Pro E Guide

UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING

PART 1A CAD COURSE

HANDOUTS & EXERCISES

K.M. Wallace P.J.G. Long D. Underhill

Jan 2006

1

Notes for students 1. Course content The course comprises the 9 introductory lectures in LT1 followed by practical sessions in the Design and Project Office (DPO). It represents the second ‘half’ of the Part 1A Drawing Course and aims to give a introduction to the use of a modern CAD package (Pro/Engineer Wildfire 2) 2. Course timetable The timetable of exercises for the Lent and Easter terms is as follows (see the contents page for further details): LENT TERM Week 1&2

Morning:

Exercise 8:

Constructing Simple Components

Afternoon: Exercise 9: Week 3&4

Morning:

Intersections, Part Drawing (1) and Patterning

Exercise 10: Components and Part Drawing (2)

Afternoon: Exercise 11: Assemblies (1) and GA Drawings Week 5&6

Morning:

Exercise 12: Assemblies (2)

Afternoon: Exercise 13: Component Design Week 7&8

Morning:

Exercise 14: Dynamic Assembly (1)

Afternoon:

Deferral Session

EASTER TERM Week 1&2

Morning:

Exercise 15: Dynamic Assmbly(2)

Afternoon: Exercise 16: Sheetmetal The lectures for the course precede the scheduled morning and afternoon practical sessions. i.e. at 11.05 and 14.15 on Thursdays, and 09.05 and 14.15 on Fridays. 3. Practical sessions As with short experiments, you are required to attend the timetabled practical sessions and you must ensure that you have been signed-in by a demonstrator shortly after arriving in the DPO after the introductory lectures. 4. DPO drawing board/PC allocation Clusters of PC’s in the DPO are assigned to specific lab groups as indicated on the attached sheet. 5. Marking Each drawing lecture and practical is self-contained, and drawings or printouts should be marked by the end of each session i.e. the morning practical should be marked up by 13.00 on Thursdays and by 11.00 on Fridays, the afternoon practical should be marked up by 16.30 on both Thursdays and Fridays. All drawings or printouts must be posted into the IA Drawing ’postbox’ at the west end of the DPO by the end of the afternoon practical sessions. Each exercise is marked as a short experiment: 2 marks for prompt attendance and satisfactory work, 0 otherwise. All sixteen exercises must be completed to obtain the 32 marks required to qualify. See ’A Guide to the Engineering Tripos, PartI’ or web page: http://eng.cam.ac.uk/teaching/tripos/four year course guide-Part I.html for further details on Part I coursework marking. As is the practice with IA and IB computing practicals, the marked coursework will be retained and not returned. 2

IA Drawing and IA Computing marks are displayed in the DPO. Please check regularly that your marks have been entered. Contact Derek Underhill in DPO Office if you have any queries about your marks. 6. Demonstrators Demonstrators are available immediately after the lecture and throughout the practical sessions (Thursday mornings until 13.00 and afternoons until 16.30; and on Friday mornings until 11.00 and afternoons until 16.30). The demonstrators are primarily there to offer help and advice, though they also attend to signing in and marking up - PLEASE use their help if you need it - you will not be penalised. 7. Deferral Deferring one drawing exercise in the Lent term is possible if you elect to miss a session for any reason. Deferred exercises may be completed and submitted without penalty but should ideally be completed within the two week ’cycle’ of that particular exercise. If this is not possible, it must be done in the deferral session at the end of term. NOTE: exercises submitted after this date will not be accepted. Permission to defer a drawing exercise must be obtained beforehand from Derek Underhill by e-mail (du203). The email should state the session you wish to defer and list the alternative sessions you can make. 8. Allowance for illness For allowances for illness and other grave causes, see ’A Guide to the Engineering Tripos, Part I’ or web page: http://eng.cam.ac.uk/teaching/tripos/four year course guide-Part I.html.

3

4

Contents Introduction to CAD

11

1 Background

11

2 Overview of Pro/ENGINEER

11

2.1

2.2

Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12

2.1.1

Datum Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

12

2.1.2

Sketched (Base) Features . . . . . . . . . . . . . . . . . . . . . . . . .

12

2.1.3

Pick and Place (or Referenced) Features . . . . . . . . . . . . . . . .

13

Modification of Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

13

Exercise 8: Simple Extruded and Revolved Parts

15

1 Key

16

2 Getting Started

16

3 Creating a Part

17

4 Task 1 (a) - Extruded Section

17

4.1

Starting an Extrusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

17

4.2

Review/Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

20

4.3

Edit Profile Dimensions

. . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21

4.4

Save Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21

4.5

Print Screen . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

21

4.6

Exiting ProEngineer Wildfire . . . . . . . . . . . . . . . . . . . . . . . . . .

21

5 Task 1 (b) - Revolved Section

22

5.1

New part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22

5.2

Revolved Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

22

5.3

Edit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

23

6 Task 2 - Woodruff Key

24

6.1

Woodruff start . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

24

6.2

CUED Quick Start . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

24

6.3

Extruded Cut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

25

7 Task 3 - Keeper Plate

25

7.1

Open an existing file . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

25

7.2

Create a ‘Round’ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

26

5

7.3

Create a ’Chamfer’ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

26

7.4

Modify the Original Extrusion . . . . . . . . . . . . . . . . . . . . . . . . . .

26

8 Task 4 - Additional Components

26

9 Construction and Editing (aide-memoire)

31

Exercise 9: Intersections, Patterns and Part Drawing (1)

39

1 Key

41

2 Getting Started

41

3 Task 1 - Cylinder/ Domed-Cylinder Intersection

42

3.1

Start Domed-Cylinder . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

42

3.2

Quick Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

42

3.3

Cylinder Section

43

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

4 Task 2 - Initial Drawing

43

4.1

Start a Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

44

4.2

First View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

44

4.3

Additional Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

45

4.4

Display Centerlines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

45

4.5

Drawing Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

46

5 Task 3 - Cylinder/Dome Intersection

46

5.1

Cylinder 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

46

5.2

Intersection Drawing Review . . . . . . . . . . . . . . . . . . . . . . . . . . .

48

6 Task 4 - Parent/Child Relationships

48

6.1

Activate Domed-Cylinder

. . . . . . . . . . . . . . . . . . . . . . . . . . . .

48

6.2

Create a shell . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

48

6.3

Check Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

48

6.4

Reordering Model Tree . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

7 Task 5 - Mounting Flange

49

7.1

Extruded Flange Notes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

7.2

Revolved Flange Notes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

7.3

Mounting Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

49

7.4

Patterned Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

50

8 Drawing 2 (Updated) 8.1

50

Tidy Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6

51

8.2

Isometric View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

51

8.3

Printing a Drawing - for information ONLY . . . . . . . . . . . . . . . . . .

52

Exercise 10: Assembly Components and Part Drawing(2)

53

1 Key

54

2 Getting Started

54

3 Task 1 Pulley

55

3.1

Start Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

55

3.2

Base Shape . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

56

3.3

Belt Groove . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

56

3.4

Keyway . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

56

3.5

Fillets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

56

4 Task 2 - Shaft

57

4.1

Start . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

58

4.2

Base Shape . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

58

4.3

Woodruff Keyway . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

58

4.4

Hole . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

59

4.5

Cosmetic Thread . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

60

4.6

Fillets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

60

4.7

Edit Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

60

5 Task 3 2D Drawing of the Pulley

60

5.1

Setting the overall Drawing Scale . . . . . . . . . . . . . . . . . . . . . . . .

61

5.2

Sectioned Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

62

5.3

Tidy Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

63

5.4

Isometric View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

64

5.5

Printing a Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

65

5.6

Shaft Drawing

66

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Exercise 11: Component Assembly and GA Drawings

67

1 Additional Parts

68

2 Sub-Assembly

68

2.1

Start Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

68

2.2

Initial Component

68

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

2.3

Exit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

69

2.4

Keeper Plate . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

69

2.5

M12 Bolt . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

70

2.6

Simplification . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

70

2.7

Roller Bearing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

71

2.8

Woodruff Key . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

71

2.9

Pulley . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

72

2.10 Nut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

72

2.11 Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

72

2.12 Resume . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

73

3 Main Assembly

73

3.1

Tensioner . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

74

3.2

Sub-Assembly. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

74

3.3

Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

74

3.4

Remove Cut . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

75

3.5

Transparency . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

75

4 Drawing

75

4.1

Load Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

75

4.2

Datum Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

75

4.3

Section View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

76

4.4

BOM Ballons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

76

4.5

Additional View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

76

5 Modified Pulley (Optional)

77

5.1

Load . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

77

5.2

Thicken Flange . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

77

5.3

Mounting Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

78

5.4

Patterned Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

78

6 Drawing 2 (Optional) 6.1

78

Suppress . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

Exercise 12: Assemblies (2)

79

81 8

Exercise 13: Component Design

83

Exercise 14: Dynamic Assembly (1)

87

1 Dynamic Analysis

89

2 Dynamic Model Assembly

90

2.1

Crankshaft Sub-Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . .

90

2.2

Piston Sub-Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

91

2.3

Conrod Sub-Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

91

3 Manipulation of Dynamic Assembly

91

3.1

Manual Movement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

92

3.2

Automatic/Driven . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

92

3.3

Results Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .

93

Exercise 15: Dynamic Assembly (2)

95

1 Key

96

2 Getting Started

96

3 Task 1 - Static Assembly 1

97

4 Task 2 - Static Assembly 2

97

5 Task 3 - Dynamic Assembly of lift mechanism

98

6 Task 4 - GA drawing 2

98

Exercise 16: Sheetmetal

99

1 Key

100

2 Getting Started

100

3 Sheetmetal Fundamentals

101

4 Task 1 - Extruded Bracket

101

5 Task 2 - Adding an additional Wall 1

102

5.1

Flat wall . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102

5.2

2-D drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103

6 Task 3 - Robot Chassis

104

6.1

Solid Model of chassis

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105

6.2

Conversion of chassis to sheetmetal . . . . . . . . . . . . . . . . . . . . . . . 105

7 Task 4 - ‘Ripping’ the 3-D model

105

7.1

Insert ‘rips’ . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105

7.2

Second Drawing Sheet + Development . . . . . . . . . . . . . . . . . . . . . 106 9

8 Task 5 - Adding Tabs to the Chassis

106

8.1

’Flat Wall’ Tab . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106

8.2

Bend relief . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106

8.3

Drawing Update . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107

9 Task 6 - Copying Tabs

107

10 Task 7 - Predefined wall extensions

108

10

Introduction to CAD - (Pro/ENGINEER)

1

Background Methods of Recording, Transferring & Illustrating Design Information Method Freehand Sketching

System

Date

Still the basis for most designers

3000 B.C. +

Isometric 2D Drawing 2D CAD 2/3D CAD 3D Modellers

2

Current Cost Cheap

∼ 1800

Decreasing

Manual

∼1700

Increasing

Autosketch, CoCreate,Visio, ProCAD, etc

1960’s

upto £2000

AutoCAD, CADKey

1970’s

Up to ∼£3000

CATIA, Unigraphics, ProEngineer, IDEAS

1980 →

(PC Based - Solidworks, Solidedge, Pro/Desktop)

2000

upto ∼£100,000 upto ∼£5000

Overview of Pro/ENGINEER

Pro/ENGINEER (Pro/E for short) is a commercial CAD/CAM package that is widely used in industry. It is one of the newer generation of systems that not only offer a full 3-D solid modeller, in contrast to purely 2-D and surface modellers, but also has parametric functionality and is fully associativity. This means that explicit relationships can be established between design variables and changes can be made at any point in the modelling process and the whole model will be updated. The version used in this course is Pro/Engineer Wildfire 2 which has a new icon based user interface, a trend becoming more common in engineering applications. The method of constructing a model of an object is very similar to that followed in the production of a physical component. For example the manufacture of the shaped block in Figure 7:1 would start with the choice of construction environment, the selection of a piece of stock material followed by a series of manufacturing processes, e.g. milling, drilling, welding/sticking. Pro/E has direct analogues for most of these operations as various types of FEATURES which can be combined to generate a complete representation of a PART, Pro/E’s terminology for a single component. Features fall into three main categories, Construction, Sketched and Pick and Place.

11

Construction of a Part ProEngineer

Workshop Select stock

Sketch Initial

Material

Cross-section

Use Protrusion

Cutoff length of

(Extrude, Revolve etc)

Stock Material

to generate 3-D workpiece

Hole {P&P}

Turn. Mill, Drill, etc

Cut (Sketched) Round/Fillet (P&P)

Slot (Sketched)

to shape part

Use Pick and place, Sketched Feature to create finished part

Protrusion (Sketched) Chamfer (P&P)

Figure 7:1: Comparison of physical and Pro/E methods of part construction

2.1 2.1.1

Features Datum Features

These features are purely used as an aid to the construction of the part, a number of various forms are available the most commonly used are the: • Csys Coordinate systems which aid in the orientation of additional features and the assembly of the part in to subsequent assemblies. CSYS feature is normally the first feature in a part definition and is used as the basis for the placement of all subsequent features. • Datums These are an extension of the idea of construction lines as used on a traditional drawing. The most used type is a DATUM PLANE which allows a 2-D reference plane to be defined in space. Additional forms include DATUM AXES, DATUM POINTS and DATUM CURVES. It is normal to add three DEFAULT datum planes, immediately after the initial coordinate system, to effectively generate default x-y, x-z and y-z planes (called respectively Front, Top, Mid in the CUED standard part.) 2.1.2

Sketched (Base) Features

These features are so named because they all involve the use of the SKETCHER mode within Pro/E, (see below for more details on its use). The main features that use this functionality are: 12

• Extrude/Revolve (Protrusions) Using these features material can be added to/taken away from a part by sketching a cross-section and then extruding/revolving/sweeping the section to produce a 3-D solid/cut. A additive protrusion is normally the first non-constructional feature in a part, and is used to produce the base solid entity of the part. • Sweep/Blend These features allow the user to define more complicated protrusions with multiple cross-sections • Style/Wrap More advanced Surfacing and distortion features • Rib This allows the user to produce a thin rib or web. This is a specialised version of the protrusion function. 2.1.3

Pick and Place (or Referenced) Features

Pick and place features derive their form from existing geometry and do not need to be sketched e.g. HOLES, ROUNDS and CHAMFERS. The action to produce the required effect has been preprogrammed into Pro/E, thus only requiring the user to indicate the position of the operation on the existing model.

