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Autodesk Inventor® 11

Autodesk, Inc. 111 McInnis Parkway San Rafael, CA 94903, USA Tel.: +1/415-507 5000 Fax: +1/415-507 5100

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Autodesk Inventor 11 Hands-on Test Drive 000000000000116862

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Autodesk Inventor

Autodesk Inventor Table of Contents Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 Chapter 1: Creating Your First 3D Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 Chapter 2: Creating a Production Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Chapter 3: Completing the Part Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Chapter 4: Using AutoCAD Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Chapter 5: Assembly Basics – Creating & Assembling Components . . . . . . 69 Chapter 6: Assembly Documentation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Chapter 7: Working with Assembly Configurations . . . . . . . . . . . . . . . . . . .107 Chapter 8: Performing Stress Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .113 Chapter 9: Designing Welded Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . .123 Chapter 10: Creating a Sheet Metal Design . . . . . . . . . . . . . . . . . . . . . . . . . . .131 Chapter 11: Photo-Realistic Rendering . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .141 Chapter 12: Designing Tubes, Pipes, and Hoses . . . . . . . . . . . . . . . . . . . . . . .145 Chapter 13: Designing Cables and Wire Harnesses . . . . . . . . . . . . . . . . . . . .159 Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .171

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Introduction Table of Contents Welcome to the Autodesk Inventor® 11 Hands-on Test Drive . . . . . . . . . . . . . . . . . . . 3 Installing Your 30-Day Autodesk Inventor Test Drive . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Setting up Your System . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6 Getting Started . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 Getting Familiar with the User Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11

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Introduction Welcome to the Autodesk Inventor® 11 Hands-on Test Drive This Test Drive is designed to guide you through the principal processes of 3D product design. While working on the design of a go-cart, you will see how, with 3D modeling, you can quickly create and refine your complete product design while simplifying the production and revision of manufacturing drawings. Many of you have a large inventory of design data created in AutoCAD®. For this reason, we devote an entire chapter to showing you how easy it is to include 2D AutoCAD data into your 3D designs. The exercises illustrate key elements of workflows involved in the design of fabricated parts and multi-part assemblies. You will also take a look at how to design welded assemblies and sheet metal parts. Once you’ve created a 3D model of the proposed product, you can save valuable time and money by testing the model on your computer. The Autodesk Inventor product line includes tools for stress analysis using Finite Elements as well as tools for simulating and analyzing the dynamic behavior of systems under load. This Test Drive will show you how to perform a basic stress analysis on a part. Powered products invariably contain routed systems—both electrical systems containing cables and wire harnesses and tube and pipe for cooling, fuel and hydraulic systems. Traditional design techniques for routed systems are time consuming and often result in unforeseen delays and unnecessary engineering changes. In the final two chapters, you will see how routed systems can be developed as an integral part of the 3D model resulting in accurate manufacturing documentation and designs that work right the first time. Thank you for your interest in Autodesk Inventor. We sincerely hope that this tutorial will give you insight into the benefits of using Autodesk Inventor to improve your product development operations. We recommend that you work closely with your Autodesk Authorized Reseller to develop a detailed plan for deploying 3D design and simulation within your organization. The Autodesk Inventor Team

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Installing Your 30-Day Autodesk Inventor Test Drive System Requirements These are the recommended system requirements for the Autodesk Inventor 11 Test Drive 30-day trial software version: •

Windows 2000 Professional SP4

•

Windows XP Professional SP1 & SP2

•

Windows XP Professional x64 Edition

•

Recommended: Part and assembly design (less than 1000 parts)

•

Intel Pentium 4, Xeon, or AMD Athlon 2.0 GHz or better processor

•

1 GB+ RAM

•

128+ MB DirectX or OpenGL Capable Workstation Class Graphics Card

•

3.5+ GB Free Disk Space

For the latest system requirements, please visit www.Autodesk.com. Note: Less capable machines can run Autodesk Inventor 11, but the results will be less than ideal.

Installing the Autodesk Inventor Software 30-day Trial Version Follow these steps to install your 30-day Autodesk Inventor software trial. Prepare for software installation: 1. Close all open applications. 2. Insert the Autodesk Inventor 11 Test Drive CD disk 1 of 1 (in the back cover of this booklet) into the CD-ROM drive and follow the onscreen instructions. Note: During the installation process, follow the on-screen instructions to insert additional disks as necessary. 3. If the CD does not start automatically, go to D:\ (where D is the CD-ROM drive), and double-click the file setup.exe.

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4. On the Install page, follow Step 1: Review Product Documentation. • Click System Requirements to review the recommended and minimum system requirements. •

Click Graphics Card Driver Update to review important graphics card and driver information.

•

Click Autodesk Inventor Professional 11 Readme to read important application information.

Install Autodesk Inventor software: 1. On the Install page under Step 2, click Install Autodesk Inventor Professional 11 (30-day Trial Version). 2. On the Welcome Wizard page, click Next. 3. Read the license agreement; confirm by clicking I accept the license agreement and then click Next. 4. On the Destination Folder page, click Next to accept the default destination folder, or click Browse to define an alternate location. We highly recommend you install to the default location. 5. On the Products page, click Next. 6. On the Product Pre-Installation Checks page, click Next. 7. On the Pre-Installation Checks results page, click Next. 8. On the Installing Specified Autodesk Products page, click Install.

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9. When the installation is complete, click Next.

10. Review the Readme and Getting Started guides and then click Finish.

Installing the Hands-on Test Drive Sample Files After installing the Autodesk Inventor trial version, copy the sample files from the CD to your computer. •

On the Install page, click Install Hands-on Test Drive Sample Files and follow the onscreen instructions.

Note: We highly recommend installing the files in the default folder C:\Inventor_R11_TestDrive.

Setting up Your System In order to have the most productive experience with the Autodesk Inventor Hands-on Test Drive, we recommend you review your computer hardware settings and configure your Autodesk Inventor software display to ensure an optimal software experience.

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Optimizing Your System Graphics Settings Autodesk Inventor is a graphically rich design application. In order to maximize behavior and performance, optimize your computer’s graphics display. 1. Right-click in the Windows desktop background and choose Properties. 2. In the Display Properties dialog, click the Settings tab. 3. In the Color quality section of the dialog, select Highest (32 bit) and then click OK.

Using a Compatible Graphics Card Autodesk Inventor software is a high-performance 3D modeling application that uses the 3D rendering features of your graphics card to properly display the parts and assemblies on your computer screen. It is important to make sure your computer has both a compatible graphics card and the correct driver before using Autodesk Inventor software. To find information about your graphics card and download the correct drivers, visit www.inventor-certified.com/graphics and choose Card Certification.

Starting Autodesk Inventor Software Start Autodesk Inventor:

1. Double-click the Autodesk Inventor 11 application icon

on the desktop.

The Authorization dialog box is displayed with a reminder of the number of days remaining for your trial version of Autodesk Inventor. 2. Select the Run the product option and then click Next. The Getting Started page is displayed. This page offers many useful tools for learning how to work with Autodesk Inventor software, including what is new in the latest release, help for the AutoCAD user, tutorials, and so on. 3. Click Cancel in the lower-right corner of the Open dialog to close this window. You have opened the Autodesk Inventor software application.

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Setting the Default Color Scheme Autodesk Inventor software offers many different color schemes. For your first experience using Autodesk Inventor, we recommend using a simple color scheme with a white background. 1. From the Tools menu, choose Application Options. 2. On the Colors tab, choose the Presentation color scheme. 3. For those using less powerful machines or laptop systems, we also recommend that you clear the Show Reflections and Textures check box. 4. Click Apply and then click Close to close the Options dialog box.

Getting Started Using this Booklet Although you can use this Test Drive at your own pace, these materials are intended for use in an Autodesk Authorized Reseller-led workshop environment. To optimize learning, your Reseller will guide you through the exercises. This Test Drive is intended to give you an overview of 3D solid modeling and illustrate how Autodesk Inventor software can help you gain design efficiencies by moving to 3D. You should be able to complete all of the exercises in this booklet in approximately 6 to 8 hours. For convenience, each chapter begins with all the files necessary for the given exercise. If necessary, this allows you to move to the next chapter without requiring that you complete the current exercise. For more information or assistance using your Autodesk Inventor Hands-on Test Drive, contact your Autodesk Authorized Reseller.

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Helping the Project Team Design a Go-Cart As your design task, you will help design a go-cart.

Your work will focus on the rear-axle assembly and begin with the creation of a part which is the carrier for the sprocket.

You will then help finish the rearaxle assembly and create detailed drawings of your part and assembly. You will also learn how the design team uses the configurations functionality of Autodesk Inventor to design an entire family of gocart designs. Using the built-in Stress Analysis functionality, you will learn how to validate the strength of your 3D carrier part. Also, you design a welded assembly and create a sheet metal part. You complete the go-cart design by creating a photo-realistic rendering of the design. In addition to the design of the go-cart, you will complete a skid assembly by adding a pipe, rigid tube, and hose run to the assembly.

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In the final design exercise you create the wires, harness, and corresponding nailboard drawing of a pcb enclosure assembly.

Starting with a Project Autodesk Inventor uses project files to organize and manage the multiple files associated with a design. You will use one project file, provided for you, for all of the exercises in this Hands-on Test Drive. Activate the project: 1. From the File menu, choose Projects. 2. In the project window, right-click and choose Browse. 3. Browse to the folder where you downloaded the sample files (default was C:\Inventor_R11_TestD rive), select the file R11 Test Drive.ipj and then click Open. 4. If a check mark does not display next to the R11 Test Drive entry, then in the project window, double-click R11 Test Drive to activate the project.

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Opening Your First Assembly To gain familiarity with the Autodesk Inventor user interface, open a finished version of the go-cart rear axle assembly: 1. In the What to Do area of the Open dialog, click Open. 2. In the Open dialog, browse to the Intro folder and double-click Rear_Axle_Assy.iam. A finished version of the go-cart rear axle assembly is now open.

Getting Familiar with the User Interface Now that you have started Autodesk Inventor and set the project file, you will gain familiarity with the user interface. You can move and resize the various aspects of the user interface to your liking.

Menu Bar At the top of the screen is the menu bar (arrow 1), which includes menus and important commands. You may notice that the menu bar is similar to a standard Windows menu. For example, on the File menu you find tools like Open, Save, Print, and Exit. On the View menu, you find tools for model and view orientation like Rotate, Pan, and Zoom.

Standard Toolbar Below the menu bar is the Autodesk Inventor Standard toolbar (arrow 2) containing commonly used icons. You can use the tools on this toolbar to perform common tasks, including Open, Save, Sketch, Return, Rotate, Pan, and Zoom.

Panel Bar The Panel bar (arrow 3) includes specialized design tools that automatically change to reflect the environment in which you are working. The commands change based on whether you are working in Sketch, Part, Assembly mode, etc. When you finish sketching, the Panel bar automatically changes to offer the tools to convert your sketch to a feature.

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The Panel bar offers two modes: Learning and Expert. Learning mode is used by default. It displays the tool icons with descriptions and provides a good introduction to all of the commands. Typically, when using Learning mode, you will need to scroll to find all the commands and tools available to that design environment. Once you become familiar with the icons associated with each tool, you can use the Expert mode to display only the icons. To change the Panel bar to Expert mode, you click the title bar or right-click the Panel bar background and then choose Expert.

The Browser The browser (arrow 4), by default, is located below the Panel bar. The browser displays essential information about your 3D designs. When working with an assembly, the browser displays the hierarchy of the subassemblies and components. When designing a part, the browser shows the features that you have added to the model.

Changing the View Orientation To change to the default isometric view of the go-cart assembly: •

In the graphics window, right-click and choose Isometric View (F6). The view orientation rotates to the default isometric view.

To return to the previous view orientation: •

In the graphics window, right-click and choose Previous View (F5). Tip: You can also use the shortcut key (F5) to return to the previous view orientation.

To magnify your view of the sprocket and right wheel: 1. On the Standard toolbar, click the Zoom Window 2. In the graphics window, click once near the upper-left of the sprocket and then click again near the lowerright of the wheel.

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Your view of the rear axle assembly should be similar to the image shown on the right. The image shows the carrier, sprocket, axle and other components you will create in this hands-on Test Drive.

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Chapter 1: Creating Your First 3D Part

Chapter 1: Creating Your First 3D Part Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 Starting a New Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 Creating Your First Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Adding Dimensions to Your Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Finishing the Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 Creating Your First Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 Creating Another Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 23 Constraining Your Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26 Creating Another Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29 Creating a Pattern . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31

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Chapter 1: Creating Your First 3D Part

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Chapter 1: Creating Your First 3D Part

Chapter 1: Creating Your First 3D Part In This Chapter Your first step in the go-cart design is to create a new 3D component for the rear axle assembly. The part you will design is a carrier for the sprocket. The finished carrier is shown on the right. You will learn the fundamentals of creating 3D solid models— sketching profiles, turning those profiles into solid geometry, and adding features.

The Autodesk Inventor Advantage Improving on 2D drafting tools, the 3D modeling environment of Autodesk Inventor provides a realistic representation of your design. Instead of using lines, arcs, and circles to represent one view of your design, Autodesk Inventor builds a model from a palette of features that describe the shape of your product in 3D. Placing these 3D features is analogous to how manufacturing processes shape and create parts through extruding, milling, turning, or casting (3D features can either add or remove material). These features interact together to define the whole part. In addition, since they each may be modified through dimensional changes or by repositioning, it is easy and intuitive to later make predictable changes to your design. Using Autodesk Inventor for 3D you're able to see your design come to life—allowing you to more easily visualize the solutions to your engineering tasks.

Starting a New Part Create a new part using a standard template: 1. On the Standard toolbar, click New

.

2. In the Open dialog, click the Metric tab and then double-click the Standard (mm).ipt icon to create a new standard part. Note: With Autodesk Inventor, you can create parts independently or in the context of an assembly. For the purposes of this project, design your first part independently.

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Chapter 1: Creating Your First 3D Part

Creating Your First Sketch Begin your part design by creating a sketch of the 2-dimensional profile of what will be the base feature of the carrier part. The first feature of this part is cylindrical, so start by sketching two concentric circles: 1. In the 2D Sketch Panel, click the Center Point Circle

tool.

2. Move the cursor into the sketch area. The cursor becomes a yellow point. 3. Move the cursor over the intersection of the main axes. 4. Click to define the center point of the first circle and then move the cursor to the upper right. As you move the cursor to the right, a dynamic circle displays and the radial value displays in the lower-right corner of the Autodesk Inventor window. 5. Continue moving the cursor to the upper right until the radial value is about 25. 6. Click to create the first circle. The Center Point Circle tool is still active, enabling you to create another circle. Create a second circle, concentric to the first: 1. Move the cursor back to the center of the existing circle. As you move the cursor over the center point of the existing circle, the yellow point turns to green and a coincident symbol displays. 2. Click to define the center point of the second circle and then move the cursor to the upper right.

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Chapter 1: Creating Your First 3D Part

3. Continue moving the cursor to the right until the dynamic circle is slightly larger than the first circle. Click to define the circle. 4. In the graphics window, right-click and choose Done to quit the Center Point Circle tool. You have just created the basic contour of your first sketch. Note: At this point, your sketch can be considered complete. With Autodesk Inventor, you can design conceptually and do not need to fully dimension your sketches.

Adding Dimensions to Your Sketch Next, you fully define the size of your sketch by adding dimensions. Autodesk Inventor provides improvement over AutoCAD dimensioning tools by using a single command to generate many different dimension types. Add dimensions to your sketch: 1. On the Panel bar, scroll down and click the General Dimension

tool.

2. Move the cursor over the edge of the inner circle. A diameter dimension symbol

displays next to the cursor.

Add a diameter dimension: 1. Select the inner circle and move the cursor to the upper right. Click to place the dimension. The value of your dimension will be different. The General Dimension tool remains active, enabling you to continue adding dimensions. 2. Select the edge of the outer circle, move the cursor to the lower right of the first dimension and then click to place the second dimension.

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Chapter 1: Creating Your First 3D Part

Defining Dimension Values Next, modify the dimensions to make them precise values. The dimensions in Autodesk Inventor are more than just text, they are values that drive the size of the geometry. Modify the dimensions: 1. Select the diameter dimension on the inner circle. A dialog displays highlighting the current value of the dimension. 2. Type a value of 50 and click the green check mark on the right of the dialog (or press Enter) to accept that value.

Defining Dimension Values Using Formulas Ensuring proper thickness of the part design requires that you define a dimensional offset between the two circles. With Autodesk Inventor, you can create mathematical relationships between dimensions. Specify the value for the outer diameter dimension: 1. With the General Dimension tool still active, select the diameter dimension on the outer circle. 2. With the value of the dimension highlighted in the Edit Dimension dialog, select the 50 diameter dimension of the inner circle. The parameter d0 displays in the Edit Dimension dialog. 3. Type +20 after the d0 entry so that the value reads d0+20. 4. Click the green check mark to accept this value and close the Edit Dimension dialog.

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Chapter 1: Creating Your First 3D Part

Test the formula for the outer dimension: 1. Select the 50 dimension. 2. In the dialog, type a value of 70 and click the green check mark

to accept that value.

Both circles update to reflect the new values. 3. Press the Esc key to quit the General Dimension tool.

Creating Driven Dimensions Because you are early in the design phase of the carrier part, you will want the ability to change the size of the inner diameter later in the design process. You will change the inner diameter dimension value to be driven. Create a driven dimension to show the diameter of the hub: 1. In the graphics window, click the 70 dimension. 2. With the dimension selected, on the right side of the Standard toolbar, click the Driven Dimension tool to toggle the default dimension style to driven. Because the dimension style is driven, notice you cannot change the value in the dialog.

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Chapter 1: Creating Your First 3D Part

Finishing the Sketch Finish the sketch: 1. Change to an isometric view by right-clicking and choosing Isometric View in the graphics window. 2. In the graphics window, right-click and then choose Finish Sketch. Notice that the grid is no longer displayed because it is needed only during sketching. Also notice on the Panel bar that the sketch commands have been replaced by the 3D part modeling feature tools.

