Autodesk AutoCAD AutoCAD Mechanical Desktop - 6.0 Instruction Manual

Autodesk® Mechanical Desktop

User’s Guide

20507-010000-5020A May 3, 2001

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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

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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

iv | 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 | v

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

vi | 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 | ix

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

x | 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 | xi

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

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

and the migration of files

received with your Mechanical Desktop software. Information about training courseware

and Internet resources are also included.

2 |

Welcome

In This Chapter

This chapter provides an overview of the capabilities of

Autodesk

about the transition from AutoCAD

and the migration of files from previous releases with the

Mechanical Desktop Migration Assistance.

Mechanical Desktop® 6 software. You learn

, data exchange,

About Mechanical Desktop

■

■ Making the transition from

AutoCAD

■ Migrating files from previous

releases

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.

4 | 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

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

XREF, and XBIND commands could corrupt Mechanical Desktop data.

■ Use the Mechanical Desktop drawing view commands to create drawing

views. The AutoCAD

of your parts.

UCS command does not associate the current plane with

INSERT, WBLOCK,

MVIEW command does not create associative views

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 | 5

To install the Mechanical Desktop Migration Assistance from your product CD 1 Hold down the

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.

SHIFT key while you insert the product CD into the CD-ROM

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.

6 | Chapter 1 Welcome

Modeling with Autodesk® Mechanical Desktop

This chapter describes the basic concepts of mechanical

design with Autodesk Mechanical Desktop software,

including fundamentals of parametric design.

If you understand the underlying concepts in this chap-

ter, you can become proficient in using the Mechanical

Desktop software.

In This Chapter

Mechanical Desktop basics

■

■ Mechanical Desktop work

environments

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 drawin

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.

3D part

revolved feature

extruded feature

8 | Chapter 2 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 | 9

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

surface cut applied to a part

10 | Chapter 2 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 | 11

The User Interface

In This Chapter

When you start the Autodesk® Mechanical Desktop® 6

software, a page called the Today window is displayed.

This chapter provides an overview of the options on the

Today window to help manage your work, collaborate

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.

The Today window

■

■ Work environm e nts

■ Mechanical Desktop interface

■ Working in the Browser

■ Methods for issuing commands

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

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.

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.

14 | 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 exter-

nally 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 | 15

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.

16 | 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 repre-

senting 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 | 17

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.

18 | 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 | 19

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

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

Assembly Modeling environment

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.

20 | 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 | 21

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.

22 | 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 | 23

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.

24 | 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 | 25

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 while selecting the underlined letter of the menu option. For example, to

AMPROFILE from the keyboard, press ALT, then P, S, P.

select

ALT

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.

26 | Chapter 3 The User Interface

Documentation and Support

In This Chapter

This chapter provides an overview of the printed and

online documentation provided with Autodesk

Mechanical Desktop

product learning, training, and support.

Read this section so that any time you need product

information, you will know where to locate it.

6. It guides you to resources for

Mechanical Desktop print

■

documentation

■ Mechanical Desktop online

documentation

■ Product Support Assistance in

Help

■ Mechanical Desktop learning

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

■ AutoLISP

■ Visual LISP

■ DXF

■ Driver Peripheral Guide

■ Connectivity Automation Reference

■ Network Administrator’s Guide

and VBA Developer’s Guide*

and VBA Reference

Reference

Developer’s Guide*

Tutorial*

Reference

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 | 29

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 | 31

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

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

Tutorials

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.

34 |

Using the Tutorials

In This Chapter

This Introduction presents information that is useful to

know before you start performing the tutorials for

Autodesk

of how the tutorials are structured, and the methods

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.

Mechanical Desktop®. It provides a summary

Finding the right tutorial

■

■ Accessing commands

■ Controlling the appearance of

the Desktop Browser

■ Backing up tutorial files

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.

36 | 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.

Too lbutton New Part

Desktop Menu Part ➤ Part ➤ New Part

Command

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:

AMNEW to create a new part.

3 Use

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

AMNEW

Part.

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

Accessing Mechanical Desktop Commands | 37

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.

38 | 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 | 39

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.

40 | Chapter 5 Using the Tutorials

Creating Parametric Sketches

In This Chapter

Autodesk® Mechanical Desktop® automates your design

and revision process using parametric geometry.

Parametric geometry controls relationships among

design elements and automatically updates models and

drawings as they are refined.

The sketch is the basic design element that defines the

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

Analyzing a design and creating a

■

strategy for sketching

■ Text sketch profiles

■ Open profile sketches

■ Closed profile sketches

■ Path sketches

■ Cut line sketches

■ Split line sketches

■ Break line sketches

to learn how to add constraints to sketches.