2.2

Modification of Features The parametric nature of Pro/E means that the

modification of features is relatively easy, individual features can be selected and the associated parameters/dimensions changed. However, it should be noted that Pro/E produces a HISTORY based model in which features can be dependant on one or more previous features for their definition, e.g. a chamfer on an edge generated by a cut or protrusion. These PARENT-CHILD dependencies mean that when a parent feature is modified its children are automatically revised to reflect the changes. Care should be taken not to remove references used by child features. In most cases it is best to leave in definition of Pick and Place features until the end of the design to reduce these problems. This has a parallel in physical construction where the adding of chamfers, rounds and holes etc is left as late as possible to reduce measurement difficulties.

13

14

Exercise 8 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This exercise gives a introduction to the use of an industrial standard solid modelling CAD package, Pro/Engineer Wildfire. Problem Use Pro/Engineer Wildfire to model the following parts: 1. A Cylindrical Spacer using (a) A extruded section. (b) A revolved section. 2. Woodruff Key using an extrude followed by a cut. 3. Keeper plate produced by modifying an existing object. (a spacer) 4. Non-functional Block Example to see how many features can be combined to achieve the desired result. N.B. Save your work at regular intervals and print out your work after each item has been competed to avoid clogging the printer at the end of the session. PLEASE MAKE SURE YOU HAVE PUT YOUR NAME, LAB. GROUP AND COLLEGE ON YOUR PRINTOUTS. THESE SHOULD BE PUT IN THE ’POST BOX’ ONCE THEY HAVE BEEN SIGNED UP.

15

1

Key

To aid in the use of this handout a number of conventions/fonts/abbreviations have been used to indicate the difference between keyboard entry, menu titles, menu items etc. These are listed below: Font Used

Item

Abbreviation

Action

Bold/Times:

menu item

LMB

Left Mouse Button

CAPITALS:

WINDOW/MENU TITLE

MMB

Middle Mouse Button

Italic:

Keyboard inputs

RMB

Right Mouse Button

Bold/Helvetica:

Hint

Menu items followed by a → indicate that the user should follow the input to a cascaded or flyout menu. N.B. In many cases the choices required are the default and therefore do not need to be individually selected. Central to the use of the package is the ability to obtain the best view of the object you are constructing, e.g. the orientation and the display mode. Access to commands affecting the display are concentrated under the View pull down menu and the top icon bar. In addition the orientation can be manipulated with a combination of the Ctrl/Shift keys and the mouse. Key/Mouse

Action

(N.B. The Ctrl key can normally be released once the action has been initiated.) Ctrl - Middle Mouse Button

Zoom in/out

- Middle Mouse Button

Spin

Shift - Middle Mouse Button

2

Translate

Getting Started • Close down unused programs, ProE imposes a large load on the system • Select Start from the main icon bar and then select Pro/Engineer Wildfire 2 from the Programs→3D Modelling submenu.

This will start the package, and set the working directory (where your files will be stored) to /userid/ProE/. Within this area are a number of predefined directories, ex8 11, ex12 13, ex14.., which will be used to store the work for each of the drawing exercises. To change to the directory for this exercise select FILE → Set Working Directory (or use the hotkey option cd) and then select the directory ex8 11 from the file browser window, close with OK.

16

3

Creating a Part

Use the LMB to select NEW PART icon ( ) on the top menu bar, this will start an automatic procedure to generate a new part using the default CUED settings. After a few seconds a menu will appear prompting for the name of a part, type spacer1 xxx123 (where xxx123 is your userid) and then press ENTER or click (LMB) on OK. This will initiate a procedure to set up the default coordinate system and datum planes (Front, Mid, Top) which will appear in the main window. N.B. The brown Datum icons ( toggle the display of datum features

) on the top icon bar can be used to

Cylindrical Spacer

Extruded Sketched X-section

(a)

(b)

Figure 8:1: (a) Example Cylindrical Spacer (b) ‘Extrude Tool’ used to generate Spacer

4

Task 1 (a) - Extruded Section

The ”Extrude” function, often used to generate an initial part (c.f. the concept of stock material in a workshop), is used to produce the basis of a cylindrical spacer, as shown in figures 8:1 (a) & (b).

4.1

Starting an Extrusion Create a base protrusion (stock material) by

selecting the Extrude Tool icon ( ’Extrude Dashboard’ (

) from the right hand icon-bar, this will initiate the ) just below the message window.

• Create a Section It is possible to use an exisiting sketch as the basis of a sketched feature, here however use the internal sketch option by RMB→Define Internal Sketch. This will open a SECTION window and a prompt in the message window to ”Select a plane or surface to define sketch plane”. Moving the mouse over the main window will highlight (in light blue) each of the possible sketch planes. 17

Section Menu

Using the LMB, select the plane FRONT when highlighted or the Model Tree window. Immediately the menu will be populated with default values and also indicated on the main window. 1. An arrow indicates the direction of view of the sketch plane The direction can be changed using the Flip button, in this example any direction will be suitable. 2. The sketchplane can be presented on the screen in any angle and a preferred orientation can be selected by using the reference and orientation menu items. In most cases ProEngineer makes an intelligent guess at the required orientation and therefore the default can be accepted. In this case choose the defaults, by selecting Sketch. N.B. Sketch is highlighted on a raised button in the menu and can thus be selected as the default option in the menu by pressing the MMB (with the pointer in the main window), see above. 3. Dimension References

Reference Menu

To automatically dimension any entity drawn the system needs a local dimensioning reference. When the sketcher mode is entered a REFERENCES window is displayed which lists the entities that have been choosen as default references and indicated in the sketching window by brown dash-dot-dot lines. 18

In this example the default references should be ‘F1(MID)’ and ‘F2(TOP)’ thus select (LMB) Close . Any further drawing on this plane will be referenced to this temporary coordinate system. (N.B. It can be useful at this stage to Deselect the Datum Plane icon to simplify display) 4. Sketching a Section

Figure 8:2: Initial sketcher mode layout. Using the sketch circle function, accessed via either the circle icon (3rd icon down) or by selecting the Circle entry on the floating menu (Opened by using the RMB while the pointer is over the main drawing window), draw two concentric circles, of arbitary size, centered on the intersection of the reference lines, see Figure 8:2. To draw a circle move the pointer, (modified to a cross once the circle function has been selected) over the intersection, click/select (LMB) to set the centre then drag the pointer and click/select to define the circle radius. Click LMB once to place circle, click MMB once to end the operation and to return to standard pointer. To delete unwanted items, select the entity (line will turn red) and then select delete by holding down RMB → Delete. Multiple entities can be selected by dragging a boundary using the LMB (Should artifacts be left on the window use VIEW → Repaint, the Repaint icon on the top menu bar ( ) or the hot-key sequences (CTRL) + R or vr) to refresh the screen. Note : (a) The pointer has ‘intellegence’ and snaps as it approaches an intersection/circle centre/line etc (b)Pressing MMB once while drawing an entity will abort the operation and return to the standard select option. Once drawn the system will allocate default dimensions to the entities, which are displayed in grey. The values are based on the screen resolution/setup and 19

any previous components of the part. (It is worthwhile spending some time familiarising yourself with the sketcher mode - add lines, rectangles etc and then delete them.) Although the dimensions for our spacer are not correct at this stage the sketch is complete and the sketcher mode can be exited be selecting the ‘Tick’ at the bottom of the side icon bar or from the pull-down menu SKETCH → Done. This changes the colour of the extrusion to a transparent yellow and re-enables the protrusion dashboard. • Solid/Surface (

)

Leave the default setting of the first and second dashboard icons, e.g. the ”extrude as solid” option (first icon) selected. • Depth (

)

The left depth icon allows the user to select details of the extent of the extrusion, accept the default (”Extrude from sketch plane by a specified depth value.”) Adjust the depth to 32 by chosing one of the following techniques: 1. Enter value in the field on dashboard 2. Selecting and dragging the square handle (small white square, on axis) on the extrusion in the main window. Note it can be difficult to acccurately choose a value using this technique. 3. Double clicking, with LMB, on the dimension in the main window and entering the required value. • Verify/Preview (

)

The defined feature can now be temporarily previewed by verify icon ( ), from the right hand end of the dashboard. If an error exists individual elements of the protrusion can be modified by re-selecting the appropriate icon. • Exit (

)

Once completed the protrusion can be accepted by selecting the tick ( Selecting the cross will cancel the generation of the feature.

4.2

). N.B.

Review/Display The Protrusion can now be rotated and/shaded to improve

the view of the feature. 1. Press the MMB to rotate the model. Use SHIFT and CTRL to zoom and pan. 2. Select Shading, Wireframe etc icons (

)

3. You can also reset the view and repaint it. These options are available by choosing VIEW pull down menu or from the icon bar ( )( ).

20

(a)

(b)

Figure 8:3: (a) Editing the Outer diameter (b) Edit Definition, selecting Edit internal sketch

4.3

Edit Profile Dimensions There are several ways of modifying a features

dimensions, including 1. Select the feature (Extrude 1) in the Model Tree or drawing screen, (Highlight protrusion feature in light blue and select with LMB) and then using the RMB select Edit. The defining dimensions are displayed in the main window, Select the value to be modified (double click LMB) and enter the value at the prompt. Modify the inner diameter to 13, the outer diameter to 40 and the length to 80. N.B. Dimension values switch from yellow to green when they have been modified. To action the modifications select Regenerate from the EDIT menu, the image will animate to the new dimensions. (N.B. The regenerate function can also be actioned by (a) Using the hotkeys rg (b) Selecting the Regenerate icon 2. Select the required feature and in the flyout menu (RMB) select Edit Definition which will return to the protrusion dashboard. Where the feature can be edited and previewed prior to regeneration. If required the section can be redefined by selecting RMB→Edit Internal Sketch.

4.4

Save Part Use the FILE → Save function or save icon (

) to save the part

in its current form.

4.5

Print Screen To record the current work, arrange the windows on the desktop

to show the main drawing window, with the part displayed, the MODEL TREE menu and ) from the top icon bar. When the mouse pointer changes to a cross then select ( click over the window and wait for a quiet beeb.

4.6

Exiting ProEngineer Wildfire If you need to exit ProEngineer, select

FILE→Exit. The system will then prompt the user to save each of the components, constructed to date, in turn. (To speed the exit process type either a or q (save all items or discard all items, respectively) at the prompt) 21

5

Task 1 (b) - Revolved Section

Cylindrical Spacer

Revolved Sketched X-section

Figure 8:4: Revolve Tool used to generate Spacer This example demonstrates an alternative method of producing a spacer, using a revolved cross-section to define the solid material. The procedure is very similar to the previous example and therefore less explanation has been included

5.1

New part Select the NEW PART icon again and name the new part spacer2 xxx123. (xxx123=userid) Selecting OK will set up the default datum planes as in the last Task 5.2

Revolved Feature Select the Revolve Tool icon (

) and then

systematically work from left → right along the dashboard • Section Use the internal sketch option (RMB → Define Internal Sketch) and choose FRONT as the sketch plane and accept the defaults for the direction, reference plane and orientation. Accept the default drawing references

Figure 8:5: Axis of rotation and cross-section for the revolved section. 22

To complete the section it is neccessary to define both the axis of rotation and the revolved section 1. To define the axis of rotation select RMB → Centreline to choose the centreline tool. To place select (LMB) the intersection of the reference line and drag and reselect vertically above to produce a vertical centreline aligned to the reference origin. 2. Use either the Rectangle or line functions to sketch one side of the spacer parallel to the axis of rotation, see Figure 8:5 By default the soft dimensions chosen by the system are shown as one radius + a thickness. To redefine dimensions, select the RMB → Dimension tool and then select the two ends of the dimension required and then MMB to place the dimension. 3. Exit the sketcher mode using the ‘Tick’ at the bottom of the side icon bar

(a)

(b)

Figure 8:6: (a) Use drag handles (white square) to dynamically adjust the angle of rotation (b) Preview of 360o revolved section • Edit Experiment using the drag handle to adjust the angle of rotation and then ensure that the dimension field is 360o.

The dimension pulldown menu has standard dimensions and recently used dimensions, useful when switching between trial values. • Preview ( • Exit (

5.3

) Use the Verify/Preview icon to check the completed revolved entity

) Exit the revolve tool

Edit . Using LMB to select and the RMB → Edit command change the inner

radius to 16, the outer radius to 35 and the length to 80. Do not forget to regenerate (select , Regenerate from the EDIT menu) or hotkey ‘rg’ to update the values. 23

Save Part Use the FILE → Save function or save icon (

) to the save the part in

its current form.

Print Display the main window and MODEL TREE menu on the screen and select the PrintScreen icon (

).

