Autodesk Auto CAD Mechanical Desktop 6.0 Instruction Manual Autocad 6 En

User Manual: autodesk AutoCAD Mechanical Desktop - 6.0 - Instruction Manual Free User Guide for Autodesk AutoCAD Software, Manual

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Autodesk Mechanical Desktop
®

User’s Guide

6
20507-010000-5020A

May 3, 2001

Copyright © 2001 Autodesk, Inc.
All Rights Reserved
This publication, or parts thereof, may not be reproduced in any form, by any method, for any purpose.
AUTODESK, INC. MAKES NO WARRANTY, EITHER EXPRESSED OR IMPLIED, INCLUDING BUT NOT LIMITED TO ANY IMPLIED
WARRANTIES OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE, REGARDING THESE MATERIALS AND MAKES
SUCH MATERIALS AVAILABLE SOLELY ON AN “AS-IS” BASIS.
IN NO EVENT SHALL AUTODESK, INC. BE LIABLE TO ANYONE FOR SPECIAL, COLLATERAL, INCIDENTAL, OR CONSEQUENTIAL
DAMAGES IN CONNECTION WITH OR ARISING OUT OF PURCHASE OR USE OF THESE MATERIALS. THE SOLE AND EXCLUSIVE
LIABILITY TO AUTODESK, INC., REGARDLESS OF THE FORM OF ACTION, SHALL NOT EXCEED THE PURCHASE PRICE OF THE
MATERIALS DESCRIBED HEREIN.
Autodesk, Inc. reserves the right to revise and improve its products as it sees fit. This publication describes the state of this product at the time of its publication,
and may not reflect the product at all times in the future.

Autodesk Trademarks
The following are registered trademarks of Autodesk, Inc., in the USA and/or other countries: 3D Plan, 3D Props, 3D Studio, 3D Studio MAX, 3D
Studio VIZ, 3DSurfer, ActiveShapes, ActiveShapes (logo), Actrix, ADE, ADI, Advanced Modeling Extension, AEC Authority (logo), AEC-X, AME,
Animator Pro, Animator Studio, ATC, AUGI, AutoCAD, AutoCAD Data Extension, AutoCAD Development System, AutoCAD LT, AutoCAD Map,
Autodesk, Autodesk Animator, Autodesk (logo), Autodesk MapGuide, Autodesk University, Autodesk View, Autodesk WalkThrough, Autodesk World,
AutoLISP, AutoShade, AutoSketch, AutoSurf, AutoVision, Biped, bringing information down to earth, CAD Overlay, Character Studio, Design
Companion, Design Your World, Design Your World (logo), Drafix, Education by Design, Generic, Generic 3D Drafting, Generic CADD, Generic
Software, Geodyssey, Heidi, HOOPS, Hyperwire, Inside Track, Kinetix, MaterialSpec, Mechanical Desktop, Multimedia Explorer, NAAUG, ObjectARX,
Office Series, Opus, PeopleTracker, Physique, Planix, Powered with Autodesk Technology, Powered with Autodesk Technology (logo), RadioRay,
Rastation, Softdesk, Softdesk (logo), Solution 3000, Tech Talk, Texture Universe, The AEC Authority, The Auto Architect, TinkerTech, VISION*, WHIP!,
WHIP! (logo), Woodbourne, WorkCenter, and World-Creating Toolkit.
The following are trademarks of Autodesk, Inc., in the USA and/or other countries: 3D on the PC, 3ds max, ACAD, Advanced User Interface, AEC
Office, AME Link, Animation Partner, Animation Player, Animation Pro Player, A Studio in Every Computer, ATLAST, Auto-Architect, AutoCAD
Architectural Desktop, AutoCAD Architectural Desktop Learning Assistance, AutoCAD Learning Assistance, AutoCAD LT Learning Assistance, AutoCAD
Simulator, AutoCAD SQL Extension, AutoCAD SQL Interface, Autodesk Animator Clips, Autodesk Animator Theatre, Autodesk Device Interface,
Autodesk Inventor, Autodesk PhotoEDIT, Autodesk Software Developer’s Kit, Autodesk Streamline, Autodesk View DwgX, AutoFlix, AutoPAD,
AutoSnap, AutoTrack, Built with ObjectARX (logo), ClearScale, Colour Warper, Combustion, Concept Studio, Content Explorer, cornerStone Toolkit,
Dancing Baby (image), Design 2000 (logo), DesignCenter, Design Doctor, Designer’s Toolkit, DesignProf, DesignServer, DWG Linking, DWG
Unplugged, DXF, Extending the Design Team, FLI, FLIC, GDX Driver, Generic 3D, gmax, Heads-up Design, Home Series, i-drop, Kinetix (logo),
Lightscape, ObjectDBX, onscreen onair online, Ooga-Chaka, Photo Landscape, Photoscape, Plasma, Plugs and Sockets, PolarSnap, Pro Landscape,
QuickCAD, Reactor, Real-Time Roto, Render Queue, SchoolBox, Simply Smarter Diagramming, SketchTools, Sparks, Suddenly Everything Clicks,
Supportdesk, The Dancing Baby, Transform Ideas Into Reality, Visual LISP, Visual Syllabus, VIZable, Volo, and Where Design Connects.

Third Party Trademarks
All other brand names, product names or trademarks belong to their respective holders.

Third Party Software Program Credits
ACIS Copyright © 1989-2001 Spatial Corp.
Anderson, et. al. LAPACK Users’ Guide, Third Edition. Society for Industrial and Applied Mathematics, 1999.
Portions Copyright © 1991-1996 Arthur D. Applegate. All rights reserved.
Typefaces from the Bitstream ® typeface library copyright 1992.
Cypress Enable™, Cypress Software, Inc.
dBASE is a registered trademark of Ksoft, Inc.
Portions licensed from D-Cubed Ltd. DCM-2D and CDM are a trademark of D-Cubed Ltd. DCM-2D Copyright D-Cubed Ltd. 1989-2001.
CDM Copyright D-Cubed Ltd. 1998-2001.
SPEC is a registered trademark of Associated Spring/Barnes Group, Inc.
Portions of this software are based on the work of the Independent JPEG Group.
InstallShield™ 3.0. Copyright © 1997 InstallShield Software Corporation. All rights reserved.
Licensing Technology Copyright © C-Dilla Ltd. UK 1996, 1997, 1998, 1999, 2000, 2001.
MD5C.C - RSA Data Security, Inc., MD5 message-digest algorithm Copyright © 1991-1992, RSA Data Security, Inc. Created 1991. All
rights reserved.
International CorrectSpell™ Spelling Correction System © 1995 by Lernout & Hauspie Speech Products, N.V. All rights reserved.
LUCA TCP/IP Package, Portions Copyright © 1997 Langener GmbH. All rights reserved.
Copyright © 1997 Microsoft Corporation. All rights reserved.
Microsoft® HTML Help Copyright © Microsoft Corporation 2001.
Microsoft® Internet Explorer 5 Copyright © Microsoft Corporation 2001. All rights reserved
Microsoft® Windows NetMeeting Copyright © Microsoft Corporation 2001. All rights reserved
Objective Grid ©, Stingray Software a division of Rogue Wave Software, Inc.
Typefaces from Payne Loving Trust © 1996. All rights reserved.
PKWARE Data Compression Library ©, PKWARE, Inc.
SMLib © 1998-2000, IntegrityWare, Inc., GeomWare, Inc., and Solid Modeling Solutions, Inc.

GOVERNMENT USE
Use, duplication, or disclosure by the U. S. Government is subject to restrictions as set forth in FAR 12.212 (Commercial Computer
Software-Restricted Rights) and DFAR 227.7202 (Rights in Technical Data and Computer Software), as applicable.

1 2 3 4 5 6 7 8 9 10

Contents

Part I

Getting Started with Autodesk Mechanical Desktop . 1

Chapter 1

Welcome . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3
What is Autodesk Mechanical Desktop?. . . . . . . . . . . . . . . . . . . . . . . . . . . . 4
Making the Transition from AutoCAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Migrating Files from Previous Releases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5
Data Exchange. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 6

Chapter 2

Modeling with Autodesk®Mechanical Desktop®. . . . . . . . . . . . . . . 7
Mechanical Desktop Basics . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

Chapter 3

The User Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13
Mechanical Desktop Today . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14
Mechanical Desktop Environments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
Assembly Modeling Environment . . . . . . . . . . . . . . . . . . . . . . . . . . . 15
Part Modeling Environment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16
Mechanical Desktop Interface. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17
Desktop Browser. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18
Issuing Commands . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24

Chapter 4

Documentation and Support . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27
Printed and Online Manuals . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
Mechanical Desktop Printed Manual . . . . . . . . . . . . . . . . . . . . . . . . 28
AutoCAD Printed Manual . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
Online Installation Guide . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28
AutoCAD 2002 Documentation . . . . . . . . . . . . . . . . . . . . . . . . . . . . 29

iii

Mechanical Desktop Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30
Updating Help Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30
Product Support Assistance in Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
Updating the Support Assistance Knowledge Base. . . . . . . . . . . . . . .31
Learning and Training Resources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31
Internet Resources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32

Part I

Autodesk Mechanical Desktop Tutorials. . . . . . . . . . 33

Chapter 5

Using the Tutorials . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35
How the Tutorials are Organized . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .36
Accessing Mechanical Desktop Commands. . . . . . . . . . . . . . . . . . . . . . . . .37
Positioning the Desktop Browser . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .38
Backing up Tutorial Drawing Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .40

Chapter 6

Creating Parametric Sketches. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .42
Basic Concepts of Parametric Sketching . . . . . . . . . . . . . . . . . . . . . . . . . . .43
Sketching Tips . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .44
Creating Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .45
Creating Text Sketch Profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .45
Creating Open Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . .46
Creating Closed Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . .46
Using Default Sketch Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .47
Using Custom Sketch Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .51
Using Nested Loops. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .56
Creating Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .58
Creating 2D Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .58
Creating 3D Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .62
Creating Cut Line Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .72
Creating Split Line Sketches. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .77
Creating Break Line Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .80

Chapter 7

Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .84
Basic Concepts of Creating Constraints. . . . . . . . . . . . . . . . . . . . . . . . . . . .85
Constraining Tips. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .86
Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .86

Contents

Applying Geometric Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88
Showing Constraint Symbols. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90
Replacing Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91
Applying Dimension Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94
Creating Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96
Adding Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 97
Appending Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100
Modifying Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 104
Using Construction Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105
Creating Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105
Adding Project Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107
Adding Parametric Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109
Constraining Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 111
Controlling Tangency . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 115

Chapter 8

Creating Sketched Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 121
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 122
Basic Concepts of Sketched Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123
Creating Extruded Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124
Extruding Closed Profiles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124
Editing Extruded Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130
Extruding Open Profiles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133
Creating Rib Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133
Creating Thin Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 136
Creating Emboss Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140
Editing Emboss Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 143
Creating Loft Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 143
Creating Linear Lofts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 143
Creating Cubic Lofts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145
Editing Loft Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149
Creating Revolved Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150
Editing Revolved Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 151
Creating Face Splits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152
Editing Face Splits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155
Creating Sweep Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 155
Creating 2D Sweep Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156
Creating 3D Sweep Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157
Editing Sweep Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163
Creating Bend Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163
Editing Bend Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165

Contents

Chapter 9

Creating Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .168
Basic Concepts of Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .169
Creating Work Planes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .170
Editing Work Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .173
Creating Work Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .174
Editing Work Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .177
Creating Work Points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .179
Editing Work Points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .182

Chapter 10

Creating Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .186
Basic Concepts of Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .187
Creating Hole Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .188
Creating Thread Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .190
Editing Hole Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .192
Editing Thread Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .193
Creating Face Drafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .194
Editing Face Drafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .198
Creating Fillet Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .199
Editing Fillet Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .202
Creating Chamfer Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .204
Editing Chamfer Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .208
Creating Shell Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .209
Editing Shell Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .210
Creating Surface Cut Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .212
Editing Surface Cut Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .213
Creating Pattern Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .214
Editing Pattern Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .223
Editing Array Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .223
Creating Copied Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .224
Editing Copied Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .227
Creating Combined Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .227
Editing Combined Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .228
Creating Part Splits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .229
Editing Part Splits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .231

Chapter 11

Using Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .234
Basic Concepts of Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .235
Preparing The Drawing File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .236

Contents

Using Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Active Part Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Global Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Creating Active Part Design Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . 239
Assigning Design Variables to Active Parts . . . . . . . . . . . . . . . . . . . . . . . . 242
Modifying Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 244
Working with Global Design Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . 246

Chapter 12

Creating Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 253
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 254
Basic Concepts of Creating Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 255
Creating Base Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 257
Sketching Base Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 258
Creating Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 264
Defining Sketch Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 267
Creating Extruded Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 270
Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 271
Dimensioning Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 274
Creating Constraints Between Features . . . . . . . . . . . . . . . . . . . . . . 276
Editing Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 280
Extruding Profiles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 282
Creating Revolved Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 284
Creating Symmetrical Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 290
Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 291
Refining Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 297
Shading and Lighting Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 304

Chapter 13

Creating Drawing Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 307
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 308
Basic Concepts of Creating Drawing Views . . . . . . . . . . . . . . . . . . . . . . . 309
Planning and Setting Up Drawings. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 309
Creating Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 310
Cleaning Up Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 322
Hiding Extraneous Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 322
Moving Dimensions. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 325
Hiding Extraneous Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 328
Enhancing Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 330
Changing Dimension Attributes . . . . . . . . . . . . . . . . . . . . . . . . . . . 330
Creating Reference Dimensions. . . . . . . . . . . . . . . . . . . . . . . . . . . . 332
Creating Hole Notes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 333
Creating Centerlines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 336
Creating Other Annotation Items . . . . . . . . . . . . . . . . . . . . . . . . . . 337
Modifying Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 340
Exporting Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 343

Contents

vii

Chapter 14

Creating Shells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 345
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .346
Basic Concepts of Creating Shells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .347
Adding Shell Features to Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .347
Using Replay to Examine Designs . . . . . . . . . . . . . . . . . . . . . . . . . .348
Cutting Models to Create Shells . . . . . . . . . . . . . . . . . . . . . . . . . . . .350
Editing Shell Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .352
Adding Multiple Wall Thicknesses . . . . . . . . . . . . . . . . . . . . . . . . . .354
Managing Multiple Thickness Overrides . . . . . . . . . . . . . . . . . . . . .358

Chapter 15

Creating Table Driven Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 361
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .362
Basic Concepts of Table Driven Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . .363
Setting Up Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .364
Displaying Part Versions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .366
Editing Tables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .367
Resolving Common Table Errors . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .369
Suppressing Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .371
Working with Two Part Versions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .377
Creating Drawing Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .379
Cleaning Up the Drawing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .384
Displaying Dimensions as Parameters . . . . . . . . . . . . . . . . . . . . . . .384
Hiding Extraneous Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . .385
Moving Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .387
Enhancing Drawings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .390
Creating Power Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .390
Creating Hole Notes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .393
Pasting Linked Spreadsheets . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .396

Chapter 16

Assembling Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 399
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .400
Basic Concepts of Assembling Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .401
Starting Assembly Designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .402
Using External Parts in Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .403
Assembling Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .406
Constraining Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .407
Using the Desktop Browser . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .414
Getting Information from Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . .417
Checking for Interference . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .417
Calculating Mass Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .418
Creating Assembly Scenes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .420

viii

Contents

Creating Assembly Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 425
Editing Assemblies. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433
Editing External Subassemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433
Editing External Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 434
Editing Assembly Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 438

Chapter 17

Combining Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 443
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 444
Basic Concepts of Combining Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 445
Working in Single Part Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 446
Creating Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 447
Creating Toolbody Part Definitions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 449
Working with Combine Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 458
Creating Relief Toolbodies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 461
Combining Toolbodies with Spacers . . . . . . . . . . . . . . . . . . . . . . . . . . . . 463
Adding Weight Reduction Holes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 465
Adding Weight Reduction Extrusions. . . . . . . . . . . . . . . . . . . . . . . . . . . . 471
Adding Mounting Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 474

Chapter 18

Assembling Complex Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . 477
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 478
Basic Concepts of Complex Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . 479
Starting the Assembly Process . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 479
Creating Local and External Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 481
Applying Assembly Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 483
Creating New Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 491
Creating Subassemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 494
Defining and Activating Subassemblies. . . . . . . . . . . . . . . . . . . . . . 494
Using External Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 495
Instancing Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 496
Completing Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 497
Applying Assembly Constraints. . . . . . . . . . . . . . . . . . . . . . . . . . . . 497
Restructuring Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 504
Analyzing Assemblies. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 506
Editing Mechanical Desktop Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 508
Reloading External References . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 509
Assigning Mass Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 510
Calculating Mass Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 511
Reviewing Assembly Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 513
Creating Exploded Assembly Scenes . . . . . . . . . . . . . . . . . . . . . . . . 513
Using Tweaks and Trails in Scenes. . . . . . . . . . . . . . . . . . . . . . . . . . 515
Creating Assembly Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . 518

Contents

Creating Bills of Material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .522
Customizing BOM Databases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .523
Working with Part References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .525
Adding Balloons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .527
Placing Parts Lists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .529
Finishing Drawings for Plotting . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .531

Chapter 19

Creating and Editing Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . 533
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .534
Basic Concepts of Creating Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . .535
Working with Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .536
Creating Motion-Based Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .538
Revolved Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .538
Extruded Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .539
Swept Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .540
Creating Skin Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .546
Ruled Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .546
Trimmed Planar Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .554
Lofted Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .555
Creating Derived Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .559
Blended Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .559
Offset Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .563
Fillet and Corner Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .565
Editing Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .569
Adjusting Adjacent Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .569
Joining Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .570
Trimming Intersecting Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . .571
Trimming Surfaces by Projection . . . . . . . . . . . . . . . . . . . . . . . . . . .573

Chapter 20

Combining Parts and Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . 575
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .576
Basic Concepts of Combining Parts and Surfaces . . . . . . . . . . . . . . . . . . .577
Using Surface Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .577
Creating Surface Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .579
Attaching Surfaces Parametrically . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .582
Cutting Parts with Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .584
Creating Extruded Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .586
Creating Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .598
Creating Features on a Work Plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .601
Modifying Designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .609
Finishing Touches on Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .611

Contents

Chapter 21

Surfacing Wireframe Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . 613
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 614
Basic Concepts of Surfacing Wireframe Models . . . . . . . . . . . . . . . . . . . . 615
Discerning Design Intent . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 615
Identifying Logical Surface Areas. . . . . . . . . . . . . . . . . . . . . . . . . . . 616
Identifying Base Surface Areas . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 617
Using Trimmed Planar Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . 619
Choosing a Surfacing Method . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 620
Verifying Surfacing Results . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 623
Surfacing Wireframe Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 624
Creating Trimmed Planar Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 626
Joining Surfaces on Complex Shapes . . . . . . . . . . . . . . . . . . . . . . . . . . . . 634
Creating Swept and Projected Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . 645
Creating Complex Swept Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 655
Using Projection to Create Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 661
Using Advanced Surfacing Techniques . . . . . . . . . . . . . . . . . . . . . . . . . . . 665
Viewing Completed Surfaced Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . 669

Chapter 22

Working with Standard Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . 671
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 672
Tutorial at a Glance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 673
Basic Concepts of Standard Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 673
Inserting Through Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 674
Using Cylinder Axial Placement . . . . . . . . . . . . . . . . . . . . . . . . . . . 674
Using Cylinder Radial Placement . . . . . . . . . . . . . . . . . . . . . . . . . . 677
Inserting Screw Connections . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 681

Chapter 23

Creating Shafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 689
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 690
Tutorial at a Glance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 691
Basic Concepts of the Shaft Generator . . . . . . . . . . . . . . . . . . . . . . . . . . . 691
Using the Shaft Generator. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 692
Getting Started . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 692
Creating Shaft Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 693
Adding Threads to Shafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 695
Adding Profile Information to Shafts . . . . . . . . . . . . . . . . . . . . . . . 697
Editing Shafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 698
Adding Standard Parts to Shafts. . . . . . . . . . . . . . . . . . . . . . . . . . . . 701
Displaying and Shading 3D Views. . . . . . . . . . . . . . . . . . . . . . . . . . 705

Contents

Chapter 24

Calculating Stress on 3D Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 707
Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .708
Tutorial at a Glance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709
Basic Concepts of 3D FEA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709
Using 3D FEA Calculations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .710
Performing Finite Element Analyses. . . . . . . . . . . . . . . . . . . . . . . . .710
Defining Supports and Forces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .711
Calculating and Displaying the Result . . . . . . . . . . . . . . . . . . . . . . .715
Desktop Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .720
Part Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .721
Part Modeling ➤ New Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .721
Part Modeling ➤ New Sketch Plane . . . . . . . . . . . . . . . . . . . . . . . . .722
Part Modeling ➤ 2D Sketching . . . . . . . . . . . . . . . . . . . . . . . . . . . . .722
Part Modeling ➤ 2D Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . .725
Part Modeling ➤ Profile a Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . .726
Part Modeling ➤ Sketched Features . . . . . . . . . . . . . . . . . . . . . . . . .727
Part Modeling ➤ Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . .727
Part Modeling ➤ Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . .727
Part Modeling ➤ Power Dimensioning . . . . . . . . . . . . . . . . . . . . . .728
Part Modeling ➤ Edit Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .728
Part Modeling ➤ Update Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .728
Part Modeling ➤ Part Visibility . . . . . . . . . . . . . . . . . . . . . . . . . . . .729
Part Modeling ➤ Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .729
Toolbody Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .730
Toolbody Modeling ➤ New Toolbody . . . . . . . . . . . . . . . . . . . . . . .730
Toolbody Modeling ➤ Part Catalog . . . . . . . . . . . . . . . . . . . . . . . . .730
Toolbody Modeling ➤ 3D Toolbody Constraints . . . . . . . . . . . . . .731
Toolbody Modeling ➤ Power Manipulator . . . . . . . . . . . . . . . . . . .731
Toolbody Modeling ➤ Check Interference. . . . . . . . . . . . . . . . . . . .731
Toolbody Modeling ➤ Toolbody Visibility . . . . . . . . . . . . . . . . . . .732
Assembly Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .732
Assembly Modeling ➤ New Subassembly. . . . . . . . . . . . . . . . . . . . .733
Assembly Modeling ➤ Assembly Catalog . . . . . . . . . . . . . . . . . . . . .733
Assembly Modeling ➤ 3D Assembly Constraints. . . . . . . . . . . . . . .733
Assembly Modeling ➤ Assign Attributes . . . . . . . . . . . . . . . . . . . . .734
Assembly Modeling ➤ Power Manipulator . . . . . . . . . . . . . . . . . . .734
Assembly Modeling ➤ Mass Properties. . . . . . . . . . . . . . . . . . . . . . .734
Assembly Modeling ➤ Assembly Visibility. . . . . . . . . . . . . . . . . . . .734

xii

Contents

Surface Modeling. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 735
Surface Modeling ➤ AutoSurf Options . . . . . . . . . . . . . . . . . . . . . . 735
Surface Modeling ➤ Swept Surface . . . . . . . . . . . . . . . . . . . . . . . . . 736
Surface Modeling ➤ Loft U Surface . . . . . . . . . . . . . . . . . . . . . . . . . 736
Surface Modeling ➤ Blended Surface. . . . . . . . . . . . . . . . . . . . . . . . 736
Surface Modeling ➤ Flow Wires . . . . . . . . . . . . . . . . . . . . . . . . . . . 737
Surface Modeling ➤ Object Visibility . . . . . . . . . . . . . . . . . . . . . . . 737
Surface Modeling ➤ Surface Display . . . . . . . . . . . . . . . . . . . . . . . . 737
Surface Modeling ➤ Stitches Surfaces . . . . . . . . . . . . . . . . . . . . . . . 738
Surface Modeling ➤ Grip Point Placement . . . . . . . . . . . . . . . . . . . 738
Surface Modeling ➤ Lengthen Surface . . . . . . . . . . . . . . . . . . . . . . 738
Surface Modeling ➤ Extract Surface Loop . . . . . . . . . . . . . . . . . . . . 739
Surface Modeling ➤ Edit Augmented Line . . . . . . . . . . . . . . . . . . . 739
Surface Modeling ➤ Wire Direction . . . . . . . . . . . . . . . . . . . . . . . . 739
Scene . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 740
Scene ➤ New Scene . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 740
Scene ➤ Scene Visibility. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 741
Drawing Layout . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 741
Drawing Layout ➤ Power Dimensioning . . . . . . . . . . . . . . . . . . . . 742
Drawing Layout ➤ Drawing Visibility . . . . . . . . . . . . . . . . . . . . . . . 744
Mechanical View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 744
Mechanical View ➤ Zoom Realtime . . . . . . . . . . . . . . . . . . . . . . . . 745
Mechanical View ➤ 3D Orbit . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 745
Mechanical View ➤ Sketch View . . . . . . . . . . . . . . . . . . . . . . . . . . . 746
Mechanical View ➤ Restore View #1. . . . . . . . . . . . . . . . . . . . . . . . 746
Mechanical View ➤ Toggle Shading/Wireframe . . . . . . . . . . . . . . . 747

Index . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 749

Contents

xiii

xiv

Part I
Getting Started
with Autodesk
Mechanical Desktop
®

Part I provides information for getting started with your Mechanical Desktop 6 software. It
includes information to help in the transition from AutoCAD® and the migration of files
from previous releases. It explains the user interface and the basics of modeling in the
different work environments in Mechanical Desktop.
In addition, Part I provides a guide to both the print and online documentation that you
received with your Mechanical Desktop software. Information about training courseware
and Internet resources are also included.

Welcome

In This Chapter

This chapter provides an overview of the capabilities of
Autodesk® Mechanical Desktop® 6 software. You learn
®

about the transition from AutoCAD , data exchange,

■ About Mechanical Desktop
■ Making the transition from

AutoCAD
■ Migrating files from previous

releases
and the migration of files from previous releases with the
Mechanical Desktop Migration Assistance.

What is Autodesk Mechanical Desktop?
Mechanical Desktop is a powerful and easy-to-use 3D parametric modeler
used in mechanical design. Built on AutoCAD 2002, the Mechanical Desktop
6 design software package includes:
■
■
■

AutoCAD Mechanical 6 with the power pack (2D Parts and Calculations)
Mechanical Desktop 6 with the power pack (Mechanical Desktop 6, 3D
Parts and Calculations)
AutoCAD 2002

When you start Mechanical Desktop 6, you have the option to run it with or
without the power pack.
The Mechanical Desktop software provides design tools to
■
■
■
■
■
■
■
■

Create parts from sketched and placed features
Combine parts and toolbodies
Build assemblies and subassemblies
Define scenes for drawing views
Set up drawing sheets and views
Annotate drawings for final documentation
Manage and reuse design data
Migrate and edit legacy solids data

Productivity and collaboration tools in Mechanical Desktop enable you to
improve workflows and comply with company practices.
Web tools are provided in a design portal called the Today page. From the
Today page, you can
■
■
■
■
■

Start a new drawing or open an existing drawing
Access symbol libraries
Communicate to design team members through a Web page you create
from a template provided
Link directly to design information on the Web
Link directly to Autodesk Web pages

For more information about the Today page, see “Mechanical Desktop
Today” on page 14.

Chapter 1

Welcome

Making the Transition from AutoCAD
Mechanical Desktop 6 is built on AutoCAD 2002 and uses many of the tools
you may already be familiar with. Because Mechanical Desktop is a parametric
modeling program, exercise care in using standard AutoCAD commands.
In the sketching stage, you can use any AutoCAD command to create the
geometry for your sketch. You can use AutoCAD drawing and editing tools
to edit sketch geometry after it has been consumed by a feature.
In general, follow these rules:
■

■

■
■

■

Use Mechanical Desktop dimensions. AutoCAD dimensions are not
parametric and cannot control the size, shape, or position of Mechanical
Desktop parts and features.
Use sketch planes and work planes to control the UCS orientation. Using
the AutoCAD UCS command does not associate the current plane with
your part.
Do not use the command EXPLODE. Exploding a part deletes the part
definition from a Mechanical Desktop drawing.
Use the Assembly Catalog or the Browser to insert external part files into
drawings and externalize part files. Using the AutoCAD INSERT, WBLOCK,
XREF, and XBIND commands could corrupt Mechanical Desktop data.
Use the Mechanical Desktop drawing view commands to create drawing
views. The AutoCAD MVIEW command does not create associative views
of your parts.

Migrating Files from Previous Releases
In Mechanical Desktop 6, you can add more than one part to a part file for
creating combined parts. The first part becomes the part definition, while all
other parts become unconsumed toolbodies. You combine toolbodies with
each other and the first part to create a complex part.
To migrate parts from a part file that contains more than one part and was
created before Mechanical Desktop Release 2, you need to follow specific
procedures. See "Running the Desktop File Migration Utility" in the Autodesk
Mechanical Products Installation Guide on the product CD.
The File Migration Tool (FMT) is a component of Mechanical Desktop
Migration Assistance, an independent Visual Basic (not VBA) application
located on your product CD. The FMT migrates multiple files from previous
releases of Mechanical Desktop to the current format. You can install
Mechanical Desktop Migration Assistance during or after the installation of
your Autodesk mechanical product.

Making the Transition from AutoCAD

To install the Mechanical Desktop Migration Assistance from your product CD
1 Hold down the SHIFT key while you insert the product CD into the CD-ROM
drive. This prevents Setup from starting automatically.
2 In the file tree of the CD-ROM drive, navigate to the Migrate folder and click
setup.exe.
3 Respond to the directions in the Mechanical Desktop Migration Assistance
installation dialog boxes.

NOTE For more information about installing the Migration Assistance and
running the FMT, see "Mechanical Desktop Migration Assistance" in the
Autodesk Mechanical Products Installation Guide on your product CD.

Data Exchange
During your design process, you may want to complement Mechanical
Desktop with other computer-aided design (CAD) software. Mechanical
Desktop 6 includes the STEP translator and the IGES Translator. The Standard
for the Exchange of Product Model Data (STEP) is International Standards
Organization (ISO) 10303. The Initial Graphics Exchange Specification
(IGES) is the ANSI standard for data exchange between CAD systems and is
supported by many CAD vendors.
The IGES Translator is compliant with the most recent version of IGES and
related standards. It supports both the United States Department of Defense
Continuous Acquisition and Life-cycle Support initiative (CALS) and the Japanese Automotive Manufacturers Association subset of IGES (JAMA).
Besides creating and maintaining a flexible CAD tool environment, the
Translator preserves the investment you have made in previous designs
developed with other CAD systems.
The Translator supports the following types of design objects:
■
■
■

2D and 3D wireframe geometry
Ruled, parametric, and NURBS surfaces
Mechanical Desktop and AutoCAD native solids, and IGES boundary
representation solids (B-rep).

For more information, see STEP and IGES in the Mechanical Desktop Help.

Chapter 1

Welcome

Modeling with Autodesk
Mechanical Desktop

In This Chapter

This chapter describes the basic concepts of mechanical
design with Autodesk Mechanical Desktop software,

■ Mechanical Desktop basics
■ Mechanical Desktop work

environments

including fundamentals of parametric design.
If you understand the underlying concepts in this chapter, you can become proficient in using the Mechanical
Desktop software.

Mechanical Desktop Basics
Mechanical Desktop is an integrated package of advanced 3D modeling tools
and 2D drafting and drawing capabilities that helps you conceptualize,
design, and document your mechanical products.
You create models of 3D parts, not just 2D drawings.
You use these 3D parts to create 2D drawings and 3D assemblies.

2D drawing

3D part

Mechanical Desktop, a dimension-driven system, creates parametric models.
Your model is defined in terms of the size, shape, and position of its features.
You can modify the size and shape of your model, while preserving your
design intent.

original part

revised part

You build parts from features—the basic shapes of your part.
Building blocks like extrusions, lofts, sweeps, bends, holes, fillets, and chamfers are parametrically combined to create your part.

revolved feature

Chapter 2

extruded feature

Modeling with Autodesk Mechanical Desktop

You create most features from sketches.
Sketches can be extruded, revolved, lofted, or swept along a path to create
features.

sketch for revolved feature

sketch for extruded feature

You work in the Part Modeling environment to create single parts.
In this environment, only one part can exist in a drawing. Additional parts
become unconsumed toolbodies for the purpose of creating a combined part.
Use part files to build a library of standardized parts.

examples of single part files

You work in Assembly Modeling to create multiple parts and assemblies.
In this environment, any number of parts can exist in one drawing. Parts can
be externally referenced from part and assembly files, or localized in the
assembly drawing.

assembly file containing four external part files

Mechanical Desktop Basics

Individual parts can be fit together to create subassemblies and assemblies.
Assembly files contain more than one part. Parts are fit together using assembly constraints to define the positions of the individual parts that make up
your final product.

individual parts in an assembly file

completed assembly

For standard parts, you can define different versions using a spreadsheet.
Instead of a large library of parts that differ only in size, like springs, bolts,
nuts, washers, and clamps, you can create one part and define different versions of that part in a spreadsheet that is linked to your drawing.

table driven part versions

You can also create 3D surface models.
Surface modeling is useful in the design of stamping dies, castings, or injection molds. You can also use surfaces to add to or cut material from a solid
part to create hybrid shapes.

surfaces used to create a part

Chapter 2

surface cut applied to a part

Modeling with Autodesk Mechanical Desktop

You can create scenes to define how your design fits together.
To better conceptualize the position of the parts in your assembly, you define
scenes using explosion factors, tweaks, and trails that illustrate how your
design is assembled.

exploded scene

You can create base, orthogonal, isometric, section, and detail views.
To document your design, drawing views can be created from scenes, parts,
or groups of selected objects. Any design changes are automatically updated
in these drawing views.

parametric drawing views

Add annotations and additional dimensions to finalize your documentation.
After you have created drawing views, finalize your design by adding balloons, bills of material, notes, reference dimensions, and mechanical
symbols.

annotations added to drawing

Mechanical Desktop Basics

The User Interface

In This Chapter

When you start the Autodesk® Mechanical Desktop® 6
software, a page called the Today window is displayed.

■ The Today window
■ Work environments
■ Mechanical Desktop interface

This chapter provides an overview of the options on the

■ Working in the Browser

Today window to help manage your work, collaborate

■ Methods for issuing commands

with others, and link to information on the Web.
Information about the work environments and the user
interface are included to help you get started using the
Mechanical Desktop software.

Mechanical Desktop Today
The first time you open the Mechanical Desktop 6 program, the Today window
is displayed on top of the program interface, along with instructions about how
to use it. The Today feature is a powerful tool that makes it easy to manage drawings, communicate with design teams, and link directly to design information.
In the Today Window, you can expand the following options for access to the
the services you require.
My Workplace

Connect directly to files on your computer and your local
network.

My Drawings

Open existing drawings, create new ones, or access
symbol libraries.

Bulletin Board

Post your own Web page with links to block libraries, CAD
standards, or other folders and directories on your
company network. CAD managers can use the Bulletin
Board to communicate with their design teams. An HTML
bulletin board template is provided.

The Web

Connect directly to the Internet.

Autodesk
Point A

Link directly to design information and tools such as
Buzzsaw.com on the Web. Use the units converter, link to
Autodesk Web sites, and much more.
Login and create your free account. Customize the
information in Autodesk Point A for your specific needs.

You can close the Today Window and use the File menu to create new drawings or open existing drawings.
To reopen Today, in the Assist menu choose Mechanical Desktop Today.
If you prefer not to see the Today Window when you start Mechanical
Desktop, you can turn it off in Assist ➤ Options ➤ System ➤ Startup.

Chapter 3

The User Interface

Mechanical Desktop Environments
Mechanical Desktop has two working environments: Assembly Modeling
and Part Modeling.

Assembly Modeling Environment
This is the environment Mechanical Desktop uses when you start the
program or create a new file by using File ➤ New. Any number of parts and
subassemblies can coexist in the same drawing.
The advantages of the Assembly Modeling environment are
■
■
■
■

More than one part can be created in the same drawing.
Individual part files, and other assemblies or subassemblies, can be externally referenced or localized and used to build a complex assembly.
Different versions of a part can be displayed in the same file.
Scenes containing explosion factors, tweaks, and trails can be created.

There are three modes in the Assembly Modeling environment: Model,
Scene, and Drawing.

Model Mode
In Model mode, you create as many parts as you need. Parts may be local or
externally referenced. Create subassemblies and save them for use in larger
assemblies. Build assemblies from any number of single part files, subassemblies, and assemblies. You can also generate a BOM (Bill of Material) database
so a list of parts can be placed in your final drawing.

Scene Mode
In Scene mode, you set explosion factors for your assembled parts and create
tweaks and trails. These settings govern how your drawing views represent
your assemblies.

Drawing Mode
In an assembly file, you can place balloons to reference the parts in your
assembly. You can create a parts list with as much information as you need
to define your parts. To illustrate how parts in an assembly fit together, you
can create base views on exploded scenes.

Mechanical Desktop Environments

Part Modeling Environment
To begin a new drawing in the Part Modeling environment, choose File ➤
New Part File. Only one part may exist in the drawing. If you add more parts,
they automatically become unconsumed toolbodies. You use toolbodies to
create complex combined parts.
The advantages of the Part Modeling environment are
■
■
■

A library of standard parts can be created for use in assembly files.
The interface is streamlined to allow only those commands available in a
part file.
File sizes are minimized because the database doesn’t need additional
assembly information.

There are two modes in the Part Modeling environment: Model and Drawing.

Model Mode
In Model mode, you build and modify your design to create a single parametric part. The part takes the name of the drawing file.

Drawing Mode
In Drawing mode, you define views of your part and place annotations for
documentation. You can also create a parts list and balloons to reference a
combined part and its toolbodies.

Chapter 3

The User Interface

Mechanical Desktop Interface
When you open a new or existing drawing in Mechanical Desktop 6, four
toolbars and the Desktop Browser are displayed.
■

■
■

■

The Mechanical Main toolbar provides quick access to select commands
from the AutoCAD Standard and the Object Properties toolbars, some
Mechanical Desktop commands, and the Web. Icons are available for
direct links to Mechanical Desktop Today window and Web tools such as,
Point A, Streamline, RedSpark, MeetNow, Publish to Web, and eTransmit.
The Desktop Tools toolbar acts as a toggle, giving you quick access to Part
Modeling, Assembly Modeling, Scenes, and Drawing Layout.
The Part Modeling toolbar is the default, but, when you use the Desktop
Tools toolbar or the Desktop Browser to switch modes, the toolbar representing the mode you have chosen is displayed.
The Mechanical View toolbar is designed to give you full control over how
you view your models, including real-time pan, zoom, dynamic 3D
rotation, and shading commands.
The Desktop Browser is docked at the left side of the screen.

Desktop Tools toolbar
Mechanical Main toolbar
Help
Mechanical View toolbar
Desktop Browser
Part Modeling toolbar

Mechanical Desktop Interface

There are four main toolbars controlled by the Desktop Tools toolbar: Part
Modeling, Assembly Modeling, Scene, and Drawing Layout.
Part Modeling
Assembly Modeling
Scene
Drawing Layout

If you begin a drawing in the Part Modeling environment, the Desktop Tools
toolbar changes to display three buttons that control the Part Modeling,
Toolbody Modeling, and Drawing Layout toolbars.
Part Modeling
Toolbody Modeling
Drawing Layout

In addition to controlling the Mechanical Desktop toolbars, the Desktop
Tools toolbar switches between Part, Toolbody/Assembly, Scene, and
Drawing modes.
For a complete description of Mechanical Desktop toolbars, see appendix A,
“Toolbar Icons.”

