Proe Fundamentals

Pro/ENGINEER

WILDFIRE 2.0 Fundamentals Written By: Michael A. Drum

Lesson 01 – Pro/ENGINEER Basic Elements 1-1 Lesson 02 – Taking a Look Around 2-1 Lesson 03 – Selecting Objects 3-1 Lesson 04 – Sketcher Basics 4-1 Lesson 05 – Sketch Feature 5-1 Lesson 06 – Extrude Feature 6-1 Lesson 07 – Making Changes 7-1 Lesson 08 – Datums Part 1 8-1

Lesson 09 – Revolve Feature 9-1 Lesson 10 – Datums Part 2 10-1 Lesson 11 – Sweep Feature 11-1 Lesson 12 – Blend Feature 12-1 Lesson 13 – Rounds 13-1 Lesson 14 – Chamfers 14-1 Lesson 15 – Draft 15-1 Lesson 16 – Hole Feature 16-1 Lesson 17 – Shell Feature 17-1 Lesson 18 – Rib Feature 18-1 Lesson 19 – Patterns 19-1 Lesson 20 – Variable Section Sweeps 20-1 Lesson 21 – Swept Blends 21-1 Lesson 22 – Boundary Blended Surface 22-1 Lesson 23 – Copy & Paste Tool 23-1 Lesson 24 – Fill Tool 24-1 Lesson 25 – Merge Tool 25-1

Lesson 26 – Trim Tool 26-1 Lesson 27 – Intersect Tool 27-1 Lesson 28 – Offset Tool 28-1 Lesson 29 – Solidify Tool 29-1 Lesson 30 – Thicken Tool 30-1 Lesson 31 – Extend Tool 31-1 Lesson 32 – Mirror Tool 32-1 Lesson 33 – Layers 33-1 Lesson 34 – Parameters & Relations 34-1 Lesson 35 – Family Tables 35-1 Lesson 36 – View Manager 36-1 Lesson 37 – Assembly Mode – Bottom-Up Design 37-1 Lesson 38 – Assembly Mode – Top-Down Design 38-1 Lesson 39 – Assembly Mode – Assembly Cuts 39-1 Lesson 40 – Assembly Mode – Assembly Operations 40-1 Lesson 41 – Drawing Mode – Drawing Fundamentals 41-1 Lesson 42 – Drawing Mode – Creating A Drawing 42-1

Lesson 43 – Drawing Mode – General Views 43-1 Lesson 44 – Drawing Mode – Projection & Section Views 44-1 Lesson 45 – Drawing Mode – Auxiliary & Detailed Views 45-1 Lesson 46 – Drawing Mode – Show Axes & GTOL Datums 46-1 Lesson 47 – Drawing Mode – Dimensioning 47-1 Lesson 48 – Drawing Mode – Broken & Partial Views 48-1 Lesson 49 – Drawing Mode – GTOLS & Symbols 49-1 Lesson 50 – Drawing Mode – 2D Drafting 50-1 Lesson 51 – Drawing Mode – Tables & Balloons 51-1 Lesson 52 – Drawing Mode – Adding Sheets & Finalize 52-1 Lesson 53 – Miscellaneous System Functions 53-1 Appendix A1 A-1 Appendix A2 A-2 Appendix A3 A-3 Appendix A4 A-4 Tutorial Data Files Fundamentals.zip

Les son

1 Lesson Objective: In this lesson, we will learn about the basic elements of Pro/ENGINEER, including the different object types, parametric modeling and design intent.

Pro/ENGINEER OBJECT TYPES Before we get into Pro/ENGINEER and start poking around, it is good to understand the different types of files created and used in Pro/ENGINEER so you will understand the terminology as we go forward. PARTS – filename.prt A Part in Pro/ENGINEER is a model that represents an individual product component. Each part is made up of features that define its size, shape, color and function. As each feature is created, a history is kept that defines how the model is made. This is known as Regeneration History. A successful feature is one that regenerates without any errors or warnings. We will see in a later topic how to deal with these situations. Parts are the building block of all Pro/ENGINEER objects. Without parts, assemblies and drawings can not exist. ASSEMBLIES – filename.asm An Assembly in Pro/ENGINEER is nothing more than a container that points to part files. Parts can be assembled into an assembly (bottom-up design), or created within an assembly (top-down design). In either method, assemblies still rely on the part file to exist. In assemblies, we can define rigid constraints (such as two objects fastened or welded together), or degree of freedom connections (such as a pin joint or a bearing). Assemblies also maintain a history of the order in which components were either assembled or created, as well as features that are created in the assembly itself (such as holes or cuts). This history must be successfully regenerated for the assembly to work properly. DRAWINGS – filename.drw

A Drawing is a two-dimensional representation of a part or assembly file. It relies on either the part or assembly to exist in order to work. Drawings contain views, tables, notes, dimensions, symbols, and other entities designed to fully describe the model for the purpose of manufacturing. FORMATS – filename.frm A Format is a file that overlays on a drawing to create the border, title block, revision block, and other company-specific standards that must always appear on that drawing. A Drawing can exist without the actual format file. SECTIONS – filename.sec A Section is a two-dimensional sketch that is used to create certain features. Sections are widely used when you are in Part or Assembly mode, and are most often created within the model, not as a separate file. A section file can be created and re-used many times. In this case the section will be saved out as a stand-alone file. We will see both types of sections in this training guide.

ADDITIONAL FILE TYPES Pro/ENGINEER also creates other types of files that may appear on your computer. The following table outlines some of these file types and their usage. File Type

Configuration Files

Error Files

Graph

Information

File Ext. .cfg .dtl .map .pcf .pnt .pro .scl .win .crc .err .out

.gph

.inf

Log Files

.log

Markups

.mrk

File Usage Govern the look, feel and behavior of the application. The extensions are: Model Tree Configuration – CFG, Drawing Setup File – DTL, User Defined Colors – MAP, Plotter Configuration – PCF, Pen Table File – PNT, Main Pro/E Configuration – PRO, System Color File – SCL and Main User Interface Configuration – WIN. These files should not be deleted. Examples: tree.cfg, e.dtl, color.map, plotter.pcf, plotter.pnt, config.pro, syscol.scl, and config.win. These files generally do not exist unless there is a problem or potential problem with something in Pro/ENGINEER. Either the model or the setup of Pro/E has an error. The extensions are: Circular Reference – CRC, Bad Geometry – ERR, Config.pro Error – OUT. These files can be deleted. Examples: 12345.crc, bad_geometry.err, and std.out Graph features can be created to drive the creation of some features using an equation. User Defined Features (UDF’s) also use this file extension when saved. These files should not be deleted. Example: holes.gph Typically created when performing an information query on an object in Pro/ENGINEER using the Info menu commands. These files can be deleted. Example: feature.inf Certain functions, such as exporting a model to an IGES format, will generate log files. These files can be deleted. Example: iges_out.log A markup file, or redline file, can be created for parts, assemblies or drawings. These can be used to convey changes electronically. The

original model or drawing must exist for these to work. These files should not be deleted.

Mass Property

.m_p .sym

Symbols

Tables

.tbl .txt

Trail Files

Example: 12345.mrk File created when running a mass property calculation on a part of assembly. These files can be deleted. Example: 12345.m_p Two-dimensional entities created in a drawing that can be re-used in other drawings. Examples of these include revision hex symbols, part marking symbols, weld symbols, etc. These files should not be deleted. Example: revision_hex.sym.1 Drawing tables that can be re-used in different drawings. Bill of material tables are a good example. These files should not be deleted. Example: bom.tbl.1 A running log file of the current session, from the moment Pro/ENGINEER is opened until the moment it closes. Stored in the c:\trails directory. These files can be deleted. Example: trail.txt.1

If you are not sure whether you can or should delete a certain file, please contact your CAD Administrator for guidance.

PARAMETRIC MODELING Pro/ENGINEER is a feature-based, parametric solid modeling tool. As described in the first section, when you create a part file, you create a series of features that add or remove material, resulting in a final model. This is what is known as feature-based modeling. Each feature contains parametric information that defines the size, shape and relationship to other features. For example, when you create an extruded protrusion that is shaped as a rectangular block, you can define the following: Length, Width and Depth of block. • Sketching Plane where you initially sketched the rectangle before extruding • it. Orientation Plane to define how you look at the sketch when you enter into • section mode. Dimensional references (such as other geometry edges, planes, surfaces, • etc.) Direction of the extrude • Parametric information comes in one of the many forms listed below. Dimensions • Relations • Parameters • References • Color (although not to a major degree that might cause a failure of the model • if missing) Some of these parameters directly affect the ability of a model to regenerate successfully, while others affect information about those features. Even if we create

features in Pro/ENGINEER that are less constrained (such as Style curves and surfaces), we are still embedding parametric information in these features. As you learn more about using Pro/ENGINEER, the idea of using parametric information becomes second nature to you, so we won’t spend any more time on it at this early juncture.

DESIGN INTENT This is, perhaps, the most important thing you should take away from this lesson, if not the entire course. Design intent is the practice of following best practices and standards to generate robust models that react well to change and function the way you intended with the fewest amount of time spent on rework. Throughout this guide, we will illustrate best ways of approaching modeling in Pro/ENGINEER, and we will also learn all about implementing design intent into a model. For now, consider this… In traditional 2D cad/drawing packages, as well as many 3D designer tools, the result is an image that best represents the final product being made. With great care and determination, you can end up with a representation that is very exact to the size and shape of the final product, but you will always lack the one thing that defines design intent, the ability to dynamically adapt to the types of changes that come about in a manufacturing environment. Sure, you can add/delete entities, drag a few curves, etc., but you will not capture the true nature of robust modeling, which is the ability to adapt to change with minimal rework. If you are using Pro/ENGINEER to simply arrive at a size and shape that represents your final product, then you are using the software as a sculptor would use clay, and are not getting the best return on your time. Design intent can be captured in the smallest details, such as the way in which you might dimension a sketch for an extruded protrusion. By dimensioning one way, you can drastically affect the way in which the part can be manufactured (tolerance stackup affects). Look at the following figure.

In this figure, we can see the overall length is called out as 8.0. If we had an overall tolerance in our model of +0.1in., then the length could vary from 7.9 to 8.1 inches when manufactured.

Now, look at the next figure, which still gives the same overall shape and size.

With the same tolerance, the overall length could vary from 7.7 to 8.3 inches, or a difference of +0.2in., which is twice the standard tolerance. This is not to say that the second dimensioning scheme is incorrect, because we might not care about the overall length, and we might be more concerned with the exact width and location of the center groove. Also, the way in which you dimension can make drastic changes easy or very difficult. You must always anticipate that you will need to change the model. This will affect the decisions you make early on when modeling. For example, in the two figures above, if we were asked to increase the length to 9.000 inches, we could simply change one dimension in the first figure, while we would have to decide which dimension we needed to change in the second figure. One might argue that simply changing the 2.5 dimension to the far right will produce the same result, and they would be correct, however in most cases, such a change is not so cut and dry. We will see this in more detail as this guide progresses.

COMMON MODELING APPROACH BOTTOM-UP DESIGN The following flowchart represents the basic steps on bottom-up design.

With Bottom-Up Design, parts are created as stand-alone files with an appropriate drawing. As you create enough parts, you begin to assemble them into an assembly file. Once the assembly is created, you create a drawing for the assembly. Each individual part has a strong chance of existing independently from each other. The assembly and the drawing files will require the part files to exist. The ability to adapt to change is reduced in this mode, because there is very little tying the parts together. For example, if you design a tote with a lid, there is no guarantee that the tote base and lid will line up. If a dimensional change is made to the base, the lid will probably not fit correctly unless it is updated as well.

TOP-DOWN DESIGN The following flowchart shows the basic steps to the top-down approach to design.

In contrast to bottom-up design, a top-down approach to design involves building the individual part files in the context of an assembly file. A neutral skeleton part captures all interface information between the components (a 3D layout), then only information needed for a particular part file is passed into that file to be used as a starting point for the geometry. Once the skeleton geometry is in the individual part, you can work in the part by itself and be confident that it will completely fit when you go back to the assembly (provided that you use the skeleton geometry to mark the location where all of the boundaries and interconnects occur. A MELTING POT Ultimately, you can choose to work in either a bottom-up or top-down approach, or choose to perform a hybrid of these two where it suits you. The type of product you are designing may help you choose which method will work better. In this guide, we will demonstrate both methods.

LESSON SUMMARY Pro/ENGINEER, like many other software packages, produces results that are only as good as the information going in. Using standards and best practices, you can master your design intent to give you robust, easy to change models and drawings. There are many different files used or created in Pro/ENGINEER, but the most common ones are Parts, Assemblies, Drawings, Sections and Formats. Parts are the building blocks for assemblies and drawings and must always be present for these others to work. When designing in Pro/ENGINEER, you may choose to build your parts then assemble them (a bottom-up approach to design), or you may wish to build your parts in an assembly to provide a more accurate and complete fit (a top-down approach to design). The type of project will determine which approach works best.

Lesson

2 Lesson Objective: In this lesson, we will learn about the User Interface of Pro/ENGINEER Wildfire 2.0, file operations, viewing modes and how to spin, pan and zoom in this release.

STARTING Pro/ENGINEER Pro/ENGINEER Wildfire 2.0 is installed in the C:\ptc\proewf2 directory. On your desktop, you will find the following shortcut.

When Pro/ENGINEER launches, it will start in the following directory. C:\Data\proewf2

Every time you open up a new session of Pro/ENGINEER, a file is created that captures every command, menu pick, and operation you perform. This file is called a trail file, and it is created and stored in your C:\Data\trails folder. Trail files can be used (with some limited degree of success) to restore work that is lost if you crash out of Pro/ENGINEER without having saved, however most of the time, this is not successful. Trail files do not need to be saved. Since they take up some disk space, it is recommended that you clean out your c:\trails directory from time to time.

USER INTERFACE Once you launch Pro/ENGINEER Wildfire 2.0, you will see the following user interface.

The following figure shows the different components of this interface when a model is opened.

The Wildfire 2.0 interface is made up of the following main areas (from top to bottom and left to right): Title Bar – Lists the currently object, and indicates whether the object is • active. Menu Bar – Every command in Wildfire 2.0 can be accessed from the • menus at the top of the application. System Toobar – Contains icons that control system-wide functions, such • as the file operations, model display, datum display, window controls, etc. Navigator – Contains several different tools used to navigate through the • model or the interface, such as the model tree, layers, file explorer, favorites, and web browser controls. Web Browser – This is a fully functional web browser. Upon the initial • startup of the application (or by clicking on the home icon), you can get to a web page with helpful information regarding this release. It also doubles as an information window for various tools in the software, such as a feature information window, bill of material reports, and when you click on a folder in the file explorer, it shows the contents in this browser. Working Window – This is the main working area in Pro/E. Your geometry • or drawing will appear in this window, and you select and build features in this area. Feature Toolbar – Contains icons used to create or edit geometry. These • are context-sensitive, which means that as you are in a specific function, you will see additional or fewer icons. Dashboard – Appears in most of the common feature creation modes. • Contains options and elements for defining features. Message Bar – Area where information is displayed in the form of prompts, • warnings, general information, etc. Status Bar – Provides additional information if necessary. It also displays • the tool tip when the mouse is placed over an icon, menu or geometry in the main working window or in any of the other toolbars. Selection Filter – Used to select different filter options for picking. Displays • the total number of selected objects.

COLOR SCHEME Every command or function in Wildfire 2.0 that displays graphically will have a different color associated with it. For example, when you move your mouse over a model, you will see geometry highlight in blue. Once you select geometry, it turns red. As you create features, you will see a yellow preview of the geometry. Datum planes have a positive brown side and a negative black side, etc. For the purpose of being able to clearly print and read this training guide on most Black & White LaserJet printers, most of the system colors will not appear in the pages of this booklet. We will clearly describe colors that you should see at the time you should see them, so you should be able to follow along very easily. The following figure describes the convention that we will use for this guide.

FILE OPERATIONS SET WORKING DIRECTORY If you recall from the first section of this lesson, we mentioned that Pro/ENGINEER Wildfire 2.0 starts up in the C:\Data\proewf2 folder. You can change over to any folder on your computer after you open up the software. The folder that you change to is called the Working Directory. If you choose not to change over to a new folder, then the start up directory is the working directory. To change your working directory, there are three ways to do this. Using the menu bar, go to File, Set Working Directory, or click on the following icon in the system toolbar.

With either of these options, you will get a new window that appears, as shown below.

In this window, select the folder you wish to use as a working directory. You can use the Directory Pull-Down to switch to a folder or network drive, use the Up One Level icon to go up one folder level, or you can even create a new folder in the current location using the Create New Folder icon. Once you have selected or created the working directory folder, click on OK. The third way to set your working directory is to go to your Navigator and access the file explorer. Find the folder that you want to work out of, then hold down the right mouse button over that folder and select Make Working Directory, as shown in the following figure.

OPEN FILES Opening files in Pro/ENGINEER is the same as in any windows application. Either go to File, Open from the menu bar, or select on the following icon from the system toolbar.

You will get a window that is very similar to the one you saw when setting your working directory, as shown below.

Initially, all Pro/ENGINEER items (parts, assemblies, sections, drawings, formats, etc.) will show up in the window for the current directory that you are in. If you want to apply a filter to only see part files, use the Type Filter pull-down towards the bottom of the window. If you are browsing through other folders and wish to return to the current working directory to look there, click on the Working Directory icon. To browse through favorite locations that you set up, click on the Favorites icon. You can also change the display type using the Change Display Options icon. This would allow you to see a list, or icons, or details, etc. In Session Memory Every time you open up a file in Pro/ENGINEER, it gets stored into memory. This is called Session Memory. The item does not have to be open to remain in memory. To view what is currently in memory, go to the open file window, and click on the In Session Memory icon (shown above). Only items that are in memory will be listed. Preview To see what the object looks like before opening it, you can click on the Preview button in the lower right portion of this screen. It will expand the window open to the right, and you will see the file, as shown in the figure at the top of the next page.

Once you find the file you want, either double-click on it using the left mouse button, or click on it once to highlight it, then click on the Open button in the lower left of the File Open window. Another way you can open a file in Pro/ENGINEER Wildfire 2.0 is to go to your file explorer in your Navigator, locate the folder that contains your file, and click on that folder once with the left mouse button. The contents of the folder will appear in the Web Browser, as shown below.

To preview the geometry before opening it, click once on the file in the File Names column. The preview appears at the top of the screen as shown at the top of the next page.

To open the file, either double-click on it using the left mouse button, or drag the file from this list out to the Working Window. ERASE As we mentioned previously, once you open up a file in a current session of Pro/ENGINEER, it remains open until one of two things happens. You exit the application using File, Exit. • You erase the object from memory. • Simply closing the file will not erase it from memory. To erase a file, go to File, Erase from the menu bar. You will see two options for erase. These are: Current – Open erases the active file from memory (next topic). • Not Displayed – Erases all objects that are not currently open. • EXAMPLE: Suppose you open three part files, A.prt, B.prt and C.prt. All three files are currently in session memory. If you were to close part B, it is still in memory. If C were the active model, and you used File, Erase, Current, then C (and only C) would be closed and erased from memory. If you used File, Erase, Not Displayed, then B (and only B) would be erased from memory. A and C would remain open and in memory. ACTIVATE OBJECT The object you are currently working on is considered the Active object. You can have as many files open at the same time, but only one can be active at any time. To activate an object, go to Window from the menu bar. At the bottom of this menu, you will see a list of currently open objects, as shown below.

The object that has the black circle to the left of it (currently shown as the CROSS_FEED_STOP.PRT file in the figure at the bottom of the previous page) is the active model. To activate a different model in this list, simply select it from the list at the bottom. To close a file, it must be the active file, then you can use Window, Close or File, Close Window from the menu bar. If you were to open a file at this point in time, it will become the active model automatically. You might notice that you have icons in your Windows Start Bar on your desktop for each of the objects that are currently open in Pro/ENGINEER. If you were to select the icon in this Start Bar, it will bring that object to the front of the Pro/ENGINEER interface, but it does not automatically make that model active. You can activate it by going to Window, Activate from the menu bar once the file is in the foreground. You will be able to tell if the currently visible object is active by looking at the title bar in the upper left corner. The following figure illustrates an active and inactive object indicated by the title bar.

SAVE FILES To save the current file, go to File, Save or click on the following icon in the system toolbar.

In the message window, you will be shown the part that is being saved. Click on the Enter key on the keyboard, or the green check mark to the right of the message window. File Versions

Most Pro/ENGINEER files append a number at the end of the file extension – filename.prt.1 for example. Every time you save that object, a new file will be created with the next higher integer – filename.prt.2 in this case. Your working directory will start to fill up with versions of the same file. For example, if you create a new part called mypart, and save it for the first time, you would see the following in your working directory. mypart.prt.1 As you continue to work with this part, you will save often. By the end of the day, you may have saved this part 10 times, and so you would see the following in your working directory. mypart.prt.1 mypart.prt.3 mypart.prt.6 mypart.prt.9 mypart.prt.10 mypart.prt.4 mypart.prt.7 mypart.prt.2 mypart.prt.5 mypart.prt.8 You will notice that, sorted by name, the .10 file comes right after the .1 file. Be aware of this if you decide to manually delete older versions. DELETE FILES Before you delete any Pro/ENGINEER files, be absolutely sure that no other Pro/E files are dependent on the files you wish to delete. For example, suppose you created an assembly and used a particular component. If you delete this part before you take it out of the assembly, then the assembly will fail when you try to open it. To delete a Pro/ENGINEER file (part, assembly or drawing), the best way to do this is to go to the menu bar and select File, Delete. When you do this, you will see two options. • Old Versions – Delete all of the versions from the hard drive except the most recent for the currently active file. This method purges old versions but leaves the most recent in memory. All Versions – Delete all versions of the file from the hard drive, including • the most recent, and erase the current file from memory. This is a total loss of data for this file. It is not recommended that you blindly delete files from your hard drive through a windows explorer unless you really know the relationships. It is recommended that you purge your working directory once you are satisfied with the most recent version of the file that you are working on. This will free up disk space. SAVE A COPY This command is used to do one of the following: Make an exact copy of the current object with a new name. • Export the file into a different file type (such as IGES, STEP, STL, etc.) • With the current object open, go to File, Save A Copy from the menu bar. You will see the following window.

To make an exact copy with a different name, first select the directory where the file is going – or leave this step out to make the copy to your current working directory. Then, enter a name in the New Name field. Once you are done, click on OK. To export the model as a different file type, first select the directory where the file is going – or leave this step out to create the new file in the current working directory. Then, use the Type pull down to find the file type that you wish to create (IGES, for example). The name should appear automatically in the New Name field with the appropriate extension added. Click on OK to complete the file export. BACKUP The backup command creates the exact file that you are working with, but in a different directory. The difference between a Backup and a Save A Copy is that a Backup allows you to keep the same name, but Save a Copy forces you to specify a different name. The backup command is really useful if you need to make a duplicate copy of an entire assembly, because it copies the assembly and all of its components to the directory you specify. To perform a backup, go to File, Backup from the menu bar. You will get the following window.

Click on OK to complete the backup operation. RENAME You must really be aware of relationships when renaming in Pro/ENGINEER. NEVER rename a part using a windows explorer, always rename through Pro/ENGINEER. When you rename a part file, you must have any assembly and/or drawing file also open. If you do not, then the assembly or drawing will still be looking for the old file name when it tries to open, and when it doesn’t find it, it will fail. To rename the currently active file in Pro/ENGINEER, use File, Rename. This will bring up the following window.

Enter a new name for the file in the New Name field, then select the option below this. There are two options: Rename on disk and in session – renames the file in memory, and • renames it on the hard drive (for all versions that exist). This is the preferred option for most renaming operations. Rename in session – renames the file only in memory. • There are only two reasons why you might want to rename in session only. The first is if you accidentally renamed a part, and forgot to open the drawing or assembly file that uses it, then you could rename the part to the old name temporarily in memory to

allow the assembly and drawing to open up, then rename it back to the new name once those files are open. The net change would be zero for the part. The other case would be if you wanted to perform a “Save A Copy” type of command. If you rename the current file in memory only, then save it, it creates a new file in the working directory. This might be useful if you already made changes to an existing file, then realized that you forgot to save a copy of it first. By renaming it in memory then saving it, you left the original file at its last save. The proper order of operations should be followed when performing a rename on disk and in session. 1. Open up the object to rename. 2. Open up all drawing or higher level assemblies where this object reports. 3. Rename the object then save it. 4. Change over to one of the other files (drawing or assembly) where the object reports and verify that the name has been changed for these files, then save them. 5. Repeat step 4 for every drawing or assembly file that contains the renamed object. 6. Close all objects and erase session memory (not displayed). 7. Retrieve each file to make sure the rename was successful. NEW FILES To create a new file in Pro/ENGINEER, go to File, New from the menu bar, or click on the following icon in the system toolbar.

This will bring up the figure at the top of the next page.

In this window, start by selecting the primary type of file being created (Part, Assembly, Drawing, Sketch). Our Pro/ENGINEER license only permits the following primary types to be created: Sketch • • Part Assembly • Drawing • Format • Report • • Layout Markup • Once you select the primary object type, the Sub-Type options will change to reflect possible choices. In the figure above, we can see the sub-types for a part file. Select the appropriate choice. Finally, enter a name for the file. Always remember to do this so you can avoid a rename condition later. Once you are done, click on OK to continue. You will now see the following figure.

For this next window, the template should automatically select one of the following: Startpart – if you selected Part for the primary type, and Solid for the sub• type. Sheetmetal – if you selected Part for the primary type, and Sheetmetal for • the sub-type. Startassy – if you selected Assembly for the primary type, and Design for • the sub-type. If you selected Drawing for the primary type, there are no sub-types. We will talk about all of these in more detail starting in the next chapter.

VIEWING MODES There are four primary viewing modes in Pro/ENGINEER for Parts and Assemblies. To select a viewing mode, pick one of the following icons in the system toolbar: •

Shaded – All external surfaces of the model are rendered and all hidden edges and surfaces will not be visible.

•

No Hidden – All external edges of the model are shown in the primary model color, but all hidden edges and surfaces will not be visible.

•

Hidden Line – All external edges of the model are shown in the primary color, while all hidden edges are displayed in a muted color.

•

Wireframe – All edges of the model (external or hidden) are shown in the primary color.

The following figure shows the four different viewing modes for a part file.

Shaded mode requires the least amount of time to display, and provides the best results for spinning. Wireframe is the second fastest in terms of display and spin, but is the least user friendly from a viewing standpoint.

MOUSE CONTROLS (SPIN, PAN & ZOOM) LEFT MOUSE BUTTON

• Stand-alone, it is used to select/deselect objects • Ctrl + = Select/deselect multiple objects • Shift + = Select Seed and Boundary or Chain of objects

RIGHT MOUSE BUTTON

• Context sensitive commands when held down • Click to “Query Select” through model where mouse pointer is located • Shift + = When selecting, it queries through multiple choices for the selected object. For example, when a single edge is selected, it will go through one-by-one, tangent chain, from-to chain, etc.

MIDDLE MOUSE BUTTON (Standard Mouse) • Used to accept selections or finish commands when clicked

3D Modes • Used to spin the model when dragged in all directions • Ctrl + = Zoom In/Out (drag mouse in front [F] or back [B] direction) or Turn (drag mouse in Left [L] or right [R] direction – snaps to 90 degree locations). • Shift + = Pan when dragged in all directions 2D Modes • Used to pan when dragged in all directions • Ctrl + = Zoom In/Out (drag mouse in front or back direction) MIDDLE MOUSE BUTTON (Wheel Mouse)

Same functions as regular middle mouse, PLUS… • By itself, it does quick zooming in and out when wheel is rolled Front or Back • Ctrl + = 2X Quick Zoom speed (for rapid zoom). • Shift + = 0.5X Zoom Speed (for slower zoom).

When spinning the model, you have two different ways to control the spin using the spin center. The spin center on/off control is located in the system toolbar, and it looks like the following.

When the Spin Center is turned ON, Wildfire 2.0 will always spin about the spin center, usually located at the geometric center of the model. This is the easiest spinning method to use, but does not give much control when you are zoomed into the model. When the Spin Center is turned OFF, Wildfire 2.0 will spin about the location of your mouse cursor at the time you press down the middle mouse button/wheel. This allows for more control of the spin, especially when zoomed in close enough that the spin center is off the screen.

VIEW ORIENTATIONS In addition to being able to spin, pan or zoom using the mouse and keyboard, you have other ways to control the orientation of the model on the screen. This section will discuss these different methods. SAVED VIEWS Built into the start part or start assembly, there are pre-defined saved views. These are FRONT, BACK, TOP, BOTTOM, LEFT, RIGHT, ISOMETRIC and TRIMETRIC. These views were created so the positive side of the default datum planes (which we will talk about in lesson 6) faces in the orientation of its name. For example, the FRONT datum plane’s positive side faces the FRONT orientation. The FRONT datum plane’s negative side faces the BACK orientation. To access saved views, click on the following icon in your system toolbar.

It will expand to show the views that are available to pick on, as shown below.

DEFAULT VIEW The default view is a system-defined view that exists for all models, even if there are no other saved views. Many times in Pro/ENGINEER, you will return to a default

orientation to make seeing or selecting easier. To go to the default view, click on the following icon from the system toolbar.

PREVIOUS VIEW To toggle between the current orientation and the last orientation, click on the following icon in the system toolbar.

RE-ORIENT To create new orientations, click on the re-orient tool in the system toolbar (the icon shown below).

This will bring up the following window.

The default type of orientation type is Orient by Reference. The goal in this section is to pick two planar surfaces or datum planes that are perpendicular to each other and face them towards specified directions. Once you enter into this tool, you are automatically asked to select the first reference, as we can see in the figure above. Using the pull-down, we can change the direction the first reference will face. In this case, the first reference will face the Front (or face the screen). Look at the following figures to see an example of using this tool. Start by selecting the first reference and its resulting orientation.

Once you select the first reference, it will appear in the field to the right of the selection arrow. Next, select the orientation and reference for the perpendicular direction. In the next figure, we will chose to face our reference towards the right, therefore we will select the right side of the model, as shown below.

If the two references we selected are perpendicular to each other, the model should snap to its new orientation, as shown below.

In addition to selecting references to re-orient our model, we can dynamically control the spin, pan and zoom of our model by using the pull-down at the top of this Orientation window, and selecting Dynamic Orient. This will change the window to look like the following.

In the top portion, we can control the Pan of the model on the screen. In the second section, we can contrl the Zoom, and in the third section, we can control the Spin. Use the sliders or type in exact values in the spaces provided. Under the Spin portion, you can select whether you are spinning about the spin center or about the screen center. Down at the bottom of the Orientation window, you can also access the Saved Views functionality. Click on the blue bar where the name Saved Views appears to expand or collapse it. Expanding it will show the following.

You can double-click on any of the pre-existing orientations to set the model to that orientation, or type in a new name in the Name field, then click on Save to create additional saved views.

The last option at the top of this window is to change preferences for the re-orient tool. When you select Preferences you see the following.

At the top of this window, select where the spin center will be. By default it is located at the model center (geometric center of the model). In the lower window, you can specify which orientation will be used for the default view.

MISCELLANEOUS PRINT When printing in Pro/ENGINEER, use one of the three non-shaded modes for printing parts or assemblies. To print, go to File, Print from the menu bar, or select the following icon on the system toolbar.

This will bring up the following window.

The first thing you want to do is select the printer that you are going to print to. Do this by selecting on the down arrow at the top, as shown in the following figure.

This list of printers is defined using Plotter Configuration Files (PCF). If you do not see a printer listed that should be listed, please contact your system administrator. Once you select your printer, the rest of the options on the Print window will become active. To change any of the print job settings, click on the Configure button, which will bring up the configuration for the current printer selected, as shown below.

There are three tabs on this window. Within this section, you can select paper size, orientation, print zoom options, etc. The PCF files should be set up to use the optimal print settings for the printer, including the correct paper size. You should not have to change any settings in this window for most print jobs. ZOOM CONTROLS In addition to the dynamic orient and mouse controls, you have a few additional options for zooming on the system toolbar. These are:

•

Window Zoom – Click the opposite corners of a box around any object you want to zoom in on.

•

Zoom Out – Each time you select this icon, it will zoom out a small amount.

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Refit – Zooms out/in until all objects are visible and centered in the working window. This does not work if you are in a sketch for the first feature of the model.

REDRAW (REPAINT/REFRESH) Occasionally, you will need to redraw your screen to eliminate any graphical blips or ghost images, etc. This is also referred to as repaint or refresh. To redraw your screen, click on the following icon in the system toolbar.

LESSON SUMMARY When you start Pro/ENGINEER, you will be placed into a working directory. Change over to the working directory you wish to use then start working. When you save a file in Pro/ENGINEER, new versions of the file will appear in your working directory. Use Delete, Old Versions to purge all versions except the most recent. If you must rename a file in Pro/ENGINEER, always make sure that any required files are also open and in session. Start renames with the lowest level object (Part Files), then rename assemblies, then drawings. Remember to save as you go. To save session memory, erase non-displayed objects once you have saved and closed them. The middle mouse button (MMB) is used for spinning when used by itself. Use Ctrl with the MMB to zoom, and Shift with the MMB to pan. You can select from pre-existing saved views, or re-orient the model to create your own saved views. There are four viewing modes. Shading is the best for spinning, panning, zooming and visualizing the model. Hidden line and No Hidden take longer to display.

EXERCISES Once Pro/ENGINEER is opened, set your working directory to C:\Data\ProETrain.

Click on this folder in the file explorer (navigator) to see the contents. Click once on the Idler_Arm.prt part file to see the preview in the web browser. Try spinning the model in the preview window. Place your mouse over the icon to the left of the Idler_Arm part file and drag it into the working window to open it. Inside the working window, try spinning, panning and zooming using the mouse and keyboard controls. Once you are done, go back to a default view. Try looking at the different display modes. Use the Saved Views icon to go to a FRONT view. Close the model but don’t exit out of Pro/ENGINEER. Use File, Erase, Not Displayed once the file is closed to erase session memory.

Les son

3 Lesson Objective: In this lesson, we will learn about action-object versus object-action selecting, query select, as well as pre-selecting.

ACTION-OBJECT / OBJECT-ACTION SELECTING Some of the features in Pro/ENGINEER are created by selecting on an action first (Insert, Blend, Surface, for example), then later you select your references, such as curves, planes, etc. In Pro/ENGINEER Wildfire 2.0, most of the common feature types can also be created using an Object-Action method of selecting. For example, to create a surface copy, you would have to select your surfaces first, then click on the copy icon. In order to make Object-Action selecting easier, there is a Pre-Selecting function that allows you to see a preview of the geometry you are going to select before you select it.

PRE-SELECTION

As you move your mouse over a model in the working window, you will see objects highlight in blue. When you move your mouse past the object, the highlight disappears, and a new one appears at the next location. This blue highlighting is called Pre-Selection. If you leave your cursor over a highlighted object long enough, a tool tip will appear showing you the feature that is currently highlighted. In the following figure, we can see a protrusion highlighted.

With the highlight visible on the feature or geometry we want to select, we use the left mouse button to click on that object. The object will turn red, which indicates that it has been selected, as shown below.

To remove any selections you may have made, click anywhere outside of the model in the working window.

SELECTION FILTER During pre-selection highlighting, you may see only features highlighting. This is due to a filter that is applied by default, called Smart. We can see the selection filters in the lower right corner of the Pro/ENGINEER interface, as shown below.

The smart filter performs a “Drill Down” approach to selecting. You begin by selecting features (Protrusions, Cuts, Drafts, Rounds, etc.), then you pre-select geometry, such as surfaces, edges, vertices, etc.

If we click on the pull-down arrow in this field, we can see the other filters that can be applied.

The other, different filters are: Features – only features will be selectable. • Geometry – only geometry (surfaces, edges, etc.) will be selectable. • Datums – only datum geometry (planes, axes, points, curves, etc.) will be • selectable. Quilts – only surface quilts will be selectable • Annotation – only notes, geometric tolerances, etc. will be selectable. • For example, if we change our selection filter to Geometry, then place our mouse over the same protrusion as we did before, we will only see a surface pre-select highlight, as shown in the figure below.

Then, if we click with our left mouse button to select the surface that is highlighted, we see something slightly different than what we saw when we selected the protrusion before.

A surface, when selected, will shade or mesh, depending on what view display you have set. In No Hidden, Hidden Line and Wireframe, the selected surface will mesh, as we see in the figure above. In Shaded mode, the entire surface will shade a rose color, as we can see in the following figure.

For the remainder of this training guide, we will only show figures in a non-shaded mode (unless it is necessary for clarification to show it in shaded mode). This is due to the ability for you to see these figures when reproduced on a black & white color copier.

QUERY SELECT Often times, what we want to select is not at the front of the model in the current orientation. Instead of rotating the model around every time we want to select hidden geometry, we can use a tool called Query Selection, which allows us to query through possible objects until we see the one we want in a pre-selection highlight (blue highlight).

For example, suppose I want to select the two surfaces of the hole indicated below.

If I have my selection filter set to Geometry, and place my cursor over the hole, I can see that the back half of the hole can be picked without querying through the possible choices, as shown below.

Now, I want to pick the other half. The first thing I need to do is hold down the Ctrl key on my keyboard to select multiple objects. When I place my mouse cursor over the end of the hole, only edges highlight in blue. I could zoom in or rotate and get a clear view of the other half of the hole, but that would defeat the point to this discussion. Instead, I am going to place my mouse cursor over the model in an area that is in front of the surface that I want to select. Imagine if the mouse cursor were a drill bit going into the screen of the computer and into the model in its current orientation. You want to place your cursor over the model so that as you “drill” down into the part, you come in contact with the object you want to select. The figure at the top of the next page shows a possible location that clearly sits in front of the surface that we ultimately want to select.

Since the outside surface of the protrusion is in front of our hole, only the protrusion surface highlights initially, as we can see in the figure above. To query through the possible choices, click on the right mouse button (remember to keep the Ctrl key pressed to select multiple objects). A single click results in the hole surface highlighting, as shown below.

Now that the surface we want to select is highlighted in blue, we can click with the left mouse button to select it, as shown below.

REMEMBER! – Even though we are working in a non-shaded mode, we still have surfaces on this model. To select a surface, you want to pick out in the middle of the surface and not near its edges, otherwise you might select an edge instead.

This is one of the biggest mistakes new users make that come from 2-D or other drawing packages. The following figure shows the correct and incorrect place to pick for selecting a surface.

EDGE SELECTING Using the same selecting techniques, we will talk about selecting edges. To start with, you can select a filter, such as Geometry, which will allow you to pick just edges, surfaces, etc. Then, bring your mouse over the edge to select. As with surfaces, it will pre-highlight in blue, as shown below.

When you click with the left mouse button, the edge becomes selected, as indicated by a bold red highlight, shown below.

You can hold down the Ctrl key to select multiple edges independently, however we are going to demonstrate how to pick edge chains. If you hold down the Shift key, then move your mouse cursor over to a different edge (in this case, on the same surface), we will see different objects highlight, as shown below.

The first thing it looks for is any tangent chain of edges to the one we originally selected. From the figure above, we can see that there are four other edges (two straight edges at either end, and two circular edges around the corners) that connect up to the first selected edge to form a tangent chain of edges. The Tool Tip indicates Tangent. If we query select (click with the right mouse button), we will see another possible option for edges, which in this case is the entire set of edges that go around the top surface (connected to the edge that we previously selected). The tool tip indicates Surface Loop, as shown below.

Click again with the right mouse button, and we will see a From-To surface loop starting from the selected edge and going around the top surface boundary until it gets to the edge our mouse is currently over, as shown below.

Click one more time with the right mouse button, and we see the opposite surface loop condition (going the other direction around the top surface boundary).

If this were the set of edges we wanted, we could now click with the left mouse button to select it (remember, we are still holding down the Shift key on the keyboard.)

SEED AND BOUNDARY SURFACE SELECTING One last method of selecting is to get all of the surfaces between two boundary surfaces. One of the boundary surfaces actually lies within the set of surfaces to be selected. This is known as the Seed surface. The other surface lies at the external end of the surfaces to be selected, and is called the Boundary surface. The following figure illustrates the seed and boundary surface you would select to get all of the internal surfaces of our cavity.

Therefore, we will begin by selecting the seed surface, as shown in the following figure.

Next, hold down the Shift key and select the top surface of the part (the Boundary surface). While the Shift key is still depressed, you should see the following.

Once you let go of the Shift key, the proper surfaces will be selected, as shown in the next figure.

The Boundary surface is never selected, only the Seed surface and all of the other surfaces between the seed and the boundary. To select additional surfaces at this point, use the Ctrl key. To deselect any of the selected surfaces, also use the Ctrl key and select the surfaces to exclude. For example, selecting the back surface with the Ctrl key gives us the figure at the top of the next page.

A RUNNING TOTAL Within the selection filter area, we will see some text indicating how many objects are currently selected. For example, if we were to select the following surfaces and edges using the Ctrl key, we would have 8 items selected.

In the selection filter area, we see text that says 8 Selected, as shown below.

If you double-click on the actual text, it opens up the window shown at the top of the next page.

As you move your mouse over this list, the items will highlight in blue on the model itself. You can remove any unwanted selections by selecting them in this list, then clicking on the Remove button at the bottom.

LESSON SUMMARY Many of the features in Pro/ENGINEER use an object-action method of selecting, or selecting the surfaces or edges that you are going to act upon, then pick the feature to create, such as picking on an edge, then picking the round tool. You can pre-highlight objects before selecting them. This makes it easier to know what you are going to pick. Use the selection filter in the lower right corner to pick only on the types of objects you want. Use Query select to drill down into the model to pick hard to reach items, or to scroll through a set of possible edge chain options.

Finally, use the Shift key to perform Seed and Boundary or Edge Chain selecting, and use the Ctrl key to pick many individual items.

EXERCISES Open up the Idler_Arm part file and go to a default view. Using techniques learned in this lesson, try selecting all of the edges that touch the front face of the part, as shown in the following figure.

Next, use whatever method you want to select the following surfaces (NOTE: This can be done with a seed and boundary if you pick the right combination of surfaces).

Close out of this model when done, and erase session memory.

Les son

4 Lesson Objective: In this lesson, we will learn about the sketcher functionality.

STAND-ALONE SKETCHER Many of the features in Pro/ENGINEER require you to sketch a profile then perform some sort of operation on that sketch, such as extrude, revolve, sweep, etc. When you are creating features that require a sketch, you enter sketch mode through the feature. To introduce sketcher functionality, we are going to create stand-alone sketches. The only time you ever create stand-alone sketches (besides for training purposes), is to create sketches that you can re-use. We will see examples of importing saved sketches into feature creation later in this guide. For now, please understand that you normally will not enter sketch mode as a standalone process. To start a sketch in stand-alone mode, go to File, New from the menu bar, or click on the following icon in the system toolbar.

When the window pops up, select the Sketch type, which has no sub-types. In this example, I am going to call this sketch Latch_Plate. The window will look like the following.

Clicking on OK brings you into the sketch. The figure at the top of the next page shows the sketcher toolbar, which appears at the right side of the working window, in the feature toolbar.

SKETCHER STEPS To effectively use sketcher, it is highly recommended that you follow these steps in this order. 1. Select/Deselect References – If entering sketch mode in the middle of creating a feature, and there is already geometry in your model, then this step applies. Otherwise, for stand-alone mode, skip this step. 2. Sketch Quickly – Your goal when sketching is to capture the basic shape, but not to worry about looking perfect, or even getting close to the proper size. If you spend too much time sketching, then you are using it incorrectly.

3.

Add Constraints – Add any constraints to the sketch to reduce the number of necessary dimensions (such as equal length, or perpendicular, etc.) 4. Dimension Completely – As you will see, sketcher does not allow you to under- or over-dimension a sketch, but you should use basic manufacturing principles when adding dimensions. Remember design intent when doing this, because the dimensions that you add in the sketch are the ones that you are going to use to make changes later, so pick dimensioning references wisely. 5. Modify Dimensions – Only after all of your entities are sketched, constrained and fully dimensioned, should you modify the dimensions to their proper values. Modifying the dimensions as you go may cause the sketch to warp or fail regeneration. There are tools in the modify command to stop regeneration or to scale the sketch. We will see this in more detail coming up. 6. Finish – Once your sketch looks good, accept the sketch to continue the feature creation, or to finish out of the stand-alone sketch.

LINE TOOLS If you click on the Line Tools Icon, it will expand to reveal the following line types.

LINE Using the left mouse button, click where the start of the line is, then move your mouse to the location where the end of the line is. Click again with the left mouse button to place the end of the line. The line tool remains active, allowing you to pick the endpoint of the next line (which starts at the end of the first line). Continue selecting locations for line endpoints until you have sketched all lines, then use the middle mouse button to complete the line tool. The following figure shows sample lines. NOTE: The display of dimensions and constraints have been turned off in the figure below. Each sketch segment contains a blue dot locating its endpoint.

TWO-TANGENT LINE This line entity is created tangent to two circles, arcs or combination of the two. With the left mouse button click on one arc/circle, then move your mouse over to the other

arc/circle. The line should automatically adjust itself to snap tangent to both entities (at both ends). Click with the left mouse button once you see the tangent snap occur. This line tool remains selected, but not active (in other words, you must start a new one by picking on the first arc/circle again, instead of continuing at the endpoint of the previous line). The following figure shows a sample two-tangent line between an arc and a circle. NOTE: The display of constraints has been turned on, but the display of dimensions still remains off. Notice the small “T” symbol that appears at each endpoint. This shows the tangent condition.

CENTERLINE Centerlines are used as snap lines, symmetry lines (for mirroring) or as axes of revolution if creating a revolved feature. When you sketch a centerline, its length occupies the entire working window. You click once with the left mouse button to locate a point on the line, then move your mouse until it is in the orientation that you want. Click with the left mouse button again to finalize the line. The centerline tool remains selected, but not active in the working window. The following figure shows three centerlines. At their intersection, a sketch point appears automatically.

RECTANGLE TOOL The rectangle tool is only a single icon, shown below.

To use the rectangle tool, use the left mouse button to locate one corner of the rectangle. Move your mouse to the location of the opposite corner, and then click with the left mouse button again to finish the rectangle. The following figure shows a sample sketched rectangle. Again, the display of dimensions and constraints has been turned off.

CIRCLE TOOLS If you click on the Circle Tools icon, it will expand to reveal the following tools.

CIRCLE To use the circle tool, click with the left mouse button to locate the center of the circle, then move your mouse to adjust the diameter. Click again with the left mouse button to place the diameter. The following figure shows a sample circle.

CONCENTRIC CIRCLE The concentric circle tool creates a circle whose center lies at the center of an already existing circle or arc. To create this, use the left mouse button to select an existing circle or arc on the sketch. Then, move the mouse cursor to drag out the diameter. Click with the left mouse button again to place the diameter. This circle tool remains active, and allows you to create multiple circles with different diameters located at the same center point. To cancel out of this circle, click on the middle mouse button. The following figure shows a concentric circle at the center of an existing arc.

THREE-POINT CIRCLE The three point circle is created by clicking or selecting any three sketch points, vertices or general locations on the sketch. When you click on the second point, the circle will appear, and the third point locates the diameter.

The following figure shows a sample three-point circle using three random locations on the sketch.

THREE-TANGENT CIRCLE The three-tangent circle is created tangent to three entities (lines, arcs, etc.) To create this, use the left mouse button to select the three entities the circle is to be tangent to, and the circle is created automatically. The following figure shows a sample three-tangent circle using two lines and an arc.

ELLIPSE An ellipse is a circle that is longer in one direction and shorter in another (like an egg). The ellipse tool in sketcher creates only horizontal or vertical ellipses, however you can use the transform tools to rotate it 45 degrees, for example. To create the ellipse, use the left mouse button to locate the center of the ellipse, then move the mouse to locate the horizontal and vertical radii. If you move more to the left or right away from the first point than you do up or down, you create a horizontal ellipse, and the opposite creates a vertical ellipse. The figure at the top of the next page shows a sample horizontal ellipse.

ARC TOOLS Clicking on the arc tools icon expands it to reveal the following tools.

TANGENT-END / THREE-POINT This general arc tool gives you two different options. The Tangent-End arc tool creates an arc that is tangent to an existing line or arc at its endpoint. To create this arc, use the left mouse button to select the open end of an existing line or arc segment. When you do this, a special symbol appears at the end, which looks like a green circle with a big “X” through it, as shown below.

The “X” breaks up the circle into quadrants. Depending on which quadrant you move your mouse out from, you will either get a tangent arc or a three-point arc. The following figure shows the quadrants that affect the result.

To create the tangent arc, bring your mouse out of the circle in the quadrant at the end of the line segment (indicated above), and then use the left mouse button to locate the free end of the arc.

The following figure shows the resulting tangent-end arc. Note the “T” symbol at the intersection of the arc and line segments. This is the tangent constraint.

The Three-Point arc is created by picking on the two endpoints of the arc, then dragging out the radius. When starting from an existing line or arc segment, be sure to come out of the quadrants to the side of the existing segment to avoid a tangentend arc. The following figure shows two three-point arcs (one from an existing segment, and the other just by itself.

CONCENTRIC A concentric arc is created by using the left mouse button to select on an existing arc or circle, then move the mouse cursor to drag out the radius. While the radius shows up in a dashed circle, use the left mouse button to select the start of the arc, then move your mouse to locate the end of the arc. Click with the left mouse button to place the end of the arc. As with the concentric circle tool, the concentric arc tool remains active, allowing you to create multiple concentric arcs on the same center. To finish out of this tool, use the middle mouse button once you have completed your desired arc(s). The following figure shows a concentric arc using an existing circle to determine the arc center.

CENTER-ENDS The center-ends arc is created by using the left mouse button to select the center of the arc. Move your mouse cursor to drag out the radius of the arc (which is indicated by a dashed circle), as shown in the following figure.

Use the left mouse button to select the start point of the arc, then move your mouse to locate the end point. Once you have located your end point, click with the left mouse button to place this end point. The figure below shows the resulting centerend arc.

THREE-TANGENT Similar to a three-tangent circle, a three-tangent arc is created by using the left mouse button to select three entities the arc will be tangent to. The first two points determine the endpoints of the arc, while the third point selected is used to determine the radius. The following figure shows a three-tangent arc using two line segments and an arc.

The “T” constraint symbols appear at the location where the tangency condition exists. CONIC A conic arc is an arc that does not have a circular profile to it (similar to an ellipse). You create the conic arc by using the left mouse button to pick the two endpoints of the arc, then drag out the radius. A centerline is created automatically through the endpoints. The following figure shows a sample conic arc.

FILLET TOOLS Expanding the fillet tools icon reveals the following tools.

CIRCULAR A circular fillet creates an arc tangent to two entities (lines, circles, other arcs, etc.) that has a circular profile. The result is the removal of the corner (or projected corner if the two entities are currently not intersecting) and the creation of the arc.

To create, use the left mouse button to select the two entities at the location where you want the fillet. The fillet will be created automatically using a best-fit method. The figure below shows a sample circular fillet.

CONICAL The conical fillet is created the same way you create a circular fillet. The only difference is that the resulting fillet does not assume a circular profile, and therefore does not have to do a best fit. The following figure shows a sample conical fillet.

SPLINE TOOL The spline tool is used to create a continuous, tangent entity that passes through specified points. To create a spline, pick on the following icon.

Then, use the left mouse button to select points in a row. As the points are selected, the spline will update to remain tangent and continuous (no sharp corners). Once you are done selecting points, use the middle mouse button to complete the spline.

The following figure shows a sample spline.

SPECIAL ENTITY TOOLS Clicking on the icon will reveal two special sketcher tools, as shown below.

POINT A sketcher point is used in various ways. One simple way it is used is to create a snap point to tie multiple entities together. For example, you might use a point to force an arc to lie on a line segment. Sketcher points are also used to create Datum points if you use the “Sketched Datum Point” feature. Another use for sketcher points would be to create blend vertices. This is, for example, when you blend a square into a triangle, you have four endpoints in one entity but only three in the other. The blend vertex forces two entities in the square to connect up to a single vertex in the triangle. The following figure shows a point used to tie two entities together, and a point all by itself.

COORDINATE SYSTEM A sketched coordinate system is used for some specialized features, such as torroidal bends, helical sweeps, general blends, etc. To sketch a coordinate system, pick the location where you want the coordinate system. The coordinate system always has the X-Y arrows in the sketch, and Z points outwards. The following figure shows a sketched coordinate system.

USE EDGE / OFFSET EDGE TOOLS When we are sketching a new feature in a model that already has geometry, we have the ability to use existing edges in the model as a basis for the sketch entities. Clicking on the Use Edge / Offset Edge icon shows us the two tools.

USE EDGE To create a sketched entity by exactly placing it on top of existing edges in the model, use this tool. Click with the left mouse button on the model edges you wish to use. The complete edge will be copied into the sketch, and a backwards “S” symbol appears on the edge, indicating that it is a use edge. The following figure illustrates this. NOTE: The existing model edges are blue in this figure, and the sketched entities are black.

OFFSET EDGE To create a sketched entity by offsetting existing edges in the model, use this tool. When you click on the Offset Edge icon, you get the following menu choices (which you also got for the Use Edge command as well).

If you use Single you will pick on an edge, then specify the offset distance for that single edge. To get all of the edges around a surface, select Loop, then specify the overall offset distance for all edges. To select a chain of edges, pick on Chain, then pick the first edge in the chain, followed by the last edge in the chain, as shown in the figure at the top of the next page.

A new menu will appear giving you the choice to accept the highlight as it currently shows, or to toggle through other possible edge chains based on the two segments you selected. The menu looks like the following.

Once you accept the chain, a red arrow will appear on the sketch, and the message window will prompt you to enter an offset value. The direction of the arrow indicates a positive offset. The following figure shows this arrow.

If we were to enter a positive value for the offset distance, then our sketch entities would appear outside of the existing model. If we enter a negative value, then our entities offset towards the inside of the model. The following figure shows a negative offset value entered. Again, note the backwards “S” symbol indicating that these edges are offset.

DIMENSION TOOL As you sketch, dimensions should appear on the model automatically. These dimensions initially appear gray and muted. This is known as a weak dimension. Weak dimensions are added to ensure that the sketch is always fully defined (no over- or under-dimensioning). The following figure shows an example of weak dimensions applied to a sketch before any dimensions were manually applied.

Let’s take a minute to break down what we see above. We can see the existing model geometry (in blue), and the sketched entities (the lines that form a sort of “L” shape). We can see some constraints that are already on the sketch (the “H” and “V” symbols). In addition, we can see two dashed lines. These lines are sketch references. We will talk about these later in this lesson. There are two sets of dimensions that you will have when you sketch to create a feature in an existing model. These are: • Locating Dimensions – Dimensions that locate the sketch with respect to existing geometry. Often, these dimensions go between the sketch references and the sketched geometry. Shape/Size Dimensions – Dimensions that control the shape and size of • the sketch that we made. You may not always have locating dimensions if you constrain the sketch to existing references or geometry (such as using a Use Edge or Offset Edge tool). Initially, all of these dimensions are weak. You want to make sure that you never leave weak dimensions in your sketch, because they are not stable, and could disappear. We will demonstrate this as we start to add dimensions.

NORMAL DIMENSIONS To create normal dimensions, click on the following icon in the sketcher toolbar.

Click on the entities to dimension using the left mouse button, then place the dimension using the middle mouse button. Now, we will demonstrate the different types of dimensioning schemes. Linear Dimensions Linear dimensions measure the distance between two entities in a single distance, or the length of a line segment. The following figures illustrate linear dimensions.

results in…

The strong dimension shows up in a creamy yellow on the sketch (shown in black in this training guide). Notice how one of our weak dimensions disappeared? The weak 2.046 dimension in the first figure went away once we added our strong dimension, because it maintained a fully-defined sketch. We could have just as easily lost the 4.092 dimension instead of the one we did lose. The fact that weak dimensions can arbitrarily disappear when we add strong dimensions is the primary reason we want to make sure all the dimensions are strong.

We don’t have to redo create a dimension if we already have a weak dimension where we need one. To make the weak dimension strong, we can either modify the dimension, or force it to be strong. To force a weak dimension to be strong, first select the dimension so it highlights in red, then click with the right mouse button to see a list of options. Select the Strong option to make this dimension strong, as shown below.

Once we do this, the dimension should turn creamy yellow (black in our case), as we can see in the following figure.

To create a dimension for the length of a line, click once on that line with the left mouse button, the place the dimension using the middle mouse button. The following figure illustrates this.

You can also create linear dimensions by picking on two arc/circle centers or two vertices. The following figure illustrates a linear dimension between two vertices.

Angular Dimensions To create an angle dimension between two entities, click on the two entities with the left mouse button, the place the dimension in the correct location with the right mouse button. The location determines what type of angle you are going to get. Consider the sketch below.

There are four possible places to specify and angle on this sketch. The following figure shows the different scenarios for specifying the location to get the different angles.

In the figure above, you select both line segments with the left mouse button, and if you click with the middle mouse button in the shaded area, you get the resulting angle dimension shown to the right of that figure.

Radius/Diameter Dimensions To create a radius dimension on an arc or circle, click once on the arc or circle with the left mouse button, and then place the dimension with the middle mouse button. To create a diameter dimension on an arc or circle, click twice on the arc or circle with the left mouse button, and then place the dimension with the middle mouse button. The following figure illustrates this.

REFERENCE DIMENSIONS If you need to call out more dimensions than are necessary for the sketch to be fully defined, you should use reference dimensions. Reference dimensions, unlike normal dimensions, can not be modified directly. They are what are called driven dimensions. Changing normal dimensions will cause the reference dimension to update. A reference dimension is created exactly the same as normal dimensions (from a standpoint of picking with the left mouse button and placing with the middle mouse button), but to access reference dimensions, go to Sketch, Dimension, Reference from the menu bar at the top. Then, pick your references. The following figure shows a reference dimension.

Notice how reference dimensions have parenthesis “( )” around them? ORDINATE DIMENSIONS Typically, you use ordinate dimensioning to reduce the screen clutter on a drawing. These are very useful for objects with hole patterns, or many, complex shapes. To start an ordinate dimension, we need to create Baseline dimensions. A Baseline dimension marks the “Zero” location from which all ordinate dimensions are measured from. There are typically two baseline dimensions in an “X-Y” coordinate system, one that determines the horizontal zero and the other that determines the vertical zero. The following figures show the difference between linear and ordinate dimensioning (maintaining the same design intent).

Linear Dimensioning Scheme

Ordinate Dimensioning Scheme Notice how much cleaner the ordinate dimensioning looks? You can also create a combination of the two. The following figure shows this for the same sketch, preserving design intent.

Would you want to do this? You’ll notice that in the figure above, ordinate dimensioning is used for the hole locations, but the rest of the model uses linear dimensions. Perhaps on your drawing, you may have a separate view detailing the hole pattern, and may wish to use ordinate dimensions for that view, but for the other view that calls out the overall dimensions of the part, you may wish to maintain the linear dimensioning scheme.

My recommendation is to reduce the number of views in the drawing that it takes to CLEARLY call out your design intent, and using ordinate dimensioning across the board may accomplish this where linear dimensions may be too messy. To create ordinate dimensions, go to Sketch, Dimension, Baseline, and then click on the entity with the left mouse button that represents one of the “Zero” locations. Place the “0.000” dimension along the entities’ direction, as shown in the figure below.

The baseline dimensioning tool remains active, so you can simply pick the next line and place the dimension, as shown below.

Once you have your baseline dimensions created, you can create the ordinate dimensions. To do this, click on the dimension icon in the sketcher toolbar (just like we do to create normal dimensions), then click in this order. 1. Pick on the baseline dimension, with the left mouse button, that runs in the same direction as the ordinate dimension you wish to create. 2. Pick on the entity to dimension with the left mouse button. 3. Use the middle mouse button to place the dimension. The following figure illustrates this.

Repeat this process to create the other ordinate dimension; (pick the other baseline to start, followed by the top edge, and then place the dimension).

MODIFY TOOL The easiest way to modify a dimension in the sketch is to double-click on that dimension with the left mouse button and type in a new value. Once you hit the Enter key (after modifying the value), your sketch should automatically regenerate to reflect this change. The following figure shows what the screen would look like once you double-click on the dimension.

Once you modify a dimension, it becomes strong (if it was previously weak).

MODIFY TOOL ICON If you have a complex sketch, sometimes modifying dimensions using the doubleclick method causes the sketch to distort. Sometimes, you can not modify a dimension value if the starting value and ending value are so drastically different that the sketch can not successfully regenerate. In these cases, you will want to use the modify tool by picking on the following icon in the sketcher toolbar.

Before using this tool, you have two choices. You can either select the icon, then select on the dimensions to modify, or use the select tool and the Ctrl key on your keyboard to select all of the dimensions ahead of time and then click on the icon. We will do the latter for this example. We will modify all of the dimensions in the figure below.

To do this, use the select tool ( ), and then drag a box around the entire sketch. When you release the left mouse button, all entities and dimensions will highlight in red. At this time, click on the modify tool icon. A window will appear. I have moved this window next to the sketch so you can see both simultaneously, as shown below.

You will notice that all dimensions that are highlighted are listed in this window. One of them is currently selected (indicated by the blue shading in the field). On the sketch itself, the selected dimension will have a box around it (currently the total height dimension). The components of this window are shown in the following figure.

You can change the dimensions by typing a new value in the field provided, or by moving the sliders to the right of the dimension to dynamically update them. We want to pay close attention to the two options in the lower left, which are: Regenerate – By default this is selected (green check mark). Turn this off to • prevent the sketch from automatically regenerating as you modify the dimension values. This will let you modify all of the dimensions and then regenerate the sketch all at once. Lock Scale – To use, turn this on BEFORE modifying any dimension • values. Once activated, the first dimension you modify will drive all other dimensions to update so the sketch maintains its current aspect ratio. For example, suppose you have a rectangle that is 2 inches long and 1 inch wide. The length to width ratio is 2:1. If we really want the length to be 200 inches long, to maintain the same aspect ratio, the width would have to be 100. If we were to click on Lock Scale, then modify the length dimension to 200, the width would automatically update to 100. This is very useful if you need to make a drastic dimension change and you don’t want your entire sketch to distort or warp on you.

CONSTRAIN TOOL As we sketch in Pro/ENGINEER, we will notice some constraints that appear automatically. Pro/ENGINEER’s sketcher tool is smart enough to make some assumptions (which may not be what you ultimately want sometimes). For example, if you sketch a line approximately in the horizontal direction, sketcher will assume you want a horizontal line and snap it to that automatically. An “H” symbol will appear on the line when this occurs. If you don’t want a horizontal line,

then exaggerate your line so it is more of a 30 degree angle (for example) with the horizontal. You can disable an automatic constraint by simply selecting on it after you sketch so it highlights, and press the Delete key on your keyboard. For example, if you sketched a horizontal line, and really wanted it to be angled, you would click on the “H” symbol so it highlights in red, then delete it. To add additional constraints to your sketch that might not have been “assumed” click on the following icon.

This will bring up the following window.

The different tools are: Vertical Line / Line up Vertically – Make any line segment a vertical line or • take two vertices and line them up on an invisible vertical line. Horizontal Line / Line up Horizontally – Make any line segment a • horizontal line, or take two vertices and line them up on an invisible horizontal line. Perpendicular – Take two entities and make them perpendicular to each • other. Tangent – Take two entities and make them tangent to each other (usually • an arc to a line, an arc to an arc, or a circle to a line or arc). Midpoint – Force a point, coordinate system or entity endpoint and make it • at the midpoint of another entity. Collinear / Aligned – Make two line segments line up with each other, or • place the endpoint of an entity and snap it to another entity (anywhere on that entity). Symmetric – Make two vertices lie equidistant from a sketched centerline to • create a “mirror” effect. Equal Length / Radii – Make two line segments equal in length, or make • two circles or arcs or combination of both equal in radii. Parallel – Make two line segments parallel to each other. •

To demonstrate this, look at the following initial sketch.

The display of dimensions has been turned off so we can more clearly see the constraints that are on the entities. As we can see, there are a few horizontal and vertical constraints added automatically as we sketched this profile. Now, suppose we want the bottom line to be horizontal, the three top horizontal lines to be equal in length, and finally the top left and top right horizontal lines to line up with each other. First, we’ll address the equal length lines. Start by clicking on the constraint icon that represents Equal Length / Radii. Then, select the two lines shown in the following figure.

The lines should snap to be the same length, and an L# symbol appears next to each line. The # in this case represents a number that is sequential every time this constraint is uniquely applied. Since this is the first equal length condition, # = 1, as shown in the following figure.

Now, we are going to make the third horizontal line equal to the first two. By selecting the Equal Length / Radii tool (which should still be selected from the previous time), and picking on one of the existing “L1” lines, we will force the third to be the same condition. The following figure shows what we are selecting.

When we do this, we get the following result.

You can see that the third line also has a L1 applied to it instead of L2. The reason for this is that all three lines are the same length. If we had picked two lines that had no “equal” condition on it, then we would have seen two “L2” constraints on the sketch.

To make the bottom line a horizontal line, pick on the Horizontal Line / Line up Horizontally constraint, then pick on the edge, as shown below.

Once we do this, an “H” should appear on this line, and it will snap to a horizontal orientation, as shown in the following figure.

Finally, we will use the same constraint tool to line up the left and right top horizontal lines. We will pick on two vertices to do this, as shown below.

The result will be the following.

The little rectangle icons facing each other is the symbol for this constraint. These same rectangles will appear for the Collinear constraint when two lines are selected, but the icon for Aligned looks different. If we turn the view of dimensions back on, we can see that we only have three dimensions left.

Compare that to the original sketch before we started adding constraints.

Because we are not allowed to over-dimension the model, the addition of constraints has forced many of the weak dimensions to disappear.

The following table shows the symbols that will appear for each type of constraint. Constraint Type

Symbol(s)

Vertical Line / Line up Vertically , Horizontal Line / Line up Horizontally

,

Perpendicular

Tangent

Midpoint

Collinear / Aligned ,

,

Symmetric

Equal Length / Radii

,

Parallel

Within the constraint window, there is a button called Explain. If you click on this button, then on any constraint symbol on the sketch, it will highlight the entities that are affected by that constraint, and in the message window, it will describe the condition that has been set. For example, if you click on an L1 symbol, it will highlight two or more line entities, and the message window will say “Highlighted linear segments have equal lengths.”

TEXT TOOL To create logos, part markings, and other text-type features on the model, you will probably have to sketch text at some point in time. This tool is used for that purpose. To start creating text in your sketch, click on the icon shown below.

Then, sketch a line that represents the start of the text. The first point of the line that you pick represents the lower left corner of the text as it reads from left to right, as shown below.

The second point on the line represents the height and orientation of the text. If you sketch a vertical line straight up (as we see in the figure above), then the text will be readable from left to right. If we sketch the line straight down, the text will be upside down and backwards. If you sketch a slanted line, then the text will be at an angle. Once we sketch the line, we see a window appear that looks like the following.

In the top field, type in the words you want for the text. In the middle section, you can change the font used, the aspect ratio (the width of the word), and the slant angle (to control italics). You can use any True-Type fonts (like you might find in Microsoft Word). See your system administrator if you need a font added to the list. The following figure shows text using CG Times (Times New Roman equivalent).

You can also get your text to follow a sketched curve (spline, arc, etc.) Suppose we want to have the text follow a three-point arc. We sketch the arc, then click on the text tool. The start point of our text will be at the left end of the arc, and we will sketch a line perpendicular to the arc (look for the perpendicular constraint symbol to appear as we sketch). Once we sketch the line, our text window appears, and we enter the text, but we notice the text is still perpendicular to the line that we sketched, as shown in the figure at the top of the next page.

In the text window, click on the Place Along Curve option, then select the arc. The text will automatically wrap around this arc. Use the Aspect Ratio slider to get the text to fit on the line. The result is shown below.

Once you finish, click on the green check mark to complete the text, then adjust the height of the text by modifying the dimension, or dragging the top end of the line that starts the text. To modify the text (get back to the text window), click on the modify tool icon, then pick on one of the letters.

TRIM TOOLS If you click on the trim tool icon, you see the following trim options.

DYNAMIC TRIM The dynamic trim tool is used to eliminate portions of the sketch you do not want to keep by clicking on the items or drawing a path through the items. Take the following sketch for an example.

Suppose we only want to keep the portion in the middle where all of the lines intersect. We would select the dynamic trim icon, then either pick on all of the outside portions of the lines one-by-one, or draw a path that goes through the outside sections at once, as shown below.

Once we are finished dragging the path around the part, let go of the mouse. The result will be as follows.

CORNER TRIM The corner trim tool is both a trim for intersecting entities, or an extend for nonintersecting entities. For this tool, you want to select on the part of the entity that is going to remain after the trim. For example, look at the following sketch.

We want to connect up the two line segments (extend), and then trim away the small portion of the line that lies past the arc intersection. Therefore we would use the corner trim tool and select in the areas indicated in the following figure.

The resulting sketch after this trim will look like the following.

DIVIDE TOOL The divide tool is used to break up a single sketched entity into multiple entities. You might use this when sketching for a blend feature, because the number of entities has to be equal. Therefore, if you were blending a circle to a square, the circle would have to be divided into four sections. The following figure shows where you might pick on a line to divide it, and then its resulting sketch after the divide.

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TRANSFORM TOOLS Selecting on the transform tools icon gives you the following choices.

MIRROR This tool is used to mirror selected entities about a sketched centerline. You always want to take advantage of symmetry in your models, and this is a great way to save time in sketch mode. To use the mirror tool, select all of the entities you wish to mirror, click on the mirror tool icon, and then click on the centerline that acts as the mirroring plane. The following sketch is an example of how the mirror tool works.

results in…

SCALE AND ROTATE This tool is used to resize, move and/or rotate an existing set of entities in the sketch. To use, select all of the entities you wish to affect, then click on the scale and rotate tool icon. Enter the appropriate scaling factor and/or angle, or dynamically drag these values on the screen. To demonstrate this, look at the following sketch.

Using the select tool, we will drag a box around the entire sketch, and then click on the Scale and Rotate icon. The dimensions disappear from the sketch temporarily, and three symbols appear, as shown in the figure at the top of the next page.

Using the left mouse button, we can select once on any of these items then move the mouse cursor to see it dynamically change. Once we are done, click again with the left mouse button to place the entity at its new location/orientation/size. At the same time we see these symbols, a window pops up in the upper right corner. It looks like the following.

We can type in a value for the scale factor or rotation angle. In this example, we will enter a Scale of 1.5, and a Rotate value of 45 degrees. Once we are done, we will click on the green check mark. Our sketch now looks like the following.

We can see that the dimensions are now 1.5 times larger, and the rectangle has been rotated 45 degrees. Since we don’t have any other entities in our sketch, a weak dimension had to be added to account for the rotation, and we can see this in the figure above.

COPY The last transformation tool is the copy tool. To use this, select the entities you wish to copy, and then click on the copy icon. It performs a “Copy and Paste” operation right in the sketch, and the new copy will appear in the upper left corner of the sketch with the same symbols we saw in the Scale and Rotate tool. Use the same techniques to move, scale or rotate the copied entities. To demonstrate this, look at the following initial sketch.

We want to make a copy of the inside closed set of entities. Therefore, we use the select tool, and we drag a box around these entities to select them. Once they are selected, we click on the Copy tool, and we can see a copy of these entities appear in the upper left corner, as shown in the following figure.

Using the dynamic move and rotate symbols, I will locate the copied entities the way I need them, as shown below.

Once they look the way I want them, I click on the green check mark in the pop-up window, and my sketch looks like the following.

ACCEPT / CANCEL When we are finally done with our sketch, we will click on the accept icon, which looks like the following.

If we were in a sketch that was part of a feature creation method, such as an Extrude feature, then we would be placed in the next sequence of events for creating that feature. If we are in a stand-alone sketch and click on this icon, we are placed back

out into the Pro/ENGINEER interface, ready to open a new file or activate an already open file. To cancel out of a sketch, click on the following icon.

You will be asked to confirm the cancel of the sketch. If you accidentally cancel the sketch, it should still be in session memory, and you can simply open it again.

SKETCH MENU So far, we have spent a great deal of time going over the sketcher toolbar. Many of these same functions are available in the Sketch menu, located in the menu bar. The sketch menu has a few functions, however, that are not icons. This section will talk about some of these. CENTERLINE TANGENT This tool creates a centerline tangent to two entities. Use Sketch, Line, Centerline Tangent from the menu bar to access this tool. Use the left mouse button to select the two entities that the centerline will be tangent to. The centerline will still span the entire sketch window. The following figure shows a sample centerline tangent entity.

AXIS POINT An axis point is a sketched point that, when extruded, generates a datum axis on the model. We will learn more about datum axes later, but the following figure illustrates this. Use Sketch, Axis Point from the menu bar to create this entity. NOTE: This only is available if you are currently sketching as part of an extrude feature, it does not work in stand-alone sketch mode.

AXIS OF REVOLUTION When you create a sketch for a revolved feature, you must create a centerline that acts as the axis of revolution. By default, the first centerline that you sketch becomes the axis of revolution. If, by mistake, you realize that you didn’t sketch an axis of revolution, and you already have several centerlines on your sketch, you can use this feature to specify a different axis of revolution. Click on the centerline that you wish to use, and then select Sketch, Feature Tools, Axis of Revolution from the menu bar to create this entity. The following figure illustrates this. NOTE: This also will not work if you are in a stand-alone sketch, it only works if you are in the sketch to create a revolved feature.

TOGGLE SECTION When you create a parallel blend feature, you must sketch at least two different sections. Every section that you create is done in a single sketch. To tell Pro/ENGINEER which sketched entities belong to one sketch and which belong to another, we toggle between sketches. To toggle between sections, go to Sketch, Feature Tools, Toggle Section from the menu bar. Again, this will only work if you are trying to create a blended feature, not in stand-alone sketch mode. The current sketch is in the color of the sketched entities (yellow in Wildfire 2.0), while the inactive sketch becomes a muted gray color (similar to the weak dimensions). Suppose we want to blend between a circle and a rectangle. We might start by sketching the circle, then use Sketch, Feature Tools, Toggle Section. The circle becomes a muted gray color, and then we sketch the rectangle, which is still in the primary sketch color (in this guide that will be black). The following figure demonstrates this.

Using the Toggle Section command again will cause the circle to become the active sketch, and the rectangle will become the inactive sketch. We will see more of this when we get to the blend feature. START POINT In several features in Pro/ENGINEER, we must define a vertex that acts as the starting point of our sketch. We can see this in the figure above for Toggle Section. The bold arrow pointing towards the right from the upper left vertex is the symbol for a start point. To change the start point, we select a different vertex on the sketch, and then use Sketch, Feature Tools, Start Point. The arrow will switch to that new vertex. BLEND VERTEX A blend vertex is used in the blend feature sketch to force multiple entity sections to converge into fewer entity sections. For example, blending a square into a triangle forces two corners of the square to converge into one corner of the triangle. To specify which corner of the triangle will accept the two corners of the square, we select that vertex, and then use Sketch, Feature Tools, Blend Vertex. The blend vertex is represented by a larger circle around the vertex selected. The following figure shows the blend vertex and the start points for this example.

DATA FROM FILE To re-use saved sketches, or to import neutral data into your sketch (such as IGES, DXF, Adobe Illustrator, Images, etc.) use Sketch, Data From File. This will bring up the following window.

Each data type that we bring in prompts us for different options, so we will only talk about inserting saved Pro/ENGINEER sections (.sec files). When you select the file you wish to bring in, it will look and behave exactly the same as the Scale and Rotate or Copy tools under the Transform icon. Scale, move and/or rotate the sketch that you are bringing in, and then click on the green check mark in the pop-up window to place the sketched entities. Continue to add/remove from this sketch as necessary, and then accept it once you are done. This is the way you will bring in the logo sections, part markings, recycle symbols, etc. OPTIONS The last item in the Sketch menu is the sketcher options or preferences. When you select this option, you will get the following window.

There are three tabs: Display, Constraints, and Parameters. On the display tab, we can toggle on/off the display of sketched entities. We can see that we currently do not have dimensions or constraints shown in our sketch. The second tab, entitled Constraints, looks like the following.

In this section, you can disable automatic constraints while sketching. Right now, sketcher can assume any one of the above conditions if it looks like that is your intention. I would recommend exaggerating your sketch instead of turning off automatic constraints. The third tab is the Parameters tab, which looks like the following.

At the top of this section, we can define the grid type, origin and angle. The default grid type is Cartesian, which creates an X-Y sketching grid. The other option is Polar, which can be used to help you sketch entities which predominantly lie around an axis normal to the screen.

In the second section, we can define the grid spacing. This only helps you if you turn on the display of the grid, and set the sketch to snap to grid. These settings are on the first tab. In the third section, we can define the number of decimal places for our sketcher dimensions, and the relative accuracy of the sketch. This is useful if you are sketching very small entities in the same sketch where you have much larger entities. The smaller entities might appear to Pro/ENGINEER as having zero length. Increasing or decreasing this number may help fix sketch regeneration errors.

EDIT MENU The Edit menu in the menu bar has some of the sketcher options, such as Modify and Trim. There is one additional item that is very important to discuss here. That is Replace. REPLACE If you are creating a model, and you sketch a feature, such as an Extrude. When you created the sketch, the single line entity in the sketch extrudes to form a surface that has an edge that lies on the sketching plane, and an edge that is projected to the depth location. Both edges of this surface rely on the single sketched entity. If we add a round to one of the edges of this extruded feature, then that round now relies on that sketched entity (by way of the extrude feature). If we were to go into the sketch again after we created the round, and deleted the entity that eventually made up the edge, then the round would fail. We can use the replace command to sketch a new entity and make the downstream features use it instead of the original one. To do this, you would sketch a new entity. Once the entity has been sketched, you would select it so it becomes highlighted in red. Then you would use Edit, Replace. You will then pick the old entity that the new one replaces. You will probably be prompted to delete dimensions that were applied to the old entity. Re-dimension the new entity as needed, then finish out of the sketch. The features downstream should regenerate successfully. The following figure shows the original sketch, extrude feature, and round for this example.