Woodruff Key

Circular Blank

Extruded Cut X-section

Extruded Sketched X-section

Figure 8:7: Two Feature construction (Extrusion - Cut ) used to generate Woodruff Key

6

Task 2 - Woodruff Key

This Task demonstrates the use of multiple sketched features to define a Woodruff Key

6.1

Woodruff start Select the NEW PART icon again and name the new part

woodruff xxx123.( xxx123=userid) → OK.

6.2

CUED Quick Start To produce the initial circular protrusion select the

CUED fast start option from the CUED menu, Extrude 2s, to start the sketcher mode for a two sided extrusion. . (Extrude 1s and Revolve 360 give similar quick starts for 1 sided extrusion and revolve respectively) Select the default drawing references by selecting Close or using MMB • Section Draw a single circle centred on the dimension references. Adjust the diameter to 16 mm, by double clicking on the dimension in the sketcher display and entering 16 at the prompt. Alternatively select the dimension with the LMB and then use RMB to access the floating menu, select Modify and use the resultant MODIFY DIMENSIONS window to adjust the value. Exit the sketcher mode using the ‘Tick’ ( ). • Depth Set the extrusion to a blind depth of 4. • Verify/Preview ( • Exit (

)

) Once complete exit the Extrude tool. 24

6.3 (

Extruded Cut The cut function is generated with the same extrude tool ) as the extrusion.

• Section Select the same plane as before as the sketching plane, and accept the defaults for the direction and orientation. Accept the default dimension references. Sketch an oversized rectangle covering the top section of the circular entity and set the centre-of-circle to base of rectangle dimension to 1.5 (above or below the centreline) and exit the sketch with ‘Tick’ ( ).

• Depth Set the extrusion to be a symmetrical two-sided, with a total depth of 8mm. ) Switch from a material extrude to a cut by selecting the cut icon (radio • Cut ( button down). • Preview (

) Use the Verify/Preview icon to check the completed revolved entity

• Cut (material) Direction ( ) if required, use the material direction function to swap the side of the section that is cut. • Exit (

) Exit the extrude (cut) tool.

Save Part Save the completed part using the save icon (

) or FILE → Save .

Print Display the main window and MODEL TREE menu on the screen and select PrintScreen (

7

).

Task 3 - Keeper Plate

This exercise demonstrates the reuse of existing data and use of ‘Pick-and-Place’ Features.

7.1

Open an existing file Use the FILE → Open or file open icon ( ) to activate the FILE OPEN selection menu. Select the part file spacer1 userid and OK. This will reopen the file with the previously saved parameters and place the window on the top of the desktop. 25

7.2

Create a ‘Round’ Selecting the round tool icon ( ) or (INSERT→Round ....) starts the ’round’ dashboard and a message prompt ‘Select an edge or chain of edges, or a surface to create a round set’.

• Radius Set the round radius to 3.5 mm. • Edges Although there are a large number of options, accept the defaults and using the highlight/select function select the two outer edges of the spacer. N.B. the most recently accepted edge is highlighted in red and is dynamically adjustable. • Review Check, preview and Exit round tool

7.3

Create a ’Chamfer’ The chamfer tool (

) operates in a similar manner to the round tool. Use it to add chamfers to each end of the bore.

• Style Select the chamfer style to 45 x D • Size Set D to 1.0 mm • Edges Select the two edges of the bore

7.4

Modify the Original Extrusion Select the original extrusion from the

main screen or the MODEL TREE and RMB → Edit the length to 9 mm.

Save A Copy Generate a new part using the FILE → Save A Copy... command save the modified file with the name Keeper userid

Print Display the main window and MODEL TREE menu on the screen and select PrintScreen. (

8

).

Task 4 - Additional Components

Experiment using the methods you have learnt so far modelling one or more entities similar to that shown in figure 8:8. Use the supplied isometric paper or plain paper to sketch the stages of various operations on the entities prior to trying to model them. 26

(a)

(b)

Figure 8:8: Non-functional Blocks. (a) Sketch using ‘isometric paper’ (b) Corresponding CAD model K.M. Wallace P.J.G. Long D. Underhill

Jan 2006

27

28

29

9

Construction and Editing (aide-memoire)

Base (Sketched) Feature Creation

• Select (RMB) required feature icon and wait for the dashboard to appear

⇓ • If an internal sketch is required, RMB→ Define Internal Sketch • Select (RMB) required drawing surface (typically a datum plane or existing surface) • Accept the default references or select and additional plane for orientation of the sketcher view.

⇓ • Accept (reset or augment) the sketching references • Sketch required section • Exit sketcher with tick • Select OK from the sketch menu to return to the dashboard. (N.B. Selectable with MMB as it is the default option)

⇓ • Set additional feature parameters (typically work from left → on dashboard. • N.B. Additional options available from the pull down menus below the dashboard icons

⇓ • Preview the feature to allow the system to check the feature’s parameters fully before accepting the feature • Click resume to return to the dashboard or the tick/X to exit the feature creation. 31

Methods for Editing a Feature EDIT • Select a feature. (N.B. If the model is complicated it can be easier to select in the model tree) • Use RMB to select Edit, shows all the dimensions used to define the feature in yellow in the main drawing window. • Use double click select to an dimension and then edit the value in the edit box. (Dimension will change green once it has been edited) • To action edit(s) select the regenerate icon, or use the hotkey rg EDIT DEFINITION • Select a feature. • Using RMB to select Edit Definition, returns the system to the feature definition dashboard. • Modify/Select feature options/parameters as if defining the initial feature. (N.B. Some changes may effect child features or references used by other components in an assembly) • Preview the changes and re-edit required • Exit the feature redefinition using the tick icon EDIT INTERNAL SKETCH • Select the main feature (or internal sketch from the menu tree) and RMB → Edit Definition returns the system to the feature definition dashboard as above. • Selecting RMB→Edit Internal Sketch over the main window or Sketch→Edit from the dashboard PLACEMENT menu returns the system to the SKETCH menu. • Selecting sketch initiates the Sketcher mode with the original settings. • Edit the sketch as required and exit using the Tick. (N.B. Deletion/modification of a line may cause child features to fail if they 32 are used as a reference.)

38

Exercise 9 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This exercise introduces some extensions to the techniques learnt in the previous lesson to model a water fitting. In addition, the the method of generating 2D drawings is introduced. Problem 1. Cylinder/Domed-Cylinder Intersection 2. Initial Drawing 3. Extrusion using an auxiliary plane 4. Update Drawing Note the changes in the drawing and update the dimensions on the drawing. 5. Parent/Child Relationships 6. Flange and Patterned Holes PLEASE MAKE SURE YOU HAVE PUT YOUR NAME, LAB. GROUP AND COLLEGE ON YOUR PRINTOUTS Overleaf are a number of questions designed to test your understanding of the tasks. The questions can be be answered during or after the whole exercise, but it is useful to refer to them as you undertake individual tasks.

39

Questions 1. Why do the two cylinders act differently when shelled? • Rearrange Protrusions/Shell Features Select (RMB) individual features (e.g. the extrudes and shell) and attempt to rearrange the order by dragging and dropping them in the Model Tree. 2. Why can you not place the shell before all the protrusions? 3. Why can one of the plain protrusions be placed before the domed cylinder and not the other? 4. Why does the flange have to be added as an additional feature rather than as part of the first revolve with this type of model construction? 5. Why is the first of the mounting holes set at 55o and not 0o ? (N.B.) Write your answers on the back of your last drawing.

40

1

Key

To aid in the use of this handout a number of conventions/fonts/abbreviations have been used to indicate the difference between keyboard entry, menu titles, menu items etc. These are listed below: Font Used

Item

Abbreviation

Action

Bold/Times:

menu item

LMB

Left Mouse Button

CAPITALS:

WINDOW/MENU TITLE

MMB

Middle Mouse Button

Italic:

Keyboard inputs

RMB

Right Mouse Button

Bold/Helvetica:

Hint

Menu items followed by a → indicate that the user should follow the input to a cascaded or flyout menu. N.B. In many cases the choices required are the default and therefore do not need to be individually selected. Model Manipulation Key/Mouse

Action

(N.B. The Ctrl key can normally be released once the action has been initiated.) Ctrl - Middle Mouse Button

Zoom in/out

- Middle Mouse Button

Spin

Shift - Middle Mouse Button

2

Translate

Getting Started

To start Pro/Engineer Wildfire login to the teaching system and • Close down unused programs, Pro/E imposes a large load on the system • Select Start from the main icon bar and then select Pro/Engineer Wildfire 2 from the Programs→3D Modelling submenu. This will start the package, and set the working directory (where your files will be stored) to /userid/ProE/. Within this area are a number of predefined directories, ex8, ex9, ..., which will be used to store the work for each of the drawing exercises. To change to the directory for this exercise select FILE → Set Working Directory (or use the hotkey option cd) and then select the directory ex8 11 from the file browser window, close with OK.

41

Figure 9:1: Construction of the initial revolved feature and first extrusion

3

Task 1 - Cylinder/ Domed-Cylinder Intersection

Using the techniques described in exercise 8, produce a domed-ended cylinder, see Figure 9:1, intersected by a second cylinder.

3.1

Start Domed-Cylinder Select the NEW PART icon again and name the

new part water fitting1 xxx123 → OK. (xxx123=userid)

3.2

Quick Feature To produce the domed-cylinder protrusion select the fast start

option from the CUED menu, CUED → Revolve360, which sets up the sketcher mode for a revolved extrusion. • Domed-Cylinder Section 1. Insert a vertical centreline/axis-of-rotation vertical aligned to the vertical reference (From the ‘line’ pullout menu or RMB → Centerline). 2. Draw a half section of the cylinder, and set the defining dimensions to be a base diameter of 75 mm, a dome radius of 37.5 mm and an overall height of 100 mm. N.B. To override the default radius dimension and generate a diameter is a 4 click operation. Using the dimension tool select (1) a base corner of the cylinder (2) the centreline (3) the corner again and finally MMB to place 3. Exit Exit the sketcher mode using the ‘Tick’ (

)

) Accept Use the default 360o revolution, check the 4. Preview/Exit ( completed entity and exit with the ( )

42

Figure 9:2: Sketcher layout of cylinder

3.3

Cylinder Section Generate a intersecting cylinder by using the extrude tool

to generate a protrusion from the MID datum plane. • Start Extrusion (

)

1. Select the MID plane as the sketching plane and accept the default directions 2. Accept the default dimension references (REFERENCES →Close) • Cylinder Geometry Sketch a small circle in approximately the right position and then dimension as shown in Figure 9:2, i.e. horizontal offset 20 mm, diameter 15 mm, vertical position 20 mm and then exit the sketcher mode. • Depth Set the extrusion to a blind depth of 75 mm. • Preview and Accept (

,

).

If the screen becomes confused due to incorrect redrawing, select VIEW→Repaint, the repaint icon ( ) or ’vr’ to refresh the display

Save Part Use the FILE → Save function or (

) to save the part in its current

form.

Print Display the main window and MODEL TREE menu on the screen and select (

4

)

Task 2 - Initial Drawing

Even though the direct link from CAD to CAM (Computer aided manufacture) is increasingly common there is still a need to produce 2-D drawings, in Pro/Engineer this is 43

a relatively painless procedure as the hard work has already been completed in the model generation. In addition, when constructing a model it is often useful to be able to see a standard set of orthogonal views of the object or assembly being drawn. The drawing can aid with visualisation and with design, a pencil sketch on paper is often faster than the generation of complex CAD constructions when trying to get a feel for orientation, and sizing etc. The advantage of the associativity of packages like Pro/Engineer mean that as features are added or dimensions changed the model and drawing are both updated

4.1

Start a Drawing (By default the system attempts to draw the currently

active solid model, so to draw the water fitting, ensure that this is selected. If required reselect the window, use the WINDOW menu, or reload/open the model) To open a new drawing select FILE→New→drawing. Enter the name of the drawing, wfitting and select OK The NEW DRAWING menu should now appear, ensure that the default model field is water fitting.prt, ensure the Empty with format option is selected and the format field is a4 part.frm. (Use the browse facility if required) Selecting OK will initiate the drawing window.

Figure 9:3: Initial General View and Orientated of master view

4.2

First View To generate and locate the first view

• Insert View select RMB → Insert General View or INSERT →Drawing View → general. • Placement The user is now requested to choose the location for the master view by a prompt in the message window ‘select CENTER POINT for drawing view. Selecting (LMB) a position near the bottom right of the drawing surface will result in a default (isometric) view being placed followed by the opening of the DRAWING VIEW window, see Figure 9:4, set in the VIEW TYPES mode. • View Orientation The Orientation functions can be used to obtain the direction of a view. A number of predefined named views are available and normally enable the 44

Figure 9:4: Setting initial view orientation initial view to be placed simply. See the scrollable list shown when the views names in model option is selected. A suitable master view for this drawing is probably FRONT or BACK, select the view e.g. Front and then Apply. Review and correct if required. Select OK to exit back to the drawing.

4.3

Additional Views Additional views can now be added, with the view

orientated automatically. Using the default menu choices add two more views to your drawing. • Add View Select the view you wish to project from using the LMB, the view will be highlighted with a dashed red box. Use RMB → Insert Projection View, ( ) or INSERT →Drawing View →Projection to initiate the generation of new views. N.B. If an existing view is selected the system assumes that the next view required is a projection. • Placement Use the LMB over the drawing area to select the position of the two views, the system will ensure that the correct projection is shown. • Relocate views Using LMB to select a view (highlighted in with a red box) and then holding LMB down drag the view to the required location. Select with LMB in a clear area of the drawing to deselect a view. (If the view does not move deselect the Lock View Movement option from the RMB context sensitive menu) • Set Display mode Select the Hidden Line display option ( ) on the icon bar and deselect the datum icons to display a clean drawing. N.B. No Hidden (and Wireframe) can be used if required.