Desktop Browser
When you start Mechanical Desktop 6, the Desktop Browser is displayed in
the default position at the left of your screen.

Docking the Desktop Browser
Right-click the gray area at the top of the Browser for a context menu of docking
controls. You can turn the following Browser docking options on and off.
Allow Docking

With Docking on, you can drag a corner of the Browser to
change its shape and size, and you can drag the Browser
to a new location on your screen.
To return the Browser to its default position, turn on
Allow Docking, and double-click the Browser title bar.

Chapter 3

The User Interface

AutoHide

With AutoHide on, choose Collapse to minimize the
Browser. When you move the cursor over and off of the
Browser, it expands and collapses.
Choose Right or Left to hide the Browser off a side of the
screen. When you move your cursor to the corresponding
edge of the screen, the Browser is displayed. Move the
cursor off the Browser, and it is hidden again.
To turn AutoHide off, in the Browser docking menu
choose AutoHide ➤ Off.

Hide

Hides the Browser entirely. To restore it, in the Desktop
menu choose View ➤ Display ➤ Desktop Browser.

Working with the Desktop Browser
When you begin, Mechanical Desktop starts a new drawing in the Assembly
Modeling environment. The assembly is named for the current file.

When you create the first sketch, a part is automatically named, numbered,
and represented in the Browser. Because the first thing you create is a sketch,
it is nested under the part. As these objects are created, they are displayed
automatically in a hierarchy.

In the Browser, you can show as much or as little detail as you wish. When
there is more information, a plus sign is shown beside an object. You click
the plus sign to reveal more levels.

Mechanical Desktop Interface

You collapse levels by clicking the minus sign beside an object, or collapse
the entire hierarchy by right-clicking the assembly name and choosing
Collapse from the menu.
When you start a new drawing in the Part Modeling environment, or open
an existing part file, the Desktop Browser contains two tabs: Model and
Drawing. In the Assembly Modeling environment, the Browser contains
three tabs: Model, Scene, and Drawing. You can choose the tabs at the top of
the Browser window to navigate from one mode to another.

Part Modeling environment

Assembly Modeling environment

Icons at the bottom of the Browser provide quick access to frequently-used
commands.

Using the Browser in Part Modeling
When you are working in the Part Modeling environment, the Browser
contains two tabs: Model and Drawing.
Model Mode in Part Modeling
In Model mode, seven icons are displayed at the bottom of the Browser.

The two at the left are quick filters. These filters are available so that you can
control the visibility of features and assembly constraints in the Browser
when you are creating combined parts.

Chapter 3

The User Interface

The first icon, the Part filter, controls the display of assembly constraints
attached to a part and its toolbodies. If the Part filter is selected, only the
features of your part and its toolbodies are visible in the Browser. If it is not
selected, assembly constraints are also visible.
The second icon is the Assembly filter. If you select this filter, only assembly
constraints that are attached to your part and its toolbodies are visible.
The third icon accesses the Desktop Options dialog box where you control
the settings for your part, surfaces, drawing views, and miscellaneous desktop
preferences.
The middle icon provides immediate access to the Part Catalog. You use the
Part Catalog to attach and localize external part files, and instance external
and local parts in your current file for the purpose of creating combined parts.
The fifth icon opens the Desktop Visibility dialog box where you control the
visibility of your part, toolbodies, and drawing objects. The sixth icon
updates your part after you have made changes to it, and the last icon
updates assembly constraints if you are working with a combined part.
Drawing Mode in Part Modeling
In Drawing mode, six icons are displayed at the bottom of the Browser.

The first two icons on the left are toggles to control automatic updating of
your drawing views or part. The last four icons access desktop options,
control visibility, and manually update your drawing views or part.

Mechanical Desktop Interface

Using the Browser in Assembly Modeling
In the Assembly Modeling environment, the Browser displays three tabs:
Model, Scene, and Drawing. With these tabs, you can create multiple parts,
assemblies, scenes, BOMs, and documents, and you can reorder assemblies.
You can localize and externalize parts in the Browser without opening the
Assembly Catalog.
Model Mode in Assembly Modeling
Model mode in the Assembly Modeling environment has the same icons at
the bottom of the Browser as Model mode in the Part Modeling environment.
Because you are working in the Assembly environment, these icons provide
more functionality.

The first icon is the Part filter which you use to control the display of the
features that make up your parts. If the Part filter is selected, only part
features are visible in the Browser. If it is not selected, assembly constraints
are also visible.
The second icon is the Assembly filter. When you select this filter, only the
assembly constraints attached to your parts are visible.
The third icon opens the Mechanical Options dialog box. From this dialog
box you can manage your settings and standards for parts, assemblies,
surfaces, drawings, shaft generators, calculations, standard parts, and various
desktop preferences.
The middle icon provides access to the Assembly Catalog, a powerful interface for attaching and localizing external part and assembly files as well as
instancing both external and local parts in your current assembly.
The fifth icon controls the visibility of parts, assemblies, drawing entities, layers,
and linetypes. The sixth icon updates the active part after you have made
changes to it, and the last icon updates the active assembly or subassembly.

Chapter 3

The User Interface

Scene Mode in Assembly Modeling
In Scene mode, three icons are displayed at the bottom of the Browser.

The first icon accesses Desktop Options, where you can control the settings
for scenes. The second icon accesses Desktop Visibility, where you can
control the visibility of your parts, assemblies, and individual drawing
objects. The last icon updates the active scene.
Drawing Mode in Assembly Modeling
In Drawing mode, six icons perform the same functions as those in Drawing
mode in the Part Modeling environment.

Mechanical Desktop Interface

Issuing Commands
You can issue commands in several ways:
■
■
■
■
■
■

Select an option from a right-click menu in the Desktop Browser.
Select an option from a right-click menu in the active screen area of your
drawing.
Select a toolbar icon.
Select an option from a pull-down menu.
Enter the command name on the command line.
Use an abbreviation of the command, called an accelerator key, on the
command line.

Using Command Menus in the Desktop Browser
Many of the commands in Mechanical Desktop can be accessed using the
Browser menus. The Browser has two types of menus. One you activate by
right-clicking an existing object in the Browser. The other you activate by
right-clicking the Browser background. Options that are not available are gray.

The type of object you select with a right-click determines the menu displayed.
The mode you are in, Model, Scene, or Drawing, when you right-click the
Browser background determines the menu displayed.

Chapter 3

The User Interface

Using Context Menus in the Graphics Area
In addition to the Browser menus, context-sensitive menus are available in
the graphics area during the modeling process. When you start Mechanical
Desktop, the Part menu is available in the graphics area. You can toggle
between the Part and Assembly menus as you build your models. When you
are in Scene mode, the Scene menu is available. In Drawing mode, you can
toggle between the Drawing and Annotate menus.

Using Toolbars
Toolbars have icons to represent frequently-used commands, settings, and
environments. You can choose an icon instead of selecting a command from
a menu or entering its name on the command line. When you pause with
the mouse selection arrow on an icon, the command action is shown at the
bottom of the screen. A tooltip also appears under the cursor. Click the left
mouse button to select the command.

Some icons have a subtoolbar (flyout) with related icons. If the icon has a
small arrow in the lower right corner, drag the mouse to reveal the additional
icons, and then select one.

To hide a toolbar, click the button in its upper right corner. To unhide it,
right-click any toolbar. In the pop-up menu, select the toolbar to redisplay.
The toolbar is automatically redisplayed.
To reorient the Mechanical Desktop toolbars to their default positions,
choose View ➤ Toolbars ➤ Desktop Express (Left). If you prefer the toolbars
at the right of your screen, choose Desktop Express (Right).
You may want to view larger toolbar icons. To do so, right-click any toolbar
and choose Customize. Select Large Buttons at the bottom left of the Toolbars
dialog box.
If you choose Large Buttons and then dock the toolbars in the screen header
area above the command line or at either side of the screen, some icons may
not be visible. In that case, you can drag the toolbar onto the screen.

Mechanical Desktop Interface

Using Pull-down Menus
To select a menu option, or access a submenu, hold down the left mouse
button while you navigate through the menu. When you find the command
you want to use, release the mouse button.
You can also access menu commands by using the keyboard. Hold down ALT
while selecting the underlined letter of the menu option. For example, to
select AMPROFILE from the keyboard, press ALT, then P, S, P.

Selecting Command Options from Dialog Boxes
Many commands have options within dialog boxes. As the term dialog box
suggests, you interact by selecting options to make a particular setting active,
display a list from which to choose an option, or enter a specific value. If a
command has a dialog box, it is displayed when you access the command,
regardless of whether you did so on the command line or from a menu or
toolbar icon.
When you need information about a dialog box you are working with, click
the Help button located in the dialog box.

NOTE If the Mechanical Desktop dialog boxes do not display, on the
command line enter CMDDIA, and change the system variable to 1.

Using the Command Line
You can access a command or system variable directly by entering its name
on the command line. Many experienced users prefer this method because it
is faster than using menus. Some experienced users are familiar with specifying command options from the command line and prefer to turn off the
display of dialog boxes.
However, because many Mechanical Desktop commands require input
through their dialog boxes, it is recommended that you use the dialog boxes
instead of the command line to ensure that you have access to the full
functionality of each feature.
All the commands and system variables for Mechanical Desktop and
AutoCAD are documented in Help.

Using Accelerator Keys
Many commands also have shortcuts called accelerator keys. To issue a
command using an accelerator key, simply enter the command alias on the
command line.
For a complete list of Mechanical Desktop accelerator keys, see “Accelerator
Keys” in the Command Reference in Help.

Chapter 3

The User Interface

Documentation and
Support

In This Chapter

This chapter provides an overview of the printed and

■ Mechanical Desktop print

documentation
online documentation provided with Autodesk®
®

Mechanical Desktop 6. It guides you to resources for

■ Mechanical Desktop online

documentation
■ Product Support Assistance in

product learning, training, and support.

Help
■ Mechanical Desktop learning

Read this section so that any time you need product
information, you will know where to locate it.

and training
■ Your Internet resources

Printed and Online Manuals
The extensive set of printed and online documentation provided with your
purchase of Mechanical Desktop 6 software includes the printed Autodesk
Mechanical Desktop 6 User’s Guide, AutoCAD Mechanical 6 User’s Guide, and the
AutoCAD 2002 User’s Guide.
The online AutoCAD Mechanical 6 and Mechanical Desktop 6 Installation Guide
is provided on the product CD.
All of the Mechanical Desktop 6 manuals are available in PDF format on the
product CD, and on the Mechanical Desktop product page of the Autodesk
Web site at http://www.autodesk.com/mechdesktop ➤ Product Information ➤
Online and Print Manuals.

Mechanical Desktop Printed Manual
The printed Autodesk Mechanical Desktop 6 User’s Guide is divided into two
parts.
Part I

An introduction to the product and information you need
to get started using the software.

Part II

A set of tutorials to expand your skills in using Mechanical
Desktop and understanding mechanical design.
Chapters 5 through 21 focus on Mechanical Desktop,
while chapters 22 through 24 focus on Mechanical
Desktop with the power pack.

AutoCAD Printed Manual
The printed AutoCAD User’s Guide contains comprehensive information and
instructions for using AutoCAD. This manual is also available online in the
AutoCAD Help.

Online Installation Guide
The AutoCAD Mechanical 6 and Mechanical Desktop 6 Installation Guide is
available on the product CD. It provides the following information:
Introduction

What’s in the software.

Chapter 1

System requirements and recommendations for installing
and running the software.

28 |Chapter 4 Documentation and Support

Chapter 2

Procedures to install, upgrade, authorize, and maintain
the software for a single user, and information you need
to know before you begin your installation.

Chapter 3

Information for network administrators. Instructions for
installing and configuring for a network environment.

Chapter 4

Technical information about environment variables and
performance enhancements to optimize performance of
the software.

Chapter 5

Information about cabling and option settings, plus other
information necessary to link and configure plotters and
printers with AutoCAD Mechanical/Mechanical Desktop.

Chapter 6

Instructions to uninstall the software, maintain your hard
disk, and recover data in case of a system failure.

AutoCAD 2002 Documentation
You should be familiar with AutoCAD before you use Mechanical Desktop.
The complete set of AutoCAD 2002 documentation is available in the
AutoCAD Help. It includes:
■
■
■
■
■
■
■
■
■
■
■
■

User’s Guide*
Command Reference*
Customization Guide*
ActiveX® and VBA Developer’s Guide*
ActiveX® and VBA Reference
AutoLISP® Reference
Visual LISPTM Developer’s Guide*
Visual LISPTM Tutorial*
DXFTM Reference
Driver Peripheral Guide
Connectivity Automation Reference
Network Administrator’s Guide

AutoCAD 2002 manuals marked with an asterisk can be ordered in print from
your local reseller.
The AutoCAD 2002 Learning Assistance CD that is included in your package
is a multimedia learning tool for intermediate to experienced AutoCAD users.
If you currently own a valid license for an Autodesk product and require
replacement media or documentation, please call the Customer Service
Center at 1-800-538-6401 to order.

Printed and Online Manuals

Mechanical Desktop Help
The Help in Mechanical Desktop provides integrated information about
AutoCAD Mechanical and Mechanical Desktop.
The Help is formatted for easy navigation, and includes:
■
■
■
■
■
■
■

Content organized by the major functional areas of Mechanical Desktop,
with How To, Reference, and Learn About pages for each functional area
Specific information about each of the features in the program
Concepts and procedures for the new features in this release
A keyword index, search function, and Favorites tab
Printable Command Reference
Guides to system variables and accelerator keys
Access to Support Assistance with integrated links to solutions

For access to Help, you can choose from the following methods:
■
■
■
■

From the Help menu, select Mechanical Help Topics.
Select the Help button in the standard toolbar.
Press F1. This opens the topic for an active button or command.
Click the Help button within a dialog box.

Updating Help Files
If you have access to the Internet, you can download updated Help files from
the Autodesk Web site.
To update your Help files
1 In Mechanical Desktop Today, choose Autodesk Point A. In Useful Autodesk
Links, choose Autodesk Product Support Index.
2 Follow the links to Mechanical Desktop 6 product support and updates.

30 |Chapter 4 Documentation and Support

Product Support Assistance in Help
When you need product support, refer to Support Assistance in the Help
menu. Support Assistance ensures quick access to technical support information through an easy-to-use issue/solution format with self-help tools and a
knowledge base.
Product Support Assistance provides information about support options
available from resellers, Autodesk System Centers (ASCs), user groups in your
area, and those available directly from the Autodesk Web pages, including
the Autodesk Product Support Index.

Updating the Support Assistance Knowledge Base
You can update your Support Assistance knowledge base with the latest
support information about Mechanical Desktop by using the
Documentation Update utility in the Support Assistance Welcome.
To update your Support Assistance Knowledge Base
1 From the Help menu, choose Support Assistance, then choose Download.
2 Follow the prompts to update your knowledge base.

Learning and Training Resources
Many sources for learning and training are listed on the Mechanical Desktop
Learning and Training Web page. From the Mechanical Desktop Web site at
http://www.autodesk.com/mechdesktop, navigate to Learning and Training. You
can link directly to sources for
■
■
■

Online courses and tutorials
The Autodesk Official Training Courseware (AOTC)
A list of Autodesk authorized resellers and trainers

Autodesk Official Training Courseware (AOTC) is the Autodesk-endorsed
courseware for instructor-led training. To register for a training course,
contact an Authorized Autodesk Training Center, Authorized Autodesk
Reseller, or Autodesk System Center.

Product Support Assistance in Help

Internet Resources
Following are resources for information about Autodesk products and assistance with your Mechanical Desktop questions.
■
■
■
■
■
■

Autodesk Web site: http://www.autodesk.com
Mechanical Desktop home page at the Autodesk Web site:
http://www.autodesk.com/mechdesktop
AutoCAD Mechanical home page at the Autodesk Web site
http://www.autodesk.com/autocadmech
Mechanical Desktop discussion groups:
http://www.autodesk.com/mechdesktop-discussion
AutoCAD Mechanical discussion groups:
http://www.autodesk.com/autocadmech-discussion
To locate an authorized reseller in your area, go to:
http://www.autodesk.com/support.

32 |Chapter 4 Documentation and Support

Part II
Autodesk Mechanical
Desktop Tutorials
®

The tutorials in this section teach you how to use Mechanical Desktop 6, and provide a
comprehensive overview of mechanical design. The lessons range from basic to advanced,
and include step-by-step instructions and helpful illustrations.
You learn how to create parts, surfaces, assemblies, table driven parts, and bills of material.
You will also learn how to prepare your designs for final documentation. Specific drawing
files for each lesson are included with the program. These drawing files provide design
elements that help you understand and learn mechanical design concepts.
There are lessons designed for learning to model with Mechanical Desktop, and others
designed specifically for learning to use Mechanical Desktop with the power pack.

Using the Tutorials

In This Chapter

This Introduction presents information that is useful to
know before you start performing the tutorials for

■ Finding the right tutorial
■ Accessing commands
■ Controlling the appearance of

Autodesk® Mechanical Desktop®. It provides a summary
of how the tutorials are structured, and the methods

the Desktop Browser
■ Backing up tutorial files

you can use to issue commands. You learn how to
manipulate the position of the Browser to best suit your
work space.
As you work through the tutorials, you use a set of
drawing files that are included with your software. In
this section, you learn how to locate, back up, and
maintain these drawings.

How the Tutorials are Organized
Read the Key Terms and Basic Concepts sections at the beginning of each
tutorial before you begin the step-by-step instructions. Understanding this
information before you begin will help you learn.
Key Terms

Lists pertinent mechanical design terms and definitions
for the lesson.

Basic Concepts

Gives you an overview of the design concepts you learn in
the lesson.

The tutorials begin with basic concepts and move toward more advanced
design techniques. They are presented in three design categories: part modeling, assembly modeling, and surface modeling.
For best results, run Mechanical Desktop 6 to perform the tutorials in chapters 1 through 16, and Mechanical Desktop 6 with the power pack to perform
chapters 17 through 19.

Chapters 6 Through 15 Part Modeling
These tutorials guide you through the basics of part modeling. Starting with
a basic sketch, you learn how to create fully parametric feature-based models
and generate drawing views.

Chapters 16 Through 18 Assembly Modeling
The assembly modeling tutorials show you how to create, manage, and document complete assemblies and subassemblies, and create exploded views of
your assembly design. You also learn how to use assembly techniques to
build a combined part in the Part Modeling environment.

Chapters 19 Through 21 Surface Modeling
These tutorials cover the techniques of surface modeling. You start by learning how to create and edit different types of surfaces. Then you create a surface and use it to cut material from a parametric part. You also learn how to
surface a wireframe model from the ground up.

Chapters 22 Through 24 2D and 3D Parts and Calculations
These tutorials focus on features in the Mechanical Desktop 6 with the power
pack. Included are tutorials working with standard parts and the shaft
generator and 3D finite element analysis (FEA) features. The exercises in
these tutorial chapters are designed to help you understand and use the
power pack features to simplify your work.

Chapter 5

Using the Tutorials

Accessing Mechanical Desktop Commands
Mechanical Desktop provides several methods to access commands and
manage your design process.
The following are samples of the access methods available to you:
Browser

Right-click the window background and choose New Part.

Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

Toolbutton

New Part

Desktop Menu

Part ➤ Part ➤ New Part

Command

AMNEW

The step-by-step procedures in the tutorials indicate the command name in
the opening procedural text. The appropriate toolbutton is displayed in the
margin next to the preferred access method. In the tutorials, the context
menu method is used when the menus are sensitive to what you are doing.
The Browser method is used when you can save time and steps. You can use
any of the alternate methods as well.
If you are in Model mode, you can toggle between the Part and Assembly
context menus. If you are in Scene mode, the Scene menu is available. When
you are working in Drawing mode, you can toggle between the Drawing and
Annotate context menus.
Here is an example of how methods are used in the tutorials:
3 Use AMNEW to create a new part.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

NOTE To find the location of a particular toolbutton, refer to Appendix A.

Accessing Mechanical Desktop Commands

Positioning the Desktop Browser
The Desktop Browser is a graphical interface that is useful in both creating
and modifying your designs. You can do much of your work in the Browser
as you proceed through the lessons in the tutorials.
By default, the Browser is located on the left side of your screen. You may
want to move, resize, or hide the Browser to suit your working conditions.
This section provides instructions to control the size, shape, and location of
the Browser, and to return it quickly to the default location.
The Browser behaves differently when it is in the Auto Hide state. The following are procedures for positioning the Browser both in and out of the Auto
Hide state.

To minimize and expand the Desktop Browser
To minimize the Browser double-click the gray area above the tabs.

To expand the Browser, double-click the gray area again.
To minimize the Browser in the Auto Hide state, right-click the gray area and
choose Auto Hide ➤ Collapse.
After you minimize the Browser in Auto Hide, you control the expand and
collapse function by moving your cursor onto and off of the Browser.
To turn off Auto Hide, right-click the gray area and choose Auto Hide ➤ Off.
With Auto Hide off, the Browser remains expanded when you move your cursor away from it.

To move the Browser out of the default position
To move the Browser to another location on the screen, right-click the title
bar and choose Move. Click the title bar and drag the Browser to a location
on your screen.

To return the Browser to the default position
To return the Browser to the default position, double-click the title bar. The
Browser is docked in the default position along the left side of the graphics
screen.
To return to the previous location, right-click the gray area and turn off Allow
Docking.

Chapter 5

Using the Tutorials

To hide and unhide the Browser
To hide the Browser, right-click the gray area above the tabs and choose Hide.
To unhide the Browser, choose View ➤ Display ➤ Desktop Browser.
To move the Browser off the screen with Auto Hide, right-click the gray bar
above the tabs and choose Auto Hide ➤ Left (or Right).
After you move the Browser off the left or right side of the screen with Auto
Hide, if you move your mouse to the corresponding edge of the screen, the
Browser is displayed along that edge. Move your mouse off the Browser, and
the Browser returns to the location off the screen.
To turn off Auto Hide, right-click the gray area and choose Auto Hide ➤ Off.
The Browser remains positioned on the screen when you move your cursor
away from it.
To move the Browser directly from Auto Hide to another location on your
screen, choose Auto Hide ➤ Allow Docking. Click the title bar and drag the
Browser to a new location. The Browser is docked in the new location.

To resize the Browser
Right-click the title bar and choose Size. Then drag a corner to resize the
Browser.

To return the Browser to its previous size, double-click the title bar.

Positioning the Desktop Browser

Backing up Tutorial Drawing Files
For each tutorial, you use one or more of the master drawing files that contain the settings, example geometry, or parts for the lesson. These files are
included with Mechanical Desktop. Before you begin the tutorials, back up
these drawing files so you always have the originals available. Any mistakes
you make while you are learning will not affect the master files.
To back up tutorial drawing files
1 From the Windows Start menu, choose Programs ➤ Windows Explorer.
2 In the folder where Mechanical Desktop is installed (by default this is Program
Files\Mdt\desktop), choose File ➤ New ➤ Folder.

3 Create a new folder called tutorial backup.
4 Open the desktop\tutorial folder that contains all the tutorial drawing files
and copy them into your new folder.
Now you can use the tutorial drawings in the desktop\tutorial folder as you
work through the tutorials in this book.

NOTE Keep your working tutorial files in the desktop\tutorial folder so that
external references in the assembly tutorials can update correctly.

Chapter 5

Using the Tutorials

Creating Parametric
Sketches

In This Chapter

Autodesk® Mechanical Desktop® automates your design

■ Analyzing a design and creating a

strategy for sketching
and revision process using parametric geometry.
Parametric geometry controls relationships among
design elements and automatically updates models and

■ Text sketch profiles
■ Open profile sketches
■ Closed profile sketches
■ Path sketches

drawings as they are refined.
The sketch is the basic design element that defines the

■ Cut line sketches
■ Split line sketches
■ Break line sketches

approximate size and shape of features in your part. As
the name implies, a sketch is a loose approximation of
the shape that will become a feature. After a sketch is
solved, you apply parametric constraints to control its
shape.
After you learn to create sketches, move on to chapter 2
to learn how to add constraints to sketches.

Key Terms
Term

Definition

2D constraint

Defines how a sketch can change shape or size. Geometric constraints control the
shape and relationships among sketch lines and arcs. Dimensional constraints
control the size of sketch geometry.

closed loop

A polyline entity, or group of lines and arcs that form a closed shape. Closed loops
are used to create profile sketches.

closed profile

A constrained sketch that is a cross section or boundary of a shape, such as an
extrusion, a revolved feature, or a swept feature.

construction geometry

Any line or arc created with a noncontinuous linetype. Using construction
geometry in paths and profiles may mean fewer constraints and dimensions are
needed to control size and shape of symmetrical or geometrically consistent
sketches.

cut line

Used to specify the path of a cross-section drawing view. Unlike a profile sketch,
the cut line sketch is not a closed loop. There are two types of cut line sketches—
offset and aligned.

feature

An element of a parametric part model. You can create extruded features,
revolved features, loft features, and swept features using profiles and paths. You
can also create placed features like holes, chamfers, and fillets. You combine
features to create complete parametric part models.

nested loop

A closed loop that lies within the boundary of another closed loop. Nested loops
are used to create more complex profile sketches.

open profile

A profile created from one or more line segments sketched to form an open
shape. Open profiles are used in bend, rib, and thin wall features.

path sketch

A constrained sketch that is a trajectory for a swept feature.

sketch

A planar collection of points, lines, arcs, and polylines used to form a profile, path,
split line, break line, or cutting line. An unconstrained sketch contains geometry
and occasionally dimensions. A constrained sketch, such as a profile, path, split
line, cut line, or break line that contains “real” and construction geometry, and is
controlled by dimensions and geometric constraints.

sketch tolerance

Tolerance setting that closes gaps smaller than the pickbox and snaps lines to
horizontal, vertical, parallel, or perpendicular.

split line

A sketch, either open or closed, used to split a part into two distinct parts. Also
known as a parting line.

text sketch profile

A profile created from a single line of text in a selected font and style. Text-based
profiles are used to emboss parts with text.

Chapter 6

Creating Parametric Sketches

Basic Concepts of Parametric Sketching
You create, constrain, and edit sketches to define a
■
■
■
■
■
■

Profile that governs the shape of your part or feature
Location for a bend feature in a part design
Path for your profile to follow
Cut line to define section views
Split line to split a face or part
Break line to define breakout section views

After you create a rough sketch with lines, polylines, arcs, circles, and ellipses
to represent a feature, you solve the sketch. Solving a sketch creates a parametric profile, path, cut line, split line, or break line from your sketched
geometry.
When you solve a sketch, Mechanical Desktop converts it to a parametric
sketch by applying two-dimensional constraints to it, according to internal
rules. This reduces the number of dimensions and constraints you need to
fully constrain it. In general, a sketch should be fully constrained before it is
used to create a feature.
You can control the shape and size of the parametric sketch throughout multiple design revisions.
In this tutorial, you learn to create and solve sketches. Chapter 7, “Constraining Sketches,” introduces you to creating, modifying, and deleting the constraints and parametric dimensions that control a sketch.

Basic Concepts of Parametric Sketching

Sketching Tips
Some of these tips do not apply to this chapter, but you will see their usefulness when you use sketches to create complex parts.

Tip

Explanation

Keep sketches simple

It is easier to work with a single object than a multiple-object
sketch. Combine simple sketches for complex shapes.

Repeat simple shapes

If a design has repeating elements, sketch one and then copy or
array as needed.

Define a sketching
layer

Specify a separate layer and color for sketching. Your sketch is
visible with other part geometry but easy to identify when you
need to modify it.

Preset sketch
tolerances

Define characteristics, such as sketch precision and angular
tolerance of sketch lines, if the default values are not sufficient.

Draw sketches to size

When your sketches are roughly correct in size and shape, your
design is less likely to become distorted as dimensions or
constraints are added. Sketch a rectangle to serve as a boundary
for the base feature to set relative size. Sketch the feature, but
delete the rectangle before you create a profile.

Use PLINE

Whenever possible, use the PLINE command to create your
sketches. With PLINE, you can easily draw tangent lines and arcs.

Chapter 6

Creating Parametric Sketches

Creating Profile Sketches
In Mechanical Desktop, there are three types of profile sketches:
■
■
■

Text-based profiles, used to create parametric 3D text-based shapes
Open profile sketches, used to define features on parts
Closed profile sketches, used to outline parts and features

You can solve and apply parametric constraints and dimensions to all three
of these profile sketch types.

Creating Text Sketch Profiles
A text sketch profile is a line of text displayed in a rectangular boundary. You
extrude a text sketch profile to create the emboss feature on part models.
To create a text sketch profile, you use the command AMTEXTSK. A dialog box
opens where you can enter text and choose a font style and size, or you can
enter the information on the command line.
You define an anchor point for the rectangle on your part and a point to
define the height of the text. You have the option to define a rotation value
on the command line to position the text at an angle. As you move your cursor to define the anchor and height points, the rectangular boundary scales
appropriately to accommodate the size of the text.
You can change the size of the text by changing the value of the height
dimension. You can apply typical parametric dimensions and constraints
between the rectangular boundary and other part edges or features.
When the text sketch profile is sized correctly and in the right position on
your part, you extrude it to create the emboss feature.

text sketch

text sketch with rotation defined

To learn more about using text sketch profiles in the emboss feature, see
“Creating Emboss Features” on page 140.

Creating Profile Sketches

Creating Open Profile Sketches
You can create an open profile from single or multiple line segments, and
solve it in the same way as you solve a closed profile.
An open profile constructed with one line segment is used to define the location of a bend feature on a flat or cylindrical part model. To bend an entire
part, you sketch the open profile over the entire part. If you sketch the open
profile over a portion of a part, only that portion of the part bends.
Open profiles constructed with one or multiple line segments are extruded
to form rib features and thin features. For a rib feature, the open profile
defines the outline of the rib, and is sketched from the side view. For a thin
feature, the open profile defines the shape of a wall and is extruded normal
to the work plane.

profile for bend feature

profile for rib feature

profile for thin feature

To learn more about open profiles in features, see “Creating Bend Features”
on page 163, “Creating Rib Features” on page 133, and “Creating Thin Features” on page 136.

Creating Closed Profile Sketches
A profile sketch is a two-dimensional outline of a feature. Closed profile
sketches are continuous shapes, called loops, that you construct from lines,
arcs, and polylines. You use closed profile sketches to create features with custom shapes (unlike standard mechanical features such as holes, chamfers,
and fillets).
Profile sketches can be created from a set of objects, or a single polyline, that
defines one or more closed loops. You can use more than one closed loop to
create a profile sketch if the loops are nested within each other.
You cannot create profile sketches with loops that are
■
■
■
■

Chapter 6

Self-intersecting
Intersecting
Tangential
Nested more than one level deep

Creating Parametric Sketches

In this section, you create three profile sketches.

Open the file sketch1.dwg in the desktop\tutorial folder. This drawing file is
blank but it contains the settings you need to create these profiles.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Using Default Sketch Rules
Mechanical Desktop analyzes individual geometric elements, and operates
on a set of assumptions about how they should be oriented and joined.

rough sketch

profile sketch

Before you begin, look at the Desktop Browser. It contains an icon with the
drawing file name. There are no other icons in the Browser, which indicates
that your file contains no parts.
You can move the Browser on your desktop and resize it to give yourself more
drawing area. See “Positioning the Desktop Browser” on page 38.

Creating Profile Sketches

To create a profile sketch from multiple objects
1 Use LINE to draw this shape, entering the points in the order shown.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Line.

Specify first point: Specify a point (1)
Specify next point or [Undo]: Specify a second point (2)
Specify next point or [Undo]: Specify a third point (3)
Specify next point or [Close/Undo]: Specify a fourth point (4)
Specify next point or [Close/Undo]: Specify a fifth point (5)
Specify next point or [Close/Undo]: Specify a sixth point (6)
Specify next point or [Close/Undo]: Specify a seventh point (7)
Specify next point or [Close/Undo]: Specify an eighth point (8)
Specify next point or [Close/Undo]: Press ENTER
1

8
4

You do not need to make the lines absolutely vertical or horizontal. The
objective is to approximate the size and shape of the illustration.
2 Using ARC, sketch the top of the shape, following the prompts on the
command line.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Arc.

Specify start point of arc or [CEnter]: Specify the start point (9)
Specify second point of arc or [CEnter/ENd]: Specify the second point (10)
Specify end point of arc: Specify the endpoint (11)
10
11

You do not need to use OSNAP to connect the arc to the endpoints of the
lines.

Chapter 6

Creating Parametric Sketches

Your sketch should look like this.

3 Create a profile sketch from the rough sketch, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Profile.

Select objects for sketch: Select the arc and the lines
Select objects for sketch: Press ENTER

As soon as the sketch is profiled, a part is created. The Browser contains a new
icon labelled PART1_1. A profile icon is nested under the part icon.

According to internal sketching rules, Mechanical Desktop determines
whether to interpret the sketch geometry as rough or precise and whether to
apply constraints.
By default, Mechanical Desktop interprets the sketch as rough and applies
constraints, redrawing the sketch. You can customize these default settings
with Mechanical Options.

Creating Profile Sketches

When redrawing, Mechanical Desktop uses assumed constraints in the
sketch. For example, lines that are nearly vertical are redrawn as vertical, and
lines that are nearly horizontal are redrawn as horizontal.
After the sketch is redrawn, a message on the command line tells you that
Mechanical Desktop needs additional information:
Solved under constrained sketch requiring 5 dimensions or constraints.
Depending on how you drew your sketch, the number of dimensions
required to fully constrain your sketch may differ from that in this exercise.
This message tells you that the sketch is not fully defined. When you add the
missing dimensions or constraints, you determine how the sketch can
change throughout design modifications. Before you add the final constraints, you need to show the assumed constraints.
4 Use AMSHOWCON to show the existing constraints, following the prompt.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] :

Enter a

The constraint symbols are displayed.

NOTE The numbers in your sketch might differ, depending on the order in
which you created the geometric elements.
The sketch has eight geometric elements, seven lines and an arc, each identified by a number in a circle. Four lines have a V symbol (vertical) and three
lines have an H symbol (horizontal). Two of the horizontal lines have constraints denoted by symbols that begin with the letter C (collinear), and three
of the elements have constraints denoted by symbols that begin with the
letter T (tangent).

Chapter 6

Creating Parametric Sketches

If your sketch does not contain the same constraints, redraw it to more
closely resemble the illustrations in steps 1 and 2.
Notice the letter F, located at the start point of line 0. It indicates that a fix
constraint has been applied to that point. When Mechanical Desktop solves
a sketch, it applies a fix constraint to the start point of the first segment of
your sketch. This point serves as an anchor for the sketch as you make
changes. It remains fixed in space, while other points and geometry move
relative to it.
You may delete this constraint if you wish, and apply one or more fix constraints to the endpoints of sketch segments, or to the segments themselves,
in order to make your sketch more rigid.
5 To hide the constraints, respond to the prompt as follows:
Enter an option [All/Select/Next/eXit] : Press ENTER
Save your file.
You have successfully created a profile sketch. In chapter 7, “Constraining
Sketches,” you learn to create, modify, and delete constraints and parametric
dimensions.

Using Custom Sketch Rules
Custom settings affect how Mechanical Desktop analyzes rough sketches. In
this exercise, you sketch with PLINE and convert your drawing to a profile
sketch. You will modify one of the Mechanical Options sketch rule settings
and see its effect on the sketch.

rough sketch

profile sketch

Before you begin the next exercise, create a new part definition.

Creating Profile Sketches

To create a new part definition
1 Use the context menu to initiate a new part definition.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

2 Respond to the prompts as follows:
Select an object or enter new part name : Press ENTER

NOTE The command method you use determines which prompts appear.
A new part definition is created in the drawing and displayed in the Browser.
The new part automatically becomes the active part.

3 Pan the drawing so you have room to create the next sketch.
Context Menu

In the graphics area, right-click and choose Pan.

You are ready for the next exercise.
To create a profile sketch from a single polyline
1 Use PLINE to draw this rough sketch as a continuous shape, following the
prompts for the first four points.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

Specify start point: Specify a point (1)
Current line-width is 0.0000
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a second point (2)
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a third point (3)
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a fourth point (4)

Chapter 6

Creating Parametric Sketches

5
1

2 Following the prompts, switch to Arc to create the arc segment, then switch
back to Line. Switch to Close to finish the sketch.
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]: Enter a
Specify endpoint of arc or
[Angle/CEnter/CLose/Direction/Halfwidth/Line/Radius/Second pt/Undo/Width]:
Specify a fifth point (5)
Specify endpoint of arc or
[Angle/CEnter/CLose/Direction/Halfwidth/Line/Radius/Second pt/Undo/Width]:
Enter l
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a sixth point (6)
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]: Enter c
3 Use AMPROFILE to create a profile sketch from the rough sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

NOTE If you used line segments and an arc to draw your sketch you cannot
use Single Profile. This command profiles single object sketches only. For
sketches containing more than one object, use Profile.
When you use Single Profile, you are not prompted to select the sketch geometry. Mechanical Desktop looks for the last entity you created. If it is a valid
closed loop, Mechanical Desktop analyzes the sketch, redraws it, and displays
the following message:
Solved under constrained sketch requiring 5 dimensions or constraints.

Creating Profile Sketches

All lines were redrawn as horizontal or vertical except one. L1 remains angled
because the angle of the line exceeds the setting for angular tolerance. By
default, this rule makes a line horizontal or vertical if the angle is within 4
degrees of horizontal or vertical.

You can modify this and other sketch tolerance settings to adjust the precision of your sketch analysis.
4 Change the angular tolerance setting.
Browser

Click the Options button below the window.

5 In the Mechanical Options dialog box, choose the Part tab and change the
angular tolerance from 4 degrees to 10 degrees, the maximum value.

Choose OK.

Chapter 6

Creating Parametric Sketches

6 Reprofile the sketch, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Profile.

NOTE You cannot use Single Profile to reprofile a sketch.
Select objects for sketch: Use a crossing window to specify the sketch
Select objects for sketch: Press ENTER

If your sketch shows line L1 unchanged, the angle was greater than 10
degrees. You need to edit or redraw the shape and append the sketch.

NOTE When adding geometry or changing a sketch, you must append the
new geometry so that the sketch is reanalyzed and constraints are reapplied. See
chapter 7, “Constraining Sketches,” to append geometry to a sketch.
When L1 was made vertical, it required one less dimension or constraint to
fully solve the sketch. The following message is displayed on the command
line.
Solved underconstrained sketch requiring 4 dimensions or constraints.
Save your file.
You can adjust sketch rules that determine how precisely you need to draw.
For most sketching, you should use the default settings. However, you can
change the default settings as needed.

Creating Profile Sketches

Using Nested Loops
You can select more than one closed loop to create a profile sketch. A closed
loop must encompass the nested loops. They cannot overlap, intersect, or
touch. With nested loops you can easily create complex profile sketches.
To create a profile sketch using nested loops
1 Use AMNEW to create a new part definition.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

2 Accept the default part name on the command line.
The Browser now contains a third part.

3 Pan the drawing so you have room to create the next sketch.
Context Menu

In the graphics area, right-click and choose Pan.

4 Create the following sketch using lines or polylines, and circles. Then, in the
graphics area, right-click and choose 2D Sketching ➤ Trim and follow the
prompts on the command line to remove the section from the smaller circle.