Now, suppose we want to make the following change.

When we go back into the original sketch, if we simply pick on the edge and hit the Delete key, we get the following warning in the message window.

This is letting us know that if we delete this entity, other features downstream will fail. We will click on No to the right of the message window to cancel the deletion of this entity. Therefore, we will sketch the new arc that will soon replace the edge, as shown below.

The old edge is still in the sketch, because we can’t delete it just yet. Once we have the new arc sketched, we will click on it to highlight it in red, then go to Edit, Replace. We are prompted in the message window to select the old entity to replace. We will pick on the vertical edge. When we do, we get the following window.

You may or may not get this window, depending on how your sketch is dimensioned. If you are prompted with this window, do not worry. Click on Yes to delete any necessary dimensions, and then re-apply the necessary dimensions to the new arc.

Once you are done, you r final sketch, extrude and round feature will look like the figure at the top of the next page.

We can clearly see that the Extrude and Round features are able to use this new arc. If we had deleted the edge and sketched the arc in its place, the round would certainly have failed. The extrude would not have failed, because it will successfully use any regenerated, closed sketch, and because the sketch was for this feature.

RIGHT MOUSE BUTTON You will also find that most of the common functionality in Sketcher can be carried out using the right mouse button. Lines, arcs, circles, rectangles, as well as dimension and modify are a few of the items that show up on the screen when you click on the right mouse button. If you have an entity selected, you may get additional menu items. Feel free to use the right mouse button for easy and fast switching between common tools and functions.

LESSON SUMMARY Many of the features in Pro/ENGINEER require a sketch of some sort. This lesson went into great detail to cover most aspects of sketching and sketch mode. Remember to always sketch in the following order: Select References • Sketch Quickly but Accurately • • Constrain Entities Dimension • Modify Dimensions • Accept Sketch • Make use of symmetry whenever possible and mirror your sketch to save time. You can use the menus at the top, the icons in the sketcher toolbar or the right mouse button to access common sketcher commands and tools.

EXERCISES

Create the sketches shown on the following pages as stand-alone sketches. Be sure to follow the proper sketcher steps (with the exception of the “Select References” for these exercises. Save each sketch once you are complete before Accepting them.

Sketch 1 – Shear_Plate.sec

Sketch 2 – Latch_Plate.sec

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5 Lesson Objective: In this lesson, we will learn about the Sketch Feature. We will also learn how to start a new part.

USAGE The Sketch feature is used to create a curve on a 2D plane or planar surface. This curve can then be used to create a variety of different features.

STARTING A NEW PART Up to now, we have not created a part file yet. We will now create one before we can create our sketch feature. To start a new part, click on File, New, or click on the following icon.

In the New window, make sure Part is selected in the first column, and Solid is selected in the sub-type column. Enter a name for the part in the field at the bottom. The window looks like the following.

Click on OK to complete this window. A new window appears as shown below.

In the upper portion, we want to make sure the appropriate start part is selected in blue. In this example, we will show the Startpart_English start part. You can enter parameter values in the spaces provided at the bottom and then click on OK to continue. The part will open in your working window. By default, datum planes should be visible, so the model looks like the following.

The model tree will appear in the Navigator, showing all of the existing geometry.

We can see that there are three datum planes, one datum coordinate system, and three datum axes in every part created from the start part. This is intentional. We will learn more about datum features in upcoming lessons. Depending on the organization, you may have different start parts with different start part geometry.

CREATING A SKETCH FEATURE On the Feature Toolbar, you will find a fly-out icon that represents datum features. Fully expanded, it will look like the following.

As indicated in the above figure, the Sketch feature is the icon that appears as a blue squiggly line on a dotted grid. When you pick on this feature, you are prompted to pick your sketching plane. The next section will describe the dialog box for selecting sketching planes.

SELECTING SKETCHING PLANES For any feature where a sketch is required, you are prompted to select a sketching plane. In the Sketch feature, when prompted to pick a sketching plane, we will see the following dialog box.

In Wildfire 2.0, dialog boxes that contain more than one field will indicate the active field by filling it yellow. In the figure above, the field used to select the sketching plane is currently filled in yellow. A field that is white (Reference in this case) is an available field to select but is not the currently active field. To activate a “Non-Active” field, simply click once in the field with the left mouse button. Any field that is grayed out is currently “In-Active” until enough references are picked to make that filed active. Therefore, we would start by picking on the sketching plane. In this example, we use the TOP datum plane.

Once we select this, we may see another datum plane or planar surface on the model get selected automatically as the horizontal/vertical reference, and its orientation will be selected as well. This is a good thing from a time saving standpoint, but you will want to be aware which entity is selected, and how it is facing. NOTE: There are times when it won’t automatically assume an H/V reference. In this example, when we pick on the TOP datum plane, it automatically assumes we want to face the RIGHT datum plane towards the Right. Our window shows this in the next figure.

To change the reference entity, you can simply pick a new one on the model, because it is currently the active field. Be sure to note the orientation, as you may need to change it for the new reference. For example, if we wanted to face the FRONT datum plane towards the Bottom, we would need to first select the plane, and then change the orientation to “Bottom” in this window. In Wildfire 2.0, the arrow is always the viewing direction in this dialog box. To change this, click on the Flip button. On the model, we can see which entities have been selected based on the color. The sketching plane will always highlight in an orange color. The horizontal / vertical reference will always highlight in red, and the direction arrow will always be yellow. The following figure shows this.

As mentioned before, the sketch feature looks like a datum curve, but is a slightly lighter shade of blue to make it stand apart. The following figure shows the difference between a sketch feature and a datum curve (through points – which are currently not shown).

Printed out in black and white, you may not see the subtle difference, but it is there.

LESSON SUMMARY A Sketch Feature creates a 2D curve. It can be selected directly to create certain solid features. We will see this in the next lesson.

EXERCISES Create a brand new part called Plate_Layout. On the TOP datum plane, create the following sketch feature.

When finished, your sketch feature should look like the following from a TOP orientation.

Save and close this part. We will come back to it in the next lesson.

Les son

6 Lesson Objective: In this lesson, we will learn about the extrude feature, and the different depth options available.

EXTRUDE DEFINITION An Extrude is created by taking a sketch and pulling that sketch in a straight direction to a specified depth. The following figure illustrates this concept.

Within the extrude feature, you can create solid protrusions, thin protrusions, solid cuts, thin cuts or surfaces, and can switch back and forth between these. The following figure shows these different types of entities.

We will see these entity types in many of the common features in Pro/ENGINEER. There are two different ways to approach an extrude feature. The first approach assumes you have no sketch features in your model that you will use as the basis for the extrude. The second assumes you are going to use a sketch feature already in your model.

EXTRUDE STEPS The steps to create an extrude feature are as follows: 1.

Use Insert, Extrude from the Menu Bar, or select on the Feature Toolbar.

2.

Select one of the feature types: Solid (

3. 4. 5. 6. 7.

), Surface (

icon in the

), Cut (

),

and/or Thin ( ). If no sketch feature was selected, hold down the Right Mouse Button, and select Define Internal Sketch. Select a sketching plane, horizontal/vertical reference and orientation in the Sketch dialog box. Sketch the profile to be extruded, followed by the blue check mark in sketcher mode. Select depth option and enter depth value (if blind). Accept the feature.

If you are starting off with an existing sketch feature as the basis for the extrude feature, the steps are as follows:

1.

Select the Sketch Feature (either in the working window, or in the model tree).

2.

Use Insert, Extrude from the Menu Bar, or select on the Feature Toolbar.

3.

Select one of the feature types: Solid (

4. 5.

and/or Thin ( ). Select the depth option and enter depth value (if blind). Accept the feature.

), Surface (

icon in the

), Cut (

),

EXAMPLE 1 – Internal Sketch In this example, we will assume that we do not have a sketch feature to pick on to create the extrude feature. To begin, create a new part called Safety_Key. We will use the Startpart_English as the template for this part since our dimensions will be in inches. We will start off with a protrusion (Solid Extrude) feature. Therefore, click on the extrude icon ( ), or use Insert, Extrude from the Menu Bar. Down in the lower left corner of our interface, the dashboard for the Extrude feature will open up. It looks like the following figure.

Along the bottom row of this dashboard are the different feature types, depth and direction options. Along the top of this dashboard are feature-specific menu options. These menu options are referred to as “Slide-Up Panels”, because they open up into little panels of information when you click on them. By default, the solid option is selected for the Extrude feature. Since this is the first solid feature in the entire model, the Cut option is currently not available. We will leave the default of Solid selected, and now it is time to create the sketch for our first extrude feature. We will therefore hold the Right Mouse Button down over the working window, and select Define Internal Sketch, as shown in the next figure.

This will bring up the Sketch window, as we can see in the next figure.

We will select the TOP datum plane as our sketching plane, and accept the default select of the RIGHT datum plane facing towards the Right. Click on the Sketch button to enter into the sketch. In sketch mode, sketch a horizontal centerline on the existing horizontal reference line. Then, sketch a 1.12” x 2.4” rectangle to the right of the vertical reference line, symmetric about the centerline, as shown below.

When you click on the blue check mark to complete this sketch, go to a default orientation to see the dynamic preview better. If we look at the dynamic preview of our extrude feature we can see the following.

For the extrude feature, you will see a yellow outline of the feature being created. There is a yellow arrow that indicates the direction the feature is going. If you simply click on this arrow, you can flip it to the other direction. There is also a depth dimension (for blind extruded features). At the end of the dimension, there is a white square. This is a drag handle. You can use your left mouse button and drag the depth value dynamically. To change the depth value, you can either enter the value in the depth field in the dashboard, or double-click on the yellow dimension on your model. We will enter the depth of 1.9, as shown in the previous figure. The lower right side of our working window is also associated with the dashboard, and has the following icons.

I recommend always leaving the Dynamic Preview On (Checked). We will talk about the pause feature a little later – but for now, understand that it is associated with “OnThe-Fly” Datum creation. You can use the full preview (eyeglasses) to see what the final model would look like when the feature is done. We are going to click on the Accept Feature icon to complete this first protrusion. Our model looks like the following.

Now, we will create another extrude feature that will remove material from this block. Start by selecting the extrude icon again. This time, however, we want to make sure that we select the Cut icon in the dashboard, as shown below.

NOTE: When you select the Cut option, another icon appears at the end of the dashboard that allows you to specify which side of the sketch the material is being removed from, as we can see in the previous figure. Once we have selected Solid (by default) and Cut, we will use the Right Mouse Button to select Define Internal Sketch. We want to use the same sketching plane that we did before (TOP datum plane). Instead of selecting it again, we will click on the Use Previous button in the Sketch window. This will automatically select the last sketching plane, H/V reference, and orientation that was used for the previous feature. Click on Sketch to get into sketch mode, and sketch the following 1.4” x .5” rectangle.

Once you sketch the rectangle, click on the blue check mark to complete the sketch, and then go to a default view to see the dynamic preview better.

From the previous figure, we can see that our cut is going in the wrong direction. We can also see an additional arrow. One of the yellow arrows indicates the direction the feature is going, while the other one shows up for cuts to represent the side of the sketch from which the material is being removed. In this case, we will click on the arrow to flip the direction of feature creation and then we need to change our depth option. In the Dashboard, we will click on the arrow to see the different depth options, as shown in the next figure.

Currently, we have the Blind depth option selected. We want to use the Through All depth option. NOTE: We could have flipped the direction of feature creation by clicking on the icon to the right of the depth value, as indicated in the figure above. Once you select the Through All depth option, the depth value should gray out, and our dynamic preview will extend beyond the top of the part to indicate that it is going all the way through the model, as shown in the next figure.

The depth dimension and drag handle have also disappeared from the preview, since we can not change the depth value with the “Through All” option. Now, we can click on the green check mark icon to accept this cut feature. The model now looks like the following.

The model tree will only indicate Extrude features with an incremental number. The biggest reason it only says “Extrude #” is the fact that we could change the cut to a protrusion or a surface, etc. at a later time, and therefore, the “Extrude” name is generic enough to allow for this flexibility. Save and close this model – we will return to complete it in the exercise.

EXAMPLE 2 – EXTERNAL SKETCH In this example, we will see how to use a sketch feature to create an extrude feature. To demonstrate this, we will start by opening up the Plate_Layout part that we created in Lesson 5. If you recall – this part consists of a single sketch feature, and it looks like the following from a TOP view with the datum planes turned off.

We will start by selecting the sketch feature (either by picking it in the Working Window, or in the Model Tree). Next, we will pick on the extrude icon. Right away, we will notice a dynamic preview of the feature when we are placed into the extrude feature, as shown below.

We will change the depth value to 2.0 and then click on the green check mark. Our model looks like the following.

IMPORTANT: When you select on a sketch feature, the entire sketch is used. In this case we created a plate with four holes in it. Even if we were to select only portions of this sketch feature (as we learned in Lesson 3), it still uses the entire sketch. Therefore, if we had wanted to have a plate with four cylindrical feet sticking out (or if we had wanted the holes to be blind instead of through all) we would have to make the holes as a separate sketch feature, or we could create regular extrude features with internal sketches and use the “Use Edge” command to pick only the pieces from the sketch that we wanted. When we use a sketch feature to create a solid feature, it becomes hidden in the model tree, as shown in the next figure.

A hidden feature in the model tree has a shaded block around its icon, as shown above. We can unhide this feature and continue to use it for more features if we needed to. The Extrude feature is completely associative with the sketch feature. If we make a change to the sketch, it updates the extrude. There is an option in Extrude mode when we use an external sketch to break that associativity. In the dashboard, we would pick on the Placement slide-up panel, and click on the Unlink button, as shown below.

When you click on the Unlink button, you will get the following prompt.

Click on OK to finish the unlink. In the slide-up panel, we can now see an Edit button that replaces the “Unlink” button, as shown below.

When you click on Edit you are brought into the standard Sketch window to redefine the placement and sketch of this feature. It will automatically take on the sketching plane, H/V reference and orientation of the original sketch feature (in this case the TOP datum plane as the sketching plane, and the RIGHT plane facing towards the Right). If we make a change to the original sketch feature after the Unlink, we will not see the extrude feature update.

DEPTH OPTIONS There are six depth options that are available at different times when creating extruded features. These are: •

Blind – Extrudes a section from the sketching plane by the specified depth value. Specifying a negative depth value flips the depth direction.

•

Symmetric – Extrudes a section on each side of the sketching plane by half of the specified depth value. Negative values are not allowed.

•

Through Next – Extrudes a section to the next surface. Use this option to terminate a feature at the first surface the entire sketch profile reaches. You cannot use datum planes as terminating surfaces.

•

Through All – Extrudes a section to intersect with all surfaces. Use this option to terminate a feature at the last surface it reaches.

•

Through Until – Extrudes a section to intersect with a selected surface or plane. You can use any part surface, datum plane, quilt composed of several surfaces or another component in an assembly.

•

To Selected – surface.

Extrudes a section to a selected point, curve, plane or

The following figure illustrates these depth option.

EXTRUDED SURFACE You go about creating the extrude feature the same way you have so far. When you get into the dashboard, you will select on the Surface option. When you create your sketch, you can have an open section or a closed section. The following figures show the difference between an open section and a closed, and their resulting extruded surface features.

Open Section

Closed Section SLIDE-UP PANELS Within the dashboard, we have some menus. These are called Slide-Up Panels, because, when you pick on the menu, a panel slides up to show the contents of that menu command. In the case of the extrude feature, there are three slide-up panels. These are: Placement, Options and Properties. The Placement slide-up panel is used to define the sketch. We can see this in the figure below.

Instead of clicking on the Define button, we can also right-click out in the working window and select Define Internal Sketch. The Options slide-up panel is used to define additional depth options, and behavior as the depth is applied. We can see this in the following figure.

For a Blind depth, we have the ability to control the depth differently on either side of the sketching plane. For example, we could have the depth go through all in one direction, and up to surface in another.

The other option on this panel – Capped Ends – will be discussed shortly. The third panel, entitled Properties, is used to rename the feature. The current name is shown below.

We can see that this feature will be called EXTRUDE_1. This is the name that appears in the model tree once we create the feature. We can edit it here to give it a meaningful name. The little blue “I” next to the name field brings up an information window in the built-in web browser with information about this feature that we are creating (sort of a summary). It looks like the figure at the top of the next page.

CAPPED ENDS When we create a surface that has a closed section, we can cap off the starting and ending surfaces of the feature. In the case of an extruded surface, this creates a surface on the sketching plane and at the end of the depth that have the profile of the sketch. The following figures show this last surface that we defined with the capped ends in a no hidden and shaded mode.

In shaded mode, the capped surface looks exactly like a solid protrusion, but in nohidden mode, we can clearly see the purple and pink edges of the surface.

THIN OPTION For either a solid or a cut, we can select the Thin option. This adds a thickness to the sketch when extruding. The thickness can be added to one side of the sketch or the other, or it can be added equally to both sides. When we create the thin feature, we use the same methods that we have for the other extruded features. In the dashboard, we will select our main feature type (Solid or Cut), then pick on the Thin option icon. This will bring up another field to enter the thickness, and another arrow icon to define the side of the sketch the thickness will be added to. The following figure shows the dashboard for a thin protrusion.

The dynamic preview shows us the thickness applied to the feature, as shown in the following figure.

Use the arrow icon at the right end of the dashboard to see the different ways it applies the thickness (inside, outside, or equal about sketch). Once you have what you are looking for, accept the feature. It will look like the following.

LESSON SUMMARY An extrude feature takes a sketched profile and adds depth in a single direction. You can create a Solid or Thin Protrusion, a Solid or Thin Cut, or a Surface in a single extrude command. Be sure to check the reference plane and its orientation once you select a sketching plane. You don’t want any surprises in case it decides to pick a surface or orientation you weren’t expecting. Use capped ends to close off the ends of a surface extrude, but only if you sketched a closed section.

EXERCISES Using the extrude feature, create the following parts on the pages that follow. Be sure to use a start part for each separate part, and save your models when you are done. Plate_Layout2.prt

Open up the Plate_Layout2 part. In this exercise, you will do the following: Create two extrude features – one for the rectangular plate, and one for the holes. The rectangular plate is extruded to a depth of 2.0 inches. The holes are only going to be extruded 1 inch into the plate – making them blind holes. Use external sketches already in the model to create this part. The following figure shows the resulting model.

Save and close this model.

Safety Key – Finish this model that we already started in this lesson.

Rod_Support

Les son

7 Lesson Objective: In this lesson, we will learn about Edit, Edit Definition and Edit References.

EDIT The Edit command is only used to make a dimensional value change. For example, if we want to modify a dimension from 1” to 2”, we would use Edit. If we needed to change the location where the dimension is going to, we would have to use Edit Definition or Edit References. To edit the dimensions of a particular feature, select on that feature (either in the model tree or on the model itself), and then hold down the right mouse button, and select Edit, or just double-click on that feature in the working window. The dimensions appear on the part, and you can now double-click on them to change their value. Once the dimension has been modified, it turns green, as shown in the following figure for the hole diameter in our Plate_Layout2.prt model.

To regenerate the model, click on Edit, Regenerate from the Menu Bar, or click on the Regenerate icon (

) in the System Toolbar.

EDIT DEFINITION The Edit Definition command is used to change anything about the feature, such as the depth value or option, dimensional changes, references used, the feature type (solid to surface, for example), etc. To use Edit Definition, first select the feature on the model or in the model tree, hold down the right mouse button, and then select Edit Definition. This brings up the dashboard that we saw at the time we created the feature.

EDIT REFERENCES The Edit References command is used to reroute features to different references, such as the sketching plane, horizontal and vertical references, or any sketcher references. You can not modify dimension values, or change depth options or the sketch itself using this command. To use Edit References, first select the feature on the model or in the model tree, hold down the right mouse button, and then select Edit References. The following menu appears:

Reroute Feat This option is used to re-select references for the existing feature. This is the most commonly used command for Edit References. Replace Ref This option allows us to specifically pick on certain references of the feature to replace with different references. In the message bar, we are prompted whether we want to roll back the model to the time in which the feature was created or not. This is a personal decision. I personally think it is a good idea, because if the change causes a failure, you will not be hit with all of the failure windows. Instead, you can now resume features selectively, and address each failure one-by-one. Once you have made the decision to roll back the model or not, each reference used to create the feature will highlight one-by-one on the working window, and you will be prompted in a menu whether to keep the same reference, or select a new one. The following figure shows this menu.

The default action is to pick a new reference (Alternate). If we wanted to keep the same reference that is shown on the screen, and go onto the next reference, you would select Same Ref. Had we picked Replace Ref, we would see the following menu.

LESSON SUMMARY Use Edit to make dimensional changes only. Use Edit References to change the different references used to define the feature only. Use Edit Definition to change anything about the feature.

EXERCISES Plate_Layout2.prt Open up the Plate_Layout2 part that we changed in Lesson 6. We are going to change the blind holes to be feet that stick out of the bottom of the plate at 0.5”. Use the appropriate Edit command to accomplish this task. The final part should look like the following (from the bottom).

Save and close this part.

Les son

8 Lesson Objective: In this lesson, we will learn about Datum Planes, Datum Axes, Datum Points, and Datum Coordinate Systems.

DATUMS – WHAT ARE THEY? Datum features are widely used in the creation of other features. They are lightweight, don’t affect mass properties, can be hidden when you don’t want to see them, and very powerful in providing necessary ties and references for other features. The most common datum feature types are accessed in the feature toolbar by selecting the very top icon in this toolbar. When we select this icon, we see the following datum feature types.

DATUM PLANES When we create a new part or assembly, we see datum planes already built into the model, as shown for a part file below.

As indicated in the figure above, datum planes have two sides, a positive side and a negative side. The positive side (if you are using the default system colors), is brown. The negative side is black (or actually, a very dark gray – but we’ll consider it black for this training guide). When we are in a default orientation, we can see the positive sides for all three default datum planes. If we rotate the model slightly to see the back side of the FRONT plane, then we can see the negative side, as seen in the figure at the top of the next page. To turn on/off the display of datum planes, click on the toolbar.

icon in the system

The positive side of the datum plane is the one that is used when picking orientation references. For example, if we pick on the TOP plane as a sketching plane, we know we will be looking at the TOP plane in the sketch. If we pick the FRONT plane as a sketcher reference, and pick Bottom as the orientation, then the brown side of the FRONT plane will face towards the bottom of the screen in sketch mode. Datum planes are widely used for sketch planes, sketch reference planes, sketcher references, depth references, cross-section planes, etc. They are probably the most used datum feature in Pro/ENGINEER. To demonstrate the creation method, we will create the following part.

Before we do this, however, we will change a setting that will allow us to see datum planes when we spin the model. Typically, datum planes temporarily turn off until you stop spinning, panning or zooming.

To change this setting, go to View, Display Settings, Model Display. This will bring up the following window.

In the middle of this window is a section entitled “Display While Reorienting”. The only items that are checked by default are Surface Mesh and Orientation Center. We want to check Datums, so datum features become visible when we spin.

Now, we will create this part, and call it Dtm_Planes. We will create the part using a start part so we have our default datum planes, as we can see below.

The first feature that we will create is the semi-circular extruded protrusion that forms the main shape of this part. We will use the RIGHT datum plane as a sketching plane and pick the TOP plane to face towards the Top as the sketching reference. Our sketch will look like the following.

The display of datum planes was turned off in the previous figure to see the sketch easier. Once we are done the sketch, we want to extrude to a depth of 10.000 inches. Our first feature looks like the following.

Be sure your RIGHT datum plane is at the left side of the model. If not, edit the definition, and change the direction of feature creation by clicking on the yellow arrow in the dynamic preview. Our next feature will be a datum plane that is offset the RIGHT plane by an amount of 4.00 inches. Therefore, we will pick on the datum plane icon in the datum flyout icon. This will bring up the following window.

The first tab, entitled Placement is active. We are asked to pick references to define the plane. The datum plane creation tool is pretty smart. Depending on the type of reference we pick, it will assume the most logical choice for creation. Therefore, if we pick on the RIGHT datum plane, we should see the preview of a plane that is parallel and slightly offset from the RIGHT plane. Drag the white square out towards the right, and you will see it moves the preview of plane, as shown below.

In the Datum Plane window, we see the following.

The RIGHT datum plane is listed in the References field, and to the far right is the type of creation method it assumed, which is Offset in this case. Down in the bottom, we can see the offset value, which shows in this figure as 3.500. We will change the value to 4.000 (either here in this window, or on the model).

The second tab in this window is entitled Display, and if we click on it, the window will look like the following.

You can use this tab to change the positive side of the plane. In this window, it is called the Normal Direction, and there is a Flip button next to it. There is also an option to Adjust Outline, which allows you to resize the datum plane. By default, it assumes the size of the model. I recommend you let it resize itself. The third tab is entitled Properties, and looks like the following.

This tab is used to rename the datum plane, or get information about it. We are going to go ahead and click on OK to finish creating this offset datum plane. Our model should now look like the following.

Now that we have this datum plane, we can create our first extruded cut feature. We will use the new datum plane (DTM1) as the sketching plane, and face the TOP plane towards the top again as the sketcher reference. Our sketch will look like the following.

Extrude this cut to the right of the datum plane a distance of 5.00 inches. The model will now look like the following.

Our next datum plane will be another offset plane, a distance of 3.5 inches up from the TOP plane. Click on the datum plane tool, then select on the TOP plane. It should automatically assume an offset creation type.

Make sure it is going above the TOP plane, and change the distance to 3.5. Our datum plane will look like the following once we create it.

Use this new datum plane (DTM2) as a sketching plane for our next extruded protrusion feature. Pick the RIGHT datum plane to face towards the right. Create the following sketch (with datum planes turned off for easier viewing).

Once we accept this sketch, go back to a default view. The feature is probably trying to extrude up from this plane. If so, click on the yellow arrow to flip the direction so the feature is going down. Then, change your depth option to Through Next ( ). When you accept this feature, your model will look like the following.

Our final feature will be the cut that is angled. We could create this cut by extruding symmetrically about the FRONT datum plane, but then we wouldn’t learn another method for creating datum planes. Therefore, we will create a new datum plane. This time, we are going to use two references to create the plane, an edge to go Through, and a surface to measure an Angle from. Therefore, pick on the datum plane tool. First, pick the TOP datum plane. It will initially assume an offset, as we can see from the datum plane window.

To add additional references, hold down the Ctrl key on the keyboard, and select them. To get an angled plane, we need a reference that acts as an axis of rotation. Therefore, we will also select the following edge (using the Ctrl key).

Once we select the edge, we see the Datum Plane window update to show the new creation type applied.

We can see the “Through” condition, and a rotation angle in the bottom. You will want to look at your model to see how the angle is being measured. Often times, the order you pick the references, as well as the references themselves determine how the angle is measured. Since we picked the TOP datum plane (whose positive side is pointing upwards), and an edge, the angle is measured from the brown side of the datum plane. Therefore, we can enter a value of 20 in the rotation field. The dynamic preview of the plane will look like the following.

We will click on OK from the datum plane menu to finish off the plane. The model will look like the following now.

Now that we have this plane, we can create our cut. Use the top surface of the first cut as the sketching plane, and face the left side surface towards the bottom. The figure below shows the references we are picking.

In our sketch, we want to take advantage of symmetry, and put in a vertical centerline on the vertical sketcher reference. When we sketch our rectangle, we will make sure to look for the little arrow symbols that show it is symmetric about this centerline. Our sketch should look like the following.

Once we are done sketching, go to a default view to see the dynamic preview. We want to make sure the direction is going down, then change our depth option to To Selected ( ), and pick the angled datum plane that we just created. The dynamic preview (in No Hidden model), will look like the following.

It may not look like it is going to angle down, but if we were to click on the Full Preview icon (the eyeglasses) or accept the feature, we would see that it does stop at the datum plane, as shown in the final model image below.

You can also create datum planes using other references. The following describes the most common methods and references for creating datum planes: Through – Create a datum plane to be co-planar with another datum plane • or planar surface. Pick on a Datum Plane or Planar Surface as the only reference. When window shows offset, change the value in the window to “Through”, as shown below. Another set of references would be an edge that lies in a single plane, but has at least two directions to it, such as the edge of a cylinder. Offset – Create a datum plane offset an existing plane or planar surface. • Pick on a plane or planar surface as the only reference. The default type should be “Offset” in the window. Enter the offset value. At Angle – Create a datum plane through an edge or axis and at an angle to • another plane or planar surface. Pick on a plane or planar surface for one reference and an edge or datum axis for the other reference. Enter the angle. Parallel – Create a datum plane parallel to another plane or planar surface • through some selected reference. Pick a plane or planar surface as one reference to determine parallelism, then pick on a datum point, vertex, edge, axis or coordinate system as the second reference to determine the location. Through Points – Create a datum plane through three datum points or • vertices. Pick on three points or vertices or a combination to determine plane.

DATUM POINTS Datum points are most commonly used for creating other datum entities, such as an axis, plane or curve. Datum points can also be used as sketcher references or for assembling two components into an assembly. To turn on/off the display of datum points and their tags (names), click on the following icons in the system toolbar.

The left icon is used for turning on/off the point completely. The icon on the right is only used to turn on/off the point names (tags). We will open the model Dtm_Pac for an example, and we will show all of the most common methods for creating datum points. To create a datum point, click on the datum point icon in the datum flyout icons. We will see the following window.

We can create as many different points as we want in a single datum point feature. This is different from the datum plane tool where we could only create one plane at a time. For each point that you create, you select references. The Properties tab is used to rename the entire datum point feature (not each individual point created). ON SURFACE This is a datum point that lies on a selected surface, and its location is measured from two references. To create this, click on the datum point tool, and then pick anywhere on a surface (planar or otherwise). The following figure shows a sample surface pick to place a point, and the Datum Point window when you select on the surface.

The point shows up on the surface along with three white squares. The square next to the point name (PNT0, in this case), is used to show the location of the point. You can drag this square to locate the point on the surface. The other two white squares are used to tie to references to locate the point. We will start by dragging the right-most square until it comes to the side surface and snaps there. The model and window will look like the following once we let go of the mouse.

We can see the white square has gone away, and is replaced by a filled dot. This dot shows us that we are lying on that surface edge. The window also reflects this by listing the first Offset Refrence in the field at the bottom of the window. We will drag the other white square over to the front surface, as shown below.

This white square should also be replaced by a filled dot, and the other offset dimension and reference shows up in the window. We would now edit the values of these offset dimensions. To create a new point, we would click on the New Point item in the left column of the window. To complete this datum point feature, click on OK. The completed point looks like the figure at the top of the next page.

OFFSET SURFACE This is a datum point that lies offset a surface by a specified amount, and located from two references. The creation method is very similar to an “On Surface” with the addition of an offset distance and direction. The following figure shows a sample surface pick, and the resulting window.

Just like the “On Surface” point, this starts out the exact way. It even assumes the “On Surface” constraint type. To change this, click where you see the word On, and change it to Offset, as shown below.

A third dimension appears on the model, and a field for the Offset has become active in the window. We will drag the locating squares to the same surfaces that we did before, then enter the offset value as 1.5, and change the locating dimension to those shown in the following figure.

When we see the point as we intended, we click on OK to finish the datum point feature, or click on New Point to create additional points. The final point looks like the following.

ON VERTEX This is a datum point that lies on the end of an edge or edge segment. You create this by clicking on the datum point tool, then pick on any vertex in the model. The following figure shows the pick and the window that result.

If we click on OK now, we would have a datum point at this corner vertex. Instead, we will continue with this same window to show the next type. OFFSET VERTEX From the last figure, we had picked a vertex to place the point, and the window indicated a constraint of On, which placed our datum point exactly on the selected vertex. If we change the type from On to Offset, then we must pick another entity that defines the offset direction. We will hold down the Ctrl key and select the edge just below the highlighted vertex, we see the following.

We can enter an offset distance of 1.5, as shown above. The constraint of Parallel applied to this selected edge means that the point will offset from the vertex parallel to the direction of the edge. Now, let’s try a different offset reference. First, right mouse click over the word Parallel and select Remove, as shown below.

Now, we’ll hold down the Ctrl key and select the DEF_CS coordinate system from the model tree. We see the following in the window and on the model.

Next to the Offset field, we can see another pull-down that currently indicates “X”. This is letting us select which axis of the coordinate system is driving our offset direction. We can change this to “Z” as shown in the following figure.

We will now remove this reference the same way we removed the edge. Once it is removed, we will hold down the Ctrl key again, and this time select the top surface. We will see the following.

Now, the reference becomes a surface and the offset direction is normal to the surface. As we have demonstrated, you have the ability to select a wide array of references to determine the offset direction. ON CURVE Another common point creation is to locate the point on a datum curve or existing edge. We will demonstrate this by selecting the top, front edge of the model. Our model and window will look like the following.

When you select a curve or edge as the reference, you get a variety of options to further refine your point definition. The first is to determine whether the distance is a ratio or a real value. The ratio option represents the percentage along the edge or curve where the point resides. For example, if you wanted the point to be at the exact midpoint of the edge, you would enter a ratio of 0.5. Real represents the actual distance along the curve the point resides at. For example, suppose you want the point to be exactly 1.5 inches in from the back left surface. You would change the Ratio option to Real as shown in the following figure.

Then, you would enter a value of 1.5 in the offset field. Once you have determined how the dimension value is being measured, you can pick your reference that the dimension value is coming from. In this window, we can see that the dimension is being measured from the End of Curve. If you want the opposite end to be used, click on the Next End button.

Or, if you want to use a datum plane or other reference other than one of the endpoints, select the Reference option, then select the actual reference on the model. Using the Reference option means that you are using a Real dimension value instead of a ratio. AT CENTER This creates a datum point at the center of a circular edge, such as the edge of a cylinder or a hole. To create, click on the datum point tool, then select on the circular edge. Initially, it will assume an “On Curve” constraint, as shown in the following figure.

As the figure above illustrates, we want to change the On value to Center. This will remove all other options, and place a point at the center of this circular edge, as shown below.

SKETCHED The previous points were created using the datum point icon in the feature toolbar. This is the first of the point definitions that can only be accessed through the menu bar. Go to Insert, Model Datum, Point, Sketched. This will bring up the Sketch window to select a sketching plane and a sketching reference. We will pick the top flat surface as a sketching plane, and then select the front surface to face towards the bottom. Inside our sketch, we will use the sketcher point icon ( ) and pick the location on the surface for the points. Dimension the points in whatever style you need. The figure at the top of the next page shows a sample sketch for these points.

Accept the sketch once you are done, and your datum points will appear on the model, as shown in the next figure.

OFFSET COORDINATE SYSTEM The next type of non-standard datum point creation method allows you to create multiple datum points by offsetting a coordinate system. Use Insert, Model Datum, Point, Offset Coordinate System. This brings up the following window.

The first thing you are asked to pick is the coordinate system you are going to use. We will pick the default coordinate system DEF_CS from the model tree. Then, pick in the first row to start defining points. The window will now look like the following.

You can type in the X, Y, and Z values directly in this window. The following shows how the point moves on the model once you edit the dimension values.

You can also drag the point around the model by placing your mouse over the white square until you see the axis highlight that you are changing. The figure at the top of the next page shows how the “Z” axis becomes visible just before you drag it.

To create another point, click in the next row in the main portion of the window. This will now look like the following.

At the bottom of this window, there are three other options. The first is used to import in a point file (has a PTS extension). The second button allows you to create a point file. If we click on this, we can save a file to our working directory. Opening the file in notepad, it looks like the following.

As you can see, this is a simple file to create and edit. You only need to enter X, Y, and Z values in this file. The third button is used to remove all dimensional information from the point array. You might want to do this if you know you are not going to change these points, and you want to potentially speed up a very large point array.

DATUM AXES Datum axes are used to create other datum features, such as planes, and they are also very useful in assembly mode to align components, set up pin constraints, etc. To show datum axes, click on the following icon in your system toolbar.

To create a datum axis, click on the datum axis icon in the datum flyout toolbar. This brings up the following window.

THROUGH EDGE One way to create datum axes is through an existing straight edge. To create this, pick on the edge as a reference, as shown below.

The datum axes will be created through this edge. NORMAL TO SURFACE If you select just a surface as a reference, you get the following window.

Just as we did with the “On Surface” datum point, drag the white squares to the references you wish to use to locate the point on the surface, and the axis will be created at this point, as shown below.

THROUGH POINTS/VERTICES With this axes creation method, select any two vertices, datum points, or combination of them to create an axis that goes through these points, as shown below.

THROUGH CYLINDER This creates a datum axes through the center axis of a revolved surface, such as a cylinder. By default, most cylindrical surfaces or revolved surfaces will already have an axis, so you may not need to create this type very often. The following window shows the model and Datum Axis window when you pick on the cylindrical surface.

POINT NORMAL TO PLANE With this creation type, select on a datum point, then select a planar surface that the axis will be normal to. This creates an axis normal to the selected plane passing through the datum point. No dimensions are necessary for this one.

INTERSECTION OF TWO SURFACES / PLANES This is an axis that is created where surfaces or planes meet. They must intersect to form a single straight line, otherwise the axis does not lie in a single plane, and therefore can not be created. The following window shows the intersection of the front surface and a datum plane.

DATUM COORDINATE SYSTEMS You may need to create a datum coordinate system for some features. To show coordinate systems, click on the following icon in the system toolbar.

When you click on the datum coordinate system icon in the datum flyout tool, you get the following window.

The most common way to create a datum coordinate system is to pick three surfaces or planes. The following shows a coordinate system window and model when three surfaces are selected.

We can see that all three surfaces are highlighted and each has a constraint of “On” set. We will need to go to the Orientation tab next to define the X, Y, and Z directions. Clicking on this tab, we see the following.

The objective in this tab is to select a surface whose normal represents the coordinate system axis. I have selected the front surface to determine the Z direction, and then selected the side surface (still highlighted) to project the X direction. I had to Flip the X-direction to get the result that you see above. This same method works for selecting datum points and vertices as the original reference. Another method for creating datum coordinate systems is to select an axis as the original reference. When we do this, it places one of the three axes along the axis that we select. We must then select at least one surface that is normal to the axis as a second reference, as shown in the following figure.

On the Orientation tab, we will select a third surface that will define the projected axis direction. Then we can set which one is X, Y, or Z. The following figure shows this tab, and the selected surface.

The last method for creating datum coordinate systems that we will cover is to offset an already existing coordinate system. Therefore we will select the DEF_CS coordinate system as our first reference. The window will look like the following.

We can use the mouse to drag the white square, or enter values for X, Y, and Z offsets in the fields provide. On the second tab, we can specify its orientation by entering rotation angles in the fields, or by selecting references on the model to orient to. I have chosen to rotate the coordinate system about the Y axis (this is the Y axis of the DEF_CS coordinate system). The result is shown below.

LESSON SUMMARY Datum features are very common in Pro/ENGINEER. You will get to know them very well. Use datum planes, axes, points, and coordinate systems to aid in the creation of other features.

EXERCISES Create the following part files using the extrude feature. Create datum planes and/or axes to aid in the creation of the extrude features. Angle_Bearing

Les son

9 Lesson Objective: In this lesson, we will learn about the Revolve Feature.

REVOLVE DEFINITION The Revolve feature is created by revolving a sketched profile around an axis of revolution. The angle and direction can be controlled independent of the sketch.

CREATING A REVOLVE FEATURE The Revolve feature is very similar to the Extrude feature (Lesson 6) from the way that it is created. The biggest differences are in the depth options (fewer for the Revolve feature) and the sketch itself (only a half sketch with a centerline that acts as an axis of revolution). The steps for a revolve feature with an internal sketch are: 1. 2. 3. 4. 5.

6. 7.

Use Insert, Revolve from the Menu Bar, or select on the icon in the Feature Toolbar. Select one of the feature types (Solid, Surface, Cut and/or Thin). Hold down the right mouse button and select Define Internal Sketch. Select the sketching plane, horizontal/vertical reference and orientation in the Sketch window. Sketch the profile to be revolved – making sure you only sketch half of the feature and a centerline that acts as an axis of revolution. Click on the blue check mark to finish the sketch. Select the depth option and enter depth value (if blind). Accept the feature.

When using external sketches, you either need to have a centerline defined in the sketch that will be picked as the axis of revolution, or you need to specify a datum axis or straight edge that lies in the plane of the sketch to act as the axis of revolution. The steps for a revolve feature with an external sketch are: 1. Select the Sketch Feature (either in the working window or in the model tree).

2. 3. 4. 5. 6.

Use Insert, Revolve from the Menu Bar, or select on the icon in the Feature Toolbar. Select one of the feature types (Solid, Surface, Cut and/or Thin). If a centerline was not used in the Sketch Feature, use the Placement slideup panel to define a datum axis or edge as the axis of revolution. Select the depth option and enter depth value (if blind). Accept the feature.

EXAMPLE 1 – Internal Sketch In this example, we will create a revolve feature that uses an internal sketch. To demonstrate this, open up the part entitled Bearing1. It contains a single sketch feature, which we will use later. The following figure shows this part.

We are going to create a new revolve feature by clicking on the revolve icon ( ). Inside the feature, the dashboard for the revolve feature looks like the following.

As you can see, the dashboard for the revolve feature looks very similar to the extrude dashboard. We will keep the default feature type of “Solid” and then we will right mouse click in the working window and select Define Internal Sketch. When the sketch window appears, click on the Use Previous button to sketch on the same plane as the first Sketch feature. Click on Sketch from this window to proceed into sketch mode, and sketch the following profile (don’t forget the vertical centerline sitting on the existing vertical reference).

In the figure above, the sketch is shaped like a “P” with all straight edges and sharp corners, and the top of the “P” is tied to the top edge of the sketch feature. When finished with the sketch, click on the blue check mark. We will now see the preview of the feature.

As with the extrude feature, we can see a drag handle on the angular dimension that we can dynamically drag to see the model update. Under the depth options, we only have the following options: Blind (specify angle), Symmetric, and Up to Selected. We will leave the depth option at 360 degrees. We will click on the green check mark to complete this feature. Our model currently looks like the following.

EXAMPLE 2 – External Sketch In this example, we will finish this bearing by cutting out the middle using the existing sketch feature. To do this, we will first start by selecting the sketch feature from the model tree so it highlights in read on the model. Next, click on the revolve feature icon. In the revolve feature, we do not see a preview yet, because we currently do not have a centerline in the sketch feature to act as an axis of revolution. Until the feature definition is complete, our dynamic preview will not appear, indicating to us that we have not defined enough yet. In our dashboard, we can see a field that is used to select the axis of revolution, as shown in the next figure.

This field is currently highlighted in yellow. This means that we can go ahead and select the datum axis or edge to use. If it were not highlighted in yellow, we could pick once inside this field to make it active. Once the field is active, we can pick on the axis or edge to use. In this case, we have the Z_AXIS datum axis in our model tree that would work. We can also select the inside edge of our sketch feature, since it lies in the plane of the sketch, and it lies at the center of our model. We will select the edge, as shown in the next figure. When we do this, the dynamic preview appears as shown.

There is only one thing we have to do for this feature, and that is to select the Cut icon to remove material from the model. The preview will change to show a cut instead of a protrusion, and then we can click on the green check mark to accept this feature. The model now looks like the following (in hidden line mode).

LESSON SUMMARY The revolve feature is not very different from an extrude feature in terms of the menu picks to create it. The biggest differences lie in the rules for the sketch and the depth options. When sketching, be sure to create or specify an axis of revolution, and sketch on only one side of this axis. You can also use an existing edge or axis in the model for the axis of revolution if you do not wish to sketch one. When specifying depth, remember that it is an angle in degrees.

EXERCISES Create the part below using a combination of extrude and revolve features. Create datum geometry if necessary. Bearing2

Lesso n

1 0 Lesson Objective: In this lesson, we will learn about Datum Curves.

DATUM CURVE USAGE Datum curves are used in a wide range of applications. They can be the trajectory for a sweep, variable section sweep or swept blend. They can also be the boundary edges for blended surfaces. They are often used as tools to create or modify surfaces. We are going to learn about a variety of methods for creating datum curves. We have already learned how to create a sketch feature, which produces a 2D curve on a plane or planar surface. We will now look at the other types of datum features and tools.

PROJECTED DATUM CURVES A projected datum curve is made by projecting a sketch or existing datum curve onto a nearby set of surfaces. You can either project normal to the sketch or normal to the surface. We will demonstrate both of these options, and discuss what is happening when you do this. We will start by looking at the following part (Dtm_Curve1).

This part has a sketch feature on a datum plane (DTM1) that lies above the cylindrical surface, as we can see above. We will use this curve to project down onto the cylindrical surface. From a TOP view, we can see this circular datum curve takes up most of the width of the cylindrical surface, as shown below.

Therefore, we click on the Project Tool icon, as shown below.

When the dashboard opens, we will click on the References slide-up panel to see all of the options, as shown in the following figure.

At the very top, there is a pull-down field. Use this field to specify whether we are projecting an existing datum curve (Project chains), or whether we are going to sketch (Project a Sketch). If we were to select the Project a Sketch option, our panel would look like the following.

We can see a Define button that will allow us to go in and sketch the profile to project. Instead, we are going to continue with the Project chains option. Therefore, we need to select the existing edges or curves to project. We will select the circular sketch that is already in the model. When we select it, it becomes a bold red, as shown in the figure at the top of the next page.

The References panel looks like the following.

In the Chains field, we can see that “1 One-by-One Chain” is listed. Now, we must pick the surface(s) we are going to project onto. To initiate this selection, we can either pick in the next field down in the panel, or pick in the first field in the lower portion of the dashboard. We will select the cylindrical surface, as shown below.

Our panel now shows this surface listed in the Surfaces field, as we can see in the next figure.

Now we come to the part where we pick to project from the sketching plane, or whether we will project normal to a surface. Our two options are shown in the following figure.

If we choose Along direction, then we must specify a plane or planar surface that the normal direction is based on. If we choose Normal to surface we will not have to specify this. We will select the “Along Direction” option and then pick the DTM1 datum plane. The following figure shows the dynamic preview for the Along Direction with the DTM1 plane selected as the reference.

NOTE: The arrow doesn’t seem to make a difference in this case. You could try flipping it, but it does not change the preview. If we accept this result, from a TOP view, this is what we would see.

The projected curve is in exact alignment with the original sketched datum curve. If we were to select Normal to Surface, our result would be the following.

We notice that the projected curve is now more of an ellipse than a circle. Why? The reason is simple. If we look at the following figure, we will see the answer.

When you use Along Direction, the curve is almost extruded down onto the cylindrical surface, and the intersection of this imaginary extrusion and the surface creates the projected curve. When you use Normal to Surface, the surface takes control of the projection. It tries to locate the spot on the cylindrical surface that, when projected normal to the surface from that spot, it intersects with the original curve. We can see that, due to the curvature of the surface, it actually starts up higher and in more to get to the same original circular curve.

In many cases, you may have problems getting a “Normal to Surface” projected curve to work unless you really understand what is going on with the way it projects. Hopefully this will help you in getting the hang of it.

THROUGH POINTS The next type of datum curve we are going to show is the Through Points (or in Pro/ENGINEER – it is spelled “Thru Points”). This is a curve that passes through datum points or vertices. We are going to work with the following part (Dtm_Curve2) for this demonstration.

To create this curve, click on the general curve icon. It brings up a set of menus called the Menu Manager, which looks like the following.

The first option on this list is the Thru Points curve, which is the one we want. In the menu manager, you generally pick options at the top of the menu, then select Done, Done Sel or Done/Return at the bottom to continue. In this case, since the Thru Points menu item is already selected (shown in a black highlight), we will pick on Done to continue. This brings up the CURVE: Thru Points window, which looks like the following.

This is a different feature window than the dashboard. Many of the more advanced features still use this type of window. In the first column, entitled Elements, there is a list of items that we can define. The second column, entitled Info describes what is happening or what needs to happen to the element in the first column. You can see that we are currently defining the curve points. Below this window, we can see more menus, that look like the following.

In the top portion, we define the way it handles corners (at the points along the curve). If we use Spline, we get a continuous curve that is tangent along its entire length. If we use Single Rad, then we will specify a single bend radius that it will apply at each corner. If we select Multiple Rad, then we will be prompted to enter the bend radius at each point we select. In this example, we are going to stay with the default choice of Spline. In the second set of options, we can select Single Point if we want to pick individual points, even if they all belong to the same datum point feature. If we pick Whole Array, then we will get all of the points in the datum point feature. Since we are only going to go between to vertices, we won’t care what option it uses here. Finally, we have one last section of this menu. There is only one choice at this time, and that is to Add Points. Down below this menu manager, we see another little window, which looks like the figure below.

You are going to see this a lot. Every time you are prompted to select something, this window will appear. When you are finished selecting items, you click on OK to finish selecting. The easier thing to do, however, is to use the middle mouse button to click once to indicate that you are finished. It is the same as clicking OK. We are going to pick on the two vertices, shown in the figure below.

Once we select the second vertex, a blue arrow will appear, indicating the start point of the curve, as shown below.

Since we are done selecting, we will click with the middle mouse button, then select Done from the menu manager. We are now placed back into the CURVE: Thru Points window. We are technically done defining all of the required elements. There are still two optional elements we can define. We will double-click on Tangency from

the element list, which will bring up the menu manager shown at the top of the next page.

Looking at the menu above, we are asked to pick a Curve, Edge or Axis that defines the tangency for the start of our curve. On our model, the start point is highlighted with a red circle, as shown below.

We will pick the edge at the top of the front surface that intersects this start point. When we do, we will see the following on the model.

At the bottom of the menu manager, we see two options: Flip or Okay. The arrow points towards the direction that tangency is measured from. Many times, you will get it right the first time, and many times you will have to try again. If we pick Okay at this point (with the arrow going away from the curve that we are creating), we will get the following.

This is one of the times that we got it wrong. Not to worry, however. All we need to do is pick on the Start menu item, pick the edge again, and this time flip the arrow, then click on Okay. The result from doing it over looks like the following.

That is much better. Once we define the start point, it automatically jumps to defining the End point. We will pick on its adjacent edge, and flip the arrow so it is pointing in the direction shown at the top of the next page.

Once it is flipped to face in this direction, click on Okay to finish it. The curve now looks like the following.

This looks pretty good – much better than the straight line we had originally. Now that we have finished defining the references at each end for the tangency condition, we are placed back at the start point, and a new menu item appears in the menu manager, called Curvature. If we select this, the curve will take on the curvature of the entity that acted as the tangency reference. Since our entity was a straight edge, our curve will receive a small straight portion to it at that end. The figure at the top of the next page shows what would happen if we selected Curvature for the start point.

If we click on the end point, and select Curvature for this end as well, we get the following curve.

This is an even better curve, because it creates a smoother transition into the existing edges. If we were to use this curve to create a surface between the two protrusions, then our surface would have very good continuity with the surrounding surfaces. We are done defining tangency conditions, so we can select Done/Return at the bottom of the menu manager. We are placed once again into the CURVE: Thru Points window. We can see one last optional element, called Tweak. If we doubleclick on this element, we see the following window.

The curve on our model will show a control curve overlaid on it, as we can see below.

Using this menu, and/or dragging the control points on the model, we can adjust our curvature even more, or shorten/lengthen the straight portion of the curve as it goes into the adjacent edges. This basically gives us more control to Tweak the shape of our curve. We are going to cancel out of this tweak window by clicking on the red “X” in the lower left corner. Back in our CURVE: Thru Points window, click on OK to finish this feature. The resulting datum curve will look like the following.

USE CROSS-SECTION We haven’t talked about creating cross-sections yet, so we’ll just go into a part that already has one. The “Use Cross-Section Datum Curve” creates a curve that represents the boundary of the entire cross section. These curves are very useful for rib features, or other features that need a sketching reference but the shape of the surrounding geometry does not allow for picking as a sketcher reference. The curve segments at this area are always selectable. To demonstrate this, we will go back to a model that we saw in Lesson 3 – Selecting Objects (Selecting.prt). When we open it, it looks like the following.

To access the cross-section functionality, go to View, View Manager from the menu bar. We will get the following window.

Click on the Xsec tab at the top to get to Cross-section functionality. The window will now look like the following figure.

In this window, we can see a cross-section that already exists, called A. If your section is not visible on the model, click on the A row in the main window. The cross section looks like the following on the model when it is visible.

Now, we can close out of this window (which will make the cross-section disappear from the model), and create our curve. To create a cross-section datum curve, click on the General Curve tool. When the menu appears in the upper right corner of the screen, select Use Xsec, followed by Done. The menu will list all of the available cross-sections in the model, as shown below.

We can see the cross section “A” that we just looked at a minute ago. When we select A from this list, the curve is automatically created, as shown below.

The curve takes on any external edge that the cross-section goes through. That is why it goes around the entire part.

COPY CURVE (COMPOSITE) There are many times when you will need to have a single curve defined. A trajectory for a sweep might be a great example. However, many times you are unable to create a single curve that captures what you want. Therefore, you create multiple curves, and then you need a way to splice them all together to form a single curve. This is where the Copy Curve comes in. With this curve tool, you can select from existing edges or datum curves to form a single curve. To demonstrate this, go back to the Dtm_Curve2 model that we just worked with.

In this example, we want to create a single curve using the following three edges.

To create the copy curve, we first need to select the entities. Therefore, we will make sure our Smart filter is turned on, and we’ll begin by selecting the solid protrusion so it highlights in red. While this protrusion is highlighted, move your mouse over to the

edge labeled (1) in the figure above and select it. It should be bold, as shown in the following figure.

Something unique to the copy curve feature is the fact that we can NOT hold down the CTRL key and pick the other two entities. We must first hold down the SHIFT key on the keyboard, then RE-SELECT the same edge that we already selected. Once that edge is selected, keep the SHIFT key pressed and pick the other two entities. They should all be bold, as shown below.

Now that all of our edges are selected, we will go to Edit, Copy from the menu bar (or select Ctrl-C on your keyboard). Next, use Edit, Paste from the menu bar (or select Ctrl-V on your keyboard).

When we do this, our model will look like the following.

There is a yellow arrow at one of the endpoints (in this case the right-most end), which indicates the start point for the newly created curve. The little “T” symbols at the ends represent the distance away from the end that we want to end the curve. A value "0.00" will cause it to be at the exact length of the original geometry. Any value other than 0.0 will cause the curve to extend beyond the geometry or end before the vertex. The default value is 0.000, which assumes that the new curve takes on the exact length of the existing curves/edges. The dashboard for this copy command looks like the following.

In the Curve Type field, we have two choices. They are: Exact – The new curve takes on the exact shape of the selected entities. • Approximate – The new curve creates a C2 Continuous curvature condition • from existing C1 continuous entities. The only potential problem with the “Approximate” option is that the new curve may “liftoff” from the existing curves. The “Exact” option will keep the original curves as they are. The only restriction with using the “Approximate” option is that the curves already have to be tangent. Exact will allow you to use non-tangent entities. Therefore, we will change the Curve Type to Exact, and then accept this feature. The following figure shows the resulting curve in our model.

The curve may be difficult to see that it extends into the existing edges, but if you pick on it from the model tree to see it highlight, then you will see the figure above.

INTERSECT SURFACES Another curve type is created by the intersection of two surfaces. To demonstrate this, look at the following surface model (Dtm_Curve3).

We will make a datum curve at the intersection of these two surfaces. Therefore, we will begin by changing our selection filter to Quilts, and then pick the cylindrical surface, followed by the revolved surface.

The figure below shows both of these surfaces selected (in No Hidden viewing mode).

Once both surfaces are selected, we will pick on the Intersect icon in the feature toolbar, which looks like the following.

NOTE: There are three icons in the feature toolbar that look very similar. These are: •

Merge – Merges two surfaces together to form a single quilt.

•

Trim – Uses a surface or a curve as a trimming tool to act on another surface or curve.

•

Intersect – Intersects two surfaces to form a datum curve, as we see in this lesson.

Be sure you are grabbing the correct one. Once we select on the Intersect tool, the datum curve should be created automatically, as shown in the following figure.

TRIM CURVE Another operation that can be performed to create a new curve is to trim the curve using another curve or surface as the trimming tool. In this example, we will use a surface as a trimming tool. Look at the following model (Dtm_Curve4).

We are going to use the surface as a cutting tool to remove the portion of the curve that sticks out to the right of it. When creating a trim curve feature, always start by selecting on the object that you are trimming, in this case the curve. Use the Smart filter to select the curve, as shown below. NOTE: If the curve is made of multiple segments, as it is in this case, you will need to pick on the part of the curve that is being trimmed.

Once you have the curve selected, pick on the trim icon, as shown below.

When we enter this feature, we will click on the References slide-up panel in the dashboard to see the different entities we are selecting. It will look like the following figure.

We can see that the curve we selected shows up in the Trimmed Curve field. We are prompted to select the Trimming object. We will pick on the extruded surface. Our model now looks like the following.

An arrow appears at the cut location, and points towards the part of the curve that we want to keep. Flip the arrow if it is not pointing in the correct direction. Once you approve of the cutting direction, click on the green check mark to accept this. The curve will be trimmed up to the surface, as we can see in the following figure.

LESSON SUMMARY Datum curves are very useful tools for creating other datum features, surfaces or solid geometry. There are a variety of tools available for creating or editing curves. The most common curve types are sketched and projected. Remember that with the projected curve, normal to surface may give you results that you do not expect.

EXERCISES Create a new part called Basket, and create the two sketched curves (as individual curve features) that you see below (complete with dimensions). Create these on the TOP datum plane as the sketching plane.

Less on

1 1 Lesson Objective: In this lesson, we will learn about the Sweep feature.

SWEEP DEFINITION A sweep feature is created by taking a sketched profile and sweeping it along a sketched or selected trajectory. The cross-section of the feature along the entire length of the trajectory is constant. In a later chapter, we will learn all about variable section sweeps, and how you can create a basic sweep in this feature. For now, we will concentrate only on the standard sweep feature.

CREATING THE SWEEP To create a sweep, you must use the menu bar, and go to Insert, Sweep. When you pick on the Sweep menu, you will get another menu showing all of the different options, as shown below.

Unlike the extrude and revolve features that we have already seen, the Sweep feature makes you decide whether you are doing a Protrusion, Thin Protrusion, Cut, Thin Cut or Surface. Once you decide, you can not change it without deleting the feature and starting over. The method for creating the five different types is identical, therefore we will demonstrate this with a solid Protrusion. Therefore, we would select the Protrusion menu option. Once we do this, we see the following window.

We saw a similar window earlier in lesson 8 when we created a datum curve through points. We can see in this window that we are currently defining the trajectory for our sweep. The menu manager appears just below this, and looks like the following.

We can either sketch a trajectory (if one does not yet exist), or select an existing set of edges or datum curves for a trajectory. We will choose the Sketch Traj option to sketch our trajectory. Once we pick this option, we get the next menu.

In this menu, we are asked to create or select a sketching plane. This is a different way to prompt us for this information than we have been used to, but we will see this type of prompt quite often with some of the more advanced (or less commonly used) features. In this menu, the option to select an existing plane is already selected (Plane). Therefore, we just need to pick the datum plane or planar surface that we want as our sketching plane. We will pick the TOP datum plane. When we do this, an arrow appears on the model, as shown below.

In the message window, we are asked to select the direction for VIEWING the sketching plane. The menu manager gives us two options, as shown at the top of the next page.

We can either flip the direction then click on Okay, or accept the current selection by clicking only on Okay. We will accept the downward direction for viewing. Once we do this, the menu changes once more.

Here, we are asked to select or create the sketching reference plane and its orientation. We will select the Bottom orientation, then pick on the FRONT datum plane on the model. Once we do this, we are placed into sketch mode. We will create the following sketch.

We notice a yellow arrow on the sketch. This is the start point for our trajectory. This sketch is called an “Open Section”, since some of its endpoints are not touching each other. In an Open Section, the start point must be one of the open endpoints of the sketch (as it is above). If it is not, you must pick on one of the endpoints with the left mouse button so it highlights, and then right mouse click and select Start Point. The Start Point represents the location where your profile starts from. We want it to be on the straight segment for this example. Once our sketch is complete, we accept it by clicking on the blue check mark. We are then placed into the sketch for the profile that we are sweeping. We will create the following sketch for this profile.

When you sketch the sweep section (profile), there will always be a horizontal and vertical reference line that forms a “Crosshairs”. This “Crosshairs” marks the location

of the start point. If you are not sure how you are looking at the trajectory, I strongly recommend rotating your model slightly to see. You can always pick View, Orientation, Sketch Orientation to return to the sketch view. IMPORTANT! – When you have an open trajectory, you must have a closed section for your profile for a solid protrusion. We will see how to handle a closed trajectory in a few minutes. Once you are done sketching the profile, accept this sketch. All of the elements are now defined for this trajectory. We can click on OK from the window to complete the feature. Our model now looks like the figure at the top of the next page.

The symbol for a sweep can be seen by looking at our model tree, as shown below.

CLOSED TRAJECTORIES In this example, we will show the slight difference in creating a sweep that has a closed trajectory. We will start the same way that we did before by going to Insert, Sweep, Protrusion from the menu bar at the top. We will continue the same way by sketching a trajectory, and then using the TOP datum plane as our sketching plane, and FRONT datum plane facing towards the Bottom. Our sketch for our trajectory will look like the figure on the next page.

This is a simple closed rectangle. Once we are done sketching our trajectory and accept our sketch, we get a different menu option.

Our two choices are: Add In Fcs – Add Inner Faces – This requires you to sketch an open profile, • and as it sweeps around, it connects across all of the open endpoints to form

•

an inner face. This is great for closed picture frames, or other parts where the outside is definitely a swept profile, but the middle is closed. No Inn Fcs – No Inner Faces – This requires you to sketch a closed profile. There will be no inner face that results from this. This would be ideal for an open picture frame (with no back plate).

In this example, we will select Add Inn Fcs, and then click on Done to continue. We are now placed into our section for our profile. We will sketch an “OPEN” section, as shown below.

We can see the two endpoints of this sketch. As the profile is swept around the rectangle, the top endpoint will connect to itself at all locations across the center of the part, while the bottom endpoint does the same. Everything in between becomes a solid mass. When we accept this sketch and click on OK to complete the feature, we can see the following model.

If we made a cross section through the middle, we would clearly see the solid mass that was created, as shown below.

SWEEPING SURFACES Sweeping surfaces is no different than sweeping protrusions, cuts, etc. The biggest difference is that you don’t need to have a closed section. If you have an open trajectory or closed trajectory, you can still have an open profile. The biggest difference is that if the trajectory you are using is the edge of another surface, you may be asked to Join or No Join. If you select Join, then you are performing a Surface Merge at the same time. If you select No Join, then the new swept surface will be separate from the surface whose edge acted as the trajectory, and a merge operation will still need to be performed to get them to be one large quilt.

SELECT TRAJECTORY We will finish this lesson off with a demonstration of the select trajectory by picking on an existing curve to create a swept surface. Let us look again at the following part that we saw earlier.

If you recall, we have a copied curve that makes up the top left edge, the datum curve in the middle, and the top right edge. We will use this curve as our trajectory for our surface sweep. NOTE: Sometimes copied curves do not work for regular sweeps if they lie in three directions. The curve that we are using here is still a two-dimensional curve, because it is co-planar with the front surface of our part. We will start the sweep the same way, picking Insert, Sweep, Surface from the menu bar. When prompted, pick on Select Traj to select the trajectory. You will then see the following menu.

Since we are picking a datum curve, we will use the Curve Chain option, then pick on the top left edge, as shown below.

When you pick on a single segment of a curve chain, we get a little menu that pops up that looks like the following.

If you want the entire curve used as the trajectory, pick on Select All. If you only want a certain portion, then select From-To and pick the starting and ending endpoints of the curve. We want the entire curve, therefore we will pick Select All. The entire curve highlights in blue, and our start point is shown with the blue arrow, as we can see below.

Now that we have what we want for a trajectory, we click on Done to stop selecting and accept what we have. Another arrow appears on the model, as shown below.

If you recall when we sketch the profile, there is a horizontal and vertical reference line on the sketch at the location of the start point. When you select a trajectory, Pro/ENGINEER wants to know which way to orient the sketch. It highlights an adjacent surface or part of the trajectory selected, and in the message window it says. “Select upward direction of the horizontal plane for sweep section.” If we click on Okay in the menu manager, then the front surface of our part will be facing up in the sketch. You will want to pay close attention to which surface it is pointing, because it may make it easier or harder to sketch your profile. We will click on Okay to accept the default direction. Had there been more than one possible surface to pick, it would have prompted us to first pick the surface that we are going to face upwards before picking the direction. With a surface feature, we are given the option to create end surfaces or leave them open. The menu that comes up gives us these options, as shown below.

We will leave the ends open, so click on Done to continue. We are then placed into sketch mode to sketch our profile. We will sketch an open profile (which if you remember was not allowed for a solid protrusion). The figure at the top of the next page shows our profile.

We just sketched a straight line at an angle to the vertical reference. Once we are done, we accept the sketch then click on OK to complete the feature. Our model looks like the following.

LESSON SUMMARY The sweep tool is used to pass a profile along a trajectory that you either sketch or select. Depending on the section for the trajectory (open or closed), you will have restrictions on what type of section you can have in the profile. For a closed trajectory, you can add inner faces or leave the part hollow. For surfaces, you can also create end surfaces as well.

EXERCISES Create the parts shown on the following pages. Use a combination of extrude, revolve and sweep features where applicable, and create any datum geometry necessary to complete your model. Dash_Pot_Lifter

Basket_Prt (Continued) Open up the Basket part that we started in lesson 8. Create a swept surface using the inside trajectory. For the profile, sketch a line angled inwards from the trajectory by 5 degrees to a depth of 18 inches, as shown below.

Les son

1 2 0 Lesson Objective: In this lesson, we will learn about the Blend Feature.

BLEND DEFINITION A Blend feature creates a single feature by blending sections of varying size, shape, and orientation. There are three types of blend features. Parallel – All sections are parallel to each other separated by a blind depth • for each section. Rotational – The sections are offset each other by an angle around a • central axis of revolution, and a distance along the axis itself. General – The sections can be rotated in the X, Y, or Z direction as you • create them. To create a blend feature, we must use the menu commands Insert, Blend, then select one of the feature types shown in the following menu.

As with the sweep feature, the method for creating a blend is very similar from type to type.

PARALLEL BLEND To demonstrate the parallel blend, we will create a part called Parallel_Blend. We will start by going to Insert, Blend, Protrusion. This brings up the following menu.

In the top portion of this menu, we are defining the type of blend we are going to create. We will keep Parallel as the option. In the middle portion of this menu, we are defining how the section will be handled. There are two options. • •

Regular Sec – The section will be sketched on a plane or planar surface, and remain there when blended together with the other sections. Project Sec – The section will be sketched on a plane, but it will be projected onto a surface as part of the blend.

For now, we will keep the default option of Regular Sec as our choice. In the third section, we only have Sketch Sec available. For a Rotational or General blend, we would have the ability to select sections instead of sketching every one. Once we have all of the options picked, we will click on Done. We will now be placed into the definition of the feature, and we see the following window.

We are currently defining the attributes, which are in the following menu.

There are two attributes to choose from: Straight or Smooth. If our blend feature only has two sections being blended together, then this will make no difference. If our blend feature has three or more sections, then a straight attribute connects them lienearly, almost like a connect the dot with straight lines. A Smooth attribute connects them as a spline would going through points. You get a continuous, tangent edge from section to section. To start, we will keep Straight selected, and click on Done to continue. We are now prompted to select or create a sketching plane. We will select the TOP datum plane. When we pick this plane, an arrow appears, as shown below.

Unlike all of the other times when we were asked to accept the direction of viewing the sketching plane, we see the following prompt in the message window: “Arrow shows direction of feature creation. Pick FLIP or OKAY.” We know we are still going to be looking at the TOP plane, but for a protrusion, the feature always comes towards us in sketch mode, while for a cut, the feature always goes away from us in the sketch. It will take a little getting used to, but eventually you will understand just how the sketch is going to orient based on what you pick. Therefore, click on Okay to accept the direction as up, then face the FRONT datum plane towards the Bottom. We will now be placed in sketch mode. We are going to sketch three rectangles to blend. We start by sketching the one that will eventually lie on the sketch plane, as shown below.

I am taking advantage of symmetry by using two centerlines. That way I only need to use two dimensions. I want to note where the start point is on this sketch. I will demonstrate why this is important a little later. For now, we just want to make sure that the start point is in the upper left corner for all three of our sketches. Once I am done sketching this profile, I need to toggle to the next section using Sketch, Feature Tools, Toggle Section. The first rectangle becomes grayed out, and I can start sketching my second profile. The figure at the top of the next page shows this sketch with the second rectangle.

Note how the start point on this rectangle is equivalent to the location on the first one. Now we are ready to make our last rectangle. Once again, we will use Sketch, Feature Tools, Toggle Section. Now both our rectangles are grayed out for us to sketch the third, as shown below.

Once again, we are keeping the start point the same on all three. When we are finished with this rectangle, we will accept the sketch. In the message window, we are prompted for the depth of section 2. In other words, what is the blind depth between the sketching plane and the second rectangle that we sketched. We will enter 8.0. We are then prompted for the depth for section 3. This is the depth between section 2 and 3 (not the distance from the sketching plane to section 3). We will enter 5.0. We are then back at the window, where we can click on OK to finish this feature. The model looks like the following.

You can clearly see what the Straight attribute does, it makes sharp edges between sections. We will go to the model tree, right mouse click on this feature, and select Edit Definition to go back in and redefine this feature.

We are placed back at the window where we see the different elements we defined. The first one on the list is Attributes. If we double-click on this, we see the menu again where we originally picked Straight. Now, this time, we are going to select Smooth, followed by Done, then click on OK in the window to finish out the redefine. The model will regenerate, and look like the following.

This is quite a difference. Now, we have tangent edges going through the three sections. This makes for a more pleasing part. Now, we will edit the definition of this feature again. When we see the window pop up, we will double-click on section, followed by Sketch in the menu manager. This will bring us back into the sketch, which now has the first rectangle active while the other two are grayed out. We will turn off the display of dimensions and constraints using the icons in the system toolbar for easier viewing of the sketch, as shown below.

We will toggle to the next section, and change the start point. To change the start point, click on a different vertex to highlight it, the right mouse click and select Start Point. We want to use the next corner in a clockwise direction, as shown below.

Toggle to the third section, and change its start point to the one shown in the figure below.

Once we have changed this last start point, accept the sketch, and then click on OK from the window to finish the redefine. The model will regenerate, and it should now look like the following.

There is a twisting effect going on here. The start point location is used to define how the entities are connected. Imagine that the sketch starts off by connecting all of the corners that have the start point, then it goes to the next clockwise corner for each section and connects those, and so on. This is how we got the twisting, because each section was connecting 90 degrees clockwise from the previous one.

ROTATIONAL BLEND A rotational blend takes advantage of a sketched coordinate system. Instead of sketching all the profiles in a single sketch like we did with the parallel blend, we only sketch one, however, we must include a coordinate system in each sketch to tie the sections together. This will make more sense in the following demonstration. We will begin by creating a new part called Rotational_Blend. Once inside, we will go to Insert, Blend, Protrusion from the menu bar. When the first menu comes up, we will pick on the following options: Rotational, Regular Sec, and Sketch Sec. This will bring up the following window.

We are currently defining the attributes. In addition to Straight and Smooth which we had in the parallel blend, we have two other choices: Open and Closed, as shown at the top of the next page.

We will see the difference between these two during this example. For now, we will keep the default of Open, select Smooth from the top choices, then click on Done to continue. We are prompted to select a sketching plane. We are going to pick FRONT. When we do, an arrow appears on the front plane, as we have seen it do many times before.

This time, however, the message window is asking for us to pick the direction of VIEWING the sketching plane again. The lesson you should have learned by now is to always look at the message window to see what you are being asked. It will save you a lot of time later. We will accept this direction of viewing by clicking on Okay, then we will select the TOP plane to face towards the Top. Inside the sketch we will create our first section, which looks like the following.

The first sketch will be the only one that contains sketcher references. We want to create a sketched coordinate system and locate it at the intersection of the two sketcher references. The coordinate system shows the sketch as lying in the X-Y plane, where Y is going upwards. Once we have finished creating this sketch, we accept it. In the message window, we are prompted to enter the rotation angle about Y. Using the right hand rule (thumb points in the direction of Y, and the direction your fingers curl represents the positive angle), we will enter a value of 30 degrees. We are then placed into a new section. We are going to sketch the same profile as we did before. HINT: Use Sketch, Data from File, then click on the “In session” icon (little blue computer screen) to list all of the current sections that are in memory. The latest one on the list represents the one you are currently working on,

so the one before that numerically is the last one that you did. Retrieve or sketch the following for the second section.

You will notice that there is a coordinate system in this sketch, because it is what ties this section’s location to the first one. Once we are done with this sketch, accept it. Down in the message window, we are asked if we want to continue on to another section. We will type Y for “Yes” and hit the enter key. We will now be asked for the rotation angle for the next section about the Y axis. This will be the angle between section 2 and 3, so we will enter 60 degrees. We will be placed into the sketch, where we will create the figure at the top of the next page.

This sketch has different dimension values for the arc and the horizontal dimension at the top. If you choose to re-use a previous sketch, you will need to make these adjustments before moving on to the next section. Once you are done, accept this sketch, answer Y to create another section and then enter 60 for the angle. Create the following sketch for the fourth section.

Accept this sketch and answer Y to create another section. Enter 30 degrees for this last angle, then sketch the following.

Once we are done with this last section, we will accept it, then answer N so that we don’t go on to another section. We will be placed back at the feature window. This time, make sure shading is turned on, and hit the Preview button in the window. Your model should look like the following.

Looking at the window, we can see there is an optional element we did not define. This is called Tangency, and it allows you to specify other surfaces that the open sections might be tangent to. In our model, we do not have any other features, so we really can not use this option at this time.

We will, however, change our attribute value. Double-Click on Attributes, and change the option from Open to Closed. Make sure you still have Smooth selected. Click on Done to accept this choice, then OK to finish the feature. You will now see the following model.

So, have you guessed how the Closed attribute works? It takes the first and last sections (as long as they are not touching), and attempts a revolve around the Y axis, blending the two together. It just happened that our first and last sections were identical, so it was able to create a semi-circular revolve to blend the two. If you just looked at this model without knowing that it only took one feature to create this, you might think it was made up of complex surfaces, and datum curves, etc. This just goes to show you that you can get pretty complex shapes with very little feature headcount or complexity.

GENERAL BLEND A General Blend combines the parallel and rotational blends, and adds the ability to rotate about more than one axis. Consider the following part (General_Blend.prt).

We can see the sections in the order in which we are going to pick them. These sections are already sketched datum curves. When creating general blends, it is often easier to create your sections as curves before you create the feature. We will create the blend by going to Insert, Blend, Protrusion from the menu bar. At the first menu, we want to select the following options: General, Regular Sec, and Select Sec. We will hit Done to continue. The window for the general blend opens up as follows.

This is the same window that we saw for the rotational blend, but the options we pick a little later will be different because we chose to select the sections. For the attributes, select Smooth, followed by Done. The following menu comes up.

We are being asked to select the first curve. We want to select all four edges of each rectangle, so we are going to select on the Sel Loop option in the lower part of the menu, then pick on the first section curve, as shown below.

We can see that all four edges of this curve were selected, and we have a start point in the upper left corner. As we rotate our model around to select the other entities, we want to make sure we pick the same corner or we’ll get that twisting effect we saw earlier. Once we have the curves selected, pick on Done. We should see the same menu again (almost as if it didn’t take our previous selection). This is normal, because we have to specify at least two sections. We are going to pick the Sel Loop menu command again, and this time we will select the second rectangle. When we pick it, it looks like the following.

All four edges were selected, but our start point is not in the right place. Therefore, click on the Start Point menu command, and pick the upper left corner. Once we do this, our sketch will update as follows.

Even though the arrow is pointing in a different direction, the fact that it is on the upper left corner is all that we care about. Pick on Done to finish this second section.

In the message window, we are asked if we want to continue on to the next section. Type in Y for yes. Repeat the process of picking using the Sel Loop command until all of the remaining three sections have been picked and the start points for all of them is in the correct orientation. On the last section, we want to make sure that the point selected when looking from a top view is the lower left corner (because we want the part to rotate up 90 degrees at this point. Once all of our sections are done, answer N to the last prompt about creating additional sections, then click on OK in the feature window to complete it. Our final feature looks like the following.

If the general blend fails, it is most likely that one of the start points was in the wrong location. Go back into the sections to fix any that were failing.

LESSON SUMMARY Blends are a great tool to create complex transitions between different shapes. You can accomplish with a single blend feature what you might take dozens of surfaces, datum features and other entities to create, so don’t be afraid to try them. You can either select sections or sketch them. Parallel blends will only let you sketch all of the sections in a single sketch using Toggle to go between them. Always check the start points in the sections. Arranging them in different locations can cause twisting to occur, or feature failure.

EXERCISES

Create the part shown on the next page. Use a blend feature to create the main shaft of this part. Use Extrude and Revolve features for the remainder of the features. Hand_Rail_Column

Les son

1 3 0 Lesson Objective: In this lesson, we will learn about Rounds.