4.4

Display Centerlines Select VIEW → Show/Erase or (

) to open the

SHOW/ERASE window. Select the axis icon and Show All, see Figure 9:5(a), confirm ‘Are you sure that you want to show all?’ and then Accept All 45

Figure 9:5: (a) Show-Erase Menu (b) Accept All

4.5

Drawing Dimensions To dimension the drawing use the same ‘Show and

Erase’ function ( ) as above (section 4.4). Select show ( ( ) → ShowAll → Accept All.

) and dimension

N.B. there may be duplicate or superfluous dimensions, these can be deleted by selecting RMB→Delete.

Print Display the main window and MODEL TREE menu on the screen and select Print Screen (

5

).

Task 3 - Cylinder/Dome Intersection

In this task the extrude function is used with an auxiliary plane together with a non-blind depth. The cylinder intersects with the domed-end of the main cylinder and extends to 75mm from the centerline. Figure 9:6 is an incomplete version of the drawing, sketch your estimate of the line of intersection on each of the views, denote hidden lines of intersection as dashed line. Check your answer once you have completed the next section.

5.1

Cylinder 2 The generation of the offset extrusion, (i.e. starting from a plane

‘offset’ from another plane) is very similar to the that of a normal extrusion but with the additional requirement of defining an new datum plane. Start an extruded feature with ( ) or INSERT → Extrude .... • Generate section When prompted to ‘Select a plane...’ a new plane is required : 1. choose the Datum Plane Tool (

) from the side tool bar.

2. Select the FRONT plane to complete the Reference in the DATUM PLANE→Placement window that opens 3. Set the Offset (Translation) to 75 mm → OK 4. Check (modify) the Sketch Orientation and then exit the SECTION window. 46

Figure 9:6: Incomplete drawing of the second extrusion intersection 5. accept the default dimension references 6. Sketch a second protrusion, diameter 35 mm and tangent to the top of the dome. The tangent constraint can be achieved either by adjusting the dimensions or using a fixed constraint which adapts to future changes in dimensions etc. To fix an tangent constrain select the constraint menu icon ( ) and then the tangent constraint icon ( ). Selecting the top of the dome and the circle of the cylinder will force a tangent constraint

Constraint Actions Make lines vertical

Make lines horizontal

Perpendicular

Tangent

Point in the middle of line

Align line/point

Symmetry about C-line

Equal lengths

Parallel

7. Exit the Sketcher Mode with ‘Tick’. • Depth select Upto Surface (

), see Figure 9:7(a).

• Direction Ensure the extrusion is towards the existing model, us ( 47

), to flip.

(a)

(b)

Figure 9:7: (a) Set Material Depth (b) Completed Modified fitting • Preview and Accept (

,

).

N.B. The combination of the datum plane and extrusion are combined as a Group, see the MODEL TREE. The group can be expanded to allow edit access to the individual features. The group (as can other features) can be renamed with select RMB→Rename

5.2

Intersection Drawing Review re-activate the ‘wfitting’ drawing and

after selecting no-hidden

Save and Print Screen

6

Task 4 - Parent/Child Relationships

Pro/Engineer is a history based CAD package, where features can be dependant on previous features.(N.B. In most case, all features are children of the initial datum planes.) In this task the modified domed-cylinder is ‘shelled’ and the position of the shell operation/feature is moved in the model tree.packages.

6.1 Activate Domed-Cylinder Ensure that the Water Fitting window is active, select via the WINDOW pull-down menu. 6.2

Create a shell Activate the shell tool, (

) or INSERT → Shell ....

Select (LMB) the flat surface at the base of the domed-cylinder, (note the selection filter, at the bottom right of the window, switches to surface). Complete the shell by setting the (wall) thickness to 3.0 mm. ( , ) when complete).

6.3

Check Drawing Reload the Drawing window, and note that the drawing has

been updated. 48

6.4

Reordering Model Tree Select the shell feature in the MODEL TREE

menu and the drag/drop, in the tree, before the various protrusions. Note the effect after each insertion.

Figure 9:8: Water fitting with mounting flange

7

Task 5 - Mounting Flange

The water fitting is designed to bolt to the end of a pipe with a flanged-joint. Using either a extrude or a revolved section add an additional 20 mm thick x 120 mm OD flange to the base of the domed-cylinder, see Figure 9:8, together with 4 x φ10.5 mm holes equi-spaced on a 100mm PCD.

7.1

Extruded Flange Notes

1. Although it may be possible to use an existing datum plane as the sketching plane it is recommended to use the end of the domed-cylinder. This will ensure that the flange remains attached if the cylinder length is altered. 2. Make the internal radius of the flange identical to that of the domed-cylinder by using the ’equal dimension’ constraint. ( )

7.2

Revolved Flange Notes

1. In order that the flange is always attached to the end of of the domed-cylinder, even if its dimensions are changed, ensure that (a) The attachment edge is ‘aligned’ to the end of the cylinder (b) The inner diameter is aligned to the inner diameter of the cylinder, as generated by the shelling operation.

7.3

Mounting Holes Use the Hole Tool (

diameter clearance hole. 49

) to model a simple φ10.5 mm

Hole Type Select a Simple Hole Hole Dimensions

Set the Diameter to 10.5 mm Depth - Upto next surface ( ) This option ensures the hole depth will be automatically adjusted if the surface is moved, e.g flange thickness is changed.

Hole Placement

1. Select a point on the flat surface of the flange. 2. Select Placement Type Radial 3. Highlight the second reference field and select the axis of the domed cylinder unit as the Axial Reference 4. Set the Radius, (PCD/2) to 50 mm 5. Using and LMB, select a datum plane (typically FRONT or TOP) as the angular reference and set the angle to 55o .

7.4

Patterned Holes The previous section (7.3) defined a simple hole on a PCD

offset at an angle (55o ) from a datum. This angle can now be used to duplicate the holes. Select hole feature from the model tree or from the main drawing window and then using RMB → Pattern (or EDIT → pattern) activate the Pattern dashboard. 1. In response to the request to ‘Select dimensions to vary in the first direction’ select the offset angle of 55o. (It may be necessary to rotate the model around to see this dimension clearly.) 2. A prompt will now appear requesting the dimension increment, enter 90. 3. At the Number of Pattern Members (1) field (second from left) enter 4 Exit the dashboard ( ) and after a few seconds the pattern should appear on the part and in the MODEL TREE.

8

Drawing 2 (Updated)

Reselect the window containing the drawing, and see that the drawing has been updated. 50

8.1

Tidy Drawing The position of symbols and text can be moved using the

LMB to select a item which can then be dragged to the required position. MMB to stop, LMB to exit move. A large number functions are available via the RMB context sensitive menus, see Figure 9:9, and from the INSERT and FORMAT menus. (See FORMAT → Decimal Places.. to change default number display and therefore implied accuracy)

(a)

(b)

(c)

Figure 9:9: Examples of context sensitive Pull out Menus, (a) On background (b) On selection of 1 dimension (c) Multiple dimension selection Use the functions, details about some are given below, to tidy the dimensioning etc. (Also see Figure 9:10) • Cleanup Dimensions: Multiple selection → RMB automatically aligns dimensions on a user definable spacing. • Move Item to View: Single or Multiple selection allows dimension etc to be switched between views. • Flip Arrows: Single or Multiple selection allows dimension arrows to be realigned • Properties (Background): Allows sheet/layout to be changed • Properties (Single): Change value, format, font etc. • Text Style: Change text in multiple dimensions etc.

8.2

Isometric View The advantage of CAD is that it is relatively easy to add

additional views. It is often useful to add an Isometric view to aid visualisation. To add a general view select RMB → Insert Drawing View or ( ) Accept the default settings, except choose General instead of Projection, and Scale instead of No Scale. Place and orientate the view in a blank part of the drawing, see Figure 10:15.

Print Display the main window and MODEL TREE menu on the screen and select Print Screen (

). 51

Figure 9:10: Example of a dimensioned drawing of the completed water fitting

8.3

Printing a Drawing - for information ONLY **** USE Print Screen for this exercise (see above)****

N.B. By default the system prints the drawing that is visible on the screen, To print the whole drawing either select VIEW→ ORIENTATION → View Refit or use LMB + CTRL to zoom to the required view. • Select the printer icon or Print from the File pull down menu. • Select Generic Postscript • Enter printer command, e.g. lp -dljmr1 for the laser printer on the teaching system.

K.M. Wallace P.J.G. Long D. Underhill

Jan 2006

52

Exercise 10 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction These tasks build on the experience gained in Exercises 8 and 9, to model two components of the belt tensioner assembly drawn last term. The simplicity and power of CAD is then used to modify the pulley and produce an detail drawing. Problem Use ProEngineer Wildfire to model draw the following sample parts: 1. Pulley 2. Shaft 3. Drawing of the Pulley 4. Drawing of the Shaft N.B. Save your work at regular intervals and print out your work after each item has been completed to avoid clogging the printer at the end of the session.

53

1

Key

To aid in the use of this handout a number of conventions/fonts/abbreviations have been used to indicate the difference between keyboard entry, menu titles, menu items etc. These are listed below: Font Used

Item

Abbreviation

Action

Bold/Times:

menu item

LMB

Left Mouse Button

CAPITALS:

WINDOW/MENU TITLE

MMB

Middle Mouse Button

Italic:

Keyboard inputs

RMB

Right Mouse Button

Bold/Helvetica:

Hint

Menu items followed by a → indicate that the user should follow the input to a cascaded or flyout menu. N.B. In many cases the choices required are the default and therefore do not need to be individually selected. Model Manipulation Key/Mouse

Action

(N.B. The Ctrl key can normally be released once the action has been initiated.) Ctrl - Middle Mouse Button

Zoom in/out

- Middle Mouse Button

Spin

Shift - Middle Mouse Button

2

Translate

Getting Started

To start ProEngineer Wildfire login to the teaching system and • Close down unused programs, ProE imposes a large load on the system • Select Start from the main icon bar and then select Pro/Engineer Wildfire 2 from the Programs→3D Modelling submenu. This will start the package, and set the working directory (where your files will be stored) to /userid/ProE/. Within this area are a number of predefined directories, ex8, ex9, ..., which will be used to store the work for each of the drawing exercises. To change to the directory for this exercise select FILE → Set Working Directory (or use the hotkey option cd) and then select the directory ex8 11 from the file browser window, close with OK.

54

Figure 10:1: Section of the basic Pulley

3

Task 1 Pulley

Generate a model of a pulley, see Figure 10:1, using the following constructional steps. (The pulley is identical in size to that used in Exercise 7, and will be used again in Exercise 11.) 1. Revolve general shape 2. Revolve a cut to generate the belt groove 3. Use a ‘both’ sided cut to produce the keyway 4. Add fillets (Round tool)

3.1 Start Part Use the New Part ( pulley xxx123 (xxx123 = userid)

) function to start a part called

13 25 5

Ø100 Ø36 Ø20

(a)

(b)

Figure 10:2: Basic Pulley Section. (a) Section Dimensions & (b) Finished protrusion 55

3.2 (

Base Shape Use the CUED → Revolve 360 tool or the basic revolve tool ) to generate the basic pulley shape, Figure 10:2(a) for dimensions.

Occasionally it can be difficult to resize a complex sketch, where the system has choosen oversized dimensions. Select all the dimensions and RMB → Modify. Select Lock Scale and adjust one dimension to keep the general shape. 3

3

15°

15°

Ø64

(a)

(b)

Figure 10:3: Belt groove. (a) Dimensions & (b) Pulley with the basic cut.

3.3

Belt Groove Again use the revolve tool, with the remove material option, to

generate the base shape of the belt groove in the pulley, see Figure 10:3.

1.8 (Depth 4mm) Cut Section

(a)

(b)

Figure 10:4: Keyway. (a) Dimensions & (b) Finished keyway

3.4

Keyway Use the extrude tool, (

) with the remove material option, to generate the keyway, Figure 10:4. Draw the section oversize and only modify the one ) for depth, by default critical dimension. Use the ‘ Extrude on both sides...’ option ( this sets the extrude depth symetrically about the sketch plane.

3.5

Fillets Use the round tool, ( ), to insert four 4 mm rounds in the groove and at the end of the pulley, see Figure 10:5(a). Use LMB select on the second and subsequent edge selections to ensure that all the rounds are part of one set, and are driven by one dimension 56

R4

R4

R4

(a)

(b)

Figure 10:5: Casting/Machined Fillets (a) Fillet Positions (b) Finished Pulley

Print an image of the completed pulley, using the Print Screen command ( N.B. Arrange the windows on the screen so that the main window and model tree are visible. Position the cross pointer over the window and select with the LMB.

Save the model using the FILE →save, (

) or hotkey sequence sw, (Save Window).

Figure 10:6: Shaft

4

Task 2 - Shaft

Generate a model of the main shaft, see Figure 10:6 using the following constructional steps. 1. Revolve general shape 2. Use a ‘both’ sided cut to produce the keyway 3. Create a coaxial threaded hole 4. Add Cosmetic thread 5. Add fillets (Round function) 6. (Correct overall dimensions) 57

).

16

15 (150)*

16

42

22

(See Note)

Ø32

Ø25 Ø20

Ø25

Ø16

(a)

(b)

Figure 10:7: Basic Shaft. (a) Section dimensions & (b) Extrusion

4.1

Start a new part shaft xxx123 (xxx123 = userid)

4.2

Base Shape Use the CUED → Revolve 360 function to generate the basic

shape, see Figure 10:7 for dimensions. Exaggerate the initial sketch, do not try to draw the shaft to scale. When the section is complete and the required dimension locations chosen use, either a critical dimension and the scale hint given above or accept the section and edit the dimension values in the main window. N.B. Leave the central section at 15 (NOT 150) at this stage to aid future modifications and screen manipulation. 46

ø16 (Depth 3.5 mm)

13

(a)

(b)

Figure 10:8: ‘Woodruff’ Keyway. (a) Section dimensions & (b) finished keyway

4.3

Woodruff Keyway Using a similar technique to that used to produce the

keyslot in the pulley, generate a slot for a ‘Woodruff’ key in the shaft. Drill Ø10.2, 30 Deep Tap M12x1.75, 24 Deep

Hole Placement and Dimensions

Finished construction 58

4.4 Hole Use the hole tool ( ) to generate a threaded hole in the end of the shaft, Figure 10:9 shows the hole dashboard.

(a)

(b)

Figure 10:9: Hole dashboard. (a) Placement options & (b) Shape Options Adjust the hole parameters as below, note the use of the additional placement menu to change the default ‘linear’ placement to ‘coaxial’: Hole Type

Standard Hole, ISO, Tapped Hole, M12 x1.75 , Add Thread Surface, (Deselect Add Countersink)

Hole Dimension

Leave as defaults, i.e. Thread depth = 24.48, Hole Depth=30.6, Internal angle 118.

Hole Placement

Choose the shaft end with a single step as the Primary Reference, i.e. surface from which the hole starts. Select Placement Type Coaxial and then select the Secondary references menu and then select the axis of the shaft as the Axial Reference, using LMB.

Select Preview, (edit if required) and ‘Tick’ to complete.You will notice that the threaded portion of the hole is indicated in purple in the wireframe mode. This is described as a cosmetic feature as it indicates the position but not the full details which would require significant graphical processing. N.B. A note is added to give information about the threaded hole. To switch this off select TOOLS → Environment and then deselect 3D Notes( hotkey ’3d’.

Figure 10:10: External Thread - Cosmetic thread function

59

) or use the

4.5

Cosmetic Thread To add a cosmetic thread to the pulley end of the shaft

create a cosmetic thread on an existing surface use INSERT → Cosmetic → Thread. This will initiate a Cosmetic Thread definition menu requiring the following elements to be defined. Thread Surf

Select the cylinder surface on which the thread will run

Start Surf

End of the shaft

Direction

Along the shaft (use Flip if required)

Depth Major Diam

Blind → DONE and 20 long Enter 18

Note Params By default the system tries to create an internal thread, select Mod Params from the FEAT PARAM menu and then modify the thread placement definition to A (external) in the Pro/Table spreadsheet. Select Save and then Exit from the Pro/Table pull down File menu. Then Done Return. Preview / re Define / OK the cosmetic thread.

Fillets - ‘Rounds’ function R1 R1

R1

Fillet Positions

4.6

Finished Shaft

Fillets Place three 1 mm rounds (Fillets) on the shaft to reduce the stress

concentration, using the default settings for the round tool. (Use to choose multiple edges)

4.7

Edit Dimensions Now that the feature definitions are complete, use the

Edit command to change the central section of the shaft from 15 mm to 150 mm. Notice the additional scrolling etc required to obtain views at large scales.

Print Arrange the windows on the screen and print a copy. Save the model.

5

Task 3 2D Drawing of the Pulley

Use the techniques learnt in exercise 9 to generate a 2-D drawing of the pulley. 60

Figure 10:11: Dimensioned drawing of the Pulley

Start a Drawing To open a new drawing select FILE→New→drawing. Enter the name of the drawing, pulley and select OK The NEW DRAWING menu should now appear, ensure that the default model field is pulley.prt, ensure the Empty with format option is selected and the format field is a4 part.frm. (Use the browse facility if required) Selecting OK will initiate the drawing window.

First View Generate and locate the first view • Insert View select RMB → Insert General View or INSERT →Drawing View → general. • Placement Place a general (isometric) view (‘select CENTER POINT for drawing view’) • View Orientation Orient the view as required using the predefined view names, e.g.Front. • Scale, Display type etc Adjust as required, see next section.

5.1

Setting the overall Drawing Scale To change the overall scale of a drawing double click LMB on the scale information at the bottom left of the main window. At the prompt line enter the value you require, 1.0 is a suitable scale for this drawing.

N.B. Normally drawings scales are limited to multiples of standard scales, e.g. 1:1 1:2 1:2.5 1:4 1:5 (1, 0.5, 0.4, 0.25, 0.2)

Additional Views Again using the techniques used in exercise 9 add additional views, to recap:61

• Add View Select the view you wish to project from using the LMB, the view will be highlighted with a dashed red box. Use RMB → Insert Projection View, ( ) or INSERT →Drawing View →Projection. • Placement Use the LMB over the drawing area to select the position of the two views, the system will ensure that the correct projection is shown. • Relocate views Use the LMB to select a view (highlighted in with a red box) and then holding LMB down drag the view to the required location.

Figure 10:12: Drawing View/Sections menu completed for a half section view similar to that in figure 10:11

Display Centerlines Add centerlines to the drawing. Select VIEW → Show/Erase or (

) to open the SHOW/ERASE window.

Select the axis icon and Show All, confirm ‘Are you sure that you want to show all?’ and then Accept All

Drawing Dimensions Add the basic dimensions the drawing using the ‘Show and Erase’function ( ) as above. Select show ( ShowAll → Accept All.

) and dimension (

)→

5.2

Sectioned Views As ProEngineeer is a solid modeller it can be used to automatically generate cross-sections. To change an existing view to a cross section • Drawing View Select the view you wish to change and use RMB → properties to start the DRAWING VIEW menu. • Sections Selecting the menu option Sections will open the SECTION Options sub-menu. • 2D Section Selecting the option 2D cross-section and then pressing the add icon activates the section table. Selecting create opens the XSEC CREATE menu. Accept the defaults (Planar, Single and Done). 62

• Section Name At the prompt enter the name for the section, normally a single letter, e.g. X. N.B. Parts started with the CUED new part function will have sections A,B and C predefined and the system will by default choose the most appropriate. A is defined on the FRONT plane, B - MID and C - TOP • Section plane The system now prompts the user for the plane of section via the SETUP PLANE menu. Using the default option Plane select the plane of section you require. Normally a datum plane in an adjacent projected view, this is from ease of selecting and stability of the drawing should an associated dimension be changed in the model. • Section Area The system offers a number of standard sectioning techniques, Full, Half, Local, Full (Unfold) Full (Aligned) (Only the Full, Half,and local options are considered here). Each require various amounts of additional information to be completed. Details of the options required are: 1. Reference and Boundary These options are only used for the Half and Local section options. In the Half section option the Reference is used to define the plane at which the section begins, the boundary option defines which side of the line is sectioned. The Local section option allows small areas to be sectioned, see Section 5.6. The Reference is used to define a point near the center of the area to be setioned and the Boundary defines the extent of the section using a user defined spline. 2. Arrow Display (Available for use with all sections) This option allows the user to place arrows on another view to indicate the line of the section. (NB This is the last column in the table and may require the table to be scrolled). Select the appropriate table cell and then the view required. The length and position of the arrows can be adjusted by selecting and dragging. Thus to produce a half section similar to that in Figure 10:11 select a reference plane through the middle of the pulley and then the area to be sectioned. Select the view on which to show the arrows, see figure 10:12. • Apply/OK Selecting Apply at any stage will cause the system to try and action the requested section. OK closes the DRAWING VIEW menu. • Hatching Properties The system tries to make an intelligent guess at the required hatching spacing however it is a common requirement to modify this to match a particular material type or fit a detail. The spacing etc can be modified by selecting the hatching and then RMB → properties opens the MOD XHATCH menu. Selecting Spacing or Angle from this menu open sub-menus which allow the hatching to be changed by factors of two or to predfined values, see figure 10:13.

5.3

Tidy Drawing The position of symbols and text can be moved using the

LMB to select a item which can then be dragged to the required position. MMB to stop, LMB to exit move. A large number of functions are available via the RMB context sensitive menus, see Figure 10:14, and from the INSERT and FORMAT menus. (See FORMAT → Decimal Places.. to change default number display and therefore implied accuracy) 63

Figure 10:13: (a) General Hatching modifcation menu (b) Spacing specific options (c) Angle specific options.

(a)

(b)

(c)

Figure 10:14: Examples of context sensitive Pull out Menus, (a) On background (b) On selection of 1 dimension (c) Multiple dimension selection Use the functions, details about some are given below, to tidy the dimensioning etc. (Also see Figure 10:15) • Cleanup Dimensions: Multiple selection → RMB automatically aligns dimensions on a user definable spacing. • Move Item to View: Single or Multiple selection allows dimension etc to be switched between views. • Flip Arrows: Single or Multiple selection allows dimension arrows to be realigned • Text Style: Change text in multiple dimensions etc. • Properties : Gives access to the DRAWING VIEW menu

5.4

Isometric View The advantage of CAD is that it is relatively easy to add additional views. It is often useful to add an Isometric view to aid visualisation. To add a general view select RMB → Insert General View or ( ) Set specific view properties from the DRAWING VIEW menu, e.g. Scale, Figure 10:16. 64

Figure 10:15: Detail of a dimensioned drawing of the Pulley

Figure 10:16: Example of a view specific scaled general view the pulley

5.5

Printing a Drawing

N.B. By default the system prints the drawing that is visible on the screen, To print the whole drawing either select VIEW→ ORIENTATION → View Refit or use LMB + CTRL to zoom to the required view.

• Select the printer icon or Print from the File pull down menu.

• Select Generic Postscript

• Enter printer command lp -dxxxx, where xxxx is the printer name, e.g. ljmr1 for the printer at CUED. 65

Partially completed drawing of the shaft.

5.6

Shaft Drawing

Complete a basic dimensioned drawing of the shaft and then add additional views to generate a drawing as shown above. K.M. Wallace P.J.G. Long D. Underhill

Jan 2006

66

Exercise 11 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This task builds on the experience gained in Tasks 8 -10, to build the tensioner unit as an assembly and produce an assembly drawing. Modifying the pulley allows a single assembly (+ associated drawings) to be used for two configurations. Problem Using Proengineer first create a sub-assembly of the shaft and then place this sub-assembly into a given housing and bearings. Finally generate two assembly drawings showing two arrangements of the tensioner. 1. Shaft Sub-Assembly • Shaft

.

• Keeper Plate • Bolt • Woodruff Key • Pulley • Nut • Check Interferences (Modify if required) 2. Bearing Assembly • Assemble Shaft • Check Interferences • Insert Sub-Assembly • Check Interferences 3. Drawing • Generate Drawing 4. Modify Pulley (Optional) • Generate Drawing • Update Drawing N.B. Save your work at regular intervals and print out your work after each item has been competed to avoid clogging the printer at the end of the session.

67

Woodruff Key M12 Bolt Keeper

Shaft

Pulley

Roller Bearing

M18 Nut

Figure 11:1: Shaft Sub-Assembly

1

Additional Parts

To complete the following exercise you will require a number of additional components and assemblies, these should be found in your directory ‘ex8 11’. To ensure correct operation FILE → Set Working Directory (or hotkey cd) to ex8 11, i.e. change directory to /ProE/ex8 11.

2 2.1

Sub-Assembly Start Assembly using the (New Assy) function (icon in CUED area) called

shaftassy xxx123 (xxx123 = userid)

Placement Menu

2.2

Initial Component Insert the shaft as the initial component by using

INSERT → Component → Assemble or ( 68

) (from the right icon bar) then

• Component Selection Select shaft xxx123.prt from the list of files. (If your version is missing use shaft mast.prt) N.B. You can limit the list of files to just parts by selecting TYPE part at the bottom of the window. • Placement By default the system will try and automatically place the shaft in the main drawing window. To specifically place the shaft restraining constraints in three planes need to be added. It is normal with the first component in an assembly to constrain it via it’s base coordinate system, this can be done by either placing the shaft using the ‘Assemble component at default location’ tool (

)

or 1. CONSTRAINT TYPE → Coord Sys 2. Select the Component Reference CSO, (picked from the window) 3. Assembly reference A-CSO, (picked from the window or MODEL TREE) N.B. To aid the selection of constraint references it is often useful to toggle the display of datum planes/axis/points/coordinate systems to simplify the view. These can be switched on/off via the icon bar or hotkey sequences (ed - Datum planes, ec - Cordinate systems, ea - Axis, ep - datum Points).

2.3

Exit If the references have been selected correctly the placement status should

show ‘Fully Constrained’, references can be re-picked by selecting the associated arrow in ). the menu and reselecting in the window. Accept the placement with ‘OK’ ( Align

Mate

Keeper Plate Placement Constraints

2.4

Keeper Plate To assemble the Keeper Plate use the same basic command

structure as with the shaft, i.e. ( ) or INSERT → Component → Assemble, but then select your keeper plate from the previous session, keeper xxx123.prt (or a master copy keeper mast.prt). N.B. To manipulate the component being assembled use + mouse buttons • Align constraint using the axis of the shaft and the plate as references. This constrains the keeper in the two dimensions perpendicular to the axis of the shaft. N.B. It is often useful to use the RMB select option in conjunction with the SMART selection tool to ‘drill’ to the selection of references 69

• Mate To restrict motion along the shaft add a second constraint, TYPE Mate and choose the side of the keeper and the end of the shaft as the references. If the system prompts for an offset dimension, enter 0 mm. The keeper plate should now snap to the correct position and the Placement Status indicate ‘Fully Constrained’. (Leave the Allow Assumptions box ticked) ) If you are not satisfied with the placement re-edit the • Review ( constraints/references, then click OK ( ) to accept the placement. N.B. In many cases the Automatic alignment function, i.e. allowing the system to guess the type of alignment, is successful. It can be aided by choosing the driving feature first, e.g the major axis on an assembly, the system will then look for another axis + alignment as the preferred option

Align

Mate

Bolt Placement Constraints

2.5

M12 Bolt Assemble the bolt (m12 bolt.prt) in a similar manner to the Keeper

Plate aligning the axis with the Shaft axis and mating the undersurface of the bolt head with the outer side of the Keeper Plate.

2.6

Simplification To improve the response of the system and to remove screen

clutter temporarily suppress or hide the keeper/bolt. Select the keeper and bolt from the screen or MODEL TREE and then RMB → Suppress or Hide. • ‘Hide’ removes the items from the screen • ‘Suppress’removes the items from the display and reduces regeneration calculations but keeps the assembly definitions.

70

Mate

Align

Roller Bearing Placement Constraint

2.7

Roller Bearing Assemble the roller bearing, again using the same basic

command structure, but at the opposite end of the shaft. Use • Component roll bearing25x62.prt • Constraints 1. align the bearing axis with the axis of the shaft and the bearing as references 2. Mate the side of the bearing with the location shoulder on the shaft. • Check and Exit (

,

). Align Axis Align Offset (Surfaces/Datum Planes)

Align Planes

Woodruff Key Placement Constraints

2.8

Woodruff Key The placement of the key ( woodruff xxx123.prt or

woodruff 16mm.prt) requires, depending on the method of construction, two or three constraints :71

• Constraints 1. Align the central-axis of the key with the axis of the circular cut used to generate the key slot. 2. Constrain the third dimension by aligning the central plane of the key with the centre plane of the shaft. 3. In some constructions the key will appear inverted. Correct this by adding another constraint, Align + Oriented or Mate Oriented, using the surfaces/datums perpendicular to the center planes. N.B. Normally the system will prompt for an offset distance, even if the planes are not aligned. Accept the default values and then change the offset column to read oriented using the pulldown menu in the table cell. • Preview/Check ( with OK ( ).

2.9

) the placement status, redefine if required and accept

Pulley Assemble the pulley ( pulley xxx123.prt or pulley mast.=prt) in a similar

maner to the keeper plate and bolt, i.e. align with the central axis and mate the side of the pulley with the outer face of the roller bearing. Check the relative orientation of the key/keyslots in the shaft and pulley. If incorrect add an additional align or mate constraint based on the datum planes or flat surfaces associated with the slots/key.

2.10

Nut Assemble the nut M18 nut.prt using align to central axis and mate to the outer surface of the pulley.

Shaft Interference Analysis

2.11

Analysis The system has numerous checking and analysis routine, one that is

useful on the completion of a (sub-)assembly is Global Interference to check that the parts are correctly defined/assembled. 72

• Model Analysis From the ANALYSIS pull down menu select Model Analysis. In the new menu select analysis TYPE → Global Interference. Accept the default setting by selecting Compute. After a few seconds the system will return with information about any interferences in the lower scrollable window. • Correction Depending on the construction/errors made in the assembly there are likely to be one interference shown, the Woodruff Key with the associated volume of interference in mm3 . To correct this interference it is neccessary to understand the error and modify the parts or assembly settings. Checking the parts should show that the keyway slot is 3.5 mm wide and the Key 4 mm. Modify the slot width in the shaft to be 4 mm wide. N.B. Modification of parts can be carried out by reloading the individual part file or from the assembly itself. (Select SETTINGS (above model tree) → Tree Filters → Display Features (‘tick’) → OK will allow individual features to be accessed from the assembly MODEL TREE.) The box by the component’s name allows the feature information to be expanded/contracted. • Re-check Return to the assembly window, (reactivate if required) and re-run the analysis to confirm the interference has been eliminated.

2.12

Resume To return the components hidden/suppressed earlier, (bearing/keeper/bolt), select RMB → unhide or EDIT → Resume → All. Print Arrange the assembly on the screen, ensure that the MODEL TREE menu is visible, and print using Print Scrn.

Save Save the assembly

Assemble Shaft assembly into the housing

3

Cut away model of the basic Tensioner

Main Assembly

The basis of the main assembly is given as a predefined file: 73

3.1

Tensioner Load the partially completed file of the total assembly, filename

tensioner assy.asm. DO NOT assemble the tensioner assembly into the shaft! N.B. The view looks partially complete as there is an active assembly cut, removing the front half of the housing to aid the location of the shaft sub-assembly.

3.2

Sub-Assembly. Locate the shaft sub-assembly into the Tensioner, using a

similar manner to that used to align the keeper/bearing/pulley etc. Mate the inner surface of the Roller Bearing with the locating step in the left end of the housing, i.e. opposite end from the circlip/roller bearing. Align the central axis of the housing with that of the shaft. N.B. The order of the choice of assembly references. If the axis alignment is chosen first the shaft will snap to the centre of the housing making the selection of the mating surface more difficult. An alternative method of assembly keeps the component in a separate window, see ‘separate window’ tick box, prior to accepting the placement. When fully constrained Preview (redefine if required) and accept OK.

3.3

Analysis Rerun the model analysis to check the Global Interferences

This should show one interference between the shaft and the ballbearing. This is a result of the mate constrain of the keeper on the end of the shaft leaving only 16 mm for a 17 mm bearing and not allowing for a clamping force. This can be modified by either defining the ball bearing as part of the shaft sub-assembly and using stacked mate constraints. Or by adjusting the keeper placement by 1 mm. • Correction Switch the active window to the shaft assembly. Select the keeper plate from the window or MODEL TREE and then RMB → Edit Definition. When the placement window appears select the mate constraint and set the Offset to 1 mm accept the placement. N.B. The placement of the bolt is automatically updated as it is a ‘child’ of the keeper • Reload Return to the Tensioner assembly window. (Remember to reactivate the window from the WINDOW pulldown menu or CTRL-A) • Check Rerun the global interference analysis and confirm that the interference has been removed.

Print Arrange the assembly on the screen, ensure that the MODEL TREE menu is visible, and print using Print Screen. N.B. The assembly can be slow to orient in shaded mode, to speed up placement zoom out reorient as a small item on the screen and then zoom in to the required magnification. The amount of information transfer required to update the screen is significantly reduced thus increasing the update speed especially on slow graphics cards or on remote displays.

Save Save the assembly 74

Figure 11:2: General Assembly Drawing of Tensioner

3.4

Remove Cut

• Display Features Ensure that the MODEL TREE display option to show features has been actioned. (Select SETTINGS (above model tree) → Tree Filters → Display Features (‘tick’) → OK) • Suppress Cut Select the assembly feature HOUSING CUT from the MODEL TREE, the RMB → Suppress. N.B. HOUSING CUT is a standard extruded cut but the feature has been renamed (RMB→ Rename) to make it easier to identify in the model tree. This technique is often used in parts/assemblies with a large number of features.

3.5

Transparency ProE allows colours to be changed and textures/lighting and

transparency etc to be modified. As an example select VIEW (pulldown) → Display Settings → Model Display → SHADE (menu tab) → toggle Transparency /Apply. N.B. The transparency can be accessed through the hotkeys et Enable Transparency and te Transparency disEnable

4 4.1

Drawing Load Drawing Open the drawing file tensioner drawing.dwg which

contains an end view of the assembly.

4.2

Datum Planes Select the datum planes on ( 75

) and repaint the screen (

).

4.3

Section View Add a side view of the tensioner and section the view on the

centerline using similar techniques that were used to section a part(See Figure 11:2), e.g. • Select the existing view and RMB→Insert Projection View • Select the new view RMB→Properties • Select the Sections option in the DRAWING VIEW menu, and complete the options for a full section N.B. The drawing table, above the information box has been updated to contain information on all the parts now in the drawing

4.4

BOM Ballons Display the Bill Of Material ballons by selecting from the

TABLE pull down menu • Select BOM Balloon → Set Region → Simple from the menus and then select the table of parts just above the title block, i.e. the Region to be used to define the balloons. Finish with Done. • Select Create Balloon from the BOM BALLOON menu and then the cross section view to place the balloons.

4.5

Additional View Add an additional isometric view and set the individual

view scale to 0.5.

Print Arrange the windows on the screen, ensure that the MODEL TREE menu is visible, and print using Print Screen.

Save Save the updated drawing

76

5

Modified Pulley (Optional) Modified Pulley

In some applications a cooling fan is added to the pulley end of the tensioner, to update the pulley to allow for this reload the pulley and add the following features

• Thicken the outer flange of the pulley • Create a radial threaded hole • Pattern the hole on a 70mm PCD

5.1

Load or reactivate the pulley window Base Auxiliary Drive Section - Revolved Protrusion 10

32

Ø36

Section Dimensions

5.2

Finished protrusion

Thicken Flange Create a revolved protrusion, centred on the axis of the

pulley with dimensions as shown above, i.e. thickness 10 mm, ID 36 mm and OD 100 mm. (If the sketch align options are used it is possible to draw the addition with only 1 (10mm) dimension.) N.B. If there is no preview option available it is likely that the axis of revolution has been obmitted, re-edit the section or select the axis via PLACEMENT→Axis 77

5.3

Mounting Holes Use the Hole Tool (

) to model one tapped (threaded)

hole for a M5 bolt. Hole Type Select a Standard Hole, ISO, M5 x 0.8 , Tapped Hole (N.B. Deselect the ‘Add Countersink’ option) Hole Dimensions

Leave as defaults, i.e. Hole Depth 12.6 mm (and Threaded Depth 10.1mm)

Hole Placement 1. Select a point on the outer surface of the new protrusion. 2. Select Placement Type Radial 3. Highlight the second reference field and select the axis of the pulley unit as the Axial Reference 4. Set the Radius, (PCD/2) to 35 mm 5. Using and LMB, select a datum plane (typically FRONT or TOP) as the angular reference and set the angle to 45o .

5.4

Patterned Holes The previous section (5.3) defined a tapped hole on a PCD offset at an angle (45o ) from a datum. This angle can now be used to duplicate the holes. Select hole feature from the model tree or from the main drawing window and then using RMB → Pattern (or EDIT → pattern) activate the Pattern dashboard. 1. In response to the request to ‘Select dimensions to vary in the first direction’ select the offset angle of 45o. (It may be necessary to rotate the model around to see this dimension clearly.) 2. A prompt will now appear requesting the dimension increment, enter 45. 3. At the Number of Pattern Members (1) field (second from left) enter 8 Exit the dashboard ( ) and after a few seconds the pattern should appear on the part and in the MODEL TREE.

6

Drawing 2 (Optional)

Reselect the window containing the drawing, and see that the drawing has been updated. 78

Print Tidy up the drawing, arrange the windows on the screen and print using Print Screen. Use Move to rearrange the position of the balloons. Use Edit Attachment to change the end location of the balloon leaders.

Save Save the updated drawing 6.1 Suppress Re-activate the pulley and select the additional revolved protrusion from the screen (or the model tree) and then RMB → Suppress. As the Holes are a child of the protrusion you are prompted to confirm that you wish to suppress all the highlighted features, select OK. (N.B. Suppressed features are indicated in the model tree with a black square) Note that the pulley is now represented on the screen and on the screen in it’s original form, however the information about the modifications is still available should both alternatives are required. N.B. If the feature is not visible in the MODEL TREE Select SETTINGS (above model tree) → Tree Filters → Display Suppressed (‘tick’) → OK. K.M. Wallace P.J.G. Long D. Underhill

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80

Exercise 12 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This task builds on the experience in the previous CAD exercises to assemble the tensioner you constructed in task 11 on to an engine block and produce an Assembly drawing and 3D views. Problem Complete tasks 1, 2 3 and 4 below 1. Tensioner If you did not complete question 11, do so such that you have a complete tensioner assembly. 2. Engine Assembly Load the blank assembly called, ‘engine-assy’ and assemble the following items (see Figure 12:1) using the constraints indicated below. Engine block

Coordinate System

Representation of a 4 cylinder engine block

Alternator

Mate, Align (axis)

M12 bolt

Mate, Align (axis)

(pattern)

Ref Pattern

Pattern the Alternator fixing bolts using the reference pattern used to generate the location holes.

Belt

Align (Axis & Plane)

Use the main crankshaft axis and the predefined belt location plane

Tensioner Assy

Align(axis) & Mate

Align pivot axis and mate to the mounting lug, and then locate in position using the axis on the belt. Locate Tensioner bolt NB allows tensioner to pivot.

Tensioner Bolts Mate, Align (axis) 3. CAD Drawings

(a) Load the predefined assembly drawing file called eng assembly and insert 3 orthogonal views. Print Screen (b) Arrange the view on the screen to shown the area around the tensioner, use suppress/resume to expose the components of the tensioner. Print screen of the detailed view. 4. Drawing Updates • Ensure the additional boss on the pulley is resumed and then add the fan + bolts 81

• Update the drawing • Using VIEW → Model Setup → color and appearances change the colour of parts and surfaces in the assembly to make it more understandable • Add an additional detailed view to the 2D drawing showing the tensioner in detail, see Figure 12:2. (Use INSERT → Drawing View → Detailed).

Figure 12:1: Completed Engine Assembly

Figure 12:2: 2D drawing of the Engine Assembly showing the Detailed View K.M. Wallace P.J.G. Long D. Underhill

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Exercise 13 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This task builds on the experience gained in previous CAD exercises in the design of parts but introduces more flexibility in the design process. Problem The A3 drawing shows an air compressor with the piston and crankshaft removed. Using ProE design a piston and crankshaft for the compressor shown in the drawing. To help the interpretation of the drawing bring up the compressor assembly in ProE before you begin the process. Design Considerations 1. PISTON The flap valve on the top of the piston is spot welded in position. Details of the flap valve are shown on the drawing provided. The piston seal is an ‘O’ ring of φ 2mm cross section diameter. Details of the connecting rod are shown on the drawing provided. 2. CRANKSHAFT To be machined from a one piece casting. The main gear to be bonded to the crankshaft with suitable adhesive. The counterbalance shape to be similar to the drawing provided. A circlip 0.2 mm thick should be used on the smallest diameter to prohibit axial movement of the shaft. CAD Drawings After modelling the two parts produce orthogonal drawings of them showing front and side elevations only. Show all necessary manufacturing dimensions. N.B. Save your work at regular intervals and print out your work after each item has been competed to avoid clogging the printer at the end of the session.

83

84

86

Exercise 14 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction Using the experience gained in the previous exercises to produce an assembly and animation including the parts completed in question 13. (i.e. the piston and crankshaft) plus the library parts available in your shared directory. Problem 1. To assemble the piston and crankshaft you have produced into a complete compressor assembly (compressor v2) and to produce and detail an othogographic drawing with 3 views, including one cross section, and an exploded isometric view. 2. Finally animate the moving parts of the assembly Method 1. Assemble the piston and crankshaft you produced in exercise 12. It is recommended that a series of sub-assemblies are first produced with all items arranged in the top dead centre position including :(a) Piston sub-assembly - containing Piston, Flap valve, ‘O’ ring and gudgeon pin (b) Con-rod sub-assembly - containing Con-rod with Big End bearing. (c) Crankshaft sub-assembly - containing Crankshaft, large gear and circlip. (d) Moving parts sub-assembly - items 1,2 & 3 above (e) Add ‘Moving Parts’ sub-assembly to the given compressor (f) Produce an assembly drawing, (use the A3 Assy Drw icon to start the drawing) 2. Animate the model using both manually (using the ‘drag’ option ) and automatically using the analysis and servo drivers. Colour the parts introduced to give a contrast to existing parts. N.B. Save your work at regular intervals and print out your work, using the PRINT SCREEN function, after each item has been competed to avoid clogging the printer at the end of the session.

87

ø 4.0

CRANKSHAFT ø 8.0 ø 7.0 0.2

45° X

0.5

ø 3.5

7.5

ø 4.0

5.0 10.0

8.0

16.0

9.0

7.0

PISTON ø19.5 5.0

ø16.5

ø3.0

15.5

2.5

45° X 1.0

X

ø14.0 SECTION X-X

88

10.0

6.0

20.0

ø4.0

X

Complete Compressor

1

Dynamic Analysis

To define a mechanism within ProEngineer location connections are added to a assembly in a very similar way to normal fixed assembly constraints. Although it is possible to modify an existing assembly to allow motion it is often easier to restart. Thus in your completed assembly delete or suppress the piston, conrod subassemblies and the crankshaft. Although, as with other parts of Proengineer, it is possible to assemble the moving parts in a number of different ways it is suggested that you follow the procedure below. Once you have completed it you may experiment with the assembly options/funtionality to discover what other features are available. There is further information on the how to use the motion options within ProEngineer Wildfire to be found on the web, see the help pages at www.eng.cam.ac.uk/DesignOffice, in particular the link relating to Design Dynamics. There are 7 standard joint types available (+ user defined joint), see below, that can be combined in a similar method to that found with fixed constraints to achieve the particular type of motion required. In many cases it is useful to think of the 6 Degrees of Freedom (DOF) available (3 Translation + 3 Rotation) and confirm the the choice of constraints limits the motion to only the DOF’s you require. 89

Joint Type

Constraints Required

DOF

Ball

Point alignment to point

3xR

Bearing

Point alignment to edge or axis

3xR, 1xT

Sliding idealised ball joint

Cylinder

Axis alignment

1xR, 1xT

Cylinder, plain bearing

Pin

Axis alignment, mate/align

Planar

Plane alignment

Slider

Axis alignment, mate/align

Weld

Coordinate system ment

Rigid

One or more constraints

2

Planar

Planar align-

Real Life Joint Idealised Ball joint

1xR

Bearing with no axial movement, e.g. Roller bearing

2xT

2-D sliding, e.g. plate-plate.

1xT

Slot Welded/bolted/glued joint Specialised joint

user

defined

Dynamic Model Assembly

Crankshaft Placement Constraints

2.1

Crankshaft Sub-Assembly As noted above the joint that actually

simulates a plain bearing best is a ‘Cylinder’, however it is often easier to use a ‘Pin’ joint that allows rotation and also restricts axial displacements in one constraint. Thus the first component, the crankshaft, is assembled using a Pin joint. Start the assembly procedure as for a fixed constraint, i.e. using INSERT → Component ) (from the right icon bar) → Assemble or ( Select the connections option, which will cause a new set of options to be available. Add a PIN connection and use 1. The axis of the crankshaft and the axis of the small bush to complete the axis alignment. 90

2. The step in the shaft and the edge of a bush to give an axial translational placement. select OK when the PLACEMENT STATUS indicates Connection Definition Complete. N.B. The crankshaft is now displayed in the model tree with a small white square, indicating that the component is not fully constrained.

2.2

Piston Sub-Assembly The piston can be assembled in a number of ways,

but it is most convienent to use the cylinder option. Use the central axis of the piston and the cylinder to align the subassembly. N.B. The flip option can be used to reorientate the piston if it appears in the model upside down. To simplify the assembly of the conrod use to move the piston subassembly into the approximately correct position.

Connections displayed on the assembly and details of the conrod definitions

2.3

Conrod Sub-Assembly Assembly of the Con-Rod completes the

mechanism and is assembled using a combination of a ‘Pin’ connection to locate the little end bearing in the middle of the gudgeon pin and a cylinder connection to locate the big-end bearing on the crankshaft. N.B. In some situations the system can lock into the secondary stable positions, e.g. with the piston below the unit and the conrod passing through the piston assembly. (There is no collision checking at this stage of the assembly process) In these situations place the conrod subassembly into the approximately correct position using and mouse movements, and then redefine the piston position. This will force the piston into position.

3

Manipulation of Dynamic Assembly

Once assembled with connections the mechanism can be manipulated either manually or automatically with one or more predefined motions. A limited amount of analysis of the system is also available at this point. To activate this mode select APPLICATIONS → Mechanism. The change of mode is indicated by the appearance of a new set of icons in the right menu and a new set of features in the model tree. 91

3.1

Manual Movement The mechanism can be manipulated ‘by hand’ using the

drag function, ( ) or MECHANISM → drag. This will highlight the connections and prompt the user to select a component. Selecting a movable item, e.g. the crankshaft balanceweight, results in a small white circle appearing on the component at which point the mouse can be used to move the item as though it was being dragged/pushed. Any connecting parts also move as defined by the connections.

3.2

Automatic/Driven

Servo Motor Definition Menus The system allows a number of different analyses to be undertaken, However in all cases ‘drivers’ need to pre-set. To setup a ‘servomotor’, select ( ) or MECHANISM → servomotors. In the new window select NEW and enter a name of your choice (or accept the default) in the SERVO MOTOR DEFINITION window. Select the crankshaft axis (the yellow highlighted joint) as the Driven Entity and selecting the PROFILE submenu define the servo motor to have a profile of specification of Position, Magnitude Ramp with position values of A=0 and B=360. Accept the Servo Motor definition and return to the main screen.

Analysis Definition Menus 92

Select ( ) or Mechanism → Analyses followed by New, choose a Repeated Assembly TYPE and enter 1. START TIME = 0 2. Length and Rate type 3. END TIME = 1 4. FRAME RATE = 20 5. MINIMUM INTERVAL = 0.05 Selecting Motors choose the motor definition entered previously. Selecting Run from the ANALYSIS DEFINITION menu will run the basic analysis and store the results. Return to the main screen using OK and Close.

3.3 Results Display Select ( ) (MECHANISM → Playback or Playbacks from the model tree). Accepting the defaults select the small playback arrow at the top of the menu and then use the cassette recorder like controls to display the motion. If you are using your own piston/crankshaft you might like to check for inteferences. Selecting the Global Interference option on the PLAYBACKS menu will set going an analysis of the interferences thoughout the motion. Any collision volumes are shown in red wireframe, c.f. the interference between the motor shaft and the small gear.

Trace Curve Menu Another interesting and often useful facility is to trace the position of a component/part of a component thoroughout a cycle. Although very simple in this instance, this functionality can be demonstrated by selecting Trace Curve from the MECHANISM menu and then selecting the Trace curve pnt on the con rod. This will automatically select the Paper Part entry and by selecting Preview the trajectory is displayed as a purple line in the main screen. (N.B. It may be neccessary to select the display datum point icon on the top menu bar to make the point visible.) 93

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Exercise 15 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This exercise extends your experience in animating mechanisms using a IDP robot as the basic model. The task is to complete a static assembly and associated 2-D assembly drawing and then using the techniques learnt in Exercise 14 to convert the lifting system into a mechanism and to update the Assembly drawing to show the extremities of travel. N.B. The components required for this excercise can be found in your subdirectory /ProE/ex15 16. Do not forget to set your working directory before starting to work. Problem 1. Add the castors and cable support to an existing model and generate an assembly drawing. 2. Complete the ‘static’ model, adding the lift mechanism, drive units, controller etc and update the drawing 3. Modify the lifting system to be a mechanism 4. Add the new lift sub-assembly to the model and produce a drawing showing the extremities of the motion. N.B. Save your work at regular intervals and print out your work, using the PRINT SCREEN function, after each item has been competed to avoid clogging the printer at the end of the session.

95

1

Key

To aid in the use of this handout a number of conventions/fonts/abbreviations have been used to indicate the difference between keyboard entry, menu titles, menu items etc. These are listed below: Font Used

Item

Abbreviation

Action

Bold/Times:

menu item

LMB

Left Mouse Button

CAPITALS:

WINDOW/MENU TITLE

MMB

Middle Mouse Button

Italic:

Keyboard inputs

RMB

Right Mouse Button

Bold/Helvetica:

Hint

Menu items followed by a → indicate that the user should follow the input to a cascaded or flyout menu. N.B. In many cases the choices required are the default and therefore do not need to be individually selected. Model Manipulation Key/Mouse

Action

(N.B. The Ctrl key can normally be released once the action has been initiated.) Ctrl - Middle Mouse Button

Zoom in/out

- Middle Mouse Button

Spin

Shift - Middle Mouse Button

2

Translate

Getting Started

To start ProEngineer Wildfire login to the teaching system and • Close down unused programs, ProE imposes a large load on the system • Select Start from the main icon bar and then select Pro/Engineer Wildfire 2 from the Programs→3D Modelling submenu. This will start the package, and set the working directory (where your files will be stored) to /userid/ProE/. Within this area are a number of predefined directories, ex8, ex9, ..., which will be used to store the work for each of the drawing exercises. To change to the directory for this exercise select FILE → Set Working Directory (or use the hotkey option cd) and then select the directory ex15 16 from the file browser window, close with OK.

96

Top view of Robot

3

Underneath view of Robot

Task 1 - Static Assembly 1 1. Load the partially completed assembly robot1 2. Assemble the two castors, (castor.asm). 3. Assemble cable support, (support supply.prt). Hint: use the tangent constrain to locate the support 4. Generate a A3 Assembly drawing 5. Print drawing

4

Task 2 - Static Assembly 2 1. Assemble the pre-defined, lift static.asm, lifting mechanism onto the robot Hint: Think how the unit would be assembled in real life 2. Assemble the drive units, drive unit.asm (motor/wheels/supports). Suggestion: Use second assembly window, or suppress a constrain if you find aligning the axes confusing. 3. Update the drawing and print 97

Lift Mechanism

5

Task 3 - Dynamic Assembly of lift mechanism 1. Load the static lift mechanism, lift static, and save a copy lift dynamic 2. Load lift dynamic Hint: Select Mechanism application temporarily to show any existing dynamic constraints 3. Modify the pivot points etc. to allow rotation Hint: You should only need to change 4 joint definitions. Start redefining the constraints from the bottom of the model tree to remove problems associated with parent-child rconstraints 4. Check the motion by using drag and the predefined motion of the pnuematic cylinder. Hint: Be careful not to drag the mechanism beyond its normal limits. Run analysis and use the predefined servo-motor, set analysis type to Repeated Assembly

6

Task 4 - GA drawing 2 1. Assemble the new lift sub-assembly into the existing main assembly, robot1. Hint: Suppress the static assembly to aid visualisation. See how defining a useful CSO can aid assembly 2. Arrange the mechanism at the end of its travel 3. Update the drawing to show the mechanism at the extremities of its motion Hint: Use the static assembly.