Chapter 6

Creating Parametric Sketches

5 Profile the sketch, following the prompts to select the objects with a crossing
window.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Profile.

Select objects for sketch: Specify a point to the right of the sketch (1)
Specify opposite corner: Specify a second point (2)
5 found
Select objects for sketch: Press ENTER
1

Mechanical Desktop calculates the number of dimensions or constraints
required to fully constrain the profile.
Solved underconstrained sketch requiring 7 dimensions or constraints.

NOTE You may need more dimensions or constraints, depending on how you
created your sketch.
Save your file.
This simple cam illustrates how you can easily create complex shapes to
define parts and features. Experiment on your own to create profiles from
nested loops.

Creating Profile Sketches

Creating Path Sketches
Path sketches can be both two dimensional and three dimensional. Like
open profile sketches, they can be open shapes. In this exercise, you create
only the path sketches, but not the profiles that would sweep along the
paths.

Creating 2D Path Sketches
A 2D path sketch serves as a trajectory for a swept feature. You create a swept
feature by defining a path and then a profile sketch of a cross section. Then,
you sweep the profile along the path.

path sketch

profile sketch

swept feature

The geometry for the 2D path must be created on the same plane.
Valid geometry that can be used to create a 2D path includes
■
■
■
■
■

Lines
Arcs
Polylines
Ellipse segments
2D splines

When you solve a 2D path sketch, you can automatically create a work plane
normal to the start point of the path. You use this work plane to create a profile sketch for the swept feature, and then constrain the profile sketch to the
start point of the path.

Chapter 6

Creating Parametric Sketches

To create a 2D path sketch
1 Create a new part definition.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

2 Press ENTER on the command line to accept the default part name.
3 Pan the drawing so you have room to create the next sketch.
Context Menu

In the graphics area, right-click and choose Pan.

4 Use PLINE to draw the rough sketch as a continuous shape, responding to the
prompts to specify the points in the following illustration.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

Specify start point: Specify a point (1)
Current line-width is 0.0000
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a second point (2)
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Enter a to create an arc segment
Specify endpoint of arc or
[Angle/CEnter/CLose/Direction/Halfwidth/Line/Radius/Second pt/Undo/Width]:
Specify a third point (3)
Specify endpoint of arc or
[Angle/CEnter/CLose/Direction/Halfwidth/Line/Radius/Second pt/Undo/Width]:
Enter l to create a line segment
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]:
Specify a fourth point (4)
Specify next point or [Arc/Close/Halfwidth/Length/Undo/Width]: Press ENTER

Make sure to switch between drawing lines and arcs at points (2) and (3).

Creating Path Sketches

5 Use AM2DPATH to convert the rough sketch to a path sketch, following the
prompts.
Context Menu
Select objects:
Select objects:

In the graphics area, right-click and choose Sketch Solving
➤ 2D Path.
Specify the polyline shape
Press ENTER

At the prompt for the start point of the path, you select the point where the
path begins. This determines the direction to sweep the profile of the cross
section.
Select start point of the path: Specify the start point (1)

You can also specify whether a work plane is created perpendicular to the
path. In this example, a work plane is not required.
Create a profile plane perpendicular to the path? [Yes/No] : Enter n

NOTE If you choose to create a sketch to sweep along the path, Mechanical
Desktop can automatically place a work plane perpendicular to the path.
Press the F2 function key to activate the AutoCAD Text window. Examine the
prompts for the AM2DPATH command. The following line is displayed:
Solved underconstrained sketch requiring 3 dimensions or constraints.
The sketch analysis rules indicate that the path sketch needs three more
dimensions or constraints to fully define the sketch.

Chapter 6

Creating Parametric Sketches

A work point is automatically placed at the start point of the path. The
Browser displays both a 2DPath icon and a work point icon nested below the
part definition.

6 Use AMSHOWCON to display the existing constraints, responding to the
prompt.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] : Enter a

The start point of the path is fixed. Both lines are vertical and are tangent to
the endpoints of the arc. The missing information is the length of each line and
the radius of the arc. Given these values, the sketch would be fully constrained.
Enter an option [All/Select/Next/eXit] : Press ENTER
Save your file.
Next, you create a three-dimensional path.

Creating Path Sketches

Creating 3D Path Sketches
3D path sketches are used to create
■
■
■
■

A 3D path from existing part edges
A helical path
The centerline of a 3D pipe
A 3D spline path

3D paths are used to create swept features that are not limited to one plane.
See chapter 8, “Creating Sketched Features,” to learn more about sweeping
features along a 3D path.
Open the file sketch2.dwg in the desktop\tutorial folder. The drawing contains
four part definitions and the geometry you need to create the 3D paths.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Creating a 3D Edge Path
A 3D edge path is used to create a path from existing part edges. After you
create the path, you can sweep a profile and use a Boolean operation to combine the feature with the existing part.

3D edge path and profile sketch

Chapter 6

Creating Parametric Sketches

3D sweep along edge path

Before you can work on a part, it must be active. Activate PART1_1, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Part ➤
Activate Part.

Select part to activate or [?] : Enter PART1_1
PART1_1 is activated, and highlighted in the Browser.
Use Pan to center PART1_1 on your screen.
Context Menu

In the graphics area, right-click and choose Pan.

PART1_1 contains an extruded part.

To create a 3D edge path
1 Use AM3DPATH to define the 3D edge path, following the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ 3D Edge Path.

Select model edges (to add): Specify the first part edge (1)
Select model edges (to add): Specify the next edges in a clockwise sequence
Select model edges (to add): Specify the last edge (9)
Select model edges (to add): Press ENTER
Specify start point: Specify start point (1)
Create workplane? [Yes/No] : Press ENTER
The command method you use determines the prompts that are displayed.

Creating Path Sketches

2 Continue on the command line to place the work plane.
Plane=Parametric
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER
The path is created, and a work point is located at the start point. A work
plane is placed normal to the start of the path so you can sketch the profile
for the sweep feature.

In the Browser, the new geometry is nested below the extrusion and fillets in
PART1_1.

Save your file.

Chapter 6

Creating Parametric Sketches

Creating a 3D Helical Path
A 3D helical path is used for a special type of swept feature. Helical sweeps
are used to create threads, springs, and coils. You create a 3D helical path
from an existing work axis, cylindrical face, or cylindrical edge.

3D path

profile sketch

3D helical sweep

When you create a 3D helical path, you can specify whether a work plane is
also created. The work plane can be normal to the path, at the center of the
path, or along the work axis. You use this work plane to draw the profile
sketch for the helical sweep.
Before you begin, activate PART2_1, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Part ➤
Activate Part.

Select part to activate or [?] : Enter PART2_1
PART2_1 is highlighted in the Browser and on your screen.
Use Pan to center PART2_1 on your screen.
Context Menu

In the graphics area, right-click and choose Pan.

PART2_1 contains a cylinder and a work axis.

work axis

Creating Path Sketches

To create a 3D helical path
3 Use AM3DPATH to define the 3D helical path, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ 3D Helix Path.

Enter path type [Helical/Spline/Edge/Pipe] : Enter h
Select work axis, circular edge, or circular face for helical center:
Select the work axis (1)
The command method you use determines the prompts that are displayed.

4 In the Helix dialog box, specify the following:
Type: Revolution and Height
Revolutions: Enter 8
Height: Enter 2
Diameter: Enter .5
Orientation: Counter-Clockwise

Choose OK.

NOTE The path is automatically constrained with the parameters defined in
the Helix dialog box. You can edit the path at any time with AMEDITFEAT.

Chapter 6

Creating Parametric Sketches

The 3D helix path is created. A work point is placed at the beginning of the path.

You can also specify that a work plane is placed normal to the start point of
the 3D path, at the center of the path, or along the work axis. This option
makes it easier for you to create the sketch geometry for the profile you sweep
along the path.
Save your file.

Creating a 3D Pipe Path
A 3D pipe path is used to sweep a feature along a three-dimensional path
containing line and arc segments or filleted polylines. You can modify each
of the control points and the angle of the segments in the 3D Pipe Path
dialog box.

3D pipe path and profile sketch

3D sweep along pipe path

Before you begin, activate PART3_1. This time use the Browser method to
activate the part.
Browser

In the graphics area, double-click PART3_1.

PART3_1 is activated, and highlighted in the Browser.

Creating Path Sketches

Use Pan to center PART3_1 on your screen.
PART3_1 contains an unsolved sketch of line segments and arcs.

To create a 3D pipe path
1 Use AM3DPATH to define the 3D pipe path, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ 3D Pipe Path.

Select polyline path source: Select the first line (1)
Select polyline path source: Select the remaining arcs and lines in sequence
Select polyline path source: Press ENTER
Specify start point: Specify a point near the start of the first line (1)
The command method you use determines the prompts that are displayed.

Chapter 6

Creating Parametric Sketches

2 In the 3D Pipe Path dialog box, examine the vertices and angles of the path.
Verify that Create Work Plane is selected.

NOTE Your numbers might not match the illustration above.
Choose OK to exit the dialog box.
3 Place the work plane, following the prompts.
Plane=Parametric
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER
The Desktop Browser now contains a 3D Pipe icon, a work plane, and a work
point nested below the PART3_1 definition.

Save your file.

Creating Path Sketches

Creating a 3D Spline Path
In this type of path, you sweep a feature along a 3D spline created with fit
points or control points. Working in one integrated dialog box, you can modify any fit point or control point in a 3D spline path, and you can convert fit
points to control points, and control points to fit points.
In this exercise, you work with a fit point spline.

3D spline path and profile sketch

3D sweep along spline path

Before you begin, activate PART4_1 from the Browser.
Browser

In the graphics area, double-click PART4_1.

PART4_1 is highlighted in the Browser and on your screen.
Use Pan to center PART4_1 on your screen.
PART4_1 contains an unsolved spline sketch.

To create a 3D spline path
1 Use AM3DPATH to define the 3D spline path, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ 3D Spline Path.

Select 3D spline path source: Specify the spline
Specify start point: Specify the start point
The command method you use determines the prompts that are displayed.

Chapter 6

Creating Parametric Sketches

2 In the 3D Spline Path dialog box, examine the vertices of the spline, and verify that Create Work Plane is selected.

NOTE Your numbers might not match the illustration above.
Choose OK to exit the dialog box.
3 Create the work plane, responding to the prompts.
Plane=Parametric
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER
The path is created, and a work point is located at the start point. A work
plane is placed normal to the start of the path so you can begin to sketch the
profile for the sweep feature.

Save your file.
Creating a path sketch is similar to creating a profile sketch. The difference
between the two sketch types is their purpose.
■
■

Profile sketches provide a general way to create a variety of features.
Path sketches are used exclusively for creating trajectory paths for 2D and
3D swept features.

Creating Path Sketches

Creating Cut Line Sketches
When you create drawing views, you might want to depict a cut path across
a part for offset, cross-section views. After you have extruded or revolved a
profile sketch to create a feature, you can return to an original sketch and
draw the cut line across the features you want to include in the cross section.
There are two types of cut line sketches: offset and aligned. An offset cut line
sketch is a two-dimensional line constructed from orthogonal segments. An
aligned cut line sketch is a two-dimensional line constructed from nonorthogonal segments.

offset cut line

section view

aligned cut line

section view

Two general rules govern cut line sketches:
■
■

Only line and polyline segments are allowed.
The start and end points of the cut line must be outside the part.

These additional rules apply to cut line sketches:
■
■
■
■

Chapter 6

The first and last line segments of an offset cut line must be parallel.
Offset cut line segments can change direction in 90-degree increments
only.
Only two line segments are allowed in an aligned cut line.
Line segments of aligned cut lines can change direction at any angle.

Creating Parametric Sketches

In the following exercise, after you create a cut line sketch on these models,
the resulting cross-section drawing views can be generated in Drawing mode.
A cut line sketch is needed when you want to define a custom cross-section
view only, but not for a half or full cross-section view.
Open the file sketch3.dwg in the desktop\tutorial folder. The drawing contains
two parts.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
Before you begin, click the plus signs in front of SKETCH3 and PART1_1 to
expand the Browser hierarchy.

Creating Cut Line Sketches

To create an offset cut line sketch
1 Use PLINE to sketch through the center of the holes on the square part.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

Next, analyze the cut line sketch according to internal sketching rules.
2 Use AMCUTLINE to solve the cut line, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Cut Line.

Select objects to define the section cutting line: Select the polyline (1)
Select objects to define the section cutting line: Press ENTER
1

A new icon called CutLine1 is added to the PART1_1 hierarchy in the
Browser.

Save your file.

Chapter 6

Creating Parametric Sketches

As with the other sketches you created, a message tells you how many dimensions and constraints are needed to fully solve the sketch. In this case, you
need five dimensions or constraints to complete the definition of the sketch:
three to define the shape of the sketch, and two to constrain it to the part.
When you create a cross-section drawing view, this sketch defines the path
of the cut plane. If you change the size of the part or holes, or their placement, the cut line is updated to reflect the new values.
For the next exercise, you use the circular part. In the Browser, click the
minus sign in from of PART1_1 to collapse the part hierarchy. Then click the
plus sign in front of PART2_1 to expand the circular part hierarchy.

Before you begin, you need to activate the circular part.
Browser

Double-click PART2_1.

PART2_1 is activated, and highlighted in the Browser and on your screen.

NOTE Before you can work on a part, it must be active.

Creating Cut Line Sketches

To create an aligned cut line sketch
1 Use PLINE to sketch through the centers of two of the holes on the circular
part.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

2 Define a cut line on your sketch, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Cut Line.

Select objects to define the section cutting line: Select the polyline (2)
Select objects to define the section cutting line: Press ENTER
2

A message states that you need five dimensions or constraints to fully solve
this sketch.
3 In the Browser, the new CutLine1 icon is part of the PART2_1 hierarchy.

Save your file.

Chapter 6

Creating Parametric Sketches

Creating Split Line Sketches
A molded part or casting usually requires two or more shapes to define the
part. To make a mold or a cast, you create the shape of your part and then
apply a split line to split the part into two or more pieces. You may also need
to apply a small draft angle to the faces of your part so that your part can be
easily removed from the mold.
Split lines can be as simple as a planar intersection with your part, or as complex as a 3D polyline, or spline, along planar or curved faces.
You can also split parts using either
■
■

A selected planar face or a work plane
A sketch projected onto a selected set of faces

In this exercise, you create a split line to split a shelled part into two separate
parts.

shelled part

split part

Open the file sketch4.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
The drawing file contains a simple shelled box. Two viewports have been
defined: the right side of the part, and an isometric view. You’ll define a new
sketch plane in the right viewport and sketch a split line in the left viewport.

Creating Split Line Sketches

To create a split line
1 Expand the Browser hierarchy of SKETCH4 and PART1_1.

The part consists of an extrusion, three fillets, and a shell feature. Next, you
create a sketch plane on the outside right face of the part.
2 In the right viewport, define a new sketch plane, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Sketch
Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Specify the outside right face of the part (1)
Enter an option [Accept/Next] : Press ENTER
Plane = Parametric
Select edge to align X axis [Flip/Rotate/Origin] : Press ENTER

Next, create a sketch and convert it to a split line.

Chapter 6

Creating Parametric Sketches

3 In the left viewport, use PLINE to sketch the split line.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

4 Use AMSPLITLINE to create a split line from your sketch, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Split Line.

Select objects for sketch: Select the polyline
Select objects for sketch: 1 found
Select objects for sketch: Press ENTER
Select edge to include in split line or press to accept: Press ENTER
Mechanical Desktop solves the sketch and displays the number of constraints
required to fully constrain it.
Solved underconstrained sketch requiring 5 dimensions or constraints.
5 Look at the Browser. SplitLine1 is now nested under the part definition.

Save your file.

Creating Split Line Sketches

Creating Break Line Sketches
When you want to document complex assemblies, it is not always easy to display parts and subassemblies that are hidden by other parts in your drawing
views. By creating a break line sketch, you can specify what part of your
model will be cut away in a breakout drawing view so that you can illustrate
the parts behind it.

break line path

breakout drawing view

Open the file sketch4a.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
The drawing file contains a simple part. An unsolved sketch lies on a work
plane. You create a break line from this sketch.

Chapter 6

Creating Parametric Sketches

To create a break line
1 Use AMBREAKLINE to define the break line sketch, following the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Break Line.

Select objects for sketch: Specify the sketch (1)
Select objects for sketch: Press ENTER

The break line is created. The Browser contains a break line icon nested below
the work plane.

Save your file.
Now that you have learned the basics of creating sketches, you are ready to
constrain them by adding geometric and parametric dimension constraints.

Creating Break Line Sketches

Constraining Sketches

In This Chapter

When you solve a sketch in Autodesk® Mechanical

■ Creating a strategy for

constraining and dimensioning
Desktop®, geometric constraints are applied in
accordance with internal rules. To fully constrain the
sketch, you apply the remaining parametric dimensions
and geometric constraints that are necessary to meet
your design goals.

■ Defining sketch shape and size

with dimensions and geometric
constraints
■ Using construction lines, arcs,

and circles to create and control
sketches
■ Modifying a design
■ Re-creating a constrained sketch

Any time you modify a sketch, the parametric geometry
retains the relationships among design elements.
To reduce the number of constraints required to fully
constrain a sketch, you can use construction geometry.
Construction geometry becomes part of the sketch, but
is ignored when the sketch is used to create a feature.
In the next chapter, you learn to add sketched features
to your constrained sketches.

Key Terms
Term

Definition

2D constraint

Defines how a sketch can change shape or size. Geometric constraints control the
shape and relationships among sketch lines and arcs. Dimensional constraints
control the size of sketch geometry.

degree of freedom

In part modeling, determines how a geometric object such as a line, arc, or circle
can change shape or size. For example, a circle has two degrees of freedom,
center and radius. When these values are known, degrees of freedom are said to
be eliminated.

dimensional constraint

Parametric dimension that controls the size of a sketch. When changed, the
sketch resizes. May be expressed as a constant value, a variable in an equation, a
variable in a table, or in global parameter files.

geometric constraint

Controls the shape and relationships among geometric elements in a sketch.

parametrics

A solution method that uses the values of part parameters to determine the
geometric configuration of the part.

Chapter 7

Constraining Sketches

Basic Concepts of Creating Constraints
A sketch needs geometric and dimensional constraints to define its shape and
size. These constraints reduce the degrees of freedom among the elements of
a sketch and control every aspect of its final shape.
When you solve a sketch, Mechanical Desktop applies some geometric
constraints. In general, use the automatically applied constraints to stabilize
the sketch shape.
Depending upon how accurately you sketch, you may need to add one or
more constraints to fully solve a sketch. You can also add construction
geometry to your sketch to reduce the number of additional constraints
required. After you add further constraints, you might need to delete some
of the applied constraints.
In most cases, you need to fully constrain sketches before you use them to
create the features that define a part. As you gain experience, you will be able
to determine which constraints control the sketch shape according to your
design requirements.

Basic Concepts of Creating Constraints

Constraining Tips
Tip

Explanation

Determine sketch
dependencies

Analyze the design to determine how sketch elements
interrelate; then decide which geometric constraints are
needed.

Analyze automatically
applied constraints

Determine the degrees of freedom not resolved by automatic
constraints. Decide if any automatic constraints need to be
deleted in order to constrain elements as you require.

Use only needed
constraints

Replace constraints as needed to define shape. Because
constraints often solve more than one degree of freedom, use
fewer constraints than degrees of freedom.

Stabilize shape
before size

If you apply geometric constraints before dimensions, your
sketch shape is less likely to become distorted.

Dimension large
before small

To minimize distortion, define larger elements that have an
overall bearing on the sketch size. Dimensioning small elements
first may restrict overall size. Delete or undo a dimension if the
sketch shape is distorted.

Use both geometric
constraints and
dimensions

Some constraint combinations may distort unconstrained
portions of the sketch. If so, delete the last constraint and
consider using a dimension or a different constraint
combination.

Constraining Sketches
Constraining a sketch defines how a sketch can change shape or size. In addition to the inferences by the software, you often need additional dimensions
or constraints.
Constraints may be fixed or variable, but they always prevent unwanted
changes to a feature as you make modifications.

Chapter 7

Constraining Sketches

The ways a sketch can change size or shape are called degrees of freedom. For
example, a circle has two degrees of freedom—the location of its center and
its radius. If the center and radius are defined, the circle is fully constrained
and those values can be maintained.

radius
center

Similarly, an arc has four degrees of freedom—center, radius, and the endpoints of the arc segment.
endpoint
radius
center

endpoint

The degrees of freedom you define correspond to how fully the sketch is constrained. If you define all degrees of freedom, the arc is fully constrained. If you
do not define all degrees of freedom, the sketch is underconstrained.
Mechanical Desktop does not allow you to define a degree of freedom in
more than one way and thus prevents you from overconstraining a sketch.
Before you add constraints, study your sketch, and then decide how to constrain it. Usually, you need both geometric constraints and dimensions. See
“Constraining Tips” on page 86.
You should fully constrain sketches so that they update predictably as you
make changes. As you gain experience, you may want to underconstrain a
sketch while you work out fine points of a design, but doing so may allow
that feature to become distorted as you modify dimensions or constraints.

Constraining Sketches

Applying Geometric Constraints
When constraining a sketch, begin by defining its overall shape before defining
its size. Geometric constraints specify the orientation and relationship of the
geometric elements. For example
■
■

Constraints that specify orientation indicate whether an element is horizontal or vertical.
Constraints that determine relationships specify whether two elements
are perpendicular, parallel, tangent, collinear, concentric, projected,
joined, have the same X or Y coordinate location, or have the same radius.

Mechanical Desktop displays geometric constraints as letter symbols. If the
constraint specifies a relationship between two elements, the letter symbol is
followed by the number of the sketch element to which the constraint is
related. In the example below,
■
■
■

■

Chapter 7

The start point of the arc (0) has a fix constraint. This point is anchored
and will not move when changes are made to the sketch constraints.
The lines (2, 3, 4, and 6) have constraint symbols of either H (horizontal)
or V (vertical).
All lines except one are tangent to at least one of the arcs (0 and 1). Each
symbol T (tangent) is followed by the number of the arc to which it is
tangent.
Each arc is tangent to its connecting lines, as shown by T constraint
symbols, and the arcs have the same radius, as indicated by the R
constraint symbols.

Constraining Sketches

As you apply geometric constraints, you should continue to analyze your
sketch, reviewing and replacing constraints.
In the next exercise, you gain experience with constraining techniques by
analyzing and then modifying geometric constraints to reshape the sketch.
Open the file sketch5.dwg in the desktop\tutorial folder. Use the before-andafter sketches below to determine what changes you must make. Then
change the constraints and see the results of your analysis.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

before geometric constraints

after geometric constraints

In the before-and-after sketches, you can see that the constraints and dimensions differ, but you cannot discern which geometric constraints Mechanical
Desktop has assumed. You will notice that
■
■

The linear dimensions are the same for both sketches.
The angular relationships of the vertical lines differ.

Applying Geometric Constraints

Showing Constraint Symbols
You can change the parametric relationships of the lines by modifying
geometric or dimensional constraints. Because geometric constraints control
the overall shape of the sketch, you cannot safely make any changes until
you know the current geometric constraints. Therefore, the next step is to
show the symbols.
To show constraint symbols
1 Use AMSHOWCON to display constraint symbols, responding to the prompt.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] :

Enter a

Parallel constraints exist between lines 0, 2, 4 and 6. Lines 1, 3, 5, and 7 have
horizontal constraints. Lines 3 and 7 are also collinear and equal in length.
You begin reshaping your sketch by removing the parallel constraints.
To understand the constraints, look at symbol P0 (on line 2). This symbol
indicates that line 2 is parallel to line 0.

Chapter 7

Constraining Sketches

Similarly, the constraint symbols (P2, P4, and P6) show that line 0 is parallel
to lines 2, 4 and 6.

2 Hide the constraint symbols.
Enter an option [All/Select/Next/eXit] :

Press ENTER

Replacing Constraints
After you delete the unwanted constraints, you can add constraints to
reshape the sketch. In this exercise, you delete the parallel constraints that
control the inner and outer angled lines in the sketch and replace them with
vertical constraints.
To replace a constraint
1 Use AMDELCON to replace the constraints, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Delete Constraints.

Select or [Size/All]: Select the parallel constraint symbols (1), (2), and (3)
Select or [Size/All]: Press ENTER

The parallel constraints are deleted. The sketch shape looks the same until
you add constraints or change dimensions.

Applying Geometric Constraints

2 Use AMADDCON to add vertical constraints to the two inner angled lines,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Vertical.

Valid selection(s): line, ellipse or spline segment
Select object to be reoriented: Specify line (3)
Solved under constrained sketch requiring 2 dimensions or constraints.
Valid selection(s): line, ellipse or spline segment
Select object to be reoriented: Specify line (4)
Solved under constrained sketch requiring 1 dimensions or constraints.
Valid selection(s): line, ellipse or spline segment
Select object to be reoriented: Press ENTER
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER

4
3

The vertical constraints are applied, and your sketch should look like this.

You removed the constraints that forced these lines to be parallel to one
another. In order to force the outer lines to be complementary angles to one
another, you need to add an angular dimension to the leftmost line.

Chapter 7

Constraining Sketches

3 Use AMPARDIM to add an angular dimension, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select near the middle of line (1)
Select second object or place dimension: Select near the middle of line (2)
Specify dimension placement: Place the dimension (3)
Enter dimension value or [Undo/Placement point] <75>: Enter 105
Solved fully constrained sketch.
Select first object: Press ENTER

NOTE If you do not select the lines near their midpoints, you may be
prompted to specify the type of dimension to create. Choose Angular.

1
3
2

You have modified the geometric constraint scheme to reshape the sketch.

Save your file.
Next, you learn to use parametric dimensions to constrain the shape of a
sketch.

Applying Geometric Constraints

Applying Dimension Constraints
It is good practice to stabilize the shape of a sketch with geometric constraints
before you specify size with dimensional constraints.
Dimensions specify the length, radius, or rotation angle of geometric elements
in the sketch. Unlike geometric constraints, dimensions are parametric;
changing their values causes the geometry to change.
Dimensions can be shown as numeric constants or as equations. Although
you can use them interchangeably, they each have specific uses.
■
■

Numeric constants are useful when a geometric element has a static size
and is not related to any other geometric element.
Equations are useful when the size of a geometric element is proportional
to the size of another element.

In the following illustration, all of the lines and the angles are constant, and
stated as numeric values.

In the next illustration, the dimensions are expressed as equations.

Chapter 7

Constraining Sketches

In this case, the height of the sketch must maintain the same proportion to
the length, even if you change dimensions later. In an equation, you can
state the height relative to the length. The dimension for the vertical line is
defined as an equation of d1 = d0/.875 where d1 is the parameter name for
the vertical line and d0 is the parameter name for one of the horizontal lines.
The d variables in the equations are parameter names assigned by Mechanical
Desktop when you define the parameters. The letter d indicates that the
parameter is a dimension. The number signifies the dimension number relative to the beginning of the dimensioning sequence.
Open the file sketch6.dwg in the desktop\tutorial folder. Add and modify
dimensions to complete the definition of the following sketch.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
The before-and-after sketches reveal where dimensions are needed and in
what order you should place them. The dimensions needed here have
already been identified and are expressed as numeric constants.

dim 1

dim 4
dim 5

dim 3

dim 2
original sketch

profiled sketch

To keep the sketch shape from becoming distorted as the dimensions resize
it, define larger dimensions first: the left vertical line (dim 1) and the bottom
horizontal line (dim 2).
By adding geometric constraints, you can reduce the number of dimensions
you need. Later, you can modify the sketch with fewer changes.
After the basic shape has been defined, you replace the rightmost vertical line
and the top horizontal line with fillets, and add geometric constraints and
dimensions to finish the profile.

Applying Dimension Constraints

Creating Profile Sketches
First, convert the unconstrained sketch to a profile sketch before you add
dimensions. Then examine the default geometric constraints.
To create a profile from a sketch and examine constraints
1 Use AMPROFILE to create a profile from the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Mechanical Desktop redraws the sketch and reports that it still needs six
dimensions or constraints to solve the sketch:
Solved under constrained sketch requiring 6 dimensions or constraints.

Examine the inferred geometric constraints and determine if the default constraints are correct or whether they inhibit the dimensions you want to add.
2 Use AMSHOWCON to display the constraints, responding to the prompt.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] :

Chapter 7

Constraining Sketches

Enter a

Mechanical Desktop recalculates the sketch and displays the constraints.
■

■
■

A fix constraint is added to the start point of the first line of the sketch.
This point is anchored and will not move when changes are made to the
sketch constraints.
Nearly horizontal and vertical lines have been assigned horizontal (H) and
vertical (V) constraints.
Nearly vertical lines are assumed to be parallel (P) to one another.

For this exercise, all of the assumed geometric constraints are correct and
none of them restrict the dimensioning scheme shown earlier.
Exit from Show Constraints, responding to the prompt as follows:
Enter an option [All/Select/Next/eXit] : Press ENTER

Adding Dimensions
The rough sketch is converted to a profile sketch, and default geometric
constraints are applied. Now you need to fully constrain the sketch by adding
four dimensions and two geometric constraints. Parts are resized as you
change parametric dimensions to refine your design, while all geometric
relationships are maintained.
Keep the following points in mind as you are adding dimensions:
■
■
■
■

Select the elements to dimension and choose where to place the dimension.
Dimension type depends on the element you choose and where you place
the dimension. The current size of the selected element is shown.
You can accept the calculated size or specify a new value.
The sketch element is resized according to the dimension value and the
dimension is placed at the location you chose.

It is good practice to accept the automatically calculated dimensions to
stabilize the sketch shape, particularly large outer dimensions. When you
later modify dimensions to exact sizes, the sketch shape is less likely to
become distorted.
In this exercise, you create horizontal and vertical dimensions. Then you
modify the sketch by appending geometry, and applying angular and radial
dimensions.

Applying Dimension Constraints

To add a dimension to a profile
1 Use AMPARDIM to add dimensions to your profile, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the line (1)
Select second object or place dimension: Place the dimension (2)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<1.9606>: Enter 2
Solved under constrained sketch requiring 5 dimensions or constraints.

1
2

The sketch is updated with the new dimension value.
The command line lists several options. These options and the number of
elements you select determine the type and placement of dimensions.
In this example, you choose a line and the placement of the dimension. If
you selected two elements and specified a location, Mechanical Desktop
would place a dimension that gives the distance between the two elements.
2 Continue dimensioning the sketch by choosing the bottom horizontal line.
Select first object: Specify the line (3)
Select second object or place dimension: Place the dimension (4)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<2.1123>: Enter 2
Solved under constrained sketch requiring 4 dimensions or constraints.
Select first object: Press ENTER
Mechanical Desktop redraws the sketch according to the new dimension value.

Chapter 7

Constraining Sketches

Now that the default constraints and larger dimensions have stabilized the
sketch shape and size, you can begin to make changes to the sketch. To
practice changing and updating the sketch, you add fillets to the two legs of
the sketch.
To add a fillet to a sketch
1 Use AMFILLET to apply a fillet, entering the points in the order shown.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.1250
Select first object or [Polyline/Radius/Trim]: Specify the line (1)
Select second object: Specify the line (2)

NOTE Because you selected parallel lines, FILLET ignores the radius value and
joins the endpoints of the selected lines with a continuous arc.

3
4

2 Apply a fillet to the other leg of the sketch.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.1250
Select first object or [Polyline/Radius/Trim]: Specify the line (3)
Select second object: Specify the line (4)
Your sketch should now look like this.

Applying Dimension Constraints

Before you continue defining your sketch, erase the horizontal line and the
vertical line joining the endpoints of the new arcs.
3 Erase the two lines.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Erase.

Your drawing should look like this.

Because you have changed the sketch, you must re-solve it before you can use
it to create a feature.

Appending Sketches
By adding the fillets and removing the lines, you have changed the sketch
geometry. Whenever you add, modify, or remove geometry you must append
the changed geometry to the profile sketch. You will be prompted to select
any new geometry you have created. Mechanical Desktop appends the new
geometry and recalculates the sketch, assigning new geometric constraints.
After appending the sketch, re-examine the geometric constraints to see if
they affect your dimensioning scheme.

100

Chapter 7

Constraining Sketches

To append a profile sketch and re-examine geometric constraints
1 Expand the hierarchy of PART1_1.
2 Use AMRSOLVESK to append the existing fillets, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Append
Sketch.

Select geometry to append to sketch: Specify the first arc
Select geometry to append to sketch: Specify the second arc
Select geometry to append to sketch: Press ENTER
Redefining existing sketch.
Solved under constrained sketch requiring 4 dimensions or constraints.
Mechanical Desktop analyzes and redraws the profile in accordance with its
sketch analysis rules. Four additional constraints are needed to fully
constrain the sketch.
3 Use AMSHOWCON to display the constraint symbols.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

Press ENTER to exit the command.
4 Display all of the symbols. Several tangent (T) constraints are added to the
original geometric constraints.

The tangent constraints join the arcs to their adjoining lines. Notice that
although the sketch segment numbers have changed because of the new
geometry, the fix constraint remains in the same location.

Applying Dimension Constraints

101

For this exercise, do not delete any constraints because the tangent constraints
do not adversely affect the dimensioning scheme. Now that you have
recreated the profile sketch, you can continue to add geometric constraints
and dimensions to the sketch, starting with a radial constraint to the two arcs.
Depending on how you drew your sketch, your default dimension values
may differ from those in this exercise.
To add constraints to a re-created profile sketch
1 Use AMADDCON to add a radial constraint to the two arcs, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Radius.

Valid selections: arc or circle
Select object to be resized: Specify an arc
Valid selections: arc or circle
Select object radius is based on: Specify the other arc
Solved under constrained sketch requiring 3 dimensions or constraints.
Valid selections: arc or circle
Select object to be resized: Press ENTER
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER
Mechanical Desktop adds radius constraints to the two arcs.

Finish constraining the sketch by adding three dimension constraints.

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Chapter 7

Constraining Sketches

2 Use AMPARDIM to dimension the leftmost arc, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the lower arc
Select second object or place dimension: Place the dimension
Enter dimension value or [Undo/Diameter/Ordinate/Placement point]
<0.3687>: Enter .4
Solved under constrained sketch requiring 2 dimensions or constraints.

After you enter the new radius value, the arcs are updated because the radius
constraint makes both arcs equal.
3 Add the final two dimensions by responding to the prompts as follows:
Select first object: Specify the line (1)
Select second object or place dimension: Place the dimension (2)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.8753>: Enter .75
Solved under constrained sketch requiring 2 dimensions or constraints.
Select first object: Specify near the middle of line (1)
Select second object or place dimension: Specify near the middle of line (3)
Specify dimension placement: Place the dimension (4)
Enter dimension value or [Undo/Placement point] <138>: Enter 135
Solved fully constrained sketch.
Select first object: Press ENTER

2
3
4

Applying Dimension Constraints

103

The dimensions are placed. Your sketch should be fully constrained..

Save your file.

Modifying Dimensions
Because your design changes during development, you must be able to delete
or modify dimension values. Mechanical Desktop parametric commands
ensure that relationships among geometric elements remain intact.
To finish the sketch, change the dimension of the top horizontal line and the
angular dimension.
To change a dimension
1 Use AMMODDIM to modify the dimensions, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify the dimension (1)
New value for dimension <.4>: Enter .375
Solved fully constrained sketch.
Select dimension to change: Specify the dimension (2)
New value for dimension <.75>: Enter .5
Solved fully constrained sketch.
Select dimension to change: Press ENTER

2
1

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Constraining Sketches

Your finished sketch should now look like this.

Save your file.

Using Construction Geometry
Construction geometry can minimize the number of constraints and dimensions needed in a sketch and offers more ways to control sketch features.
Construction geometry works well for sketches that are symmetrical or have
geometric consistencies. Some examples are sketches that have geometry
lying on a radius, a straight line, or at an angle to other geometry.
Construction geometry is any line, arc, or circle in the sketch profile or path
that is a different linetype from the sketch linetype. By default, construction
geometry is placed on the AM_CON layer. To make construction geometry
easier to see, you can change its color, linetype, or linetype scale.
Construction geometry can be used to constrain only the sketch it is
associated with. When you create a feature from a sketch, you also select the
construction geometry with the path or profile sketch. After the feature is
created, the construction geometry is no longer visible.

Creating Profile Sketches
In this exercise, you follow a typical sequence. As always, study the sketch to
determine what constraints and dimensions you need and decide where to
place construction geometry to make solving the sketch easier.
Open the file sketch7.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Using Construction Geometry

105

To create a single profile sketch
1 Use PLINE to draw the rough sketch.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

2 Use AMSOLVE to solve the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

The polyline is automatically selected.
Mechanical Desktop applies constraints according to how you sketch and
then reports that the sketch needs six or more additional constraints. A fix
constraint is automatically applied to the point where you started your sketch.
3 Use AMSHOWCON to display the existing constraints.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

4 Display all of the assumed constraint symbols. Each of the eight lines should
have a vertical or horizontal constraint.
Next, create a construction line to assist in constraining the sketch.

NOTE If necessary, remove the fix constraint using AMDELCON. This constraint
prevents you from projecting the sketch to the construction line.

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To create a construction line
1 Create a construction line.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Construction Line.

2 Draw the line diagonally across the sketch.

Mechanical Desktop draws the line on a new layer called AM_CON. The line
is yellow and drawn with the HIDDEN linetype. Because the linetype is
different from the one used to draw the sketch, the line is considered
construction geometry. It is used only in this sketch.
3 Use AMRSOLVESK to append the profile.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Append.

4 Select the construction line.
5 Re-examine the assumed constraints.

Adding Project Constraints
Mechanical Desktop recognizes nine lines in the sketch. The sketch requires
two more constraints because you added a construction line.
Next, project the construction line to each vertex that serves as an inner
corner of a stair.
To place a project constraint, specify a vertex and then select the construction line. Depending on how closely you drew the construction line to the
vertices, some constraints may have already been applied.

Using Construction Geometry

107

To add a project constraint
1 Use AMADDCON to add the project constraints, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Project.

Valid selections: line, circle, arc, ellipse or spline segment
Specify a point to project: Enter end
of: Specify point (1)
Valid selections: line, circle, arc, ellipse, work point or spline segment
Select object to be projected to: Specify the construction line (5)
Valid selections: line, circle, arc, ellipse or spline segment
Specify a point to project:
Repeat this process for points (2) through (4), then press ENTER
4
3
2
5
1

NOTE If you do not use the endpoint object snap, you will not be able to
correctly constrain the sketch.
By defining the slope of the stairs with the construction line, you have
reduced the number of required constraints and dimensions to four.
2 Use REDRAW to clean up the screen display.
Desktop Menu

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Chapter 7

View ➤ Redraw

Constraining Sketches

Adding Parametric Dimensions
To fully define the sketch, dimension one of the risers and apply a slope angle
for the construction line. Each step is equal in height, so you can add equal
length constraints to the remaining steps later.
To add a parametric dimension
1 Use AMPARDIM to dimension the slope angle, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify near the middle of the construction line (1)
Select second object or place dimension:
Specify near the middle of the bottom horizontal line (2)
Specify dimension placement: Specify a point to right (3)
Enter dimension value or [Undo/Placement point] <31>: Enter 30
Solved under constrained sketch requiring 3 dimensions or constraints.