ROUND USAGE Rounds are used to remove sharp edges/corners in your model. They are generally very easy to create, but very easy to fail. For this reason, they should be modeled as some of the last features in your part, unless they are needed to complete another feature (other than another round). Rounds that add material should be created separate from rounds that remove material, especially if they potentially intersect each other. There are basically two types of rounds: Constant – the radius value is the same along the entire length being rounded, and Variable – the radius can change along the length being rounded. Both of these rounds are created using the same round tool.

CREATING ROUNDS To create rounds, click on the following icon in the feature toolbar.

Specify references to round. The thing to keep in mind is the concept of round sets. A round set is a single, tangent edge, or multiple, tangent edges that all have the same radius value. You can create as many round sets as you need (following the rule about adding/removing material). To pick multiple edges to be in a single round set, use the Ctrl key on your keyboard, then pick the edges. To create a new round set, simply pick a new reference without holding down any keys on the keyboard.

You can still use the Shift key to get a chain of edges.

CONSTANT ROUNDS SELECTING EDGES We will start by demonstrating how to create round sets with constant radii values. To do this, we will open up a part called Headset, which will initially look like the following.

We will start creating rounds by picking on the round icon. In the dashboard, we will click on the Sets slide-up panel to see its contents. The dashboard looks like the following with the panel open.

We can see a column in the upper left. This column will keep track of the different round sets that we create. To the right of this column are several fields that define the shape of the round. The default, and most commonly used settings are shown above (Circular cross-section for the round, and Rolling Ball for the type of milling operation that would create such a round). There are other settings, but since they are not widely used, they will not be discussed in this guide. In the References field, we will see a tally of entities that we select for the current active round set. Below this is a field that lists the radius values used for the active round set. We will see this field in more detail when we talk about variable rounds. Right now, there are no references picked (hence the “No Items” text in the References field). We will start by picking on the sharp edge at the top of the model. When we pick on it, it will highlight in a bold red, and a preview of the round with its current radius dimension will show up, as we can see in the figure below.

We can drag the white squares to dynamically update the radius value, or we can double-click on the radius dimension itself and enter a new value. We are going to change this radius to 0.7. The model will update, as shown below.

If we look back at the Sets panel, we can see the first round set listed, and we can see the references field includes the single edge that we picked. The radius value appears in the lower field, and in the icon bar at the very bottom of the dashboard.

Now, without holding down the Ctrl key, we will select one of the vertical edges at the other end of the rounded surface. Once we have one of them selected, we will hold down the Ctrl key to select the other. With both selected, modify the radius value to 1.2. Our model should look like the following figure.

The Sets panel now shows the second round set, the two edges used for this set, and the radius value applied.

It is currently the active round set because it shows up in red and yellow on the model. The first round set should be a muted cream color (when using the standard color scheme). In my illustrations, it appears as a dark gray outline of the dynamic preview for the round. Now, we will create a third round set and pick the bottom two vertical edges. Remember to start the round set by picking on one of the edges without holding down any keys on the keyboard. Once you have the first edge selected, use the Ctrl key to select the other. Initially, they will take on the radius value of the previous round set, as we can see in the following figure.

What we actually want is to remove the surface at the bottom with a full round that goes all the way around, forming a semi-circle. We could enter a radius value that is equal to half of the width of the part, but if we later change the width, the round might fail, or at the least, no longer be a full round. To preserve design intent, we will turn this round set into a full round. Looking at the Sets slide-up panel, we can see the third round set highlighted.

To the right of the sets list, we can see a button that is called Full Round. It will only be available if the current round set has two edges that are across from each other on the same surface. Picking on this button gives us the following result on the model.

We can see that the radius value has disappeared. If we look at the sets panel, the radius value is dimmed here as well.

Now that we have all three round sets defined, we will click on the accept icon to complete this round feature. The model looks like the following.

If we were to look at the model tree, we would only see one round feature listed. This single round feature contains three separate round sets. We will create one additional round for this model at this time, and that will be along the entire top edge of the model, with a radius value of 0.4. To create this, we will pick on the round icon, and then select one of the edges. It will automatically assume that any tangent edges to the one that we selected should also be rounded. This is a good assumption, because 99% of the rounds created are intended to round an entire tangent chain of edges. The preview for this round looks like the following.

Accepting this gives us the following model at this time.

We will save this model and come back to it later. SURFACE TO SURFACE ROUND In addition to selecting edges to round, we may also select two surfaces that share a common edge. Look at the following model (Round2.prt).

We are going to round the front, top edge by selecting two surfaces that share this edge. Therefore we will go into the round tool. Instead of picking on the edge (which is probably the easiest thing to do), we will pick on the left front surface, and then hold down the Ctrl key and pick the top flat surface. We will see a preview of the round, as shown below.

We will modify the radius to 0.5, and then accept this round feature. Our round will look exactly like an edge round, as we can see below.

ROUND THROUGH CURVE Another type of round is one that rounds an edge chain, but the radius is controlled by a datum curve or set of nearby tangent edges. We will continue with the same model as the previous section to demonstrate this. We can see from the figures on the previous page, that we have a datum curve sketched on the top surface. We are going to use this datum curve to define the radius for an edge round on the back edge. We will start by clicking on the round tool. We will pick the edge that we want to round first, as we can see in the following figure.

Then, we will expand the Sets slide-up panel to see the options, as shown below.

In this panel, we see a button entitled Through Curve. We want to pick on this. When we do, the panel will change slightly, as we can see below.

Instead of the field at the bottom with the radius values, we now have a field used to define the curve that we are going to follow. We will pick the datum curve on the model, and when we do, we will see the dynamic preview of the round.

We will accept this round, and our model will now look like the following.

THROUGH VERTEX/POINT ROUND The last constant round we will demonstrate is one that uses a nearby vertex or datum point to define the radius value. Look at the figure below to see the model that we are going to work with (Round3.prt).

We are going to round the front edge at the base of the rim that sticks up from the top of this part. But, we want the round to come up to the front edge. We could measure

this distance and use that for the round, but if we change the model, that round will remain at a fixed radius. Therefore, we want to use a vertex on the front edge as the radius value. That way, if we change the dimensions of the model, the round remains up to the front edge. We will start by going into the round tool, and select the edge to round, as shown below, and use a value of 0.100.

We can see that the round goes up to the top of the rim, but stops short of the front. We will open up the Sets panel to make our change.

At the bottom of this panel, we see a field with the word Value in it. This field is used to determine how the radius is measured. Value means that we are going to enter a

dimension value for the radius. This is the most common way to specify the radius, and that is why it is the default value. If we pull-down this field, we see another option, called Reference. Reference allows us to specify the location by picking on existing geometry. The following figure shows what we are going to pick.

Once we select the vertex, our round should update, and the dimension value should disappear. We see a reference to the vertex instead.

In the lower right corner of the dashboard, we will click on the preview button (the eyeglasses) to see what this would look like if we accepted it right now.

VARIABLE ROUNDS A variable round is one that changes in radius value as it traverses its edge. To demonstrate this, we are going to open the Var_Round model, which looks like the figure below.

We want to round the top edge where the extruded and the revolved protrusions meet. We notice at the very right end of this edge, we come very close to the side of the plate. We could create a constant radius around this entire edge, but it will create a very ugly condition at the end, because it won’t be able to maintain its nice shape all the way to the endpoint. Therefore, we are going to taper the round at this point. To do this, we will go into the round feature, and then select on one of the segments of this tangent chain of edges. Initially, the radius may come in very large. We want to modify it to 0.075, which will be our primary radius value for this edge. The round will initially look like the following.

You can see with the dynamic preview (shown above) that the round does not go all the way to the end as a constant radius. Therefore we need to make this a variable round. In order to make this a variable round, we need more than one radius. To add additional radii, hold the right mouse button down over one of the white squares (drag handles) where you see the existing radius dimension. When we do this, we should get an option to Add Radius, as shown below.

When we select this option, the existing radius dimension will snap to one end of the tangent edge chain, and a new radius will appear at the opposite end, as we can see in the figure at the top of the next page.

We could change the dimension value at the end now, but it would create a gradual taper across the entire length. We actually only want to start tapering as we come across the top of the rounded edge. Therefore, we will need another radius. Holding the right mouse button over one of the drag handles on the leftmost dimension, we will select the Add Radius option again. It creates a new radius point, but places it on the same segment that the existing radius is on, as shown below.

We can see from the above figure that it has the same radius value as the original (0.075), but it also has another dimension (0.200). This is the length ratio for this radius. In other words, it represents how far along the current segment it lays in terms of a percent of the length. If we wanted this radius to be exactly at the midpoint of this arc, we would change this dimension to 0.5. To move the radius to its proper location, we could place our mouse cursor over the white circle (which sits on the edge being rounded), and slowly drag it across the edge. You must keep your mouse cursor over the edge as you drag it, otherwise it doesn’t work.

For a very long edge, this could take some time. Instead, we are going to specify the exact location ourselves. To do this, open up the Sets panel. We can see the three radius points in the field at the bottom of this panel, as shown below.

For points 1 and 2 (which are at the endpoints of the tangent edge), we can see a Location called out as Vertex:Edge… For the third point (the new one that we just added), we can see a location of 0.200 (which was our length ratio). Below this field, we can see the word Ratio in a pull-down field. To specify an exact location, we will use the pull-down to select Reference. When we do this, we can pick the exact vertex or datum point where we want to place the radius. We will pick on the vertex of the round going across the top, as shown in the following figure.

Now that we have specified all of the radius points, it is time to modify the values. The design intent for this round is to maintain the 0.075 radius until we get to the rounded edge, then taper down to a 0.0 radius value at the small end. Therefore, we will modify the rightmost dimension to 0.0. Our dynamic preview will show us the result.

This is exactly what we want, so we will accept this round. The nice thing about the dynamic preview is that you can use it as a gauge to let you know if the feature will work or not. If the dynamic preview shows gaps across the edge, or is not visible at all, then the feature will not work. NOTE: Not all features in Pro/ENGINEER use a dynamic preview, however, so don’t get confused if you do not see one. You can always click on the full preview icon to test it before accepting it. Our final model looks like the following.

ROUND TRANSITIONS So far, we have only been talking about round sets. When you create a round feature, you start by defining all of the round sets. In many cases, that is all you have to do. There are some cases, however, where you will need to define transitions. A transition is generally needed when two or more round sets converge at a nontangent location, such as a sharp corner. The transition defines how the shape of the round will behave at such a location. To demonstrate this, we will open up the following part (Round4.prt)

We want to round the three edges that converge into the sharp corner where the two protrusions meet. Each one of these rounds needs a different radius value per our design intent. The following figure shows what we want to do.

We know that we can create three separate round sets, each with a unique radius value, so that is how we will start. We will go into the round tool, then select the three edges as separate round sets, and give each their respective radius value. It will not matter which order we go in, only that we have three separate round sets. The following figure shows these three sets after their radii values have been modified.

We can see that the dynamic preview for the three do not meet at the corner. They each have their own stopping point (at the ends of their segments). We will need to define a transition to ease these three rounds together. The Sets panel at this point looks like the following.

Down in the lower left corner of the dashboard, we see two icons, as follows.

The left icon is used to define Sets. It is selected as a default when you create a round. The icon on the right is used to define Transitions. We will click on that now. In the model, any transition will highlight. You will have a possible transition at each of the following. Intersection of two or more rounds at a non-tangent location • Any free end of a round set (where the end of the round is) • Our model has four potential transitions we could define, as shown below.

We only need to worry about the transition where the three round sets meet. If you move your mouse over the transition, it will pre-highlight. Select it so it becomes active. When active, it will turn yellow, as shown in the following figure.

In the dashboard, we will see a field that lists the current, default transition type.

The default transition type in this case is a Round Only 1. That is what you see in the preview on the model. If we use the pull-down arrow, we can see the other transition types that would work for this intersection. They are shown in the following figure.

There are actually more transition types in Pro/ENGINEER, but you will only see the ones that will work at this time. If we move our mouse over the transition in this pulldown list, and watch our model at the same time, we will see it dynamically preview the transition in blue. If I move the mouse over the Patch transition type, I would see the following preview on the model.

You can see that there are still some gaps in this transition type, so I would not put a lot of faith in the transition looking like it does above. If I place my mouse over the Round Only 2 transition type, I would see the following.

This looks as if it will bring my two larger rounds to a sort of chamfer, then round the top edge with the smallest round. I will go ahead and accept the default Round Only 1 transition type, then accept the round feature to complete it. Our final model looks like the following.

Just in case you are wondering what the result is for the other two transitions, here they are.

As I mentioned before, the Patch preview looked like it wasn’t working properly, so it defaulted to a Round Only 2 condition. That is why they both look the same.

LESSON SUMMARY It is very easy to create rounds in Pro/ENGINEER, but you should try to create most of them as the last features, since they are primarily used to remove sharp corners.

The best reason for putting them last in the model is because they are often suppressed before exporting the model to an analysis package, such as ANSYS. If you must create them early, it should be because you need them for downstream features. You should always avoid creating a non-round feature by tying it to an existing round. For example, you should not create an extrude feature and “Use Edge” on the round in the sketch. Of course, there are always exceptions in rare cases. Create multiple rounds into a single set if they have the same radius value. Use Ctrl to do this. Create multiple round sets if you need different radius values. For multiple round sets that converge to non-tangent corners or edges, define transitions to smooth out the round.

EXERCISES Open up the Hand_Rail_Column.prt part that we created in Lesson 12. Add the rounds shown in the figure on the next page.

Open up the Dash_Pot_Lifter and apply the rounds shown below. HINT: The order in which you create the rounds will have an effect on your ability to create them.

Les son

1 4 0 Lesson Objective: In this lesson, we will learn about Edge and Corner Chamfers.

CHAMFER USAGE The chamfer tool is used to create a bevel on an edge or corner. I truly believe that it is an under-used feature. Many times, people will use an extruded cut or a swept cut to accomplish this, but you are adding complexity and regeneration time when a simple chamfer can be used. Just like the round tool, there are no sketches that need to be created, you only have to pick on edges or corners to chamfer, then modify dimensions. Also like the round tool, you can create sets with transitions.

EDGE CHAMFERS To demonstrate an edge chamfer, we will use the following model (Chamfer.prt).

To access the Edge Chamfer functionality, click on the following icon in the feature toolbar.

When we enter into the edge chamfer tool, we see the following dashboard (with the Sets panel opened up).

The top of the dashboard lists the different chamfer sets we create. The middle portion is used to list references for each set. The next field down will list the values entered for angles or linear dimensions. Down in the icon bar, we can see the familiar Sets and Transitions icons, but the next field over is new. This field is used to pick the chamfer scheme. There are four schemes to choose from, as shown below.

These are: D X D – You only need to specify the edge to be chamfered, and the • distance away from that edge (D). It creates a chamfer that is symmetric about the edge selected. D1 X D2 – You specify the edge to be chamfered, and then you edit two • linear dimensions. The chamfer is created with the ends of the chamfer at the distances specified from the edge. Angle X D – You specify the edge to be chamfered, and then enter a value • for an angle and a linear dimension. You can reverse the direction of the chamfer with a single click. 45 X D – This creates a chamfer that is identical to the D X D. The • difference is how it reports on a drawing when dimensions are shown. We will see this in more detail when we cover drawing mode. The following figure graphically shows how these different schemes work.

For now, we are going to keep the D X D chamfer scheme selected, and then pick on the edge shown in the figure below.

Change the “D” dimension value to 0.500 so it looks like the figure above. When we go to our Sets panel, we see the following.

At the bottom of the sets panel, we have a few other things we can define. The first field, that shows the word Value, can be used to switch to Reference. Choosing reference lets us pick a vertex or other entity to determine the distance “D”. The other field, which says Offset Surfaces determines how “D” is measured. Currently, it is set to go along the edge at a distance “D” from the surfaces that intersect where the edge is being chamfered. This is the most common method for doing chamfer dimensioning. You can also choose to determine the distance from a tangent reference which you will pick. We will not demonstrate this, but you are encouraged to try it out for yourself.

We are going to continue to create additional chamfer sets. Just like we did in the creation of rounds, if we hold down the Ctrl key, we would add more edges to the current chamfer set. If we just pick a new reference without holding the Ctrl key down, then it starts a new set. We will pick on the back edge of the model, as shown below.

Only after you start a new chamfer set can you change the scheme. Once we pick the edge shown above, we select a D1 X D2 scheme, then modify our values to the ones shown above. Now, our panel looks like the figure at the top of the next page.

We will create one more Chamfer set for this chamfer feature. Without holding down the Ctrl key, select the rim of the topmost hole, then hold down the Ctrl key and select the other rim. Once you start this round set, change over to an Angle X D scheme, and modify the D value to 0.25 and the Angle to 60.0 degrees. Your model should initially look like the following.

The entire dashboard at this time looks like the following.

We can see the Angle X D scheme is selected, and the values of our angle and linear dimensions. At the very far right of these icons and fields is an icon with a blue slanted line and two arrows. Use this to reverse the direction of the chamfer. When we do this, our model will now look like the following.

We will accept our chamfer once we are done defining these three sets. Our model will look like the following.

We will now create one more chamfer feature. This time we will use the 45 X D scheme, modify our “D” value to 0.25 and select the edge of the model shown below.

Once we have done this, accept this chamfer feature. The final model will look like the following.

CORNER CHAMFERS A corner chamfer creates a bevel on a corner of a part. To demonstrate this, we are going to open up the Corner_Chamfer part, which is a simple 5 x 3 x 2 rectangular block, as shown below.

There is no icon in the feature toolbar to access this feature, so we must use Insert, Chamfer, Corner Chamfer from the menu bar, as shown below.

When we do this, it brings up the following window.

The first thing we are asked to do is select the corner to chamfer. We will pick the front right corner. One of the edges will highlight, as shown below. (NOTE: Your edge may be different from my edge, and that is okay for this demonstration).

In the menu manager, we see the following choices.

Enter-input is used to type in an exact dimension value measured along that highlighted edge from the specified corner. For quick creation of the chamfer, we can initially use Pick Point and pick anywhere on the edge. We will use this option, and pick approximately halfway along the length of this highlighted edge. Once we select the first point, another one of the edges will highlight in a faint green color, as shown below.

We will pick approximately halfway along this edge as well. Once we pick, the edge that we just picked on will become highlighted in a bold red (just as the first one did), and the last edge will highlight in green.

As with the other two, we will pick approximately halfway along the length of this little edge. Once we do this, all three edges become highlighted in the bold red color, and we can pick OK from the feature creation window to finish this corner chamfer. Our finished chamfer looks like the following.

Now that we have the chamfer, we will select it from the model tree, click with the right mouse button, and select Edit. This will bring up the dimensions for the corner chamfer, as shown below.

We will double-click on each dimension and modify its value to be the entire length of the line that the dimension is on. When we modify the dimensions, they will turn green, indicating that they have not been regenerated yet, as shown below.

We will click on the regenerate icon in the system toolbar ( chamfer will look like the figure below.

), and our final

LESSON SUMMARY Use chamfers when you need to create a bevel on an edge. It is better to use a chamfer than an extrude or sweep feature (when applicable) because it does not involve any sketching. It will regenerate faster as well. Create chamfer sets just as you did with the round feature. Use Ctrl to add edges to the same set with the same dimensioning scheme (D X D, for example). Or, select a new edge to create a new round set, then change the scheme for that set. Use Pick Point for corner chamfers as a quick and easy way to initially create the chamfer, then Edit the dimension values to get exact results. This is especially important if you don’t know the length of the line on which the corner chamfer dimension is being measured, but you can always pick on that line.

EXERCISES Finger_Guide Create the model shown on the next page. NOTE: You may need to play around with chamfer transitions if you create the cuts first.

Les son

1 5 0 Lesson Objective: In this lesson, we will learn about the Draft Feature, including constant draft, variable draft, split draft, etc.

DRAFT USAGE You create a draft feature to remove perpendicularity between model surfaces and the parting line (for molded parts). This is such a critical feature for many of the products we design. At the end of this lesson, we will also see how to perform a draft check. Before we begin, we need to define a few key terms. DRAFT SURFACES These are the model surfaces that draft will be applied to. They can be solid surfaces or surfaces created as actual surface features. There are only two rules that are applied to draft surfaces. They must be closed in on the top, sides and bottom. Therefore, you can • not extrude a single line as a surface, then expect to add draft to that surface, because there is no top, side or bottom surfaces. Any tangency with adjacent surfaces may cause the draft to fail. For • example, suppose you have a rectangular block. You want to add draft to the front of the block, but you already have a round at the top edge. This front surface can not be used for draft. DRAFT HINGES These are planes, planar surfaces, datum curves or model edges that act as the axis of rotation for the drafted surfaces. When defining the draft hinge as a plane or planar surface, be aware of the distance from the surface being drafted, because it does affect it. When defining curves or edges for the draft hinge, you must also supply another entity to define the “Pull Direction” or the direction the part comes out of the mold. The following figure shows the potential problem with choice of draft hinge when using planes or planar surfaces.

Looking at the figures above, there is a datum curve that shows the original surface that is being selected as the Draft Surface. In the figure on the left, we use the top surface of the model as the Draft Hinge. In the figure on the right, we use a datum plane above the model. When the draft is calculated, it will project the draft surface up to the draft hinge, then apply the angle at their intersection. We can see that the overall width of the top of the part on the left is still the original length, but we’ve actually made the part bigger on the right.

DRAFT ANGLE The draft angle is the dimension value applied to the surface. There is a maximum of 30 degrees that can be applied as a draft. If you need more than 30 degrees, you will need to use a different modeling method, such as extrude, sweep, etc.

CREATING DRAFTS The draft tool is located in the Feature Toolbar, in the top most grouping of blue icons, and looks like the following.

To demonstrate the new draft tool, we will open up the model entitled Draft1.prt. It will initially look like the following.

We are going to draft all of the vertical surfaces in this model. Therefore, we start by clicking on the Draft icon in the Feature Toolbar. The dashboard (with the references panel open) looks like the following.

When creating a draft feature, the first thing you specify are the surfaces to be drafted. This is the top field in this References panel, and is activated by default. That is why it is not a field at the bottom of the dashboard. Therefore, we will select all of the surfaces (using the Ctrl key) that are shown in the next figure.

Once all of these surfaces are selected, we need to click into the Draft Hinges field (either in the References panel, or by picking the first field in the dashboard). With this field active, we can pick a planar surface, datum plane, or chain of edges/curves to act as our draft hinge. Therefore, using selecting techniques learned in lesson 3, we will pick the chain of tangent edges that go around the top, as shown in the next figure.

Since we did not use a plane or planar surface as our draft hinge, we must pick a datum plane or other planar surface in the model that is perpendicular to the pull direction. First, however, we must pick in the Pull Direction field to activate it. Once

activated, click on the TOP datum plane in the model tree. At this time, all elements are defined, so we can see an angle on our model for the draft, as shown in the following figure.

NOTE: If you don’t see the yellow arrow and angle dimension, you have not defined enough references for this draft feature. We can drag the handle for the angle dimension to dynamically see the draft preview update. We want to make sure we are drafting outwards as we go down from the top of the model. Once your draft is going in the right direction, enter 8.0 as the draft angle. Our preview now looks like the following.

Click on the green check mark to complete this first draft feature. The model will look like the next figure.

Save this model for later, and then close it.

SPLIT In Pro/ENGINEER, you can split a draft up with datum planes or sketch features. To demonstrate how to split draft, we will open the model entitled Draft2.prt, which looks like the following.

We will start by creating a draft feature. For our draft surface, we will pick the following surface.

Once this surface is selected, click into the Draft Hinges field, and pick on the FRONT datum plane as our neutral plane. When we do this, our model automatically

assumes the pull-direction plane is the same as the existing draft hinge that we picked. We can change this if we want, but we will leave it the way it is. Our model now shows the arrow and angle.

Change the angle value to 5.0, and our model will now look like the following.

So far we haven’t done anything related to splitting up the draft. The fact that we used a plane in the middle of the part as our draft hinge has only resulted in rotating the selected surface about that plane as draft was applied. We will now apply the split. To do this, open up the Split slide-up panel, which looks like the following.

Currently, the Split Options field is set to “No Split”. We will use the pull-down to select a different option. We have two additional options: 1. Split by Draft Hinge – Causes the surface to break at the FRONT datum plane, and each side will be drafted independently. 2. Split by Split Object – We can select or sketch a profile that splits up our part. The object must lie on the surface being drafted, and it must be planar. We can not split using a projected curve on a non-planar surface. We will choose the Split by Split Object option. This activates the Split Object field, and we will pick on the oval datum curve on the model. When we do this, our Split window looks like the following.

The model currently looks like the following.

We can see a clear independent oval surface in the middle of our existing drafted surface. We can also see two dimensions, one that will control the draft on the large surface, the other on the oval surface. We are not done yet. We want to remove the draft from the original surface, causing only the oval surface to remain drafted. To do this, we go back to our Split panel. At the bottom, in the “Side Options” field, the current value is Draft sides independently. There are three other options in this pull-down field. These are: 1.

Draft Sides Dependently – Both surfaces will have the same, but opposite draft angle. Only one dimension will control both. 2. Draft First Side Only – Only the large surface will contain draft, the oval surface will remain flat. 3. Draft Second Side Only – Only the oval surface will contain draft. The large surface will remain flat. We will use the Draft Second Side Only to give the illusion that we are creating a light switch. When we select this option, our model will look like the following.

We will change the angle to 10.0 degrees, making our switch more pronounced, and then click on the green check mark to complete this draft feature. Our final model looks like the following.

VARIABLE DRAFT The draft feature also allows you to make variable draft. It works just like the variable round tool. You would right click on the angle dimension and use Add Angle. This creates a second angle. The biggest difference is that both angles don’t automatically jump to other locations. You will need to drag these angles to the locations you want and then modify their values.

DRAFT ANALYSIS The Draft Check analysis is a little more streamlined in this release, as are many of the other analysis types. To perform a draft check on this model (Draft2.prt), we would go to Analysis, Geometry, Draft from the Menu Bar. This brings up the following interface.

We can run a quick check on the model, or we can retrieve a saved analysis that we have already created. We will keep the Quick option selected, and the click on the Definition tab at the top. This will bring up the following.

By default, we are being prompted to pick on the surfaces to check. To check an entire part, we hold the mouse cursor over the model so that one of the features highlights in blue. Then, we continue to click (slowly) with our right mouse button until the entire model highlights in blue, and we see our status window (or the tool tip) indicate SolidGeom, as shown in the following figure.

Once we see this condition, click with the left mouse button to select the entire part. Now, we will skip over the next field and go straight to the Draft Angle section in our window. For this, we are going to pick on the icon that has the arrows going in both directions (this indicates the “Both Sides” option). Then, we are going to enter the minimum draft we are checking against. In this model, we are going to check against 5.0 degrees.

Once we have entered this data, we will pick in the Direction field and select on a plane or planar surface that is perpendicular to the pull direction. In our example we will pick on the top flat surface (not the oval surface). Our window looks like the following once we have done all of this.

Our model will be shaded in colors, as shown below.

These colors correspond to the legend that pops up at the left of our screen, as shown in the next figure.

There are three black triangles on the left side of this legend. The top and bottom represent the positive and negative draft that we are measuring (since we picked “Both sides”). The max/min value is 5/-5 respectively. The center black triangle represents no draft (0.0), and this corresponds to the lime green color. On our model, we can see that any surface in this green color has no draft whatsoever. Any surface that is magenta or blue is at least 5.0 degrees, and any other colors are between 0 and 5 or 0 and -5.

LESSON SUMMARY The draft tool is absolutely necessary when working with plastic molded parts (or any molded parts for that matter). You will need to choose your Draft Hinge wisely to avoid growing or shrinking the model. Always perform the basic draft check outlined in this lesson to ensure you have enough draft on your model.

EXERCISES Open up your Safety_Key part file that you created back in Lesson 5. Perform a draft check to make sure you have at least 2 degrees of draft on every surface of the

model. Add draft where necessary. Assume the pull direction is perpendicular to the following surface.

Les son

1 6 0 Lesson Objective: In this lesson, we will learn about the Hole Feature.

HOLE USAGE This is another widely underused feature that should be used more often. Many people use extruded cuts or revolved cuts instead of holes, but many of the straight holes or even standard holes do not need to be sketched, and that will save time (both in regeneration and in the user’s time). There are two main types of holes: Straight – The profile is either a plain circle extruded to a certain depth, or • you can sketch a profile that creates a revolved cut. Standard – Select from industry sized holes (UNC/UNF, etc.) • Once you pick the type of hole you are going to create, you can place the hole using one of the following methods.

• • • •

Linear – Hole lies on a plane or planar surface and is located from two references (similar to a datum point on surface). Radial (Cylindrical) – Hole lies on the outside of a cylindrical surface, measured from a reference that is perpendicular to the cylinder’s axis, and located about the axis by some angle reference. Radial (Axial) – Hole lies on a plane or planar surface, but is located about an axis normal to that surface. Dimensions are radius or diameter around axis, and an angle through the axis. Coaxial – Hole lies along a datum axis and starts from a specified plane or planar surface to a desired depth.

CREATING A HOLE FEATURE The Hole feature is located on the Feature Toolbar in the same group of blue icons as the round, chamfer, rib, shell and draft, and represents the last of the pick-andplace features covered in this guide. The icon looks like the following.

To demonstrate the hole functionality, we will open up the Hole_Definition part, which initially looks like the following.

When you create holes, you generally have four types of placement: Linear, Radial, Diameter and Coaxial. We will use the next sections to show these different types.

LINEAR HOLE We will start by clicking on the hole feature, and then we will click on the model in the location shown below.

A preview of the hole appears on the model, as shown in the next figure. For a linear placement, there are a number of different drag handles that appear on the hole feature. They are shown in the figure.

Our dashboard looks like the following.

Depending on the type of hole you are creating, you will see different options in the dashboard. For a straight hole (circular cross-section along the entire length), the options represent the following.

For this first linear hole, we will change the diameter to 0.625 and change the depth option to Through All. Our preview will look like the next figure.

We still have two drag handles that need to be addressed. We will drag the two handles over to the following references.

Once we do this, we will see two dimensions on the model.

In the dashboard, we will click on the Placement slide-up panel, which looks like the following.

We can see the two references and the respective dimensions. We can also see a middle column that defines the relationship to the references. For the FRONT datum plane row, we will click on the word “Offset” and change the option to Align, and change the remaining offset dimension to 1.000, as shown below.

This will make the center of the hole line up with the FRONT datum plane, as we can see on the model preview.

Now we will click on the green check mark to complete this first hole, which will look like the following.

COAXIAL HOLE We are going to create another straight, simple hole. The first thing we are going to do is turn on the display of axes. Next, we will create a new hole and pick on the axis A_10 that is going through the large circle on the end. You will see an outline of the hole that is lined up with the axis that we selected. We will change the diameter value to 1.0, and the depth to Through All. When we do this, our preview looks like the following.

The “depth” of the hole seems to have gone to zero – even though it isn’t. The reason it does this is that there still is not enough information to fully define this hole. To see what is left, we need to expand the Placement panel, which looks like the following.

With a coaxial hole, the primary reference is the axis that we picked. The hole knows it is lined up with the axis, but it doesn’t know where it starts from. This is the Secondary Reference. Therefore, pick in the Secondary References field, and then pick on the large, flat, circular surface. The preview now looks like the following.

Click on the green check mark to complete this hole. The model now looks like the following.

RADIAL/DIAMETER HOLE The next hole we create will demonstrate the Radial and/or Diameter placement, but we will also shake it up a bit and switch from a straight, simple hole to a standard hole. Therefore, we will start by creating a new hole feature, and then pick on the following surface.

The hole will initially preview like a Linear placement, as we can see in the following figure.

Before we start dragging handles, we should open up the Placement panel, and use the pull-down field at the top right to change from Linear to Radial, as shown in the next figure.

In the figure above, you can see the four placement options. In this example, we use Radial, but we could pick on Diameter and the rest of these steps would be identical. The difference between “Radial” and “Diameter” is how it is dimensioned for the drawing. Once you pick on Radial, you must select additional references. Therefore, click into the Secondary References field to make it active, and then pick on the A_10 axis that we picked for the last hole. This will create a radius dimension from the axis to the center of the hole, as shown below.

Change this radius dimension to 0.875, as shown in the above figure. The second drag handle must be tied to a datum plane or planar surface that either passes through the A_10 axis, or is parallel to an imaginary plane that would pass through the axis. Therefore, we will drag the reference handle over to the FRONT datum plane. When we do this, an angle will appear on the preview, as we can see in the next figure.

We will modify this angle dimension to 60.0. The Placement panel will look like the following.

Now that we have successfully placed this hole, we will change it to a standard hole. NOTE: You could have selected standard to begin with, but I think it is easier to make the standard hole once it is fully placed, otherwise, you won’t see the correct shape in the preview. Click on the Standard Hole icon in the lower left of the dashboard. This will change the dashboard to look like the following (with the Shape panel expanded).

For the Thread Type field, we will keep the UNC option. Other options include UNF and ISO. For the Thread Size field, use the pull-down to select a 10-24 thread. For the depth option, we will pick on the Through All icon. This will make the Depth Value disappear. At the end of the dashboard icons, we will keep the Tapping and Countersink options selected. Up in the Shape panel, we want to change the depth of the thread to Thru Thread, so the threaded surface goes along the entire length of the tapped hole. We will leave the angle and diameter for the countersink alone, but we could change this if we needed. Our dashboard should now look like the following.

If we look at the preview on the part, we can see the shape and size has updated to reflect this standard hole. If we had not placed it fully, it would still look like a big yellow cylinder.

If we expand the Note panel, we can see the standard not that it creates by default. We can edit and add to this note. This note can be shown in the drawing to save us some time re-creating it.

We will now click on the green check mark to complete the hole. The model will look like the following.

To hide the view of the note on the model, we can go to Tools, Environment and uncheck the 3D Notes option. Our model will now look like the following.

Save and close this model. We will come back to it in the lesson on Patterns.

SKETCHED HOLES

The last option we have for the hole feature is a sketched hole. It is created by starting with a straight hole. In the dashboard, use the first pull-down field to change from Simple to Sketched. When we do this, the dashboard looks like the following.

The sketch must meet the following requirements: 1. Must have a vertical centerline that acts as the axis of revolution 2. Must only be a half-model of the hole (one side of the centerline) 3. Must be closed The “vertical” centerline is important to remember. Even if you are making a hole in the side of a block, where normally you would sketch a horizontal profile, you still make it vertical in this feature. The following figure shows the correct and incorrect way to do this.

LESSON SUMMARY Hole features should be used over extruded or revolved cuts. Placing the hole is simple and straightforward once you know what you need to select, and you can pick from standard, industry sizes and take the guesswork out of knowing the exact thread diameter to use. As you saw in this lesson, you can mix and match hole placement types and hole types. But perhaps the biggest benefit to using the hole feature is when you go to pattern, which we will see in a later lesson.

EXERCISES Open up the Hole_Exercise.prt part and add the three holes shown on the figure on the next page.

Les son

1 7 0 Lesson Objective: In this lesson, we will learn about the Shell Feature.

SHELL USAGE The shell feature is designed to take a solid part, and hollow it out to create a thinwalled part. Any exposed surface that is not selected to be removed will get a uniform thickness applied to it. Some surfaces can be specified with non-default thicknesses if necessary. To demonstrate the shell feature, we will open the Shell.prt part, which looks like the following.

If we look at the default cross-section for this part initially, we can see that it is a complete solid, as shown in the following figure.

We are going to hollow this part out so water will actually be able to fill it, and pour from it.

CREATING THE SHELL To create a shell, click on the following icon in the feature toolbar.

We will instantly see a preview of the shell, and an overall thickness value. Our thickness might be too large initially to see the preview, which means that if we were to accept the default thickness, our shell would fail. We will modify the thickness to 0.125, and then we will be able to see our preview, as shown below.

The dashboard for a shell feature looks like the following.

It is pretty simple. We only have a few things to define. In the icon row, we will define the overall thickness, and the side of the material the thickness is being added to. We can actually shell outwards if we wanted to. If we open up the References panel, we will see the following.

Initially, no surfaces will be removed, and there are no “Non-Default Thicknesses” defined. In other words, if we accept the feature right now, we will have a completely hollow, but closed part. We will accept it right now to show you what I mean. After we accept this, we will go to a FRONT view and look at the cross-section again. We can see that the part is hollow, but we can also see that it is closed the entire way around the part. So if water were in this part, it would have to have been poured as it was molded shut.

We will edit the definition of this feature in the model tree to make some changes. The first change we will make will be while we still have a completely hollow but closed model. In the References panel, click on the field for Non-Default Thicknesses, then select the top flat surface of this part, as shown below.

We can see another dimension appear on this part. If we change the thickness for this surface to 0.5, accept the part, and then look at the cross-sectional view again, we would see the figure at the top of the next page.

Any external surface can have a non-default thickness as long as it is not tangent to any other surfaces. Had we had a round at the top of this model where the flat surface met the side domed surface, then we would not have been able to perform this operation. Actually, we wouldn’t be able to remove it either. We will edit the definition once more. Go into the References panel again. In the Non-Default Thicknesses field, right mouse click on the surface that is listed, and select Remove. Then, in the Removed Surfaces field, click on the words “No Items” to activate this field. Pick the top flat surface, and the surface at the end of the spout to remove them, as shown in the following figure.

When we accept this part, and shade the model for better clarity, we can see that we have a hollow part, as shown in the figure at the top of the next page.

If we were to go back to our cross-section and use the clipping tool (Select Display, Set Visible, and then select Clip Front, we would see the following.

LESSON SUMMARY Use the shell tool to hollow out a complex part. The important thing to note is that you will want to use this feature later in the model, after you have defined all features that will need to be hollowed out. If you create a shell early in the part, then you might want to consider using surfaces instead, and thicken the surfaces later. We will see how to do this in an upcoming lesson.

Select surfaces to remove unless you want to design a blow molded part, and select non-default thicknesses, as long as they are not tangent to other surfaces that must be at the default thickness.

EXERCISES Draft1 Open up the Draft1 part that we created, and add a 0.1” round to both the top edge and the middle edge, as shown below.

Next, hollow out the model, removing the bottom surface with a wall thickness of 0.0625”, as shown below.

If we look at a cross-section through the middle of the part, it looks like the following figure.

Save and close this model.

Headset Open up the Headset part file that we created in Lesson 11, and add a Coaxial hole and Shell feature, as shown in the following figure.

HINT: You may need to create a datum axis first for the coaxial hole.

Les son

1 8 0 Lesson Objective: In this lesson, we will learn about the Rib Feature.

RIB USAGE The Rib feature is designed to create a thin walled protrusion between two or more surfaces in the model. The unique behavior of the rib as it can adapt to changing geometry better than an extrude feature makes is a great, but underused feature.

CREATING THE RIB The rib feature is located in the Feature Toolbar in the top grouping of blue icons, and looks like the following.

To demonstrate this feature, we will open up the Draft1 part that we have been working with. We will create a support/stack rib for this model. Therefore, we will start by clicking on the Create rib icon. The dashboard appears as follows.

We need to start by sketching our rib profile. In the References slide-up panel, we can see a Define button. When we click on this, we see the familiar sketching window.

We will pick the RIGHT datum plane as our sketching plane, and accept the TOP datum plane facing towards the top. When we get into the sketch, we will pick the inside elliptical edge as a sketcher reference, as shown in the next figure.

We are going to create the following sketch. NOTE: We will use an ellipse for the arc portion of this sketch, centered on the vertical reference line, located 0.464” below the horizontal reference line.

When we complete the sketch, we should see a preview of the rib. If the yellow arrow is not facing into the rib geometry, we will need to click on it to flip it. The preview should look like the following.

We will change the rib thickness value to 0.1”. Rotated, our final preview will look like the following.

Just like the shell feature, we have an icon next to the thickness field that is used to flip which side of the sketching plane our rib is added. By default, it wants to be symmetric about the sketching plane (0.05” on each side in this example). You can flip it to either side as well using this icon. We will click on the green check mark to complete this feature. Our model looks like the following.

Save this model and close it. We will return to this in the lesson on patterns.

LESSON SUMMARY Use a rib feature when you must add a thin wall between existing surfaces of a model. This is preferable to extruding a protrusion on both sides of the datum plane, because the rib feature will follow curving geometry where an extrude just goes straight out from the sketching plane. Use Cross-section datum curves when necessary to snap to the geometry at the location where you want the rib, especially if the geometry is curved.

EXERCISES Open up the Headset part that we have been working on. We are going to add a rib within the shelled out area. After we add the rib, we are going to add some rounds to make it look nice. Use the figure below as a guide for this.

Les son

1 9 0 Lesson Objective: In this lesson, we will learn about Patterns.

PATTERN USAGE Patterns are used to replicate a feature (or group of features) multiple times in a repetitive manner. Patterns can be as simple as three holes with equal spacing in a row, or one-hundred bumps on a surface to create a non-skid texture. There are three primary types of patterns. These are: Dimensional – You want to pattern an entity in a certain direction. A • dimension is selected that already goes in that direction. You provide the incremental spacing between entities, and the number of entities that will result. Table – You create a table based on selected driver dimensions. The table • can indicate non-uniform patterns. You can put as much or as little information into a pattern table as you need. Fill – You create a feature, then pattern that feature within a boundary that • you sketch. You can change the shape, spacing, angle and visibility of the instances in that pattern. Within a Dimensional pattern, you also have the ability to define one of three attributes. These are: Identical – Each instance is completely identical to the one that is being • patterned. The pattern can not intersect itself or leave the current surface boundary that the lead entity is located on. Varying – You can vary different aspects of the entity, such as depth, • diameter (for a hole), etc. for each instance in an incremental fashion. The instances are able to leave the current surface boundary, but they can not intersect themselves. General – There are no restrictions on this type, but it takes longer to • regenerate than an identical pattern. If you can’t get an identical or varying pattern to work, try setting it as a general pattern first. If this does not work, then there are bigger issues at work.

CREATING PATTERNS

The pattern tool is commonly activated using the right mouse button (either on the feature itself or on the model tree). You can also get to patterns through the Edit menu, or using the following icon in the Feature Toolbar.

You must start by picking on a feature to pattern, otherwise the tool is not active. To demonstrate the pattern tool, we will start with the Hole_Definition part that we saved from lesson16. It will look like the following.

We created three different holes in this part in lesson 16. The first (Hole 1) was a linear hole. The second (Hole 2) was a coaxial hole, and the third (Hole 3) was a radial/diameter hole. The following figure shows these holes.

We will start by clicking on the Hole 1 feature in our model tree (or the hole that corresponds to “Hole 1” in the previous figure). Once selected, click on the Pattern tool. The dimensions for the hole feature should appear on the model, as we can see in the next figure.

The dashboard appears and looks like the following.

By default, most features will assume a dimensional pattern type. This is the common one in 2001 – which requires you to pick a dimension that drives the first and second directions. Other pattern types exist in Wildfire 2.0, but we will start with the standard Dimensional pattern. Therefore, we start by picking on the dimension that drives the first direction of the pattern. We will pick on the 1.000 dimension. When we do this, a field appears right beneath the selected dimension, as we can see in the next figure.

We will use this field to specify the increment between holes. Type in 3.25 and then hit the <ENTER> key on your keyboard. You should now see little black circles indicating where the holes will be when completed as shown in the next figure.

If we open up the Dimensions panel, we will see the following.

We can see the dimensions and increment values defined for the first and second directions. We can also see that we can define the increment by relations. Currently, we have defined a single driving dimension for direction1, and the spacing is 3.250. If we go to the Options panel, we can see the three different classifications of patterns.

We will leave these alone right now. Click on the green check mark to complete this pattern, and you will see the following.

Next, we are going to create a radial pattern using Hole 3. For this pattern, we will use a reference instead of an actual dimension to drive the pattern. Therefore, start by picking on the hole in the model tree and then click on the pattern tool. We can see the dimensions show up in the next figure.

We could select on the 60.000 dimension to drive the angle, but we will demonstrate a different type of pattern, called Axis. In the dashboard, use the first pull-down field to change the option from Dimension to Axis, as we can see in the next figure.

Once we select Axis, we must select a datum axis or edge that will act as the pattern reference. We will turn on our datum axes and select the A_10 axis. Once we do this, we can see a different look on the model.

There are now two arrows, one for the first direction (maroon arrow labeled “1”) and one for the second direction (yellow arrow labeled “2”), as we can see in the figure above. We can also see the default increment is currently 90.000 degrees, and there are four black dots representing four holes. In the dashboard, we can see the following.

There is still a section for first direction and second direction. We will change the total number of instances from 4 to 3, and the angle from 90.000 to 120.000, as shown below.

This change is also reflected on the model itself.

We will now click on the green check mark to complete this hole pattern. Our model will now look like the following.

Save and close this model.

FILL PATTERN The next pattern type that will discuss is the Fill pattern. This is new in Wildfire, and offers a huge benefit to users that create very large identical patterns that fill in a grid on a model. For example, suppose you are creating a non-skid surface with all of the little diamond shape bumps on it. This would be one way of doing that. The advantage of a fill pattern over an identical dimensional pattern is the fact that you don’t have to stay within a rectangular grid, and the second is that the lead feature doesn’t have to have any dimensions associated with it, nor do you have to even keep the lead pattern. To demonstrate this pattern type, we will open up the model entitled Boat. It will initially look like the following.

This is a bath mat, and requires suction cups along the bottom to prevent it from sliding. If we turn the model around, we can see one of these suction cups that we created.

If we zoom in close on this model, we can also see a sketch feature. This sketch feature defines the area that is going to be filled. We can either use a sketch feature (as we are in this example), or we can sketch a shape once we get into the pattern itself.

If we look at the model tree, we can see that we created the suction cup as a revolve feature, and we used an “on-the-fly” datum plane, which caused the features to be grouped together.

With a regular dimensional pattern, this would be necessary to include the offset dimension for the plane to be tied to the feature being patterned. In a fill pattern, however, we don’t need the datum plane at all. We could even ungroup this current group and pattern the revolve feature all by itself. Instead, we will simply pick on the Revolve 1 feature in the model tree and then click on the pattern tool. When the dashboard appears, switch the pattern type to Fill, as shown in the next figure.

When we do this, the dashboard will change to look like the following.

We must start by defining the fill boundary. If we needed to sketch a boundary, we could right click in the working window and use the Define Internal Sketch option. Instead, we will pick on the sketch feature on the model. NOTE: If you are going to use a pre-defined sketch (as we are in this example), it must come before the feature being patterned in the model tree. This is because the model is rolled back to the time just before the feature was created for the pattern. When we pick on the sketch feature, we will see the following in the model. Go to a BOTTOM view for the rest of this example.

A grid of black circles appears on the model. This is the preview for the pattern. In the dashboard, we have a variety of options to chose from for defining the shape of this pattern. The first field to the right of the sketch definition is the shape of the pattern. The default is Square, which gives you the effect above. There are other shapes, such as Triangle, Diamond, Circle, Spiral, Curve, etc. that give you different results. Try each one until you find the one you want. In our example, we are going to stay with the Square option. The next field to the right is the spacing between instances. We are going to change this value to 0.750. The next field is the distance from the boundary that we sketched/selected. We will use a value of 0.300 for this fill. The last field is used to rotate the entire grid about the lead instance. We will use a value of 57.000 degrees to line the suction cups up with the long angled edge. The dashboard, when completed will look like the following.

The preview of the pattern will look like the next figure.

If we wanted to remove one or more of the instances from the resulting pattern, we would click on the black circle and turn it white. We, however, are going to keep each of these instances. When we click on the green check mark, each of the instances will regenerate, and then we will be left with our final pattern, as shown in the next figure.

Save and close this model.

TABLE PATTERNS The next pattern type that we will look at is the Table Pattern option. We will demonstrate this functionality with the Plate3 model, which looks like the following.

We are going to start by picking on the hole and then select the pattern tool. When the dashboard appears, change the pattern type from Dimension to Table, as shown in the next figure.

When we do this, the dashboard will look like the following.

The first thing we must do is select any dimension we want to control in the table. I find it best to pick them in the order you want to see them in the columns of the table. Therefore, we will pick the 0.625 “x” dimension, followed by the 0.750 “y” dimension, and lastly the 0.750 diameter dimension. Once all three dimensions are selected, we will click on the Edit button next to the “TABLE1” field. This brings up the table editor, which will look like the following.

We can see four columns. The first is used to identify the hole by a unique incrementing number. The first hole that we selected represents “1”, therefore, we will start with “2” in the second row.

The remaining columns are our three dimensions that we selected, in the order in which we selected them. I always find it easier to sketch out the hole pattern on paper prior to filling out the table to make it easier to fill out. My sketch for this hole pattern might look like the following.

Using this information, I will fill out the table as follows.

Once the table is filled out, I will select File, Exit from the menu at the top of this window. This saves and exits the table. Back in the model, we will see the preview of this pattern, which looks like the following.

At this time, we could create more than one pattern table for this hole. The reason you might do this would be for different family table instances, or to try out different patterns until you know which one will work for you. We will click on the green check mark to complete this pattern. Our final model will look like the following.

Save this model for the next pattern type.

REFERENCE PATTERNING A reference pattern is a feature pattern that follows an existing pattern. In order to make this work, the feature you are trying to pattern must be tied to the lead feature of the existing pattern in such a way that it could be translated to each of the instances of that pattern. To demonstrate how this works in Wildfire 2.0, we will continue to work with the Plate3 model that we have open. We are going to add two features that will both be referenced patterned. The first will be an extruded thin protrusion. Start by going to the extrude feature, and be sure to select the solid and thin material options, as shown below.

Change the wall thickness to 0.125, as we can see in the above figure. Next, use your right mouse button to Define Internal Sketch. For the sketching plane, use the top surface of the plate, and accept the RIGHT datum plane facing towards the Right. Inside the sketch, use the “Use Edge” tool to select both halves of the lead hole (the one in the lower left corner), as shown in the next figure.

Once we complete the sketch, be sure to flip the material side to the outside of the hole, and change the depth to 0.25. The preview will look like the following.

Click on the green check mark to complete this feature, which looks like the following.

Now, select the extrude feature and then click on the pattern tool. Since this feature is already tied to the lead hole in the hole pattern, the default type listed is Reference, as shown in the next figure.

Click on the green check mark to complete this pattern, and our model will update as shown in the following figure.

Notice that the diameter was controlled by the hole pattern, so it got bigger around the center hole as it should. The next feature will be a round at the base of the extrude feature on the lead hole. The radius will be 0.05, as shown below.

Once you finish this round, select it in the model tree and click on the pattern tool. This time, the dashboard will not open. Instead, it will automatically pattern the round to all of the instances. Rounds and Chamfers do this automatically. The following figure shows the resulting model once the reference pattern is done.

LESSON SUMMARY Patterns are great tools to reduce the amount of repetitive work you might incur otherwise. You need to build in the proper dimensioning scheme so you have dimensions available to drive pattern directions, sizes, etc. In dimensional patterns, you define the instance spacing and number of instances. In table-driven patterns, you spell out exactly the location and size based off of references that the lead entity used. In a fill pattern, you sketch a boundary that the fill resides within, and then you indicate size, shape and orientation. To successfully group or reference pattern, all entities must be tied only to the lead feature being patterned first (or first in the group). If they reference stationary, nonmoving references, the pattern will fail.

EXERCISES Open up the Headset part that we have worked with in the past, and pattern the rib and all of its rounds, as shown below. The spacing for the ribs is 1.25 inches.

HINT: Since we have not learned how to create a group by combining already created features, you will not be creating one for this exercise. You will, however need to find out which feature drives the 1.25 spacing dimension and pattern that first.

Cup_Washer Create the part below.

Les son

2 0 0 Lesson Objective: In this lesson, we will learn about Variable Section Sweeps.

VARIABLE SECTION SWEEP DEFINITION A variable section sweep is an advanced sweep feature that, instead of maintaining a constant section shape and size along the length of the trajectory, is varying along the trajectory by specifying additional trajectories that push or pull the section as it goes.

CREATING A VSS (Variable Section) To demonstrate this functionality, we will open up the Variable_Section1.prt file, which initially looks like the following.

In this example, we are going to create a cut out of the block that is rectangular in shape, but changes size according to the datum curves/sketches that are on the model. To create a variable section sweep, click on the following icon in the Feature Toolbar.

This will open up the variable section sweep tool, and its dashboard looks like the following (with the References panel open).

By default, variable section sweeps start out as surfaces. Therefore, we will need to first click on the Solid icon (first icon in the dashboard). Once we pick on this option, select the Remove Material icon. Our dashboard should now look like the following.

We are now ready to start selecting our trajectories. One of the big differences in Wildfire 2.0 is that we don’t have to specify whether it is a curve or an edge chain. We can simply pick on the reference, and it will be smart enough to know whether it is valid or not. We will begin by picking on the origin trajectory. The first trajectory that we pick in a VSS feature is always treated as the origin. The best trajectory in our model to use as the origin trajectory is the dark blue straight curve on the top of the block. Therefore, we will pick on it. The model will highlight the curve, as shown.

There is a label on the curve that identifies it as the “Origin”. In addition, there are two dimensions and two yellow arrows. The two dimensions can be used to extend or shorten the trajectory for our origin even if the selected trajectory is longer/shorter. It does not change the length of the original curve, only the origin trajectory in this feature. The yellow arrow that is pointing down the trajectory is the start point. If we were to click on it, we could change the start point to the other end of the trajectory. The second yellow arrow is used to identify the Horizontal/Vertical orientation when no other trajectories are specified as the “X-Trajectory”. In a regular sweep feature, this would be used to help orient the sketch, as there is only one trajectory. Our References panel looks like the following.

We can see our Origin trajectory listed, and there is a check in the box in the “N” column, indicating that our section, when swept, will be normal to this trajectory. We could change the section plane control to Normal to Projection or Constant Normal Direction using the first pull-down field, entitled “Section Plane Control”. We will now start to pick our other trajectories. The order doesn’t matter once you select your origin, but for consistency, we will pick the next curve shown below as our second trajectory. Be sure to hold down the Ctrl key when picking this second trajectory – otherwise, you will re-select the “Origin”.

We can see that this trajectory is labeled “Chain 1”, and since it is currently active in the reference window, we can see the two dimensions used to extend/shorten it. We will now hold down the Ctrl key again, and select our third trajectory, shown below.

This trajectory is now labeled “Chain 2”. Hold down the Ctrl key once again, and select our fourth trajectory, shown in the next figure.

It is labeled “Chain 3”. We now have all of our necessary trajectories. Our References panel looks like the following.

We can see all four trajectories listed with their labels. We can also see a column entitled “X”. This column allows us to specify a trajectory from our list to act as our “X-Trajectory”. We will click in the check box for “Chain 2”, so it looks like the following.

When the check mark appears, you will notice that our Horizontal/Vertical control field has changed to X-Trajectory. This allows the application to automatically line up the Origin and the Chain 2 start points on the same horizontal when inside sketch mode. We are now ready to create our section. Therefore, we will click on the pencil and paper icon in the dashboard (just to the left of the “Remove Material” icon). This brings us into our sketch, which initially looks like the following.

The figure above illustrates the location of the different start points for these trajectories, based on the start point for the origin. It is upside down from how we were looking at it before, but that is okay, because we can always rotate the sketch to see how we are looking at it. We are going to sketch a rectangle that has corners that touch the end of “Chain 1” and “Chain 2”, and is controlled by the Chain 3 for its height, as shown in the next figure.

If we go back to a rotated view, we can see exactly where our section sits with respect to the trajectories.

When we click on the check mark to complete the sketch, we will see the profile of our VSS feature, as shown below.

The downward arrow in this preview indicates the material removal side. We will click on the green check mark to complete our feature. Our model now looks like the following.

CREATING A VSS (Constant Section) In this next section, we are going to see how to create a regular sweep using the Variable Section Sweep feature. To demonstrate this, open up the Variable_Section2 part, which looks like the following.

We are going to cut out a special lip around the front top edge of this part, but we only want it to be a certain location. Therefore, we will start by going into our variable section sweep tool. Make sure that you select the Solid and Remove Material options from the dashboard, as shown below.

Next, pick on the front, top edge so it highlights as shown in the next figure.

At the two ends of the highlighted edge, we can see the T=0.000 dimensions that allow us to extend or shorten the length of our trajectory. We will shorten the trajectory by 2” on each end, therefore, we will double-click on the 0.000 dimension, and change it to -2.0 for each end. The result is shown in the following figure.

Next, we will go to the dashboard and pick on the Options slide-up panel, and select Constant Section, as shown in the next figure.

We actually may not need to do this to get our final result, but I would get in the habit, because there may be a time down the road where this feature could fail, because it may be looking for more than one trajectory (Variable section option), and we only want a single trajectory (Constant section option). Now, we will click on the sketch icon, and when we are placed into sketcher, we will see the following.

The intersecting dashed lines represent the start of our trajectory (where the yellow arrow was). If you are not sure how you are looking at the part, you can rotate it, and then return to the sketch view after that. We will sketch four lines and dimension as shown.

When we finish our sketch, and rotate our model, we can see the dynamic preview (another advantage of using a VSS over a regular sweep, which currently does not have a dynamic preview).

The completed model looks like the next figure.

Had we needed more control over the end points of the trajectory, we would need to use the regular sweep feature and sketch our trajectory on top of the existing model edges. The following figure shows an example of a case where a variable section sweep would have to be combined with additional features to accomplish what a regular sweep would do.

LESSON SUMMARY The variable section sweep is a very powerful tool to take a standard swept type feature, and stretch and pull it in different directions by defining datum curves that the section will ride along. Be sure to create your datum curves ahead of time. If you happened to forget one, you could pause the feature and create one on the fly. Use the variable section sweep for regular swept features if you don’t need to add inner faces

EXERCISES Open up the basket part in our ProETrain folder. It should look like the following.

We want to create a surface variable section sweep at the top of the existing surface as shown below.

The section for the rim profile is a semicircle that is normal to the top rim of the existing surface as it goes around.

Les son

2 1 0 Lesson Objective: In this lesson, we will learn about Swept Blends.

SWEPT BLEND USAGE A swept blend is used when you must blend together several sections, but the path that the blend takes must follow a specific trajectory. It is sort of a combination between a general blend and a sweep feature. Unlike a variable section sweep, you can only use one trajectory, but you can vary the shape of the sections drastically along the trajectory, which you can not do with a variable section sweep. To demonstrate this, we will create the following swept blend protrusion.

We will open up the Swept_Blend.prt part file in our ProETrain directory. It will initially look like the following.

The trajectory will be the long, open ended sketched curve, and the three sections that we are gong to blend are indicated in the order in which we will pick them.

Like the General Blend, it is easier to select your trajectory and sections, although you have the ability to sketch them. For this lesson, we will select the entities.

CREATING THE SWEPT BLEND There is no icon on the feature toolbar for this tool, and like a regular sweep feature, you have to decide ahead of time what type of material condition are you creating (Protrusion, Cut, Surface, etc.). We will use Insert, Swept Blend, Protrusion from the menu bar, as shown below.

This brings up the following menu.

At the top of this menu, we will define how we are going to create the sections. By default, the option Sketch Sec is selected. We have already selected Select Sec in the figure above. This means that when we come to defining sections, we are going to select them instead of sketching them.

The options at the bottom are similar to the ones we have seen in the variable section sweep. These are: • NrmToOriginTraj – Normal to origin trajectory. We will only pick one trajectory with this option, which acts as the origin. Pivot Dir – Pivot Direction. Choose a datum plane or planar surface that the • sections will be perpendicular to along the length of the trajectory. Norm To Traj – Normal to Trajectory. In this option, you actually will pick • two trajectories, but the sections don’t follow both. One of the trajectories will be the one that the sections follow, while the other one determines perpendicularity of the sections. We are going to keep the first option by default, and then select Done. This will bring up the Swept Blend window, as shown below.

We can see that we are defining the origin trajectory. We have the following menu options that appear.

To sketch a trajectory, you would use the Sketch Traj option. We, however, want to select an existing curve or edge as the trajectory; therefore we will pick on the Select Traj option. This will bring up a menu giving us options for how to select the trajectory. We want to select the Curve Chain option, since we are picking on a sketched datum curve.

We will then select on the straight portion of the trajectory, shown with the bold red highlight in the figure below. When we do this, one of the ends of the trajectory will have a bold, blue arrow, indicating the start point.

We want to start at the other end, so we will click on Start Point from the menu. A smaller menu appears with the options Next and Accept. We want to click on Next, which will cause the vertex at the other end of the curve to highlight. We will then click on Accept to move the start point to this end, as shown below.

With the start point in the right spot, we will click on Done to move forward. We are now placed into a menu to select our sections.

We will keep the default option of Pick Curve selected, but at the bottom, we want to select Sel Loop, which will let us pick the entire closed loop of curve segments that make up the section. We will then pick on the bottom edge of the first section. When we do this, the entire first curve highlights, and a start point arrow appears. As in all other blends that we have talked about, we want to make sure the start point is in the same location on all of the sections. There is a point on each of the sections that never changes, and that is the one that lies on the trajectory. Therefore, we want our start point to look like the figure below.

Once it looks like the figure above, click on Done. We see the same menu again, and we want to pick the same options. This time, we will pick on the bottom edge of the second section, and make sure our start point arrow is on the point that lies on the trajectory, as shown below.

Click on Done for this section once it looks like the figure above. In the message window, we are asked if we want to continue selecting sections. We will enter Y. For the third section, we will still use the Sel Loop, and we will pick on the flat edge. When we do this, the start point shows up on the following vertex.

We want to switch the start point to be on the other end of this edge, so it lies on the trajectory. Therefore, we select Start Point from the menu, and then pick on the opposite vertex for this straight segment. It will now look like the following.

BLEND VERTEX If you look at the first two sections, there are four entities that make up these. There is a straight edge on the bottom, two edges on the sides, and an arc at the top. This third section only has two entities, the straight edge at the bottom and the arc at the top. We must have the same number of entities for this to work, so we will create two blend vertices. A Blend Vertex is a selected vertex on the section that will force two vertices from the previous section to blend into this one. Since we are eliminating the

two side edges from the third section, we need to have the vertices from these edges in section two blend into a single vertex in section three. So, we will pick Blend Vertex from the menu, and select the two endpoints of the straight segment. When we do this, a large circle appears around the vertex, as shown below.

Once we have done this, click on Done. At the prompt to create additional sections, type in N. We can now click on OK to complete this feature, as shown below.

There were two other options in the Swept Blend window. These were. Blend Control – Specify how the blend will be controlled. You can create • an area graph specifying the exact smoothness of the blend. You can also ask it to create more of a linear blend. The default blending method usually gives good results, so we didn’t have to define other options. Tangency – If you have existing geometry at the ends of the trajectory, you • can specify whether the swept blend should be tangent to these entities. This is very useful if doing this as a surface feature. Since we don’t have any other features in this model, we don’t need to define this option.

LESSON SUMMARY A swept blend is a great tool to use if you must blend together multiple sections, and control the shape between the sections by a trajectory. You can select or sketch the sections and trajectory, but it is often easier to select. Remember to check your start points and number of entities. Create blend vertices where necessary.

EXERCISES

Open up the Swept_Blend2.prt part file, and create a swept blend cut around the bottom rim of the part, as shown below. Use the outside edge as the trajectory, and use the existing datum curves as the sections.

Les son

2 2 0

Lesson Objective: In this lesson, we will learn about the Boundary Blended Surface tool.

BOUNDARY BLEND SURFACE USAGE None of the tools that we have used so far would help you take boundary curves to define a surface, and internal curves to control the shape across the boundaries. This is what a boundary blended surface is all about. To demonstrate this, we will open up the following part (Boundary1.prt)

We are going to create a new surface by blending the outside curves together, but using the internal curves to define the shape. DIRECTION CURVES When you define boundary blend surfaces, you define curves or edges in one or two directions. It doesn’t matter what you consider the first or second direction, as long as you keep track of it yourself. In our example, we are going to consider the following directions, and curves in those directions.

CREATING THE SURFACE To create a Boundary Blended Surface, click on the following icon in the feature toolbar.

The dashboard for this feature looks like the following figure. The fields at the bottom are not labeled, but they are used to pick curves in the first, second and approximate directions.

The first direction curve field is currently highlighted in yellow, meaning that it is active. We will select the first and third curve in the first direction, as shown below. NOTE: Use the Ctrl key to select both of these.

Once we select these, the first field at the bottom will say 2 Chains. We can see a plane highlighted, and we can also see two circles with little symbols in them. We will discuss what these mean a little later. Now, we will click in the second direction field, and select the first and third curves in this direction, as shown in the figure at the top of the next.

If we look at a full preview, and rotate the model, we can see that our surface does not intersect the two curves in the middle of the part, as shown below.

Click on the full preview button again to return to the feature definition. We are going to pick on the Curves slide-up panel. It will look like the following.

As you can tell, this panel is used to define the first and second direction curves. Currently, we are active in the second direction, so we will pick in the first field to activate first direction curves. We are going to hold down the Ctrl key and pick on the second curve in the first direction. It will appear in this panel as the third chain on the list.

On the model, the dynamic preview has disappeared, because it can not build the surface in the order the curves were picked. We need to move the new curve to the middle of the list so it acts as if we picked it second instead of last. To do this, we will select on the 3 Chain item so it becomes highlighted, then select the up arrow that appears, as shown below.

As soon as we do this, the dynamic preview appears again, as shown below.

Now, repeat this process for the second direction curves. We are going to hold down the Ctrl key and select the middle curve in the second direction, then repeat the process of moving it up the list so it becomes the second curve listed. When we do this, we can see the preview for the final surface, shown at the top of the next page.

We will now accept this surface, and it will look like the following.

If you rotate the model, you will find that it goes through all of the curves.

EDGE ALIGNMENT AND ADVANCED OPTIONS One of the more common options you will adjust in boundary blended surfaces is edge alignment (boundary conditions) and advanced options (edge influence). To demonstrate this, open up the Boundary2.prt part file. It will look like the following.

Constraints If you recall from the last section, on each selected boundary curve, there is a white circle with markings in it. These circles are used to identify and define the boundary conditions (constraints) that exist. There are four possible constraints to choose from. They are shown in the following figure.

When selecting constraints, you should be aware which surface(s) is being referenced, as it will determine whether the condition can be satisfied. In our current model, we are going to create a surface that will connect these two sides and then adjust boundary conditions to get the final result. To do this, we will go back into our boundary blended surface. For the first direction curves, we will pick the top edges of each side, as shown below.

We don’t have any side curves to define a second direction, but that is okay. The problem that we have right now is that it is a flat surface connecting the two edges that we selected. We actually want the surface to be tangent to the existing surfaces. Therefore, we will define edge alignment (or boundary conditions). When we click on the Constraints slide-up panel, we see the following.

It lists the first and last curves/edges selected in the first direction. Currently, the boundary condition at both of these sides is “Free” or in other words, no condition is set. When we pick on one of the edges in the panel, the adjacent surface highlights in an orange outline, as shown in the following figure.

We are going to change, for both edges, the boundary condition from Free to Tangent as shown below. We can do this directly in the slide-up panel, or by rightclicking on the circle on the model.

The surface to which the boundary surface assumes tangency will be listed in the field below. In many cases, it will assume a surface that shares the edge selected, so we won’t have to change anything in this field, but you will want to verify this. As soon as we set the tangent conditions for both edges, click on the “Display drag handles” check box, and our dynamic preview will update to show the result.

For each of the tangencies defined, there is a dimension that appears on the model. This dimension determines how far from the edge into the surface does the tangency exist. The larger the number, the more domed the surface will be. The smaller the number, the flatter the surface will be. We will change these values to both be 1.5, which gives us a nice dome, as we can see from the side.

SIDE CURVE INFLUENCE Now that we have a nice dome to our surface, we can still see that it looks a little strange. We don’t have a tangency condition with the sides of the original surfaces. This is really evident from a TOP view. Therefore, for both edges, we will click on the “Add side curve influence” option at the bottom of our Constraints panel, as shown in the next figure.

The model now looks like the following.

This is exactly what we wanted to accomplish for this surface. We will accept this surface, and the model will look like the following.

CONTROL POINTS The last thing we can define in a boundary blended surface is any control points. To demonstrate how this might make a difference, we will open up the Boundary3.prt file, which looks like the following.

We will create a boundary blended surface by selecting the left curve and the right curves in the first direction. The initial surface will look like the following.

We can see from the figure above that Pro/ENGINEER must create internal surface edges to blend these two curves together. This isn’t necessarily a bad thing, but the more internal surface edges you have, the less smooth the blend will be. If we were to perform a full preview, and rotate the model, you would see shadows all across this surface, indicating high and low spots. These spots occur where the internal surface edges are. We will try to reduce the number of internal edges, thus performing a better blend. To start, we will open up the Control Points slide-up panel, which looks like the figure below.

In the Sets section, we can see that we are defining a control point set. In the field to the right, we will pick on the top-most Undefined. When we do this, our model will highlight the first curve we selected, and place red “X’s” where there are internal vertices, as shown below.

We can see four vertices, but only two of them are internal to the first curve. We aren’t going to worry about the outside points, because they connect directly up to the endpoints on the second curve. We are asked to select one of the vertices from this first curve. We will select the topmost internal vertex, as indicated in the figure above. When we do this, the second curve will now highlight with its internal vertices.

We will select the vertex on the second curve that is approximately opposite the one we just selected on the first curve (as shown in the previous figure). When we do this, the top two internal edges become a single internal edge connecting the two, and we can now pick a second set of points, starting with the vertex shown below.

Once we pick the first vertex for the second set, the second curve will highlight, and we will pick the corresponding point on this edge, as shown below.

When we do this, we will see the bottom two internal edges replaced by a single internal edge, as shown in the next figure.

We do not have any additional internal curve vertices to select, and our Control Points panel looks like the following.

We will finish out of this boundary blend surface, and our model will now look like the following.

CURVATURE CHECK Under Analysis, Geometry, Shaded Curvature, we have the ability to select all three surface pieces to perform a Gaussian curvature check. If we were to perform a Gaussian curvature analysis on the original surface before we added the control points, and compare that to the same analysis on the newly reformed surface, we would see a big difference in the smoothness, as shown in the following two figures.

ORIGINAL SURFACE

NEW SURFACE

As we can see, there are ups and downs in the curvature of the first surface (it goes from magenta to red to green to blue to green again to yellow to red again to yellow again then to green again). In the second surface, there is a continuous curvature change (it goes from magenta to red to yellow to green to blue). This is a much cleaner and smoother surface, and will result in a more appealing product when light shines on it.

LESSON SUMMARY

Use a boundary blended surface to create a single surface connecting curves in one or two directions. Use or create internal curves to help define the shape between the boundaries. Always be aware of existing boundary conditions. You want to make sure you are normal or tangent to entities that touch the surface to give you the smoothes transition. Try to reduce the number of internal edges that result from the blend by using control points. The fewer the edges, the smoother the surface will be.

EXERCISES Open up the Boundary4 part file and turn shading on. Notice that our surface does not look smooth across the center. It has seam lines.

The model tree for this part looks like the following:

We will need to edit the definition of the feature called MAIN_SURFACE and adjust boundary conditions. HINT: Since this surface was created by itself, then the model was mirrored twice to form the full part, you will not be able to use tangent. Try one of the other boundary conditions. The final result should look like the following.

Les son

2 3 Lesson Objective: In this lesson, we will learn about the Copy & Paste Tool.

COPY & PASTE USAGE The Copy & Paste Tool is used to do the following things: Surface Copy – Make a quilt surface from a set of selected solid or existing • quilt surfaces. Surface Transform – Translate or rotate a copy of an existing quilt surface. • Composite Curve – Create a new curve from the combination of existing • stand-alone curves or edges. This was covered in Lesson 10 – Datums Part 2. Feature Copy/Move – Copy a feature with new placement references, • translate or rotate the copy as needed. In the next sections, we will show how to use the new Copy & Paste for each feature/operation listed above (with the exception of Composite Curves)

SURFACE COPY The surface copy creates a new surface quilt by copying existing solid surfaces or quilt surfaces. To demonstrate this functionality, we will open up the part called Copy_Paste1, which will initially look like the following.

We are going to copy some solid surfaces to make a single quilt surface. To make selection easier, change your selection filter in the lower right corner of the working window to Geometry instead of Smart. We will now select the following four surfaces using the Ctrl key to select them all at the same time.

Once all four surfaces are selected, you can use Edit, Copy or just use Ctrl-C on your keyboard to copy the four surfaces. Next, use Edit, Paste or just use Ctrl-V on your keyboard to paste the new surface. It will open up the Copy Surface dashboard, and you should see a preview of the new surface in yellow, as shown below.

In the dashboard, if you click on the Options slide-up panel, you will still have the ability to exclude internal loops or fill holes, or even copy just inside a selected boundary. The following shows this panel.

Click on the green check mark to complete this surface copy, and you will now see a surface sitting on top of the existing geometry, as shown in the next figure.

We will continue with this same part for the next operation.

SURFACE TRANSFORM

You use the Copy & Paste tool to move or rotate surfaces as well. NOTE: You must have the surface feature first to rotate or translate it. Start by changing the selection filter to Quilts to make sure we are only selecting the surface that we just created in the previous section. Once this surface is selected, use Ctrl-C to copy it into the clipboard. Next, go to the Edit menu, and you will see two Paste commands: Paste and Paste Special. If you just used Paste, it would make another copy right on top of the existing quilt. To get to the Move or Rotate options, you must use the Paste Special. Therefore, we will select Paste Special. NOTE: Ctrl-V does not work for Paste Special – only Paste. Once we select “Paste Special” we see the following dashboard.

The first two icons determine what type of move operation you are performing. The default is Translate (just called Move in this feature). The second is Rotate. We will start by picking on the Rotate icon. We must start by picking on an edge or axis about which to rotate. We will select the short edge at the end of the revolved surface, shown highlighted in red in the next figure. When we do this, a default angle of 0.000 appears on the model, as shown.

We will enter a value of 270.00 for the angle, which will put it in the correct orientation for what we want. The next figure shows this rotation.

Before we move this surface over to the other side, we will open up two of the different slide-up panels. The first is the Options panel, which shows the following.

Since this is a surface copy, it actually will keep the original copied surface intact. By default, it hides the original geometry so it appears as if it was just a move/rotate. If you wanted to see the original surface, just uncheck this option. We will leave it hidden. Next, we will look at the Transformations slide-up panel, which looks like the following.

We can see that we have defined our first move (Move 1) as a Rotate with an angle of 270.000 degrees. To create our translation, we will now click on the New Move option, and then change our pull-down to Move. For our Direction Reference, pick on the edge shown highlighted in the following figure.

Enter a value of 6.000 for the translation amount, and it should preview in the correct location. NOTE: If you have to, enter a -6.000.

Click on the green check mark to complete this surface transform. Our model now looks like the following.

In our model tree, we can see the difference in a Surface Copy versus a Surface Transform, as shown in the next figure.

Save and close this model for now – we will come back to it in a later topic.

FEATURE COPY/MOVE The final Copy & Paste operation that we will show is how to copy an existing solid feature and re-use it in a new location. To demonstrate this, open up the model called Copy_Paste3, which looks like the following.

We are going to copy the Extrude 2 feature. When we select this feature in the model tree and then use Ctrl-C, we will go to the Edit menu and see that we have Paste and Paste Special, just like we saw earlier. We will start with a Paste command, which kicks us into the dashboard for an Extrude 3 feature, as shown in the following figure.

All of the definitions are identical as the Extrude 2 feature, except for the placement. We will start by right clicking in the working window, and select Edit Internal Sketch. When we do this, the Sketch window appears as follows.

We have to re-select a new sketching plane and Horizontal/Vertical reference. We will click on the top surface of the model where the Extrude 2 feature is. When we do this, accept the default H/V reference of RIGHT facing towards the Right. Click on the Sketch button to get placed back into sketch mode. Inside the sketch, we will see an outline of the feature as if we had brought in a saved sketch. The only difference is we don’t have the scale or rotate options as we have with a saved sketch. We will place this new sketch approximately next to the existing feature, as shown in the next figure.

Click with the left mouse button to place the sketch. Dimensions will appear on the model. The dimensions for the sketch itself will be the same as the first feature. The only two dimensions we will change are the locating dimensions, circled in the following figure.

Once your dimensions are the values shown above, click on the blue check mark to get out of sketch mode. This brings us back to the Sketch window, where we will click OK. We will now see the preview of the feature. Click on the green check mark to complete it. Our model now looks like the following.

Now, we are going to demonstrate the Paste Special option. Therefore, re-select the Extrude 2 feature in the model tree, and then use Ctrl-C to copy it. Next, go to Edit, Paste Special menu option. When we do this, we get a window that pops up with three options, as shown in the following figure.

The following options are: 1. Make copies dependent on dimensions of originals. This places the feature right on top of its existing one. If you use Edit Internal Sketch, it will break the dependency on the first one. 2. Apply Move/Rotate transformations to copies. This will allow you to change the location of the feature and rotate it as well as you are copying it. 3. Advanced reference configuration. This brings up a window that shows all of the references used for the first feature to reroute the new copy that you are making. We are going to select the “Apply Move/Rotate transformations to copies” option, as shown in the previous figure, and then click on OK. When we do this, we can see a bounding box representing the new copied feature, as shown below.

This brings up the transform dashboard that we saw earlier, as shown in the next figure.

We will start by selecting the Rotate icon, and then turn on the datum axes. We will select the A_10 axis at the center of our Extrude 2 feature. When we do this, enter a value of 60 for the rotation angle. Our model should look like the following at this time.

Next, go to the Transformations slide-up panel, and click on the New Move option. We are going to use a “Move” (translate) option this time. For the reference, we are going to select on the bottom edge of our top surface and enter a value of -0.625. Our Panel looks like the following.

And our model – showing the selected edge looks like:

Now, we are going to click on the New Move option again, and this time pick the right edge of the top surface and translate the object 1.5 inches. The model should look like the following.