Key Terms

Te r m Definition

2D constraint Defines how a sketch can change shape or size. Geometric constraints control the

closed loop A polyline entity, or group of lines and arcs that form a closed shape. Closed loops

closed profile A constrained sketch that is a cross section or boundary of a shape, such as an

construction geometry Any line or arc created with a noncontinuous linetype. Using construction

cut line Used to specify the path of a cross-section drawing view. Unlike a profile sketch,

feature An element of a parametric part model. You can create extruded features,

nested loop A closed loop that lies within the boundary of another closed loop. Nested loops

open profile A profile created from one or more line segments sketched to form an open

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

shape and relationships among sketch lines and arcs. Dimensional constraints

control the size of sketch geometry.

are used to create profile sketches.

extrusion, a revolved feature, or a swept feature.

geometry in paths and profiles may mean fewer constraints and dimensions are

needed to control size and shape of symmetrical or geometrically consistent

sketches.

the cut line sketch is not a closed loop. There are two types of cut line sketches—

offset and aligned.

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.

are used to create more complex profile sketches.

shape. Open profiles are used in bend, rib, and thin wall features.

sketch A planar collection of points, lines, arcs, and polylines used to form a profile, path,

sketch tolerance Tolerance setting that closes gaps smaller than the pickbox and snaps lines to

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

text sketch profile A profile created from a single line of text in a selected font and style. Text-based

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.

horizontal, vertical, parallel, or perpendicular.

known as a parting line.

profiles are used to emboss parts with text.

42 | 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, “Constrain- ing Sketches,” introduces you to creating, modifying, and deleting the con- straints and parametric dimensions that control a sketch.

Basic Concepts of Parametric Sketching | 43

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

Repeat simple shapes If a design has repeating elements, sketch one and then copy or

Define a sketching layer

Preset sketch tolerances

Draw sketches to size When your sketches are roughly correct in size and shape, your

Use PLINE Whenever possible, use the PLINE command to create your

sketch. Combine simple sketches for complex shapes.

array as needed.

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.

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

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.

sketches. With PLINE, you can easily draw tangent lines and arcs.

44 | 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 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.

AMTEXTSK. A dialog box

Creating Profile Sketches | 45

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 rib featureprofile for bend 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.

profile for thin feature

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

■ Self-intersecting

■ Intersecting

■ Tangential

■ Nested more than one level deep

46 | Chapter 6 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 | 47

To create a profile sketch from multiple objects

LINE to draw this shape, entering the points in the order shown.

1 Use

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

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)

911

You do not need to use

OSNAP to connect the arc to the endpoints of the

lines.

48 | 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 | 49

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.

AMSHOWCON to show the existing constraints, following the prompt.

4 Use

Context Menu In the graphics area, right-click and choose 2D

Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] <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).

50 | 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] <eXit>: Press

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.

ENTER

Using Custom Sketch Rules

Custom settings affect how Mechanical Desktop analyzes rough sketches. In this exercise, you sketch with sketch. You will modify one of the Mechanical Options sketch rule settings and see its effect on the sketch.

PLINE and convert your drawing to a profile

rough sketch profile sketch

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

Creating Profile Sketches | 51

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 <PART2>: 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)

52 | Chapter 6 Creating Parametric Sketches

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

AMPROFILE to create a profile sketch from the rough sketch.

3 Use

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 | 53

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.

54 | 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 | 55

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

AMNEW to create a new part definition.

1 Use

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.

56 | 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

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 | 57

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.

The geometry for the 2D path must be created on the same plane.

swept featurepath sketch profile sketch

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.

58 | 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 | 59

5 Use AM2DPATH to convert the rough sketch to a path sketch, following the

prompts. Context Menu In the graphics area, right-click and choose Sketch Solving

➤ 2D Path.

Select objects: Specify the polyline shape Select objects: 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] <Yes>: 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.

60 | 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.

AMSHOWCON to display the existing constraints, responding to the

6 Use

prompt. Context Menu In the graphics area, right-click and choose 2D

Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] <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] <eXit>: Press

ENTER

Save your file.

Next, you create a three-dimensional path.

Creating Path Sketches | 61

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 3D sweep along edge path

62 | Chapter 6 Creating Parametric Sketches

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 [?] <PART1_1>: 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] <Yes>: Press

ENTER

The command method you use determines the prompts that are displayed.

Creating Path Sketches | 63

2 Continue on the command line to place the work plane.

Plane=Parametric Select edge to align X axis or [Flip/Rotate/Origin] <accept>: 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.

64 | 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

rofile sketch

3D helical swee

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 [?] <PART1_1>: 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 | 65

To create a 3D helical path

AM3DPATH to define the 3D helical path, responding to the prompts.

3 Use

Context Menu In the graphics area, right-click and choose Sketch Solving

➤ 3D Helix Path.

Enter path type [Helical/Spline/Edge/Pipe] <Edge>: 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.

66 | 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 | 67

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

AM3DPATH to define the 3D pipe path, responding to the prompts.

1 Use

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.

68 | 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] <accept>: Press

The Desktop Browser now contains a 3D Pipe icon, a work plane, and a work point nested below the PART3_1 definition.

ENTER

Save your file.

Creating Path Sketches | 69

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

AM3DPATH to define the 3D spline path, responding to the prompts.

1 Use

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.

70 | Chapter 6 Creating Parametric Sketches

2 In the 3D Spline Path dialog box, examine the vertices of the spline, and ver-

ify 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] <accept>: 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 | 71

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.

section viewoffset cut line section viewaligned cut line

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:

■ 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.

72 | Chapter 6 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 | 73

To create an offset cut line sketch

PLINE to sketch through the center of the holes on the square part.

1 Use

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

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

Save your file.

74 | 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 | 75

To create an aligned cut line sketch

PLINE to sketch through the centers of two of the holes on the circular

1 Use

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

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.

76 | 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 | 77

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] <Accept>: Press

ENTER

Plane = Parametric Select edge to align X axis [Flip/Rotate/Origin] <accept>: Press

ENTER

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

78 | 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.

AMSPLITLINE to create a split line from your sketch, responding to the

4 Use

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 <ENTER> 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 | 79

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.

80 | Chapter 6 Creating Parametric Sketches

To create a break line

AMBREAKLINE to define the break line sketch, following the prompts.

1 Use

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 | 81

Constraining Sketches

In This Chapter

When you solve a sketch in Autodesk® Mechanical

Desktop

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.

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.

, geometric constraints are applied in

Creating a strategy for

■

constraining and dimensioning

■ 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

In the next chapter, you learn to add sketched features

to your constrained sketches.

Key Terms

Te r m Definition

2D constraint Defines how a sketch can change shape or size. Geometric constraints control the

degree of freedom In part modeling, determines how a geometric object such as a line, arc, or circle

dimensional constraint Parametric dimension that controls the size of a sketch. When changed, the

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

shape and relationships among sketch lines and arcs. Dimensional constraints

control the size of sketch geometry.

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.

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 configuration of the part.

84 | 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 | 85

Constraining Tips

Tip Explanation

Determine sketch dependencies

Analyze automatically applied constraints

Use only needed constraints

Stabilize shape before size

Dimension large before small

Use both geometric constraints and dimensions

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

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.

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

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

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.

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.

86 | Chapter 7 Constraining Sketches

Autodesk AutoCAD AutoCAD Mechanical Desktop - 6.0 Instruction Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

Welcome

What is Autodesk Mechanical Desktop?

Making the Transition from AutoCAD

Migrating Files from Previous Releases

Data Exchange

Mechanical Desktop Basics

The User Interface

Mechanical Desktop Today

Mechanical Desktop Environments

Assembly Modeling Environment

Part Modeling Environment

Mechanical Desktop Interface

Desktop Browser

Issuing Commands

Documentation and Support

Printed and Online Manuals

Mechanical Desktop Printed Manual

AutoCAD Printed Manual

Online Installation Guide

AutoCAD 2002 Documentation

Mechanical Desktop Help

Updating Help Files

Product Support Assistance in Help

Updating the Support Assistance Knowledge Base

Learning and Training Resources

Internet Resources

Using the Tutorials

How the Tutorials are Organized

Accessing Mechanical Desktop Commands

Positioning the Desktop Browser

Backing up Tutorial Drawing Files

Creating Parametric Sketches

Key Terms

Basic Concepts of Parametric Sketching

Sketching Tips

Creating Profile Sketches

Creating Text Sketch Profiles

Creating Open Profile Sketches

Creating Closed Profile Sketches

Using Default Sketch Rules

Using Custom Sketch Rules

Using Nested Loops

Creating Path Sketches

Creating 2D Path Sketches

Creating 3D Path Sketches

Creating Cut Line Sketches

Creating Split Line Sketches

Creating Break Line Sketches

Constraining Sketches

Key Terms

Basic Concepts of Creating Constraints

Constraining Tips

Constraining Sketches