1
3

2 Continue, adding dimensions to the first vertical riser.
Select first object: Specify a point near the center of the lower left vertical line (4)
Select second object or place dimension: Specify a point to left of first point (5)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.9463>: Enter 1
Solved under constrained sketch requiring 2 dimensions or constraints.
Select first object: Press ENTER

To finish constraining the sketch, add equal length dimensions to the
remaining two risers.

Using Construction Geometry

109

To add an equal length constraint
1 Use AMADDCON to add an equal length constraint, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Equal Length.

Valid selections: line or spline segment
Select object to be resized: Specify the second riser (2)
Valid selections: line or spline segment
Select object to base size on: Specify the dimensioned riser (1)
Solved under constrained sketch requiring 1 dimensions or constraints.
3
1

2 Continue on the command line to place the last constraint.
Valid selections: line or spline segment
Select object to be resized: Specify the third riser (3)
Valid selections: line or spline segment
Select object to base size on: Specify the dimensioned riser (1)
Solved fully constrained sketch.
You should now have a fully constrained sketch. Exit the command by
pressing ENTER twice.

3 Use AMMODDIM to change the angular dimension, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify the angular dimension
New value for dimension <30>: Enter 25
Select dimension to change: Press ENTER
Save your file.

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Constraining Path Sketches
Construction geometry helps you constrain sketches that may be difficult to
constrain with only the geometry of the sketch shape. In this exercise, you
create a path sketch, add a construction line, and constrain the sketch to the
line.
Before you begin this exercise, create a new part definition for the sketch.
To create a new part definition
1 Use AMNEW to create a new part definition.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

2 Press ENTER on the command line to accept the default part name.
3 Pan the drawing so you have room to create the next sketch.
Context Menu

In the graphics area, right-click and choose Pan.

You are ready for the next exercise.
To use construction geometry in a swept path
1 Use PLINE to draw the following sketch.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

Use the arc/direction option of PLINE to draw the arcs. You can also use your
cursor crosshairs to visually align the endpoints of each arc as you sketch.

NOTE To enlarge the crosshairs, choose Assist ➤ Options. Under Crosshair
Size, set the size to 15 or larger.

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111

2 Use AM2DPATH to create a 2D path from your sketch, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ 2D Path.

Select objects: Specify the polyline
Select objects: Press ENTER
Specify the start point of the path: Specify one of the ends of the path
Solved under constrained sketch requiring 10 dimensions or constraints.
Create a profile plane perpendicular to the path? [Yes/No] : Enter n
You can use either end for the start point.
Mechanical Desktop reports that the sketch needs ten or more additional
constraints, depending on how you drew the sketch.
3 Draw two construction lines. The goal is to have each of the ends of the arcs
meet the construction lines.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Construction Line.

4 In the Desktop Browser, expand the PART2_1 hierarchy.
5 Use AMRSOLVESK to append the construction lines to your sketch, following
the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Append.

Select geometry to append to sketch: Specify a construction line
Select geometry to append to sketch: Specify the other construction line
Select geometry to append to sketch: Press ENTER
Redefining existing sketch.
Specify start point of path: Specify one of the ends of the path
Solved under constrained sketch requiring 6 dimensions or constraints.
The construction lines have reduced the number of constraints or dimensions needed by constraining the arc endpoints and centers to the line. The
construction lines have been made horizontal as well.

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To check for and add missing constraints
1 Use AMSHOWCON to check for constraints that are still needed.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

2 Display all the constraints and press ENTER to exit the command.
3 Use AMADDCON to add constraints and dimensions to the sketch, following
the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the upper left arc (1)
Select second object or place dimension:
Specify the vertical line on the left below its midpoint (2)
Specify dimension placement: Specify a point to the left of the sketch (3)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<3.1069>: Enter 3
Solved under constrained sketch requiring 5 dimensions or constraints.
4
1

4 Add a second dimension.
Select first object: Specify the upper left arc (1)
Select second object or place dimension:
Specify a point above and left of sketch (4)
Enter dimension value or [Undo/Diameter/Ordinate/Placement point]
<0.2788>: Enter .25
Solved under constrained sketch requiring 4 dimensions or constraints.
Select first object: Press ENTER
Next, you fully solve the path by adding 2D constraints.

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113

5 Constrain all the arcs with the same radius as the one you just dimensioned,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Radius.

Valid selections: arc or circle
Select object to be resized: Specify the lower left arc
Valid selections: arc or circle
Select object radius is based on: Specify the arc with the radial dimension
Solved under constrained sketch requiring 3 dimensions or constraints.
Valid selections: arc or circle
Select object to be resized: Specify the upper arc that is second from the left
Valid selections: arc or circle
Select object radius is based on: Specify the arc with the radial dimension
Solved under constrained sketch requiring 2 dimensions or constraints.
Valid selections: arc or circle
Select object to be resized: Specify the lower arc that is second from the left
Valid selections: arc or circle
Select object radius is based on: Specify the arc with the radial dimension
Solved under constrained sketch requiring 1 dimensions or constraints.
Valid selections: arc or circle
Select object to be resized: Specify the upper right arc
Valid selections: arc or circle
Select object radius is based on: Specify the arc with the radial dimension
Solved fully constrained sketch.
Valid selections: arc or circle
Select object to be resized: Press ENTER
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER
Your sketch should now be fully constrained. You may need to use the Equal
Length constraint for the beginning and end vertical line segments of your
sketch. Experiment with this sketch by changing the values of the two
dimensions.
If arc centers do not lie on the construction line, use the project constraint.
Add project constraints until the sketch is fully constrained.

NOTE Depending on how accurately you sketched the path, you may need to
add other constraints. Experiment until your sketch is fully constrained. If you
have difficulty, delete the sketch and try again.
Save your file.

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Controlling Tangency
A single piece of construction geometry can manage the size and shape of
entire sketches. Circles and arcs are particularly useful for constraining the
perimeter shapes of nuts, knobs, multisided profiles, and common polygons.
In this exercise, you create a triangular sketch and then constrain the sides of
the triangle and the internal angles to remain equal. In this manner, you
could form the basis for a family of parts in which the only variable is a single
diameter dimension.
Create a new part definition for the next sketch.
To create a new part definition
1 Use AMNEW to create a new part definition.
Context Menu

In the graphics area, right-click and choose Part ➤ New
Part.

2 Accept the default part name.
3 Pan the drawing so you have room to create the next sketch.
Context Menu

In the graphics area, right-click and choose Pan.

You are ready to create the next sketch.
To control tangency with construction geometry
1 Use PLINE to create the triangular shape.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

2 Draw a circle inside the triangle.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Construction Circle.

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115

3 Use AMPROFILE to turn the sketch into a profile sketch, making sure to select
both the polyline and the circle.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Profile.

At this point, the circle may be tangent to some or all of the sides of the
triangle.
4 Use AMADDCON to add Tangent constraints to the sketch, following the
prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Tangent.

Valid selections: line, circle, arc, ellipse or spline segment
Select object to be reoriented: Specify the line (1)
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be made tangent to: Specify the circle (2)
Solved under constrained sketch requiring 5 dimensions or constraints.
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be reoriented: Specify the line (3)
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be made tangent to: Specify the circle (4)
Solved under constrained sketch requiring 4 dimensions or constraints.
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be reoriented: Specify the line (5)
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be made tangent to: Specify the circle (6)
Solved under constrained sketch requiring 3 dimensions or constraints.
Valid selections: line, circle, arc, ellipse or spline segment
Select object to be reoriented: Press ENTER
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER

2
6
4
3

Mechanical Desktop now needs three or more dimensions or constraints to
fully solve the sketch.

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To add a dimension to an angle
1 Use AMPARDIM to apply angular dimensions to the triangle, following the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify near the middle of the line (1)
Select second object or place dimension: Specify near the middle of the line (2)
Specify dimension placement: Place the dimension (3)
Enter dimension value or [Undo/Placement point] <67>: Enter 60
Solved under constrained sketch requiring 2 dimensions or constraints.

2 Continue on the command line.
Select first object: Specify near the middle of the line (4)
Select second object or place dimension: Specify near the middle of the line (5)
Specify dimension placement: Place the dimension (6)
Enter dimension value or [Undo/Placement point] <78>: Enter 60
Solved under constrained sketch requiring 1 dimensions or constraints.
Select first object: Press ENTER

NOTE If you do not select the lines near their midpoints, you may be
prompted to specify the type of dimension to create. Choose Angular.
The angular dimensions should look like these.

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117

To add a dimension to a circle
1 Add a dimension to the diameter of the construction circle, following the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify a point on the circle
Select second object or place dimension: Specify a point outside of the triangle
Enter dimension value or [Undo/Radius/Ordinate/Placement point]
<3.1541>: Enter 10
Solved fully constrained sketch.
Select first object: Press ENTER
The sketch should now be fully constrained.
2 Zoom out to view the entire sketch.
Context Menu

In the graphics area, right-click and choose Zoom.

NOTE If the bottom segment of your triangle is still not horizontal, you will
need to add a Horizontal constraint to fully constrain the sketch.
3 Experiment with the size of the sketch. Use AMMODDIM to change the
diameter dimension of the circle, following the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify the diameter dimension
New value for dimension <10>: Enter 5
Solved fully constrained sketch.
Select dimension to change: Press ENTER
Save your file.

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All sides remain equal in length and tangent to the circle, and the bottom of
the triangle remains horizontal. If you used this sketch as a base feature of a
part, you could change the overall size of the part simply by changing the
diameter of the construction circle.
This technique could be applied to more complex geometry such as
pentagons, octagons, and odd-shaped polygons. These shapes can form the
base feature for a family of nuts, bolts, fittings, and so on. Try these types of
sketches on your own.

Using Construction Geometry

119

120

Creating Sketched Features

In This Chapter

Features are the parametric building blocks of parts. By
creating and adding features you define the shape of

■ Extruded features
■ Loft features
■ Revolved features

your part. Because features are parametric, any changes

■ Face splits

to them are automatically reflected when the part is

■ Sweep features

updated.
In Autodesk® Mechanical Desktop®, there are three
types of features—sketched, work and placed.
In this tutorial, you learn to create and modify sketched
features. In chapter 4, you learn about work features.

121

Key Terms
Term

Definition

base feature

The first feature you create. As the basic element of your part, it represents its
simplest shape. All geometry you create for a part depends on the base feature.

Boolean modeling

A solid modeling technique in which two solids are combined to form one
resulting solid. Boolean operations include cut, join, and intersect. Cut subtracts
the volume of one solid from the other. Join unites two solid volumes. Intersect
leaves only the volume shared by the two solids.

consumed sketch

A sketch used in a feature, for example, an extruded profile sketch. The sketch is
consumed when the feature is created.

cubic loft

A feature created by a gradual blending between two or more planar sections.

draft angle

An angle applied parallel to the path of extruded, revolved, or swept surfaces or
parts. A draft angle is used to allow easy withdrawal from a mold or easy insertion
into a mated part.

extrude

In part modeling, to create a geometric sketch defined by a planar profile
extended along a linear distance perpendicular to the profile plane.

feature

helical sweep

A geometric feature defined by the volume from moving a profile along a 3D
path about a work axis.

linear loft

A feature created by a linear transition between two planar sections.

lofted feature

A parametric shape created from a series of sketches defining the cross-sectional
shape of the feature at each section.

revolve

In part modeling, to create a feature by revolving a profile about an axis of
revolution.

sketch plane

A temporary drawing surface that corresponds to a real plane on a feature. It is an
infinite plane with both X and Y axes on which you sketch or place a feature.

sketched feature

A three-dimensional solid whose shape is defined by constrained sketches and
located parametrically on a part. Sketched features are extrudes, lofts, revolves,
sweeps, or face splits.

sweep

A geometric sketch feature defined by the volume from moving a profile along a
path.

swept profile

A special parametric sketch used to create a swept feature from the cross section
of a profile.

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Basic Concepts of Sketched Features
Features are the building blocks you use to create and shape a part. Because
they are fully parametric, they can easily be modified at any time.
The first feature in a part is called the base feature. As you add more features,
they can be combined with the base feature or each other to create your part.
Boolean operations, such as cut, join, and intersect, can be used to combine
features after a base feature has been created.
You create a sketched feature from a profile, which is an open or closed
parametric sketch that has been solved. You can also create a feature from
a text-based sketch. In most cases, you fully constrain the profile before
you create a feature. Because a sketch is parametric, you can easily modify
it to change the shape of the feature. When you update your part, the
changes you made are displayed automatically.
Sketched features include extrusions, lofts, revolutions, sweeps, and embossing. Face splits are also considered sketched features, but they are created by
splitting a part face using an existing face, a work plane, or a split line. If you
choose the split line method, you are using a sketched feature to split the
face.
In this tutorial you learn how to create and edit sketched features. Later you
learn how to create and edit work features and placed features.
Open the file s_feat.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Basic Concepts of Sketched Features

123

The drawing file includes fifteen parts which contain the geometry you need
to create the sketched features in this section.

NOTE For clarity, the work features are not shown.
First, you create an extruded feature.

Creating Extruded Features
Extrusions are the most common sketched features. An extruded feature can
be created from a closed profile, an open profile, or a text-based profile.

Extruding Closed Profiles
A closed profile is used to create a base feature, or in Boolean modeling to cut,
intersect, and join with other features.
In the first exercise, you use the part EXTRUDE_1. Activate the part, and
expand the hierarchy of EXTRUDE_1.
To activate a part
Browser

Double-click EXTRUDE_1.
Click the plus sign in front of EXTRUDE_1 to expand the
hierarchy.

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Clear the visibility of the other parts, and display the dimensions and work
features of the active part.
To turn off the visibility of multiple parts
Browser

Select EXTRUDERIB_1, then hold down SHIFT as you
select BEND_1. Right-click the selected block and choose
Visible.

NOTE Because most of the parts do not contain features yet, you cannot use
the toolbutton, menu, or command methods to make the part instances
invisible.
Click the plus sign in front of EXTRUDE_1 to expand the hierarchy.
To thaw dimension and work layers
Desktop Menu

Assist ➤ Format ➤ Layer

The Layer Properties Manager dialog box is displayed.
In the AM_PARDIM layer, select the On icon and the Freeze icon to unthaw
the layer. Repeat for the AM_WORK layer.
Choose OK to exit the dialog box.
The parametric dimensions and work features for each part are now visible.

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125

To zoom in to a part
Browser

Right-click EXTRUDE_1, and choose Zoom to.

The EXTRUDE_1 part is positioned on your screen.
To create an extruded feature
1 Use AMEXTRUDE to create an extruded feature from Profile1.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Distance: Enter 0.5
Termination: Type: Blind

The image tile indicates the direction of the extrusion.
Choose OK.

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The profile is extruded perpendicular to the plane of the profile.

Next, you create and constrain another profile, and extrude it to cut material
from the base feature.
To create a profile sketch
1 Change to the top view of your part.
Desktop Menu

View ➤ 3D Views ➤ Top

2 Use RECTANGLE to sketch a rectangle as shown in the following illustration,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

Specify first corner point or [Chamfer/Elevation/Fillet/Thickness/Width]:
Specify a point (1)
Specify other corner point: Specify a second point (2)

Creating Extruded Features

127

3 Use AMRSOLVESK to solve the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

The command line indicates the number of constraints required to fully constrain the profile.
Solved underconstrained sketch requiring 4 dimensions or constraints.
Before you extrude the profile, fully constrain it by adding four dimensional
constraints.
To constrain a sketch
1 Use AMPARDIM to add parametric dimensions to fully constrain the sketch,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the top edge (1)
Select second object or place dimension: Place the dimension (2)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.1574>: Enter .16
Solved underconstrained sketch requiring 3 dimensions or constraints.
Select first object: Specify the top edge again (1)
Select second object or place dimension: Specify the top arc (3)
Specify dimension placement: Place the dimension (4)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.0730>: Enter .08
Solved underconstrained sketch requiring 2 dimensions or constraints.
2
4
3
1
9
8

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2 Continue creating the parametric dimensions.
Select first object: Specify the right edge (5)
Select second object or place dimension: Place the dimension (6)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.4500>: Enter .5
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Specify the left edge (7)
Select second object or place dimension: Specify the left arc (8)
Specify dimension placement: Place the dimension (9)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.2430>: Enter v
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.2430>: Enter .25
After you finish dimensioning, the following message is displayed on the
command line:
Solved fully constrained sketch.
Select first object: Press ENTER
Your sketch should look like this.

NOTE For clarity, the parametric dimensions controlling Profile1 are not
shown.
Now that the profile is fully constrained, you extrude it into the base feature
to cut material from your part.

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129

To add an extruded feature to a part
1 Change to an isometric view.
Desktop Menu

View ➤ 3D Views ➤ Front Right Isometric

2 Extrude the profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

3 In the Extrusion dialog box, specify the following:
Operation: Cut
Distance: Enter 0.25
Termination: Blind
4 Choose OK to exit the dialog box.
Your part should look like this.

Save your file.

Editing Extruded Features
Because an extruded feature is controlled by parametric dimensions, you can
easily make changes to it by modifying the values of the profiled sketch, or
the extruded feature itself.

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To modify a consumed profile
1 Expand ExtrusionBlind2 in the Browser.
2 Edit the dimensions of the profile used to define the shape of the extrusion,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] :
Press ENTER, and select the cut extrusion
Enter an option [Next/Accept] : Press ENTER
2 In the Extrusion dialog box, specify a distance of .15 and Choose OK.
3 Continue on the command line.
Select object: Press ENTER
4 Use AMUPDATE to update the part.
Context Menu

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In the graphics area, right-click and choose Update Part.

Creating Sketched Features

Your part should look like this.

Save your file.

Extruding Open Profiles
You extrude open profiles to create rib features and thin features.
For more information about sketching open profiles, see “Creating Open Profile Sketches” on page 46.

Creating Rib Features
To create a rib feature on a part model, you sketch an open profile to shape
the rib, define the thickness of the rib, and extrude it to part surfaces.
Observe these rules when you sketch open profiles for ribs:
■
■
■

Sketch the side view of the rib.
The sketch can have any number of segments.
The ends of the sketch need not touch surfaces the rib will attach to, but
when extended must meet valid active part surfaces, without holes in the
extrusion path.

You solve the sketch to create an open profile, and apply parametric constraints and dimensions as with any other profile sketch.
Like other features, the rib feature can be edited and it has dependencies. If
you delete something in your model that a rib feature depends upon, such as
a face that a profile plane is based on, you delete the rib feature as well.

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133

In this exercise, you extrude a rib feature to two perpendicular walls of a part.
Turn off visibility for EXTRUDE_1, and make EXTRUDERIB_1 visible.
Browser

Right-click EXTRUDE_1 and choose Visible. Then rightclick EXTRUDERIB_1 and choose Visible.

Activate EXTRUDERIB_1 and position it on your screen.
Browser

Double-click EXTRUDERIB_1. Then right-click
EXTRUDERIB_1 and choose Zoom to.

In the previous exercise, you made the work feature layer visible.

To create a rib feature
1 Change to the front view so you can sketch the rib from its side.
Desktop Menu

View ➤ 3D Views ➤ Front

2 Use PLINE to sketch a rough outline of the rib, as shown in the following illustration. The sketch doesn’t have to be touching the surfaces.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

NOTE For clarity, the work plane is not shown.

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3 Use AMPROFILE to solve the sketch, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Select part edge to close the profile : Press ENTER
An icon for the open profile is displayed in the Browser.
4 Use AMPARDIM to add an angular dimension between the lower wall and the
lower section of the rib, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify a point on the rib (1)
Select second object or place dimension: Specify a point on the lower wall (2)
Specify dimension placement: Specify a point to place the dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<71>: Enter a value of 73
Select first object: Specify the next dimension to add
Continue adding dimensions, as shown in the illustration, to fully constrain
the open profile sketch.
Solved fully constrained sketch.
Select first object: Press ENTER

5 Use AMRIB to create the rib.
Browser

In the Browser, right-click the open profile icon, and
choose Rib.

Editing Extruded Features

135

In the Rib dialog box, specify:
Type: Midplane
Thickness: .05

Choose OK.
6 Use 3DORBIT to rotate your part so you can see the rib feature.
Your part should look like this.

Creating Thin Features
To create a thin feature, you sketch an open profile and extrude it to part surfaces. When you extrude an open profile, the Extrusion dialog box includes
the options for defining a thin wall feature. When you sketch open profiles
for thin features
■
■
■

Sketch must be an open profile from the front view
Sketch is extruded normal to the sketch plane
Ends of the open profile need not touch surfaces, but when extended must
meet valid active part surfaces, without holes in the extrusion path

For more information about sketching open profiles, see “Creating Open Profile
Sketches” on page 46.

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In this exercise, you create a thin wall in a shell. In the Browser, turn off
visibility for EXTRUDERIB_1, and make EXTRUDETHIN_1 visible.
Browser

Right-click EXTRUDERIB_1 and choose Visible. Then
right-click EXTRUDETHIN_1 and choose Visible.

Activate EXTRUDETHIN_1 and position it on your screen.
Browser

Double-click EXTRUDETHIN_1. Then right-click
EXTRUDETHIN_1 and choose Zoom to.

To create a thin feature
1 Use AMWORKPLN to create a work plane for the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:
1st Modifier: Planar Parallel
2nd Modifier: Offset
Offset: Enter .75
Choose OK.
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the back face of the shell
Enter an option [Next/Accept] : Press ENTER
Enter an option [Flip/Accept] :
Flip to point arrow to back face, or press ENTER
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER

2 Change to the Right view to sketch the thin feature.
Desktop Menu

View ➤ 3D Views ➤ Right

Editing Extruded Features

137

3 Use LINE to sketch the thin feature.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Line

Specify first point: Specify the start point of the line (1)
Specify next point or [Undo]: Specify the end point of the line (2) and press ENTER

NOTE Turn OSNAP off so that you will not snap to the back face when you pick.
4 Use AMRSOLVESK to solve the sketch, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Select part edge to close the profile : Press ENTER
In the Browser, an open profile icon is displayed.
5 Change to the front right isometric view to extrude the profile.
Desktop Menu

View ➤ 3D Views ➤ Front Right Isometric

6 USE AMEXTRUDE to extrude the open profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify
Operation: Join
Termination: Type: Face
Thickness: Type: Midplane
Thickness: Enter .05

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Choose OK.
7 Respond to the prompt:
Select Face: Select the back face of the shell and press ENTER
Enter an option [Next/Accept] : Press ENTER
Your part should look like this.

A thin wall is created with equal thickness on each side of the profile. In the
Browser, an icon is displayed for the thin extrusion.

NOTE When you extrude an open profile, the Extrusion dialog box contains
options for defining a thin feature.
Save your file with a new name so you can use the same shell part for the next
exercise.

Editing Extruded Features

139

Creating Emboss Features
Emboss features are text sketch profiles extruded on part models. A text
sketch profile is one line of text displayed in a rectangular boundary.
To create a text sketch profile, you define a font and a style, and enter one
line of text. Then you place the text on an active sketch plane on your part,
and extrude it to emboss the surface of your part with the text.
Delete the thin extrusion from your shell part.
Browser

Right-Click ThinExtrusionToFace1 and choose Delete.

Highlighted features will be deleted. Continue? [Yes/No] : Press ENTER
Change to the Front view to create the emboss feature.
Desktop Menu

View ➤ 3D Views ➤ Front

To create an emboss feature
1 Use AMWORKPLN to create a work plane for the text sketch.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:
1st Modifier: On Edge/Axis
2nd Modifier: Planar Parallel
Choose OK.
2 Respond to the prompts:
Select work axis, straight edge or [worldX/worldY/worldZ]:
Select the top edge of the shell
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the front face of the shell and press ENTER
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER

NOTE Verify that CMDDIA is set to 1 so that the Text Sketch dialog box will be
displayed. On the command line, enter CMDDIA, then enter 1.
3 Use AMTEXTSK to create a text sketch profile.
Command

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In the Text Sketch dialog box, specify:
True Type Font: Sans Serif
Style: Regular
Text: Enter Autodesk

Choose OK.
4 Define a location for the text sketch with a rotation angle of 15, responding
to the prompts.
Specify first corner: Specify a point in the lower left corner of the shell
Specify opposite corner or [Height/Rotation]: Enter r and press ENTER
Specify second angle endpoint or [Direction] <0>:
Move the cursor to the right and specify a rotation angle of 15
Hold the cursor in one location momentarily to display the angle dimension.

NOTE For clarity, the work plane is not shown.
Continue on the command line.
Specify opposite corner or [Height/Rotation]:

Specify a point for the height

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141

As you move the cursor, the rectangular border adjusts to accommodate the
size of the text.

In the Browser, an icon is displayed for the text sketch.
You can change the parametric dimension for the height, and you can control
the placement of the text object with typical 2D constraints and parametric
dimensions between the rectangular boundary and other edges or features on
your part.
After the text sketch is positioned on the part, you can extrude it.
5 Use AMEXTRUDE to extrude the text sketch.
Browser

Right-click the text sketch icon and choose Extrude.

In the Extrusion dialog box, specify:
Operation: Join
Distance: Enter .5
Termination: Type: Blind
Choose OK.
6 Use 3DORBIT to rotate your part so you can see the emboss feature.
Toolbutton
Your part should look like this.

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Editing Emboss Features
You can edit the text in an emboss feature using the Text Sketch dialog box
before the text sketch is consumed. After a text sketch is consumed by a feature, you can edit the feature dimensions or the sketch font and style.

Creating Loft Features
You create loft features by defining a series of cross sections through which
the feature is blended. Lofts may be linear or cubic. Both types can be created
with existing part faces as the start and end sections.

Creating Linear Lofts
A linear loft is a feature created by a linear transition between two planar
sections.
First, activate the next part in your drawing.
To activate a part
1 Make LOFT1_1 visible.
Browser

Right-click LOFT1_1 and choose Visible.

NOTE Because LOFT1_1 does not contain any features, you cannot use the
toolbutton, menu, or command methods to make it visible.
2 Activate LOFT1_1.
Browser

Right-click LOFT1_1 and choose Activate Part

3 Make EXTRUDE_1 invisible.
Browser

Right-click EXTRUDE_1 and choose Visible.

4 In the Desktop Visibility dialog box, select the Assembly tab.
5 Choose Select and continue on the command line.
Select assembly objects to hide: Select EXTRUDE_1
Select assembly objects to hide: Press ENTER
6 Choose OK to exit the dialog box.
If you choose the Browser method, the dialog box is not displayed.
Next, create the lofted feature.

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143

To create a linear loft
1 Expand LOFT1_1 in the Browser. Minimize EXTRUDE_1.

2 Zoom in to LOFT1_1.
Desktop Menu

View ➤ Zoom ➤ All

The LOFT1 part contains two planar sections you use to create a linear lofted
feature.

3 Create the loft feature, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Loft.

Select profiles or planar faces to loft: Specify the bottom profile
Select profiles or planar faces to loft: Specify the top profile
Select profiles or planar faces to loft or [Redefine sections]: Press ENTER
4 In the Loft dialog box, specify:
Type: Linear

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5 Choose OK to exit the Loft dialog box.
Mechanical Desktop® calculates and displays the loft feature.

Save your file.
Next, you create a cubic loft blended through three planar sections.

Creating Cubic Lofts
A cubic loft is created by a gradual blend between two or more planar sections. Before the loft begins blending with the next section, you can control
the tangency and the take-off angle at the start and end sections, and the distance the loft follows the tangent or angle options.
To create a cubic loft
1 Make LOFT2_1 visible.
2 Activate LOFT2_1.
3 Make LOFT1_1 invisible.
4 Zoom in to LOFT2_1.
Browser

Right-click LOFT2_1, and choose Zoom to.

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145

LOFT2 contains three profiles defining the sections you use for the loft feature.

5 Create the loft, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Loft.

Select profiles or planar faces to loft: Select the bottom profile
Select profiles or planar faces to loft: Select the middle profile
Select profiles or planar faces to loft or [Redefine sections]: Select the top profile
Select profiles or planar faces to loft or [Redefine sections]: Press ENTER
6 In the Loft dialog box specify:
Type: Cubic
7 Choose OK to exit the Loft dialog box.
The loft is displayed with isolines because it is created from elliptical and circular sections. The default isoline setting displays the loft as in the following
illustration.

For a better view of the loft, increase the number of isolines defining the
feature.

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To change the number of isolines
1 Modify the ISOLINES system variable.
Command

ISOLINES

New value for ISOLINES <4>: Enter 6
2 Regenerate your drawing.
Desktop Menu

View ➤ Regen

Mechanical Desktop regenerates the drawing and displays the loft using
more isolines.

NOTE A higher value for ISOLINES increases the time it takes to recalculate a
part. In general, keep ISOLINES at its default value (4).
3 Reset the value of ISOLINES to its default setting.
Command

ISOLINES

New value for ISOLINES <6>: Enter 4
4 Regenerate your drawing.
Desktop Menu

View ➤ Regen

Save your file.
In the next exercise you create a cubic loft using an existing part face as the
start section of the loft.

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147

To create a cubic loft from an existing face
1 Make LOFT3_1 visible.
2 Activate LOFT3_1.
3 Make LOFT2_1 invisible.
4 Zoom in to LOFT3_1.
LOFT3 contains an existing extrusion and two profiles parametrically constrained to it.

NOTE For clarity, the parametric dimensions are not shown.
5 Select the profiles to use for the cubic loft, following the prompts, and join
the loft to the existing extrusion.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Loft.

Select profiles or planar faces to loft: Select the front planar face (1)
Enter an option [Accept/Next] :
Highlight the front face and press ENTER
Select profiles or planar faces to loft: Select the first profile (2)
Select profiles or planar faces to loft or [Redefine sections]:
Select the second profile (3)
Select profiles or planar faces to loft or [Redefine sections]: Press ENTER

1
2
3

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6 In the Loft dialog box, specify:
Operation: Join
Type: Cubic
Choose OK to exit the Loft dialog box.
Your drawing should look like this.

Save your file.

Editing Loft Features
You edit loft features the same way extruded features are edited—change the
profiles or modify the loft feature itself.
Try editing the loft features you created in this section.

Editing Loft Features

149

Creating Revolved Features
You create revolved features by revolving a closed profile about an axis. The
axis may be a work axis or a part edge.
To create a revolved feature about a work axis
1 Make REVOLVE_1 visible.
2 Activate REVOLVE_1.
3 Expand REVOLVE_1 and make Work Axis1 visible.
4 Make LOFT3_1 invisible.
5 Zoom in to REVOLVE_1.
REVOLVE_1 contains a profile parametrically constrained to a work axis.

work axis

NOTE For clarity, the parametric dimensions are not shown.
6 Create a revolved feature.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Revolve.

7 Respond to the prompt as follows:
Select revolution axis: Specify the work axis
8 In the Revolution dialog box, specify:
Angle: Enter 360
Termination: By Angle

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Choose OK.
Mechanical Desktop calculates and displays the feature.

Save your file.

Editing Revolved Features
Edit a revolved feature by making changes to the profile, or by modifying the
feature itself (like editing extruded and lofted features).
Try editing your revolved feature following the procedures for editing
extruded features you learned earlier in this tutorial.

Editing Revolved Features

151

Creating Face Splits
Use face splits to split existing part faces. They can be created with
■
■
■

An existing part face
A work plane
A split line

First, use one of the part’s existing faces to split a face.
To split a face using an existing part face
1 Make FSPLIT_1 visible.
2 Activate FSPLIT_1.
3 Make REVOLVE_1 invisible.
4 Zoom in to FSPLIT_1.
FSPLIT_1 contains a part, a work plane, and a split line.

work plane

split line

NOTE For clarity, the parametric dimensions are not shown.
5 Create the face split, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] : Enter p
Select faces to split or [All]: Specify the left back face (1)
Enter an option [Accept/Next] :
Enter n to flip to the back face or press ENTER to continue
Select faces to split or [All/Remove]: Press ENTER
Select planar face or work plane for split: Specify the top right face (2)
Enter an option [Accept/Next] :
Enter n to flip to the top face or press ENTER

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Mechanical Desktop splits the back face into two faces.

Next, split a face using a work plane.
To split a face using a work plane
1 Create the face split, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] : Enter p
Select faces to split or [All]: Specify the top right face (1)
Enter an option [Accept/Next] :
Enter n to flip to the top face or press ENTER to continue
Select faces to split or [All/Remove]: Specify the right front face (2)
Enter an option [Accept/Next] :
Enter n to flip to the front face or press ENTER to continue
Select faces to split [All/Remove]: Press ENTER
Select planar face or work plane for split: Specify the work plane (3)

3
1
2

Creating Face Splits

153

Your drawing should look like this.

Now split the front face using the split line sketch.
To split a face using a split line
1 Make Work Plane2 invisible.
2 Create the face split, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] : Press ENTER
Select faces to split or [All]: Specify the left front face (1)
Enter an option [Accept/Next] :
Enter n to flip to the front face or press ENTER to continue
Select faces to split or [All/Remove]: Press ENTER

If you use the Browser method, the prompts are not displayed.

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When you choose the Project option, Mechanical Desktop automatically
looks for an unconsumed split line. If more than one split line exists, you are
prompted to select the split line for the face split.
Mechanical Desktop displays the new face split.

The Browser contains three face split features.
Save your file.

Editing Face Splits
Face splits created from an existing planar face can be edited by modifying
the position of the face on the part. Face splits created from a work plane can
be edited by modifying the dimensions controlling the location of the work
plane. Face splits created from a split line can be modified by editing the
parametric dimensions that control the split line.
Try editing the face splits you just completed in this exercise.

Creating Sweep Features
Sweep features can be either 2D or 3D. Both are created by sweeping a closed
profile along a path.

Editing Face Splits

155

Creating 2D Sweep Features
You create a 2D sweep feature by sweeping a profile along a path that lies on
a 2D plane. The feature may be the base feature of your part, or you can use
Boolean operations to cut, intersect, split, or join the feature to your part.
To create a 2D sweep
1 Make SWEEP1_1 visible.
2 Activate SWEEP1_1.
3 Make FSPLIT_1 invisible.
4 Zoom in to SWEEP1_1.
SWEEP1_1 contains a solved profile constrained to the start of a 2D path.

NOTE For clarity, the parametric dimensions and the work point are not shown.
5 Create the 2D sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep dialog box, choose OK to accept the settings.

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Your drawing should look like this.

NOTE Increase the value of ISOLINES for a more accurate display of the sweep.
Save your file.

Creating 3D Sweep Features
With Mechanical Desktop, you can also sweep profiles along a variety of 3D
paths. Use these paths to create a feature swept along
■
■
■
■
■

A helical path
A spiral path
A path defined by a 3D spline
A path created from filleted 3D polylines and lines
A path created from existing part edges

For more information about creating 3D paths, see chapter 6, “Creating Parametric Sketches.”
First, create a 3D helical sweep.
To create a 3D helical sweep
1 Make SWEEP2_1 visible.
2 Activate SWEEP2_1.
3 Make SWEEP1_1 invisible.
4 Zoom in to SWEEP2_1.

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157

SWEEP2_1 contains a cylinder and a helical path. A solved profile is constrained
to the start of the path.

5 Create the 3D helical sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep Feature dialog box, choose OK to accept the settings.
You can create a cut, join, intersection, or split feature. These options are
available because there is a base feature in the part definition.
Choose OK to exit the dialog box.
Mechanical Desktop calculates the sweep and displays your part.

Save your file.
Next, create a spiral 3D sweep.

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To create a spiral 3D sweep
1 Make SWEEP3_1 visible.
2 Activate SWEEP3_1.
3 Make SWEEP2_1 invisible.
4 Zoom in to SWEEP3_1.
SWEEP3_1 contains a spiral helical path and a solved profile constrained to
the start of the path. The spiral path is elliptical.

5 Create the 3D sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep Feature dialog box, choose OK to accept the settings.
Your drawing should look like this.

Save your file.
Next, create a sweep using a 3D edge path.

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159

To create a sweep from a 3D edge path
1 Make SWEEP4_1 visible.
2 Activate SWEEP4_1.
3 Make SWEEP3_1 invisible.
4 Zoom in to SWEEP4_1.
SWEEP4_1 contains a 3D edge path and a solved profile constrained to the
start of the path.

5 Create the sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep Feature dialog box, choose OK to accept the settings.
Your drawing should look like this.

Save your file.
Next, sweep a feature along a path created from non-planar lines and arcs.

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To create a sweep from a 3D pipe path
1 Make SWEEP5_1 visible.
2 Activate SWEEP5_1.
3 Make SWEEP4_1 invisible.
4 Zoom in to SWEEP5_1.
SWEEP5_1 contains a 3D pipe path and a solved profile constrained to the
start of the path.

5 Create the sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep dialog box, choose OK to accept the settings.
Your drawing should look like this.

Save your file.
Finally, create a swept feature using a path created from a 3D spline.

Creating Sweep Features

161

To create a sweep from a 3D spline path
1 Make SWEEP6_1 visible.
2 Activate SWEEP6_1.
3 Make SWEEP5_1 invisible.
4 Zoom in to SWEEP6_1.
SWEEP6_1 contains a 3D spline path and a solved profile constrained to the
start of the path.

5 Create the sweep.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Sweep.

6 In the Sweep Feature dialog box, choose OK to accept the settings.
Your drawing should look like this.

Save your file.

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Editing Sweep Features
As with all sketched features, sweep features can be edited by modifying the
profile, the path, or the feature itself.
Try modifying the sweep features you just created.

Creating Bend Features
The bend feature is for bending flat or cylindrical parts.
To create a bend feature, you sketch a single line segment on your part and
create an open profile to define the tangency location where the part transitions from its current shape to the final bent shape.
To bend an entire flat part, sketch the open profile to extend over the entire
part. To bend only a portion of a flat part, sketch the open profile over only
the portion you want to bend.
By choosing options and entering values in the Bend dialog box, you design
a theoretical cylinder tangent to the open profile, about which the part
bends. The bend feature is placed automatically in one operation.
In the next exercise, you create a bend feature on a portion of a flat part.
Make the BEND_1 part visible. Then activate it and use ZOOM to position the
part on your screen.

Editing Sweep Features

163

To create a bend feature on a flat part
1 Use LINE to sketch a line on one side of the plate, responding to the prompts.
Context Menu

In the graphics area, right click and choose 2D Sketching ➤
Line.

Specify first point: Select the start point of the line
Specify next point [or Undo]: Select the end point of the line, and press ENTER
2 Use AMPROFILE to create an open profile, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Select part edge to close the profile : Press ENTER

In the Browser, an icon for the open profile is displayed.
3 Use AMBEND to create the bend feature.
Context Menu

In the graphics area, right-click and choose Sketched
Work Features ➤ Bend.

4 In the Bend dialog box specify:
Combination: Angle+Radius
Radius: 1.0
Angle: 90
Flip Bend Side: Verify that the direction arrow points toward the hole
Flip Direction: Verify that the arrow points up

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Choose OK.
Hide the hidden lines to see your part better. To display silhouette edges, you
set the DISPSILH system variable to 1 first.
5 Change the setting for DISPSILH.
Command

DISPSILH

New value for DISPSILH <0>: Enter 1
6 Use HIDE to hide the hidden lines.
Desktop Menu

View ➤ Hide

Your part should look like this.