Our panel looks like the following.

Click on the green check mark to complete this feature. The model will look like the following.

On your own, edit this last feature, and change the horizontal dimension from 0.625 to 0.75 and regenerate the model. Save and close.

LESSON SUMMARY The Copy & Paste tool is used to create copied surfaces, transformed surfaces, composite curves, and to copy and move existing solid features. NOTE: You can also get to feature copy/move operations through Edit, Feature Operations, Copy.

EXERCISES Open up the model called Toy_Block, which looks like the following.

In the model tree, there is a feature called BLOCK, which is the overall square block. The second feature is called LETTER_A, which is an extruded cut that creates the rim around the block and the letter A itself. The goal for this exercise is to use the Copy and Paste commands to create the rest of the letters (B-F) for this block in the orientations shown in the following figure.

NOTE: You will need to edit the sketch to change the letter each time. Try to use an aspect ratio that centers the letter within the construction square surrounding it. When done, the model tree should show the names of the features that were added by copying the LETTER_A feature.

Save and close this model.

Les son

2 4 Lesson Objective: In this lesson, we will learn about the Fill Tool.

FILL TOOL USAGE The fill tool creates a 2D quilt based on a sketch. Fill surfaces are often used to help create surface models.

CREATING A FILL The Fill tool is the following icon on the Feature Toolbar.

To demonstrate this feature, we will create a brand new part called Fill_Surface from the Startpart_English template. Make sure your default datum planes are visible, and then click on the Fill tool icon in the Feature Toolbar. The following dashboard appears.

The only thing we have to do for this feature is define a sketch, either by selecting an existing sketch feature, or by sketching on-the-fly. We will use the right mouse button and select Define Internal Sketch, to sketch on-the-fly. For a sketching plane, use the TOP datum plane, and face the RIGHT datum plane towards the Right. Our sketch will look like the following.

When we click on the blue check mark to complete our sketch, we will see the preview of the surface in yellow.

Click on the green check mark to complete the fill surface, which now looks like the following.

That is all there is to creating a fill feature.

LESSON SUMMARY The Fill tool is very easy to use, and replaces the flat surface in 2001. Simply define your sketch and finish the feature.

EXERCISES

None

Les son

2 5 Lesson Objective: In this lesson, we will learn about the Merge Tool.

MERGE TOOL USAGE The Merge Tool is used to take two quilt surfaces and combine them into a single quilt – allowing you to trim away portions of the quilts that intersect each other.

USING THE MERGE TOOL The Merge Tool is located on the Feature Toolbar, and looks like the following icon.

This tool will only be active once two quilts are selected to merge together. To demonstrate this functionality, we will open the Funnel part. It should look like the following.

Before we use the Merge tool, we will add a 0.25” round to one of the surfaces, as shown below.

Once the round is created, our model should look like the following.

Now we will merge these two quilt surfaces together. To make it easier to select them, change the selection filter to Quilts, and then select one of the two quilts, followed by the second one using the Ctrl key. You may want to switch to a no hidden view to make it easier to graphically see what is selected, as shown in the next figure.

Click on the Merge Tool, which should now be active, and you may see the following.

Depending on which quilt you selected first, you may or may not have the same thing highlighted on your screen. In the previous figure, the yellow shaded portion is what will remain if you finish the merge. We can see that the incorrect side of the revolved surface is selected. Therefore, click on the appropriate yellow arrow to flip the side of the surface to keep. When we pick on the arrow that is pointing down in the above figure, it will now look like the following.

This is what we want, so we will pick on the green check mark to complete this merge. Our final model looks like the following.

NOTE: As you have already seen, the color of surfaces in Wildfire 2.0 is different from 2001. A pink surface edge is an open edge, while a purple edge is an internal edge. When merged, there will now be a purple edge between these two quilts where they intersect.

MERGE DASHBOARD The dashboard for the Merge Tool looks like the following.

You can see the two quilts selected. You can also see two arrows used in flipping the sides to be kept for both the first and second quilt. The Options panel looks like the following.

The Dynamic preview is very useful for seeing the difference between options, and to see if the selected option will work (you won’t see the yellow shaded surfaces if it fails).

LESSON SUMMARY The merge tool has a new interface, but it is the same tool that existed in 2001. The dynamic preview and ease of use of this new merge tool makes this tool better in the Wildfire 2.0 release.

EXERCISES Open up the Project_Exercise part. It will look like the following (from the bottom).

Merge these two surface quilts together to get the following model.

Save and close this model when done.

Les son

2 6 Lesson Objective: In this lesson, we will learn about the Trim Tool.

TRIM TOOL USAGE If you recall from Lesson 10 – Datums Part 2, we learned how to trim a curve using this tool. In this lesson, we will see how to trim surfaces using curves or other quilt surfaces as trimming tools.

USING THE TRIM TOOL The Trim Tool is located on the Feature Toolbar, and is very similar in appearance to the Merge Tool that we learned in the last lesson. It looks like the following.

To demonstrate the trim tool, we will open up the part entitled Trim_Surface, which looks like the following.

We are going to start by using the wavy surface to remove the top of the basket. Therefore, we will change our selection filter to Quilts to make picking surface quilts easier. Pick on the basket itself, as shown in the next figure.

Once the basket quilt is selected, your Trim tool should be available. Pick on this trim tool. When the dashboard opens up, pick on the wavy surface to use as a trimming object. The model will highlight the side to be kept, as shown in the next figure.

Obviously, this is the incorrect side to keep, therefore, we will click on the yellow arrow to flip it to the other side, so it looks like the following.

Currently our dashboard looks like the following.

Since we had to pick the quilt surface that was being trimmed first, the only reference we had to pick was the trimming object – in this case Quilt:F11, indicated in the field with the scissors icon next to it. The References panel shows us both quilts (the one to be trimmed, and the one acting as the trimming object), as shown in the next figure.

Finally, our Options panel shows us that we are going to keep the wavy surface when we are done.

We will uncheck this option, and then click on the green check mark to complete this trim. Our model will now look like the following.

We are going to create a second trim now using the circular projected curve. Therefore, pick on the basket surface once more, as shown in the following figure.

With the basket selected, click on the trim tool, and then pick on the blue circular curve. It will highlight, and the shaded preview will show what we are keeping, as shown below.

In this case, the preview is what we want, so we will pick on the green check mark to complete this model, which looks like the following.

Save and close this model.

LESSON SUMMARY The trim tool is used to trim away surfaces or curves using other geometry, such as points, curves, surfaces, planes, etc. as cutting tools. Select the side to keep and the trim operation will be complete.

EXERCISES Open up the Indexing_Surface model. We are going to use the wavy surface as a trimming tool to trim the cylindrical surface. The following figure shows this.

We do not want to keep the trimming surface when we are done. Our final model will look like the following.

Save and close this model.

Les son

2 7 Lesson Objective: In this lesson, we will learn about the Intersect Tool.

INTERSECT TOOL USAGE The intersect tool is used to create datum curves by either the intersection of two surfaces, or the projection of two curves/sketches. In Lesson 10 – Datums Part 2, we saw how to use two surfaces to make a curve, in this lesson, we will learn how to intersect two curves to make a new one, as well as making a curve at the intersection of a datum plane and solid model (similar to the Xsec datum curve).

USING THE INTERSECT TOOL The intersect tool is the last of the “similar” icons on the feature toolbar, and looks like the following.

This tool looks like the “Merge” and “Trim” tools, but have a slightly different shading of the objects. This one has the thick curve at the intersection of the dimmed circle and square

PROJECTION OF TWO CURVES/SKETCHES To demonstrate this intersection type, open up the Intersect2 part, which looks like the following.

To create this intersection, start by picking both sketch features so they are both highlighted in red, as shown below.

With both sketches highlighted, click on the Intersect tool. A new curve will appear at the “projected” intersection of both sketches, as shown in the following figure.

The original sketches are hidden, but still exist. To projection works by almost performing an extrude on each of the selected sketches, and where the extruded surfaces would meet would be the new curve. The following figure shows how this is working.

Save and close this model.

INTERSECTION OF PLANE AND SOLID GEOMETRY In Wildfire 2.0 and 2001, you have the ability to create a datum curve using an existing cross-section. In Wildfire 2.0, however, you can create a datum curve at the intersection of a datum plane and a solid model without having to have a created cross-section. To do this, we will open up the Intersect3 model, which looks like the following.

To create the intersected curve, start by picking on the FRONT datum plane, and then click on the Intersect tool. The plane will be highlighted, but we will still need to pick additional entities, as shown below.

Since we already have the datum plane selected, we will hold down the Ctrl key, and place our mouse over the solid model. Query through using the right mouse button until you see the entire model highlight in blue, and the words SolidGeom appear in the tool tip. Once you see this, click with the left mouse button to select the entire solid geometry. A preview of the curve appears on the model as we can see in the next figure.

Click on the green check mark, and our intersection curve is created.

This is a useful tool for setting up the model for a rib feature that lies on non-straight geometry. Save and close this model.

LESSON SUMMARY In Wildfire 2.0, it is very easy to create a datum curve at the intersection of two surfaces, projected from two existing curves or sketches, or at the intersection of a solid model and a datum plane. You must have your stand-alone curves/sketches before you can create the intersection of them.

EXERCISES Open up the Intersect_Ex part. It will look like the following.

This model consists of two sketch features. In this example, we are trying to make a surface, and all we know is that from the top it looks like the following:

And, from the front, it looks like the following:

Therefore, we created two sketch features that represent what we see from the Top and from the Front. We will intersect these two curves, then use the one on the TOP plane to extrude a surface. We can then use the newly created intersection curve as a trimming tool to remove the top part of the surface, leaving us with the following model.

Save and close this model when done.

Les son

2 8

Lesson Objective: In this lesson, we will learn about the Offset Tool.

OFFSET TOOL USAGE The offset tool is a very versatile tool. It can be used to create a new quilt surface by offsetting an existing solid or quilt surface. It can also be used to replace a solid surface with quilt surface.

Another use for this tool is to create an emboss on a solid or quilt surface by a defined shape. The last use of this tool that we will demonstrate is the ability to offset curves.

USING THE OFFSET TOOL The Offset tool is located on the feature toolbar, and looks like the following:

We will devote a separate section to each of the offset types.

SURFACE OFFSET The first type of offset we will demonstrate is one where either a solid surface or an existing quilt is used to create a new offset quilt. This is also known as a standard offset. To demonstrate this, we will open up the part called Offset_Standard. It looks like the following.

We will start by selecting the outside solid surface of this part, as shown in the next figure.

Next, we will click on the Offset tool. A preview of our new surface will appear on the model, as shown in the next figure.

We can use the yellow arrow to flip the offset direction. We will leave it going to the outside. The dashboard for this standard offset looks like the following.

The References panel lists the surfaces selected to offset. The Options panel shows us some additional options for the creation method of this offset, as shown below.

If we were to select the Controlled Fit option, then we would see the following additional items to specify.

We will leave it at the Normal to Surface option, and then click on the Create Side Surface check box. This adds surfaces to the sides of our offset surface, as shown in the following figure.

Go ahead and uncheck this box to remove the side surfaces. In our dashboard, we have another pull-down that defines the type of offset feature we are creating. By default, the Standard offset is selected. The different types are:

We will leave the type at Standard, change the offset distance to 1.0, and then click on the green check mark to complete this first offset feature. Our model now has a quilt surface as shown in the next figure.

EXPAND OFFSET Solid Surface Expand Working with the same model (Offset_Standard), we will use Edit Definition to go back into our offset feature. Once you are back at the preview, change the offset type to Expand. This changes the surface offset into a solid offset, because our surface was solid to begin with. The preview of this solid expand offset looks like the following.

When we click on the green check mark to complete this change, our model now looks like the following.

If we take the length of the edge of this part (from the center), we can see that it is 1.0” longer than it was before this offset feature. Close this model.

Surface Expand – Sketched Region The expand feature also doubles as a Tweak Offset (for both solids and surfaces). We will demonstrate this using the Offset_Expand model, which initially looks like the following.

This model consists of a surface quilt (boundary blend surface) and a sketched star on the TOP datum plane. We are going to offset the quilt within the star to make almost a punch out on the original surface. Therefore, we will begin by picking the surface quilt, as shown below.

Once this surface is selected, click on the offset tool. Change the offset dimension to 0.5, and our preview currently looks like the standard offset, as shown in the next figure.

Now, we will change the offset type to Expand. When we do this, the preview disappears, and the dashboard now includes an area where you will define a sketch, as shown below.

If you don’t have a pre-defined sketch feature, you can right click out in the model and select Define Internal Sketch. We, however, are going to pick the star-shaped sketch. When we do this, we will see the following.

If you rotate this model, you will see that the only offset area is within the star shape itself. It also automatically creates side surfaces. A FRONT view looks like the following.

We can see that the sides of this offset are going straight up and down. This is due to the fact that our offset is being defined as Normal to Sketch. We can see this if we open up the Options panel again.

We will change the option to be normal to Surface, and our preview will change to look like the following.

Click on the green check mark to complete this offset expand feature. Our model now looks like the following figure.

You could have done this same thing if the model were completely solid instead of surface quilts.

WITH DRAFT The next type we will show will use the same model that we just worked on (Offset_Expand). Start by using Edit Definition to go back into the offset feature again. We will change our type from Expand to With Draft. A new dimension will appear on the model, and our dashboard will look like the following.

Initially, the draft angle will be 0.000 degrees. Change this to 15.000, as shown above, and then our preview will update to show draft along the offset.

This is really useful, because it makes the draft hinge the bottom of the offset feature where it intersects the original selected quilt/solid surface. You also have the ability to add rounds, but I don’t recommend this, because you have no control over the radius for the round. Click on the green check mark to complete this change, and our model now looks like the following.

REPLACE SURFACE The next type of offset is used as a “Tweak Replace”. To do this, we must have a solid surface to replace, and a quilt that acts as the replacement surface. Therefore, we will demonstrate this with the Offset_Replace model, which looks like the next figure.

This model is shelled out, as we can see from a bottom view.

The model tree for this model looks like the following.

Before we create our offset feature, we will roll the model back before the shell. To do this, drag the red arrow in the model tree up until it is just before the shell, and then let go. The shell will go away temporarily, and the screen will indicate that we are in insert mode. The model tree will look like the following figure.

We are almost ready to create our offset replace feature. If you recall, we must have a surface quilt to use as a replacement surface. We want to replace the larger angled surfaces with the taller swoopy surface. Therefore, we will start by picking the following surface.

With this surface selected, use Crtl-C top copy it, and then Ctrl-V to paste it. This brings us into the surface copy mode, and we will click on the green check mark to finish the surface copy. We can now see a surface quilt on the model.

Now that we have our replacement quilt, we will pick on the first of the two solid surfaces to replace, as shown in the next figure.

We will click on the Offset tool, and we can initially see a standard offset, as shown below.

Change the offset type from Standard to Replace. When we do this, we can see the following dashboard.

We are prompted to select the quilt that acts as the replacement surface. We will pick on our newly copied surface. When we do this, our preview now looks like the following.

Before we finish this first replace surface command, we will go to the Options panel, and check the box to keep the replacement quilt, as shown below.

The reason we are doing this, is because we have to perform this operation for the back surface, and we don’t want to have to re-create our copied surface. Click on the green check mark, and we can see our first replace feature.

We can now select our back surface, and repeat these steps to create our second replace feature. For the second one, do not select the check box to keep the replacement quilt. When we create the second one, our model will now look like the following.

Now, drag the red arrow in the model tree back to the bottom to resume the shell feature. Our final model when viewed from the bottom will look like the following.

Close this model.

OFFSET CURVES The last offset functionality we will demonstrate is how to make offset curves. To demonstrate this, open up the part entitled Offset_Curves, which initially looks like the following.

To create an offset curve, select the curve to offset (in this case the straight blue projected curve on the right side of the model), and then pick on the offset tool. When we do this, we will get the following preview on the screen.

If you grab the white square (drag handle) and move the curve over to the left along the surface, you will notice that the curve remains on the surface at all times. We will drop it on the left side of the originally selected curve, and change the offset distance to 1.0, as shown below.

The dashboard for the offset curve looks like the following.

The first pull-down icon lets you select from three different offset types. The default is the “Offset Along Surface” option, which gives us the behavior that we have already seen. The three offset types are:

We will demonstrate each of these in upcoming sections. For now, we will click on the Measurements slide-up panel, which looks like the following.

Down in the lower left corner, there is another pull-down icon. The different options are:

Pictorially, the different options would give you the following result.

As we can see from the above figure, the option you choose will change the resulting curve drastically. We will leave it at the default of “Distance normal to curve/sketch”. Close the Measurements slide-up panel. Offset Normal to Surface In the dashboard, change the type to the “Offset normal to surface”. Rotate the model so you can see that the preview of the resulting curve now sits below the surface. Flip the arrow to place it above the surface at the same offset distance of 1.0, as demonstrated in the next figure.

NOTE: When creating an offset normal to surface, it is possible that not all segments of the selected curve/sketch will be created in the same offset feature. If this happens, you will need to split up your initial sketch into several and offset each segment individually. Fan Offset A “Fan Offset” occurs when you have two curves/sketches on the same surface, and you want to create curves between these – transitioning from one shape to the other at equally spaced intervals. We will change our offset type to the “Fan Offset”. When we do this, our dashboard looks like the following.

We have already selected our first curve/sketch to offset, now we are prompted to select the second curve/sketch. We will pick on the wavy curve on the left side of our surface, as shown in the next figure.

After we select this curve, we still need to define the offset direction. To do this, we must first click in the white field with the words “Click here to add…”, and then select a datum plane that is parallel to the offset direction.

We will turn on our datum planes and select the FRONT plane. When we do this, we will see the following preview.

Currently, the last field in the dashboard, labeled “23” represents the total number of curves to be created between our selected curves. The default value is 1, which is what we see on our model. Change this value to 50, and then click on the green check mark once you see the preview to finish this offset curve feature. Our resulting model will look like the following.

We can see that the curves start with the straight line and slowly develop into the wavy curve at the end. Close this model when done.

LESSON SUMMARY The Offset tool combines several different 2001 features into a single interface, controlled by what is initially selected (solid surface, quilt surface or curve).

EXERCISES

None

Les son

2 9 Lesson Objective: In this lesson, we will learn about the Solidify Tool.

SOLIDIFY USAGE The solidify tool is used to create a solid protrusion or cut by using a quilt surface. You would use this method to create a solid model from a set of closed surfaces that are completely merged together.

USING THE SOLIDIFY TOOL The Solidify tool is located on the feature toolbar and looks like the following icon.

It will only become available when a quilt surface is selected. To demonstrate this tool, we will open up the Copy_Paste1 part that we worked on in Lesson 23. It currently looks like the following.

We will start by selecting Quilts in the selection filter, and pick on the surface feature on the model, as shown in the next figure.

With our quilt selected, we will now pick on the Solidify tool in the feature toolbar. Our model will look like the following.

The dashboard for this tool looks like the following.

Across the bottom, from left to right, are the following icons: Create solid volume from quilt • Remove material using quilt • Create patch surface using quilt • Flip side of quilt to create feature • Since our edges of our quilt lie on the solid volume surfaces, it automatically assumes we want to create a patch. We could use this if we wanted, and would end up with the correct model. For demonstration purposes, however, we will pick on the “Remove Material” icon. When we do this, our preview looks like the following.

Since the shaded yellow volume represents what we will be left with, our arrow is obviously facing the wrong direction. Therefore, click on the yellow arrow or the “Flip” icon in the dashboard to point it in the opposite direction. Our preview will now look like the following.

This is what we want, so we will click on the green check mark to complete our feature. The model now looks like the following.

Save and close this model.

LESSON SUMMARY The solidify tool uses surface quilts to add, remove or replace solid volume.

EXERCISES Open up the model BBS1. It looks like the following.

The middle of this part is a boundary blended surface that is open on the bottom. We will need to add a Fill surface (Lesson 24) to the bottom of this quilt, and then merge the two together (Lesson 25) to create a quilt that we can use for this operation. NOTE: Because our quilt completely touches solid volume on its sides, we will not have to copy the surfaces in between the solid features. It will work fine as long as the quilt does not touch air around the model. The final model will look like the following.

Save and Close this model.

Les son

3 0

Lesson Objective: In this lesson, we will learn about the Thicken Tool.

THICKEN TOOL USAGE The Thicken tool is used to create a thin-walled protrusion or cut by adding thickness about a quilt surface.

USING THE THICKEN TOOL

The thicken tool is located on the feature toolbar, and looks like the following.

You must select a quilt surface before this tool will become active. To demonstrate the thicken tool, we will open up the BBS2 part. It looks like the following.

If you rotate this model, you will notice that these surfaces have not been merged yet. Therefore, that is the first thing we are going to do. Change your selection filter to Quilts and select both surfaces (using the Ctrl key). Once both surfaces are selected, click on the Merge tool. Flip the arrows as necessary until you see both sides shaded in yellow, as shown in the next figure.

Click on the green check mark and we will now have one large surface quilt. To clean up the display of the model, we will right click on the Style id 33 and Project 1 features in the model tree and select Hide to temporarily turn off the display of these features. When hidden, the model tree shows them with a gray box around the corresponding icon, as shown in the next figure.

The model will now look like the following.

With the Quilts filter still active, pick this entire surface so it highlights, as shown in the next figure.

Once this surface is selected, click on the Thicken tool. We should see the following.

IMPORTANT NOTE: Sometimes, the side to be thickened is not the one you want, and based on the default wall thickness selected by the program, one or more surface quilts may fail as it tries to thicken it. You will get a warning indicating that certain regions can not be thickened, and it will ask you if you want to exclude them. Say NO to this message. Then, you can adjust the thickness and flip the direction if necessary. If it still fails, then you may have to fix your model or adjust the wall thickness. For our model, the default side was the outside. We want to click on the yellow arrow to flip it to the inside, and change the wall thickness to 5.0. Our preview will look like the following when this is done.

If we were to open up the Options panel, we can see similar options to the Offset feature. After all, a wall thickness is very similar to an offset where the volume is added at the same time. The following figure shows this Options panel.

In the dashboard, we see an icon for adding material and one for removing material. In our example, we are adding material, but the process is exactly the same for removing material. Click on the green check mark to complete this feature, and our model will look like the next figure.

Save and close this model for a later lesson.

LESSON SUMMARY The Thicken tool is used to add or remove material uniformly about a surface quilt. Be careful not to exclude surfaces if it initially fails, because it might just be an issue with the thickness value or material side that results as a default.

EXERCISES Open up the Project_Exercise part that we have been working on. It looks like the following.

We will add a 0.25” round on the intersecting edge between the handle and the top, and then thicken the part to the inside with a wall thickness of 0.05”. The final model will look like the following figure.

Save and close this model for a later lesson.

Les son

3 1 Lesson Objective: In this lesson, we will learn about the Extend Tool.

EXTEND TOOL USAGE The Extend tool is used to extend the edge of a quilt surface by a specified amount. This would be used if you needed to merge two surfaces together that are completely touching all along the surface boundary.

USING THE EXTEND TOOL The Extend tool is located on the feature toolbar and looks like the following icon.

It can only be accessed if an edge chain of a surface quilt is selected. To demonstrate this tool, we will open up the model entitled Extend1, which looks like the following.

This model consists of a revolved surface quilt, and a swept surface quilt. We could have sketched the swept surface in such a way that it would have completely intersected the revolved surface, but for the sake of this lesson, we will leave it the way it is. The goal is to extend the edge chain of the swept surface, which is an arced surface, over to the revolved surface. The following figure shows the edge chain being selected.

Therefore, select the tangent set of edges shown in the next figure.

Once these edges are selected, click on the Extend tool. When we do this, we will see the following.

We will start by changing the dimension value to 1.375, which makes our preview look like the following figure.

The dashboard for our extend tool looks like the following.

Along the bottom, there are two icons. The first one is used to extend the surface along its current direction. This is the default. The second icon is used to extend up to a selected plane. Be careful when using this, because it takes the surface at the selected edge, and brings it straight over to the plane, normal to it the whole way. It does not merely extend the arced surface over to the plane. The following figure shows what this model would look like with this option and the RIGHT datum plane selected.

We will keep the surface extend type at the default for now. If we look at the Measurements slide-up panel, we see the following.

Down in the lower left corner, there are two options for how the distance is measured. The following figure shows these two options.

The following two figures show the difference between these options. Measure Distance in Reference Surface

Measure Distance in Selected Plane (TOP Plane Selected)

We will leave the default alone (in Reference Surface). We will now click on the Options panel, which looks like the following.

For the Method field, there are three options: Same (default), Tangent and Approximate. “Same” keeps the curvature of the original surface. This is what we have seen so far. “Tangent” extends the surface out tangentially from the edge selected. The following two figures show how these options differ (as seen from the BACK view):

Same

Tangent

As we can see, the curvature is kept in the “Same” option, but the extension goes straight in the “Tangent” option. We will leave the default of Same for this model. Click on the green check mark to complete this surface extension, and our model now looks like the following.

The final thing we will do is merge these two surfaces together to get the following model.

Save and close this model.

LESSON SUMMARY The surface extend tool is used to extend the edges of a surface by a specified amount and based on a specified method.

EXERCISES Open up the Extend2 model, which looks like the following figure.

The goal is to extend up the “U” shaped surface and merge it with the larger revolved surface. A wall thickness of 0.125” should be applied to the inside of the model. While extending, we want the top edge of the extension to remain tangent to the arced edge on the original surface being extended. The resulting model will look like the following.

Save and close this model.

Les son

3 2 Lesson Objective: In this lesson, we will learn about the Mirror Tool.

MIRROR TOOL USAGE The Mirror tool in can be used to mirror an entire part, or just a single solid, surface or datum feature about a datum plane or planar surface.

USING THE MIRROR TOOL The mirror tool is located on the Feature Toolbar, and looks like the following.

It becomes active when you select a feature or the model name from the model tree. To demonstrate this tool, we will open up the part entitled Mirror, which initially looks like the following.

On the inside of this model, there is a support rib. We want to mirror this rib about the FRONT datum plane, and then mirror the entire part about the RIGHT datum plane. The following figure shows this rib.

Therefore, we will find the RIB 1 feature in the model tree and select it (or pick it directly on the model). Once highlighted, click on the Mirror tool in the Feature Toolbar. The dashboard for the Mirror tool looks like the following.

As we can see in the above figure, the Options panel allows us to determine whether this mirror will be dependent (default) or independent on the originally selected feature. The only other thing we need to define is the mirroring plane. Therefore, pick on the FRONT datum plane. When everything is defined, the green check mark is now active. NOTE: When you select a solid feature to mirror, you will not get a preview option, nor will there be a dynamic preview. Click on the green check mark to complete this mirror, and you will see the following.

To mirror the entire model, we go to the model tree and pick on the MIRROR.PRT label at the very top. This selects the entire part file. The Mirror tool will now be active, and we will pick on it. In the dashboard, we no longer have the ability to pick on the Options panel, as the mirror feature is dependent when it is the entire model being mirrored. In the References panel, we can see the name of the part/feature being mirrored.

Now, we have to pick on the mirroring plane. We will pick the RIGHT datum plane. Unlike a solid feature mirror, an entire part mirror will have a dynamic preview, as shown in the next figure.

Click on the green check mark to complete this mirror feature.

NOTE: The sketch and datum curve features were hidden in the model, but appear on the mirrored side. This will be true of surfaces and all other datum features. To hide them, you can either hide the Mirror feature (which will only hide non-solid geometry) or add the Mirror feature to a layer and hide it. Save and close this model.

LESSON SUMMARY The mirror tool allows you to mirror the entire part, or a selected feature. You will not see a preview if you select a solid feature to mirror.

EXERCISES We are going to go back to several models that we created or worked on in earlier lessons and mirror the entire model to get the final part. Save each one before closing. Funnel In this model, we will end up with the following surface model. NOTE: To turn this into a solid part, you would have to merge the four surfaces together.

BBS2

Project_Exercise

Extend1 For this model, we will mirror the surface model first, and then add a 0.25” round along the two outside rims. Thicken this model to the inside with a wall thickness of 0.125”. The final model will look like the following:

Les son

3 3 Lesson Objective: In this lesson, we will learn about Layers.

LAYER USAGE Layers are used to organize information in the model. Typically, layers are used to group specific types of datum entities, such as planes, axes, curves, points, etc. Layers can be shown or hidden to help organize and clean up your working environment. Layers are not like AutoCAD in the sense that they are controlled by colors, or affect printing of certain model entities, although in drawing mode, layers can be used to turn off entities that will then not print.

WORKING WITH LAYERS The Layers tool is located on the System Toolbar, and looks like the following.

Hide Layer: To demonstrate layers in Wildfire 2.0, we will open up the Assembly1 assembly. It will look like the following.

We will be learning about Assembly mode in a later lesson. For now, the Navigator shows the Model Tree. If we click on the Layers tool, the Model Tree is replaced by the Layers interface, which looks like the following for this model.

Most of the layer functionality is carried out with the right mouse button. For example, turn on the visibility of datum planes. From the following figure, we can see how jumbled our model looks with all of the datum planes turned on.

In the Navigator, we can see a layer called _Defaults, which contains all of the default datum planes, datum axes and datum coordinate system. We will click on the “+” box to the left of the name _Defaults to expand it. Once expanded, there are four models listed under this layer – the assembly itself, and the three UNIQUE components that make up the assembly.

We will use the Ctrl key to select Component1, Component2 and Component3, and then hold down the right mouse button over any one of them. In the RMB menu, select Hide, as shown in the next figure.

Gray shaded squares appear around the icon for these three components, and when you click on the refresh button ( ), you will only see the default datum planes from the assembly, as well as any planes that are on the _PLANES layer.

We will now turn off the datum curve that resides in the Component3 model. Therefore, we go to the _Curves layer and expand it to see the single component that has this layer.

We will right click on that component and use the Hide command again. Refresh the model to see that the blue curve is no longer visible. Save Status To have the layer status changed for all components affected, you must first hold down the right mouse button over the Layers name in the navigator, and select Save Status, as shown in the next figure.

Then, you would save the assembly, which will save all changed components. Be careful, because in Pro/INTRALINK a “Save Status” will be treated as a modified object, and will need to be checked back in once you save. To return to the last SAVED status, you would click on Reset Status. Hide All Layers To hide all layers, you would right click on the word Layers and select Hide. This will gray out all layers, as shown in the next figure.

If you do this, use the Reset Status to undo this so we are back to our last status save (which only hid the _Defaults layer in the three components and the _Curves layer in the component3 model. Creating a New Layer To create a new layer, right click on the word Layers, and select New Layer, as shown in the following figure.

This will bring up the following window.

The first thing we want to do is to give this layer a name. We will call it FASTENERS, as shown in the next figure.

Now it is time to start adding items. Down at the lower portion of this window, we see two buttons: Include and Exclude. The default is Include, which means that anything we pick will be included in this layer, and subject to the status of the layer. Exclude is used to exempt added items from being subject to the status of the layer, but include them in the layer so we can change their status at a later time. The Remove button is used to completely take an item (whether included or excluded) off the layer permanently. We will keep the default of Include, and select the four screws, as shown in the next figure.

As we pick on the component, it will become added in our list with a green “+” in the status column, indicating that it is included, as shown in the following figure.

Once you are done adding items to this layer, click on OK to complete the layer, and it will show up in the navigator.

Now we could hide this layer, and all the screws on the assembly will disappear with the refresh button.

Layer Properties To get back into a layer definition to add/remove/exclude items, right mouse click on the selected layer, and pick the Layer Properties command, as shown in the next figure.

Once inside, we will click on the Exclude button, and select the last two components in the list. The green “+” status turns into a red “-“ status, as shown below.

If we had hidden this layer, these last two components would now be unhidden, even though the first two are still hidden. We will click on Cancel to undo this change. Remove Items To remove an item from a layer, you could go to the Layer Properties, select on the item in the list, and then click on the Remove button. The other way would be to expand the layer itself in the navigator, as shown for the FASTENERS layer.

We will remove the last component in the layer (C14). Select this component, and then hold down the right mouse button over it and select Remove Item, as shown in the next figure.

When you do this, you will get a confirmation, as shown below.

Click on Yes to remove this item from the layer. Now, if we were to hide this layer, one of the four screws is not going to be hidden. If we go back to the Layer Properties for this layer, we can see that it is no longer listed.

Changing the displayed component’s layers:

Currently, we have been looking at all of the layers for the assembly and any of its components. If we wanted to just look at the layers for Component3, we would use the pull-down field at the top of our navigator to change over to this component, as shown in the next figure.

Now, we can see and manipulate just the layers that exist in this component. Moving items from one layer to another To move an item from one layer to another, you can cut and paste the item. To demonstrate this, we will create a new layer for cross-section planes, and then move the XSEC_A_PLANE from the _Planes layer to this new layer.

Create New Layer XSEC_DTMS. First, we will right click over the word Layers, and use the New Layer option. When the window appears, enter XSEC_DTMS for the name, but don’t include any items. If you include the existing plane, it will now be in two different layers. The following figure shows us our new layer properties window.

Click on OK to get out of the properties. Now, we will expand the _PLANES layer to see the plane we want to move.

We will right click on the datum plane and select Cut Item, as shown in the next figure.

When we do this, it disappears from the navigator. We will now right click on the XSEC_DTMS layer and select Paste Item, as shown in the next figure.

A “+” box appears next to the layer, and if we expand it, we can see the item now in this layer.

Now, we could go back and delete the _Planes layer, since it is now empty.

LESSON SUMMARY The layer functionality is completely contained within the navigator, and works off of right mouse button commands (which are also available in the three tabs at the top of the navigator). Be sure to save your layer status before saving your assembly or part files.

EXERCISES None

Les son

3 4 Lesson Objective: In this lesson, we will learn about Parameters and Relations.

USAGE OF PARAMETERS & RELATIONS Parameters are attributes that exist in the model. These attributes can be used to search on in PDM/PLM systems, and are most commonly used to fill in drawing title blocks automatically. Parameters can also be used to drive dimensional information in relations. Relations are mathematical expressions that help you control your model. If you recall from the very first lesson, we talked about design intent and parametric modeling. Relations can be used to ensure that your model will react to change in a predictable manner. For example, suppose you always need your width of your block to be half the length. Instead of modifying two dimensions every time your length changes, you can write a relation that will automatically govern the width dimension.

PARAMETERS To access parameters, go to Tools, Parameters from the menu bar. To demonstrate this, we will open up the Assembly1 assembly that we saw in the last lesson. Once open, go to Tools, Parameters. We will get the following window appear.

The main portion of this window lists the current parameters and their values and properties in table format. You can edit many of the property cells directly in this table. To add a parameter, use the green “+” button at the bottom, and then fill in the information. To remove a parameter, select it in the table, and then use the red “-“ button. Along the bottom, there is a pull-down field and two buttons. The pull-down field allows you to look at the reported and alternate mass property parameters. The following figure shows the Alternate Mass Properties.

The following window shows the Reported Mass Properties.

These are system parameters that are derived from mass property calculations. Switching over to another part Currently, we are looking at the parameters defined in the assembly file. To view the parameters from a different model, or to look at component parameters, etc., we would use the pull-down field in the upper left of the model, as shown in the next figure.

We will select on Part, and then we are instantly placed into the working window to select the part from the model of which we wish to view the parameters. We will pick

on one of the screws to access Component3’s parameters. The window now looks like the following.

We can see the type as Part, and then name COMPONENT3 listed at the top now. Parameter Properties To view all of the properties in a single window for a selected parameter, use the Properties button in the lower right corner of the window. This would bring up the following window (shown for the APPROVED_DATE) parameter.

You can edit the data in this window as well.

Customizing the table The last icon in the lower right corner is used to customize the table display for this window. When you click on this icon, it brings up the following.

You can remove columns, reorder them, and change their size.

RELATIONS Relations are accessed in the Menu Bar using Tools, Relations. To demonstrate this, we will open up the Plate3 model that we worked with a while ago. It currently looks like the following.

Dimension Symbol Editing Before we add relations to this block, we should rename the dimension symbol for any dimension that is going into the relation so it makes more sense when viewing the relation later. For example the outer shape of the plate is currently a 10”W x 5”D x 0.5”H rectangular block. The dimension symbols for this are: d4 x d3 x d2. Unless you are very familiar with this model, you would not know which one of these is the height or the depth or the width. Therefore, it makes more sense to rename these to the following:

Current Symbol D4 D3 D2

New Symbol Width Depth Height

To do this, we will first go to the model tree and select the first Extrude feature. Once selected, hold down the right mouse button and select Edit. The dimensions for this block will appear on the model, as shown in the next figure.

Single click on the 10.000 dimension (Width) so it highlights in red, and then right click and select Properties. This brings up the following window.

This is the Dimension Properties window, which can be used to change tolerances, edit the text, change text style, change dimension type (basic, inspection, etc.), and change dimension symbol. We are going to go to the second tab, entitled Dimension Text, and then edit the Name field value from d4 to Width, as shown in the next figure.

Click on OK, and then repeat this for the other two dimensions. Be sure to rename the 0.5 dimension to Height (from d2), and the 5.0 dimension to Depth (from d3). We are also going to rename the hole dimensions as shown in the next figure.

Once all of your dimension symbols are renamed, we will create some relations so all we have to modify is the width of the block and everything will update.

Go to Tools, Relations, and you will see the following window.

There is a default relation to calculate the MASS parameter based on a mass property calculation result. We will start a new line at the bottom, and then start to enter our relations. We are going to enter the following. Depth=Width/2 Height=Depth/10 These two relations will govern the size of the plate itself, always making the depth half the width, and the height 1/10th the size of the depth. Now, we will enter relations governing the X-Locations of the holes. X1_Location=Width/10 X2_Location=X1_Location X3_Location=Width-X1_Location X4_Location=X3_Location X5_Location=Width/2 This sets all of the small holes equally away from their closest edge, at a distance 1/10th the size of the width. The larger hole in the middle is placed at the halfway point along the width. Now we will enter the Y-Locations of the holes. Y1_Location=X1_Location Y2_Location=Depth-Y1_Location Y3_Location=Y2_Location Y4_Location=Y1_Location Y5_Location=Depth/2 This makes the small holes equally away from their closest edge, at a distance equal to the X-Location distance. The larger hole in the middle is placed at the halfway point along the Depth. Our final entries will govern the diameter of the holes.

Dia1=X1_Location*.75 Dia2=Dia1 Dia3=Dia1 Dia4=Dia1 Dia5=Dia1*2 This makes the diameters of the small holes ¾ the size of the X-Location distance. The larger hole is twice as large as the smaller holes. The relations window will look like the following figure when complete.

Had we not remembered the dimension names, we could have picked a feature from the model, and its dimensions would have showed up on the screen, as shown for the extrude feature.

The icons at the top of the relations window provide some additional functionality for testing the relation, reporting values, etc. We will click on OK and then regenerate the model to see the change. Our model now looks like the following figure.

Save and close this model.

LESSON SUMMARY Use Parameters and Relations to capture design intent and model attribute information. Remember to always rename dimension symbols that you wish to use in relations so that individuals reading the relations later have an idea of what you are trying to do with them.

EXERCISES Open up the Draft1 part that we worked on earlier. If you recalll, it has a pattern of ribs around the inside. Currently, there are 5 ribs equally spaced at 72 degrees. We are going to create a relation for this rib pattern that, based on the number of ribs specified, keeps the ribs evenly spaced around the center axis. Test your relation with a rib count of 10, as shown below.

Les son

3 5 Lesson Objective: In this lesson, we will learn about Family Tables.

USAGE OF FAMILY TABLES Family tables are used to capture “like” models – or models that typically only change in size or minimal feature definition from one part to another. A perfect example of a family table is a family of socket head cap screws. Each individual instance of the screw is only different from a dimensional or material specification. You can create multi-dimensional family tables (or what is referred to as nested family tables) that can capture a larger family of parts/assemblies. Until you are comfortable working with family tables, I would stick with single level family tables. An example of a nested family table would be to create an entire family of screws. At the top level, you would distinguish between head types (SHCS, FHD, HHD, etc.). Then, at the second level, you could break each of these into dimensional and material types.

PREPARING THE MODEL

To demonstrate this functionality, we will open up the model called Mounting_Rail, which looks like the following.

The goal for this lesson is to be able to make different sizes for this mounting rail, and yet maintain a proper slot spacing and number of holes. Dimension Symbol Names As you learned in the last lesson (Parameters & Relations), you should rename any dimension symbols that are going to be used in Relations. The same is true for dimensions that will be used in family tables. In this example, we have already renamed the dimension symbols of the primary features used in both the relations (that we will see in a minute) and the family table that we will create. The following are some of the key symbol names: • Length – The overall length of the rail, which is currently at 10”. Size – The height of the rail (both sides are equal in size), which is currently 1”. • Radius – The radius of the inner fillet, which is currently 0.125”. • • Lead_Offset – The spacing from the left edge of the rail to the first slot. Spacing – The spacing between slots on the first slot pattern • Slotnum – The total number of slots in the first slot pattern • Slot_Length – The length of the lead slot • Slot_Width – The width of the lead slot. •

Relations Whenever possible, you should use relations before creating family tables. This is especially true if there is a ratio between two or more dimensions that should always exist, regardless of overall size of the model. This is the case in this model. The spacing of the slots is always 1”, regardless of the length of the rail. Therefore, we need to change the total number of holes when the length changes. To do this, we could have added the Slotnum dimension to a family table and controlled it there, but then we would have a lot of calculations to do each time we wanted a new size for our rail. Instead, we will do this with relations. The relations for this model can be found using Tools, Relations, as shown in the next figure.

The relation that controls the overall number of holes is the following: Slotnum=(floor(Length/Spacing)+1) What this does is first calculate the overall length divided by the spacing. For our current example, the Length=10 and the Spacing=1, therefore this equation results in 10/1 = 10. Then, it adds one additional hole, making a total of 11 holes. When the length of our rail is an exact increment of 1, such as 10, 11, 12, etc., then we always end up with one slot outside of the model. That is okay, because if our rail has a decimal attachment, such as 12.75”, then it will make a difference. Floor(Length/Spacing) always rounds the final number down to the nearest integer, therefore, if we have a length of 12.75”, then Floor(12.75) = 12. If we only had 12 slots, then we would have a large portion at the end of our rail that did not have a slot in it (or even a partial slot). Adding the 13th slot takes care of this. The last portion of this relation sets the dimensions of the second set of slots equal to the first so that the overall impression is that both are identical.

CREATING THE FAMILY TABLE To create the family table, go to Tools, Family Table from the Menu Bar. When we do this, it will bring up the following interface.

Currently, there are no instances created for this model. Across the top of this window is a toolbar. The first available icon is used to add instances (adding rows to the table). It looks like the following.

We will click on this icon five times in a row to create five different instances. When we do this, we will see the following.

Before we add any dimensions, features, parameters, etc. to our family table, we will change the names of our rails. We are going to create rails in 2” increments starting at 2 and ending at 10. Therefore, we will click in each cell starting with MOUNTING_RAIL_INST and rename them as follows:

We are now ready to start defining the items that vary from instance to instance. We will therefore click on the following icon to add columns to our table.

This brings up the following window.

Down at the bottom, you would start by selecting the type of entity you are going to add to the family table. In this case, the default is Dimension, which is what we will use. We will now pick out on the first extrude feature and then pick on the 10.000 length dimension. When we do this, it becomes added to our table, as shown in the next figure.

We will also pick on the 1.000 size dimension, and the 0.125 radius dimension. The following shows this window once all three dimensions are added.

We can see our modified symbol names listed next to the original symbol name. This makes it easier for us to identify which dimension is which. If we accidentally added a dimension that we didn’t want, we would highlight it and click on the button with the red “X”.

Next, we will add a parameter to our table. Therefore, click on the Parameter option at the bottom, and you will get the following window.

We will scroll down until we find the parameter called Title. Click on this parameter, and then click on the Insert Selected button at the bottom of this window. The TITLE parameter now shows up in our window, as shown in the next figure.

Click on the Close button to close out of the parameters window. We are done defining our family table. You can see in the above figure that we can add features,

groups, pattern tables, etc. to our family table, and we can also temporarily filter out what we are looking at by using the upper right corner of this box. Click on OK to return to edit the table. The table now has a column for each of the items that we added, in the order in which they were added, as shown below.

We will edit each cell with the values that we want. The following figure shows our completed table.

Once you have your table filled out, it is time to verify the instances. This is very important before you check them into Pro/INTRALINK. To verify the instances, click on the following icon.

This brings up the following window.

This window will list all instances, and show which ones have not been verified. Currently all five instances are “Unverified”. Click on the Verify button, and each one will be opened and regenerated behind the scenes. If all goes well, you will be left with a status of “Success” for each instance, as shown in the next figure.

If any fail, it will list that. You will then need to go back and fix the instance. The most common problem with a failed instance is a decimal point error while typing. Once all instances are successfully verified, click on the Close button. Back in the family table, we can preview our instances by highlighting the instance and clicking on the following icon.

The following figures show the preview for the 8” and 2” versions of our part.

8”

2” You can spin, pan, zoom, change display type, etc. while in the preview window. When you are done, click on the Close button at the bottom. Once you are happy with your family table, click on OK to complete the family table, and then save your model.

LESSON SUMMARY The interface for family tables is now more streamlined.

EXERCISES None

Les son

3 6 Lesson Objective: In this lesson, we will learn about the View Manager.

2001 EQUIVALENTS The View Manager is a single interface used to access the following functionality: Simplified Reps • • Cross-Sections Exploded States • Component Display •

ACCESSING THE VIEW MANAGER The view manager is accessed through the Menu Bar, using View, View Manager. To demonstrate this functionality, we will use the Assembly1 model that we worked with earlier. Open up this assembly, and then go to the View Manager. It will look like the following.

There are six tabs when you are in assembly mode (only three in part mode). The six tabs are for the following:

• • • • • •

Simp Rep – Access simplified representations Style – Access component displays Xsec – Access cross-sections Explode – Access Exploded States Orient – View the different saved views All – Create a combination of multiple view states (exploded with cross-section with simplified reps, etc.)

Each of these will be shown in a different section below.

SIMP REP The first one we will show is the Simplified Representation. A Simplified Representation is used to manage large assemblies. It allows you to create different “views” of an assembly by adding/removing components. A great example might be in the design of a car. A top-level assembly model of a car would have tens of thousands of components, and would require a supercomputer to open the entire model. In most cases, individual designers and engineers are only tasked to work on specific regions of the car – electrical wiring harness, for example. With Simplified Reps, you can create a representation that would only include the wiring harness and any other components necessary to define/redefine the harness. The user only needs to open the rep to work on the model, and therefore doesn’t need the entire car assembly in session. The really nice thing about simplified reps is that you can eliminate a component that may be a parent or child of one that you need to keep in your rep, and it will not cause a regeneration failure. If a change needs to happen to the child in your rep, then it brings in the necessary parent components just for that change. To demonstrate Simplified Reps, we are going to create two different simplified representations. The first will be the fasteners only. The second will be the model with no fasteners. Therefore, click on the Simp Rep tab in the view manager, and you will see the following.

As you can see, there are several built-in representations. Currently, we are looking at the Master Rep, because it has the red arrow next to it. If we wanted to change over to the Graphics Rep, we would simply double-click on it. To create a new rep, click on the New button. The window will look like the following.

Type in NO_FASTENERS in the field provided, as shown in the next figure.

When done, it will become the active rep. Now, we will right-click on this rep and select Redefine. When we do this, it brings up the following window.

Our model tree will also update to look like the following.

If you notice, the default rep state for the assembly is shown as Graphics Rep. This is because we started this new simplified rep with the graphics rep active. We will make sure the Master Rep option is selected on the Include tab, and then pick on the assembly in the model tree. It will now look like the following.

Now, we want to exclude all of the COMPONENT3 models from our assembly. Therefore, we will click on the Exclude tab, and then pick on the COMPONENT3 files in the model tree. In the second column, we should see the word “Exclude” next to each one, as shown below.

Now, we will click on the green check mark button to accept this, and our model will now update, as shown in the next figure.

In the working window, we can see which rep is currently active by the following text:

Now we are going to create a second one called FASTENERS_ONLY, and exclude COMPONENT 1 and COMPONENT 2 from the assembly. All you should see when this one is done is the following.

Double-click on the Master Rep once again, and then close out of the view manager. Save the assembly, but don’t close it yet.

STYLE The next tab is entitled Style, and is used to create different graphical displays for your assembly. A good example is the car again. You might want to keep the outer body of the car to show how the wiring goes through the model. If you were in shaded mode, you wouldn’t be able to see the wiring harness through the body of the car. Therefore, you can create a style where the body of the car is in a no-hidden display, while your harness is shaded. Therefore, in the assembly, we will go to View, View Manager, and when this opens, click on the Style tab, which looks like the following.

We will click on the New button to create a new style, and enter Fasteners_Visible in the name field, as shown in the following figure.

Next, we will right-click on this style and select Redefine. This will bring up the next window.

We want to change the display of Component 1 and 2 to be in No Hidden mode, and put all of the fasteners in shaded mode. Therefore, we will click on the Show tab, and then select the No Hidden option, as shown below.

In the model tree, click on Component1 and Component2. The second column should now indicate this status change, as shown in the next figure.

Now, select the Shading option, and pick the four Component3 models in the tree. They now indicate their status, as shown in the figure below.

When we click on the green arrow to accept this change, our assembly will update (as long as we are not in shaded mode).

Double-click on the Master Style and then close out of the view manager. Save the assembly but do not close it.

XSEC The next tab we will talk about is creating cross-sections. Therefore, go to View, View Manager, and click on the Xsec tab, which will look like the following figure.

Click on the New button, and enter A for the name, as shown in the next figure.

When you click on the ENTER key, it replaces this interface with the menu manager, as shown in the next figure.

This is the old interface for selecting options for the cross-section. You can see we have the planar and offset types, just like we did in 2001. We will click on Done to accept the default options, and then the next menu shows up.

As we know from 2001, we now have the ability to pick an existing plane or create one on-the-fly. We will pick on the XSEC_A_PLANE plane in the model. A brief flash will appear on the model, and then disappear. In the view manager, highlight the “A” xsec and go to Display, Show X-Hatching, as shown in the next figure.

The cross-section will now appear on the model, as shown in the next figure.

If we double-click on the cross-section in the main window to make it active, it will remove the geometry on one side of the cross-section plane, as shown in the next figure.

To flip the side removed, go to Display, Flip. To return back to the full assembly, double-click on the No Cross Section item to make it active. Close out of this section and save the model but do not close it.

EXPLODE Next, we will talk about Exploded states. Therefore, go to View, View Manager and click on the Explode tab, which will look like the following.

Click on New and enter a name of Main_Explode, as shown in the next figure.

When you redefine this explode state, it will bring up the following menu.

This is the same functionality as 2001, so to edit the explode position, you would click on Position, which brings up the following window.

The most common thing to do in an example like this is to pick on a vertical edge or vertical axis to define the translation direction, and then move the components until they are in a position you want them in, like the one shown in the next figure.

Click on OK to finish the position definition. Next click on Offset Lines to create any dashed offset lines between components to show placement. When you click on this option, another menu appears, and we will click on Create, as shown in the next figure.

When you are lining up holes and shafts, like we are in this case, the easiest thing to do is use the Axis option, and then pick on the cylindrical surface of one component and the corresponding surface on the other. Repeat for each screw to the green part, and then from the green part to the brown part, to get the following result.

When done, click on Done/Return from the menus until you get back to the View Manager. Click on Close and then save your model.

ORIENT When you go to View, View Manager and then click on the Orient tab, you get the following.

You can double-click on a view to see that orientation. If you use Edit, Redefine, it brings you back to the re-orient window, as shown in the next figure.

Cancel out if you tried this, and then close the view manager. You do not need to save your model at this time.

ALL The last tab in the view manager allows you to combine different created view states from the other tabs that you saw. If you were to click on this tab, initially you will see the following.

We will click on New, and accept the default name COMB0001. When you hit the enter key, a window pops up as follows:

You can either reference the existing states so that a change to them will update your combination state, or create copies so that your combo state becomes independent. We will pick on the Reference Originals option. Back in the View Manager, redefine this new state, and you will see the following window.

In this window, we will select the different states that we created for each tab. Use the figure above to create your COMB0001 state, and when you click on the green check mark, this is what you will see (in No-Hidden line mode):

LESSON SUMMARY The view manager combines several functions into a single, consistent interface. You can create exploded views, simplified reps, component displays, cross-sections, saved views, and/or a combination of these.

EXERCISES None

Les son

3 7 Lesson Objective: In this lesson, we will get started with assemblies by demonstrating bottom-up design. The primary focus for this lesson will be to learn how to assemble in existing components into an assembly.

BOTTOM-UP DESIGN If you recall from Lesson 1 – Pro/ENGINEER Basic Elements, we learned that one approach to assembly design is to start by modeling individual parts, and then start to construct assemblies. As we create sub-assemblies, we can then assemble these into higher level assemblies. This lesson will go through the steps to assemble components.

CREATING A NEW ASSEMBLY We will get started by switching our working directory to the Machine_Vise folder. Next, we will go to File, New and when the New window opens, we want to select Assembly in the first column. The second column will list possible assembly subtypes, as shown in the next figure.

For most assembly mode usage, we will stick with a Design assembly. Many of the other ones on this list are specific for manufacturing.

We will give this assembly a name of MV_Screw_Assy, as shown in the previous figure, and then click on OK to continue to the next window, which looks like the next figure.

In this example, we will select the Startassy_English assembly because our units are English. You can use whatever template assembly your division uses, just be consistent with your units. Just like Part mode, we can enter parameter values for the assembly file in this window as well. Click on OK to finish the definition of the assembly. Assuming that your datum planes are visible, you should now see the following in your working window.

There are three default datum planes, called ASSY_FRONT, ASSY_TOP and ASSY_RIGHT, which are similar to the default part datums, but named with the prefix of ASSY_ to be able to quickly identify assembly datum planes from part datums. In the Model Tree, we currently only see the name of the assembly, as shown in the next figure.

By default, only part mode shows feature definition in the Model Tree. To see features in assembly mode, we must go to the top of the Model Tree, and pick on the Settings button, which expands to give us the following options.

We will pick on the first option (Tree Filters), which brings up the following window.

In the right column on this window, we can see a list of different entities that are displayed or can be displayed. Check the box next to Features, and then click on OK. We should now be able to see the default datum features in the assembly.

We are now ready to start building our assembly.

ASSEMBLE COMPONENTS On the Feature Toolbar, we can see an icon that looks like the following.

This is the Assemble Component icon. We will click on this and get the following window.

We are asked to select the component to assemble into the current assembly. We will pick on the 07_MV_Vise_Screw part, followed by Open. When we do this, the component shows up on the assembly in the working window, as shown in the following figure.

The component comes into the window in a default orientation, and location. To the right of our screen, we have a Component Placement window, which looks like the following figure.

The purpose of this placement window is to allow you to pick on geometry from the component as well as geometry from the assembly and define a relationship between those entities. Typically, the first component in a bottom-up design assembly is fixed to the assembly (can not move with respect to the assembly), and therefore we use the Default Placement icon to locate our first component. When we pick on this icon, the three default datum planes of the part align with their corresponding default datum planes in the assembly, as indicated below: FRONT (component) aligns with ASSY_FRONT (assembly) TOP (component) aligns with ASSY_TOP (assembly) RIGHT (component) aligns with ASSY_RIGHT (assembly) Go ahead and pick on the Default Placement icon, and you will see that the status in the bottom of our window now lists Fully Constrained. We are done placing our first component.

PLACEMENT CONSTRAINTS If you recall, when we first got into the placement window for a new component, the current constraint was listed as Automatic. It was awaiting entity selection to determine automatically which of the pre-defined constraints made the most sense. I would recommend starting off with Automatic and then adjust the constraints

accordingly. In this section we will look at the pre-defined constraints that can be assumed or selected directly. Mate A mate takes two surfaces and points their normals towards each other and lines up both surfaces, as shown in the next figure.

Mate Offset This is the same as a Mate except that the distance between the surfaces can be less than or greater than zero.

Align An Align takes two surfaces and points their normals in the same direction and lines up both surfaces, as shown in the next figure.

Align Offset This is the same as an Align except that the distance between the surfaces can be less than or greater than zero.

Orient (Parallel) This is similar to an Align offset, except that you don’t specify the distance between the surfaces.

Insert (Coaxial) An insert takes two cylindrical surfaces and lines up their axes, as shown in the next figure.

Tangent A Tangent constraint takes two cylindrical surfaces, or a planar and cylindrical surface and makes them tangent to each other, as shown in the next figure.

Point on Surface Places a datum point or vertex on a surface, as shown in the following figure.

Edge on Surface Places a straight edge on a cylindrical or planar surface, as shown in the next figure.

APPLYING CONSTRAINTS UPON ASSEMBLY To show these constraints, we will continue to assemble components into the MV_Screw_Assy. Therefore, click on the Assemble Component icon, and when the Open window appears, select the 08_MV_Collar component. When the Component Placement window appears, select the following two entities:

The order doesn’t matter, because it knows that the 07_MV_Vise_Screw component is now part of the assembly, and the 08_MV_Collar is the component part. When we pick both cylindrical surfaces, the axes line up as shown in the next figure.

In our Component Placement window, we can see that it automatically assumed an Insert constraint for this first selection of entities, as shown in the following figure.

We can also see that the status is only Partially Constrained, and we are prompted to create a second constraint in the constraint list window. Therefore, we will now pick on the following two entities.

When we select both flat surfaces, we see a magenta arrow on the part, as shown in the next figure.

In the message bar, we get the following prompt: “Offset (ins) in indicated direction:” Since our component surface was relatively far away from the assembly surface

selected, it assumed we wanted an offset constraint. Since we picked two surfaces that were facing in the same direction, it automatically assumed an Align Offset. We will enter a value of 0.0 in the message bar, and hit the enter key. When we do this, the blue component will snap over to the following location.

If we look at our placement window, we can see that it is Fully Defined, but there is an option to allow assumptions, and this option is currently checked, as shown in the next figure.

In reality, there is still a rotational degree of freedom open for this component, but that may not be critical in our design, so we can allow the system to fix this rotational degree of freedom for us. If we were to uncheck the “Allow Assumptions” box, we would have to define additional placement constraints to fix this rotational degree of freedom. Also, if you look up at the constraint list, we can see the last Align constraint that was created. In the Offset column, we can see our entered value of 0.0000. We could leave this the way it is, and it would remain aligned, but if we want to be certain that both surfaces always line up, we can use the pull-down field to change the option to Coincident, as shown in the next figure.

We will do this for our component so we are guaranteed that the placement stays at an Align. If we wanted the flexibility to move the component along the axis, we would have left it as an Align Offset. Our assembly currently looks like the following.

We will now assemble the last component for this particular assembly. Therefore, click on the assemble component icon and select the 09_MV_Special_Key. Initially, it comes into the assembly at the following location.

We will start defining our first constraint using the following cylindrical surfaces.

This will create an Insert constraint for us, and line up the axis of the component and assembly. Now, we will finish off this component by picking the following two planar surfaces.

NOTE: We are selecting the back flat surface of the key (the one that we can not directly see in this figure). When we do this, we again get an assumption of an “Offset” condition, and we will enter 0.0 for the offset value. A Mate Offset constraint is created, and we can now change the Offset column to indicate Coincident, as shown in the next figure.

We can also see that we are allowing it to fix the rotational degree of freedom on this key, which is okay for this component. We will click on OK to complete this component placement, and our assembly model will now look like the following.

Save and close this assembly.

LESSON SUMMARY For Bottom-Up design, we start by creating an assembly, and bring in components one-by-one. The first component is typically fixed by using the Default Placement constraint. For the rest of the assembled components, we will select an entity on the component and an entity on the assembly, and let Pro/E assume the constraint we want. We can then adjust the constraint as necessary to finalize the placement.

EXERCISES Create another assembly called Machine_Vise in the same working directory we’ve been working in for this lesson. Begin assembling components starting with 01_MV_Base to create the top-level assembly. Be sure to assemble in the subassembly that we created in this lesson (MV_Screw_Assy) instead of assembling the individual 07, 08 and 09 components. The final assembly will look like the following:

An exploded view of this assembly is shown on the next page for reference in determining how some of the components are assembled.

Les son

3 8 Lesson Objective: In this lesson, we will continue to learn about assemblies by a top-down design approach.

TOP-DOWN DESIGN The idea behind Top-Down design is to try to build in intelligence between the fit, form and function of parts that reside in an assembly. You try to capture this fit, form and function into the assembly first, and then pass the appropriate information down to the part level so that a change made at the assembly level or to one component in the assembly can drive updates to the rest of the critical parts. In this method, many of the components are created in the assembly, instead of being assembled into the assembly.

SKELETON MODELS The best way to capture fit, form and function for the assembly is to create a special kind of component called a Skeleton Model. A Skeleton model is similar to a regular part, but it is treated specially in the assembly. For example, a skeleton model is automatically excluded from the Bill of Material, where if you just created a regular part and used it like a skeleton, it would still be reported. There are also restrictions that can be placed on regular parts that skeleton models are exempt from, or get special rights to deal with. For example, you can make it so you are not allowed to copy surfaces from a regular part to another regular part, but you can still pass surfaces from the skeleton model to a regular part. In defining such restrictions, you avoid creating parent-child relationships between individual part files, making the model more robust. To demonstrate this principal, we will first create a new assembly file called Stacker. Be sure to use a Design sub-type for this assembly, just as we did for the last lesson. Also, once you have the assembly started, be sure to turn on the features in the model tree.

CREATE COMPONENT - SKELETON On the feature toolbar, we have another assembly icon that looks like the following.

This is the Create Component icon. When we pick on it, we get the following window.

We can see in this window that we have the ability to create parts, sub-assemblies, skeleton models, and bulk items. We will talk about bulk items in a later lesson. For now, select Skeleton Model. The default name for skeleton models is the name of the assembly appended with “_SKEL”, as shown in the next figure.

We can also see that there are no sub-types for a skeleton model. I recommend leaving the default name alone, and click on OK to continue. We get the next window.

In this window, we are asked to specify how the model will be created. We want to always use the Copy from Existing option, and browse to get to our start part that

we want to use. In this case, the startpart_english is already selected, so we will click on OK to continue. The skeleton model has now been added to our assembly, as we can see in the following figure.

In our model tree, we can see that the skeleton model has been placed at the top of the list, even before assembly features. This is one of the hints that lets us know that it is a skeleton model versus a regular part, which would have showed up at the end of the list.

We will now open up the skeleton model separately to add datum geometry to this model. If we right-click on this component in the model tree, we will see the following options.

Select the Open option, and the skeleton model will open up in a new window.

SKELETON GEOMETRY Skeleton models typically only contain datum or surface geometry. You should only try to capture enough information to drive the models where they interface. I have seen individuals create almost an entire assembly and all of its components in the skeleton so no changes have to be made at the part level, but this is overkill, and will over-complicate the model. Therefore, the less you can place in the skeleton but still maintain the complex relationships between parts, the better. In this example, we will start by creating a sketch feature (Lesson 5). Use the FRONT datum plane as the sketching plane, and face the RIGHT datum plane towards the Right. We will then create the following sketch.

NOTE: There is a vertical centerline in this sketch that allows for the diameter dimensions at the top and bottom. When we complete this sketch feature, we have the first curve in our skeleton model, as shown in the next figure.

In our model tree, we will right click on this sketch feature and select Rename, and rename the sketch to STEM, as shown in the next figure.

You are not required to rename the feature, but I recommend it so you know what it controls if you need to make a change later. Now, we are going to create a second sketch feature using the same sketching plane and horizontal/vertical reference. Our sketch will look like the following.

When completed, the skeleton model now looks like the following.

We will rename this second sketch feature to BASE, as shown in the next figure.

We have one more sketch feature for this skeleton model, which will be on the same sketching plane and H/V reference, and looks like the following figure.

The completed skeleton model will look like the following.

We will rename this last sketch feature to RINGS, as we can see in the figure below.

Save and close the skeleton model, and then return to the assembly. We can see the curves in our assembly, because the skeleton model is already assembled. Save the assembly.

CREATE ADDITIONAL COMPONENTS The next thing we are going to do is create parts in the assembly for each of the individual components that will ultimately make up this assembly. We are going to have seven components in this assembly, as shown in the following product structure. STACKER • Base • Stem Blue_Ring • Green_Ring • Yellow_Ring • Orange_Ring • Red_Ring • Base Component Therefore, return to the assembly file, and then click on the Create Component icon again. This time, select Part, Solid, and enter Base for the name, as shown in the next figure.

Click on OK, and in the next window, be sure that you are copying from an existing start part (in this case Startpart_english.prt). We can also see that when we are

creating a part object, we see a slightly different window than what we saw when creating a skeleton model.

At the bottom of the window, we have an option to leave the component unplaced. The reason you might do this is if you were simply trying to capture the product structure at this time, but then you wanted to come back later and locate the component once you have geometry. This might be especially true if you have mechanism connections that are going to exist. Even if you don’t check this option, you can always come in later and edit the definition of the component, and re-define the placement constraints. Therefore, we will leave it unchecked whenever we create a component in the context of an assembly. Click on OK to continue, and we now have our Component Placement window. We will click on the Default Placement icon to allow the part to be fixed to the assembly datum planes. Click on OK once you select the Default Placement icon. In the working window, you may not be able to distinguish the new part, because we only have default datum planes, but in the Model Tree, we can see the Base component added, as shown in the next figure.

We will repeat this same process to create the remaining six components in the order in which they are listed in the product structure on the previous page. The model tree, when complete, will look like the following.

Save this assembly once you have added the rest of the components.

PUBLISH GEOMETRY When you want to pass data from one model to another in top-down design, you use a tool called Copy Geometry. Copy Geometry is done in the component where you want to copy the geometry to (called the Target). The Source of the geometry comes from the Skeleton Model, assembly or other component. In our case, we are going to copy geometry from the skeleton model into each of the seven individually created components. Preparing the Skeleton If you recall, we have three sketch features in our skeleton model. At this time, we don’t have to do anything. When we use the copy geometry command within one of the components, we will be able to selectively pick the curve segments we want to pass. Left the way it is, there is no guarantee that the user that is responsible for creating the individual component will grab just enough references into his/her model. Too few, and they won’t have enough information to define the connection between the part and the skeleton. Too many, and it just wastes features and disk space in the component. Pro/ENGINEER has a tool that allows you to pre-define groups of data to pass from one model to the other. This tool is called Publish Geometry. It allows you to define all of the necessary items (curves, surfaces, points, planes, axes, etc.) and group them logically so when the user goes to copy the geometry, they only have to pick one item and get all of the necessary entities. For our example, it might be a bit overkill to define the individual publish geometry features, but we will do it for practice. For large, complicated models, you will want to use publish geometry features. It will become more clear as we go through an example.

The limitation of a publish geometry feature is that it can only be created from entities that exist in the model where the publish geometry is being created. With regular copy geometry features, you can copy external references into your model. But, by working with skeleton models, we are better positioned to have all of the entities within the skeleton model. Base Publish Geometry Therefore, go back and open the skeleton model. From the menu bar, select Insert, Shared Data, Publish Geometry. This will bring up the following window.

As you can see, we can optionally define surface references, edge references, curve references, or a variety of miscellaneous references (Axes, points, csys, etc.). This is nice, because we can publish all of the entities for the base that we need, regardless of what type of entity they are. We only have curves in our skeleton model, therefore, we will pick on the Curve Refs item, followed by the Define button. We will get the following menu.

We can select entire chains of curves, or individual curve segments using the default option of One By One. We will keep the default option, and then select the following four segments using the Ctrl key.

When all four are selected, they will be highlighted in a bold red, as shown in the next figure.

Click on the middle mouse button to accept this selection, and then click on Done in the menu manager. In the Published Geometry window, click on OK. In our Model Tree, we can see the current publish geometry feature.

We will want to rename this feature to BASE_PG. NOTE: When you rename features in the model tree, they have to have unique names. Therefore, we append the “_PG” at the end so we can tell that this is the Publish Geometry feature for the base.

Stem Publish Geometry For the stem, we will repeat this same process, but select the following entities.

Don’t forget the small horizontal curve segment. You may need to use the Right mouse button to query select until you see this segment highlight. Rename the finished feature to STEM_PG, as shown in the next figure.

Ring Publish Geometry Repeat this same process to create the publish geometry features for the individual rings, starting with Blue and ending at the Red ring. The following figure shows which curve references to pick for each publish geometry feature.

The completed model tree for the skeleton model will look like the following.

Again, using publish geometry for our simple example may be overkill, but you should get in the habit of using publish geometry to organize the data you want to pass from the skeleton to the individual parts.

The nice thing to point out is that each publish geometry is not a copy of the entities, and therefore doesn’t take up a lot of regeneration time or disk space. It is merely an organizational tool. Save and close the skeleton model once you are done creating all of the individual publish geometry features.

COPY GEOMETRY Now that we have created the individual components in our assembly, and we have defined all of the publish geometry in our skeleton, we are ready to pass the information from the skeleton down into the individual part files. To do this, we will go back to the assembly file. Base In the Model Tree for the assembly, right click on the Base component, and select Activate. This makes the active working model the base, even though we are currently in the top-level assembly. This is critical, because if we just went back to the base model itself, the skeleton would not be there to pick from, and we would be forced to work in multiple windows. By activating the part in the assembly, we can work in a single window. The trade-off is with the amount of clutter you have on the screen for large assemblies. This is where simplified reps or component displays, or merely hiding components will help organize your working environment. We know the base is active, because the model tree has a green pinwheel symbol on the base part, and in the working window, we can see text indicating the active object, as shown in the next figure.

With the Base part active, we will go to Insert, Shared Data, Copy Geometry from the menu bar. This brings up the following window.

From this window, we can see that we have the ability to define surfaces, edges, curves, etc. just like we did when we created the publish geometry. We could have selected Curve Refs here, and picked the same references in the skeleton model that we picked before. This would by-pass the publish geometry feature, and for our simple model would have worked just as well.

You can also see a Publish Geom line item in this window. We will click on this, followed by Define. This brings up the following menu manager.

Out on our working window, we can move our mouse over one of the entities that made up the base publish geometry, and it will highlight the entire publish geometry for the base, as shown in the next figure.

We can now pick this. We could have also expanded the features of the skeleton model in our model tree and picked the publish geometry for the feature directly. Once you select the BASE_PG publish geometry feature, click on the middle mouse button to accept it, followed by Done in the menu manager. Click on OK in the Copy Geometry window, and the copy of the curves should be complete. To verify this, open up the Base.prt part file by itself, and you should see only the curve entities that were part of the publish geometry feature, as shown in the next figure.

We will now activate the rest of the components (one-by-one), and use the Insert, Shared Data, Copy Geometry, Publish Geom tool to grab the appropriate publish geometry feature and place it in the active part.

Save the assembly when you have finished copying the geometry into each part. Open each one to verify that you have the correct data.

FINISH COMPONENTS Now, we can open up the individual components and add any necessary solid/surface features to create our models. We will go through each one individually now. Base Open up the base part, which should have the existing datum curves copied from the skeleton. In our model tree, we can see a copy geometry feature listed, as shown in the next figure.

We will now create a revolve feature. Use the FRONT datum plane as a sketching plane, and face the RIGHT datum plane towards the Right. Inside the sketch, use the Copy Edge tool to grab the existing curves from our copy geometry feature, and trim away the left side of the top-most horizontal line. Complete the sketch with three additional line entities, as shown in the next figure.

Don’t forget a vertical centerline as the axis of revolution. Revolve 360 degrees to get our first protrusion.

Finally, add a 0.75” round to the outside top edge, as shown in the next figure.

Save and close this part. When we return to the assembly, we can see the base part geometry.

Stem Open up the stem model. Create a revolve feature using the FRONT datum plane for our sketching plane, and face the RIGHT datum plane to the Right. Use the Copy Edge tool to get all of the existing curves from the copy geometry feature, and then close the left side with a line. Don’t forget the vertical centerline for the axis of revolution. Our sketch should look like the following.

Revolve this feature 360 degrees to create the first protrusion, and then add a 0.25” round on the top edge of this model to produce the final stem part, as shown in the following figure.

Save and close the stem part. Blue Ring Open up the Blue_Ring model. Repeat the same process to create a revolved protrusion. Don’t forget to add a vertical centerline on the existing vertical sketcher reference, as shown in the next figure.

The completed ring will look like the following.

Save and close this part. Green, Yellow, Orange and Red Rings Repeat the same process that we did for the blue ring to create the remainder of the rings. When you are done, and have saved each ring model, return to the assembly, and it will now look like the following.

MAKING CHANGES From the previous figure, we can see that the diameter of the base is too large. We can also see that the angle on the stacking rings is not quite big enough. With traditional bottom-up design, we would have to modify every single component. With our approach to top-down design, we only have to modify the skeleton model to accomplish this change. Therefore, go back to the skeleton model, and edit the stem sketch feature. Change the length of the small horizontal line from 0.125” to 0.375”. Next, edit the base sketch feature, and change the length of the horizontal line from 2.0” to 1.0”. Regenerate the skeleton model, and we should now see the following profile.

BEFORE

AFTER

Go back to the assembly, and regenerate it. The final stacker assembly looks like the following.

Save and close this assembly. We will come back to it in a later lesson.

LESSON SUMMARY Top-Down design is an approach that passes critical fit, form and function information from the top-level assembly down into the individual components/sub-assemblies. By using Skeleton Models with published geometry, you can make changes to the entire assembly by controlling the skeleton model.

EXERCISES None.

Les son

3 9 Lesson Objective: In this lesson, we will learn how to create exploded states, complete with offset lines.

USAGE OF ASSEMBLY CUTS There are a variety of reasons to create cuts in the context of an assembly. The most common are: Cut-Away Views – You create a cut that removes volume from some or all of • the components in the assembly. Unlike a cross-section, which will remove volume from all of the components when you set the visibility to view the cutaway, an assembly cut allows you to selectively pick which components are affected. Holes/Cuts in Weldments – Adding a hole pattern or cut to an assembly that • represents a single weldment. The ability to create the holes in the individual parts is minimized, because of dimensional references that may or may not exist.

CUT-AWAY VIEW We will work with the stacker assembly that we created in Lesson 38 to demonstrate cut-away views. Open up this assembly, and it will look like the following.

We want to make a cut that removes half of the volume from all of the components except the stem part. Before we do this, however, let us look at a cross-section for this part. To do this, go to View, View Manager. When the view manager opens, click on the Xsec tab. Create a new cross-section called Cut_Away, and use the ASSY_RIGHT datum plane as our reference (pick it from the model tree). Once you have created this cross-section, double-click on it. We see the following.

As you can see, the cross-section view removes half of the stem as well as the rest of the components. We want to see the entire stem. Therefore, we will use an assembly cut. First, close out of the view manager, and go into the layer tool. Hide all _Defaults layers except for the assembly itself. Your assembly should look like the following with datum planes visible.

Now, click on the Extrude tool. Down in the dashboard, you will notice that the “Remove Material” icon is grayed out. The reason for this is that any solid feature created in assembly mode can only remove material, not add material.

Now, click on the Placement slide-up panel. It looks like the following.

We can either select a sketch feature in the assembly, or create a sketch. We will click on the Define button. For a sketching plane, select the ASSY_TOP datum plane, and face the ASSY_RIGHT plane towards the Right. Inside the sketch, select the outermost circle (both halves) as sketching references. Then, sketch the following rectangle. Be sure to impose a tangent condition with the side, and snap to the top and bottom of the circle.

Finish out of the sketch, and make sure you go to the Options slide-up panel and select Through All for both directions, as shown below.

Finally, go to the Intersect slide-up panel. It looks like the following.

By default, all components in the path of the cut are going to be listed in the window. In this case, all seven parts are listed. We will start by un-checking the Automatic Update option at the top. This allows us to selectively add/remove models from the list. We will scroll to find the STEM model, and right click on it. Select Remove from the list of options, as shown in the next figure.

Click on the green check mark to finish this extrude feature, and we will be left with the following.

The Stem part is completely unaffected by this cut. The other models are only cut away in the assembly. If you open the Base or any of the rings, they still are whole. We will show something different in the next section. To turn off the cut-away, either delete the extrude feature or suppress it. Save and close this assembly. We will come back to it in the last lesson.

WELDMENT CUTS/HOLES The other common usage for assembly cuts would be in an instance where you can not easily define a hole or cut in a single part that may affect a group of parts. A good example might be a welded frame that will get items mounted to it. The spacing of the holes, as well as the locating dimension for the holes is usually determined after the frame is completely welded. But, for manufacturing reasons, we need to model the members of the frame separately and use an assembly to define the overall frame. Change working directories over to the Weldment folder, and open the assembly entitled Welded_Frame.asm. It looks like the following.

If we expand the model tree, we can see the product structure as follows:

The overall frame (gray bars) is welded together. The plate on the side (green) will be bolted onto the frame. In order to ensure that our bolt holes line up perfectly, we could do a number of things. Perhaps the cleanest would be to develop a skeleton for the interface points, and develop the weldment and the plate from this information. In this case, we are working with existing assemblies, so we only have two choices. We can go into each model, create separate holes/cuts and then build in relations between components to determine the location in case a change is made. This is a perfectly acceptable way of doing it, but creates a lot of book keeping. It also assumes that each hole can be manufactured off of existing references in the part file. In our assembly, we want to locate the holes from the extreme ends of the assembly, so it won’t work at the part level without adding extra datum planes or surfaces to capture the envelope of the assembly. Therefore, we will create the cut at the assembly level, and then discuss how we might be able to transfer that information into the parts (if required). Creating the Cut Click on the Extrude tool once more. Define the sketch, and use the front of the plate as a sketching plane, and point the ASSY_RIGHT datum plane towards the left. In sketch mode, change your display to a hidden line mode. If your sketch

doesn’t automatically pick references, select ASSY_RIGHT and ASSY_TOP for sketching references. Zoom in on the upper left corner, and sketch the following:

Now, pan over to the upper right corner and sketch two more circles – making sure to align the centers where applicable, and dimensioning where necessary.