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Exercise 16 UNIVERSITY OF CAMBRIDGE DEPARTMENT OF ENGINEERING DRAWING COURSE Introduction This exercise builds on your experience of Pro/Engineer and introduces a new module ’Sheetmetal’ that enables a designer to generate development drawings of sheetmetal constructions. Complete the sub-tasks listed below, items 1 & 2 use a number of the standard functions in the sheetmetal module to produce a support bracket. Items 3 & 4 are based around a chassis for an Part IB Intergrated Design Project robot used in Qu 15. The emphasis is on completing well laid out dimensioned 2-D drawings suitable for design acceptance in this project. The additional items 5 - 7 give experience in using more of the sheetmetal functionality. Problem 1. Construct a support bracket 2. Add a flat ‘wall’ to [1] and produce a 2-D development drawing 3. Construct the outline of an example IDP robot chassis in solid, convert to sheetmetal. 4. Add ‘edge rips’ and ‘flat pattern’ features to the model. Generate a drawing containing 2 sheets showing the isometric + development of the chassis. 5. Construct a simple metal tab to the chassis 6. Copy existing tab 7. Add Wall extensions to [1] N.B. Save your work at regular intervals and print out your work, using the PRINT SCREEN function, after each item has been competed to avoid clogging the printer at the end of the session.

99

1

Key

To aid in the use of this handout a number of conventions/fonts/abbreviations have been used to indicate the difference between keyboard entry, menu titles, menu items etc. These are listed below: Font Used

Item

Abbreviation

Action

Bold/Times:

menu item

LMB

Left Mouse Button

CAPITALS:

WINDOW/MENU TITLE

MMB

Middle Mouse Button

Italic:

Keyboard inputs

RMB

Right Mouse Button

Bold/Helvetica:

Hint

Menu items followed by a → indicate that the user should follow the input to a cascaded or flyout menu. N.B. In many cases the choices required are the default and therefore do not need to be individually selected. Model Manipulation Key/Mouse

Action

(N.B. The Ctrl key can normally be released once the action has been initiated.) Ctrl - Middle Mouse Button - Middle Mouse Button Shift - Middle Mouse Button

2

Zoom in/out Spin Translate

Getting Started

To start ProEngineer Wildfire login to the teaching system and • Close down unused programs, ProE imposes a large load on the system • Select Start from the main icon bar and then select Pro/Engineer Wildfire 2 from the Programs→3D Modelling submenu. This will start the package, and set the working directory (where your files will be stored) to /userid/ProE/. Within this area are a number of predefined directories, ex8, ex9, ..., which will be used to store the work for each of the drawing exercises. To change to the directory for this exercise select FILE → Set Working Directory (or use the hotkey option cd) and then select the directory ex15 16 from the file browser window, close with OK.

100

3

Sheetmetal Fundamentals

The user interface employed by the ‘sheetmetal’ module of Pro/Engineer is very similar to the default solid modelling part. The same principles hold, select the type of feature to generate, sketch/pick&place the feature completing all the elements required and then preview/accept.

4

Task 1 - Extruded Bracket

In this section we use a standard technique in the sheetmetal module to produce material, an extruded section. This is similar to the extrude function in the solid module, but only one side of the section needs to be drawn as the sheetmetal thickness is defined.

Figure 16:1: Basic Bracket Start a new part, bracket userid, invoke the ‘Sheetmetal’ option from the APPLICATIONS menu and start to create a one-sided ‘Unattached Extruded Wall’ ( ) feature, (in the flyout menu on the fourth icon down or INSERT → Sheetmetal Wall → Unattached → Extrude). Once in the sketcher draw the general bridge outline of the part with the dimensions shown in the figure above. Ensure that the ‘bridge’ is centred about the MID datum plane. Hint: If a centreline is placed on the desired mid plane, the ‘symmetric about a centreline’, constraint can be used. Select the centreline followed by the two vertices to be made symmetric Whilst in the sketcher mode, select the thicken function (RMB → Thicken) and then choose the direction to retain the internal dimensions, e.g. internal radii 1.5 mm (See Figure 16:1). Enter a material thickness of 1.5 mm. Exit the sketcher, accept the default direction and enter a blind depth of 60 mm. Preview and accept. Create a Flat Pattern feature, using the bottom icon on the side icon bar, selecting the top of the bracket as the plane to remain fixed. N.B. Once created the Flat Pattern feature will automatically remain the last feature. To return to the folded state suppress the feature. 101

Print an image of the bracket Use the ANALYSIS → measure function to manually check the calculated value for the bend allowance and compare it with a hand calculated figure. Add the calculation, and comments about any differences, to the printout.

5

Task 2 - Adding an additional Wall 1

Additional flaps etc can be added to a part by using the various attached wall features, here the Create Flat Wall feature is used.

5.1 Flat wall Select the ‘Create Flat’ ( ) feature, (second icon down or INSERT → Sheetmetal Wall → Flat), which opens the associated dashboard (Figure 16:2)

Figure 16:2: Standard setting for the Flat Wall dashboard Accepting the default settings and selecting an attachment edge immediately generates an additional wall.

Figure 16:3: Initial Display of the flatwall, having chosen an attachment edge A Flat wall is simply additional material attached to an existing piece of sheetmetal work. It can be an arbitary shape and attached at a user defined angle, see the first two dashboard items. The default Rectangle shape can be modified in the SHAPE dashboard pulldown menu, see Figure 16:4. If a different shape, e.g. Trapezoid, L, T is chosen from the wall shape selection both the shape display and the model automatically change. An arbitary shape can be defined in a sketcher window by selecting the User Defined option or selecting sketch from the SHAPE menu. Hint: Although it is additional work it is often useful to use the User defined option even to define a rectangular wall, when the dimensions can be constrained by an existing feature/dimension. 102

Figure 16:4: Screenshot showing both the interactive SHAPE menu and the pulldown menu allowing the selection of predefined shapes

5.2

2-D drawing Start a new A4 part drawing (using the a4 part.frm format),

named bracket1, and place an edge view and a plan view of the bracket development fully dimensioned. Reminder: To change the scale double click on the value at the bottom left of the screen In many cases it is useful to also display one or more views of the finished folded item. This can be done on another drawing or second sheet of the same drawing. Alternatively the concept of a ’family table’ combined with the ability of the system to include drawings of more than one item on one drawing can be used. Add row

Add item

Figure 16:5: Typical layout of a ‘Family Table’ The family table allows a series of similar ‘instances’ of one model each differing by one or more dimensions/features, the details of which are contained in a table. In this situation a family table needs to be produced with two instances differing by the inclusion/exclusion of the flat pattern feature. To set up a Family table for the bracket, return to the part window, ensure that the bracket has the Flat Pattern feature resumed and then select Family Tab from the TOOLS menu. Following the instructions in the Family Table window first add the Flat Pattern feature as column to the table. (Add item → feature → Select the feature → OK). Add a second instance, using the add row icon, and set the Instance Name to Bracket1 folded and the feature setting to N (Use the pulldown options.), see Figure 16:5. 103

When you have complete the table, exit using OK. N.B.: A suppressed feature cannot be selected. Also, it is often useful to add three instances, generic, folded and flat. This allows drawings and models to remain correct even if the flat pattern status is changed in the generic mode

Figure 16:6: Dimensioned Drawing

To add views of the folded bracket to the drawing, the folded instance of the part needs to be made active by, selecting RMB → Properties → Dwg Models → Add Model. Select Bracket1 userid and then Bracket1 folded → Open in the SELECT INSTANCE menu. To select the folded model as the current model select Set Model → Folded bracket → Done/Return. Add a general view as shown in the figure above. Update any dimensions required in the 2-D drawing and print. Although the show all option can be used from the show and erase menu this often produces a large number of awkward dimensions. It is often better to manually insert dimensions using the INSERT→Dimensions →New references or ( )

6

Task 3 - Robot Chassis

A powerful facility within Pro/Engineer and a number of the other large CAD packages is to be able to construct a model in solid and then finally shell it, c.f. the cylinder intersection problem, and then generate the development. The next two tasks are examples of this process being used to produce drawings, and therefore possible CNC codes, for the manufacture of a typical IDP robot chassis. 104

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General view of the final assembled robot

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Overall dimensions of the chassis

6.1 Solid Model of chassis Construct a new part names chassisshell, constructed using a solid one-sided extrusion to the dimensions shown in the figure above. Hint. While the cross-section of the extrusion can be sketched on any plane it is often useful to arrange for them to be named correctly to aid with future assemblies, i.e. sketch the section on the ‘yellow’ side of the top plane and orientated with the front of the vehicle aligned with the yellow side of the FRONT plane

6.2

Conversion of chassis to sheetmetal In essence this is very similar to a standard shell operation, but the system recognises the resulting shell as a sheetmetal object. While the solid chassis window is still active select APPLICATIONS → Sheetmetal → shell. Then select the surfaces to be removed, the base + four surfaces in the slots. Once selected, complete the feature definition with Done → Done Refs and enter the material thickness, 1.6 mm. An indication that the model is now in sheetmetal mode is that this shelling results in a new ’First Wall’ feature.

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Task 4 - ‘Ripping’ the 3-D model

Inserting a flat pattern feature at this point indicates that only the flap at the centre of the front is available for automatically bending.

7.1 Insert ‘rips’ Although the chassis part is recognised as a sheetmetal element the system does not automatically choose cut lines. These are normally added by using the ‘Conversion’ feature. Select the ‘Create Conversion’ feature ( )and select to define (from the SMT Conversion menu), Edge Rip. Add the four outer corner edges of the chassis together with the outer return edges by the notches at the front of the chassis, then Done Sel → Done Sets, Preview/Redefine/Accept. Hint. If the material is thick there can be problems with too much material in the corners of bends. The problem can be eleviated by adding ‘Corner Relief’ either when defining the conversion or afterwards using the Create Corner Relief feature. 105

7.2

Second Drawing Sheet + Development To fully describe an object

or assembly it is often neccessary to produce a number of drawings. These can be separate drawings, however it is often useful to have sub-sheets with different aspects of the item described. In the case of the chassis it may be useful to have one sheet with the orthographic views and a second with the development. Use the technique described in 2 to generate folded and unfolded instances of the chassis. Produce a A4 drawing of the folded chassis and then add a dimensioned development drawing on the second sheet. To add a second sheet to a drawing select INSERT → Sheet. The sheets can be switched using VIEW → Go To Sheet or use the sheet selection icon ( ). Print the two sheets.( Note any differences to the length of the sides of the chassis and propose a reason(s).)

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Task 5 - Adding Tabs to the Chassis

It is often required to increase the torsional stiffness of a chassis (or other sheetmetal object) by adding tabs at corners, which are subsequently attached with bolting, riveting or spot-welding. The simplest method to add tabs is to use the ‘Create Flat Wall’ feature used in task 2.

8.1

’Flat Wall’ Tab Select the ‘Create Flat’ (

) icon and when the dashboard has loaded select an edge of one of the exisiting chassis walls. Although a rectangular tab can be used it often useful to choose a Trapezoid shape with a shallow angle to allow for variations in bending, see Figure 16:7 for typical dimensions. Use the first flip option, on the dashboard, to orientate the tab if required. If the tab is coincident with the second wall use the ‘offset’ pulldown options to automatically realign the bend.

8.2

Bend relief In the corner where the tab,top and walls meet there is an area of high deformation. By default, Wildfire defines a rip in the material, see Figure 16:8. In manufacture it is better to control the deformation by the removal of material in this area, which can be done automatically with a predefined relief option, e.g. Obround, see Figure 16:9. Before this form of relief can be used the tab needs to be reduced in size.

Select/redefine the Flat Wall feature used to define the tab and reduce the size by 2mm. Then insert a default Obround feature at the corner end of the tab, N.B. Inserting a relief 106

Figure 16:7: Placement/Shape/Dimensions of a tab at the corner of the chassis

(a)

(b)

Figure 16:8: Rendered images of (a) ‘Rip’ (b) ‘Obround’ relief at the open end will cause a simply recoverable error.

8.3

Drawing Update Add a detail scrap view of the tab/relief to the existing 2D

drawing of the flat chassis.

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Task 6 - Copying Tabs

Experiment with the Feature → Copy feature to generate a second ‘dependant’ tab on another corner. Hint: This functionality can be used to copy features in both Solid and Sheetmetal parts. Select the tab completed in section 8 and then using the EDIT→Copy (or C) and EDIT→Paste Special add the same wall definition to another corner. When the paste Special option is selected choose the option make copies dependent on dimensions of originals. This ensures that changes to the master tab are propagated to all copies, this can subsequently be disabled by selecting the feature and RMB→Make Sec indep. 107

(a)

(b)

Figure 16:9: (a) Adjustment of Tab size (b)‘Obround’ relief default definition Pasting a copied object initates the normal dashboard, but ony requires the placement references to be picked from the model, here an external edge at another corner, before the feature is defined and the dashboard can be exited.

Figure 16:10: Example of Extended Wall

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Task 7 - Predefined wall extensions

It is often useful to add small extensions to walls to close a box for instance, see Figure 16:10. While it is possible to manually add wall extensions, there is an automatic feature. Reload/re-Activate the bracket and then choose the Create Extended Wall feature ( ) and then select the outer edge of the tab and the side of the existing bracket to extend the tab. Update the 2-D drawing and print K.M. Wallace P.J.G. Long D. Underhill

Jan 2006

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Pro/Engineer Wildfire 2 Sheet metal Menus & Bend Allowance Calculation CUED Part 1A Drawing

Sheet metal Conversion Flat Wall Revolved Wall

Flange Wall

Offset Wall

Sheet metal Cut Extended Wall

Unattached Flat Wall

Bend

Edge Bend

Unbend

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Corner Relief

Punch

Notch

Blended Wall

Unattached Extruded Wall

Rip

Bend Back

Merge

Flat Pattern

Form

Flatten Form

Deform Area

pjgl2/April05