The bend is completed, and an icon for the bend feature is displayed in the
Browser. Save your file.

Editing Bend Features
Use typical editing methods to edit a profile for a bend feature or to redefine
the bend.
Try redefining the bend feature you just created.

Editing Bend Features

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166

Creating Work Features

In This Chapter

In Autodesk® Mechanical Desktop®, work features are
special construction features that you use to place

■ Work planes
■ Work axes
■ Work points

geometry that would otherwise be very difficult to
position parametrically.
By constraining sketched and placed features to a work
feature, that is in turn constrained to your part, you can
easily control their location by changing the position of
the work feature.
This tutorial teaches you how to use work features to
control the position of sketched features. You learn
about each of these features as you work through the
tutorial.

167

Key Terms
Term

Definition

nonparametric work
plane

A work plane fixed in location with respect to a part. If the part geometry is
parametrically changed, the work plane is unaffected.

parametrics

A solution method that uses the values of part parameters to determine the
geometric configuration of the part.

parametric work plane

A work plane associated with and dependent on the edges, faces, planes, vertices,
and axes of a part.

sketch plane

A temporary drawing surface that corresponds to a real plane on a feature. It is an
infinite plane with both X and Y axes on which you sketch or place a feature.

work axis

A parametric construction line created along the centerline of a cylindrical feature,
or sketched on the current sketch plane. A work axis can be used as the axis of
revolution for a revolved or swept feature, an array of features, to place a work
plane, and to locate new sketch geometry. It can be included in dimensions.

work feature

Planes, axes, and points used to place geometric features on an active part.

work plane

An infinite plane attached to a part. A work plane can be designated as a sketch
plane and can be included in a constraint or dimension scheme. Work planes can
be either parametric, or nonparametric.

work point

A parametric work feature used to position a hole, the center of an array, or any
other point for which there is no other geometric reference.

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Basic Concepts of Work Features
When you build a parametric part, you define how the part’s features are
associated. Changing one feature directly affects all the features related to it.
Work features are special construction features that help you define the relationships between the features on your part. They provide control when
placing sketches and features. Any changes to the position of a work feature
directly affect the placement of the sketches and features constrained to it.
You use work features to define
■
■
■

A plane to place sketches and features
A plane or edge to place parametric dimensions and constraints
An axis or point of rotation for revolved, swept, and array features

There are three types of work features: work planes, work axes, and work
points. In this tutorial, you learn the basics of creating and modifying each
of these work features.
Open the file w_feat.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
The drawing contains three simple parts.

Each part has a profile sketch associated with it. You create work features to
control the behavior of each of the sketches.

Basic Concepts of Work Features

169

Creating Work Planes
A work plane is an infinite plane that you attach to your part. It can be either
parametric or nonparametric. A work plane can also be used to define a sketch
plane for new geometry. To position a feature that does not lie on the same
plane as your base feature, you define a new plane and then create the feature.
If the plane is parametric, any changes to it affect the position of the feature.
Work planes are defined using two modifiers. The modifiers determine how
the plane will be oriented. By selecting the right modifiers, you can create a
work plane wherever you need a plane to place geometry.
Parametric work planes can be created by specifying edges, axes, or vertices,
and defining whether the plane is normal, parallel, or tangent to selected
geometry. Nonparametric work planes can be created on the current coordinate system (UCS), or on any of the three planes of the World Coordinate
System (WCS).
For more information about creating work planes, see AMWORKPLN in the
online Command Reference.
PART1_1 contains an extrusion with a profile constrained to its back face.

NOTE For clarity, the parametric dimensions are not shown.
In this tutorial, you use this profile to cut material from the part. By extruding the profile to a work plane, you can easily control the depth of the extrusion by changing the position of the plane.

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First, you create a work plane through the midplane of the part and extrude
the profile to it. Later, you edit the position of the work plane to modify the
depth of the new extrusion.
Activate PART1_1 and use ZOOM to position it on your screen.
Browser

Double-click PART1_1. Now right-click PART1_1 and
choose Zoom to.

To create a work plane
1 Use AMWORKPLN to create a work plane through the midplane of PART1_1.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

2 In the Work Plane dialog box, specify:
1st Modifier: Planar Parallel
2nd Modifier: Offset
Offset: Enter .5
Choose OK.
3 Continue on the command line.
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Specify the front face
Enter an option [Next/Accept] :
Enter n to cycle to the front face or press ENTER
Enter an option [Flip/Accept] :
Enter f to point direction arrows into the part
Enter an option [Flip/Accept] : Press ENTER
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER
A work plane now bisects the part.

work plane

Next, extrude the profile to the work plane.

Creating Work Planes

171

To extrude a profile to a plane
1 Use AMEXTRUDE to extrude the profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

2 In the Extrusion dialog box, specify the following:
Operation: Cut
Termination: Plane
Choose OK to exit the dialog box.
3 Continue on the command line.
Select face or work plane: Specify the work plane
The profile is extruded to the work plane.

Now edit the location of the work plane to control the depth of the extrusion
you just created.

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Editing Work Planes
Because a nonparametric work plane is static, any features constrained to it
are restricted to the original plane. If you change the position or orientation
of your part, the features remain associated with the work plane and your
part could fail to update.
Whenever possible, locate your features on parametric work planes. When
you change the location of a parametric work plane, you change the position
of any features created on it or constrained to it.
To modify the position of a work plane
1 Use AMEDITFEAT to reposition the work plane, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature]
: Press ENTER
Select feature:
Specify the work plane
Select object: Specify the 0.5 dimension
Enter dimension value <.5>: Enter .15
Select object: Press ENTER
2 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Enter an option [active Part/aLl parts] : Press ENTER
If you use the Browser, the prompt is not displayed.
Your part should look like this.

Save your file.

Editing Work Planes

173

Creating Work Axes
A work axis is a parametric construction line used as the axis of revolution
for a revolved or swept feature, or an array of features; it is also used to place
a work plane, and to locate new sketch geometry. You can create a work axis
through the center of a cylindrical edge, or draw it on the current sketch
plane by specifying any two points.
PART2 contains a simple revolved feature, a work plane, and a partially constrained profile. You create a work axis through the center of the part. Then
you constrain the profile to the work axis so you can cut material from the
base feature.

NOTE For clarity, the parametric dimensions are not shown.
Activate PART2 and use ZOOM to position it on your screen.
Browser

Double-click PART2_1. Now right-click PART2_1 and
choose Zoom to.

To create a work axis
1 Use AMWORKAXIS to create a work axis, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Axis.

Select cylinder, cone or torus [Sketch]: Select a cylindrical edge
Because the work axis is created through the center of the part, no constraints
are necessary.

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work axis

Next, constrain the profile to the new work axis and create a revolved feature
from it.
Depending on your drawing, your default dimension values may differ from
those in this exercise.
To constrain and revolve a profile
1 Use AMPARDIM to constrain the profile to the work axis. Add two dimensions,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the right edge of the profile (1)
Select second object or place dimension: Specify the work axis (2)
Specify dimension placement: Place the dimension (3)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.8324>: Enter h to force a horizontal dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.1671>: Enter 0
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Specify the top edge of the profile (4)
Select second object or place dimension: Specify the top edge of the part (5)
Specify dimension placement: Place the vertical dimension (6)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.1333>: Enter 0
Solved fully constrained sketch.
Select first object: Press ENTER
5
6
4

3
2
1

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175

2 Use AMREVOLVE to revolve a feature from the profile, responding to the
prompt.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Revolve.

Select revolution axis: Select the work axis
3 In the Revolution dialog box, specify:
Operation: Cut
Angle: Enter 360
Termination: By Angle

Choose OK to exit the dialog box.
Your drawing should look like this.

Save your file.

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Editing Work Axes
Work axes are parametric, so any changes to the parameters controlling a
work axis affect the location of features constrained to it.
In this exercise, the work axis was created through the center of a cylindrical
object and cannot be repositioned. But by changing one of the dimensions
that constrains the profile to the axis, the revolved feature changes.
To modify the revolved feature, you change the horizontal dimension constraining the profile to the work axis. In this exercise, because the value of
the dimension is 0, modifying it forces the profile in the wrong direction. To
relocate the profile correctly, erase the dimension, move the profile slightly,
and then add a new horizontal dimension.
To reposition a profile constrained to a work axis
1 Edit the revolved feature with the Browser.
Browser

Right-click Revolution Angle1 and choose Edit Sketch.

2 Use ERASE to erase the 0.00 dimension constraining the profile to the work
axis.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Erase.

3 Use MOVE to move the profile and its dimensions, following the prompts.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Move.

Select objects: Enter w
Specify first corner: Specify a point above and left of the 0.15 dimension
Specify opposite corner: Specify a point below and right of the 0.30 dimension
11 found
Select objects: Press ENTER
Specify base point or displacement: Specify any point
Specify second point of displacement or :
Specify a point to the left of the base point

NOTE Press F8 to turn on orthographic mode before you specify the base and
second points.

Editing Work Axes

177

4 Use AMPARDIM to create a new parametric dimension, following the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the right edge of the profile
Select second object or place dimension: Specify the work axis
Specify dimension placement: Place the dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.4347>: Verify that the dimension is horizontal, then enter .15
Solved fully constrained sketch.
Select first object: Press ENTER
5 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Enter an option [active Part/aLl parts] : Press ENTER
Your drawing should look like this.

Save your file.

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Creating Work Points
A work point is a parametric point for positioning features that cannot easily
be located on a part. By constraining a feature to a work point and then constraining the work point to the part, you control the position of the feature.
Use work points to
■
■
■
■

Position sketched features
Create centers for polar arrays
Place surface cut features
Place holes when concentric cylindrical edges, or two planar edges, are not
available

PART3 contains a simple cylindrical extrusion with a work axis at its center,
and a sketch on its top face.

You place a work point on the sketch plane and profile the sketch. Then, you
constrain the profile to the work point, and the work point to the work axis.
Activate PART3, and use ZOOM to position it on your screen.
Browser

Double-click PART3_1. Then right-click PART3_1 and
choose Zoom to.

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179

To create and constrain a work point
1 Use AMWORKPT to create a work point, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Point.

Specify the location of the workpoint: Specify a point near the center of the sketch

NOTE You may prefer to turn OSNAP off before you create and constrain the
work point. Click the OSNAP button at the bottom of your screen.
2 Use AMPARDIM to constrain the work point to the work axis, following the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Specify the work point
Select second object or place dimension: Specify the work axis
Specify dimension placement: Place the dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.5890>: Verify the dimension is horizontal and enter .6
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Specify the work point
Select second object or place dimension: Specify the work axis
Specify dimension placement: Place the dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.6130>: Verify the dimension is vertical and enter .6
Solved fully constrained sketch.
Select first object: Press ENTER

Solve the sketch and constrain it to a work point.
Change to a top view of your part.
Desktop Menu

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View ➤ 3D Views ➤ Top

Creating Work Features

To solve a sketch and constrain it to a work point
1 Use AMPROFILE to solve the sketch, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Profile.

Select objects for sketch: Specify the polygon sketch
Select objects for sketch: Press ENTER
Solved underconstrained sketch requiring 8 dimensions or constraints.

NOTE Although the polygon is a single object, you cannot use Single Profile
to solve it because it was not the last object created.
The profile requires eight constraints: six to solve it, and two to constrain it
to the work point.
2 Zoom in to the profile and constrain it using the dimensions in the following
illustration.

You could also use Equal Length constraints on the line segments to reduce
the number of dimensions required.
3 Constrain the profile to the work point as in the following illustration.

NOTE For clarity, the dimensions of the profile are not shown.
The profile is now fully constrained. Next, you create an extrusion to cut
material from the base feature.

Creating Work Points

181

To extrude a feature through a part
1 Change to an isometric view.
Desktop Menu

View ➤ 3D Views ➤ Front Right Isometric

2 Use AMEXTRUDE to extrude the profile through the part.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Through
Choose OK.

The dimensions controlling the work point are still visible because the work
point has not been consumed by a feature.
Save your file.

Editing Work Points
Next, to relocate the extrusion you change the dimensions constraining the
work point to the work axis. The extrusion and the work point are parametrically associated; any change to the position of the work point causes the
extrusion to move.

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Creating Work Features

To edit a work point
1 Use AMMODDIM to modify the vertical sketch dimension controlling the
work point, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify the vertical dimension
New value for dimension <0.6000>: Enter 0
Solved fully constrained sketch.
2 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Enter an option [active Part/aLl parts] : Press ENTER
3 Use AMMODDIM to modify the horizontal sketch dimension controlling the
work point, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify the horizontal dimension
New value for dimension <0.6000>: Enter .75
Solved fully constrained sketch.
4 Update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Enter an option [active Part/aLl parts] : Press ENTER
5 Turn off the visibility of the work point and its dimensions.
Browser

Right-click WorkPoint1 and choose Visible.

Save your file.
You learn more about creating work features as you go through the rest of the
tutorials in this book.

Editing Work Points

183

184

Creating Placed Features

In This Chapter

This tutorial introduces you to placed features, and
builds on what you learned in previous tutorials. A

■ Holes
■ Face drafts
■ Fillets

placed feature is a well-defined common shape, such as

■ Chamfers

a hole or a fillet. To create a placed feature, you only

■ Shells

need to supply its dimensions. Autodesk® Mechanical
Desktop® creates the feature for you.
In this lesson, you learn how to create and modify

■ Surface cuts
■ Patterns
■ Copied features
■ Combined features
■ Part splits

placed features.

185

Key Terms
Term

Definition

chamfer

A beveled surface between two faces.

combine feature

A parametric feature resulting from the union, subtraction, or intersection of a
base part with a toolbody part.

draft angle

An angle applied parallel to the path of extruded, revolved, or swept surfaces or
parts. A draft angle is used to allow easy withdrawal from a mold or easy insertion
into a mated part.

face draft

A part face that has a draft angle applied to it. Used to create an angle on a face
that will be needed when pulling a part out of a mold.

fillet

A curved transition from one part face or surface to another. The transition cuts
off the outside edge or fills in the inside edge. The fillet can have a constant or
variable radius.

hole

A geometric feature with a predefined shape: drilled, counterbore, or countersink.

pattern feature

A parameter-driven collection of duplicate features. You can create rectangular,
polar, and axial patterns. If you change the original patterned feature, all the
elements in the pattern change.

placed feature

A well-defined mechanical shape that does not require sketches, such as a hole,
chamfer, or fillet. Placed features are constrained to the feature on which they are
placed, and they are geometrically dependent.

shell

A Mechanical Desktop feature that cuts portions of the active part by offsetting its
faces.

surface cut

A feature on a part created when a surface is joined to the solid. Where the
surface cuts the part or protrudes, the part face assumes the curved shape of the
surface. The surface, like other features, is parametric; both the surface and the
part retain their parametric relationship whenever either is modified.

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Basic Concepts of Placed Features
Placed features are well defined features that you don’t need to sketch, such
as fillets, holes, chamfers, face drafts, shells, surface cuts, patterns, combined
features, and part splits.
You specify values for their parameters and then you position them on your part.
To modify placed features, you simply change the parameters controlling them.
Open the file p_feat.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
The drawing includes thirteen parts which contain the geometry you need to
create the features in this tutorial. If you are interested in how the parts in
this drawing were created, activate a part and use AMREPLAY.

Before you begin, expand the Browser hierarchy by clicking the plus sign in
front of P_FEAT. Expand the hierarchy of the active part HOLE_1.

NOTE For clarity, the work features are not shown.

Basic Concepts of Placed Features

187

Creating Hole Features
You can create drilled, counterbore, and countersink hole features. Each may
be assigned tapped hole information. Holes can extend through the part,
stop at a defined plane, or stop at a defined depth. You can change a hole
from one type to another at any time.
When you create a hole, you can use the Thread tab in the Hole dialog box
to include threads. Threads can also be added to existing holes.
Instead of creating a custom hole, you can specify a standard hole from an
external file. Standard holes can be tapped or untapped.
In this exercise, you create hole features first. Then you add thread data to
the hole you created.
To create a hole feature
1 Activate HOLE_1 part, and zoom in to it.
Browser

In the Browser, double-click HOLE_1. Now right-click
HOLE_1 and choose Zoom to.

HOLE_1 is created from two extrusions.

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Chapter 10 Creating Placed Features

2 Use AMHOLE to create two drilled holes.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Hole.

NOTE Hold your cursor over an icon to see a tooltip that identifies the icon.
In the Hole dialog box, on the Hole tab, select the Drilled hole type icon, and
specify:
Termination: Through
Placement: Concentric
Diameter: Enter .25

Choose OK to exit the dialog box.

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189

3 Define the locations for the holes, responding to the prompts.
Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:
Specify a face (1)
Select concentric edge: Specify an edge (1)
Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:
Specify a face (2)
Select concentric edge: Specify an edge (2)
Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:
Press ENTER
1

Your drawing should look like this.

Next, add internal threads to the HOLE_1.

Creating Thread Features
You can create internal or external threads on cylindrical, conical, and elliptical shapes. You edit existing threads from within the Thread dialog box. As
with holes, you can specify standard threads from an external file.
In the following exercise, you add an external thread to one of the cylindrical
holes you created.

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Chapter 10 Creating Placed Features

To create a thread feature
1 In the Browser, select the hole to add threads.
Browser

Select Hole1.

2 Define the thread for Hole1
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Thread

Respond to the prompts:
Select cylindrical/conical edge or face: Select the circular edge of Hole1
Enter an option [Next/Accept] : Press ENTER
In the Threads dialog box, specify:
Thread Type: Custom
Full Thread: Select the check box
Major Dia: 0.2009
Minor Dia: 0.1709
Choose OK.

The thread feature is placed on Hole1 and an icon representing the external
thread is added to the Browser hierarchy.
Next, you change one of the drilled holes to a counterbore hole, and change
the minor diameter of the thread feature.

Creating Thread Features

191

Editing Hole Features
You can change a hole feature from one type of hole to another by modifying
the parameters defining the hole.
To edit a hole feature
1 Use AMEDITFEAT to change the second hole to a counterbore hole, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] :
Press ENTER
Select feature: Select the ExternalThread1 feature
2 In the Threads dialog box, specify:
Thread Type: Custom
Display Thread: Select the check box.
Minor Diameter: 0.1805
Choose OK.
3 Continue on the command line.
Select object: Press ENTER
The thread feature is displayed, and reflects the new minor diameter value.
Next, you learn how to create and edit face drafts.

Editing Thread Features

193

Creating Face Drafts
Face drafts are used to add a small angle to one or more faces of a part; then
the part can be easily extracted from a mold after it is manufactured.
Face drafts can be applied from a specified plane, an existing part face, or a
part edge. You can also create a shadow draft from a circular face. If you are
creating a face draft from a plane, the plane can be either an existing face, or
a work plane offset from the part.
First, activate F-DRAFT_1 and zoom in on the part. Turn off the visibility of
HOLE_1.

The part contains a simple extrusion.
To create a face draft from a plane
1 Use AMFACEDRAFT to create a face draft.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Face Draft.

In the Face Draft dialog box, specify:
Type: From Plane
Angle: Enter 10

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Chapter 10 Creating Placed Features

2 Choose Draft Plane and continue on the command line.
Select draft plane (planar face or work plane): Specify the bottom face
Draft direction [Accept/Flip] : Enter f to flip the direction arrow up
Draft direction [Accept/Flip] : Press ENTER
3 In the Face Draft dialog box, in Faces to Draft, press Add.
4 Continue on the command line.
Select faces to draft (ruled faces only): Specify the left side face
Select faces to draft (ruled faces only): Specify the right side face
Select faces to draft (ruled faces only): Press ENTER

NOTE Refer to the UCS icon to orient yourself when selecting faces.
5 Choose OK to exit the Face Draft dialog box. Draft is applied to the two faces.

A face draft can also be applied from an existing edge.
To create a face draft from a fixed edge
1 Create a face draft.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Face Draft.

In the Face Draft dialog box, specify:
Type: From Edge
Angle: Enter 10
Choose Draft Plane.

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195

2 Respond to the prompts as follows:
Select draft plane (planar face or work plane): Specify the back face
Enter an option [Next/Accept] :
Enter n to cycle to the back face, or press ENTER
Draft direction [Flip/Next] :
Enter f to flip the arrow away from the part, or press ENTER
3 In the Face Draft dialog box, specify:
Faces to Draft: Add
4 Continue on the command line.
Select faces to draft (ruled faces only): Specify the bottom face
Select faces to draft (ruled faces only): Press ENTER
Select fixed edge: Specify the bottom edge of the back face
Select fixed edge: Press ENTER
5 In the Face Draft dialog box, choose OK to exit.

Draft is applied to the bottom face.
Next, create a shadow draft along the circular face of the part.

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To create a shadow draft
1 Create the shadow draft.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Face Draft.

In the Face Draft dialog box, specify:
Type: Shadow
Angle: Enter 45
Choose Draft Plane.
2 Respond to the prompts as follows:
Select draft plane (planar face or work plane): Specify the top right face
Enter an option [Next/Accept] :
Enter n to cycle to the top right face or press ENTER
Draft direction [Flip/Accept] :
Enter f to flip the arrow away from the part or press ENTER
3 In the Face Draft dialog box, specify:
Faces to Draft: Add
4 Continue on the command line.
Select faces to draft (ruled faces only): Specify the cylindrical face
Enter an option [Next/Accept] :
Enter n to cycle to the cylindrical face or press ENTER
Select faces to draft (ruled faces only): Press ENTER
5 In the Face Draft dialog box, choose OK to exit.
Your part should look like this.

The Browser contains three face draft icons nested below the FDRAFT_1 part
definition.
Save your file.
Next, you modify one of the face drafts you just created.

Creating Face Drafts

197

Editing Face Drafts
To modify a face draft, you change the parameters that control it.
To edit a face draft
1 Use AMEDITFEAT to change FaceDraft2, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] :
Specify Fillet4
Enter an option [Next/Accept] :
Enter n to cycle to Fillet4 or press ENTER
Select object: Specify the .1 radius
Enter Radius <0.100000000>: Enter .5 and press ENTER
Select object: Specify the original .5 radius
Enter Radius <0.500000000>: Enter .1 and press ENTER
Select object: Press ENTER
2 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Your part should look like this.

Save your file.
Delete some or all of the fillets you created in these procedures, and replace
them with your own fillets to change the shape of your part.

Editing Fillet Features

203

Creating Chamfer Features
A chamfer feature is a bevelled face created between two existing faces on a
part. Chamfers can be created with an equal distance, two different distances,
or a distance and an angle. You can select an edge or a face to place a chamfer.
If one or more of the edges of a face you want to chamfer have been altered,
you need to use the edge selection method to place chamfers around that face.
First, activate CHAMFER_1 and zoom in on the part. Turn off the visibility of
FILLET_1.

The part contains a simple extrusion.
To create a chamfer defined by an equal distance
1 Use AMCHAMFER to create the chamfer.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Chamfer.

In the Chamfer dialog box, specify:
Operation: Equal Distance
Distance1: Enter .5

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2 Choose OK and respond to the prompts as follows:
Select edges or faces to chamfer: Specify an edge (1)
Select edges or faces to chamfer : Press ENTER

Mechanical Desktop creates the chamfer along the edge you selected.

You can also create chamfers by specifying two different distances. After you
select the edge, you specify a face for Distance 1, called the base distance. Distance 2 is applied to the other face.

Creating Chamfer Features

205

To create a chamfer defined by two distances
1 Use AMCHAMFER to create the chamfer.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Chamfer.

In the Chamfer dialog box, specify:
Operation: Two Distances
Distance1: Enter .25
Distance2: Enter .15
Choose OK.
2 Respond to the prompts as follows:
Select an edge or face to chamfer: Specify the edge (2)
Press to continue: Press ENTER
The specified face will be used for base distance.
Specify face for first chamfer distance (base) [Next/Accept] :
Press ENTER

Mechanical Desktop calculates and displays the chamfer. Your drawing
should look like this.

You can create a chamfer defined by a distance and an angle. You select an
edge, and then specify the face for the angle. The distance is applied to the
other face.

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Chapter 10 Creating Placed Features

To create a chamfer defined by a distance and angle
1 Define the chamfer.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Chamfer.

In the Chamfer dialog box, specify:
Operation: Distance and Angle
Distance1: Enter 1
Angle: Enter 10
Choose OK.
2 Continue on the command line.
Select an edge or face to chamfer: Specify the edge (3)
Press to continue: Press ENTER
The specified face will be used for base distance.
Specify face for chamfer distance (base) [Next/Accept] :
Press ENTER
3

Mechanical Desktop calculates and displays the chamfer.

If you need to place a chamfer on all sides of a face, you can select the face
and place a chamfer on all of the edges in one operation. This works on faces
where none of the edges to be chamfered have been altered.

Creating Chamfer Features

207

To create a chamfer on all edges of a face
1 Define the chamfer.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Chamfer.

In the Chamfer dialog box, specify:
Operation: Equal Distance
Distance1: Enter .04
Choose OK.
2 Continue on the command line.
Select edges or faces to chamfer: Select the face (4)
Enter an option [Next/Accept] : Press ENTER
Select edges or faces to chamfer : Press ENTER

A chamfer is placed on all edges of the face you selected.

Four chamfer icons are nested below the CHAMFER_1 part definition in the
Browser.
Save your file.

Editing Chamfer Features
As with all placed features, chamfers can be edited by selecting the feature,
changing parameters, and updating the part. Try editing some of the chamfer
features you created in this section.

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Chapter 10 Creating Placed Features

Creating Shell Features
You use shell features to hollow parts that are used in a variety of industrial
applications. For example, you shell parts to create molds, castings, containers, bottles, and cans.
Activate SHELL_1 and zoom in on it. Turn off the visibility of CHAMFER_1.

The part is constructed from two extrusions and one fillet feature.
Next, you shell the part, and then modify it to exclude the top and bottom faces.
To create a shell feature
1 Use AMSHELL to create a shell.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Shell.

In the Shell Feature dialog box, specify:
Default Thickness: Inside: Enter .1

Choose OK to exit the dialog box.

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209

Mechanical Desktop offsets all faces by the thickness you specified in the
Shell Feature dialog box.

2 Change to a front view for a better view of the feature.
Desktop Menu

View ➤ 3D Views ➤ Front

Save your file.
Next, you edit the feature to exclude the top and bottom faces from the shell.

Editing Shell Features
You modify shell features by changing the parameters that control them.
Shells can also have multiple thickness overrides applied to individual faces.
You learn to use multiple thickness overrides in chapter 14, “Creating Shells.”
To edit a shell feature
1 Return to an isometric view.
Desktop Menu

View ➤ 3D Views ➤ Front Right Isometric

2 Use AMEDITFEAT to modify the shell feature, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] :
Enter c
Select surfcut feature: Specify the surface
The surface is recovered.

In this state, you can modify the actual shape of the surface by editing its
grips, or change the location of the work point that controls the position of
the surface on the part.

Editing Surface Cut Features

213

2 Use AMMODDIM to change the vertical dimension controlling the work
point, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Specify .75
New value for dimension <.75>: Enter .5
Select dimension to change: Press ENTER
3 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

The part is updated to reflect the new location for the surface cut feature.

4 Save your file.
Experiment with the surface by editing its control points. Use AMEDITFEAT to
recover the surface. Then select a grip to activate it. When you move the grip
to another location you will see the surface deform. Update your part to
examine the effect of your changes.

Creating Pattern Features
A pattern is a collection of duplicate features. You can create patterns with
rectangular, nonorthogonal rectangular, polar, and axial configurations, and
patterns of other pattern features.
By default, a pattern feature uses the active sketch plane as the distribution
plane for pattern instances.

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While selecting a feature set for a pattern, you select each graphically dependent feature individually. You can select multiple independent features.
Single instances in a pattern can be made independent of an existing pattern
feature. Once a feature is independent, it can be altered while its position
remains intact.
In this tutorial, you create several different types of patterns, using both
incremental and included spacing. In the polar pattern exercise, you make
one instance independent and alter it.
Activate R-PATTERN_1, and zoom to it. Turn off the visibility of SURFCUT_1.

R-PATTERN contains a filleted plate and one counterbore hole. You create a
rectangular pattern of the hole with incremental spacing and alignment to
an edge.
To create a rectangular pattern
1 Use AMPATTERN to create a rectangular pattern, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Rectangle Pattern.

Select features to pattern: Specify the hole
Select features to pattern or [liSt/Remove] : Press ENTER
If you use multiple features to create a pattern, you select each one individually, regardless of feature dependencies.

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2 In the Pattern dialog box, specify:
Type: Rectangular
Column Placement: Choose Incremental Spacing, the leftmost button
Row Placement: Choose Incremental Spacing, the leftmost button

NOTE Hold the cursor over an icon for a tooltip to identify the icon.
Enter the values shown for column and row instances and spacing.

3 Choose Preview, and view your pattern on the screen.
At this point, you can redefine the pattern by changing your selections in the
Pattern dialog box, and then preview the changes. Preview becomes unavailable once the parameters in the dialog box match the display on the screen.
Using the preview image, you can suppress instances of features in patterns.
4 Choose OK to create the pattern and exit the dialog box.
Your drawing should look like this.

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Use R-PATTERN again to create a nonorthogonal rectangular pattern with
included spacing and a value entered for the angle.
In the Browser, right-click the icon for the pattern you just created, and
choose delete. Verify that the R-PATTERN part is activated.
To create a nonorthogonal rectangular pattern
1 Use AMPATTERN to create a nonorthogonal rectangular pattern, responding
to the prompts.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Rectangular Pattern.

Select features to pattern: Specify the hole
Select features to pattern or [liSt/Remove] : Press ENTER
2 In the Pattern dialog box, in Column Placement, select Included, the second
button from the left. Specify:
Instances: Enter 3
Angle: Enter 60
Spacing: Angle: Enter 1
In Row Placement, select Included, and specify:
Instances: Enter 2
Spacing: Enter .75

Choose OK.
The hole pattern is created at a 60-degree angle from the side of the part.

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Next, create a full circle polar pattern using a work axis as the center and a
specified number of instances. When you choose a different pattern type, the
appropriate options are displayed in the Pattern dialog box.
Activate P-PATTERN_1 and zoom to the part.

The part is constructed with a circular plate and two holes.
To create a polar pattern
1 Use AMPATTERN create a polar pattern, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Polar Pattern.

Select features to pattern: Specify Hole2
Enter an option [Next/Accept] : Press ENTER
Select features to pattern or [liSt/Remove] : Press ENTER
Valid selections: work point, work axis, linear edge, cylindrical edge/face
Select rotational center: Specify the work axis
2 In the Pattern dialog box, specify:
Polar Placement: Choose Full Circle
Instances: Enter 5

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Choose Preview and view the pattern. Then choose OK.

Next, make one instance of the pattern independent and then alter it.
To make a pattern instance independent
1 Select the pattern instance to make independent.
Browser

Right-click PolarPattern, and choose Independent
Instance.

Respond to the prompts.
Select feature pattern or array instance: Select hole instance #4
An independent hole based on a work point is copied from the selected hole
instance. Dependent features are maintained and copied with the pattern
instance.
Icons for the work point and independent Hole3 are displayed in the
Browser.

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The previous hole instance is suppressed. It can be reclaimed using the
Pattern dialog box.
2 Use AMEDITFEAT to resize the independent pattern instance.
Browser

Right-click the independent Hole4, and choose Edit.

The Hole dialog box is displayed.
3 In the Hole dialog box, change the diameter to .4, and choose OK.
4 Use AMUPDATE to update the part, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

The Hole3 is resized, while it maintains its position in the pattern.

You can create axial patterns, and you can create a pattern from another
pattern.
In the Browser, right-click A-PATTERN_1 and choose Activate Part. Rightclick A-PATTERN_1 again, and choose Zoom to. Turn off the visibility of
P-PATTERN_1.

A-PATTERN_1 contains a cylinder with a polar pattern of three holes. In this
exercise, you use this polar pattern to create an axial pattern, specifying a
work axis as the rotation center. You specify the number of instances, and
incremental column and row placement.
After you create the axial pattern, you use it to create another polar pattern.
In the Browser, expand A-PATTERN_1.

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To create an axial pattern
1 In the Browser, under A-PATTERN_1, right-click WorkAxis1 and choose
Visible.
2 Use AMPATTERN to create an axial pattern, responding to the prompts.
Browser

In the Browser, right-click Polar Pattern1 and choose
Pattern ➤ Axial.

Valid selections: work point, work axis, linear edge, cylindrical edge/face
Select rotational center: Specify the work axis
In the Pattern dialog box, in Axial Placement, specify:
Instances: Enter 12
Column Placement: Select Incremental Angle, the button on the left
Spacing Angle: Enter 30
Row Placement: Select Incremental Offset, the button on the left
Offset Height: Enter .2

3 In the Pattern Dialog box, press Preview to view the pattern, then press OK.
The axial pattern is created on the surface of the cylinder. Hide the hidden
lines to see your part better. Because the part is cylindrical, to display silhouette
edges, you set the DISPSILH system variable to 1 first.
4 Change the setting for DISPSILH.
Command

DISPSILH

New value for DISPSILH <0>: Enter 1

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5 Use HIDE to hide the hidden lines.
Desktop Menu

View ➤ Hide

Your part should look like this.

6 Finish the part by using the new axial pattern to create another polar pattern.
Browser

In the Browser, right-click Axial Pattern1 and choose
Pattern ➤ Polar.

Select Rotational Center: Select the work axis
7 In the Pattern dialog box, specify:
Polar Placement: Select Incremental Angle
Instances: Enter 2
Spacing Angle: Enter 180
Choose OK.
8 Use HIDE to hide the hidden lines.
Desktop Menu

View ➤ Hide

Your finished part should look like this.

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Editing Pattern Features
You edit pattern features in the Pattern dialog box. In the Pattern Control
tab, you modify the instancing controls. In the Features tab, you redefine the
features in the pattern. Once a pattern is created, you cannot change the pattern type.
When you delete a feature from a pattern set, you also remove other graphically dependent features that are children of that feature, such as fillets. If
you want to add a feature to the set, a feature rollback is required.
A pattern is associative to the original feature that was patterned. When you
modify the sketch of a patterned feature, you also modify the entire pattern.
Use the Pattern dialog box to preview and redefine the orientation of the distribution plane at any time. If you want to change the distribution plane to
a different plane, a feature rollback is required.
Try editing the rectangular and polar patterns you created in this section.

Editing Array Features
Although you cannot create a new array, you can edit a previously-created
array by editing the dimensions and instance constraints of the array using
command line prompts. There is no dialog box available for editing arrays.
Pre-existing array features cannot be migrated to pattern features.
The following procedure is available only when you open a drawing file that
contains a previously-created array.
To edit a previously-created array
9 Use AMEDITFEAT to edit a previously created array, responding to the
prompts.
Context Menu

Right-click the graphics area and choose Edit Features ➤
Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select
Feature] : Enter s
Select sketched feature: Specify the extrusion
2 Modify the height of the sketch, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Edit Dimension.

Select dimension to change: Select the 0.20 dimension (1)
New value for dimension <.20>: Enter .12
Solved fully constrained sketch.
Select dimension to change: Press ENTER

3 Use AMUPDATE to update the model, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Update Part.

Your part is updated according to the changed dimension and looks like this.

Save your file.

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263

Creating Work Features
Now that you have created the base feature, add the feature that defines the
rough shape of the bracket. First, create work features to maintain symmetry.
Then, use them to draw, constrain, and extrude the sketch.
The first work feature is a work axis along the centerline of the arc on the base
feature. This work axis anchors your next sketch to the base feature.
To create a work axis
1 Use AMWORKAXIS to create the work axis, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Axis.

Select cylinder, cone or torus [Sketch]: Specify the cylindrical face (1)

The work axis is displayed as a line along the center of the arc.

work axis

If the work axis is not visible, the work axis display is probably turned off.
2 To turn on the display, in the Browser right-click Work Axis1. Choose Visible.
The next work feature, the work plane, forms the second axis of symmetry.
This plane is parallel to the front face and intersects both lugs. You specify
the work plane position as parallel to the selected face and offset one-half the
depth of the part.

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work plane

To locate the work plane parametrically, specify the offset depth as an equation. By using an equation, the work plane tracks changes in the bracket
width and always remains centered. To use an equation, you must determine
the dimension parameter before you define the work plane.
To create a work plane
1 Use AMDIMDSP to set dimensions as equations.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ Dimensions as Equations.

2 Redisplay the sketch dimensions, following the prompt.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] :
Press ENTER
Select Edges: Specify the circular lug
Select Edges: Press ENTER
In the Edge Properties dialog box, choose Color.
In the Select Color dialog box, select red, and press ENTER.
Choose OK to close the Edge Properties dialog box.
Choose OK to close the Edit Drawing View dialog box.

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The lug color in the detail view changes to red. However, the lug color
remains unchanged in the parent view.
For practice, create the same detail view using a circle for selection. Notice
how the command line prompts change according to the selection type you
use.
Next, you create a cross section—a view that cuts through a point on the part
along a work plane, or if the part is an offset section, through a sketch. Work
planes are often easier to visualize and select than cutting planes.
If you choose not to create a work plane, you will find it easier to select only
the endpoints of edges and the centers of circles or arcs to specify a cutting
plane.
In this tutorial, you will create a work plane for the cross-section view, using
an axis and an existing work plane.
To create a cross-section and isometric view
1 Return to Model mode.
Browser

Select the Model tab.

2 Use AMWORKPLN to create a work plane for the cross-section view.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:
1st Modifier: On Edge/Axis
2nd Modifier: Planar Normal
Create Sketch Plane: Clear the check box
Choose OK.

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3 On the command line, respond to the prompts as follows.
Select work axis, straight edge or [worldX/worldY/worldZ]:
Specify the work axis (1)
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Specify the work plane (2)

2
1

Your model should now look like this.

Next, you create a full cross-section view of the part that is an orthographic
projection of the front view.
4 Return to Drawing mode.
Browser

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Select the Drawing tab.

Chapter 13 Creating Drawing Views

5 Create a new drawing view.
Context Menu

In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:
View Type: Ortho
Choose the Section tab and specify:
Type: Full
Label: Enter A
Label Pattern: Section A-A
Hatch: Select the check box, and press Pattern
Use the Hatch Pattern dialog box to define the hatch pattern, and choose OK.
Choose OK to close the Create Drawing View dialog box.
6 Define the orthogonal view, responding to the prompts.
Select parent view: Specify a point anywhere inside the front view
Specify location for orthogonal view:
Specify a point to the right of the front view (3)
Specify location for orthogonal view: Press ENTER
Enter section through type [Point/Work plane] :
Press ENTER
Select work plane in parent view for the section:
Select the edge of the second work plane at a point inside the view box (4)

4
3

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319

Your display should now look like this.

7 Create an isometric view, using the base view as the parent view.
Context Menu

In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:
View Type: Iso
Scale: Enter 1
Relative to Parent: Select the check box
Choose OK.
8 Define the isometric view, responding to the prompts.
Select parent view: Specify the base view (1)
Location for isometric view: Specify a point to the right of the top view (2)
Location for isometric view: Press ENTER

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Your drawing should look like this.