In the lower right corner, sketch two more circles, as follows:

Finally, in the lower left corner, finish sketching the last two circles, as shown. NOTE: You shouldn’t need any dimensions for these holes, as the centers should line up with existing circles or references.

Zooming out, our entire sketch should look like the following.

Finish out of the sketch. For a depth option, pick on the To Select icon (the one with the red), and pick the following surface.

Now, we will click on the Intersect slide-up panel. It currently looks like the following.

We can see four MAIN_BAR models listed. In reality, the holes that we are creating are not going to intersect these models, so we will remove them. To do this, uncheck the Automatic Update option, and then right click on each of these bars to remove them. We are left with two SIDE_BAR, two MID_BAR, and one SIDE_PLATE components, as shown in the next figure.

One other thing we can see in this window is that each component has a value of Top Level, in the Display column. This means that the cut will only show up in the top-level assembly where it is created. We will right-click on each of these models in the list and change the option to Part Level. The intersect window will look like the following when we do this.

Click on the green check mark to complete this extrude feature, and you will see the following on your model.

From this figure, we can clearly see holes on all of the mid and side bars. The reason for this is the cut has been translated into the actual part file. If we open the SIDE_BAR component, for example, we see the holes.

In the model tree, it indicates the Assembly Cuts, as shown in the following figure.

If you try to edit or edit the definition of these features in the part itself, you will find that you can not. You have to go back to the assembly to edit them. This is intended functionality.

If we had kept the models at the Top Level scope, this is what we would have seen at the assembly level.

We can see that the holes are only on the side with the plate. All other Side and Mid bars are unaffected. If we open up the same SIDE_BAR model, we don’t see the holes, and the model tree does not list the assembly cut features.

The advantage of placing the visibility of the holes at the part level is that we can detail out the part in drawing mode and dimension the holes accordingly to perform the drilling at the part level. Of course, if this had been the original intention, we might have wanted to just create them as part cuts, and then tie them together with relations at the assembly level. The disadvantage of placing the visibility of the holes at the part level is that the model being cut will now have the holes in every instance that is used in the assembly, as we saw in our model. The work-around to this would be to model completely different bars for the side with the plate than what is on the rest of the frame. This creates more models than we really need. Of course, had we needed to add a plate to the other side, we can now just assemble in one more with the bolts and nuts and we won’t have to necessarily cut additional holes out.

LESSON SUMMARY

Assembly cuts are great for creating cut-away views that can’t be done with crosssections, or for creating cuts/holes in an assembly and showing the visibility at the part level. Be sure to look at the list of models that the cut will intersect, and remove any models that you don’t need in the list.

EXERCISES Open up the model entitled Shelf.asm. It will initially look like the following.

For this exercise, we need to drill holes to screw the pieces together. The following figures show the locations for the holes. We also need these holes to appear at the part level to be able to detail out the individual boards.

Les son

4 0 Lesson Objective: In this lesson, we will learn about Flexible Components, Merge and Cut-Out, and Repeat Component Placement.

FLEXIBLE COMPONENTS There are some models that change each time you use them. Typically, there is a “steady-state” for these components, but when they are used, dimensionally they are altered. A perfect example of such a component is a compression spring. In its steady-state, it has a certain length. When used, the length is either compressed or stretched out. If you recall from Lesson 35 – Family Tables, we can create a family of “like” components. Many users might consider using Family tables to create different spring models, but the problem is two-fold: 1)

There can be an unlimited number of possible lengths that can be achieved with the spring, so you would have to almost create a new instance for each usage. 2) Family table instances are unique parts, each with its own unique name. When used in an assembly in multiple configurations, this approach would create as many individual components. A Bill of Material would not be very accurate unless you specifically altered each component’s parameters to be identical. The advantage of using flexible components is that the new dimensional data for that model is stored with the assembly, so the original part is not altered, and yet we can capture an infinite number of lengths for the component when used. Each instance is the original model, so the quantity in a BOM is accurate. To demonstrate this concept, we will switch our working directory over to the Flex_Asm folder. Open up the Flexible_Spring.asm model. It consists of a rim part and three instances of the same spring, as shown in the figure below.

The model tree confirms the fact that all three spring models are the same part.

What we want to be able to do is have the length of the three springs be different for each one so they fit in the space provided, which is shown in the next figure.

Preparation of Spring For the spring to work properly, we have a relation that calculates the pitch based on the length of the spring (between TOP and DTM2) divided by 10 coils. Therefore, if we change the length, the spring compresses or extends. If we turn on datum planes, we can see DTM2 for each of the springs. DTM2 controls the length of the spring, but unfortunately, based on the way the spring was created does not go from one extreme to the other. The following figure shows the actual length of the spring relative to the bottom of the spring as it would rest in our part.

We can see DTM1 at the bottom of the spring. Each spring, when assembled, lines up the DTM1 plane with the bottom inside of the rim part so the spring is resting on the bottom without any interference. The length of the spring in its steady state is 10.000”, the distance from TOP to DTM2. The remaining distance is 0.25” – therefore, we need to subtract ¼” from the actual distance we want to cover to modify the length of the spring. Therefore, from left to right, the new length of the spring would be 4.5, 7.0 and 9.5 respectively. Make Flexible Now that we got that out of the way, we are ready to adjust each of the springs. We will start with the first one in the model tree. Right click on the spring and select Make Flexible, as shown in the next figure.

This brings up the following window.

By default, we are placed into the Dimensional variation tab. In the working window, we can see the component highlighted in red, as shown below.

We need to pick on the feature that contains the dimension to vary. In this case we will pick on the DTM2 datum plane. This will show the 10.000 dimension. Pick on this dimension, followed by the middle mouse button, and it will be added into our window, as shown below.

When adding dimensions, the default method for entering the new value is based on data entry. We simply pick in the field and type in the new value (9.5 in this case). There are other ways to calculate the new value if you don’t already know it. If we use the pull-down field Method, we see other options. One of these, for example, allows you to measure the distance between two entities. We will click on OK to complete this change, and our model updates. We will repeat this process for the other two springs, entering 7.0 for the second one, and 4.5 for the third. When complete, our assembly will look like the following.

Our model tree has a little “Spring” icon on top of the blue cube indicating that the components are flexible, as shown in the next figure.

Save and close this assembly. Aside from controlling dimensions, the flexible component can also vary parameter values, feature regeneration status (keep in mind suppressing a feature will suppress all of its children), surface finish and geometric tolerance data.

MERGE A merge operation is performed in the context of an assembly. It takes one or more parts and merges them into a single, specified part. To demonstrate this functionality, open up the model entitled Assy_Merge.asm. It will look like the following:

We will take a moment to interrogate this assembly. It is made up of four components. The first three contain solid features. The fourth (Stand_Alone_D) contains only the default datum information. We will come back to this part a little later. If we go to View, View Manager and click on the Explode tab, we can see a default explode state. Double-clicking on this shows us the following.

Right click on the default explode state and select Unexplode View. Now, click on the Xsec tab, and we can see two cross-section views listed, A and B. Double click on A and you will see the following.

Double-click on B to see the following.

We can clearly see the boundaries of the individual components in the two crosssectional views. We will come back to the cross-section views once we perform the merge operation to show you the result. Example 1 – Merge into Existing Component w/Solid Geometry In this example, we will merge Components “B” and “C” into Component “A”. Therefore, go to Edit, Component Operations, which will bring up the following menu manager.

We will click on Merge. When we do this, the message bar prompts us with the following: “Select parts to perform MERGE process to.” For future reference, we will refer to the model we select as the TARGET. We will pick on the Stand_Alone_A component (either directly, or in the model tree). Click on the middle mouse button to accept this selection. We are now prompted to “Select reference parts for MERGE process.” For future reference, we will refer to these models as REFERENCE MODELS. We will pick Stand_Alone_B and Stand_Alone_C using the Ctrl key to pick multiple items. Once both are selected, click on the middle mouse button to accept these selections. The menu manager now looks like the following.

This menu has two sections. The first deals with how the new merged model behaves with respect to the original model. The options are: Reference – The TARGET model will be dependent on the REFERENCE • model. A change to the REFERENCE model will update the TARGET model. Copy – The TARGET model will be independent of the REFERENCE model. A • change to the REFERENCE model will not update the TARGET model.

The second section is used to copy datums from the REFERENCE model to the TARGET model. The options are: No Datums – Only solid volume will get merged into the new part. Typically, if • you are merging into a part that already contains default datum planes, you don’t need to duplicate the planes. Copy Datums – Datums will be copied along with the solid volume into the new • part. You may wish to use this if you are merging into an empty part (without any datum features). We will accept the default options of Reference and No Datums, and click on Done to continue. In the message bar, we get the following prompt:

Before we explain this, we ought to define one additional piece of information. If the placement constraints of the REFERENCE MODEL are tied completely to the TARGET model, then we will consider this to be a LOCAL REFERENCE. If the placement constraints of the REFERENCE MODEL are tied to any other reference other than a TARGET reference (i.e. – other part in the assembly, or assembly datum plane, for example), then we will consider this an EXTERNAL REFERENCE. When you select the option Reference in the menu manager, and your model is a LOCAL REFERENCE, then you will get this prompt. If your model is an EXTERNAL REFERENCE, then you will not get this prompt. If you used Copy instead of Reference, then you will not get this prompt. Okay – so what is this prompt asking? Since the model in question (Stand_Alone_B) is being merged using the Reference option, and it is a LOCAL REFERENCE to the TARGET part (Stand_Alone_A), then answering Yes to this prompt will allow an update to the placement of this part to update the TARGET as well. For example, if we used a MATE OFFSET to locate Component “B” to “A”, and later changed the

offset distance, the TARGET part would update with the new position of component “B”. If we answer No, then we can change the original placement of the REFERENCE part and the TARGET will not update. We will answer Yes to this prompt. When we do this, we get the next prompt:

Answering Yes to this will remove STAND_ALONE_B from the assembly, leaving only three components. Since we answered Yes to the previous prompt, then we should answer No to this, otherwise, we will never be able to re-define the placement of this component. Therefore, we will answer No. At this point in time, we are now asked to deal with Stand_Alone_C, and we see the same menu as before.

Now, this component is not a LOCAL REFERNCE. It is an EXTERNAL REFERENCE, because it is assembled to Stand_Alone_B, and not to the TARGET (Stand_Alone_A). Therefore, if we pick either Reference or Copy, we will not get the first prompt that we got before. We will accept the defaults for this menu, and pick Done. We are not prompted at all for this component. On our model (with shading on) we can see that there is now overlapping geometry, as shown in the next figure.

Go ahead and hide Stand_Alone_B and Stand_Alone_C in the model tree, and you will see that our Stand_Alone_A component now has the volume of B and C added to it, as shown in the next figure.

Try looking at your cross sections, and you will see that this is truly one solid volume made up of three separate components. Now, open up Stand_Alone_C, and add a 1.0” round to the edge shown below.

Switch back over to your assembly, and regenerate it. You can see (even with the part hidden) that the round has transferred to the TARGET part. This is because of the Reference option that we picked.

What is Happening at the Part Level? If we open up the Stand_Alone_A part, and look at the model tree, we can see the following.

We can see two merge features at the bottom of the tree. If you click on the first one, the geometry representing Stand_Alone_B highlights. if you pick on the second one, the geometry representing Stand_Alone_C highlights. If we wanted to return to the original “A” part, we would have to delete the two merge features. This is something important to keep in mind. The TARGET part will be altered when you merge. If we were trying to create a temporary model for analysis or other reason, we might want to consider using an empty part (such as our Stand_Alone_D) model. To demonstrate this, go ahead and delete the two merge features from this part, return to the assembly, and unhide the “B” and “C” components. We are going to create a new merge by using Edit, Component Operations, Merge. For the TARGET part, select Stand_Alone_D from the model tree. Click on the middle mouse button to accept this. Next, for the REFERENCE PARTS, select “A”, “B” and “C” components form the model tree. Click on the middle mouse button to accept these. For all three, select Reference and No Datums from the menu manager when it comes up. As you do this, you will notice new geometry appearing on the model embedded into the three existing components. When done, hide the first three components, and you will see the following.

Copy

Now, we will demonstrate the difference between Reference and Copy. Up to now, we have referenced the original models in the TARGET. Now, we will open up the Stand_Alone_D model, delete the three merge features that we just created, and return to our assembly. Unhide all three components. This time, when you perform the merge as we just did, use Copy instead of Reference. Hide the three components again in the assembly, and you still see the same result. The difference is when you open up the Stand_Alone_D part. What do you notice? Well, the first thing you might have noticed is that when you picked the Copy option, the option to include or exclude datums was not available. In a Copy datums are automatically copied. The second thing you might notice is that in the part (Stand_Alone_D), the model tree now contains all of the features for all three components, in addition to the default datums it had. The model tree is shown in the next figure.

All of these features are now completely independent of the models that created them. An update to Stand_Alone_A, for example, will not update this model. We can, however make changes now to any of these features in this part. The other thing we might want to do is go through and edit references for the added datum planes to get them to use the default planes for this model. For example, if we look at the top of the model tree, we can see that we have our default model datum planes (RIGHT, TOP and FRONT).

The next set of datum planes (DTM1, DTM2 and DTM3) correspond to the features merged from Stand_Alone_A. We can edit the references for DTM1, and re-route all features to RIGHT. Doing the same for DTM2 and DTM3 would allow us to delete these planes from this model to reduce clutter. Again, using an empty part is ideal if you don’t want to alter the original models being merged. Save and close this part, and the assembly.

CUT-OUT A Cut-Out is exactly the same as the merge in almost all respects. The only difference is that it removes material from the TARGET instead of adding material to it. To demonstrate this, open up the assembly entitled Assy_Cut-Out.asm. It looks like the following.

This assembly consists of two components (Stand_Alone_E and Stand_Alone_F). The “F” component sits within the “E” component. The purpose of this is to extract the volume of “F” from “E”. A good example of using this is to create a die model. Another reason you might use this is for dual-material parts, or parts that are over molded. You can create a volume, assemble another volume into it, and then subtract the interfering volume. We will go to Edit, Component Operations and we see the same menu as before.

This time, we will select the Cut Out command, as shown above. When we do this, we get the following prompt in the message bar: “Select parts to perform CUT OUT process to”. This is the TARGET part, as we remember from the merge operation. We will select the Stand_Alone_E part from the model tree.

Click on the middle mouse button to accept our choice. Now the message bar reads: “Select reference parts for CUT OUT process”. We will pick Stand_Alone_F from the model tree, followed by the middle mouse button. We see a somewhat familiar menu as before.

The biggest difference is the ability to include or exclude datums. The same rules still apply for Reference and Copy as the merge operation. We will pick Reference, followed by Done. When we do this, we get the same prompt: “Support associative placement for the feature?” Remember, this prompt comes up if you select Reference and the REFERENCE MODEL (“F”) is tied to the TARGET (“E”) in terms of placement (which it is). We will answer Yes to this prompt. Another difference between merge and cut-out is the fact that we do not get another prompt at this point. Instead, our cut-out is complete. If we hide component “F” in our model tree, we can see the following.

In our part file for Stand_Alone_E, we see the following model tree.

Save and close this part and assembly.

REPEAT COMPONENT PLACEMENT When you are assembling a component multiple times into an assembly, you can repeat the placement process to save time. A great example would be to assemble in a fastener where a pattern is not readily available to take advantage of. To demonstrate this, we will open up the assembly called Repeat.asm. It looks like the following:

It currently consists of a single part called Repeat_Base. This part has notches cut out along the length. Each notch is the same width, but is spaced differently, and at different heights. The notches are not patterned. We are going to assemble in a bar across each of these notches. Since the notches are not patterned, we can’t simply assemble the bar on the lead notch, and then reference pattern it. We also don’t want to have to go through the complete assembly placement commands for each one independently. Therefore, we will learn about a tool that will save time in a case like this. We have to start by assembling one of the bars. Therefore, pick on the assemble component icon, and select the Repeat_Arm part. When it shows up in the window, we will start picking references, starting with the following on the arm.

For the assembly reference, select the following surface on the far left side of the base.

This should create a Mate placement constraint with a “Coincident” type applied. Now, back on our arm, select the next surface.

Then, on the base, pick the following surface.

This should create a second Mate “Coincident” constraint. Finally, pick the last surface on the arm, as indicated below.

On the base, select the following thin surface at the far left of the part.

We will be prompted for an offset distance. Type in 0.0, and then change the type to “Coincident” in the placement window. Our Component Placement window will look like the following when done. Click OK to complete the placement.

On the assembly, we can see the first arm assembled.

Now, to be able to use the repeat command, we need to remember what assembly references we picked, and in what order. If you recall, we picked the following surfaces in the order indicated in the figure.

Remember this, because we’ll come back to this. To access the repeat command, first select the component to repeat. Therefore, we will pick on the Repeat_Arm component in the model tree so it highlights in red in the working window. Next, go to Edit, Repeat from the menu bar. This will bring up the following window.

At the top of this window, we can see the three placement constraints used to assemble this arm, and in the order in which they were picked starting from the top to the bottom of the list. These correspond to the 1-Mate, 2-Mate and 3-Mate two figures back. What we need to do is pick which references are different for each new instance of the arm we add. If we remember the three references, the second one was the large flat front surface, which all of the notches share as a common reference. The first and third mate commands, however, used surfaces that were unique to each notch. Therefore, the only references that will be unique for each bar placement will be the first and last ones. We will pick both of these in this window, as shown in the next figure.

If you imagine what would be the first and second reference for each additional arm being placed, it would be the following.

“Pick 1” represents the surface that we would pick for the first mate, while “Pick 2” represents the surface we would pick for the last mate. Now, we will pick on the Add button. When we do this, the reference used for the first Mate command highlights on the model, and we are asked to pick the equivalent. This is where we pick the first “Pick 1” in the previous figure. Then, the second reference highlights, and we will pick on the first “Pick 2” reference from the previous figure. All of a sudden, an arm appears in the second notch, as shown in the next figure.

In the Repeat window, we can see one instance added to the list at the bottom.

The first reference is highlighted again, so we go back to picking the “Pick 1” surface for the next notch, followed by the “Pick 2” reference for that same notch. Keep picking the “Pick 1” and “Pick 2” references for each additional notch until you see an arm in each one. At this time, our model looks like the following.

Our Repeat window now lists all of the instances in the bottom.

If we don’t have any more to add, we will click on the Confirm button, and our placements will be complete. As you can see, you can save a lot of time by just picking the assembly references that are unique to place each arm. Save and close this assembly.

LESSON SUMMARY Flexible components are great when you need to use the same model, but vary it each time. Merge and Cut-Out operations add/remove material from a TARGET part by using one or more REFERNCE PARTS. Just be careful to select the options that will work for your needs.

Finally, use the Repeat command to bring in more than one of the same objects where tedious repetition would otherwise be required.

EXERCISES None

Les son

4 1 Lesson Objective: In this lesson, we will learn about the basic flow for creating drawings.

3D to 2D Pro/ENGINEER is a highly advanced three-dimensional solid modeling package. The benefits to modeling in three-dimensions are: Easier to visualize and interpret the product being defined – ambiguity of 2D • drawings being perhaps the biggest problem with 2D Faster for making drastic changes (assuming that design intent is followed • when modeling the part) Direct 3D manufacturing and analysis capability (CNC, CMM, STL, FEA, etc.) – • Rapid prototyping all the way to full manufacturing processes, 3D translation into international exchange formats makes manufacturing much easier Higher quality of products – more design iterations can take place with 3D over • 2D, allowing for fit, form and function checks Lower unit costs – a by-product of faster, more reliable computer prototyping, • resulting in fewer samples being produced or purchased Improved MRP data – fully defined product structures that are easy to create, • and maintain allow for more accurate data transfer to MRP systems. Others… • Even with the benefits to generating product designs in 3D, the reality is that many companies (ours included) still rely on 2D drawings to convey product information (in addition to 3D models). Having said that, it is important to learn the proper way to generate 2D Detailed Drawings from Pro/ENGINEER 3D models. Practice Makes Perfect When you talk to many Pro/ENGINEER users, they will complain about the 2D mode of Pro/ENGINEER – either because of ease of use, perceived lack of functionality, or performance issues. Unfortunately, many of the complaints that come up are a result of inexperience with this tool. Pro/ENGINEER has one of the best 2D Drawing packages out there (aside from AutoCAD). The huge advantage over AutoCAD is the associative nature with the 3D

modeling world. The problem is that most users spend about 95% of their time in 3D modeling modes, and only about 5% of their time in drawing mode. Because of this, it is very easy to fall behind the learning curve on the tools and functionality of this module. This training guide will serve as a reference for users to recall such tools and techniques, but the reality is that unless you spend a lot of time in drawing mode, you may forget many of these tools.

DRAWING 101 A Drawing in Pro/ENGINEER is a by-product of the 3D model. When done properly, the majority of drawing mode steps should be automated by the definition of the model. If you recall from our first lesson, drawings can not exist without the 3D part or 3D assembly of which the drawing represents. The typical steps to creating a drawing are: 1. Model Definition – Create the part and/or assembly files that the drawing represents. Be sure to follow design intent and model in dimensions that must be shown on the drawing, especially critical dimensions. 2. Create Drawing – Start a new drawing. Select the model for the drawing. 3. Load in Drawing Setup File – Load in the appropriate drawing setup file for your units and sheet size. This is critical to getting your text, arrows and line styles to appear properly on the drawing. Ours our based off of ASME Y14 standards. 4. Add Views – Add all of the views you will need for your drawing. For crosssection views, define the cross-sections in the model itself (much faster and easier than doing it in the drawing). 5. Show Axes – Show axes for any features/views that require them. Clean up any axes as necessary. 6. Show GTOL Datums – Show the datum references for any GTOL Datums created. Again, the GTOL datums themselves should be created in the part or assembly. 7. Show Dimensions – Show dimensions from the model that exist and need to be captured in the drawing. Clean up dimensions as necessary. Modify the dimension to add specific text, tolerances, or symbols. 8. Create Additional Dimensions – Create any additional dimensions in the drawing that do not already exist in the model. Modify the dimension to add specific text, tolerances or symbols. 9. Create/Show GTOLs – Create or show already created geometric tolerance blocks on the model. Associate to any dimensions as necessary. 10. Add Notes and Symbols – Add notes and symbols to your drawing views. Relate any symbols that must move with the views. 11. Create Any Necessary Draft Entities – Create any geometry that does not currently exist in the model that is necessary for further defining the drawing. This might include things like parting lines that weren’t already created as datum curves, etc. Relate any draft entities that must move with the views. 12. Add Tables – If your drawing requires a table (BOM, for example), add it to the drawing. 13. Add Balloons – Add any table-driven balloons and clean-up as required. 14. Add Additional Sheets – This can be done earlier, but it is easier to define all views, notes, etc. on one sheet (even if outside the border at first), and then move to additional sheets as space requires. 15. Add Format – Assuming that your drawing is not based on a template (covered later in this lesson), you will need to add your drawing format. You can add the drawing format at any time in this list. I find that it is easier to

add the format once you are pretty sure your drawing sheet size is the one you want. 16. Finalize – Tweak any additional items on the drawing, filling in parameters, etc. If you try to follow these steps in this order, you will be more efficient in creating drawings, as well as adapting to changes to your model in the meantime. In the rest of this lesson, and additional lessons coming up, we will go through these steps in more detail.

FORMATS, TEMPLATES AND SETUP FILES A Drawing Format is another Pro/ENGINEER object type (.frm) that typically defines the borders and tables in the drawing. Typically, these are created by system administrators, and maintained by the same individuals. Most users only apply already created company formats to their drawings. The creation and maintenance of drawing formats is not covered in this training guide – only how to apply/change the applied format on the drawing. A Drawing Template is an actual drawing file that contains a format, an associated drawing setup file, and some pre-defined information (such as pre-defined views, notes, tables, symbols, etc.). These are designed to help automate the creation of drawings further, but can cause problems if the company doesn’t always follow the same rules for creating drawings from one product to the next. For the purpose of this training guide, we will not go into further detail about templates. We will learn how to do everything from scratch. A Drawing Setup File is a configuration file that controls the look and feel of the drawing. It defines such things as the drawing units, the text heights, the line and arrow styles, the format for dimensions, symbols, tolerances, gtols, etc. These files are typically created by system administrators and applied by the users. We will not go into detail on how to create one of these files, nor will we go through the myriad of options controlled in these files. Suffice it to say that our company has a pre-defined set of files that are based on industry standards (ASME Y14).

LESSON SUMMARY Drawings are critical to the release of products, but the creation of drawings doesn’t have to be a time-consuming and confusing process. By following the typical steps to creating a drawing, users can be confident in the quality of their drawings, and be happy with the methods for creating these drawings.

EXERCISES None

Les son

4 2 Lesson Objective: In this lesson, we will learn how to create a new drawing, apply a drawing format, and a drawing setup file.

CREATING A NEW DRAWING To demonstrate how to create a new drawing, we will start by opening a model that the drawing is going to be created from. Therefore, open up the model called Lesson41a.prt, which looks like the following:

We are going to demonstrate how to create the new drawing file, add the format and drawing setup file. In later lessons, we will learn how to create views, show dimensions, create geometric tolerances, etc.

In this lesson, we are going to start the new drawing, associate the model to it, add a drawing format, and add the drawing setup file in preparation for adding views, dimensions, etc. We will look at parameters in the model and how they fill in the title blocks, etc.

NEW DRAWING Before we get started, switch your working directory over to Drawing, located in your ProETrain folder. We are going to start by going to File, New, and pick on Drawing as the primary object type. For the name, type Lesson41a, which is the exact name of the part file we are working with. NOTE: It is important to use the same name as the primary model in your drawing. The reason for this is due to making a copy of the drawing. If your model and drawing have the same file name, when you perform a SAVE_AS on the part, it makes a copy of the part, and its drawing as well. This will save you from having to re-create the drawing for the copied part. The New window currently looks like the following:

Down at the bottom, you can see a check box labeled Use Default Template. If we were using a company-created template drawing, we want this to be checked. For our training class, we are not going to use template drawings, so we will leave this unchecked. You can also see that there are no sub-types for drawings. Click on OK to continue. We now see the following window.

The first thing we need to check is the model listed at the top of this window. By default, it uses the last model that was active. Since we just opened our Lesson41a.prt part file, it should be listed. If this is not the case, or if you have not opened a model recently, click on the Browse button to find the model to use.

Next, we have another chance to specify a template drawing, or to bring the drawing in empty with an associated drawing format, or just empty. The default is Empty, which we will leave. Next, we can specify the orientation of the drawing. We always want to use Landscape, but it won’t really matter once we apply the actual drawing format, which will replace all settings as they are now. That is why we will leave this default at landscape. Finally, we have the ability to pick a sheet size to start with. We will pick C to start. Once your window looks like the previous figure, click on OK to continue. We can now see an empty drawing. There is a rectangular border around the drawing that represents the sheet boundary (“C” in this case). At the bottom of our working window, we can see a summary of the drawing to this point, which looks like the following:

From this we can see that the overall drawing scale is 1:1, the active model is a Part, and the name of that part is Lesson41A. Finally, we can see that our current sheet size is C. If we needed to change the scale or sheet size, we could double-click on these values in the summary and these would invoke the proper interface to make those changes. For now, we will leave these alone.

ADDING A DRAWING FORMAT For this lesson, we are going to add a drawing format at this time. Normally, we would add the format once we are ready to release the drawing, and have created and cleaned up our views. If you recall, we picked an empty “C” size drawing sheet. We are now going to add a format to this sheet. To do this, go to File, Page Setup from the menu bar. This brings up the following window:

Currently, there is only one sheet, so there is only one row in our window. Had we had multiple sheets, we would see a row for each sheet. We can apply different

formats for different sheets. Generally, I would recommend against this. The only thing we will do is have a different format sheet for the first sheet of the drawing and one that is used for the rest of the sheets. This will make more sense in a little later. Currently, we can see that for sheet one, we have a C Size format applied. This is the generic empty “C” size that we picked. If we click on the word C Size, we can see that it becomes a pull-down field to select from other formats in our library. We can see the following.

In this list, we can see all of the default PTC sheet sizes for English (A, B, C, D and E) and Metric (A4, A3, A2, A1 and A0). We can also see a choice called Variable Size. We could use this to create a custom sheet size, which would invoke the rest of the options in this window. The last choice is Browse, which will let us search for a format to use. We will click on Browse, which brings up the following window.

Typically, companies use a configuration file called Config.pro, which defines the location for global standards. The location of company-approved formats is often one

of these standards defined. If you have a config.pro file that calls out the location for standard formats, it comes up by default, as shown in the figure above. For this training class, we will all work off the same formats for consistency, therefore, we will want to click on the folder that brings us into our current working directory (which we selected as the folder called Drawing). The figure above shows the icon to select to get to our working directory. Once we pick on this, we see the following drawing formats to choose from.

We will pick on the Train_Frm_C format, followed by Open. Our page setup window now lists this format, as shown in the next figure.

We can see that for sheet one, the current format is TRAIN_FRM_C (Sheet 1). Notice the “Sheet 1” comment at the end. Why is this? In ASME Y14 standards, the first sheet of a drawing has more information than the rest of the sheets (referred to as continuation sheets). Therefore, Pro/ENGINEER formats can contain two sheets. The first sheet of the format is typically applied to the first sheet of a drawing when used. The second sheet of the format is typically applied to the second, third, etc. sheets of a drawing. Therefore, our drawing sheet 1 in this example is using the first sheet of the drawing format. When we click on OK to complete this page setup, we can see the drawing format applied to our drawing.

DRAWING SETUP FILES The Config.pro file that we talked about before governs the behavior of Pro/ENGINEER as a whole, but there is a special file that governs the behavior of drawings. This is called a Drawing Setup File, and has a .dtl extension. The Drawing Setup File controls the units of the drawing, the text properties, line styles, view display styles, rules for tolerances, etc. We have drawing setup files that follow the ASME Y14 standards in their values for these types of controls. For the purpose of the training class, we have included a copy of these in our current working directory. By default, Pro/ENGINEER has its own drawing setup files. The Config.pro file that we use calls out a company standard setup file as the default, but this may be different for each division, so we want to get in the habit of retrieving one into our current drawing before we add views, notes, dimensions, etc. Failure to add the drawing setup file before the views may result in some re-work. To access the drawing setup file and its options, go to File, Properties. This brings up the following menu manager.

In this menu, we can see three different options. The first (Drawing Models) is used to access the current drawing models in the drawing. The last (Tolerance Standard) is used to control tolerance mode. We will pick Drawing Options, which brings up the following window.

At the top, there is a File Open icon. Pick on this, and you will be brought into your working directory. We will stop a minute to talk about something. If you were to look at the units of our model, they are in Millimeters. If you recall, we chose a C size sheet for our drawing. It might seem logical to select a drawing setup file that is tied completely to the sheet being used. This would be an incorrect assumption. Why? The rules governing metric drawings are completely different than those governing English drawings. For example, dimensions in millimeters are not allowed to have trailing zeros (zeros after the decimal point). English dimensions are not allowed to have leading zeros (zeros before the decimal point). The drawing setup files have the correct settings to control this. If we were to pick a drawing setup file in English units, then our drawing would have the rules for English dimensions applied to metric dimensions. This could throw off Tolerancing, etc.

We do need to understand the sheet size that we are using to make sure our text heights, arrow lengths, line weights, etc. are appropriate for reading the values when printed, so we can not completely ignore the “C” size sheet. Therefore, we need to pick a drawing setup file for millimeter dimensions that corresponds to an approximate “C” size sheet. So, what are the equivalents for metric and English paper sizes? The following table shows the equivalents. English Paper Sizes (inches) A (8.5 x 11) B (11 x 17) C (17 x 22) D (22 x 34) E (34 x 44)

Metric Paper Sizes (millimeters) A4 (210 x 297) ~ (8.23” x 11.7”) A3 (297 x 420) ~ (11.7” x 16.54”) A2 (420 x 594) ~ (16.54” x 23.39”) A1 (594 x 841) ~ (23.39” x 33.11”) A0 (841 x 1189) ~ (33.11” x 46.81”)

Even though there is a clear difference in size from English to metric sheet sizes, we can see that the equivalent for a “C” size is an A2 size. Therefore, the drawing setup file that we will pick will be the a2a3a4.dtl drawing setup file (located in our current “Drawing” working directory. Our window looks like the following:

Click on Open once you have selected this drawing setup file. The Options window now lists the settings that correspond to this file, as shown in the next figure.

We are not going to go through all of these settings. Suffice it to say that they do follow ASME standards, so we can be confident in the outcome of our drawings using these files. Click on OK to apply the settings and close out of the window. Save the drawing.

LESSON SUMMARY When creating a new drawing, be sure to name it the same as the primary model used in the drawing. Before adding any views to a drawing, add the drawing setup file that corresponds to the model units and sheet size being used. Drawing formats are added to the sheets. Formats should be applied once you know how big your sheet size will need to be to accommodate the different views, their dimensions, notes, symbols, etc.

EXERCISES None

Les son

4 3 Lesson Objective: In this lesson, we will learn about adding general views, and some basics about the view properties window. We will also learn about the drawing mode toolbar.

DRAWING MODE TOOLBAR In the System Toolbar, there is a set of icons for drawing mode. These icons look like the following.

From left to right, these icons do the following: Set Current Drawing Model – If you have more than one model associated • with the drawing, you can use this tool to make one of the models the current active model. We will talk about this in more detail in a later lesson. You can also get to this functionality through File, Properties, Drawing Models. Update Views – Certain changes update in the drawing automatically, while • other changes require you to update all of the sheets and all of the views. This icon is used to do this. You can also get to this through View, Update, All Sheets. Add General View – This icon lets you add general views to your drawing. • You can also get to this through Insert, Drawing View, General from the menu bar. Show/Erase Tool – This icon accesses the tool used to show or erase • dimensions, axes, reference dimensions, notes, geometric tolerances, set

•

• • • •

datums, etc. already created in the model. You can also access this tool through View, Show and Erase. Create Dimensions – This tool allows you to create driven dimensions in the drawing. These dimensions do not exist in the model, and can not be used to change the model itself. This functionality can also be accessed through Insert, Dimension, New Reference. Notes – This tool allows you to create notes on the drawing. You can also access this functionality through Insert, Note. Balloon Note – This tool allows you to create balloon notes on the drawing. You can also access this functionality through Insert, Balloon. Drawing Symbols – This tool allows you to access your custom symbols library. You can access this functionality through Insert, Drawing Symbol, Custom. Sheet Selector – When you have more than one sheet on your drawing, the current sheet is listed in this field. You can use the up/down arrows to go through the sheets. You can access this functionality through View, Go to Sheet.

GENERAL VIEWS The first view that you add to a drawing is called a General view. It has no predefined orientation, scale or style. To demonstrate this functionality, we will go back to the Lesson41a.drw drawing that we started earlier. Currently, it looks like the following:

Click on the Add General View icon in the system toolbar, and the message window will show the following prompt: “Select CENTER POINT for drawing view.”

We will pick out in the middle of the drawing. Initially, the view appears in the default orientation, as shown in the next figure.

A properties window appears for the view, as shown in the next figure.

The first thing we will do is select the orientation for the general view. In the main portion of this window, we can see a list of saved views. We will scroll down, and double-click on TOP. When we do this, we can see the view update on the drawing. Click on OK to continue. Our view now looks like the following.

One of the things you might immediately notice about this view is that there are little letters enclosed in squares, with leaders going to triangular bases. These are called Set Datums (or Datum Features in ASME Y14). They are used in conjunction with geometric tolerances. This model has some set datums defined, and they appear on the view when we create it. We can clean these datums up on this view. First, look at the following figure.

The figure on the left shows the datum feature before we select it. We can see that there are two main components to this datum feature – a leader that identifies which surface/entity the reference is tied to, and the identifier, which gives the label for the datum. If we pick on this datum feature, it highlights in red, and we can see some little red squares appear (as shown in the figure on the right). The squares on the leader line can be used to move the leader endpoints. The square at the base of the identifier is used to move the text in and out from the base. If you place your mouse over the base, you will see a four-arrow symbol that allows you to move the datum identifier along the leader. We will clean up the leader lines so our datums look approximately like the following figure.

We will now go back and look at the view properties window for this general view.

GENERAL VIEW PROPERTIES When we place our mouse over the drawing view, we can see a light blue dashed rectangle appear. Click once to highlight the box in red. We can now right click and go to Properties which brings up the view properties window. (NOTE: We can also double-click on the view once we see the blue rectangle to get to the properties window).

On the left side of this window is a list of Categories that we can select for the particular view. The first category is View Type, which defines type of view, the system name for the view, and the orientation. We can see that the view type is grayed out (but indicates General). At this time, we have no other views on the drawing from which we could convert this to a different type (like projection, or auxiliary, etc.) We can also see the default system name for this view is New_View_2. The name can be shown on the drawing for projection views, or for defining templates. Finally, we can see that we have the ability to re-orient this view using the saved view list, or by picking on a different method for orientation. Visible Area The next category down is used to create broken views, partial views, half views, or to add z-direction clipping of the view (like cutting away the part from the point of view of the screen behind a certain planar surface) This category looks like the following for this general view.

We will come back in a later lesson to see how to create half, partial and broken views. For now, click on the Clip view in Z-direction box, and then pick the following flat surface on the view:

Click on Apply, followed by Close. What do you notice? All of the geometry beyond this flat surface is no longer visible in this view, as we can see in the next figure.

Go back into the properties window, return to the Visible Area category, and uncheck the box. Click on Apply. Now we will continue to the next category. Scale When we apply a default view, we have the ability to change its scale with respect to the current drawing scale. If you recall, the current drawing scale is 1:1. This means that as long as we print this drawing on the same paper size as the drawing format or

sheet size selected, the views will be at a 1 to 1 scale. A 1” dimension should measure 1” with a ruler. In Pro/ENGINEER, we don’t scale the model. We always create the 3D models at full scale. We only scale the drawing or drawing views. The Scale category for this drawing view looks like the following:

The default option is to keep the view at the current drawing scale. If we wanted the view to have a different scale, we would pick Custom Scale, and enter a value in decimal or fractional format (.5 or ½, for example). NOTE: It is better to scale the drawing if most of the views are going to have to be scaled, and then use this interface to scale selected views differently. You should not scale all general views on the drawing, and leave the drawing view at its original scale. We can also add perspective to a general view. Sections The next category is used to create cross-sectional views, or views of distinct surfaces of the model. It looks like the following for this general view.

Currently, the default option is No Section. If we wanted to add/create a crosssection (planar or offset), we would use the 2D Cross-Section option. We will demonstrate this in an upcoming lesson. If you want to create a view of a particular surface only (perhaps for calling out special instructions for painting or coating of a surface), you can use the Single part surface option, and then select the surface on the model. NOTE: If you do this, and then decide later that you don’t want this, you will have to delete and re-create the view. View States This category is used to define exploded views, simplified representations of assemblies, and mechanism snapshots. It looks like the following.

Because this view is of a PART model, and not an assembly model, these options are currently unavailable. View Display

The next category is used to define the display mode for the drawing and entities on the drawing. It looks like the following.

Currently, this view is in Wireframe display. Tangent edges (like those created by the round features), are currently displayed in Phantom mode (dashed lines). The hidden line removal for quilts is currently grayed out, because it is not applicable in Wireframe display mode. You can also define how colors, skeleton models, and weldments are displayed on the drawing view. We will change the display style from Wireframe to No Hidden, as shown in the next figure.

Click on Apply to see the model update. In this particular case, there is no difference for this view. Origin The next category helps you define the origin of the view. By default, the origin of a drawing view is at the center of the view. We can see a red square at the center of our view to indicate this when we select the view. If you wanted the origin to be at the corner or other location on a view, you could specify it here, and then you can use the X and Y coordinate locations to define the exact location of a view on the sheet. This category window looks like the next figure.

Alignment If we had other views on the sheet that came before this general view, we could align this view to one of the views. You might do this to align two general views, or a separate detailed view with its parent. The alignment category window looks like the following.

You specify whether the alignment is a horizontal or vertical one, and then you pick the references or view origins on the current general view to the other view.

NOTE: You are not converting the view to a different type, only lining it up with another view so they move together. Click on Close to get out of the properties window.

LESSON SUMMARY The first view in any drawing is a general view. Use the different categories in the properties window to further define the view once it is placed.

EXERCISES None

Les son

4 4 Lesson Objective: In this lesson, we will learn how to create projected and cross-sectioned views.

PROJECTED VIEWS Many drawings use orthographically projected views. These create 90 degree rotated views that represent such orientations as: FRONT, TOP, RIGHT, BACK, BOTTOM and LEFT. For this reason, we have created default saved views in the start parts. Depending on the product and company, you will have third angle or first angle projection. Third angle projection places the view on a plane that lies between the observer and the object. This is the most commonly accepted view configuration used in the United States. It looks like the following:

THIRD ANGLE PROJECTION First angle projection places the object between the observer and the plane where the view is created. This type of projection can be found in many countries outside of the United States. It looks like the following:

FIRST ANGLE PROJECTION By default, we use the third angle projection in our configuration settings. To enable first angle projection, you must set the drawing setup file option PROJECTION_TYPE to FIRST_ANGLE. For the rest of this training guide, we will continue to work with Third Angle projection.

ADDING PROJECTED VIEWS To add a projected view, you must have at least one general view already defined in your drawing. We will demonstrate a projected view with the drawing that we have been working on (Lesson41a.drw). We will start by selecting the general view that we created earlier so a red dashed rectangle appears around it, as shown in the following figure.

Next, we hold the right mouse button down over the view, and select Insert Projection View, as shown in the next figure.

Once we select this option, move your mouse cursor (without picking) over your existing general view. You will notice an orange rectangle that appears as your mouse leaves the boundary of the general view. Depending on whether you leave the boundary to the left, top, right, or bottom, you will get a different projection. We will move our mouse below the general view, and click to create a FRONT view (remember our first view was actually a TOP view). When you create this view, it appears initially with the red dashed rectangle around it. Click anywhere outside of the two views to clear this. Our drawing currently looks like the following.

We will first double-click on this view to go to the properties window. On the first category, View Type, you can see that this is a projected view.

We can see that the name of this projected view is Bottom_3, just because we came off the bottom of the existing view. We can also see that it lists the parent view as new_view_2, which (if you recall) was the name of our first general view. There is an option to Add projection arrows. This creates arrows on the first general view that we can move and clean up that indicate where this view came from. This is helpful if we need to move a projected view to a different sheet from the parent view. The only catch – you will want to show view names for this to be effective, otherwise you may not know which view it is. In the config.pro file, there is an option called MAKE_PROJ_VIEW_NOTES, which currently is set to NO. If you decide to use this, you have to have this enabled BEFORE you project your view to get the label to show up. Within the properties window, we will look at a couple of other categories which are different for this view than the general view. First, look at the Scale category.

Notice that we can not change the scale of this view. Why? A projection view always takes on the scale of its parent view. The only way to be able to scale this new view independently, would be to convert it to a general view (using the View Type category window). In the View Display category, change the display type from Wireframe to No Hidden. Finally, if we look at the Alignment category, we can see that, by default, there is an alignment between this view and the general view, as indicated in the following figure.

Click on Apply to make the display change to the view, and then close out of this window. On our drawing we see the following.

For the set datums on this view, we will start by selecting the “A” datum feature on the right side of this view. Once selected, right click and select Erase. This will get rid of this datum feature on this view. Next clean up the “C” datum feature as we did in the other view to get the following.

Save the drawing.

CROSS-SECTION VIEWS

For this lesson, we will learn how to create a cross-section view where a crosssection already exists. We will start by returning to the Lesson41a.drw drawing. We are going to convert our existing projected view into a cross-section view. Therefore, double-click on the projected view to get back to the properties for the view. Once inside the properties window, go to the Sections category. It will look like the following.

We are going to add the existing cross-section into our view. Therefore, click on 2D cross-section, and we will see the following.

We have a “+” button available now, so we will click on this to add a cross-section to this view. This will give us the following.

At this time, we can either select a cross section from the list (here we see “A” available), or we can click on Create New, and create a cross-section right inside drawing mode. We will select the existing “A” section. Once we select the crosssection, we can define how the section will be created. We have several options shown in the next figure.

The options are: Full – The entire model will be cross-sectioned in the view. This is the default. • Half – We select a datum plane perpendicular to the view, and select on which • side of the plane the model will be sectioned. Local – We sketch a boundary on the view, and only the portion of the model • within the boundary will be sectioned. Full(Unfold) – This section type works for offset cross-sections on axially • symmetric models (such as ones that are revolved). We will keep the default of Full. Above the list of sections, we can see some radio dials in a section entitled Model edge visibility. There are two options for this: Total – All model geometry will be visible past the cutting plane. • • Area – Only the cross-section will be visible – all geometry past the cutting plane will not be shown. We will keep the default of Total for this. At this time, we could add additional crosssections to this view. This would enable us to do a Full and Local type cross-section, by selecting one section to be full, and then sketching a boundary on top of this section to show another section that might lie further into the part. We are done once we add this section. Click on OK to complete this cross-section, and we will see the following on our drawing.

When we create a cross-section view, we have the ability to show arrows on another view to indicate where the section cuts through the part. To do this, we will first click on the section view to activate it, and then hold down the right mouse button to select the Add Arrows option, as shown in the next figure.

We are prompted to pick on the view to show the arrows. We will pick on the TOP view that we started with. When we do this, we can see the cross-section arrows, as shown in the following figure.

We can click on the arrows themselves to move them (and the text) to a new location. If we wanted the cross-section view to be flipped to see the other side, you would select the cross-section itself so it highlights in red, and then right click and select Flip Material Removal Side. We are NOT going to do this at this time. NOTE: When dealing with a projected cross-section view, flipping the material side technically means your view is now the opposite of what it was before. Therefore, our cross-section view (which is currently a FRONT view) would become a BACK view if we flipped the arrows, and therefore, should be positioned according to the first or third angle projection rules. To clean up our cross-section a bit, we are first going to move the view name. To do this, click on the text (SECTION A-A) so it highlights, and then move it to the following location.

Next, we will change the spacing of the cross-hatching, as it is a little too close together. To do this, click on the hatching itself so it highlights in red, and the right mouse click and select Properties. This brings up the following menu manager.

There are many different options in this menu. We will select on Spacing, which brings up the following menu.

We will keep the default option of Overall, to increase the spacing for all lines. Then, click once on Double to double the width of the spacing. We should see the update in our view. Now, before we exit out of this menu, we will click on Angle to see what options we have here. This makes the menu look like the following.

By selecting a value from the list, we can change the angle of the hatching. This would be important if we had an assembly with several members. Each member would have its own angle to avoid confusion between the boundaries of the models. We will now click on Done to finish this hatching change. Our view now looks like the following.

Save this drawing.

CROSS-SECTION TYPES In this section, we will explore the Half, Local and Area cross-section options. We will use the same drawing. Half Section In order to create a half section, we need to have a datum plane in the model that represents the break in the section. Therefore, go back to the model (Lesson41a.prt). Click on the “Create Datum Plane” tool, and then pick the cylindrical surface on the inside of the taller hole, hold down the Ctrl key, and select the RIGHT datum plane from the model tree. Be sure to use the Parallel option instead of Normal in the datum plane window. Our window will look like the following.

The preview of the new plane on our model should look like the following.

Click on OK to complete the datum plane. We should now have DTM1 in our model tree that we can use for this cross-section. Return to the drawing, and double-click on the existing cross-section view to get back to the properties window. Once inside the window, go back to the Sections category.

We will use the pull-down to change from Full to Half. When we do this, we are prompted to pick on the datum plane to cut the section. From the model tree, pick on the datum plane that we just created (DTM1). When we do this, we see a red arrow pointing to the side that will be cross-hatched, as shown in the next figure.

We will pick out to the left of the arrow (sort of near that red rectangle), which will cause the arrow to flip to the other direction. Click on OK to complete this crosssection. Move the view name text to clean it up, and your view will look like the following.

NOTE: Typically, half sections are used when you have a symmetrical object where cutting half away can give you (in one view) a good representation of the interior and exterior of the object. Our example doesn’t fall into this category, but it does demonstrate how to create a half section view. Local Section Now, we are going to create a local cross-section. To demonstrate this, go back into the properties for this section view. Return to the Sections category, and change the option from Half to Local. When we do this, we get the following message bar prompt: “Select the center point for a breakout to section < A >.” We will pick out in the middle of the view (on the blue line that appears when you place your mouse just below the little red square), and sketch an approximate circular spline as shown in the next figure.

Once you pick your last point (indicated by the “End Here” location in the previous figure), click on the middle mouse button. You will see the boundary close itself, and appear in blue, as shown in the next figure.

Click on OK to complete this cross-section view. We will see the view now looks like the following.

Area Section We will now create a Full, Area cross-section. To do this, return one more time to the properties window for this view, and return to the Sections category. Change the type from Local back to Full, and above the list of cross-sections, change the display from Total to Area. The window should look like the following at this time.

Click on OK, and your view will now only show the cross-hatching. All model geometry is missing from the model, as shown in the next figure.

We will go back one more time and change it back to a Total view with a full crosssection, to get back to our original cross-section view that we started with, as shown in the next figure.

Save and close this drawing.

LESSON SUMMARY Projection views are 90 degree rotated views off of existing views in the drawing. You can use first or third angle projection schemes in your drawings. When creating cross-section views, it is easier to create the cross-section in the model, and then show it in the drawing. You can use different types of cross-section definitions to get what you are after.

EXERCISES

None

Les son

4 5 Lesson Objective: In this lesson, we will learn how to create Auxiliary and Detailed views.

AUXILIARY VIEWS To demonstrate how to create an auxiliary view, we will open up a drawing called Lesson45.drw. It will look like the following.

This drawing uses a B size sheet, and the 1abc.dtl drawing setup file has been applied. No drawing format has been applied at this time. Three views exist on this drawing already. The first view (General View) is the front view in the lower left corner. The second and third views are projected views to make the TOP and RIGHT views in the drawing. We are going to add an auxiliary view in the upper right corner of this drawing. Therefore, we will go to Insert, Drawing View, Auxiliary from the menu bar. This will give us the following message bar prompt: “Select edge of or axis through, or datum plane as, front surface on main view.”

Since an auxiliary view is often created from an angled surface, we will pick on the edge indicated in the following figure.

When we select this edge, an orange square appears showing us the location of the view to place it, as shown in the next figure.

As you move your mouse, you will notice that the view stays in a line normal to the edge that we selected. We will drop the view in the upper corner of the “invisible” square that makes up the views, as shown in the next figure.

At this point in time, we will drag all of the views in towards the general view to get them a little closer together. This is optional, as we have not added all of the dimensions yet so real-estate might be a problem if the views are close to each other, but we will need some room for our detailed view that we will add next. Our drawing (with the views closer together), looks like the following.

Save the drawing.

DETAILED VIEWS

A Detailed view is a drawing view that represents only a portion of the parent view from which it comes, but it is intentionally scaled independently so we have the ability to “blow up” the magnification of the view to see more detail – hence “detail” view. We are going to create a detail view that zeros in on the top of the auxiliary view that we just created. Therefore, we will go to Insert, Drawing View, Detailed. When we do this, we get the following prompt in our message bar: “Select center point for detail on an existing view.” We are going to pick in the following location.

When we pick here, a solid red dot appears on the model, as we can see in the next figure.

And, in our message bar, we see the following prompt: “Sketch a spline, without intersecting other splines, to define an outline.” We are going to sketch a spline (similar to how we did it for the local cross-section boundary in the last lesson) as shown in the following figure.

When we pick our last point (indicated by “End Here” in the figure above), click on the middle mouse button, and you will see a dashed circle appear around the region with text indicating “SEE DETAIL A”, as shown in the next figure.

In the message bar, we are prompted to select the center point for the view on the drawing. We will pick out to the left of our existing four views. When we do this, we see the new detailed view, as shown in the next figure.

Okay – a couple of things to point out. By default, the new view comes in at a 2X scale to the existing drawing view scale. The boundary of the detailed view is a circle by default. Also, the name of the detailed view is assigned at “A”. We want to change all of these things at this point. Scale To change the scale of this view, simply double-click on the “2/1” text in the detail view name. In the message bar, type in 4, and then hit the <ENTER> key on your keyboard. The view will enlarge by a factor of 2 again, as shown in the next figure.

NOTE: You must first select the entire note, and then you will notice that the “2/1” text highlights independently. Once you see it independently highlighting, that is when you double-click on it to change the value in the message bar.

View Name In this drawing, it is okay that the detail name is “A”, because we currently do not have any section views that may already be using this designation. As a general

rule, view names should never repeat themselves, even if one is a section and the other is a detail view. To demonstrate how to rename a view, we will change the name of this view to B. To do this, double click on the “A” note in the view name, and enter “B” in the message bar. The following figure shows the new view name (in both locations). NOTE: You can change the name in either location where it appears.

Boundary Shape By default, the boundary is approximated into a circle with the minimum radius being the maximum distance from the filled in dot to the sketched boundary at the time we made the view. We can use other shapes for our boundary (Ellipse, H/V Ellipse, Spline and ASME 94 Circle). To edit this, we will click on the detailed view so it becomes selected, and then right click and go to Properties. This brings up the properties window for this view, as shown in the next figure.

We can (of course) rename the view here as well. On the View Type category, we can see an option entitled Boundary type on parent view. It is currently set to Circle. If we use the pull-down, we can see the other options.

We will select the Spline option, just to show you something different. Click on OK when you are done, and your view will update as follows.

NOTE: You may need to move the text around on the parent view to get it to be the way you want it, as shown in the figure above. One last thing to mention. In our properties window, we saw a check box labeled Show boundary on detailed view. If our sketched boundary intersects view geometry, leaving this checked will show a solid line where the boundary exists. We can see this in the lower right corner of our detailed view. If you were to uncheck this option, then the boundary will not show. The boundary edge that is out in space (not touching any of the model) will not show regardless. Save and close this drawing.

LESSON SUMMARY

An Auxiliary view is a projected view that is normal to an angled surface in the model. A detailed view takes a portion of the parent view that you sketch around and blows it up into an independent view. The boundary can be changed to one of a variety of formats. Both views are accessed through the menu bar.

EXERCISES None

Les son

4 6 Lesson Objective: In this lesson, we will learn how to show axes on our drawing view, and also how to show GTOL Datums. We will have a general discussion on the Show/Erase tool as well.

SHOWING AXES If your model has holes, slots or cylindrical surfaces, you will want to show axes in your drawing view – especially if you intend to dimension to these axes. All axes should exist in the model prior to showing them in the drawing. Most cylindrical-like features in Pro/ENGINEER generate axes. Full Rounds, for example, do not, so they will need to be added afterwards. To demonstrate this functionality, we are going to open up a drawing entitled Axis_Model.drw, which initially looks like the following.

This drawing consists of three views. The upper left view is a general view oriented to the TOP saved view. The second view is a projected section view (using a Full(Align) section type so it unfolds the geometry). The third view is a general view in a TRIMETRIC orientation, and at a ½ scale.

For the first and second view, we want to show the axes that go through the two holes, but we don’t want axes on our general view. SHOW/ERASE TOOL Therefore, to show axes, we will go to View, Show and Erase from the menu bar (or select on the Show/Erase icon in the drawing toolbar). This brings up the following window.

This tool is used to show most of the detail-oriented entities in the model, such as axes, dimensions, notes, GTOLS, etc. The figure above shows what each of the individual buttons are for. The most important thing to note when you enter this tool is whether you are in SHOW or ERASE mode. The tool will start out in the last mode that was used in the same session. Once you have selected your mode, you pick on the object button(s) you wish to control. You can show more than one type of entity at the same time, although I highly recommend against it. For a simple model like this, it might be okay, but when you have hundreds or thousands of features in your model, it can get very messy very quickly. My advise is to start with axes, and then move on to dimensions, and then on to more specialized entity types. Therefore, we are going to pick on the Axes button, which will make the window look like the following.

In the Filter region of the tool we have the following options: Feature – When you select on a feature in any view, it shows the axis in all • views for that feature. Part – Shows all of the axes for a selected part (usually use this in assembly • mode where you have more than one part) View – Shows all of the axes for a selected view. All other views will not show • axes yet. Feature and View – Shows the axes for the particular feature, but only in the • view where you picked the feature. All other features and views will not show the axis yet. Part and View – Shows the axes for the entire part in a selected view. Again, • this is used more in Assembly mode. Show All – Shows all axes in all views. For part mode, this would do the same • as the Part option. Okay – here’s my advice on selecting a filter. If your model is small in terms of the number of features, and the amount of entities that might be shown, then using Show All is faster for getting all of the entities to show up. Then, you can optionally keep or remove entities from the preview, or erase them later. The disadvantage of “Show All” is the fact that it will take you longer to perform a clean-up of entities. If the model is very complex with a lot of features, I recommend using the Feature or Feature and View options, because you may not want all of the dimensions for the entire part shown. The disadvantage of using these two is that to show all dimensions for an entire part, you would have to pick on each feature in turn, where a “Show All” would do it in one shot. As you show the entities per feature, you can then clean them up and move on to the next feature. We are going to keep the default of Feature selected, and pick out on the large revolved protrusion as shown in the next figure.

When we do this, an axis will show up in each of the views, as we can see in the next figure.

We could continue to pick more features, but we will click on the middle mouse button at this time to accept our current selection. When we do this, we get the following.

At the bottom of this window, we have four options for dealing with the entities that have appeared on our views. These options are: Sel to Keep – (Select to Keep). Only axes that we pick on the views will be • kept when we are done, all others will be erased automatically. Sel to Remove – (Select to Remove). Only axes that we pick on the views will • be erased, all others will be kept. Accept All – Keeps all of the axes that we see on the screen. • Erase All – Cancels the current show/erase by erasing all axes that popped up • on the screen. We only want to get rid of the axis that appeared on the general trimetric view. Therefore, we will pick on the Sel to Remove button, and then pick on the axis on the general view. It will highlight red when we select it. We could hold down the Ctrl key and select additional axes to remove, but we are done at this time. When we click on the middle mouse button to finish selecting objects to remove, we are left with the following.

As you can see, the axis is gone from the general view, but still remains in the two other views. Click on Close to get out of the Show/Erase tool. Now, we have some clean-up to do on these axes. RESIZE AXES If we zoom in on the first general view we created, we can see that the axis is very small. Normally, when you show axes on a drawing view, the axis lines extend beyond the cylindrical surface to which they apply (and sometimes even longer if the axis represents other items on the model, such as a bolt pattern). When we zoom in, we see the following.

We can see the tiny axis that we just showed on this view. When we pick on the axis, we can see it highlight in red, and little red squares appear at the ends of each of the axis lines, as shown in the next figure.

You can drag the axis lines independently of each other by placing your mouse over the square and drag it. The following figure shows such a drag.

This is useful if you need to extend one or more of the lines further than the others. To resize all of the lines at once, place your mouse over the selected axis until you see four arrows on the mouse icon. Then drag out one of the axis lines. The following figure shows what we want to end up with.

Once you have the axis looking the way you want, click on the drawing outside of the view to de-select it. Our axis on our view now looks like the following.

We will go to the cross-section view, and drag out the axis on both sides just to make it a little more clear that this is an axis, as shown in the next figure.

Remaining Axes We still have one more axis we have to show for these two views, the one that goes through the hole in the handle. Repeat the same process that we just went through to create the following.

NOTE: You don’t want to have any axes on the second general view, and you may want to use Sel to Keep this time instead of Sel to Remove (fewer items to pick). You also may be wondering why the axis in the big hole showed up again. When creating the handle, a “Use Edge” command was used in the sketch, which grabbed the outer edge of the revolve feature, thus creating another axis for this feature. ROTATE AXIS Another thing you may wish to do for your axes, is have the axis lines rotated to line up with the model edges. On our first general view, we might want to do this for the new axis that sits on the handle. To rotate an axis, you first select the axis, as shown in the next figure.

Next, right click on the axis and select Edit Attachment, as shown in the next figure.

This will bring up the following menu manager.

We can use a variety of methods for defining the angle for the axis, but we will pick Parallel on the menu, and then select the following edge.

When we do this, the axis rotates as expected.

Now, we will resize one of the axis lines to bring it back just outside the small circle, as shown in the next figure.

Click anywhere outside of the view to de-select the axis, and save the drawing.

GTOL DATUMS If you recall from our Lesson41a drawing, we saw some geometric set datums. These datums were planes created in the model, and then converted over to set datum features. We will go through an example using our current model (Lesson45) to show how to create set datums. Therefore, open up the axis_model.prt model. Currently, we have all of our default datum planes turned off on a layer. That is okay, because when you create set datums, you should use new datum planes instead of existing default datum planes. Why? In the process of creating the set datums, we will give the datums new names (A, B, C, etc.). We don’t want to rename our FRONT, TOP or RIGHT datum planes, or our default axes, as well in this process. AXES AS SET DATUMS We will start by going to our layers, and turning on the AXES layer, and then save status. Turn on the visibility of axes and you should see two axes on the model, as shown in the next figure.

We want to create a set datum on the A_5 axis. To create a set datum, we will go to Edit, Setup from the menu bar. This brings up the following menu manager.

We will click on the Geom Tol command, which brings us to the next menu.

Within this menu, we can create inspection and basic dimensions, and create our set datums. We will pick on Set Datum, and then pick on the A_5 axis on the model. This brings up the next window.

On the model, we can see a box around the dimension, and dashes on either side of the name, as shown in the next figure.

We have two different ways we can place this datum. The first is Free, which keeps it tied to the axis itself. This is the one shown above. The second is In Dim, which ties the datum to a selected dimension (usually a diameter or radius in this type of selection). We will keep the default of Free selected. You may also notice two buttons in this window. The First button, labeled A, is used to unset the axis if it was previously set as a datum. The button labeled -A- is used to set a datum. We will leave this latter button pressed. The last thing we need to do for our axis is rename it. We will give it a name of A. Click on OK to complete the definition, and we will see the following on our model.

PLANAR SET DATUMS We will now create a planar set datum. Therefore, turn on the display of datum planes, and then create a new datum plane through the bottom planar surface of our part (not the side with the handle). Rename the plane to B. Our model should currently look like the following.

Now, I am going to show you a different way to set datum planes/axes as set datums without having to go through the Edit, Setup, Geom Tol, Set Datum menu structure. Right click on this datum plane in the model tree and select Properties. This brings up the following window.

Click on the -A- button to turn this into a set datum, followed by OK. We will now see the datum symbol on the datum plane on the model, as shown in the next figure.

Now we are ready to show these datums on our drawing. If we switch back over to our drawing file, we can see that our planar set datum is there already.

In fact, we can see two set datums right now. The reason for this is the nature of the cross-sectional view. Since this is an “unfolded” or “aligned” cross-section, it is almost like two separate views in one, and that is why we are seeing two datums. We will pick on the middle datum so it highlights in red, and then using the right mouse button, select Erase. Then, clean up the remaining datum to look like the following.

Now we will show the axis set datum. To do this, go to View, Show and Erase and you get the following window.

To show axis set datums, we actually have to show axes again. Therefore, we will click on the Show button, and then the Axis button. We will use the Show All this time. When we do this, we get the following:

Remember, a show all may give you a very cluttered screen to sift through, so you get a prompt asking if you are really sure you want to do this. We will click on Yes, which will bring back all axes, including ones that we didn’t select before, and the default datum axes as well, as shown in the next figure.

The default option at the bottom of our window is Sel to Keep, and we will keep this selected. On our cross-section view, we will select the box with the “A” inside it, as shown in the next figure.

Click on the middle mouse button once you have selected this set datum. The rest of the axes disappear, and we are left with just the newly added set datum for the axis. Move the datum to clean it up as shown in the next figure.

So, you might be wondering why we didn’t need to show the set datum planes, and yet there is a button on the show/erase tool to show these. Actually, these are the only set datums that come on by default. If you erase a set datum, as we have in this lesson, you can use the show/erase tool to bring them back. Save and close this drawing.

LESSON SUMMARY The Show/Erase tool allows you to turn on/off many entities in your drawing. In this lesson we saw how to show axes using some of the different ways to use this tool. We also learned how to create set datums for axes and planes, and show them on the drawing.

EXERCISES None

Les son

4 7 Lesson Objective: In this lesson, we will learn how to show and create dimensions in our drawing.

SHOW VS. CREATE – THE GREAT DEBATE One of the biggest debates in the Pro/ENGINEER community is the question of whether you should show dimensions that are in the model, and design accordingly, or whether you will just simply create dimensions in the drawing. The reality is that it depends on several things: 1. Product Definition – If we are talking about fixtures, sheet metal parts, or parts that have predominantly linear or cylindrical surface definitions, then I personally feel that users should show more dimensions than create. For products that are defined with many swoopy 3D curves and surfaces, the availability of well-defined dimensional constraints in the model is less, so showing dimensions may not present a realistic solution to creating drawings. 2. Fit, Form and Function versus Manufacturability – The other driving factor is whether it is possible to capture manufacturing dimensions in the model and preserve design intent. This is, perhaps, one of the biggest cases made for creating dimensions. For an example, we will look at the following bracket design:

Suppose that the bracket in the previous figure must be designed so that it always mounts perfectly depending on the spacing of the two posts. Another requirement might be that the outside of the bracket must line up perfectly with the outside edges of the posts. Therefore, the direct spacing between the holes is critical for satisfying the first condition, but the overall width of the bracket can not be specified and still maintain design intent for the second condition. Instead, the dimensioning scheme for the model might have to be created as follows.

From the previous figure, we can see that the dimension between the two holes is defined, and the distance from the hole to the outside of the bracket on each side is defined. This scheme will allow us to take the width of the posts, as well as the spacing of the posts into consideration for our bracket design. Unfortunately, we can not manufacture the bracket this way, because we would first start with the metal and bend it to form the main geometry of the bracket, and then put the holes in afterwards. Therefore, on the drawing, we might have a different dimensioning scheme, as indicated in the next figure.

Another possible manufacturing scheme might be…

As you can see, both of these schemes allow for the creation of the bracket geometry first, and then the holes second. Unfortunately, all three modes potentially create a different result based on dimensional tolerances. The good news, you can combine both schemes into the drawing, by showing the fit, form and function dimensions, and then specify the overall length as a reference, or a “Basic” dimension, and then specify the three shown dimensions as critical or “inspection” dimensions, as shown in the next figure.

In this lesson, we will see how to do both – show dimensions in the drawing that were created in the model definition, and how to create dimensions directly on the drawing.

SHOW DIMENSIONS To demonstrate this functionality, we will open up the drawing called Show_Draw.drw. It currently contains four views, as shown in the following figure.

Our first general view creates the front view in the lower left corner. We then added a projected view off of this towards the top to create our next view. From that TOP view, we projected another view, and made it a section view (Section A). From the first general view, we projected a RIGHT view, and used an offset crosssection for this view (Section B). On the views, you can see axes where appropriate, and you can also see three set datums for this part (A, B, and C – on the FRONT and TOP views). We are now going to show the dimensions for this part. Therefore, we will go to our Show/Erase tool in our drawing toolbar (the one that looks like a flashlight), or go to Edit, Show and Erase from our menu bar. We get the familiar show and erase window. We want to make sure that the Show button is pressed in, and that the first dimension button is pressed in. All other buttons should be depressed, as shown in the next figure.

For this example, we will click on the Show All button (since we don’t have that many dimensions on our model). We get the confirmation window, as shown below.

Click on Yes to confirm showing all of the dimensions in the model. When we do this, dimensions show up on the drawing views where they are able to be shown, and we will pick on the Accept All button in our Show/Erase window. When we do this, all of our dimensions are currently highlighted in red, as shown in the next figure.

It keeps the dimensions highlighted until you click on the refresh button. We will zoom in on the TOP view first to clean up the dimensions. CLEANUP DIMENSIONS If we zoom in on the TOP view, we can see the following.

We only have seven dimensions on this view so far, so dragging each one to clean up the view isn’t really that big a deal, however, we will take a moment to show the cleanup tool. First, click anywhere on the drawing (away from any entity), and the dimensions will de-select. We can use the clean-up tool to clean up all dimensions on the drawing, but we will just focus on this view right now. Once all of the dimensions are no longer selected, drag a box around this view (make sure it is big enough to go around all of the dimensions. Do not worry if it gets a dashed border around the view as well. Once you have all of the dimensions highlighted for this view, go to Edit, Cleanup, Dimensions, from the menu bar, which brings up the following window.

We will take a moment to talk about this window, and what it does. First of all, we notice at the top that it says 3 Selected. If you remember, we have 7 dimensions on this view, so why is it only reporting 3? Only linear dimensions are affected in the cleanup process. Diameter/Radius dimensions are not included. If we look at the view, we can see that we have only 3 linear dimensions (the width of the block (10”), the height of the block (8”), and the width of the protrusion on top of the block (2.5”)). The next thing we see are two tabs. The first tab, which is currently selected is Placement. The first thing we can define in this tab is how it spaces out the linear dimensions. If you notice, we have only one linear dimension on the right side of this view, but we have two dimensions on the bottom of this view. When we space out the dimensions, one of the dimensions will start out a distance away from the view specified by the Offset value. In this case, our first dimensions will be spaced 0.5” away from the view. The next dimension, and the one after that, and so on will be spaced according to the Increment value. On the right side of the view, we only have the one dimension, so it will sit out 0.5” from the view. On the bottom side of the view, we have two dimensions, so one of them will sit out 0.5” from the view, and the second will sit out 0.375” from the first one. So, what determines the starting point for the offset value of 0.5”? Currently, the Offset Reference is specified as the View Outline. In other words, when you pick on a view, and you see a dashed rectangular border around the view, that is the view outline. Therefore, the first dimension will be offset 0.5” from the dashed rectangle. If you want to use a different reference, such as an edge of the model, you can select the Baseline option, and choose the reference. We will keep it as the “View Outline”. Finally, we have the option to create snap lines and to break witness lines. A Snap Line is a dashed, muted line that only appears electronically on the drawing, and is used to allow you to snap dimensions to it. If we were going to show more dimensions later, we could snap the newly shown dimensions to the existing snap lines. If we select this option, we will get snap lines at 0.5” from the border, and

0.375” from the first snap lines for any additional dimensions that we have. We will leave this option selected right now. By default, we don’t have the Break Witness Lines option selected. A “Witness Line” is the leader line that goes from the dimension back to the geometry. If you have lines that overlap in the drawing, you can have one of the lines broken so there is a small gap, as shown in the next figure.

The figure on the left above shows overlapping witness lines without a break, while the figure on the right shows the witness line for the 8.0” dimension broken to make it easier to see the lines. This is a cosmetic feature, but I recommend it. Now, in our drawing, none of the linear dimensions will overlap witness lines, so we really don’t have to worry about checking this option. For now, we will change the two offset values as follows: Offset = 1.0, Increment = 0.5. The Placement tab should now look like the following.

Now, we will click on the Cosmetic tab, which looks like the following figure.

On this tab, we have some additional ways to control the look of the dimensions and arrows. If the witness lines are too close together, the system can automatically flip arrows to the outside of the lines. We can also center our text on our lines. We will leave both of these options selected. Down in the lower part of this tab, we can see how to adjust our text if we have to place it outside of the witness lines. We will leave the default options of placing the text to the left and/or top (depending on the orientation of the dimension). We will now click on Apply to see how these settings affect our view. We see the following.

We can see that our linear dimensions have moved to the outside of our drawing view. We can also see that there are three dashed snap lines. One is really obvious – the one that the 2.5” dimension sits on. The others are harder to see, because the dimensions and leader lines are sitting right on top of them. For this drawing view, we really didn’t have to use the cleanup tool for only three dimensions, but it was a good exercise to learn how to do it, because, if you have a model with a lot of features, and you decide to use the “Show All” option, you can perform an initial clean-up that will make it easier to come back and perform your manual clean-up later. If we didn’t like the way the clean-up looked, we could click on the Undo button, and reset our values, and re-apply the clean-up. We will click on Close to accept this clean-up. Click outside of the view to de-select all dimensions. MANUAL CLEANUP Staying on this view, we will perform some manual clean-up. Just as we did with axes and GTOL datums, we can drag dimensions around to where we want them. If we pick on one of the squares at the end of leaders or witness lines, we can control the length of the lines, and the distance of the text. We will drag our dimensions around so we are left with the following.

Since we moved our dimensions off the snap line, we probably don’t need them anymore. Therefore, click on a snap line, and then hit your key on your keyboard. Click outside the view to refresh it. HINT: As you drag a dimension, if you click on the right mouse button, it flips the arrows on-the-fly. Now, we will go to the FRONT view. It currently looks like the following.

Okay, we can see that this view has several things that need to be fixed. All of the linear dimensions across the top describe holes in the model. The problem is that we can not see the holes on this view.

NOTE: Even if you were to turn on hidden line display for this view, it is against ASME Y14 standards to dimension to hidden entities. We will have to move these dimensions to a view where we can clearly see the holes. MOVE ITEM TO VIEW To move a dimension from one view to another, we first select the dimension to move. In this case, select the 7.000, and 1.500 linear dimensions at the top of this view using the Ctrl key to get both of them. Be sure not to select the 0.250” radius dimension, or the 5.000” linear dimension. Once these dimensions are selected, hold down the right mouse button over one of the selected dimensions, and select Move Item to View. (You can also access this through Edit, Move Item to View from the menu bar). We must now select the view we want to move them to. We will select on the Section A-A view (at the top of our drawing). When we do this, the dimensions leave the FRONT view, and jump to our section view, as shown in the next two figures.

FRONT VIEW

ALIGN DIMENSIONS When you have two linear dimensions that are next to each other, as we do in our section view, we can line them up on the same horizontal or vertical without having to use snap lines. In our Section view, we want to move these dimensions above the view, so the witness line for the 7.000” dimension doesn’t cut through the view, overlapping the geometry.

Therefore, we will select both of these dimensions using the Ctrl key, and then right click on one of them and pick Align Dimensions. When we start dragging, we can see that both dimensions move at the same time. We will drop the dimensions as shown in the next figure.

Notice that when we do this, our witness lines are still embedded in the drawing. One thing to point out is that when you print out this drawing, the witness lines will clip back to the ends, but from an electronic viewing, this is still messy. I personally like to keep my drawings clean on the screen as well. Therefore, we will drag our witness lines to clean them up as shown in the next figure.

Return to the FRONT view, and we will clean up the dimensions as shown in the next figure.

Again, we will have to move one more dimension. The 5.000 dimension goes to the center of the large hole. We will need to move this dimension to our TOP view. Therefore, click on this dimension, hold down the right mouse button and select Move Item to View, and then pick on the TOP view. Clean up this dimension as shown in the next figure.

This was the only view that would accommodate this dimension, because it is the only view that has the center of the large hole visible, and where we can see the right edge of the model where the dimensions goes to. Finally, we will go to the Section B-B view to clean it up. It currently looks like the following.

We can keep two of these linear dimensions, but we will need to move the 5.000 dimension to the TOP view. This view, when cleaned up will look like the following.

Clean up the TOP view once more for this newly moved dimension. NOTE: You may need to move the section view arrows for A-A to get it clean, as shown in the next figure.

FLIP ARROWS On two of our view, we may wish to flip the arrows of some of the dimensions to clean it up a bit. Go to the FRONT view. As you can see, we have a linear dimension on the left side for the height of the plate. We are going to demonstrate how to flip arrows and we want to move the dimension over to the right side of the view, where it makes more sense to show it. Just Flipping the Arrows If you don’t want to move the dimension, just flip the arrows, you select the dimension first, and then hold the right mouse button down and select Flip Arrows. We will do this first for the 1.0 dimension. When we do this, our view looks like the following.

Flipping Arrows While Moving Now, we will click on the dimension to move it to the right side. As you are dragging the dimension, try clicking with the right mouse button. What happened? The arrows went back to the inside of the witness lines. Click once more with the right mouse button (while still dragging), and you will see the arrows flip back to the outside. Place the dimension and clean-up as shown below.

This works just as well for radius and diameter dimensions, as well as angular dimensions. At this point in time, our dimensions are all placed, as shown in the next figure.

Save this drawing. We will continue to work with it in the next section.

EDIT MODEL THROUGH DRAWING One of the advantages of shown dimensions is the ability to make design changes from within the drawing. Created dimensions are read-only, but shown dimensions are fully associative and parametric with the model, since they came directly from the model definition. To demonstrate this, go to the TOP view in our drawing. It currently looks like the following.

We want to change the large hole diameter from 3.000 to 2.000. Therefore, click once on the 3.000 diameter dimension to select it, and then double-click on the “3.000” text. (We will explain in a minute why we did this in a two-step select process). When we do this, an edit field appears on the dimension, as shown in the next figure.

Change the value to 2.0, and then hit the enter key. Now, using Edit, Regenerate, Model or click on the following icon in the system toolbar:

The model will regenerate, and the drawing view will update to show the new geometry and dimension value, as shown in the next figure.

If we look at our Section B-B view, we can see that the cross-section has updated as well.

If we open up the model, we can see that (as expected) the hole is at the smaller diameter.

This is a two-way associativity. If we make a dimensional change in the model, it updates the drawing as well. In the case of created dimensions, the dimensions will update, but you can not drive the model from the drawing with created dimensions. Save the model and close it. Save the drawing, but leave it open for the next section.

CREATE DIMENSIONS

As we talked about in the beginning of this lesson, there are many times when you may need to create a dimension in your drawing instead of showing one. My absolute advice is the following: 1. 2.