Creating Your First Feature For this portion of the design, use the Extrude tool. 1. On the Panel bar, click the Extrude

tool.

The Extrude dialog displays. 2. In the graphics window, identify the portion of the sketch you want to extrude by selecting the area between the two circles. 3. Click the Centered dialog.

option in the Extrude

A preview of the 3D model displays. 4. Move the cursor to an edge of the preview and drag the extrusion to a slightly larger height. Notice that the value in the Extrude dialog automatically updates. You can also specify an exact distance. 5. In the Extrude dialog, highlight the current distance value, type 40, and click OK to close the dialog and create the extrusion feature.

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Chapter 1: Creating Your First 3D Part

Creating Another Sketch To create another sketch, first define the orientation of the sketch plane. For the flange, use the same plane that you used to define the previous extrusion feature: 1. In the browser, click the plus sign (+) in front of Origin. The names of the principal orientation planes and axes display. 2. In the browser, right-click the name XY Plane and choose New Sketch. Notice that several elements in the browser have a gray background. The browser uses shading to identify active and inactive elements. In this case, Sketch2 is active.

Viewing Normal to the Sketch Plane Before you start to sketch the geometry for the flange, change the orientation of your view to be perpendicular to the sketch plane: 1. On the Standard toolbar, click the Look At

tool.

2. In the graphics window, select the top face of the part.

Changing the Default Sketch Behavior At any time, you can change the default sketching behavior in Autodesk Inventor. Next, you will change the display settings of the grid and specify that you want to edit the value of a dimension when it is created. Change the default 2D sketching behavior: 1. From the Tools menu, choose Application Options. 2. Click the Sketch tab.

23

Chapter 1: Creating Your First 3D Part

3. Clear the Minor Grid Lines and Axes check boxes. 4. Select the Edit dimension when created check box. 5. Click OK to close the Options dialog. Notice that the grid display has changed and the axes are no longer visible on the sketch plane.

Referencing Existing Geometry The flange must maintain a geometric relationship with the existing solid. You can easily use existing geometry by referencing existing dimensions or by projecting geometry onto the current sketch plane. Project the outer circular edge of the solid: 1. On the Panel bar, scroll down and click the Project Geometry 2. In the graphics window, select the outer edge of your 3D part. A circle and centerpoint are created on the sketch plane. This geometry is fully associative to the outer edge of the part. That means this geometry automatically updates when the part edge changes. 3. Right-click in the graphics window and chose Done to quit the Project Geometry tool.

Sketching the Flange Next, sketch a line that defines the shape of the flange: 1. On the Panel bar, click the Line

24

tool.

tool.

Chapter 1: Creating Your First 3D Part

2. In the graphics window, move the cursor to the upper right of the projected edge, as shown in the image on the right. A coincident symbol displays next to the cursor. 3. Click to define the start point of the line.

4. Move the cursor to the right and slightly down, as shown in the image on the right and then click to define the second point of the line While using the Line tool, you can also create arcs. Create an arc that is tangent to the previous line segment: 1. Pause your cursor at the end of the line, then click, hold, and drag the cursor to see a dynamic preview of your arc. Note: To view a Help video on arc creation, right-click in the graphics window and choose How To. In the Show Me dialog, in the Sketch Line section, choose Arcs and then click Tangent. 2. Move the cursor directly below the start point of the arc, as shown on the right and then release the mouse button to create the arc. Continue sketching the final line segment: 1. Move the cursor over the lower right of the projected edge until a coincident symbol the cursor and a tangent symbol the endpoint of the arc.

displays next to displays next to

2. When both symbols display, click to define the endpoint of the final line segment. Note: An additional dotted line may display while sketching this final line segment. Dotted reference lines display when the cursor is aligned with other geometry in the sketch. In this case, the cursor may be vertically aligned with the start point of the first line segment. 3. In the graphics window, right-click and choose Done to quit the Line tool.

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Chapter 1: Creating Your First 3D Part

Constraining Your Sketch Creating Construction Geometry Construction geometry often simplifies the process of constraining a sketch. You will define sketched geometry as construction geometry. Create a horizontal construction line: 1. On the Panel bar, click the Line

tool.

2. On the right side of the Standard toolbar, click the Construction

tool to turn on construction mode.

3. In the graphics window, select the center point of the hub to define the start point of the line. 4. Move the cursor to the right of the arc on the flange. A horizontal symbol displays next to the cursor when the preview of the line is nearly horizontal. 5. With the horizontal symbol displayed, click to define the endpoint of the construction line. A horizontal dashed line is created. Notice the difference in line type and color of the construction line. 6. In the graphics window, right-click and choose Done to quit the Line tool. 7. On the Standard toolbar, click the Construction

tool to turn off construction mode.

Constraining the Flange The center points of the hub and the arc on the flange must be aligned horizontally. You will control this behavior by making the center point of the arc coincident with the horizontal construction line. Align the arc on the flange with the construction line: 1. On the Panel bar, click the down arrow Perpendicular

next to the

tool.

The tools in this list are all the constraint tools. 2. Click the Coincident

tool.

3. Select the center point of the arc and then select the construction line.

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Chapter 1: Creating Your First 3D Part

4. The center point of the arc adjusts to become coincident with the construction line. The two angled lines adjacent to the arc need to be symmetrical about the construction line. To make the two lines symmetrical: 1. On the Panel bar, click the down arrow next to the Coincident tool. 2. Click the Symmetric

tool.

3. Click the top angled line, the bottom angled line and then select the construction line. The two angled lines are now symmetrical about the construction line.

Displaying Existing Constraints At any time while you are sketching, you can display the constraints on your sketch. Display the constraints: 1. On the Panel bar, click the Show Constraints tool. 2. Select the arc. The constraint icons display, showing all the constraints associated with the arc. Highlight the geometry associated with each constraint: 1. Move the cursor over the constraint icons. Both sketch objects associated with that constraint are highlighted in the sketch.

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Chapter 1: Creating Your First 3D Part

2. Click the X to the right of the constraint icons to close the constraints display. 3. Press Esc (or right-click and choose Done) to quit the Show Constraints tool.

Finishing the Sketch with Dimensions Next, finish constraining the size of the sketch by creating dimensions: 1. On the Panel bar, click the General Dimension tool. Note: Ensure the Driven Dimension

tool on the Standard toolbar is not active.

2. Select the arc and place the dimension to the upper right of the arc. Because you changed the default behavior for dimensioning, the Edit Dimension dialog displays, enabling you to define the value. 3. In the dialog, type 6 and then click the green check mark

to accept that value.

Create an angular dimension between the two angled lines: 1. Select the top angled line, select the bottom angled line and then place the dimension between the two lines. 2. In the dialog, type 20 and press Enter to accept that value. The lines update to reflect the new angular value. Define the length of the flange by adding another dimension: 1. Select the center point of the arc, select the center point of the hub, and place the dimension near the bottom of the sketch. 2. In the dialog, with the dimension value highlighted, type 66 and then press Enter to accept that value. 3. Press Esc to quit the General Dimension tool.

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Chapter 1: Creating Your First 3D Part

Creating Another Feature Extruding the Flange The sketch for the flange is now complete. Next, use the Extrude tool to create another feature: 1. Press F6 to display an isometric view. 2. In the graphics window, right-click and choose Finish Sketch. 3. In the Panel bar, click the Extrude

tool.

4. In the graphics window, click inside the sketch geometry defining the flange. 5. In the Extrude dialog, click the Centered

option.

6. Highlight the distance value, type 12 and then click OK to create the second extrusion feature.

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Chapter 1: Creating Your First 3D Part

Zooming and Rotating Now it is time to visually examine your model. In Autodesk Inventor, you can easily do this at any time—even while you are using another tool. View your model: 1. On the Standard toolbar, click the Zoom All

tool.

2. The Zoom All tool adjusts the view of the model so that you can see the entire model onscreen. 3. On the Standard toolbar, click the Rotate

tool.

The Rotate tool displays an Orbit symbol as a circle. 4. Dynamically rotate the model and view it from different directions by moving the cursor inside the Orbit circle and then clicking and holding the left mouse button while moving the cursor. 5. Rotate the model about its vertical or horizontal axis by moving the cursor over the quadrant lines on the perimeter of the Orbit circle and then dragging. 6. Spin the model on an axis perpendicular to your screen by moving the cursor just outside the Orbit circle and then dragging. 7. Redefine the center of rotation by clicking at the point you want to rotate around. 8. Press Esc or right-click and choose Done to quit the Rotate tool. 9. Press F6 or right-click and choose Isometric View to return to the isometric view.

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Chapter 1: Creating Your First 3D Part

Creating a Pattern Create a circular pattern: 1. On the Panel bar, click the Circular Pattern

tool.

The Circular Pattern dialog displays. The Features button is selected, enabling you to identify the features to pattern. 2. In the graphics window, select the flange extrusion (arrow 1). 3. In the Circular Pattern dialog, click the Rotation Axis button. 4. In the graphics window, select the inner face of the hub (arrow 2). A preview of the circular pattern displays. 5. In the Circular Pattern dialog, click OK to create the circular pattern feature. A circular pattern of the flange with six equally spaced occurrences is created.

Saving Your Work Save your design: 1. On the Standard toolbar, click the Save

tool.

2. In the Save As dialog, browse to the folder Chapter 1_Creating Your First 3D Part. 3. In the Save As dialog, type My_Carrier as the file name and then click Save to save your design. 4. From the File menu, click Close.

Chapter Summary Autodesk Inventor software includes a wide range of 3D part modeling tools helping you expedite the design of simple or complex shapes. The part design environment offers a complete set of commands that add or remove material using intuitive workflows, making it the industry’s shortest path to full 3D productivity.

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Chapter 1: Creating Your First 3D Part

32

Chapter 2: Creating a Production Drawing

Chapter 2: Creating a Production Drawing Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Starting a New Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Changing the Default Sheet Size . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 Generating the First View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 36 Creating More Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37 Shading a View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 37 Adding a Section View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 38 Retrieving Model Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39 Adding Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Working with Styles and Layers . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 42

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Chapter 2: Creating a Production Drawing

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Chapter 2: Creating a Production Drawing

Chapter 2: Creating a Production Drawing In This Chapter As opposed to the design and documentation techniques of AutoCAD, where you create the design representation in the drawing environment, Autodesk Inventor creates detailed drawings directly from the geometry of the 3D model. All of the geometry needed to define the part in a 2D view exists in the 3D Model. In this chapter you will create a detailed drawing from the carrier part. You will place multiple drawing views, add dimensions, and experience productivity gains integral to the Autodesk Inventor drawing environment.

The Autodesk Inventor Advantage Simplify the creation of accurate detail drawings using Autodesk Inventor. All 2D entities are generated for you automatically in the desired drawing view from the 3D model. It is quick and easy to generate your drawing views, place dimensions and other annotations. Since the drawing geometry is created directly from the 3D model, you benefit from the security of knowing any changes made to the 3D model will be properly reflected in your drawing. As opposed to complete recreation of the 2D design views, rework from design changes consists of repositioning or adding annotations if needed.

Starting a New Drawing Create a drawing of the carrier part. First, open the carrier part: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 2_Creating a Production Drawing folder and double-click Chapter 2_Carrier.ipt. Create a new drawing of your 3D part: 1. On the Standard toolbar, click the New

tool.

2. In the Open dialog, click the Metric tab, then double-click the ISO.idw

tool.

Autodesk Inventor creates a new A3 size drawing sheet with a frame and title block. Notice that the Panel bar has automatically changed to offer the appropriate drawing tools.

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Chapter 2: Creating a Production Drawing

Changing the Default Sheet Size Next, change the sheet size from A3 to A2: 1. In the browser, right-click Sheet:1 and choose Edit Sheet. 2. In the Edit Sheet dialog, select A2 from the Size drop-down list and click OK.

Generating the First View Create the first view of your 3D part: •

On the Panel bar, click the Base View

tool.

The Drawing View dialog displays, and a preview of the base view is shown at the current cursor location. Create a drawing view of the carrier part: 1. In the Drawing View dialog, ensure the scale is set to 1:1 and the style is set to Hidden Line . 2. Move the cursor to the lower-left side of the drawing sheet and then click to place the view. Tip: If the dialog is in the way, simply drag it by clicking the blue title bar at the top.

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Chapter 2: Creating a Production Drawing

Creating More Views 1. Create a side and isometric view of the part: 2. On the Panel bar, click the Projected View

tool.

3. Select the front view you just created and then click to the right to define the location of the side view. A rectangular preview of the view displays. 4. Move the cursor to the upper right (as shown in the image), and click again to define the location for an isometric view. 5. Right-click and choose Create to finalize these drawing views. Your drawing should now show three different drawing views similar to the image.

Shading a View You can also enhance the appearance of your drawing views by shading the isometric view: 1. Move the cursor over the isometric view (avoid placing the cursor over lines in the view), right-click and choose Edit View. 2. In the Drawing View dialog, click the Shaded tool and then click the Display Options tab. 3. In the upper-right corner, clear the Tangent Edges check box and then click OK.

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Chapter 2: Creating a Production Drawing

Adding a Section View You can also create section views: 1. On the Panel bar, click the Section View

tool.

2. Select the front view (the view in the lower-left corner of the sheet) to identify the parent view. Identify the position of the horizontal section line in the parent view: 1. Move the cursor over the center of the radius of the right-most flange. A green dot displays. 2. Move the cursor to the right of the hole (a dotted line displays as you move the cursor) and then click to define the start point of the section line.

3. Move the cursor to the left side of the front view. When the cursor is outside the left flange and the preview of the line is horizontal, click to define the endpoint of the section line. Tip: When sketching the line, ensure that the horizontal constraint displays next to the line before you click the second point on the line. 4. To finish defining the horizontal section line, right-click in the graphics window and choose Continue. 5. To place the section view, click the location above the front view.

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Chapter 2: Creating a Production Drawing

Note: If the section view does not go completely through the front view, you can correct this by dragging the end of the section line to the left. The section view automatically updates after you adjust the location of the section line.

Retrieving Model Dimensions Because you are designing in 3D you will simply display the dimensions that were used to define the 3D part. Retrieve the model dimensions for a specific drawing view: 1. Move the cursor into the front view (lower-left corner of the drawing sheet), right-click and choose Retrieve Dimensions. 2. In the Retrieve Dimensions dialog, click the Select Parts option and then select any line in the front view. The model dimensions appropriate for the front view of the part display. 3. In the Retrieve Dimensions dialog, click Select Dimensions. 4. To identify the dimensions you want to keep, click and drag a window box selection over all the dimensions in the front view. 5. In the Retrieve Dimensions dialog, click OK. 6. To clean up the dimension display, in the graphics window, click on each dimension and drag to a new location to reposition.

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Chapter 2: Creating a Production Drawing

Adding Dimensions Next, you add baseline dimensions to the section view. Display drawing annotation tools on the Panel bar: •

Click the title bar on the Panel bar and choose Drawing Annotation Panel.

Add baseline dimensions to the section view: 1. Zoom in on the section view. 2. On the Panel bar, click the Baseline Dimension Set tool. 3. In the section view, from bottom to top, select the four horizontal lines shown in the image to the right. 4. Right-click and choose Continue. 5. Click to the right of the view to place the baseline dimensions. 6. In the graphics window, right-click and choose Create to place the dimensions.

Working with Styles and Layers With Autodesk Inventor software, much like AutoCAD, you can control the visibility, color, linetype, and lineweight of objects. First, use the Select Layer tool to control the visibility of objects in your drawing: 1. On the Standard toolbar, click the down-arrow next to the Select Layer drop-down list, as shown in the image. 2. In the list, click the light bulb symbols next to the Hatch (ISO) and Dimension (ISO) entries. The hatch and dimensions are no longer visible in your drawing. 3. Repeat this process to turn the visibility of the hatch and dimensions back on.

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Chapter 2: Creating a Production Drawing

Change the color of the dimensions: 1. On the Standard toolbar, click the Edit Layers

tool.

2. In the Styles and Standards Editor dialog, in the Dimension (ISO) row, click the Color box. 3. In the Color dialog, choose Red and then click OK. The color for the Dimension (ISO) layer is now set to red. Next, create a new layer and move a dimension to that layer. 1. At the bottom of the Layer Styles section of the Styles and Standards Editor dialog, click Click here to add. 2. Type the name My Layer, change the color to Blue, and ensure the linetype is set to Continuous. 3. At the top of the Styles and Standards Editor dialog, click Save and then click Done.

Move a dimension to the new layer: 1. In the graphics window, select the R6 dimension in the lowerleft view. 2. On the Standard toolbar, click the Select Layer drop-down, scroll to the bottom and then choose My Layer. The dimension color changes to the color you defined on your custom layer.

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Chapter 2: Creating a Production Drawing

Saving Your Work Save your production drawing of the carrier part: 1. On the Standard toolbar, click the Zoom All

tool and then click the Save

tool.

2. In the Save As dialog, browse to the Chapter 2_Creating a Production Drawing folder and ensure the file name is Chapter 2_Carrier.idw and then click Save. 3. Close the Chapter 2_Carrier.idw drawing window and then close window.

the Chapter 2_Carrier.ipt part

Chapter Summary Increase accuracy and save time in both creation and modification of your detail drawings with the automatic drawing functions of Autodesk Inventor.

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Chapter 3: Completing the Part Design

Chapter 3: Completing the Part Design Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Opening the Part and Drawing Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Creating Fillets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 45 Calculating Mass Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 Creating Work Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Creating a Work Plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Creating Another Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Creating a Revolve Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Changing Object Visibility . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50 Associative Drawing Updates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 51

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Chapter 3: Completing the Part Design

44

Chapter 3: Completing the Part Design

Chapter 3: Completing the Part Design In This Chapter In this chapter, you will see how to change designs with complete confidence, even after drawings are created. Next, you round the edges of your carrier part by applying fillets to the 3D model. You also calculate the part’s weight and create cuts in the flanges to reduce weight and raw material. Your views are updated automatically when you review the drawing.