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321

Each drawing view is represented as it relates to other views. For example, the
ortho, section, and iso views are derived from the base view. Also, it is clear
that the detail view is based on the ortho view. Detail and section views are
named according to the labels you specified.

Save your file.

Cleaning Up Drawings
After creating the drawing views, you need to clean up the parametric dimensions and some extraneous lines.
Parametric dimensions are automatically placed on the AM_PARDIM layer.

Hiding Extraneous Dimensions
Because dimensions originate on the model, some might be redundant or
conflict with others. For example, because the saddle bracket is symmetrical,
one dimension states the overall length of a feature while another states the
length of one side. Only one of these dimensions is necessary because the
other can be derived. Decide which dimensions to show, and then selectively
hide the others. Hiding dimensions does not delete them. They can be redisplayed from the Desktop Visibility dialog box.
Other dimensions may be redundant because you created the model by
constructing individual features. For example, when you sketched the arc
that represents the rough saddle form, you specified a radius of .33. This
dimension appears in the top view of the drawing. When you created the
boss, you specified a dimension of .33 to revolve the boss. This dimension
appears in the front view of the saddle bracket. Only one of the .33 dimensions is needed.

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To hide extraneous dimensions in a front view
1 Zoom to the base view.
Context Menu

In the graphics area, right-click and choose Zoom.

2 Activate the Desktop Visibility dialog box.
Desktop Menu

Drawing ➤ Drawing Visibility

In the Desktop Visibility dialog box, verify that the Hide option is selected.
Then choose Select.
3 On the command line, respond to the prompts to select the redundant .33
and .74 dimensions to hide.
Select drawing objects to hide: Specify the 0.33 dimension
Select drawing objects to hide: 1 found
Select drawing objects to hide: Specify the 0.74 dimension
Select drawing objects to hide: 1 found, 2 total
The view also contains a number of dimensions associated with the rib
sketch. The ribs were created from a trapezoid shape, where only two of the
sides are used by the part. The other sides are not visible, so their dimensions
should not appear in the drawing.
Select drawing objects to hide: Specify the 1.00 dimension
Select drawing objects to hide: 1 found, 3 total
Select drawing objects to hide: Specify the 0.50 dimension
Select drawing objects to hide: 1 found, 4 total
Select drawing objects to hide: Specify the 14° dimension
Select drawing objects to hide: 1 found, 5 total
Select drawing objects to hide: Press ENTER
Choose OK to exit the dialog box.

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4 Your display should look like this.

In the top view, the 1.16 dimension specifies the distance between arc centers. You can hide the extraneous .58 and 0.08 dimensions.
To hide extraneous dimensions in a top view
1 Zoom to the top view.
Browser

Right-click Ortho and choose Zoom to.

2 Activate the Desktop Visibility dialog box.
Desktop Menu

Drawing ➤ Drawing Visibility

3 In the Desktop Visibility dialog box, verify that the Hide check box is selected
and choose Select.
4 Respond to the prompts as follows.
Select drawing objects to hide: Specify the 0.58 dimension
Select drawing objects to hide: Specify the 0.08 dimension
Select drawing objects to hide: Press ENTER
Choose OK to exit the dialog box.
The dimensions should be hidden on the view.

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Moving Dimensions
Mechanical Desktop places dimensions on the drawing according to the way
they were created during sketching. Usually, some cleanup is required, to
comply with drafting standards.
In the following exercises, you will move dimensions within and between views
until all the dimensions needed to define the part are visible on the drawing.
All the dimensions for the drawing currently exist in the front and top views.
Originally these views were cluttered with extraneous dimensions. Now that
those dimensions are gone, it is much easier to move the remaining dimensions to other views.
To move a dimension within a view
1 Zoom to the base view.
Browser
.

Right-click Base and choose Zoom to.

2 Use AMMOVEDIM to move some dimensions to clean up your view, following
the prompts.
Context Menu

In the graphics area, right-click and choose Annotate
Menu ➤ Edit Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] : Press ENTER
Select dimension to move: Specify the 1.48 dimension (1)
Select destination view: Specify a point near the center of the front view (2)
Select location: Specify a point slightly below the A for the section cut (3)
Select location: Press ENTER
Press ENTER to repeat the command.

1
3

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3 Continue moving dimensions until the front view looks like this.

4 Zoom to the top view.
Browser

Right-click Ortho and choose Zoom to.

5 Use AMMOVEDIM to move some of the dimensions in the top view.
Context Menu

In the graphics area, right-click and choose Annotate
Menu ➤ Edit Dimensions ➤ Move Dimension.

Follow the command line prompts to move dimensions until your view
looks like this.

Because dimensions are placed on the first true-size view of the part, most
dimensions clutter the first few views you create. In this exercise, you move
a dimension from the front view to its cross-section view.
6 Zoom to return to the drawing layout.
Context Menu

326

In the graphics area, right-click and choose Zoom. Rightclick again, and choose Zoom Extents. Right-click again
and choose Exit to close the command.

Chapter 13 Creating Drawing Views

To move a dimension to a different view
1 Zoom in to view the front and cross-section views.
Context Menu

In the graphics area, right-click and choose Zoom.

2 Use AMMOVEDIM to move a dimension from the front view to the crosssection view, following the prompts.
Context Menu

In the graphics area, right-click and choose Annotate
Menu ➤ Edit Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] : Press ENTER
Select dimension to move: Specify the 0.78 dimension (1)
Select destination view: Specify the cross-section view (2)
Select location: Place the dimension to the left of the cross-section view (3)
Select location: Press ENTER

1
3

Your drawing views should look like this.

Cleaning Up Drawings

327

Hiding Extraneous Lines
Although Mechanical Desktop eliminates lines when it creates views, you
may want to edit the views to remove additional, unwanted lines.
To hide an extraneous line
1 Zoom to the isometric view.
Browser

Right-click Iso and choose Zoom to.

2 Use AMEDITVIEW to edit the Iso view.
Context Menu

In the graphics area, right-click and choose Drawing
Menu ➤ Edit View.

3 Specify the isometric view.
4 In the Edit Drawing View dialog box, choose the Display tab and then choose
Edge Properties.

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5 On the command line, respond to the prompts as follows:
Enter an option (edge properties) [Remove all/Select/Unhide all] : Enter a

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Your drawing should look like this.

Next, hide the extraneous dimensions.

Hiding Extraneous Dimensions
When drawing views are created, Mechanical Desktop displays all the parametric dimensions that are related to the part display in each view. Usually,
some cleanup is required because of overlapping or redundant dimensions.

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385

To hide an extraneous dimension in a base view
1 Use AMVISIBLE to hide extraneous dimensions.
Desktop Menu

Drawing ➤ Drawing Visibility

In the Desktop Visibility dialog box, choose Select.

NOTE If you choose the toolbutton method to hide the dimensions, the
Desktop Visibility dialog box is not displayed. Select the dimensions to hide. Use
Zoom Realtime while selecting the dimensions.
2 Respond to the prompts as follows:
Select drawing objects to hide:
Select drawing objects to hide:
Select drawing objects to hide:
Select drawing objects to hide:
Select drawing objects to hide:

Specify the d1+d2 dimension (1)
Specify the ab dimension (2)
Specify the tb dimension (3)
Specify the tb dimension (4)
Press ENTER

1,4
3

In the Desktop Visibility dialog box, choose OK.

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To hide a dimension in an orthographic view
1 Use AMVISIBLE to hide dimensions.
Desktop Menu

Drawing ➤ Drawing Visibility

2 In the Desktop Visibility dialog box, choose Select.

NOTE If you choose the toolbutton method to hide the dimensions, the
Desktop Visibility dialog box is not displayed. Select the dimensions to hide.
3 In the side ortho view, hide the db dimension, the two db/2 dimensions, and
the db/4 dimension.
You do not need to hide dimensions in the bottom ortho view.
The ortho views should look like this.

side view

bottom view

Now that the extraneous dimensions are hidden, it is easier to move the
remaining dimensions for clarity.

Moving Dimensions
Because several of the remaining dimensions overlap, you need to rearrange
them so that they are easy to view.

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387

To move a dimension
1 Use AMMOVEDIM to move the parametric dimensions in the base view,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit
Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] : Press ENTER
Select dimension to move: Select the dimension for the long leg of the bracket (1)
Select destination view: Specify a point in the base view (2)
Select location: Specify a point to the right (3)
Select location: Press ENTER

1
2

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2 Continue moving dimensions until your base view looks like this.

3 Move the dimensions in the ortho views.
The ortho views should look like this.

side view

bottom view

Next, add reference dimensions, to fully define the part.

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389

Enhancing Drawings
To finalize the presentation of the drawing, you add power dimensions, displayed as parameters and create a hole note to describe the three holes in the
bracket.

Creating Power Dimensions
The drawing views are intended to display the generic part. When you display parametric dimensions using design variables, and you power dimension your drawing views, the views represent the generic part.
Because reference dimensions are not displayed as parameters, you use power
dimensioning to create dimensions represented as parameters. Power dimensioning allows you to specify tolerance and fit information for your parts as
you dimension and to modify the default value of a dimension as you create it.
Later, when you paste the spreadsheet into the drawing, you will have a list
of values for the variables in each version that cross-references the dimensions in each view.
To add a reference dimension
Before you begin this procedure, enable Osnaps. If Osnaps are set to off, you
will be unable to create the dimension. Work in the base view.
1 Use AMPOWERDIM to create power dimensions, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Power
Dimensioning.

(Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/
Update] : Press ENTER
Select arc, line, circle, or dimension: Specify the arc
Enter an option [Next/Accept} : Press ENTER
Specify dimension line location or [Linear/Diameter/Options]:
Specify a location for the dimension
(Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/
Update] : Press ENTER
Select part and subassembly instances: Select PLIERB
Select part and subassembly instances: Press ENTER
2 In the Assembly Mass Properties dialog box, select the Setup tab and specify:
Input units: US Customary (in, lbm)
Output units: US Customary (in, lbm)
Coordinate system: User coordinate system (UCS)
Display Precision: Enter 2.0
Part List: Select PLIERB
Materials available: Select Mild_Steel.

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419

3 Select the Results tab. The results window for PLIERB remains empty until
you calculate the results.
4 Choose Calculate. Message dialogs appear warning that density is not specified for the other parts in the assembly. Choose OK to proceed.
Mass properties are calculated according to the values you set.

Choose Done.

NOTE You can save mass properties calculations to a file to use in design analysis,
and you can export the results.
Next, you create scenes of the assembly.

Creating Assembly Scenes
Now that you have instanced the parts and applied the assembly constraints,
you can create and lay out assembly scenes. A scene is an exploded view that
separates the parts of an assembly or subassembly to show how they fit
together. You can create a scene quickly; it updates automatically every time
you change the assembly. The separation of the parts is based on an explosion factor you set and the assembly constraints you used to position the
parts. You can create multiple exploded scenes of the same assembly and save
them for later use.

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Assembly trails indicate the path of the assembly explosion. With the exception of the grounded part, assembly trails can be created for all parts. When
you create assembly trails, a new layer is automatically created for them. You
can automatically create trails when you create tweaks.
First, you set an explosion factor and then create an exploded assembly
scene. Then you add trails to show how parts are assembled. From a scene,
you create drawing views.
To create an exploded view
1 Use AMNEW to create a new scene.
Context Menu

In the graphics area, right-click and choose New Scene.

The Create Scene dialog box is displayed.
2 In the Create Scene dialog box, specify:
Target Assembly: S_PLIER
Scene Name: SCENE1
Auto Explode: Scene Explosion Factor: 1.5
Synchronize Visibility with Target Assembly: Select the check box

Choose OK.
The exploded assembly scene is displayed. Its name is shown below the command line. The Browser shows all parts in the scene.

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421

Next, align the exploded parts in the assembly scene. You can tweak the position and orientation of individual parts or rotate them for better visibility.
In the Browser, verify that the Scene tab is selected. Unless the scene is activated, you cannot tweak parts to adjust their position or add trails to show
how they are assembled.
To align scene parts
1 Use AMTWEAK to move the HEXNUT part closer to the other parts, responding to the prompt.
Context Menu

In the graphics area, right-click and choose New Tweak.

Select part or subassembly to tweak:

Select HEXNUT (1)

2 In the Power Manipulator dialog box, on the General tab, verify that Place
Objects (ALT) is selected.

Choose Done.
The Power Manipulator dialog box is displayed automatically only the first
time you create a new tweak. After that, to access the Power Manipulator
dialog box, right-click the Power Manipulator symbol on your screen, and
select Options.
3 Continue on the command line.
Select handle or Geometry
[undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] :
Enter z
Enter tweak distance [Rotate]<1.0000>: Enter .25
Select handle or Geometry
[undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] :
Press ENTER.

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The HEXNUT position is tweaked by the specified distance.

NOTE The grounded part of an assembly or subassembly cannot be tweaked.
Its position is fixed.
4 Use AMTRAIL to show the direction of the explosion and tweak paths,
responding to the prompt.
Context Menu

In the graphics area, right-click and choose New Trail.

Select reference point on part or subassembly: Select the end of HEXBOLT (1)

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423

5 In the Trail Offsets dialog box, specify:
Offset at Current Position: Distance: Enter 1
Over Shoot: Select the option
Offset at Assembled Position: Distance: Enter 1
Over Shoot: Select the option

Choose OK.
The assembly trail for HEXBOLT is displayed.

6 Apply assembly trails to the PLIERB and HEXNUT parts, responding to the
prompt.
Context Menu

In the graphics area, right-click and choose New Trail.

Select reference point on part or subassembly:
Select the outside hole of HEXNUT (2)

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7 In the Trail Offsets dialog box, specify:
Offset at Current Position: Distance: Enter 1
Over Shoot: Select the option
Offset at Assembled Position: Distance: Enter 1
Over Shoot: Select the option
Choose OK.
The assembly drawing automatically updates the current scene to reflect the
tweaks and assembly trails.

Save your file. Choose OK in the External Part Save dialog box to bring all
parts up to date.
Next, you create drawing views of the assembly scene.

Creating Assembly Drawing Views
After you complete the assembly model and the scene, you can create 2D
orthogonal views or 3D isometric and exploded views of the entire assembly.
Then you add reference dimensions.
You can set up as many drawing layouts as you need to document your
design. Because this assembly is small, you create only one layout.
Before creating the base view of the pliers assembly, modify a plotter setup to
include a custom paper size. Then set up the drawing layout to arrange the
drawing views on paper.

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To add a custom paper size to a plotter setup
1 Use AMMODE to switch to Drawing mode.
Browser

Choose the Drawing tab.

2 Add a custom paper size to an existing plotter.
Browser

Right-click Layout1 and choose Page Setup.

3 In the Page Setup dialog box, select the Plot Device tab and specify:
Name: DWF Classic.pc3

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4 Choose Properties.
5 In the Plotter Configuration Editor dialog box, expand User-Defined Paper
Sizes and Calibration. Select Custom Paper Sizes and choose Add.

6 Use the Custom Paper Size Wizard to define a paper size of 18 x 12 inches
with no indents. Choose Next until the setup is finished.
7 Save your changes to the DWF Classic.pc3 file.
Next, you set up the drawing layout and insert a title block.

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To set up a drawing layout
1 In the Page Setup dialog box, select the Layout Settings tab and specify:
Paper Size: User 1 (18.00 x 12.00 inches)
Plot Scale: 1:1
Choose OK.
2 Use MVSETUP to insert a title block.
Browser

Right-click Layout1 and choose Insert Title Block.

In the AutoCAD text window, respond to the prompt as follows:
Enter number of title block to load or [Add/Delete/Redisplay]: Enter 8
3 Continue on the command line.
Create a drawing named ansi_b.dwg? : Enter n
Enter an option [Align/Create/Scale viewports/Options/Title block/Undo]:
Press ENTER
The title block is inserted into the drawing.
4 Use MOVE to center the title block in the layout, responding to the prompts.
Desktop Menu

Modify ➤ Move

Select objects: Select the title block
Select objects: Press ENTER
Specify base point or displacement: Specify a point
Specify second point of displacement or :
Specify another point

Next, define drawing views to display the assembly.

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To create a base assembly drawing view
1 Use AMDWGVIEW to create a base view.
Context Menu

In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:
Type: Base
Data Set: Scene: SCENE1

Choose OK.
2 Respond to the prompts as follows:
Select a planar face, work plane, or [Ucs/View/worldXy/worldYz/worldZx]:
Enter z
Select work axis or straight edge [worldX/worldY/worldZ]: Enter x
Adjust orientation [Flip/Rotate] : Press ENTER
Specify location of base view: Specify a point
Specify location of base view: Specify another point or press ENTER

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The base drawing view is displayed.

Next, create an isometric view of the assembly.
To create an isometric assembly drawing view
1 Create an isometric view.
Context Menu

In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:
View Type: Iso
In the Hidden Lines tab, specify:
Calculate Hidden Lines:
Choose OK.

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Clear the check box

2 Respond to the prompts as follows:
Select parent view: Specify the base view
Specify location for isometric view: Specify a point to place the isometric view
Specify location for isometric view: Specify another point or press ENTER

Examine the Browser. The views are nested under a Scene icon which is
nested under Layout1.
Save your file.
Now you can add reference dimensions, which can be moved, frozen, and
thawed in each drawing view. Reference dimensions are not parametric, but
they update when the model changes.

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To add a reference dimension
1 Zoom in to enlarge the area you want to dimension.
Context Menu

In the graphics area, right-click and choose Zoom.

2 Use AMREFDIM to add a reference dimension, following the prompts.
Context Menu

In the graphics area, right-click and choose Reference
Dimension.

Select first object: Select the endpoint of the pliers (1)
Select second object or place dimension: Select the bolt (2)
Specify dimension placement: Specify a point above the pliers
Specify placement point or [Undo/Hor/Ver/Align/Par/aNgle/Ord/reF/Basic]:
Press ENTER
Select first object: Press ENTER

The reference dimension is added to the current view.

Save your file.
Now that you have created drawing views, you edit a part and automatically
update the drawing views.

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Editing Assemblies
Design or specification changes require most assembly designs to be documented and edited frequently. You modify parts, rearrange parts and features
in the hierarchy of the assembly tree, and change or delete constraints.
Because the parts and assembly are parametric, changes are fast and updates
are immediate.
Editing an external part definition automatically changes the assembly
model wherever the part is instanced.

Editing External Subassemblies
The process for editing external subassemblies and combined parts is much
like the one for editing external parts. To begin, you activate the subassembly
by double-clicking it in the Browser or entering information on the command line. When external files are active in the ref-edit state, they are not
available for simultaneous use by others.
The active subassembly retains its color on the screen, while other geometry
is dimmed. Non-active instances of the active subassembly dim one-half as
much. This indicates which instance is active and reflects all of the instances
that will be updated as a result of the change.
When active, you can edit the subassembly. The editing operations take place
as if the active subassembly was an open document. You alter subassemblies
by adding or removing components, changing constraints, adding new features, or restructuring the assembly. Newly created non-part based geometry
such as surfaces and wires are created in the master assembly until made part
of a component.
You can save your changes to an external subassembly file in several ways.
■
■
■
■

Use an option in AMUPDATE to commit the changes to the external file.
Activate a part or subassembly that is contained in another file and, in the
resulting dialog box, commit to changes.
Activate another subassembly that is external to the active subassembly.
Save the assembly and choose either to not save changes or to save the
pending changes to any external files.

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Editing External Parts
To update all instances of a part in assemblies, you need to edit the original
part. You alter part features by changing dimensions, changing the
constraints, or adding new features. The changes take effect in the assembly.
In this tutorial, you edit the external PLIERT part from within your assembly
drawing. This is called editing in place. In the following steps, you add another
hole to the PLIERT part, and modify assembly constraints.
To edit an external part in place
1 Use AMMODE to return to Model mode.
Browser

Select the Model tab.

2 Use AMACTIVATE to activate the PLIERT part.
Context Menu

In the graphics area, right-click and choose Part ➤
Activate Part.

The inactive parts are grayed out in the Desktop Browser, and dimmed on
screen.

By dimming the inactive parts, it is easier for you to work on the active external part without moving other parts.
3 Notice the red lock preceding the PLIERT icon in the browser. This indicates
that the file has been locked and cannot be modified by another user.

NOTE For clarity, the visibility of the other parts has been turned off in this section. If you prefer, turn off the visibility of PLIERB, HEXBOLT, and HEXNUT before
you activate PLIERT.

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4 Zoom in on PLIERT.

5 Use AMSKPLN to create a new sketch plane, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Sketch
Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Make sure the front face of the part is highlighted, and press ENTER
Plane=Parametric
Select edge to align X axis or [Z-flip/Rotate] :
Make sure the UCS icon is upright and the Z axis points away from the part,
and then press ENTER

The sketch plane is defined on the front face of the pliers. Now, create the
new slip hole to increase movement of the slip pliers.

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435

To create a new feature on an external part
1 Use CIRCLE to place a new hole, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Circle.

CIRCLE Specify center point for circle or [3P/2P/Ttr (tan tan radius)]:
Select a point near the existing hole
Specify radius of circle or [Diameter]:
Draw a circle approximately the same size as the other hole

2 Use AMPROFILE to solve the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving ➤
Single Profile.

Mechanical Desktop indicates that three dimensions are required to fully
constrain the sketch.
3 Use AMPARDIM to add the parametric dimensions, responding to the
prompts. Zoom in as needed to magnify the holes.

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Context Menu

In the graphics area, right-click and choose Dimensioning ➤
New Dimension.

Select first object: Select the circle (1)
Select second object or place dimension:
Specify a point for the location of the dimension (2)
Enter dimension value or [Undo/Radius/Ordinate/Placement point]
<0.2003>: Enter .22
Solved underconstrained sketch requiring 2 dimensions or constraints.
Select first object: Select the circle (1)
Select second object or place dimension: Select the existing extruded hole (3)
Specify dimension placement: Specify a point for the location of dimension (4)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.0454>: Enter 0
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Select the circle (1)
Select second object or place dimension: Select the top line on PLIERT (5)
Specify dimension placement: Specify a point for the location of dimension (6)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.5093>: Enter .45
Solved fully constrained sketch.
Select first object: Press ENTER
The circle is now constrained.
5
4
3
6

1
2

4 Use AMEXTRUDE to extrude the new hole through the pliers.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Termination: Through
Operation: Cut

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437

Choose OK to exit the dialog box.
The new hole is extruded, and its position is constrained to the original hole.

Save your file.
5 The External Part Save dialog box indicates a change in the PLIERT drawing.
Choose OK to save the changes you have made.

new bolt hole

The Browser returns to normal. The inactive parts are no longer dimmed, and
the assembly reflects the new PLIERT part.

Editing Assembly Constraints
Using the Browser, you can selectively delete, edit, and add constraints to
realign or change relationships of parts.
Use MOVE to reposition the parts as you edit and add constraints. If you do
not want the parts to reassemble throughout editing, set AMAUTOASSEMBLE
to 0 (off). To reassemble parts after you add a constraint, select the Update
icon on the Desktop Browser.

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To delete an assembly constraint
1 In the Desktop Browser, click the plus sign on PLIERB_1 to expand the hierarchy. Select the Assembly filter at the bottom of the Browser to filter out all
information except the assembly constraints.

2 In the Browser, click the plus sign on HEXBOLT_1 to expand the hierarchy.
Right-click the Mate ln/ln constraint of HEXBOLT_1, and choose Delete.
3 Delete the Mate pl/pl constraints of HEXBOLT_1.
4 Delete constraints for PLIERB, PLIERT, and HEXNUT.
5 Use MOVE to separate the parts to apply the new constraints.
Context Menu

In the graphics area, right-click and choose 2D Sketching ➤
Move.

Next, you apply new assembly constraints. You use an insert constraint to
align HEXBOLT to the new hole along their axes while mating the face of
PLIERT and the corresponding face of the bolt head.
Use the DOF symbol to illustrate how many rigid body degrees of freedom
are eliminated for each part.

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439

To apply an assembly constraint
1 Use AMINSERT to constrain PLIERT_1 and HEXBOLT_1, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose 3D
Constraints ➤ Insert.

Select first circular edge: Select the new bolt hole of PLIERT (1)
First set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward HEXBOLT, and press ENTER
Select second circular edge: Select the bolt shaft near the head (2)
Second set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward PLIERT, and press ENTER
Enter offset <0.0000>: Press ENTER

The bolt is now inserted through the new hole.

Now you can align the new hole in PLIERT and the corresponding hole in
PLIERB along their axes.

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2 Use AMINSERT to constrain PLIERB and PLIERT, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 3D
Constraints ➤ Insert.

Select first circular edge: Select the new bolt hole of PLIERT (3)
First set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward PLIERB and press ENTER
Select second circular edge: Select the hole on the inner face of PLIERB (4)
Second set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward PLIERT and press ENTER
Enter offset <0.0000>: Press ENTER

The PLIERB and PLIERT parts are constrained to each other on the inside face
and along the axes of the lower hole of PLIERT and the single hole of PLIERB.
Transactional degrees of freedom are solved. In this case, you want to allow
the pliers and hexbolt to rotate on the axes, so you leave the rotational
degree of freedom unsolved.

3 Use AMINSERT to constrain the facing planes of HEXNUT and PLIERB at the
bolt holes, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 3D
Constraints ➤ Insert.

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441

Move parts so you can easily see selection points.
Select first circular edge: Select the bolt hole on PLIERB (5)
First set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward HEXNUT and press ENTER
Select second circular edge: Select the hole on HEXNUT (6)
Second set = Plane/Axis
Enter an option [Clear/Flip] :
Flip the direction arrow toward PLIERB and press ENTER
Enter offset <0.0000>: Press ENTER

The PLIERB and PLIERT parts are constrained on their facing planes. The bolt
passes through both parts, and the holes and bolt shaft are aligned along
their axes.

4 Check that the parts are assembled correctly.
Desktop Menu

View ➤ 3D Views ➤ Top

5 Return to the isometric view.
Desktop Menu

View ➤ 3DViews ➤ Front Right Isometric

Save your file.

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Combining Parts

In This Chapter

This Autodesk® Mechanical Desktop® tutorial builds on
the part and assembly modeling techniques that you

■ Working in Single Part mode
■ Changing part definitions
■ Combining and intersecting

learned in previous chapters. In this chapter, you create
a part and combine toolbodies with it, using parametric
Boolean operations such as cut, join, and intersect, to

parts
■ Creating toolbody and nested

toolbody parts
■ Reducing weight parametrically

construct a single part. You also learn how the display of
complex parts is organized in the Desktop Browser.
In this tutorial, you work in Single Part mode to create a
complex part to be used as a component for an off-road
vehicle. You build the part by combining several
toolbodies with a base part.

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Key Terms
Term

Definition

base part

The active part where toolbody parts are aligned and subsequently combined.

Boolean modeling

combine feature

A parametric feature resulting from the union, subtraction, or intersection of a
base part with a toolbody part.

complex part

A parametric part containing one or more parametric parts as features.

Part Catalog

The means of attaching and cataloging local and external parts in the Part
Modeling environment. Use the All and External tabs to specify contents, which
can be instanced, copied, renamed, replaced, externalized, removed, localized
and sorted.

part definition

Contains information about a part, including its name, geometric data,
specifications, and parameters. If you instance a part multiple times, the
assembly contains only one definition of the part.

part instance

A copy of the part definition. The part instance is inserted into the drawing and
is visible as a solid object on the graphics screen. When a part definition is
changed, so are all of its instances. Part instance names are displayed in the
Desktop Browser.

toolbody

A part that is aligned with the base part and then used to join, intersect, or cut
volume from the base part. In the Part Modeling environment, a part created
after a base part, that automatically becomes an unconsumed toolbody.

toolbody consumption

When a toolbody part is combined with a base part, the toolbody part instance
disappears from the graphics screen and appears as a new combine feature of
the base part in the Desktop Browser.

toolbody rollback

A special option of the AMEDITFEAT command that enables you to change a
toolbody part after it has been consumed as a combine feature.

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Chapter 17 Combining Parts

Basic Concepts of Combining Parts
In Mechanical Desktop® the parametric Boolean capabilities for combining
parts provide a combination of modeling flexibility and convenience. To
combine two parts, you identify which part you want to use as the base part
and make it active. Then, you position the toolbody part on the base part,
using the MOVE or ROTATE command or assembly constraints. You use
AMCOMBINE to cut, join, or intersect the toolbody part with the base part.
You can combine as many toolbodies with a base part as you like, but the
base part and the toolbody must be instances of different parts. In other
words, you cannot combine a part with an instance of itself.
Because the end result is a single part, you can create combined parts in Single
Part mode. If you place more than one part in a part file, the additional parts
automatically become unconsumed toolbodies.
To combine a toolbody with a base part in an Assembly file, both parts must
exist in the same active assembly.
When you create a complex part, the complete definitions of the toolbodies
are stored in the assembly model file. To avoid creating files that are unnecessarily complex, use simple parts as toolbodies. In the following illustration,
the highlighted parts are used to cut a slot. The resultant parts look identical,
but the one created with the complex toolbody part consumes more disk
space. Feature editing operations, such as cutting a slot, take longer.
complex toolbody part

simple toolbody part

With Mechanical Desktop, you can create toolbody parts that contain other
toolbody parts. These are called nested toolbodies. However, you may be able
to achieve the same result without nesting toolbodies.

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445

In the following illustration, the appearance of the part is the same, whether
or not you nest the toolbodies, but the part displayed in the Desktop Browser
on the left is easier to manage and has a less cumbersome display than the
one in the Browser on the right.

To edit CAM_1, on the left, you need to expose only one toolbody. Nested
toolbody parts, like those in the example on the right, usually have more complex constraint systems and require multiple part updates after modification.

Working in Single Part Mode
If you are creating combined parts, you can work in Single Part mode. In a
single part file, you can only have one part definition, but you can work with
more than one part. If you create or externally reference more than one part,
the additional parts become unconsumed toolbodies that you can use to
combine with the first part created in the drawing.

In the Browser above, TOOLBODY1 and TOOLBODY3 are unconsumed.
TOOLBODY2 is consumed, since it has been combined with TOOLBODY1.

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Chapter 17 Combining Parts

Creating Parts
In this tutorial, you create a chassis suspension component for an off-road
recreational vehicle. The part is an axle spacer. You create most of the features
of this part by first creating the basic shape. Then, you create separate parts
that you use as tools to add additional features to the basic shape.
Open the file spacer.dwg in the desktop\tutorial folder. This drawing contains
a fully constrained profile sketch of the basic shape of the axle spacer.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

To create an axle spacer, you begin by extruding the part. First, review the
constraint system for this sketch.
To extrude a part
1 Use AMSHOWCON to check the existing constraints.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

2 Choose All.
Each arc uses the geometric constraints tangent and radius. The upper and
lower outside arcs are aligned using the X Value constraint, and the left and
right outside arcs use the Y Value constraint.
3 Press ENTER.
Because this part is cast aluminum, you must extrude it with a draft angle.
Expand the part hierarchy by clicking the plus icon next to the part name in
the Desktop Browser. The Browser shows an existing part, SPACER, that contains an unconsumed profile.
4 In the Desktop Browser, expand SPACER. Under SPACER, select the Profile1
icon. The sketch is highlighted.

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447

5 Use VIEW to change your viewpoint to a previously saved view.
Desktop Menu

View ➤ Named Views

In the View dialog box, select SPACER_VIEW, and choose Set Current.
Choose OK.
6 Use AMEXTRUDE to extrude the profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Distance: Enter 64
Draft Angle: Enter -2
Termination: Type: MidPlane

Choose OK.
Next, adjust the system settings so that you can hide the silhouette edges of
your part.
To hide silhouette edges
1 Set the AutoCAD system variable that controls the display of silhouette
edges, responding to the prompt.
Command

DISPSILH

Enter new value for DISPSILH <0>: Enter 1

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Chapter 17 Combining Parts

2 Use HIDE to hide the silhouette edges.
Desktop Menu

View ➤ Hide

The spacer has a boss at the bottom and a relief at the top. Next, you use two
part definitions to construct the toolbody parts. You combine those toolbody
parts with the spacer to create the boss and relief.

Creating Toolbody Part Definitions
The shapes of the new toolbody parts are similar to the shape of the spacer
profile. The easiest way to create the toolbodies is to use copies of the spacer
to construct the new toolbody parts. Because you cannot copy a base part
definition in the Part Modeling environment, you use the Part Catalog to
attach a copy of the part to the current drawing as a toolbody definition.
To externally reference a toolbody definition
1 Change the display back to wireframe.
Desktop Menu

View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen

2 Use AMCATALOG to attach the boss.dwg file as a toolbody. This drawing is a
duplicate of the spacer.
Context Menu

In the graphics area, right-click and choose Toolbody
Menu ➤ Catalog.

In the Part Catalog, choose the External tab and select Return to Dialog.
Right-click in Directories, and choose Add Directory.
3 In the Browse for Folder dialog box, select the folder containing your tutorial
drawings. Choose OK.

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449

Because you are working in the Part Modeling environment, Mechanical
Desktop filters the part and assembly drawings in your working directory and
lists only the part files. A thumbnail preview of the part icon precedes the
drawing name. If a part file does not contain features, it is preceded by a red
AutoCAD icon.
4 In the Part Catalog, right-click BOSS and choose Attach.

5 Respond to the prompts as follows:
Specify new insertion point: Specify a point above and to the right of the spacer
Specify insertion point for another instance or : Press ENTER

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Chapter 17 Combining Parts

The Part Catalog is displayed.
6 Choose the All tab. The boss toolbody is listed in External Toolbody Definitions.

Choose OK.
Next, localize and make a copy of the boss toolbody, to create a definition for
the relief toolbody using the Browser shortcut methods.
To localize an external toolbody and copy its definition
1 Localize external toolbody BOSS_1.
Browser

Right-click BOSS_1, and choose All Instances ➤ Localize.

The boss toolbody is localized.
Next, copy the boss toolbody definition to create a relief toolbody.
2 Copy the boss toolbody
Browser

Right-click BOSS_1, and choose Show Definition.

3 In the Part Catalog, choose the All tab. The boss toolbody is listed in Local Toolbody Definitions.
Right-click BOSS, and choose Copy Definition.

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451

4 The Copy Definition dialog box is displayed. In New Definition Name , enter
relief.

Choose OK.
5 Position the instance of the relief toolbody definition to the right of the boss
toolbody, and press ENTER.

The new relief toolbody definition is listed under Local Toolbody Definitions
in the Part Catalog. Choose OK.
Examine the Browser. It contains one part and two unconsumed toolbodies.

Save your file.

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The boss toolbody on the completed spacer follows the profile of the spacer,
but its corners are rounded. The next step is to combine a cylinder with the
boss toolbody.

boss

In the Browser, right-click BOSS_1 and choose Activate Toolbody. Right-click
BOSS_1 again, and choose Zoom To.
To create a cylinder toolbody to combine with the boss toolbody
1 Use AMNEW to create a new toolbody definition, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Toolbody ➤
New Toolbody.

Enter an option [Instance/Part} : Press ENTER
Select an object or enter a new part name :
Enter boss_cylinder and press ENTER
The new toolbody is created, and the toolbody name is added to the Browser.
In the graphics area, right-click and choose Part Menu.
2 Use CIRCLE to create a circle close to the boss toolbody.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
2D Sketching ➤ Circle.

3 Use AMPROFILE to create a profile from the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving ➤
Single Profile.

4 Use AMPARDIM to constrain the profile.
Context Menu

In the graphics area, right-click and choose Dimensioning ➤
New Dimension.

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453

5 Select the circle, and enter a dimension of 86.

6 Use AMEXTRUDE to extrude the profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Distance: Enter 5
Draft Angle: Enter 2
Termination: Type: Blind
Choose OK.
Next, you use assembly constraints to position the cylinder at the bottom of
the BOSS_1 toolbody. Then you use a Boolean intersect operation to combine
the two parts.
To align the cylinder with the boss toolbody, you create two mate-line constraints. Follow the prompts carefully, using the illustrations as your guide to
selecting the correct part edges.
To align a part with a relief toolbody
1 Use AMMATE to create a mate constraint, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Toolbody
Menu ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the bottom edge of the cylinder (1)
First set = Axis, (arc)
Select first set or [Clear/Face/Point/cYcle] : Enter p
First set = Point, (arc)
Select first set or [Clear/aXis/fAce/cYcle] : Press ENTER

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Select second set of geometry: Select the arc (2)
Second set = Axis, (arc)
Select second set or [Clear/fAce/Point/cYcle] : Enter p
Second set = Point, (arc)
Select second set or [Clear/aXis/fAce/cYcle] : Select the arc (3)
Second set = Plane, (arc)
Enter an option [Clear/aXis/Flip/cYcle] : Enter x
Second set = Axis, (arc)
Select first set or [Clear/fAce/Midpoint/cYcle] : Enter m
Second set = Axis, (arc)
Select first set or [Clear/fAce/Midpoint/cYcle] : Press ENTER
Enter offset <0>: Press ENTER

3
2

The center of the cylinder is aligned with the line between the two spacer arc
centers.

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455

2 Use MOVE to move the cylinder for easier selection, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
2D Sketching ➤ Move.

Select objects: Specify the cylinder
Select objects: Press ENTER
Base point or displacement: Specify a point
Second point of displacement: Specify a second point and press ENTER
3 Create the second mate-line constraint, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Toolbody
Menu ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the bottom edge of the cylinder (4)
First set = Axis, (arc)
Select first set or [Clear/fAce/Point/cYcle] : Enter p
First set = Point, (arc)
Select first set or [Clear/aXis/fAce/cYcle] : Press ENTER

Select second set of geometry: Select the arc (5)
Second set = Axis, (arc)
Select second set or [Clear/fAce/Point/cYcle] : Enter p
Second set = Point, (arc)
Select second set or [Clear/aXis/fAce/cYcle] : Select the arc (6)
Second set = Plane, (arc)
Enter an option [Clear/aXis/Flip/cYcle] : Enter x
Second set = Axis, (arc)
Select first set or [Clear/fAce/Midpoint/cYcle] : Press ENTER
Enter offset <0>: Press ENTER

5
6

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The center of the cylinder is aligned with the line between the two boss arc
centers. Together, the two mate constraints position the cylinder at the bottom of the boss. The center of the cylinder is coincident with the center of
the boss.

Now, you are ready to combine the boss toolbody with the cylinder. Because
the boss toolbody will be the base part in the Boolean operation, you need to
make it active.
To create a combine feature
1 Use AMACTIVATE to activate BOSS_1.
Browser

In the Browser, right-click BOSS_1 and choose Activate
Toolbody.

2 Use AMCOMBINE to combine the toolbody and the cylinder, responding to
the prompts.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
Placed Features ➤ Combine.

Enter parametric boolean operation [Cut/Intersect/Join] : Enter i
Select part (toolbody) to use for intersecting: Select the cylinder

Save your file.

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Working with Combine Features
The Desktop Browser now shows that the boss toolbody has a combine feature. The boss cylinder is a toolbody in the combine feature.

The next step is to constrain and combine the boss toolbody with the spacer.
To constrain and combine a toolbody to the base part
1 Use AMACTIVATE to activate the SPACER.
Browser

In the Browser, right-click SPACER and choose Activate
Part.