Rule 1 – If you have the dimension already in the model, always show it. Rule 2 – If the dimension is going to be an inspection dimension (critical), it should probably be in your model to drive changes to the model, and to perform any necessary analysis on the dimension as you are designing. Critical dimensions should typically be shown dimensions (not always, but I make it a habit of trying to do it as much as possible). 3. Rule 3 – If you need to dimension to geometry within a cross-section, you might want to create a cross-section datum curve first so you have welldefined entities (edges, vertices, etc.) to select from when dimensioning. Often it is difficult in drawing mode to select the entity you want. You can then hide the curves in layers when done. 4. Rule 4 – Avoid creating draft geometry to facilitate dimensioning. In a later lesson, we will learn all about draft geometry. For now, suffice it to say that it is easier to create the geometry as curves in the model and then reference these entities in the drawing. You can always hide this geometry in layers when you are done.

I can not stress the importance of following these rules. If you don’t you may find yourself frustrated with using the tool the way it was not intended to be used. Having said all that, we will get into learning how to create dimensions. To demonstrate this functionality, we will return to our drawing that we’ve been working with in this lesson. Go to the Section A-A view. We are going to create couple of dimensions for this view just to show how it is done. NOTE: You want to avoid an over-dimensioned drawing. Because all of our current dimensions are shown, and we are showing every one from the model, any ones that we add as standard dimensions now will over constrain the drawing, and could confuse manufacturers – especially if we specify conflicting tolerances. So, we will put aside common sense for the purpose of this exercise. Standard Created Dimensions We will start by adding a radius dimension to the round at the right side of this section view. Therefore, we will go to the create dimension tool on our drawing toolbar, or go to Insert, Dimension, New Reference. Pick once on the arc shown in the next figure.

When we do, it highlights in a bold red, as shown in the next figure.

Now, click with the middle mouse button where you want the dimension to be, and you will get the following.

Try to change this dimension value here in the drawing. What happens? Down in the message bar, we get the following error:

Now, we will add a linear dimension from the axis of the left hole to the right edge of the protrusion sticking out of the plate. Therefore, click on the create dimension tool again, and this time start by picking on the axis. It will highlight in red. Next select the right edge, and it will highlight in a bold red, as shown in the next figure.

Now, using the middle mouse button, pick outside of the geometry below, and in between the two selected references to place the dimension as shown.

We can clean up created dimensions the same way we clean up shown dimensions. Therefore, flip the arrows to get the following.

Save the drawing. CREATED REFERENCE DIMENSIONS Whenever you need to add a dimension that is not critical, but may potentially over constrain the drawing, you should use a reference dimension. Tolerance is not applied to reference dimensions, so be careful which dimensions you choose to consider “for reference only”. To create a reference dimension, you would select Insert, Reference Dimension, New Reference, and then select the references as you would with the creation of any type of dimension. We will create a reference dimension for the distance from the left edge of the section view to the left hole axis, as shown in the next figure.

We can see the parenthesis placed around this newly created reference dimension. We will flip the arrows and align this dimension to the other two linear dimensions to clean it up as we can see in the figure above. As a typical rule, reference dimensions are the most commonly “created” dimensions in drawing mode. You can, however, create reference dimensions in the part and show them in drawing mode – the choice is up to you. I personally find it easier to create reference dimensions in the drawing. Save the drawing and close it. We will come back to it in a later section of this lesson.

ORDINATE DIMENSIONING If you recall from Lesson 4 – Sketcher Basics, we learned how to create ordinate dimensions when sketching a feature (Pg 4-22). Sometimes, you don’t have the luxury of having the forethought to use ordinate dimensioning from the start. Once you get to the drawing, you might think it is too late to show ordinate dimensioning, but it isn’t. In this section, we will learn how to convert a set of linear dimensions to ordinate dimensions. To do this, we will open up a drawing called Ordinate.drw, which currently looks like the following.

Okay, let us first take a look at this drawing and point out a couple things. The first is that any radius or diameter dimension can not be converted to an ordinate dimension. The second thing we notice is that in the horizontal direction, we have two linear dimensions that represent the distance between similar holes (8.000 and 5.000 dimensions at the top of the FRONT view). In order to convert dimensions from linear to ordinate, the witness lines for the dimensions must share the same reference. For example, all of the linear dimensions at the bottom of the FRONT view all reference the left edge of the model. Therefore, all of these can be converted to ordinate dimensions using the same baseline (where the dim is 0.0). The two hole spacing dimensions at the top of the view do not share a common reference with each other or with the linear dimensions at the bottom. Therefore, we will either leave these as linear dimensions

in this drawing, or go back and edit the sketch for these features and change the dimensioning scheme. NOTE: Remember your design intent. If the fit, form or function of this drawing requires the distance between the holes to be maintained, then you should leave them as linear dimensions in the drawing. For the vertical dimensions, all of them reference the bottom edge of the model, so all of these can be turned into ordinate dimensions. We will now demonstrate how to do this conversion. First, start by selecting all of the linear dimensions at the bottom of the FRONT view, as shown in the next figure.

With these four dimensions highlighted, go to Edit, Toggle Ordinate/Linear. When we do this, we see the following.

We have a “.000” baseline at the left of our model, and all the other dimensions for the holes and the plate are in ordinate dimensions. We can use the Align Dimensions command to clean them up as shown.

Now, select the three linear dimensions on the left side of the view, and the one on the right side of the view using the Ctrl key, as shown in the next figure.

Once all four dimensions are selected, use Edit, Toggle Ordinate/Linear once more. We will get the following ordinate dimensions.

Align the dimensions, and clean up the view as shown in the next figure.

Save and close the drawing. BACK IN THE MODEL So, what effect did converting the dimensions do to the model? If we open up the Ordinate.prt model, and edit the second extrude feature. We will see the following.

As you can see, the dimensions are now in ordinate form in the part as well. Remember, these were associative, shown dimensions, so they updated automatically. So, this begs the question, can you do this with Created Dimensions?

The answer is yes. As long as your created dimensions are going to the same reference (in this case the left edge of the model), we can toggle them to ordinate as well. Close this part.

SKETCHER TO DRAWING When you are showing dimensions on a drawing, the approximate placement of the dimension will be as it was when you sketched the feature that created that dimension. So what does this mean? If you get in the habit of cleaning up your sketches as you make features, you will have a lot less clean-up to do in drawing mode. To demonstrate this, we will go through an example. Create a brand new part called Sloppy. Create an extrude feature using the TOP datum plane as the sketching plane, and face the RIGHT datum plane towards the right. Create the following sketch (be sure all dimensions are strong and located exactly where you see them in the next figure).

Now, extrude this to a depth of 1.0 to create our model, as shown in the next figure.

Now, we will go and create a new drawing called Sloppy, and use a C size sheet, as shown I the next figure.

Create a general view and use the TOP saved view to orient it. Next, go to the Show/Erase tool and show all dimensions. This is what you will get when you Accept All.

Notice how the dimensions came in exactly as they were in the sketch? Think this is a coincidence? Go ahead and close out of this drawing and close the part, and create a brand new part called Clean. Create an extrude using the exact shape and size as before, but clean up the dimensions in the sketch to look like the following.

Extrude to 1.0 to complete this model, and then create a new drawing called Clean. Use the same sheet size of C, and make sure that the model is the Clean.prt file that we just created. Add a General view, and use the TOP orientation as before. Show all dimensions, and accept all that show up. Notice a difference?

As we can clearly see, the time spent cleaning up our sketch is well worth it if we know we are going to show dimensions in our drawing. I would get in the habit of cleaning up your sketches anyway, because someone may inherit your model later, and it will be easier to figure out what you were doing with a clean sketch (remember, don’t leave any weak dimensions either). Close these models without saving.

DIMENSION PROPERTIES When you show or create a dimension on your drawing, it takes on the characteristics of the drawing setup file in terms of text height, text spacing, arrow size, arrow length, etc. There are a lot more things we can do with dimensional properties within the drawing itself. To demonstrate this, go back to the Show_Draw.drw drawing that we started with in this lesson. It should currently look like the following.

We will go into the FRONT view in the lower left corner, which currently looks like the following.

Do you remember when we changed the dimension of the model directly in the drawing? Do you remember how we clicked once to select the dimension, and then double-clicked to edit the dimension? Well, if we were to simply double-click on a dimension (shown or created), it brings up the properties of that dimension. For example, double-click on the 3.000 height dimension on the left side (be sure that it was not previously selected). When we do this, we see the following.

The Dimension Properties window contains three tabs: Properties, Dimension Text and Text Style. We will focus on each one independently. PROPERTIES TAB The properties tab is used to specify the format of the dimension. It includes the ability to set dimensional tolerances, change the fraction from a decimal format to a fractional format, specify the number of decimal places shown (which will affect rounding), control dual dimension text formatting, witness line visibility and also specify whether this dimension is a Basic or Inspection dimension. Display We will come back to Tolerancing in the next section. For now, we will look at the Display section, which looks like the following.

Currently, this dimension is displaying as a regular dimension. We will select on the Basic option, and then click on OK to make the change. On our drawing view, we can see the result.

Double-click on the dimension again to get back to the properties. This time, pick the Inspection option, followed by OK. We now have the following.

So, what is the difference between a Basic and an Inspection dimension? Inspection Dimensions Typically, all standard dimensions on a drawing (with the exception of reference dimensions) are subject to inspection for quality purposes. The practice of calling out a sub-set of dimensions that must regularly be checked after first article release has led to the creation of inspection dimensions in drawings. In some cases, separate drawings were created for quality control that only contained specific dimensions to inspect to as the product came back from manufacturing. For companies that prefer to create a master document and reduce potential error from multiple copies floating about, it became common practice to use special symbols to represent dimensions that needed extra attention. Today, most CAD systems include a built-in mechanism that helps identify these dimensions by applying an oblong shape around the dimension. An oblong is used because there are no other oblongs defined in ASME/ISO standards. Tolerances can be shown within the oblong. Basic Dimensions

A basic dimension represents a numerical value used to describe the theoretically exact size, profile, orientation, or location of a feature or datum target. It is the basis from which permissible variations are established by tolerances on other dimensions, in notes, or in feature control frames. In other words, a basic dimension is not subject to tolerances, is not necessarily important enough to inspect in every time, and yet is held to its value, unlike a reference dimension. Use a basic dimension, when you know this is the exact value it should be, regardless of applied tolerances. Typically, basic dimensions are denoted by a rectangular box around the dimension, and no tolerance appears in the box. Format Double-click on the dimension again to get back to the properties window, and then change the display back to Neither to remove the Inspection symbol. Now, we will look at the Format section, which currently looks like the following.

Currently, our dimensions are shown in decimal format, and the number of decimal places shown is three. Change the option to Fractional, and you will see the following.

Instead of the number of decimal places, we are asked to enter the largest denominator for the fraction. In this case, it is 32. Therefore, if our dimension had been 1.500, it would have shown up as 1-1/2 (it doesn’t automatically try to make a fraction with a denominator of 32, which in this case would be 48/32). If we click on OK you will get the following.

We can see that no decimal places are shown in fractional form (as expected). IMPORTANT: For tolerance reasons, you have to be extremely careful when using fractional dimensions. Why? Isn’t “3” the same as “3.000”? Not to a manufacturer. Suppose we have a general tolerance as follows: x. .x .xx .xxx

+ .5 + .1 + .05 + .01

Now do you still think they are the same? “3” can be any number in the range of 2.5 < x < 3.5, while “3.000” can be any number in the range of 2.99 < x < 3.01. This is a huge difference if tight fits are required. We will set the dimension back to decimal format with three decimal places. Dual Dimension In this drawing, we currently don’t have dual dimensioning turned on. Had we had dual dimensioning on, we would have two dimension values shown for each dimension on this drawing – one on top of the other. The dimension on top represents the Primary Units of the drawing, while the dimension on the bottom represents the Secondary Units of the drawing. In this example, our primary dimensional units are Inches, so the secondary units would be Millimeters. The typical format for a dual dimension is as follows:

PRIMARY UNITS [SECONDARY UNITS] The following figure shows what this drawing view might look like if we had dual dimensioning turned on:

Okay, a few things to point out. First, the number of decimal points are going to be equal. The reason for this deals with the idea of trailing zeros. In Metric, trailing zeros are not permitted. Pro/ENGINEER knows this based on the drawing setup file. Therefore, our 3.000 dimension (which goes to 3 decimal places) equates to 76.2 millimeters (3.0 * 25.4). It is not shown as 76.200. Why is this important? We do a lot of manufacturing oversees, where the metric system is prevalent. If we model our designs in inches, and then produce drawings with dual dimensions, there is a good chance that the manufacturer will look at the bottom number for manufacturing or inspecting. Generally, this isn’t a problem. Sure, there is some rounding going on when converting from English to Metric, but generally Pro/ENGINEER does a good job in maintaining consistency in the conversion. The problem could arise if general tolerances are used on the drawing. Going back to our example before, we might have English tolerances as follows: x. .x .xx .xxx

+ .5 + .1 + .05 + .01

From a conversion standpoint, the equivalent in metric would be: x. .x .xx .xxx

+ 12.7 + 2.54 + 1.27 + .254

Okay, if we look back at our current dimension, we know that our height can vary from 2.99 to 3.01 (based on three decimal places). If the manufacturer is looking at the metric dimensions (but following the general tolerances listed on the drawing), there is a chance (possibly slight – but it still exists), that they might end up doing 76.2 + .1 (which is the metric dimension with the English tolerance for one decimal place applied). This gives us a range of 76.1 to 76.3 millimeters, which is equivalent to 2.996 to 3.004 inches.

Okay, you might be saying – wow, this would actually be better, because it is a tighter tolerance, and still leaves room for most of the English range. Aside from a potential in cost difference to hold to this tolerance, going from English to metric doesn’t seem as bad. If we had the opposite, a metric drawing with English secondary units, and we called out general metric tolerances, the results are quite different. We won’t go through an example of this, but try it on your own. The bottom line is that when you use dual dimensioning, you should watch out for possible rounding or misinterpretation errors that may occur. Witnessline Display The last section on this tab that we will talk about here is the witness line display section, which looks like the following:

Working with the same 3.000 dimension, we will click on the Erase button. We are prompted to pick one or more lines. We will pick the top witness line for this dimension, followed by the middle mouse button to complete the selection. Click on OK to close the properties window, and you will see the following.

Notice that a Double arrow appears on the end of this dimension where the witness line used to be. Typically, you see this in partial or detail views where the geometry the dimension connects to on one side is not in the current view. The recommend practice for this is to set up a set datum on the reference that is not visible, and then call out the datum in the dimension, as shown in the next figure (assuming Datum “D” is the datum that is not on this view)

This can be done in the second tab of our Dimension Properties window, which is coming up soon in this lesson. For now, we will double-click on the dimension once more, and click on Show back in the Witnessline Display section to get back the witness line that we erased. DIMENSION TEXT TAB The next tab in our properties window is the Dimension Text tab, which looks like the following for our current dimension:

In the main field, we can see a value of @D. This is telling how to display the dimension value. There are three options that can follow the “@” symbol. These are: @D – Shows the actual dimension value on the drawing. This is the default for • dimensions. @S – Shows the symbolic name for the dimension on the drawing. For • example, you can see in this figure that our dimension’s symbolic name is currently d5, so if we edit this large field and type in “@S”, our drawing would show the following:

This is especially useful for tabulated drawings where you might want to call out the length dimension on a part, and then have a table that defines what “Length” actually is for the different parts. A family table drawing is a good example where using the symbolic name instead is common. •

@O – Can only be used for created dimensions. This overrides the value of the dimension, allowing you to enter any value in. I highly recommend against using this. An example where you might use this is in a part that you only want to model part of it, like a din rail that might be 10 feet long. Perhaps you only want to model 1 foot, because all of the detail along the rail is the same from one end to the next, so you only need to call out a portion of it.

In this case, we can enter “10” for the value, and on the drawing it will appear as 10. Changing the actual dimension in the model will not update the drawing. That is why it is better not to use it. For this same example, it would be better to use a Broken view instead. We will see how to create partial and broken views in an upcoming lesson. Remember our Section A-A view has two created standard dimensions. We could take the one at the bottom of the view and change its text to read: “@O 1396500.4” (without the parenthesis). This would result in the following on our drawing.

Clearly, this is not correct, and could never possibly be this way, but we have the ability to do this with created dimensions. This is just one more reason not to use created dimensions over shown dimensions (which don’t let you override them). Now, within this large field, we can add any additional text we want to the existing dimension. For example, we can edit the height dimension again, and add the following:

This, combined with erasing the top witness line is what was able to give us the following:

Down at the bottom of our Display Properties window, we have a button called Text Symbol, which, if clicked, brings up the following window.

This Text Symbol window has many commonly used drafting symbols used in dimensional notes. For example, if our small holes were only 0.25” deep, instead of calling out the depth dimension on another view, we could update the dimension text with the depth symbol, followed by the symbolic name of the depth (&d31, for example), which might give us the following.

In our current tab, we also have three fields at the bottom. These fields are: Name – the symbolic name for the dimension (d5 in an earlier example). We • can rename the dimension in this location (“Height” for example). Prefix – Specify a prefix in front of the current dimension (3X for example). • • Postfix – Specify text at the end of our current dimension (TYP, for example). You can add prefix and postfix text in the large window as well, as we saw. TEXT STYLE TAB The last tab in our Dimension Properties window is used to modify the style of the text, including font, text size, text angle, text color, etc. This tab looks like the following.

Copy From At the top of this window is a section that allows us to re-use any style libraries that might be set up, or to pick another dimension/note on the drawing to copy its current style. Character The next section down allows us to specify the font we are using. Any true-type font can be used. If you don’t have a font in your pull-down list that you need, contact your system administrator for help on getting that text into your list. In addition to the font, you can specify the height, thickness, width factor, and slant angle for the text. Most of these use the values set by the drawing setup file. I would not override these unless you absolutely had to, as these are based on current standards. If you need to underline your text, you can click on the check box entitled Underline.

Note/Dimension In the final section, we can specify some effects for the text, such as the justification (center, left, right), the alignment (vertical/horizontal), the color of the text, line spacing for multi-line dimensions or notes, whether the text is mirrored, and margins for text inside table cells. Again, I would keep the default settings for most of these, as they are driven by the setup file. Justification is the only one that is often changed. BUTTONS At the bottom of the Display Properties window, we see a row of buttons. They do the following: • Move – pick a new location on the screen where you want the text to be, and the dimension or note will jump to that location. Move Text – Keeps the witness lines and leaders stationary, and just allows • you to pick where you want the text to be. This is good if you want to move a radius or diameter dimension text without moving the leader. Edit Attach – Allows you to specify alternate attachments for the • note/dimension. For dimensions with leaders (such as radius or diameter dimensions), this is more common. For linear dimensions, you really can’t change the location where the witness lines are going. For example, you might have a round feature in the model that goes along many edges. By default, the first edge you select in the round feature is the one that shows the dimension in the drawing. By using the Edit Attach button, you could select a different arc on your drawing that is tied to the same round feature. Close out of this properties window, and save the drawing.

DIMENSIONAL TOLERANCES The last topic for this lesson is how to apply dimensional tolerances. If you doubleclick on a dimension to get the properties window back, you can see a section on the first tab for tolerance specification. To demonstrate this, we will go to our TOP view in the same drawing, and doubleclick on the overall length dimension (10.000”) to bring up the properties window. The following figure shows the tolerance section of the Display Properties window.

Currently, our dimension is at its Nominal value – meaning that there is no tolerance shown for this dimension. The Nominal Value is 10.000 (which is what the dimension was set to). If we wanted to change the value of the dimension, we could do it here. The upper tolerance is currently set at 0.010, meaning that our dimension can go up to 10.010. The lower tolerance is set at 0.010 as well, meaning that our dimension can start at 9.990. We will change them to the following for demonstration purposes: Upper Tolerance: 0.05 Lower Tolerance: 0.02 Our window should look like the following:

Using the pull-down field, we can see the following tolerance modes available to select from:

The following figures show us what our dimension would look like with the different tolerance settings:

LIMITS

PLUS-MINUS

+- SYMMETRIC Okay, you might have noticed something a little strange. First, on the Limits setting, it used the “nominal value” + “Upper Tolerance” to arrive at the top number (10.000 +

0.050 = 10.050). For the lower number, it used the “nominal value” – “Lower Tolerance” (10.000 – 0.020 = 9.980). This isn’t strange, it is exactly what we expected. When we picked on the PlusMinus setting, however, our nominal value changed to 10.015 instead of 10.000. Why? It took the average of the previous result (10.000 + 9.980)/2, which gave us 10.015. Then, it divided the tolerance difference (0.05 + 0.02)/2, which gave us 0.035. Had we picked this tolerance mode first, we would have gotten the following result.

This is what we expected to see, so why didn’t it do this? Unlike AutoCAD or other 2D drafting packages, Pro/ENGINEER is a fully parametric solid modeling tool. It gives us the ability to set our dimensions to different ranges of tolerances to check stack-up, so when we change the tolerance mode for a dimension in the model, it actually updates the model with these values. It was not simply a text edit on the drawing, it was an update to the 3D data. Just keep this in mind if you decide to go from one tolerance mode to another, you will want to verify your numbers are correct. Now, with the Symmetric setting, we will get something different if we had started with this. The result is:

This kept the nominal value correct (10.000), but it didn’t average the upper and lower tolerance. Instead it used to upper tolerance value. Again, if this is not what you want, make sure you change it. Try these out for yourself. When you are done, save and close the drawing. TOLERANCE STACK-UP ANALYSIS In the model itself, we can set our dimensions to their upper, lower, or nominal values, or a combination of these and regenerate the model. Then, we can run interference checks with our assemblies to see the effects of tolerance. Typically, you will only be concerned with certain fit dimensions, and therefore, we want to leave most of the dimensions at their nominal value. If you have more than one dimension adding up in the direction of the fit (for example, instead of an overall length of the plate, if we had dimensioned from edge to hole, to edge, causing two separate dimensions, then we would want to try different scenarios with both of these dimensions. To set a dimension to a particular tolerance limit, we go to Edit, Setup, and then pick on Dim Bound from our Menu Manager when it appears. This will give us the following.

In the DIM BOUNDS menu, we can see options for which dimensions we are selecting. These are: Set All – Sets all dimensions in the model to the tolerance limit specified in the • next section. Set Selected – Allows you to select specific dimensions (such as the length • dimension) and only set that one to the tolerance limit specified in the next section. The next section of options defines the tolerance limit. The choices are: Upper – Sets the dimension value(s) to the maximum value based on the • tolerance(s) specified. Lower – Sets the dimension value(s) to the minimum value based on the • tolerance(s) specified. Nominal – Sets the dimensions back to their nominal values. • Dim Bnd Table – Lets you read from a dimension boundary table that you can • create. The following figure shows a sample Dim Bound Table.

I recommend setting up these tables to make quick work of stack-up analyses. The way they work, you can specify the Set All option, and then pick on the Dim Bnd Table. This brings up the following menu.

Starting from scratch, you would select Edit, which brings up the figure at the top of this page. In the table, the dimension symbol names are listed across the columns.

Here, only four of the many dimensions are visible. If we scroll to the right, we would see the rest of them. For each of the symbols, you can specify whether they should be at the Upper, Lower, Middle or Nominal values. You could set up a table for each type of stack-up you want to try. Then, when you are ready, use the Apply Set to read in one of the tables. Regenerate the model, run your analysis, then apply a different set.

NOTES Creating notes on the drawing is easy. Demonstrate this, go back to the Show_Draw drawing that we have been working with. We will create a note at the bottom left corner of the drawing. Before we do this, we are going to first go to our TOP view, and find out the dimension symbol name for one of our radius values. Therefore, double click on the radius dimension that is currently out in the middle of the view (near the large hole). When the properties window opens up, go to the Dimension Text tab, and you should see the dimension name is d7. Close the properties window. In the drawing toolbar, click on the create note icon, or go to Insert, Note from the menu bar. This brings up the following menu.

The top section of this menu deals with leaders. To create a general note on the drawing, we will use the No Leader option (which is currently the default). If we wanted to make a leader that pointed to an edge or surface, we would use the With

Leader option. There is also an ISO leader option, an On Item leader option, and an Offset leader option. These are probably less used, so we won’t cover them in this guide. Next, we can specify whether we are going to enter the note ourselves, or we are going to import a text file from disk. We will keep the default option of Enter. The next section defines the orientation of the note. The default is Horizontal, but we also have Vertical, or Angular options as well. We will keep the default option. The next section only applies if you are using leaders. Since we are not going to use a leader, we will skip this section. The section following this justifies the text, and the section after this allows us to specify a style to use. We will leave the Default option selected. Finally, we have the option to make the note or cancel out (Done/Return). We will therefore pick Make Note, and then pick down in the lower left corner of our drawing (out in the open area – not on the actual corner of the sheet). When we do this, the message bar becomes a text field and we can enter the first line of our note. We will enter: NOTES: When done, click on the <ENTER> key on your keyboard. We are now prompted to enter text for the second line of our note. We want to have a space in the note, so we will hit our spacebar once, followed by <ENTER>. NOTE: If you don’t hit the spacebar, and just hit <ENTER>, you will be done creating the note. We are now prompted to enter the next row of text. We will type: UNLESS OTHERWISE SPECIFIED, ALL ROUNDS Hit on the <ENTER> key, and type the last part of the note: AND FILLETS SHALL BE &d7. Hit the <ENTER> key, and then hit the <ENTER> key once more to complete the note. We will see the following on the drawing.

We can see that instead of “&d7” in our note, we can actually see the dimension value for our radius (.500), and if we go to our TOP view, we can see that the radius dimension is no longer on the drawing view.

Why is this? If you remember, our drawing can not be over constrained with dimensions that come from the model, therefore, if we use the syntax &d# in a note, that dimension that represents d# will transfer over to the note, and disappear from the drawing where it was used. This same thing works with created dimensions, which are typically &ad#. The only difference is that you can over constrain your drawing with created dimensions, and the system won’t stop you. If you delete the note, the dimension will re-appear on your view. As I mentioned a few paragraphs back, there are so many possible combinations of leader types and attachments for creating notes that we won’t cover them all in this guide. If you have questions about notes, please don’t hesitate to contact your CAD Administrator or the online help for more information. Save and close this drawing.

LESSON SUMMARY Dimensions are probably the most time-consuming entities to place on your drawing. Using shown dimensions, you can save some time in creation, and by applying clean-up techniques (both in sketch mode, and in drawing mode), you can save a lot of time. Created dimensions are often used when you need to specify manufacturing dimensions that conflict with your current fit, form and function dimensioning scheme, or where no such dimension exists in the model.

Always try to show dimensions that must be “inspection” dimensions. Apply tolerances to your dimensions, and perform stack-up analyses to test your design. You can also embed dimensions into notes and remove them automatically from the drawing.

EXERCISES None

Les son

4 8 Lesson Objective: In this lesson, we will learn how to create Broken and Partial view types.

BROKEN VIEWS Broken views are used to shorten a view of an elongated feature/model. Typically, the elongated model does not vary in features from one end to the other, and therefore, you can remove the middle of this model, and not lose any detail. A perfect example of an elongated model is a din rail, or a broom handle, or any object that has a constant cross-section along its length. To demonstrate this, we will open up the drawing called Broken_View.drw, which will look like the following.

The rectangle in the figure above represents the boundary of the sheet size we are using (which happens to be a “D” size sheet). We could use an “E” size sheet, and possibly get more of the model to fit, but the height of the model would be too small in comparison to the size of the sheet. Therefore, to be able to detail out this model, we will use a broken view from the existing RIGHT view to make the entire model fit on this sheet of paper, and not lose any manufacturing detail.

CREATING THE BROKEN VIEW Double-click on the RIGHT view to bring up the properties window. Once open, go to the Visible Area category, which will look like the following.

Currently, the visibility is set to a Full View. We will use the pull-down field to see the other options, shown in the next figure.

We can see that one of the options is Broken View. We will select on this option, and we see the following.

Click on the “+” button to add a broken view definition. When we do this, we are asked to select on the view where we want our first break line. We will pick in the following location.

When we pick in this location, a vertical blue line appears on the drawing view, and we are prompted to pick the location for the second break line, which will be in the location indicated in the next figure.

When we pick in the second location, we get our second vertical blue line, as shown in the next figure.

At this point in time, if we scroll over in our broken view definition, we can see additional fields that we can define. One of them defines the shape of the cut on the view. Currently, we are seeing the Straight option, as shown in the next figure.

We will keep this option of Straight selected, and click on OK. Our view collapses, and we can see the following when we click outside of the view to de-select it.

As you can see, we have vertical lines where the handle is broken. Our view is now made up of two parts, which can be moved independently in the horizontal direction, as shown in the following figure.

We will double-click on the larger of the two view segments to get back into the properties window. Return to the Visible Area category, and then scroll over to see the other options for the shape of the break. This time, select Sketch. When you do this, you are asked to sketch a spline that represents the shape of the break. We will sketch the following spline in the location shown in the next figure.

NOTE: You should try to stay within the two black dots. Once you are done picking the last spline point, click on the middle mouse button to complete the spline. Two identical blue splines show up on the view, as shown in the following figure.

Click on OK to complete this view, and we will see the following.

The following figures show the rest of the view shapes available. NOTE: For the two “Geometry” options, you have to pick two points to define the geometry. You should pick near one of the black dots for the first point, and then approximately the same location on the bottom line, under the dot you previously selected. S-Curve on View Outline

NOTE: Because our handle is so small in height, the “S” shape doesn’t really manifest itself well. The other “S-Curve” option is better, as shown in the next section.

S-Curve on Geometry

Heartbeat on View Outline

Heartbeat on Geometry

By contrast, this “Geometry” option doesn’t work as well as its previous counterpart. The “Heartbeat” is too small to be effective in this case. BENEFIT OF BROKEN VIEW The benefit of making this a broken view is that we can now detail out the model, and the portion of the handle that is missing from the view is not critical to the definition of that model. The following view shows how we can show the entire length of the model, but still get it on the drawing sheet.

NOTE: The dimension on the figure above is a created dimension. The model is actually an assembly consisting of a base and handle. Neither of these independent models has the entire length as a dimension. We could have done this assembly

with top-down design, and introduced the overall length as a variable in our skeleton model that could be controlled, and then shown on the drawing. Save and close the drawing.

PARTIAL VIEWS A partial view should only be used to show pertinent features not described by true projection in other views on the drawing. They are used when you want to zero in on the model to detail out a feature or set of features but to simplify the drawing by removing all non-necessary geometry from the view that is already detailed out in other views. To demonstrate this, we will create two partial views for a bracket. Open up the drawing entitled Aux_Partial.drw, which contains a RIGHT view of the bracket, as shown in the next figure.

We could easily project a FRONT view, as shown in the next figure.

The problem occurs when we add an auxiliary view. In order to get all three views on the drawing (without changing the sheet size or scale), we would have to arrange them as follows.

But, that brings up a good question… Should we opt to change sheet size or scale as opposed to adding partial views? I don’t think it really matters either way. The thing to keep in mind is that a partial view allows you to remove geometry that is not directly detailed in that view, and is detailed in another view. Therefore, looking at the last figure, the auxiliary view contains geometry for the lower two holes that we are never going to detail in this view. Similarly, the FRONT view contains geometry for the raised protrusion that we are never going to detail in

this view, so why not create partial views for the FRONT and AUXILIARY views? That is what we are going to do. If you have not added the two additional views, go ahead and do this using techniques already described in this guide. Partial FRONT View We will start by creating our partial view on the FRONT view. Double-click on the FRONT view to open the view properties window. Under the Visible Area category, use the pull-down to select Partial View, as shown in the next figure.

Just like when we created the detail views earlier, we have to sketch a spline around the geometry we want to show in the view. We have to start by picking on a vertex of one of the existing geometric entities in our view as the center of the spline. We will pick on the end of one of the hole arcs, as shown in the next figure.

A blue dot appears where we picked, and we will start sketching our spline (remember not to close it completely, as shown in the next figure).

When you have finished sketching the spline, click on the middle mouse button to have the spline closed, and then you will see a blue outline for the spline, as shown in the next figure.

Click on OK to complete this view, and our FRONT view will now look like the next figure.

At this point, our drawing looks like the following.

Partial Auxiliary View Now, we will repeat this same process to turn our auxiliary view into a partial auxiliary view. Double-click on the auxiliary view to get to the properties window, and then click on the Visible Area category. Change the type to Partial View. Sketch the following spline (using the blue dot as an indication of where we picked for the center of the spline.)

Click on OK to complete this view. Our drawing should now look like the following.

We can now move the views back in towards each other and complete detailing it, as shown in the next figure.

Save and close the drawing.

LESSON SUMMARY Broken and Partial views are used to save “Real-estate” on the drawing. By eliminating unnecessary portions of the geometry, while still being able to convey the necessary information, we can make our drawings easier to read and follow.

EXERCISES None

Les son

4 9

Lesson Objective: In this lesson, we will learn how to create Geometric Tolerances (GTOLS) and how to access symbol libraries.

DEFINITIONS Before we jump into Geometric Tolerances, we will take a moment to look at some definitions that pertain to concepts behind GTOLS. These definitions come from the ASME Y14.5 standard. Datum A Datum is a theoretically exact point, axis or plane. It is the origin from which the location of geometric characteristics of features of a part is established. For example, if we specify the bottom, planar surface of a model as a datum, then defining a “parallel” tolerance to that surface assumes that the datum surface is (for all intents and purposes) perfectly flat. We already learned how to define a datum (planar and axial) in Lesson 46. Feature of Size One cylindrical or spherical surface, or a set of two opposed parallel surfaces associated with a size dimension. Least Material Condition (LMC) The condition in which a feature of size contains the least amount of material within the stated limits of size. For example, the maximum hole diameter and minimum shaft diameter. Maximum Material Condition (MMC) The condition in which a feature of size contains the maximum amount of material within the stated limits of size. For example, the minimum hole diameter and maximum shaft diameter. Regardless of Feature Size (RFS) This term is used to indicate that a geometric tolerance or datum reference applies at any increment of size of the feature within its size tolerance. True Position The theoretically exact location of a feature established by BASIC dimensions.

GEOMETRIC TOLERANCES Geometric Tolerancing, and dimensional Tolerancing in general is not something that we can teach in the scope of this training guide. For more information on GD&T (Geometric Dimensioning and Tolerancing), you are encouraged to read the ASME Y14.5 standard. The following table lists the common geometric tolerances that are used.

Usage

Tolerance Type

Characteristic Straightness

Flatness For Individual Features

Form

Circularity (Roundness) Cylindricity

Profile of a Line For Individual or Related Features

Profile

Profile of a Surface

Angularity

Perpendicularity Orientation Parallelism

Position For Related Features

Concentricity Location Symmetry

Circular Runout Runout

FEATURE CONTROL FRAMES

Total Runout

Symbol

A Geometric Tolerance Feature Control Frame is the method used to display these tolerances on the drawing view. It is a rectangular block that is divided into different sections, as shown in the example in the next figure.

The block can be a single row, as we see in the previous figure, or it can have multiple rows for composite tolerances. The following table lists the common Modifying Symbols that are present in these tolerances. Term At Maximum Material Condition At Least Material Condition

Projected Tolerance Zone

Free State

Tangent Plane Diameter Spherical Diameter Radius Spherical Radius Controlled Radius Reference Arc Length

Symbol

Statistical Tolerance Between We will demonstrate how to build these control frames with an example.

CREATING A GTOL CONTROL FRAME To demonstrate how to create Geometric Tolerances, we will open up the drawing entitled GTOL_Create.drw, which currently looks like the following.

We can see axes, dimensions, a note, and some set datums. We are going to create our first geometric tolerance by going to Insert, Geometric Tolerance, which will bring up the following window.

This window has four main tabs. These are: Model Refs – Define the type of tolerance, and specify how it is going to be • placed on the drawing. Also allows you to specify which model to use in the case of an assembly. NOTE: Your set datum must be in the model where you want to show it. Therefore, if you have an assembly, you can not create a GTOL for one part, and reference a set datum in another. Datum Refs – Specify the datum references. • Tol Value – Specify the tolerance value. • Symbols – Add modifying symbols to your frame. • The first tolerance we are going to create will be a Flatness tolerance. Therefore, we will pick on the symbol that corresponds to the flatness. Refer back to the first table to identify which button corresponds to the different tolerances, or move your mouse over the buttons until you see it listed in the tool tip. Once we pick on the “Flatness” symbol, we will see that the type of reference to select changes from an Edge to Surface, as shown in the next figure.

We will pick on the Select Entity button, and then pick the edge that represents the surface, as shown in the next figure.

When we do this, we now see another portion of our window become active, as shown in the next figure.

The Placement section will specify how the frame is to be placed. If we use the pulldown we can see a variety of methods for placing the control frame on our drawing.

We are going to place our first frame using the With Leader option, which will place a leader from the frame to the model on the view. Once we select this option, we get the following menu.

Currently, the default settings indicate that our leader will have an arrow head and will go to an entity, such as an edge, axis or vertex. We will pick the same edge that we picked before for defining the surface that is to get the flatness tolerance. Once you pick on the edge, it will become a bold red. Use the middle mouse button out in the view to place the frame, and you will see the following.

A preview of the frame is now on our drawing view, and it will update as we continue to fill in the frame. We will now click on the Datum Refs tab, which currently looks like the following.

The GTOL frame builder is intelligent. It knows that since we picked a “Flatness” tolerance type, there are no datum references that we can call out. Therefore, it gave us this window. Click on the Tol Value tab to continue. It looks like the following.

Currently, the default tolerance is 0.001. We will change this value to 0.02, and then hit the <ENTER> key on the keyboard. The preview updates.

Within this “Tol Value” tab, we also can define material conditions for the tolerance. We will not be specifying any for this particular tolerance. Therefore, we will click on the Symbols tab to continue. It looks like the following.

In this window, we can see some symbols that are available for this type of tolerance and any references we’ve defined so far. We will not define any additional symbols; therefore click on OK to complete this first tolerance frame. Our drawing view will currently look like the following.

Save the drawing. GTOL FRAME IN NOTE The next Geometric Tolerance we will create will be attached to a note containing a dimension. In general, Geometric Tolerances can not be attached to a free note, but they can be created as a free note. Therefore, go back to Insert, Geometric Tolerance to start a new GTOL. We can see that the window is exactly as we left it for our last tolerance definition. We will pick a Position tolerance this time. Once we do this, our window will look like the following.

In the Reference field, we can see that Edge is currently selected. If we use the pulldown, we can see other reference types we can select.

We will use the default of Edge, and select the edge shown in the next figure.

You should always try to pick on geometry that the GTOL controls. In this case, we are going to be attaching our GTOL frame to the “M42 X 1.5 – 6g” note, which is currently going to the same edge. Once we pick the edge, the Placement type we are going to use is Dimension. Remember, we can not attach to a free note, but the “42” in our current note is actually a dimension that was used in the note. Therefore, we can click on the Select Entity button for the Placement filed, and select on this note. When we do, we can see a preview attach itself to the note, as shown in the next figure.

Now, we will go to the Datum Refs tab. It currently looks like the following.

For a positional tolerance, we do have fields that we can define on this tab. In the middle of the window, we see three tabs entitled Primary, Secondary and Tertiary. For this tolerance, we are only going to define one datum reference, therefore we will stay on the “Primary” section. Since we are not doing a compound tolerance, we will use the Basic row, and use the pull-down to select which datum acts as the primary reference for this tolerance, as shown in the next figure.

We will use B for this reference. Once you select a reference, you have the ability to define material condition for this reference. We will use the pull-down to see a list of possible material conditions.

In this case, we will select the MMC (Maximum Material Condition) option. When we do this, our window will now look like the following.

We will now click on the Tol Value tab. For the tolerance value, enter 0.1 in the field provided, and then we will use the Material Condition pull-down at the bottom to specify a material condition for the tolerance itself.

We will select the same material condition (MMC) that we used for the reference. Our window now looks like the following.

Finally, we will click on the Symbols tab, and add a Diameter Symbol to our tolerance field, as shown in the next figure.

Click on OK to complete this tolerance, and our note will now look like the following.

The FRONT view for our drawing now looks like the following.

Save the drawing. TANGENT LEADER PLACEMENT The next Geometric Tolerance we will create will use a tangent leader as the placement type. Therefore, go to Insert, Geometric Tolerance once more from the menu bar. This time, select a Parallelism tolerance. For the reference type, make sure Surface is selected, and pick on the following surface in the FRONT view.

When we do this, for the placement field, use the pull-down to select Tangent Leader, as shown in the next figure.

Once we select this, we get the following menu.

Typically, with a Tangent Leader, you use the No Arrow leader type. Therefore, we will select on this option from the menu above, and then pick on the same edge we picked on before. Using the middle mouse button, place the frame above the existing dimensions, as shown in the figure below.

Currently, the definition of the tolerance, datum reference, and material conditions are still left over from the previous tolerance that we defined. Therefore, we will need to go in and edit it to get the following.

For the material condition fields, set it back to RFS (no symbol), which will eliminate the “M” symbol. Also don’t forget to remove the diameter symbol. The FRONT view will look like the following once you complete this tolerance.

Save this drawing. DIMENSIONS WITH SET DATUMS We are now going to create a geometric tolerance tied to a dimension that has a set datum attached to it. Create a new geometric tolerance, and pick a Perpendicularity tolerance. For the reference, we are going to pick Surface, and then pick on the same surface that we used for our first Flatness tolerance definition. Once we pick on this surface, use the Dimension placement type, and pick on the 44.60/44.45 limits dimensions to the left of our FRONT view (the one that currently has the “C” set datum attached to it. When we pick on this dimension, we can see the GTOL frame attach itself to the dimension, and the set datum attaches itself automatically to the frame, as shown in the next figure.

On the tolerance creation window, there is a button called Move, which will allow us to temporarily move the GTOL while we are still defining it. Click on this button and move the tolerance to the following location.

Now we will go in and edit the values and add any material and modifying symbols as necessary to get the final tolerance, as shown in the next figure.

Save and close this drawing. We will come back to it in the exercises for this lesson.

SYMBOL LIBRARIES There are several libraries of symbols that are available in Pro/ENGINEER and in our company. These are: Surface Finish Symbols • Weld Symbols • Custom Company Symbols • CUSTOM COMPANY SYMBOLS In an upcoming lesson, we will learn how to create draft entities in drawing mode – which is the method to define symbols. For now, we will learn how to access already created symbols. By default, we have a config.pro file that points to the location of our custom symbols. If you have the correct config.pro loaded, then you will always end up in the custom symbol location when you go to insert a symbol. To demonstrate this, create a brand new drawing. Accept the default name, and the default model that is associated (even if it says None). Use an A size sheet. We are not going to add any views to this drawing. To access our symbols, go to Insert, Drawing Symbol, Custom, which will bring up the following window.

You can see the location is listed as User Syms in the pull-down field. Out in the main window, you will see a list of defined symbols. Your list may be different depending on the organization. To demonstrate the symbol window, we will open up the tri_flag.sym symbol. When we open this symbol, we get the following window.

As we move our mouse around the drawing, a preview of the symbol follows the mouse, as shown in the next figure.

Looking back at our Custom Drawing Symbol window, we can see that there are three tabs. The first tab (General) is used to define the symbol, the placement, and the size/rotation/color of the symbol. For the placement types, you have the same sort of options you have for GTOL frames, and notes. Depending on the symbol definition, you may or may not be able to use leaders. For this symbol, it is most commonly used without leaders, so we will leave the placement type as Free. For now, we will also leave the height and angle at the default values. If we click on the Grouping tab, we see the following.

As you can see from this figure, no grouping has been defined for this symbol. Grouping allows you to create different configurations of the same symbol instance. Each defined group can turn on/off draft entities or text in the group definition. We will see this in more detail in the next two symbol types (Weld and Surface Finish). If we continue on to the next tab, called Variable Text, you can see the following.

When you define a symbol, if you place text in back slashes - \text\, you can create variable text that can be changed each time the symbol is used. Text that is not in back slashes will be read-only in the symbol.

We can see that we have a variable text that currently has a value of A. We will edit this and enter 5. Click anywhere on the drawing to place the symbol, and then click on OK to complete this symbol. On our drawing, we see the following symbol.

To edit this symbol, you would simply double-click on it to get back to the symbol window. SURFACE FINISH SYMBOLS To access surface finish symbols, go to Insert, Drawing Symbol, Custom, which this time brings us back into the surface window, where the last symbol we used is still active. We will click on the Browse button next to the name of the symbol (on the General) tab. This brings us back into the file open window. In the pull-down field at the top, select System Syms, as shown in the next figure.

This brings us into the following window:

In this window, we can see two different Surface Finish folders, and a weld symbol folder. The first folder is for surface finishes following the ISO 1302-1978(E) standard. The second folder is for surface finishes following the ASME Y14.36-1978 standard. We will double-click on the ASME Y14 standard folder. This reveals a single surface finish symbol, as shown in the next figure.

We will open this single symbol (surftexture.sym), and we will get the symbol creation window, which looks like the following.

We will leave the defaults alone on the first tab, and go to the Grouping tab. We will see the following options in the group window.

This is a perfect example for using groups. There are hundreds of possible surface finish combinations, and instead of creating hundreds of individual symbols, a single symbol was created that contains all of the possible definitions. By turning on/off certain options, we can get all of the different combinations possible. At the top level, we can specify whether this is for an Unspecified, Machined, or No-Removal surface. Within each of these options, are further options that can be defined. If we were to expand all three options to see the possible sub-options, our window would look like the following.

We will expand the Unspecified option to see the detail up close.

As you check items, and sub-items, it starts to build your custom symbol in the window to the right. We will select the Average Roughness option, as shown in the previous figure, which adds variable text to our symbol. If we go to the Variable Text tab, we can edit the value for this variable text. In this case, we will enter 3.2 for the average surface roughness, as shown in the next figure.

Clicking out on our drawing gives us our current symbol.

If we had more than one of these surface finish symbols to define, we could go back to the General tab, and click on the New button, which starts a new surface finish symbol, using the current definition as the starting point. Every time we click on the drawing, we place this symbol in its location, and then click on New to add a new one. Click on OK to complete this symbol. WELD SYMBOLS To create a weld symbol, we repeat the process as the last section until we get to the folder where we see the three different system symbol directories. This time, we select the Weldsymlib folder, which gives us the following.

As with the surface finish symbols, there are two standards to choose from for weld symbols: ISO 2553:1992(E) and ANSI/AWS A2.4-93. We will double-click on the ansi_weld folder, which gives us the following folder options.

These are the first of the different categories for weld symbols. We will double-click on the Simple folder to continue. This brings up the following window:

From this window, we can see a list of individual symbol definitions. We will open up the first one (bevel.sym), which brings up the following symbol create window.

One of the differences in this symbol is that we can use a Free placement type. We will have to pick a location for the leader to go to, but we will come back to that once we have defined the group options. Therefore, click on the Grouping tab, and select the options shown in the following figure.

When we have defined these group options, click on the Variable Text tab, which shows two parameters we can modify based on our selection of options.

Go ahead and enter any values you want. I will leave the current values for this example. To place this symbol, we need to go back to the General tab. We will leave the Placement Type at With Leaders, but we will change the New Leader value to Free Point, and then click out in the drawing. After you click, you will notice a preview of the symbol with its leader appears.

Drag the symbol to the location you want, and then click on the middle mouse button to finish the drag. Click on OK to complete this symbol. The following figure shows the location where I dragged it.

Close this drawing without saving.

LESSON SUMMARY Geometric Tolerances can be applied to your drawing in a variety of ways. Be sure you have your set datums, axes and dimensions fully detailed before adding the Geometric Tolerance to make it easier. Symbols can be created to automate common drafting tasks. In a later lesson, we will learn how to create a basic symbol with some grouping.

EXERCISES Now, using techniques learned in this lesson, complete the Geometric tolerances on the GTOL_Create.drw drawing, as shown in the next figure.

Les son

5 0

Lesson Objective: In this lesson, we will learn about the 2D Drafting capabilities and how to create a symbol from scratch.

2D DRAFTING There are times in drawing mode where you may need to sketch entities. Creating symbols and formats is the most common usage for the 2D drafting tools in drawing mode, but often, we create geometry on the drawing (such as parting lines, arrows, etc.) The 2D Drafting tools are not the most user-friendly tools in the Pro/ENGINEER drawing arsenal. In fact, compared to the part mode sketcher functionality, the 2D Drafting tools seem very clunky. In a future release of Wildfire, the 2D drafting functionality is going to be replaced by the regular sketcher tools, which will make it much easier to use. The 2D Drafting tools are located on the feature toolbar in drawing mode, and look like the following:

We will go through these tools in the next section.

2D DRAFTING TOOLS To demonstrate the different drafting tools, open up the 2D_Draft.drw drawing. It contains three views, as shown in the next figure.

We will work out in the upper right corner for most of these tools, but some of them require actual geometry to work off of, so we will come back to the views in a minute. Enable Sketching Chain If you depress this tool, a command remains active until you select a different command. For example, if you start to sketch a line, once you place the endpoint of the first line, it becomes the start point for the next line. If you don’t have this active, then the line tool is still the active tool, but you have to pick the start of the next line. We will demonstrate this once we get into the line tool. Remember Parametric Sketching References When you sketch draft entities in drawing mode, you can pick on existing draft geometry or view geometry as references (just like we pick references in sketch mode). If you press this button, and then sketch an entity parametrically related to a view, an update to the model will update the parametric information (collinear constraint, for example). We will see an example of this with the line tool. Line Tools The line tool is a fly-out consisting of the following tools.

2 Point Line The two-point line creates a line by picking on the start point, and then picking on the end point. When you pick on the tool, you will see a red cross-hairs on the mouse cursor as it moves across the drawing, as shown in the next figure.

A window appears for capturing sketching references, as shown in the following figure.

Currently we don’t have any references. We will come back to this in a minute. Out on the drawing, if you hold down the right mouse button, you will see the following options.

The following commands directly relate to the sketch that we are creating. These are: Select Reference – Takes us back to the Snapping Reference window that • appeared. Angle – Specify an angle for the line entity that we are currently sketching or • will sketch. To make a horizontal line, enter 0.0 or 180 for the angle. For a vertical line, enter 90 or 270 degrees for the value. Relative Coordinates – This is usually used for the end point of the line, giving • you exact control of the vector from the start point. For example, a horizontal line exactly 1.5” long going to the right of the start point would result in the following: X = 1.5, Y=0. Absolute Coordinates – This can be used for either endpoint. It gives you the • ability to sketch using the entire sheet size as a grid, where X=0, Y=0 is in the lower left corner of the sheet. For an “A” size sheet, your maximum X that you would want to go is 11.0”, and your maximum Y that you would want to go is 8.5”. Regenerate Draft – Regenerates all of the draft entities. Any parametrically • linked entities would update. Properties – Select line size, color, style, etc. • We will select Angle, which will give us the following window.

We will keep the default value of 0.0000 to create a horizontal line. Click on <ENTER> on your keyboard, or click on the green check mark to accept this. Click anywhere on the drawing to start the line. As you move your mouse, you will see a magenta preview of the line going to the left or right of your first point (depending on which side you are on when you drag).

We will make this line segment exactly 3.0” in length, therefore, before you select your end point, right click again, and select Relative Coordinates, which brings up the following window.

As indicated in the window above, if we enter 3.0 in the “X” field, we will get a line that is 3 inches long going to the right. If we entered -3.0, it would go 3 inches to the left. Click on the green check mark to accept this, and we get the following line.

In our Snapping References window, we can see the line added to the list of active references.

If we move our mouse back over to one of the end points of the line, we can see that it will snap there for the beginning of our next line.

Go ahead and snap to the right end as shown above, and click to start a new line. As you move your line up, and away from the first line, you will notice that it will snap at perpendicular, as shown in the next figure.

We would use this to make a square or rectangle. Instead, we are going to hold down the right mouse button, select Angle, and enter 135 for the angle. This forces the line to go at 45 degrees with respect to the first line, as shown in the next figure.

Drag the line well over to the right of the middle, and click to create it, as shown in the next figure.

Now, we have two lines in our References window – the first horizontal line and now the new angled line. We will create a third line starting at the left end of the horizontal line, and select Angle and enter a value of 45 to get a line going up towards our last one. When you get to the first angled line, our new line will snap to it, as shown in the next figure.

Click to accept this snap and finish the line. Click on the middle mouse button to finish out of line mode, and we are left with the following on our drawing.

Trim We will take a moment to see how to trim a line. From the menu bar, we would select Edit, Trim, which gives you the following options for trimming.

•

Divide at Intersection – divides up the entities where they intersect. You can then delete the extra pieces you don’t need.

• • • • •

Divide by Equal Segments – Breaks up an entity into equal length segments. For example, breaking up a line into 10 pieces of equal length. Corner – Trims two intersecting entities at their intersection point. The entities need to either already touch, or project to touch at a corner. Bound – Extends an entity up to another one. The entities must project to a corner intersection Length – Trims an entity to an exact length by extending or shortening the entity near the endpoint selected. Increment – Extends or shortens an entity by a specified amount.

We will choose the Corner option, and then pick on the two angled lines on the portion we want to keep using the Ctrl key, as shown in the next figure.

This will eliminate the small portion that extends out to the upper left, resulting in the following.

Construction Line The second line tool is the Construction Line. It creates a line just like the two-point line, but it behaves like a sketcher centerline or construction line. It will not print out on a drawing if used. Select this tool from the line tools fly-out. When the Snapping References window appears, you will notice that there are no references listed. What happened to our three lines that we created? The lines are still there, but their presence in the references window was only while we were still active in the line tool. Once we went back to the select tool, it cleared the references. Therefore, we will pick on the arrow button in this window to add references, and we will pick on the two angled lines in our triangle. They will show up in the window, as shown in the next figure.

Click on the middle mouse button to finish picking references, and then bring your mouse over to the left of the two angled lines. Around the middle of the line, it should snap to the midpoint, as shown in the next figure.

Click here, and then go over to the midpoint on the other line, as shown in the next figure.

When you click on this endpoint, a dashed line appears across the working window. Click on the middle mouse button to complete the creation of construction lines and return to the select tool. We can see a light gray dashed line on our drawing.

Unlike sketcher, where you can convert a line to a construction line, and still have it be within the endpoints selected, this construction line will use the start and end points as vectors to define an infinite line. Go ahead and use the select tool to drag a box around the triangle to select it, and hit the delete key on your keyboard. Pick on the construction line that we just created and delete it as well. Crossed Construction Lines The Crossed Construction Line tool creates two perpendicular construction lines. The first line you draw determines the location of the origin of the lines (where they intersect) by using the start point. The end point determines the horizontal vector. The perpendicular construction line is created automatically. To demonstrate this, click on this tool from the line tools fly-out icon. Pick out on the drawing, and then move your mouse over and down to create an angled line, as shown in the following figure.

When you click on the end point, the two construction lines appear. The location of the intersection of the two lines is where our start point was before, while the angle of the lines is determined by the end point that we picked, as shown in the next figure.

Go ahead and delete these two lines. Enable Chain Sketching – Revisited We will now take a look at this option. If we click this icon, and then go into our line tool, we start to create a line the same way we normally do. This time, however, when you pick on the endpoint for the first line, notice how the next line starts automatically at the endpoint of the first one?

This is similar to the way it works in Sketcher mode with the line tool. To complete your chain of lines, click on the middle mouse button. The line tool will still remain active for you to start a new set of lines. To get back to the select tool, click on the middle mouse button again. Delete any entities that you just sketched. Keep this tool active for our next topic. Remember Parametric Sketching References – Revisited Now, we will look at this option again using the line tool. To start, click on the icon to activate this. You must have the icon active before you sketch your geometry. Activating it after will only enable it for newly sketched entities. Once you have pressed the button, click on the line tool. In the Snapping References window, click on the arrow button, and we will pick the following edge on our RIGHT view.

When we select this edge, its endpoints highlight in a blue dot, as shown in the next figure.

We will see this edge listed in our References window.

Click on the middle mouse button to finish selecting references, and then our line command becomes active. Sketch a perpendicular line starting on the left point of the reference edge (be sure you are snapped to it). Stop the line before you get to an “equal length” condition between the line and the edge. The next line segment should start automatically (because we still have our chain sketching enabled). Sketch a horizontal line over until you get an equal length condition with the edge, then create the last segment down to the right vertex of the edge. The following figure shows this sketch.

To demonstrate the parametric nature of our references, we will change a model dimension to force the top edge of the model to translate down. To do this, we will show some dimensions. Alternate way to Show Dimensions Another way to show dimensions on your drawing for a specific feature is to go to the model tree, right click on the feature, and select Show Dimensions, as shown in the next figure.

Unlike the Show/Erase tool, we have no ability to only select certain ones to keep, but that is okay for this instance. On our drawing, we can see the three dimensions that make up our selected feature.

We will select on the 2.000 dimension once to activate it, and the double-click on it to modify the value to 1.5. Regenerate the model, and you will notice that as the top edge of the model translates down, the sketched entities move with it to remain snapped to the edge, as shown in the next figure.

Edit the dimension back to 2.000, regenerate the model, and then delete the three sketched entities that we made. By contrast, if we try this same thing again without using the Remember Parametric Sketching References activated, the sketched entities will not translate with the top edge, as we can see in the following figure.

Try this out for yourself by repeating this same process, but de-select the tool first. When done, set the dimension back to 2.0, and regenerate the model. Delete the sketched entities. Finally, de-select the Chain Sketching command. Circle Tools The circle tools is a fly-out consisting of the following.

Circle Tool To create a circle, click on the drawing, and then drag out the diameter. Click to complete the circle. If the Chain Sketching is active, a new circle starts again at the same center, allowing you to create concentric circles. If you click with the right mouse button with the circle tool active, you see the following.

This is very similar to the RMB functionality with the line tool, but instead of an Angle to define, we can specify the Radius. When we select this option, we get the following window.

We will enter a value of 1.0 in this field, and then click on the green check mark, or hit the <ENTER> key on the keyboard. When we do, we see the outline of the circle at the specified dimension.

We then click to place the circle. Remember, this is the RADIUS of the circle that we entered, not the DIAMETER. The following shows the circle after it has been created.

Delete this circle when complete. Construction Circle This is done exactly the same as the regular circle. The only difference is that the circle that results is only used to aid in the creation of other entities, and will not print. It is a dashed gray entity, just like the construction line.

Ellipse by Major Axis End Points

The first ellipse tool is created by first selecting the start point and then end point of a line that represents the length of the ellipse. This line can be at any angle you want. The following figure shows the creation of this first line.

Once you pick on the end point, the ellipse will appear, and you can drag out the width, as shown in the next figure.

The following figure shows the created ellipse.

Delete this ellipse.

Ellipse by Center and End of Major Axis The last ellipse is very similar to the previous one. The biggest difference is that instead of picking the start point of the line that defines the length, we are picking the center of the ellipse. Once we pick on the location, the line grows out on both sides of this point, and rotates about it. Once you pick the second time to finish dragging out the length, you drag out the width of the ellipse just as we did before. Arc Tools The Arc Tools is a fly-out icon that contains the following:

3 Point/Tangent-End Arc Click on the 3 Point/Tangent Arc tool and click out on the drawing. This creates the start point for our arc. Next, drag your mouse over to the location for the end point, as shown in the next figure.

When you click on the end point, you now drag out the radius of the arc, as shown in the next figure.

When you click once more, you finish the first arc. Since the arc tool remains active, we can go straight into demonstrating the tangent-end arc. Therefore, bring your cursor over the end point of the arc that we just created, and you will see it snap to this point. A small “T” appears to indicate that it will be tangent, as shown in the next figure.

Click on this end point to start the arc, and then drag out the end point for the tangent arc, as shown in the next figure.

When you click to place the end point, we can continue to make additional arcs, or click on the middle mouse button to complete the arc tool. The following figure shows the completed set of arcs.

Delete these arcs when done. Center-Ends Arc When you click on this tool, the first point you will pick is the center of the arc. Once you pick the center point on your drawing, a circle will appear. Your cursor will ride on the circle to define the start point of the arc, as shown in the next figure.

Once you click to create the start point, you are now dragging out the location on the circle where the end point will be, as shown in the following figure.

The following figure shows the completed arc.

Delete this arc when done. Fillet Tools The fillet tools is a fly-out, but there is only one fillet tool in our current fly-out. This is the Round Fillets Tangent To 2 Edges command. To demonstrate this, first create two lines that connect to each other, as shown in the next figure.

Now, click on the fillet tool, and you will be asked to select one entity. We will pick on the first line as shown below.

Next, we will pick on the second line. Once we pick on the second line, a prompt appears in the message bar, as shown in the next figure.

We will enter 0.75, as shown in the figure above. When we do this, an arc appears on the sketch, as shown in the next figure.

Click on the middle mouse button to complete the arc tool, and you will see the following on your drawing.

Delete these entities when done. Spline Tool To create a spline, start by selecting on this tool to activate it. Next, pick on the first endpoint of the spline, and then continue to pick intermediate points. When you have picked your last point, click on the middle mouse button to complete it. The following figure shows a spline as it is being defined.

Once you click on the middle mouse button (after picking the end point), you will see the end points highlighted in blue, while the intermediate points are in the curve color, as shown in the next figure.

Click on the middle mouse button again to exit out of the spline tool. The following figure shows the completed spline.

Delete this spline when done.

Point Tool The Point tool creates a single point on the drawing. The following figure shows some completed points.

NOTE: The shape and size of the point can be controlled by the drawing setup file. There are two options: Datum_point_shape – Controls the shape of the point. The values available • are:

•

Datum_point_size – Controls the height of the symbol used for the point.

Delete these points when you are done. Chamfer Tool The chamfer tool adds an angled line at the intersection of two entities. To demonstrate this tool, first start by creating two connecting lines, as shown in then next figure.

Now, click on the chamfer tool. This brings up the following menu.

From here on out, we will assume that when prompted to select the entities, that we will pick the following lines in the order shown in the next figure.

When you click on one of the schemes, you are then prompted to pick the entities. Once we pick the entities in the order shown above (using the Ctrl key), a blue circle appears at the intersection, and the message bar prompts us for the necessary chamfer values. 45 x d You are prompted to pick the value for d. We will enter 0.5. It automatically measures the 45 degree angle from the first line picked. The chamfer is added. The following figure shows the resulting scheme for this chamfer.

The value for d is measured along the first line selected. To get back to the line before we added the chamfer, click on the Undo button, or delete the chamfered edge, and then use Edit, Trim, Corner and select the two lines again using the Ctrl key. dxd You are prompted to pick the value for d. We will enter 0.5. The chamfer is added equally to both lines, as shown in the next figure.

Undo this chamfer or trim to get back to the starting two lines. d1 x d2 You are prompted to enter the value for d1. Whatever line you pick first will have d1 measured along it. We will enter 0.5. We are then prompted for d2, and we will enter 0.625. The chamfer is created as shown in the following figure.

Undo this chamfer or trim to get back to the starting two lines. Ang x d When you click on this option, you are asked to pick the reference line. This will be the line that the distance and angle are measured from. We will still pick the first line as indicated in an earlier figure. We then pick the second line. We are prompted to enter a value for d. We will enter 0.5. For the angle (measured from the first line), we will enter 20.0. This creates the chamfer with the following scheme.

Delete these lines when done. Edge Tools The Edge Tools icon is a fly-out that contains the following:

This tool allows you to create draft entities right on, or offset model edges or datum curves on the drawing. You might want to use this tool to show parting lines in a different line style than the existing drawing entities, or for identifying a surface boundary for a special finish, etc. Use Edge To demonstrate this, go to the FRONT view, which currently looks like the following.

We want to indicate a parting line for this view. Therefore, we will click on the Use Edge tool, and select (using the Ctrl key) the following entities on this view.

Once you have all the entities selected, click on the middle mouse button to accept this selection. In the message bar, you will get the following prompt.

In this particular case, we do want to erase the edges, because our copied draft entities will be right on top of the existing lines, and if we change the line style, we don’t want the model edges to interfere with the visibility of the lines. Therefore, click on Yes. You are then told that you will need to refresh the drawing views. To do this, click on the following icon in your drawing toolbar.

Now, select each of the entities that we just created, and right click on them and select Line Style, as shown in the next figure.

This will bring up the following window.

To get a nice dashed line, we will pick on the CTRLFONT_S_L option, as shown in the next figure.

Click on Apply, followed by Close to see the new style on the view.

Now, we can use Edit, Trim, Increment and extend each end 0.5 inches, to get the following.

The nice thing is that the Use Edge command keeps the entities tied to that view, so if we move the view around, the entities move with it.

Offset Edge To demonstrate the offset edge tool, we will look at the TOP view in our drawing. Click on this tool, and you will get the following menu.

The default option is Single Ent, which stands for “single entity”. If you use this option, then you can only pick one edge at a time and enter the offset right after picking it. If you want to offset more than one edge that forms a chain, use the Ent Chain option. We will use the Ent Chain option for our selection. Next, using the Ctrl key, select the following edges to offset.

Once all edges are selected, click on the middle mouse button. An arrow will show up on one of the selected entities, as shown in the next figure.

Enter the offset distance where positive is going in the direction of the arrow. For our example, we will enter -0.05 (negative). This will add the following entities to our view.

We will change the line style for these entities to the CTRLFONT_S_L style that we used before, and we get the following.

We will repeat this same process to offset the circle in this view as well. Once we have both sets of offset edges created and set to the CTRLFONT_S_L line style, we will select all of them by dragging a box around the view. Next, go to Edit, Fill, Hatched and down in the message bar, you are asked to enter a name for the hatched surface. Give it any name you want. I will use SURF_A. When you accept the name, hatch marks appear on the view, as shown in the next figure.

The following menu also appears.

We will click on Spacing, followed by Half (four times) to get the following.

Doing this can make it clear to a manufacturer any comments you might have that require the application to the entire surface, such as a finish note, etc. On the Fill menu, there is also a Solid option, which will create a shaded surface in this region. You can then go to the properties of the filled area and change the color for more emphasis in electronic mode, as shown in the next figure.

These are just some examples where the edge tools can be used. Save the drawing. Mirror Tool The mirror tool is the last toolbar icon. It is used to mirror draft entities about a draft line. Therefore, we will start by creating a series of lines on our drawing as shown in the next figure (NOTE: do not worry about the exact shape and size, just get it close).

Now, sketch a single line at an angle to the right of this shape, as shown in the next figure.

To mirror the sketch, start by clicking on the mirror tool. Drag a box around the closed sketch (don’t include the angled line). These entities highlight in red. Click on the middle mouse button to finish selecting the objects to mirror. Down in the message bar, it prompts you to pick on a draft line to mirror about. We will pick on the angled line that we sketched. When we do this, we can see the new mirrored entities, as shown in the following figure.

Delete these entities when done.

SKETCH MENU & OTHER DRAFT TOOLS Up to now, we have focused primarily on the 2D Drafting toolbar. We will now take a look at other, related drafting tools in drawing mode. Sketch Menu In the menu bar, there is a sketch menu. If we click on it, we get the following.

For the most part, this menu contains all of the commands that are covered in the icons that we have gone over. We will look at one in particular, called Sketcher Preferences. When we click on this, it brings up the following window.

This menu controls the automatic snapping constraints that can be applied while sketching. For example, if you recall when sketching in previous sections, we saw that the entities snapped to each other and their vertices. These are on by default in this sketcher preferences window. We can see that we can enable Horizontal and Vertical snapping, which would be very useful to save us some time in specifying right mouse button commands. We will enable this, and the Angle snapping (leave at 45 degrees). Now, try sketching lines on your drawing. You can see that the objects will snap at 45 degrees, as well as horizontal and vertical orientations. Transform In the Edit menu, there is a command called Transform, which gives you the following options.

This set of commands will let you move, move and copy, rotate, scale, mirror and stretch your draft entities. Translate / Translate and Copy To demonstrate the translate functionality, go ahead and sketch a circle with a radius of .25 located at absolute coordinates of X=6.0 and Y=6.0. This will create the circle as shown in the next figure.

Now, we will go to Edit, Translate. We are asked to pick on the entities to translate. We will pick on the circle, and then click on the middle mouse button to finish selecting objects. This will bring up the following menu.

The options at the top are: Horiz – Enter a distance in the X-direction. • Vert – Enter a distance in the Y-direction. • Ang/Length – Enter a distance in polar coordinates • From-To – Enter a distance by taking a vector using one of the methods in the • second section. The second section gives the following options: Pick Pnt – Pick a point on the screen for the start/end of the vector. • • Vertex – Select a vertex for the start/end of the vector. On Entity – Pick a point on a draft entity for the start/end of the vector. • Rel Coords – Pick a point a certain x and y distance from the current circle • center for the start/end of the vector. Abs Coords – Pick an exact x and y location for the start/end of the vector. • NOTE: You can use one option for the start, and a different option for the end of the vector. For example, you could pick Vertex for the start of the translation vector, and then use Rel Coords to locate the end of the vector. We will use Horiz in the top menu, and enter a value of 1.0. The circle will move 1 inch in the X direction. Now, we will click on Edit, Transform, Translate and Copy, and pick on the circle again. After using the middle mouse button to accept the selection, pick on Horiz again, and enter 1.0 for the incremental distance between copies. Once you enter this number, you are prompted for the number of copies. The number that you enter does not include the first circle, so if you want a total of 10, you need to enter 9. We will enter 3, and then hit the <ENTER> key. we should see three additional circles created, each spaced 1.0 inch from each other, as shown in the next figure.

Delete all four circles. Rotate / Rotate and Copy These commands are similar to the Translate and Translate and Copy commands. We will first start by sketching the following shape on our drawing.

We are going to rotate the triangular object about the center of the circle. Therefore, go to Edit, Transform, Rotate, and then drag a box around the two lines and the arc that make up the piece to rotate (don’t include the circle in the box).

Once all three objects are selected, click on the middle mouse button. We will get the following menu.

We will use the Vertex option to be able to select the center of the circle/arc. Once you pick this option, move your mouse over to the center of the circle. You should see a light blue circle appear at the center. Click on this vertex, and then you will get the following prompt in the message bar:

We will enter 90 as shown above, and then click on the <ENTER> key on our keyboard. The draft entities will rotate to the bottom of the circle, as shown in the next figure.

Now, we will try out the Rotate and Copy command to make five of these wedges equally spaced about the circle. Therefore, click on Edit, Transform, Rotate and Copy. Drag a box around the entities again, and then click on the middle mouse button. Select Vertex once more from the menu, and pick on the center of the arc/circle. When prompted for the angle of rotation, we will type in 360/5 (you can enter equations in dimension fields). For the number of entities to create, we will enter 4 to create a total of five of these wedges. The result will be the following.

Keep these entities on the drawing for the next topic. Rescale We are now going to see how to scale the object. Currently, the scale is at 1.0. To make this half as big, we would enter a scale of 0.5. Once the object is scaled, it is reset at 1.0 again, so to make it half as big again, we would still use 0.5 (not 0.25 from the original starting size). Therefore, click on Edit, Transform, Rescale. Drag a box around all of these objects to select them, and then click on the middle mouse button. We will get the following menu.

We are asked to select the point/vertex about which to scale. The point that we pick will remain where it is, and the rest of the entities will scale about that point, potentially causing some translation if you pick an extremity as the scaling point (such as one of the tips of the wedges). We will click on Vertex, and select the center of the circle to scale about. When we do this, we are asked to enter the scale in the message bar. Enter 0.5, and then hit the <ENTER> key on your keyboard. The entities scale down to half of the original size, as shown in the next figure.

We will use these entities once more for the next topic. Stretch We are going to skip over Mirror, because we already covered this as a tool on the 2D Drafting toolbar. The Stretch tool is used to elongate or shrink the draft entities, but not proportionally (like a scale command). Therefore, we will go to Edit, Transform, Stretch. You are asked to draw a box about the entities to stretch. NOTE: Unlike the previous commands where you had to get the box around the entire entity to select it, this time the box only has to touch the entities to select them. We only want to stretch out the bottom wedge, so we will draw a box that only touches the two angled lines on the bottom wedge. Do not touch the arc at the top of the wedge, or any other entities on this drawing. Once both lines are selected, click on the middle mouse button. We get the following menu.

The stretch command uses the translate option to define a vector for the length and direction of stretch. We will start by selecting Vertex, and then picking on the following vertex to act as the starting point of our vector.

Once you pick this vertex, you are prompted to define the end point. We will use Rel Coords to enter an X and Y translation from the selected vertex. When prompted, enter X=0 and Y=-0.5. This will result in the following.

Group Create We will now talk about grouping objects. If you were to select just one of the entities in this current set of draft objects, you could then drag it and it would separate from the rest of the entities. Even though we snapped to end points when defining the sketch, the entities are not completely connected. Therefore, we will want to group these entities together to be able to manipulate them as a single entity. Therefore, go to Edit, Group, Draft Group from the menu bar. This brings up the following menu.

We have the ability to create groups, suppress them, resume any suppressed groups, ungroup (explode) and edit groups within this menu. We will click on Create, and then drag a box around all of the draft entities. Click on the middle mouse button to finish selecting objects, and then in the message bar we will be prompted to enter a group name. Type in STAR, and then hit the <ENTER> key. The group is created, and now we can select additional entities to group. Click on the middle mouse button to finish creating draft groups. Now, if you try dragging just one entity, the entire group moves. Edit To edit a group, click on Edit, Group, Draft Group, and then select Edit from the menu. This brings up a sub-menu, as follows:

You can either select the group from the drawing (which is the default), or you can pick from a list of created group names. We will click on By Name, which brings up the following.

We can see the current group that we created, called STAR. Pick on this name, and you will get the following options.

We can add additional entities to our group, or remove current entities from the group. To cancel out of this, click on the middle mouse button. Additional Comments The thing that makes 2D drafting less user friendly than regular sketch mode (intent manager), is the fact that you should be more exact in your sketching, because making changes to your sketch is more difficult. Dimensions can not be modified to shorten, lengthen, or move draft objects. Therefore, if you sketch a rectangle using four lines, you can add dimensions. To get the exact length and width of the rectangle, you would need to either do this up front, or trim to length the entities after the fact. Once you trim to the length, the entities become disjointed, and you will need to translate other entities to get it back. Therefore, I highly recommend being precise up front.

SYMBOL CREATION Creating a symbol is an extension of 2D Drafting – since most of what you do involves sketching the shape of the symbol. The advantage of creating symbols is to create a library of commonly used shapes that appear in the drawing. You can also scale symbols upon retrieval, so changing the size is easier. To demonstrate this, we will continue to work in the same drawing, but delete any draft entities in the drawing already.

Starting a New Symbol To start a new symbol, you go to Format, Symbol Gallery from the menu bar. This will bring up the following menu.

The options in this menu do the following: Define – Create a new symbol • Redefine – Change an existing symbol • Delete – Delete a symbol from the library • Write – Save the symbol to the library • Symbol Dir – Define the directory where you will save symbols for this session. • Show Name – Pick on a symbol in your drawing to identify the symbol name in • the library that represents the symbol. Symbol Dir Normally, our symbol library is governed by our Config.pro file, as we saw in Lesson 49 – GTOLS and Symbols. For the purpose of this training guide, we do not want to write our temporary symbols to this location. Therefore, we will need to use Symbol Dir to select our current training directory as the location to save any symbols we create. Click on Symbol Dir, and you will get the following.

We can see that the current directory is our Symbols system folder. Therefore, click on the Working Directory icon (the one with the little blue diamond in the upper right corner), followed by Open. Down in the message bar, we see the confirmation that our working directory is now the active symbol library directory, as shown in the following figure.

Define We will now define a new symbol. Therefore, click on Define in the menu manager. Down in the message bar, we are prompted to enter a symbol name. We will enter MY_SYMBOL for the name, and then hit the <ENTER> key on the keyboard. The following menu manager appears:

On our working window, it looks as if all the drawing entities and views have disappeared. In reality, a new window has opened with a blank drawing sheet. In

the title bar at the upper left corner of the Pro/ENGINEER interface, we can see that our symbol is currently active, as shown in the following figure.

We can start to define our symbol in this blank drawing. The location of the symbol on the drawing is not important, but the shape and size of the symbol is important. We want to create a series of entities that will ultimately allow us to pick the shape of the symbol when we use it. We are going to create three possible shapes for this symbol: Rectangle, Oblong and Oval, as shown in the next figure.

For each of these symbols, we want the ability to show text in the center (as shown above), or not have text. This text has to be different every time it is used, so it must be variable. In addition, we want the ability to place these symbols on the drawing without leaders, or with a leader on the left or right side of the symbol. Sketching The Rectangle The first thing we are going to do is sketch our rectangle. From a size standpoint, we should consider what is more critical, the length or the height. We also want to understand what the relationship is between the two. Why do we care? When we bring in a symbol instance, we have the ability to scale it. Therefore, it makes the most sense to pick whether the length or the height is going to be the driving force behind the scale. For example, if we needed to have a 1” long rectangle one time, and a 2.5” rectangle the next, then we should make the length the driving force behind the size of the rectangle. If we make the length 1” in our symbol definition, then we can directly scale it to the size we want. If we sketch the rectangle at 2” in the symbol, we would have to scale it to 0.5 to get a 1” rectangle, for example. Therefore, we will assume that our rectangle is going to be 4 times longer than it is high. So we want to sketch a 1.0 x 0.25 rectangle on our drawing. Use the tools that we have learned in this lesson to create it, as shown in the next figure.

Now, before we go any further, we might want to turn on grid lines, and snap to grid. To turn on the grid lines, you will select View, Draft Grid from the menu bar. This brings up the following menu.

We will click on Show Grid to see the grid lines on the drawing. Currently we see the following.

We can see that the grid is too large to be useful, and the lines don’t sit squarely on the rectangle that we have sketched. Therefore, we will start by re-sizing the grid. Click on Grid Params, which brings up the following:

We can control the X and Y spacing equally (X&Y Spacing), or set them independently (X Spacing and Y Spacing). We can also change the Angle of the grid. We will pick on X&Y Spacing, and then enter 0.0625 in the message bar. The grid changes to the following.

Clearly, this grid size is better, but the location is not. Therefore, click on Done/Return to get back to the previous menu. On this menu, click on Origin, and select Vertex as the method to select the origin. Pick on the lower left corner of the rectangle, and you will see the grid shift. A coordinate system appears at the origin, as shown in the next figure.

To snap to the gridlines for additional sketching, we will need to go to Sketch, Sketch Preferences, and then click on the Grid Intersection option to activate it. Click on Close, and now we can start to sketch again. Variable Text We are now going to add the text inside the rectangle that will become the variable text in the symbol. If you remember from Lesson 49, variable text is a text note that has backwards slashes around it. Therefore, we will go to Insert, Note from the menu bar, which brings up the following menu.

Many of the options are grayed out while in symbol definition mode. We will leave most of the defaults, but we will change the justification of the text to Center, and then click on Make Note. For the location of the note, click on the grid intersection at the center of our rectangle. Down in the message bar, we will enter \TEXT\ for the note. Be sure to use the back slash before and after the word. Click on <ENTER> twice to finish the note. Our rectangle now looks like the following.

We will want to adjust the text height to make sure it is the correct size for our symbol. We want the text height to be fixed at 0.125 inches. Therefore, click once

on the note to select it, and then right mouse click and select Text Style. This brings up the following window.

Currently, the text height is being driven by the drawing setup file at 0.12 inches. We will uncheck the Default box for the height field, and then enter 0.125, as shown in the next figure.

Click on OK, and you will see the text change slightly. We are now ready to create our first grouping of entities. Group 1 – Rectangle The grouping functionality for symbol definition is slightly different from what we saw in the 2D Draft Group section earlier in this lesson. We will pick on Groups in the menu manager. It brings up the following menu.

Click on Create. In the message bar, you are prompted to enter a name for the group. Enter RECTANGLE and then click on the <ENTER> key. You are now asked to pick the entities to include in this group. Using the Ctrl key, pick the four sides of the rectangle, and also the text note. Click on the middle mouse button once all of these five entities have been selected. You will get a confirmation that the group has been created. Group Attributes Currently, we are defining groups for the top level. We will define the attributes for this level of groups by going to Group Attr, which brings up the following menu.

We want to specify whether the groups at this level are exclusive or independent. Exclusive means that only one option can be selected at any time. If you remember back to when we added a weld symbol, there was a top level that had two or three choices. Only one choice could be selected from this level. This is an example of Exclusive.

Independent means that we can include more than one option from the list in the symbol instance. In the weld symbol that we worked with earlier, you remember how we added two different text notes to the same symbol. These were independent group options at a sub-level. We will click on Exclusive to ensure that we can only show one of the shapes at any given usage of the symbol. Click on Done/Return to get back to our original symbol menu. We will now sketch our oblong shape. Sketching the Oblong We can sketch our oblong shape directly on top of the rectangle, but that might get a little confusing. Therefore, we will sketch the following shape above the rectangle:

Then, we can translate this down to its correct position, as shown in the next figure.

Now, we can click on Groups, Create and enter OBLONG for the group name. When selecting the entities, be sure you are getting the shorter line on the top and bottom, as well as the two arcs and the text note (we need this text note in all of our groups). Sketching the Oval (Ellipse) Now, we will repeat this same process to create the oval shape. The final sketch should look like the following.

Create another group called OVAL, and include the ellipse and the text note for this group. Click on Done/Return from the groups menu when done. Symbol Attributes Now that we have finished defining the entities and groups that make up our symbol, we are ready to define the symbol attributes. Therefore, at the SYMBOL EDIT menu, click on Attributes. This brings up the following window.

This window contains two tabs at the top. The General tab is used to define most of the attributes for the symbol, while the Var Text tab is used to define the variable text in the symbol. Allowed Placement Types On the General tab, the first section is used to define how the symbol will be placed on the drawing. The choices are: • Free – The symbol can be placed anywhere on the drawing with no leaders. • On Entity – The symbol is tied to a geometric entity, such as an edge or vertex on the drawing view. Normal to Entity – The symbol will have a leader normal to the entity selected. • • Left Leader – A leader will be on the left side of the symbol. Right Leader – A leader will be on the right side of the symbol. • Radial Leader – A leader will be attached to a circle, and free to travel around • the circumference. Since we don’t have any complete circles in our symbol definition, this option is currently grayed out. You can select more than one type of placement for a single symbol instance. If you recall, we want to be able to bring the symbol in with or without a leader, and the leaders should either be on the left or right side of the symbol. Therefore, we want to pick Free, Left Leader and Right Leader.

For each of these, you will need to pick the location on the symbol where the leader line goes to. The following figure shows where we would pick for each of these options.

Symbol Instance Height The next section is used to define the height of the symbol. The choices are: Fixed – The symbol height is driven from the original definition, and can not • change. I do not recommend this, because you won’t be able to scale it or change the size later. Variable - Drawing Units – The height is driven by the units on the drawing. • For example, if the drawing is in inches, then the height is governed by inch values, even if the model is metric. Variable – Model Units – The height is driven by the units of the model. For • example, if the model is metric, and the drawing is in inches, then you will be governing the height in mm. Variable – Text Related – You will pick on a text note in the symbol to drive • the height. If you later modify the height of the text, the symbol will grow/shrink accordingly. The unit of height for the text is governed by the drawing units. We will pick on Variable – Text Related, and then pick on the “\TEXT\” note in our symbol as the driving text for the height of the symbol. Attributes The last section on this tab defines how the leaders and text behave. The options are: Fixed Text Angle – The text can not be rotated in the event the symbol is • rotated. Allow Elbow – Allows jogs in the leaders if defined. • Allow Geometry to Mirror – Allows you to mirror the symbol geometry • Allow Text to Mirror – Allows text in the symbol to mirror when the symbol • geometry is mirrored. Allow Text to Flip – Allows the text in the symbol to be flipped and rotated to • maintain its original orientation as the symbol is rotated through 90 degree increments. We will keep the default settings for this section. Variable Text Now, we will click on the Var Text tab at the top of the attributes window, and we will see the following.

The left side of this window lists all text notes that it finds that have back slashes around them. In this case, we only defined one text note. The other large field is used to pre-define values that are available for the symbol. By default, it put the current text in the field. Just to see what this does, add the following words to your list of preset values:

Down at the bottom of the window, we can see some check boxes. The first (Preset Values Only) is used to force people from only choosing from the list of preset values (like the ones that we just entered). If you leave it unchecked, you can type in whatever you want for the value or pick from a list. We will leave it unchecked. The other three boxes are used to define the type for the variable text. Currently, any value we put in (regardless of numeric or alphabetic characters), will be treated as a text string. If we only wanted to use numbers in this field, we could pick on Integer or Floating Point. We will leave it alone at Text. The last thing we can do is add any symbols to our list of preset values by clicking on the Text Symbol button in the lower right corner. This is the same symbol tool we saw when creating notes or changing the properties of dimensions. Click on OK once you have completed all of these attribute settings. Click on Done to complete the definition of this symbol. Write

Now, we will click on Write to save our symbol to our working directory. If we fail to do this, the symbol will remain available in this session, but as soon as we exit out of Pro/E it no longer exists. When you click on Write, you get the following.

This gives you a chance to enter a new directory path to store your symbol, but we will just click on <ENTER> to accept the current location (which is the one we set earlier). You will get the following confirmation: “Symbol [C:\Data\Proetrain\Drawing\my_symbol.sym.1] has been stored.” Here, we can see the full path to the location of the symbol, and the name of the symbol is my_symbol.sym.1. Using the New Symbol in Our Drawing Now, we will test out this new symbol that we created by using it in our current drawing (which should now be back up on the screen). Therefore, go to Insert, Drawing Symbol, Custom. The symbol instance window should appear with the symbol that we just created. If not, click on your Working Directory icon from the Open window that appears, and then open the symbol that we just created. It should look like the following:

We can see that the rectangle version of this symbol is currently active. It is also a good time to point out something critical. If you remember, we used a 1.0” dimension to define the length of our rectangle. Unfortunately, the height of the symbol is being driven from the text height (which by default is 0.12 as defined in the drawing setup file). If you recall, we made the symbol dependent on the text note. Not a big deal, we can live with this, but you will want to make a mental note that 1) height is the most important dimension when text is not being used to drive it, and 2) the text height drives it when you do specify this attribute.

We will enter 0.25 for the height of the symbol. For now, we will also leave the placement type as Free. Click on the Grouping tab, and you will see the following.

You can see the three groups that we created in the symbol. Try picking on each of them to see the shape update in the right side of this window. You will also notice that we can only select one of these options at a time (based on the Exclusive group attribute that we defined). We will select OBLONG for our first symbol instance, and then click on the Variable Text tab, which looks like the following.

We can see our text note is listed as variable text, and we can also see if we use the pull-down field, that our preset values are there, as shown in the next figure.

NOTE: The order in which you entered these preset values is the order that shows up here. It does not automatically sort the words/numbers, so keep that in mind if you want to make a large list of possible values for your symbol. We will enter our own names in the field instead of picking from the list, and then click anywhere on the drawing to place the first symbol. Our first symbol instance is created, and an outline appears immediately for any additional symbols we want to create, as shown in the next figure.

Go back to the General tab. This time, we will change the placement type from Free to With Leaders. When we do this, we see the menu for placing the leader. We will use the On Entity and Arrow Head options (that are there by default), and select on the following edge on the TOP view.

When we do this, we can see a preview of the symbol appear on the drawing.

Click on the middle mouse button to finish the placement for this symbol instance, and you will see it as shown in the next figure.

Click on OK to complete the definition for these two symbols. Try moving around the symbol with the leader, you will notice that you can move the symbol to the other side of the leader line, and an elbow appears automatically. You will also notice that the leader which was on the left, automatically jumps to the right side if the symbol is moved to the left. The following figure shows this.

Save and close this drawing.

LESSON SUMMARY 2D Drafting in drawing mode is somewhat clunky compared to the robust sketcher used in part mode. This will change in a new release. For now, this lesson teaches you how to use the 2D Drafting tools, and some best practices for using them. Symbols are used to reproduce common draft sketches. You can create simple symbols, or even multi-level symbols with groups and variable text.

EXERCISES None

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5 1

Lesson Objective: In this lesson, we will learn how to create basic tables and show balloons.

TABLES vs. REPORT TABLES In Pro/ENGINEER Drawing mode, there are two different types of tables that you can create. They both start off the same way, but a report table takes it to the next level. To clearly define the difference, we will first need to define some key terms:

Parameter – As we learned in Lesson 34 – Parameters and Relations, a parameter is used to capture data for the model that can then be used later for different purposes. A good example of a user defined parameter is PART_NO. This parameter is used to capture the part number of the object. Typically, you would report this information on the title block in a drawing, and in Bill of Material tables. Repeat Region – A repeat region is a grouping of table cells that gather information from the model, process it according to different rules set up by the user, and then reported back to the table in as many rows as it needs to accomplish the reporting. A good example of a repeat region is one that gathers Bill of Material information from an assembly. Depending on the type of information gathered, and what you want to output, the table can be as long as the number of models in the total assembly. Report Symbol – A report symbol is a special parameter used in repeat regions. It represents a full path to the location where data is stored. For example, the PART_NO parameter that we talked about earlier is typically stored in the model (part and assembly files). When the repeat region wants to extract this information from an assembly, the first thing it needs to know is how to get to this parameter. In plain English, one might say that the PART_NO parameter resides in the model which is a member of the assembly. In report symbol language, this would look like the following: asm.mbr.part_no Where asm represents Assembly, mbr represents Member, and part_no is the parameter that we are looking for. There are hundreds of possible report symbol paths that can be used to pull data from models of varying types. So, if you think back to a Bill of Materials table, as the repeat region starts to gather information, it goes from one component of the assembly to the next, gathering the value of Part_No for each model it encounters. Some models are used more than once (screws, for example), so the value that it finds is duplicated, but counted. When it is done gathering the values, it processes them. We might set up a rule that we don’t want to have duplicate rows, therefore, when the output is created, for every value of Part_No that is identical, it tries to combine them into a single row of the table. The more report symbols you have reported in your table (in separate columns), the better the chances are that there will be fewer identical rows created. This helps in calculating quantities. We will see all of this in more detail as we create a bill of material table in an upcoming example.

CREATING A TABLE Since Report Tables and regular Tables start off the same, the first thing we’ll learn is how to create a table. Therefore, we will open up the 51_BOM.drw drawing located in our working directory. It looks like the following.

This is an assembly drawing (the model is 51_BOM.asm). There are two views. Both of these are general views. One of them is showing an exploded state that was created in the assembly. The other is a scaled isometric view to show what the assembly looks like together. We are going to be creating a Bill of Materials table in the lower right of this drawing. Building Rows and Columns To start a table, we will go to Table, Insert, Table in the menu bar. This will bring up the following menu.

At the top, we have two options: Descending and Ascending. Descending means that the table is typically read from top to bottom, and any repeat regions that may expand in this table will expand downwards. Ascending means that the table is typically read bottom-up, and any repeat regions will expand upwards. Our BOM tables are typically Ascending, because they start just above the title block, and expand upwards. For the purpose of this training guide, we will use the default of Descending. The next section has two options as well: Rightward and Leftward. Rightward means that we will read from left to right, and any two-dimensional repeat regions will expand out to the right. Leftward means that we will read from right to left, and any two-dimensional repeat regions will expand out to the left. We will talk about twodimensional repeat regions later in this lesson. For now, we will keep the default of Rightward. The third section from the top contains two options also. These are: By Num Chars and By Length. By Num Chars means that the width and height of the cells we create will be based off of the number of characters of text that will fit exactly in that space. By Length means that we will specify the actual length in the drawing units we use. For example, we may want a cell to be 1.5” wide, and .25” tall. The choice here really doesn’t matter, because most of the time we will adjust the actual width and height of the cells after the fact. I do find it easier to use By Num Chars when defining the table initially, because there is fewer input needed. Therefore, we will keep this default option. We are now asked to start the upper left corner of the table (because of Descending, Rightward options). We will pick out on the drawing to the right of the exploded view, and below the scaled general view. Once we pick the location for the upper left corner, we see the following.

The numbers across the top of this figure indicate the number of characters. Each zero represents the next “tens” of characters. The single vertical line at the left of this figure represents the left border of the first cell being created, as shown in the next figure.

The purpose here is to pick on the number that represents the number of characters you want for the width of the column. Personally, I pick at about the “10” location for each column I want to add just to do it fast. Therefore, we will do the same. Pick on

the first 0 (or close to it) that you see in the line of numbers. When we do, we see the following.

From this figure, we can see that we have defined our first column (left and right border). Every “0” that we pick on from here adds one more column. We want to have three columns in our table, therefore we will pick on the first 0 in this list, and then the first 0 of the next list of numbers, until we see the following.

When we are done defining columns, we click on the middle mouse button. This will cause the table definition to switch over to defining rows, as shown in the next figure.

Again, the numbers going down in the list represent the number of characters for the row height. I like to pick on the 3 for each row I want to add. We will add three rows, therefore, pick on 3 a total of three times to get the following.

We will click on the middle mouse button to finish defining rows once we have three created. This will give us the table shown in the next figure.

We are now ready to start setting up the table. Selecting Table Entities We are going to take a moment to learn about selecting a table or selecting rows, columns or cells. Start by clicking anywhere outside the table to make sure it is completely unselected. Then, bring your mouse cursor just outside the upper left corner of the table. When you do this, you should see the entire table highlight in blue, and if you wait a few seconds, a tool tip will appear, indicating that you are previewing the entire table, as shown in the next figure.

Selecting now will select the entire table, and then you would have the ability to perform any operation that can be done on the table as a whole, such as move or delete the table, rotate it, change the height and width of all cells simultaneously, etc. This works for any of the corners, just by bringing your mouse to the corner itself. If you place your mouse to the left or right of any row in the table, you will see the entire row highlight, as shown in the next figure. NOTE: Your mouse must be outside of the table, or on the outer edge of that row.

If you place your mouse just over or just below any column in the table, that column will highlight, as shown in the next figure.

Finally, if you place your mouse cursor into the middle of any cell, just that cell highlights, as shown in the next figure.

Clicking with the left mouse button once you see the entity highlight will select that entity, whether it is the entire table, the row, the column or the cell. To select multiple rows, columns or cells, use the Ctrl key. Merge Cells Before we start adding any text to the table, we should perform any merge cell operations. We want to merge all of the cells in the top row into a single cell. Therefore, we are going to select all three cells using the Ctrl key to do this. Once you have all three cells selected, go to Table, Merge Cells. Click outside of the table, and you will see the following.

We are now ready to add the static text to the table. Entering Text (Static) Static text is text that is not part of a repeat region. Basically, all text not in a repeat region is going to be static text. To add text to a table cell, double-click on that cell, which brings up the following properties window.

We will type in the following text in the large field provided: BILL OF MATERIALS, as shown in the next figure.

Next, click on the Text Style tab at the top. When the text style window opens, make the following changes: Font = filled • Text height = 0.1875 • Width Factor = 1.0 • Horizontal Justification = Center • • Vertical Justification = Middle The following figure shows what this window should look like.

To see what the text will look like, click on the Preview button. Click on OK to complete this text. Our table now looks like the following:

We will repeat this process to add text to each of the cells in the middle row. The only text style change that we have to make for each cell is: Horizontal Justification = Center • Vertical Justification = Middle • When done, your table now looks like the following.

Obviously our first and third columns are not wide enough – even for the titles. We could fix this right now, but we still don’t know how much room our repeat region is going to need once it fills in with data, so it really is up to you whether you want to fix it now, or wait until later. For practice, we will change it now, and probably again later. To adjust the width of the first column, we first select the entire column (as discussed in the section Selecting Table Entities earlier). Once we have the column selected, we right click and select Width. This brings up the following window.

We can see that the Row fields are currently grayed out, because we selected a column. We can change the width in the number of characters (currently 9) or the actual length (1.248” currently). So you see, when we first started creating the table, it was easier to just pick random cell widths using By Num Char, because we can come in here later and specify exactly what we want. We will change the width of the column using the drawing units field with a value of 1.5”, and then click on OK. Our table updates as follows.

Repeat this for the third column, and use a width of 3.0”. The table will look like the following after this change.

The only other change I might make at this time is to change the height of the last row (bottom) to 1 Character. To do this, select the entire row, right click and select Height. This will bring up the following window.

This time, since we only picked a row, the column fields are inactive. We will change the 2.0 to 1.0. Click on OK, and you will have the following table.

We are now ready to create a repeat region. Save this drawing first.

REPEAT REGIONS Not all tables that you create will have repeat regions. In fact, most of the tables you create may only have static text in them. The most common tables with repeat regions that I have created or have seen created are: Bill of Material Tables • • Pipe/Cable Cut-Length Tables Part Parameter Tables • Family Table Driven Tables (Two-Dimensional) • Miscellaneous Manufacturing-Mode Tables • By contrast, all of the tables in the drawing formats are tables with static text. Some of the static text actually pulls value from part, assembly or drawing parameters, but does not belong to a repeat region. Creating A Repeat Region There are two ways to create a repeat region. The first is to select a row, and then right click and select Add Repeat Region. The second method is to go to Table, Repeat Region, and then select Add from the menu manager that appears. We will do the latter of these two, since most of the other Repeat Region functionality is through the menu manager. Therefore, go to Table, Repeat Region. This brings up the following menu.

To add a repeat region to a table that currently does not have one, we would use Add. when we click on this option, we get the following sub-menu:

Simple is used to create most repeat regions. Two-D is only used to create twodimensional repeat regions. We will have a completely different section devoted to two-dimensional repeat regions, so for now, we will click on Simple (which is already the default). In the message bar, we get the following prompt: “Locate corners of the region.” We are supposed to pick the first and last cells that make up the region in a row. Therefore, we will click on the following.

NOTE: You do not need to hold down the Ctrl key for this. When you select both cells, the only way you’ll know that you successfully created the region will be the following message bar statement: “Region has been successfully created.”

To verify that a region exists, we will go to the TBL MANAGER table, and select on the Switch Syms command. If we have a repeat region in our table, the region will outline in green, as shown in the next figure.

The Switch Syms command is used to let you get back to the report symbol names once you add them to the table to see what they are. We will see this soon. For now, just remember that it is the way to see into the repeat region. We will click on Switch Syms once more to go back to the table view (the green outline should disappear). Removing Repeat Regions Had we needed to remove a repeat region from our table, you would go to Table, Repeat Region, and then select Remove from the menu manager. We will leave our repeat region in our table. Adding Report Symbols The method to add a report symbol to our repeat region cell is the same as entering static text, but the result is quite different. Therefore, double click in the first cell of the repeat region. When we do this, we see the following.

The way this works is that you select a category for the first screen. For example, if you were adding a parameter from the model to fill in a Bill of Materials table, (PART_NO, for example), you would select asm in this first screen. Once you select a category, the screen updates to show only additional subcategories that are related to the first one you picked. We will pick on asm first, and our window updates as follows.

On this window, we can see three options. The first one, labeled UP, takes you back to the previous screen (in case you made a mistake). We then have mbr and name to choose from. One other thing to point out is that one of the options has three dots (periods) following it, while the other one does not. Any symbol that has dots means that there are further sub-options for this selection. In this case, name does not go any further. In case you are wondering, asm.name would report back the name of the top level assembly, which for a bill of materials table doesn’t do much for us. Therefore, we will click on mbr…, which brings up the next set of options.

We can see that there are a lot of options at the assembly member level. There are a few to point out here. First, the name option doesn’t go any further. Asm.mbr.name will give back the actual file name for the model in the assembly. This might be useful if the name used for the part is the same as the part number parameter. Often, this is not the case (especially for inseperable assemblies). Type also does not go any further. Asm.mbr.type would give back the type of file it is (PART, ASSEMBLY, BULK-ITEM, etc.)

The third one that doesn’t go any further is User Defined. User Defined allows you to type in a value for the last symbol. This is what we use for capturing model parameters (PART_NO, for example). Therefore, if we select on User Defined, the message bar prompts for the name of the symbol text we want to enter. We will type in PART_NO, as shown in the next figure.

When we click on the <ENTER> key, we will see the following in our table.

We will continue this same process by double-clicking on the last two cells and entering the following: Second cell – rpt.qty • Last cell – asm.mbr.TITLE (NOTE: Use the User Defined option, and type in • TITLE) Rpt.qty will give us the reported quantity. We will describe how this works soon. asm.mbr.TITLE will give us the description of the part by using the TITLE parameter in the model. The table should look like the following when these two cells are done.

Don’t worry about the fact that the first report symbol (asm.mbr.PART_NO) doesn’t completely fit inside the cell. The actual value that is reported from the parameter is what we care about, not the entire path to that value. To see the actual values from the model, we need to update the repeat region. To do this, go to Table, Repeat Region, Update Tables. When we do this, we see the following.

Do you know what is going on here? Unfortunately, the PART_NO and TITLE parameters were never filled in for the models. Therefore, their default values are reporting, and are all identical. We have no idea which row represents what component on the assembly. This is why it is critical to fill in parameter information in the model. Therefore, we will have to go do this. MODIFYING PARAMETERS The easiest, and fastest way to do this will be to open up the assembly model itself. Once you have the 51_BOM.asm assembly open, we are going to focus on the model tree. At the top of the model tree, pick on Settings, Tree Columns, as shown in the next figure.

This brings up the following window.

Using the Type pull-down menu, select Model Params, and then add PART_NO and TITLE to the list on the left, as shown in the next figure.

Click on OK, and your model tree will update as follows.

Now, we can click on the value in the PART_NO and TITLE columns and edit the value. We will type in the following parameter values for each part and the top level assembly.

Save the assembly, and return to the drawing, which should now show the updated table, as we can see in the next figure.

Now we can see that our DESCRIPTION column is not wide enough to accommodate the values. We will change the width of this column to 4.0 inches, and our table now looks like the following.

We are getting close to a completed table. There are some attributes we should set to get the table to be completed. Repeat Region Attributes Go to Table, Repeat Region, Attributes, and pick on the repeat region in the table. This brings up the following menu.

In the first section, we see the following options: Duplicates – Allows multiple rows with the same data to exist. This is why we • see several rows that look identical to each other. Unfortunately, Duplicates will not show a quantity in the quantity column (which is why we don’t see any right now). No Duplicates – Does not allow duplicate rows to exist in the table. For any • two or more rows that are the same, the repeat region will calculate the total number of these rows and report that quantity in the second column. No Dup/Level – Does not allow duplicate rows to exist for each level of the • assembly. This option only works if you have your level reporting set to Recursive. The second section is used to identify the level of the assembly reported. The options are: Recursive – Shows all levels of the assembly, including the assembly itself. • Sub-assemblies will show all of their components on the table as well. Flat – Only reports the items at the top level of the current assembly. • The next option, Min Repeats, allows you to specify the minimum number of repetitious rows allowed in the repeat region. The default is 1, which will allow for blank lines to appear if data is missing from certain components. I recommend keeping this setting at 1 unless you have an advanced table function you are trying to work with that requires the number to be set to something else. The following section deals with indexing numbers. The options are: Start Index – Allows you to specify the number that the repeat region starts at • when indexing rows. No Start Idx – Always starts the numbering at “1”. • In the next section, we see the following two BOM Balloon options: Bln By Part - When you suppress or replace a component to which a BOM • balloon is attached, this command reattaches the balloon to another placement of the same part. If no other copy of the part exists in the assembly, then the BOM balloon disappears from the drawing. Bln By Comp – Specifies that simple BOM balloons reattach themselves to • whatever component replaced the one that originally owned the BOM balloon.

The last section deals with Electrical Cable reporting. Since we don’t use this module, we will not go over this section. For our table, we will set the attributes to No Duplicates, Flat, and Bln By Part. When we select these options, and then click on Done/Return, the table updates to the following.

We can see the quantity field has now updated to show the quantities. Again, keep in mind that the quantity field (rpt.qty), will report the total number of rows that contain the identical information. If we were to change the PART_NO parameter and TITLE parameter values for the 51_A component to match those of the 51_B component, then we would see one row with a quantity of 5 instead of 4. So this quantity is only as accurate as your parameter information. The good news is that we can assemble in two models that (for one reason or another) had to be modeled as separate parts but they represent the same part. By making their parameter information identical, the BOM table will report 2 for the quantity instead of two separate lines. To go back and see the report symbols that were used in this table, we would click on Switch Syms again, and we would see the following.

We can still see all three rows, but only the first row shows values (the report symbols that we used). Click on Switch Syms again to get back to the parameter values.

ADDING ROWS/COLUMNS One column that we typically show in BOM tables is an indexing number that is used to correlate to BOM balloons. Unfortunately, we do not have one in our table right now.

To add a column to our table, we go to Table, Insert, Column, and then pick close to the side of the cell where we want to add the column. If we pick toward the left side, it adds a column before the one we picked in. If we pick toward the right side, it adds a column after the one we picked in. The index column typically comes first in the table, so we would want to pick in the following location.

When we do this, a column is indeed added to our table, as shown in the next figure.

Unfortunately, if we use the Switch Syms command, we can see that our repeat region was not expanded into the new column.

Therefore, we will delete this column that we just added. Click on Done from the repeat region menu. Select this column, and then hit the delete key. We get the following warning.

You will get this message because a repeat region exists in the table, not because we actually do span a repeat region. So we will click on Yes, and our column is now gone. Therefore, we will have to do something else to get the column into the table. We will go to Table, Insert, Column again, and this time pick on the following location.

The column is now added in between PART NUMBER and QTY, as shown in the next figure.

The good news is that our repeat region does span the entire table, and we can now cut and paste the text from the first column into the second. To do this, we will click once on the cell containing the static text “PART NUMBER”. While this cell is highlighted, click on Ctrl-C (Edit, Copy) and then click into the empty cell to the right of it, and press Ctrl-V (Edit, Paste). The text appears in the second cell, as shown below.

We will do the same for the report symbol in the next row, giving us the following.

Now, we can go in and edit the text style to justify them like the originals, as we can see in the next figure.

The last thing we need to do is edit the text in the first column. For both cells, double-click and enter the appropriate values: INDEX for the static text cell, and rpt.index for the repeat region report sym cell. The following figure shows the table when changed.

Now, go back to Table, Repeat Region, Switch Syms, which will give us the following.

On your own, center justify the report symbols for the INDEX and QTY columns. HINT: You only need to do it for the cell that contains the report symbol, and all other filled in cells will get the same result. The table will look like the following with the justification.

At this time, our drawing should now have a completed bill of material table, as shown in the next figure.

Save the drawing.

BOM BALLOONS In Drawing mode, there are two types of balloons you can show/create. On the drawing toolbar, there is a balloon note. This is nothing more than a balloon symbol with variable text that you manually input. The other type is tied to repeat regions, and fills in automatically from the BOM table. You can show these balloons on the views automatically, just like dimensions, and then clean them up. I always recommend using the automatic balloons for linking to BOM tables instead of creating balloon notes. Showing BOM Balloons We are going to continue to work with the same drawing (51_BOM.drw). From the menu bar, select Table, BOM Balloons. This brings up the following menu.

At this time, we need to identify what type of balloon we want to use. There are three choices: Simple – Creates a circular balloon that only lists the index number. You have • the ability to report any report symbol in the balloon, but no quantity is shown. With Qty – Creates a circular balloon that lists the index number and quantity. • The index number can be replaced with any other report symbols in your table. Custom – Can use any custom symbol you have defined as long as it as either • \index\ or \index\ and \qty\ defined as variable text. This would allow you to create a balloon that was oblong in shape, or oval, or a star, etc. To start, we will select Simple, and then pick on the repeat region in the table. NOTE: You need to pick what type of balloon you are going to use BEFORE you select the repeat region. If you pick the repeat region first, it takes whatever value is highlighted in the bottom section (which is usually Simple by default).

Now that we have picked the repeat region, the rest of the menu options become available, as shown in the next figure.

We will now click on Create Balloon, which brings up the next menu.

We can show balloons by view, by component, or by component and view, or we can simply show all balloons. Since we will only have three balloons (one for each row in the BOM table), we will click on Show All. When we do this, the three balloons appear on the drawing, as shown in the next figure.

We can see that the shape is a circle, and there is an indexing number that corresponds directly with the index number in the BOM table. These balloons are directly linked to the table. If we were to sort the table differently from how it is now, the index numbers would change to match the table. Edit Attachment for Balloons By default, the balloons are going to appear on the drawing view where you can clearly see the component that the balloon references. In this case, all three balloons went to the larger exploded view – which is perfect for what we need. The default attachment type is a leader with an arrow head that points to an edge on the component that represents the row the balloon is tied to. You can not change a balloon reference to point to a different component than what it currently belongs to. This is not true with balloon notes, which have no intelligence. For example, component “1” and component “3” only exist once in the assembly. The balloons for these can only touch edges or surfaces for the single models in the drawing view. Component “2” however is used four times in the assembly. Therefore, it could be attached to any one of the four components on the drawing view. We will show how to change the entity to which the balloon references. To do this, first select the balloon with the “2” in it. When it highlights in red, use the right mouse button to select Edit Attachment. This is shown in the next figure.

This will bring up a familiar menu that we saw when placing notes on the drawing.

We will select the On Surface and Filled Dot options, as shown above, and then pick out in the middle of the surface that the balloon is currently touching. Click on Done/Return, and refresh your window to see the following.

Typically, you should use an arrow head when pointing to an edge, axis, vertex, or datum curve. Use a filled dot when pointing out in the middle of a surface. Clear Region If you want to remove all balloons from a drawing, the easiest, and preferred method is to clear the region. We are not going to do this, but if you did want to – you would use Table, BOM Balloons, Clear Region, and then pick on the repeat region. You will get a prompt to clear the region. Change Type We want to use a With Qty balloon instead of a simple. To change all balloons over to a different type, we use Table, BOM Balloons, Change Type, and then pick on the repeat region. This brings back up the menu with the three types: Simple, With Qty, and Custom. We will pick on With Qty, followed by Done/Return. The balloons will change to look like the following.

In this symbol, there are two numbers. The number on top is the index number. The number on the bottom is the quantity. We can see that the balloon for item “2” shows a quantity of “4”. Split When you have quantity balloons, any balloon that is reporting more than a quantity of “1” can be split up. This is extremely common for fasteners or library-type items that may be used all over your assembly, and in sub-assemblies. We will demonstrate this with a simple example. We can split up the quantity balloon for component “2”, because our quantity is “4”. We can not split up the balloon for components “1” or “3”, because they only have a quantity of 1. To split the balloon, go to Table, BOM Balloons, Split, and then pick on the balloon to split. We will pick on the component “2” balloon. When we do this, we get the following prompt in the message bar: “Enter amount [Quit]”. We will enter 1 and then hit the <ENTER> key. We are now asked to pick the location on a different instance of this component, and we will pick in the following location.

The surface will become selected, and we will use the middle mouse button to locate the balloon out to the location where the “Select Here” note is in the figure above. Our completed balloon is shown in the next figure.

We can see that the new balloon contains only the quantity that we specified (1), which is subtracted from the original balloon (4-1=3). We can now edit the attachment for this new balloon to select Filled Dot, to get the following.

Save the drawing. Merge The opposite of splitting up a balloon is to merge a balloon. When you merge two quantity balloons together one of two things will happen: If the two balloons represent the same component, a single balloon will result • with the sum of the two quantities. If the two balloons represent different components, the one that is merging with • the other will attach itself to the outside of the other, and its leader will disappear. We will demonstrate both of these. Same Component Merge We will start by going to Table, BOM Balloons, Merge. In the message bar, we get the following prompt: “Select quantity balloon to be merged.” We will pick on the component “2” balloon that has a quantity of “1”. Once we pick this, we get the following prompt: “Select quantity balloon to be merged onto.” We will pick on the

other component “2” balloon with a quantity of “3”. When we do this, only one balloon remains, with a quantity of “4”, as shown in the next figure.

Different Component Merge Now, we will go to Table, BOM Balloons, Merge, and for the first balloon, pick on the component “3” balloon. For the second balloon, pick on the component “1” balloon. We will get the following result.

We can see that the component “3” balloon attached itself to the side of the component “1” balloon. If we drag around the “1” balloon, “3” moves with it. When do you typically use something like this? Suppose you are mounting a plate that gets fastened down with four hex head machine screws, four lock washers, four flat washers, and four lock nuts. Instead of showing balloons for the plate, the screw, the washer, the lock washer, and the nut, having leaders going all over the place, it is cleaner to show the balloon for the plate with the leader, and then merge the rest of the balloons to this one. Doing this sort of “implies” that the hardware is tied to the plate, and also helps in the assembly of the plate. Another good usage is if it is part of a kit that came with these different (but separate) components. By merging the balloons together, you can imply that they are all together, possibly even before they are assembled together into the top level assembly. Save and close this drawing.

TWO-DIMENSIONAL REPEAT REGIONS In this section, we will learn about two-dimensional repeat regions. If you recall from our repeat region tables before, our regions expanded in a single direction. A 2D Repeat region expands in two directions. The most common type of 2D repeat region is a family table driven table. To demonstrate this, we will open up the 2D_Rpt_Region.drw drawing, which initially looks like the following.

This drawing will be a tabulated drawing for a family table of steel blocks of varying sizes. As we learned in Lesson 35 – Family Tables, there is some preparation that is done to the model to get it ready for a family table. This model has three dimensions: LENGTH, WIDTH, and HEIGHT. It also has parameters. Our family table has all of these dimensions as varying items, and we also have the TITLE parameter to capture the different descriptions for the individual sizes. We went ahead and modified the dimension symbol names to their respective titles (LENGTH, WIDTH, and HEIGHT). We then created the family table and added these three dimensions, followed by the TITLE parameter. The family table was then verified to make sure all instances are working. On the drawing, we added two views, and we are showing the dimensions for the block. We went into the properties for these dimensions, and changed the display from “@D”, which displays dimensional values, to @S, which displays the symbolic name for the dimension. That is why you can see “LENGTH”, “WIDTH” and “HEIGHT” on the drawing views. Then, we created a simple 2-column, 3-row table, and merged the two cells together in the first row. We added some static text in the first row, and in the first cell of the second row. The last thing that was done was to justify the text in the cells. I took the liberty of adjusting the text justification in the empty cells as well, because I know what the final result will look like, and I wanted to clean it up ahead of time. Creating the 2D Repeat Region We will now go to Table, Repeat Region, Add. In the lower section of the menu manager, we will select Two-D. We get the following prompt in the message bar: “Locate corners of the outer boundary of the two-dimensional region.” We will pick on two cells that define the upper left corner and lower right corner of the region we are creating. Therefore pick the cells in this order:

NOTE: If your table were ascending and/or leftward, the order of selecting the corners would be different. Once we pick the second cell, we get the following prompt: “Select a cell to set the upper border of the row & column subregions.” This time, we have to pick the cell that is going to be expanding in two directions simultaneously. If you imagine that the last cell in the second row only expands to the right, and the first cell in the third row only expands down, then the cell in the lower right corner of the table (the one that is labeled “Pick Second” in the figure above) is the one that expands both down and to the right.

Therefore, we will pick on the cell in the lower right corner of the table. When we do this, we get the following confirmation: “Region has been successfully created.” Click on Done to complete the definition of this region. We will now go to Table, Repeat Region, Switch Syms, and we see the following.

We can see a single green rectangle that goes around all four cells. Then, we have a rectangle that just goes through the last row, and another rectangle that goes through the last column. We will now add our report symbols. Report Symbols Double-click on the second cell in the second row, and use the following report symbol path: fam.inst.param.name, as shown in the next figure.

This report symbol will take the parameter name from the family table instances (such as LENGTH, WIDTH, HEIGHT and TITLE) and add them as columns to the table. Notice how this text is already centered and is in a bold (filled) style? Now, double-click on the first cell in the last row, and add fam.inst.name to this cell, as shown in the next figure.

This report symbol will show the family table instance names and report them as rows in the family table. Again, we have already left justified this text, and made it bold. The last cell will contain the fam.inst.param.value report symbol, as shown in the next figure.

This report symbol will show the value for the parameter (LENGTH, for example) for each instance in the family table. Therefore, this will report as the columns are added, and as the rows are added. If we now go to Table, Repeat Region, Switch Syms, we will see our expanded table.

There are a few things to point out that we will need to address. The first is that our header row isn’t merged all the way across. Therefore, we will need to pick on each cell (while holding down the Ctrl key), and then go to Table, Merge Cells. This will fix this, as shown in the next figure.

The second thing to point out is that all of our columns (starting with the HEIGHT column) are all the same length. We can not change this. Because the original table

didn’t have all of these columns, it takes its width from the last one in the repeat region. We had to make the column wide enough to accommodate the TITLE column, which meant that all the rest of our cells are large compared to their data. The last thing to note is that the columns (starting with HEIGHT) are in alphabetic order. This is okay, except that we might want to show the WIDTH right after the other dimensional columns. When we create our family table, we add dimensions and parameters in a particular order (or at least we should). The order in the family table itself can be shown on the drawing by going to Table, Repeat Region, Sort Regions, and then pick on the repeat region. This brings up the following menu.

To create your own sorting, you would click on Add and then define the type of sort (ascending or descending), and then pick on the cell to sort by. There is a Default Sort, which is already selected. This default sort is what is currently controlling our table. We also can see an option called No Default, which will show the table columns in the same order as they appeared in the family table itself. We will click on this option, followed by Done, which will make our table appear the way we want it.

Save and close this drawing.

LESSON SUMMARY Tables are used frequently in drawing mode, especially for assembly drawings where Bills of Materials are common. Take advantage of repeat regions to make your tables dynamic.

You can save out your tables and retrieve them in later. The report symbols in the tables will automatically read from whatever model is currently active at the time the table is created or updated. Use BOM Balloons in conjunction with BOM Tables to get the maximum automation out of your drawings. There is a lot more functionality with Report Tables and Balloons that wasn’t covered in this fundamentals course. Feel free to contact your CAD Administrator to learn more.

EXERCISES None

Les son

5 2 Lesson Objective: In this lesson, we will learn how to add additional drawing sheets, and finalize the drawing.

MULTI-SHEET DRAWINGS Most of the drawings we create are multi-sheet drawings. There just isn’t enough room on one sheet for the drawing format, BOM Tables (for assemblies), revision history blocks that grow over time, and all of the views, dimensions, notes, symbols and balloons necessary to detail out the drawings. You can create drawings with as many sheets as you need to clearly define your product. As you have learned over the last 10 lessons, it is easy to add views, show/create dimensions, move those dimensions around to other views, create geometric tolerances, etc. It is often easier to do these steps on one sheet and then move views (completely detailed) to their final residence – even if that means it is five sheets into the drawing. Therefore, we will look at a drawing example to learn how to add sheets and move views to other sheets. Adding Sheets To demonstrate this, we will open up the drawing entitled Multi_Sheet.drw, which currently has one sheet with many views that are detailed. A lot of these views reside outside of the boundary of the first sheet. The following figure shows this drawing currently.

Most of the views that are outside of the sheet boundary are detailed or sectioned views. There is an auxiliary view as well. In preparation for moving the auxiliary to a different sheet, view arrows have been shown, and a view note is currently related to the view to indicate which view it is. This is a good practice to get into, because otherwise, someone may not understand how the auxiliary view was projected. The first step is to add an additional sheet. Therefore, go to Insert, Sheet. A new drawing sheet is added to the drawing. Notice how the drawing format is different for the second sheet. All other sheets added will use this format.

At the right end of the drawing toolbar, use the up or down arrows to switch back to sheet 1. Back on sheet 1, we will use the Ctrl key and select all of the drawing views that are outside of the border. Once all are selected, go to Edit, Move Item to Sheet. In the message bar, you will see the following prompt: “Destination sheet number (you can start a new sheet) [Quit].” We will enter 2 in this field, and then press <ENTER>. When we do this, we are placed back into sheet 2, and we can see the views where they were previously.

We will now move these views into the border for the second sheet, as shown in the next figure.

Save this drawing.

FINALIZING THE DRAWING The biggest thing you can do to make sure your drawing is ready to go is to make sure your parameters are filled in completely. You can tell by looking at your title blocks, revision history block, and drawing margin blocks to ensure the data is accurate. Check your weight on your drawing and make sure it is reporting the correct mass. If not, you may have to adjust your density (if you hadn’t already). If you use more than one model for your drawing, then make sure the active model is the primary model for your drawing. Be sure all of your views have been regenerated and refreshed, and ensure your layer status is set to blank the necessary items. This is critical, because if you just turn off the display of datums on your computer, the next person might not, and they will see screen clutter.

LESSON SUMMARY Add additional sheets to your drawing as necessary to fit your drawing views clearly. It is easier to detail your views on a single sheet, and then move them to other sheets. Finalize your drawing by checking parameters, layers and active models.

EXERCISES None

Les son

5 3

Lesson Objective: In this lesson, we will learn about some additional miscellaneous system functions, such as the configuration files, model setup, feature operations, color and appearance, model player, cosmetic sketches, analyses and how to obtain floating modules.

CONFIG.PRO As we have mentioned throughout this guide, there is a configuration file that drives the behavior of Pro/ENGINEER. This file is called Config.pro. When you launch Pro/ENGINEER, the software automatically reads in this file from two locations, in the following order: Loadpoint\text Directory (C:\ptc\proewf2\text, for example) • Start-In Directory (C:\Data\proewf2, for example) •

If you launch from a batch file, as we typically do, a global config.pro file gets copied to the first location listed above. This file may get updated periodically to ensure consistency throughout the user base. If you choose to add mapkeys, or other options to your environment, you are encouraged to create a brand new, blank config.pro in the second location. IMPORTANT: Do NOT simply copy the one from the first location to the second location, and then make changes. The reason for this is because any option that is listed in the first file will be overwritten by the second file if it contains that same option. For example, there is a bell that beeps every time you execute a command in Pro/E. We turn this bell off. If the global config.pro as the option BELL No, and the one in the start in directory has BELL Yes, then the bell will always be on. This might seem trivial, but if we change a global setting because of potential issues that we have seen in the software, and your start-in config was a copy of the global before the change was made, then the net effect will be that the change was never made for your computer. To access the Config.pro file options, go to Tools, Options. You will see the settings that are currently read into your session. If you make any changes, it automatically saves it to the location indicated in the upper left corner. In addition, a Session.pro file is created that only lists the changed options.

CONFIG.WIN There is a second configuration file that defines the look of the tool. This is called Config.win. The Config.win file is used to define what icons you see in the different modes, the location of model trees, dashboards, browser settings, etc. There is a global config.win file as well, and I recommend using it. To access the Config.win file options, go to Tools, Customize Screen. If you need assistance in customizing one of these files, please see your CAD Administrator.

MODEL SETUP (Units, Density, etc.) To get to some setup options for the model, go to Edit, Setup from the menu bar. You will get the following menu.

Units When you select Units you will get the following window.

The red arrow and highlighted row show you what unit is currently set. We would pick on the units that we wanted to change it to, and then click on Set. This brings up another window, which is shown at the top of the next page.

You have two options, which are: Convert Dimensions – This will keep the overall size of the geometry the • same, and do a straight conversion on the numbers. For example, suppose you had a cube that was 1.0 inches in size. If you use this option, the cube will still be 1.0 inch in size, but if you were to edit the feature, you would see 25.4 if you switched to millimeters. Interpret Dimensions – This does the reverse. This keeps the dimension • value the same, and turns it into a different unit. In the same example, the 1 inch cube would become a 1 millimeter cube with this option, since the value of 1.0 stayed the same. Density (Mass Property) To set the density for the part, pick on the Mass Props menu choice. It brings up the following window.

FEATURE OPERATIONS (Copy, Group, etc.) When you select Edit, Feature Operations you get the following menu.

Copy Use this command to copy any solid feature by either translation, rotation or mirroring about a selected plane. This is the only way to mirror a solid feature. To mirror, click on this command, then pick the feature(s) to be copied. You will get the choice to make the copy dependent on the original for size and shape, or make it independent so you can modify it separately. Once you have picked the feature(s), click on Done, then pick the mirroring plane or planar surface. The feature will be mirrored. Group When you click on this command, you will get a File Open window to go out and try to retrieve a user defined group. In the menus, you will select Local Group, and then enter a name for the group in the message window. After you enter a name for the group, pick on the features in the model tree that are going to be grouped together. The features should be modeled sequentially. To ungroup, right mouse click on the group in the model tree and select Ungroup. Reorder You can and should reorder in the model tree by dragging the feature up or down to its new place. If you have a lot of features, you can save some dragging time by going straight to this command. When you use this command, it asks for the feature(s) to reorder, then it asks you to select the feature that you wish to reorder after. Assuming that there are no problems with parent/child relationships, it will reorder then regenerate the model. Insert Mode You can and should drag the red arrow that says “Insert Here” in the model tree to the location where you want to insert a new feature. If you have a lot of features, you can save some time by using the command here. After you select this command, click on Activate. You will be asked to pick on the feature to insert after. To cancel out of insert mode, click on Cancel. This will regenerate all the features that were currently suppressed, and take you back to the end of the model tree. Read-Only Be careful using this. When you click on this command, you will pick a feature in the model tree. All features before the selected one become read-only. You can’t edit a dimension or redefine the features if they are read-only. You will need to use Clean in the Read-only menu to clear this status. Suppress

Suppress is used to turn off features from the regeneration sequence. They disappear from the model. You should only use suppress in the following cases: Family table features. Use suppress in the generic and instances to turn of • features that are not in that instance. Failure recovery. Temporarily suppress failing features so you can go in and • fix them or other features one at a time. Design Iterations. Temporarily suppress a feature to try a different • possibility. Delete the ones you end up not using. Other than in family tables, there should never be any suppressed features in your model when you go to release it.

COLOR AND APPEARANCE Adding color to your models is a great way to visualize them. To add colors, go to View, Color and Appearance from the menu bar. It will open up the window shown in the next figure.

If you have a saved color file, then you can load it in, or it may already be loaded. We can see from this figure above that there are no pre-defined colors in this session. To add a new color, click on the “+” symbol at the top. A name appears in the bottom field of this portion of the window. You can and should edit the name to something meaningful, as shown below for a bright red color that we are adding.

Once you add the new color, go to the Properties portion of this window, click on the Color swatch and define your color, as shown in the next figure.

When you click on Close you will want to change other settings, such as brightness, transparency, etc. These choices are in the tabs at the bottom of the window, as we can see below.

When you are ready to assign the color, go to the Assignment portion of the window. Use the pull-down to select the scope. By default, Part is chosen. This means that we will assign the selected color to the whole part. You can also choose surfaces, components (in assembly mode), etc. The following figure shows the assignment of this color to one of the parts we have been working with in the past lessons.

PARENT/CHILD RELATIONSHIPS Because Pro/ENGINEER is a feature-based modeling tool, we are bound to have features that rely on other features to exist. Every time we pick a surface as a reference, or an edge, or a plane, etc. we are creating these dependencies.

These dependencies are classified as either parents or children. For example, suppose we create an extruded protrusion. Then we round an edge on that protrusion. The protrusion is the parent, and the round is the child. You can delete the round and the protrusion won’t care. But, if you try to delete the protrusion, the round will be directly affected. To view existing parent-child relationships for any given feature, select that feature, and then right-mouse click on it and go to Info, Parent/Child. You get a window that looks like the following.

At the top, it shows the feature that we are running the report on. In the bottom left, we get a list of all of the parents of this selected feature. On the right, we get a list of all of the children of this feature. Can you reduce parent child relationships in your model? Sure you can. The easiest way to reduce the number of relationships is to try to use the default datum planes as much as possible for sketching planes, sketching references, and dimensional references. But, the moment you use a Use Edge or Offset Edge or select a vertex or edge or surface as a reference in the sketch, you have created that parent/child relationship. It is unavoidable. My advice is to never delete or suppress a feature until you have run this query. Then, at least, you will be prepared to see things disappear.

MODEL PLAYER Whenever you get a model to work on that you didn’t create, you should immediately use the model player, found under Tools, Model Player in the menu bar. This will bring up the following window.

You will use the arrows at the top to step through the model from start to finish. As you pick on the “Next” arrow, the feature that is displayed will appear in the working window. You can pick on the Show Dims button at any time to see the dimensions used for that feature (if any).

COSMETIC SKETCHES A cosmetic sketch is used to convey information on the part without creating a solid or datum feature to do it. A great example is a logo or part marking. There are a few restrictions when using them. The first is that the cosmetic sketch can not cross over surface boundaries if projected. The other is that you can not hatch a projected cosmetic sketch. Cosmetic sketches are either sketched directly on a surface similar to a sketch feature, or they are projected onto a single surface, similar to a projected datum curve. The following figure shows a cosmetic sketch for our logo on a part.

Cosmetic sketches are accessed through Insert, Cosmetic, Sketch in the menu bar.

ANALYSES

There are a lot of different analysis tools in Pro/ENGINEER. We went through a draft check analysis back in Lesson 15, and we saw the results of a Gaussian Curvature analysis in Lesson 22. There are three additional analysis that are used widely. Mass Property Calculation Use Analysis, Model Analysis then select Model Mass Properties from the pulldown. This gives us the following window.

Most of the time, you can just hit the Compute button. The analysis results include (but are not limited to): Mass, Volume, Density, Center of Gravity, Total Surface Area, Moments of Inertia, etc. We need to run this analysis before our mass parameter will show the correct value in the drawing title block. Global Interference Check In an assembly, you can run this analysis to check for interference between parts. Go to Analysis, Model Analysis, then select Global Interference from the pulldown. It will look like the following.

Measure Use this to take measurements between surfaces, planes, points, vertices, axes, or other entities. This is found under Analysis, Measure. It brings up the following window.

FLOATING MODULES To access any floating modules, go to Tools, Floating Modules. Floating modules are applications that we have with the software, but they are not tied to any particular license. They float on the network, and can be accesses on a first-come-first-serve basis. Two are shown in the window that pops up.

LESSON SUMMARY This Lesson marks the end of this training guide. Be sure to keep this guide handy. If you have any Pro/ENGINEER questions, contact your CAD Administrator or PTC through one of the following methods. PTC Phone Support: 1-800-477-6435 PTC Online Support: www.ptc.com – select on the support link at the top.

EXERCISES None

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A Appendix Summary: In this Appendix, we will see the solutions to all of the exercises for this training guide. Lesson 1 Lesson 2 Lesson 3 Lesson 4 Lesson 5 Lesson 6 Lesson 7 Lesson 8 Lesson 9 Lesson 10 Lesson 11 Lesson 12 Lesson 13 Lesson 14 Lesson 15 101 Lesson 16 107 Lesson 17 113 Lesson 18 117 Lesson 19 121 Lesson 20 130 Lesson 21 132 Lesson 22 137 Lesson 23 140 Lesson 24 143 Lesson 25 143 Lesson 26 145

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LESSON 1 – Pro/ENGINEER Basic Elements There are no exercises for this lesson.

LESSON 2 – Taking a Look Around Set Working Directory The first part of this exercise is to set your working directory to C:\Data\ProETrain. There are three different (and equally preferred) ways to do this. Using the Navigator Using the navigator, locate the folder that we want to switch over to. If you are not in the file explorer portion of the navigator, click on the following icon at the top of the navigator.

Once you find the ProETrain folder, hold down the right mouse button over this folder to see the available options, as shown below.

As indicated above, select the Set Working Directory menu option. Using the System Toolbar

A second way to select your working directory was to click on the following icon in the system toolbar (the row of icons across the top).

This brings up a separate window, entitled Set Working Directory, and looks like the figure at the top of the next page.

Use the pull-down field in the upper left of this window to start your search, and then select the ProETrain folder in the main portion of this window. Click on OK to finish. Menu Bar The third way to set your working directory uses the menu bar at the top of the Pro/ENGINEER window. We would select File, followed by Set Working Directory, as shown below.

This brings up the same window shown previously. Select the folder, and then click on OK to finish setting the working directory. Spinning, Panning and Zooming the Model To spin the model, use the middle mouse button all by itself. Hold down this button and keep it held down during the duration of the spin, then release to stop the model in its new orientation. To zoom the model, hold down the Ctrl key on the keyboard and then press and hold the middle mouse button. Moving the mouse up and down will zoom the model in or out. Moving the mouse from right to left will tilt the model about an axis normal to the

screen. Once you initiate a zoom or tilt, you must let go of the mouse button and press it again to select the other option. To pan the model, hold down the Shift key on the keyboard and then press and hold the middle mouse button. Release the middle mouse button to stop the model in its current location. If you have a scroll button for a middle button, you can use this wheel to zoom in or out. If you press the scroll button down, it behaves as if you only had a plain middle mouse button for the regular spin, pan and zoom options. Default and FRONT Views The default view icon is located in the system toolbar, and looks like the following.

To access other saved views (such as FRONT, TOP, RIGHT, etc.) click on the following icon in the system toolbar.

Then, select one of the views listed below this icon. In this case, we select the FRONT view.

LESSON 3 – Selecting Objects Edge Selecting The easiest way to do this is to first start by changing your selection filter to Geometry. This is located in the lower right corner of the Pro/ENGINEER window, as shown below.

Next we will begin by selecting one of the edges on the outside of the flat surface, as shown in the figure below.

It will turn a bold red. Now, we will hold down the Shift key on the keyboard, and then move our mouse cursor to the rounded edge just above (and connected to) the line that we just selected. The entire outside surface edge should highlight in blue, as shown below.

While we can see the entire outside boundary loop of this surface highlighted in blue, we will click once with the left mouse button. The blue highlight should turn into a bold red outline, which indicates that it is selected, as shown below.

We still have two additional sets of edges to select, so we will begin by holding down the Ctrl key on the keyboard to select multiple objects, and then select the bottom flat edge of the next set, as shown below.

As we did before, release the Ctrl key and press the Shift key on the keyboard. Move your mouse cursor over one of the two vertical edges that touch our selected edge. The entire loop of edges around this hole/keyway should be highlighted in blue, as shown in the next figure.

With the entire set of edges highlighted, click once with the left mouse button to select these edges, as we can see in the following figure.

Release the Shift key, and then hold down the Ctrl key on the keyboard to make our third selection. This time, select one of the two halves of the upper hole, as shown below.

Once again, hold down the Shift key and place your mouse cursor over the other half of the circle to see the whole circle highlight in blue, as we can see below.

Finally, click once with the left mouse button to select this hole once it is highlighted in blue. It will be selected as shown in the following figure.

Seed-and-Boundary Surface Selecting The last part of this exercise could have been done using the Ctrl key and selecting all of the surfaces that are shown (the ones that are meshed). We wanted you, however, to try using the seed and boundary method for selecting. To do this, we first have to determine which surface is the seed and which surface(s) represent the boundary. Remember – the boundary surface can be made up of multiple surfaces, and is not included in the final selection. The seed surface can only be a single surface, and it is included in the final selection. Knowing this, we would pick the following surfaces for our seed and boundary selections.

To actually perform the selecting, do the following steps. First, make sure that you still have Geometry selected for the selection filter. Then, click on the seed surface first (the large half cylindrical surface at the bottom of our model). Next, hold down the Shift key on the keyboard and start selecting the surfaces of the boundary that you can easily get to. Once you have selected the first part of the boundary surface chain, let go of the Shift button. You will most likely see a set of selected surfaces that do not conform to what you want. Do not worry about this. Use the middle mouse button to rotate the model until you can see the next set of boundary surfaces to select, and then press the Shift key again. Do you notice something? The only selected surfaces that we see are the ones that we selected before we let go of the shift key the first time. It remembers what we already selected, so when we let go of the key to spin the model, then pressed it again, it was as if we never let go of the key in the first place. Finish selecting the rest of the boundary surfaces with this technique, and once they are all selected, release the Shift key again. You should see all of the surfaces that touch the boundary surfaces (but not the boundary surfaces themselves). Included in this will be our seed surface. The figure below shows this.

Close out of this model using Window, Close from the menu bar, and then erase session memory using File, Erase, Not Displayed. Click on OK to confirm the objects being erased.

LESSON 4 – Sketcher Basics Sketch 1 – Shear Plate For this sketch, start by going to File, New, and then select the Sketch type. Be sure to enter the name Shear_Plate in the appropriate field, as shown in the next figure.

Click on OK to get into the sketch. Once inside sketch mode, it is easier to start sketching if we turn off the display of dimensions. Therefore, we will click on the following icon in the system toolbar to de-select it.

Next, we are going to use the line tool ( ) and sketch the outline of our overall shape. Remember, the goal is to sketch quickly and somewhat accurately. We are going to watch our constraints to make sure we see the “H” at the bottom of the sketch, and we also are going to look for the perpendicular symbol in the upper left of the sketch. When we are done sketching the lines, click on the middle mouse button to get out of line creation mode. Our sketch looks like the following.

Next, we are going to sketch the two circles using the circle tool ( ). Start with the leftmost circle and try to line up the center of the circle with the vertex shown in the following figure. Then, create the second circle to the right of the first one. As you move your mouse to locate the center of the next circle, you should see the symbol to assume that they are lined up horizontally. As you sketch the circle, look for the equal radii symbol to appear. The resulting sketch will look like the figure below.

Now, we are going to go back to the line tool, and sketch a line starting at the center of the rightmost circle, and going parallel to the side edge, as we can see in the following figure.

Be sure to see the parallel symbol appear when the line is parallel to the appropriate side. Since we don’t really need this line to create geometry, we are going to turn it into a construction line (similar to a centerline, but with a fixed length). To do this, we are first going to select on the line so it turns red. Then, we will hold down the right mouse button over the line and select the Construction option, as shown in the next figure.

Once we do this, the line will become dashed, indicating that it is not a solid sketcher line anymore, but a construction line that is for reference only. The figure below shows this resulting construction line.

We are going to repeat this same process to create another construction line. This will be the line that runs down the center of our slot. Therefore, start by creating a solid line that originates at the top of our existing construction line, as shown below.

Be sure that no automatic constraint is applied (such as another parallel or perpendicular or equal length, etc.). Next, select this new line and right mouse click on it and select Construction, just as we did with the last line. It will become a construction line, as shown in the following figure.

Now, we will sketch our slot. To start the slot, we know that the top arc’s center lies on the intersection of the two construction lines, therefore, we will use a center-ends arc (

) and start by clicking on the vertex where the two construction lines meet.

When you drag out the diameter/radius for the arc, try to get your starting location to be on an invisible line that is perpendicular to the second construction line, through the center of the arc that we are sketching, as shown below.

Once you click with the left mouse button to start the arc, move your mouse cursor to the opposite side of the construction line, thus forming an approximate 180 degree arc, as shown in the following figure.

Now, we will return to our line tool, and sketch a line at the right endpoint of this new arc. We want to make sure the line is tangent (look for a “T” symbol) to the arc, and parallel and equal in length to the short construction line, as shown on the next page.

To sketch the bottom arc, we will use a tangent-end/3-point arc ( ). Start by clicking on the end of the solid line that we just sketched. When the green circle with the “X” appears, come out of the bottom quadrant, and move the end of the arc over so it creates an approximate 180 degree arc, as shown below (NOTE: the arc center should snap to the end of the construction line, and our equal length symbols disappear).

When we click with the left mouse button to finish the arc, the green circle will go away, and our resulting arc will look like the following.

To finish the slot, we are going to use a line tool again, and connect the two open arc ends. A tangent symbol “T” should appear at both ends if we sketched the arcs at approximately 180 degrees.

Now that we have sketched the entities for our section, we are going to address any constraints that we have. Remember, the sketcher steps start with sketching, followed by adding/removing constraints. We have a lot of “weak” constraints on the sketch already. To turn a weak constraint into a strong constraint, you first select the constraint so it highlights in red, the hold down the right mouse button and select Strong. We will do this for all of our weak constraints, shown in the following figure.

Once you make these constraints strong, they will turn into a bold yellowish cream (black in this guide) instead of the gray color they once were, as shown on the next page.

There is only one constraint that we are missing. To add a constraint, we will click on the following icon in the sketcher toolbar.

When the constraint window appears, select on the icon used to line up two vertices on an invisible vertical line, as shown below.

We will then select the center of the right leftmost circle, and the vertex below it on the outside boundary, as shown below.

Once we do this, two bold rectangles will appear that face each other, indicating that these entities are lined up vertically.

Our sketch is now fully constrained the way we want it. Now, we must address the dimensions. Therefore, turn back on the view of dimensions. Your model should have a lot of gray (weak) dimensions on it. The figure below shows the dimensions that are on my model but yours may be slightly different.

You should NEVER leave dimensions weak. Therefore we will either add new dimensions (which automatically come in strong), or convert weak dimensions over to strong dimensions that are already in the sketch that we want. For example, there are many angular dimensions on this sketch that are the ones that we want, so instead of re-creating these dimensions, we can simply select them with the left mouse button, then hold down the middle mouse button and select Strong. In this example, we have the following dimensions that already exist that we will make strong. (NOTE: Your sketch may or may not have these exact dimensions, but don’t worry, you can always create the correct ones). Also, the figure below omits the rest of the dimensions for clarity; on your screen you will see all of the dimensions that are available.

Once the dimensions are made strong, they will appear in a bold yellowish cream color (black in this guide), and they stand out from the weak gray dimensions, as shown below.

Now, we are going to create the rest of the dimensions that we need. When we create a dimension, it comes in strong automatically, and one or more weak dimensions will disappear to leave the sketch fully constrained. ). The first dimensions that we We will start by clicking on the dimension tool ( will add will be the lengths of the lines around the border of the sketch. To dimension the length of a line, simply click on the line once with the left mouse button, and then

place the dimension by clicking with the middle mouse button where you want the dimension, as illustrated for our first dimension below.

We will repeat this process to create all of the rest of the seven linear dimensions around the outside of the sketch, as shown below.

Notice that many of our weak dimensions are gone. Now, we will repeat this same sort of process to dimension the distance between the slot and the left hole, and the length of the slot itself. We will click once with the left mouse button on the construction line between the left hole and the top of the slot, and then use the middle mouse button to place the dimension. Do the same for the other construction line that goes between the two arcs in the slot. The resulting dimensions look like the following.

The next dimension will be the width of the slot itself. To create this dimension, click on the right outside straight edge of the slot with the left mouse button, then click on the left outside straight edge of the slot with the left mouse button, and then use the middle mouse button to place the dimension, as shown below. Again, the surrounding dimensions have been omitted from the following figure for clarity only.

Our next dimension is the distance between the two holes. To create this dimension, select on one of the circle centers with the left mouse button, followed by the other circle center (using the left mouse button again), and then click with the middle mouse button to locate the dimension.

There is only one more dimension on this sketch that needs to be created. It is an angular dimension on the right side of the sketch. To create an angular dimension, select on one of the angular lines with the left mouse button, followed by the other angular line (also using the left mouse button). Once both lines are selected, place the dimension using the middle mouse button. The following figure shows this angular dimension.

All of the weak dimensions should be gone. If not, you either do not have all of the dimensions placed on the sketch, all of them have not been made strong yet, or you do not have enough constraints, as defined earlier. The fully dimensioned sketch should look like the figure at the top of the next page.

Once we have all of the dimensions created and strong, it is time to modify them. Notice that most of our linear dimensions are on the order of a few inches (largest is about 4.3 inches). However, in our exercise, the smallest linear dimension is actually 19 (the width of the slot). If we were to simply try to modify each dimension one-by-one, our sketch would either fail regeneration, or it would terribly distort. The best approach in this case is to use the lock scale option to scale up the sketch to a better range of dimensions. To do this, we will first click on the following icon in the sketcher toolbar.

We will drag a box around the entire sketch. All of the dimensions, constraint symbols and sketched entities (lines, arcs, circles, etc.) will turn red.

Next, we will click on the modify icon ( at the top of the next page.

). This will bring up the window shown

To lock the scale, we will first click in the box to the left of the words “Lock Scale”. Next, we select on the dimension that we want to change that will drive all other dimensions to update. In this case, we will scroll through the available dimension fields until we see the one that represents the linear dimension on the horizontal line (the one marked “H”). When we select on this dimension from this window, a box will appear around the dimension on the sketch, as shown in the following figure.

We will then edit the value for this dimension to 94.0. Once we hit the enter key, all of the dimensions in this modify window will change to match the same scale as the dimension value that we entered, as we can see in the following figure.

Now, we can click on the green check mark, and the entire sketch will re-appear in the window. Notice that all of the dimensions are closer in value to the correct values in the exercise. This is shown at the top of the next page.

We can now modify each of the dimensions separately by double-clicking on them and entering a new value. Because the dimensions are closer to the correct value, the sketch shouldn’t warp as bad as it would had we tried to go from 1.5 to 81 (for example). Once all of the dimensions are modified, our sketch looks like the picture on the exercise page, as shown below.

Save the sketch, then use Window, Close to finish.

Sketch 2 – Latch Plate When we look at this sketch, we can see that it is symmetric about a horizontal centerline. Therefore, our goal is to take advantage of this symmetry by sketching only half of the shape, and then mirror it. Therefore, we will start by creating a new sketch, called Latch_Plate. The first entity will be a centerline. To create this, click on the following icon in the line tool flyout.

Click out in the middle of the sketch window, and snap the centerline so it is horizontal (you should see the “H” symbol), as shown below.

Now, we are going to use the line tool to sketch the following shape (and it probably works best and fastest in the order shown below).

In the figure above, “LMB” means “Left Mouse Button” and “MMB” means “Middle Mouse Button”. Be sure to avoid any equal length constraints or any “line up horizontal or vertical” constraints. You should only see horizontal “H” and vertical “V” constraints, and two collinear constraints where the lines connect to the centerline. Also, there is no line connecting the two points that lie on the centerline, it is left open for now. The next thing we will do is create a fillet at the upper left corner of the sketch. To do this, click on the following icon.

Then select the two lines that intersect in the upper left corner of the sketch, as shown in the figure at the top of the next page.

The resulting fillet will look like the following.

Repeat this process to create the other fillet near the right side of the sketch, as shown completed below.

The next thing we will sketch will be the circle that lies at the center of the first fillet that we created. Therefore, click on the circle tool, and then click with the left mouse button on the fillet arc center and drag out the radius. Click with the left mouse button to finish the circle, which will look like the figure at the top of the next page.

Next, create another circle. When selecting the location for the center of the circle, try to get the “Line up Horizontal” symbol to appear first, and then click on the sketch approximately below the vertex shown in the following figure. Drag out the radius until you see the “Equal Radii” symbol appear.

We have two arcs left to create. Therefore, click on the center-ends ( and create a 90-degree arc at the location shown in the following figure.

) arc tool,

Be sure to make the arc large enough so that no equal radii symbols appear on it. If you get an equal radii symbol, you can delete it later.

Now, we are going to use a tangent-end/3-point arc ( ) and click at the end of the arc that we just made, and drag out the end of the arc to other line end, as shown below.

The following figure shows our half section after we are done sketching all of the entities.

Normally, we would finish sketching the entire section before addressing the constraints, but in the case of mirroring, it is best to get your section and constraints in order before you mirror, but we will not deal with dimensions at this time. Therefore, we will first start by turning all of our weak constraints into strong ones. The figure at the top of the next page shows all of our constraints once we turn them to strong constraints. NOTE: If you do not have one or more of these constraints, you can always add them at this time.

We need to add one additional constraint before we mirror. We will use the icon, followed by and select the center of the right circle with the vertex at the top of the model that is lined up with this circle. The result is shown below.

To mirror the sketch, we will first use the select tool ( ) to drag a box around the entire sketch so that all the entities, and constraints become selected. Next, we will click on the mirror tool, which looks like the following icon.

Select on the horizontal centerline that we sketched, and our section should now be one complete sketch, as shown at the top of the next page.

You will see a bunch of arrows. These arrows represent a “symmetric” constraint, and are always set on vertices or arc centers when you mirror a sketch. We will need to add one additional constraint before we are ready to dimension. To do this, we are going to go back into the constraint tool, then select the collinear constraint ( following figure.

). We are going to select on the two arc centers shown in the

When we do this, they will snap on top of each other (align). The result will look like the following.

Our sketch should now look like the following.

Now, we are going to turn off the display of constraints by clicking on the following icon.

Then, turn on the display of dimensions (use the dimensions appear on the sketch, as shown below.

icon to do this). Our weak

NOTE: I have moved the weak dimensions around to see them more clearly.

As we did in the last exercise, we will look for any dimensions that we need that are already in the sketch, and turn them into strong dimensions. We do this by selecting all of them using the Ctrl key, and then hold down the right mouse button and select Strong. The following figure shows the resulting dimensions in this example that are already there and have been converted to strong.

Now it is just a matter of adding additional dimensions until we get the dimensioning scheme that we saw in the exercise. The resulting dimensioning scheme is shown below.

The last thing we must do is modify the dimensions to their correct values. Unlike the last exercise, we don’t have a huge jump, but we want to be careful in the order that we pick if we just want to modify one-by-one. The other option is to select all of the dimensions by dragging a box around the entire sketch, select the modify tool, uncheck the Regenerate option, and then modify all of the dimensions one-by-one in the modify window. When we are done, we click on the green check mark, and our sketch will regenerate and look like the final version that we need, as shown below.

Save this sketch, and click on Window, Close to finish out of the section.

LESSON 5 – Sketch Feature Start by going to File, New from the menu bar, and when the window opens, make sure that Part is selected, and enter Plate_Layout, for the name, as shown in the next figure.

The Sub-Type should be Solid. Click on OK and you will get the next window.

For this model, our units are in inches, so select the startpart_english file, or whatever equivalent English start part you may have. Click on OK to continue. You will see your default datum planes (assuming they are turned on).

From the datum fly-out icon, select on the Sketch tool, or use Insert, Model Datum, Sketch, from the menu bar. We will get the following window.

We will pick on the TOP datum plane to use as our sketching plane. When we do this, it automatically assumes we want to use the RIGHT datum plane as a reference, and faces it towards the Right, as shown in the next figure.

There is a yellow arrow pointing down from the TOP datum plane, indicating the viewing direction. We will accept this, and click on the Sketch button. This places us into our 2D sketch mode. Turn off datum planes, and you will see the following.

We can see two orange dashed lines. These lines are NOT centerlines. They represent sketcher references. Our sketcher references window should be open, and we can see that the FRONT and RIGHT datum planes (which are perpendicular to the TOP datum plane – our sketching plane) have been selected automatically as sketcher references.

We will not need to select any additional references at this time, so we will click on the Close button. We will now use a rectangle tool and sketch a rectangle where the lower left corner lays at the intersection of the two sketcher reference lines. When the rectangle is done, we will go ahead and modify the dimensions to 10.000 and 5.000. NOTE: The reasons we are going ahead and modifying the dimensions at this time are two-fold: • The sketch is simple enough that modifying the dimensions now will not cause the sketch to fail. The dimensions originally come in very large compared to our final values. • Modifying the two dimensions now will cause the sketch to scale down so our remaining entities will be closer to their final values. The sketch should look like the following at this time.

We will now switch to the circle tool. Sketch a circle in the upper left corner of the rectangle. Change the dimension values to their correct values as shown in the next figure.

Next, we will sketch a second circle in the upper right corner of the rectangle. When placing the circle, snap to a horizontal alignment, and also snap to equal radii. Modify the single dimension to its correct value, as shown in the next figure.

Now, we will sketch the circle in the lower left corner. Be sure to align vertically with the first circle, and snap to equal radii. Modify the single dimension that appears, as shown in the following figure.

The last circle should be easy. It will snap at the horizontal alignment to the third circle, and vertically to the second circle. The equal radii value will also snap. No dimensions will be necessary for this circle. The final sketch looks like the following.

Click on the blue check mark to complete the sketch, turn on your datum planes, and go to a default orientation. Your model will look like the following.

Save and close this model.

LESSON 6 – Extrude Feature Plate_Layout Open up the Plate_Layout2 model. It consists of two sketched features, as we can see in the model tree.

The model looks like the following.

We will start by selecting on the Sketch_Plate sketch from the model tree so it highlights in red on the model. Now, pick on the Extrude feature. When we do this, the dynamic preview automatically appears, because we have decided to use an external sketch.

We will change the depth to 2.0 inches, and then click on the green check mark to complete this first extrude feature. Our model looks like the following (no hidden mode).

In our model tree, we can see that the first sketch is now hidden, because it has been used in an extrude feature.

If we need to see this or use this sketch again, we can always unhide it. For now, we will pick on the second sketch (SKETCH_CIRCLES), and then click on the extrude icon again. This time, when our dashboard opens, be sure to select on the Remove Material icon. Change the depth value to 1.0, and be sure it is going up into the part, as shown in the next figure.

Click on the green check mark to complete this extruded cut, and then rotate the model to see the result.

Save and close this part.

Safety_Key Create a brand new part called Safety_Key. Use an English start part (if available). While there may be multiple ways to create this part, we will demonstrate one method that utilizes simple sketches, and a low number of features. We will also use internal sketches. To do this, first select the extrude tool, and then right click on the working window and select Define Internal Sketch. The following images show the progression of this model. Extrude 1 – TOP plane as Sketching Plane, RIGHT plane facing towards the Right.

SKETCH

DYNAMIC PREVIEW

FINISHED EXTRUDE

Extrude 2 – Select Use Previous for sketching plane and sketching reference.

SKETCH

DYNAMIC PREVIEW

FINISHED

EXTRUDE Extrude 3 (Cut) – FRONT plane for sketching plane, RIGHT plane facing towards the Right.

SKETCH

OPTIONS SLIDE-UP PANEL

DYNAMIC PREVIEW

FINISHED EXTRUDE

Extrude 4 (Cut) – RIGHT plane as sketching plane (default viewing direction), TOP plane facing towards the Top.

SKETCH

DYNAMIC PREVIEW

FINISHED EXTRUDE

NOTE: For the dynamic preview, you will need to change the depth option to Through All, and flip the direction to go back into the part, as shown in the figure above. Save and close this model. IMPORTANT: For the first cut feature, we chose to combine the circular hole and the rectangular cut-out in a single extrude feature. For greater flexibility, you may wish to separate them, but for this example, both are very simple shapes, and easy to modify in the same sketch. If you were required to delete one of these entities, you would have to edit the sketch and remove the profile.

Rod_Support Create a brand new part called Rod_Support. Use a metric start part (if available). As with the last part, we will demonstrate the preferred method for creating this part using simple sketches and flexible features. Extrude 1 – RIGHT plane for Sketching Plane, and TOP plane facing towards the Top.

SKETCH

DYNAMIC PREVIEW

FINISHED EXTRUDE

Extrude 2 (Cut) – FRONT plane for Sketching Plane, RIGHT plane facing towards the Right.

SKETCH

OPTIONS SLIDE-UP PANEL

DYNAMIC PREVIEW

FINISHED EXTRUDE

Extrude 3 (Cut) – TOP plane for Sketching Plane, RIGHT plane facing towards the Right.

SKETCH

DYNAMIC PREVIEW

FINISHED EXTRUDE

NOTE: A Through All depth is used for this cut, and the direction must be flipped to go through the part.

Extrude 4 (Cut) – RIGHT plane for Sketching Plane, TOP plane facing towards the Top.

SKETCH

DYNAMIC PREVIEW

FINISHED EXTRUDE

Again, the dynamic preview indicates a Through All cut that goes back into the part, resulting in the finished part shown above on the right. We could have created this hole in our first extrude feature as well. The same rules apply, if we needed to separate out the features later, we would have to redo the sketches for the features. Save and close this model.