The Autodesk Inventor Advantage Quickly create and revise your designs using Autodesk Inventor 3D software. Understand the physical properties of your designs. By monitoring the effects a design change or assembly reconfiguration may have on physical properties such as center-of-gravity, you can make informed, intelligent design decisions and engineer with confidence.

Opening the Part and Drawing Files First, open the carrier 3D part and its corresponding drawing: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 3_Completing the Part Design folder and then double-click Chapter 3_Carrier.idw. 3. On the Standard toolbar, click the Open

tool again.

4. In the Open dialog, browse to the Chapter 3_Completing the Part Design folder and double-click Chapter 3_Carrier.ipt.

Creating Fillets Next, you will create rounds and fillets on the sharp edges of the carrier part. Create the first set of fillets: 1. On the Panel bar, click the Fillet

tool.

Rather than selecting individual edges, you will select multiple edges of a specific type.

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Chapter 3: Completing the Part Design

2. In the Fillet dialog, check the All Rounds check box and then click OK to create the fillet feature. This creates a fillet feature with a default 2 mm radius on all the sharp edges of your part. Create the second set of fillets: 1. Click the Fillet

tool again.

2. In the Fillet dialog, check the All Fillets check box.

3. Highlight the 2 mm radial value and type 3. 4. Click OK to create the second fillet feature. You have created another fillet feature with a 3 mm radius.

Calculating Mass Properties When using Autodesk Inventor for 3D design, at any point in the design cycle, you can calculate your part or assembly’s mass properties—mass, area, volume, center of gravity, and so on. View mass properties: 1. In the Model browser, right-click on Chapter 3_Carrier.ipt and choose iProperties. 2. In the Properties dialog, click the Physical tab to view the mass properties of your part. 3. In the Properties dialog, click to expand the Material list and select Steel from the list. Notice that the physical properties update. 4. Click OK.

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Chapter 3: Completing the Part Design

Creating Work Axes Next, you use the axes and planes work feature to create the proper orientation for the upcoming cut feature. Create a work axis on the hub: 1. On the Panel bar, click the Work Axis

tool.

2. In the graphics window, select the inner face of the hub (arrow 1). You have created the first work axis. Create another work axis on the radius of the flange: 1. Click the Work Axis

tool again.

2. Select the outer radius of the flange extrusion (arrow 2).

Creating a Work Plane Next, create a work plane on the two work axes: 1. On the Panel bar, click the Work Plane tool. 2. In the graphics window, select the two work axes. You have created a work plane that bisects the part on the two work axes.

Creating Another Sketch Create a new sketch on the new work plane: 1. On the Standard toolbar, click the 2D Sketch tool. 2. In the graphics window, click on the work plane you just created.

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Chapter 3: Completing the Part Design

Viewing the Sketch Plane Notice that the grid on the sketch plane interferes with the model. Use the Slice Graphics tool to see the entire sketch plane or to work inside solid models. To use the Slice Graphics tool: •

In the graphics window, right-click and choose Slice Graphics.

Creating a Rectangular Sketch Next create a rectangular sketch by orienting your view normal to the sketch plane: 1. On the Standard toolbar, click the Look At 2. Click the Zoom Window

tool and then select the work plane.

tool (or use the wheel on your mouse) to zoom in on the right side of the part.

Tip: When you use the mouse wheel for zooming, the current cursor location is used as the zoom area target. Create a rectangle: 1. On the Panel bar, click the Two Point Rectangle

tool.

2. At the approximate location shown in the image on the right, click once to define the upper left of the rectangle and then click again to define the lower right of the rectangle. 3. Press Esc to quit the Two Point Rectangle tool. Dimension the rectangle: 1. On the Panel bar, click the General Dimension tool. 2. Select the right vertical edge of the rectangle and place the dimension to the right. 3. In the Edit Dimension dialog, type 8 and press Enter. 4. Select the lower horizontal edge of the rectangle and place the dimension below the rectangle. 5. In the Edit Dimension dialog, type 20 and press Enter.

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Chapter 3: Completing the Part Design

6. Press Esc to quit the General Dimension tool.

Aligning the Sketch with the Part Edges Next, you project the edges of the part to the sketch plane and then use colinear constraints to align the rectangular sketch with the edges of the flange. Project the edge of the flange: 1. On the Panel bar, click the Project Geometry

tool.

2. Select the lower edge of the flange and then select the right (silhouette) edge of the flange. Two lines, representing the edges of the flange, display. 3. Press Esc to quit the Project Geometry tool. Align the rectangle with the projected edges: 1. In the graphics window, right-click, choose Create Constraint and then click the Colinear

tool.

2. Select the right edge of the rectangle and then select the projected right edge of the flange. The rectangular sketch aligns vertically with the projected edge. Finish constraining the rectangle from an isometric view: 1. In the graphics window, rightclick and choose Isometric View (or press F6). 2. With the Colinear tool still active, select the lower edge of the rectangle and then select the projected lower edge of the flange. The rectangular sketch is now fully constrained to the proper location on the flange. 3. Press Esc to quit the Colinear tool.

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Chapter 3: Completing the Part Design

Creating a Revolve Feature Now that you have finished the sketch, you will use the Revolve tool to create the feature. 1. To start the Revolve tool using a keyboard shortcut, press the R key on your keyboard. Because there is only one closed profile in the sketch, the rectangle is automatically selected for you. 2. To define the center axis for the revolution, select the work axis at the center of the hub. 3. In the Revolve dialog, click the Cut option and then click OK to create the Revolve feature.

Changing Object Visibility By now, you have probably noticed that several new items appear in the browser. The model tree in the browser shows each step in the modeling process. See how the elements in the browser are related to the geometry on your part: •

Move the cursor over the elements in the browser. The corresponding part geometry highlights in the graphics window.

Because you no longer need to use the two work axes and the work plane, you can use the browser to turn off their visibility: 1. In the browser, click the plus sign (+) next to Work Plane1 in the browser. 2. Press and hold the Ctrl key, then select Work Plane1, Work Axis1 and Work Axis2. All three items in the browser are highlighted. 3. Right-click one of the highlighted items and then choose Visibility. The work axes and work plane are no longer visible in the graphics window and the feature icons in the browser are grayed.

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Chapter 3: Completing the Part Design

Associative Drawing Updates Next, you will revisit the production drawing of the carrier part. Autodesk Inventor drawings are always in sync with the 3D model. Any change you make to the 3D model associatively updates the drawing geometry. View the carrier drawing: •

From the Window menu, click Chapter 3_Carrier.idw. Note: The features you just created, the fillets and the revolved cut, were automatically updated in the drawing.

Saving Your Work You have completed your design of the carrier. Save your design and drawing: 1. Close

the Chapter 3_Carrier.idw drawing window.

2. When prompted to save changes to your model and its dependents, click Yes. 3. Close

the Chapter 3_Carrier.ipt part window.

Chapter Summary Improve every aspect of your design before it is built, reducing manufacturing costs and decreasing time to market using Autodesk Inventor for 3D design.

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Chapter 3: Completing the Part Design

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Chapter 4: Using AutoCAD Data

Chapter 4: Using AutoCAD Data Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Creating a 3D Part Using AutoCAD Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Importing AutoCAD Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Using Imported Geometry to Create a Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58 Creating a Feature Using a Shared Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59 Creating Another Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60 Importing More AutoCAD Data . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61 Rotating and Aligning DWG Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 64 Finishing the Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65 Creating a Revolve Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

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Chapter 4: Using AutoCAD Data

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Chapter 4: Using AutoCAD Data

Chapter 4: Using AutoCAD Data In This Chapter In this chapter, you will create a new part using AutoCAD geometry as the basis for the design. You create a 3D bearing housing for the rear axle. The finished 3D bearing housing is shown on the right. Autodesk Inventor gives you the ability to import AutoCAD geometry in two different ways—you can simply copy and paste from AutoCAD or you can use the import utility. Both methods are described below—you may choose which workflow to follow. If you have AutoCAD installed on your computer it is suggested you follow the Workflow Option 1: Using the Copy and Paste from AutoCAD Import Method. If you do not have AutoCAD on your computer please follow the Workflow Option 2: Using the Autodesk Inventor Import DWG Import Method.

The Autodesk Inventor Advantage Autodesk Inventor makes it easy to re-use existing DWG data, capturing geometry and converting dimensions to enable part modification, providing you with the best possible workflow for maximizing the value of your AutoCAD data. Autodesk Inventor allows valuable, proven designs created in AutoCAD to be incorporated into new 3D designs or continue to be available in 2D—giving you the right tool for the job and allowing you to move to 3D at your own pace.

Creating a 3D Part Using AutoCAD Data To create a new part using a standard template: 1. On the Standard toolbar, click New

.

2. In the Open dialog, click the Metric tab and then double-click Standard (mm).ipt

.

Importing AutoCAD Data If you have AutoCAD installed on your computer, we suggest you follow the Workflow Option 1: Using the Copy and Paste from AutoCAD Import Method. If you do not have AutoCAD on your computer, please follow the Workflow Option 2: Using the Autodesk Inventor Import DWG Method.

Workflow Option 1: Using the Copy and Paste from AutoCAD Import Method To complete this workflow you use both Autodesk Inventor and AutoCAD applications. If you do not have a version of AutoCAD or AutoCAD Mechanical installed on your computer, proceed to Workflow Option 2. Keep the Autodesk Inventor application running, but minimize the application while you work in AutoCAD.

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Chapter 4: Using AutoCAD Data

•

In the upper right-hand corner of the Autodesk Inventor window, click the Minimize

tool.

If you have AutoCAD on your computer: 1. Start AutoCAD. 2. In AutoCAD, from the File menu, click Open. 3. In AutoCAD, in the Select File dialog, browse to the Chapter 4_Using AutoCAD Data folder (default was C:\Inventor_R11_TestDrive\Workspace\) and then choose the file Chapter 4_Axle_Bearing.dwg and then click Open.

Copying the AutoCAD Data to Import 1. In AutoCAD, turn off the Dimension, Hatch, Hidden, Hidden Narrow, Section Line, Sketch Geometry, and Symbol layers. 2. In the AutoCAD graphics window, select the outer square profile of the part (arrow 1), the triangular edges (arrow 2), the four small holes in each corner (arrows 3, 4, 5, 6), and the smallest circle at the center of the part (arrow 7). 3. In the AutoCAD graphics window, right-click and choose Copy. The AutoCAD geometry is placed on your clipboard. 4. To minimize your AutoCAD application, in the upper right-hand corner of the AutoCAD window, click the Minimize tool.

Pasting the AutoCAD Data into Autodesk Inventor 1. Maximize the Autodesk Inventor application window. 2. In the Autodesk Inventor graphics window, right-click and choose Paste. A dotted blue rectangle displays. 3. In the Autodesk Inventor graphics window, rightclick and choose Paste Options. 4. In the Paste Options dialog, click Specify Units and ensure the value is set to mm.

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5. In the Paste Options dialog, verify that Constrain End Points is checked. 6. Click OK. 7. In the graphics window, click to paste the AutoCAD data. 8. On the Standard Toolbar, click the Zoom All

tool.

You have just copied and pasted AutoCAD data directly into your Autodesk Inventor sketch. Proceed to the Using the Imported Geometry to Create Features section.

Workflow Option 2: Using the Autodesk Inventor DWG Import Method To use Autodesk Inventor sketch environment’s Insert AutoCAD file tool, please follow the steps below: 1. On the Panel bar, click the Insert AutoCAD File

tool.

2. In the Open dialog, browse to the Chapter 4_Using Autocad Data folder, choose Chapter 4_Axle Bearing.dwg and then click Open. The Layers and Objects Import Options dialog displays.

Using the DWG Import Tool Next, you identify the layers or geometry you want to import. Although you can import the entire drawing, you may import only the contents you need. Import content: 1. In the upper right-hand corner of the Layers and Objects Import Options dialog, click the White Background

tool.

2. In the Selective import area, clear the check boxes for all layers including and between Dimension and Symbol. Tip: You can use the Shift key to select all items between these two layers and then click the check box once to clear all the check boxes. Notice as you select or deselect the layers that the preview window dynamically updates.

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3. In the Selection area, clear the All check box. This enables you to select geometry in the Import Preview window. 4. In the Import Files Units area, ensure Specify Units is selected and set to mm. 5. Verify that Constrain End Points is checked. 6. In the Import Preview window, drag a rectangle around all the geometry in the right-hand view, as shown in the image. Note: To zoom and pan inside the Import Preview window, you can use the wheel mouse or rightclick in the Import Preview window and choose the Zoom and Pan commands. 7. In the Import Preview window, select the outer square profile of the part (arrow 1), the triangular edges (arrow 2), the four small holes in each corner (arrows 3, 4, 5, 6), and the smallest circle at the center of the part (arrow 7). Tip: If you select the wrong geometry, press and hold the Shift key and reselect the geometry to remove it from the selection set. 8. Click Finish. The geometry you selected is imported as sketch geometry for your part.

Using Imported Geometry to Create a Feature You need to have completed either Workflow 1 or Workflow 2 at this point. Next, you use the imported geometry to create the base of the bearing housing. The base will be created using two extrusion features. 1. In the graphics window, right-click and choose Finish Sketch.

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2. To display an isometric view, press F6. 3. On the Panel bar, click the Extrude

tool.

4. To identify the profile to extrude, select just outside the large center circle (arrow 1) and then select the four triangular shapes near each edge (arrows 2-5). Autodesk Inventor enables you to select multiple separate regions to extrude. 5. In the Extrude dialog, for the distance value, type 6 mm. 6. Click OK to create the first extrusion feature.

Creating a Feature Using a Shared Sketch To finish the base of the bearing housing, you will create another extrusion by reusing the imported AutoCAD geometry. 1. Near the bottom of the Model browser, click the plus sign (+) next to Extrusion1. 2. Right-click on Sketch1 and choose Share Sketch. The imported sketch geometry displays in the graphics window. Create the second extrusion feature for the base: 1. On the Panel bar, click the Extrude

tool.

2. To define the profile to extrude, in the graphics window, select the area just outside the center hole on the base. 3. In the Extrusion dialog, for the distance value, type 10 mm.

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4. Click OK to create the second extrusion defining the shape of the base. 5. In the browser, right-click Sketch1 (just above the Extrusion1 feature), and choose Visibility to turn off the visibility of the shared sketch.

Creating Another Sketch Next, you create a new sketch for the revolve feature.

Creating a Work Plane You create a work plane at the center of the part that will be used to orient the sketch for the revolve feature. 1. On the Panel bar, click the Work Plane

tool.

2. In the graphics window, right-click and choose Create Axis. Then select the face of the large hole at the center of the part, as shown on the right (arrow 1). 3. Select the right planar face of the part, as shown on the right (arrow 2). 4. In the Angle dialog, type 0 (zero) and press Enter.

A work plane is created parallel with the side face and centered in the hole. In the browser, notice the work axis is nested under the work plane.

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Creating the Sketch 1. In the graphics window, right-click the new work plane you just created and choose New Sketch. 2. Press the F7 key to slice the graphics. 3. On the Standard toolbar, click the Look At tool and then select the work plane.

Creating Reference Geometry Next, you project the right edge of the part and then create a point that is later used to orient the imported sketch geometry for the revolution feature. 1. On the Panel bar, click the Project Geometry

tool.

2. In the graphics window, select the bottom, horizontal edge of the part. 3. In the graphics window, right-click and choose Done. 4. On the Panel bar, click the Point, Center Point

tool.

5. Move the cursor near the center of the projected line, and when a green dot is displayed on the line, click to place the point. 6. In the graphics window, right-click and choose Done.

Importing More AutoCAD Data If you have AutoCAD installed on your computer, we suggest you follow the Workflow Option 1: Using the Copy and Paste from AutoCAD Import Method. If you do not have AutoCAD on your computer, please follow the Workflow Option 2: Using the Autodesk Inventor Import DWG Method.

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Workflow Option 1: Using the Cut and Paste from AutoCAD Import Method To complete this workflow you will use both the Autodesk Inventor and AutoCAD applications. If you do not have a version of AutoCAD or AutoCAD Mechanical installed on your computer, proceed to Workflow Option 2. Keep the Autodesk Inventor application running, but minimize the application while you work in AutoCAD. •

In the upper right-hand corner of the Autodesk Inventor window, click the Minimize

tool.

Copying the AutoCAD Objects to Import To copy AutoCAD geometry: 1. Maximize the AutoCAD application window. Note: The Dimension, Hatch, Hidden, Hidden Narrow, Section Line, Sketch Geometry, and Symbol layers should already be turned off. 2. In the AutoCAD graphics window, drag a rectangle around all of the geometry in the right-hand view as shown in the image. 3. In the AutoCAD graphics window, right-click and choose Copy. The AutoCAD geometry has been placed on your clipboard. 4. Minimize the AutoCAD application by clicking the Minimize tool in the upper right-hand corner of the AutoCAD window.

Pasting the AutoCAD Data into Autodesk Inventor 1. Maximize the Autodesk Inventor application window. 2. In the Autodesk Inventor graphics window, right-click and choose Paste. A dotted blue rectangle will appear. 3. In the Autodesk Inventor graphics window, right-click and choose Paste Options. 4. In the Paste Options dialog, click Specify Units and ensure the value is set to mm. 5. In the Paste Options dialog, verify that Constrain End Points is checked.

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6. Click OK. 7. In the graphics window, click to paste the AutoCAD data beneath the existing geometry. You have just copied and pasted AutoCAD data into your Autodesk Inventor sketch. Proceed to the Rotating and Aligning the Geometry section.

Workflow Option 2: Using the Autodesk Inventor DWG Import Method Follow the steps below to use the Autodesk Inventor sketch environment’s Insert AutoCAD file tool. 1. On the Panel bar, click the Insert AutoCAD File

tool.

2. In the Open dialog, browse to the Chapter 4_Using AutoCAD Data folder, select Chapter 4_Axle_Bearing.dwg and then click Open. The Layers and Objects Import Options dialog displays.

Using the DWG Import Tool 1. In the upper right-hand corner of the Layers and Objects Import Options dialog, click the White Background

tool.

2. In the Selective import area, clear the check boxes for all layers including and between Dimension and Symbol. 3. In the Selection area, clear the All check box. 4. In the Import Files Units area, ensure Specify Units is selected and set to mm. 5. Verify that Constrain End Points is checked. 6. In the Import Preview window, drag a rectangle around all the geometry in the right-hand view. 7. Click Finish.

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Moving Imported Geometry 1. In the graphics window, drag a rectangle around the geometry you just imported. 2. With the geometry highlighted, click on the geometry and drag the geometry just below the part as shown in the image on the right (the placement location is only approximate).

Rotating and Aligning DWG Geometry You need to have completed either Workflow 1 or Workflow 2 at this point. Next, you rotate and align the sketch geometry with respect to the reference geometry of the 3D part. 1. On the Panel bar, click the Rotate

tool.

2. Ensure all the geometry is selected, and then, in the Rotate dialog, click Center Point and then select any point along the centerline of the sketch geometry. 3. In the Rotate dialog, enter an Angle value of 180. 4. Click Apply to rotate the geometry. 5. Click Done to close the Rotate dialog. Align the geometry: 1. On the Panel bar, click the Move

64

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Chapter 4: Using AutoCAD Data

2. Ensure all the geometry is selected and then click the Move From tool and select the point shown in the image to the right (arrow 1). In the Move dialog, the Move To automatically selected.

tool is

3. To identify the location to move to, select the Point, Center Point you placed on the bottom midpoint of the part (arrow 2). 4. Click Apply to move the geometry.

5. Click Done to close the Move dialog. The imported sketch geometry is now aligned at the proper location on the 3D part.

Finishing the Sketch 1. In the graphics window, right-click and select Finish Sketch. 2. Press F6 to rotate to an isometric view.

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Creating a Revolve Feature To finish the design of the bearing housing, create a revolve feature: 1. On the Panel bar, click the Revolve

tool.

2. Select the profile shown on the right (arrow 1). 3. In the Revolve dialog, click Axis and in the browser, expand Work Plane 1 and then select Work Axis 1. 4. Click OK to create the Revolve feature.

Saving Your Work Turn off the visibility of the work plane and save your work: 1. In the Model browser, right-click Work Plane1 and choose Visibility. 2. On the Standard toolbar, click the Save

tool.

3. In the Save As dialog, browse to the Chapter 4_Using AutoCAD Data folder and type My_Bearing. 4. Click Save. 5. From the File menu, click Close.

Chapter Summary Autodesk Inventor provides you with the best functionality for leveraging your investment in AutoCAD designs. You can use your existing AutoCAD data with Autodesk Inventor, while continuing to accurately collaborate with AutoCAD users, suppliers, and customers.

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Chapter 5: Assembly Basics – Creating & Assembling Components

Chapter 5: Assembly Basics – Creating & Assembling Components Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69 Opening the Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69 Adding Parts to an Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69 Adding Assembly Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 70 Mirroring in an Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71 Working with a Subassembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 72 Using the Shaft Generator Tool . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 73 Running an Interference Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78 Making a Design Change Using Grip Editing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79 Adding Components to a Subassembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81 Creating an Adaptive Link between Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 84 Creating a Keyway . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86 Creating a Bolted Connection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91

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Chapter 5: Assembly Basics – Creating & Assembling Components

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Chapter 5: Assembly Basics – Creating & Assembling Components

Chapter 5: Assembly Basics – Creating & Assembling Components In This Chapter So far, you have been learning about creating and documenting individual parts. Next, you will combine components into the go-cart assembly and learn the fundamentals of assembly modeling. You will add the bearing housing into the assembly. In addition, you will learn how the functional design technology of Autodesk Inventor simplifies selecting engineering components and streamlines adding shafts, keyways, bolted connections, and other devices to your designs.

The Autodesk Inventor Advantage Functional Design delivers context-sensitive design elements that understand the tasks for which they will be used. They take design requirements as their input and use built-in design rules to deliver components that satisfy the given requirements, elevating the 3D design process from mere geometric description. The Design Accelerator functionality in Autodesk Inventor allows you to automate the process of creating common mechanical components and assemblies based on real-world attributes such as speed, power, and material properties. Move beyond 2D drafting and 3D modeling to create designs in terms of mechanical requirements, rather than geometric descriptions and constraints.

Opening the Assembly Open the go-cart assembly: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 5_Assembly Basics folder and double-click Chapter 5_Go_Cart.iam.

Adding Parts to an Assembly Next, you add the bearing housing to your assembly. 1. Press F6 to view the go cart in an isometric view.

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Chapter 5: Assembly Basics – Creating & Assembling Components

2. Zoom in to the back left section of the assembly as shown. Add a component to the assembly: 1. On the Assembly Panel bar, click the Place Component

tool.

2. In the Open dialog, choose Chapter 5_Bearing.ipt and then click Open. A preview of the part is positioned at the cursor location. 3. Move the cursor slightly below the axle mount and click to place one occurrence of the bearing. 4. In the graphics window, right-click and choose Done.

Adding Assembly Constraints Create constraints to define the location of the bearing housing within the context of the assembly: 1. On the Panel bar, click the Constraint

tool.

2. In the Place Constraint dialog, click the Insert

option.

3. On the axle mount plate of the chassis frame, select the inner edge of the center hole, as shown (arrow 1).

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4. Use the Rotate

tool to view the opposite side of the bearing housing. Press Esc to quit the Rotate tool.

5. Select the circular edge of the bearing housing, with the arrow facing outward as shown (arrow 2). 6. Click Apply to create the constraint.

Fully constrain the component by adding an angle constraint: 1. In the Place Constraint dialog, click the Angle tool. 2. For the first selection, click the top face of the bearing. 3. For the second selection, click the top face of the axle mount as shown. Note: You may need to use the Select Other tool to select the correct face. 4. In the Angle section of the Place Constraint dialog, type a value of 0. 5. Click Apply to create the constraint. 6. Click Cancel to close the Place Constraint dialog.

Mirroring in an Assembly Next, you will mirror the bearing housing to the opposite side of the chassis frame. 1. On the Panel bar, click the Mirror Components tool. 2. Select the bearing housing to identify the part to mirror (arrow 1). 3. In the Mirror Components dialog, click Mirror Plane.

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4. In the browser, choose Work Plane7 (arrow 2). 5. In the graphics window, zoom out and rotate for a better view of the entire rear axle. A preview of the mirrored part displays. 6. In the Mirror Components dialog, click the green icon Chapter 5_Bearing:1.

to the left of

The green mirror icon changes to a yellow plus (+) icon . Tip: The yellow plus (+) icon signifies that another instance of the part will be placed, rather than actually mirroring the part. Because there is no physical difference between the left and right versions, you can simply place another instance. 7. Click Next.

8. In the Mirror Components: File Names dialog, click OK.

Working with a Subassembly Next, you will create the shaft of the rear axle. You will create the new shaft as part of the Rear Axle subassembly. The Design Accelerator functionality of Autodesk Inventor guides you through the creation of common engineering components. Work in the context of the Rear Axle subassembly: •

In the browser, double-click Rear Axle Assy:1. Note: The components of the active subassembly remain visible while the rest of the assembly components gray out.

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Using the Shaft Generator Tool Create a shaft: 1. Click the Assembly Panel drop down list and select Design Accelerator. Note: The tool pallet changes. 2. In the Design Accelerator Panel bar, click the Shaft

tool.

3. In the upper right-hand corner of the dialog, set Standards to ISO (arrow 1) and then click Yes to confirm. For the first element of the shaft: 1. In the Shaft Component Generator dialog, click the No Groove tab as the element type (arrow 2). 2. In the Current Element Parameters section of the Shaft Component Generator dialog (arrow 3), do the following: • Type 40 for Diameter. •

Type 400 for Length.

•

Click the left-hand chamfer tab (arrow 4) and type 2 for size.

•

To switch to the next section of the shaft, change Active Part to 2.

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For the second element of the shaft: 1. In the Shaft Component Generator dialog, click the Cone tab as the element type (arrow 1). 2. In the Current Element Parameters section of the Shaft Component Generator dialog, do the following (arrow 2): • Type 40 for Diameter. •

Type 75 for Length.

•

In the Cone section of the dialog, type 60 for Second Cone Diam (arrow 3).

•

To switch to the next section of the shaft, change Active Part to 3.

For the third element of the shaft: 1. In the Shaft Component Generator dialog, click the No Groove tab as the element type (arrow 1). 2. In the Current Element Parameters section of Shaft Component Generator dialog, do the following (arrow 2): • Type 60 for Diameter.

74

•

Type 300 for Length.

•

To switch to the next section of the shaft, change Active Part to 4.

Chapter 5: Assembly Basics – Creating & Assembling Components

For the fourth element of the shaft: 1. In the Shaft Component Generator dialog, click the Cone tab as the element type (arrow 1). 2. In the Current Element Parameters section of Shaft Component Generator dialog, do the following (arrow 2): • Type 60 for Diameter. •

Type 75 for Length.

3. In the Cone section of the dialog, type 40 for Second Cone Diam (arrow 3). 4. To switch to the next section of the shaft, in the Current Element Parameters section, change Active Part to 5. For the fifth element of the shaft: 1. In the Shaft Component Generator dialog, click the No Groove tab as the element type as shown on the right. 2. In the Current Element Parameters section of Shaft Component Generator dialog, do the following: • Type 40 for Diameter. •

Type 400 for Length.

•

Click the right-hand chamfer tab (arrow 3) and then type 2 for size.

•

To switch to the next section of the shaft, change Active Part to 6.

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Remove the sixth element of the shaft: •

At the bottom of the Current Element Parameters section, click Remove (arrow 1). The Total length of your shaft should equal 1250 mm, as shown in the dialog near the right-hand side of the shaft image (arrow 2).

Add an internal hole to the shaft: 1. Click the Outer Shaft Shoulder 1).

tool (arrow

2. In the Inner Hole Parameter section of the dialog, click the Insert to Left tool (arrow 2). 3. In the Inner Hole Parameter section of the dialog, do the following (arrow 3) • Type 25 for Diameter. •

Type 1250 for Length.

4. Click OK to complete the shaft creation.

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Place the shaft into the rear axle subassembly: •

A preview of the part is positioned at the location of the cursor. Note: Zoom and rotate your model as necessary to complete placing the shaft near the right wheel.

1. Move the cursor to the right of the wheel and click to place one occurrence of the shaft. 2. In the graphics window, right-click and choose Done.

Constrain the shaft in place: 1. Type C on your keyboard to activate the Constraint tool. 2. In the Place Constraint dialog, click the Insert tool. Note: Zoom and rotate your model as necessary to complete the constraint selections. 3. For Selection 1, click the end of the shaft as shown (arrow 1). 4. For Selection 2, click the inner diameter of the wheel rim as shown (arrow 2). A preview of the shaft’s placement displays in the graphics window. 5. If your shaft did not insert in the correct direction, in the Solution section of the Place Constraint dialog, click the Aligned

tool.

6. Click OK to close the dialog.

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Running an Interference Analysis Next, you will check if the newly created shaft causes any interference with the rear axle assembly. Because your solid models understands their size and location, you can automatically check your assemblies for interferences. Check for interference: 1. On the Standard toolbar click the Return tool to focus your work at the main assembly level. 2. Zoom and rotate your assembly so that it is oriented similarly to the image shown. 3. From the Tools menu, click Analyze Interference. In the Interference Analysis dialog, Define Set #1 is automatically selected. Add components to Set #1: 1. Click the left instance of the Axle Mount component (arrow 1). 2. Then click the Chapter 5_Bearing component (arrow 2). 3. Then click the right instance of the Axle Mount component (arrow 3). 4. In the Interference Analysis dialog, click the Define Set #2 tool.

5. To add components to Set #2: Click the Shaft component (arrow 4). 6. Click OK.

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An Interference Detected dialog displays stating the volume of the detected interference. The graphics window graphically displays in red the interference volume between the involved components. 1. In the Interference Detected dialog, click >> to display information about the components that interfere. 2. In the Interference Detected dialog, click OK.

Making a Design Change Using Grip Editing To remove the interference between the shaft and the Axle Mount components, you will make a design change to the Axle Mount component. You will increase the size of the hole in the center of the Axle Mount. Edit the Axle Mount component: •

In the graphics window, double-click the left instance of the Axle Mount component.

All assembly components other than the Axle Mount should be dimmed. If not, change the component opacity setting: •

On the Standard toolbar, click the Component Opacity Off

tool and select the

Component Opacity On

tool instead.

Edit the diameter of the hole in the center of the Axle Mount: 1. On the Standard toolbar, click the Select tool and select the Feature Priority tool.

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2. In the graphics window, click the hole in the center of the Axle Mount (arrow 1). 3. In the graphics window, right-click and choose 3D Grips. A set of grip handles displays on the circular feature.

4. In the graphics window, pause your cursor over the circular grip at the top edge of the circle (arrow 2). A yellow arrow displays. Drag the size of the circle bigger: 1. Pause your cursor over the yellow grip arrow until it turns red, indicating it is selected. 2. With the arrow selected, click and drag your cursor upward to make the circle larger. Note: The radius value changes as you move the grip arrow. You can use 3D grips to edit dimensions of many features in Autodesk Inventor. Change the radius dimension value: 1. Pause your cursor over the yellow grip arrow until it turns red, indicating it is selected. 2. With the arrow selected, right-click and choose Edit Radius. 3. In the Edit Radius dialog, type 25 and then press Enter. 4. In the graphics window, right-click and choose Done. 5. To return your focus to the top level assembly, on the Standard toolbar, click Return

.

Note: Notice that the diameter change is reflected in all three of the Axle Mount instances that are in the assembly.

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Adding Components to a Subassembly The next step in your design is to add the carrier part you designed in the beginning of the test drive to the Rear Axle subassembly. You will constrain the carrier into place and modify its size to ensure proper fit in your design. Work in the context of the Rear Axle subassembly: 1. In the graphics window, double-click the shaft component. Because the shaft is part of the Rear Axle subassembly, all components other than those of the Rear Axle subassembly should be grayed out. If not, change the component opacity setting: •

In the Standard toolbar, click the Component Opacity Off Opacity On

tool and select the Component

tool instead.

Add the carrier part to your subassembly: 1. On the Assembly Panel bar, click the Place Component

tool.

2. In the Open dialog, browse to the Chapter 5_Assembly Basics folder and double-click Chapter 5_Carrier.ipt. A preview of the part is positioned at the cursor location. 3. Move the cursor slightly above the shaft and click to place one occurrence of the carrier. 4. In the graphics window, right-click and choose Done.

Define the location of the carrier within the context of the subassembly by adding constraints. Align the center axis of the carrier with the center axis of the shaft:

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1. On the Panel bar, click the Constraint

tool.

In the Place Constraint dialog, the Mate constraint is automatically selected. 2. For Selection 1, click the inner diameter of the carrier (arrow 1). 3. For Selection 2, click the shaft (arrow 2). 4. In the Place Constraint dialog, ensure the Offset value is 0. 0. 5. Click Apply to create the constraint. 6. Click Cancel to close the Place Constraint dialog.

By creating constraints you define and limit the degrees of freedom of your components. Graphically see that the carrier is constrained to the axis of the shaft: 1. In the graphics window, position your cursor on the carrier and click and drag your cursor horizontally back and forth to see the carrier move along the axis of the shaft. 2. Place the carrier in the position shown.

Next, you create an orientation constraint between the carrier and the shaft so the two components will always rotate together.

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Create the constraint: 1. On the Panel bar, click the Constraint

tool.

In the Place Constraint dialog, the Mate constraint is automatically selected. 2. For Selection 1, in the Model browser, click the plus sign (+) next to Chapter 5_Carrier:1 to expand the list of features. 3. Click the plus sign (+) next to Origin and then click YZ Plane (arrow 1). 4. For Selection 2, in the Model browser, click the plus sign (+) next to Shaft:1 to expand the list of features. 5. Click the plus sign (+) next to Origin and then click YZ Plane (arrow 2). 6. In the Place Constraint dialog, ensure the Offset value is 0. 0. 7. Click Apply to create the constraint. Next, you will create an insert constraint between the carrier and the sprocket. 1. In the Place Constraint dialog, click the Insert

option.

2. For Selection 1, click the gold-colored small hole on the sprocket. 3. For Selection 2, click the outer radius on one of the arms of the carrier (arrow 2). 4. In the Place Constraint dialog, ensure the Offset value is 0. 0. 5. Click Apply to create the constraint. 6. Click Cancel to close the Place Constraint dialog.

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Graphically see that the carrier is constrained to the sprocket: •

In the graphics window, position your cursor on the carrier and then click and drag your cursor vertically up and down to see the carrier and sprocket rotate around the shaft.

Creating an Adaptive Link between Parts Next, you will use the Adaptive functionality of Autodesk Inventor to ensure the diameter of your carrier part always fits the diameter of the rear axle shaft. You will define the inner diameter of your carrier so it is allowed to adjust in size—be adaptive—to other geometry. You will then link the inner diameter of the carrier to always be slightly larger than the diameter of the shaft. Define the diameter of the carrier to be adaptive: 1. In the Model browser, double-click Chapter 5_Carrier:1 to focus your edits on the carrier part (arrow 1). 2. In the Model browser, under Chapter 5_Carrier:1, on Extrusion1 (arrow 2), right-click and choose Adaptive. Note: An adaptive indicator names in the browser.

displays next to the feature and part

Return to editing the Rear Axle subassembly: •

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Create an adaptive link between the inner diameter of the carrier and the outer diameter of the shaft: 1. On the Panel bar, click the Constraint

tool.

In the Place Constraint dialog, the Mate constraint is automatically selected. 2. For Selection 1, pause your cursor over the inner diameter of the carrier and wait until the Select Other tool displays. Click the arrow once to highlight the inner face of the carrier. Click the center green circle of the Select Other tool to accept the inner face selection. IMPORTANT: Ensure you select the inner diameter FACE, not the face/axis combination. The carrier axis should NOT be displayed when you make your selection. 3. For Selection 2, click the shaft. 4. In the Place Constraint dialog, type 2 for the Offset value. 5. Click Apply to create the constraint. 6. Click Cancel to close the Place Constraint dialog. You have fully constrained the carrier part to the Rear Axle subassembly. The diameter of the carrier has become 2 mm larger than the shaft.

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Creating a Keyway Next, you will create a keyway in the shaft and carrier using the Design Accelerator functionality of Autodesk Inventor. Work in the context of the Rear Axle subassembly: •

In the browser, double-click Rear Axle Assy:1. Note: The components of the active subassembly remain visible while the rest of the assembly components gray out.

You will turn off the visibility of the wheel components to more easily create the keyway on the shaft and carrier components. Turn off the visibility of the wheel components: 1. In the graphics window, position your cursor over the right tire, right-click, and choose Visibility. The wheel components are no longer visible.

2. Zoom and rotate your model so you view the right end of the shaft—a position similar to the one shown.

Create a keyway: 1. Click the Assembly Panel drop down list and select Design Accelerator from the list. 2. In the Design Accelerator Panel bar, click the arrow and click the Key Connection

next to the Shaft

tool.

Note: You may experience a delay while the Content Center database loads.

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3. In the Parallel Key Connection Generator dialog, in the Shaft Groove section, Reference 1 is automatically selected. In the graphics window click the outer face of the shaft (arrow 1). 4. In the Shaft Groove section, for Reference 2, in the graphics window click the end face of the shaft (arrow 2).

5. In the Hub Groove section, for Reference 1, in the graphics window, click the flat, vertical face on the end of the carrier (arrow 3). 6. In the Hub Groove section, for Reference 2, in the graphics window, click the inner diameter of the carrier (arrow 4). Change the location of the shaft keyway: 1. In the graphics window, click the right-most grip arrow on the shaft keyway preview.

2. Click and drag the cursor horizontally along the shaft until the shaft keyway is in line with the carrier. The tooltip should display approximately 180 mm.

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Increase the length of the keyway: 3. Click and drag the left-most grip arrow until the tooltip displays 63.000 mm.

4. To complete the creation of the keyway, in the Parallel Key Connection Generator dialog, click OK.

Creating a Bolted Connection Next, you will create a bolted connection between the carrier and the sprocket parts using the Design Accelerator functionality of Autodesk Inventor. Ensure you are working in the context of the Rear Axle subassembly: 1. In the browser, double-click Rear Axle Assy:1. 2. Zoom and rotate your model to a position similar to the one shown. On the sprocket part, position the gold colored hole to be visible.

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Create a bolted connection: 1. In the Design Accelerator Panel bar, click the Bolted Connection

tool.

2. In the Bolted Connection Component Generator dialog, in the Placement section, ensure By hole is the selected placement type. 3. In the Bolted Connection Component Generator dialog, in the Placement section, Start Plane should be automatically selected. If not, click the Start Plane tool. 4. To select the start plane, in the graphics window, click on the sprocket face (arrow 1). 5. In the dialog, in the Placement section, Existing Hole should be automatically selected. If not, click the Existing Hole

tool.

6. To select the existing hole, in the graphics window, click on the inner diameter face of the gold-colored hole (arrow 2). 7. In the dialog, click the Follow pattern check box. 8. In the dialog, in the Placement section, click the Termination tool

.

9. To select the termination plane, in the graphics window, select the back face of the carrier part (arrow 3).

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10. In the dialog, at the top of the fasteners and holes list, click the Click to add a fastener tool. Note: You may experience a delay while the Content Center database loads.

11. Ensure the Standard is set to ISO and then click the ISO 4762 fastener, as shown on the right.

12. In the dialog, click OK to create the pattern of bolted connections.

Saving Your Work Turn the visibility of the Rear Wheel Assembly back on: 1. In the Model browser, right-click on Rear Wheel Assy:2 and choose Visibility. 2. On the Standard toolbar click the Return

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3. Press F6 to return to an isometric view. 4. Close the Chapter 5_Go_Cart.iam window. 5. When prompted to save changes and dependents, click Yes.

Chapter Summary Designing with Autodesk Inventor means you take advantage of a 3D model to create a virtual prototype. Improve your designs while using the time-saving functionality in Autodesk Inventor for finding and incorporating standard content into your 3D designs. Replacing physical prototypes with virtual ones allows you to bring products to market faster.

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Chapter 6: Assembly Documentation

Chapter 6: Assembly Documentation Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Creating an Assembly Presentation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 95 Illustrating Assembly Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96 Animating Assembly Steps . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 98 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 98 Starting a New Assembly Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 98 Changing the Default Sheet Size . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Generating the First View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Creating Another View of the Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99 Creating a Detail View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 Creating a Broken View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101 Adding Balloons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102 Creating a Parts List . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103 Printing and Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104

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Chapter 6: Assembly Documentation In This Chapter Now you will see how you can use Autodesk Inventor 3D assemblies to complete your product documentation. You will create a technical illustration and assembly instruction video. You will create a detailed assembly drawing using the annotation abilities of Autodesk Inventor, and automatically create an accurate parts list using the information of the 3D assembly.

The Autodesk Inventor Advantage Significantly increase the accuracy of your detail drawings using Autodesk Inventor. Easily include isometric, detail and broken views. Automatically maintain an accurate parts list with quantities that are always kept up to date and have associated balloons, numbers, and arrows. Speed the creation of technical illustrations, process sheets, and training materials by leveraging the 3D parts and assemblies you design in Autodesk Inventor.

Creating an Assembly Presentation Open the presentation file that has already been started for you: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 6_Assembly Documentation folder and double-click Chapter 6_Rear_Axle_Presentation.ipn. Note: The Panel bar now displays the Presentation tools. 3. Use the Zoom All parts.

tool to see all the

The parts that define the right wheel have already been exploded to show the individual parts. 4. In the browser, click the plus signs (+) next to Explosion1 and Rear Axle Assy.iam. Notice that the part and assembly structures are shown in the browser. This structure is defined by the assembly file.

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5. Rotate your view to an orientation similar to the image shown.

Illustrating Assembly Steps Tweak the position of the carrier: •

On the Presentation Panel bar, click the Tweak Components

tool.

Define the direction of the tweak: 1. Move the cursor over the end of the axle to display a preview of the triad. 2. When the Z direction of the triad preview is aligned with the center of the axle, click to accept. 3. To define the component, in the graphics window, select the carrier part. Define the transformation of the carrier: 1. Once the carrier is selected, drag the carrier to the right between the end of the axle and the sprocket. 2. To define the exact distance of the tweak, type 250 in the Tweak Component dialog. Then click the green check mark to accept that value.

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Next, you tweak the position of the key: 1. With the Tweak Component dialog still displayed, click Clear to define a new set of components for the next tweak sequence. 2. Zoom and rotate your view to an orientation similar to the image shown on the right.

Define the direction of the tweak: 1. Move the cursor over the outer face of the key to display a preview of the triad. 2. When the Z direction of the triad preview is pointing perpendicular to the top face of the key, click to accept. Define the component: •

In the Model browser, choose Key Connection:1.

Define the transformation of the key: 1. Drag the key away from the shaft. 2. To define the exact distance of the tweak, type 50 in the Tweak Component dialog and then click the green check mark

to accept that value.

3. To finish tweaking components, click Close.

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Animating Assembly Steps Create an animation of the assembly process. 1. On the Standard toolbar, click the Zoom All tool to see all the parts. 2. On the Presentation Panel bar, click the Animate

tool.

3. In the Animation dialog, type 10 for the interval and then click Apply.

Watch an animation of how to assemble and disassemble the parts: 1. Click the Play Forward

tool.

2. Click the Play Reverse

tool.

3. Click Cancel to close the Animation dialog.

Saving Your Work •

On the Standard toolbar, click Save its dependents.

and then OK to save your modifications to the presentation file and

Starting a New Assembly Drawing Next, create an assembly drawing of the rear axle assembly using the presentation file and assembly file with which you have been working. Start a new assembly drawing: 1. On the Standard toolbar, click the New

tool.

2. In the Open dialog, click the Metric tab and then double-click the ISO.idw This creates a new drawing with an A3 sheet size.

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Changing the Default Sheet Size The assembly drawing needs a larger sheet size. Next, you will change the sheet size from A3 to A1. Change the sheet size: 1. In the browser, right-click Sheet:1 and choose Edit Sheet. 2. In the Edit Sheet dialog, select A1 from the Size drop-down list and then click OK.

Generating the First View The first drawing view you create is an exploded view of the rear axle assembly. 1. On the Panel bar, click the Base View

tool.

2. In the Drawing View dialog, click the File drop-down list and select Chapter 6_Rear_Axle_Presentation.ipn. 3. In the Drawing View dialog, under Orientation select Right, change the scale to 0.25 (shown as 1:4 in the drop down list) and then ensure Style is set to Hidden Line Removed

.

4. To place the drawing view on the sheet, in the graphics window, click the approximate location shown. Tip: If the dialog is in the way, drag it to a new location using the title bar at the top.

Creating Another View of the Assembly Next, you will create an assembled view of the rear axle assembly on the same drawing sheet. 1. On the Panel bar, click the Base View

tool again.

2. In the Drawing View dialog, click the File Browse tool, and browse to the Chapter 6_Creating Assembly Documentation\Assemblies folder and then double-click Rear Axle Assy.iam.

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3. In the Drawing View dialog under Orientation, choose Iso Top Right, change the scale to 0.25 (shown as 1:4 in the dropdown list) and then change the Style to Shaded

.

4. To place the drawing view on the sheet, in the graphics window, click the approximate location shown.

Creating a Detail View Because the assembly view of the rear axle is small, you create a detail view that focuses on the sprocket area. 1. On the Drawing Views Panel bar, click the Detail View tool. 2. Click anywhere in the lower-left isometric view. 3. In the Detail View dialog under Scale, type .75 and then select the Shaded

style.

Define the circular boundary of the view: 1. Click once near the center of the sprocket and then click again when the preview circle is slightly larger than the sprocket.

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2. Place the drawing view on the right side of the sheet just above the title block.

Creating a Broken View The exploded view of the rear axle assembly is an ideal situation for a broken view. Convert the exploded view to a broken view: Note: Ensure that no drawing views are selected (red borders should not display on any of your drawing views) before starting the next step. 1. On the Panel bar, click the Broken View

tool.

2. To define the view to be broken, select the top exploded view. 3. In the Broken View dialog, type 10.00mm for the Gap value. Define the left and right boundaries to be removed from the view: •

Click just to the right of the left cone on the axle (arrow 1). Then click just to the left of the right cone on the axle (arrow 2).

The view is converted to a broken view and break symbols identify the section that was removed.

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Adding Balloons Identify all the parts in the exploded view of the rear axle by adding balloons. Before you add balloons, clean the drawing sheet and move the broken view slightly to the left. 1. Click near the center of the broken view (without selecting any view geometry). A red border displays around the perimeter of the view. 2. Drag the drawing view border and place the view near the upper-left corner of the sheet as shown.

Display drawing annotation tools on the Panel bar: •

Click the Panel bar and choose Drawing Annotation Panel.

Automatically add balloons to the broken view: 1. On the Drawing Annotation Panel bar, click the down arrow to the Balloon

tool and then click the Auto Balloon

next tool.

2. In the graphics window, select the broken view you just moved. 3. To identify the parts you want to balloon, drag a rectangle around all the parts in the view. 4. Ensure the Ignore Multiple Instances selection is checked. 5. To define the balloon placement, click the Select Placement move the cursor around the drawing view.

tool, click the Around option and then

Notice the balloons dynamically move around the center of the view. 6. Click the Horizontal option, place the balloons above the view and then click OK to create the balloons. Balloons are created and automatically distributed along the top of the broken view.

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Even though you created the balloons as a set, you can modify balloons individually. Modify the arrow on a balloon: 1. Use the Zoom Window balloon for the carrier.

tool to zoom in on the

2. Move the cursor over the arrow on the balloon for the carrier.

3. Click and drag the tip of the arrow to the center of the hub so that the arrow is not touching any part geometry. Because the balloon no longer touches the geometry on the part, the balloon arrow changes to a dot (below right).

Creating a Parts List Include a parts list with your balloons: 1. On the Drawing Annotation Panel bar, click the Parts List

tool.

2. Click once on the broken view and then click OK to exit the Parts List dialog. A rectangular preview of the parts list boundary now displays, enabling you to identify a location. 3. Move the cursor near the right side of the drawing sheet. As the upper-right corner of the preview boundary nears the upper-right corner of the border, it snaps into place temporarily. 4. Click to accept the location and create the parts list.

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Printing and Saving Your Work If you have a printer or plotter available, you can now print your drawing the same way you print documents in other Windows applications. After printing, you can save your assembly drawing. If you would like to print your drawing: 1. From the File menu, choose Print. 2. To save your drawing, on the Standard toolbar, click the Save tool, type the name My _Rear_Axle_Drawing.idw and then click Save. Because you are finished with the assembly drawing and presentation, you can now close the files. 3. Close the My_Rear_Axle_Drawing.idw and Chapter 6_Rear Axle Presentation.ipn files. 4. Click Yes to save the file and any dependents.

Chapter Summary Dramatically improve drawing accuracy and the need for manual checking using Autodesk Inventor. Improve the communication to your manufacturing floor and your customers with high-quality, accurate assembly drawings and technical illustrations created with Autodesk Inventor.

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Chapter 7: Working with Assembly Configurations

Chapter 7: Working with Assembly Configurations Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107 Opening the Assembly File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107 Working with an Assembly Configuration . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108 Opening the Drawing File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110

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Chapter 7: Working with Assembly Configurations In This Chapter Next, you will see how you use Autodesk Inventor to design product families containing many varying components or sizes. You will see how a master assembly contains a table specifying the design differences between the various configurations of the design. Also, you will see how to document and accurately communicate your configured assemblies.

The Autodesk Inventor Advantage It is common to design products that come in various sizes or with several options, often referred to as product families. Using Autodesk Inventor, you can quickly create 3D models of an entire product family with configurations of varying geometry, dimensions, and components. You can quickly create dozens of design variants, and the associative drawing environment of Autodesk Inventor makes documenting configurations automated and easy.

Opening the Assembly File Open the go-cart assembly: 1. On the Standard toolbar, click the Open tool. 2. In the Open dialog, browse to the Chapter 7_Working with Assembly Configurations folder and double-click Chapter 7_Go_Cart_i_assembly.iam. If prompted to update the assembly, click Yes.

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Working with an Assembly Configuration If you design product families—many designs containing similar subassemblies and parts—you can gain design efficiency by using the assembly configuration functionality of Autodesk Inventor. Next, see how one master assembly file contains a table that drives the definition of all the possible design variations of that assembly. In the go-cart assembly, you will see that you have many different size and style configurations of the front wheel subassembly. •

In the Model browser, click the plus sign (+) next to Table. Each of the assemblies listed under Table represents a unique configuration of the go-cart assembly.

View a different configuration of the assembly: 1. In the Model browser, double-click the first item in the table list, Dia140-Wide-Gray. The go-cart assembly now contains a front wheel subassembly with a 140-diameter-wide tire, gray rim wheel assembly.

2. In the Model browser, double-click the last item in the table list, Dia100-Narrow-Red to view another configuration of the assembly.

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Opening the Drawing File Open the drawing of the go-cart assembly configuration: 1. On the Standard toolbar, click the Open tool. 2. In the Open dialog, browse to the Chapter 7_Working with Assembly Configurations folder and double-click Chapter 7_Go_Cart.idw. If notified to update member files, click OK. 3. In the graphics window, right-click the assembly view and choose Edit View.

4. In the Drawing View dialog, click the Model State tab. The drawing environment allows you to choose which member of the configuration you would like to display in the drawing. 5. In the Drawing View dialog, in the Assembly Member section, choose Dia100Narrow-Red. If notified to update member files, click OK. 6. Click OK. Your assembly view updates to display the instance of the assembly that includes the narrow,100-diameter, red-rim front wheel assembly.

Saving Your Work Save your work: 1. Close

the Chapter 7_Go_Cart.idw window.

2. Click Yes when prompted to save changes.

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3. Close

the Chapter 7_Go_Cart_i_assembly.iam window.

4. Click Yes when prompted to save files and dependents.

Chapter Summary Autodesk Inventor allows you to quickly create and document entire product families saving you design time and increasing the quality of each and every one of your products.

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Chapter 8: Performing Stress Analysis Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Opening the Part File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Performing Stress Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Material Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113 Applying a Bearing Load . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 114 Applying a Fixed Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 114 Applying a Pin Constraint . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115 Running Stress Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115 Reviewing Analysis Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115 Making a Revision . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 117 Updating the Stress Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 118 Generating a Report . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119

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Chapter 8: Performing Stress Analysis In This Chapter You will use the built-in finite element analysis (FEA) functionality of Autodesk Inventor Professional to improve the carrier part you designed in the beginning of this test drive. You will define the loading of the carrier part, review the results of your analysis, make a necessary design change, and validate that the change will work by running the analysis again, all without ever leaving the familiar Autodesk Inventor design environment.

The Autodesk Inventor Advantage By performing finite element analysis on your parts within the Autodesk Inventor environment, you can validate design decisions based on analytic results rather than intuition. Autodesk Inventor 3D part designs carry full physical and material properties, so by applying forces and identifying fixed points you can easily perform reliable analyses of how your parts will perform under load. Test various material types and geometric changes to design more robust parts, reduce material costs, and decrease the number of physical prototypes necessary using the FEA functionality of Autodesk Inventor.

Opening the Part File First, open the carrier 3D part: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 8_Performing Stress Analysis folder and double-click Chapter 8_Carrier.ipt.

Performing Stress Analysis •

On the Panel bar, click the Part Features drop-down arrow and select Stress Analysis.

Material Properties At any time, you have the ability to change and update the material properties of the part being analyzed. Change the material of your part: 1. In the Choose Material dialog, click the Material drop-down list and select Cast Steel. 2. Click OK.

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Applying a Bearing Load By applying a specific bearing load, you can predict how the part might behave under real-life conditions: 1. On the Stress Analysis Panel bar, click the Bearing Load

tool.

2. In the graphics window, for the Faces selection, select the inner face of the hole on the flange that is opposite the keyway (arrow 1). 3. In the Bearing Load dialog, click the Direction select tool and then, in the graphics window, select the vertical face on the side of the flange (arrow 2). 4. Enter a Magnitude of 500N. 5. Click OK to create the load. Notice that Bearing Load 1 has been added to the Stress Analysis browser.

Applying a Fixed Support A fixed constraint simulates a connection to a rigid, immovable object. Apply a constraint that depicts how the carrier is assembled to the drive shaft. 1. On the Stress Analysis Panel bar, click the Fixed Constraint tool. 2. In the graphics window, select the keyway face as shown. Note: This fixed constraint will oppose the rotational force created by Bearing Load 1. 3. Click OK.

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Applying a Pin Constraint A pin constraint is used to simulate a radially, axially, or tangentially fixed cylindrical surface, so that the applied curved surface cannot move, rotate, or deform in the selected direction. Apply a pin constraint: 1. On the Panel bar, click the Pin Constraint tool. In the Pin Constraint dialog, the Fix Radial Direction and Fix Axial Direction options should be checked. 2. Select the inner diameter face of the carrier. 3. Click OK.

Running Stress Analysis 1. Press F6 to switch to an isometric view. 2. On the Panel bar, click the Stress Analysis Update

tool.

The mesh and solution are calculated automatically in the background. Tip: If the Stress Analysis Update tool is grayed out, the solution is either current, missing at least one load and one support, or one of the boundary conditions is invalid.

Reviewing Analysis Results Running an analysis generates plots for Equivalent Stress, Principal Stresses, Deformation, and Safety Factor. The mesh used in the analysis is also available for display. In addition to the numerical values of your results, the 3D model visually displays the results and even allows you to animate results under various frequencies. Turn on the visibility of the mesh: •

On the Standard toolbar, click the Element Visibility

tool.

Animate your results: 1. On the Stress Analysis Panel bar, click the Animate Results

tool.

2. In the Animate Results dialog, click Play, Pause, and Stop. 3. Click OK.

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Equivalent Stress Autodesk Inventor Professional calculates the Equivalent Stress of a model using the von Mises theory. The von Mises stress simplifies the solution into a single scalar number, which is used to estimate Yield criteria for ductile materials and also calculate fatigue strength. The Equivalent (von Mises) Stress Plot is the default display. Note the Maximum Equivalent Stress for your model, displayed above the legend.

Deformation Results Autodesk Inventor describes Deformation as a change in shape when a force is applied. By measuring the amount of deformation that occurs to a model, you can analyze whether a design will hold or maintain dimensional tolerances when subjected to the specified forces. Display the Deformation plot: 1. In the Stress Analysis browser, double-click Deformation. 2. On the Standard Toolbar, click the Deformation Style drop-down arrow and select 2:1 Automatic. An exaggerated deformation plot of the bracket displays at a ratio of 2:1 to provide a better visual reference of how the model is being deformed. 3. In the Deformation Style drop-down list, select Actual to return to the original state of the model. Note: The Maximum Deformation value for the model displays above the legend.

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Safety Factor The Safety Factor of a model is the ratio of the limit strength of a material to the maximum stress predicted for the design. A Safety Factor of less than 1 indicates Material Yield and possible design failure. The Material Yield is the stress at which permanent deformation takes place. •

In the Stress Analysis browser, double-click Safety Factor. The Safety Factor Plot displays. Note: The Minimum Safety Factor value for the model displays above the legend.

Making a Revision After running an analysis, return to the modeling environment and make modifications. In this exercise, the carrier flange shows a possible failure point where the bearing load is applied. Modify the geometry to help strengthen the arm. Modify the flange radius: 1. On the panel bar, click the Stress Analysis dropdown arrow and select Part Features. 2. In the Model browser, right-click the Extrusion 2 feature and choose 3D Grips.

3. In the graphics window, right-click the 6 dimension and choose Edit Dimension. 4. In the Edit Dimension dialog, type 8 and then click OK. 5. In the graphics window, right-click and choose Done.

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Modify the cutout width: 1. In the Model browser, right-click the Revolution1 feature and choose 3D Grips. 2. In the graphics window, pause your cursor over the grip handle on the left-hand side of the rectangular profile. A yellow arrow displays. 3. Pause your cursor over the yellow grip arrow until it turns red, indicating it is selected (arrow 1). 4. With the arrow selected, click and drag your cursor to the right, making the width of the rectangle smaller. Drag the arrow until the width dimension displays a value of 14 (arrow 2). Modify the cutout height: 1. With 3D Grip Edit still active, in the graphics window, pause your cursor over the grip handle on the top of the rectangular profile. 2. Pause your cursor over the yellow grip arrow until it turns red, indicating it is selected (arrow 3). 3. With the arrow selected, click and drag your cursor downward, making the height of the rectangle smaller. Drag the arrow until the height dimension displays a value of 5 (arrow 4). 4. In the graphics window, right-click and choose Done to accept the change.

Updating the Stress Analysis Re-run the analysis of the part: 1. On the panel bar, click the Part Features drop-down arrow and select Stress Analysis. 2. On the Stress Analysis panel, click the Stress Analysis Update

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View the new analysis results: 1. In the Stress Analysis browser, note the new value of the Equivalent Stress results. 2. In the Stress Analysis browser, double-click Deformation to view the updated results. 3. In the Stress Analysis browser, double-click Safety Factor to view the updated results.

Generating a Report When you complete your analysis and are ready to communicate your results to management, peers, customers, and suppliers, you can generate a professional report using the automatic Report Generator. •

In the Stress Analysis panel, click the Report automatically.

tool. Autodesk Inventor creates the document

Tip: By default, Autodesk Inventor creates the report in HTML format. You can also save and edit the document in MS Word format.

Saving Your Work 1. Close

the Chapter 8_Carrier.ipt window.

2. When prompted to save changes, click Yes.

Chapter Summary Using Autodesk Inventor for 3D design enables you to analyze your product virtually. Create higher quality parts and experience fewer field failures while making better decisions about parts before entering the physical prototyping or manufacturing design stage.

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Chapter 9: Designing Welded Assemblies

Chapter 9: Designing Welded Assemblies Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 Welding the Flanges on the Steering Column . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123 Converting the Assembly to a Welded Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 Creating a 3D Fillet Weld . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 Creating a Drawing of the Welded Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125 Reusing Welding Symbols and Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Finishing the Welded Drawing with Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 126 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127

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Chapter 9: Designing Welded Assemblies In This Chapter Next, you will work in the dedicated weld environment of Autodesk Inventor. You will add welds to the steering column of the go-cart design and create a detail drawing to document your welded assembly.

The Autodesk Inventor Advantage The built-in weldment design environment in Autodesk Inventor makes it easy to model welds in 3D and automatically generate associative 2D documentation and symbology of the welds. This advantage improves design quality by automatically updating the weldments when designs change, and by including the mass of weld material in the properties of the assembly. The associative documentation always reflects the correct symbols for downstream use in the manufacturing process.

Welding the Flanges on the Steering Column In the go-cart design, you will weld the parts defining the steering column. First, open the go-cart and steering column assemblies: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 9_Designing Welded Assemblies folder and double-click Chapter 9_Go_Cart.iam. 3. Use the Zoom

tool to zoom in on the steering column.

4. In the graphics window, right-click the steering column assembly and choose Open. The steering column assembly is opened in a separate window. Notice in the browser that the steering column assembly contains a steering column shaft and two steering column flanges.

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Converting the Assembly to a Welded Assembly To create welds between the parts in the assembly, you must convert the assembly to a welded assembly: 1. From the Convert menu, choose Weldment. 2. When the dialog displays asking you to confirm the conversion of the assembly to a welded assembly, click Yes to continue. 3. In the Convert to Weldment dialog, ensure the Standard is set to ISO and the Weld Bead Material is Welded Aluminum-6061 and then click OK. Notice in the browser that the assembly now has Preparations, Welds, and Machining entries. Each of these entries contains the individual features associated with that specific process.

Creating a 3D Fillet Weld Autodesk Inventor can create cosmetic welds and 3D fillet welds. Next, you will create 3D fillet welds between the two flanges and the steering column. Since our weldment is fairly simple and requires no preparation, you can go directly to the welding process: 1. In the browser, double-click Welds. The Panel bar displays the appropriate welding tools. 2. On the Panel bar, click the Fillet Weld

tool.

3. Click the Bead 1 button and then select the steering column shaft. 4. Click the Bead 2 button and then select the top face of the upper flange. 5. Click the Leg Length value and type 4 mm for the weld leg length (arrow 1). 6. Check the Create Welding Symbol option.

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7. Enter a for prefix (arrow 2) and 4 for Leg 1 (arrow 3). 8. Click Apply. The 3D fillet weld seam is created along the intersection of the two parts. Also, notice that the weld symbol displays. 9. Use the F4 key to rotate your view so you can see the bottom of the lower flange. 10. Click the Bead 1 column shaft.

button and then select the steering

11. Click the Bead 2 button, select the bottom face of the lower flange and then click OK to create the second fillet weld. The final weld seam and associated weld symbol are created. 12. To finish your welded assembly, on the Standard toolbar, click Return

and then click Save

.

Creating a Drawing of the Welded Assembly Next, create a drawing of the welded assembly: 1. On the Standard toolbar, click the New

tool.

2. In the Open dialog, click the Metric tab and then double-click ISO.idw . A new A3 size drawing sheet with a frame and title block is created. 3. On the Panel bar, click the Base View tool. 4. In the Drawing View dialog, click the File drop-down list and then choose Chapter 9_Steering Column Assy.iam.

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5. In the Drawing View dialog under Orientation, select Right, change the scale to 0.5 (shown as 1:2 in the drop-down list), and ensure Style is set to Hidden Line Removed

.

6. Place the drawing view on the sheet by clicking the approximate location shown in the image. Create a projected view: 1. On the Panel bar, click the Projected View

tool.

2. Select the view you just created and then click to the right to define the location of the side view. 3. To create the drawing view, right-click and choose Create.

Reusing Welding Symbols and Annotations Since the welding symbols already exist in the model, you can simply retrieve them for the drawing. 1. Right-click in the drawing view on the left and choose Get Model Annotations and then choose Get Welding Symbols. 2. If the welding symbols are not located as shown, click the green dot and drag them into the desired position. 3. Repeat this procedure for the projected view on the right.

Finishing the Welded Drawing with Dimensions Finish your drawing of the welded assembly by adding baseline dimensions showing the proper location of each flange: •

Click the Panel bar and choose Drawing Annotation Panel.

Add baseline dimensions to the view: 1. Zoom in on the flanges and the right end of the shaft in the left drawing view. 2. On the Panel bar, click the Baseline Dimension Set

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3. In the left view, select the three vertical lines from right to left, as shown in the image above. 4. Right-click and choose Continue. 5. Click above the view to place the baseline dimensions. 6. Right-click and choose Create to quit the Baseline Dimension Set tool.

Saving Your Work Save your weldment drawing of the steering column: 1. On the Standard toolbar, click the Save

tool.

2. In the Save As dialog, browse to the Chapter 9_Designing Welded Assemblies folder and type My_Weldment.idw as the file name and then click Save. 3. Close

the My_Weldment.idw

drawing window and then close the Chapter 9_Steering Column Assy.iam and Chapter 9_Go_Cart.iam windows.

Chapter Summary Modeling welds in 3D improves the accuracy of mass and center of gravity computations, completes the manufacturing documentation, and elevates the overall quality of your designs.

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Chapter 10: Creating a Sheet Metal Design

Chapter 10: Creating a Sheet Metal Design Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 131 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 131 Creating a Sheet Metal Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 131 Mirroring Sketch Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 132 Adding Dimensions to the Contour . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 132 Defining the Sheet Metal Thickness . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133 Creating the Sheet Metal Part from the Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133 Creating a Flange . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Creating a Hole in the Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Defining the Location of the Cutouts for the Gauges . . . . . . . . . . . . . . . . . . . . . . . . . 135 Using the Punch Tool . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 136 Finishing the Design Using Corner Rounds . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137 Creating a Flat Pattern . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 138

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Chapter 10: Creating a Sheet Metal Design In This Chapter Next, you use the sheet metal-specific design features of Autodesk Inventor to create a sheet metal bracket and the associated flat pattern.

The Autodesk Inventor Advantage Designing quality sheet metal parts requires the ability to design and visualize parts in both the flat and folded state. The 3D design environment of Autodesk Inventor enables you to work in either state, enabling you to account for bend thickness and precise dimensioning. The software automatically calculates bend allowances, provides customizable bend tables, and automates the creation of detail drawings. Using 3D to design sheet metal parts helps improve the accuracy and quality of your parts and documentation.

Creating a Sheet Metal Part With Autodesk Inventor software, you can design a sheet metal part in several convenient ways. In this exercise, you design a sheet metal part from a simple contour. Start a new sheet metal part: 1. On the Standard toolbar, click the New

tool.

2. In the Open dialog, click the Metric tab and then double-click the Sheet Metal (mm).ipt a new sheet metal part.

icon to create

Once again, you start your part with a sketch. Since you are now somewhat familiar with the sketching tools, the descriptions are brief: •

Click the Line tool and then create the open, foursegment sketch shown on the right (arrow 1). Tip: Use the grid to sketch the line segments as closely as possible to the size shown on the right.

Create a vertical construction line at the midpoint of the upper line segment: 1. Click the Line

tool and then, on the Standard

toolbar, click the Construction

tool.

2. Using the green dot at the midpoint of the upper horizontal line as a starting point, sketch a construction line that is perpendicular to that line (arrow 2).

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3. Click the Construction

tool on the Standard toolbar to turn construction mode off.

Mirroring Sketch Geometry Next, mirror the three line segments from the left to the right side of the sketch using the construction line: 1. On the Panel bar, click the Mirror

tool.

2. Drag a window (from left to right) around the three line segments on the left side of the sketch (see arrows). 3. In the Mirror dialog, click Mirror line. 4. Select the construction line, click Apply and then click Done.

Adding Dimensions to the Contour Next, add dimensions to define the size of the contour: 1. Using the General Dimension tool, create the 60, 180, 155, 100, and 30 dimensions respectively. Note: As you add dimensions, notice that both sides of the sketch update. Tip: To create the 155 dimension, select the upper horizontal line and then select the endpoint of the lower-left line segment. 2. Press F6 to restore the isometric view. 3. In the graphics window, right-click and choose Finish Sketch.

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Defining the Sheet Metal Thickness The default thickness of the sheet metal part is a bit thin. Change the sheet metal thickness and other crucial parameters globally: 1. On the Panel bar, click the Sheet Metal Styles tool. 2. In the Sheet Metal Styles dialog, type 3 mm for the thickness, click Save and then click Done. Your default settings have now been changed.

Creating the Sheet Metal Part from the Sketch Next, you turn your sketch into a 3D, solid sheet metal feature. 1. On the Panel bar, click the Contour Flange

tool.

2. For the profile selection, in the graphics window, select the open contour sketch you just created. 3. In the Contour Flange dialog, type a distance of 26 mm. 4. If the preview of the part is not offset to the outside of the sketch, click the Offset button. 5. Click OK to create the sheet metal part.

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Creating a Flange Next, create a flange that will support the RPM and speedometer gauges of the go-cart design: 1. On the Panel bar, click the Flange

tool.

2. Select the long, inner edge of the part shown in the image on the right. 3. In the Flange dialog, type a distance of 100 mm.

4. If your preview does not match the image shown on the right, use the Flip Offset Flip Direction settings.

and

options to adjust your

5. Click OK to create the flange.

Creating a Hole in the Part Next, create a hole through the short tabs of the part: 1. On the Panel bar, click the Hole

tool.

2. Ensure the Linear placement option is selected.

3. Click Face and then, in the graphics window, select the outer face of the right tab.

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4. Select the upper edge of the tab and type a distance of 13 and then press Enter to define the first edge and offset.

5. Select the left edge of the tab and type a distance of 13 and then press Enter to define the second edge and offset. 6. In the Holes dialog, choose a termination of Through All. 7. Type a diameter value of 10 mm and then click OK to define the size of the hole.

Defining the Location of the Cutouts for the Gauges Next, sketch two points that define the location of the cutouts for the gauges: 1. On the Standard toolbar, click the 2D Sketch 2. Use the Look At

tool and then select the top face of the flange.

tool to view the top face of the flange.

3. Using the Line and Construction tools, create a vertical construction line that is centered on the midpoint of the upper edge of the sketch, as shown (arrow 1). 4. Click the Construction tool on the Standard toolbar to turn construction mode off. 5. On the Panel bar, click the Point, Center Point tool and then place one point at the approximate location shown in the image (arrow 2). 6. Use the Mirror tool again to mirror the Point, Center Point to the right side of the sketch using the construction line as the mirror line.

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7. In the graphics window, right-click and choose Finish Sketch.

Using the Punch Tool Next, use the punch tool to create the cutouts for the gauges: 1. On the Panel bar, click the Punch Tool

tool.

2. In the Punch Tool dialog, choose Keyway.ide and then click Next. 3. Since the geometry for the location of the punch is automatically selected using the points on the sketch, click Next again.

Define the size of the keyway: 1. For the diameter, highlight the current value and then type 2 in. Tip: Autodesk Inventor software enables you to mix units of measurement. 2. For the keyway width, highlight the current value and then type 5 mm. 3. For the keyway depth, highlight the current value and then type .9 in. 4. Click OK to create the two cutouts for the gauges.

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Finishing the Design Using Corner Rounds Finally, you use the corner round tool to remove some sharp edges on the part. 1. On the Panel bar, click the Corner Round

tool.

2. Select the six edges of the part shown on the right (the sharp corners of the short tabs and the flange), enter 6 mm for the corner radius and then click OK to create the corner rounds. Note: Notice that Autodesk Inventor automates the selection process of these short edges.

Creating a Flat Pattern Flat patterns are the “flat blanks” used to manufacture sheet metal parts. Create a flat pattern for your sheet metal part: •

On the Panel bar, click the Flat Pattern

tool.

Autodesk Inventor automatically performs the required calculations for the bending allowance and correctly displays the flat pattern as a flat 3D part. Identify the bending lines and bending zones on the flat blank: •

On the Standard toolbar, click the down arrow Shaded Display

next to the

tool and then click the Hidden Edge Display

tool. You can create engineering drawings using both the folded and unfolded versions of the sheet metal part on the same drawing sheet. Flat patterns can also be exported as AutoCAD® DWG or DXF™ files and can then be imported into CAM (Computer Aided Machining) software for nesting, punching, or even laser cutting.

Saving Your Work Save your sheet metal part: 1. Click the Save tool, browse to the Chapter 10_Creating a Sheet Metal Design folder, type the name My_Bracket.ipt and then click Save.

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2. Close

the My_Bracket.ipt window.

Chapter Summary Autodesk Inventor software includes a set of powerful sheet metal tools, enabling you to create high-quality parts and reliable manufacturing documentation.

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Chapter 11: Photo-Realistic Rendering

Chapter 11: Photo-Realistic Rendering Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Opening the Assembly File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Creating an Autodesk Inventor Studio Rendering . . . . . . . . . . . . . . . . . . . . . . . . . . . 141 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 142 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 142

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Chapter 11: Photo-Realistic Rendering In This Chapter Now that you have finished your go-cart design, you can create a photo-realistic rendering of your assembly.

The Autodesk Inventor Advantage Communication of final and conceptual engineering designs is an important aspect a successful product. Autodesk Inventor makes it easy for design engineers to create high quality photo-realistic renderings and animations. State-of-the-art rendering and animation tools are built into the 3D design environment, allowing engineers to quickly set up and create renderings and animations any time during the design cycle.

Opening the Assembly File Open the go-cart assembly: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 11_PhotoRealistic Rendering folder and double-click Chapter 11_Go_Cart.iam.

Creating an Autodesk Inventor Studio Rendering Use the Autodesk Inventor Studio functionality to create a photo-realistic rendering of the go-cart assembly: 1. From the Applications menu, choose Inventor Studio.

2. On the Inventor Studio Panel bar, click the Render Image

tool.

3. On the Render Image dialog, click Render to create a photo-realistic rendering of the go-cart. 4. Close the Render Output window.

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Saving Your Work Save your work: 1. Close

the Chapter 11_Go_Cart.iam window.

2. When prompted to save changes, click Yes.

Chapter Summary Communicate your designs and communicate more clearly with those outside of engineering with the rendering capabilities of Autodesk Inventor. Visually prove concepts, reduce physical prototypes, and save time and money typically required for generating product renderings.

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Chapter 12: Designing Tubes, Pipes, and Hoses

Chapter 12: Designing Tubes, Pipes, and Hoses Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145 Opening the Assembly File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145 Starting a Pipe Run Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 146 Creating a Pipe Route . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 147 Finishing the Pipe Run Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149 Starting a Flexible Hose Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150 Creating a Flexible Hose Route . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150 Finishing the Flexible Hose Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151 Making a Design Change . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151 Starting a Rigid Tube Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152 Creating a Rigid Tube Route . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152 Finishing the Rigid Tube Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153 Reviewing Additional Tube and Pipe Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153 Reviewing Tube, Pipe and Hose Assembly Documentation . . . . . . . . . . . . . . . . . . . 154 Saving Your Work . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155

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Chapter 12: Designing Tubes, Pipes, and Hoses In This Chapter You will now use Autodesk Inventor to create a series of pipe, tube, and flexible hose runs in an existing skid assembly. The assembly you will work with is shown below.

The Autodesk Inventor Advantage Ensure that the flexible hoses, pipes, and tubes of your final product fit correctly the first time. Extend your 3D design by routing pipes, tubes, and hoses through your assemblies. Include fittings, unions, and other plumbing accessories. Apply bend and material rules to ensure manufacturable designs. Autodesk Inventor alerts you of interferences, calculates material lengths, and generates a Bill of Materials. You can quickly generate accurate manufacturing documentation using the automatic drawing views, parts lists, and cut lengths in the Autodesk Inventor drawing environment. Design your entire product line and increase the accuracy of your material requirements and assembly documentation using the tubing, piping, and hose design functionality of Autodesk Inventor.

Opening the Assembly File Rather than designing an assembly from scratch, open an existing assembly: 1. On the File menu, click Open. 2. In the Open dialog, browse to the Chapter 12_Designing Tubes, Pipes, and Hoses folder, choose _Chapter 12_skid_assembly.iam and then click Open.

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Starting a Pipe Run Design Start by adding a pipe run to the assembly: 1. On the Assembly Panel bar, click the Create Pipe Run

tool.

2. In the Create Tube & Pipe Run dialog, click OK to accept the default settings. Note: The Model browser now displays a folder named Tube & Pipe Runs. All pipe runs created in the main assembly will be stored automatically in this folder.

Defining a Pipe Style Autodesk Inventor allows you to define design rules that enforce consistency in the size, material, and components used in your Tube & Pipe assemblies. Set up your Styles in advance and let the software guide you as you add pipes, tubes, and hoses to your design. 1. On the Tube & Pipe Panel bar, click the Tube & Pipe Styles

tool.

2. In the Style list, click ISO 7598/ISO 49 Threaded Steel Pipe with Iron Fittings. 3. Click OK.

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Creating a Pipe Route Add a new pipe route to the Tube & Pipe Runs assembly: 1. Rotate and Zoom your model similar to the image on the right. 2. On the Tube & Pipe Panel bar, click the New Route tool and then click OK to accept the default Route file name. 3. From the Tools menu, click Document Settings. 4. In the Document Settings dialog, click the Units tab, and for Length, choose millimeter from the list. 5. Click OK. 6. On the Route Panel bar, click the Route

tool.

7. Pause your cursor over the inner diameter of the fitting. 8. When the green dot displays and the yellow arrow points away from the fitting, click to place the first node. Note: After placing the first node, you are automatically prompted to place a second node. When you move your cursor over the axis, a series of colored glyphs displays. The location of these glyphs is dependent upon the design rules set in your tube and pipe styles. By using these glyphs you can quickly see where nodes in a route should be placed, ensuring that the route meets the minimum and maximum pipe length rules. •

A blue dot means the pipe segment meets the minimum length but is too short for an additional fitting or bend.

•

A green dot indicates a valid location for your next node.

•

A yellow X means your node doesn't meet the minimum length segment setting.

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Using Precise Value Entry Define the second node of your route using precise numerical input: 1. Anywhere in front of the fitting, pause the cursor over the axis and then right-click and choose Enter Distance. 2. In the Enter Distance dialog, type 100 mm and then click the green check mark to accept.

Using the 3D Orthogonal Route Tool Define the next node of your route using the 3D Orthogonal Route graphical orientation tool. This tool assists in creating or repositioning the nodes that define the pipe route. 1. Pause the cursor over the lower section of the vertical axis and then right-click and choose Enter Distance. 2. In the Enter Distance dialog, type 200 mm and then click the green check mark to accept.

Using Point Snap Next, use the Point Snap functionality to define your pipe route in relation to other assembly geometry. You can create route node points by snapping to faces, edges, or work points that exist within the tube and pipe assembly. Point Snap on: 1. While pausing the cursor over the blue axis, right-click and choose Point Snap. With Point Snap turned on, you can now reference other objects in the assembly. 2. Move and pause the cursor over objects to see how Point Snap determines its location. 3. Pause the cursor over the support beam face shown (arrow) on the right (do not select the beam face). 4. Once the distance tool tip displays, type 10 mm to bring up the Enter Distance dialog and then click the green check mark. This newly created node is now 10 mm past the beam. 5. To turn the feature off, right-click and uncheck Point Snap.

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Finishing with Auto-Route Use Auto-Route to finish defining the path of your first route: 1. Locate the outlet fitting of the pump as shown on the right. 2. Move your cursor over the circular edge of the fitting. Click when the green dot appears and the arrow points away from the fitting. Tip: To change the direction of the fitting during insertion, press the spacebar. Auto-Route cycling displays its first routing solution. Select from other possible route solutions: 1. Use either the mouse wheel or the left and right arrows on the Select Other tool to cycle through all solutions. 2. Cycle through to the first solution and then click the Green Select button on the Select Other tool to accept the routing. 3. Right-click and select Done (or press Esc) to finish the route.

Finishing the Pipe Run Design Finish the pipe design and apply 3D geometry to the pipe run. You can now see a single line representation of the route in the context of the assembly. This representation serves as a placeholder until you are ready to apply the physical characteristics specified by the tube and pipe style. •

In the graphics window, right-click and select Finish Edit.

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Turn pipe routes into physical pipe runs and automatically place fittings and pipe segments as needed: 1. On the Tube & Pipe Panel bar, click the Populate Route tool. 2. In the graphics window, right-click and select Finish Edit to return to the top-level assembly. You have created a new 3D pipe run.

Starting a Flexible Hose Design Autodesk Inventor allows you to create flexible hose routes. 1. Use the Zoom and Rotate tools to view the area shown in the image to the right. 2. On the Panel bar, click the Create Pipe Run click OK to accept the default settings.

tool, and

Defining a Flexible Hose Style 1. On the Tube & Pipe Panel bar, click Tube & Pipe Styles. 2. In the Style drop-down menu, select Hydraulic Hose - Male Straight Thread and then click OK.

Creating a Flexible Hose Route Define the start and end points for the route: 1. On the Tube & Pipe Panel bar, click the New Route click OK to accept the default settings. 2. On the Route Panel bar, click the Route

tool and

tool.

3. Select the circular edge of the DBW20:1 fitting as shown on the right (arrow 1). Tip: To change the direction of the fitting during insertion, press the spacebar.

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4. For the second fitting, select the circular edge of the bottom tap of the Junction Box:1. 5. To accept the previewed auto-route, in the graphics window, rightclick and choose Done.

Finishing the Flexible Hose Design 1. In the graphics window, right-click and choose Finish Edit. 2. In the Tube & Pipe Panel bar, click the Populate

tool.

Making a Design Change Autodesk Inventor allows you to make design changes that automatically update your tube, pipe, and hose designs. Make a design change: 1. Double-click _Chapter 12_skid_assembly.iam to activate the main assembly. 2. Click the plus sign (+) in front of Junction Box:1. 3. Click the assembly constraint Mate:15(100.00 mm). 4. At the bottom of the Model browser, change the value to 500 mm and then press Enter. Notice that when the Junction Box position changes, the hose routing automatically updates according to the applied design criteria.

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Starting a Rigid Tube Design Create the first run in the tubing assembly: 1. On the Assembly Panel bar, click the Create Pipe Run

tool.

2. In the dialog, click OK to accept the default settings. 3. Use the Rotate and Zoom tools to view the area shown in the image to the right.

Defining a Rigid Tube Style Define the Tube and Pipe Style: 1. On the Tube & Pipe Panel bar, click the Tube & Pipe Styles

tool.

2. In the Style drop-down list, select ASTM B 88-ASME B16.22 - Soldered Copper Tubing and then click OK.

Creating a Rigid Tube Route Define the route: 1. On the Tube & Pipe Panel bar, click the New Route

tool and then click OK to accept the default settings.

2. Ensure you are working in millimeters: • From the Tools menu, click Document Settings. •

In the Document Settings dialog, click the Units tab, and for Length, choose millimeter from the list.

•

Click OK.

3. On the Route Panel bar, click the Route

tool.

4. Select the circular edge of the fitting for the first point, ensuring the yellow arrow points away from the fitting. Use Enter Distance to define the tube route: 1. Pause your cursor over the axis, right-click and choose Enter Distance. 2. Type 100 mm in the Enter Distance dialog and then press Enter.

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3. Pause your cursor over the green axis that extends left and then right-click and choose Enter Distance. 4. Type 200 mm in the Enter Distance dialog and then press Enter. 5. To define the final point in the route, select the diameter of the opening on the top of the tank. 6. Click the Green Select button to accept the first solution displayed. 7. Press Esc to exit the command, then right-click and choose Finish Edit.

Finishing the Rigid Tube Design •

On the Tube & Pipe Panel bar, click the Populate Route

tool.

Reviewing Additional Tube and Pipe Assemblies Rather than designing the entire assembly, you will review a completely finished design of the skid assembly. 1. On the File menu, click Open. 2. In the Open dialog, browse to the Chapter 12_Designing Tubes, Pipes, and Hoses folder, select Chapter 12_finished.iam and then click Open. Notice the multiple pipe and tube runs in the completed assembly.

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Reviewing Tube, Pipe and Hose Assembly Documentation Next, open and review a finished drawing of the skid assembly. To learn how to create assembly drawings, please review Chapter 6: Assembly Documentation. 1. On the File menu, click Open. 2. In the Open dialog, browse to the Chapter 12_Designing Tubes, Pipes, and Hoses folder, select Chapter 12_finished.idw and then click Open. 3. Review the contents of the assembly drawing and parts list. 4. In the browser, right-click Sheet:2 and choose Activate. 5. Review the contents of the pipe run drawing and parts list. Autodesk Inventor allows you to quickly document tube, pipe, and hose designs. The drawing environment includes built-in templates specifically for creating tube and pipe assembly documentation. As you can see, using the drawing capabilities in Autodesk Inventor, you can easily create orthographic and isometric views of your tube and pipe designs.

Parts List Capabilities With Autodesk Inventor, you can create a comprehensive parts list of your tube and pipe design. Parts lists can include a cut list or the rolled-up length of each type of piping or tubing used in the design. You can configure the parts list to collect all common tubes or pipes of a specific type and display it as a single line item with the length summed. You can use balloons to display the individual length of a pipe or tube segment that is part of a summed row. Each type of tube (different diameter, raw material, and so forth) used in an assembly has a unique part number and its own line in the parts list.

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When you use the template provided by Autodesk Inventor, the total length of the pipe is automatically calculated. You can also take advantage of this summation feature by adjusting the Value Substitution format option. Using the roll-up and ballooning capabilities, you can communicate accurate data to purchasing and manufacturing.

Saving Your Work Close and save the drawing and assembly files: •

Close the Chapter 12_finished.idw, Chapter 12_finished.iam, and _Chapter 12_skid_assembly.iam files. Click Yes to save changes.

Chapter Summary Create and communicate your complete design with the robust tubing and piping functionality in Autodesk Inventor. Increase the quality and manufacturability of your designs by ensuring that tube and pipe runs will fit properly before entering the prototyping or manufacturing stage.

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Chapter 13: Designing Cables and Wire Harnesses

Chapter 13: Designing Cables and Wire Harnesses Table of Contents In This Chapter . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 The Autodesk Inventor Advantage . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Opening the Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Working with the Wire Harness Subassembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159 Working with Electrical Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160 Working with Wires . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 161 Working with Segments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163 Viewing a Wire Path . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Viewing Segment Contents . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168 Creating a Nailboard Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 168 Chapter Summary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 170

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Chapter 13: Designing Cables and Wire Harnesses In This Chapter In this chapter you will design a wire harness for a printed circuit board (PCB) enclosure. The assembly with its wire harness is shown on the right. After you create the wire harness you will create a nailboard drawing to communicate your design.

The Autodesk Inventor Advantage Improve quality, reduce material costs, and streamline design time by incorporating your cable and wire harness design into the 3D design process. Using a 3D design environment means the software automatically calculates wire lengths and a Bill of Materials that update as the design changes, allowing you to skip the time-consuming and error-prone process of manually measuring a hardware prototype. Create accurate nailboard drawings that are always up to date reducing manufacturing and purchasing errors. Reduce overall design time and increase quality by using Autodesk Inventor to complete your cables and wire harness in the 3D design environment.

Opening the Assembly Open the assembly: 1. On the Standard toolbar, click the Open

tool.

2. In the Open dialog, browse to the Chapter 13_Designing Cables and Wire Harnesses folder and doubleclick Chapter 13_PCB Enclosure.iam. Take a moment to familiarize yourself with the assembly. It is a sheet metal enclosure with a printed circuit board mounted inside. The electrical connectors have already been inserted to aid in the wire harness design.

Working with the Wire Harness Subassembly To create a wire harness, you must first create a harness subassembly. To expedite this exercise, this step has already been completed for you. Edit the subassembly: 1. In the browser, double-click the Wire Harness subassembly. Note: If you receive the message, “The Cable & Wire Harness Library could not be found at:”, select Yes and then browse to the following path: C:\Program Files\Autodesk\Inventor 11\Cable & Harness\Library\Cable&HarnessDefaultLibrary.iwl, and click Open.

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Notice that the Panel bar has changed to the Cable & Harness toolbar. Most of the tools required to design a wire harness are on this toolbar. Other tools can be accessed through the context-sensitive menus. 2. In the browser, click the plus sign (+) next to Wire Harness 1 to expand it. The browser has been customized to handle the unique harness geometry that you will create.

Working with Electrical Parts Electrical parts provide the starting and ending points for wires in a wire harness assembly. Any Autodesk Inventor part can be turned into an electrical part by adding pins to it. Pins are work points placed by the Cable & Harness module with specialized harness information. Each pin has a unique name to distinguish it from the other pins on the part. Cable & Harness properties are also added to these parts. 1. In the graphics window, right-click and choose Isometric View. 2. In the browser, right-click the part D SUB 9 PIN:1 and choose Find in Window. 3. In the browser, click the plus sign (+) next to D SUB 9 PIN:1 to display the feature list. This part has nine pins, identified with the pin icon

.

Adding a RefDes Property RefDes, short for reference designator, is an important property for electrical parts in Cable & Harness. The RefDes is the unique identifier for each connector instance in a cable and harness design. RefDes and Pin Name together provide the information needed to terminate a wire. 1. Ensure the Wire Harness subassembly is active: In the browser double-click Wire Harness. 2. In the browser, right-click the D SUB 9 PIN:1 part and choose Harness Properties. 3. In the Part Properties dialog, type J1 in the RefDes field and then click Apply. 4. Click the Custom tab to view the custom properties that have been added to the part. 5. Click Cancel to close the Part Properties dialog.

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You can add any number of user-defined or custom properties to the components of a harness design. These properties are then available for later use when generating manufacturing documentation.

Working with Wires In Autodesk Inventor Professional, a wire represents both the physical geometry (diameter, color, length) of the wire as well as the electrical connectivity data such as wire ID, signal name, and from/to connection information. Each wire connects two pins and establishes electrical design intent, similar to mechanical design intent.

Inserting Wires Manually 1. On the Standard toolbar, click the Zoom All

tool.

2. On the Cable & Harness Panel bar, click the Create Wire tool. 3. Choose Belden from the Category drop-down list. 4. Choose 9916-RED from the Name drop-down list. 5. In the graphics window, move the cursor over the points on the D SUB 9 PIN:1 connector. A tooltip identifies the connector RefDes and pin name. 6. Select Pin 5 as shown in the image to the right to identify the first pin (starting point). In the Create Wire dialog, the arrow button next to Pin 2 is automatically selected. 7. Select Pin 10 on the PCB Connector (rectangular connector located on the PCB) to identify the second pin (ending point). A preview of the wire displays. 8. In the Create Wire dialog, change the Wire ID field to 10010. Wire ID is the unique name for the wire. The Wire ID is used as the browser name for the wire as well. 9. Click OK. The wire you just created is drawn between the two pins as a straight line.

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Importing Harness Data Many wires can be added automatically to the assembly using the Import Harness Data tool. A CSV (comma separated value) file is used to specify the point-to-point connectivity of each wire. These files can be generated from an AutoCAD® Electrical file, a spreadsheet, or a database of the wire connections in the harness. Following is an image of the text file you will import.

The CSV file lists the wires to be imported into the assembly. Each row represents a wire to be imported. The wire ID is unique for each wire in the design. The Part Name references a wire in the Wire Library. The RefDes and Pin columns correspond to the part and pin the wire will be attached to on each end. Other user-defined properties can be imported onto the wires during the Import Wire List function. Import a wire list for this assembly: 1. On the Panel bar, click the Import Harness Data tool. 2. In the Harness Data File section of the Import Harness Data dialog, click Browse and navigate to the Chapter 13_Designing Cables and Wire Harnesses folder. Ensure that Files of type is set to (*.csv), then select Wire List Data.csv and click Open. 3. In the Configuration File section of the Import Harness Data dialog, click Browse and navigate to the Chapter 13_Designing Cables and Wire Harnesses folder. Select Wire List configuration.cfg and then click Open. 4. Click OK. 5. In the Imported Harness Data dialog, click OK. 6. In the Imported Harness Data log file dialog, click Close. The wires are created in the assembly.

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Working with Segments Segments define virtual paths for wires to take through the assembly. Their diameters can be set to update automatically as wires are added to reflect the size of the wires bundled in them. You add segments by clicking geometry in the assembly. Each click defines a work point that provides the 3D spline path for the segment. These work points can be associated to geometry in the assembly or can be grounded by coordinates.

Creating Segments You first need to create a segment that goes between the two connectors on the walls of the enclosure. You are going to use work points placed on the connector and the zip ties as the locations for your points. Create a segment: 1. In the graphics window, right-click and choose Isometric View. 2. Use the Zoom connector.

tool to zoom in on the D SUB 9 PIN

3. On the Cable & Harness Panel bar, click the Create Segment

tool.

4. Move the cursor over the first point coming out of the connector (arrow 1). 5. When the point turns white, click to select it as your first point. You have just created an associative relationship between this point and the segment point. Now if the connector has to be moved, the segment moves with it. Notice that as you move the cursor, a line is drawn back to your first point.

6. Pause the cursor over the work point to the right of the first point (arrow 2), and when it turns white, click it. A yellow line represents the first part of your segment. As you continue picking the rest of the points for the segment, the line becomes a spline, previewing your segment’s path.

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Continue defining the segment: 1. Return to the isometric view, and, if necessary, zoom in on the cable zip ties so that you can see them all. 2. Pause the mouse over the outside circular edge of the first cable zip tie. 3. When the edge turns red and a green dot displays at the center of the edge, click the mouse button. The next point is created as well as another associative relationship to the cable zip tie. 4. Repeat the procedure, selecting the back edge of the cable zip tie, as shown. 5. Repeat this procedure for the three remaining cable zip ties in the assembly. Complete the segment by selecting points on the circular connector: 1. Zoom in on the circular connector. 2. Pause the cursor over the outer point until it turns white and then select it (arrow 1). 3. Select the point to the right of it (arrow 2). 4. To complete the first segment, in the graphics window, right-click and choose Continue. The segment sweeps along the path you created. The Create Segment tool is still active so that you can add the next segment.

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Inserting a Branch Next, you add another segment to allow the wires attached to the PCB connector to enter the harness. Insert a branch: 1. Click the Look At tool and then select the top of the green PCB so that you are looking straight down on the harness, as shown on the right. 2. Zoom in so that you can clearly see the connector on the PCB and the segment you just created. 3. Select the centerline of the first segment directly above the middle of the connector. The first segment is split into two connected pieces, and a third segment is started at the junction. 4. In the graphics window, right-click and choose Edit Offset. 5. Type 30 mm for the offset distance and then click OK.

6. Click on a point over the PCB board, midway between the first point and the PCB connector on the board, to select the top face of the PCB board. Click again to specify the point’s location on the face. 7. In the graphics window, right-click and choose Edit Offset again. 8. Change the distance to 6.5 mm, and click OK. 9. Select a point between the pins on the top surface of the PCB connector. 10. In the graphics window, right-click and choose Finish. 11. Press F6 to switch to an isometric view. You have now developed a network of segments that you can route the wires into.

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Routing Wires There are several ways to bundle the wires into the network of segments. You will use two of them to complete the harness.

Route wires: 1. In the graphics window, right-click the yellow wire running from the 9 Pin D-Sub connector to the circular connector (arrow 1) and then choose Route. The Route Wires dialog displays, with your wire already selected. All that is necessary is to choose the segment for the wire to enter and exit. 2. Select the segment ending at the 9 Pin D-Sub connector (arrow 2) for the first segment.

3. Select the segment ending at the circular connector (arrow 3) for the last segment. 4. In the Route Wires dialog, click OK to route the wire. You have just routed the wire. Notice that the segment diameters have changed from their initial default diameters to now reflect the diameter of the wire running through them. This individual wire routing method is handy if you need to control exactly how the wires are routed through your harness.

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Route the remaining wires using the Automatic Route tool: 1. On the Cable & Harness Panel bar, click the Automatic Route

tool.

2. Select All Unrouted Wires, and click OK. The remaining wires are routed and the diameters of the segments are updated to reflect the bundled diameter of the wires running through them.

Viewing a Wire Path Often, it is important to see where a particular wire is running through the assembly. You next use the View Path tool to highlight the segments that the wire is running through. View the path of a wire: 1. In the browser, under Wire Harness 1, expand the Wires folder so that you can view all the wires you have created. 2. In the browser, right-click wire 10015 and choose Find in Window. The graphics window zooms in so that you can see the two ends of the wire. 3. In the browser, right-click the wire 10015 again, and choose View Path. The wire stubs and the centerlines of the segments that the wire runs through are highlighted.

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Chapter 13: Designing Cables and Wire Harnesses

Viewing Segment Contents You can also view the contents of a segment by viewing the segment’s harness properties. View the contents of a segment: 1. In the graphics window, right-click one of the centerlines of the segments and choose Harness Properties. The Occurrence tab controls information about the segment like its browser name and diameter. 2. Click the Wires/Cables tab to view the wires that are routed through that segment. 3. In the Segment Properties dialog, double-click one of the wires to view its properties. The Cable & Harness module recognizes the relationships among all of these harness objects and enables you to navigate through them nongraphically. 4. Click Cancel to close each of the Properties dialogs.

Creating a Nailboard Drawing Nailboard drawings are automatically created by flattening the harness from the 3D representation in the assembly. The 3D curves are flattened into a 2D plane and are displayed in a 2D view on the drawing sheet. The 3D path determines the wire length, and the length can only be updated in the 3D model. Any changes made to the 3D harness will be automatically updated in the 2D nailboard drawing. Create a new 2D nailboard drawing: 1. On the Standard toolbar, click the New tool. 2. In the Open dialog, click the Metric tab and then double-click ISO.idw A new drawing with an A3-size sheet is created. 3. In the Drawing Views Panel bar, click the Nailboard View

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Chapter 13: Designing Cables and Wire Harnesses

4. In the Nailboard View dialog, ensure the selected file is set to Chapter 13_PCB Enclosure.iam and then click OK. This automatically creates a 2D drawing of your wire harness.

Property Display The property display tool allows you to selectively filter and display property names for the wire harness. Large harness drawings can be printed across multiple sheets of paper, or shortened to fit a single sheet, while still reporting their correct overall length. 1. On the Panel Bar, click the Property Display

tool.

2. In the Property Display dialog, select All Pins in the Selection Filter section and Pin Name in the Property Name list. 3. To zoom in on the harness drawing, click the Zoom Window tool and drag a selection box around the left end of the harness.

4. In the Property Display dialog, click Apply and click near the end of the pin to place the names on the drawing sheet. 5. From the Standard toolbar, click the Zoom All

tool.

6. With the Property Display dialog still open, select Object in the Selection Filter. In the graphics window, click on the long harness segment located on the left-hand side of the drawing (each individual segment will highlight as you move the cursor over it).

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7. In the Property Display dialog, select Segment Name under the Property Name list and click Apply. 8. In the graphics window, move your mouse just above the selected segment and click to place the segment name on the drawing. 9. Repeat the Object selection and Segment Name procedure to name the remaining two segments. When all segments have been named, click OK.

Harness Dimensioning You can use the Harness Dimension tool on the Nailboard Panel bar to add a driven, aligned dimension between two points. The two points can span wires and segments, but dimensions from a segment or wire to a connector are not allowed. 1. On the Nailboard Panel bar, click the Harness Dimension

tool.

2. To create the dimension, first select the center point at the left end of Segment 1. Next, select the center point at the right end of Segment 1. 3. Click just below the segment to place the dimension. 4. Repeat the dimensioning steps to add length dimensions to Segment 2 and Segment 3. 5. Right-click and select Done when finished dimensioning. 6. Right-click and select Finish Sketch to complete the drawing. 7. To save your drawing, on the Standard toolbar, click the Save dependents. Enter My_Nailboard.idw for the drawing name.

tool, click Save and OK to save

Chapter Summary Easily create and maintain your full-routed systems designs with Autodesk Inventor. By creating your wire harness in 3D, you can improve the quality and manufacturability of your entire product design.

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Conclusion We hope you have enjoyed your 3D design experience. This test drive only scratches the surface of the full capabilities of Autodesk Inventor. You now have 30 days to continue using Autodesk Inventor software before your trial version expires. Autodesk supports products through Autodesk Authorized Resellers, industry experts who offer consultation, training, support, and other related services to help meet your business needs. We encourage you to contact an Autodesk Authorized Reseller or your local Autodesk representative to learn how Autodesk Manufacturing Solutions can help you get to market faster and at a lower cost. To find an Authorized Autodesk Reseller in your area, call 800-964-6432 (United States and Canada only) or visit our website at www.autodesk.com/reseller. The Autodesk Inventor Team

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Top 10 Reasons to Move from AutoCAD to Autodesk Inventor 11 2D and 3D Tools You Need-Right Out of the Box Take advantage of all that Autodesk Inventor software has to offer, and get the best of both worlds with 2D and 3D design tools in one package. The Autodesk Inventor product line provides a comprehensive and integrated set of design tools. It includes Autodesk Inventor Series software for 3D design and documentation, Autodesk Inventor Professional products for creating routed systems and validating designs, AutoCAD® Mechanical for 2D drawing and detailing, and Autodesk Vault® software for data management. Autodesk Inventor also delivers a new ground-breaking modeling paradigm, Functional Design. Functional Design allows designers to move beyond geometric modeling and into an environment where they can focus on the problem they are trying solve rather than spending time solely on the 3D geometry required to build the design. Create better products, manage your design process, and share data with your extended design team with Autodesk Inventor-the best choice for AutoCAD users.

1. Automatic Drawing Views Dramatically reduce drafting time by automatically creating front, side, ISO, detail, section and auxiliary views of parts and assemblies from the model. Quickly annotate drawings by retrieving the dimension information directly from the design. Generate item numbers and part lists automatically. Complete the drawing using a robust set of dimension, annotation, and 2D symbols with full support for technical drawing standards, including GB, JIS, BSI, ISO, DIN, ANSI, and GOST.

2. Automatic Drawing Updates Change it once, change it everywhere. Autodesk Inventor associates drawing views to the original components so a change made to any part or assembly is automatically reflected in all associated drawing sheets. For example, with the intuitive 3D Grips functionality, you can quickly make changes to your model and all related drawing views will automatically update.

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3. Bill of Materials Manage the Bill of Materials (BOM) as you develop the design. With Autodesk Inventor, the BOM is an integral part of the assembly model that allows you to include purchased and non-purchased components including virtual items such as grease, paint, and glue. Autodesk Inventor automatically synchronizes BOM items with the parts lists and balloons in your drawings making it easier than ever to keep the drawings in sync with changes to the 3D model. By managing parts lists and quantity information in the Autodesk Inventor BOM you can easily provide accurate and up-to-date parts lists for purchasing and manufacturing.

4. Virtual Prototyping Building physical prototypes is expensive and time consuming. By creating a 3D model with Autodesk Inventor you can create and test a complete virtual prototype ensuring all parts fit correctly before you commit to manufacturing. Autodesk Inventor also includes tools to detect interference and other design errors reducing or eliminating the need for physical prototypes while delivering better products at a reduced cost.

5. DWG Interoperability As the creators of AutoCAD software, Autodesk understands your design process and created the Autodesk Inventor product line to make the move from 2D to 3D as easy as possible, preserving your investment in AutoCAD while simplifying your transition to 3D. If you are like thousands of companies across the world, you trust AutoCAD to create and revise production drawings. With Autodesk Inventor you can reuse existing AutoCAD geometry by copying and pasting your AutoCAD geometry directly into Inventor to begin creating a new 3D model. Every copy of Autodesk Inventor includes AutoCAD Mechanical-the industry’s leading 2D mechanical design solution so you will always have a real version of AutoCAD to edit your valuable DWG design data. AutoCAD Mechanical and Autodesk Inventor have been carefully integrated to support parallel 2D and 3D workflows, allowing you to open native Autodesk Inventor parts and assembly files in AutoCAD Mechanical and create

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drawings of your Autodesk Inventor design in a familiar AutoCAD environment. Best of all, when the design changes in Autodesk Inventor, the AutoCAD Mechanical drawing updates automatically.

6. Component Generators Save time with Autodesk Inventor Component Generators. Create parts and assemblies from real-world design parameters such as speed, power, and material properties allowing you to focus on design rather then geometric modeling. Autodesk Inventor includes component generators for bolted connections, shafts and hubs, o-rings, gears, belt and chain drives, and power screws and springs. The AutoDrop feature of Autodesk Inventor is fast, easy and accurate. It automatically adjusts the bolt diameter as you move the mouse over the hole and it lets you adjust the length based on the bolt sizes in the library.

7. Technical Documentation With drawing views, you can quickly create assembly drawings and exploded assembly views for use in training manuals and manufacturing instructions. With the Autodesk Inventor presentation environment you can easily create compelling animated sequences for use in training videos, assembly instructions, and sales presentations, helping you visually communicate your design intent.

8. Pipe and Cable Routing Autodesk Inventor Professional gives you the power to quickly and accurately add routed systems, tube and pipe runs, or cables and wiring harnesses to your 3D designs. Routed designs automatically comply with userdefined design rules to reduce errors and save time. And just

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like with all Autodesk Inventor files the assembly drawings automatically update whenever the routing model is modified.

9. Stress Analysis and Simulation Create better quality parts and avoid field failures by using the Finite Element Analysis (FEA) functionality in Autodesk Inventor Professional to determine the stresses and deflections under load. Use FEA to optimize part strength and reduce material costs without compromising performance. The Dynamic Simulation functionality in Autodesk Inventor Professional extends the benefit of your 3D prototype enabling you to predict the forces and accelerations experienced by each part in the assembly under real world conditions with timevarying loads, friction characteristics, and dynamic components such as springs and dampers.

10. State of the Art Rendering and Animation Autodesk Inventor Studio provides state-of-art rendering and animation tools within the Autodesk Inventor design environment. Use Autodesk Inventor Studio to quickly and easily create high-quality photo-realistic renderings and animations that improve communication with customers and other decision makers.

Now is the Time Now is the time to take a look at the Autodesk Inventor software and make the transition to 3D at your own pace. Protect existing 2D investments and work with the most DWG compatible platform available. For more information about Autodesk Inventor, go to www.autodesk.com/inventor. To locate the reseller nearest you, visit www.autodesk.com/reseller. Autodesk, AutoCAD, and Autodesk Inventor are registered trademarks or trademarks of Autodesk, Inc. in the USA and/or other countries. All other brand names, product names, or trademarks belong to their respective holders. Autodesk reserves the right to alter product offerings and specifications at any time without notice, and is not responsible for typographical or graphical errors that may appear in this document. © 2006 Autodesk, Inc. All rights reserved.

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