2 Use AMMATE to apply a mate constraint to the boss toolbody and the spacer,
responding to the prompts.
Desktop Menu

Toolbody ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the top edge of the boss toolbody (1)
First set = Axis, (arc)
Select first set or [Clear/fAce/Point/cYcle] : Enter p
First set = Point, (arc)
Select first set or [Clear/aXis/fAce/cYcle] :
Select the opposite edge of the boss toolbody (2)
First set = Plane, (arc)
Enter an option [Clear/aXis/Flip/cYcle] : Enter x
First set = Axis, (arc)
Select first set or [Clear/fAce/Midpoint/cYcle] : Press ENTER

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1
2

Select second set of geometry: Select the bottom right edge of the spacer (3)
Second set = Axis, (arc)
Select second set or [Clear/fAce/Point/cYcle] : Enter p
Second set = Point, (arc)
Select second set or [Clear/aXis/fAce/cYcle] :
Select the opposite edge of the spacer (4)
Second set = Plane, (arc)
Enter an option [Clear/aXis/Flip/cYcle] : Enter x
Second set = Axis, (arc)
Select second set or [Clear/fAce/Midpoint/cYcle] : Press ENTER
Enter offset <0>: Press ENTER

3
4

3 Move the boss toolbody, and repeat step 2 for the second constraint. Be sure
to select the top edges of the boss toolbody.

1
2
4
3

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459

The boss toolbody is now aligned with the spacer.

4 Use AMCOMBINE to combine the spacer and the boss toolbody, responding to
the prompts.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
Placed Features ➤ Combine.

Enter parametric boolean operation [Cut/Intersect/Join] : Enter j
Select part (toolbody) to be joined: Select the boss toolbody

Save your file.

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Creating Relief Toolbodies
The Desktop Browser now shows a nested toolbody construction. The boss
cylinder toolbody is a combine feature of the boss toolbody, and the boss
toolbody is a combine feature of the spacer.

Next, you create the relief toolbody, to cut material from the spacer.
In the Browser, right-click RELIEF_1 and choose Zoom To.
To add a new toolbody name in the Browser
1 Use AMNEW to create a new toolbody called RELIEF_CYLINDER, responding
to the prompts.
Context Menu

In the graphics area, right-click and choose Toolbody
Menu ➤ Toolbody ➤ New Toolbody.

Enter an option [Instance/Part} : Press ENTER
Select an object or enter new part name :
Enter relief_cylinder and press ENTER
The new part name is added to the Desktop Browser.

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To create a new part
1 Use CIRCLE to draw a circle near RELIEF_1.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
2D Sketching ➤ Circle.

2 Use AMPROFILE to create a profile from the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving ➤
Single Profile.

3 Use AMPARDIM to constrain the profile.
Context Menu

In the graphics area, right-click and choose Dimensioning ➤
New Dimension.

Select the circle, and enter a dimension of 90.
4 Use AMEXTRUDE to extrude the profile.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion Feature dialog box specify:
Termination: Blind
Distance: Enter 10
Draft Angle: Enter 2
Choose OK.
Next, you position the cylinder at the top of RELIEF_1, using assembly constraints just as you did for the boss cylinder. As you select geometry for the
constraints, be sure to select the top edges of both the relief cylinder and the
relief toolbody.
To constrain the toolbodies
1 Use AMMATE for two mate constraints to align the toolbodies.
Desktop Menu

In the Desktop Menu, choose Toolbody Menu ➤ Toolbody
➤3D Constraints ➤ Mate.

first mate constraint

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second mate constraint

result

2 After adding the constraints, use AMACTIVATE to activate RELIEF_1.
Browser

In the Browser, right-click RELIEF_1 and choose Activate
Toolbody.

3 Combine the relief cylinder and the relief toolbody.
Context Menu

In the graphics area, right-click and choose Part Menu ➤
Placed Features ➤ Combine.

4 Choose Intersect, and select the relief cylinder as the toolbody.

Save your file.

Combining Toolbodies with Spacers
In the Desktop Browser, make sure that the relief toolbody has a combine feature and that it contains the relief cylinder toolbody.

In the Browser, right-click SPACER and choose Activate Part.

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To combine a relief toolbody with a spacer
1 Use AMMATE for assembly constraints just as you did to align the relief toolbody with the spacer.
Desktop Menu

Toolbody ➤ 3D Constraints ➤ Mate.

When you combine the spacer and the relief toolbody in step 3, you will cut
the spacer with the toolbody. Therefore, be sure to align the top of the toolbody with the top of the spacer.
After you constrain the relief toolbody, your model should look like this:

2 Use AMCOMBINE to combine the spacer and the relief toolbody.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Combine.

3 Choose Cut, and select the relief toolbody.

Save your file.

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Adding Weight Reduction Holes
The axle spacer is a high-performance chassis component, so its weight must
be kept to a minimum. To achieve this, you cut weight reduction holes into
the part. The manufacturer of the part offers several size spacers with different size weight reduction holes. The use of parametric Boolean operations is
an ideal way to model the part, because it is easy to replace one combine feature with another.
The file spacer.dwg already contains the geometry you need to create a weight
reduction extrusion that cuts material from the middle of the spacer. An
external file contains the part that you will use to remove material from each
of the spacer’s four sides.
First, you attach the external file.
To minimize the weight of a part, using an external toolbody
1 Use AMCATALOG to attach the weight reduction holes toolbody.
Context Menu

In the graphics area, right-click and choose Catalog.

In the Part Catalog, choose the External tab. Clear the Return to Dialog check
box. Right-click WR_HOLES, and choose Attach.
2 Respond to the prompts as follows:
Specify new insertion point: Specify a point to the left of the spacer
Specify insertion point for another instance or Press ENTER

The spacer is created as a midplane extrusion. Therefore, the parting line
appears as a profile that encircles the part at its midsection. When you constrain the weight reduction extrusion to the spacer, you select the partingline geometry.
3 Use AMMATE to constrain the two parts.
Context Menu

In the graphics area, right-click and choose 3D
Constraints ➤ Mate.

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4 Align the axis of one of the reduction extrusion cylinders with a line that
runs through the center points of the spacer arcs. Use the point option when
you define the axis, as you did with previous mate constraints.

5 Use another mate constraint to align the axis of the adjacent weight reduction extrusion cylinder with a line that runs through the center points of the
spacer arcs.

6 Make sure that the spacer is the active part, and use AMCOMBINE to combine the two parts.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Combine.

7 To cut the weight reduction extrusion from the spacer, choose Cut, and select
the weight reduction extrusion as the toolbody.
8 Remove the hidden lines.
Desktop Menu

View ➤ Hide

Save your file.

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The weight reduction holes are very close to the relief cut. For balance, the
holes must remain centered in the spacer. To provide enough material
between the holes and the relief, you need to reduce the depth of the relief
and the diameter of the holes.
To make the change, you edit the nested relief cylinder toolbody and reduce
its extrusion distance.

NOTE When you edit more complex parts, it is sometimes easier to select
commands from menus or toolbars instead of searching for the feature in the
Browser and using the Browser menus.
To center the weight reduction holes
1 Return to wireframe display.
Desktop Menu

View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen

2 Use AMEDITFEAT to recover the relief toolbody, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features ➤
Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select
Feature] : Enter t
Mechanical Desktop recovers the relief cylinder toolbody and displays it in
its constrained position on the relief toolbody.

4 Change the thickness of the relief cylinder, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select
Feature] : Select one of the drilled holes
Enter an option [Accept/Next] : Enter n or press ENTER
The Hole dialog box is displayed.
4 In the Hole dialog box, enter 15 in the Drill Size field. Then choose OK.
5 Repeat steps 3 and 4 for Hole2 and Hole3.
6 Use AMUPDATE to update the edited part.
Context Menu

In the graphics area, right-click and choose Update Part.

The pulley plate reflects the new design.
Save your file.

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Reloading External References
To update the assembly to reflect the changes you made to the external part,
reload the external definition.
To reload an external definition
1 Switch to the window containing the assembly.
2 Use AMCATALOG to reload the PPULLEY definition.
Context Menu

In the graphics area, right-click and choose Catalog.

In the Assembly Catalog, in External Assembly Definitions, right-click
PPULLEY and choose Reload.
Choose OK.
The pulley plate reflects the new design.

redesigned part

If the assembly looks incorrect, choose Assembly ➤ Assembly Update to
update the assembly constraints.
Save your file.
Check the assembly again for interference.

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To check for interference
1 Use AMACTIVATE to activate the SUBPULLY subassembly.
Context Menu

In the graphics area, right-click and choose Assembly ➤
Activate Assembly.

Specify the SUBPULLY subassembly.
2 Use AMINTERFERE to check for interference.
Context Menu

In the graphics area, right-click and choose Analysis ➤
Check Interference.

3 Specify DPULLEY3. No interference should be detected.

Assigning Mass Properties
Next, calculate mass property information. You can analyze parts and assemblies during the course of designing. You may need to optimize weight, maximize stiffness, balance loads, ease assembly, or meet particular requirements.
One mass properties dialog box contains both Setup and Results tabs that
function the same for both parts and assemblies. In this case, the parts list in
the dialog box displays all parts and part properties in the activated assembly
to be analyzed. Item numbers are also displayed if a BOM exists. When you
select an item in the parts list, it is graphically highlighted on the screen.
In these steps, you analyze the bracket and change tolerance values and
material types.
To set up mass properties
1 Activate the PULLYASM assembly.
Context Menu

In the graphics area, right-click and choose Assembly ➤
Activate Assembly.

2 Use AMMASSPROP to analyze the mass properties of the assembly, responding
to the prompt.
Context Menu

In the graphics area, right-click and choose Analysis ➤
Mass Properties.

Select parts or subassemblies: Select the bracket, and press ENTER
The Assembly Mass Properties dialog box is displayed with the Setup tab
active. In the Materials Available window, the materials listed are all of those
defined in the active assembly.

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3 In the Assembly Mass Properties dialog box Setup tab, specify:
Output Units: Metric (mm, g)
Coordinate System: User coordinate system (UCS)
Display Precision: Select 0.00000
Part Name: Select BRACKET
Materials Available: Material: Select Stainless_Steel
Choose Assign Material.
The material information is transferred to the part material attribute and
BOM, and is updated in the part name list.
Next, change the material definition for a part in the assembly.
4 In the Part Name list, select BRACKET, and then select Edit Materials.
5 In the Physical Materials List dialog box Material List, select Stainless_Steel.
In the Properties Window, specify
Density:

8.5

Choose OK.
The new material definition information is transferred to the part, BOM, and
is updated in the Assembly Mass Properties dialog box Part List view.
Choose Done to exit the Assembly Mass Properties dialog box.
You are ready to calculate the mass properties based on the new information
you entered.

Calculating Mass Properties
In the Mass Properties dialog box the Results tab is blank until you use the
Calculate button to retrieve the results of your input in the Setup tab.

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To calculate mass properties
1 In the Mass Properties Dialog Box, select the Results tab. Then select the
Calculate button.
The results are calculated and displayed.

The Calculate button is no longer available because the Setup and Results
fields are in sync. If you change an item on the Setup tab, the results are
cleared and the Calculate button becomes available.
You can use the Insert UCS button to create and insert a user coordinate system (UCS) based on a parts or assemblies center of gravity (CG).
2 Choose Export Results.
In the File dialog box, define a file name and save the file.
This report file can be imported by many external programs.
3 Choose Done to close the Assembly Mass Properties dialog box.
Save your file.
Now, you create an exploded view of the assembly.

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Reviewing Assembly Models
Assembly scenes and drawing views are essential for reviewing the assembly
model. For this lesson, you first create an exploded assembly scene, and then
tweak the positions of parts and add assembly trails and annotations.

Creating Exploded Assembly Scenes
After assembly constraints have been applied to each part, you can create a
scene (an exploded view of the entire assembly). Multiple scenes can be
created and named. You set an explosion factor to determine the separation
of parts in the scene. If you do not want an exploded view in a scene, set the
explosion factor to 0.
Before you begin, select the Scene tab to switch to Scene mode.
To create an exploded assembly scene
1 Use AMNEW to create a new scene, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Scene.

In the Create Scene dialog box, specify:
Target Assembly: PULLYASM
Scene Name: Enter design1
Scene explosion factor <.0000>: Specify 0.0000
Synchronize Visibility with Target Assembly: Select the check box

Choose OK.

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The scene, design1, is displayed.

2 Look at the Browser. The names of all parts in the design1 scene are listed.

Next, align the exploded parts in the assembly scene.

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Using Tweaks and Trails in Scenes
In an exploded scene, sometimes parts obscure other parts. You can use tweaks
to change the positions of individual parts and then adjust the positions of the
parts in the design1 scene. Zoom in to magnify the parts to be tweaked.
In the Browser, tweaks are nested under the respective parts. You can select and
multi-select tweaks in the Browser to delete them. When you pause the cursor
over a tweak in the Browser, a tooltip displays the distance factor for the tweak.

NOTE The grounded part of an assembly or a subassembly cannot be
tweaked. Its position is fixed.
Assembly trails use a continuous or other defined linetype to indicate the
path of the explosion. These trails use assembly constraint information to
visually demonstrate how the assembly design fits together.
To tweak an exploded assembly scene
1 Use AMTWEAK to open the Power Manipulator dialog box.
Context Menu

In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on BUSHING_1 (1)
Enter an option [Next/Accept] : Press ENTER

The Power Manipulator dialog box is displayed only the first time you create
a new tweak.

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In the Power Manipulator dialog box, on the Move tab, verify that Place
Objects (ALT) is selected.

Choose Done.

NOTE To access the Power Manipulator dialog box later, right-click the Power
Manipulator symbol on your screen, and select Options.
2 Use AMTWEAK to tweak the BUSHING part, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on DPULLEY_1 (1)
Enter an option [Next/Accept] : Press ENTER
This time, the Power Manipulator symbol is displayed on the BUSHING part
you selected.
3 Click the -Z axis on the Power Manipulator symbol, drag away from the
assembly, and click at a distance of -150.
4 Continue on the command line.
Select handle or Geometry
[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] :
Press ENTER
The BUSHING is moved away from the assembly. In the Browser, a Tweak
icon is displayed.
1 Use AMTWEAK to tweak the DPULLEY part, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on DPULLEY_1 (1)
Enter an option [Next/Accept] : Press ENTER
2 Click the -Z axis on the Power Manipulator symbol, drag away from the
assembly, and click at a distance of -70.

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3 Continue on the command line.
Select handle or Geometry
[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] :
Press ENTER.
4 Use AMTWEAK to tweak the SHAFT part, responding to the prompts.
Context Menu

In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on SHAFT_1 (1)
Enter an option [Next/Accept] : Press ENTER
The Power Manipulator symbol is displayed on the SHAFT part.
5 Click the -Z axis on the Power Manipulator symbol, drag away from the
assembly, and click at a distance of -200.
6 Continue on the command line.
Select handle or Geometry
[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] : Enter r
Create Trails? [Yes/No] : Enter y
[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] :
Press ENTER
The BUSHING, DPULLEY, and SHAFT part tweaks are displayed with trails.

assembly trail added
tweaked
bushing

tweaked
dpulley

tweaked
shaft

You can adjust assembly trails.

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To adjust assembly trails
1 Use AMTRAIL to adjust your assembly trails, responding to the prompt.
Command

AMTRAIL

The Trail Offsets dialog box is displayed.
2 Use the options in the Trail Offsets dialog box, to adjust over shoots and
undershoots for your trails.

Choose OK to apply your selections.
Next, create an assembly drawing view.

Creating Assembly Drawing Views
An assembly drawing view shows a 2D representation of the 3D assembly.
You use the base part for a base view. Then you create an isometric view of
the entire assembly model. Drawing views are automatically updated when
you change a part or subassembly.
Before you begin, select the Drawing tab to switch to Drawing mode.

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To create a drawing view
1 Use AMDWGVIEW to create a new drawing view.
Context Menu

In the graphics area, right-click and choose New View.

2 In the Create Drawing View dialog box, specify:
Type: Base
Data Set: Scene: DESIGN1
Scale: Enter .03 (or .75 mm)

Choose OK.
3 Respond to the prompts as follows:
Select planar face, work plane or [Ucs/View/worldXy/worldYz/worldZx]:
Enter z
Select work axis, straight edge or [worldX/worldY/worldZ]:
Enter x
Adjust orientation [Flip/Rotate]
Enter r until the UCS icon is upright
Adjust orientation [Flip/Rotate] : Press ENTER
Specify location of base view: Specify a point in the left of the title block
Specify location of base view: Press ENTER

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The base assembly drawing view is displayed.

4 Create an isometric view of the assembly.
Context Menu

In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:
View Type: Iso
Scale: Enter 1
Relative to Parent: Select the check box
Choose OK.
5 Respond to the prompts as follows:
Select parent view: Select the base view
Specify location for isometric view: Specify a point to the right of the base view
Specify location for isometric view: Press ENTER
An isometric view of the assembly is displayed.

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6 Use AMMOVEVIEW to align the views, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Move View.

Select view to move: Select the isometric view
Specify new view location or [Layout]: Align the views and press ENTER

Examine the Browser. The isometric view is listed under the base view.
Now, create a BOM database, and add a parts list and associative balloon callouts.

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Creating Bills of Material
After you have assembled your parts, you can create a bill of material (BOM)
database. This database contains a list of attributes assigned to each part. The
attributes store information such as manufacturer, description, and vendor
part number.
The attributes are contained in part references that are assigned to each part.
Part references can also be created to reference other geometry in your drawing, such as surfaces. The geometry can then be included in a parts list.
The BOM database counts the number of instances in an assembly and tallies
instances for each part. In the BOM table, defined columns can be edited,
added, deleted, moved, and sorted.
By accessing the information in the BOM database, you can add balloons and
insert parts lists into your drawing. You can edit part references, balloons,
and parts lists. The BOM database is automatically updated.
Because the BOM database is fully parametric, any changes to it update the
information stored in balloons, part references, and parts lists.
To create a BOM database
1 Use AMBOM to create the BOM database.
Command

AMBOM

In the BOM dialog box, review the parts in the database.

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Notice the SUBPULLY definition in the list of parts. The plus sign in front of
it indicates that it is a subassembly.
2 Click the plus sign in front of SUBPULLY.
The BOM database now lists all the parts in the assembly, including those in
the subassembly.
Choose OK to exit the BOM dialog box.
3 Select the Model tab in the browser. A BOM icon is located under PULLYASM.

By default, the BOM takes the same name as the assembly file. You can
change this setting by editing the name of the BOM directly in the Browser.
To edit the name of a BOM
1 Using the Browser, rename the BOM database.
Browser

Right-click the BOM icon and choose Rename.

2 Change the name to BOM_1.

Customizing BOM Databases
Mechanical Desktop provides symbol standards for major drafting conventions, including ANSI, BSI, CSN, DIN, GB, ISO, and JIS. By modifying the
symbol standards, you can control the way symbols, balloons, and parts lists
are displayed in the drawing, when you create them.
Next, modify the symbol standards to control the number of columns used
in the parts list and the name of one of the columns.

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To modify symbol standards
1 Use AMOPTIONS to access the Mechanical Desktop symbol standards.
Command

AMOPTIONS

In the Mechanical Options dialog box, expand the hierarchy of ANSI, and
double-click the icon in front of BOM Support.

2 In the BOM Properties for ANSI dialog box, in Columns select Material and
specify:
Caption Alignment: Select the Center Align Text icon
Data Alignment: Select the Center Align Text icon

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Choose Apply, then OK.
The Mechanical Options dialog box is still open.
3 Choose OK to close the Symbol Standards dialog box.
Save your file.

Working with Part References
When you create a BOM database, each part in the assembly is assigned a part
reference. A part reference is an attributed block that can be modified to
include any information you want to attach to the part. That information is
used by the BOM database and included in the parts lists you generate.
Before you begin, in the Browser, select the Drawing tab to switch to Drawing
mode.

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525

To edit a part reference
1 Use AMPARTREFEDIT to edit a part reference, responding to the prompt.
Context Menu

In the graphics area, right-click and choose Annotate
Menu ➤ Parts List ➤ Part Reference Edit.

Select pick object: Select the part reference for BRACKET (1)

2 In the Part Ref Attributes dialog box, double-click in the Name field and enter
Pulley Bracket.
Choose OK.

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3 Use AMBOM to display the BOM database.
Context Menu

In the graphics area, right-click and choose Parts List ➤
BOM Database.

Bom table [Delete/Edit] :

Press ENTER

Notice that Pulley Bracket is now listed under Note for BRACKET.

Choose OK to exit the BOM dialog box.
Next, add balloon callouts to the isometric view.

Adding Balloons
Balloons are used to reference parts in your drawing to a parts list. They contain the same information as the part reference they are attached to. You can
edit that data by selecting balloons. Changes made to the data associated
with a balloon are reflected in the BOM database and the parts list.
You can control the size and appearance of balloons, using the Symbol Standards dialog box.

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527

To place a balloon callout
1 Use AMBALLOON to create balloon callouts for BRACKET, DPULLEY, BUSHING, SHAFT, and NUT3, responding to the prompts.
Desktop Menu

Choose Annotate ➤ Parts List ➤ Balloon.

Select part/assembly or [auTo/autoAll/Collect/Manual/One/ Renumber/
rEorganize]: Enter T
Align [Angle/Standalone/Horizontal/Vertical] : Press ENTER
Select pick object: Select the part reference for BRACKET (1)
Select pick object: Select the part reference for DPULLEY (2)
Select pick object: Select the part reference for BUSHING (3)
Select pick object: Select the part reference for SHAFT (4)
Select pick object: Select the part reference for NUT3 (5)
The objects are aligned after you pick them.

2
3
4

528

Continue on the command line:
Select pick object: Press ENTER
Align Standalone/Horizontal/:
Specify a point between the two drawing views

Next, place the parts list in the drawing.

Placing Parts Lists
A parts list is an associative block of information about your assembly. It displays information about the parts, according to the settings specified in the
BOM database. Because it is parametric, any changes you make to the BOM
database or symbol standards are automatically reflected in the parts list.

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529

To place a parts list
1 Use AMPARTLIST to place the parts list under the base view of your assembly,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Parts List ➤
Part List.

The Parts List dialog box is displayed.
2 In the Parts List dialog box, in Title, enter the new name Pulley Parts List.
3 Choose Apply, then choose OK.
Specify location:

Specify a point under the base view

The parts list is placed in the drawing.

NOTE You may need to move the drawing views to make room for the parts
list. Place the parts list first, and then move the views as needed. Because the balloons are associated with the views, they will also move.

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Chapter 18 Assembling Complex Models

When the parts list is created, a parts list icon is displayed in the Browser.

Save your file.

Finishing Drawings for Plotting
Now that the assembly has been documented, plot the drawing.
Paper drawings are useful for reviewing the entire assembly to make sure that
the design is feasible and can be manufactured. The Parts List on the assembly drawing provides information about the parts needed to manufacture the
assembly. If you wish, add more reference dimensions, fill in the title block,
and add some notes to your drawing before you plot.
This tutorial has demonstrated the flexibility of using subassemblies to create
complex models. Even a complex assembly can be easily modified and documented, if it is truly a parametric assembly.

Finishing Drawings for Plotting

531

532

Creating and Editing
Surfaces

In This Chapter

This Autodesk® Mechanical Desktop®tutorial

■ Creating surfaces—motion

based, skin, and derived
introduces surfaces grouped by function, and provides
instructions for creating the different types of surfaces.

■ Joining and trimming surfaces
■ Editing surfaces

You learn surface types, practice surface modeling, and
work with modeling some typical surfaces.
Once you have completed this lesson, you will
understand the techniques required to surface a more
complex part.

533

Key Terms
Term

Definition

augmented line

A 3D polyline with vector information at each vertex. An augmented line is a
surface creation tool that allows you to control the curvature and the tangency
of a surface.

base surface

A basic underlying surface that carries a shape across a larger area. Can be
trimmed to precise shapes as needed, but the base surface remains intact and
may be displayed.

derived surface

A surface that gets some or all of its attributes from one or more base surfaces.

motion-based surface

A surface created by moving wires through space.

rail

One or more curved lines along which a surface is swept. Rails form the
curvature of a swept surface.

skin surface

The surface draped over a wireframe.

surface normal

A short line perpendicular to a surface that shows where the surface starts and
which direction is out.

surface primitive

Surface created by values you specify. It does not require a wireframe model.

U or V display lines

Lines that correspond to rails and wires.

wire

Generic term for lines, arcs, circles, ellipses, 2D and 3D polylines, augmented
lines, and splines.

wireframe modeling

Wires and surface parts intermixed to construct the basic framework of a 3D
model. The initial step in creating a surfaced model.

wireframe surfacing

Covering a wireframe model with surfaces.

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Chapter 19 Creating and Editing Surfaces

Basic Concepts of Creating Surfaces
Three-dimensional surface modeling can be compared to constructing a
building. You start by establishing the initial shape. Then you cover the
rough framing with siding and roofing.

rough frame

siding applied

One approach to surface modeling is to create a 3D framework of wires. Wire
is a generic term for lines, arcs, circles, ellipses, 2D and 3D polylines, augmented lines, and splines, including splines created from existing part edges.
This framework is called a wireframe.

circle

line

spline

ellipse

polyline

augmented line

Wires and surface parts can be intermixed to construct the framework of your
3D model. This initial step in creating a surfaced model is called wireframe
modeling.
Once the 3D wireframe model is created, the next step is to cover the framework with a surface. This task is called wireframe surfacing. This technique is
one approach to creating surfaces.

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Working with Surfaces
In this tutorial you’ll learn about these types of surfaces:
■
■
■
■

Primitive, created by specifying values
Motion-based, created by moving wires through space
Skin, applied over a wireframe
Derived, generated from existing surfaces

Primitive surfaces (cone, cylinder, sphere, and torus) do not require wireframes for their construction. To create a sphere surface, for example, you
determine the center of the sphere and then enter a value for its radius. Primitive surfaces are most often used for conceptual design.

You can practice creating primitive surfaces on your own by choosing Surface
➤ Create Primitives.
In this tutorial, you’ll practice working with motion-based, skin, and derived
surfaces you create from wireframes. You’ll also work with simple wireframe
geometry to learn surfacing techniques.
After you create each surface, use the Extents option of the ZOOM command
to redisplay all of the wireframes provided in the drawing file. Then zoom to
enlarge the object you need for the next exercise.

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Chapter 19 Creating and Editing Surfaces

To set up your file
1 Open the file t_surfs.dwg in the desktop\tutorial folder. The wireframe objects
you need for this lesson are included in this file.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Surface lines, called U and V lines, indicate the direction of the surface.
Increasing the number of lines increases the density of the surface image.
2 Use the Mechanical Options dialog box to change the number of surface
lines used to display surfaces.
Desktop Menu

Surface ➤ Surface Options

Choose the Surface tab, and in Surface Properties specify:
U Display Wires: Enter 7
V Display Wires: Enter 7
Choose OK.

NOTE If you shade the surfaces you create to better view them, adjust the
AutoCAD setting that controls back faces. Go to Assist ➤ Options and select the
System tab. Choose Properties, then clear the check box for Discard Back Faces.
Choose Apply & Close, then OK.
You are ready to create your first surfaces.

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537

Creating Motion-Based Surfaces
Some surfaces are created by “moving” wires through space. These motionbased surfaces are revolved, extruded, and swept.

Revolved Surfaces
A revolved surface uses two wires: one establishes the constant shape of the
surface, and the other is the axis about which to spin the shape. The revolved
surface is created by the motion of a wire shape through space.
To revolve a surface
1 Use AMREVOLVESF to revolve a spline curve about an axis, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Revolve

Select path curves to revolve: Select spline (1)
Select path curves to revolve: Press ENTER
Specify axis start point or [Wire]: Enter w
Select wire to define axis: Select line (2)
Enter start angle <0>: Press ENTER
Enter included angle (+=ccw, -=cw) : Press ENTER

1
2

The curve revolves about the vertical line.

2 Use the Zoom Extents option of ZOOM to redisplay all the wireframes and
select the object for the next exercise.

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Chapter 19 Creating and Editing Surfaces

Extruded Surfaces
An extruded surface is created by a 3D wire shape moved along a straight line.
You select a line, polyline, arc, or spline to extrude, and you specify the direction and magnitude of the extrusion.
To extrude a surface
1 Use AMEXTRUDESF to extrude a circle into a cylinder, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Extrude

Select wires to extrude: Select circle (1)
Select wires to extrude: Press ENTER
Define direction and length.
Specify start point or [Viewdir/Wire/X/Y/Z]: Enter w
Select wire to define direction: Select line (2) above its midpoint
Enter an option [Accept/Flip] :
Press ENTER to accept the extrude direction
Enter taper angle <0>: Press ENTER to accept the default

1
2

The extrusion direction is determined by your selection point on the wire.
You selected the upper half of the line to extrude the circle along the length
of the line. To extrude the circle in the opposite direction, select a location
below the midpoint of the line.

Creating Motion-Based Surfaces

539

The extruded surface should look like this.

2 For more practice, choose Extrude again. Select the spline and then a location
on the line to determine the length and direction.

Because the line is obscured by the first surface you created, you may have
difficulty selecting it. Press CTRL as you select, to cycle through the objects.
Press ENTER when the line is highlighted.
3 Use the Zoom Extents option of ZOOM to redisplay all the wireframes and
select the object for the next exercise.

Swept Surfaces
A swept surface is a wire cross section moved along a curved line called a rail.
You can use multiple cross sections and one or two rails. The lines on the
swept surface in the illustration are U and V display lines. Cross sections can
be dissimilar but you need to select them in order.
In this exercise, you use different combinations of cross sections and rails to
create four swept surfaces.

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Chapter 19 Creating and Editing Surfaces

To create a swept surface
1 Use AMSWEEPSF to sweep two cross sections along a rail, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select the first cross section (1)
Select cross sections: Select the second cross section (2) and press ENTER
Select rails: Select line (3) and press ENTER

2 In the Sweep Surface dialog box, choose OK to accept default settings.

A message tells you that four surfaces will be created. Choose Continue. The
surfaces should look like this.

Creating Motion-Based Surfaces

541

You can select the individual surfaces to see the shape of each one.
Because one of the cross sections has sharp corners, a single surface cannot
be created. Instead, four separate surfaces are created, each corresponding to
one side of the rectangular cross section. For more information, see “To surface polylines with sharp corners” on page 550.
3 Use the Extents option of ZOOM to redisplay all the wireframes and select the
object for the next exercise.
To sweep a spline along a rail
1 Sweep one spline along a rail, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select spline (1) and press ENTER
Select rails: Select line (2) and press ENTER

1
2

2 In the Sweep Surface dialog box, choose OK to accept the default settings.
Your surface should look like this.

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Chapter 19 Creating and Editing Surfaces

You created a nonuniform rational B-spline (NURBS) surface from a spline.
You can convert a NURBS surface into a part by adding thickness.

NOTE Save a copy of your NURBS surface if you will need it later. When you
thicken a surface, the original surface is consumed and disappears.
To convert a NURBS surface to a solid
1 Use AMTHICKEN to convert a NURBS surface to a thin solid, responding to the
prompts.
Desktop Menu

Surface ➤ Surface Thicken

Select surfaces to thicken: Select the surface
Select surfaces to thicken: Press ENTER
Select direction to thicken [Flip/Accept] :
Flip to point the direction arrow down, and press ENTER
Thickness <1.0000>: Press ENTER

A solid is created, and a new part icon is displayed in the Browser.
2 Use the Extents option of ZOOM to redisplay all the wireframes and select the
object for the next exercise.
A swept surface is useful when your design has different shapes at either end.

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543

To sweep dissimilar shapes
1 Sweep two dissimilar shapes along two nonparallel rails, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select first shape (1)
Select cross sections: Select second shape (2) and press ENTER
Select rails: Select first rail (3)
Select rails: Select second rail (4)

1
3
4
2

2 In the Sweep Surface dialog box, choose OK to accept the default settings.
The swept surface should look like this.

3 Use the Extents option of ZOOM to redisplay all the wireframes and select the
object for the next exercise.

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Chapter 19 Creating and Editing Surfaces

To sweep multiple cross sections along two rails
1 Sweep multiple cross sections along two rails, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections:
Select cross sections (1) through (5) in consecutive order and press ENTER
Select rails: Select first rail (6)
Select rails: Select second rail (7)
1
2

6
7

3
4
5

2 In the Sweep Surface dialog box, choose OK to accept the default scale.
Because the cross sections have rounded corners, a single surface results. If
the cross section had square corners, three surfaces would have been created.

3 Use the Extents option of ZOOM to redisplay all the wireframes and select the
object for the next exercise.

Creating Motion-Based Surfaces

545

Creating Skin Surfaces
A skin surface drapes over a wireframe model. After the wireframe is
removed, the surface retains the shape of the wireframe. Skin surfaces are
ruled, planar, lofted U, and lofted UV.

Ruled Surfaces
A ruled surface is a straight, flat shape stretched between two wires of any 3D
shape. You can create a ruled surface between any two nonintersecting wires
that can represent the top and the bottom. The top and bottom can be open
or closed wires. You can create a ruled surface from two augmented lines as
well, and from a single augmented line by adding thickness to it.
To surface two wires
1 Use AMRULE to create the ruled surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Rule

Select first wire: Select line (1)
Select second wire: Select line (2)
1

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Chapter 19 Creating and Editing Surfaces

The ruled surface shows the surface normal, a short vertical line in one corner.
A surface normal shows where the surface starts and which direction is out.

If surface normal indicators are too small, use the DISPSF system variable to
change the size. In the Individual Surface Display dialog box, change the
value in the Normal Length field. Adjust the setting as needed.
You can create a ruled surface from two augment lines, or by adding width to
a single augmented line. Besides using the command method, you can access
AMAUGMENT in the Desktop menu by choosing Surface ➤ Create Wireframe
➤ Augmented Lines.
To create an augmented line on a surface
1 Use AMAUGMENT to create an augmented line on the surface.
Command

AMAUGMENT

Select surface wire or [Angle/Distance/Spacing]:
Select the leftmost wire of the surface
Select surface wire or [Angle/Distance/Spacing]: Press ENTER

When you use an augmented wire to create a surface, the vectors are ignored.
You specify a value for the width of the surface.

Creating Skin Surfaces

547

To surface an augmented line
1 Use AMRULE to create a surface from the augmented wire, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Rule

Select first wire: Select the augmented line
Enter an option [Next/Accept] : Press ENTER
Enter width (or) [Select second wire] <1.0000>: Press ENTER

The surface extends beyond the vectors to the specified width.
You can use this technique to create a ruled surface normal to any existing
ruled surface. First you create a parting line on the surface and project it to get
an augmented line, and then create the ruled surface from the augmented line.
2 Undo the surfaces you created so that you can use the two original augmented lines in subsequent exercises.
Desktop Menu

Edit ➤ Undo

3 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

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Chapter 19 Creating and Editing Surfaces

To surface two arcs with different radii
1 Create a surface from two arcs of different radii, responding to the prompts.
Surface ➤ Create Surface ➤ Rule

Desktop Menu

Select first wire: Select arc (1)
Select second wire: Select arc (2)

The ruled surface should look like this.

surface normal

2 To experiment, use the previous example and select the arcs in a different order.
3 Erase the surface you just created.
Desktop Menu

Modify ➤ Erase

Select the surface and press ENTER.
If creating the surface was the last command, you can use UNDO.
4 Create a surface again, selecting the arcs in reverse order.
Desktop Menu

Surface ➤ Create Surface ➤ Rule

Select first wire: Select arc (2)
Select second wire: Select arc (1)

Creating Skin Surfaces

549

Selecting the arcs in different order changes the surface normal.

surface
normal

5 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.
In the next exercise, you surface polylines. A surface follows a spline exactly
but approximates the polyline by a curve. The Polyline Fit default setting of
150 maintains all corners less than 150 degrees as sharp corners. In such
cases, multiple surfaces are created.
To surface polylines with sharp corners
1 Use the Mechanical Options dialog box to adjust the Polyline Fit settings:
Desktop Menu

Surface ➤ Surface Options

Choose the Surfaces tab and then choose Polyline Fit.
2 In the Polyline Fit dialog box, change the angle setting to 0 and change the
length setting to inf (infinity) or a specific length longer than the longest line
segment.

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Chapter 19 Creating and Editing Surfaces

Choose OK.
These settings force sharp corners to convert to a smooth curved surface.
3 Choose OK to exit the Mechanical Options dialog box.

Creating Skin Surfaces

551

4 Use AMRULE to create a curved surface from polylines drawn with sharp corners, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Rule

Select first wire: Select polyline (1)
Select second wire: Select polyline (2)

A continuous smooth curved surface is created.

5 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.
Now use the same polylines, but choose a fit angle to recognize sharp corners.
Use the Polyline Fit dialog box to change the angle setting until the image
tile resembles the angles you want to recognize as corners. Choose a setting
between 150 and 165 to recognize most corners.

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Chapter 19 Creating and Editing Surfaces

To create surfaces with sharp angles
1 Use AMOPTIONS to reset the fit angle to 150 and re-create the ruled surface.
Desktop Menu

Surface ➤ Surface Options

2 Erase the surface you just created.
Desktop Menu

Modify ➤ Erase

3 Use AMRULE to create three ruled surfaces from polylines drawn with sharp
corners, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Rule

Select first wire: Select polyline (1)
Select second wire: Select polyline (2)

4 A message tells you that three surfaces will be created. Choose Continue.

The three surfaces follow the sharp corners of the polylines.

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553

5 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

Trimmed Planar Surfaces
A planar surface may be constructed from lines, arcs, splines, polylines, or
simply two locations, if the selected objects are closed and on the same plane.
The exterior shape of the 2D wire shape becomes the trimmed edge of the
surface. In this exercise, you create trimmed planar surfaces.
To create a planar trimmed surface using a closed polyline
1 Use AMPLANE to create a planar trim surface from a closed polyline, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Planar Trim

Specify first corner or [Plane/Wires]: _wire
Select wires: Select object (1)
Select wires: Press ENTER

The planar surface is trimmed, using the closed polyline as the border. The U
and V lines appear inside the border.

2 Use the Extents option of ZOOM to redisplay all of the wireframes, and select
the object for the next exercise.
The closed polyline for the next exercise contains two interior circles that are
coplanar. You create a trimmed surface using the polyline and circles.

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Chapter 19 Creating and Editing Surfaces

To create a trimmed planar surface using three closed polylines
1 Create a planar trim surface from three polylines, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Planar Trim

Specify first corner or [Plane/Wires]: _wire
Select wires: Select object (1)
Select wires: Select interior circle (2)
Select wires: Select circle (3)
Select wires: Press ENTER

2
3

Instead of selecting the objects individually, you could also drag a crossing
window around all of them and press ENTER.
A trimmed planar surface is automatically trimmed to the largest boundary
created by the wire. As in this example, when closed areas exist inside the
boundary, these holes are trimmed out.

2 Use the Extents option of ZOOM to redisplay all of the wireframes, and select
the object for the next exercise.

Lofted Surfaces
You can create a lofted surface from one or two sets of wires, each with similar
attributes, such as having approximately the same direction. You must select
the wires in consecutive order.