LESSON 7 – Making Changes

Open up the Plate_Layout2 model that we created in Lesson 6. Right now, we have a 10” x 5” x 2” plate that has four 1” holes going 1” into the part. To turn these holes into feet sticking out of the model, we must change a protrusion into a cut, and we must change both the direction and depth of the feature. To do all of this, we will need to use the Edit Definition command. Therefore, we will select on the Extrude 2 feature from the model tree with the right mouse button, and select Edit Definition, as shown in the next figure.

This brings us back into the dashboard for the feature, and it looks like the dynamic preview we saw before:

The first thing we will do is to de-select the Remove Material icon, turning the extrude from a Cut into a Protrusion. The preview now shows solid shading for these holes, as shown in the next figure.

Next, we will click on the yellow arrow to flip the direction of the feature, and change the value to 0.5. The preview now looks like the following.

Click on the green check mark to complete the changes to this feature, and now our model looks like the following:

Save and close this model.

LESSON 8 – Datums Part 1 Create a new part called Angle_Bearing. The trick to this exercise model is to understand that our raised cylindrical protrusion, and the hole that goes down it are perfect circular shapes when viewed at the section A angle.

Therefore, we need to have a sketching plane that is parallel to this section plane. So, the trick is getting that sketching plane. Once you have that, everything else is relatively simple.

Extrude 1 – “T” shaped base We will start by creating an extrude feature. Use an internal sketch, and use the FRONT datum plane as the sketching plane. Face the RIGHT datum plane towards the Right, and sketch the following profile.

Click on the blue check mark to complete the sketch, and use a symmetric depth of 103.0, as shown in the dynamic preview.

Click on the green check mark to complete this first extrude feature. The model currently looks like the following.

Now, we will start to create our datum features. Datum 1 – Datum Axis To get started, we need to create a datum axis. Why? In order to have a datum plane that is at an angle (as our section “A” plane is), we need an edge or axis to revolve through. We can’t simply use an edge on the model, because we need to control where the axis of the cylinder connects with the right edge of the model (as indicated by the 33.0” dimension). Therefore, we will click on the datum axis tool (or use Insert, Model Datum, Axis from the menu bar). This brings up the following window.

We will create an axis that is normal to a surface, located from two additional surfaces. Therefore, select on the following surface location.

When we do this, the surface highlights in a mesh (in no hidden mode – or a rosecolor shade in shaded mode). We can also see two drag handles to locate the axis, as shown in the next figure.

We will drag one of the handles over to the front “T-shaped” face, and the other to the side rectangular surface, giving us two linear dimensions, as shown in the next figure.

Your dimensions will be different unless you picked the exact location I picked in this example. We will modify the distance to the front face to 33.0, and the distance to the side as 0.0, as we can see in the following figure.

This places the axis exactly where we need it for our first datum plane. At this time, our axis window looks like the following.

We will click on OK to finish this axis, and turn on the display of datum axes to see the result.

We can see our new axis, as well as the three default axes in the start part. We will turn off the display of axes, because we will be able to pick from the model tree, which looks like the following.

Datum 2 – Datum Plane Now, we will create our first datum plane. Therefore, click on the datum plane tool, or select Insert, Model Datum, Plane from the menu bar. This brings up the following window.

We will start by picking on the A_1 axis from the model tree. The dynamic preview shows a plane going through this axis, and it is at an angle, as shown in the next figure.

Now, hold down the Ctrl key, and select the side surface that the axis goes through. When we do this, an angle appears on the dynamic preview and the datum plane rotates, as shown below.

Change the angle to 60.0 as shown in the previous figure, and then our window will look like the following.

You may notice that the yellow arrow is facing to the back side of the datum plane (as viewed from a default orientation). We want this to be this way, so if you accidentally flip the arrow to the front, flip it back to the back by clicking on it. Click on OK to finish this datum plane, and then turn on the display of datums to see the result.

We should be able to see the black side of the DTM1 datum plane in a default orientation, as shown in the previous figure.

Datum 3 – Datum Plane Our last datum plane will be our eventual sketching plane. To create this, go back to the datum tool, and for our references, we will select the A_1 axis, followed by DTM1 (using the Ctrl key). When we do this, we will see the following.

Currently, our datum plane window looks like the following.

We could change the angle to 90 degrees, but instead, we will go to the datum plane window, and change the second reference type from Offset to Normal, as shown in the next figure.

Next, click on the Display tab in the window. It currently looks like the following figure.

We will flip the direction for the positive side of the datum plane. We could have picked on the yellow arrow on the model itself, or click on the Flip button from this tab. Once we do this, we see the following.

Click on OK to complete this datum plane, which now looks like the following.

We can see the positive brown side of DTM2 facing towards the front right, as shown in the previous figure. We are now ready to continue with solid features.

Extrude 2 – Cylindrical Protrusion Create another extrude feature. Use an internal sketch, and select the DTM2 datum plane as the sketching plane. Use DTM1 as the reference, facing towards the Right. Inside the sketch, create the following.

NOTE: We can’t create the hole at the same time, because we can’t remove material and add at the same time. Also, you will have to select sketcher references for this model, because the system doesn’t automatically select them. Click on the blue check mark to complete this sketch, and your dynamic preview will look like the following.

Here is the other tricky part about this problem. Since our sketching plane rests at the edge of our model, we actually need to have geometry created in two directions. The following figure shows the area that needs to be created (shaded in red).

As we can see from the previous figure, we have to stop the protrusion at the two side surfaces, therefore, we will change our depth option to “To Selected” (the one with the red in it), and select the surface shown in the next figure.

When we do this, we see the following dynamic preview.

We are not done yet. Using the Options slide-up panel, set the depth in the second direction to “To Selected” as well.

For the second direction reference, pick on the opposite surface, shown in the next figure.

Our dynamic preview now looks like the following.

Click on the green check mark to complete this extrude feature, which now looks like the following.

Extrude 3 (Cut) – Axial Hole through top Cylindrical Protrusion To create the hole that goes through the cylindrical protrusion that we just created, we will use the same sketching plane, reference plane, orientation, and sketcher references, but this time our sketch will look like the following.

When you complete the sketch, be sure that you have selected the Remove Material option, and change the depth option to Through All for both directions, as shown in the next figure.

Our dynamic preview should look like the following.

Click on the green check mark to finish this extruded cut, which now looks like the following.

Extrude 4 – Final cuts For our last feature in this model, we will create another extruded cut, and use the TOP datum plane for the sketching plane. Be sure the arrow for viewing is going into the part, and then use the RIGHT datum plane to face towards the Right.

Inside sketch mode, sketch the following.

When finished sketching, change the depth option to Through All, and our dynamic preview will look like the following.

Click on the green check mark to complete this extrude feature. Our final model looks like the following.

Save and close this model.

LESSON 9 – Revolve Feature Create a new part called Bearing2.

Revolve 1 – Body of the Bearing For our first feature, we will click on the revolve icon. Use an internal sketch, and select the RIGHT datum plane for our sketching plane, and then use the TOP datum plane to face towards the Top. Inside the sketch, start off with a horizontal centerline on the existing horizontal sketcher reference, and then sketch the following profile. NOTE: Many of the dimensions are diameters, even though we only sketched half a model. The way you create this type of dimension is to select on the line/vertex followed by the centerline, and then select the same line/vertex again. When you place the dimension with the middle mouse button, a diameter dimension (or symmetric dimension) appears on the sketch.

Click on the blue check mark to complete the sketch. Our dynamic preview looks like the following.

Click on the green check mark to complete this revolve feature, and then you will have the following.

Extrude 1 – Holes The last feature for this bearing is the set of holes in the center of the bearing. We will click on the extrude tool, followed by the Remove Material option. For the sketching plane, use the FRONT datum plane, and face the RIGHT datum plane towards the Right. Sketch the following.

NOTE: To make the construction circle, sketch a regular circle, select it, and then right click and select Construction. When finished, our dynamic preview (with a depth option of Through All) looks like the following.

The final model will look like the following once you finish this extruded cut.

Save and close this model.

LESSON 10 – Datums Part 2 Create a new part called Basket. In this exercise, we are asked to create two sketched curves. We can do this with the sketch feature that we learned about in Lesson 5. These curves are going to be used later as trajectories to create the main body of the basket part. Sketch 1 Click on the sketch feature, or go to Insert, Model Datum, Sketch. For the sketching plane, select the TOP datum plane, and face the RIGHT datum plane towards the Right. For the first sketch, it will be easier to start with the internal curve. Therefore, we will sketch the following profile, which consists of two centerlines, two lines and an arc.

The finished sketch feature will look like the following.

NOTE: Be sure to use symmetrical dimensions as indicated in the figure. Therefore, you will need two centerlines in this sketch. Sketch 2 The next sketch will complete the outside curve. For sketcher references, be sure to pick all three entities from the first sketch that we made, and then sketch in the order starting with Line 1 in the following figure.

This completed sketch (and part) will look like the following.

Save and close this part for a later lesson.

LESSON 11 – Sweep Feature Dash_Pot_Lifter This is (admittedly) the most difficult exercise, but the actual definition of the model is not difficult once you see the solution. It just seems overwhelming, because you may not know where to get started.

If we take a look at the exercise figure, and pay close attention to the dimensions, we can see that there is a progression that must exist. For example, in the FRONT view, we see a hole-to-hole dimension of 140 mm. In order to be able to do this, we have to have the hole on the left, but to have the hole on the left, we have to have the farthest hole on the left side of the part. Therefore, we will need to work from left to right on the part. To do this part, we are going to use a combination of Datum, Extrude, Revolve and Swept features. Start by creating a new part called Dash_Pot_Lifter, and use a metric start part (if available). Feature 1 – Extrude The first feature we will create is an extrude. Use the FRONT datum plane as the sketching plane, and face the RIGHT plane towards the Right. We will sketch the following profile.

Extrude this feature to a depth of 38 mm. The first feature will look like the following in a default orientation.

Feature 2 – Extrude (Cut) The next feature will be an extrude that cuts out material from this first feature. For the sketching plane, use the TOP datum plane, and face the RIGHT datum plane towards the Right. Sketch the following rectangle.

For the depth option, go Through All in both directions (using the Options slide-up panel). The finished extrude will look like the following.

Feature 3 – Extrude The next feature will be an extruded protrusion. The sketching plane will be the top flat surface of the first extrude. Be sure the viewing direction is going into the part. Face the RIGHT datum plane towards the Right. Inside the sketch, use the right surface as a sketcher reference, and sketch the following.

When you finish the sketch, be sure the feature is going in the right direction, and flip it if it is not. Use the To Selected depth, and pick the opposite surface of the first extrude feature, and the completed feature looks like the following.

Feature 4 – Datum Plane If we look at the first cylindrical protrusion in the part, we can see that the back side of the cylinder sits 10mm away from the main body of the part, but the overall length of the cylinder (27mm) is based on this same reference point. Therefore, we should create a datum plane 10mm offset from the back side of the part. Therefore, click on the create datum plane icon (or use Insert, Model Datum, Plane), and pick on the following reference.

When the preview for the plane appears, change the offset distance to 10, and flip the positive side of the datum plane so it faces into the part, as shown in the next figure.

The reason we flipped the positive side, is so we can see the brown side when we are in a default orientation, as shown in the next figure for the completed datum plane.

Feature 5 – Extrude The next feature will be the cylindrical protrusion that extrudes from the DTM1 plane up 27mm into the part. Therefore, use DTM1 as the sketching plane, and make sure the viewing direction is facing away from the part. Use the flat, topmost surface of the part as the reference surface, and face it towards the Top. Add the TOP datum plane as a sketcher reference in addition to the RIGHT plane and the top flat surface of the part (which should already be selected as references). Sketch a circle centered on the TOP datum plane reference, tangent to the top surface sketcher reference, as shown in the following figure.

Extrude this circle into the part a distance of 27mm to create the following.

Feature 6 – Extrude (Cut) Even though we could do this next feature any time in the model, we will do it now, since we are working left to right. Therefore, we will create another extrude, and use the front flat surface of the cylindrical protrusion we just created, and face the TOP datum plane towards the Top. For a sketcher reference, add at least one of the circular edges of the cylinder that we just created, and sketch a circle, as shown in the next figure.

Extrude Through All to get the following.

Now might be a good time to save this part if you haven’t already. Feature 7 – Revolve (Cut) This next feature is one that can be done several different ways. If you look at the cross-section “A” through the bend in the part, we can see an “I” profile. We can always add this “I” in later as an extruded cut on each side, but because we have a width of 8mm for the middle of the “I” we might want to do it a different way to preserve the dimensioning intent of this exercise. Therefore, we will create the half-circle portion of the cut out by using a revolved cut. Click on the revolve tool, and the remove material icon. For the sketching plane, use the small rectangular surface at the right of our model. Face the TOP datum plane towards the Top. When we get into sketch mode, select the right edge of the rectangle as a sketching reference (the left side should be covered by the FRONT datum plane already), and be sure to sketch a horizontal centerline on the TOP sketcher reference. Then, sketch two rectangles on the top half of the centerline, and dimension according to the following figure.

For the depth option, accept the default of 360 degrees. NOTE: You could use 180 and make sure it is inside the part. The reason for using 360 at this time, is because there is no geometry outside of the model to the right that we are worried about

cutting, and we want to make sure we completely cut through the right side of the part. Depending on part accuracy, we could end up with a very small surface with 180. The final revolve feature looks like the following.

If you rotate the model, you will see the semi-circle on both sides of the part, forming the “I” profile at the end. We could have done this with extruded cuts, but would have had to make two separate cuts to do what we did in one revolve cut. Feature 8 – Sweep We are finally ready to perform our sweep operation (the whole point of this exercise). The good news is that we have already prepared our sweep profile (the “I” beam shape), all we need to do is define the appropriate trajectory. Therefore, go to Insert, Sweep, Protrusion, and the following window comes up.

We can see we are currently defining the trajectory. We can also see the following menu manager.

We will pick on the Sketch Traj option to sketch a trajectory. When we do this, pick on the FRONT datum plane for the sketching plane. An arrow appears, indicating the direction of viewing the sketch, as shown in the next figure.

Make sure it is going in the direction shown above, and then click on Okay. In the next menu, pick on the Right option, and then pick on the “I” shaped surface. We are placed into the sketch. For a sketching reference, pick on the top, flat surface of the part as a sketcher reference, and then sketch the following profile.

NOTE: Be sure the start point is at the top of the arc where it intersects the solid geometry. The start part can not be out in the middle of the trajectory. The “Line up Vertically Constraint” is applied between the arc 2 center and arc 2 endpoint. Once your trajectory is done, click on the blue check mark to finish the sketch. You will now have the following menu options.

We can go ahead and use Free Ends, because our trajectory is normal to the surface where the solid geometry exists. If the trajectory were not normal, we might want to use Merge Ends to have the gap filled between the end of the sweep and the existing geometry. Click on Done to continue. We are now placed into the sketch. Because we already have the profile of the sweep defined (the “I” shape), we can use the Use Edge, Loop option and select the I-shaped surface. Each edge will show the “use edge” constraint symbol, as shown in the next figure.

Click on the blue check mark to complete this, followed by OK in the sweep window. We will see our finished sweep feature, as shown in the next figure.

Save this model at this time before continuing. Feature 9 – Datum Plane In preparation for the next feature, we will create another offset datum plane. This one will use the same reference as the last one we created (DTM1), but will be 12mm instead of 10, like we did in the last one. The preview for this datum plane while creating it will look like the following (again, flip the positive side to be visible from the front of the model).

Feature 10 – Extrude The next extrude feature will actually be disconnected from the model temporarily. If you look at the figure, we can’t see a dimension going from the end of the sweep to the next section. We do see the 140mm distance between the first cylindrical protrusion to the hole on the right side, so we will create the protrusion that generates this hole as the next feature. For the sketching plane, use the DTM2 plane that we just created, and make sure the viewing direction arrow is facing towards the back of the part. Face the RIGHT datum plane towards the Right. Inside the sketch, we want to use the vertices at the top and bottom end of our swept feature as a reference (as indicated in the next figure). Then, sketch the following profile.

The next figure shows a close-up of the section and what is going on.

Finish the sketch by clicking on the blue check mark, and then extrude this feature to the front of the part a distance of 38mm. The result is shown in the next figure.

We can see that our protrusion is entirely outside of the rest of the model, but we will be closing that gap in two more features. Save the model. Feature 11 – Extrude (Cut) The next extrude feature we are going to create will cut out the opening on the right side of the feature we just created. Therefore, use the bottom, flat surface of the last extrude feature as the sketching plane. Flip the viewing direction arrow so it is facing down, away from the existing extrude feature, and face the flat front surface of the same extrude towards the Bottom. Inside the sketch, be sure to select the silhouette edge of the extrude feature as a sketching reference, as well as the axis that goes through the hole in this feature (you may need to temporarily turn on the axes to select it). Then, sketch the following rectangle and dimension it accordingly.

NOTE: The 16 mm dimension is missing from the exercise figure. If you notice, this feature is dimensioned exactly the same as the second feature we created for this model. Therefore, go ahead and add this 16 mm dimension. When finished with the sketch, extrude the cut up into the part using the Through All depth option. The finished extrude will look like the following.

Save this model before continuing. Feature 12 – Extrude The last extrude for this model will close the gap that exists. We will use the “I” shaped surface as the sketching plane, and face the viewing direction in towards the sweep feature. Face the FRONT datum plane towards the Left. Inside the sketch, use a Use Edge command, and select the top and bottom edge of the “I” beam profile, but do not select any of the sides. IMPORTANT: Because there are no assumed sketcher references, when you pick on the “Use Edge” command, you will get a warning that no references have been defined, and do you want to continue to sketch. Click on Yes, then proceed to select the top and bottom edge of the “I” shaped surface. Fill in the sides with two lines to complete the rectangle shown in the next figure (which shows the sketch in a rotated orientation from the 2D sketch view).

Finish the sketch by clicking on the blue check mark, and then use the To Selected depth option to go up to the larger flat surface of the disconnected extrude feature. The finished extrude feature looks like the following.

Notice that we don’t have the semi-circular cut out on this side yet. That will be our last feature for this exercise. Save the model first. Feature 13 – Revolve (Cut) We will create a very similar revolved cut to finish this model. For the sketching plane, we are going to pick on the very thin, flat surface shown in the next figure.

For the reference surface, select the front surface of the sweep, as indicated in the figure above, and face it towards the Right. Be sure your viewing direction is aiming out to the left, away from the end of the sweep. Inside the sketch, we want to use the Use Edge command and select the four vertical edges on the sketching plane, as well as the two short edges at the top of these lines, as shown in the next figure.

Next, sketch a horizontal centerline snapped to the midpoint of one of the vertical lines that we just created, as shown in the next figure.

Finally, trim up the vertical lines so only the top half remain, and close off the rectangles with two more short lines. The final sketch looks like the following.

Revolve this cut 360 degrees (which will not interfere with any other geometry in the model), and the final model will look like the following figure.

Save and close this model.

Basket The last exercise in this Lesson, is to create a swept surface for our basket. Open up the Basket part that we created in Lesson 10, which currently looks like the following.

Go to Insert, Sweep, Surface from the menu bar. The Sweep window opens, and we see the familiar menu manager.

This time, we are going to select the Select Traj option (because we have our trajectory already defined by a curve or existing geometry). When we do this, we get the following menu.

Since we have sketched curves in our model, we will use the Curve Chain option (indicated above). Place your mouse over one of the segments of the first sketch in the model (the one with two lines and an arc), and right click until you see the entire curve highlight in blue. Select the curve once it is completely highlighted, and you will get the following menu.

Since we want to use the entire curve as our trajectory, we will select on the Select All option. Had we only wanted to go from one vertex to another on the trajectory, we could have used the From-To option. When we click on Select All, an arrow appears on one of the endpoints, as shown in the next figure.

If your start point is not the same as the one shown above, then you will need to click on Start Point, in the menu manager, followed by Next, until you see this vertex highlight, at which point you would select Accept. Click on Done once your start point is in the correct location, and you will get the following menu manager.

If you are sketching a closed profile (like a rectangle or a circle), you can have the final surface closed off at the ends. We are only going to be sketching a single line, therefore, we will leave the default of Open Ends selected, and click on Done to continue. We are placed into sketch mode, where we will sketch an angled line dimensioned as shown in the following figure.

When you are done with the sketch, click on OK in the sweep window, and you will have your swept surface as shown in the next figure (in the default orientation).

Save and close this model.

LESSON 12 – Blend Feature Hand_Rail_Column Create a new part called Hand_Rail_Column, and use a metric start part if available. For this model, we will use a combination of datum, extrude, revolve and blend features. Feature 1 – Extrude The first feature we will create is an extruded protrusion. The TOP datum plane will be our sketching plane, and we will face the RIGHT datum plane towards the Right. Sketch a single circle as shown in the next figure.

Extrude this circle a depth of 12mm upwards to complete the first extrude feature, as shown in the next figure.

Feature 2 – Extrude Our next feature is going to be the extruded section at the top of this part. We are going to skip over the blended section for now, and the reason will become apparent as we create the blend feature next. Therefore, we will create an extrude feature, and use the FRONT datum plane for the sketching plane and face the RIGHT plane towards the Right. We will sketch the following profile.

Use a symmetric depth option, and a depth value of 42mm. The finished extrude feature looks like the following figure.

Feature 3 – Blend The next feature will be our blend that goes between the first and second extrude features. The reason we created the top extrusion before the blend is because of the depth of the blend feature.

Based on the fact that our blend sections are going to be parallel to each other, we will end up using a parallel blend. If you recall from the lesson, if you were to define the depth of the blend sections using a numerical value, that value goes from one section to the next. Unfortunately, if you look at the design intent of this model, the bottom section of the blend is on the top of the cylindrical protrusion. The depth of the second section (88mm), however, is based off the bottom of the cylinder. Therefore, to preserve design intent, we can’t simply create the blend and use a depth of 76mm (88-12). We can, however, use references to define the depth instead of an actual value, and that is where the second extrude comes in. By defining the extruded feature’s base at 88mm above the TOP datum plane, we can use that base as the stopping point for our blend. Therefore, go to Insert, Blend, Protrusion, and you will get the following menu.

We will keep all of these default options to create a parallel blend where we use regular sections that we sketch. Click on Done, and this brings up the blend window, as shown in the next figure.

We are currently defining the attributes, and our choices are shown in the following menu.

Since we only will have two sections, either one of these choices will do the same thing. Therefore, we will keep the default of Straight, and click on Done to continue.

We are asked to pick on a sketching plane, so we will pick on the top circular surface of the first extruded cylinder. When we do this, an arrow appears indicating the direction of feature creation, as shown in the next figure.

If the arrow is going in this direction, click on Okay. If not, flip it and then hit Okay. Next, select Bottom, and pick the FRONT datum plane. When we are placed into sketch mode, we will start by sketching two centerlines on the existing sketching references, followed by a square with a side of 42mm, as shown in the next figure.

Once you have the first square sketched, right click out in the working window, and select Toggle Section, as shown in the next figure.

This should mute your first square, and now you will sketch a second square with a side length of 32mm, as shown in the next figure. NOTE: You do not need a second set of centerlines, the first ones should still work for your symmetry constraints.

Once you have this second circle sketched, click on the blue check mark to complete the sketch. You will get the following menu to select the depth options.

We will select the Thru Until option, followed by Done, and then select the square surface at the bottom of the second extrude feature. Once you select this, click on OK to complete the feature, which is shown in the next figure.

Feature 4 – Extrude (Cut) The next feature will create the hole in the side of the second extrude feature. Therefore, for our sketching plane, use the RIGHT datum plane. Make sure your viewing direction is going back into the model. Face the TOP datum plane towards the Top. Inside the sketch, select the bottom surface of the second extruded feature to use as a sketching reference, and sketch the following circle.

Extrude this cut back into the part using the Through All option, and your feature looks like the following.

Feature 5 – Revolve (Cut) The last feature we will create will be a revolved cut. We will use the FRONT datum plane as the sketching plane, and face the RIGHT plane towards the Right. Sketch a vertical centerline on the RIGHT sketcher reference, and then sketch the following.

NOTE: This sketch consists of six lines forming an “L” shape. Use symmetrical dimensions to represent the diameters of the holes. The final model, shown in hidden line mode, looks like the following figure.

Save and close this model for the next lesson.

LESSON 13 – Rounds Hand_Rail_Column Open up the Hand_Rail_Column that we created in the last lesson. We are going to add rounds to this model. The goal when creating overall part rounds is to try to create them in the following order: 1. Individual edges/chains that create tangencies on other edges that must be rounded. 2. Edges that share the same radius value that do not intersect. 3. Edges that have different round values that do not intersect can be done in the same round as #2 as another set. 4. All other rounds. Therefore, keeping this in mind, we may want to create our first round feature using the following:

NOTE: I would recommend viewing this figure in color – either printed that way or electronically. Round 1 – Set 1 Create a new round feature. Change the radius value to 3, and select all of the edges shown in the colored schematic above using the Ctrl key so they are all part of a single round set. The preview for this first set will look like the following.

Round 1 – Set 2 Now, without holding down the Ctrl key, select the edge indicated by the color schematic for Round 1 – set 2. Change the diameter once selected to 1.0. The preview for this looks like the following. NOTE: You are still in the same round feature, so do not complete the round yet. The first round set should be muted.

Round 1 – Set 3 Once more, without using the Ctrl key, click on one of the slanted edges on the blend feature. When the radius appears, right click on one of the drag handles, and select Add Raidus to turn this round into a variable round. When the two dimensions appear for this selected line, change the one near the base to 12.0, and the one near the top to 6.0. Now, hold down the Ctrl key, and select the other three slanted lines and add them to the same round set. The preview for this set will now look like the following.

Click on the green check mark to complete this first round feature, and you will see the following.

Round 2 – Set 1 Start a new round feature. Change the radius to 1.0 and select on one of the edges indicated in the color schematic as the Round 2 – Set 1. Because we rounded all of the edges in the first round, a tangent chain should exist that propagates this new round all the way around the head. Continue using the Ctrl key to select the other edge, as shown in the following preview.

Round 2 – Set 2 Release the Ctrl key, and select one of the edges at the intersection of the blend feature and the extrude feature at the top. Again, a tangency condition should propagate this round along the entire intersection. Change the radius to 3.0, and the preview will look like the following.

Round 2 – Set 3 Again, without holding down the Ctrl key, select one of the edges at the bottom of the blend feature where it meets the cylindrical extrusion. Change the radius to 6.0, and the preview should look like the following.

The preview for this entire round feature should look like the following at this time.

Click on the green check mark to complete our second round feature, and the model will look like the following.

Round 3 – Set 1 For our last round feature, there will only be one round set. Create a new round, and change the radius to 3.0. Select the circular edge at the top of the first extruded cylinder. The preview for this round will look like the following.

Click on the green check mark to complete this round, and our model is now finished. The following figure shows the completed model with the three round features.

Save and close this model. Dash_Pot_Lifter Using the same method as in the last model, we will create the rounds for the dash pot lifter using the following round features and round sets. NOTE: Again, this schematic is better viewed in color for clarity.

Round 1 – Set 1 Create a new round and set the radius value to 2.0. Select all of the edges using the Ctrl key indicated in the color schematic. The preview for this round set will look like the following.

There are no other sets for this round feature. The finished feature looks like the following.

Round 2 – Set 1 The next round will take advantage of tangency conditions that now exist. Therefore, create a new round feature, change the radius to 1.0, and then select on the appropriate edges indicated in the color schematic. The preview for this round set will look like the following.

Again, there are no other round sets for this round feature. The completed round will look like the following.

Round 3 – Set 1 The last round has to be done separately, and after the second round feature. These are the rounds that go around the cylindrical protrusion. Even though they share the same radius value as round 2, the way that the cylinder intersects the existing geometry, creates a weird transition that even the Transition tool in the round feature can’t address.

Therefore, we will create our third round feature, and select the remaining edges to round. The preview for this round set looks like the following figure.

NOTE: You have to select all four circular edges, because no tangency condition exists at the top or bottom. The final model with this round feature completed looks like the following.

Save and close this model.

LESSON 14 – Chamfers Create a new part called Finger_Guide. We are going to use a combination of extrude and chamfer features to complete this model. Feature 1 – Extrude The first feature will capture most of the shape of the model as seen from the top view (with the exception of the chamfered edges. Therefore, we will use the TOP datum plane as the sketching plane, and face the RIGHT plane towards the Right. Sketch the following profile. NOTE: Take advantage of symmetry to reduce the number of required dimensions.

Extrude this profile 1.5 inches to create our first extrude feature, as shown in the next figure.

Feature 2 – Extrude (Cut) The second feature will be a cut that leaves the “L” shape seen in the Front view of the exercise. Therefore, use the FRONT datum plane as a sketching plane, and face the RIGHT datum plane towards the right. Inside the sketch, select the top and right surface of our first feature as sketching references, and then sketch and dimension the following rectangle.

Extrude this Through All on both sides of the datum plane using the Options slideup panel to define the depth in both directions. The final result is shown in the next figure.

Feature 3 – Chamfer For this chamfer feature, we are going to create three different sets. One of the sets will even have transitions to deal with. Set 1 For the first set, we will start by clicking on the chamfer icon, and then select the following edge.

By default, the scheme is D x D, and in our example, the “D” value is 0.060. We will change the scheme to D1 x D2, and then enter 1.9 and 0.3 for the dimensions, as shown in the next figure of the preview for this scheme.

Set 2

For the second chamfer set, we will pick (without using the Ctrl key) the equivalent vertical edge on the back side of this model. You may need to use the “Flip” button to the right of the D2 field to get the right scheme, as shown in the next figure.

Set 3 For this set, we will start by picking on the horizontal line that forms the top of the “L” front surface. Do not use the Ctrl key, so you can create a third set. Change the scheme to Ang X D, and use 60.0 for the angle and 0.44 for the “D” value. Flip the dimensions if necessary to get the following.

Now, hold down the Ctrl key and select the equivalent edge on the back side. The preview should now look like the following.

If we were to click on the preview button (the one with the glasses in our dashboard), we would see the following.

Clearly, the third chamfer set is not ending properly – it should go all the way to the back of the model. Therefore, we will need to use transitions to fix this. Click on the transitions button in the lower left corner of our dashboard. Next, pick on the following transition (shaded in blue in the next figure for more clarification).

When we select this, we can see that the transition assigned right now is called Default (Stop Case 2). We will change this to Stop Case 1, which looks like the following.

If we click on the preview button now, we see the following.

This looks correct. Now, click on the equivalent transition on the other side. Its default transition is Default (Stop Case 1). We will use the Stop Case 2 for this one, and now our transitions are correct on both sides. Finish out of this chamfer feature, and our model is done, as shown in the next figure.

Save and close this model.

LESSON 15 – Draft Open up the Safety_Key part that we created in Lesson 6 – Extrude. It currently looks like the following.

Draft Check The first step to this exercise is to perform a draft check on this model to see where we need to add draft. We need at least 2 degrees of draft on all vertical surfaces. Therefore, we will go to Analysis, Geometry, Draft, which brings up the following window.

Go to the Definition tab, which looks like the following.

We will start by right clicking over the model until we see the entire part highlight in blue, and the tool tip says SolidGeom, as shown in the next figure.

Then, click with the left mouse button to select the entire model. In our Draft window, we should see this selection as follows.

Now, we will skip over the next field, and in the Draft Angle section, click on the Both Sides button, and change the angle to 2.0, as shown in the next figure.

Now, go back and click on the Direction field to activate it, and select on the TOP datum plane. The model will change color, as shown in the next figure.

On the left side of our screen, a legend appears that indicates the draft angle currently assigned to each color, as we can see in the following figure.

From this legend and our model, we can see that all of the vertical surfaces are shaded in green, which indicates a 0.0 degree draft. This is obviously unacceptable, so we must add draft to all of these green surfaces. Adding Draft Close out of this analysis window, and click on the draft tool. For the surfaces to draft, we will use the Ctrl key to pick all of the surfaces that touch the bottom surface of the model, as shown in the next figure.

Next, click in the Draft Hinge field to activate it, and pick on the bottom surface of the model. We are using this surface, because we have been told in the exercise that the footprint of the model can not change size, therefore, it should be our draft hinge. When we do this, the preview shows the surfaces angled, and we will enter 2.0 for the draft angle. Make sure the surfaces angle into the model as they go up, as we can see in the following preview.

Click on the green check mark to complete the first draft feature, and our model will currently look like the following.

We still have three surfaces that needed draft, but these surfaces did not touch the bottom of the model, so we did not include them in the first draft feature. We will now add draft to two more of these surfaces. Start a new draft feature, and pick on the following two surfaces (using the Ctrl key).

For the draft hinge, select the surface at the bottom of these two surfaces, and then enter 2.0 degrees for the draft, and make sure the draft is going into the part, as we can see in the following preview.

The model will look like the following once this draft has been completed.

Create one more draft feature, and select the following surface to draft.

For the draft hinge, select the triangular surface that this surface touches. Enter 2.0 for the draft angle, and make sure it is going back into the part, as shown in the following preview.

Finish this draft feature by clicking on the green check mark, and your finished model will look like the following.

Verification Run the draft check again using the entire model, and the same TOP plane as the direction. This time, our entire model is in magenta or blue, which indicates that we have at least 2 degrees of draft on all surfaces relative to the pull direction.

Close the analysis, and then save and close the model.

LESSON 16 – Hole Feature Open up the Hole_Exercise part, which looks like the following.

We are going to add three separate hole features to this model. The order does not matter.

Hole 1 – Coaxial Hole We will start with the coaxial hole at the left end of this part. To start, turn on the display of datum axes. Now, click on the hole feature. When the dashboard opens up, enter 0.625 for the diameter. Change the depth option to Through All, and now we are ready to pick references. We will pick on the A_3 axis. When we do this, we can see the following preview.

All we see is the end of the hole, but the depth part of the preview is not visible yet, indicating that we have not picked enough references. In this case, we need to define the surface that we are starting the hole from. To do this, right click out in the working window and select Secondary References Collector, as shown in the next figure.

Now, pick on the flat surface at the front of this tab that sticks out, as shown in the next figure as the meshed surface.

We can now see the preview for the hole in its entirety. Click on the green check mark to complete this hole, and our model looks like the following.

Hole 2 – Linear Hole The next hole we will create will be the one on the right side of the model. Therefore, create a new hole. The diameter is the same as the one we just did (0.625), and the depth option should be set to Through All again. Now, pick on the flat surface indicated by the mesh below.

We can see two drag handles. We need to drag these to references to locate the hole. We will drag the first one over to the right surface of the model, as shown in the next figure.

A dimension now appears locating the hole from this surface. Now, drag the other handle over to the flat surface of the tab where we placed the coaxial hole. When we do this, we see the other dimension, as shown in the following figure.

If we open up the Placement slide-up panel, we see the following.

We will start by changing the first dimension value to 0.75. Next, we want to line up the hole with the tab surface, therefore, we will change the Offset type to Align, as shown in the next figure.

The preview for this hole now looks like the following (note the absence of the second dimension).

The completed hole looks like the following.

Hole 3 – Sketched Hole The last hole will be the one in the middle. Since this hole has a counterbore profile, we will use a sketched hole to accomplish this. We could have also used a standard hole, but the dimensions wouldn’t be exactly the sizes we see here. Therefore, click on the hole feature again. This time, we will change the hole type from Simple to Sketched. When we do this, the dashboard looks like the following.

Click on the Sketch icon, and a new window will open for the sketcher tool. Sketch a vertical centerline, and the following profile.

NOTE: Since we are sketching the depth of the hole, we should use a dimension that will go past the part. We can later set up relations to make sure that it will always go

through the entire part. Since the height of the part is 1.94”, we decided to use 2.0” for this sketch. Once you finish the sketch, you will need to pick the placement point for the hole. Pick on the top surface of the model. Drag handles appear on the simplified preview.

Drag one handle to the right edge of this surface, and the other to the flat front surface of the tabbed section, as shown in the next figure.

Now that the placement is fully defined, we can see the correct shape and size of our hole. Open up the Placement slide-up panel, and change the edge dimension to 0.75 and change the offset type to Align for the other reference, as shown in the next figure.

The preview will look like the following.

Finish this hole, and our completed model looks like the following.

Save and close this model.

LESSON 17 – Shell Feature Draft1 Open up the Draft1 part, which should look like the following.

There should already be a draft of 8 degrees added to the outside of the protrusion from Lesson 15. If not, you can go back and add it before continuing. The next step is to add a 0.1 inch round to the top and bottom edge of this protrusion. We will therefore, click on the round tool, enter 0.1 for the radius value, and then pick the two edges shown below.

Once you add the round, rotate the model so you can see the large flat side of the part. Next, click on the shell tool icon from the feature toolbar, or go to Insert, Shell from the menu bar. When the dashboard appears, enter 0.0625 for the thickness, and then select the large flat side of the model, as shown in the next figure.

If you forget to pick on the surface, the shell will still be created, but no surfaces will be removed – it will be a hollow part. Click on the green check mark to finish this shell feature, which will look like the following.

Save and close this part. Headset Open up the headset that we have been working with. It should currently look like the following.

The first part of this exercise is to create the coaxial hole. If you recall from Lesson 16, to create a coaxial hole, we first need an axis to select. If you turn on the visibility of axes, you will see the following.

From the previous figure, we can see that we do not have any axes at the center of the cylindrical end. Therefore, we will need to create one. Click on the create axis tool, and then pick on the cylindrical surface at the end of the headset model. When we do this, we see the following.

The axis window will show Through as the placement type, as we can see in the next figure.

Click on OK, and our axis will be created. Now, click on the hole tool, and select this axis as the primary reference. We will see the following in our dynamic preview.

Change the diameter to 1.0, and the depth option to Through All. The preview will change to the following.

Now, right click on the window and select Secondary References Collector, as shown in the next figure.

Pick on the top, flat surface of the headset model, and you will see the following.

Click on the green check mark to complete the hole, and then rotate your model around to see the flat bottom surface, as shown in the next figure.

Now, we will create the shell for this model. Start by clicking on the shell tool, and enter 0.2 for the thickness. Pick on the large flat surface to remove, as shown in the following figure.

Next, click on the References slide-up panel, which looks like the following.

There is a field used to define non-default thicknesses. We will click in this field to turn it yellow and make it active, and then pick on one of the surfaces inside the hole (you only need to pick one). Another thickness dimension shows up on the model, and we will change its value to 0.5, as shown in the next figure.

Click on the green check mark to complete this feature, and our model now looks like the following.

Save and close this model.

LESSON 18 – Rib Feature Open up the headset model once more. It should look like the last figure above. The first thing we need to do is create a datum plane to use for our rib. Therefore, click on the create datum tool, and then select on the FRONT datum plane. Enter an offset direction of 3.75 into the model, but keep the positive side of the datum plane (indicated by the yellow arrow), going back towards the FRONT datum plane. The following preview shows this plane being created.

Once you finish creating this plane, we are going to use it to create the rib. Therefore, click on the rib tool, or go to Insert, Rib, from the menu bar, and then right click on the screen to select Define Internal Sketch. For the sketching plane, select on the datum plane that we just created. Accept the viewing direction as going away from the hole, and accept the RIGHT datum plane facing towards the Left. Click on the Sketch button, and sketch the following profile.

NOTE: Switch over to a hidden line view so you can see the internal edges, and select the two vertical internal edges near the outsides as sketcher references, as shown in the figure above. The sketch is symmetric about the center, and consists of five lines, as we can see if we go to a no hidden view.

Complete the sketch by clicking on the blue check mark. An arrow appears showing the material side for the rib, and it may be sticking up, which is in the wrong direction. Click on the yellow arrow if this is the case to reverse it to pointing down.

We should now see the dynamic preview for the rib. Enter 0.2 for the thickness, and our preview looks like the following.

Click on the green check mark to complete the rib, which looks like the following figure.

Now, we will add the rounds to this rib. First, create a round feature using a 0.125 radius value, and pick on the following references.

Finish this round, and it will look like the following.

The next round will be a full round that uses the following two references.

The completed round will look like the following.

The final round will be the 0.05” round that goes around the entire rib. Therefore, create a new round, enter 0.05 for the radius, and then pick on the following reference.

The completed rib with all of its rounds is shown in the next figure.

Save and close this model for the next lesson.

LESSON 19 – Patterns Open up the headset again. Right now, we have a single rib completed. We are going to pattern this rib, along with the rounds that are tied to it. If you recall from the previous exercise, we created a datum plane that gave us our offset distance of 3.75”. Therefore, we will need to pattern this datum plane first, and then reference pattern the rib and all of the rounds. All said, we will create five individual patterns. Pattern 1 – Datum Plane In the model tree, find the datum plane that we created for the rib (DTM1 in my example). Right click on this datum plane, and select Pattern, as shown in the next figure.

The 3.75” dimension appears on the model, as shown in the next figure.

Click on this dimension, and if the field appears, type in 1.25 for the increment. If the field does not appear, you can click on the Dimensions slide-up panel, and enter the increment in the space provided, as shown below.

Once you enter the increment value, two black dots appear on the model, showing where the two pattern instances (including the original) will be created, as we can see in the following figure.

Click on the green check mark to create the pattern, and you will see the following.

Pattern 2 – Rib The next pattern will be the rib itself. Right click on this rib from the model tree, and select Pattern, just as we did for the plane. When the dashboard appears, you should see Reference as the default option in the bottom, as we can see in the next figure.

Click on the green check mark, and the rib will be patterned, as shown in the next figure.

Pattern 3 – Round When we right click on the first round and select Pattern, it automatically patterns it for us. We won’t even get a dashboard. The following figure shows us the result.

Pattern 4 & 5 – Rounds We will repeat this process for the remaining two rounds, as shown in the next figures.

Save and close this model.

Cup_Washer For this lesson, we are going to create two patterns, one for the protrusion that sticks up above the part, and one for the three small holes. We will start by creating the extruded cylinder with the large hole. Feature 1 – Extrude Create an extrude feature using the TOP datum plane as the sketching plane, and face the RIGHT plane towards the Right. Sketch the following two circles.

Extrude this section 0.56” to create the following.

Feature 2 – Extrude The next feature will be one of the protrusions that sticks up on the part. Note the dimensioning for this feature goes from the bottom of the part, so we will need to use the TOP datum plane for the sketching plane. For the reference plane, we will need to create one on the fly. Therefore, after you pick the TOP plane for a sketching plane, move your window out of the way, and click on the create datum plane tool. For the datum plane creation, click on the Z_Axis going through the center of the hole. Hold down the Ctrl key, and pick on the RIGHT datum plane. Use 45 degrees for the offset angle. Our preview for the plane looks like the following.

Allow the positive side (yellow arrow) to face towards the right. When you click on OK to complete this plane, you are returned to the section window. We must pick on the newly created datum plane to make it the reference, and face it towards the Right. When you click on the sketch icon, you will want to pick Z_Axis and DTM1 (newly created plane) as the sketching references. Do NOT pick any other planes in the model as sketching references, because they are fixed and may affect our ability to pattern this protrusion later. Sketch a vertical centerline on top of our plane, and create the following symmetric profile (two arcs and two lines).

NOTE: The perpendicular constraints allow the lines on the side to understand that they go to the center of the part, because our two sketched arcs use the Z_Axis as their centers.

Extrude this section to a depth of 1.75, and our finished extrude feature looks like the following.

In the model tree, we can see a group created for this extrude.

It is a group, because we created the datum plane in the middle of defining the extrude feature, so it becomes grouped with the extrude, and automatically hidden. Feature 3 – Pattern Now, we will right click on the entire group itself, and select Pattern, as shown in the next figure.

All of the dimensions will show up on the screen. If you only tried to pattern the extrude feature itself, you would not see the driving angular dimension tied to the datum plane, as shown in the next figure.

When you click on the 45 degree dimension, enter 120 for the increment, and change the number of instances to 3. Click on the green check mark, and the pattern will be created. NOTE: The first extrude in the pattern is currently 45 degrees from the center. For this model, we want the lead extrude to be sitting at 0 degrees, so you will need to edit the first group in the pattern list (when expanded) and change the 45 degree dimension to 0.0, and regenerate the model. From a top view, the completed pattern looks like the following.

Feature 4 – Hole For the first hole, we are going to use an actual hole feature. Click on the hole feature, and pick on the following location.

When the preview for the hole appears, enter 0.56 for the diameter of the hole, and change the depth to Through All. The preview should now look like the following.

Down in the dashboard, click on the Placement slide-up panel, and change the placement type from Linear to Radial, as shown in the next figure.

Once we do this, we will need to drag the two drag handles over to an axis and a plane. We will start by dragging one of the handles over to the Z_AXIS axis. When we do this, a radial dimension appears, and we will change its value to 1.44, as shown in the next figure.

Next, drag the other handle over to the RIGHT datum plane. When we do this, an angle appears, and we will change it to 60.0 degrees, as shown in the next figure.

The Placement slide-up panel for our feature looks like the following.

Click on the green check mark to complete this first hole, which looks like the following.

Feature 5 – Hole Pattern The last feature for this model will be to pattern the newly created hole. Right click on the hole, and select Pattern from the model tree. The dimensions show up on the model.

We will pick on the 60.0 degree dimension, and enter an increment of 120 degrees. Change the number of instances to 3. Unlike the group pattern that we did previously, this pattern will show the black dots indicating the location of the patterned instances, as shown in the next figure.

Click on the green check mark to complete this pattern, and our finished model will look like the following.

Save and close this model.

LESSON 20 – Variable Section Sweeps Open up the Basket part that we created earlier. It should look like the following.

We are going to use Sketch 1 and Sketch 2 to create a new surface that has a semi-circular profile all along its length, but the radius of the semi-circle will be dependent on the outer trajectories used. Therefore, we will click on the Variable Section Sweep tool, or use Insert, Variable Section Sweep from the menu bar. When the dashboard appears, select Sketch 1 on the model. Make sure the entire curve is highlighted before you select it. Once you select it, your model should look like the following.

The yellow arrow indicates the start of the trajectory, and should be located where shown above. If not, click on the yellow arrow to flip it to the other end. Now, hold down the Ctrl key, and select the entire Sketch 2 curve, as shown in the next figure.

Now that both trajectories are selected, we will click on the sketch icon in the dashboard. NOTE: By default, the surface option is selected, which is what we want for this model. When we click on the sketch icon, we are placed into the section, looking at the two ends of the trajectories that we selected. These ends are indicated by the “X” symbols in the sketch. We want to sketch a semi-circle using these two “Xs” for the arc ends, as shown in the next figure.

When we finish the sketch, we should see the following dynamic preview.

We can see the semi-circular shape all along the trajectories, but increasing in size at the other end. Click on the green check mark to complete this feature. Our basket now looks like the following.

Save and close this part.

LESSON 21 – Swept Blends Open up the Swept_Blend2 part. It looks like the following.

We can see three individual rectangular sketches. Each of these shares the outside edge of the model, which we can use as a trajectory. We will go to Insert, Swept Blend, Cut from the menu bar, and the following menu manager appears.

We will select the Select Sec option (as shown above), because we are going to select the sections. We will leave the Normal to Origin Trajectory (NrmToOriginTraj) option selected. Click on Done to continue. This brings up the following window.

The menu manager gives us the following choices.

We will select the front edge of the model, therefore, select the Select Traj option. When we pick this option, we get the following menu manager.

We want to pick on the entire tangent set of front edges, therefore, we will pick on the Tangent Chain option, and pick the first arc indicated by the bold red selection in the next figure.

An arrow appears, indicating the start of the trajectory. We will leave it in the location shown. The entire edge should be highlighted in blue, showing the full tangent chain of edges. Click on Done to continue. A surface should highlight in green. Click on Accept if it is the bottom surface of the part, as shown in the next figure. If not, click on Next until you see this surface highlight, and then click on Accept.

We are placed into the menu to select the sections, which looks like the following.

We will use the Sel Loop option to select the entire loop of edges that make up the rectangle in our section. Once we pick this option, pick on one of the lines of the rectangle sketch that sits at the beginning of our trajectory. When we do this, an arrow appears on one of the vertices, as shown in the next figure.

In order to avoid a twisting effect, we want the vertex for each section to be the same one. For consistency, we want to use the vertex that sits on the trajectory. Therefore, click on Start Point in the menu manager, and select on the vertex that lies on the trajectory, as shown in the next figure.

The arrow now appears on this vertex. Do not worry about the direction of the arrow. Click on Done to move on to the next section.

Use the Sel Loop option again, and pick on the small rectangle in the center of the model. Make sure the start point is sitting on the vertex that lies on the trajectory, as shown in the next figure.

Click on Done to continue. In the message bar, we are prompted to create another section. Click on Yes to create one more section. Repeat the same process to pick the last section (Sel Loop). Make sure the start point is in the correct spot, as shown in the next figure.

Click on Done. In the message bar, enter No to finish creating sections. An arrow appears on the model indicating direction of material removal, as shown in the next figure.

We want to click on Flip, followed by Okay to get the material to remove inside the rectangle. Click on OK to complete this feature, which looks like the following.

If you hide the three sketched rectangles and shade the part, it will look like the following.

Save and close this model.

LESSON 22 – Boundary Blended Surface Open the Boundary4 part. It looks like the following.

We can clearly see the seam lines in this model, due to poorly defined boundary conditions. We will fix this by editing the definition for the MAIN_SURFACE feature in the model tree. When we use Edit Definition on this feature, we see the following.

Right now, we can see that all boundary edges have a Free state associated with them. Because we are going to be mirroring this surface about two planes, we want to make sure that our edges on those planes have a Normal condition applied to them, as indicated in the next figure.

We will start by right-clicking on one of the boundary condition symbols and select Normal, as shown in the next figure.

When we do this, the boundary condition symbol changes to the appropriate condition, as we can see in the next figure.

We will do the same thing to the next boundary condition, as we can see in the following figure.

Its resulting condition will look like the following.

When we click on the green check mark to complete these changes, the rest of the features resume, and our finished surface model will look like the following.

We can now see that the seam lines are gone. Save and close this model.

LESSON 23 – Copy & Paste Tool Open up the model entitled Toy_Block, which currently looks like the following.

In the model tree, we have a feature called Letter_A, which is an extruded cut that creates the letter. We are going to copy this feature to create the rest of the letters. For the purpose of saving space, we will only demonstrate how to do this with the letter “B”, but you can continue to create the rest of the letters (C-F). The first thing we will do is highlight Letter_A in the model tree, and then go to Edit, Copy from the menu bar. Once we do this, select Edit, Paste from the menu bar, which will bring us into the dashboard for an Extrude feature. We will notice in our dashboard, that the remove material icon is already selected, as it should be.

We will need to edit the placement of the sketch, and possibly tweak the sketch itself. Therefore, right click on the working window, and select Edit Internal Sketch, which brings up the section window, as shown below.

We can see that we must re-select our sketching plane and sketching reference plane. For the sketching plane, we will pick on the front side of the block where we currently see the “B” letter in our exercise. We will face the RIGHT datum plane towards the Right. When you are placed into the sketch, you can see an outline of the current sketch floating along with your mouse, as shown in the next figure.

We want to move our mouse so the letter appears like the following (approximately centered on the block face).

Click once to place the sketch. The dimensions will appear, and we want to make sure we have two locating dimensions, each modified to 0.1875”, as shown in the next figure.

Next, pick on the letter “A”, and then click on the Modify icon. This will bring up the following window.

Change the text to “B”, and then you can adjust any other settings as necessary to get the letter looking like you want it. Click on OK once you are happy with your letter, and your sketch will look like the following.

You could further change your letter by modifying the 2.5” dimension. We will leave it alone, and click on the blue check mark to finish this sketch. We are placed back into the section window, where we will click on OK. Finally, click on the green check mark to complete this feature, and we can now see our finished letter “B”, as shown in the next figure.

On the model tree, we should see an Extrude 1 feature. We want to rename this to LETTER_B, as shown in the next figure.

Save and close your model.

LESSON 24 – Fill Tool There are no exercises for this lesson.

LESSON 25 – Merge Tool Open up the model entitled Project_Exercise, which looks like the following (no hidden mode):

The goal for this exercise is to merge the two surfaces together to make a single quilt surface. When selecting surfaces, it is easier to change your selection filter to Quilts, as shown in the next figure.

Then, select one of the surfaces, hold down the Ctrl key, and then select the second surface. Both surfaces will mesh in no hidden mode, as shown in the next figure.

Once both surfaces are selected, the merge tool is available. Click on this tool, and we will see the following preview.

Both surfaces highlight in a yellowish hue. The first surface that you pick (considered to be the parent surface) is more of a yellow color, while the second surface you selected (considered the child) is more of a cream color. A yellow arrow will indicate which side of the quilt(s) will be kept after the merge. We want it to look like the figure above. If it does not, you will need to click on the yellow arrow to flip the material side. Once it looks like the figure above, click on the check mark to complete the merge. The model will now look like the following.

We can see that the top edge of the cylindrical surface has been removed within the adjoining curve. If we hide the project feature and the sketch features in the model, we get a clear picture that these two surfaces are indeed merged, because we can see a purple internal edge between the two surfaces, as shown in the next figure.

Save and close this model.

LESSON 26 – Trim Tool Open up the Indexing_Surface model. It will look like the following figure.

We are going to use the indexing surface (the wavy one) as a trimming tool to cut out the bottom of the cylinder, thus retaining the indexing edge. Unlike the merge, which would have kept the index surface, we only want to have the cylinder when we are done, therefore, a trim is a better tool. We will start by going to our Quilts selection filter, and the pick on the cylindrical surface, as shown in the next figure.

Once you have the cylinder selected, click on the trim tool. When the trim dashboard appears, select on the indexing surface. We will see the following.

From this preview, we can see that we will be getting rid of the top of the cylinder, and only keeping the bottom portion, under the indexing surface. This is not what we want, therefore, click on the yellow arrow to flip the material side, and you will see the following.

This is exactly what we want, but before we finish the model, we need to remove the trimming quilt. To do this, click on the Options slide-up panel, and uncheck the Keep Trimming Surface option, as shown in the next figure.

Now, click on the green check mark to complete this feature. Our model now looks like the following.

Save and close this model.

LESSON 27 – Intersect Tool Open up the Intersect_Ex part, which looks like the following. NOTE: Datum planes have been turned off to view these sketches easier.

To be able to create this model, we are going to need to do a combination of three things. Feature 1 – Intersect Curves Be sure your selection filter is not on Quilts anymore. Select one of the two sketches, then hold down the Ctrl key, and select the other. Once both are selected, click on the Intersect tool. This will create the following curve at the projected intersection of both curves.

The original two sketches are automatically hidden in the model tree. That is okay – because for our next feature, we can pick the first sketch directly in the model tree. Feature 2 – Extruded Surface In the model tree, select Sketch 1, and then click on the Extrude tool. When we do this, the dynamic preview shows a surface, as shown in the next figure.

For the depth of the surface, change to the To Selected option, and pick on the upper end of the curve, as shown in the next figure.

Click on the green check mark to complete this surface, which looks like the following.

Now, we can use the intersected curve as a trimming tool on the surface. Therefore, pick once on the surface to select it (or select it from the model tree), and then click on the trim tool. Once the trim dashboard appears, click on the curve. A preview will show which side of the surface will be kept. Flip the arrow if necessary to arrive at the following preview.

Click on the green check mark to complete this trim, and your finished surface will look like the following.

Save and close this model.

LESSON 28 – Offset Tool

There are no exercises for this lesson.

LESSON 29 – Solidify Tool Open up the BBS1 model, which will look like the following.

We want to take the middle of this part (which is a surface) and turn it into a solid. If we rotate and shade the model, we can see that the surface is not closed, as shown in the next figure.

Therefore, the first thing we need to do is to create a Fill surface. Click on the Fill tool, or go to Edit, Fill, and when the dashboard appears, right click in the working window and select Edit Internal Sketch. For the sketching plane, select the TOP datum plane. Face the RIGHT plane towards the Right, and then use the Use Edge tool to get the two sides of the surface, as well as the two solid edges that close off the boundary, as shown in the next figure.

When we click on the blue check mark, we see the following preview.

Click on the green check mark to complete the feature. Now, we have two surfaces that are not connected, so we will need to merge them together. Change over to the Quilts selection filter, pick both surfaces (using Ctrl), and merge them together. You should now be left with a single quilt in the middle with purple internal edges. The only pink edges are the ones that touch the solid volumes on either end, as shown in the next figure.

Now we can solidify the model. Click on the single quilt surface in the middle so it highlights, as shown in the next figure.

Next, click on the Solidify tool. Initially we see the following preview.

If we look in the dashboard, we can see that the Patch option is selected, as shown in the following figure.

We want to switch over to the Solid option (the first icon all the way to the left), and then flip the yellow arrow so it points into the model. The preview should now show the entire model highlighted, as shown in the next figure.

Click on the green check mark to complete the solidify tool, and we should be left with a completely solid model, as shown in the next figure.

Save and close this model.

LESSON 30 – Thicken Tool Open up the Project_Exercise model again, which looks like the following if all previous lessons have been completed.

The first thing we are going to do is add a round to the intersection of these two surfaces. Therefore, click on the Round tool, enter 0.25” for the radius, and pick the following edge.

Complete this round. Now, switch over to the Quilts selection filter, and pick on the entire surface model. Once the entire model is highlighted, click on the Thicken tool. In the dashboard, enter 0.05” for the thickness, and flip the arrow if necessary to get it to the inside. The preview for the thicken tool should look like the following.

Complete this tool, and the model will look like the following.

Save and close this model.

LESSON 31 – Extend Tool Open up the Extend2 model, which looks like the following figure.

We are going to start by setting our selection filter to Geometry, and then we are going to pick on the following surface edge.

Once the edge is selected, click on the Extend tool. We will see a preview for the extend, as shown below.

Before we extend this out we will go to the Options slide-up panel and change the type from Same to Tangent, as shown in the next figure.

Now, change the extend distance to 3.5, which should clear our domed surface, as shown in the next figure.

Click on the green check mark to complete this first extend. Repeat this process for the other side, to arrive at the following.

Now that we have both sides extended, we will switch over to the Quilts selection filter, and pick both quilt surfaces. Click on the Merge tool, and you will get the following.

If your preview looks like the one above, click on the green check mark to get the following quilt surface.

Click on the entire quilt surface, and then select the Thicken tool. Flip the arrow so it is pointing into the inside of the surface, and change the thickness to 0.125”. The following figure shows the preview for this.

Click on the green check mark, and our part is completed, as shown in the next figure.

Save and close this model.

LESSON 32 – Mirror Tool Funnel Open up the funnel model that we worked with in an earlier lesson. It looks like the following.

Since this is a surface model, we will mirror the surface instead of the entire part. The advantage of mirroring individual features is that it does not mirror the default datum geometry or anything else, just the surface. Therefore, we will use the Quilts selection filter, and pick on the single quilt. Once the quilt is selected, click on the mirror tool, or go to Edit, Mirror from the menu bar. When the dashboard appears, click on the FRONT datum plane to mirror about. We will see the following preview.

Click on the green check mark to complete this mirror, and then merge the two surfaces together using the Merge tool. The result will be the following.

Now, pick this entire surface, followed by the Mirror tool again, and then pick on the RIGHT datum plane. The preview looks like the following.

Complete this mirror, merge the two sides together, and you will have your final funnel part.

Save and close this part.

BBS2 Open up the BBS2 part. Since this is a solid model, we will mirror the entire part. Therefore, in the model tree, select on the BBS2.PRT words at the top of the tree. Once you have selected this, click on the Mirror tool. When the dashboard appears, use the TOP datum plane to mirror about, and you will see the following preview.

Click on the green check mark to complete this mirror. Hide the mirror in the model tree to eliminate any extra curves, planes, etc. that may have been in the first side. The following figure shows this completed model.

Save and close this model. Project_Exercise Open up the Project_Excercise model. It too is a solid model, so we will select the entire model by picking on its name in the model tree, followed by the Mirror tool. For a mirroring plane, pick on the TOP datum plane again. The following shows the preview for this mirror.

The completed part will look like the next figure.

Save and close this model. Extend1 Open up the Extend1 model that we worked with earlier. It should currently look like the following.

The first thing we are going to do is mirror this surface. Therefore, use the Quilts selection filter, and pick the entire surface, followed by the Mirror tool. For a mirroring plane, select the RIGHT datum plane. We will see the following preview.

Once you mirror the surface, perform a merge operation to create one larger quilt, as shown in the next figure.

Now, we are going to create a mirror that goes around the top edge. Often, when you have a round that traverses a mirroring plane, it is better to mirror first, and then add the round. Therefore, we will click on the round tool, enter a radius of 0.25”, and then select on the following edge.

Once you create the round, select the entire quilt, followed by the Thicken tool. Enter a thickness of 0.125”, and point the direction to the inside of the surface, as shown in the following preview.

Finish the thicken tool, and our model will be complete, as shown in the next figure.

Save and close this model.

LESSON 33 – Layers There are no exercises for this layer.

LESSON 34 – Parameters & Relations Open up the Draft1 part. It should have a rib that is patterned five times (every 72 degrees). If not, start by patterning this rib. To do this, right click on the rib and select Pattern. For the pattern type, change it to Axis, and select the Z_AXIS. For the increment, enter 72 degrees, and a total count of 5. The part with the pattern of ribs should look like the following.

In order to drive the pattern, we will need to see not only the angular spacing between the ribs, but the number of ribs itself. Therefore, we will right click on the pattern in the model tree and select Edit. This will bring up the following dimensions.

We can see the angular spacing (72.000) and the number of ribs (5). With these dimensions visible, go to Tools, Relations, which will cause the dimensions to temporarily switch to their symbolic names, as shown in the next figure.

Therefore, to drive the equally spaced ribs based off of the number of ribs, the equation that we need to write (in words) would be: Angular Spacing = 360 Degrees / Number of Ribs Therefore, we must enter: d33=360/p36 We have a window that opens for us to enter the equation, which currently looks like the following.

We will enter the equation exactly as we specified into this window, as shown in the next figure.

NOTE: Be sure to look at your model to see if your symbolic names are the same as this exercise solution, if not, you will need to enter the names as they appear on your model. Once you have entered the relationship into the window, click on OK. In the model, edit the pattern again, and change the number of ribs from 5 to 10, and then regenerate your model. You should see 10 equally spaced ribs, as shown in the next figure.

Save and close this model.

LESSON 35 – Family Tables There are no exercises for this lesson.

LESSON 36 – View Manager There are no exercises for this lesson.

LESSON 37 – Assembly Mode – Bottom-Up Design Create a brand new assembly called Machine_Vise in the Machine_Vise folder. We have already created the sub-assembly called MV_Screw_Assy in this lesson, but we are going to create the top-level assembly now. Component 1 – 01_MV_BASE Click on the Assemble Component icon. When the Open window appears, select the 01_mv_base.prt component, followed by Open. This will bring the base model into our working window, and the Component Placement window appears. Since this is our first component in the assembly, we will click on the Defaut placement icon, followed by OK. Our first component looks like the following.

Component 2 – 02_MV_SLIDING_JAW Click on the Assemble Component icon again. This time, select the 02_mv_sliding_jaw.prt component. When the placement window appears, we will start picking references according to the next figure.

(1) – Mate Select on the top flat surface of the 01_mv_base part, and the underneath flat side of the 02_mv_sliding_jaw component. Be sure the placement type is Mate with a Coincident type associated to it. (2) – Mate Select on the inner front surface of the 01_mv_base, and the front surface of the 02_mv_sliding_jaw component. Use another Mate, Coincident for the placement type. (3) – Mate Offset (1.5) Select the inner left-facing surface on the 01_mv_base component, followed b component, followed by the right surface of the 02_mv_sliding_jaw component. An arrow will appear asking for the offset distance. Enter 1.5 if the arrow is pointing to the left. If the arrow is pointing towards the right, enter -1.5. The component placement window should look like the following when all references have been selected.

Click on OK, and the following figure shows the placement of this component.

Component 3 – 03_MV_SLIDE_KEY For this next component, it will be easier to hide the first component that we assembled. To do this, right click on the 01_MV_BASE component in the model tree, and select Hide. It will temporarily disappear from view, as shown in the next figure.

Click on the Assemble Component icon, and pick the 03_mv_slide_key.prt component. Use the references in the next figure to assemble this component.

(1) – Mate Select the back surface of the groove on the 02_mv_sliding_jaw component with one of the two side surfaces on the 03_mv_slide_key component. Make sure the constraint is a Mate with a type of Coincident. (2) – Mate Select the bottom of the groove on the 02_mv_sliding_jaw component, and the bottom flat surface (back in this figure) of the 03_mv_slide_key component. Use a Mate, Coincident constraint with this one as well. (3) - Tangent This one is sort of tricky. You may want to use Ctrl-Alt and the right mouse button to slide the key over until the square cut-out on the “03” component lines up with the hole on the “02” component, and then using a hidden line view, select one side of the cylindrical hole and one side of the square cut, thus producing a tangent constraint. When done, the placement of this component looks like the following.

Component 4 – 03_MV_SLIDE_KEY Repeat this same process to assemble the other slide key. The fully assembled key looks like the following.

Component 5 – 04_MV_SET_SCREW Assemble in the 04_mv_set_screw.prt component. Use the placement constraints shown in the next figure:

(1) – Insert Select on the larger cylinder on the set screw and the inside surface of the hole on the bottom of the sliding jaw component. An Insert placement type should be created automatically. (2) – Mate Select on the middle flat surface of the set screw and the first noticeable flat surface you see in the hole on the bottom of the sliding jaw. Be sure to make the offset distance 0.0 and select a Mate command. It may come in originally as an Align Offset. The final placement for the first set screw looks like the following.

Component 6 – 04_MV_SET_SCREW Repeat this process for the second set screw, whose placement looks like the following when complete.

Component 7 – 05_MV_JAW_PLATE Assemble in the 05_mv_jaw_plate.prt component, and use the following placement references and constraints.

(1) – Insert Pick on one of the holes in the sliding jaw and the corresponding hole on the jaw plate. An Insert command will be created. (2) – Insert

Do the same for the other set of holes. (3) - Mate Pick on the flat part of the jaw plate that does not have the countersink around the holes and then pick on the flat surface on the sliding jaw. Be sure to use a Mate constraint with a 0.0 offset (or coincident). Use Ctrl-Alt and the Right Mouse Button to move around the component as necessary for easier picking. The final placement of this plate is shown in the next figure.

Component 8 – 05_MV_JAW_PLATE Repeat this process to add another jaw plate to the stationary side of the base, as shown in the next figure.

Component 9 – 06_MV_FLAT_HEAD_SCREW Assemble in the 06_mv_flat_head_screw.prt into the assembly using the following two placement constraints and references.

(1) – Insert Select on the cylindrical surface of the screw and the first cylindrical surface of the jaw plate. An insert constraint will be created. Use Ctrl-Alt-RMB to move the screw so it is visible to select the next references. (2) - Align Pick on the flat head of the screw, and the flat surface of the jaw plate and use a coincident align to make them flush. The final placement of the first screw is shown in the next figure.

Components 10-12 – 06_MV_FLAT_HEAD_SCREW Repeat this same process to bring in the remaining 3 flat head screws in the locations shown in the next two figures.

Component 13 – MV_SCREW_ASSY The next component we will bring in will be the mv_screw_assy.asm assembly that we created in this lesson. We will use the following constraints for this assembly placement.

(1) – Mate

I chose to do the mate first so it would flip the assembly around to be facing the right direction. Pick the small flat surface in the middle of the collar and the first small flat surface you encounter in the hole on the sliding jaw. Change the constraint to a coincident mate. (2) – Insert Next, select the large cylindrical surface on the collar and the first cylindrical surface of the hole on the sliding jaw. The final placement for this sub-assembly is shown in the next figure.

Component 14 – 10_MV_HANDLE_ROD The next component will be the rod that goes through the end of the sub-assembly that we just placed. To do this, we will use an insert, and then a mate offset to fix the movement of this rod through the hole. The following figure shows these placements.

(1) – Insert Select the cylindrical surface of the rod and the inside of the hole on the subassembly. An insert command should be created. (2) – Mate Offset (-0.5) Select on the bottom flat surface of the rod, and the bottom flat surface of the base. It may create a coincident align, so you will need to go into the placement window and use the pull-down to change it from Coincident to 0.0, and then edit this number to -0.5 to move the rod up. The following figure shows this final placement for the rod.

Component 15 – 11_MV_HANDLE_BALL Assemble in the 11_mv_handle_ball.prt component. You may wish to turn on hidden lines to see the placement references easier. We will use the following references.

(1) – Insert Select the cylindrical surface on the rod, and the cylindrical surface of the hole in the ball. An insert command will be created. (2) – Mate Select on the top flat surface of the rod, and the inside flat surface of the hole on the ball. Use a coincident mate for this placement. The following figure shows this component’s placement.

Component 16 – 11_MV_HANDLE_BALL Repeat this process for the second ball. We will have to add a third constraint for this ball, because the holes for the taper pin will be on opposite sides when we use the same placement constraints as the first ball. To rotate the ball around, uncheck the Allow Assumptions box in the placement window, and use Ctrl-Alt and the middle mouse button to rotate the ball around 180 degrees (approximately). Once the ball is rotated, click on the “+” symbol to add

one more constraint. Turn on the visibility of datum axes, and select the two axes to Align to each other. If you need to, re-select the Allow Assumptions box if the last constraint does not change the status to fully constrained. The following figure shows this placement.

Component 17 – 12_MV_TAPER_PIN Assemble in the 12_mv_taper_pin.prt component into the assembly. Turn on the display of hidden lines, and use the following constraints and references.

(1) – Align Select on the axis of the taper pin, and on the axis of the ball. This will line up the axes using an Align constraint. (2) – Mate Select on the small flat end of the taper pin, and the inside flat surface of the rod and use a coincident mate. Be sure the Allow Assumptions box is checked, and the following figure shows the final placement for this pin.

Component 18 – 12_MV_TAPER_PIN Repeat this process for the last taper pin, which will look like the following when assembled.

The following figure shows the completed Machine Vise assembly.

Save and close this assembly.

LESSON 38 – Assembly Mode – Top-Down Design There are no exercises for this lesson.

LESSON 39 – Assembly Mode – Assembly Cuts

Switch working directories back to the ProETrain folder. Open up the assembly entitled Shelf.asm, which looks like the following.

We need to create a series of assembly cuts to create the pre-drilled holes that will later be used for wood screws. Before we get started, go to your model tree, and select on the Settings button. When this expands, select on Tree Filters, as shown in the next figure.

When you select Tree Filters, you get the following window.

Select the Features option, as shown above, and then click on OK. Features will now be shown in the model tree, as we can see in the next figure.

Now, we are ready to begin. We will start with the holes on the back of the assembly. Click on the Extrude tool. When the dashboard opens, you should notice right away that the remove material icon is selected and grayed out, because we can only create cuts in assembly mode with this tool. We will right click on the working window, and select Define Internal Sketch. When prompted, select the following references for the sketching plane, reference plane and orientation of the reference plane.

Inside the sketch, we will start on the right side of the part, and sketch 3 circles. Be sure all circles are assuming equal radii and lined up vertically. Dimension the circles as shown in the next figure.

Now, zoom in on the left side, and sketch three more circles. For each of these circles, make sure they are using the same radii as the previous three, are lined up vertically with each other, and are lined up with their respective holes horizontally. We should only need one dimension for these three circles, as shown in the next figure.

Now, sketch two remaining circles in line with the top holes, using the same radii value as the others, and dimensioned from the left as shown in the next figure.

Once you have all eight circles sketched, click on the blue check mark to complete the sketch. Change the depth of the cut to 1.5, and the preview will look like the following.

Before we go any further, expand the Intersect slide-up panel. It currently looks like the following.

We do want the holes to intersect all of the parts in this assembly, so the list of models is correct, however, we want the visibility of the holes to be at the part level, and currently, only the top-level assembly is going to show them. Therefore, we need to uncheck the Automatic Update box so we can control the values in the table. Once unchecked, pick on the Display cell that currently says Top Level, and change it to Part Level as shown in the next figure.

Do this for each of the model rows, until our slide-up panel looks like the following.

Now, we are ready to complete this extruded cut. Click on the green check mark, and our model will look like the following.

We can verify the display level by opening up the SHELF_BACK component, and we can see the holes in this part.

Before we create our new extrude, we will create a datum plane in the assembly. Therefore, click on the create datum plane tool, and select on the top flat surface of

the assembly. Use -0.25 for the offset distance, to place it into the shelf, as shown in the following preview.

Click on OK, and we will now have an ADTM1 plane in our model tree. Now, we will click on the Extrude tool again. Use Define Internal Sketch to start our sketch, and select the ADTM1 from the model tree to use as our sketching plane. Make sure the direction of viewing is going down into the shelf, and then select the following surface to face towards the Bottom.

Inside the sketch, start on the left side, and sketch a circle dimensioned as shown in the next figure.

Then, sketch a circle on the right side that is the same radius as the first one, and lines up horizontally. Dimension it as shown in the next figure.

Click on the blue check mark to complete this sketch, and change the depth option to Through All, making sure the direction of feature creation is going down through the shelf. The following shows the preview at this point.

Open up the Intersect slide-up panel, which shows only the SHELF_MAIN and the two SHELF_SUPPORT models. This is correct, but we will need to uncheck the Automatic Update box to change each of these to Part Level visibility, as shown in the next figure.

Click on the green check mark to complete this second extrude feature. We can see the following in our assembly.

If we open up the SHELF_MAIN component, we can see the holes that were created by both extrude features.

Save and close this assembly.

LESSON 40 – Assembly Mode – Assembly Operations There are no exercises for this lesson

LESSON 41 – Drawing Mode – Drawing Fundamentals There are no exercises for this lesson

LESSON 42 – Drawing Mode – Creating A Drawing There are no exercises for this lesson

LESSON 43 – Drawing Mode – General Views There are no exercises for this lesson

LESSON 44 – Drawing Mode – Projection & Section Views There are no exercises for this lesson

LESSON 45 – Drawing Mode – Auxiliary & Detailed Views There are no exercises for this lesson

LESSON 46 – Drawing Mode – Show Axes & GTOL Datums There are no exercises for this lesson

LESSON 47 – Drawing Mode – Dimensioning There are no exercises for this lesson

LESSON 48 – Drawing Mode – Broken & Partial Views There are no exercises for this lesson

LESSON 49 – Drawing Mode – GTOLS & Symbols Switch working directories over to the Drawing folder. Open up the drawing entitled GTOL_Create. It initially looks like the following figure.

We will start by completing the two geometric tolerances on the cross-section view, which currently looks like the following.

GTOL 1 – Circular Runout We will start with the Circular Runout tolerance on the larger of the two diameter dimensions on the right of this view. Therefore, go to Insert, Geometric Tolerance. When the window opens, click on the Circular Runout symbol (single arrow). This will make the screen look like the following.

Keep the Reference type at Surface and then click on the Select Entity button. Pick on the cylindrical surface that highlights in blue when you place your mouse in the following location.

For the Placement type, keep Dimension, and click on the Place Gtol button. Pick on the 31.8/31.6 limit diameter dimension to the right of this view. We will see the GTOL appear on the dimension. Use Move to clean up the location. Currently, my control frame looks like the following.

Now, we will click on the Datum Refs tab, and make sure B is the primary datum referenced. We should not have any material symbols set (RFS should be set), as shown in the next figure.

Click on the Tol Value tab, and change the tolerance to 0.1. Again, no material condition should be set, and our window should look like the following.

Click on the OK button to complete this tolerance. Our control frame looks like the following figure.

GTOL 2 – Circular Runout We will create another circular Runout. We could have clicked on the New Gtol button while we were in the last definition, but we did not, so we will have to go back through Insert, Geometric Tolerance. When the window appears, we should still have the same values as we did for the previous Runout. This time, click on the Select Entity, and pick in the location shown in the following figure.

We will use the Dimension placement type, and click on the Place Gtol button to place the control frame on the 20.13/20.00 limit diameter dimension next to the one we selected in the last GTOL. The control frame appears on the dimension, and the set datum “B” reference attaches to the bottom of it. We will use Move to clean up the location of the dimension, as shown in the next figure.

We will now edit the values. In the Datum Refs tab, make sure you are on the Primary tab, and select A for the reference, as shown in the next figure.

Now, click on the Secondary tab and select C as the datum reference, as shown in the following figure.

Now, click on the Tol Value tab, and enter 0.14 for the tolerance. We do not want any material conditions set, so our window should look like the following.

Click on OK to complete this GTOL, and our final section view looks like the following.

GTOL 3 – Position The last GTOL that we need to create is on the RIGHT view. It will be a position tolerance. Therefore, click on Insert, Geometric Tolerance, and when the window appears, click on the Position symbol. Our window will look like the following.

For the Reference type, change the option to Axis, click on the Select Entity button, and pick on the axis for the hole where the radius dimension is attached, as shown in the next figure.

For the Placement type, keep Dimension selected, and using the Place Gtol button, pick on the radius dimension (8.1/7.9 limit dimension). We can see the control frame on the drawing view, as shown in the next figure.

Go to the Datum Refs tab. The Primary tab should still show A, and the Secondary tab still shows C, but we need to add a maximum material condition symbol to the secondary reference, as shown in the next figure.

Now, go to the Tol Value tab, and add a maximum material condition to the tolerance, which should still be set at 0.14 from our previous GTOL definition, as shown in the next figure.

Go to the Symbols tab, and check the box for the Diameter symbol, as shown in the next figure.

Click on OK and our GTOL definition is complete. The completed view looks like the following figure.

Save and close this drawing.

LESSON 50 – Drawing Mode – 2D Drafting There are no exercises for this lesson

LESSON 51 – Drawing Mode – Tables & Balloons There are no exercises for this lesson

LESSON 52 – Drawing Mode – Adding Sheets & Finalize There are no exercises for this lesson

LESSON 53 – Drawing Mode – 2D Drafting There are no exercises for this lesson