Creating Skin Surfaces

555

A lofted U surface is stretched between any number of wires that share similar
characteristics. The example contains two sets of wires from which you create
two surfaces. The light blue polylines are approximately horizontal, and the
green lines are approximately vertical. First, you create a surface from the
horizontal polylines.
To create a lofted surface using a set of wires
1 Use AMLOFTU to surface a set of vertical wires, responding to the prompts.
Desktop Menu
Select U wires:

Surface ➤ Create Surface ➤ LoftU
Select lines (1) through (8) in consecutive order and press ENTER

9
18

2 In the Loft Surface dialog box, choose OK to accept the default settings.

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Chapter 19 Creating and Editing Surfaces

3 Surface a set of horizontal wires, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ LoftU

Select U wires: Select lines (9) through (18) in consecutive order and press ENTER
4 In the Loft Surface dialog box, choose OK to accept the default settings.
The two surfaces, one horizontal and one vertical, should look like these.

5 Use the Extents option of ZOOM to redisplay all the wireframes and select the
object for the next exercise.
A lofted UV surface is stretched over two sets of wires. Each wire in one set
crosses every wire in the other set. Two sets of wires can accurately describe
a complex surface.
You can select wires directly, as you did in the previous exercise, or you can
select two groups of wires. In this exercise, you create two groups of wires and
then create a lofted surface from the two groups. The wires in the U direction
are magenta (purple), and those in the V direction are cyan (light blue).
3
1

6
12
7
13

Creating Skin Surfaces

557

To create a single lofted surface from two groups of wires
1 Group the magenta U lines.
Command

GROUP

In the Object Grouping dialog box specify:
Group Name: Enter uwires
Create Group: Choose New to close the dialog box
Respond to the prompt as follows:
Select objects:

Select lines (1) through (7) in consecutive order and press ENTER

In the Object Grouping dialog box, choose OK.
2 Press ENTER to repeat the GROUP command.
In the Object Grouping dialog box specify:
Group name: Enter vwires
Create Group: Choose New to close the dialog box
Respond to the prompt as follows:
Select objects:

Select lines (8) through (13) in consecutive order and press ENTER

In the dialog box, choose OK.

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Chapter 19 Creating and Editing Surfaces

3 Use AMLOFTU to loft a surface from two groups of wires, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ LoftUV

Select U wires: Enter g
Enter group name: Enter uwires
7 found
Select U wires: Press ENTER
Select V wires: Enter g
Enter group name: Enter vwires
6 found
Select V wires: Press ENTER
Enter an option [eXit/Loft/Node check] : Press ENTER
You have created a surface from the two groups of wires.

4 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

Creating Derived Surfaces
Derived surfaces are generated from existing surfaces: blended, offset, fillet,
and corner fillet. Derived surfaces can be trimmed.

Blended Surfaces
You can create a blended surface between two, three, or four wires or surfaces.
The blended surface is tangent to the surfaces or wires from which it is created.

NOTE To create surfaces correctly, select lines at points shown in the illustrations.

Creating Derived Surfaces

559

To create a blended surface
1 Use AMBLEND to create a blended surface from two wires, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (1)
Select second wire: Select surface (2)
Select third wire [Weights]: Press ENTER

1
2

You have created the first blended surface.
The type of object you select affects the blended surface. When you select surfaces or augmented lines, you are prompted for the weight of the surface edge.
2 Create the second blended surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (3)
Select second wire: Select surface (4)
Select third wire [Weights]: Press ENTER

3
4

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Chapter 19 Creating and Editing Surfaces

3 Create the third blended surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (5)
Select second wire: Select surface (6)
Select third wire [Weights]: Press ENTER

5
6

4 Use ZOOM to enlarge the corner area created by the blended surfaces.
5 Use AMBLEND to create a corner blended surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend.

Select first wire: Select surface (7)
Enter an option [next/Accept] : Press ENTER
Select second wire: Select surface (8)
Enter an option [next/Accept] : Press ENTER
Select third wire [Weights]: Select surface (9)
Select fourth wire: Press ENTER

7
8

The order in which you select the objects to blend determines the orientation
of the corner created by the blend.

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561

Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.
Next, you create a blended surface from two surfaces and lines. To create a
blended surface from four objects, make the selections in the order shown;
the objects cannot be selected in consecutive order.
To blend surfaces and lines
1 Use AMBLEND to create a surface from two surfaces and two lines, responding
to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (1)
Select second wire: Select surface (2)
Enter an option [Next/Accept] : Press ENTER
Select third wire [Weights]: Select wire (3)
Select fourth wire: Select wire (4)
1

3
2

The new surface is created between the original surfaces and lines.

2 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.
Next, you create two surfaces, each blended from two augmented lines.

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Chapter 19 Creating and Editing Surfaces

To blend augmented lines
1 Use AMBLEND to create a surface from two augmented lines, responding to
the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select line (1)
Select second wire: Select line (2)
Select third wire [Weights]: Press ENTER

2 Use ZOOM to redisplay wireframes. Then select the second set of lines.
3 Create a surface from the second set of augmented lines, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Blend

Select first wire: Select augmented line (1)
Select second wire: Select augmented line (2)
Select third wire [Weights]: Press ENTER

Compare these two surfaces to see how the direction of the augmented line
vectors affects the resulting surface.
4 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

Offset Surfaces
An offset surface is a duplicate of an existing surface, offset by a specific distance. When you create an offset surface, you can keep the original or remove
it, as needed.

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563

To create an offset surface
1 Use AMOFFSETSF to create an offset surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Offset

Select surfaces to offset: Select surface (1)
Select surfaces to offset: Press ENTER
Distance=1.0000 Keep=Yes
Enter offset distance or [Keep] <1.0000>: Enter k
Keep original surface(s) [Yes/No] : Enter y
Distance=1.0000 Keep=Yes
Enter offset distance or [Keep] <1.0000>: Enter 0.5

The new surface is offset from the original surface, which is normal at all
locations.

2 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

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Chapter 19 Creating and Editing Surfaces

Fillet and Corner Surfaces
In this exercise, you create fillet surfaces between two selected surfaces, and
a corner fillet where three fillet surfaces intersect. You trim the original surfaces back to the fillet surfaces.
To create fillet and corner surfaces
1 Use AMFILLETSF to create a fillet between two surfaces, responding to the
prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (1)
Select second surface: Select surface (2)

2 In the Fillet Surface dialog box, specify:
Fillet Type: Constant
Trim: Both Surfaces
Create To: Surface Trim
Radius: Enter 0.5

Choose OK.

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565

3 Create a fillet between another two surfaces, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (3)
Select second surface: Select surface (4)

4 In the Fillet Surface dialog box, specify:
Fillet Type: Constant
Trim: Both Surfaces
Create To: Base Surface
Radius: Enter 0.75
Choose OK.
The Base Surface option was not available when you created the first fillet
surface. It is available now because the first surface was trimmed and now
differs from the base surface. Next, trim to the base surface, not the trimmed
surface.

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The next illustration shows both fillets, which you will trim later.
5 Create a fillet between another two surfaces, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (5)
Select second surface: Select surface (6)

6
5

6 In the Fillet Surface dialog box, specify:
Fillet Type: Constant
Trim: Both Surfaces
Create To: Base Surface
Radius: Enter 0.6
Choose OK.
The fillets overlap at the corner. You need to trim the overlap with a corner
fillet.

Creating Derived Surfaces

567

To create a corner fillet
1 Use AMCORNER to trim the overlapping fillets, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Corner Fillet

NOTE The default is set to trim the corner fillet to the three fillet surfaces. If you
do not want to trim, enter T at the first prompt and change the setting to No.
Trim=Yes
Select first fillet surface or [Trim]: Select surface (7)
Select first fillet surface or [Trim]: Select surface (8)
Select first fillet surface or [Trim]: Select surface (9)

8
7

The trimmed corner fillet looks like this.

2 Use the Extents option of ZOOM and select the object for the next exercise.

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Chapter 19 Creating and Editing Surfaces

Editing Surfaces
As you create models, you need to combine surfaces and trim them where
they overlap. You will learn four surface editing techniques: adjusting surfaces, joining surfaces, trimming surfaces at intersections, and trimming
surfaces by projection.

Adjusting Adjacent Surfaces
You can control the tangency of two adjacent surfaces by adjusting them to
create one continuous surface. When you select the edges of two adjacent
surfaces to adjust, the first edge you select is the control surface. You can use
a quilt for the control surface. By default, 20 per cent of the total area of each
surface is adjusted. You can change the percentage for either or both of the
the adjustment areas, depending on which surface shape you need to retain.
To adjust adjacent surfaces
1 Use AMADJUST to convert two surfaces into one surface, responding to the
prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Adjust

Select surface edge to adjust: Select the control surface edge (1)
Select surface edge to adjust: Select the adjacent surface edge (2)

1
2

Editing Surfaces

569

First surface=20.0000% Second surface=20.0000% cOntinuity=Smooth
Keep=No
Enter an option [First surface/Second surface/cOntinuity/Keep] :
Enter s
Enter adjustment for the second surface <20.0000%>: Enter 40
First surface=20.0000% Second surface=40.0000% cOntinuity=Smooth
Keep=No
Enter an option [First surface/Second surface/cOntinuity/Keep] :
Enter o
Continuity [Coincident/Smooth] : Press ENTER
First surface=20.0000% Second surface=40.0000% cOntinuity=Coincident
Keep=No
Enter an option [First surface/Second surface/cOntinuity/Keep] :
Press ENTER

The two surfaces are adjusted to meet.

Joining Surfaces
You can join multiple surfaces into a single surface. Each surface is indicated
by two surface normal indicators.
To join surfaces
1 Use AMJOINSF to join the surfaces you select, responding to the prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Join

Select surfaces to join: Select surface (1)
Select surfaces to join: Select surface (2)
Select surfaces to join: Press ENTER

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Chapter 19 Creating and Editing Surfaces

The two surfaces are joined. Only one surface normal indicator is shown.

To force two surfaces to join, choose Surface ➤ Surface Options. In the
Mechanical Options dialog box, choose the Surface tab and adjust the Join
Gap Tolerance. Two untrimmed surfaces are joined automatically if they are
within twice the gap tolerance.
2 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

Trimming Intersecting Surfaces
You can trim intersecting surfaces, including quilted surfaces, and create a 3D
polyline at the intersection. The 3D polyline can then be used to create
another surface.
A 3D point is created at the intersection of a wire curve and a surface or quilt.
If the wire curve intersects the surface or quilt more than once, points are created everywhere an intersection takes place.
When you trim, always make your selections on the portion of the surface
you want to keep.

Editing Surfaces

571

To trim intersecting surfaces
1 Use AMINTERSF to trim the surface you want to keep, responding to the
prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Intersect Trim

Select first surface/quilt or wire: Select surface (1)
Select second surface: Select surface (2)
2

2 In the Surface Intersection dialog box, check the options indicated in the following illustration and choose OK.

The first surface you selected is trimmed at its intersection with the second
surface.
Using the Trim options, you can trim neither, one, or both surfaces at their
intersection. As you change these options, the dynamic image in the dialog
box displays the results.

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Chapter 19 Creating and Editing Surfaces

3 Use UNDO to erase the trim. Then try selecting surfaces at different locations.
4 Use the Extents option of ZOOM to redisplay all of the wireframes and select
the object for the next exercise.

Trimming Surfaces by Projection
You can project a wire onto a surface to trim a shape that corresponds to the
wire shape. You select the portion of the surface you want to keep.
In this exercise, you trim a curved surface with a star-shaped polyline.
To trim a surface by a projected wire
1 Use AMPROJECT to project the wire to trim the surface, responding to the
prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select polyline (1) and press ENTER
Select target surfaces/quilts: Select surface (2) on the side you want to keep
Select target surfaces/quilts: Press ENTER
1

Editing Surfaces

573

2 In the Project to Surface dialog box, specify:
Direction: Choose Normal
Output Type: Choose Trim Surface
Keep Original Wire: Check the check box

Choose OK.
The polyline is projected onto the curved surface, trimming out the surface
inside the polyline.

3 Use UNDO and try different selection points and output types for the
projection.

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Chapter 19 Creating and Editing Surfaces

Combining Parts and
Surfaces

In This Chapter

In Autodesk® Mechanical Desktop®, surfaces are

■ Creating a part with multiple

features
valuable features because they can represent complex
curved shapes. When joined to a parametric part, they

■ Creating a simple surface
■ Attaching a surface

parametrically to a part
cut away an angular surface and replace it with a
sculpted face. A surface may also add material to a part
as a protrusion. In this tutorial, you combine parametric

■ Cutting out features
■ Creating mounting holes
■ Sketching on work planes
■ Revising and finishing a design

and surface modeling by creating a camera body with a
sculpted face.

575

Key Terms
Term

Definition

base surface

A basic underlying surface that carries a shape across a larger area. Can be trimmed
to precise shapes as needed, but the base surface remains intact and may be
displayed.

model view

Changes orientation of the viewer so that the object is viewed from a different
position. Individual views can be displayed in multiple viewports. For example, enter
3 at the Command prompt to create three viewports with default views: top, front,
and right isometric.

NURBS

Acronym for nonuniform rational B-spline. The SPLINE command creates a true
NURBS curve and can be used to create a surface.

rail

One or more curved lines along which surfaces are swept. They form the curvature of
a swept surface.

spline

A curved line defined by specified control points that assumes a unique shape. Used
to create curved surfaces. The radius of a spline curve is constantly changing. Splines
are used as the basis of free-form surfaces.

surface cut

A feature created when a surface is joined to a part. Where the surface cuts the part
or protrudes, the part face assumes the curved shape of the surface. The surface, like
other features, is parametric; both the surface and the part retain their parametric
relationship whenever either is modified.

wire

A generic term referring to lines, arcs, circles, ellipses, 2D and 3D polylines,
augmented lines, and splines.

work plane

An infinite plane attached to a part. Can be designated as a sketch plane and can be
included in a constraint or dimension scheme. Work planes can be either parametric,
or non-parametric.

work point

A parametric work feature used to position a hole, the center of a pattern, or any
other point for which there is no other geometric reference.

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Chapter 20 Combining Parts and Surfaces

Basic Concepts of Combining Parts and
Surfaces
You can use Mechanical Desktop® to create angular-shaped parts. You can
apply 3D surfaces to those parts to create hybrid parts consisting of a mixture
of angular and curved shapes. With Mechanical Desktop you can create
model designs with shapes of varying types.
You can apply surfaces to Mechanical Desktop parts and use those surfaces to
cut material from a parametric part, to create any hybrid shapes that your
design requires.

before surface cut

after surface cut

You can also use surfaces to add material to angular parts.

Using Surface Features
A feature created from surfaces has the shape of a contoured surface. You
either cut away material or add material as a protrusion to join it to a part.
In this tutorial, you cut away an angular face and replace it with a sculpted
surface.
Surfaces must have these characteristics to be used as features on models:
■
■
■
■
■
■

A contoured surface must have four logical boundaries.
The curved shape must be a single surface. If you need multiple surfaces
to represent the shape, you must join them into a single surface.
The surface must be a nontrimmed base surface. Join only base surfaces,
not interior trim edges of trimmed surfaces.
The surface must extend past the part on all four sides.
A surface cannot contain sharp corners.
Surfaces should have a minimum number of internal patches. These surfaces work better and faster than complex ones.

Basic Concepts of Combining Parts and Surfaces

577

First, sketch the camera from all sides (top, side, front, and isometric views).
With a complete idea, you can decide where to place features on the camera
body.
shutter release mount

film advance mount

lens sheath

viewfinder
compartment

flash compartment
film compartment
battery compartment

door cutout

The camera body, which is common to all other features, is the base feature.
The camera design has many other features, some of which are cutaways
from the body: battery and film compartments and cutouts for their doors;
mounting holes for the film advance and shutter release; and compartments
for the viewfinder and the flash. The lens sheath feature, a sculpted surface,
is joined to the camera face.

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Chapter 20 Combining Parts and Surfaces

Creating Surface Features
Open the file camera.dwg in the desktop\tutorial folder. The file contains the
settings you need, and the geometry to create the camera body—an extruded
feature and some NURBS curves. You use NURBS to create the surface for the
sculpted camera face.

NOTE Back up the tutorial drawing files so you still have the original files if you
make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
You can work on your model in any viewport, moving among views as you
create features.

First, you create two surfaces by sweeping wires along a rail. Then, you join
them into a single surface and extend the surface so that it covers the camera
body.

NOTE If you prefer to use toolbuttons to access commands, choose Surface ➤
Launch Toolbar.

Creating Surface Features

579

To create a swept surface
1 Use AMSWEEPSF to sweep a spline along a rail, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections: In the front view, choose the right horizontal spline (1)
Select cross sections: Press ENTER
Select rails: Select the vertical spline (2)
Select rails: Press ENTER

2 In the Sweep Surface dialog box, specify:
Orientation: Parallel

Choose OK. The first half of the swept surface is created.
3 Create the second half of the swept surface, responding to the prompts.
Desktop Menu

Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select the left horizontal spline (3)
Select cross sections: Press ENTER
Select rails: Select the vertical spline (2)
Enter an option [Next/Accept] : Press ENTER
Select rails: Press ENTER
In the Sweep Surface dialog box, specify:
Orientation: Parallel
Choose OK.

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Chapter 20 Combining Parts and Surfaces

4 Use AMJOINSF to join the two surfaces, responding to the prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Join

Select surfaces to join: Select the right surface (1)
Select surfaces to join: Select the left surface (2) and press ENTER

The two surfaces create a single surface. The resulting surface probably does
not extend beyond the part on all sides, so you need to lengthen the surface.
5 Use AMLENGTHEN to lengthen the surface, responding to the prompts.
Desktop Menu

Surface ➤ Edit Surface ➤ Lengthen

Base edge=Single Extension=Percent Method=Parabolic Value=110.0000%
Select surface edge or spline [eDge/Extend/Keep/Mode/Value]: Enter v
Enter percent <110.0000%>: Enter 105
Base edge=Single Extension=Percent Method=Parabolic Value=105.0000%
Select surface edge or spline [eDge/Extend/Keep/Mode/Value]:
Select the rightmost vertical edge of the surface (1)
Base edge=Single Extension=Percent Method=Parabolic Value=105.0000%
Select surface edge or spline [eDge/Extend/Keep/Mode/Value]: Press ENTER
1

The surface now extends past the cube representing the camera body.

Creating Surface Features

581

Attaching Surfaces Parametrically
Next, you create a work plane and work point and then dimension the work
point to the part. This dimension establishes a parametric relationship
between the surface and the part. The position of the surface is controlled by
the work point, and its orientation is controlled by the work plane associated
with the work point. Later, if you modify the position of the work point, the
surface location moves accordingly.
To position the work plane and work point easily, work in the isometric view.
To attach a surface to a part
1 Use AMWORKPLN to create a work plane.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

In the Work Plane Feature dialog box, specify:
1st Modifier: Planar Parallel
2nd Modifier: Offset
Offset: Enter 1
Create Sketch Plane: Select the check box
Choose OK.
2 Position the offset work plane on the part, responding to the prompts.
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the front face of the camera (1)
Enter an option [Next/Accept] :
Choose n to cycle to the front face, or press ENTER
Enter an option [Flip/Accept] :
Choose f to flip the direction arrow away from the camera body, or press ENTER
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Verify that the UCS icon is upright and press ENTER

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Chapter 20 Combining Parts and Surfaces

1
2

You have created a parallel work plane offset from the front face of the part.
3 Use AMWORKPT to place a work point on the work plane, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Point.

Workpoint will be placed on the current sketch plane.
Specify the location of the workpoint: Specify a location (2)
You have created a work point on the sketch plane.
4 Use AMPARDIM to constrain the work point to the camera body, responding
to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select the work point (3)
Select second object or place dimension:
Select the right edge of the camera body (4)
Specify dimension placement: Place the horizontal dimension (5)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<1.3316>: Enter 1
Solved underconstrained sketch requiring 1 dimensions or constraints.

Attaching Surfaces Parametrically

583

5 Continue on the command line.
Select first object: Select the work point
Select second object or place dimension:
Select the bottom edge of the camera body
Specify dimension placement: Place the vertical dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.8898>: Enter 1
Solved fully constrained sketch.
Select first object: Press ENTER

The work point is fully constrained.
Save your file.

Cutting Parts with Surfaces
Now that the surface is positioned relative to the camera body, you can use
it to cut away material from the planar camera face.
To cut away from a part
1 Use AMSURFCUT to create a surface cut, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Placed
Features ➤ Surface Cut.

(Type: Cut)
Select surface or [Type]: Select the surface
Select work point: Select the work point
Specify portion to remove: [Flip/Accept] :
Verify the direction arrow points away from the camera body and press ENTER

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Chapter 20 Combining Parts and Surfaces

One side of the part is cut away, leaving the curved face of the surface. Your
model shows the modified block and the splines used to create the surface.

2 Use REGENALL to regenerate the drawing views.
Desktop Menu

View ➤ Regen All

3 Remove the three splines used to create the surface.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Erase.

4 Select the three splines and press ENTER.

Save your file.

Cutting Parts with Surfaces

585

Creating Extruded Features
The film compartment at the back of the base feature has two features—the
compartment and the door.
The camera back is a flat plane. You specify it as the sketch plane, sketch the
profile, and extrude it directly into the camera body.
To sketch the film compartment
1 Use AMSKPLN to create a new sketch plane, responding to the prompts. Work
in the isometric view.
Context Menu

In the graphics area, right-click and choose New Sketch
Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the back face of the camera (1)
Enter an option [Accept/Next] :
Choose n to cycle to the back face, or press ENTER
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Select the bottom edge of the camera (2)
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Verify that the X axis is pointing to the left and press ENTER

1
2

The back of the camera has been specified as the sketch plane. In the isometric view, the UCS icon is displayed with the X axis pointing left.
Next, change the view to see the back of the camera. If needed, zoom out to
see the entire back of the camera.
2 Change the front view to a back view.
Desktop Menu

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View ➤ 3D Views ➤ Back

Chapter 20 Combining Parts and Surfaces

3 Use RECTANG to sketch a rectangle to the left on the camera back.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

4 Use AMPROFILE to create a profile from the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

You need to place four dimensions or constraints: two to define the sketch
size and two to specify the sketch location on the camera body.
To add dimensions and constraints to the film compartment sketch
1 Use AMPARDIM to dimension the width of the rectangle, responding to the
prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select the bottom horizontal line of the sketch (1)
Select second object or place dimension: Specify a location (2)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<3.7546>: Enter 4
Solved underconstrained sketch requiring 3 dimensions or constraints.

3
4
1

2 Define the height of the rectangle.
Select first object: Select the left vertical line of the sketch (3)
Select second object or place dimension: Specify a location (4)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<2.6011>: Enter 2.5
Solved underconstrained sketch requiring 2 dimensions or constraints.
Select first object: Press ENTER

Creating Extruded Features

587

3 Make the isometric view active.
To see the dimensions and the profile sketch more clearly, rotate the isometric view until the back of the camera faces you.
Desktop Menu

View ➤ 3D Views ➤ Back Left Isometric

Define the distance between the top of the sketch and the top of the camera
back.
4 Use AMPARDIM to constrain the rectangle to the camera body, responding to
the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select line (1)
Select second object or place dimension: Select line (2)
Specify dimension placement: Specify a location (3)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.2355>: Enter .1626
Solved underconstrained sketch requiring 1 dimensions or constraints.
3

2 1

5
4
6

5 Define the distance between the right side of the sketch and the right edge
of the camera back.
Select first object: Select line (4)
Select second object or place dimension: Select line (5)
Specify dimension placement: Specify a location (6)
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.8583>: Enter .8426
Solved fully constrained sketch.
Select first object: Press ENTER
Next, cut the film compartment from the camera body.

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Chapter 20 Combining Parts and Surfaces

To cut the film compartment
1 Use AMEXTRUDE to cut the film compartment from the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Blind
Distance: Enter 1.2
Flip: Point the direction arrow into the camera body

Choose OK.
The cut-out compartment is displayed in all four views.

Creating Extruded Features

589

2 Activate and then restore the viewports to the original orientation.
Upper right viewport: Front Right Isometric View
Lower left viewport: Front View
Cutting the door is similar to cutting the film compartment. You sketch a
rectangle on the right side of the camera and blindly extrude it as a cut into
the camera body.
To sketch the film compartment door
1 Use AMSKPLN to create a new sketch plane, responding to the prompts. Work
in the isometric view.
Context Menu

In the graphics area, right-click and choose New Sketch
Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the side face of the camera (1)
Enter an option [Accept/Next] :
Verify that the side face is highlighted and press ENTER
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Verify that the Z axis points away from the camera and press ENTER

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Chapter 20 Combining Parts and Surfaces

2 Set the UCS origin to the lower-left corner of the right side of the camera,
responding to the prompts.
Desktop Menu

Assist ➤ New UCS ➤ Origin

Specify new origin point <0,0,0>: Enter end
of: Specify a point near the lower-left corner of the side view

NOTE If the UCS icon does not snap to the lower-left corner of the camera,
set the AutoCAD system variable UCSICON to On.
3 In the side view, zoom in on the camera face.
Context Menu

In the graphics area, right-click and choose Zoom.

4 Hold down the left mouse button to size the view, and then press ENTER to
end the command.
5 Sketch a rectangular shape for the door cutout.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

6 Create the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

You need four dimensions or constraints to solve the sketch. Add constraints
that define the location of the profile on the camera side.

Creating Extruded Features

591

To constrain the film compartment door
1 Use AMADDCON to make the bottom edge of the profile sketch collinear with
the bottom line of the film compartment, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Collinear.

Valid selection(s): line or spline segment
Select object to be reoriented: Select line (1)
Valid selection(s): line or spline segment
Select object to be made collinear to: Select line (2)
Solved underconstrained sketch requiring 3 dimensions or constraints.

3
4
1
2

2 Make the right side of the profile sketch collinear with the right edge of the
camera body.
Valid selection(s): line or spline segment
Select object to be reoriented: Select line (3)
Valid selection(s): line or spline segment
Select object to be made collinear to: Select line (4)
Solved underconstrained sketch requiring 2 dimensions or constraints.
Valid selection(s): line or spline segment
Select object to be reoriented: Press ENTER
Enter an option
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER

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Chapter 20 Combining Parts and Surfaces

3 Use AMPARDIM to dimension the width and height of the profile sketch,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select a horizontal profile edge
Select second object or place dimension: Place the horizontal dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.6840>: Enter .6
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Select a vertical profile edge
Select second object or place dimension: Place the vertical dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<2.3218>: Enter 2.5
Solved fully constrained sketch.
Select first object: Press ENTER
The horizontal dimension makes the width of the profile equal to half the
depth of the film compartment and the height of the profile equal to the
height of the compartment.
For practice, express the width and height of the profile as equations.
To cut the film compartment door
1 Use AMEXTRUDE to cut the profile from the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Blind
Distance: Enter .1574
Flip: Point the direction arrow into the camera

Creating Extruded Features

593

2 Choose OK to create the extrusion.
Save your file.
The battery compartment also has a cutout for a door. The order in which
you create these features does not matter, but the natural order would be to
create the film compartment first.
The cutout for the battery compartment is more complicated because of its
shape. The key to creating this feature is to locate the sketch plane properly
on the bottom left side of the camera body.

NOTE Watch the UCS icon in the isometric view and make sure it is positioned
on the bottom of the camera.
To sketch the battery compartment
1 Change the top view to a bottom view.
Desktop Menu

View ➤ 3D Views ➤ Bottom

2 Use AMSKPLN to create a new sketch plane, responding to the prompts. Work
in the isometric view.
Context Menu

In the graphics area, right-click and choose New Sketch
Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Select the bottom face of the camera (1)
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Verify that the Z axis arrow points down, away from the camera body
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Verify that the X axis points to the left and press ENTER

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Chapter 20 Combining Parts and Surfaces

3 Use PLINE to sketch the profile of the battery compartment on the bottom of
the camera body. Work in the bottom view.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Polyline.

4 Use AMPROFILE to create the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

The sketch needs seven to nine dimensions or constraints, depending on
how precisely you drew the sketch. If you need more than seven constraints,
you need to add some missing geometric constraints.
To constrain the battery compartment
1 Use AMSHOWCON to view the current geometric constraints.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Show Constraints.

2 Add any missing geometric constraints.
Typically, the radial (R) constraints and one of the tangent (T) constraints are
missing from the arcs.

NOTE When you add constraints, the sketch shape might become distorted,
but you can restore it when you complete the dimensions. Dimension the largest
vertical dimension and the arcs before you dimension smaller objects.

Creating Extruded Features

595

3 Use AMPARDIM to add the following dimensions.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

The sketch is fully constrained.
To cut the battery compartment
1 Use AMEXTRUDE to cut the profile from the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Blind
Distance: Enter 2.4
Flip: Point the direction arrow into the camera body
Choose OK.

The door opening of the battery compartment is located on the same plane
as the battery compartment. Therefore, you need only to sketch and constrain a rectangle, cutting it into the camera body to the proper depth.

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Chapter 20 Combining Parts and Surfaces

To sketch and constrain the battery compartment door
1 Use RECTANG to sketch the profile of the cutout. Work in the bottom view.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

2 Use AMPROFILE to create the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

The sketch requires four dimensions or constraints.
3 Use AMADDCON to constrain the sketch to the bottom of the camera body.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Collinear.

Select lines that make the outside edges of the sketch collinear with the outside edges of the camera body.
4 Use AMPARDIM to dimension the length and width of the profile sketch,
responding to the prompts.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

Select first object: Select the narrow side of the rectangle
Select second object or place dimension: Place the horizontal dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<0.7463>: Enter .76
Solved underconstrained sketch requiring 1 dimensions or constraints.
Select first object: Select the long side of the rectangle
Select second object or place dimension: Place the vertical dimension
Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]
<1.1274>: Enter 1.3
Solved fully constrained sketch.
Select first object: Press ENTER

The sketch is fully constrained.

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To cut the battery compartment door
1 Use Extrude to cut the door opening from the camera body. Make sure the
direction of the cut is into the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Blind
Distance: Enter .1574
Flip: Point the direction arrow into the camera body
Choose OK.

Save your file.

Creating Holes
Both the shutter release and the film advance mounts are counterbored holes
that you can create as placed features.
To create shutter release and film advance mount holes
1 Change the upper-left viewport to a top view.
Desktop Menu

View ➤ 3D Views ➤ Top

2 Zoom in to enlarge the view as needed, and then activate the isometric view.
3 Use AMHOLE to place the holes for the shutter release and the film advance.
Context Menu

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In the graphics area, right-click and choose Placed
Features ➤ Hole.

Chapter 20 Combining Parts and Surfaces

In the Hole dialog box, select the Counterbore hole type icon and specify:
Termination: Blind
Placement: 2 Edges
Dia: Enter .5
Depth: 1.0
Pt. Angle: Enter 180
C’Dia: Enter .65
C’Depth: Enter 1

Choose OK.
4 Respond to the prompts as follows:
Select the first edge: Select the top, back edge in the isometric view (1)
Select the second edge: Select the top, left edge in the isometric view (2)
Specify the hole location: Specify a location (3)
Enter the distance from first edge (highlighted) <0.4146>: Enter .5
Enter the distance from second edge (highlighted) <4.3456>: Enter 4.25
Select the first edge: Press ENTER
2
1
3

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599

A hole is created for the film advance component.

5 Press ENTER to redisplay the Hole Feature dialog box. Specify:
Operation: C’Bore
Termination: Blind
Placement 2 Edges
Drill Size: Custom, enter .2 diameter, 1.0 depth, and 180 degrees point angle
C’bore/Sunk Size: Enter .3 diameter and .1 depth and choose OK
6 Respond to the prompts as follows:
Select the first edge: Select the top, back edge in the isometric view
Select the second edge: Select the top, left edge in the isometric view
Specify the hole location: Specify a location
Enter the distance from first edge (highlighted) <0.6946>: Enter .85
Enter the distance from second edge (highlighted) <1.7487>: Enter 1.6
Select the first edge: Press ENTER
A hole is created for the shutter release mount.

Save your file.

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Chapter 20 Combining Parts and Surfaces

Creating Features on a Work Plane
The camera body is complete except for features on the camera face. Unlike
the previous features, you sketch these features on a work plane parallel to
the front of the camera. You extrude the features from the work plane and
into the camera body to the correct depth.
You sketch on the work plane because 2D sketches cannot be drawn and profiled on a NURBS surface.
The lens sheath, a hollow cylinder joined to the face of the camera, has two
features: a solid cylinder and a circle used to cut out the center of the
cylinder.
To extrude the lens sheath on a work plane
1 Use AMWORKPLN to create a new work plane on which to locate the sketch
plane.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Work Plane.

In the Work Plane Feature dialog box, specify:
1st Modifier: Planar Parallel
2nd Modifier: Offset
Offset: Enter 1.25
Create Sketch Plane: Select the check box
Choose OK.

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601

2 Respond to the prompts as follows:
Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:
Specify a point (1)
Enter an option [Next/Accept] :
Press ENTER when the front of the camera is selected
Enter an option [Flip/Accept] :
Verify that the work plane is offset from the camera front and press ENTER
Plane = Parametric
Select edge to align X axis or [Flip/Rotate/Origin] :
Point the Z axis away from the camera front and press ENTER
1

The work plane is created in front of the camera face. Because the sketch
plane is specified on the work plane, the UCS icon is also displayed on the
work plane.
3 Use CIRCLE to sketch a circle in front of the camera face. Work in the front
view.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Circle.

4 Use AMPROFILE to create the profile sketch.
Context Menu

602

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Chapter 20 Combining Parts and Surfaces

To position the circle, you need three dimensions or constraints: a diameter
and two dimensions to locate the circle on the sketch plane relative to the
camera body.
5 Use AMPARDIM to dimension the sketch with the following values.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

6 Use EXTRUDE to extrude the profile to create the outer cover of the lens
sheath. Work in the isometric view.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Join
Termination: Blind
Distance: Enter 1.25
Flip: Point the direction arrow into the camera body
Choose OK.

The lens sheath is complete. Now, cut a smaller cylinder to hollow out the
sheath.

Creating Features on a Work Plane

603

To hollow out the lens sheath
1 Activate the front view, and sketch a circle on the work plane.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Circle.

2 Profile the sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

Three dimensions or constraints are needed to solve the sketch.
3 Use AMADDCON to constrain the sketch to be concentric with the lens
sheath, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Concentric.

Valid selection(s): arc, circle, or ellipse
Select object to be reoriented: Select the small circle
Valid selection(s): arc, circle, ellipse, or work point
Select object to be made concentric to: Select the large circle
Solved underconstrained sketch requiring 1 dimensions or constraints.
Valid selection(s): arc, circle, or ellipse
Select object to be reoriented: Press ENTER
Enter an option
[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]
: Press ENTER
4 Use AMPARDIM to dimension the sketch to the value shown.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

5 Make the isometric view active and use AMEXTRUDE to extrude the sketch to
hollow out the lens sheath.
Context Menu

604

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

Chapter 20 Combining Parts and Surfaces

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Through
Flip: Point the direction arrow into the camera body
Choose OK.

Save your file.
Next, you create the viewfinder compartment, a filleted rectangle that is cut
from the camera face.
To cut the viewfinder compartment
1 Use RECTANG to sketch a rectangle on the sketch plane above the lens sheath.
Work in the isometric view.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

2 Use FILLET to define the fillet for the corners of the rectangle, responding to
the prompts.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.5000
Select first object or [Polyline/Radius/Trim]: Enter r
Specify fillet radius <0.5000>: Enter .1, and choose OK.
3 Press ENTER to restart FILLET. Apply the fillet, responding to the prompts.
Current settings: Mode = TRIM, Radius = 0.1000
Select first object or [Polyline/Radius/Trim]: Enter p
Select 2D polyline: Specify the rectangle

Creating Features on a Work Plane

605

4 Use AMPROFILE to create the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

You need five or more dimensions or constraints to solve the sketch. Add the
dimensions for the length and width of the shape, one dimension for the fillets, and two dimensions to locate the sketch in relationship to the camera
body.
5 In the front view, zoom in to enlarge the model as needed.
6 Use AMPARDIM to add the following dimensions.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

7 Use AMEXTRUDE to cut the sketch through the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Through
Flip: Point the direction arrow into the camera body
Choose OK.

The last feature is the flash compartment. It has a shape similar to the viewfinder but is larger and located in the upper-right corner of the camera face.

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Chapter 20 Combining Parts and Surfaces

To cut the flash compartment
1 Sketch a rectangle to the right of the viewfinder.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Rectangle.

2 Define a fillet for the corners of the rectangle, responding to the prompts.
Context Menu

In the graphics area, right-click and choose 2D Sketching
➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.5000
Select first object or [Polyline/Radius/Trim]: Enter r
Specify fillet radius <0.5000>: Enter .1
3 Press ENTER to restart FILLET. Apply the fillet, responding to the prompts.
Current settings: Mode = TRIM, Radius = 0.1000
Select first object or [Polyline/Radius/Trim]: Enter p
Select 2D polyline: Specify the rectangle
4 Create the profile sketch.
Context Menu

In the graphics area, right-click and choose Sketch Solving
➤ Single Profile.

You need five or more dimensions or constraints to solve the sketch, just as
you did when you sketched the viewfinder. Dimension the length, width,
and the fillets, and locate the sketch in relationship to the camera body.
Zoom in on the front view as needed.
5 Use AMADDCON to make the top and right edges of the sketch collinear with
the upper-right corner of the film compartment.
Context Menu

In the graphics area, right-click and choose 2D
Constraints ➤ Collinear.

Creating Features on a Work Plane

607

6 Add the following dimensions.
Context Menu

In the graphics area, right-click and choose Dimensioning
➤ New Dimension.

7 Extrude the sketch to cut it through the camera body.
Context Menu

In the graphics area, right-click and choose Sketched &
Work Features ➤ Extrude.

In the Extrusion dialog box, specify:
Operation: Cut
Termination: Through
Flip: Point the direction arrow into the camera body
Choose OK.

Save your file.

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Chapter 20 Combining Parts and Surfaces

Modifying Designs
As with all projects, designs change during the development process. For
example, you might want to scale the camera to a smaller size and change
the dimension that positions the camera face on the solid model. Because
you want both the surface and the camera body at the same scale, you first
resize them.
In this exercise, you specify a percentage of the camera’s current size. Then,
to position the surface on the camera proportionately, you modify the parametric dimension.
To scale the camera body and face
1 Zoom in to magnify the isometric view.
2 Use SCALE to reduce the scale of the part, responding to the prompts.
Desktop Menu

Modify ➤ Scale

Select objects: Select the camera and press ENTER
Specify base point: Select the rear corner of the camera
Specify scale factor or [Reference] <1.0000>: Enter .9 and press ENTER

full-scale camera body

scaled camera body

The camera and surface are resized to 90 percent of their original size. The
surface and other features retain their original geometric relationships.

Modifying Designs

609

To reposition the camera face
1 Use AMEDITFEAT to edit the surfcut feature, responding to the prompts.
Context Menu

In the graphics area, right-click and choose Edit Features
➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature]