Autodesk Auto CAD Mechanical Desktop 6.0 Instruction Manual Autocad 6 En

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

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Getting Started with Autodesk® Mechanical Desktop®
Autodesk® Mechanical Desktop® Tutorials

Autodesk® Mechanical Desktop®

User’s Guide

20507-010000-5020A May 3, 2001

12345678910

This publication, or parts thereof, may not be reproduced in any form, by any method, for any purpose.

AUTODESK, INC. MAKES NO WARRANTY, EITHER EXPRESSED OR IMPLIED, INCLUDING BUT NOT LIMITED TO ANY IMPLIED

WARRANTIES OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE, REGARDING THESE MATERIALS AND MAKES

SUCH MATERIALS AVAILABLE SOLELY ON AN “AS-IS” BASIS.

IN NO EVENT SHALL AUTODESK, INC. BE LIABLE TO ANYONE FOR SPECIAL, COLLATERAL, INCIDENTAL, OR CONSEQUENTIAL

DAMAGES IN CONNECTION WITH OR ARISING OUT OF PURCHASE OR USE OF THESE MATERIALS. THE SOLE AND EXCLUSIVE

LIABILITY TO AUTODESK, INC., REGARDLESS OF THE FORM OF ACTION, SHALL NOT EXCEED THE PURCHASE PRICE OF THE

MATERIALS DESCRIBED HEREIN.

Autodesk, Inc. reserves the right to revise and improve its products as it sees fit. This publication describes the state of this product at the time of its publication,

and may not reflect the product at all times in the future.

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iii

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

iv |Contents

Mechanical Desktop Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30

Updating Help Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30

Product Support Assistance in Help. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31

Updating the Support Assistance Knowledge Base. . . . . . . . . . . . . . .31

Learning and Training Resources. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31

Internet Resources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .32

Part I Autodesk®

Mechanical Desktop®

Tutorials. . . . . . . . . . 33

Chapter 5 Using the Tutorials . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

How the Tutorials are Organized . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .36

Accessing Mechanical Desktop Commands. . . . . . . . . . . . . . . . . . . . . . . . .37

Positioning the Desktop Browser . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .38

Backing up Tutorial Drawing Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .40

Chapter 6 Creating Parametric Sketches. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .42

Basic Concepts of Parametric Sketching . . . . . . . . . . . . . . . . . . . . . . . . . . .43

Sketching Tips . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .44

Creating Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .45

Creating Text Sketch Profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .45

Creating Open Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . .46

Creating Closed Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . .46

Using Default Sketch Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .47

Using Custom Sketch Rules . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .51

Using Nested Loops. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .56

Creating Path Sketches. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .58

Creating 2D Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .58

Creating 3D Path Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .62

Creating Cut Line Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .72

Creating Split Line Sketches. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .77

Creating Break Line Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .80

Chapter 7 Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .84

Basic Concepts of Creating Constraints. . . . . . . . . . . . . . . . . . . . . . . . . . . .85

Constraining Tips. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .86

Constraining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .86

Contents |v

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

vi |Contents

Chapter 9 Creating Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .168

Basic Concepts of Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .169

Creating Work Planes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .170

Editing Work Planes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .173

Creating Work Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .174

Editing Work Axes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .177

Creating Work Points. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .179

Editing Work Points . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .182

Chapter 10 Creating Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 185

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .186

Basic Concepts of Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .187

Creating Hole Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .188

Creating Thread Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .190

Editing Hole Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .192

Editing Thread Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .193

Creating Face Drafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .194

Editing Face Drafts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .198

Creating Fillet Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .199

Editing Fillet Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .202

Creating Chamfer Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .204

Editing Chamfer Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .208

Creating Shell Features. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .209

Editing Shell Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .210

Creating Surface Cut Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .212

Editing Surface Cut Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .213

Creating Pattern Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .214

Editing Pattern Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .223

Editing Array Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .223

Creating Copied Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .224

Editing Copied Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .227

Creating Combined Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .227

Editing Combined Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .228

Creating Part Splits. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .229

Editing Part Splits . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .231

Chapter 11 Using Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 233

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .234

Basic Concepts of Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .235

Preparing The Drawing File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .236

Contents |vii

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

viii |Contents

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

Contents |ix

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

x|Contents

Creating Bills of Material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .522

Customizing BOM Databases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .523

Working with Part References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .525

Adding Balloons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .527

Placing Parts Lists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .529

Finishing Drawings for Plotting. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .531

Chapter 19 Creating and Editing Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . 533

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .534

Basic Concepts of Creating Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . .535

Working with Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .536

Creating Motion-Based Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .538

Revolved Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .538

Extruded Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .539

Swept Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .540

Creating Skin Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .546

Ruled Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .546

Trimmed Planar Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .554

Lofted Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .555

Creating Derived Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .559

Blended Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .559

Offset Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .563

Fillet and Corner Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .565

Editing Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .569

Adjusting Adjacent Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .569

Joining Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .570

Trimming Intersecting Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . .571

Trimming Surfaces by Projection . . . . . . . . . . . . . . . . . . . . . . . . . . .573

Chapter 20 Combining Parts and Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . 575

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .576

Basic Concepts of Combining Parts and Surfaces . . . . . . . . . . . . . . . . . . .577

Using Surface Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .577

Creating Surface Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .579

Attaching Surfaces Parametrically . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .582

Cutting Parts with Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .584

Creating Extruded Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .586

Creating Holes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .598

Creating Features on a Work Plane . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .601

Modifying Designs . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .609

Finishing Touches on Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .611

Contents |xi

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

xii |Contents

Chapter 24 Calculating Stress on 3D Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 707

Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .708

Tutorial at a Glance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709

Basic Concepts of 3D FEA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709

Using 3D FEA Calculations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .710

Performing Finite Element Analyses. . . . . . . . . . . . . . . . . . . . . . . . .710

Defining Supports and Forces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .711

Calculating and Displaying the Result . . . . . . . . . . . . . . . . . . . . . . .715

Desktop Tools. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .720

Part Modeling. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .721

Part Modeling ➤ New Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .721

Part Modeling ➤ New Sketch Plane . . . . . . . . . . . . . . . . . . . . . . . . .722

Part Modeling ➤ 2D Sketching. . . . . . . . . . . . . . . . . . . . . . . . . . . . .722

Part Modeling ➤ 2D Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . .725

Part Modeling ➤ Profile a Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . .726

Part Modeling ➤ Sketched Features . . . . . . . . . . . . . . . . . . . . . . . . .727

Part Modeling ➤ Placed Features . . . . . . . . . . . . . . . . . . . . . . . . . . .727

Part Modeling ➤ Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . .727

Part Modeling ➤ Power Dimensioning . . . . . . . . . . . . . . . . . . . . . .728

Part Modeling ➤ Edit Feature . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .728

Part Modeling ➤ Update Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .728

Part Modeling ➤ Part Visibility . . . . . . . . . . . . . . . . . . . . . . . . . . . .729

Part Modeling ➤ Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .729

Toolbody Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .730

Toolbody Modeling ➤ New Toolbody . . . . . . . . . . . . . . . . . . . . . . .730

Toolbody Modeling ➤ Part Catalog . . . . . . . . . . . . . . . . . . . . . . . . .730

Toolbody Modeling ➤ 3D Toolbody Constraints . . . . . . . . . . . . . .731

Toolbody Modeling ➤ Power Manipulator . . . . . . . . . . . . . . . . . . .731

Toolbody Modeling ➤ Check Interference. . . . . . . . . . . . . . . . . . . .731

Toolbody Modeling ➤ Toolbody Visibility . . . . . . . . . . . . . . . . . . .732

Assembly Modeling . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .732

Assembly Modeling ➤ New Subassembly. . . . . . . . . . . . . . . . . . . . .733

Assembly Modeling ➤ Assembly Catalog. . . . . . . . . . . . . . . . . . . . .733

Assembly Modeling ➤ 3D Assembly Constraints. . . . . . . . . . . . . . .733

Assembly Modeling ➤ Assign Attributes . . . . . . . . . . . . . . . . . . . . .734

Assembly Modeling ➤ Power Manipulator . . . . . . . . . . . . . . . . . . .734

Assembly Modeling ➤ Mass Properties. . . . . . . . . . . . . . . . . . . . . . .734

Assembly Modeling ➤ Assembly Visibility. . . . . . . . . . . . . . . . . . . .734

Contents |xiii

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

xiv

Part I

Getting Started

with Autodesk®

Mechanical Desktop®

Part I provides information for getting started with your Mechanical Desktop 6 software. It

includes information to help in the transition from AutoCAD® and the migration of files

from previous releases. It explains the user interface and the basics of modeling in the

different work environments in Mechanical Desktop.

In addition, Part I provides a guide to both the print and online documentation that you

received with your Mechanical Desktop software. Information about training courseware

and Internet resources are also included.

In This Chapter 1

Welcome

This chapter provides an overview of the capabilities of

Autodesk® Mechanical Desktop® 6 software. You learn

about the transition from AutoCAD®, data exchange,

and the migration of files from previous releases with the

Mechanical Desktop Migration Assistance.

■About Mechanical Desktop

■Making the transition from

AutoCAD

■Migrating files from previous

releases

4|Chapter 1 Welcome

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.

Making the Transition from AutoCAD |5

Making the Transition from AutoCAD

Mechanical Desktop 6 is built on AutoCAD 2002 and uses many of the tools

you may already be familiar with. Because Mechanical Desktop is a parametric

modeling program, exercise care in using standard AutoCAD commands.

In the sketching stage, you can use any AutoCAD command to create the

geometry for your sketch. You can use AutoCAD drawing and editing tools

to edit sketch geometry after it has been consumed by a feature.

In general, follow these rules:

■Use Mechanical Desktop dimensions. AutoCAD dimensions are not

parametric and cannot control the size, shape, or position of Mechanical

Desktop parts and features.

■Use sketch planes and work planes to control the UCS orientation. Using

the AutoCAD UCS command does not associate the current plane with

your part.

■Do not use the command EXPLODE. Exploding a part deletes the part

definition from a Mechanical Desktop drawing.

■Use the Assembly Catalog or the Browser to insert external part files into

drawings and externalize part files. Using the AutoCAD INSERT, WBLOCK,

XREF, and XBIND commands could corrupt Mechanical Desktop data.

■Use the Mechanical Desktop drawing view commands to create drawing

views. The AutoCAD MVIEW command does not create associative views

of your parts.

Migrating Files from Previous Releases

In Mechanical Desktop 6, you can add more than one part to a part file for

creating combined parts. The first part becomes the part definition, while all

other parts become unconsumed toolbodies. You combine toolbodies with

each other and the first part to create a complex part.

To migrate parts from a part file that contains more than one part and was

created before Mechanical Desktop Release 2, you need to follow specific

procedures. See "Running the Desktop File Migration Utility" in the Autodesk

Mechanical Products Installation Guide on the product CD.

The File Migration Tool (FMT) is a component of Mechanical Desktop

Migration Assistance, an independent Visual Basic (not VBA) application

located on your product CD. The FMT migrates multiple files from previous

releases of Mechanical Desktop to the current format. You can install

Mechanical Desktop Migration Assistance during or after the installation of

your Autodesk mechanical product.

6|Chapter 1 Welcome

To install the Mechanical Desktop Migration Assistance from your product CD

1Hold down the SHIFT key while you insert the product CD into the CD-ROM

drive. This prevents Setup from starting automatically.

2In the file tree of the CD-ROM drive, navigate to the Migrate folder and click

setup.exe.

3Respond to the directions in the Mechanical Desktop Migration Assistance

installation dialog boxes.

NOTE For more information about installing the Migration Assistance and

running the FMT, see "Mechanical Desktop Migration Assistance" in the

Autodesk Mechanical Products Installation Guide on your product CD.

Data Exchange

During your design process, you may want to complement Mechanical

Desktop with other computer-aided design (CAD) software. Mechanical

Desktop 6 includes the STEP translator and the IGES Translator. The Standard

for the Exchange of Product Model Data (STEP) is International Standards

Organization (ISO) 10303. The Initial Graphics Exchange Specification

(IGES) is the ANSI standard for data exchange between CAD systems and is

supported by many CAD vendors.

The IGES Translator is compliant with the most recent version of IGES and

related standards. It supports both the United States Department of Defense

Continuous Acquisition and Life-cycle Support initiative (CALS) and the Japa-

nese 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.

In This Chapter 2

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.

■Mechanical Desktop basics

■Mechanical Desktop work

environments

8|Chapter 2 Modeling with Autodesk Mechanical Desktop

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.

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.

You build parts from features—the basic shapes of your part.

Building blocks like extrusions, lofts, sweeps, bends, holes, fillets, and cham-

fers are parametrically combined to create your part.

2D drawin

art

original part revised part

extruded feature

revolved feature

Mechanical Desktop Basics |9

You create most features from sketches.

Sketches can be extruded, revolved, lofted, or swept along a path to create

features.

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.

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.

sketch for revolved feature sketch for extruded feature

examples of single part files

assembly file containing four external part files

10 |Chapter 2 Modeling with Autodesk Mechanical Desktop

Individual parts can be fit together to create subassemblies and assemblies.

Assembly files contain more than one part. Parts are fit together using assem-

bly constraints to define the positions of the individual parts that make up

your final product.

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 ver-

sions of that part in a spreadsheet that is linked to your drawing.

You can also create 3D surface models.

Surface modeling is useful in the design of stamping dies, castings, or injec-

tion molds. You can also use surfaces to add to or cut material from a solid

part to create hybrid shapes.

individual parts in an assembly file completed assembly

table driven part versions

surfaces used to create a part surface cut applied to a part

Mechanical Desktop Basics |11

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.

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.

Add annotations and additional dimensions to finalize your documentation.

After you have created drawing views, finalize your design by adding bal-

loons, bills of material, notes, reference dimensions, and mechanical

symbols.

exploded scene

parametric drawing views

annotations added to drawing

In This Chapter 3

The User Interface

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 environments

■Mechanical Desktop interface

■Working in the Browser

■Methods for issuing commands

14 |Chapter 3 The User Interface

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 draw-

ings, communicate with design teams, and link directly to design information.

In the Today Window, you can expand the following options for access to the

the services you require.

My Workplace Connect directly to files on your computer and your local

network.

My Drawings Open existing drawings, create new ones, or access

symbol libraries.

Bulletin Board Post your own Web page with links to block libraries, CAD

standards, or other folders and directories on your

company network. CAD managers can use the Bulletin

Board to communicate with their design teams. An HTML

bulletin board template is provided.

The Web Connect directly to the Internet.

Autodesk

Point A

Link directly to design information and tools such as

Buzzsaw.com on the Web. Use the units converter, link to

Autodesk Web sites, and much more.

information in Autodesk Point A for your specific needs.

You can close the Today Window and use the File menu to create new draw-

ings 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.

Mechanical Desktop Environments |15

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, subassem-

blies, 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.

16 |Chapter 3 The User Interface

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 paramet-

ric 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.

Mechanical Desktop Interface |17

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

Desktop Browser

Part Modeling toolbar

Mechanical Main toolbar

Mechanical View toolbar

Help

18 |Chapter 3 The User Interface

There are four main toolbars controlled by the Desktop Tools toolbar: Part

Modeling, Assembly Modeling, Scene, and 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.

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.

Part Modeling

Assembly Modeling

Scene

Drawing Layout

Toolbody Modeling

Part Modeling

Mechanical Desktop Interface |19

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.

20 |Chapter 3 The User Interface

You collapse levels by clicking the minus sign beside an object, or collapse

the entire hierarchy by right-clicking the assembly name and choosing

Collapse from the menu.

When you start a new drawing in the Part Modeling environment, or open

an existing part file, the Desktop Browser contains two tabs: Model and

Drawing. In the Assembly Modeling environment, the Browser contains

three tabs: Model, Scene, and Drawing. You can choose the tabs at the top of

the Browser window to navigate from one mode to another.

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

commands.

Using the Browser in Part Modeling

When you are working in the Part Modeling environment, the Browser

contains two tabs: Model and Drawing.

Model Mode in Part Modeling

In Model mode, seven icons are displayed at the bottom of the Browser.

The two at the left are quick filters. These filters are available so that you can

control the visibility of features and assembly constraints in the Browser

when you are creating combined parts.

Part Modeling environment Assembly Modeling environment

Mechanical Desktop Interface |21

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.

22 |Chapter 3 The User Interface

Using the Browser in Assembly Modeling

In the Assembly Modeling environment, the Browser displays three tabs:

Model, Scene, and Drawing. With these tabs, you can create multiple parts,

assemblies, scenes, BOMs, and documents, and you can reorder assemblies.

You can localize and externalize parts in the Browser without opening the

Assembly Catalog.

Model Mode in Assembly Modeling

Model mode in the Assembly Modeling environment has the same icons at

the bottom of the Browser as Model mode in the Part Modeling environment.

Because you are working in the Assembly environment, these icons provide

more functionality.

The first icon is the Part filter which you use to control the display of the

features that make up your parts. If the Part filter is selected, only part

features are visible in the Browser. If it is not selected, assembly constraints

are also visible.

The second icon is the Assembly filter. When you select this filter, only the

assembly constraints attached to your parts are visible.

The third icon opens the Mechanical Options dialog box. From this dialog

box you can manage your settings and standards for parts, assemblies,

surfaces, drawings, shaft generators, calculations, standard parts, and various

desktop preferences.

The middle icon provides access to the Assembly Catalog, a powerful inter-

face 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.

Mechanical Desktop Interface |23

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.

24 |Chapter 3 The User Interface

Issuing Commands

You can issue commands in several ways:

■Select an option from a right-click menu in the Desktop Browser.

■Select an option from a right-click menu in the active screen area of your

drawing.

■Select a toolbar icon.

■Select an option from a pull-down menu.

■Enter the command name on the command line.

■Use an abbreviation of the command, called an accelerator key, on the

command line.

Using Command Menus in the Desktop Browser

Many of the commands in Mechanical Desktop can be accessed using the

Browser menus. The Browser has two types of menus. One you activate by

right-clicking an existing object in the Browser. The other you activate by

right-clicking the Browser background. Options that are not available are gray.

The type of object you select with a right-click determines the menu displayed.

The mode you are in, Model, Scene, or Drawing, when you right-click the

Browser background determines the menu displayed.

Mechanical Desktop Interface |25

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.

26 |Chapter 3 The User Interface

Using Pull-down Menus

To select a menu option, or access a submenu, hold down the left mouse

button while you navigate through the menu. When you find the command

you want to use, release the mouse button.

You can also access menu commands by using the keyboard. Hold down ALT

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

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

Selecting Command Options from Dialog Boxes

Many commands have options within dialog boxes. As the term dialog box

suggests, you interact by selecting options to make a particular setting active,

display a list from which to choose an option, or enter a specific value. If a

command has a dialog box, it is displayed when you access the command,

regardless of whether you did so on the command line or from a menu or

toolbar icon.

When you need information about a dialog box you are working with, click

the Help button located in the dialog box.

NOTE If the Mechanical Desktop dialog boxes do not display, on the

command line enter CMDDIA, and change the system variable to 1.

Using the Command Line

You can access a command or system variable directly by entering its name

on the command line. Many experienced users prefer this method because it

is faster than using menus. Some experienced users are familiar with specify-

ing 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.

In This Chapter 4

Documentation and

Support

This chapter provides an overview of the printed and

online documentation provided with Autodesk®

Mechanical Desktop® 6. It guides you to resources for

product learning, training, and support.

Read this section so that any time you need product

information, you will know where to locate it.

■Mechanical Desktop print

documentation

■Mechanical Desktop online

documentation

■Product Support Assistance in

Help

■Mechanical Desktop learning

and training

■Your Internet resources

28 |Chapter 4 Documentation and Support

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.

Printed and Online Manuals |29

Chapter 2 Procedures to install, upgrade, authorize, and maintain

the software for a single user, and information you need

to know before you begin your installation.

Chapter 3 Information for network administrators. Instructions for

installing and configuring for a network environment.

Chapter 4 Technical information about environment variables and

performance enhancements to optimize performance of

the software.

Chapter 5 Information about cabling and option settings, plus other

information necessary to link and configure plotters and

printers with AutoCAD Mechanical/Mechanical Desktop.

Chapter 6 Instructions to uninstall the software, maintain your hard

disk, and recover data in case of a system failure.

AutoCAD 2002 Documentation

You should be familiar with AutoCAD before you use Mechanical Desktop.

The complete set of AutoCAD 2002 documentation is available in the

AutoCAD Help. It includes:

■User’s Guide*

■Command Reference*

■Customization Guide*

■ActiveX® and VBA Developer’s Guide*

■ActiveX® and VBA Reference

■AutoLISP® Reference

■Visual LISPTM Developer’s Guide*

■Visual LISPTM Tutorial*

■DXFTM Reference

■Driver Peripheral Guide

■Connectivity Automation Reference

■Network Administrator’s Guide

AutoCAD 2002 manuals marked with an asterisk can be ordered in print from

your local reseller.

The AutoCAD 2002 Learning Assistance CD that is included in your package

is a multimedia learning tool for intermediate to experienced AutoCAD users.

If you currently own a valid license for an Autodesk product and require

replacement media or documentation, please call the Customer Service

Center at 1-800-538-6401 to order.

30 |Chapter 4 Documentation and Support

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

1In Mechanical Desktop Today, choose Autodesk Point A. In Useful Autodesk

Links, choose Autodesk Product Support Index.

2Follow the links to Mechanical Desktop 6 product support and updates.

Product Support Assistance in Help |31

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 informa-

tion 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

1From the Help menu, choose Support Assistance, then choose Download.

2Follow 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.

32 |Chapter 4 Documentation and Support

Internet Resources

Following are resources for information about Autodesk products and assis-

tance 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.

Part II

Autodesk® Mechanical

Desktop® Tutorials

The tutorials in this section teach you how to use Mechanical Desktop 6, and provide a

comprehensive overview of mechanical design. The lessons range from basic to advanced,

and include step-by-step instructions and helpful illustrations.

You learn how to create parts, surfaces, assemblies, table driven parts, and bills of material.

You will also learn how to prepare your designs for final documentation. Specific drawing

files for each lesson are included with the program. These drawing files provide design

elements that help you understand and learn mechanical design concepts.

There are lessons designed for learning to model with Mechanical Desktop, and others

designed specifically for learning to use Mechanical Desktop with the power pack.

34 |

In This Chapter 5

Using the Tutorials

This Introduction presents information that is useful to

know before you start performing the tutorials for

Autodesk® Mechanical Desktop®. It provides a summary

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.

■Finding the right tutorial

■Accessing commands

■Controlling the appearance of

the Desktop Browser

■Backing up tutorial files

36 |Chapter 5 Using the Tutorials

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 mod-

eling, assembly modeling, and surface modeling.

For best results, run Mechanical Desktop 6 to perform the tutorials in chap-

ters 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 doc-

ument 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 learn-

ing how to create and edit different types of surfaces. Then you create a sur-

face 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.

Accessing Mechanical Desktop Commands |37

Accessing Mechanical Desktop Commands

Mechanical Desktop provides several methods to access commands and

manage your design process.

The following are samples of the access methods available to you:

Browser Right-click the window background and choose New Part.

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

Part.

Toolbutton New Part

Desktop Menu Part ➤ Part ➤ New Part

Command AMNEW

The step-by-step procedures in the tutorials indicate the command name in

the opening procedural text. The appropriate toolbutton is displayed in the

margin next to the preferred access method. In the tutorials, the context

menu method is used when the menus are sensitive to what you are doing.

The Browser method is used when you can save time and steps. You can use

any of the alternate methods as well.

If you are in Model mode, you can toggle between the Part and Assembly

context menus. If you are in Scene mode, the Scene menu is available. When

you are working in Drawing mode, you can toggle between the Drawing and

Annotate context menus.

Here is an example of how methods are used in the tutorials:

3Use AMNEW to create a new part.

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

Part.

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

38 |Chapter 5 Using the Tutorials

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 follow-

ing 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 cur-

sor 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.

Positioning the Desktop Browser |39

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.

40 |Chapter 5 Using the Tutorials

Backing up Tutorial Drawing Files

For each tutorial, you use one or more of the master drawing files that con-

tain 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

1From the Windows Start menu, choose Programs ➤ Windows Explorer.

2In the folder where Mechanical Desktop is installed (by default this is Program

Files\Mdt\desktop), choose File ➤ New ➤ Folder.

3Create a new folder called tutorial backup.

4Open 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.

In This Chapter 6

Creating Parametric

Sketches

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

to learn how to add constraints to sketches.

■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

42 |Chapter 6 Creating Parametric Sketches

Key Terms

Te r m Definition

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

shape and relationships among sketch lines and arcs. Dimensional constraints

control the size of sketch geometry.

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

are used to create profile sketches.

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

extrusion, a revolved feature, or a swept feature.

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

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

needed to control size and shape of symmetrical or geometrically consistent

sketches.

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

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

offset and aligned.

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

revolved features, loft features, and swept features using profiles and paths. You

can also create placed features like holes, chamfers, and fillets. You combine

features to create complete parametric part models.

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

are used to create more complex profile sketches.

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

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

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

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

split line, break line, or cutting line. An unconstrained sketch contains geometry

and occasionally dimensions. A constrained sketch, such as a profile, path, split

line, cut line, or break line that contains “real” and construction geometry, and is

controlled by dimensions and geometric constraints.

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

horizontal, vertical, parallel, or perpendicular.

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

known as a parting line.

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

profiles are used to emboss parts with text.

Basic Concepts of Parametric Sketching |43

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 para-

metric 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 mul-

tiple 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.

44 |Chapter 6 Creating Parametric Sketches

Sketching Tips

Some of these tips do not apply to this chapter, but you will see their useful-

ness when you use sketches to create complex parts.

Tip Explanation

Keep sketches simple It is easier to work with a single object than a multiple-object

sketch. Combine simple sketches for complex shapes.

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

array as needed.

Define a sketching

layer Specify a separate layer and color for sketching. Your sketch is

visible with other part geometry but easy to identify when you

need to modify it.

Preset sketch

tolerances Define characteristics, such as sketch precision and angular

tolerance of sketch lines, if the default values are not sufficient.

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

design is less likely to become distorted as dimensions or

constraints are added. Sketch a rectangle to serve as a boundary

for the base feature to set relative size. Sketch the feature, but

delete the rectangle before you create a profile.

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

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

Creating Profile Sketches |45

Creating Profile Sketches

In Mechanical Desktop, there are three types of profile sketches:

■Text-based profiles, used to create parametric 3D text-based shapes

■Open profile sketches, used to define features on parts

■Closed profile sketches, used to outline parts and features

You can solve and apply parametric constraints and dimensions to all three

of these profile sketch types.

Creating Text Sketch Profiles

A text sketch profile is a line of text displayed in a rectangular boundary. You

extrude a text sketch profile to create the emboss feature on part models.

To create a text sketch profile, you use the command AMTEXTSK. A dialog box

opens where you can enter text and choose a font style and size, or you can

enter the information on the command line.

You define an anchor point for the rectangle on your part and a point to

define the height of the text. You have the option to define a rotation value

on the command line to position the text at an angle. As you move your cur-

sor 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.

To learn more about using text sketch profiles in the emboss feature, see

“Creating Emboss Features” on page 140.

text sketch text sketch with rotation defined

46 |Chapter 6 Creating Parametric Sketches

Creating Open Profile Sketches

You can create an open profile from single or multiple line segments, and

solve it in the same way as you solve a closed profile.

An open profile constructed with one line segment is used to define the loca-

tion 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.

To learn more about open profiles in features, see “Creating Bend Features”

on page 163, “Creating Rib Features” on page 133, and “Creating Thin Fea-

tures” on page 136.

Creating Closed Profile Sketches

A profile sketch is a two-dimensional outline of a feature. Closed profile

sketches are continuous shapes, called loops, that you construct from lines,

arcs, and polylines. You use closed profile sketches to create features with cus-

tom 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

profile for rib featureprofile for bend feature profile for thin feature

Creating Profile Sketches |47

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.

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.

rough sketch profile sketch

48 |Chapter 6 Creating Parametric Sketches

To create a profile sketch from multiple objects

1Use LINE to draw this shape, entering the points in the order shown.

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

➤ Line.

Specify first point: Specify a point (1)

Specify next point or [Undo]: Specify a second point (2)

Specify next point or [Undo]: Specify a third point (3)

Specify next point or [Close/Undo]: Specify a fourth point (4)

Specify next point or [Close/Undo]: Specify a fifth point (5)

Specify next point or [Close/Undo]: Specify a sixth point (6)

Specify next point or [Close/Undo]: Specify a seventh point (7)

Specify next point or [Close/Undo]: Specify an eighth point (8)

Specify next point or [Close/Undo]: Press ENTER

You do not need to make the lines absolutely vertical or horizontal. The

objective is to approximate the size and shape of the illustration.

2Using 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)

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

lines.

911

Creating Profile Sketches |49

Your sketch should look like this.

3Create 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.

50 |Chapter 6 Creating Parametric Sketches

When redrawing, Mechanical Desktop uses assumed constraints in the

sketch. For example, lines that are nearly vertical are redrawn as vertical, and

lines that are nearly horizontal are redrawn as horizontal.

After the sketch is redrawn, a message on the command line tells you that

Mechanical Desktop needs additional information:

Solved under constrained sketch requiring 5 dimensions or constraints.

Depending on how you drew your sketch, the number of dimensions

required to fully constrain your sketch may differ from that in this exercise.

This message tells you that the sketch is not fully defined. When you add the

missing dimensions or constraints, you determine how the sketch can

change throughout design modifications. Before you add the final con-

straints, you need to show the assumed constraints.

4Use AMSHOWCON to show the existing constraints, following the prompt.

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

Constraints ➤ Show Constraints.

Enter an option [All/Select/Next/eXit] <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 iden-

tified 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 con-

straints 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).

Creating Profile Sketches |51

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 con-

straints to the endpoints of sketch segments, or to the segments themselves,

in order to make your sketch more rigid.

5To hide the constraints, respond to the prompt as follows:

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

Save your file.

You have successfully created a profile sketch. In chapter 7, “Constraining

Sketches,” you learn to create, modify, and delete constraints and parametric

dimensions.

Using Custom Sketch Rules

Custom settings affect how Mechanical Desktop analyzes rough sketches. In

this exercise, you sketch with PLINE and convert your drawing to a profile

sketch. You will modify one of the Mechanical Options sketch rule settings

and see its effect on the sketch.

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

rough sketch profile sketch

52 |Chapter 6 Creating Parametric Sketches

To create a new part definition

1Use the context menu to initiate a new part definition.

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

Part.

2Respond 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.

3Pan 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

1Use 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)

Creating Profile Sketches |53

2Following 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

3Use AMPROFILE to create a profile sketch from the rough sketch.

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

➤ Single Profile.

NOTE If you used line segments and an arc to draw your sketch you cannot

use Single Profile. This command profiles single object sketches only. For

sketches containing more than one object, use Profile.

When you use Single Profile, you are not prompted to select the sketch geom-

etry. 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.

54 |Chapter 6 Creating Parametric Sketches

All lines were redrawn as horizontal or vertical except one. L1 remains angled

because the angle of the line exceeds the setting for angular tolerance. By

default, this rule makes a line horizontal or vertical if the angle is within 4

degrees of horizontal or vertical.

You can modify this and other sketch tolerance settings to adjust the preci-

sion of your sketch analysis.

4Change the angular tolerance setting.

Browser Click the Options button below the window.

5In 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.

Creating Profile Sketches |55

6Reprofile 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.

56 |Chapter 6 Creating Parametric Sketches

Using Nested Loops

You can select more than one closed loop to create a profile sketch. A closed

loop must encompass the nested loops. They cannot overlap, intersect, or

touch. With nested loops you can easily create complex profile sketches.

To create a profile sketch using nested loops

1Use AMNEW to create a new part definition.

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

Part.

2Accept the default part name on the command line.

The Browser now contains a third part.

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

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

4Create 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.

Creating Profile Sketches |57

5Profile 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.

58 |Chapter 6 Creating Parametric Sketches

Creating Path Sketches

Path sketches can be both two dimensional and three dimensional. Like

open profile sketches, they can be open shapes. In this exercise, you create

only the path sketches, but not the profiles that would sweep along the

paths.

Creating 2D Path Sketches

A 2D path sketch serves as a trajectory for a swept feature. You create a swept

feature by defining a path and then a profile sketch of a cross section. Then,

you sweep the profile along the path.

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

Valid geometry that can be used to create a 2D path includes

■Lines

■Arcs

■Polylines

■Ellipse segments

■2D splines

When you solve a 2D path sketch, you can automatically create a work plane

normal to the start point of the path. You use this work plane to create a pro-

file sketch for the swept feature, and then constrain the profile sketch to the

start point of the path.

swept featurepath sketch profile sketch

Creating Path Sketches |59

To create a 2D path sketch

1Create a new part definition.

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

Part.

2Press ENTER on the command line to accept the default part name.

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

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

4Use 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).

60 |Chapter 6 Creating Parametric Sketches

5Use 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.

Creating Path Sketches |61

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.

6Use AMSHOWCON to display the existing constraints, responding to the

prompt.

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

Constraints ➤ Show Constraints.

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

62 |Chapter 6 Creating Parametric Sketches

Creating 3D Path Sketches

3D path sketches are used to create

■A 3D path from existing part edges

■A helical path

■The centerline of a 3D pipe

■A 3D spline path

3D paths are used to create swept features that are not limited to one plane.

See chapter 8, “Creating Sketched Features,” to learn more about sweeping

features along a 3D path.

Open the file sketch2.dwg in the desktop\tutorial folder. The drawing contains

four part definitions and the geometry you need to create the 3D paths.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Creating a 3D Edge Path

A 3D edge path is used to create a path from existing part edges. After you

create the path, you can sweep a profile and use a Boolean operation to com-

bine the feature with the existing part.

3D edge path and profile sketch 3D sweep along edge path

Creating Path Sketches |63

Before you can work on a part, it must be active. Activate PART1_1, respond-

ing 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

1Use 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.

64 |Chapter 6 Creating Parametric Sketches

2Continue 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.

Creating Path Sketches |65

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.

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.

ath

rofile sketch 3D helical swee

work axis

66 |Chapter 6 Creating Parametric Sketches

To create a 3D helical path

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

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

➤ 3D Helix Path.

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

4In 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.

Creating Path Sketches |67

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.

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.

3D pipe path and profile sketch 3D sweep along pipe path

68 |Chapter 6 Creating Parametric Sketches

Use Pan to center PART3_1 on your screen.

PART3_1 contains an unsolved sketch of line segments and arcs.

To create a 3D pipe path

1Use AM3DPATH to define the 3D pipe path, responding to the prompts.

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

➤ 3D Pipe Path.

Select polyline path source: Select the first line (1)

Select polyline path source: Select the remaining arcs and lines in sequence

Select polyline path source: Press ENTER

Specify start point: Specify a point near the start of the first line (1)

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

Creating Path Sketches |69

2In 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.

3Place the work plane, following the prompts.

Plane=Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <accept>: Press ENTER

The Desktop Browser now contains a 3D Pipe icon, a work plane, and a work

point nested below the PART3_1 definition.

Save your file.

70 |Chapter 6 Creating Parametric Sketches

Creating a 3D Spline Path

In this type of path, you sweep a feature along a 3D spline created with fit

points or control points. Working in one integrated dialog box, you can mod-

ify 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.

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

1Use AM3DPATH to define the 3D spline path, responding to the prompts.

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

➤ 3D Spline Path.

Select 3D spline path source: Specify the spline

Specify start point: Specify the start point

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

3D spline path and profile sketch 3D sweep along spline path

Creating Path Sketches |71

2In 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.

3Create 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.

72 |Chapter 6 Creating Parametric Sketches

Creating Cut Line Sketches

When you create drawing views, you might want to depict a cut path across

a part for offset, cross-section views. After you have extruded or revolved a

profile sketch to create a feature, you can return to an original sketch and

draw the cut line across the features you want to include in the cross section.

There are two types of cut line sketches: offset and aligned. An offset cut line

sketch is a two-dimensional line constructed from orthogonal segments. An

aligned cut line sketch is a two-dimensional line constructed from non-

orthogonal segments.

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.

section viewoffset cut line section viewali

ned cut line

Creating Cut Line Sketches |73

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.

74 |Chapter 6 Creating Parametric Sketches

To create an offset cut line sketch

1Use PLINE to sketch through the center of the holes on the square part.

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

➤ Polyline.

Next, analyze the cut line sketch according to internal sketching rules.

2Use 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.

Creating Cut Line Sketches |75

As with the other sketches you created, a message tells you how many dimen-

sions 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 place-

ment, 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.

76 |Chapter 6 Creating Parametric Sketches

To create an aligned cut line sketch

1Use PLINE to sketch through the centers of two of the holes on the circular

part.

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

➤ Polyline.

2Define 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.

3In the Browser, the new CutLine1 icon is part of the PART2_1 hierarchy.

Save your file.

Creating Split Line Sketches |77

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 com-

plex 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.

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.

shelled part split part

78 |Chapter 6 Creating Parametric Sketches

To create a split line

1Expand 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.

2In 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.

Creating Split Line Sketches |79

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

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

➤ Polyline.

4Use AMSPLITLINE to create a split line from your sketch, responding to the

prompts.

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

➤ Split Line.

Select objects for sketch: Select the polyline

Select objects for sketch: 1 found

Select objects for sketch: Press ENTER

Select edge to include in split line or press <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.

5Look at the Browser. SplitLine1 is now nested under the part definition.

Save your file.

80 |Chapter 6 Creating Parametric Sketches

Creating Break Line Sketches

When you want to document complex assemblies, it is not always easy to dis-

play 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.

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.

break line path breakout drawing view

Creating Break Line Sketches |81

To create a break line

1Use AMBREAKLINE to define the break line sketch, following the prompts.

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

➤ Break Line.

Select objects for sketch: Specify the sketch (1)

Select objects for sketch: Press ENTER

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

the work plane.

Save your file.

Now that you have learned the basics of creating sketches, you are ready to

constrain them by adding geometric and parametric dimension constraints.

In This Chapter 7

Constraining Sketches

When you solve a sketch in Autodesk® Mechanical

Desktop®, geometric constraints are applied in

accordance with internal rules. To fully constrain the

sketch, you apply the remaining parametric dimensions

and geometric constraints that are necessary to meet

your design goals.

Any time you modify a sketch, the parametric geometry

retains the relationships among design elements.

To reduce the number of constraints required to fully

constrain a sketch, you can use construction geometry.

Construction geometry becomes part of the sketch, but

is ignored when the sketch is used to create a feature.

In the next chapter, you learn to add sketched features

to your constrained sketches.

■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

84 |Chapter 7 Constraining Sketches

Key Terms

Te r m Definition

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

shape and relationships among sketch lines and arcs. Dimensional constraints

control the size of sketch geometry.

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

can change shape or size. For example, a circle has two degrees of freedom,

center and radius. When these values are known, degrees of freedom are said to

be eliminated.

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

sketch resizes. May be expressed as a constant value, a variable in an equation, a

variable in a table, or in global parameter files.

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

parametrics A solution method that uses the values of part parameters to determine the

geometric configuration of the part.

Basic Concepts of Creating Constraints |85

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.

86 |Chapter 7 Constraining Sketches

Constraining Tips

Constraining Sketches

Constraining a sketch defines how a sketch can change shape or size. In addi-

tion 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.

Tip Explanation

Determine sketch

dependencies Analyze the design to determine how sketch elements

interrelate; then decide which geometric constraints are

needed.

Analyze automatically

applied constraints Determine the degrees of freedom not resolved by automatic

constraints. Decide if any automatic constraints need to be

deleted in order to constrain elements as you require.

Use only needed

constraints Replace constraints as needed to define shape. Because

constraints often solve more than one degree of freedom, use

fewer constraints than degrees of freedom.

Stabilize shape

before size If you apply geometric constraints before dimensions, your

sketch shape is less likely to become distorted.

Dimension large

before small To minimize distortion, define larger elements that have an

overall bearing on the sketch size. Dimensioning small elements

first may restrict overall size. Delete or undo a dimension if the

sketch shape is distorted.

Use both geometric

constraints and

dimensions

Some constraint combinations may distort unconstrained

portions of the sketch. If so, delete the last constraint and

consider using a dimension or a different constraint

combination.

Constraining Sketches |87

The ways a sketch can change size or shape are called degrees of freedom. For

example, a circle has two degrees of freedom—the location of its center and

its radius. If the center and radius are defined, the circle is fully constrained

and those values can be maintained.

Similarly, an arc has four degrees of freedom—center, radius, and the end-

points of the arc segment.

The degrees of freedom you define correspond to how fully the sketch is con-

strained. If you define all degrees of freedom, the arc is fully constrained. If you

do not define all degrees of freedom, the sketch is underconstrained.

Mechanical Desktop does not allow you to define a degree of freedom in

more than one way and thus prevents you from overconstraining a sketch.

Before you add constraints, study your sketch, and then decide how to con-

strain it. Usually, you need both geometric constraints and dimensions. See

“Constraining Tips” on page 86.

You should fully constrain sketches so that they update predictably as you

make changes. As you gain experience, you may want to underconstrain a

sketch while you work out fine points of a design, but doing so may allow

that feature to become distorted as you modify dimensions or constraints.

radius

center

end

oint

radius

center

endpoint

88 |Chapter 7 Constraining Sketches

Applying Geometric Constraints

When constraining a sketch, begin by defining its overall shape before defining

its size. Geometric constraints specify the orientation and relationship of the

geometric elements. For example

■Constraints that specify orientation indicate whether an element is hori-

zontal or vertical.

■Constraints that determine relationships specify whether two elements

are perpendicular, parallel, tangent, collinear, concentric, projected,

joined, have the same X or Y coordinate location, or have the same radius.

Mechanical Desktop displays geometric constraints as letter symbols. If the

constraint specifies a relationship between two elements, the letter symbol is

followed by the number of the sketch element to which the constraint is

related. In the example below,

■The start point of the arc (0) has a fix constraint. This point is anchored

and will not move when changes are made to the sketch constraints.

■The lines (2, 3, 4, and 6) have constraint symbols of either H (horizontal)

or V (vertical).

■All lines except one are tangent to at least one of the arcs (0 and 1). Each

symbol T (tangent) is followed by the number of the arc to which it is

tangent.

■Each arc is tangent to its connecting lines, as shown by T constraint

symbols, and the arcs have the same radius, as indicated by the R

constraint symbols.

Applying Geometric Constraints |89

As you apply geometric constraints, you should continue to analyze your

sketch, reviewing and replacing constraints.

In the next exercise, you gain experience with constraining techniques by

analyzing and then modifying geometric constraints to reshape the sketch.

Open the file sketch5.dwg in the desktop\tutorial folder. Use the before-and-

after sketches below to determine what changes you must make. Then

change the constraints and see the results of your analysis.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

In the before-and-after sketches, you can see that the constraints and dimen-

sions differ, but you cannot discern which geometric constraints Mechanical

Desktop has assumed. You will notice that

■The linear dimensions are the same for both sketches.

■The angular relationships of the vertical lines differ.

before geometric constraints after geometric constraints

90 |Chapter 7 Constraining Sketches

Showing Constraint Symbols

You can change the parametric relationships of the lines by modifying

geometric or dimensional constraints. Because geometric constraints control

the overall shape of the sketch, you cannot safely make any changes until

you know the current geometric constraints. Therefore, the next step is to

show the symbols.

To show constraint symbols

1Use AMSHOWCON to display constraint symbols, responding to the prompt.

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

Constraints ➤ Show Constraints.

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

Parallel constraints exist between lines 0, 2, 4 and 6. Lines 1, 3, 5, and 7 have

horizontal constraints. Lines 3 and 7 are also collinear and equal in length.

You begin reshaping your sketch by removing the parallel constraints.

To understand the constraints, look at symbol P0 (on line 2). This symbol

indicates that line 2 is parallel to line 0.

Applying Geometric Constraints |91

Similarly, the constraint symbols (P2, P4, and P6) show that line 0 is parallel

to lines 2, 4 and 6.

2Hide the constraint symbols.

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

Replacing Constraints

After you delete the unwanted constraints, you can add constraints to

reshape the sketch. In this exercise, you delete the parallel constraints that

control the inner and outer angled lines in the sketch and replace them with

vertical constraints.

To replace a constraint

1Use AMDELCON to replace the constraints, responding to the prompts.

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

Constraints ➤ Delete Constraints.

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

Select or [Size/All]: Press ENTER

The parallel constraints are deleted. The sketch shape looks the same until

you add constraints or change dimensions.

92 |Chapter 7 Constraining Sketches

2Use AMADDCON to add vertical constraints to the two inner angled lines,

responding to the prompts.

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

Constraints ➤ Vertical.

Valid selection(s): line, ellipse or spline segment

Select object to be reoriented: Specify line (3)

Solved under constrained sketch requiring 2 dimensions or constraints.

Valid selection(s): line, ellipse or spline segment

Select object to be reoriented: Specify line (4)

Solved under constrained sketch requiring 1 dimensions or constraints.

Valid selection(s): line, ellipse or spline segment

Select object to be reoriented: Press ENTER

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

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

You removed the constraints that forced these lines to be parallel to one

another. In order to force the outer lines to be complementary angles to one

another, you need to add an angular dimension to the leftmost line.

Applying Geometric Constraints |93

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

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

➤ New Dimension.

Select first object: Select near the middle of line (1)

Select second object or place dimension: Select near the middle of line (2)

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Placement point] <75>: Enter 105

Solved fully constrained sketch.

Select first object: Press ENTER

NOTE If you do not select the lines near their midpoints, you may be

prompted to specify the type of dimension to create. Choose Angular.

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

Save your file.

Next, you learn to use parametric dimensions to constrain the shape of a

sketch.

94 |Chapter 7 Constraining Sketches

Applying Dimension Constraints

It is good practice to stabilize the shape of a sketch with geometric constraints

before you specify size with dimensional constraints.

Dimensions specify the length, radius, or rotation angle of geometric elements

in the sketch. Unlike geometric constraints, dimensions are parametric;

changing their values causes the geometry to change.

Dimensions can be shown as numeric constants or as equations. Although

you can use them interchangeably, they each have specific uses.

■Numeric constants are useful when a geometric element has a static size

and is not related to any other geometric element.

■Equations are useful when the size of a geometric element is proportional

to the size of another element.

In the following illustration, all of the lines and the angles are constant, and

stated as numeric values.

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

Applying Dimension Constraints |95

In this case, the height of the sketch must maintain the same proportion to

the length, even if you change dimensions later. In an equation, you can

state the height relative to the length. The dimension for the vertical line is

defined as an equation of d1 = d0/.875 where d1 is the parameter name for

the vertical line and d0 is the parameter name for one of the horizontal lines.

The d variables in the equations are parameter names assigned by Mechanical

Desktop when you define the parameters. The letter d indicates that the

parameter is a dimension. The number signifies the dimension number rela-

tive to the beginning of the dimensioning sequence.

Open the file sketch6.dwg in the desktop\tutorial folder. Add and modify

dimensions to complete the definition of the following sketch.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The before-and-after sketches reveal where dimensions are needed and in

what order you should place them. The dimensions needed here have

already been identified and are expressed as numeric constants.

To keep the sketch shape from becoming distorted as the dimensions resize

it, define larger dimensions first: the left vertical line (dim 1) and the bottom

horizontal line (dim 2).

By adding geometric constraints, you can reduce the number of dimensions

you need. Later, you can modify the sketch with fewer changes.

After the basic shape has been defined, you replace the rightmost vertical line

and the top horizontal line with fillets, and add geometric constraints and

dimensions to finish the profile.

dim 1

dim 2

dim 5

dim 4

original sketch profiled sketch

dim 3

96 |Chapter 7 Constraining Sketches

Creating Profile Sketches

First, convert the unconstrained sketch to a profile sketch before you add

dimensions. Then examine the default geometric constraints.

To create a profile from a sketch and examine constraints

1Use AMPROFILE to create a profile from the sketch.

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

➤ Single Profile.

Mechanical Desktop redraws the sketch and reports that it still needs six

dimensions or constraints to solve the sketch:

Solved under constrained sketch requiring 6 dimensions or constraints.

Examine the inferred geometric constraints and determine if the default con-

straints are correct or whether they inhibit the dimensions you want to add.

2Use AMSHOWCON to display the constraints, responding to the prompt.

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

Constraints ➤ Show Constraints.

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

Applying Dimension Constraints |97

Mechanical Desktop recalculates the sketch and displays the constraints.

■A fix constraint is added to the start point of the first line of the sketch.

This point is anchored and will not move when changes are made to the

sketch constraints.

■Nearly horizontal and vertical lines have been assigned horizontal (H) and

vertical (V) constraints.

■Nearly vertical lines are assumed to be parallel (P) to one another.

For this exercise, all of the assumed geometric constraints are correct and

none of them restrict the dimensioning scheme shown earlier.

Exit from Show Constraints, responding to the prompt as follows:

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

Adding Dimensions

The rough sketch is converted to a profile sketch, and default geometric

constraints are applied. Now you need to fully constrain the sketch by adding

four dimensions and two geometric constraints. Parts are resized as you

change parametric dimensions to refine your design, while all geometric

relationships are maintained.

Keep the following points in mind as you are adding dimensions:

■Select the elements to dimension and choose where to place the dimension.

■Dimension type depends on the element you choose and where you place

the dimension. The current size of the selected element is shown.

■You can accept the calculated size or specify a new value.

■The sketch element is resized according to the dimension value and the

dimension is placed at the location you chose.

It is good practice to accept the automatically calculated dimensions to

stabilize the sketch shape, particularly large outer dimensions. When you

later modify dimensions to exact sizes, the sketch shape is less likely to

become distorted.

In this exercise, you create horizontal and vertical dimensions. Then you

modify the sketch by appending geometry, and applying angular and radial

dimensions.

98 |Chapter 7 Constraining Sketches

To add a dimension to a profile

1Use AMPARDIM to add dimensions to your profile, responding to the

prompts.

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

➤ New Dimension.

Select first object: Specify the line (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<1.9606>: Enter 2

Solved under constrained sketch requiring 5 dimensions or constraints.

The sketch is updated with the new dimension value.

The command line lists several options. These options and the number of

elements you select determine the type and placement of dimensions.

In this example, you choose a line and the placement of the dimension. If

you selected two elements and specified a location, Mechanical Desktop

would place a dimension that gives the distance between the two elements.

2Continue dimensioning the sketch by choosing the bottom horizontal line.

Select first object: Specify the line (3)

Select second object or place dimension: Place the dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<2.1123>: Enter 2

Solved under constrained sketch requiring 4 dimensions or constraints.

Select first object: Press ENTER

Mechanical Desktop redraws the sketch according to the new dimension value.

Applying Dimension Constraints |99

Now that the default constraints and larger dimensions have stabilized the

sketch shape and size, you can begin to make changes to the sketch. To

practice changing and updating the sketch, you add fillets to the two legs of

the sketch.

To add a fillet to a sketch

1Use AMFILLET to apply a fillet, entering the points in the order shown.

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

➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.1250

Select first object or [Polyline/Radius/Trim]: Specify the line (1)

Select second object: Specify the line (2)

NOTE Because you selected parallel lines, FILLET ignores the radius value and

joins the endpoints of the selected lines with a continuous arc.

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

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

➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.1250

Select first object or [Polyline/Radius/Trim]: Specify the line (3)

Select second object: Specify the line (4)

Your sketch should now look like this.

100 |Chapter 7 Constraining Sketches

Before you continue defining your sketch, erase the horizontal line and the

vertical line joining the endpoints of the new arcs.

3Erase the two lines.

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

➤ Erase.

Your drawing should look like this.

Because you have changed the sketch, you must re-solve it before you can use

it to create a feature.

Appending Sketches

By adding the fillets and removing the lines, you have changed the sketch

geometry. Whenever you add, modify, or remove geometry you must append

the changed geometry to the profile sketch. You will be prompted to select

any new geometry you have created. Mechanical Desktop appends the new

geometry and recalculates the sketch, assigning new geometric constraints.

After appending the sketch, re-examine the geometric constraints to see if

they affect your dimensioning scheme.

Applying Dimension Constraints |101

To append a profile sketch and re-examine geometric constraints

1Expand the hierarchy of PART1_1.

2Use AMRSOLVESK to append the existing fillets, responding to the prompts.

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

Sketch.

Select geometry to append to sketch: Specify the first arc

Select geometry to append to sketch: Specify the second arc

Select geometry to append to sketch: Press ENTER

Redefining existing sketch.

Solved under constrained sketch requiring 4 dimensions or constraints.

Mechanical Desktop analyzes and redraws the profile in accordance with its

sketch analysis rules. Four additional constraints are needed to fully

constrain the sketch.

3Use AMSHOWCON to display the constraint symbols.

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

Constraints ➤ Show Constraints.

Press ENTER to exit the command.

4Display all of the symbols. Several tangent (T) constraints are added to the

original geometric constraints.

The tangent constraints join the arcs to their adjoining lines. Notice that

although the sketch segment numbers have changed because of the new

geometry, the fix constraint remains in the same location.

102 |Chapter 7 Constraining Sketches

For this exercise, do not delete any constraints because the tangent constraints

do not adversely affect the dimensioning scheme. Now that you have

recreated the profile sketch, you can continue to add geometric constraints

and dimensions to the sketch, starting with a radial constraint to the two arcs.

Depending on how you drew your sketch, your default dimension values

may differ from those in this exercise.

To add constraints to a re-created profile sketch

1Use AMADDCON to add a radial constraint to the two arcs, responding to the

prompts.

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

Constraints ➤ Radius.

Valid selections: arc or circle

Select object to be resized: Specify an arc

Valid selections: arc or circle

Select object radius is based on: Specify the other arc

Solved under constrained sketch requiring 3 dimensions or constraints.

Valid selections: arc or circle

Select object to be resized: Press ENTER

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

Mechanical Desktop adds radius constraints to the two arcs.

Finish constraining the sketch by adding three dimension constraints.

Applying Dimension Constraints |103

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

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

➤ New Dimension.

Select first object: Specify the lower arc

Select second object or place dimension: Place the dimension

Enter dimension value or [Undo/Diameter/Ordinate/Placement point]

<0.3687>: Enter .4

Solved under constrained sketch requiring 2 dimensions or constraints.

After you enter the new radius value, the arcs are updated because the radius

constraint makes both arcs equal.

3Add the final two dimensions by responding to the prompts as follows:

Select first object: Specify the line (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.8753>: Enter .75

Solved under constrained sketch requiring 2 dimensions or constraints.

Select first object: Specify near the middle of line (1)

Select second object or place dimension: Specify near the middle of line (3)

Specify dimension placement: Place the dimension (4)

Enter dimension value or [Undo/Placement point] <138>: Enter 135

Solved fully constrained sketch.

Select first object: Press ENTER

104 |Chapter 7 Constraining Sketches

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

Save your file.

Modifying Dimensions

Because your design changes during development, you must be able to delete

or modify dimension values. Mechanical Desktop parametric commands

ensure that relationships among geometric elements remain intact.

To finish the sketch, change the dimension of the top horizontal line and the

angular dimension.

To change a dimension

1Use AMMODDIM to modify the dimensions, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the dimension (1)

New value for dimension <.4>: Enter .375

Solved fully constrained sketch.

Select dimension to change: Specify the dimension (2)

New value for dimension <.75>: Enter .5

Solved fully constrained sketch.

Select dimension to change: Press ENTER

Using Construction Geometry |105

Your finished sketch should now look like this.

Save your file.

Using Construction Geometry

Construction geometry can minimize the number of constraints and dimen-

sions needed in a sketch and offers more ways to control sketch features.

Construction geometry works well for sketches that are symmetrical or have

geometric consistencies. Some examples are sketches that have geometry

lying on a radius, a straight line, or at an angle to other geometry.

Construction geometry is any line, arc, or circle in the sketch profile or path

that is a different linetype from the sketch linetype. By default, construction

geometry is placed on the AM_CON layer. To make construction geometry

easier to see, you can change its color, linetype, or linetype scale.

Construction geometry can be used to constrain only the sketch it is

associated with. When you create a feature from a sketch, you also select the

construction geometry with the path or profile sketch. After the feature is

created, the construction geometry is no longer visible.

Creating Profile Sketches

In this exercise, you follow a typical sequence. As always, study the sketch to

determine what constraints and dimensions you need and decide where to

place construction geometry to make solving the sketch easier.

Open the file sketch7.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

106 |Chapter 7 Constraining Sketches

To create a single profile sketch

1Use PLINE to draw the rough sketch.

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

➤ Polyline.

2Use AMSOLVE to solve the sketch.

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

➤ Single Profile.

The polyline is automatically selected.

Mechanical Desktop applies constraints according to how you sketch and

then reports that the sketch needs six or more additional constraints. A fix

constraint is automatically applied to the point where you started your sketch.

3Use AMSHOWCON to display the existing constraints.

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

Constraints ➤ Show Constraints.

4Display all of the assumed constraint symbols. Each of the eight lines should

have a vertical or horizontal constraint.

Next, create a construction line to assist in constraining the sketch.

NOTE If necessary, remove the fix constraint using AMDELCON. This constraint

prevents you from projecting the sketch to the construction line.

Using Construction Geometry |107

To create a construction line

1Create a construction line.

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

➤ Construction Line.

2Draw the line diagonally across the sketch.

Mechanical Desktop draws the line on a new layer called AM_CON. The line

is yellow and drawn with the HIDDEN linetype. Because the linetype is

different from the one used to draw the sketch, the line is considered

construction geometry. It is used only in this sketch.

3Use AMRSOLVESK to append the profile.

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

➤ Append.

4Select the construction line.

5Re-examine the assumed constraints.

Adding Project Constraints

Mechanical Desktop recognizes nine lines in the sketch. The sketch requires

two more constraints because you added a construction line.

Next, project the construction line to each vertex that serves as an inner

corner of a stair.

To place a project constraint, specify a vertex and then select the construc-

tion line. Depending on how closely you drew the construction line to the

vertices, some constraints may have already been applied.

108 |Chapter 7 Constraining Sketches

To add a project constraint

1Use AMADDCON to add the project constraints, responding to the prompts.

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

Constraints ➤ Project.

Valid selections: line, circle, arc, ellipse or spline segment

Specify a point to project: Enter end

of: Specify point (1)

Valid selections: line, circle, arc, ellipse, work point or spline segment

Select object to be projected to: Specify the construction line (5)

Valid selections: line, circle, arc, ellipse or spline segment

Specify a point to project:

Repeat this process for points (2) through (4), then press ENTER

NOTE If you do not use the endpoint object snap, you will not be able to

correctly constrain the sketch.

By defining the slope of the stairs with the construction line, you have

reduced the number of required constraints and dimensions to four.

2Use REDRAW to clean up the screen display.

Desktop Menu View ➤ Redraw

Using Construction Geometry |109

Adding Parametric Dimensions

To fully define the sketch, dimension one of the risers and apply a slope angle

for the construction line. Each step is equal in height, so you can add equal

length constraints to the remaining steps later.

To add a parametric dimension

1Use AMPARDIM to dimension the slope angle, responding to the prompts.

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

➤ New Dimension.

Select first object: Specify near the middle of the construction line (1)

Select second object or place dimension:

Specify near the middle of the bottom horizontal line (2)

Specify dimension placement: Specify a point to right (3)

Enter dimension value or [Undo/Placement point] <31>: Enter 30

Solved under constrained sketch requiring 3 dimensions or constraints.

2Continue, adding dimensions to the first vertical riser.

Select first object: Specify a point near the center of the lower left vertical line (4)

Select second object or place dimension: Specify a point to left of first point (5)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.9463>: Enter 1

Solved under constrained sketch requiring 2 dimensions or constraints.

Select first object: Press ENTER

To finish constraining the sketch, add equal length dimensions to the

remaining two risers.

110 |Chapter 7 Constraining Sketches

To add an equal length constraint

1Use AMADDCON to add an equal length constraint, responding to the

prompts.

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

Constraints ➤ Equal Length.

Valid selections: line or spline segment

Select object to be resized: Specify the second riser (2)

Valid selections: line or spline segment

Select object to base size on: Specify the dimensioned riser (1)

Solved under constrained sketch requiring 1 dimensions or constraints.

2Continue on the command line to place the last constraint.

Valid selections: line or spline segment

Select object to be resized: Specify the third riser (3)

Valid selections: line or spline segment

Select object to base size on: Specify the dimensioned riser (1)

Solved fully constrained sketch.

You should now have a fully constrained sketch. Exit the command by

pressing ENTER twice.

3Use AMMODDIM to change the angular dimension, responding to the

prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the angular dimension

New value for dimension <30>: Enter 25

Select dimension to change: Press ENTER

Save your file.

Using Construction Geometry |111

Constraining Path Sketches

Construction geometry helps you constrain sketches that may be difficult to

constrain with only the geometry of the sketch shape. In this exercise, you

create a path sketch, add a construction line, and constrain the sketch to the

line.

Before you begin this exercise, create a new part definition for the sketch.

To create a new part definition

1Use AMNEW to create a new part definition.

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

Part.

2Press ENTER on the command line to accept the default part name.

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

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

You are ready for the next exercise.

To use construction geometry in a swept path

1Use PLINE to draw the following sketch.

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

➤ Polyline.

Use the arc/direction option of PLINE to draw the arcs. You can also use your

cursor crosshairs to visually align the endpoints of each arc as you sketch.

NOTE To enlarge the crosshairs, choose Assist ➤ Options. Under Crosshair

Size, set the size to 15 or larger.

112 |Chapter 7 Constraining Sketches

2Use AM2DPATH to create a 2D path from your sketch, responding to the

prompts.

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

➤ 2D Path.

Select objects: Specify the polyline

Select objects: Press ENTER

Specify the start point of the path: Specify one of the ends of the path

Solved under constrained sketch requiring 10 dimensions or constraints.

Create a profile plane perpendicular to the path? [Yes/No] <Yes>: Enter n

You can use either end for the start point.

Mechanical Desktop reports that the sketch needs ten or more additional

constraints, depending on how you drew the sketch.

3Draw two construction lines. The goal is to have each of the ends of the arcs

meet the construction lines.

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

➤ Construction Line.

4In the Desktop Browser, expand the PART2_1 hierarchy.

5Use AMRSOLVESK to append the construction lines to your sketch, following

the prompts.

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

➤ Append.

Select geometry to append to sketch: Specify a construction line

Select geometry to append to sketch: Specify the other construction line

Select geometry to append to sketch: Press ENTER

Redefining existing sketch.

Specify start point of path: Specify one of the ends of the path

Solved under constrained sketch requiring 6 dimensions or constraints.

The construction lines have reduced the number of constraints or dimen-

sions needed by constraining the arc endpoints and centers to the line. The

construction lines have been made horizontal as well.

Using Construction Geometry |113

To check for and add missing constraints

1Use AMSHOWCON to check for constraints that are still needed.

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

Constraints ➤ Show Constraints.

2Display all the constraints and press ENTER to exit the command.

3Use AMADDCON to add constraints and dimensions to the sketch, following

the prompts.

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

➤ New Dimension.

Select first object: Specify the upper left arc (1)

Select second object or place dimension:

Specify the vertical line on the left below its midpoint (2)

Specify dimension placement: Specify a point to the left of the sketch (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<3.1069>: Enter 3

Solved under constrained sketch requiring 5 dimensions or constraints.

4Add a second dimension.

Select first object: Specify the upper left arc (1)

Select second object or place dimension:

Specify a point above and left of sketch (4)

Enter dimension value or [Undo/Diameter/Ordinate/Placement point]

<0.2788>: Enter .25

Solved under constrained sketch requiring 4 dimensions or constraints.

Select first object: Press ENTER

Next, you fully solve the path by adding 2D constraints.

114 |Chapter 7 Constraining Sketches

5Constrain all the arcs with the same radius as the one you just dimensioned,

responding to the prompts.

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

Constraints ➤ Radius.

Valid selections: arc or circle

Select object to be resized: Specify the lower left arc

Valid selections: arc or circle

Select object radius is based on: Specify the arc with the radial dimension

Solved under constrained sketch requiring 3 dimensions or constraints.

Valid selections: arc or circle

Select object to be resized: Specify the upper arc that is second from the left

Valid selections: arc or circle

Select object radius is based on: Specify the arc with the radial dimension

Solved under constrained sketch requiring 2 dimensions or constraints.

Valid selections: arc or circle

Select object to be resized: Specify the lower arc that is second from the left

Valid selections: arc or circle

Select object radius is based on: Specify the arc with the radial dimension

Solved under constrained sketch requiring 1 dimensions or constraints.

Valid selections: arc or circle

Select object to be resized: Specify the upper right arc

Valid selections: arc or circle

Select object radius is based on: Specify the arc with the radial dimension

Solved fully constrained sketch.

Valid selections: arc or circle

Select object to be resized: Press ENTER

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

Your sketch should now be fully constrained. You may need to use the Equal

Length constraint for the beginning and end vertical line segments of your

sketch. Experiment with this sketch by changing the values of the two

dimensions.

If arc centers do not lie on the construction line, use the project constraint.

Add project constraints until the sketch is fully constrained.

NOTE Depending on how accurately you sketched the path, you may need to

add other constraints. Experiment until your sketch is fully constrained. If you

have difficulty, delete the sketch and try again.

Save your file.

Using Construction Geometry |115

Controlling Tangency

A single piece of construction geometry can manage the size and shape of

entire sketches. Circles and arcs are particularly useful for constraining the

perimeter shapes of nuts, knobs, multisided profiles, and common polygons.

In this exercise, you create a triangular sketch and then constrain the sides of

the triangle and the internal angles to remain equal. In this manner, you

could form the basis for a family of parts in which the only variable is a single

diameter dimension.

Create a new part definition for the next sketch.

To create a new part definition

1Use AMNEW to create a new part definition.

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

Part.

2Accept the default part name.

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

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

You are ready to create the next sketch.

To control tangency with construction geometry

1Use PLINE to create the triangular shape.

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

➤ Polyline.

2Draw a circle inside the triangle.

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

➤ Construction Circle.

116 |Chapter 7 Constraining Sketches

3Use AMPROFILE to turn the sketch into a profile sketch, making sure to select

both the polyline and the circle.

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

➤ Profile.

At this point, the circle may be tangent to some or all of the sides of the

triangle.

4Use AMADDCON to add Tangent constraints to the sketch, following the

prompts.

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

Constraints ➤ Tangent.

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be reoriented: Specify the line (1)

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be made tangent to: Specify the circle (2)

Solved under constrained sketch requiring 5 dimensions or constraints.

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be reoriented: Specify the line (3)

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be made tangent to: Specify the circle (4)

Solved under constrained sketch requiring 4 dimensions or constraints.

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be reoriented: Specify the line (5)

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be made tangent to: Specify the circle (6)

Solved under constrained sketch requiring 3 dimensions or constraints.

Valid selections: line, circle, arc, ellipse or spline segment

Select object to be reoriented: Press ENTER

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

Mechanical Desktop now needs three or more dimensions or constraints to

fully solve the sketch.

Using Construction Geometry |117

To add a dimension to an angle

1Use AMPARDIM to apply angular dimensions to the triangle, following the

prompts.

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

➤ New Dimension.

Select first object: Specify near the middle of the line (1)

Select second object or place dimension: Specify near the middle of the line (2)

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Placement point] <67>: Enter 60

Solved under constrained sketch requiring 2 dimensions or constraints.

2Continue on the command line.

Select first object: Specify near the middle of the line (4)

Select second object or place dimension: Specify near the middle of the line (5)

Specify dimension placement: Place the dimension (6)

Enter dimension value or [Undo/Placement point] <78>: Enter 60

Solved under constrained sketch requiring 1 dimensions or constraints.

Select first object: Press ENTER

NOTE If you do not select the lines near their midpoints, you may be

prompted to specify the type of dimension to create. Choose Angular.

The angular dimensions should look like these.

118 |Chapter 7 Constraining Sketches

To add a dimension to a circle

1Add a dimension to the diameter of the construction circle, following the

prompts.

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

➤ New Dimension.

Select first object: Specify a point on the circle

Select second object or place dimension: Specify a point outside of the triangle

Enter dimension value or [Undo/Radius/Ordinate/Placement point]

<3.1541>: Enter 10

Solved fully constrained sketch.

Select first object: Press ENTER

The sketch should now be fully constrained.

2Zoom out to view the entire sketch.

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

NOTE If the bottom segment of your triangle is still not horizontal, you will

need to add a Horizontal constraint to fully constrain the sketch.

3Experiment with the size of the sketch. Use AMMODDIM to change the

diameter dimension of the circle, following the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the diameter dimension

New value for dimension <10>: Enter 5

Solved fully constrained sketch.

Select dimension to change: Press ENTER

Save your file.

Using Construction Geometry |119

All sides remain equal in length and tangent to the circle, and the bottom of

the triangle remains horizontal. If you used this sketch as a base feature of a

part, you could change the overall size of the part simply by changing the

diameter of the construction circle.

This technique could be applied to more complex geometry such as

pentagons, octagons, and odd-shaped polygons. These shapes can form the

base feature for a family of nuts, bolts, fittings, and so on. Try these types of

sketches on your own.

120

121

In This Chapter 8

Creating Sketched Features

Features are the parametric building blocks of parts. By

creating and adding features you define the shape of

your part. Because features are parametric, any changes

to them are automatically reflected when the part is

updated.

In Autodesk® Mechanical Desktop®, there are three

types of features—sketched, work and placed.

In this tutorial, you learn to create and modify sketched

features. In chapter 4, you learn about work features.

■Extruded features

■Loft features

■Revolved features

■Face splits

■Sweep features

122 |Chapter 8 Creating Sketched Features

Key Terms

Te r m Definition

base feature The first feature you create. As the basic element of your part, it represents its

simplest shape. All geometry you create for a part depends on the base feature.

Boolean modeling A solid modeling technique in which two solids are combined to form one

resulting solid. Boolean operations include cut, join, and intersect. Cut subtracts

the volume of one solid from the other. Join unites two solid volumes. Intersect

leaves only the volume shared by the two solids.

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

consumed when the feature is created.

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

draft angle An angle applied parallel to the path of extruded, revolved, or swept surfaces or

parts. A draft angle is used to allow easy withdrawal from a mold or easy insertion

into a mated part.

extrude In part modeling, to create a geometric sketch defined by a planar profile

extended along a linear distance perpendicular to the profile plane.

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

revolved features, loft features, and swept features using profiles and paths. You

can also create placed features like holes, chamfers, and fillets. You combine

features to create complete parametric part models.

helical sweep A geometric feature defined by the volume from moving a profile along a 3D

path about a work axis.

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

lofted feature A parametric shape created from a series of sketches defining the cross-sectional

shape of the feature at each section.

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

revolution.

sketch plane A temporary drawing surface that corresponds to a real plane on a feature. It is an

infinite plane with both X and Y axes on which you sketch or place a feature.

sketched feature A three-dimensional solid whose shape is defined by constrained sketches and

located parametrically on a part. Sketched features are extrudes, lofts, revolves,

sweeps, or face splits.

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

path.

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

of a profile.

Basic Concepts of Sketched Features |123

Basic Concepts of Sketched Features

Features are the building blocks you use to create and shape a part. Because

they are fully parametric, they can easily be modified at any time.

The first feature in a part is called the base feature. As you add more features,

they can be combined with the base feature or each other to create your part.

Boolean operations, such as cut, join, and intersect, can be used to combine

features after a base feature has been created.

You create a sketched feature from a profile, which is an open or closed

parametric sketch that has been solved. You can also create a feature from

a text-based sketch. In most cases, you fully constrain the profile before

you create a feature. Because a sketch is parametric, you can easily modify

it to change the shape of the feature. When you update your part, the

changes you made are displayed automatically.

Sketched features include extrusions, lofts, revolutions, sweeps, and emboss-

ing. Face splits are also considered sketched features, but they are created by

splitting a part face using an existing face, a work plane, or a split line. If you

choose the split line method, you are using a sketched feature to split the

face.

In this tutorial you learn how to create and edit sketched features. Later you

learn how to create and edit work features and placed features.

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

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

124 |Chapter 8 Creating Sketched Features

The drawing file includes fifteen parts which contain the geometry you need

to create the sketched features in this section.

NOTE For clarity, the work features are not shown.

First, you create an extruded feature.

Creating Extruded Features

Extrusions are the most common sketched features. An extruded feature can

be created from a closed profile, an open profile, or a text-based profile.

Extruding Closed Profiles

A closed profile is used to create a base feature, or in Boolean modeling to cut,

intersect, and join with other features.

In the first exercise, you use the part EXTRUDE_1. Activate the part, and

expand the hierarchy of EXTRUDE_1.

To activate a part

Browser Double-click EXTRUDE_1.

Click the plus sign in front of EXTRUDE_1 to expand the

hierarchy.

Creating Extruded Features |125

Clear the visibility of the other parts, and display the dimensions and work

features of the active part.

To turn off the visibility of multiple parts

Browser Select EXTRUDERIB_1, then hold down SHIFT as you

select BEND_1. Right-click the selected block and choose

Visible.

NOTE Because most of the parts do not contain features yet, you cannot use

the toolbutton, menu, or command methods to make the part instances

invisible.

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

To thaw dimension and work layers

Desktop Menu Assist ➤ Format ➤ Layer

The Layer Properties Manager dialog box is displayed.

In the AM_PARDIM layer, select the On icon and the Freeze icon to unthaw

the layer. Repeat for the AM_WORK layer.

Choose OK to exit the dialog box.

The parametric dimensions and work features for each part are now visible.

126 |Chapter 8 Creating Sketched Features

To zoom in to a part

Browser Right-click EXTRUDE_1, and choose Zoom to.

The EXTRUDE_1 part is positioned on your screen.

To create an extruded feature

1Use AMEXTRUDE to create an extruded feature from Profile1.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Distance: Enter 0.5

Termination: Type: Blind

The image tile indicates the direction of the extrusion.

Choose OK.

Creating Extruded Features |127

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

Next, you create and constrain another profile, and extrude it to cut material

from the base feature.

To create a profile sketch

1Change to the top view of your part.

Desktop Menu View ➤ 3D Views ➤ Top

2Use RECTANGLE to sketch a rectangle as shown in the following illustration,

responding to the prompts.

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

➤ Rectangle.

Specify first corner point or [Chamfer/Elevation/Fillet/Thickness/Width]:

Specify a point (1)

Specify other corner point: Specify a second point (2)

128 |Chapter 8 Creating Sketched Features

3Use AMRSOLVESK to solve the sketch.

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

➤ Single Profile.

The command line indicates the number of constraints required to fully con-

strain the profile.

Solved underconstrained sketch requiring 4 dimensions or constraints.

Before you extrude the profile, fully constrain it by adding four dimensional

constraints.

To constrain a sketch

1Use AMPARDIM to add parametric dimensions to fully constrain the sketch,

responding to the prompts.

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

➤ New Dimension.

Select first object: Specify the top edge (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.1574>: Enter .16

Solved underconstrained sketch requiring 3 dimensions or constraints.

Select first object: Specify the top edge again (1)

Select second object or place dimension: Specify the top arc (3)

Specify dimension placement: Place the dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.0730>: Enter .08

Solved underconstrained sketch requiring 2 dimensions or constraints.

Creating Extruded Features |129

2Continue creating the parametric dimensions.

Select first object: Specify the right edge (5)

Select second object or place dimension: Place the dimension (6)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.4500>: Enter .5

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Specify the left edge (7)

Select second object or place dimension: Specify the left arc (8)

Specify dimension placement: Place the dimension (9)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.2430>: Enter v

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.2430>: Enter .25

After you finish dimensioning, the following message is displayed on the

command line:

Solved fully constrained sketch.

Select first object: Press ENTER

Your sketch should look like this.

NOTE For clarity, the parametric dimensions controlling Profile1 are not

shown.

Now that the profile is fully constrained, you extrude it into the base feature

to cut material from your part.

130 |Chapter 8 Creating Sketched Features

To add an extruded feature to a part

1Change to an isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

2Extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

3In the Extrusion dialog box, specify the following:

Operation: Cut

Distance: Enter 0.25

Termination: Blind

4Choose OK to exit the dialog box.

Your part should look like this.

Save your file.

Editing Extruded Features

Because an extruded feature is controlled by parametric dimensions, you can

easily make changes to it by modifying the values of the profiled sketch, or

the extruded feature itself.

Editing Extruded Features |131

To modify a consumed profile

1Expand ExtrusionBlind2 in the Browser.

2Edit the dimensions of the profile used to define the shape of the extrusion,

responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Select the cut extrusion

Enter an option [Next/Accept] <Accept>: ExtrusionBlind2: Press ENTER

3Choose OK to exit the Extrusion dialog box, then continue on the command

line.

Select object: Select the 0.5 dimension (1)

Enter new value for dimension <.5>: Enter 1

Solved fully constrained sketch.

Select object: Select the 0.25 dimension (2)

Enter new value for dimension <.25>: Enter .5

Solved fully constrained sketch.

Select object: Press ENTER

NOTE For clarity, the taper and depth dimensions are not illustrated.

132 |Chapter 8 Creating Sketched Features

4Use AMUPDATE to update your part.

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

The part now reflects the changes to the profile that controls the shape of the

extrusion you used to cut material from the part.

Next, modify the extrusion feature to change the depth of the cut.

To modify a feature

1Select the cut extrusion to modify, responding to the prompt.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Press ENTER, and select the cut extrusion

Enter an option [Next/Accept] <Accept>: Press ENTER

2In the Extrusion dialog box, specify a distance of .15 and Choose OK.

3Continue on the command line.

Select object: Press ENTER

4Use AMUPDATE to update the part.

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

Editing Extruded Features |133

Your part should look like this.

Save your file.

Extruding Open Profiles

You extrude open profiles to create rib features and thin features.

For more information about sketching open profiles, see “Creating Open Pro-

file Sketches” on page 46.

Creating Rib Features

To create a rib feature on a part model, you sketch an open profile to shape

the rib, define the thickness of the rib, and extrude it to part surfaces.

Observe these rules when you sketch open profiles for ribs:

■Sketch the side view of the rib.

■The sketch can have any number of segments.

■The ends of the sketch need not touch surfaces the rib will attach to, but

when extended must meet valid active part surfaces, without holes in the

extrusion path.

You solve the sketch to create an open profile, and apply parametric con-

straints and dimensions as with any other profile sketch.

Like other features, the rib feature can be edited and it has dependencies. If

you delete something in your model that a rib feature depends upon, such as

a face that a profile plane is based on, you delete the rib feature as well.

134 |Chapter 8 Creating Sketched Features

In this exercise, you extrude a rib feature to two perpendicular walls of a part.

Turn off visibility for EXTRUDE_1, and make EXTRUDERIB_1 visible.

Browser Right-click EXTRUDE_1 and choose Visible. Then right-

click EXTRUDERIB_1 and choose Visible.

Activate EXTRUDERIB_1 and position it on your screen.

Browser Double-click EXTRUDERIB_1. Then right-click

EXTRUDERIB_1 and choose Zoom to.

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

To create a rib feature

1Change to the front view so you can sketch the rib from its side.

Desktop Menu View ➤ 3D Views ➤ Front

2Use PLINE to sketch a rough outline of the rib, as shown in the following illus-

tration. The sketch doesn’t have to be touching the surfaces.

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

➤ Polyline.

NOTE For clarity, the work plane is not shown.

Editing Extruded Features |135

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

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

➤ Single Profile.

Select part edge to close the profile <open profile>: Press ENTER

An icon for the open profile is displayed in the Browser.

4Use AMPARDIM to add an angular dimension between the lower wall and the

lower section of the rib, responding to the prompts.

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

➤ New Dimension.

Select first object: Specify a point on the rib (1)

Select second object or place dimension: Specify a point on the lower wall (2)

Specify dimension placement: Specify a point to place the dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<71>: Enter a value of 73

Select first object: Specify the next dimension to add

Continue adding dimensions, as shown in the illustration, to fully constrain

the open profile sketch.

Solved fully constrained sketch.

Select first object: Press ENTER

5Use AMRIB to create the rib.

Browser In the Browser, right-click the open profile icon, and

choose Rib.

136 |Chapter 8 Creating Sketched Features

In the Rib dialog box, specify:

Type: Midplane

Thickness: .05

Choose OK.

6Use 3DORBIT to rotate your part so you can see the rib feature.

Your part should look like this.

Creating Thin Features

To create a thin feature, you sketch an open profile and extrude it to part sur-

faces. When you extrude an open profile, the Extrusion dialog box includes

the options for defining a thin wall feature. When you sketch open profiles

for thin features

■Sketch must be an open profile from the front view

■Sketch is extruded normal to the sketch plane

■Ends of the open profile need not touch surfaces, but when extended must

meet valid active part surfaces, without holes in the extrusion path

For more information about sketching open profiles, see “Creating Open Profile

Sketches” on page 46.

Editing Extruded Features |137

In this exercise, you create a thin wall in a shell. In the Browser, turn off

visibility for EXTRUDERIB_1, and make EXTRUDETHIN_1 visible.

Browser Right-click EXTRUDERIB_1 and choose Visible. Then

right-click EXTRUDETHIN_1 and choose Visible.

Activate EXTRUDETHIN_1 and position it on your screen.

Browser Double-click EXTRUDETHIN_1. Then right-click

EXTRUDETHIN_1 and choose Zoom to.

To create a thin feature

1Use AMWORKPLN to create a work plane for the profile sketch.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:

1st Modifier: Planar Parallel

2nd Modifier: Offset

Offset: Enter .75

Choose OK.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the back face of the shell

Enter an option [Next/Accept] <Accept>: Press ENTER

Enter an option [Flip/Accept] <Accept>:

Flip to point arrow to back face, or press ENTER

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>: Press ENTER

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

Desktop Menu View ➤ 3D Views ➤ Right

138 |Chapter 8 Creating Sketched Features

3Use LINE to sketch the thin feature.

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

➤ Line

Specify first point: Specify the start point of the line (1)

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

NOTE Turn OSNAP off so that you will not snap to the back face when you pick.

4Use AMRSOLVESK to solve the sketch, responding to the prompt.

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

➤ Single Profile.

Select part edge to close the profile <open profile>: Press ENTER

In the Browser, an open profile icon is displayed.

5Change to the front right isometric view to extrude the profile.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

6USE AMEXTRUDE to extrude the open profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify

Operation: Join

Termination: Type: Face

Thickness: Type: Midplane

Thickness: Enter .05

Editing Extruded Features |139

Choose OK.

7Respond to the prompt:

Select Face: Select the back face of the shell and press ENTER

Enter an option [Next/Accept] <Accept>: Press ENTER

Your part should look like this.

A thin wall is created with equal thickness on each side of the profile. In the

Browser, an icon is displayed for the thin extrusion.

NOTE When you extrude an open profile, the Extrusion dialog box contains

options for defining a thin feature.

Save your file with a new name so you can use the same shell part for the next

exercise.

140 |Chapter 8 Creating Sketched Features

Creating Emboss Features

Emboss features are text sketch profiles extruded on part models. A text

sketch profile is one line of text displayed in a rectangular boundary.

To create a text sketch profile, you define a font and a style, and enter one

line of text. Then you place the text on an active sketch plane on your part,

and extrude it to emboss the surface of your part with the text.

Delete the thin extrusion from your shell part.

Browser Right-Click ThinExtrusionToFace1 and choose Delete.

Highlighted features will be deleted. Continue? [Yes/No] <Yes>: Press ENTER

Change to the Front view to create the emboss feature.

Desktop Menu View ➤ 3D Views ➤ Front

To create an emboss feature

1Use AMWORKPLN to create a work plane for the text sketch.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:

1st Modifier: On Edge/Axis

2nd Modifier: Planar Parallel

Choose OK.

2Respond to the prompts:

Select work axis, straight edge or [worldX/worldY/worldZ]:

Select the top edge of the shell

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the front face of the shell and press ENTER

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>: Press ENTER

NOTE Verify that CMDDIA is set to 1 so that the Text Sketch dialog box will be

displayed. On the command line, enter CMDDIA, then enter 1.

3Use AMTEXTSK to create a text sketch profile.

Command AMTEXTSK

Editing Extruded Features |141

In the Text Sketch dialog box, specify:

True Type Font: Sans Serif

Style: Regular

Text: Enter Autodesk

Choose OK.

4Define a location for the text sketch with a rotation angle of 15, responding

to the prompts.

Specify first corner: Specify a point in the lower left corner of the shell

Specify opposite corner or [Height/Rotation]: Enter r and press ENTER

Specify second angle endpoint or [Direction] <0>:

Move the cursor to the right and specify a rotation angle of 15

Hold the cursor in one location momentarily to display the angle dimension.

NOTE For clarity, the work plane is not shown.

Continue on the command line.

Specify opposite corner or [Height/Rotation]: Specify a point for the height

142 |Chapter 8 Creating Sketched Features

As you move the cursor, the rectangular border adjusts to accommodate the

size of the text.

In the Browser, an icon is displayed for the text sketch.

You can change the parametric dimension for the height, and you can control

the placement of the text object with typical 2D constraints and parametric

dimensions between the rectangular boundary and other edges or features on

your part.

After the text sketch is positioned on the part, you can extrude it.

5Use AMEXTRUDE to extrude the text sketch.

Browser Right-click the text sketch icon and choose Extrude.

In the Extrusion dialog box, specify:

Operation: Join

Distance: Enter .5

Termination: Type: Blind

Choose OK.

6Use 3DORBIT to rotate your part so you can see the emboss feature.

Toolbutton

Your part should look like this.

Creating Loft Features |143

Editing Emboss Features

You can edit the text in an emboss feature using the Text Sketch dialog box

before the text sketch is consumed. After a text sketch is consumed by a fea-

ture, you can edit the feature dimensions or the sketch font and style.

Creating Loft Features

You create loft features by defining a series of cross sections through which

the feature is blended. Lofts may be linear or cubic. Both types can be created

with existing part faces as the start and end sections.

Creating Linear Lofts

A linear loft is a feature created by a linear transition between two planar

sections.

First, activate the next part in your drawing.

To activate a part

1Make LOFT1_1 visible.

Browser Right-click LOFT1_1 and choose Visible.

NOTE Because LOFT1_1 does not contain any features, you cannot use the

toolbutton, menu, or command methods to make it visible.

2Activate LOFT1_1.

Browser Right-click LOFT1_1 and choose Activate Part

3Make EXTRUDE_1 invisible.

Browser Right-click EXTRUDE_1 and choose Visible.

4In the Desktop Visibility dialog box, select the Assembly tab.

5Choose Select and continue on the command line.

Select assembly objects to hide: Select EXTRUDE_1

Select assembly objects to hide: Press ENTER

6Choose OK to exit the dialog box.

If you choose the Browser method, the dialog box is not displayed.

Next, create the lofted feature.

144 |Chapter 8 Creating Sketched Features

To create a linear loft

1Expand LOFT1_1 in the Browser. Minimize EXTRUDE_1.

2Zoom in to LOFT1_1.

Desktop Menu View ➤ Zoom ➤ All

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

feature.

3Create the loft feature, responding to the prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Loft.

Select profiles or planar faces to loft: Specify the bottom profile

Select profiles or planar faces to loft: Specify the top profile

Select profiles or planar faces to loft or [Redefine sections]: Press ENTER

4In the Loft dialog box, specify:

Type: Linear

Creating Loft Features |145

5Choose OK to exit the Loft dialog box.

Mechanical Desktop® calculates and displays the loft feature.

Save your file.

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

Creating Cubic Lofts

A cubic loft is created by a gradual blend between two or more planar sec-

tions. Before the loft begins blending with the next section, you can control

the tangency and the take-off angle at the start and end sections, and the dis-

tance the loft follows the tangent or angle options.

To create a cubic loft

1Make LOFT2_1 visible.

2Activate LOFT2_1.

3Make LOFT1_1 invisible.

4Zoom in to LOFT2_1.

Browser Right-click LOFT2_1, and choose Zoom to.

146 |Chapter 8 Creating Sketched Features

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

5Create the loft, responding to the prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Loft.

Select profiles or planar faces to loft: Select the bottom profile

Select profiles or planar faces to loft: Select the middle profile

Select profiles or planar faces to loft or [Redefine sections]: Select the top profile

Select profiles or planar faces to loft or [Redefine sections]: Press ENTER

6In the Loft dialog box specify:

Type: Cubic

7Choose OK to exit the Loft dialog box.

The loft is displayed with isolines because it is created from elliptical and cir-

cular sections. The default isoline setting displays the loft as in the following

illustration.

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

feature.

Creating Loft Features |147

To change the number of isolines

1Modify the ISOLINES system variable.

Command ISOLINES

New value for ISOLINES <4>: Enter 6

2Regenerate your drawing.

Desktop Menu View ➤ Regen

Mechanical Desktop regenerates the drawing and displays the loft using

more isolines.

NOTE A higher value for ISOLINES increases the time it takes to recalculate a

part. In general, keep ISOLINES at its default value (4).

3Reset the value of ISOLINES to its default setting.

Command ISOLINES

New value for ISOLINES <6>: Enter 4

4Regenerate your drawing.

Desktop Menu View ➤ Regen

Save your file.

In the next exercise you create a cubic loft using an existing part face as the

start section of the loft.

148 |Chapter 8 Creating Sketched Features

To create a cubic loft from an existing face

1Make LOFT3_1 visible.

2Activate LOFT3_1.

3Make LOFT2_1 invisible.

4Zoom in to LOFT3_1.

LOFT3 contains an existing extrusion and two profiles parametrically con-

strained to it.

NOTE For clarity, the parametric dimensions are not shown.

5Select the profiles to use for the cubic loft, following the prompts, and join

the loft to the existing extrusion.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Loft.

Select profiles or planar faces to loft: Select the front planar face (1)

Enter an option [Accept/Next] <Accept>:

Highlight the front face and press ENTER

Select profiles or planar faces to loft: Select the first profile (2)

Select profiles or planar faces to loft or [Redefine sections]:

Select the second profile (3)

Select profiles or planar faces to loft or [Redefine sections]: Press ENTER

Editing Loft Features |149

6In the Loft dialog box, specify:

Operation: Join

Type: Cubic

Choose OK to exit the Loft dialog box.

Your drawing should look like this.

Save your file.

Editing Loft Features

You edit loft features the same way extruded features are edited—change the

profiles or modify the loft feature itself.

Try editing the loft features you created in this section.

150 |Chapter 8 Creating Sketched Features

Creating Revolved Features

You create revolved features by revolving a closed profile about an axis. The

axis may be a work axis or a part edge.

To create a revolved feature about a work axis

1Make REVOLVE_1 visible.

2Activate REVOLVE_1.

3Expand REVOLVE_1 and make Work Axis1 visible.

4Make LOFT3_1 invisible.

5Zoom in to REVOLVE_1.

REVOLVE_1 contains a profile parametrically constrained to a work axis.

NOTE For clarity, the parametric dimensions are not shown.

6Create a revolved feature.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Revolve.

7Respond to the prompt as follows:

Select revolution axis: Specify the work axis

8In the Revolution dialog box, specify:

Angle: Enter 360

Termination: By Angle

work axis

Editing Revolved Features |151

Choose OK.

Mechanical Desktop calculates and displays the feature.

Save your file.

Editing Revolved Features

Edit a revolved feature by making changes to the profile, or by modifying the

feature itself (like editing extruded and lofted features).

Try editing your revolved feature following the procedures for editing

extruded features you learned earlier in this tutorial.

152 |Chapter 8 Creating Sketched Features

Creating Face Splits

Use face splits to split existing part faces. They can be created with

■An existing part face

■A work plane

■A split line

First, use one of the part’s existing faces to split a face.

To split a face using an existing part face

1Make FSPLIT_1 visible.

2Activate FSPLIT_1.

3Make REVOLVE_1 invisible.

4Zoom in to FSPLIT_1.

FSPLIT_1 contains a part, a work plane, and a split line.

NOTE For clarity, the parametric dimensions are not shown.

5Create the face split, responding to the prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] <pRoject>: Enter p

Select faces to split or [All]: Specify the left back face (1)

Enter an option [Accept/Next] <Accept>:

Enter n to flip to the back face or press ENTER to continue

Select faces to split or [All/Remove]: Press ENTER

Select planar face or work plane for split: Specify the top right face (2)

Enter an option [Accept/Next] <Accept>:

Enter n to flip to the top face or press ENTER

work plane

split line

Creating Face Splits |153

Mechanical Desktop splits the back face into two faces.

Next, split a face using a work plane.

To split a face using a work plane

1Create the face split, responding to the prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] <pRoject>: Enter p

Select faces to split or [All]: Specify the top right face (1)

Enter an option [Accept/Next] <Accept>:

Enter n to flip to the top face or press ENTER to continue

Select faces to split or [All/Remove]: Specify the right front face (2)

Enter an option [Accept/Next] <Accept>:

Enter n to flip to the front face or press ENTER to continue

Select faces to split [All/Remove]: Press ENTER

Select planar face or work plane for split: Specify the work plane (3)

154 |Chapter 8 Creating Sketched Features

Your drawing should look like this.

Now split the front face using the split line sketch.

To split a face using a split line

1Make Work Plane2 invisible.

2Create the face split, responding to the prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Face Split.

Enter facesplit type [Planar/pRoject] <pRoject>: Press ENTER

Select faces to split or [All]: Specify the left front face (1)

Enter an option [Accept/Next] <Accept>:

Enter n to flip to the front face or press ENTER to continue

Select faces to split or [All/Remove]: Press ENTER

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

Editing Face Splits |155

When you choose the Project option, Mechanical Desktop automatically

looks for an unconsumed split line. If more than one split line exists, you are

prompted to select the split line for the face split.

Mechanical Desktop displays the new face split.

The Browser contains three face split features.

Save your file.

Editing Face Splits

Face splits created from an existing planar face can be edited by modifying

the position of the face on the part. Face splits created from a work plane can

be edited by modifying the dimensions controlling the location of the work

plane. Face splits created from a split line can be modified by editing the

parametric dimensions that control the split line.

Try editing the face splits you just completed in this exercise.

Creating Sweep Features

Sweep features can be either 2D or 3D. Both are created by sweeping a closed

profile along a path.

156 |Chapter 8 Creating Sketched Features

Creating 2D Sweep Features

You create a 2D sweep feature by sweeping a profile along a path that lies on

a 2D plane. The feature may be the base feature of your part, or you can use

Boolean operations to cut, intersect, split, or join the feature to your part.

To create a 2D sweep

1Make SWEEP1_1 visible.

2Activate SWEEP1_1.

3Make FSPLIT_1 invisible.

4Zoom in to SWEEP1_1.

SWEEP1_1 contains a solved profile constrained to the start of a 2D path.

NOTE For clarity, the parametric dimensions and the work point are not shown.

5Create the 2D sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

Creating Sweep Features |157

Your drawing should look like this.

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

Save your file.

Creating 3D Sweep Features

With Mechanical Desktop, you can also sweep profiles along a variety of 3D

paths. Use these paths to create a feature swept along

■A helical path

■A spiral path

■A path defined by a 3D spline

■A path created from filleted 3D polylines and lines

■A path created from existing part edges

For more information about creating 3D paths, see chapter 6, “Creating Para-

metric Sketches.”

First, create a 3D helical sweep.

To create a 3D helical sweep

1Make SWEEP2_1 visible.

2Activate SWEEP2_1.

3Make SWEEP1_1 invisible.

4Zoom in to SWEEP2_1.

158 |Chapter 8 Creating Sketched Features

SWEEP2_1 contains a cylinder and a helical path. A solved profile is constrained

to the start of the path.

5Create the 3D helical sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

You can create a cut, join, intersection, or split feature. These options are

available because there is a base feature in the part definition.

Choose OK to exit the dialog box.

Mechanical Desktop calculates the sweep and displays your part.

Save your file.

Next, create a spiral 3D sweep.

Creating Sweep Features |159

To create a spiral 3D sweep

1Make SWEEP3_1 visible.

2Activate SWEEP3_1.

3Make SWEEP2_1 invisible.

4Zoom in to SWEEP3_1.

SWEEP3_1 contains a spiral helical path and a solved profile constrained to

the start of the path. The spiral path is elliptical.

5Create the 3D sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

Your drawing should look like this.

Save your file.

Next, create a sweep using a 3D edge path.

160 |Chapter 8 Creating Sketched Features

To create a sweep from a 3D edge path

1Make SWEEP4_1 visible.

2Activate SWEEP4_1.

3Make SWEEP3_1 invisible.

4Zoom in to SWEEP4_1.

SWEEP4_1 contains a 3D edge path and a solved profile constrained to the

start of the path.

5Create the sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

Your drawing should look like this.

Save your file.

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

Creating Sweep Features |161

To create a sweep from a 3D pipe path

1Make SWEEP5_1 visible.

2Activate SWEEP5_1.

3Make SWEEP4_1 invisible.

4Zoom in to SWEEP5_1.

SWEEP5_1 contains a 3D pipe path and a solved profile constrained to the

start of the path.

5Create the sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

Your drawing should look like this.

Save your file.

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

162 |Chapter 8 Creating Sketched Features

To create a sweep from a 3D spline path

1Make SWEEP6_1 visible.

2Activate SWEEP6_1.

3Make SWEEP5_1 invisible.

4Zoom in to SWEEP6_1.

SWEEP6_1 contains a 3D spline path and a solved profile constrained to the

start of the path.

5Create the sweep.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Sweep.

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

Your drawing should look like this.

Save your file.

Editing Sweep Features |163

Editing Sweep Features

As with all sketched features, sweep features can be edited by modifying the

profile, the path, or the feature itself.

Try modifying the sweep features you just created.

Creating Bend Features

The bend feature is for bending flat or cylindrical parts.

To create a bend feature, you sketch a single line segment on your part and

create an open profile to define the tangency location where the part transi-

tions from its current shape to the final bent shape.

To bend an entire flat part, sketch the open profile to extend over the entire

part. To bend only a portion of a flat part, sketch the open profile over only

the portion you want to bend.

By choosing options and entering values in the Bend dialog box, you design

a theoretical cylinder tangent to the open profile, about which the part

bends. The bend feature is placed automatically in one operation.

In the next exercise, you create a bend feature on a portion of a flat part.

Make the BEND_1 part visible. Then activate it and use ZOOM to position the

part on your screen.

164 |Chapter 8 Creating Sketched Features

To create a bend feature on a flat part

1Use LINE to sketch a line on one side of the plate, responding to the prompts.

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

Line.

Specify first point: Select the start point of the line

Specify next point [or Undo]: Select the end point of the line, and press ENTER

2Use AMPROFILE to create an open profile, responding to the prompt.

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

➤ Single Profile.

Select part edge to close the profile <open profile>: Press ENTER

In the Browser, an icon for the open profile is displayed.

3Use AMBEND to create the bend feature.

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

Work Features ➤ Bend.

4In the Bend dialog box specify:

Combination: Angle+Radius

Radius: 1.0

Angle: 90

Flip Bend Side: Verify that the direction arrow points toward the hole

Flip Direction: Verify that the arrow points up

Editing Bend Features |165

Choose OK.

Hide the hidden lines to see your part better. To display silhouette edges, you

set the DISPSILH system variable to 1 first.

5Change the setting for DISPSILH.

Command DISPSILH

New value for DISPSILH <0>: Enter 1

6Use HIDE to hide the hidden lines.

Desktop Menu View ➤ Hide

Your part should look like this.

The bend is completed, and an icon for the bend feature is displayed in the

Browser. Save your file.

Editing Bend Features

Use typical editing methods to edit a profile for a bend feature or to redefine

the bend.

Try redefining the bend feature you just created.

166

167

In This Chapter 9

Creating Work Features

In Autodesk® Mechanical Desktop®, work features are

special construction features that you use to place

geometry that would otherwise be very difficult to

position parametrically.

By constraining sketched and placed features to a work

feature, that is in turn constrained to your part, you can

easily control their location by changing the position of

the work feature.

This tutorial teaches you how to use work features to

control the position of sketched features. You learn

about each of these features as you work through the

tutorial.

■Work planes

■Work axes

■Work points

168 |Chapter 9 Creating Work Features

Key Terms

Te r m Definition

nonparametric work

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

parametrically changed, the work plane is unaffected.

parametrics A solution method that uses the values of part parameters to determine the

geometric configuration of the part.

parametric work plane A work plane associated with and dependent on the edges, faces, planes, vertices,

and axes of a part.

sketch plane A temporary drawing surface that corresponds to a real plane on a feature. It is an

infinite plane with both X and Y axes on which you sketch or place a feature.

work axis A parametric construction line created along the centerline of a cylindrical feature,

or sketched on the current sketch plane. A work axis can be used as the axis of

revolution for a revolved or swept feature, an array of features, to place a work

plane, and to locate new sketch geometry. It can be included in dimensions.

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

work plane An infinite plane attached to a part. A work plane can be designated as a sketch

plane and can be included in a constraint or dimension scheme. Work planes can

be either parametric, or nonparametric.

work point A parametric work feature used to position a hole, the center of an array, or any

other point for which there is no other geometric reference.

Basic Concepts of Work Features |169

Basic Concepts of Work Features

When you build a parametric part, you define how the part’s features are

associated. Changing one feature directly affects all the features related to it.

Work features are special construction features that help you define the rela-

tionships between the features on your part. They provide control when

placing sketches and features. Any changes to the position of a work feature

directly affect the placement of the sketches and features constrained to it.

You use work features to define

■A plane to place sketches and features

■A plane or edge to place parametric dimensions and constraints

■An axis or point of rotation for revolved, swept, and array features

There are three types of work features: work planes, work axes, and work

points. In this tutorial, you learn the basics of creating and modifying each

of these work features.

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

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing contains three simple parts.

Each part has a profile sketch associated with it. You create work features to

control the behavior of each of the sketches.

170 |Chapter 9 Creating Work Features

Creating Work Planes

A work plane is an infinite plane that you attach to your part. It can be either

parametric or nonparametric. A work plane can also be used to define a sketch

plane for new geometry. To position a feature that does not lie on the same

plane as your base feature, you define a new plane and then create the feature.

If the plane is parametric, any changes to it affect the position of the feature.

Work planes are defined using two modifiers. The modifiers determine how

the plane will be oriented. By selecting the right modifiers, you can create a

work plane wherever you need a plane to place geometry.

Parametric work planes can be created by specifying edges, axes, or vertices,

and defining whether the plane is normal, parallel, or tangent to selected

geometry. Nonparametric work planes can be created on the current coordi-

nate system (UCS), or on any of the three planes of the World Coordinate

System (WCS).

For more information about creating work planes, see AMWORKPLN in the

online Command Reference.

PART1_1 contains an extrusion with a profile constrained to its back face.

NOTE For clarity, the parametric dimensions are not shown.

In this tutorial, you use this profile to cut material from the part. By extrud-

ing the profile to a work plane, you can easily control the depth of the extru-

sion by changing the position of the plane.

Creating Work Planes |171

First, you create a work plane through the midplane of the part and extrude

the profile to it. Later, you edit the position of the work plane to modify the

depth of the new extrusion.

Activate PART1_1 and use ZOOM to position it on your screen.

Browser Double-click PART1_1. Now right-click PART1_1 and

choose Zoom to.

To create a work plane

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

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

2In the Work Plane dialog box, specify:

1st Modifier: Planar Parallel

2nd Modifier: Offset

Offset: Enter .5

Choose OK.

3Continue on the command line.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify the front face

Enter an option [Next/Accept] <Accept>:

Enter n to cycle to the front face or press ENTER

Enter an option [Flip/Accept] <Accept>:

Enter f to point direction arrows into the part

Enter an option [Flip/Accept] <Accept>: Press ENTER

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <accept>: Press ENTER

A work plane now bisects the part.

Next, extrude the profile to the work plane.

work plane

172 |Chapter 9 Creating Work Features

To extrude a profile to a plane

1Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

2In the Extrusion dialog box, specify the following:

Operation: Cut

Termination: Plane

Choose OK to exit the dialog box.

3Continue on the command line.

Select face or work plane: Specify the work plane

The profile is extruded to the work plane.

Now edit the location of the work plane to control the depth of the extrusion

you just created.

Editing Work Planes |173

Editing Work Planes

Because a nonparametric work plane is static, any features constrained to it

are restricted to the original plane. If you change the position or orientation

of your part, the features remain associated with the work plane and your

part could fail to update.

Whenever possible, locate your features on parametric work planes. When

you change the location of a parametric work plane, you change the position

of any features created on it or constrained to it.

To modify the position of a work plane

1Use AMEDITFEAT to reposition the work plane, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature]

<selectFeature>: Press ENTER

Select feature: Specify the work plane

Select object: Specify the 0.5 dimension

Enter dimension value <.5>: Enter .15

Select object: Press ENTER

2Use AMUPDATE to update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

If you use the Browser, the prompt is not displayed.

Your part should look like this.

Save your file.

174 |Chapter 9 Creating Work Features

Creating Work Axes

A work axis is a parametric construction line used as the axis of revolution

for a revolved or swept feature, or an array of features; it is also used to place

a work plane, and to locate new sketch geometry. You can create a work axis

through the center of a cylindrical edge, or draw it on the current sketch

plane by specifying any two points.

PART2 contains a simple revolved feature, a work plane, and a partially con-

strained profile. You create a work axis through the center of the part. Then

you constrain the profile to the work axis so you can cut material from the

base feature.

NOTE For clarity, the parametric dimensions are not shown.

Activate PART2 and use ZOOM to position it on your screen.

Browser Double-click PART2_1. Now right-click PART2_1 and

choose Zoom to.

To create a work axis

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

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Axis.

Select cylinder, cone or torus [Sketch]: Select a cylindrical edge

Because the work axis is created through the center of the part, no constraints

are necessary.

Creating Work Axes |175

Next, constrain the profile to the new work axis and create a revolved feature

from it.

Depending on your drawing, your default dimension values may differ from

those in this exercise.

To constrain and revolve a profile

1Use AMPARDIM to constrain the profile to the work axis. Add two dimensions,

responding to the prompts.

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

➤ New Dimension.

Select first object: Specify the right edge of the profile (1)

Select second object or place dimension: Specify the work axis (2)

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.8324>: Enter h to force a horizontal dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.1671>: Enter 0

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Specify the top edge of the profile (4)

Select second object or place dimension: Specify the top edge of the part (5)

Specify dimension placement: Place the vertical dimension (6)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.1333>: Enter 0

Solved fully constrained sketch.

Select first object: Press ENTER

work axis

176 |Chapter 9 Creating Work Features

2Use AMREVOLVE to revolve a feature from the profile, responding to the

prompt.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Revolve.

Select revolution axis: Select the work axis

3In the Revolution dialog box, specify:

Operation: Cut

Angle: Enter 360

Termination: By Angle

Choose OK to exit the dialog box.

Your drawing should look like this.

Save your file.

Editing Work Axes |177

Editing Work Axes

Work axes are parametric, so any changes to the parameters controlling a

work axis affect the location of features constrained to it.

In this exercise, the work axis was created through the center of a cylindrical

object and cannot be repositioned. But by changing one of the dimensions

that constrains the profile to the axis, the revolved feature changes.

To modify the revolved feature, you change the horizontal dimension con-

straining the profile to the work axis. In this exercise, because the value of

the dimension is 0, modifying it forces the profile in the wrong direction. To

relocate the profile correctly, erase the dimension, move the profile slightly,

and then add a new horizontal dimension.

To reposition a profile constrained to a work axis

1Edit the revolved feature with the Browser.

Browser Right-click Revolution Angle1 and choose Edit Sketch.

2Use ERASE to erase the 0.00 dimension constraining the profile to the work

axis.

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

➤ Erase.

3Use MOVE to move the profile and its dimensions, following the prompts.

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

➤ Move.

Select objects: Enter w

Specify first corner: Specify a point above and left of the 0.15 dimension

Specify opposite corner: Specify a point below and right of the 0.30 dimension

11 found

Select objects: Press ENTER

Specify base point or displacement: Specify any point

Specify second point of displacement or <use first point as displacement>:

Specify a point to the left of the base point

NOTE Press F8 to turn on orthographic mode before you specify the base and

second points.

178 |Chapter 9 Creating Work Features

4Use AMPARDIM to create a new parametric dimension, following the

prompts.

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

➤ New Dimension.

Select first object: Specify the right edge of the profile

Select second object or place dimension: Specify the work axis

Specify dimension placement: Place the dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.4347>: Verify that the dimension is horizontal, then enter .15

Solved fully constrained sketch.

Select first object: Press ENTER

5Use AMUPDATE to update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

Your drawing should look like this.

Save your file.

Creating Work Points |179

Creating Work Points

A work point is a parametric point for positioning features that cannot easily

be located on a part. By constraining a feature to a work point and then con-

straining the work point to the part, you control the position of the feature.

Use work points to

■Position sketched features

■Create centers for polar arrays

■Place surface cut features

■Place holes when concentric cylindrical edges, or two planar edges, are not

available

PART3 contains a simple cylindrical extrusion with a work axis at its center,

and a sketch on its top face.

You place a work point on the sketch plane and profile the sketch. Then, you

constrain the profile to the work point, and the work point to the work axis.

Activate PART3, and use ZOOM to position it on your screen.

Browser Double-click PART3_1. Then right-click PART3_1 and

choose Zoom to.

180 |Chapter 9 Creating Work Features

To create and constrain a work point

1Use AMWORKPT to create a work point, responding to the prompt.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Point.

Specify the location of the workpoint: Specify a point near the center of the sketch

NOTE You may prefer to turn OSNAP off before you create and constrain the

work point. Click the OSNAP button at the bottom of your screen.

2Use AMPARDIM to constrain the work point to the work axis, following the

prompts.

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

➤ New Dimension.

Select first object: Specify the work point

Select second object or place dimension: Specify the work axis

Specify dimension placement: Place the dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.5890>: Verify the dimension is horizontal and enter .6

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Specify the work point

Select second object or place dimension: Specify the work axis

Specify dimension placement: Place the dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.6130>: Verify the dimension is vertical and enter .6

Solved fully constrained sketch.

Select first object: Press ENTER

Solve the sketch and constrain it to a work point.

Change to a top view of your part.

Desktop Menu View ➤ 3D Views ➤ Top

Creating Work Points |181

To solve a sketch and constrain it to a work point

1Use AMPROFILE to solve the sketch, responding to the prompts.

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

➤ Profile.

Select objects for sketch: Specify the polygon sketch

Select objects for sketch: Press ENTER

Solved underconstrained sketch requiring 8 dimensions or constraints.

NOTE Although the polygon is a single object, you cannot use Single Profile

to solve it because it was not the last object created.

The profile requires eight constraints: six to solve it, and two to constrain it

to the work point.

2Zoom in to the profile and constrain it using the dimensions in the following

illustration.

You could also use Equal Length constraints on the line segments to reduce

the number of dimensions required.

3Constrain the profile to the work point as in the following illustration.

NOTE For clarity, the dimensions of the profile are not shown.

The profile is now fully constrained. Next, you create an extrusion to cut

material from the base feature.

182 |Chapter 9 Creating Work Features

To extrude a feature through a part

1Change to an isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

2Use AMEXTRUDE to extrude the profile through the part.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Through

Choose OK.

The dimensions controlling the work point are still visible because the work

point has not been consumed by a feature.

Save your file.

Editing Work Points

Next, to relocate the extrusion you change the dimensions constraining the

work point to the work axis. The extrusion and the work point are paramet-

rically associated; any change to the position of the work point causes the

extrusion to move.

Editing Work Points |183

To edit a work point

1Use AMMODDIM to modify the vertical sketch dimension controlling the

work point, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the vertical dimension

New value for dimension <0.6000>: Enter 0

Solved fully constrained sketch.

2Use AMUPDATE to update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

3Use AMMODDIM to modify the horizontal sketch dimension controlling the

work point, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the horizontal dimension

New value for dimension <0.6000>: Enter .75

Solved fully constrained sketch.

4Update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

5Turn off the visibility of the work point and its dimensions.

Browser Right-click WorkPoint1 and choose Visible.

Save your file.

You learn more about creating work features as you go through the rest of the

tutorials in this book.

184

185

In This Chapter 10

Creating Placed Features

This tutorial introduces you to placed features, and

builds on what you learned in previous tutorials. A

placed feature is a well-defined common shape, such as

a hole or a fillet. To create a placed feature, you only

need to supply its dimensions. Autodesk® Mechanical

Desktop® creates the feature for you.

In this lesson, you learn how to create and modify

placed features.

■Holes

■Face drafts

■Fillets

■Chamfers

■Shells

■Surface cuts

■Patterns

■Copied features

■Combined features

■Part splits

186 |Chapter 10 Creating Placed Features

Key Terms

Te r m Definition

chamfer A beveled surface between two faces.

combine feature A parametric feature resulting from the union, subtraction, or intersection of a

base part with a toolbody part.

draft angle An angle applied parallel to the path of extruded, revolved, or swept surfaces or

parts. A draft angle is used to allow easy withdrawal from a mold or easy insertion

into a mated part.

face draft A part face that has a draft angle applied to it. Used to create an angle on a face

that will be needed when pulling a part out of a mold.

fillet A curved transition from one part face or surface to another. The transition cuts

off the outside edge or fills in the inside edge. The fillet can have a constant or

variable radius.

hole A geometric feature with a predefined shape: drilled, counterbore, or countersink.

pattern feature A parameter-driven collection of duplicate features. You can create rectangular,

polar, and axial patterns. If you change the original patterned feature, all the

elements in the pattern change.

placed feature A well-defined mechanical shape that does not require sketches, such as a hole,

chamfer, or fillet. Placed features are constrained to the feature on which they are

placed, and they are geometrically dependent.

shell A Mechanical Desktop feature that cuts portions of the active part by offsetting its

faces.

surface cut A feature on a part created when a surface is joined to the solid. Where the

surface cuts the part or protrudes, the part face assumes the curved shape of the

surface. The surface, like other features, is parametric; both the surface and the

part retain their parametric relationship whenever either is modified.

Basic Concepts of Placed Features |187

Basic Concepts of Placed Features

Placed features are well defined features that you don’t need to sketch, such

as fillets, holes, chamfers, face drafts, shells, surface cuts, patterns, combined

features, and part splits.

You specify values for their parameters and then you position them on your part.

To modify placed features, you simply change the parameters controlling them.

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

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing includes thirteen parts which contain the geometry you need to

create the features in this tutorial. If you are interested in how the parts in

this drawing were created, activate a part and use AMREPLAY.

Before you begin, expand the Browser hierarchy by clicking the plus sign in

front of P_FEAT. Expand the hierarchy of the active part HOLE_1.

NOTE For clarity, the work features are not shown.

188 |Chapter 10 Creating Placed Features

Creating Hole Features

You can create drilled, counterbore, and countersink hole features. Each may

be assigned tapped hole information. Holes can extend through the part,

stop at a defined plane, or stop at a defined depth. You can change a hole

from one type to another at any time.

When you create a hole, you can use the Thread tab in the Hole dialog box

to include threads. Threads can also be added to existing holes.

Instead of creating a custom hole, you can specify a standard hole from an

external file. Standard holes can be tapped or untapped.

In this exercise, you create hole features first. Then you add thread data to

the hole you created.

To create a hole feature

1Activate HOLE_1 part, and zoom in to it.

Browser In the Browser, double-click HOLE_1. Now right-click

HOLE_1 and choose Zoom to.

HOLE_1 is created from two extrusions.

Creating Hole Features |189

2Use AMHOLE to create two drilled holes.

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

Features ➤ Hole.

NOTE Hold your cursor over an icon to see a tooltip that identifies the icon.

In the Hole dialog box, on the Hole tab, select the Drilled hole type icon, and

specify:

Termination: Through

Placement: Concentric

Diameter: Enter .25

Choose OK to exit the dialog box.

190 |Chapter 10 Creating Placed Features

3Define the locations for the holes, responding to the prompts.

Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:

Specify a face (1)

Select concentric edge: Specify an edge (1)

Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:

Specify a face (2)

Select concentric edge: Specify an edge (2)

Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]:

Press ENTER

Your drawing should look like this.

Next, add internal threads to the HOLE_1.

Creating Thread Features

You can create internal or external threads on cylindrical, conical, and ellip-

tical shapes. You edit existing threads from within the Thread dialog box. As

with holes, you can specify standard threads from an external file.

In the following exercise, you add an external thread to one of the cylindrical

holes you created.

Creating Thread Features |191

To create a thread feature

1In the Browser, select the hole to add threads.

Browser Select Hole1.

2Define the thread for Hole1

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

Features ➤ Thread

Respond to the prompts:

Select cylindrical/conical edge or face: Select the circular edge of Hole1

Enter an option [Next/Accept] <Accept>: Press ENTER

In the Threads dialog box, specify:

Thread Type: Custom

Full Thread: Select the check box

Major Dia: 0.2009

Minor Dia: 0.1709

Choose OK.

The thread feature is placed on Hole1 and an icon representing the external

thread is added to the Browser hierarchy.

Next, you change one of the drilled holes to a counterbore hole, and change

the minor diameter of the thread feature.

192 |Chapter 10 Creating Placed Features

Editing Hole Features

You can change a hole feature from one type of hole to another by modifying

the parameters defining the hole.

To edit a hole feature

1Use AMEDITFEAT to change the second hole to a counterbore hole, respond-

ing to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Specify Hole2

Enter an option [Next/Accept] <Accept>: Press ENTER

2In the Hole dialog box, select the Counterbore icon, and specify:

Termination: Through

Dia: Enter .2

C’Dia: Enter .375

C’Depth: Enter .15

Choose OK to exit the dialog box.

3Continue on the command line.

Select object: Press ENTER

4Use AMUPDATE to update the part, responding to the prompt.

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

Your part should look like this.

Save your file.

Editing Thread Features |193

Editing Thread Features

You can redefine the size of an existing thread. If you need to change the

thread type, it is necessary to delete the existing thread and create a new one.

To edit a thread feature

1Use AMEDITFEAT to change and display the thread feature, responding to the

prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Press ENTER

Select feature: Select the ExternalThread1 feature

2In the Threads dialog box, specify:

Thread Type: Custom

Display Thread: Select the check box.

Minor Diameter: 0.1805

Choose OK.

3Continue on the command line.

Select object: Press ENTER

The thread feature is displayed, and reflects the new minor diameter value.

Next, you learn how to create and edit face drafts.

194 |Chapter 10 Creating Placed Features

Creating Face Drafts

Face drafts are used to add a small angle to one or more faces of a part; then

the part can be easily extracted from a mold after it is manufactured.

Face drafts can be applied from a specified plane, an existing part face, or a

part edge. You can also create a shadow draft from a circular face. If you are

creating a face draft from a plane, the plane can be either an existing face, or

a work plane offset from the part.

First, activate F-DRAFT_1 and zoom in on the part. Turn off the visibility of

HOLE_1.

The part contains a simple extrusion.

To create a face draft from a plane

1Use AMFACEDRAFT to create a face draft.

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

Features ➤ Face Draft.

In the Face Draft dialog box, specify:

Type: From Plane

Angle: Enter 10

Creating Face Drafts |195

2Choose Draft Plane and continue on the command line.

Select draft plane (planar face or work plane): Specify the bottom face

Draft direction [Accept/Flip] <Accept>: Enter f to flip the direction arrow up

Draft direction [Accept/Flip] <Accept>: Press ENTER

3In the Face Draft dialog box, in Faces to Draft, press Add.

4Continue on the command line.

Select faces to draft (ruled faces only): Specify the left side face

Select faces to draft (ruled faces only): Specify the right side face

Select faces to draft (ruled faces only): Press ENTER

NOTE Refer to the UCS icon to orient yourself when selecting faces.

5Choose OK to exit the Face Draft dialog box. Draft is applied to the two faces.

A face draft can also be applied from an existing edge.

To create a face draft from a fixed edge

1Create a face draft.

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

Features ➤ Face Draft.

In the Face Draft dialog box, specify:

Type: From Edge

Angle: Enter 10

Choose Draft Plane.

196 |Chapter 10 Creating Placed Features

2Respond to the prompts as follows:

Select draft plane (planar face or work plane): Specify the back face

Enter an option [Next/Accept] <Accept>:

Enter n to cycle to the back face, or press ENTER

Draft direction [Flip/Next] <Accept>:

Enter f to flip the arrow away from the part, or press ENTER

3In the Face Draft dialog box, specify:

Faces to Draft: Add

4Continue on the command line.

Select faces to draft (ruled faces only): Specify the bottom face

Select faces to draft (ruled faces only): Press ENTER

Select fixed edge: Specify the bottom edge of the back face

Select fixed edge: Press ENTER

5In the Face Draft dialog box, choose OK to exit.

Draft is applied to the bottom face.

Next, create a shadow draft along the circular face of the part.

Creating Face Drafts |197

To create a shadow draft

1Create the shadow draft.

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

Features ➤ Face Draft.

In the Face Draft dialog box, specify:

Type: Shadow

Angle: Enter 45

Choose Draft Plane.

2Respond to the prompts as follows:

Select draft plane (planar face or work plane): Specify the top right face

Enter an option [Next/Accept] <Accept>:

Enter n to cycle to the top right face or press ENTER

Draft direction [Flip/Accept] <Accept>:

Enter f to flip the arrow away from the part or press ENTER

3In the Face Draft dialog box, specify:

Faces to Draft: Add

4Continue on the command line.

Select faces to draft (ruled faces only): Specify the cylindrical face

Enter an option [Next/Accept] <Accept>:

Enter n to cycle to the cylindrical face or press ENTER

Select faces to draft (ruled faces only): Press ENTER

5In the Face Draft dialog box, choose OK to exit.

Your part should look like this.

The Browser contains three face draft icons nested below the FDRAFT_1 part

definition.

Save your file.

Next, you modify one of the face drafts you just created.

198 |Chapter 10 Creating Placed Features

Editing Face Drafts

To modify a face draft, you change the parameters that control it.

To edit a face draft

1Use AMEDITFEAT to change FaceDraft2, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Specify the part

Enter an option [Next/Accept] <Accept>: ExtrusionBlind1: Enter n

Enter an option [Next/Accept] <Accept>: FaceDraft1: Enter n

Enter an option [Next/Accept] <Accept>: FaceDraft2: Press ENTER

2In the Face Draft dialog box, change the Angle to 5. Choose OK.

3Continue on the command line.

Select object: Press ENTER

4Use AMUPDATE to update the part, responding to the prompt.

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

Your part should look like this.

Save your file.

Creating Fillet Features |199

Creating Fillet Features

Fillet features can range from simple constant fillets to complex cubic fillets.

Mechanical Desktop creates the following fillet types:

■Constant

■Fixed width

■Linear

■Cubic

A constant fillet has one radius defining it. A fixed width fillet is controlled

by a chord length. Linear and cubic fillets have a radius at each vertex of the

selected edges that you are filleting. A linear fillet has a straight transition

from one vertex to the next. A cubic fillet has a continually changing radius

from one vertex to the next.

Activate FILLET_1, and zoom to it. Turn off the visibility of F-DRAFT_1.

To create a constant radius fillet

1Use AMFILLET to create a constant radius fillet.

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

Features ➤ Fillet.

In the Fillet dialog box, choose Constant and specify a radius of .15.

Choose OK.

200 |Chapter 10 Creating Placed Features

2Continue on the command line.

Select edges or faces to fillet: Specify an edge (1)

Select edges or faces to fillet: Specify an edge (2), and press ENTER

The fillets are applied to your part.

Next, create a fixed width fillet where the cylindrical extrusion meets the

angled face.

To create a fixed width fillet

1Use AMFILLET to create a fixed width fillet.

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

Features ➤ Fillet.

In the Fillet dialog box, choose Fixed Width and specify a chord length of .1.

Then choose OK.

2Continue on the command line.

Select edges: Specify the circular edge on the angled face

Creating Fillet Features |201

Your part should look like this.

Create a linear fillet along the top left edge.

To create a linear fillet

1Create a linear fillet.

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

Features ➤ Fillet.

In the Fillet dialog box, choose Linear, then choose OK.

2Continue on the command line.

Select edge: Specify the top left edge

Select radius: Specify the back radius symbol

Enter radius <0.5000>: Enter .35 and press ENTER

Select radius: Specify the front radius symbol

Enter radius <0.0000>: Enter .15 and press ENTER

Select radius: Press ENTER

Your part should look like this.

You create a cubic fillet in the same way you create a linear fillet. Cubic and

linear fillets differ because a cubic fillet is a blend on constantly changing

radii from one vertex to the next.

202 |Chapter 10 Creating Placed Features

To create a cubic fillet

1Create a cubic fillet.

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

Features ➤ Fillet.

In the Fillet dialog box, choose Cubic, then choose OK.

2Continue on the command line.

Select edge: Specify the top right edge at the back of the part

Select radius or [Add vertex/Clear/Delete vertex]: Specify the back radius symbol

Enter radius <0.5000>: Enter .5 and press ENTER

Select radius or [Add vertex/Clear/Delete vertex]: Specify the front radius symbol

Enter radius <0.0000>: Enter .1 and press ENTER

Select radius or [Add vertex/Clear/Delete vertex]: Press ENTER

Your part should look like this.

The Desktop Browser contains four fillet icons nested under FILLET_1.

Save your file.

Editing Fillet Features

Like all placed features, fillets are modified by changing the parameters that

control them.

Editing Fillet Features |203

To edit a fillet

1Use AMEDITFEAT to modify the cubic fillet, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Specify Fillet4

Enter an option [Next/Accept] <Accept>:

Enter n to cycle to Fillet4 or press ENTER

Select object: Specify the .1 radius

Enter Radius <0.100000000>: Enter .5 and press ENTER

Select object: Specify the original .5 radius

Enter Radius <0.500000000>: Enter .1 and press ENTER

Select object: Press ENTER

2Use AMUPDATE to update the part, responding to the prompt.

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

Your part should look like this.

Save your file.

Delete some or all of the fillets you created in these procedures, and replace

them with your own fillets to change the shape of your part.

204 |Chapter 10 Creating Placed Features

Creating Chamfer Features

A chamfer feature is a bevelled face created between two existing faces on a

part. Chamfers can be created with an equal distance, two different distances,

or a distance and an angle. You can select an edge or a face to place a chamfer.

If one or more of the edges of a face you want to chamfer have been altered,

you need to use the edge selection method to place chamfers around that face.

First, activate CHAMFER_1 and zoom in on the part. Turn off the visibility of

FILLET_1.

The part contains a simple extrusion.

To create a chamfer defined by an equal distance

1Use AMCHAMFER to create the chamfer.

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

Features ➤ Chamfer.

In the Chamfer dialog box, specify:

Operation: Equal Distance

Distance1: Enter .5

Creating Chamfer Features |205

2Choose OK and respond to the prompts as follows:

Select edges or faces to chamfer: Specify an edge (1)

Select edges or faces to chamfer <continue>: Press ENTER

Mechanical Desktop creates the chamfer along the edge you selected.

You can also create chamfers by specifying two different distances. After you

select the edge, you specify a face for Distance 1, called the base distance. Dis-

tance 2 is applied to the other face.

206 |Chapter 10 Creating Placed Features

To create a chamfer defined by two distances

1Use AMCHAMFER to create the chamfer.

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

Features ➤ Chamfer.

In the Chamfer dialog box, specify:

Operation: Two Distances

Distance1: Enter .25

Distance2: Enter .15

Choose OK.

2Respond to the prompts as follows:

Select an edge or face to chamfer: Specify the edge (2)

Press <ENTER> to continue: Press ENTER

The specified face will be used for base distance.

Specify face for first chamfer distance (base) [Next/Accept] <Accept>:

Press ENTER

Mechanical Desktop calculates and displays the chamfer. Your drawing

should look like this.

You can create a chamfer defined by a distance and an angle. You select an

edge, and then specify the face for the angle. The distance is applied to the

other face.

Creating Chamfer Features |207

To create a chamfer defined by a distance and angle

1Define the chamfer.

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

Features ➤ Chamfer.

In the Chamfer dialog box, specify:

Operation: Distance and Angle

Distance1: Enter 1

Angle: Enter 10

Choose OK.

2Continue on the command line.

Select an edge or face to chamfer: Specify the edge (3)

Press <ENTER> to continue: Press ENTER

The specified face will be used for base distance.

Specify face for chamfer distance (base) [Next/Accept] <Accept>:

Press ENTER

Mechanical Desktop calculates and displays the chamfer.

If you need to place a chamfer on all sides of a face, you can select the face

and place a chamfer on all of the edges in one operation. This works on faces

where none of the edges to be chamfered have been altered.

208 |Chapter 10 Creating Placed Features

To create a chamfer on all edges of a face

1Define the chamfer.

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

Features ➤ Chamfer.

In the Chamfer dialog box, specify:

Operation: Equal Distance

Distance1: Enter .04

Choose OK.

2Continue on the command line.

Select edges or faces to chamfer: Select the face (4)

Enter an option [Next/Accept] <Accept>: Press ENTER

Select edges or faces to chamfer <continue>: Press ENTER

A chamfer is placed on all edges of the face you selected.

Four chamfer icons are nested below the CHAMFER_1 part definition in the

Browser.

Save your file.

Editing Chamfer Features

As with all placed features, chamfers can be edited by selecting the feature,

changing parameters, and updating the part. Try editing some of the chamfer

features you created in this section.

Creating Shell Features |209

Creating Shell Features

You use shell features to hollow parts that are used in a variety of industrial

applications. For example, you shell parts to create molds, castings, contain-

ers, bottles, and cans.

Activate SHELL_1 and zoom in on it. Turn off the visibility of CHAMFER_1.

The part is constructed from two extrusions and one fillet feature.

Next, you shell the part, and then modify it to exclude the top and bottom faces.

To create a shell feature

1Use AMSHELL to create a shell.

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

Features ➤ Shell.

In the Shell Feature dialog box, specify:

Default Thickness: Inside:Enter .1

Choose OK to exit the dialog box.

210 |Chapter 10 Creating Placed Features

Mechanical Desktop offsets all faces by the thickness you specified in the

Shell Feature dialog box.

2Change to a front view for a better view of the feature.

Desktop Menu View ➤ 3D Views ➤ Front

Save your file.

Next, you edit the feature to exclude the top and bottom faces from the shell.

Editing Shell Features

You modify shell features by changing the parameters that control them.

Shells can also have multiple thickness overrides applied to individual faces.

You learn to use multiple thickness overrides in chapter 14, “Creating Shells.”

To edit a shell feature

1Return to an isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

2Use AMEDITFEAT to modify the shell feature, responding to the prompt.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Specify the shell feature

3In the Shell Feature dialog box under Excluded Faces, choose Add.

Editing Shell Features |211

4Continue on the command line.

Select faces to exclude: Specify the bottom face

Enter an option [Accept/Next] <Accept>: Enter n to cycle to the bottom face

Enter an option [Accept/Next] <Accept>: Press ENTER

Select faces to exclude: Specify the top face

Enter an option [Accept/Next] <Accept>: Enter n to cycle to the top face

Enter an option [Accept/Next] <Accept>: Press ENTER

Select faces to exclude: Press ENTER

Choose OK to exit the Shell Feature dialog box.

5Use AMUPDATE to update your part, responding to the prompt.

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

Hide the hidden lines to see your part better. Because the part is cylindrical,

to display silhouette edges, you set the DISPSILH system variable to 1 first.

6Change the setting for DISPSILH.

Command DISPSILH

New value for DISPSILH <0>: Enter 1

7Use HIDE to hide the hidden lines.

Desktop Menu View ➤ Hide

Your part should look like this.

8Return to wireframe display.

Desktop Menu View ➤ Shade ➤ 3D Wireframe

Save your file.

212 |Chapter 10 Creating Placed Features

Creating Surface Cut Features

Surface cut features give you the flexibility of combining a parametric part

and a surface. While the surface is not parametric, its position on the part is

controlled by a work point which you can move parametrically.

Surface cut features may be used to add and remove material from a part.

Activate SURFCUT_1 and zoom in to it. Turn off the visibility of SHELL_1.

SURFCUT contains a simple rectangular extrusion, a work point, and a sur-

face. The work point is constrained to the part. You use the work point to

control the position of the surface cut.

To create a surface cut

1Use AMSURFCUT to create a surface cut, responding to the prompts.

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

Features ➤ Surface Cut.

Type=Cut

Select surface or [Type]: Specify the surface

Select work point: Specify the work point

Specify portion to remove: [Flip/Accept] <Accept>:

Enter f to flip the arrow away from the part, or press ENTER

The portion of the part above the surface is cut away, leaving the curved face

of the surface.

Editing Surface Cut Features |213

The Browser contains a surface cut icon at the bottom of the feature hierarchy

for SURFCUT_1.

Save your file.

Next, you edit the position of the surface to modify the surface cut feature.

Editing Surface Cut Features

You can modify surface cut features in one of two ways:

■Parametrically change its position.

■Manually change the shape of the surface.

In this section, you change the position of the feature by modifying the para-

metric dimensions controlling the work point associated with the surface.

To reposition a surface cut feature

1Use AMEDITFEAT to edit the feature, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Enter c

Select surfcut feature: Specify the surface

The surface is recovered.

In this state, you can modify the actual shape of the surface by editing its

grips, or change the location of the work point that controls the position of

the surface on the part.

214 |Chapter 10 Creating Placed Features

2Use AMMODDIM to change the vertical dimension controlling the work

point, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify .75

New value for dimension <.75>: Enter .5

Select dimension to change: Press ENTER

3Use AMUPDATE to update the part, responding to the prompt.

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

The part is updated to reflect the new location for the surface cut feature.

4Save your file.

Experiment with the surface by editing its control points. Use AMEDITFEAT to

recover the surface. Then select a grip to activate it. When you move the grip

to another location you will see the surface deform. Update your part to

examine the effect of your changes.

Creating Pattern Features

A pattern is a collection of duplicate features. You can create patterns with

rectangular, nonorthogonal rectangular, polar, and axial configurations, and

patterns of other pattern features.

By default, a pattern feature uses the active sketch plane as the distribution

plane for pattern instances.

Creating Pattern Features |215

While selecting a feature set for a pattern, you select each graphically depen-

dent feature individually. You can select multiple independent features.

Single instances in a pattern can be made independent of an existing pattern

feature. Once a feature is independent, it can be altered while its position

remains intact.

In this tutorial, you create several different types of patterns, using both

incremental and included spacing. In the polar pattern exercise, you make

one instance independent and alter it.

Activate R-PATTERN_1, and zoom to it. Turn off the visibility of SURFCUT_1.

R-PATTERN contains a filleted plate and one counterbore hole. You create a

rectangular pattern of the hole with incremental spacing and alignment to

an edge.

To create a rectangular pattern

1Use AMPATTERN to create a rectangular pattern, responding to the prompts.

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

Features ➤ Rectangle Pattern.

Select features to pattern: Specify the hole

Select features to pattern or [liSt/Remove] <Accept>: Press ENTER

If you use multiple features to create a pattern, you select each one individu-

ally, regardless of feature dependencies.

216 |Chapter 10 Creating Placed Features

2In the Pattern dialog box, specify:

Type: Rectangular

Column Placement: Choose Incremental Spacing, the leftmost button

Row Placement: Choose Incremental Spacing, the leftmost button

NOTE Hold the cursor over an icon for a tooltip to identify the icon.

Enter the values shown for column and row instances and spacing.

3Choose Preview, and view your pattern on the screen.

At this point, you can redefine the pattern by changing your selections in the

Pattern dialog box, and then preview the changes. Preview becomes unavail-

able once the parameters in the dialog box match the display on the screen.

Using the preview image, you can suppress instances of features in patterns.

4Choose OK to create the pattern and exit the dialog box.

Your drawing should look like this.

Creating Pattern Features |217

Use R-PATTERN again to create a nonorthogonal rectangular pattern with

included spacing and a value entered for the angle.

In the Browser, right-click the icon for the pattern you just created, and

choose delete. Verify that the R-PATTERN part is activated.

To create a nonorthogonal rectangular pattern

1Use AMPATTERN to create a nonorthogonal rectangular pattern, responding

to the prompts.

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

Features ➤ Rectangular Pattern.

Select features to pattern: Specify the hole

Select features to pattern or [liSt/Remove] <Accept>: Press ENTER

2In the Pattern dialog box, in Column Placement, select Included, the second

button from the left. Specify:

Instances: Enter 3

Angle: Enter 60

Spacing: Angle: Enter 1

In Row Placement, select Included, and specify:

Instances: Enter 2

Spacing: Enter .75

Choose OK.

The hole pattern is created at a 60-degree angle from the side of the part.

218 |Chapter 10 Creating Placed Features

Next, create a full circle polar pattern using a work axis as the center and a

specified number of instances. When you choose a different pattern type, the

appropriate options are displayed in the Pattern dialog box.

Activate P-PATTERN_1 and zoom to the part.

The part is constructed with a circular plate and two holes.

To create a polar pattern

1Use AMPATTERN create a polar pattern, responding to the prompts.

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

Features ➤ Polar Pattern.

Select features to pattern: Specify Hole2

Enter an option [Next/Accept] <Accept>: Press ENTER

Select features to pattern or [liSt/Remove] <Accept>: Press ENTER

Valid selections: work point, work axis, linear edge, cylindrical edge/face

Select rotational center: Specify the work axis

2In the Pattern dialog box, specify:

Polar Placement: Choose Full Circle

Instances: Enter 5

Creating Pattern Features |219

Choose Preview and view the pattern. Then choose OK.

Next, make one instance of the pattern independent and then alter it.

To make a pattern instance independent

1Select the pattern instance to make independent.

Browser Right-click PolarPattern, and choose Independent

Instance.

Respond to the prompts.

Select feature pattern or array instance: Select hole instance #4

An independent hole based on a work point is copied from the selected hole

instance. Dependent features are maintained and copied with the pattern

instance.

Icons for the work point and independent Hole3 are displayed in the

Browser.

220 |Chapter 10 Creating Placed Features

The previous hole instance is suppressed. It can be reclaimed using the

Pattern dialog box.

2Use AMEDITFEAT to resize the independent pattern instance.

Browser Right-click the independent Hole4, and choose Edit.

The Hole dialog box is displayed.

3In the Hole dialog box, change the diameter to .4, and choose OK.

4Use AMUPDATE to update the part, responding to the prompt.

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

The Hole3 is resized, while it maintains its position in the pattern.

You can create axial patterns, and you can create a pattern from another

pattern.

In the Browser, right-click A-PATTERN_1 and choose Activate Part. Right-

click A-PATTERN_1 again, and choose Zoom to. Turn off the visibility of

P-PATTERN_1.

A-PATTERN_1 contains a cylinder with a polar pattern of three holes. In this

exercise, you use this polar pattern to create an axial pattern, specifying a

work axis as the rotation center. You specify the number of instances, and

incremental column and row placement.

After you create the axial pattern, you use it to create another polar pattern.

In the Browser, expand A-PATTERN_1.

Creating Pattern Features |221

To create an axial pattern

1In the Browser, under A-PATTERN_1, right-click WorkAxis1 and choose

Visible.

2Use AMPATTERN to create an axial pattern, responding to the prompts.

Browser In the Browser, right-click Polar Pattern1 and choose

Pattern ➤ Axial.

Valid selections: work point, work axis, linear edge, cylindrical edge/face

Select rotational center: Specify the work axis

In the Pattern dialog box, in Axial Placement, specify:

Instances: Enter 12

Column Placement: Select Incremental Angle, the button on the left

Spacing Angle: Enter 30

Row Placement: Select Incremental Offset, the button on the left

Offset Height: Enter .2

3In the Pattern Dialog box, press Preview to view the pattern, then press OK.

The axial pattern is created on the surface of the cylinder. Hide the hidden

lines to see your part better. Because the part is cylindrical, to display silhouette

edges, you set the DISPSILH system variable to 1 first.

4Change the setting for DISPSILH.

Command DISPSILH

New value for DISPSILH <0>: Enter 1

222 |Chapter 10 Creating Placed Features

5Use HIDE to hide the hidden lines.

Desktop Menu View ➤ Hide

Your part should look like this.

6Finish the part by using the new axial pattern to create another polar pattern.

Browser In the Browser, right-click Axial Pattern1 and choose

Pattern ➤ Polar.

Select Rotational Center: Select the work axis

7In the Pattern dialog box, specify:

Polar Placement: Select Incremental Angle

Instances: Enter 2

Spacing Angle: Enter 180

Choose OK.

8Use HIDE to hide the hidden lines.

Desktop Menu View ➤ Hide

Your finished part should look like this.

Editing Pattern Features |223

Editing Pattern Features

You edit pattern features in the Pattern dialog box. In the Pattern Control

tab, you modify the instancing controls. In the Features tab, you redefine the

features in the pattern. Once a pattern is created, you cannot change the pat-

tern type.

When you delete a feature from a pattern set, you also remove other graphi-

cally dependent features that are children of that feature, such as fillets. If

you want to add a feature to the set, a feature rollback is required.

A pattern is associative to the original feature that was patterned. When you

modify the sketch of a patterned feature, you also modify the entire pattern.

Use the Pattern dialog box to preview and redefine the orientation of the dis-

tribution plane at any time. If you want to change the distribution plane to

a different plane, a feature rollback is required.

Try editing the rectangular and polar patterns you created in this section.

Editing Array Features

Although you cannot create a new array, you can edit a previously-created

array by editing the dimensions and instance constraints of the array using

command line prompts. There is no dialog box available for editing arrays.

Pre-existing array features cannot be migrated to pattern features.

The following procedure is available only when you open a drawing file that

contains a previously-created array.

To edit a previously-created array

9Use AMEDITFEAT to edit a previously created array, responding to the

prompts.

Context Menu Right-click the graphics area and choose Edit Features ➤

Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Enter I

Follow the command line prompts to edit the dimensions and instance con-

straints for your particular array.

224 |Chapter 10 Creating Placed Features

Creating Copied Features

You can copy a feature from any part, and place it on your active part on the

current sketch plane. If the feature you select is on the active part, you can

specify that the copy is independent. That way, you can modify either feature

without affecting the other. If you do not specify that the copy is indepen-

dent, or you copy a feature from an inactive part, any changes made to either

the feature or the copy are reflected in both features.

Once copied, you can constrain the copied feature to the part by editing the

sketch.

NOTE You cannot copy base features.

Activate CFEAT_1 and zoom in on the part. Turn off the visibility of

P-PATTERN_1.

The part has a blind slot on the left front face. The current sketch plane lies

on the right front face. You copy the feature to the current sketch plane and

then constrain it to the part.

Creating Copied Features |225

To copy a feature

1Use AMCOPYFEAT to create a copy of the slot, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Copy.

Select feature to be copied (from any part): Specify the blind extrusion

Parameters=Independent

Specify location on the active part [Parameters]:

Specify a location on the current sketch plane

Parameters=Independent

Specify location on the active part [Parameters/Rotate/Flip]: Enter f

Parameters=Independent

Specify location on the active part [Parameters/Rotate/Flip]: Enter r

Parameters=Independent

Specify location on the active part [Parameters/Rotate/Flip]: Enter r

Parameters=Independent

Specify location on the active part [Parameters/Rotate/Flip]:

Respecify the location or press ENTER

Your drawing should look like this.

Next, you constrain the copied feature to the part by editing the feature’s

sketch. Three dimensions constrain the original feature to the part. You

create three identical dimensions to constrain the new feature to the part.

226 |Chapter 10 Creating Placed Features

To constrain a copied feature

1Use the Browser to edit the sketch.

Browser Right-click ExtrusionBlind3 and choose Edit Sketch.

2Use AMPARDIM to add three parametric dimensions to constrain the sketch

to the part.

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

➤ New Dimension.

3Place a 0.25 horizontal dimension, a 0.35 vertical dimension, and a 0.25 ver-

tical dimension as illustrated below.

4Use AMUPDATE to update your part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

Save your file.

Editing Copied Features |227

Editing Copied Features

You can edit a copied feature by modifying the feature itself, or by modifying

its location on the part. If the copy is dependent on the original feature, or if

it was created from a feature on an inactive part, any changes to either feature

are reflected in both features.

The copied feature you created is independent from the original feature. Try

modifying the shape of the copied feature, using what you learned earlier in

this tutorial about editing extrusions.

Creating Combined Features

You create combined features by combining two parts, using Boolean opera-

tions. The part that is combined is called the toolbody. You position the tool-

body on the base part using assembly constraints, and then combine the parts.

Activate COMBINEFEAT_1 and zoom in so you can see it and TOOLBODY_1.

Turn off the visibility of CFEAT_1.

The parts have already been constrained with assembly constraints. You

learn to use assembly constraints in chapter 16, “Assembling Parts.”

COMBINEFEAT_1

TOOLBODY_1

228 |Chapter 10 Creating Placed Features

To create a combined feature

1Use AMCOMBINE to create a combined feature, responding to the prompts.

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

Features ➤ Combine.

Enter a parametric Boolean operation [Cut/Intersect/Join] <Cut>: Enter j

Select a part (toolbody) to be joined: Specify TOOLBODY_1

The parts are combined into one part.

2Look at the Browser. Expand the Combine1 icon nested under

COMBINEFEAT_1. TOOLBODY_1 has become a combined feature and is

no longer a separate part definition.

Save your file.

Editing Combined Features

Combined features can be modified by changing the assembly constraints

controlling the base part and the toolbody, by editing the base part, or by

making changes to the toolbody. You’ll learn more about combining parts

and editing toolbodies in chapter 17, “Combining Parts.”

Creating Part Splits |229

Creating Part Splits

You can split parts by creating a planar or a nonplanar split feature. A planar

split uses a work plane, existing part face, or a split line. A nonplanar split

uses a constrained sketch and a Boolean operation.

Activate P-SPLIT_1 and zoom in on the part. Turn off the visibility of

COMBINEFEAT_1.

The part is a simple extrusion with two holes and a work plane located at the

midplane of the part. You split the part into two distinct part definitions with

the work plane.

To create a part split

1Use AMPARTSPLIT to split the part, responding to the prompts.

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

Features ➤ Part Split.

Select planar face, work plane, surface, or split line for split:

Specify the work plane

Define side for new part: [Accept/Flip] <Accept>: Press ENTER

Enter name of the new part <PART2>: Press ENTER

The part is split along the work plane and a new part definition is created.

NOTE For clarity, the work plane is not shown.

230 |Chapter 10 Creating Placed Features

2Expand PART2_1 in the Browser and compare its features with P-SPLIT_1.

Both parts contain a Part Split feature, two holes, and a work plane.

Save your file.

You can also create planar splits with an existing part face, or a split line con-

strained to the part. Next, create a nonplanar split.

Activate N-SPLIT_1 and zoom in on the part. Turn off the visibility of

P-SPLIT_1 and PART2_1.

NOTE For clarity, the profile’s dimensions are not shown.

You create a nonplanar split by extruding the profile into the part. A new part

definition is created from the volume shared by the part and the extrusion.

To create a non-planar part split

1Use AMEXTRUDE to create the part split.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion Feature dialog box, specify:

Operation: Split

Termination: Blind

Distance: Enter .7

Flip: Make sure the direction arrow is flipped into the part

Choose OK to exit the dialog box.

Editing Part Splits |231

2Continue on the command line.

Enter name of the new part <PART3>: Press ENTER

The part is split and a new part definition is created.

Save your file.

Editing Part Splits

Parts created by a part split can be edited in the same way as the parts they

were created from. The new parts contain identical work geometry, and if any

feature was split, each part contains a version of that feature.

Nonplanar splits are used to create parts that fit together. Face drafts can be

applied to the faces of both parts to make them fit together easier.

Try editing the sketched and placed features that make up the parts you have

split in this section.

You are now ready to create a complex part.

232

233

In This Chapter 11

Using Design Variables

You can assign variables to the parametric dimensions

that control a part. Variables can be assigned to the

active part, or they can be global.

Active part design variables control only the features of

the part they are assigned to. Global design variables

control the features of any number of parts.

Autodesk® Mechanical Desktop® automatically

reevaluates parts, and updates them when design

variables have been modified.

■Creating active part design

variables

■Assigning variables to an active

part

■Modifying design variables

■Creating global design variables

234 |Chapter 11 Using Design Variables

Key Terms

Te r m Definition

active part variable A parametric variable used in the dimensions that control features of the active

part.

global variable A parametric variable that can be used by any number of parametric features and

parts. Also used for single parts and to constrain parts.

helical sweep A geometric feature defined by the volume from moving a profile along a 3D

path about a work axis.

pitch The measured distance parallel to the axis of a helical path, from one point on the

path to the corresponding point on the adjacent revolution.

profile plane A work plane at the start point of a helical path, placed normal to the start of the

path or at the center of the axis/path.

start angle The angle at which a helical path begins from the X axis of the active sketch

plane.

table driven variable A global or active part design variable controlled by values in a linked external

spreadsheet.

taper angle The angle where a helical sweep is tapered as it is created.

Basic Concepts of Design Variables |235

Basic Concepts of Design Variables

Parts and features are controlled by dimensions and other parameters that

define their shapes. By creating design variables and assigning them to these

parameters, you gain greater control over these values. There are two types of

design variables:

■Global

■Active part

You use global design variables when you want to control parameters that

belong to more than one part. When you want to control only a specific part,

you use active part design variables.

You can create design variables using the Design Variables dialog box, or you

can use the Equation Assistant dialog box to create design variables on the

fly as you are creating a part.

Design variables are also used in tables to control versions of a part. You learn

to create these tables in chapter 15, “Creating Table Driven Parts.”

This tutorial introduces design variables for controlling features. The tutorial

drawing file contains a helical sweep. For clarity, the sweep is represented by

four wires. The work features used to create the sweep are visible to help you

understand how it was created. Before you begin the tutorial, turn off the vis-

ibility of the work features, and set the number of wires to a lower value; this

increases the speed of recalculation and regeneration of the part.

Open the file helix1.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 spring created from a helical sweep.

236 |Chapter 11 Using Design Variables

Three work planes are associated with the part. Two were used to create the

sketched work axis for the sweep. The third, also called a profile plane, was

created normal to the start of the path when it was defined. It was used to

sketch the profile for the sweep. The profile is constrained to a work point at

the beginning of the path.

Preparing The Drawing File

Before you begin, turn off the visibility of the work features. Leave the work

axis visible because it will be helpful in keeping you oriented when you

change the variables that control the 3D path.

To hide a work feature

1Use AMVISIBLE to turn off the visibility of the first work plane.

Desktop Menu Part ➤ Part Visibility

2In the Desktop Visibility dialog box, with Hide turned on, choose Work

Planes and Work Points.

Choose Apply.

Choose OK to exit the dialog box.

Preparing The Drawing File |237

To speed up recalculations and regenerations of the helical sweep, set the

ISOLINES variable to its default value. This will display the sweep using only

one wire. Currently it is set to display the sweep as a helical tube.

To set isolines

1Change the setting for ISOLINES, responding to the prompt.

Command ISOLINES

New value for ISOLINES <8>: Enter 4

2Use REGEN to regenerate your drawing.

Desktop Menu View ➤ Regen

The helix should look like this.

To see your model better, use the shade button on the Desktop View toolbar

to toggle shading on and off. If you prefer, leave the shade option on.

To toggle shading of a part

1Use SHADE to shade your part.

Desktop Menu View ➤ Shade ➤ Gouraud Shaded

Your part should now look like this.

NOTE Shading is turned off throughout this tutorial.

The Desktop View toolbar also contains commands to dynamically rotate

your design and control views.

238 |Chapter 11 Using Design Variables

To dynamically rotate a part

1Use 3DORBIT to rotate the view of your part.

Context Menu In the graphics area, right-click and choose 3D Orbit.

2Select a point near the center of the part. This point acts as the central point

for the rotation. Press the mouse button as you move your cursor around the

screen. The part dynamically rotates as the cursor moves.

3Release the mouse button when the display is to your liking.

In the next procedure, you restore the view to its original display. The

helix1.dwg file has one saved view, View1.

To restore a saved view

1Use VIEW to restore the original drawing view.

Desktop Menu View ➤ Named Views

2In the View dialog box, highlight View1, and choose Set Current.

Choose OK.

Your drawing is returned to the original view.

Next, you define active part design variables and then assign them to the

existing helical part.

Using Design Variables |239

Using Design Variables

Design variables provide a tool for controlling dimensions, and using equations

and relationships between dimensions. Changing one or more variables affects

the entire part.

Design variables can be either active or global.

Active Part Design Variables

Active part design variables control only the part they are assigned to.

Global Design Variables

Global design variables allow you to use the same variables for multiple fea-

tures across multiple parts. If you are designing multiple parts in the same

file, you may use global design variables to control some or all of the parts

with the same variables.

Creating Active Part Design Variables

The helical sweep is governed by the following parameters:

■Type of sweep

■Number of revolutions

■Pitch

■Height

■Shape

■Diameter of the sweep

■Taper angle

■Orientation

■Start angle

■Radius of the swept profile

240 |Chapter 11 Using Design Variables

In addition to the method used in the following exercises, you can create

design variables in the Equation Assistant dialog box while you are in the

modeling process. In the Equation Assistant dialog box, you right-click in the

variables list area and choose New. A space for the new variable is provided

at the end of the list, and your cursor is positioned in the Name column.

There you enter a name for the new variable, and then you define it in the

Equation column.

In this lesson, you create variables and parametric equations to control the

number of revolutions, height, and diameter of the sweep. You also assign a

variable to control the radius of the profile that is swept along the helical

path. Because you are working with a single part, you create these variables

as active part design variables.

To create an active part design variable

1Use AMVARS to create a design variable.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, make sure the Active Part tab is selected

and choose New.

3In the New Part Variable dialog box, specify:

Name: Enter rev

Equation: Enter 8

Press ENTER.

Creating Active Part Design Variables |241

4Repeat step 3 to enter the following variables:

Ht 2

Dia .5

Rad .05

Choose OK.

The next step is to edit the existing part by replacing its dimensions with the

design variables you have just created.

242 |Chapter 11 Using Design Variables

Assigning Design Variables to Active Parts

Before the spring can be table driven, you need to assign the design variables

you have defined. You edit the sweep feature and the profile used to create

the sweep. You change the values controlling the feature with the design

variables you have just created.

To edit a sweep feature

1Use AMDIMDSP to set dimensions to display as equations.

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

➤ Dimensions as Equations.

2Use AMEDITFEAT to define the sweep feature to edit.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Highlight the helical sweep.

3In the Helix dialog box, enter the following:

Revolutions: rev

Height: ht

Diameter: dia

Choose OK. Then choose OK to exit the Sweep dialog box.

You have assigned design variables to the parameters controlling the sweep.

Assigning Design Variables to Active Parts |243

4Assign the last variable to the radius of the profile, responding to the prompts

as follows:

Select object: Select the dimension (1)

Enter dimension value <.1>: Enter rad

Select object: Press ENTER

NOTE For clarity, shading has been turned off in these illustrations. You may

prefer to keep it on throughout the tutorial.

5Use AMUPDATE to update the part, responding to the prompt.

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

The spring is updated. The part changes because the value for the rad design

variable you assigned is not the same as the original value used to create the

sweep.

244 |Chapter 11 Using Design Variables

Modifying Design Variables

Design variables can be added and modified anytime during the design process.

When the part is updated, changes to the design variables are automatically

applied.

In this exercise, you add a design variable for a taper angle on the active part.

To add a design variable to an active part

1Use AMVARS to add a design variable.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, with the Active Part tab selected, choose New.

3In the New Part Variable dialog box, specify:

Name: taper

Equation: Enter 0

Choose OK.

4Choose OK to exit the Design Variables dialog box.

Next, you edit the sweep feature by adding the new variable to its design

parameters.

To edit a sweep feature

1Use AMEDITFEAT to add the new design variable to the sweep feature.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

2Highlight the helical sweep.

3In the Helix dialog box, specify the following:

Taper Angle: taper

Choose OK. Then choose OK to exit the Sweep dialog box.

4Press ENTER to end the command.

Modifying Design Variables |245

To modify a design variable

1Use AMVARS to modify the design variable.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, with the Active Part tab selected, high-

light the taper variable. In the highlighted line, double-click the Equation

field and enter 15.

Choose OK to exit the Design Variables dialog box.

3Use AMUPDATE to update the part.

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

Save your file.

246 |Chapter 11 Using Design Variables

Working with Global Design Variables

You can assign global variables to more than one part to control similar fea-

tures. In this lesson, you move some of the active part design variables to glo-

bal variables and assign them to two parts.

Open the file helix2.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing contains two springs created from helical sweeps.

Both helical sweeps have active part design variables already assigned to

them. In this lesson, you create global design variables to control identical

features of each helix.

First, expand the Browser hierarchy by clicking the plus sign in front of

HELIX2. Then click the plus sign in front of PART1_1 and PART2_1. The

Browser should look like this. Notice PART1_1 is the active part.

Working with Global Design Variables |247

Next, examine the active part design variables for both parts.

To examine a design variable for an active part

1Use AMVARS to open the Design Variables dialog box.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, with the Active Part tab selected, examine

the values for the design variables assigned to PART1_1.

You should see four variables controlling the number of revolutions, height,

radius of the swept profile, and the taper angle of the active part. There is no

variable defined for the diameter of the helical sweep.

Choose OK to exit the dialog box.

3Use AMACTIVATE to activate PART2_1.

Browser In the Browser, right-click PART2_1 and choose Activate

Part.

4Examine the design variables assigned to PART2_1.

Desktop Menu Part ➤ Design Variables

248 |Chapter 11 Using Design Variables

5In the Design Variables dialog box, make sure the Active Part tab is selected.

Choose OK.

Both parts have active part design variables controlling the same features.

The variable controlling the height of both helical sweeps contains the same

value.

Next, you move this active part design variable to a global design variable so

that one variable controls both parts.

To move an active part variable to a global design variable

1Open the Design Variables dialog box.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, with the Active Part tab selected, high-

light the ht variable. Under Move to Global, choose Selected.

The variable is removed from the list of active part design variables.

3Click the Global tab and examine the list of global variables.

Working with Global Design Variables |249

Choose OK to exit the dialog box.

Mechanical Desktop re-evaluates the features of the part and updates the

part. Because the value of the variable has not changed, the part does not

change.

Although the ht variable for PART2_1 has been moved to global, the same

variable for PART1_1 is still an active part design variable. Because one global

variable will drive both parts, you remove the ht variable from the PART1_1

list of active part design variables.

To delete an active part design variable

1Use AMACTIVATE to activate PART1_1.

Browser In the Browser, right-click PART1_1 and choose Activate

Part.

2Open the Design Variables dialog box.

Desktop Menu Part ➤ Design Variables

3In the Design Variables dialog box, with the Active Part tab selected, high-

light the ht variable and choose Delete.

The variable is removed from the list of active part design variables.

Choose OK to exit the dialog box.

PART1_1 is re-evaluated and updated. The global design variable is now con-

trolling the height of both helical sweeps.

250 |Chapter 11 Using Design Variables

Next, you create a new global design variable to control the diameter of the

springs and assign it to both parts. Then you modify the value of the global

design variable controlling their height.

To create a global design variable

1Open the Design Variables dialog box.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, select the Global tab and choose New.

3In the New Part Variable dialog box, specify:

Name: Enter dia

Equation: Enter .75

Choose OK. The Global tab now contains two variables, ht and dia.

Choose OK to exit the dialog box.

The parts do not change because the variable has not yet been assigned to

them.

To assign a global design variable to a part

1Edit the sweep feature for PART1_1:

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

2Highlight the helical sweep.

3In the Helix dialog box, specify the following:

Diameter: dia

Choose OK. Then choose OK to exit the Sweep dialog box.

Working with Global Design Variables |251

4Continue on the command line.

Select object: Press ENTER

5Update the part.

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

Enter an option [active Part/Assembly/aLl parts/linKs] <active Part>:

Press ENTER

Mechanical Desktop updates PART1_1 using the new global design variable

to control the diameter of the sweep.

6Activate PART2_1.

7Repeat steps 1 through 5 for PART2_1.

Your drawing should look like this.

Next, you modify the global design variable controlling the height of the

parts.

PART1_1

PART2_1

252 |Chapter 11 Using Design Variables

To modify a global design variable

1Open the Design Variables dialog box.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, with the Global tab selected, highlight

the ht variable. In the highlighted line, double-click the Equation field and

enter 1.25.

Choose OK to exit the dialog box.

Mechanical Desktop re-evaluates the features and updates both parts.

Design variables are a powerful way to control the features of a part. Both

active part and global design variables may be table driven. To create a table

driven part, you use Microsoft® Excel software to create a spreadsheet con-

taining values for different versions of a part. You learn more about table

driven parts in chapter 15, “Creating Table Driven Parts.”

253

In This Chapter 12

Creating Parts

This tutorial continues with techniques you learned in

previous lessons. You use sketches to create features.

You position standard features, such as holes, and then

combine them to create a part. You analyze your design

and build a model so that you can easily incorporate

changes. This is a problem-solving process that you

can apply to any parts you create using Autodesk®

Mechanical Desktop®.

In this tutorial, you create a saddle bracket in two

phases. First, you create all the features of the part in

rough form. Then, you refine those features to complete

the part.

■Analyzing design ideas to simplify

sketching

■Selecting the base feature

■Planning the order in which to

add features

■Stabilizing features with

constraints and dimensions

■Creating features that remain

fixed relative to work planes and

work axes

■Refining features

■Adjusting features according to

design changes

254 |Chapter 12 Creating Parts

Key Terms

Te r m Definition

base feature The first feature you create. As the basic element of your part, it represents its

simplest shape. All geometry you create for a part depends on the base feature.

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

consumed when the feature is created.

Desktop Browser A graphical representation of the features that make up your model. You can work

in the Browser to create and restructure parts and assemblies, define scenes,

create drawing views, and control overall preferences.

placed feature A mechanical shape that does not require sketches, such as a hole, chamfer, or

fillet. Placed features are constrained to the feature on which they are placed and

are geometrically dependent.

sketch plane A temporary drawing surface that corresponds to a real plane on a feature. It is an

infinite plane with both X and Y axes, where you sketch or place a feature.

sketched feature A three-dimensional solid whose shape is defined by constrained sketches and

located parametrically on a part. Sketched features are extrudes, lofts, revolves,

sweeps or face splits.

work axis A parametric construction line created along the centerline of a cylindrical feature,

or sketched on the current sketch plane. A work axis can be used as the axis of

revolution for a revolved or swept feature, an array of features, to place a work

plane, and to locate new sketch geometry. It can be included in dimensions.

work feature A work axis, work point, or work plane used to construct and position a feature

where there is no face on which to sketch or place the feature. You constrain or

dimension work features to maintain symmetry throughout updates.

work plane An infinite plane attached to a part. Can be designated as a sketch plane and can

be included in a constraint or dimension scheme. Work planes can be either

parametric, or non-parametric.

work point A parametric work feature used to position a hole, the center of an array, or any

other point for which there is no other geometric reference.

Basic Concepts of Creating Parts |255

Basic Concepts of Creating Parts

You construct a model bit by bit, fashioning shapes to add to it and using

tools to cut away the portions of the shapes you do not need. In Mechanical

Desktop®, these shapes are the features of the part you are creating.

Analyzing Rough Sketches

You may be accustomed to jotting down design ideas on paper, starting with

a rough outline for a part and adding details as you go. Working with

Mechanical Desktop is similar: you put some thought into your idea, plan-

ning the best way to implement your concept.

In general, you follow this process to develop a part design:

■Look at the whole part and decide how to break it down into simple shapes.

■Identify the simplest element to use as your base feature.

■Decide the order for creating additional features.

■Determine the methods for creating the features.

■As you build individual features, review and adjust your ideas about how

the features work together.

■As you adjust your design strategy, you can revise the features you created

earlier.

With early planning, you can express your design in modular, simple terms.

When changes occur, as they often do in design work, you can easily accom-

modate them because of the parametric capabilities in Mechanical Desktop.

Any changes you make to your design are quickly recalculated.

As you study the part to determine the features you need and the order in

which to create them, also notice the relationships and patterns of the

shapes. Some features may be symmetrical, but others may be built most eas-

ily from simple shapes combined to form compound shapes.

The saddle bracket in this rough sketch has four distinct features: the saddle,

the mounting lugs, a boss, and strengthening ribs.

lug

boss

saddle

rib

256 |Chapter 12 Creating Parts

The part is symmetrical. Visualize two perpendicular centerlines—one along

the axis of the boss and another intersecting both lugs. As you create this

part, consider this symmetry as you constrain features.

As you build the saddle bracket, you learn to create features according to

the relationships among them. In this case, the base feature of the part is

the saddle and lugs. Because the remaining features attach to the saddle and

lugs, you create the main shape first. The next feature you create is the boss

because it rests directly on the saddle. Finally, you create the ribs because

they attach to both the saddle and the boss.

Creating Rough Parts

In the saddle bracket, features are present but lack details such as the arch of

the saddle, the mounting holes for the lugs, and the pipe hole for the boss.

Despite the missing details, the shape of the part and the placement of fea-

tures are symmetrical. Working from this basic part, you will add those

details.

Dimensioning and Constraining Parts

You apply dimensions and constraints to control the size and shape of a part,

and the position of part features. Dimensions can be expressed as numbers,

parameters, or equations.

You can use the Design Variables dialog box to create equations and control

the relationships between the dimensions on your model. Then you apply

the variables to your model and the model is updated to reflect the changes.

front view to

view

Creating Base Features |257

If you want to assign design variables as you are defining part sketches and

creating features, use the Equation Assistant. You can activate the Equation

Assistant in two ways:

■When you are prompted for a dimension value, right-click the graphics

area.

■While you are creating sketched and placed features, in the feature dialog

box, right-click a value field.

For more information about working with design variables, see “Using

Design Variables” on page 239.

To begin this lesson, open the file saddle.dwg in the desktop\tutorial folder.

The drawing is blank but contains the settings you need for this tutorial.

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 Base Features

The overall shape of the saddle bracket is simple. First, you sketch a shape to

represent the saddle and lugs.

Next, you convert the sketch to a base feature and modify its shape by inter-

secting it with a second feature. Intersecting the base feature is like cutting

away material you don’t need.

saddle arch

258 |Chapter 12 Creating Parts

When you create these features, you position them symmetrically using a

work axis and a work plane. Like other features, you include work features in

your constraint scheme to maintain symmetry throughout future updates to

the part.

Sketching Base Features

After you have a strategy, you are ready to sketch, constrain, and extrude the

base feature of the part. Begin by creating a sketch of the block and then con-

verting it to a profile sketch.

To make it easier to sketch the shape, turn off Polar, Osnap, and Otrack at the

bottom of your screen.

To create a profile sketch

1Use PLINE to sketch this shape. Draw the shape starting at the lower left of

the sketch.

You can use the cursor crosshairs to align the top horizontal lines (that is,

make them collinear). Use the Direction option of PLINE to control the direc-

tion of the arc.

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

➤ Polyline.

work plane

work axis

Creating Base Features |259

2Use AMPROFILE to profile your sketch.

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

➤ Single Profile.

Mechanical Desktop analyzes the sketch and displays a message on the com-

mand line:

Solved underconstrained sketch requiring 5 dimensions or constraints.

NOTE Throughout this tutorial, the number of constraints your sketch needs

may differ from the example, depending on how precisely you draw the sketch.

You learn how to modify constraints so that your sketch solves correctly.

Look at the assumed constraints and determine which constraints you need.

3Use AMSHOWCON to display all of the existing constraints.

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

Constraints ➤ Show Constraints.

Respond to the prompt to show all constraints.

Your sketch should look like this. However, the constraint numbering may

differ, depending on the order in which you drew the geometry.

In the example, all sketch elements have constraints except the arc. The lines

show vertical (V) or horizontal (H) constraints and the top two horizontal

lines show a collinear (C) constraint. A fix constraint is located at the start

point of line 0.

NOTE If the fix constraint in your sketch does not appear in the same location

as the illustration above, redraw the sketch starting at the lower left.

Now that the basic sketch shape is defined, you need to add dimensions to

stabilize its size. Start with its longest lengths to minimize the risk of distort-

ing the shape as it is resized.

260 |Chapter 12 Creating Parts

For this exercise, add dimensions in the order shown, starting with the

dimension for the bottom line.

Depending on your sketch, your default dimension values may differ from

those in this exercise.

To constrain a sketch

1Use AMPARDIM to add parametric dimensions to fully constrain the sketch,

following the prompts.

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

➤ New Dimension.

Select first object: Specify the line (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<1.2297>: Enter 1.48

Solved underconstrained sketch requiring 4 dimensions or constraints.

2To center the arc, create a horizontal dimension from the center of the arc to

the left edge of the sketch.

Select first object: Specify the left edge (1)

Select second object or place dimension: Specify the arc (2)

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.5944>: Enter .74

Solved underconstrained sketch requiring 3 dimensions or constraints.

Creating Base Features |261

3Create the dimension for the top left horizontal line. Continue to follow the

selection points.

Select first object: Specify the left horizontal line (4)

Select second object or place dimension: Place the dimension (5)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.3951>: Enter .28

Solved underconstrained sketch requiring 2 dimensions or constraints.

NOTE You may get a message stating that adding a dimension will overcon-

strain the sketch. This can occur if your sketch does not closely resemble this

exercise. Try adding the dimensions in a different order, or re-create your sketch.

4Finish dimensioning the sketch.

Select first object: Specify the arc (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Diameter/Ordinate/Placement point]

<0.4600>: Enter .68

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Specify the line on the right (3)

Select second object or place dimension: Place the dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.2176>: Enter .20

Solved fully constrained sketch.

Select first object: Press ENTER

Now that your profile sketch is fully constrained, create a solid feature.

262 |Chapter 12 Creating Parts

To extrude a feature

1Change to an isometric view of your part.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

You need to specify the type of extrusion operation, how to terminate the

extrusion, and its size.

2Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

3In the Extrusion dialog box, specify:

Distance: .66

Termination: Blind

Choose OK to create the feature.

The base feature should look like this.

4Refer to the Desktop Browser, which shows that you have added an extrusion

feature to the base feature and that the extrusion was blind (a specific depth).

Click the plus sign beside the extrusion feature to display a profile icon. This

display tells you that the extrusion feature originated with the profiled

sketch. If you complete a feature and then need to change its size or shape,

you can edit it and update the part to reflect the change.

Creating Base Features |263

To edit a consumed sketch in the Browser, double-click the profile icon to dis-

play the original sketch, or right-click to show the menu, and choose Edit

Sketch. Make any changes and choose Part ➤ Update to resize the part with

the changed values.

To edit a base feature

1Select the sketch to edit, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Enter s

Select sketched feature: Specify the extrusion

2Modify the height of the sketch, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Select the 0.20 dimension (1)

New value for dimension <.20>: Enter .12

Solved fully constrained sketch.

Select dimension to change: Press ENTER

3Use AMUPDATE to update the model, responding to the prompt.

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

Your part is updated according to the changed dimension and looks like this.

Save your file.

264 |Chapter 12 Creating Parts

Creating Work Features

Now that you have created the base feature, add the feature that defines the

rough shape of the bracket. First, create work features to maintain symmetry.

Then, use them to draw, constrain, and extrude the sketch.

The first work feature is a work axis along the centerline of the arc on the base

feature. This work axis anchors your next sketch to the base feature.

To create a work axis

1Use AMWORKAXIS to create the work axis, responding to the prompt.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Axis.

Select cylinder, cone or torus [Sketch]: Specify the cylindrical face (1)

The work axis is displayed as a line along the center of the arc.

If the work axis is not visible, the work axis display is probably turned off.

2To turn on the display, in the Browser right-click Work Axis1. Choose Visible.

The next work feature, the work plane, forms the second axis of symmetry.

This plane is parallel to the front face and intersects both lugs. You specify

the work plane position as parallel to the selected face and offset one-half the

depth of the part.

work axis

Creating Base Features |265

To locate the work plane parametrically, specify the offset depth as an equa-

tion. By using an equation, the work plane tracks changes in the bracket

width and always remains centered. To use an equation, you must determine

the dimension parameter before you define the work plane.

To create a work plane

1Use AMDIMDSP to set dimensions as equations.

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

➤ Dimensions as Equations.

2Redisplay the sketch dimensions, following the prompt.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Specify any point on the part

3Choose OK to exit the Extrusion dialog box.

Parameter d6 is the dimension that specifies the width of the feature. Because

the dimension parameters for your sketch may differ, make note of the

parameter for your part.

work plane

266 |Chapter 12 Creating Parts

4Press ENTER to exit the command.

5Create a parametric work plane in the center of the part, parallel to the front

surface, and offset one-half the width of the part.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

6In the Work Plane Feature dialog box, specify:

1st Modifier: Planar Parallel

2nd Modifier: Offset

Offset: d6/2 (substitute your parameter value for d6)

Create Sketch Plane: Clear the check box

NOTE By default, the Create Sketch Plane option in the Work Plane Feature

dialog box is selected. This setting automatically places the sketch plane (the

location on which the next feature will be sketched or placed) on the work plane.

For this exercise, you specify a sketch plane on a surface of the feature, not on

the work plane.

Choose OK.

7Identify the part face to which the work plane is parallel, responding to the

prompts.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the curved edge on the front face (1)

Enter an option [Next/Accept] <Accept>: Press ENTER

Enter an option [Flip/Accept] <Accept>: Enter f to flip the direction into the part

Enter an option [Flip/Accept] <Accept>: Press ENTER

Creating Base Features |267

The work plane is displayed as a planar rectangle. The Desktop Browser dis-

plays both a work axis and a work plane icon.

Save your file.

Defining Sketch Planes

Before you can sketch the next feature, you must define a new sketch plane,

an infinite XY plane that locates a 2D sketching surface in 3D space.

When you create sketched features, you determine the placement and orien-

tation of the sketch plane on a 2D plane. A 2D plane is

■A flat part surface

■The XY, YZ, or ZX axes of the World Coordinate System (WCS)

■A previously defined work plane

■The XY plane of the current user coordinate system (UCS)

Unlike a work feature, a sketch plane is a temporary object. Only one sketch

plane can exist at the same time.

NOTE Except for base features, you must specify a sketch plane before you can

draw a sketch. With base features, the sketch plane is automatically placed on

the current UCS.

work plane

work axis

268 |Chapter 12 Creating Parts

As you move your mouse over a part, Mechanical Desktop highlights the

faces that can be used to define a new sketch plane. Faces that cannot be used

are not highlighted. When you select a face, a temporary sketch plane

appears on that face.

You can choose the Z direction and orientation of the XY axes for the new

sketch plane.

After you have selected the options, the temporary sketch plane disappears

from the screen. You are ready to create the sketch geometry.

In the next exercise, the bottom face of the base feature is the sketch plane.

On this face, you sketch a profile to extrude through the part. Once placed,

the sketch and subsequent features remain attached to the base feature,

regardless of changes you make later.

To create a sketch plane

1Use MCAD2 to change your display to two viewports.

Desktop Menu View ➤ Viewports ➤ 2Viewports

The left viewport is a top view of the part; the right viewport is an isometric

view.

Before you create the sketch plane, check the system variable that controls

the UCS settings for your viewports. By default, each viewport has its own

UCS.

2If necessary, change the UCS setting so that each viewport uses the same

UCS, responding to the prompt.

Command UCSVP

Enter new value for UCSVP <1>: Enter 0

temporary sketch plane

Creating Base Features |269

3Use AMSKPLN to create a new sketch plane for the profile to be extruded,

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]:

Select the bottom face when it is highlighted (1)

Enter an option [Accept/Next] <Accept>:

Choose n to cycle to the bottom face, or press ENTER

Select edge to align X axis or [Z-flip/Rotate]:

Enter z to flip the Z axis up through the part

Plane = Parametric

Select edge to align X axis or [Z-flip/Rotate] <accept>:

Verify that the X axis is pointing to the right, and press ENTER

You can pick the Z axis arrow to flip the Z axis orientation. You can also pick

part and work feature edges to orient the XY plane.

The UCS icon in the viewports is updated to reflect changes in the sketch plane

orientation. The sketch plane is always coincident with the UCS XY plane.

270 |Chapter 12 Creating Parts

Creating Extruded Features

To define the rough shape of the saddle bracket, you sketch a diamond shape

with filleted corners and add constraints to stabilize its shape. When the fea-

ture is stabilized with geometric constraints, you add dimensions to fully

define its size. Finally, you extrude the sketch, creating a solid feature from

the combined volume of the original base feature and the extruded feature.

To create a profile sketch

1Use PLINE to sketch this shape in the left viewport. With PLINE, you may need

to use the Direction option to control the direction of arcs.

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

➤ Polyline.

NOTE To make it easier to sketch the shape, make sure POLAR, OSNAP, and

OTRACK are turned off at the bottom of your screen.

Creating Extruded Features |271

2Use AMPROFILE to create a profile from the sketch.

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

➤ Single Profile.

Mechanical Desktop analyzes the sketch, redraws it, and displays this

message:

Solved underconstrained sketch requiring 10 dimensions or constraints.

NOTE If your sketch needs more than 10 dimensions or constraints to solve

the sketch, you probably need some tangency and constraints. Look for sharp

discontinuities between the fillets and the lines they join. You make these correc-

tions when you constrain the sketch to the base feature.

3Look at the Desktop Browser. The profile you just created is represented as

Profile2.

Because you have not extruded the profile, it is not consumed by a feature.

Therefore, the Browser shows that Profile2 is aligned at the same level in the

hierarchy as ExtrusionBlind1.

Because you added this feature to the base feature, you need to constrain its

shape and size and then constrain it to the existing part.

Constraining Sketches

To constrain a sketch, first you add and change geometric constraints to

create the shape of the bracket and to define its symmetry about the two

centerlines formed by the work plane and the work axis. Then you dimen-

sion the sketch to maintain the proper length and width.

NOTE Don’t be concerned if your sketch appears to be misshapen compared

to the illustrations. Constraining the sketch to the base feature will correct its

shape.

272 |Chapter 12 Creating Parts

To geometrically constrain a sketch

1Use AMADDCON to add tangent constraints to the arcs and lines, following

the prompts.

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

Constraints ➤ Tangent.

Valid selection(s): line, circle, arc, ellipse or spline segment

Select object to be reoriented: Specify an arc segment

Valid selection(s): line, circle, arc, ellipse or spline segment

Select object to be made tangent to: Specify an adjoining line segment

Solved underconstrained sketch requiring n dimensions or constraints.

Valid selection(s): line, circle, arc, ellipse or spline segment

Select object to be reoriented:

Continue adding constraints, or press ENTER twice to end the command

NOTE If the constraint display is too small, choose Part ➤ Part Options and

adjust the constraint size in the Desktop Options dialog box. Redisplay the

constraints.

You need to add radial constraints so that opposing arcs have equal radii.

Radial constraints make the arcs the same size and maintain the symmetry

needed between the sides of the bracket.

Fewer dimensions are needed because one parametric dimension solves 2

degrees of freedom by specifying the size of 2 arcs.

Creating Extruded Features |273

2Select the arcs to constrain, following the prompts.

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

Constraints ➤ Radius.

Valid selection(s): arc or circle

Select object to be resized: Select the arc at the top of the sketch (1)

Valid selection(s): arc or circle

Select object radius is based on: Select the arc at the bottom of the sketch (2)

Solved underconstrained sketch requiring 9 dimensions or constraints.

3Add radial constraints to the left and right arcs to make them equal in size.

Valid selection(s): arc or circle

Select object to be resized: Select the arc at the right of the sketch (3)

Valid selection(s): arc or circle

Select object radius is based on: Select the arc at the left of the sketch (4)

Solved underconstrained sketch requiring 8 dimensions or constraints.

Your left viewport should look like this.

If you sketched in a different order, your arcs and lines may be numbered

differently.

Valid selection(s): arc or circle

Select object to be resized: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/

eXit] <eXit>: Press ENTER

274 |Chapter 12 Creating Parts

4Delete any parallel constraints, responding to the prompts

If your sketch doesn’t contain parallel constraints, skip this procedure.

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

Constraints ➤ Delete Constraints.

Select or [Size/All]: Specify the constraint with the P symbol (1)

Select or [Size/All]: Specify the constraint with the P symbol (2)

Select or [Size/All]: Press ENTER

These parallel constraints, although valid, conflict with adding dimensions

between arc centers. You need to remove the parallel constraints to prevent

overconstraining the sketch.

Save your file.

Dimensioning Sketches

Now that the feature is stabilized with geometric constraints, you can dimen-

sion the distance between the arc centers and specify the arc radius. You need

four dimensions: a radius dimension for each arc, a dimension between the

left and right arc centers, and a dimension between the center of the sketch

and the center of either the left or right arc.

Creating Extruded Features |275

To dimension a sketch

1Use AMDIMDSP to change the dimension display back to numbers.

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

➤ Dimensions as Numbers.

2Use AMPARDIM to dimension the radius for the top and right arcs, responding

to the prompts.

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

➤ New Dimension.

Select first object: Specify the arc (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Diameter/Ordinate/Placement point]

<0.1986>: Enter .25

3Continue on the command line.

Select first object: Specify the arc (3)

Select second object or place dimension: Place the dimension (4)

Enter dimension value or [Undo/Diameter/Ordinate/Placement point]

<0.1676>: Enter .17

Your sketch should look like this.

276 |Chapter 12 Creating Parts

4Create a horizontal dimension between the centers of the left and right arcs.

Select first object: Specify the left arc center (1)

Select second object or place dimension: Specify the right arc center (2)

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.9797>: Press ENTER

5Dimension the distance between the centers of the top and left arcs.

Select first object: Specify the left arc center (1)

Select second object or place dimension: Specify the top arc center (4)

Specify dimension placement: Create a horizontal dimension (5)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.5135>: Press ENTER

6Press ENTER to exit the command.

In this case, you do not change the values while you create the dimensions.

While a sketch is underconstrained, dimension changes can cause it to dis-

tort, and you may not be able to recover its correct shape.

Creating Constraints Between Features

The sketch geometry is now completely defined. However, to position the

sketch symmetrically on the base feature, you need to constrain the sketch to

the work plane and the work axis because they serve as centerlines for the part.

You use the project (PR) constraint to project points onto objects (similar to the

NEA object snap) and the concentric (C) constraint to force two arc or circle

centers to be coincident.

As you determined when you first analyzed the part,

■The left and right arcs of the sketch form the lugs for the saddle bracket.

The arc centers must lie on the work plane.

■The top and bottom arcs of the sketch form the base for the boss, in the

exact center of the part. The centers of both top and bottom arcs are coin-

cident with the intersection of the work plane and the work axis.

Creating Extruded Features |277

To constrain a sketch to a base feature

1Use AMADDCON to make the center of the right arc lie on the work plane,

responding to the prompts.

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

Constraints ➤ Project.

Valid selection(s): line, circle, arc, ellipse or spline segment

Specify a point to project: Enter cen

of: Specify the arc (1)

Valid selection(s): line, circle, arc, ellipse, work point or spline segment

Select object to be projected to: Specify the work plane (2)

To make selecting lines and arcs easier, use transparent ZOOM. You can zoom

in or out while using an active command. At the Command prompt, enter

‘z, and select the area of the sketch you want to magnify. Then continue with

the active command.

NOTE If you do not use the cen object snap to specify the arc centers, you will

not be able to create the project constraints.

rough shape rough shape as a part

278 |Chapter 12 Creating Parts

2Make the center of the left arc lie on the work plane.

Valid selection(s): line, circle, arc, ellipse or spline segment

Specify a point to project: Enter cen

of: Specify the arc (1)

Valid selection(s): line, circle, arc, ellipse, work point or spline segment

Select object to be projected to: Specify the work plane (2)

3Position the center of the top arc on the work plane.

Valid selection(s): line, circle, arc, ellipse or spline segment

Specify a point to project: Enter cen

of: Specify the arc (1)

Valid selection(s): line, circle, arc, ellipse, work point or spline segment

Select object to be projected to: Specify the work plane (2)

Creating Extruded Features |279

4Position the center of the top arc on the work axis.

Valid selection(s): line, circle, arc, ellipse or spline segment

Specify a point to project: Enter cen

of: Specify the arc (1)

Valid selection(s): line, circle, arc, ellipse, work point or spline segment

Select object to be projected to: Specify the work axis (2)

5Use AMADDCON to make the center of the bottom arc concentric with the

center of the top arc, responding to the prompts.

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

Constraints ➤ Concentric.

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Specify the bottom arc (1)

Valid selection(s): arc, circle, ellipse, or work point

Select object to be made concentric to: Specify the top arc (2)

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/

eXit] <eXit>: Press ENTER

280 |Chapter 12 Creating Parts

Your sketch should be fully solved and look like this.

Save your file.

Editing Sketches

Now that the sketch is fully constrained, you can change the sketch dimen-

sions to position the sketch on your part. Modify the distances between the

center of the left arc and the center of the sketch and between the centers of

the left and right arcs.

To change a sketch dimension

1Use AMMODDIM to modify the values of the dimensions, following the

prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the dimension (1)

New value for dimension: <0.25>: Enter .33

Select dimension to change: Specify the dimension (2)

New value for dimension: <0.17>: Enter .16

Select dimension to change: Specify the dimension (3)

New value for dimension: <0.98>: Enter 1.16

Select dimension to change: Specify the dimension (4)

New value for dimension: <0.51>: Enter .56

Select dimension to change: Press ENTER

Creating Extruded Features |281

Your part should look like this.

Now, you need to create an equation between the overall dimension and the

dimension that centers the feature on the part and maintains symmetry

relative to the work axis. Display the dimensions as parameters, and then use

them as variables in the parametric equation.

2Use AMDIMDSP to display the dimensions as parameters.

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

➤ Dimensions As Parameters.

NOTE Your dimension parameter numbers may differ from those shown in the

illustration.

3Make the dimension between the top and left arcs one-half the horizontal

distance between the left and right arcs, following the prompts.

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

➤ Edit Dimension.

Select dimension to change: Specify the dimension (1)

Enter new value for dimension <.56>:

Enter =dx/2, where x is the dimension that corresponds to d13 in the illustration

Select dimension to change: Press ENTER

282 |Chapter 12 Creating Parts

Now that the profile sketch is completely constrained and dimensioned, you

can use it to change the shape of the base feature.

Extruding Profiles

You create a solid feature by extruding the profile through to the boundary

of the base feature, retaining the common volume. To create the rough shape

of the saddle bracket, you extrude the profile sketch up and completely

through the base feature. Because the sketch you extrude changes the shape

of the base feature, the intersection shares the volume of both.

base features resulting intersection

Creating Extruded Features |283

To extrude a profile through a base feature

1Use AMEXTRUDE to create the extrusion.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, accept the default size and specify:

Operation: Intersect

Flip: Verify that the direction arrow is pointed up through the part

Termination: Through

Choose OK to exit the dialog box and create the extrusion.

Save your file.

284 |Chapter 12 Creating Parts

Creating Revolved Features

With the rough shape of the saddle bracket defined, you can create the next

dependent feature, the boss, which is a cylinder. The fastest and most effi-

cient method to model the cylindrical boss is to extrude a circle. Alterna-

tively, you can revolve a rectangle about a central axis. This method is used

here to teach you the revolving method.

When you finish the exercise, your model will look like this.

Before you can sketch the profile for the revolved feature, you need to create

a work axis to serve as the centerline for the revolved feature. Work in the

right viewport, the isometric view.

To sketch a profile for a revolved feature

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

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Axis.

Select cylinder, cone or torus [Sketch]: Specify the face (1)

boss

work plane

work axis

Creating Revolved Features |285

2A work axis passes vertically through the part. If the work axis is not dis-

played, use AMVISIBLE to display it.

Desktop Menu Part ➤ Part Visibility

In the Desktop Visibility dialog box, choose the Part tab and check Work

Axes. Select Unhide and choose OK.

Next, you need to create a new sketch plane. Because the cylinder is vertical,

you place the sketch plane on the previously defined work plane.

3Create 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 work plane (1)

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>: Press ENTER

The sketch plane assumes the Z direction and XY orientation of the work

plane.

4Hide the work plane. This time use the Browser method.

Browser Right-click WorkPlane1 and choose Visible

The work plane is no longer visible.

286 |Chapter 12 Creating Parts

5Make the left viewport active and change the view so that you see a front

view of the part as you look at the sketch plane.

Desktop Menu View ➤ 3D Views ➤ Front

6Sketch a rectangular outline of the cylinder, following the prompts.

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

➤ Rectangle.

Specify first corner point or [Chamfer/Elevation/Fillet/Thickness/Width]:

Specify a point

Specify other corner point: Specify a second point

7Use AMPROFILE to convert the sketch to a profile for the feature.

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

➤ Single Profile.

Mechanical Desktop selects the sketch you just drew, and converts it to a pro-

file. The sketch still needs four dimensions or constraints.

Creating Revolved Features |287

To constrain a profile sketch to revolve

1Use AMDIMDSP to change the dimension display to numbers.

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

➤ Dimensions as Numbers.

2Use AMPARDIM to dimension the length and width of the sketch, following

the prompts.

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

➤ New Dimension.

Select first object: Specify the line (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.3629>: Enter .33

Solved underconstrained sketch requiring 3 dimensions or constraints.

Select first object: Specify the line (3)

Select second object or place dimension: Place the dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.6687>: Enter .78

Solved underconstrained sketch requiring 2 dimensions or constraints.

Select first object: Press ENTER

In the right viewport, constrain the sketch to the part as follows:

■Make the bottom line of the sketch collinear with the bottom of the part.

■Make the right side of the rectangle collinear with the vertical work axis

so that it serves as the axis of revolution of the feature.

288 |Chapter 12 Creating Parts

3Use AMADDCON to add collinear constraints, following the prompts.

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

Constraints ➤ Collinear.

Valid selections: line or spline segment

Select object to be reoriented: Specify the line (1)

Valid selections: line or spline segment

Select object to be made collinear to: Specify the vertical work axis (2)

Solved underconstrained sketch requiring 1 dimensions or constraints.

Valid selections: line or spline segment

Select object to be reoriented: Specify the line (3)

Valid selections: line or spline segment

Select object to be made clinger to: Specify the part edge (4)

Solved fully constrained sketch.

Valid selections: line or spline segment

Select object to be reoriented: Press ENTER

Enter an option [Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/

Length/Mir/Fix/eXit] <eXit>: Press ENTER

In the next procedure, you create the cylinder by revolving the sketch about

the work axis. You can also revolve a sketch about a part edge or about a line

in the profile sketch.

Creating Revolved Features |289

To revolve a feature about a work axis

1Use AMREVOLVE to revolve the sketch about the work axis, responding to the

prompt.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Revolve.

Select revolution axis: Specify the axis (1)

2In the Revolution dialog box, specify the operation, termination, and angle

of revolution. Because the cylinder attaches to the part, define the revolution

to be a full (360 degrees) termination that joins to the part.

Operation: Join

Angle: Enter 360

Termination: By Angle

Choose OK.

290 |Chapter 12 Creating Parts

After specifying the type of revolution and the axis of rotation, the cylinder

is created on your model.

Save your file.

Creating Symmetrical Features

The final features are the strengthening ribs, located on each side of the saddle

just above the lugs.

The ribs can be created simultaneously from a single open profile sketch. You

sketch an outline of the ribs, and add dimensions and constraints to make

the ribs symmetrical. Then you extrude the ribs automatically with the Rib

feature.

The sketch you create lies on the same plane as the revolution feature, so it

is not necessary to create a new sketch plane.

Before you begin, change to the front view, and one viewport.

strengthening rib

Creating Symmetrical Features |291

To sketch a feature on a part

1Use PLINE to sketch the ribs.

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

➤ Polyline.

Sketch a three-segment polyline in the approximate outline of the ribs. The

lines don’t have to touch the saddle.

2Use AMPROFILE to create an open profile from the sketch.

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

➤ Single Profile.

Respond to the prompt.

Select part edge to close the profile <open profile>: Press ENTER

Next, constrain the sketch.

Constraining Sketches

When you solved the sketch, a parallel constraint was applied between the

top horizontal line of the part and the horizontal segment of the sketch. Six

additional dimension or constraints are needed to fully constrain the sketch.

Use dimensions to adjust the size of the ribs and to center them on the part.

292 |Chapter 12 Creating Parts

To constrain a sketch

1Use AMPARDIM to dimension the distance between the top of the sketch and

the top of the part.

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

➤ New Dimension.

Respond to the prompts as follows:

Select first object: Specify the line (1)

Select second object or place dimension: Specify the line (2)

Specify dimension placement: Place the vertical dimension (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.1683>: Enter .08

Solved under constrained sketch requiring 6 dimensions or constraints.

2Add dimensions for the angle between the two ribs, and the angle between

the work axis and one rib.

Select first object: Specify the line (1)

Select second object or place dimension: Specify the line (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.1683>: Enter n

Specify dimension placement: Place the dimension (3)

Enter dimension value or [Undo/Placement point] <47>: Enter 40

Select first object: Specify the vertical work axis (4)

Select second object or place dimension: Specify the line (1)

Specify dimension placement: Place the angular dimension (5)

Enter dimension value or [Undo/Placement point] <20>: Press ENTER

Creating Symmetrical Features |293

3Add horizontal dimensions for the top line of the sketch, and from the work

axis to the outer edge of the top line.

Select first object: Specify the line (1)

Select second object or place dimension: Place the horizontal dimension (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.9806>: Enter .58

Select first object: Specify the outer end of line (1)

Select second object or place dimension: Specify the work axis(3)

Specify dimension placement: Place the horizontal dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.9806>: Enter .29

4Repeat step three to add a horizontal dimension of .98 between the two lower

endpoints of the sketch, and .49 between the work axis and one lower end-

point of the sketch.

Solved fully constrained sketch.

To verify that the ribs are symmetrical, express the dimensions as equations.

Set the distance and the angle between the axis and the rib to one-half the

distance and angle between both ribs.

294 |Chapter 12 Creating Parts

To display the dimensions as parameters

1Use AMDIMDSP to change the display of the dimensions from numeric to

parametric.

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

➤ Dimensions As Parameters.

Display the dimensions as equations.

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

➤ Dimensions As Equations.

2Use AMMODDIM to edit the dimensions. Use the work axis as the centerline

of the part.

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

➤ Edit Dimension.

Select dimension to change: Specify the horizontal dimension from the work axis

to either endpoint of the top line of the sketch

New value for dimension <current>:

Enter dx/2, where x is the horizontal dimension for the top line of the sketch

Solved fully constrained sketch.

Select dimension to change:

Specify the dimension for the angle between the work axis and a side of the sketch

New value for dimension <current>:

Enter dy/2, where y is the dimension for the angle between the sides of the sketch

Solved fully constrained sketch.

Select dimension to change: Press ENTER

Creating Symmetrical Features |295

3Use AMUPDATE to apply any changes to the rib sketch.

Context Menu Right-click the graphics area and choose Update Part.

You are ready to extrude the sketch to form symmetrical ribs.

4Use 3DOrbit to adjust the view so you can see the rib feature preview before

you create the ribs.

Desktop Menu Choose View ➤ 3D Orbit. Rotate the view slightly to the

left, and tilt it slightly downward.

5Use AMRIB to extrude the ribs.

Browser In the Browser, right-click the open profile icon, and

choose Rib.

In the Rib dialog box, specify:

Type: Midplane

Thickness: Enter .08

Verify the direction arrow points into the part, and choose OK.

The two symmetrical ribs are extruded to the face of the cylinder.

Next, suppress the hidden lines so that you can see your model more clearly.

296 |Chapter 12 Creating Parts

To suppress silhouette edges from Mechanical Desktop parts

1Set the DISPSILH system variable to 1, responding to the prompts.

Command DISPSILH

Enter new value for DISPSILH <0>: Enter 1

2Use HIDE to remove the hidden lines from your display.

Desktop Menu View ➤ Hide

Your part should now look like this. The Desktop Browser shows the hierar-

chy of the part features.

3Return to wireframe display.

Desktop Menu View ➤ Shade ➤ 3D Wireframe

Save your file.

Refining Parts |297

Refining Parts

Now, you complete the part by modifying its features in the same order as

you created them: the saddle and lugs, the boss, and the ribs.

To finish the body of the saddle bracket, you need to cut the pipe saddle,

adjust the length of the lugs, and create mounting holes. To create the saddle,

you cut an arc through the front of the saddle body. To cut the arc, you create

a circle and extrude it through the part, along the horizontal work axis. For

this feature, you use the previously defined sketch plane.

To sketch and constrain the circle to be extruded

1Use CIRCLE to draw the circle to extrude, following the prompts. Work in the

left viewport.

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

➤ Circle.

Specify center point for circle or [3P/2P/Ttr (tan tan radius)]:

Specify a center point

Specify radius of circle or [Diameter]: Specify a point to define the radius

2Use AMPROFILE to solve the sketch to convert it to a profile sketch.

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

➤ Single Profile.

You need to constrain the circle to the part. The sketch also needs two more

dimensions: the location of the center and the diameter of the circle.

The work axis is the center of the saddle arcs on the front and back of the

bracket. By making the circle concentric with the arcs, you satisfy two con-

straints, the location of the center and the relationship of the circle to the part.

298 |Chapter 12 Creating Parts

3Use AMADDCON to constrain the circle to be concentric with the saddle arcs,

responding to the prompts.

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

Constraints ➤ Concentric.

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Specify the circle (1)

Valid selection(s): arc, circle, ellipse, or work point

Select object to be made concentric to: Specify the arc (2)

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/

eXit] <eXit>: Press ENTER

4Use AMDIMDSP to return the dimension display to numeric, responding to

the prompt.

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

➤ Dimensions As Numbers.

Refining Parts |299

5Use AMPARDIM to dimension the diameter of the circle, following the

prompts.

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

➤ New Dimension.

Select first object: Specify the circle (1)

Select second object or place dimension: Place the dimension (2)

Enter dimension value or [Undo/Placement point] <1.0976>: Enter 1.12

Select first object: Press ENTER

The sketch is now fully constrained and looks like this.

300 |Chapter 12 Creating Parts

To extrude a feature

1Extrude the feature, specifying a cut operation with a midplane termination.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

2In the Extrusion dialog box, specify:

Operation: Cut

Distance: Enter .66

Termination: Type: Mid Plane

Choose OK. The arc shape cuts through the saddle bracket.

To complete the body of the bracket, you need a placed feature on each of

the lugs for mounting holes.

To create a drilled hole

1Use AMHOLE to place the mounting holes. Work in the isometric view.

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

Features ➤ Hole.

2In the Hole dialog box, select the Drilled hole type icon and specify:

Termination: Through

Placement: Concentric

Diameter: Enter .09

Choose OK.

Refining Parts |301

3Respond to the prompts as follows:

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify face (1)

Enter an option [Next/Accept]<Accept>: Press ENTER

Select the concentric edge: Specify edges (1) for the first hole

4Continue on the command line to place the second hole.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify face (2)

Select the concentric edge: Specify edges (2) for the second hole

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]: Press ENTER

Your part should look like this.

To complete the boss, you create a counterbored hole through the cylinder.

You create the hole as a placed feature on the same vertical work axis as the

cylinder.

Keep the right viewport active, and specify a counterbored hole drilled

through the part, concentric with the cylinder.

302 |Chapter 12 Creating Parts

To create a counterbored hole

1Use AMHOLE to place the counterbored hole.

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

Features ➤ Hole.

In the Hole dialog box, select the Counterbore hole type icon and specify:

Termination: Through

Placement: Concentric

Hole Parameters: Size: Enter .42

C’Bore/Sunk Size: C’ Dia: Enter .48

C’Bore/Sunk Size: C’ Depth: Enter .125

Choose OK.

2Respond to the prompts as follows:

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify face (1)

Select the concentric edge: Specify edge (1)

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]: Press ENTER

The ribs currently extend too far onto the lug area, leaving little room for the

mounting holes. To adjust the design, you need to reduce the width and

angle of the ribs.

Work in the left viewport. Modify the ribs by changing a few sketch

dimensions. The previously-defined equations keep the ribs symmetrical.

Use the Browser to select the rib feature and redisplay its sketch dimensions.

After you change the dimension values, use the Update icon in the Browser

to incorporate the changes.

Refining Parts |303

To edit a feature

1Use AMEDITFEAT to edit the rib sketch.

Browser Right-click OpenProfile1 and choose Edit Sketch.

The rib sketch and its dimensions become visible on the screen.

2Change two of the dimensions in the sketch, following the prompts.

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

➤ Edit Dimension.

Select object: Specify the dimension (1)

Enter new value for dimension <40>: Enter 28

Select object: Specify the dimension (2)

Enter new value for dimension <.o8>: Enter .06

Select object: Press ENTER

3Update the part to reflect the new dimension values in the sketch.

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

The ribs are updated to reflect your dimensional changes.

In the Browser, each feature is placed in the order it was created.

304 |Chapter 12 Creating Parts

Shading and Lighting Models

To see your model better, use the shade button on the Desktop View toolbar

to toggle shading on. Then adjust the lighting of your shaded model.

To toggle shading of a part

1Use SHADE to shade your part.

Desktop Menu View ➤ Shade ➤ Gouraud Shaded

Your part should now look like this.

The Desktop View toolbar also contains commands to dynamically rotate

your design and control views.

Now adjust the ambient and direct lighting of your shaded part.

Ambient light provides constant illumination in the drawing environment.

It has no particular source or direction. You can adjust the intensity of ambi-

ent light. Keep ambient light low to prevent washing out your image.

Direct light illuminates your image from a specified direction. You can adjust

the intensity and direction of direct light.

Shading and Lighting Models |305

To control the lighting of a shaded part

1Use AMLIGHT to adjust the intensity of ambient and direct light.

Toolbutton Lighting Control

In the Lights dialog box, use the slider bars to adjust the intensity of the

ambient light and the direct light as follows.

2Use AMLIGHTDIR to specify a direction for direct light.

In the Lights dialog box, click the Light Direction button. Respond to the

prompt as follows:

Select a point that will be used with the current target point for light direction:

Specify a point in the upper left of the graphics area

The light adjustments are reflected in your drawing. Experiment with other

light settings.

Save your file.

306

307

In This Chapter 13

Creating Drawing Views

Autodesk® Mechanical Desktop® simplifies both the

drawing and the documentation of your design.

Drawing views are associated with a part and with one

another. You lay out drawing views in any position on a

screen. You can move them and make changes easily.

Most dimensions are automatically placed on the views

when you create them, but you can easily add missing

reference dimensions and other annotations. In this

tutorial, you will learn to use the Drawing tab in the

Desktop Browser to manage and edit drawing views.

■Planning and setting up your

drawing

■Multiple document layouts

■Creating drawing views

■Hiding extraneous dimensions

■Moving dimensions to a different

view

■Customizing annotations

■Relocating and editing views

308 |Chapter 13 Creating Drawing Views

Key Terms

Te r m Definition

balloon A circular annotation tag that ties components in an assembly into a bill of

material.

base view The first view you create. Other views are derived from this view.

Desktop Browser A graphical representation of the features that make up your model. You can

work in the Browser to create and restructure parts and assemblies, define

scenes, create drawing views, and control overall preferences.

Drawing mode Establishes the settings for paper space so that you can create a drawing of your

model. When Drawing mode is off, you are in model space.

hidden line A line that is not visible in a specified view. For example, in a front view, lines

behind the front plane are not visible.

Model mode Creates 3D models on which drawing views are based.

parametric dimension A dimension created during the sketch phase of feature creation. Parametric

dimensions control size and update a part when you change its values.

parent view A view on which to base another drawing view. For example, the base view is

the parent view for auxiliary and orthographic views. Any view can be the parent

view for a detail view.

reference dimension An annotation dimension placed on a Mechanical Desktop drawing. These

measurements do not control the size of the object. Instead, reference

dimensions are required for manufacturing. They are updated when the

geometry changes.

view scale The scale of a base drawing relative to the model scale. Also the scale of

dependent views relative to the base view.

Basic Concepts of Creating Drawing Views |309

Basic Concepts of Creating Drawing Views

Drawings and documentation are often the true products of design because

they guide the manufacture of a mechanical device.

Mechanical Desktop adds an important dimension to drawing creation by

doing most of the work for you. Traditional 2D orthographic, isometric, aux-

iliary, section, and detail views of parts and assemblies can be automatically

created.

Mechanical Desktop creates these views complete with dimensions derived

from the models. You can then add annotations or more dimensions.

Because the views are derived from the models, they are updated as you make

changes to your design.

In Mechanical Desktop, you can set up multiple layouts for complex models

that require more than one drawing sheet to document.

Planning and Setting Up Drawings

Before you create drawing views, plan the views you need. Set up dimension-

ing and text styles and the drafting standard for your dimensions and other

annotations.

To customize your drawing, use system parameters to specify drawing char-

acteristics. You can define parameters in a prototype drawing so that they are

automatically set before you begin a new project.

For this exercise, open the file partview.dwg in the desktop\tutorial folder. The

file contains the saddle bracket model from the previous tutorial. It has been

created in a prototype drawing that contains a predefined drawing style and

title block.

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.

310 |Chapter 13 Creating Drawing Views

Creating Drawing Views

The first view you create is a base view. In Model mode, you specify the orien-

tation of the view, and then change to Drawing mode to position it on the

page. A title block and drawing border have been placed on the TITLE_BLK layer.

When you place the base view, hidden lines are removed. Parametric dimen-

sions are shown according to the currently-defined dimension style.

By default, a dimension is shown in one view only—the first view you create

displays the object that the dimension references. You can specify that para-

metric dimensions be displayed in other views as they are created, or you can

move a dimension, if you prefer to show it on a different view.

When drawing views are created, by default their size is determined by the

size of the data set. However, you can manually grip edit a viewport border if

Parametric Border Sizing is turned off in the Edit Drawing View dialog box.

If you turn Parametric Border Sizing back on, parametric sizing is restored.

First, define a front view as a base view for the drawing. Before you begin this

exercise, select the Drawing tab to change to Drawing mode.

To create a base view

1Use AMDWGVIEW to define the base view. Verify that the Drawing tab is

selected in the Browser.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, choose OK to accept the default

options.

Creating Drawing Views |311

2Respond to the prompts as follows:

Select a planar face, work plane, or [Ucs/View/worldXy/worldYz/worldZx]:

Specify the work plane (1)

Define X axis direction:

Select work axis, straight edge or [worldX/worldY/worldZ]:

Specify the axis of revolution (2)

Adjust orientation [Flip/Rotate] <Accept>:

Enter r until the UCS icon is upright, or press ENTER

3On the command line, define a location on the drawing for the base view.

Specify location of base view:

Specify a point in the lower-left corner, inside the drawing border

Specify location of base view: Press ENTER

312 |Chapter 13 Creating Drawing Views

The base view is placed at the location you selected.

The Desktop Browser displays a hierarchy of the views you create. Because

you have only the base view, it is listed below the part. As you create views

from the base view, they are nested beneath the base view in the Browser.

Because the base view is too small to be easily read, enlarge it by changing

the view scale. Subsequent views will use the enlarged view scale until you

specify a different one.

4Use AMEDITVIEW to edit the scale of the base view.

Context Menu In the graphics area, right-click and choose Edit View.

Select the view you created.

In the Edit Drawing View dialog box, specify a scale of 2, and choose OK.

Next, create an orthographic top view for the part.

When projected orthographically from the front view, the top view is aligned

horizontally or vertically with the base view and maintains the same scale.

Creating Drawing Views |313

To create a top and detail view

1Create the orthographic view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify the Ortho view type and

Choose OK.

2Define a location for the orthographic view, responding to the prompts.

Select parent view: Specify the front view (1)

Specify location for orthogonal view:

Specify any location above the front view, within the drawing border (2)

Specify location for orthogonal view: Press ENTER

Your drawing should now look like this.

314 |Chapter 13 Creating Drawing Views

Because the orthogonal view is created from the base view, it is nested below

the Base icon in the Desktop Browser.

Next, create an independent detail view of one of the lugs. Properties of inde-

pendent detail views can be changed without affecting the properties of the

parent view.

To create a detail view, choose the parent view and the area in the parent to

show in detail. In this case, create a detail view of the rightmost mounting

lug. For detail views, you always define the viewport border. The border is not

controlled parametrically by the size of the part or geometry.

To create an independent detail view

1Use AMDWGVIEW to create the detail view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

View Type: Detail

Scale: Enter 1.75

Relative to Parent: Select the check box

Detail Symbol: Enter A

Label Pattern: Enter VIEW

Independent View Display: Select the check box

Choose OK.

Creating Drawing Views |315

2Define the detail view, responding to the prompts.

Select vertex in parent view to attach detail:

Specify the center of the rightmost lug (1)

Specify center point for circular area or [Ellipse/Polygon/Rect/Select]: Enter r

Specify first corner of rectangular area:

Specify the first point of the selection rectangle (2)

Specify opposite corner: Specify the second point of the selection rectangle (3)

Specify location for detail view:

Specify a point to the lower right of the top view (4)

Specify location for detail view: Press ENTER

NOTE To facilitate selection, turn off Object Tracking and Object Snaps by

clicking the buttons at the bottom of your screen. You may need to zoom in to

select the circle.

316 |Chapter 13 Creating Drawing Views

Your drawing should look like this.

The Browser displays a Detail icon nested below the Ortho icon.

3Use AMEDITVIEW to edit the edge properties of the detail view.

Context Menu In the graphics area, right-click and choose Edit View.

Select the detail view you created.

In the Edit Drawing View dialog box, select the Display tab, and select Edge

properties.

4Edit the detail view edge properties, responding to the prompts.

Enter an option (edge properties) [Remove all/Select/Unhide all] <Select>:

Press ENTER

Select Edges: Specify the circular lug

Select Edges: Press ENTER

In the Edge Properties dialog box, choose Color.

In the Select Color dialog box, select red, and press ENTER.

Choose OK to close the Edge Properties dialog box.

Choose OK to close the Edit Drawing View dialog box.

Creating Drawing Views |317

The lug color in the detail view changes to red. However, the lug color

remains unchanged in the parent view.

For practice, create the same detail view using a circle for selection. Notice

how the command line prompts change according to the selection type you

use.

Next, you create a cross section—a view that cuts through a point on the part

along a work plane, or if the part is an offset section, through a sketch. Work

planes are often easier to visualize and select than cutting planes.

If you choose not to create a work plane, you will find it easier to select only

the endpoints of edges and the centers of circles or arcs to specify a cutting

plane.

In this tutorial, you will create a work plane for the cross-section view, using

an axis and an existing work plane.

To create a cross-section and isometric view

1Return to Model mode.

Browser Select the Model tab.

2Use AMWORKPLN to create a work plane for the cross-section view.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

In the Work Plane dialog box, specify:

1st Modifier: On Edge/Axis

2nd Modifier: Planar Normal

Create Sketch Plane: Clear the check box

Choose OK.

318 |Chapter 13 Creating Drawing Views

3On the command line, respond to the prompts as follows.

Select work axis, straight edge or [worldX/worldY/worldZ]:

Specify the work axis (1)

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify the work plane (2)

Your model should now look like this.

Next, you create a full cross-section view of the part that is an orthographic

projection of the front view.

4Return to Drawing mode.

Browser Select the Drawing tab.

Creating Drawing Views |319

5Create a new drawing view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

View Type: Ortho

Choose the Section tab and specify:

Type: Full

Label: Enter A

Label Pattern: Section A-A

Hatch: Select the check box, and press Pattern

Use the Hatch Pattern dialog box to define the hatch pattern, and choose OK.

Choose OK to close the Create Drawing View dialog box.

6Define the orthogonal view, responding to the prompts.

Select parent view: Specify a point anywhere inside the front view

Specify location for orthogonal view:

Specify a point to the right of the front view (3)

Specify location for orthogonal view: Press ENTER

Enter section through type [Point/Work plane] <Work plane>:

Press ENTER

Select work plane in parent view for the section:

Select the edge of the second work plane at a point inside the view box (4)

320 |Chapter 13 Creating Drawing Views

Your display should now look like this.

7Create an isometric view, using the base view as the parent view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

View Type: Iso

Scale: Enter 1

Relative to Parent: Select the check box

Choose OK.

8Define the isometric view, responding to the prompts.

Select parent view: Specify the base view (1)

Location for isometric view: Specify a point to the right of the top view (2)

Location for isometric view: Press ENTER

Creating Drawing Views |321

Your drawing should look like this.

322 |Chapter 13 Creating Drawing Views

Each drawing view is represented as it relates to other views. For example, the

ortho, section, and iso views are derived from the base view. Also, it is clear

that the detail view is based on the ortho view. Detail and section views are

named according to the labels you specified.

Save your file.

Cleaning Up Drawings

After creating the drawing views, you need to clean up the parametric dimen-

sions and some extraneous lines.

Parametric dimensions are automatically placed on the AM_PARDIM layer.

Hiding Extraneous Dimensions

Because dimensions originate on the model, some might be redundant or

conflict with others. For example, because the saddle bracket is symmetrical,

one dimension states the overall length of a feature while another states the

length of one side. Only one of these dimensions is necessary because the

other can be derived. Decide which dimensions to show, and then selectively

hide the others. Hiding dimensions does not delete them. They can be redis-

played from the Desktop Visibility dialog box.

Other dimensions may be redundant because you created the model by

constructing individual features. For example, when you sketched the arc

that represents the rough saddle form, you specified a radius of .33. This

dimension appears in the top view of the drawing. When you created the

boss, you specified a dimension of .33 to revolve the boss. This dimension

appears in the front view of the saddle bracket. Only one of the .33 dimen-

sions is needed.

Cleaning Up Drawings |323

To hide extraneous dimensions in a front view

1Zoom to the base view.

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

2Activate the Desktop Visibility dialog box.

Desktop Menu Drawing ➤ Drawing Visibility

In the Desktop Visibility dialog box, verify that the Hide option is selected.

Then choose Select.

3On the command line, respond to the prompts to select the redundant .33

and .74 dimensions to hide.

Select drawing objects to hide: Specify the 0.33 dimension

Select drawing objects to hide: 1 found

Select drawing objects to hide: Specify the 0.74 dimension

Select drawing objects to hide: 1 found, 2 total

The view also contains a number of dimensions associated with the rib

sketch. The ribs were created from a trapezoid shape, where only two of the

sides are used by the part. The other sides are not visible, so their dimensions

should not appear in the drawing.

Select drawing objects to hide: Specify the 1.00 dimension

Select drawing objects to hide: 1 found, 3 total

Select drawing objects to hide: Specify the 0.50 dimension

Select drawing objects to hide: 1 found, 4 total

Select drawing objects to hide: Specify the 14° dimension

Select drawing objects to hide: 1 found, 5 total

Select drawing objects to hide: Press ENTER

Choose OK to exit the dialog box.

324 |Chapter 13 Creating Drawing Views

4Your display should look like this.

In the top view, the 1.16 dimension specifies the distance between arc cen-

ters. You can hide the extraneous .58 and 0.08 dimensions.

To hide extraneous dimensions in a top view

1Zoom to the top view.

Browser Right-click Ortho and choose Zoom to.

2Activate the Desktop Visibility dialog box.

Desktop Menu Drawing ➤ Drawing Visibility

3In the Desktop Visibility dialog box, verify that the Hide check box is selected

and choose Select.

4Respond to the prompts as follows.

Select drawing objects to hide: Specify the 0.58 dimension

Select drawing objects to hide: Specify the 0.08 dimension

Select drawing objects to hide: Press ENTER

Choose OK to exit the dialog box.

The dimensions should be hidden on the view.

Cleaning Up Drawings |325

Moving Dimensions

Mechanical Desktop places dimensions on the drawing according to the way

they were created during sketching. Usually, some cleanup is required, to

comply with drafting standards.

In the following exercises, you will move dimensions within and between views

until all the dimensions needed to define the part are visible on the drawing.

All the dimensions for the drawing currently exist in the front and top views.

Originally these views were cluttered with extraneous dimensions. Now that

those dimensions are gone, it is much easier to move the remaining dimen-

sions to other views.

To move a dimension within a view

1Zoom to the base view.

Browser Right-click Base and choose Zoom to.

.2Use AMMOVEDIM to move some dimensions to clean up your view, following

the prompts.

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

Menu ➤ Edit Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] <Move>: Press ENTER

Select dimension to move: Specify the 1.48 dimension (1)

Select destination view: Specify a point near the center of the front view (2)

Select location: Specify a point slightly below the A for the section cut (3)

Select location: Press ENTER

Press ENTER to repeat the command.

326 |Chapter 13 Creating Drawing Views

3Continue moving dimensions until the front view looks like this.

4Zoom to the top view.

Browser Right-click Ortho and choose Zoom to.

5Use AMMOVEDIM to move some of the dimensions in the top view.

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

Menu ➤ Edit Dimensions ➤ Move Dimension.

Follow the command line prompts to move dimensions until your view

looks like this.

Because dimensions are placed on the first true-size view of the part, most

dimensions clutter the first few views you create. In this exercise, you move

a dimension from the front view to its cross-section view.

6Zoom to return to the drawing layout.

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

click again, and choose Zoom Extents. Right-click again

and choose Exit to close the command.

Cleaning Up Drawings |327

To move a dimension to a different view

1Zoom in to view the front and cross-section views.

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

2Use AMMOVEDIM to move a dimension from the front view to the cross-

section view, following the prompts.

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

Menu ➤ Edit Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] <Move>: Press ENTER

Select dimension to move: Specify the 0.78 dimension (1)

Select destination view: Specify the cross-section view (2)

Select location: Place the dimension to the left of the cross-section view (3)

Select location: Press ENTER

Your drawing views should look like this.

328 |Chapter 13 Creating Drawing Views

Hiding Extraneous Lines

Although Mechanical Desktop eliminates lines when it creates views, you

may want to edit the views to remove additional, unwanted lines.

To hide an extraneous line

1Zoom to the isometric view.

Browser Right-click Iso and choose Zoom to.

2Use AMEDITVIEW to edit the Iso view.

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

Menu ➤ Edit View.

3Specify the isometric view.

4In the Edit Drawing View dialog box, choose the Display tab and then choose

Edge Properties.

Cleaning Up Drawings |329

5On the command line, respond to the prompts as follows:

Enter an option (edge properties) [Remove all/Select/Unhide all] <Select>:

Press ENTER

Select Edges: Specify the vertical line on the lug (1)

Select Edges: Specify the vertical line on the lug (2)

Select Edges: Press ENTER

6In the Edge Properties dialog box, specify:

Hide Edges: Select the check box

Choose OK.

7Choose OK to exit the Edit Drawing View dialog box.

The selected lines are removed from the view.

lines selected lines hidden

330 |Chapter 13 Creating Drawing Views

Enhancing Drawings

When you are satisfied with the drawing views, you can modify and enhance

them. Enhancements include:

■Adding more dimensions

■Adding annotations such as callouts, hole notes, and centerlines

■Relocating views

■Modifying the part from the drawing view

Changing Dimension Attributes

Even though you set up the dimension style before creating the dimensions,

some dimensions may need to be displayed in a particular way.

To edit a dimension attribute

1Zoom to the front and cross-section views.

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

2Use AMPOWEREDIT to edit a dimension on the front view to show a tolerance

range, responding to the prompts.

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

Menu ➤ Edit Dimensions ➤ Power Edit.

Select object: Specify the .12 dimension in the front view

3In the Power Dimensioning dialog box, choose the Units tab and specify:

Units: Decimal

Round Off: Enter 3

Select the Add Tolerance button in the upper right of the dialog box and

specify:

Upper: Enter +0.001

Lower: Enter -0.001

Enhancing Drawings |331

4Choose the General tab.

The .12 dimension should now be expressed as 0.120 +/- .001. Now that the

dimension is longer, it may overlap the drawing view.

Choose OK.

5Move the dimension so that it does not overlap any geometry.

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

Dimensions ➤ Move Dimension.

Move the dimension so that it looks like this.

332 |Chapter 13 Creating Drawing Views

Creating Reference Dimensions

You can supplement parametric dimensions with reference dimensions. The

reference dimensions do not control the size of the model; however, if you

change the model, the reference dimensions are updated to reflect the new

size. Reference dimensions reside on the AM_REFDIM layer.

In the next exercise, you add a reference dimension to the front view.

To add a reference dimension

1Zoom to the front view.

Browser Right-click Base and choose Zoom to.

2Use AMREFDIM to dimension the vertical distance from the top of the right-

most rib to the top of the rightmost lug, responding to the prompts.

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

Menu ➤ Reference Dimension.

Select first object: Specify a point at the top of rib (1)

Select second object or place dimension: Specify a point at the top of lug (2)

Specify dimension placement: Specify a point to place the dimension (3)

Specify placement point or [Undo/Hor/Ver/Align/Par/aNgle/Ord/reF/Basic]:

Enter v to force a vertical dimension, or press ENTER

Select first object: Press ENTER

NOTE You can move some of the dimensions to avoid a cluttered view.

reference dimension addedpoints selected

Enhancing Drawings |333

Creating Hole Notes

Mechanical Desktop does not automatically display hole dimensions on the

drawing, but you can add this information.

First, you add a hole note to the boss in the top view, and tapped hole infor-

mation to the mounting hole in the detail view.

To create a hole note

1Zoom to the top view.

Browser Right-click Ortho and choose Zoom to.

2Use AMNOTE to create a hole note for the hole through the boss, responding

to the prompts.

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

Menu ➤ Annotation ➤ Hole Note.

Select object to attach [rEorganize]: Specify one of the two inner circles (1)

Next Point <Symbol>: Specify the location (2), and press ENTER

334 |Chapter 13 Creating Drawing Views

3In the Note Symbol dialog box, choose the more button to display the Note

Templates section.

In Note Templates, choose the COUNTER BORE template.

4Select the Leader tab, and set the leader justification to Middle of All Text.

Choose OK.

A hole note with the hole diameter, the counterbore diameter, and the hole

depth is displayed on your drawing.

Next, add hole information to the mounting hole in the detail view. This

procedure is similar to adding standard hole note information, except that

you include additional information when you create the hole. You edit the

text in the hole note template, but it applies to that hole note only and does

not alter the template.

Enhancing Drawings |335

To create a modified hole note

1Zoom to the detail view.

Browser Right-click Detail and choose Zoom to.

2Create the hole note, responding to the prompts.

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

Hole Note.

Select object to attach [rEorganize]: Specify the hole in detail view (1)

Next Point <Symbol>: Specify the location (2), and press ENTER.

3In the Note Symbol dialog box, choose the more button to display the Note

Templates section.

In Note Templates, choose the THRU HOLE template.

The Multiline Text Editor is displayed.

4In the Multiline Text Editor, place the cursor at the end of the existing text

and press ENTER. Add (typ of 2) on the second line.

Select the Leader tab, and set the leader justification to Middle of All Text.

Choose OK.

Your drawing should look like this.

336 |Chapter 13 Creating Drawing Views

Creating Centerlines

In this exercise, you create a parametric centerline for the top view and a cen-

ter mark for the detail view. Centerlines and center marks are attached to the

view and move with the view as the model changes.

To create a centerline

1Add a center mark, responding to the prompts.

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

Centerline.

Select Edge: Specify the hole in the detail view (1)

Select mirrored edge or <ENTER>: Press ENTER

The size and characteristics of the center mark are defined by settings in the

Centerline Properties dialog box. To change the settings, choose Drawing ➤

Drawing Options. On the Annotation tab, choose Centerline Settings, and

choose the Center Line Properties button.

In the Center Line Properties dialog box, you can choose to use standard set-

tings, or you can enter new values for overshoot and center mark size that

will apply to this drawing only.

2Zoom to the top view.

Browser Right-click Ortho and choose Zoom to.

3Create another centerline, responding to the prompts.

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

Centerline.

Select Edge: Specify the top edge of the left lug (1)

Select mirrored edge or <RETURN>: Specify the lower edge of the left lug (2)

Enhancing Drawings |337

A centerline is placed through the view. Now, specify where to trim the cen-

terline endpoints.

Select first trim point: Specify a point to the right of the part

Select second trim point: Specify a point to the left of the part

Your display should look like this.

Creating Other Annotation Items

When you make changes to a model, the geometry and dimensions are

updated automatically. Special commands create drawing annotations such

as reference dimensions, hole notes, and centerlines.

You can create other annotations such as callout bubbles, surface finish sym-

bols, and Geometric Distancing and Tolerancing (GD&T) symbols. The anno-

tation items do not change when you make changes to the model. To make

these annotation objects parametric, you convert them after you create

them.

In the next exercise, you convert a callout bubble into a Mechanical Desktop

annotation item. The callout bubble is already created and placed on the

AM_ANNOTE layer of your drawing.

338 |Chapter 13 Creating Drawing Views

To convert a callout bubble

1Zoom out to view the entire drawing.

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

click again and choose Zoom Extents. Right-click again

and choose Exit.

2Use LAYER to turn on the AM_ANNOTE layer. You should see a callout bubble

containing the number 1 and a leader.

3Use AMMOVEVIEW to position the isometric view near the callout, respond-

ing to the prompts.

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

Menu ➤ Move View.

Select view to move: Select the isometric view (1)

Specify new view location: Specify a point (2)

Specify new view location: Press ENTER

If you use the Browser to move a view, you will not be asked to select it.

The callout does not move. Convert it to an annotation so that it is associ-

ated with the isometric view.

Enhancing Drawings |339

4Convert the callout bubble to an annotation, responding to the prompts.

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

Menu ➤ Annotation ➤ Create Annotation.

Select objects to associate with view:

Draw a selection rectangle around the callout bubble, numeral, and leader (1, 2)

Select objects: Press ENTER

Select point in view to attach annotation: Specify a point (2)

Your drawing should look like this.

340 |Chapter 13 Creating Drawing Views

Modifying Drawing Views

You can relocate views or change the model from a drawing view. The draw-

ing and, if appropriate, the model, are updated to reflect the changes you

made.

Move the isometric view. The callout bubble moves with the view because it

is associated with the part. Then, relocate the isometric and detail views, and

change the detail view. The model and all drawing views are updated.

To relocate a drawing view

1Move the Iso view back to its former location, responding to the prompts.

Context Menu In the graphics area, right-click and choose Move View.

Select view to move: Specify center of isometric view (1)

Specify new view location: Specify new location (2) and press ENTER

Specify new view location: Press ENTER

The callout bubble moves with the view.

Enhancing Drawings |341

2Relocate the detail view to the right of and below the isometric view,

responding to the prompts.

Context Menu In the graphics area, right-click and choose Move View.

Select view to move: Specify center of the detail view (1)

Specify new view location: Specify new location (2) and press ENTER

Specify new view location: Press ENTER

All annotations associated with the view move with it and keep their posi-

tions relative to the view. You can move views from layer to layer.

Now, change one of the parametric dimensions within a view and watch the

resulting changes.

342

To modify a drawing view

1Zoom to the top view.

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

2Use AMMODDIM to change the radius of the lug, responding to the prompts.

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

Dimensions ➤ Edit Dimension.

Select dimension to change: Select the .16 value of the lug radius

New value for dimension <.16>: Enter .13

Select dimension to change: Press ENTER

You must update the part to show the changes.

3Zoom out to display all the drawing views.

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

click again, and choose Zoom Extents. Right-click again

and choose Exit.

4Use AMUPDATE to update your part.

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

Update part now? [Yes/No]: Press ENTER

In the Update Dependent Part dialog box, choose Yes.

Mechanical Desktop updates the part, it also updates each drawing view.

After it completes the updating, your drawing should look like this.

Save your file.

Exporting Drawing Views |343

Exporting Drawing Views

You can save your 2D drawing views directly to Mechanical Desktop versions

other than Release 6 as DWG, DWT, or DXF files. You can export the entire

current layout, including all views and geometry, or you can select views and

entities to export.

The Export Drawing Views dialog box provides options to:

■Convert views at true scale (1:1)

■Convert circular and linear splines that project to 2D arcs, circles and lines

■Flatten all source data, including any 3D autoCAD entities, or flatten only

MDT objects

The export options in the Export Drawing Views dialog box enable you to

export drawing views to:

■A new layout in the current file

■An external file in either model space or in layout

■Past and present versions of AutoCAD and DXF

Usually, only one base view is shown in a drawing view. With the True Scale

option turned on, a warning is displayed if two or more base views are shown

with different scales. You export base views separately, whether or not they are

scaled by the same factor. In the exporting process, isometric and detail views

are scaled by the same factor as the base view.

In this exercise, you save your drawing file to AutoCAD 2000.

344 |Chapter 13 Creating Drawing Views

To export Mechanical Desktop drawing views

1Use AMVIEWOUT to save your drawing view file to AutoCAD 2000.

Browser In the Browser, right-click Base and choose Export View.

2In the Export Drawing Views dialog box, specify the following:

Source: Specify Current Layout

Data Handling:

Export Views True Scale (1:1): Select the check box

Flatten All Selected Objects: Select the check box

Convert Circular/Linear Splines to Circles/Lines: Select the check box

Generate Preview Image: Select the check box

File Name: Enter or browse to a file name for the new version

Press the More button (<<), and in Export Options, specify:

To New External File: Select the check box, and select In Layout

Save as type: Specify AutoCAD 2000 Drawing (*.dwg)

Choose OK.

The drawing view is saved into the first layout in the new external file.

345

In This Chapter 14

Creating Shells

This tutorial teaches you how to create and edit a

shelled part in Autodesk® Mechanical Desktop®. With

the shell feature, you can create complex parts with

walls of varying thickness. In the tutorial, you add a

shell feature to an existing die cast engine part, and then

edit the shell. The procedures you learn here can be

applied to a variety of shelled parts.

■Adding a shell feature to an

existing part

■Modifying wall thickness

■Adding multiple thickness

overrides

■Managing thickness overrides

346 |Chapter 14 Creating Shells

Key Terms

Te r m Definition

converging radial

shapes A sharp corner where cylindrical faces, such as fillets, are offset and converge to

form a zero radius. Parts with more complex shapes, such as variable radius

fillets and surfcuts, need a shell thickness large enough so that the offset face

does not converge.

default thickness The offset value initially applied to all faces of your part.

excluded face Face on a shelled part you select that will not be offset.

reclaimed face Face on a shelled part that was previously excluded can be selected, or

reclaimed. Reclaimed faces are offset by the default thickness.

shell A Mechanical Desktop® feature that cuts portions of the active part by offsetting

its faces.

thickness override An offset value that takes precedence over the default thickness of a shell

feature. You can define a list of thickness override values and apply them to any

face on the part.

Basic Concepts of Creating Shells |347

Basic Concepts of Creating Shells

Unlike other sketched or placed features, a shell feature is initially applied to

all the faces of your active part, instead of only those you select. It doesn’t

need parametric dimensions to control placement. A part can have only one

shell feature.

When you add a shell feature to a part, Mechanical Desktop creates new faces

by offsetting existing ones inside or outside of their original positions. You

can also choose the midplane option, which offsets faces by half the entered

value to one side and half to the other side.

Mechanical Desktop treats continuously tangent faces as a single face when

offsetting. This illustration shows the progression for adding a shell feature

to a part and then a thickness override to the cylindrical face. The faces tan-

gent to the cylindrical face are also offset in the operation.

You can change a shell feature in different ways. You can change the offset

type and offset values in the Shell Feature dialog box. If you choose to

exclude or reclaim faces, or change thickness overrides, you select faces on

your part. In both cases, to apply your modifications you must update the

part.

Adding Shell Features to Models

In this tutorial, you add a shell feature to the existing model of a clutch hous-

ing for a 250cc two-stroke engine. The shell feature requires an excluded face

and multiple thickness overrides.

You apply what you’ve learned in previous chapters about constrained

sketches and features to examine an existing part. You then add a shell fea-

ture to the part, later modifying it to suit your design requirements.

348 |Chapter 14 Creating Shells

Using Replay to Examine Designs

First, review the clutch housing design.

Open the file clutch.dwg in the desktop\tutorial folder. The clutch housing has

been modeled to a point in the design where it is ready for you to add the

shell feature. It contains six extruded features.

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.

For the constraint system in this model, construction lines were used to align

its cylindrical features. You can change the angle of the features with respect

to one another to alter the design to fit engines of different sizes.

To replay the design of a part

1Use AMREPLAY to review the process used to build this model, responding to

the prompts.

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

Closed profile

Enter an option [Display/Exit/Next/Size/Truncate] <Next>:

Press ENTER to review each design step

Enter an option [Exit/Next/suPpress/Truncate] <Next>:

Continue to press ENTER until you see the following message

Part replay complete

The construction of the model is also displayed in the Desktop Browser. Each

feature is located in the order it was created. Expand the browser and exam-

ine the feature hierarchy.

2Change your view to Back Right Isometric.

Desktop Menu View ➤ 3D Views ➤ Back Right Isometric

Adding Shell Features to Models |349

This displays the model in another isometric view.

Next, you remove the silhouette edges from your model so you can visualize

it better. Silhouette edges are similar to hidden lines, but to remove them you

need to modify a system variable.

3Change the system variable controlling the visibility of silhouette edges.

Command DISPSILH

New value for DISPSILH <0>: Enter 1

4Use HIDE to remove hidden lines from your display. This improves your view

of the features of the housing.

Desktop Menu View ➤ Hide

5Use 3DORBIT to dynamically rotate the model, and view the underside of the

housing.

Context Menu In the graphics area, right-click and choose 3D Orbit.

Click the bottom control point on the 3D orbit icon in the graphics area, and

rotate the part upward.

6Remove the hidden lines again. Your drawing should resemble the following

illustration.

350 |Chapter 14 Creating Shells

Cutting Models to Create Shells

Now that you have examined the model, the next step is to cut it, removing

the interior area, so that all that remains is a shell of the part. This part is a

magnesium alloy casting which requires a wall thickness of about 4 mm in

most areas, but some walls must be thicker to withstand forces applied to

them.

To cut a model

1Return to the back right isometric view.

Desktop Menu View ➤ 3D Views ➤ Back Right Isometric

2Return to a wireframe display of your model.

Desktop Menu View ➤ Shade ➤ 3D Wireframe

3Use AMSHELL to create a shell feature.

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

Features ➤ Shell.

4In the Shell Feature dialog box, specify:

Default Thickness: Inside: Enter 4

Choose OK.

Adding Shell Features to Models |351

The shell feature is calculated and the model is updated.

5Change your display to three viewports.

Command 3

This gives you a better view of the thickness of the walls in the model.

An isometric view of the bottom of the housing has been previously saved.

6Click in the right viewport to make it current, and restore the saved view.

Desktop Menu View ➤ Named Views

7In the View dialog box, highlight BOTTOM_ISOMETRIC and choose Set

Current.

Choose OK. The right viewport changes to display the selected view.

352 |Chapter 14 Creating Shells

When the shell feature was added, all the faces in the model were offset. The

result is a hollow model. For a better view, suppress the hidden lines.

8Use HIDE to remove the hidden lines.

Desktop Menu View ➤ Hide

Save your file.

Editing Shell Features

When you create a shell, your wireframe display becomes more complex

because Mechanical Desktop offsets each face in your model, doubling the

number of faces. One way to edit a shell feature is to use AMEDITFEAT and

select an offset face edge. However, choosing the shell feature icon from the

Desktop Browser is easier.

To remove the bottom face from the part, you need to edit the shell feature

and exclude the bottom face.

Adding Shell Features to Models |353

To exclude a face on a shell feature

1Use AMEDITFEAT to edit the shell feature.

Browser In the Browser, right-click Shell1 and choose Edit.

If you choose a method other than the Browser, you must select the shell fea-

ture first. The Shell Feature dialog box is displayed.

2In the Shell Feature dialog box, choose Add and then respond to the prompts

as follows:

Select faces to exclude: Specify a point (1)

Enter an option [Accept/Next] <Accept>:

Enter n until the bottom face is selected or press ENTER

Select faces to exclude: Press ENTER

Choose OK to exit the dialog box.

In the Browser, the shell icon has a yellow background indicating that it

needs to be updated.

354 |Chapter 14 Creating Shells

3Use AMUPDATE to update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

The model is updated to reflect the modified shell feature.

Save your file.

Adding Multiple Wall Thicknesses

When the clutch housing is attached to an operating engine, the stresses are

higher on some casting walls than on others. The walls surrounding the

water pump shaft and the clutch support the most force. You need to thicken

these walls to conform to design requirements.

Wall thickness overrides are applied to only those faces you select. A chain of

tangent faces is treated as a single face.

You can have as many wall thickness overrides as you like in a shell feature,

but most applications require only a few. Mechanical Desktop keeps track of

which faces have thickness overrides.

Adding Shell Features to Models |355

To edit a shell through the Browser

1Return to the back right isometric view.

Desktop Menu View ➤ 3D Views ➤ Back Right Isometric

The face surrounding the water pump can now be selected easily.

2Return to a wireframe display of your model.

Desktop Menu View ➤ Shade ➤ 3D Wireframe

3Edit the shell feature again.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Select the shell feature. The Shell Feature dialog box is displayed.

4In the Shell Feature dialog box, in Multiple Thickness Overrides, specify:

Set: New

Thickness: Enter 8

Faces: Add

On the command line, respond to the prompts as follows:

Select faces to add: Specify a point (1)

Select faces to add: Press ENTER

Choose OK to exit the dialog box.

356 |Chapter 14 Creating Shells

5Update the part, responding to the prompt.

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

Enter an option [active Part/aLl parts] <active Part>: Press ENTER

Refer to the top view in the upper left viewport to see the results. When you

selected the cylindrical face, tangent faces were automatically selected. The

wall thickness surrounding the water pump should look twice as thick as the

rest of the walls.

To create a multiple thickness override

1In the right viewport, change to the left isometric view of the model so that

the faces surrounding the clutch can be easily selected.

Desktop Menu View ➤ 3D Views ➤ Front Left Isometric

2Use AMEDITFEAT to create a multiple thickness override for the walls surround-

ing the water pump.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Select any one of the edges of the inside shell walls. The Shell Feature dialog

box is displayed.

Adding Shell Features to Models |357

3In the Shell Feature dialog box, specify:

Multiple Thickness Overrides: New

Thickness: Enter 6

Choose Add, and respond to the prompts as follows:

Select faces to add: Specify a point on the model (1)

Select faces to add: Specify a second point (2)

Select faces to add: Press ENTER

Choose OK to exit the dialog box.

4Update the part.

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

In the top view, the two faces you selected are thicker.

5Make the right viewport active and restore another saved view.

Desktop Menu View ➤ Named Views

358 |Chapter 14 Creating Shells

6In the View dialog box, highlight BOTTOM_PERSPECTIVE, choose Set Cur-

rent, and then choose OK.

7Use HIDE to remove the hidden lines.

Desktop Menu View ➤ Hide

Save your file.

Managing Multiple Thickness Overrides

Occasionally, you may create complex parts that require more thickness

override values. As you apply the override values to faces on your part, it is

easy to lose track of which faces are using different overrides, especially if you

are viewing a part that was designed by someone else.

However, Mechanical Desktop makes it easy to manage overrides and iden-

tify the faces with specific override values. You may have noticed that when

you chose an override from the list in the Shell Feature dialog box, all faces

with that override were highlighted.

Mechanical Desktop also audits the override list each time you edit the shell

feature. Override values that are no longer used are removed from the list.

This eliminates the need to manually delete obsolete overrides, which

ensures that the list always reflects the wall thicknesses of your current part.

Design changes are also easy to implement. When you change an override

thickness value in the Shell Feature dialog box, you change the wall thick-

nesses of all the faces that reference that override value.

Adding Shell Features to Models |359

For the clutch assembly, the wall thickness around the water pump can be

reduced from 6 to 4. Because the default wall thickness of the shell is 4, you

remove the override of 6 from the list. When you delete an override value

from the list, faces that once referenced that value revert to the default

thickness.

To change a wall thickness

1Use AMEDITFEAT to edit the shell feature again to change the wall thickness

around the water pump.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Select the shell feature. The Shell Feature dialog box is displayed.

2In the Shell Feature dialog box, specify:

Thickness: Enter 6

Set: Delete

Choose OK and then press ENTER on the command line.

3Use AMUPDATE to update the part.

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

The model is updated to reflect the modified shell feature.

Save your file.

360

361

In This Chapter 15

Creating Table Driven Parts

You can assign variables to the parametric dimensions

that control a generic part and then use a table (an

external spreadsheet) to control the size and shape of

the part. The spreadsheet can contain several versions of

the part. Each version uses different values for the

variables you define. Autodesk® Mechanical Desktop®

redraws the part using the variables linked to that

version.

Documentation for all versions can be simplified by

plotting one drawing representing the generic part. You

can paste the spreadsheet into your drawing to list the

values for each version.

For this tutorial, you need Microsoft® Excel on your

system.

■Creating a table

■Displaying part versions

■Editing a table

■Solving common problems with

table driven parts

■Suppressing features in table

driven parts

■Setting up a generic drawing to

define the table driven part

362 |Chapter 15 Creating Table Driven Parts

Key Terms

Te r m Definition

active part variable A parametric variable used in the dimensions that control features of the active

part.

feature suppression Temporarily removing features from the calculation of a part. Features can be

suppressed manually through the Desktop Browser, or through a linked external

table.

global variable A parametric variable that can be used by any number of parametric features and

parts. Also used for single parts and to constrain parts.

linked spreadsheet An external spreadsheet linked to the current drawing file. This spreadsheet can

be used to change parts in the drawing file, if the variables in the spreadsheet are

used in the drawing file.

manual suppression Suppressing features through the browser or command line. These features will

remain suppressed unless manually unsuppressed or a version of a linked table

that unsuppresses it becomes active.

part version The version of variables that the active part is currently using from the external

table. Part versions can be changed through the Desktop Browser or the Design

Variables dialog box.

table An external spreadsheet that drives versions of a part.

table driven

suppression Features suppressed in an external spreadsheet. A table driven suppressed feature

is suppressed only in the part version specified in the spreadsheet.

table driven variable A global or active part design variable controlled by values in a linked external

spreadsheet.

Basic Concepts of Table Driven Parts |363

Basic Concepts of Table Driven Parts

In the manufacturing industry, you often have parts that are similar to each

other except for size or a particular feature. Some examples are springs, brackets,

plates, nuts, and bolts. By driving part versions from an external spreadsheet,

you can document a number of similar parts using one drawing.

The external spreadsheet, or table, is where you make modifications to your

design specifications once your drawing is set up. By controlling a part from

a table, you avoid errors due to design changes that have not been imple-

mented across a number of drawings. All design data is contained in the

table, with one drawing representing many parts.

Open the file tdpart1.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 is a simple bracket that you link to a spreadsheet.

The part is controlled by its relationships to nine active part design variables.

Changing the value of one variable affects every dimension that has a rela-

tionship to it. For information on creating and modifying design variables,

see chapter 11, “Using Design Variables.”

364 |Chapter 15 Creating Table Driven Parts

Setting Up Tables

A table is a spreadsheet that contains the various part versions and the values

of the design variables for each version. You use Microsoft Excel to create

table driven parts.

First, examine the part, using the Desktop Browser. Expand the Browser by

clicking the plus sign in front of TDPART1 and PART1_1. The bracket is con-

structed from three extrusions, three holes, and five fillets.

Each feature is controlled by a design variable. In this exercise, you create a

table containing the design variables, and define four different part versions.

To set up a table

1Use AMVARS to open the Design Variables dialog box and set up a table.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, verify that the Active Part tab is selected.

Examine the active part design variables.

3Under Table Driven, choose Setup.

4In the Table Driven Setup dialog box, verify that the Active Part tab is

selected. Under Layout, specify:

Version Names: Across

Choose Create.

Setting Up Tables |365

5In the Create Table dialog box, select the desktop\tutorial folder and specify

tdpart1.xls as the name of your table.

Choose Save to exit the dialog box.

Microsoft Excel opens a new spreadsheet containing a generic part and a

value for each design variable assigned to it.

Next, change the name of the generic part to 35 and add three more part

versions.

To define additional part versions

1Fill in the value of the design variable for each new part definition, as shown

in the following illustration:

2Save the file and exit Microsoft Excel.

366 |Chapter 15 Creating Table Driven Parts

3In the Table Driven Setup dialog box, select Update Link and choose OK.

Choose OK to exit the Design Variables dialog box.

The Desktop Browser now contains a Table icon nested below PART1_1. The

four part versions you created in the spreadsheet are listed below the Table

icon.

The PART1_1 (35) icon displays the active version in parentheses. The Table

(tdpart1.xls) icon indicates the name of the spreadsheet that is linked to your

drawing.

Next, display each version of the table driven part. When you select a ver-

sion, Mechanical Desktop recalculates the part, using the values for the vari-

ables that correspond to the selected version.

Displaying Part Versions

You display part versions by selecting them from the Desktop Browser.

To display a part version

1Display the 46 part version.

Browser Double-click the 4x6 icon.

The 4x6 version is calculated and displayed.

2Repeat step 1 for the other two versions.

The part versions do not differ, except in size. In the next lesson, you add

another part version by editing the spreadsheet.

Editing Tables |367

Editing Tables

Using a table to drive multiple versions of a part gives you flexibility in

designing the part. You can quickly create variations of the part, and easily

edit the design parameters by changing values in the cells of the spreadsheet.

To add a part version to an existing table

1Open the spreadsheet to edit.

Browser Right-click Table (tdpart1.xls) and choose Edit.

NOTE The part definition in the Browser displays the current version of the

part for easy reference.

Microsoft Excel opens, displaying your spreadsheet.

368 |Chapter 15 Creating Table Driven Parts

2Add a new part version in the spreadsheet, using the values in the following

illustration:

3Save the spreadsheet and exit Microsoft Excel.

4Update the link to the spreadsheet.

Browser Right-click Table (tdpart1.xls) and choose Update.

Examine the Browser. It now displays five part versions under the Table

(tdpart1.xls) icon.

Occasionally, errors occur when you link a spreadsheet to Mechanical

Desktop. In the next section, you learn how to fix errors such as

■Spreadsheets that cannot be found

■Spreadsheets that have been modified since the drawing was saved

■Incorrect or missing data in a spreadsheet

Resolving Common Table Errors |369

Resolving Common Table Errors

Open the file tdpart2.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing contains a version of the simple bracket used in the previous

example, but it is linked to a different spreadsheet.

Before you can look for errors in the link between the drawing and the

spreadsheet, you need to expand the part hierarchy.

To expand a part hierarchy

1Expand the part hierarchy.

Browser Click the plus sign in front of TDPART2 and then click

PART1_1.

Notice the red background behind the Table icon. This indicates that the

spreadsheet cannot be found, it has been modified since the drawing was last

saved, or it contains incorrect data in one or more cells. Before the spread-

sheet can be used to drive the part, you must resolve the conflict.

370 |Chapter 15 Creating Table Driven Parts

To resolve a conflict with a linked spreadsheet

1Resolve the conflict between the drawing and the linked spreadsheet.

Browser Right-click Table (tdpart.xls) and choose Resolve Conflict.

An AutoCAD message dialog box is displayed asking if you would like to

update the table.

2In the message dialog box, choose Yes.

The HD variable controls the diameters of the holes for the bracket. The first

part version is missing an entry in cell B10.

3In cell B10, enter .1875. Then save the spreadsheet and exit Microsoft Excel.

4Update the link to the table.

Browser Right-click Table (tdpart2.xls) and choose Update.

Mechanical Desktop updates the link.

5Use AMUPDATE to update the part.

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

Next, display the part versions.

Suppressing Features |371

To display the first part version

1Display the first part version.

Browser Double-click the 35 icon nested under PART1_1.

The 35 angle bracket is recalculated from the values in the table and then

displayed.

2Repeat step 1 for the remaining four part versions.

Save your file.

Next, you suppress features for some of the part versions in your table. The

smaller brackets do not require the brace, so you will suppress the features

associated with it for those versions.

Suppressing Features

Suppressing features can be done in the Browser, in a linked table, or in the

Suppress By Type dialog box. Suppressing a feature manually in the Browser

affects all part versions. Suppressing a table driven feature gives you control

over each version.

Use the Suppress By Type dialog box to suppress and unsuppress features by

specific type.

With an existing table, you append the features you want suppressed to the

table. First, you manually suppress the brace feature and the bracecut feature

in the Browser. It is not important which version of the part is active when

the features are suppressed.

372 |Chapter 15 Creating Table Driven Parts

To suppress a feature

1Display the first part version.

Browser Double-click the 35 icon nested under PART1_1.

2Use AMSUPPRESSFEAT to suppress the brace feature, responding to the

prompt.

Browser Right-click Brace and choose Suppress.

The highlighted features will be suppressed.

Continue? [Yes/No] <Yes>: Press ENTER

The brace feature is suppressed and is no longer visible on your screen. The

bracecut feature and four fillets are dependent on the brace feature, so they

are also suppressed.

Manually suppressed features are represented in the Browser by a circle and

a dashed line preceding the grayed-out feature name. These features can be

unsuppressed at any time.

Next, append the suppressed features to the table.

Suppressing Features |373

To append a suppressed feature to a table

1Use AMVARS to append the suppressed features to the spreadsheet.

Desktop Menu Part ➤ Design Variables

2In the Design Variables dialog box, under Table Driven, choose Setup.

3In the Table Driven Setup dialog box, specify:

Type: Both

Format: Concatenate Tables

Choose Append.

Microsoft Excel spreadsheet tdpart2.xls is displayed. A new entry, brace, has

been added under the existing design variables. The letter “S” in the 35 col-

umn indicates that this feature is suppressed.

Next, suppress the brace and its dependent features for the 46 version.

4In the spreadsheet, enter S in cell C12.

For the largest bracket, you suppress the bracecut feature while retaining the

brace feature for strength.

374 |Chapter 15 Creating Table Driven Parts

To create a suppressed feature in a table

1In the spreadsheet, in cell A13 enter bracecut.

2In cell F13 enter S.

3Save the spreadsheet and exit Microsoft Excel.

4Choose OK to exit the Table Driven Setup dialog box without updating the

link.

5Choose OK to exit the Design Variables dialog box.

You have created two table driven suppressed features. To activate the table

driven suppression of these features, you update the link to the table. After

the table has been linked to the drawing, these features cannot be manually

unsuppressed. To unsuppress these features, you edit the spreadsheet.

Manually suppressed features affect all part versions so you must manually

unsuppress the features in the Browser before you update the link to the

table.

Suppressing Features |375

To manually unsuppress a feature

1Use AMUNSUPPRESSFEAT to unsuppress the brace feature.

Browser Right-click Brace and choose Unsuppress+.

NOTE By using Unsuppress+ in the Browser, you unsuppress the feature you

select and all dependent features. If you use the Browser, the dialog box is not

displayed.

2If you use the Unsuppress By Type dialog box, verify that Fillets, which are

the dependent features, and Extrudes are selected.

Choose OK.

The brace and its dependent features are unsuppressed. Look at the Browser.

There should be no suppressed features visible.

3Update the link to the table.

Browser Right-click Table (tdpart2.xls) and choose Update.

The suppressed features for the active version are now represented in the

Browser by a different symbol. A circle with a diagonal line through it indi-

cates that the feature is suppressed by the table and can be unsuppressed only

by editing the table.

Next, display the 35 version of the bracket.

376 |Chapter 15 Creating Table Driven Parts

To display a part version

1Display the part.

Browser Double-click the 35 icon nested below Table (tdpart2.xls).

The part is recalculated using the values for the 35 version in the linked

table. In the Browser, the suppressed features are grayed out.

2Repeat step 1 for the 46 version. The brace and its dependent features in this

version are suppressed.

3Repeat step 1 for the 57 and 69 versions. Note that the features are not sup-

pressed in these versions.

4Repeat step 1 for the 712 version. The brace feature remains in this version,

but the bracecut and its dependent features are suppressed.

Save your file.

35 version

712 version

Working with Two Part Versions |377

Working with Two Part Versions

You can create copies of a part and work with different versions to create

assemblies. In this lesson, you copy a part and display two versions

simultaneously.

To copy a part definition

1Display the 35 version of the bracket.

Browser Double-click the 35 icon nested below Table (tdpart2.xls).

2Use UCS to return to the World Coordinate System so that the copy of the

part is oriented the same as the original.

Desktop Menu Assist ➤ New UCS ➤ World

3Use AMCATALOG to make a copy of PART1_1.

Context Menu In the graphics area, right-click and choose Catalog.

4In the Assembly Catalog, clear the Return to Dialog check box and select the

All tab.

5In Local Assembly Definitions, right-click PART1_1 and choose Copy

Definition.

378 |Chapter 15 Creating Table Driven Parts

6In the Copy Definition dialog box, specify:

New Definition Name: Enter part2

Choose OK.

7Continue on the command line.

Specify new insertion point: Specify a point to the right of the existing part

Specify insertion point for another instance or <continue>: Press ENTER

Choose OK to close the Assembly Catalog dialog box.

The Browser now contains a PART2_1 definition. Because you copied the orig-

inal part definition, its relationship to the spreadsheet, tdpart2.xls, has been

duplicated in the new part.

Next, change the version of the copied part in your drawing.

copied part definition

Creating Drawing Views |379

To display a different version

1Use AMACTIVATE to activate PART2_1.

Browser In the Browser, right-click PART2_1 and choose Activate

Part.

2Display the 57 version for PART2_1.

Browser Double-click the 57 icon nested under PART2_1.

The 57 version of PART2_1 is displayed.

Save your file.

Next, you set up the drawing for plotting. Instead of using numeric dimen-

sions to annotate five separate parts, you define views for one part and

annotate the drawing, using active part design variables and equations.

You paste into the drawing a copy of your spreadsheet that lists the values

of those variables for each part version.

First, create drawing views to display the part.

Creating Drawing Views

The first view you create is the base view. You define the plane to orient your

view using a part face or work feature, and then position the view in Drawing

mode.

Because you are creating a generic view to represent all versions of the part,

you use the 57 version, which contains the brace. When you import the

table, it will indicate the versions for which the brace is suppressed.

PART2_1

380 |Chapter 15 Creating Table Driven Parts

To create a base view

1Use the Browser to turn off the visibility of PART1_1.

Browser Right-click PART1_1 and choose Visible.

2Use AMMODE to switch to Drawing mode.

Browser Select the Drawing tab.

Mechanical Desktop switches to Drawing mode. A title block has been

inserted into the drawing.

3Use AMDWGVIEW to create the base view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, select the Hidden Lines tab and specify:

Calculate Hidden Lines: Clear the check box

Display As: Wireframe

Choose OK, and continue on the command line.

Select planar face, work plane or [Ucs/View/worldXy/worldYz/worldZx]:

Specify the front edge (1)

Enter an option [Accept/Next] <Accept>:

Enter n to highlight the front face, or press ENTER

Select work axis, straight edge or [worldX/worldY/worldZ]:

Specify the top edge (2)

Adjust orientation [Flip/Rotate] <Accept>:

Verify that the UCS is upright, and press ENTER

Creating Drawing Views |381

4Continue on the command line to place the base view.

Specify location of base view: Specify a point in the top center of the title block

Specify location of base view: Press ENTER

Your drawing should look like this.

Next, create side and bottom orthographic views of the part.

382 |Chapter 15 Creating Table Driven Parts

To create an orthographic view

1Create the orthographic view.

Context Menu In the graphics area, right-click and choose New View.

2In the Create Drawing View dialog box, select the view type Ortho. On the

Hidden Lines tab, specify:

Display As: Wireframe

Choose OK.

3On the command line, respond to the prompts as follows:

Select parent view: Pick a point inside the base view

Specify location for orthogonal view: Specify a point to the left of the base view

Specify location for orthogonal view: Press ENTER

Your drawing should look like this.

Next, create a bottom ortho view.

4Create the orthographic view.

Context Menu In the graphics area, right-click and choose New View.

Creating Drawing Views |383

5In the Create Drawing View dialog box, select the view type Ortho. On the

Hidden Lines tab, specify:

Display As: Wireframe

Choose OK.

6On the command line, respond to the prompts as follows:

Select parent view: Pick a point inside the base view

Specify location for orthogonal view: Specify a point below the base view

Specify location for orthogonal view: Press ENTER

Your drawing should look like this.

Save your file.

Look at the Browser. There are two ortho views and a base view. Because the

ortho views are dependent on the base view, they are nested below the Base

icon.

The parametric dimensions that define the part are displayed in each view.

Because Mechanical Desktop displays the parametric dimensions in the order

in which they were created, dimensions may conflict with each other, over-

lap, or be redundant in a drawing view.

Next, clean up the display of parametric dimensions in each of the views.

384 |Chapter 15 Creating Table Driven Parts

Cleaning Up the Drawing

To clean up the drawing, you change the parametric dimensions to be dis-

played as parameters, hide extraneous dimensions, and move dimensions for

clarity.

NOTE For detailed cleanup instructions see “Cleaning Up Drawings” on page

322 in chapter 13.

Displaying Dimensions as Parameters

The parametric dimensions used to define a part are displayed with the val-

ues for the active version of the part. Because you are creating a drawing of

the generic part and linking a table to describe the values for the parameters

controlling each part version, you change dimensions to be displayed as

parameters.

To change a dimension to be displayed as a parameter

1Display the dimensions as parameters, responding to the prompt.

Desktop Menu Drawing ➤ Parametric Dim Display ➤ Dimensions as

Parameters

Select dimension or [All/View/Select dimensions] <Select dimensions>: Enter a

Cleaning Up the Drawing |385

Your drawing should look like this.

Next, hide the extraneous dimensions.

Hiding Extraneous Dimensions

When drawing views are created, Mechanical Desktop displays all the para-

metric dimensions that are related to the part display in each view. Usually,

some cleanup is required because of overlapping or redundant dimensions.

386 |Chapter 15 Creating Table Driven Parts

To hide an extraneous dimension in a base view

1Use AMVISIBLE to hide extraneous dimensions.

Desktop Menu Drawing ➤ Drawing Visibility

In the Desktop Visibility dialog box, choose Select.

NOTE If you choose the toolbutton method to hide the dimensions, the

Desktop Visibility dialog box is not displayed. Select the dimensions to hide. Use

Zoom Realtime while selecting the dimensions.

2Respond to the prompts as follows:

Select drawing objects to hide: Specify the d1+d2 dimension (1)

Select drawing objects to hide: Specify the ab dimension (2)

Select drawing objects to hide: Specify the tb dimension (3)

Select drawing objects to hide: Specify the tb dimension (4)

Select drawing objects to hide: Press ENTER

In the Desktop Visibility dialog box, choose OK.

1,4

Cleaning Up the Drawing |387

To hide a dimension in an orthographic view

1Use AMVISIBLE to hide dimensions.

Desktop Menu Drawing ➤ Drawing Visibility

2In the Desktop Visibility dialog box, choose Select.

NOTE If you choose the toolbutton method to hide the dimensions, the

Desktop Visibility dialog box is not displayed. Select the dimensions to hide.

3In the side ortho view, hide the db dimension, the two db/2 dimensions, and

the db/4 dimension.

You do not need to hide dimensions in the bottom ortho view.

The ortho views should look like this.

Now that the extraneous dimensions are hidden, it is easier to move the

remaining dimensions for clarity.

Moving Dimensions

Because several of the remaining dimensions overlap, you need to rearrange

them so that they are easy to view.

side view bottom view

388 |Chapter 15 Creating Table Driven Parts

To move a dimension

1Use AMMOVEDIM to move the parametric dimensions in the base view,

responding to the prompts.

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

Dimensions ➤ Move Dimension.

Enter an option [Flip/Move/move mUltiple/Reattach] <Move>: Press ENTER

Select dimension to move: Select the dimension for the long leg of the bracket (1)

Select destination view: Specify a point in the base view (2)

Select location: Specify a point to the right (3)

Select location: Press ENTER

Cleaning Up the Drawing |389

2Continue moving dimensions until your base view looks like this.

3Move the dimensions in the ortho views.

The ortho views should look like this.

Next, add reference dimensions, to fully define the part.

side view bottom view

390 |Chapter 15 Creating Table Driven Parts

Enhancing Drawings

To finalize the presentation of the drawing, you add power dimensions, dis-

played as parameters and create a hole note to describe the three holes in the

bracket.

Creating Power Dimensions

The drawing views are intended to display the generic part. When you dis-

play parametric dimensions using design variables, and you power dimen-

sion your drawing views, the views represent the generic part.

Because reference dimensions are not displayed as parameters, you use power

dimensioning to create dimensions represented as parameters. Power dimen-

sioning allows you to specify tolerance and fit information for your parts as

you dimension and to modify the default value of a dimension as you create it.

Later, when you paste the spreadsheet into the drawing, you will have a list

of values for the variables in each version that cross-references the dimen-

sions in each view.

To add a reference dimension

Before you begin this procedure, enable Osnaps. If Osnaps are set to off, you

will be unable to create the dimension. Work in the base view.

1Use AMPOWERDIM to create power dimensions, responding to the prompts.

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

Dimensioning.

(Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/

Update] <Select>: Specify a point at the bottom of the short leg (1)

Specify second extension line origin:

Specify a point at the inside top of the bracecut (2)

Place dimension line [Options/Pickobj] <Options>: Specify a location (3)

Enhancing Drawings |391

2In the Power Dimensioning dialog box, change the default text to tb/2.

Choose OK.

392 |Chapter 15 Creating Table Driven Parts

3Continue on the command line to add a power dimension to the fillet at the

bottom of the long leg:

(Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/

Update] <Select>: Press ENTER

Select arc, line, circle, or dimension: Specify the arc

Enter an option [Next/Accept} <Accept>: Press ENTER

Specify dimension line location or [Linear/Diameter/Options]:

Specify a location for the dimension

(Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/

Update] <Select>: Press ENTER

Select arc, line, circle, or dimension <Exit>: Specify the dimension

4In the Power Dimensioning dialog box, specify tb*.75 for the dimension text.

Choose OK.

5Continue on the command line.

Select arc, line, circle, or dimension <Exit>: Press ENTER

Enhancing Drawings |393

Your drawing should resemble the following illustration.

6Place power dimensions so that the orthographic views look like this.

Next, create a hole note that describes the three holes in the bracket.

Creating Hole Notes

Mechanical Desktop provides a tool for creating hole notes, which saves you

time when annotating your drawing.

In the side view, create a hole note for one of the holes in the long leg of the

bracket.

394 |Chapter 15 Creating Table Driven Parts

To create a hole note

1Use AMNOTE to create the hole note, responding to the prompts.

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

Hole Note.

Select object to attach [rEorganize]:

Specify the upper hole in the long leg of the bracket (1)

Next Point <Symbol>: Specify the location (2) and press ENTER.

2In the Note Symbol dialog box, select the Leader tab. In Leader Justification,

specify Middle of All Text.

Choose OK.

The hole note is displayed in your drawing.

Enhancing Drawings |395

Edit the hole note so that it is typical for all three holes.

3Use AMPOWEREDIT to edit the hole note, responding to the prompt.

Context Menu Select the hole note, then right-click the note and choose

Edit.

4In the Note Symbol dialog box, select the Note tab, and change the text to

read as follows:

%%c hd THRU

(typ of 3)

Choose OK.

The side view should now look like this.

Save your file.

Now that the power dimensions and annotations are in place, paste the

linked spreadsheet into the drawing.

396 |Chapter 15 Creating Table Driven Parts

Pasting Linked Spreadsheets

Pasting a linked spreadsheet into a drawing provides more flexibility for

working with the table that defines the values for the part versions. The

external spreadsheet can be opened and modified while you are working, and

the results are reflected in the drawing.

To paste a linked spreadsheet into a drawing

1Use AMMODE to return to the Part/Assembly environment.

Browser Select the Model tab.

2Open the spreadsheet.

Browser Right-click Table (tdpart2.xls) and choose Edit.

The Microsoft Excel spreadsheet is displayed.

3Select the cells to be copied.

4In Microsoft Excel, choose Edit ➤ Copy.

5In the drawing, return to Drawing mode.

Browser Select the Drawing tab.

Pasting Linked Spreadsheets |397

6Paste the selected area of the spreadsheet into the drawing.

Desktop Menu Edit ➤ Paste Special

7In the Paste Special dialog box, choose Paste Link.

8Place the selected cells in the drawing. Your drawing should look like this.

NOTE Depending on the zoom factor of your display at the time you paste the

image, you may have to resize it. Select the image, and use a corner grip to resize

it to fit in the drawing.

Save your file.

Now that the linked spreadsheet has been pasted into the drawing, any

changes made in the spreadsheet will automatically be reflected in the draw-

ing. Experiment with modifications to the spreadsheet to see how your part

and the table are automatically updated.

398

399

In This Chapter 16

Assembling Parts

You can build part assembly models from two or more

parts, or parts grouped in subassemblies. Like part

features, parts and subassemblies act as building blocks.

Autodesk® Mechanical Desktop® builds individual parts

and subassemblies into an assembly.

In this tutorial, you create an assembly model of a pair

of slip pliers from four parts. Three of the parts originate

in files that are externally referenced to the assembly

file.

Using externally referenced parts creates a truly parametric

assembly design. Changes to an external reference can be

made from within the assembly or in the original file.

■Using external parts in an

assembly

■Using assembly constraints

■Analyzing the assembly

■Creating assembly scenes

■Using assembly tweaks and trails

■Creating assembly drawing

views

■Editing an external reference

and updating an assembly

400 |Chapter 16 Assembling Parts

Key Terms

Te r m Definition

3D constraint In assembly modeling, an associative link between two or more parts that controls their

locations relative to each other and to their placement within the assembly.

Assembly Catalog The means of attaching and cataloging local and external parts and subassemblies in

the Assembly Modeling environment. Use the All and External tabs to specify contents,

which can be instanced, copied, renamed, replaced, externalized, removed, localized,

sorted, unloaded, and reloaded.

assembly tree A graphical hierarchy that illustrates the order in which parts and subassemblies are

combined in the current assembly. The assembly tree is managed in the Desktop

Browser.

attach The act of connecting a reference file to the current assembly file. The attachment

remains with the current file after the file is saved.

definition All information about a part or subassembly, including its name, location, and

attributes.

detach Permanently removing a file as an external reference in an assembly.

external reference A part or assembly that resides in a file other than the current part or assembly file.

insert constraint Aligns center points and planes of two circles in a specified direction. Solves translation

degrees of freedom. Used to constrain a bolt in a hole, for example.

localized part Changes the definition of a part from external to local, severing the link to the external

file. Changes made to a localized part affect only the current part or assembly file; other

part or assembly files that reference the part are not affected.

mate constraint Causes a plane or axis on one part to be coincident with a plane, point, or axis on

another part in a specified direction. Removes a translational degree of freedom.

rename definition In the Part or Assembly Catalog, an attached external part or subassembly may be

renamed. The alias name is displayed beside the drawing name in parentheses.

scene A 3D orientation of an assembly that you can use to create a 2D view in Drawing

mode. You use scenes to provide exploded or assembled views of your assembly

without destroying the constraints.

trail In an exploded view, a line that shows how parts in an assembly are assembled.

tweak Adjusts the position of parts in an assembly scene to avoid overlap in some views or to

make some parts more visible.

Basic Concepts of Assembling Parts |401

Basic Concepts of Assembling Parts

You create assemblies from parts, either combined individually or grouped

in subassemblies. Mechanical Desktop builds these individual parts and

subassemblies into an assembly in a hierarchical manner according to rela-

tionships defined by constraints. Using the Desktop Browser, you can

restructure the hierarchy of an assembly as needed, while retaining the

design constraints. See “Using the Desktop Browser” on page 414.

As in part modeling, the parametric relationships allow you to quickly

update an entire assembly based on a change in one of its parts.

You can build 3D solid assembly models from two or more parts or subassem-

blies. Like part features, parts and subassemblies act as building blocks.

The following process for building assemblies and subassemblies is similar to

that for building parts:

■Lay out the assembly.

■Create the base part.

■Create the remaining parts.

■Create the assembly and subassemblies.

■Analyze the assembly.

■Modify the assembly as necessary.

When you create an assembly file, you can create your parts in the assembly

drawing, or you can reference external files.

Using externally referenced parts gives you more flexibility over the control

of your assembly. If you need to make modifications to any of your parts, you

can open the individual part file and make changes to it. Because more than

one drawing can be open in the same Mechanical Desktop session, you can

immediately see the effects of your changes in the assembly file. You can also

edit external references from within the assembly file. This is particularly use-

ful in smaller assemblies. Depending on your system resources, you can edit

external files individually if they are part of a large assembly.

After you have assembled your parts, you need to check the assembly for

interferences. You may also want to perform mass property calculations on

your parts to ensure that they are structurally sound.

Finally, you need to document your design. To make it easier to visualize your

design, you may want to adjust, or tweak, your assembly and add trails to

indicate how your parts fit together. Then, you set up your drawing views

and add information, such as reference dimensions and annotations, before

finalizing the drawing for plotting.

402 |Chapter 16 Assembling Parts

Starting Assembly Designs

An assembly design might begin as an overall conceptual design. You may

know how the parts are assembled but you may not know all the details

about each part.

Before you begin, decide how you want to lay out your assembly.

■Start with a design idea.

■Decide whether you need to create new parts, or if you can use existing

parts.

■Start drawing the parts.

Although you can begin designing immediately and reorganize the hierarchy

of your assembly later, for this lesson you assemble parts in a logical order,

starting at the top level in the assembly tree. One part has already been cre-

ated in the tutorial file for this lesson. The other three parts reside in separate

files. You attach the files and then instance the parts into the assembly.

To begin, open the file s_plier.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.

In the Browser, the PLIERB part is nested under the assembly icon.

Next, you reference three other parts to create the assembly.

Using External Parts in Assemblies |403

Using External Parts in Assemblies

The parts that make up the assembly model can be created and maintained

in other files. These parts are called externally referenced parts. When a part

changes, all instances of that part in other files are automatically updated.

Using parts from other files as external references is similar to external refer-

encing (xref) in AutoCAD. Because they are external, you can reuse referenced

parts in future assemblies. You can start a library of commonly used parts in a

directory where you can easily locate them. Externally referenced parts can be

instanced in the current file at any time.

To attach and instance an external part

1Use AMCATALOG to attach the external parts.

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

Menu ➤ Catalog.

2In the Assembly Catalog, verify that the External tab is selected and Return

to Dialog is checked.

In the Directories window, right-click and choose Add Directory.

404 |Chapter 16 Assembling Parts

A Browse for Folder dialog box lists your network connections and

directories.

3In the Browse for Folder dialog box, specify the desktop\tutorial folder to be

your working directory.

Choose OK.

NOTE If you have installed Mechanical Desktop in a different location, browse

through your directories to locate the correct folder.

All drawing files in the desktop\tutorial folder are listed under Part and Subas-

sembly Definitions on the External tab.

4In the desktop\tutorial folder, double-click the PLIERT definition to insert an

instance into the drawing, responding to the prompts.

Specify new insertion point: Specify a point below PLIERB

Specify insertion point for another instance or <continue>: Press ENTER

You can also right-click the definition in the Catalog and choose Attach.

The pliert.dwg file is attached to the current assembly, and an instance is

inserted into the current assembly. In the Assembly Catalog, PLIERT is dis-

played on a white background.

Using External Parts in Assemblies |405

Notice that each of the external files is preceded by an icon, indicating

whether it is a part or assembly file.

5Attach and instance the HEXNUT and HEXBOLT parts to the current

assembly.

As you instance each part, you return to the Assembly Catalog. In the Part

and Subassembly Definitions list, each attached part is displayed on a white

background. When all parts are instanced into the assembly, choose OK.

Examine the Browser. Four parts are nested under the assembly definition.

Each part is followed by a number. As you create instances of a part, each

instance is numbered to indicate the order in which you added them to the

assembly.

Notice that PLIERT, HEXBOLT, and HEXNUT have teal colored icons. This

indicates that the parts are externally referenced.

6Change to an isometric view of your drawing.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

Now you are ready to start the assembly process.

NOTE For information about using the shortcut method in the Desktop

Browser to localize and externalize assembly component definitions, see “To

localize an external part with the Browser” on page 417.

hexbolt

plierb

pliert

hexnut

406 |Chapter 16 Assembling Parts

Assembling Parts

After parts or subassemblies have been created, you apply constraints to

position them relative to one another. Each time you apply a constraint to a

part, you eliminate some degrees of freedom (DOF). The number of degrees

of freedom determines the movement of a part in any direction; the more

constraints applied, the less the part can move.

A degrees of freedom symbol illustrates the instance order of the parts and

how the parts can move. The DOF symbol shows how many degrees of free-

dom are not solved and help you visualize and apply constraints to parts.

Apply multiple assembly constraints on two parts to fully position them rel-

ative to each other. A bolt might still turn (rotational degree of freedom is not

solved), but as long as the bolt and hole are aligned on their axes, and the

bolt face is flush with the hole, no other constraints are needed.

Because the parts and their assembly constraints are parametric, they can be

edited. The assembly constraints applied on each part are permanently

stored with the assembly to allow parametric updating if the parts change.

To display a DOF symbol

1Use the Browser to display the DOF symbol for HEXBOLT_1.

Browser Right-click HEXBOLT_1, and choose DOF Symbol.

The DOF symbol is displayed in the center of HEXBOLT. It indicates that the

bolt can move in any direction.

DOF symbol

Assembling Parts |407

Constraining Parts

Use a mate constraint to join the PLIERT and HEXBOLT parts. Zoom in as

needed to make the selection easier.

To add a mate constraint between parts

1Use AMMATE to select the first set of geometry, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select HEXBOLT (1)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Enter a

First set = Plane

Enter an option [Clear/aXis/Point/Flip/cYcle] <accEpt>:

Enter y to cycle to face, or press ENTER

2Select the second set of geometry to complete the mate constraint.

Select second set of geometry: Select PLIERT (2)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>:

Enter a to highlight the corresponding face of PLIERT

Second set = Plane

Enter an option [Clear/aXis/Point/Next/Flip/cYcle] <accEpt>:

Enter y to cycle to the next face, or press ENTER

Enter offset <0.0000>: Press ENTER

To select geometry, enter responses on the command line, or use the animated

cursor to cycle through options. Click the left (red) mouse button to cycle.

Then, press the right (green) mouse button to accept. You may also use the

animated cursor to select a face by picking in the area defined by the face, then

cycling to other logical faces before accepting.

408 |Chapter 16 Assembling Parts

The corresponding faces of the HEXBOLT and PLIERT parts are mate

constrained.

NOTE The DOF symbol is useful during constraining but has been turned off

for clarity in the illustrations.

3Use AMMATE to constrain HEXBOLT to the bolt hole on PLIERT along their

axes, following the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select the end of the HEXBOLT (3)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Select second set of geometry: Select the bolt hole of PLIERT (4)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

mated planes

Assembling Parts |409

In addition to a mate constraint on the faces of the bolt head and pliers, the

HEXBOLT and the PLIERT bolt hole are constrained along their axes.

4Examine the DOF symbol.

It should show that only the rotational degree of freedom remains unsolved.

In this case, it does not need to be solved.

You could use the insert constraint to solve the same degrees of freedom as

the two mate constraints. By choosing the faces of HEXBOLT and PLIERT, the

parts would be aligned on their axes and mate constrained on their corre-

sponding faces.

NOTE To make part selections easier, use MOVE to reposition a constrained

part. The part will automatically move back to its constrained position once you

have added a new assembly constraint.

mated lines

410 |Chapter 16 Assembling Parts

To mate to a grounded part

1Turn on the DOF symbol for PLIERB.

Browser Right-click PLIERB_1 and choose DOF Symbol.

The DOF symbol is represented by a number within a circle, indicating that

it has no degrees of freedom. Because it is the first part created in the assem-

bly drawing, PLIERB becomes the grounded part. As you apply assembly con-

straints, the grounded part remains stationary. If you move the grounded

part, all parts constrained to it also move.

2Mate the PLIERB and PLIERT parts, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select the inside face of PLIERB (5)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Enter a to highlight the face

First set = Plane

Enter an option [Clear/aXis/Point/Flip/cYcle] <accEpt>:

Enter y to cycle to the next face, or press ENTER

3Select the second set of geometry to complete the mate constraint.

Select second set of geometry: Select the inside face of PLIERT (6)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>:

Enter a to highlight the face

Second set = Plane

Enter an option [Clear/aXis/Point/Next/Flip/cYcle] <accEpt>:

Enter y to cycle to the inside face, or press ENTER

Enter offset <0.0000>: Press ENTER

Assembling Parts |411

The two parts of the pliers body are now plane mated on corresponding faces.

To mate parts on their axes

1Mate the HEXBOLT part to the PLIERB part along their axes, responding to

the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select the bolt hole of PLIERT (7)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Select second set of geometry: Select the bolt hole of PLIERB (8)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

The PLIERB and PLIERT parts are line mated along the axes of the holes, and

the bolt passes through both parts.

mated planes

412 |Chapter 16 Assembling Parts

2Mate the HEXNUT to the face of the pliers, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select the top face of HEXNUT (9)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Enter a to highlight the face

First set = Plane

Enter an option [Clear/aXis/Point/Next/Flip/cYcle] <accEpt>:

Enter n to highlight the top face, if necessary, and then press ENTER

3Select the second set of geometry to complete the mate constraint.

Select second set of geometry: Select the outside face of PLIERB (10)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>:

Enter a to highlight the face

Second set = Plane

Enter an option [Clear/aXis/Point/Next/Flip/cYcle] <accEpt>:

Enter f to flip the direction arrow away from PLIERB, and then press ENTER

Enter offset <0.0000>: Press ENTER

HEXNUT is plane mated to the face of PLIERB.

Assembling Parts |413

4Mate the nut to the bolt along their axes to pass the bolt through the hole.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select the bolt hole on HEXNUT (11)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Select second set of geometry: Select the bolt hole on PLIERB (12)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

The parts are now assembled.

5Check that the parts are assembled correctly.

Desktop Menu View ➤ 3D Views ➤ Top

6Return to the isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

Save your file.

414 |Chapter 16 Assembling Parts

Using the Desktop Browser

As you assemble parts, a graphical hierarchy of the assembly is illustrated in

the Desktop Browser. Each 3D constraint applied to an assembly component

is listed below the component. You can tell at a glance which constraints

exist between which components, because the other component to which

the constraint applies is shown in the hierarchy. When you hold the cursor

over a constraint, feature, or tweak in the Browser, a tooltip displays perti-

nent data. For instance, the offset value is displayed for a mate constraint,

type and size data is displayed for a hole feature, and a distance value is dis-

played for a tweak. In scenes, explosion factors are displayed in a tooltip.

Using the Browser, you can both edit the hierarchy of an assembly and move

components into an empty assembly file. To restructure the hierarchy, you

either drag components, or use the cut and paste options in cases where the

Browser display is long and detailed. The design constraints for restructured

assemblies remain unchanged.

For more information about using in the Browser to restructure assemblies,

see “Restructuring Assemblies” on page 504 in chapter 18.

You can use the Browser to add, change, delete, and copy, and to localize and

externalize component definitions. To see how this works, edit the mate con-

straint on the hexbolt. Then change the color of a part, make copies, and

externalize a component definition.

To edit an assembly constraint with the Browser

1Change your display to two viewports.

Command 2

2Zoom to enlarge the hexbolt.

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

3In the Browser, right-click the Mate pl/pl constraint under HEXBOLT_1, and

choose Edit.

Assembling Parts |415

4In the Edit 3D Constraint dialog box, change the offset to 0.05. Click the

Update icon.

You can see the hexbolt offset the new distance. Experiment with changing

the offset again, using the Update icon to see the change.

Choose Cancel. The original offset distance of 0.00 remains in effect.

You can easily edit values and see them take effect without permanently

changing your assembly. Use the Update icon in the Edit 3D Constraint dia-

log box to see the change, and then choose Cancel to return to the original

values.

To copy a part with the Browser

1Collapse the assembly tree to better visualize the changes you make.

Browser Right-click S_PLIER and choose Browser Node ➤ Collapse.

2Make a copy of HEXBOLT_1.

Browser Right-click HEXBOLT_1 and choose Copy.

3Place one or more copies near the pliers, and then press ENTER.

You can see the new hexbolts listed in the Browser hierarchy, each numbered

in the sequence you added them.

416 |Chapter 16 Assembling Parts

To change the color of a part with the Browser

1Activate HEXBOLT_1.

Browser Right-click HEXBOLT_1 and choose Activate Part.

2Open the Select Color dialog box to change the color of HEXBOLT_1.

Browser Right-click HEXBOLT_1 and choose Properties ➤ Color.

3In the Select Color dialog box, select Red, and then choose OK.

This color applies to all instances of HEXBOLT.

4Activate the assembly to view the changed color

Browser Right-click S_PLIER and choose Activate Assembly.

Next, change the bolt color to the original and remove the experimental copies.

5Activate HEXBOLT_1

Browser Right-click HEXBOLT_1 and choose Activate Part.

6Open the Select Color dialog box to change the color of HEXBOLT_1 back to

white.

Browser Right-click HEXBOLT_1 and choose Properties ➤ Color.

7In the Select Color dialog box, select White, and then choose OK.

8Activate PLIERB_1 to return the bolts back to their original color.

Browser Right-click PLIERB_1 and choose Activate Part.

To delete part copies with the Browser

1Delete the HEXBOLT copy.

Browser Right-click HEXBOLT_2 and choose Delete.

2Repeat for the other copies if needed.

Your experimental copies are no longer visible in the Browser assembly

hierarchy.

Getting Information from Assemblies |417

To localize an external part with the Browser

1Localize the external parts HEXBOLT_1 and HEXBOLT_3.

Browser Press CTRL and select HEXBOLT_1 and HEXBOLT_3.

Right-click the selected parts and choose All Instances ➤

Localize.

This shortcut method enables you to localize and externalize parts without

opening the Assembly Catalog. When you select a local part in the Browser,

the externalize option is available.

For more information about local and external assembly components, see

“Creating Local and External Parts” on page 481.

You are now ready to check the assembly for mass properties and interference.

Getting Information from Assemblies

Now that all the parts are constrained, you can check for interference and

obtain mass property information for some of the parts or the entire assembly.

Checking for interference between two or more parts in the assembly can detect

design problems before manufacturing starts. Mass property information can

tell you whether the dimensions or materials of a part need to be changed to

achieve the desired results. This analysis is critical for making decisions early in

the design phase that can prevent manufacturing problems later.

Checking for Interference

An interference analysis detects interference between two parts or all parts.

You can move up or down the assembly tree, selecting parts as you proceed.

Next, you will perform an interference analysis on the entire pliers assembly.

418 |Chapter 16 Assembling Parts

To check for interference

1Change to one viewport.

Command 1

2Change to the right isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

3Use AMINTERFERE to check for interference, responding to the prompts.

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

Check Interference.

Nested part or subassembly selection? [Yes/No] <No>: Press ENTER

Select first set of parts or subassemblies: Select the PLIERT part (1)

Select first set of parts or subassemblies: Press ENTER

Select second set of parts or subassemblies: Select the HEXBOLT part (2)

Select second set of parts or subassemblies: Press ENTER

Parts/subassemblies do not interfere.

If you have trouble selecting a part, use the Browser to change its color.

4Check for interference between the PLIERB and HEXBOLT parts.

The parts should show no interference.

Next, you will calculate the mass properties for the assembly.

Calculating Mass Properties

Once an assembly is completed, you can calculate its mass properties. Toler-

ance values control the accuracy of the mass property information. The

material types can be different for each part, resulting in accurate mass prop-

erty values no matter how complex the assembly.

Getting Information from Assemblies |419

To calculate mass properties

1Use AMASSMPROP to select the parts for the mass properties calculation, fol-

lowing the prompts, and open the Assembly Mass Properties dialog box.

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

Mass Properties.

Enter an option (parts/subassemblies) [Name/Select] <Select>: Press ENTER

Select part and subassembly instances: Select PLIERB

Select part and subassembly instances: Press ENTER

2In the Assembly Mass Properties dialog box, select the Setup tab and specify:

Input units: US Customary (in, lbm)

Output units: US Customary (in, lbm)

Coordinate system: User coordinate system (UCS)

Display Precision: Enter 2.0

Part List: Select PLIERB

Materials available: Select Mild_Steel.

420 |Chapter 16 Assembling Parts

3Select the Results tab. The results window for PLIERB remains empty until

you calculate the results.

4Choose Calculate. Message dialogs appear warning that density is not speci-

fied for the other parts in the assembly. Choose OK to proceed.

Mass properties are calculated according to the values you set.

Choose Done.

NOTE You can save mass properties calculations to a file to use in design analysis,

and you can export the results.

Next, you create scenes of the assembly.

Creating Assembly Scenes

Now that you have instanced the parts and applied the assembly constraints,

you can create and lay out assembly scenes. A scene is an exploded view that

separates the parts of an assembly or subassembly to show how they fit

together. You can create a scene quickly; it updates automatically every time

you change the assembly. The separation of the parts is based on an explo-

sion factor you set and the assembly constraints you used to position the

parts. You can create multiple exploded scenes of the same assembly and save

them for later use.

Creating Assembly Scenes |421

Assembly trails indicate the path of the assembly explosion. With the excep-

tion of the grounded part, assembly trails can be created for all parts. When

you create assembly trails, a new layer is automatically created for them. You

can automatically create trails when you create tweaks.

First, you set an explosion factor and then create an exploded assembly

scene. Then you add trails to show how parts are assembled. From a scene,

you create drawing views.

To create an exploded view

1Use AMNEW to create a new scene.

Context Menu In the graphics area, right-click and choose New Scene.

The Create Scene dialog box is displayed.

2In the Create Scene dialog box, specify:

Target Assembly: S_PLIER

Scene Name: SCENE1

Auto Explode: Scene Explosion Factor: 1.5

Synchronize Visibility with Target Assembly: Select the check box

Choose OK.

The exploded assembly scene is displayed. Its name is shown below the com-

mand line. The Browser shows all parts in the scene.

422 |Chapter 16 Assembling Parts

Next, align the exploded parts in the assembly scene. You can tweak the posi-

tion and orientation of individual parts or rotate them for better visibility.

In the Browser, verify that the Scene tab is selected. Unless the scene is acti-

vated, you cannot tweak parts to adjust their position or add trails to show

how they are assembled.

To align scene parts

1Use AMTWEAK to move the HEXNUT part closer to the other parts, respond-

ing to the prompt.

Context Menu In the graphics area, right-click and choose New Tweak.

Select part or subassembly to tweak: Select HEXNUT (1)

2In the Power Manipulator dialog box, on the General tab, verify that Place

Objects (ALT) is selected.

Choose Done.

The Power Manipulator dialog box is displayed automatically only the first

time you create a new tweak. After that, to access the Power Manipulator

dialog box, right-click the Power Manipulator symbol on your screen, and

select Options.

3Continue on the command line.

Select handle or Geometry

[undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>:

Enter z

Enter tweak distance [Rotate]<1.0000>: Enter .25

Select handle or Geometry

[undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>:

Press ENTER.

Creating Assembly Scenes |423

The HEXNUT position is tweaked by the specified distance.

NOTE The grounded part of an assembly or subassembly cannot be tweaked.

Its position is fixed.

4Use AMTRAIL to show the direction of the explosion and tweak paths,

responding to the prompt.

Context Menu In the graphics area, right-click and choose New Trail.

Select reference point on part or subassembly: Select the end of HEXBOLT (1)

424 |Chapter 16 Assembling Parts

5In the Trail Offsets dialog box, specify:

Offset at Current Position: Distance: Enter 1

Over Shoot: Select the option

Offset at Assembled Position: Distance: Enter 1

Over Shoot: Select the option

Choose OK.

The assembly trail for HEXBOLT is displayed.

6Apply assembly trails to the PLIERB and HEXNUT parts, responding to the

prompt.

Context Menu In the graphics area, right-click and choose New Trail.

Select reference point on part or subassembly:

Select the outside hole of HEXNUT (2)

Creating Assembly Drawing Views |425

7In the Trail Offsets dialog box, specify:

Offset at Current Position: Distance: Enter 1

Over Shoot: Select the option

Offset at Assembled Position: Distance: Enter 1

Over Shoot: Select the option

Choose OK.

The assembly drawing automatically updates the current scene to reflect the

tweaks and assembly trails.

Save your file. Choose OK in the External Part Save dialog box to bring all

parts up to date.

Next, you create drawing views of the assembly scene.

Creating Assembly Drawing Views

After you complete the assembly model and the scene, you can create 2D

orthogonal views or 3D isometric and exploded views of the entire assembly.

Then you add reference dimensions.

You can set up as many drawing layouts as you need to document your

design. Because this assembly is small, you create only one layout.

Before creating the base view of the pliers assembly, modify a plotter setup to

include a custom paper size. Then set up the drawing layout to arrange the

drawing views on paper.

426 |Chapter 16 Assembling Parts

To add a custom paper size to a plotter setup

1Use AMMODE to switch to Drawing mode.

Browser Choose the Drawing tab.

2Add a custom paper size to an existing plotter.

Browser Right-click Layout1 and choose Page Setup.

3In the Page Setup dialog box, select the Plot Device tab and specify:

Name: DWF Classic.pc3

Creating Assembly Drawing Views |427

4Choose Properties.

5In the Plotter Configuration Editor dialog box, expand User-Defined Paper

Sizes and Calibration. Select Custom Paper Sizes and choose Add.

6Use the Custom Paper Size Wizard to define a paper size of 18 x 12 inches

with no indents. Choose Next until the setup is finished.

7Save your changes to the DWF Classic.pc3 file.

Next, you set up the drawing layout and insert a title block.

428 |Chapter 16 Assembling Parts

To set up a drawing layout

1In the Page Setup dialog box, select the Layout Settings tab and specify:

Paper Size: User 1 (18.00 x 12.00 inches)

Plot Scale: 1:1

Choose OK.

2Use MVSETUP to insert a title block.

Browser Right-click Layout1 and choose Insert Title Block.

In the AutoCAD text window, respond to the prompt as follows:

Enter number of title block to load or [Add/Delete/Redisplay]: Enter 8

3Continue on the command line.

Create a drawing named ansi_b.dwg? <Y>: Enter n

Enter an option [Align/Create/Scale viewports/Options/Title block/Undo]:

Press ENTER

The title block is inserted into the drawing.

4Use MOVE to center the title block in the layout, responding to the prompts.

Desktop Menu Modify ➤ Move

Select objects: Select the title block

Select objects: Press ENTER

Specify base point or displacement: Specify a point

Specify second point of displacement or <use first point as displacement>:

Specify another point

Next, define drawing views to display the assembly.

Creating Assembly Drawing Views |429

To create a base assembly drawing view

1Use AMDWGVIEW to create a base view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

Type: Base

Data Set: Scene: SCENE1

Choose OK.

2Respond to the prompts as follows:

Select a planar face, work plane, or [Ucs/View/worldXy/worldYz/worldZx]:

Enter z

Select work axis or straight edge [worldX/worldY/worldZ]: Enter x

Adjust orientation [Flip/Rotate] <accEpt>: Press ENTER

Specify location of base view: Specify a point

Specify location of base view: Specify another point or press ENTER

430 |Chapter 16 Assembling Parts

The base drawing view is displayed.

Next, create an isometric view of the assembly.

To create an isometric assembly drawing view

1Create an isometric view.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

View Type: Iso

In the Hidden Lines tab, specify:

Calculate Hidden Lines: Clear the check box

Choose OK.

Creating Assembly Drawing Views |431

2Respond to the prompts as follows:

Select parent view: Specify the base view

Specify location for isometric view: Specify a point to place the isometric view

Specify location for isometric view: Specify another point or press ENTER

Examine the Browser. The views are nested under a Scene icon which is

nested under Layout1.

Save your file.

Now you can add reference dimensions, which can be moved, frozen, and

thawed in each drawing view. Reference dimensions are not parametric, but

they update when the model changes.

432 |Chapter 16 Assembling Parts

To add a reference dimension

1Zoom in to enlarge the area you want to dimension.

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

2Use AMREFDIM to add a reference dimension, following the prompts.

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

Dimension.

Select first object: Select the endpoint of the pliers (1)

Select second object or place dimension: Select the bolt (2)

Specify dimension placement: Specify a point above the pliers

Specify placement point or [Undo/Hor/Ver/Align/Par/aNgle/Ord/reF/Basic]:

Press ENTER

Select first object: Press ENTER

The reference dimension is added to the current view.

Save your file.

Now that you have created drawing views, you edit a part and automatically

update the drawing views.

Editing Assemblies |433

Editing Assemblies

Design or specification changes require most assembly designs to be docu-

mented and edited frequently. You modify parts, rearrange parts and features

in the hierarchy of the assembly tree, and change or delete constraints.

Because the parts and assembly are parametric, changes are fast and updates

are immediate.

Editing an external part definition automatically changes the assembly

model wherever the part is instanced.

Editing External Subassemblies

The process for editing external subassemblies and combined parts is much

like the one for editing external parts. To begin, you activate the subassembly

by double-clicking it in the Browser or entering information on the com-

mand line. When external files are active in the ref-edit state, they are not

available for simultaneous use by others.

The active subassembly retains its color on the screen, while other geometry

is dimmed. Non-active instances of the active subassembly dim one-half as

much. This indicates which instance is active and reflects all of the instances

that will be updated as a result of the change.

When active, you can edit the subassembly. The editing operations take place

as if the active subassembly was an open document. You alter subassemblies

by adding or removing components, changing constraints, adding new fea-

tures, or restructuring the assembly. Newly created non-part based geometry

such as surfaces and wires are created in the master assembly until made part

of a component.

You can save your changes to an external subassembly file in several ways.

■Use an option in AMUPDATE to commit the changes to the external file.

■Activate a part or subassembly that is contained in another file and, in the

resulting dialog box, commit to changes.

■Activate another subassembly that is external to the active subassembly.

■Save the assembly and choose either to not save changes or to save the

pending changes to any external files.

434 |Chapter 16 Assembling Parts

Editing External Parts

To update all instances of a part in assemblies, you need to edit the original

part. You alter part features by changing dimensions, changing the

constraints, or adding new features. The changes take effect in the assembly.

In this tutorial, you edit the external PLIERT part from within your assembly

drawing. This is called editing in place. In the following steps, you add another

hole to the PLIERT part, and modify assembly constraints.

To edit an external part in place

1Use AMMODE to return to Model mode.

Browser Select the Model tab.

2Use AMACTIVATE to activate the PLIERT part.

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

Activate Part.

The inactive parts are grayed out in the Desktop Browser, and dimmed on

screen.

By dimming the inactive parts, it is easier for you to work on the active exter-

nal part without moving other parts.

3Notice the red lock preceding the PLIERT icon in the browser. This indicates

that the file has been locked and cannot be modified by another user.

NOTE For clarity, the visibility of the other parts has been turned off in this sec-

tion. If you prefer, turn off the visibility of PLIERB, HEXBOLT, and HEXNUT before

you activate PLIERT.

Editing Assemblies |435

4Zoom in on PLIERT.

5Use AMSKPLN to create a new sketch plane, responding to the prompts.

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

Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Make sure the front face of the part is highlighted, and press ENTER

Plane=Parametric

Select edge to align X axis or [Z-flip/Rotate] <accept>:

Make sure the UCS icon is upright and the Z axis points away from the part,

and then press ENTER

The sketch plane is defined on the front face of the pliers. Now, create the

new slip hole to increase movement of the slip pliers.

436 |Chapter 16 Assembling Parts

To create a new feature on an external part

1Use CIRCLE to place a new hole, responding to the prompts.

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

➤ Circle.

CIRCLE Specify center point for circle or [3P/2P/Ttr (tan tan radius)]:

Select a point near the existing hole

Specify radius of circle or [Diameter]:

Draw a circle approximately the same size as the other hole

2Use AMPROFILE to solve the sketch.

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

Single Profile.

Mechanical Desktop indicates that three dimensions are required to fully

constrain the sketch.

3Use AMPARDIM to add the parametric dimensions, responding to the

prompts. Zoom in as needed to magnify the holes.

Editing Assemblies |437

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

New Dimension.

Select first object: Select the circle (1)

Select second object or place dimension:

Specify a point for the location of the dimension (2)

Enter dimension value or [Undo/Radius/Ordinate/Placement point]

<0.2003>: Enter .22

Solved underconstrained sketch requiring 2 dimensions or constraints.

Select first object: Select the circle (1)

Select second object or place dimension: Select the existing extruded hole (3)

Specify dimension placement: Specify a point for the location of dimension (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.0454>: Enter 0

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Select the circle (1)

Select second object or place dimension: Select the top line on PLIERT (5)

Specify dimension placement: Specify a point for the location of dimension (6)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.5093>: Enter .45

Solved fully constrained sketch.

Select first object: Press ENTER

The circle is now constrained.

4Use AMEXTRUDE to extrude the new hole through the pliers.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Termination: Through

Operation: Cut

438 |Chapter 16 Assembling Parts

Choose OK to exit the dialog box.

The new hole is extruded, and its position is constrained to the original hole.

Save your file.

5The External Part Save dialog box indicates a change in the PLIERT drawing.

Choose OK to save the changes you have made.

The Browser returns to normal. The inactive parts are no longer dimmed, and

the assembly reflects the new PLIERT part.

Editing Assembly Constraints

Using the Browser, you can selectively delete, edit, and add constraints to

realign or change relationships of parts.

Use MOVE to reposition the parts as you edit and add constraints. If you do

not want the parts to reassemble throughout editing, set AMAUTOASSEMBLE

to 0 (off). To reassemble parts after you add a constraint, select the Update

icon on the Desktop Browser.

new bolt hole

Editing Assemblies |439

To delete an assembly constraint

1In the Desktop Browser, click the plus sign on PLIERB_1 to expand the hier-

archy. Select the Assembly filter at the bottom of the Browser to filter out all

information except the assembly constraints.

2In the Browser, click the plus sign on HEXBOLT_1 to expand the hierarchy.

Right-click the Mate ln/ln constraint of HEXBOLT_1, and choose Delete.

3Delete the Mate pl/pl constraints of HEXBOLT_1.

4Delete constraints for PLIERB, PLIERT, and HEXNUT.

5Use MOVE to separate the parts to apply the new constraints.

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

Move.

Next, you apply new assembly constraints. You use an insert constraint to

align HEXBOLT to the new hole along their axes while mating the face of

PLIERT and the corresponding face of the bolt head.

Use the DOF symbol to illustrate how many rigid body degrees of freedom

are eliminated for each part.

440 |Chapter 16 Assembling Parts

To apply an assembly constraint

1Use AMINSERT to constrain PLIERT_1 and HEXBOLT_1, responding to the

prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Select the new bolt hole of PLIERT (1)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward HEXBOLT, and press ENTER

Select second circular edge: Select the bolt shaft near the head (2)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward PLIERT, and press ENTER

Enter offset <0.0000>: Press ENTER

The bolt is now inserted through the new hole.

Now you can align the new hole in PLIERT and the corresponding hole in

PLIERB along their axes.

Editing Assemblies |441

2Use AMINSERT to constrain PLIERB and PLIERT, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Select the new bolt hole of PLIERT (3)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward PLIERB and press ENTER

Select second circular edge: Select the hole on the inner face of PLIERB (4)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward PLIERT and press ENTER

Enter offset <0.0000>: Press ENTER

The PLIERB and PLIERT parts are constrained to each other on the inside face

and along the axes of the lower hole of PLIERT and the single hole of PLIERB.

Transactional degrees of freedom are solved. In this case, you want to allow

the pliers and hexbolt to rotate on the axes, so you leave the rotational

degree of freedom unsolved.

3Use AMINSERT to constrain the facing planes of HEXNUT and PLIERB at the

bolt holes, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

442 |Chapter 16 Assembling Parts

Move parts so you can easily see selection points.

Select first circular edge: Select the bolt hole on PLIERB (5)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward HEXNUT and press ENTER

Select second circular edge: Select the hole on HEXNUT (6)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow toward PLIERB and press ENTER

Enter offset <0.0000>: Press ENTER

The PLIERB and PLIERT parts are constrained on their facing planes. The bolt

passes through both parts, and the holes and bolt shaft are aligned along

their axes.

4Check that the parts are assembled correctly.

Desktop Menu View ➤ 3D Views ➤ Top

5Return to the isometric view.

Desktop Menu View ➤ 3DViews ➤ Front Right Isometric

Save your file.

443

In This Chapter 17

Combining Parts

This Autodesk® Mechanical Desktop® tutorial builds on

the part and assembly modeling techniques that you

learned in previous chapters. In this chapter, you create

a part and combine toolbodies with it, using parametric

Boolean operations such as cut, join, and intersect, to

construct a single part. You also learn how the display of

complex parts is organized in the Desktop Browser.

In this tutorial, you work in Single Part mode to create a

complex part to be used as a component for an off-road

vehicle. You build the part by combining several

toolbodies with a base part.

■Working in Single Part mode

■Changing part definitions

■Combining and intersecting

parts

■Creating toolbody and nested

toolbody parts

■Reducing weight parametrically

444 |Chapter 17 Combining Parts

Key Terms

Te r m Definition

base part The active part where toolbody parts are aligned and subsequently combined.

Boolean modeling A solid modeling technique in which two solids are combined to form one

resulting solid. Boolean operations include cut, join, and intersect. Cut subtracts

the volume of one solid from the other. Join unites two solid volumes. Intersect

leaves only the volume shared by the two solids.

combine feature A parametric feature resulting from the union, subtraction, or intersection of a

base part with a toolbody part.

complex part A parametric part containing one or more parametric parts as features.

Part Catalog The means of attaching and cataloging local and external parts in the Part

Modeling environment. Use the All and External tabs to specify contents, which

can be instanced, copied, renamed, replaced, externalized, removed, localized

and sorted.

part definition Contains information about a part, including its name, geometric data,

specifications, and parameters. If you instance a part multiple times, the

assembly contains only one definition of the part.

part instance A copy of the part definition. The part instance is inserted into the drawing and

is visible as a solid object on the graphics screen. When a part definition is

changed, so are all of its instances. Part instance names are displayed in the

Desktop Browser.

toolbody A part that is aligned with the base part and then used to join, intersect, or cut

volume from the base part. In the Part Modeling environment, a part created

after a base part, that automatically becomes an unconsumed toolbody.

toolbody consumption When a toolbody part is combined with a base part, the toolbody part instance

disappears from the graphics screen and appears as a new combine feature of

the base part in the Desktop Browser.

toolbody rollback A special option of the AMEDITFEAT command that enables you to change a

toolbody part after it has been consumed as a combine feature.

Basic Concepts of Combining Parts |445

Basic Concepts of Combining Parts

In Mechanical Desktop® the parametric Boolean capabilities for combining

parts provide a combination of modeling flexibility and convenience. To

combine two parts, you identify which part you want to use as the base part

and make it active. Then, you position the toolbody part on the base part,

using the MOVE or ROTATE command or assembly constraints. You use

AMCOMBINE to cut, join, or intersect the toolbody part with the base part.

You can combine as many toolbodies with a base part as you like, but the

base part and the toolbody must be instances of different parts. In other

words, you cannot combine a part with an instance of itself.

Because the end result is a single part, you can create combined parts in Single

Part mode. If you place more than one part in a part file, the additional parts

automatically become unconsumed toolbodies.

To combine a toolbody with a base part in an Assembly file, both parts must

exist in the same active assembly.

When you create a complex part, the complete definitions of the toolbodies

are stored in the assembly model file. To avoid creating files that are unnec-

essarily complex, use simple parts as toolbodies. In the following illustration,

the highlighted parts are used to cut a slot. The resultant parts look identical,

but the one created with the complex toolbody part consumes more disk

space. Feature editing operations, such as cutting a slot, take longer.

With Mechanical Desktop, you can create toolbody parts that contain other

toolbody parts. These are called nested toolbodies. However, you may be able

to achieve the same result without nesting toolbodies.

simple toolbody partcomplex toolbody part

446 |Chapter 17 Combining Parts

In the following illustration, the appearance of the part is the same, whether

or not you nest the toolbodies, but the part displayed in the Desktop Browser

on the left is easier to manage and has a less cumbersome display than the

one in the Browser on the right.

To edit CAM_1, on the left, you need to expose only one toolbody. Nested

toolbody parts, like those in the example on the right, usually have more com-

plex constraint systems and require multiple part updates after modification.

Working in Single Part Mode

If you are creating combined parts, you can work in Single Part mode. In a

single part file, you can only have one part definition, but you can work with

more than one part. If you create or externally reference more than one part,

the additional parts become unconsumed toolbodies that you can use to

combine with the first part created in the drawing.

In the Browser above, TOOLBODY1 and TOOLBODY3 are unconsumed.

TOOLBODY2 is consumed, since it has been combined with TOOLBODY1.

Creating Parts |447

Creating Parts

In this tutorial, you create a chassis suspension component for an off-road

recreational vehicle. The part is an axle spacer. You create most of the features

of this part by first creating the basic shape. Then, you create separate parts

that you use as tools to add additional features to the basic shape.

Open the file spacer.dwg in the desktop\tutorial folder. This drawing contains

a fully constrained profile sketch of the basic shape of the axle spacer.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

To create an axle spacer, you begin by extruding the part. First, review the

constraint system for this sketch.

To extrude a part

1Use AMSHOWCON to check the existing constraints.

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

Constraints ➤ Show Constraints.

2Choose All.

Each arc uses the geometric constraints tangent and radius. The upper and

lower outside arcs are aligned using the X Value constraint, and the left and

right outside arcs use the Y Value constraint.

3Press ENTER.

Because this part is cast aluminum, you must extrude it with a draft angle.

Expand the part hierarchy by clicking the plus icon next to the part name in

the Desktop Browser. The Browser shows an existing part, SPACER, that con-

tains an unconsumed profile.

4In the Desktop Browser, expand SPACER. Under SPACER, select the Profile1

icon. The sketch is highlighted.

448 |Chapter 17 Combining Parts

5Use VIEW to change your viewpoint to a previously saved view.

Desktop Menu View ➤ Named Views

In the View dialog box, select SPACER_VIEW, and choose Set Current.

Choose OK.

6Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Distance: Enter 64

Draft Angle: Enter -2

Termination: Type: MidPlane

Choose OK.

Next, adjust the system settings so that you can hide the silhouette edges of

your part.

To hide silhouette edges

1Set the AutoCAD system variable that controls the display of silhouette

edges, responding to the prompt.

Command DISPSILH

Enter new value for DISPSILH <0>: Enter 1

Creating Toolbody Part Definitions |449

2Use HIDE to hide the silhouette edges.

Desktop Menu View ➤ Hide

The spacer has a boss at the bottom and a relief at the top. Next, you use two

part definitions to construct the toolbody parts. You combine those toolbody

parts with the spacer to create the boss and relief.

Creating Toolbody Part Definitions

The shapes of the new toolbody parts are similar to the shape of the spacer

profile. The easiest way to create the toolbodies is to use copies of the spacer

to construct the new toolbody parts. Because you cannot copy a base part

definition in the Part Modeling environment, you use the Part Catalog to

attach a copy of the part to the current drawing as a toolbody definition.

To externally reference a toolbody definition

1Change the display back to wireframe.

Desktop Menu View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen

2Use AMCATALOG to attach the boss.dwg file as a toolbody. This drawing is a

duplicate of the spacer.

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

Menu ➤ Catalog.

In the Part Catalog, choose the External tab and select Return to Dialog.

Right-click in Directories, and choose Add Directory.

3In the Browse for Folder dialog box, select the folder containing your tutorial

drawings. Choose OK.

450 |Chapter 17 Combining Parts

Because you are working in the Part Modeling environment, Mechanical

Desktop filters the part and assembly drawings in your working directory and

lists only the part files. A thumbnail preview of the part icon precedes the

drawing name. If a part file does not contain features, it is preceded by a red

AutoCAD icon.

4In the Part Catalog, right-click BOSS and choose Attach.

5Respond to the prompts as follows:

Specify new insertion point: Specify a point above and to the right of the spacer

Specify insertion point for another instance or <continue>: Press ENTER

Creating Toolbody Part Definitions |451

The Part Catalog is displayed.

6Choose the All tab. The boss toolbody is listed in External Toolbody Definitions.

Choose OK.

Next, localize and make a copy of the boss toolbody, to create a definition for

the relief toolbody using the Browser shortcut methods.

To localize an external toolbody and copy its definition

1Localize external toolbody BOSS_1.

Browser Right-click BOSS_1, and choose All Instances ➤ Localize.

The boss toolbody is localized.

Next, copy the boss toolbody definition to create a relief toolbody.

2Copy the boss toolbody

Browser Right-click BOSS_1, and choose Show Definition.

3In the Part Catalog, choose the All tab. The boss toolbody is listed in Local Tool-

body Definitions.

Right-click BOSS, and choose Copy Definition.

452 |Chapter 17 Combining Parts

4The Copy Definition dialog box is displayed. In New Definition Name , enter

relief.

Choose OK.

5Position the instance of the relief toolbody definition to the right of the boss

toolbody, and press ENTER.

The new relief toolbody definition is listed under Local Toolbody Definitions

in the Part Catalog. Choose OK.

Examine the Browser. It contains one part and two unconsumed toolbodies.

Save your file.

Creating Toolbody Part Definitions |453

The boss toolbody on the completed spacer follows the profile of the spacer,

but its corners are rounded. The next step is to combine a cylinder with the

boss toolbody.

In the Browser, right-click BOSS_1 and choose Activate Toolbody. Right-click

BOSS_1 again, and choose Zoom To.

To create a cylinder toolbody to combine with the boss toolbody

1Use AMNEW to create a new toolbody definition, responding to the prompts.

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

New Toolbody.

Enter an option [Instance/Part} <Part>: Press ENTER

Select an object or enter a new part name <TOOLBODY1>:

Enter boss_cylinder and press ENTER

The new toolbody is created, and the toolbody name is added to the Browser.

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

2Use CIRCLE to create a circle close to the boss toolbody.

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

2D Sketching ➤ Circle.

3Use AMPROFILE to create a profile from the sketch.

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

Single Profile.

4Use AMPARDIM to constrain the profile.

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

New Dimension.

boss

454 |Chapter 17 Combining Parts

5Select the circle, and enter a dimension of 86.

6Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Distance: Enter 5

Draft Angle: Enter 2

Termination: Type: Blind

Choose OK.

Next, you use assembly constraints to position the cylinder at the bottom of

the BOSS_1 toolbody. Then you use a Boolean intersect operation to combine

the two parts.

To align the cylinder with the boss toolbody, you create two mate-line con-

straints. Follow the prompts carefully, using the illustrations as your guide to

selecting the correct part edges.

To align a part with a relief toolbody

1Use AMMATE to create a mate constraint, responding to the prompts.

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

Menu ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the bottom edge of the cylinder (1)

First set = Axis, (arc)

Select first set or [Clear/Face/Point/cYcle] <accEpt>: Enter p

First set = Point, (arc)

Select first set or [Clear/aXis/fAce/cYcle] <accEpt>: Press ENTER

Creating Toolbody Part Definitions |455

Select second set of geometry: Select the arc (2)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Enter p

Second set = Point, (arc)

Select second set or [Clear/aXis/fAce/cYcle] <accEpt>: Select the arc (3)

Second set = Plane, (arc)

Enter an option [Clear/aXis/Flip/cYcle] <accEpt>: Enter x

Second set = Axis, (arc)

Select first set or [Clear/fAce/Midpoint/cYcle] <accEpt>: Enter m

Second set = Axis, (arc)

Select first set or [Clear/fAce/Midpoint/cYcle] <accEpt>: Press ENTER

Enter offset <0>: Press ENTER

The center of the cylinder is aligned with the line between the two spacer arc

centers.

456 |Chapter 17 Combining Parts

2Use MOVE to move the cylinder for easier selection, responding to the

prompts.

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

2D Sketching ➤ Move.

Select objects: Specify the cylinder

Select objects: Press ENTER

Base point or displacement: Specify a point

Second point of displacement: Specify a second point and press ENTER

3Create the second mate-line constraint, responding to the prompts.

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

Menu ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the bottom edge of the cylinder (4)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Enter p

First set = Point, (arc)

Select first set or [Clear/aXis/fAce/cYcle] <accEpt>: Press ENTER

Select second set of geometry: Select the arc (5)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Enter p

Second set = Point, (arc)

Select second set or [Clear/aXis/fAce/cYcle] <accEpt>: Select the arc (6)

Second set = Plane, (arc)

Enter an option [Clear/aXis/Flip/cYcle] <accEpt>: Enter x

Second set = Axis, (arc)

Select first set or [Clear/fAce/Midpoint/cYcle] <accEpt>: Press ENTER

Enter offset <0>: Press ENTER

Creating Toolbody Part Definitions |457

The center of the cylinder is aligned with the line between the two boss arc

centers. Together, the two mate constraints position the cylinder at the bot-

tom of the boss. The center of the cylinder is coincident with the center of

the boss.

Now, you are ready to combine the boss toolbody with the cylinder. Because

the boss toolbody will be the base part in the Boolean operation, you need to

make it active.

To create a combine feature

1Use AMACTIVATE to activate BOSS_1.

Browser In the Browser, right-click BOSS_1 and choose Activate

Toolbody.

2Use AMCOMBINE to combine the toolbody and the cylinder, responding to

the prompts.

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

Placed Features ➤ Combine.

Enter parametric boolean operation [Cut/Intersect/Join] <Cut>: Enter i

Select part (toolbody) to use for intersecting: Select the cylinder

Save your file.

458 |Chapter 17 Combining Parts

Working with Combine Features

The Desktop Browser now shows that the boss toolbody has a combine fea-

ture. The boss cylinder is a toolbody in the combine feature.

The next step is to constrain and combine the boss toolbody with the spacer.

To constrain and combine a toolbody to the base part

1Use AMACTIVATE to activate the SPACER.

Browser In the Browser, right-click SPACER and choose Activate

Part.

2Use AMMATE to apply a mate constraint to the boss toolbody and the spacer,

responding to the prompts.

Desktop Menu Toolbody ➤ 3D Constraints ➤ Mate.

Select first set of geometry: Select the top edge of the boss toolbody (1)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Enter p

First set = Point, (arc)

Select first set or [Clear/aXis/fAce/cYcle] <accEpt>:

Select the opposite edge of the boss toolbody (2)

First set = Plane, (arc)

Enter an option [Clear/aXis/Flip/cYcle] <accEpt>: Enter x

First set = Axis, (arc)

Select first set or [Clear/fAce/Midpoint/cYcle] <accEpt>: Press ENTER

Working with Combine Features |459

Select second set of geometry: Select the bottom right edge of the spacer (3)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Enter p

Second set = Point, (arc)

Select second set or [Clear/aXis/fAce/cYcle] <accEpt>:

Select the opposite edge of the spacer (4)

Second set = Plane, (arc)

Enter an option [Clear/aXis/Flip/cYcle] <accEpt>: Enter x

Second set = Axis, (arc)

Select second set or [Clear/fAce/Midpoint/cYcle] <accEpt>: Press ENTER

Enter offset <0>: Press ENTER

3Move the boss toolbody, and repeat step 2 for the second constraint. Be sure

to select the top edges of the boss toolbody.

460 |Chapter 17 Combining Parts

The boss toolbody is now aligned with the spacer.

4Use AMCOMBINE to combine the spacer and the boss toolbody, responding to

the prompts.

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

Placed Features ➤ Combine.

Enter parametric boolean operation [Cut/Intersect/Join] <Cut>: Enter j

Select part (toolbody) to be joined: Select the boss toolbody

Save your file.

Creating Relief Toolbodies |461

Creating Relief Toolbodies

The Desktop Browser now shows a nested toolbody construction. The boss

cylinder toolbody is a combine feature of the boss toolbody, and the boss

toolbody is a combine feature of the spacer.

Next, you create the relief toolbody, to cut material from the spacer.

In the Browser, right-click RELIEF_1 and choose Zoom To.

To add a new toolbody name in the Browser

1Use AMNEW to create a new toolbody called RELIEF_CYLINDER, responding

to the prompts.

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

Menu ➤ Toolbody ➤ New Toolbody.

Enter an option [Instance/Part} <Part>: Press ENTER

Select an object or enter new part name <TOOLBODY1>:

Enter relief_cylinder and press ENTER

The new part name is added to the Desktop Browser.

462 |Chapter 17 Combining Parts

To create a new part

1Use CIRCLE to draw a circle near RELIEF_1.

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

2D Sketching ➤ Circle.

2Use AMPROFILE to create a profile from the sketch.

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

Single Profile.

3Use AMPARDIM to constrain the profile.

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

New Dimension.

Select the circle, and enter a dimension of 90.

4Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion Feature dialog box specify:

Termination: Blind

Distance: Enter 10

Draft Angle: Enter 2

Choose OK.

Next, you position the cylinder at the top of RELIEF_1, using assembly con-

straints just as you did for the boss cylinder. As you select geometry for the

constraints, be sure to select the top edges of both the relief cylinder and the

relief toolbody.

To constrain the toolbodies

1Use AMMATE for two mate constraints to align the toolbodies.

Desktop Menu In the Desktop Menu, choose Toolbody Menu ➤ Toolbody

➤3D Constraints ➤ Mate.

first mate constraint second mate constraint result

Combining Toolbodies with Spacers |463

2After adding the constraints, use AMACTIVATE to activate RELIEF_1.

Browser In the Browser, right-click RELIEF_1 and choose Activate

Toolbody.

3Combine the relief cylinder and the relief toolbody.

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

Placed Features ➤ Combine.

4Choose Intersect, and select the relief cylinder as the toolbody.

Save your file.

Combining Toolbodies with Spacers

In the Desktop Browser, make sure that the relief toolbody has a combine fea-

ture and that it contains the relief cylinder toolbody.

In the Browser, right-click SPACER and choose Activate Part.

464 |Chapter 17 Combining Parts

To combine a relief toolbody with a spacer

1Use AMMATE for assembly constraints just as you did to align the relief tool-

body with the spacer.

Desktop Menu Toolbody ➤ 3D Constraints ➤ Mate.

When you combine the spacer and the relief toolbody in step 3, you will cut

the spacer with the toolbody. Therefore, be sure to align the top of the tool-

body with the top of the spacer.

After you constrain the relief toolbody, your model should look like this:

2Use AMCOMBINE to combine the spacer and the relief toolbody.

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

Features ➤ Combine.

3Choose Cut, and select the relief toolbody.

Save your file.

Adding Weight Reduction Holes |465

Adding Weight Reduction Holes

The axle spacer is a high-performance chassis component, so its weight must

be kept to a minimum. To achieve this, you cut weight reduction holes into

the part. The manufacturer of the part offers several size spacers with differ-

ent size weight reduction holes. The use of parametric Boolean operations is

an ideal way to model the part, because it is easy to replace one combine fea-

ture with another.

The file spacer.dwg already contains the geometry you need to create a weight

reduction extrusion that cuts material from the middle of the spacer. An

external file contains the part that you will use to remove material from each

of the spacer’s four sides.

First, you attach the external file.

To minimize the weight of a part, using an external toolbody

1Use AMCATALOG to attach the weight reduction holes toolbody.

Context Menu In the graphics area, right-click and choose Catalog.

In the Part Catalog, choose the External tab. Clear the Return to Dialog check

box. Right-click WR_HOLES, and choose Attach.

2Respond to the prompts as follows:

Specify new insertion point: Specify a point to the left of the spacer

Specify insertion point for another instance or <continue> Press ENTER

The spacer is created as a midplane extrusion. Therefore, the parting line

appears as a profile that encircles the part at its midsection. When you con-

strain the weight reduction extrusion to the spacer, you select the parting-

line geometry.

3Use AMMATE to constrain the two parts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

466 |Chapter 17 Combining Parts

4Align the axis of one of the reduction extrusion cylinders with a line that

runs through the center points of the spacer arcs. Use the point option when

you define the axis, as you did with previous mate constraints.

5Use another mate constraint to align the axis of the adjacent weight reduc-

tion extrusion cylinder with a line that runs through the center points of the

spacer arcs.

6Make sure that the spacer is the active part, and use AMCOMBINE to com-

bine the two parts.

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

Features ➤ Combine.

7To cut the weight reduction extrusion from the spacer, choose Cut, and select

the weight reduction extrusion as the toolbody.

8Remove the hidden lines.

Desktop Menu View ➤ Hide

Save your file.

Adding Weight Reduction Holes |467

The weight reduction holes are very close to the relief cut. For balance, the

holes must remain centered in the spacer. To provide enough material

between the holes and the relief, you need to reduce the depth of the relief

and the diameter of the holes.

To make the change, you edit the nested relief cylinder toolbody and reduce

its extrusion distance.

NOTE When you edit more complex parts, it is sometimes easier to select

commands from menus or toolbars instead of searching for the feature in the

Browser and using the Browser menus.

To center the weight reduction holes

1Return to wireframe display.

Desktop Menu View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen

2Use AMEDITFEAT to recover the relief toolbody, responding to the prompts.

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

Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Enter t

Select parametric boolean to edit: Select the edge of the relief toolbody (1)

Enter an option [Accept/Next] <Accept>:

When the relief toolbody is highlighted, press ENTER

468 |Chapter 17 Combining Parts

Mechanical Desktop recovers the toolbody and displays it in its constrained

position on the spacer. The relief toolbody is active, and it contains the relief

cylinder toolbody.

3Use AMEDITFEAT to recover the relief cylinder, responding to the prompt.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Enter t

Mechanical Desktop recovers the relief cylinder toolbody and displays it in

its constrained position on the relief toolbody.

4Change the thickness of the relief cylinder, responding to the prompt.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Select the cylinder (1)

5In the Extrusion dialog box, change the distance to 5. Then choose OK.

6Continue on the command line.

Select object: Press ENTER

Adding Weight Reduction Holes |469

In the Browser, note that the relief toolbody and the relief cylinder toolbody

have yellow backgrounds. This indicates that they need to be updated.

7Use AMUPDATE to update the parts, responding to the prompts.

Context Menu In the graphics area, right-click and choose Update Full.

Toolbody Updates Pending: 2

Enter an option [Full/stEp/posiTioning] <Full>: Press ENTER to update both parts

Next, you change the diameter of the weight reduction holes. Because the

toolbody is an external reference, you activate it first. Then you change the

diameters of the cylinders.

470 |Chapter 17 Combining Parts

To edit the weight reduction cylinders

1In the Browser, right-click WR_HOLES_1 and choose Open to Edit.

Mechanical Desktop opens the external file containing the weight reduction

holes.

2Expand WR_HOLES in the Browser.

3Right-click ExtrusionMidplane1 and choose Edit.

4Choose OK to exit the Extrusion dialog box.

5Continue on the command line.

Select object: Specify the diameter dimension

Enter dimension value <42>: Enter 35

Solved fully constrained sketch.

Select object: Press ENTER

6Repeat steps 3 through 5 for the adjacent cylinder.

Next, commit your changes to the external file, and then update your com-

bined part.

To commit changes to an external file

1Use AMUPDATE to update the external part, responding to the prompts.

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

Part.

2Save and close wr_holes.dwg.

3Reload the external file.

Browser Right-click and choose Show Definition.

4In the Part Catalog, under the All tab right-click WR_HOLES, and choose

Reload.

5Choose OK to exit the Part Catalog.

6Use HIDE to remove the hidden lines to verify the design changes.

Desktop Menu View ➤ Hide

Save your file.

Adding Weight Reduction Extrusions |471

Adding Weight Reduction Extrusions

One more weight reduction extrusion remains. The geometry for the sketch

is stored on the WEIGHT_REDUCTION_EXTRUSION layer.

To copy a sketch to create a new sketch

1Return to wireframe display.

Desktop Menu View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen

2Use LAYER to turn on the WEIGHT_REDUCTION_EXTRUSION layer and make it

current.

Desktop Menu Assist ➤ Format ➤ Layers

This sketch was easily constructed by creating a copy of the spacer profile

sketch before it was consumed. Its scale was then reduced by 50 percent,

using a base point at the center of the sketch.

3Switch to a top view of your part.

Desktop Menu View ➤ 3D Views ➤ Top

4Use AMNEW to create a new toolbody.

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

Menu ➤ Toolbody ➤ New Toolbody.

5Enter the name wt_reduction_extrusion.

472 |Chapter 17 Combining Parts

6Turn off LAYER 0, which contains the spacer.

Desktop Menu Assist ➤ Format ➤ Layer

7Use AMPROFILE to profile the sketch.

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

Sketch Solving ➤ Profile.

8Select the sketch and all of its existing dimensions.

Mechanical Desktop converts the standard dimensions to parametric dimen-

sions and solves the sketch.

Solved underconstrained sketch requiring 2 dimensions or constraints.

To constrain and extrude sketches

1Use AMADDCON to add two X Value constraints to the profile, responding to

the prompts to fully constrain the sketch.

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

Constraints ➤ X Value.

Valid selections: line, arc, circle or spline segment

Select object to be reoriented: Select the arc (1)

Valid selections: line, arc, circle or spline segment

Select object x value is based on: Select the arc (2)

Solved underconstrained sketch requiring 1 dimensions or constraints.

Adding Weight Reduction Extrusions |473

Valid selections: line, arc, circle or spline segment

Select object to be reoriented: Select the arc (3)

Valid selections: line, arc, circle or spline segment

Select object x value is based on: Select the arc (4)

Solved fully constrained sketch.

Valid selections: line, arc, circle or spline segment

Select object to be reoriented: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/

eXit] <eXit>: Press ENTER

2Use VIEW to restore the saved view.

Desktop Menu View ➤ Named Views

In the View dialog box, make SPACER_VIEW current, and choose OK.

3Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion Feature dialog box, specify:

Termination: MidPlane

Distance: Enter 75

Draft Angle: Enter 2

Choose OK.

Next, combine the new toolbody with SPACER_1.

474 |Chapter 17 Combining Parts

To combine a weight reduction extrusion with a spacer

1Turn on LAYER 0, and make it current.

Desktop Menu Assist ➤ Format ➤ Layer

2Activate the spacer, and then combine the weight reduction extrusion and

the spacer.

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

Features ➤ Combine.

3Choose Cut, to cut the weight reduction extrusion from the spacer, and then

select the weight reduction extrusion as the toolbody.

4Remove the hidden lines.

Desktop Menu View ➤ Hide

Save your file.

Adding Mounting Holes

The final step in your model is to add the mounting holes.

To add a mounting hole

1Return to wireframe display.

Desktop Menu View ➤ Shade ➤ 2D Wireframe

2Use AMHOLE to create the mounting holes.

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

Features ➤ Hole.

Adding Mounting Holes |475

In the Hole dialog box, specify:

Operation: Drilled

Termination: Through

Placement: Concentric

Hole Parameter: Size: 12

3Respond to the prompts as follows:

Select work plane, planar face, or [worldXy/worldYz/worldZx/Ucs]:

Select the top face (1)

Select concentric edge: Select the cylindrical edge (2)

4Repeat steps 2 and 3 to create three more holes, and then press ENTER.

476 |Chapter 17 Combining Parts

5Use HIDE to remove the hidden lines.

Desktop Menu View ➤ Hide

The spacer contains one extrusion, four combine features, and four holes.

Save your file.

You have now created and edited a combined part in the Part Modeling

environment.

477

In This Chapter 18

Assembling Complex

Models

In a previous Autodesk® Mechanical Desktop® tutorial,

you created a simple assembly. In this tutorial, you

create a more complex assembly that includes a

subassembly. You work with contraints, external parts,

and part instances. Then you examine your model for

interference and edit an external part.

When the model is complete, you create assembly

scenes with tweaks, drawing views, and annotations in

preparation for plotting.

■Creating local and external parts

■Constraining parts to create an

assembly

■Creating a new part

■Creating a subassembly and

constraining it to the base

assembly

■Creating and annotating

assembly scenes

■Editing a part in a completed

assembly

■Adding annotations

■Checking for interference

■Updating an assembly and its

scenes

■Finishing a drawing for plotting

478 |Chapter 18 Assembling Complex Models

Key Terms

Te r m Definition

base view The first drawing view you create. Other drawing views are derived from this view.

bill of material

database A dynamic database containing a list of all the parts in an assembly. Used to generate

parts lists that contain associated attributes such as part number, manufacturer, and

quantity.

exploded view Separates parts and subassemblies to show how they fit together. Automatically

updated if the assembly or one of its parts changes.

explosion factor Defines separation of parts in an assembly exploded view by a set value, plus offset, if

applicable. Value is based on model units.

external part A part reference that resides in a file other than the current part or assembly file.

flush constraint Makes two planes coplanar, with their faces aligned in the same direction.

local part A part created in the current assembly file.

parent view A drawing view on which other views are based. For example, the base view is the

parent view for an isometric or orthographic view.

part reference An attributed object associated with a part. Used to provide information about the

part when generating a parts list.

parts list A dynamic list of parts and associated attributes generated from a bill of material

database and placed in the drawing. The parts list automatically reflects additions

and subtractions of parts from an assembly.

structure The hierarchical tree of component to component relationships that define the

assembly model. Assembly models can be restructured in the Browser.

subassembly A group of parts constrained together. Can be used as a single object in a larger

assembly. A subassembly may be created in the current assembly or referenced from

an external file.

trail In an exploded view in a scene, a line that shows how parts in an assembly are

assembled.

tweak Adjusts the position of parts in an assembly scene to avoid overlap in some views or

to make some parts more visible.

zero explosion

factor Allows individually specified movements of parts in an exploded view.

Basic Concepts of Complex Assemblies |479

Basic Concepts of Complex Assemblies

Assemblies can consist of any number of externally referenced and local parts.

You can also have any number of subassemblies, both local and externally

referenced. The advantage to having externally referenced parts and subas-

semblies is that you can use the files in any number of assembly files.

In complex assemblies, the same part is often used in multiple locations. Each

part definition defines a unique part. By instancing a part definition, you can

create multiple copies of a part while maintaining only one definition in your

drawing. Any change to the part definition affects all instances of the part.

After building the assembly, you check for interference between the parts, and

perform mass properties calculations to ensure that the parts are designed cor-

rectly. If a design change affects a part used in more than one assembly, make

the change in the external file.

In a previous tutorial, you made changes to an external part from within an

assembly file by editing in place. In this tutorial, you open an external file and

modify it directly. Then you update the assembly file to reflect the changes,

set up scenes to illustrate the assembly, in both exploded and non-exploded

views, create a parts list, and finalize the drawing for plotting.

Starting the Assembly Process

There are two ways to approach the design process; start by thinking about

how the assembly is organized and decide the order in which to instance the

local and external parts into the assembly, or start designing immediately

and then reorganize the hierarchy of the assembly as needed, using assembly

restructure. Constraints are maintained with parts and subassemblies that are

moved in the restructure process.

The assembly restructure feature provides more flexibility in the design pro-

cess. You can place or create an assembly of components at a single level and

subsequently adjust the assembly structure, grouping components into sub-

assemblies for manufacturing, inventory, and other uses.

For more information about using assembly restructure, see “Restructuring

Assemblies” on page 504.

480 |Chapter 18 Assembling Complex Models

In this lesson, the model is organized and assembled in a particular order.

The assembly contains existing parts and referenced external files. A new

plate design is also referenced into the current file as part of a subassembly.

Open the file pullyasm.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.

This drawing contains one local part, a bracket, and six external parts—a pul-

ley, a washer, a shaft, a bushing, and two nuts.

pulley4

bracket

nut2

washer1

nut4

shaft

bushing

Creating Local and External Parts |481

In the Desktop Browser, click the plus sign next to PULLYASM. The assembly

tree expands to reveal the part files in the order in which they were added,

or referenced, into the file pullyasm.dwg.

In the Browser, each part is followed by a number that indicates the order in

which it was instanced. In this case, each part has only one instance. As you

add more instances, each one will be numbered incrementally. Icons with a

teal background are externally referenced parts.

Creating Local and External Parts

An assembly consists of a combination of existing or new parts and local and

external parts. You create local parts in the current assembly file.

You use the Assembly Catalog to manage existing local parts and to create

new external part references and new local parts. You can use the Browser for

quick access to the localize and externalize functions without opening the

Assembly Catalog.

482 |Chapter 18 Assembling Complex Models

To localize a part

1Localize the PULLEY4, BUSHING, and SHAFT parts.

Browser Press CRTL and select PULLEY4, BUSHING, and SHAFT.

Right-click PULLEY4 and choose All Instances ➤ Localize.

In the Browser, note that the PULLEY4, BUSHING, and SHAFT icons no

longer have a teal background, which indicates that the externally referenced

Mechanical Desktop® parts are now local parts.

Links to the external files are severed. Any changes made to these parts affect

only the instances in the current assembly.

2Check the Assembly Catalog to see how the localized parts are displayed.

Context Menu In the graphics area, right-click and choose Catalog.

Choose the All tab. The PULLEY4, BUSHING, SHAFT and BRACKET are listed

under Local Assembly Definitions.

Choose OK.

When you have a library of existing parts, bring the files containing those

parts into the assembly drawing, and localize them. Parts that may change

should be externally referenced so that if the original part is changed, the

change will be reflected in the assembly drawing.

Applying Assembly Constraints |483

To reference an external part

1Use AMCATALOG to reference an external part.

Context Menu In the graphics area, right-click and choose Catalog.

In the Assembly Catalog, choose the External tab.

2In Directories, right-click and choose Add Directory.

Select the desktop\tutorial folder, and choose OK.

All the part and assembly files in the folder are displayed; the icon in front of

each file indicates whether it is a part file or an assembly file.

3Clear the Return to Dialog check box.

4In Part and Subassembly Definitions, right-click DPULLEY and choose Attach.

5In the graphics area on your screen, specify an insertion point and press ENTER.

DPULLEY is now externally referenced and instanced into your copy of the

pullyasm.dwg file.

Applying Assembly Constraints

Now that the parts are referenced or localized into the assembly drawing, you

build the assembly by applying assembly constraints. You apply them to one

part at a time, removing degrees of freedom. The more constraints a part has,

the less freedom of movement it has.

You link the parts, one by one, like a chain, by constraining each part to

another part. Use the DOF symbol to illustrate how many degrees of freedom

are removed. Usually, you need to solve at least 2 degrees of freedom to suf-

ficiently constrain a part.

Zoom in as needed to make selection points easier to see. First, you constrain

the pulley to the bracket along the common axes. Then, you add another

constraint, to mate the planes of the two parts.

dpulley

484 |Chapter 18 Assembling Complex Models

To constrain part faces along their axes using mate

1Use AMMATE to constrain the part faces, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Select a cylindrical face on BRACKET (1)

First set = Axis, (arc)

Select first set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Select second set of geometry: Select a cylindrical face on PULLEY4 (2)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

To select the geometry to be constrained, enter responses on the command

line, or use the animated mouse. Click the left (red) mouse button to cycle

through the options. Click the right (green) mouse button to select an option.

The PULLEY4 part is partially constrained to the BRACKET part along the

common axes.

Applying Assembly Constraints |485

You can move parts to make selection easier. The parts are automatically

reassembled when you add a constraint. Or, to manually reassemble parts,

set AMAUTOASSEMBLE to 0 (off). Use the Assembly Update icon in the

Browser to reassemble the parts after you finish adding constraints.

2Mate the parts on facing planes, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

Select first set of geometry: Specify the top plane on BRACKET (3)

Select first set or [Clear/aXis/fAce/Next/cYcle] <accEpt>: Enter a

First set = Plane

Enter an option [Clear/Next/Flip/cYcle] <accEpt>:

Cycle to point arrow away from the part, then press ENTER

Select second set of geometry: Specify the flange on PULLEY4 (4)

Second set = Axis, (arc)

Select second set or [Clear/fAce/Point/cYcle] <accEpt>: Enter a

Second set = Plane

Enter an option [Clear/aXis/Point/Next/Flip/cYcle] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

You have constrained BRACKET and PULLEY4 along the common axes and

mating planes.

The constraints are illustrated in the Desktop Browser as you create them,

showing the other part the constraint is applied to.

486 |Chapter 18 Assembling Complex Models

To make it easier to see the constraints you have applied, select the Assembly

filter in the Browser. Then, the features are hidden, and only the assembly

constraints are displayed.

To constrain part faces along their axes using Insert

1Use AMINSERT to constrain the part faces along the common axes and corre-

sponding planes, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Specify the hole on NUT2 (5)

First set = Plane/Axis

Enter an option [Clear/Flip] <accEpt>: Press ENTER

Select second circular edge: Specify the hole on the top flange of PULLEY4 (6)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accEpt>: Press ENTER

Enter offset <0.0000>: Press ENTER

Applying Assembly Constraints |487

Using the insert constraint removes the same degrees of freedom as

constraining planes and axes separately. This is particularly useful for bolt-in-

hole type constraints.

The NUT2 part is constrained to BRACKET and PULLEY4 along the common

axes and mating planes.

2Constrain WASHER1 to NUT2, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Zoom in as needed to see the arrows that indicate the direction of insertion.

Select first circular edge: Specify a point on WASHER1 (7)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Select second circular edge: Specify the hole on NUT2 (8)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Flip the direction arrow as needed, and press ENTER

Enter offset <0.0000>: Press ENTER

WASHER1 is constrained to NUT2. Next, constrain NUT4 to WASHER1 along

the common axes and mating planes.

488 |Chapter 18 Assembling Complex Models

3Constrain NUT4 to WASHER1.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

4Constrain BUSHING and DPULLEY along the common axes, responding to

the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Specify a point on BUSHING (9)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Select second circular edge: Specify the hole on DPULLEY (10)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>:

Enter f to flip the direction arrow away from BUSHING

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Enter offset <0.0000>: Press ENTER

Applying Assembly Constraints |489

DPULLEY is constrained to BUSHING.

To apply final mate constraints

1Use AMMATE to constrain DPULLEY and BUSHING to BRACKET with two

constraints: one to mate planes and one to mate along their axes. If you need

to, refer to “To constrain part faces along their axes using mate” on page 484.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

mating plane

mating line

490 |Chapter 18 Assembling Complex Models

2Use AMMATE to constrain SHAFT to BRACKET along the left vertical line of

the notch.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Mate.

The rotational degree of freedom is removed.

Save your file.

The parts are assembled, and all required degrees of freedom are solved by the

constraints.

3Change to a top view and then to a right view, to verify that the parts are

positioned correctly.

Use the Browser to delete unwanted assembly constraints. Right-click the

Constraint icon, and choose Delete. You can then apply new constraints.

Next, create a new part to use as part of a subassembly.

mating lines

Creating New Parts |491

Creating New Parts

Before you build the subassembly, you create a pulley plate part. First, you

open a part file containing a constrained profile. Because you can have more

than one drawing open at a time in Mechanical Desktop, you do not need to

close your assembly file. In the part file, you add thickness to the profile and

create additional features so that you can use it as a subassembly in your

assembly.

Open the file ppulley.dwg.

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 sketch of the pulley plate has already been profiled and constrained, so

you only need to extrude it. Extrusion adds thickness to a constrained profile.

492 |Chapter 18 Assembling Complex Models

To extrude a sketch

1Expand the feature hierarchy in the Browser by clicking the plus sign in front

of PPULLEY_1.

2Use AMEXTRUDE to extrude the profile.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

3In the Extrusion dialog box, specify:

Distance: Enter 10

Choose OK to create the extrusion.

To add a placed feature to a part

1Use AMHOLE to add three drilled bolt holes to the pulley plate.

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

Features ➤ Hole.

In the Hole dialog box, select the Drilled hole type icon, and specify:

Termination: Through

Placement: Concentric

Diameter: Enter 10

Choose OK.

2Continue on the command line.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the pulley plate edge (1)

Enter an option (Next/accEpt) <accEpt>: Press ENTER

Select concentric edge: Select the arc (2)

Creating New Parts |493

3Continue placing two more holes concentric to the remaining arcs. Then

press ENTER.

The drilled holes are added and cut through the pulley plate. Later, you check

for interference and modify the diameter of the holes.

4Use AMFILLET to fillet the pulley plate edges.

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

Features ➤ Fillet.

In the Fillet dialog box, select the Constant check box and specify:

Radius: Enter 1

Return to dialog: Clear the check box

Choose OK.

5Respond to the prompts as follows:

Select edges or faces to fillet: Select the pulley plate top edge (1)

Select edges or faces to fillet: Select the pulley plate bottom edge (2)

Select edges or faces to fillet: Press ENTER

The pulley plate edges are filleted.

Now that the pulley plate is complete, you have all the parts you need to

build the subassembly.

Save your file, but do not close it. You will make some changes to it later.

494 |Chapter 18 Assembling Complex Models

Creating Subassemblies

You created an assembly. Now, you will create a subassembly. Each subassem-

bly contains one or more parts or subassemblies. In the Browser, subassem-

blies and parts are nested under the assembly.

You create, instance, and constrain parts into a subassembly just as you do

into an assembly. Once the subassembly is created, it is constrained to the

assembly, completing the assembly model.

Defining and Activating Subassemblies

Before you can instance any parts into the subassembly, you must create and

activate a subassembly definition and then load and instance external part

drawings as the parts for the subassembly.

To create and activate a new subassembly

1Switch to the window containing your assembly.

2Activate the assembly, PULLYASM.

Browser Right-click PULLYASM and choose Activate.

3In the Browser, collapse the feature hierarchy.

Browser Right-click PULLYASM and ➤ Collapse. Then click the

plus sign in front of PULLYASM.

4Create a new subassembly definition, responding to the prompt.

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

New Subassembly.

Enter new subassembly name <SUB1>: Enter subpully

The Desktop Browser adds a subassembly called SUBPULLY_1 to the assembly

tree. Because there are no parts instanced or files attached, the subassembly

location is empty.

5Activate the new subassembly, responding to the prompt.

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

Activate Assembly.

Enter assembly name to activate or [?] <PULLYASM>: Enter subpully_1

Creating Subassemblies |495

The inactive PULLYASM assembly is shaded in the Desktop Browser, and the

SUBPULLY subassembly is active.

The active subassembly name is displayed below the command line (Target:

SUBPULLY).

Using External Parts

Now that you have activated the new subassembly, you use external parts to

create the subassembly.

To attach an external part drawing as an external part

1Use AMCATALOG to attach an external part.

Context Menu In the graphics area, right-click and choose Catalog.

In the Assembly Catalog, choose the External tab. Verify that tutorial is listed

in Directories and that Return to Dialog is selected.

2Double-click the file ppulley.dwg.

3Position the pulley plate on the screen, and press ENTER.

The pulley plate is attached to the SUBPULLY subassembly.

4In the Assembly Catalog, right-click DPULLEY3 and choose Attach.

5Attach WASHER3 and NUT3.

dpulley3

nut3

washer3

ppulley

496 |Chapter 18 Assembling Complex Models

Notice that an attached part is indicated by a white background in the

Assembly Catalog.

Choose OK.

Examine the Browser. The referenced parts are nested under the new sub-

assembly hierarchy.

Instancing Parts

You have already attached parts to the subassembly. Each part definition is

listed in the Assembly Catalog. When you instance a part in the current

assembly, it refers to its part definition in the Catalog. Once a part is

instanced into the subassembly, you can copy it from the Browser.

To instance a part

1Use AMCATALOG to instance a part.

Context Menu In the graphics area, right-click and choose Catalog.

In the Assembly Catalog, choose the All tab. In External Assembly Definitions,

select DPULLEY and verify that Return to Dialog is selected.

2Insert a copy of DPULLEY, and choose OK to exit the Assembly Catalog.

3Use the Browser to create another instance of DPULLEY.

Browser Right-click DPULLEY and choose Copy. In the graphics

area, click a location for the copy and press ENTER.

4Make one copy each of DPULLEY3, WASHER3, and NUT3.

The Browser is updated to include the new instances.

Save your file.

Next, apply assembly constraints to build the subassembly.

Completing Assemblies |497

Completing Assemblies

Now that the parts are instanced into the subassembly, you can complete the

subassembly and constrain it to the base assembly. When the entire assembly

is complete, check it for interference among parts, and obtain mass property

information.

NOTE The Desktop Browser shows the order in which parts and subassemblies

are assembled. You can drag a part or subassembly to a different position in the

Desktop Browser. Always save your file before you reorder the hierarchy.

Reordering may affect offsets for explosion factors in scenes.

Applying Assembly Constraints

First, constrain parts in the subassembly, and then constrain the subassembly

to the base assembly.

The instructions specify responses on the command line for constraint appli-

cation, but if you prefer, you can use the animated cursor. After you select the

object to constrain, click the left mouse button (red) to cycle through the

options. When the object you want is highlighted, click the right mouse

button (green) to accept the selection.

498 |Chapter 18 Assembling Complex Models

To constrain a subassembly part

1Use AMINSERT to constrain WASHER3 to PPULLEY, responding to the

prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Specify the hole on the bottom of WASHER3 (1)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Enter f, if needed

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Select second circular edge:

Specify the top cylindrical edge of the hole in PPULLEY (2)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Offset <0.0000>: Press ENTER

WASHER3 is constrained to PPULLEY along common axes and mating

planes.

Completing Assemblies |499

2Constrain DPULLEY to WASHER3, responding to the prompts.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Select first circular edge: Specify inner edge of hole on DPULLEY (1)

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Enter f

First set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Select second circular edge: Specify the top cylindrical edge of WASHER3 (2)

Second set = Plane/Axis

Enter an option [Clear/Flip] <accept>: Press ENTER

Offset <0.0000>: Press ENTER

The DPULLEY part is constrained to WASHER3 along the common axes and

mating planes.

500 |Chapter 18 Assembling Complex Models

3Constrain DPULLEY3 and NUT3 to the subassembly.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

4Constrain the remaining parts to finish the subassembly.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Save your file.

Next, activate the top level of the assembly and constrain the subassembly to

the top assembly.

To constrain a subassembly to a top-level assembly

1Use AMACTIVATE to activate the PULLYASM assembly, responding to the

prompt.

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

Activate Assembly.

Enter assembly name to activate or [?] <PULLYASM>: Press ENTER

Completing Assemblies |501

In the Desktop Browser, the top-level assembly is no longer shaded.

The active assembly name is displayed below the command line (Target:

PULLYASM).

2Move the subassembly, to make viewing easier. Then zoom in as needed to

magnify selection points.

Next, constrain the pulley plate subassembly to the root assembly.

3Choose Insert to constrain the shaft of NUT2 to the pulley plate hole on the

mating planes and along the common axes.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

completed subassembly

completed root assembly

502 |Chapter 18 Assembling Complex Models

The subassembly is now constrained to the root assembly.

Copy another instance of NUT3 in your drawing and constrain it to the shaft

of NUT2.

To add and constrain a part instance

1Use the Browser to copy another instance of the NUT3 external part into the

assembly.

Browser Right-click NUT3, and choose Copy. In the graphics area,

click a location for the copy, and press ENTER.

2Constrain NUT3 to the pulley plate and the shaft of NUT2.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

Completing Assemblies |503

It is a good idea to check the position of a constrained part in another view. If

the part is constrained incorrectly, use the Browser to delete the constraint.

Right-click to display the menu, and choose Delete. Then move the parts as

needed, and reapply the constraints.

One side of the pulley assembly is complete.

3Repeat steps 1 and 2 to copy and apply assembly constraints to WASHER3,

PPULLEY, and NUT3, to complete the pulley assembly.

4Add one instance of your copy of the PPULLEY external part, two copies of

WASHER3, and three copies of NUT3 into the assembly drawing.

NOTE Depending on the current UCS of your drawing, the parts may not be

oriented the same as they are in the above illustration. This does not affect your

ability to place the constraints.

504 |Chapter 18 Assembling Complex Models

5Constrain both WASHER3 parts to the DPULLEY3 parts on the pulley plate.

Context Menu In the graphics area, right-click and choose 3D

Constraints ➤ Insert.

6Use Insert to constrain PPULLEY_2 to the WASHER3 parts.

Constrain PPULLEY to any two instances of WASHER3, to remove the rota-

tional degree of freedom from the pulley plate.

7Use Insert again to constrain the NUT3 parts to the pulley plate.

Save your file. The pulley assembly is complete.

Restructuring Assemblies

The pulley assembly model in the previous exercise was planned, and then

assembled in a particular order. In Mechanical Desktop, you can use another

design process called assembly restructure. You can design and constrain parts

and create assemblies in any order, and subsequently adjust the assembly

structure within the Desktop Browser.

Using the assembly restructure feature in the Browser, you can

■Use either the drag or cut and paste method to move components

■Move components from the master assembly into a local or external sub-

assembly

■Select multiple parts and subassemblies and move them within the

Browser to restructure the assembly

■Move components while in the context of an active external subassembly

Completing Assemblies |505

In most cases, constraints are maintained with the parts and subassemblies

that you move. In the event that a constraint cannot be maintained, a warn-

ing message is displayed.

NOTE Instances can be lost if you restructure them up the assembly hierarchy

where multiple instances of the same definition exist.

Open the assembly file pullyasm.dwg from the desktop\tutorial folder, and

practice using assembly restructure.

To restructure an assembly hierarchy

1Expand the hierarchy in the Browser so you can see all of the components.

Browser Right-click PULLYASM and choose Expand.

2Select a part name to activate the part.

To select more than one part, hold down CTRL as you select.

To select all parts within a range, hold down SHIFT as you select the first and

last part in the range. All components in between are automatically selected.

3Drag the selected parts up or down in the assembly structure.

Use a left-click to drag your selection to a location and release the mouse.

Use a right-click to drag your selection to a location and release the mouse to

display a context menu with options Move Here, Copy Here, Create Subas-

sembly Here, and Cancel.

If the assembly tree is too long to scroll conveniently, right-click the compo-

nent and choose Cut, scroll to the new location, and Choose paste.

If a part cannot be moved logically, an error icon is displayed.

When restructure is activated, the cursor changes to look like a shadow of the

original part name.

4Drop the part in a valid destination.

Valid destinations are highlighted as you move the cursor over them.

The part is restructured within the assembly, and the assembly is updated.

506 |Chapter 18 Assembling Complex Models

Analyzing Assemblies

Next, check for interference between parts. This analysis is useful for detect-

ing problems that may arise during the final design stages. Check each part

for interference. If any interference is detected between parts, interference

solids can be created to illustrate where the interference occurs.

To check for interference

1Use AMINTERFERE to check for interference.

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

Check Interference.

Respond to the prompts.

Nested part or subassembly selection? [Yes/No] <No>: Enter y

Specify first set of parts or subassemblies or [?]: Select PPULLEY (1)

Instance = PPULLEY_2

Enter an option [Down/Next/Accept] <Accept>: Press ENTER

Specify first set of parts or subassemblies: Press ENTER

Specify second set of parts or subassemblies: Select DPULLEY3 (2)

Instance = SUBPULLY_1

Enter an option [Down/Next/Accept] <Accept>: Enter d

Instance = DPULLEY3_1

Enter an option [Up/Down/Next/Accept] <Accept>: Press ENTER

Specify second set of parts or subassemblies: Press ENTER

Comparing 1 parts/subassemblies against 1 parts/subassemblies.

Interference 1:

PPULLEY_2

SUBPULLY_1

DPULLEY3_1

Create interference solids? [Yes/No] <No>: Enter n

Highlight pairs of interfering part/subassemblies?[Yes/No] <No>: Enter y

Enter an option [eXit/Next pair] <Next pair>: Enter x

NOTE Resize the text window above the command line to read the results of

interference checking.

Completing Assemblies |507

You should detect two examples of interference. Both DPULLEY and

WASHER3 parts interfere with the holes on PPULLEY. The drilled holes in the

pulley plate are too small.

The pulley plate is an external part, but it can be edited from within the

assembly file. If you are working in a very large assembly, it may be easier to

open the external file and make changes.

508 |Chapter 18 Assembling Complex Models

Editing Mechanical Desktop Parts

Because interference was detected between the pulley plate and the

DPULLEY3 parts, you need to enlarge the drilled holes on the pulley plate.

Editing an external part updates all instances of the parts in the assembly

drawing. The modified part retains the applied assembly constraints.

In this tutorial, you return to the open ppulley.dwg file and make the holes

larger, to remove the interference.

To edit an external part

1Switch to the window containing the PPULLEY part you created earlier.

2In the Browser, click the plus sign in front of PPULLEY to display the part

features.

3Use AMEDITFEAT to edit the holes, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Independent array instance/Sketch/surfCut/Toolbody/select

Feature] <select Feature>: Select one of the drilled holes

Enter an option [Accept/Next] <Accept>: Enter n or press ENTER

The Hole dialog box is displayed.

4In the Hole dialog box, enter 15 in the Drill Size field. Then choose OK.

5Repeat steps 3 and 4 for Hole2 and Hole3.

6Use AMUPDATE to update the edited part.

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

The pulley plate reflects the new design.

Save your file.

Reloading External References |509

Reloading External References

To update the assembly to reflect the changes you made to the external part,

reload the external definition.

To reload an external definition

1Switch to the window containing the assembly.

2Use AMCATALOG to reload the PPULLEY definition.

Context Menu In the graphics area, right-click and choose Catalog.

In the Assembly Catalog, in External Assembly Definitions, right-click

PPULLEY and choose Reload.

Choose OK.

The pulley plate reflects the new design.

If the assembly looks incorrect, choose Assembly ➤ Assembly Update to

update the assembly constraints.

Save your file.

Check the assembly again for interference.

redesigned part

510 |Chapter 18 Assembling Complex Models

To check for interference

1Use AMACTIVATE to activate the SUBPULLY subassembly.

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

Activate Assembly.

Specify the SUBPULLY subassembly.

2Use AMINTERFERE to check for interference.

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

Check Interference.

3Specify DPULLEY3. No interference should be detected.

Assigning Mass Properties

Next, calculate mass property information. You can analyze parts and assem-

blies during the course of designing. You may need to optimize weight, max-

imize stiffness, balance loads, ease assembly, or meet particular requirements.

One mass properties dialog box contains both Setup and Results tabs that

function the same for both parts and assemblies. In this case, the parts list in

the dialog box displays all parts and part properties in the activated assembly

to be analyzed. Item numbers are also displayed if a BOM exists. When you

select an item in the parts list, it is graphically highlighted on the screen.

In these steps, you analyze the bracket and change tolerance values and

material types.

To set up mass properties

1Activate the PULLYASM assembly.

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

Activate Assembly.

2Use AMMASSPROP to analyze the mass properties of the assembly, responding

to the prompt.

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

Mass Properties.

Select parts or subassemblies: Select the bracket, and press ENTER

The Assembly Mass Properties dialog box is displayed with the Setup tab

active. In the Materials Available window, the materials listed are all of those

defined in the active assembly.

Reloading External References |511

3In the Assembly Mass Properties dialog box Setup tab, specify:

Output Units: Metric (mm, g)

Coordinate System: User coordinate system (UCS)

Display Precision: Select 0.00000

Part Name: Select BRACKET

Materials Available: Material: Select Stainless_Steel

Choose Assign Material.

The material information is transferred to the part material attribute and

BOM, and is updated in the part name list.

Next, change the material definition for a part in the assembly.

4In the Part Name list, select BRACKET, and then select Edit Materials.

5In the Physical Materials List dialog box Material List, select Stainless_Steel.

In the Properties Window, specify

Density: 8.5

Choose OK.

The new material definition information is transferred to the part, BOM, and

is updated in the Assembly Mass Properties dialog box Part List view.

Choose Done to exit the Assembly Mass Properties dialog box.

You are ready to calculate the mass properties based on the new information

you entered.

Calculating Mass Properties

In the Mass Properties dialog box the Results tab is blank until you use the

Calculate button to retrieve the results of your input in the Setup tab.

512 |Chapter 18 Assembling Complex Models

To calculate mass properties

1In the Mass Properties Dialog Box, select the Results tab. Then select the

Calculate button.

The results are calculated and displayed.

The Calculate button is no longer available because the Setup and Results

fields are in sync. If you change an item on the Setup tab, the results are

cleared and the Calculate button becomes available.

You can use the Insert UCS button to create and insert a user coordinate sys-

tem (UCS) based on a parts or assemblies center of gravity (CG).

2Choose Export Results.

In the File dialog box, define a file name and save the file.

This report file can be imported by many external programs.

3Choose Done to close the Assembly Mass Properties dialog box.

Save your file.

Now, you create an exploded view of the assembly.

Reviewing Assembly Models |513

Reviewing Assembly Models

Assembly scenes and drawing views are essential for reviewing the assembly

model. For this lesson, you first create an exploded assembly scene, and then

tweak the positions of parts and add assembly trails and annotations.

Creating Exploded Assembly Scenes

After assembly constraints have been applied to each part, you can create a

scene (an exploded view of the entire assembly). Multiple scenes can be

created and named. You set an explosion factor to determine the separation

of parts in the scene. If you do not want an exploded view in a scene, set the

explosion factor to 0.

Before you begin, select the Scene tab to switch to Scene mode.

To create an exploded assembly scene

1Use AMNEW to create a new scene, responding to the prompts.

Context Menu In the graphics area, right-click and choose New Scene.

In the Create Scene dialog box, specify:

Target Assembly: PULLYASM

Scene Name: Enter design1

Scene explosion factor <.0000>: Specify 0.0000

Synchronize Visibility with Target Assembly: Select the check box

Choose OK.

514 |Chapter 18 Assembling Complex Models

The scene, design1, is displayed.

2Look at the Browser. The names of all parts in the design1 scene are listed.

Next, align the exploded parts in the assembly scene.

Reviewing Assembly Models |515

Using Tweaks and Trails in Scenes

In an exploded scene, sometimes parts obscure other parts. You can use tweaks

to change the positions of individual parts and then adjust the positions of the

parts in the design1 scene. Zoom in to magnify the parts to be tweaked.

In the Browser, tweaks are nested under the respective parts. You can select and

multi-select tweaks in the Browser to delete them. When you pause the cursor

over a tweak in the Browser, a tooltip displays the distance factor for the tweak.

NOTE The grounded part of an assembly or a subassembly cannot be

tweaked. Its position is fixed.

Assembly trails use a continuous or other defined linetype to indicate the

path of the explosion. These trails use assembly constraint information to

visually demonstrate how the assembly design fits together.

To tweak an exploded assembly scene

1Use AMTWEAK to open the Power Manipulator dialog box.

Context Menu In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on BUSHING_1 (1)

Enter an option [Next/Accept] <Accept>: Press ENTER

The Power Manipulator dialog box is displayed only the first time you create

a new tweak.

516 |Chapter 18 Assembling Complex Models

In the Power Manipulator dialog box, on the Move tab, verify that Place

Objects (ALT) is selected.

Choose Done.

NOTE To access the Power Manipulator dialog box later, right-click the Power

Manipulator symbol on your screen, and select Options.

2Use AMTWEAK to tweak the BUSHING part, responding to the prompts.

Context Menu In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on DPULLEY_1 (1)

Enter an option [Next/Accept] <Accept>: Press ENTER

This time, the Power Manipulator symbol is displayed on the BUSHING part

you selected.

3Click the -Z axis on the Power Manipulator symbol, drag away from the

assembly, and click at a distance of -150.

4Continue on the command line.

Select handle or Geometry

[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>:

Press ENTER

The BUSHING is moved away from the assembly. In the Browser, a Tweak

icon is displayed.

1Use AMTWEAK to tweak the DPULLEY part, responding to the prompts.

Context Menu In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on DPULLEY_1 (1)

Enter an option [Next/Accept] <Accept>: Press ENTER

2Click the -Z axis on the Power Manipulator symbol, drag away from the

assembly, and click at a distance of -70.

Reviewing Assembly Models |517

3Continue on the command line.

Select handle or Geometry

[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>:

Press ENTER.

4Use AMTWEAK to tweak the SHAFT part, responding to the prompts.

Context Menu In the graphics area, right-click and choose New Tweak.

Select part/subassembly to tweak: Specify a point on SHAFT_1 (1)

Enter an option [Next/Accept] <Accept>: Press ENTER

The Power Manipulator symbol is displayed on the SHAFT part.

5Click the -Z axis on the Power Manipulator symbol, drag away from the

assembly, and click at a distance of -200.

6Continue on the command line.

Select handle or Geometry

[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>: Enter r

Create Trails? [Yes/No] <No>: Enter y

[Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] <Accept>:

Press ENTER

The BUSHING, DPULLEY, and SHAFT part tweaks are displayed with trails.

You can adjust assembly trails.

tweaked

dpulley

tweaked

bushing

tweaked

shaft

assembly trail added

518 |Chapter 18 Assembling Complex Models

To adjust assembly trails

1Use AMTRAIL to adjust your assembly trails, responding to the prompt.

Command AMTRAIL

The Trail Offsets dialog box is displayed.

2Use the options in the Trail Offsets dialog box, to adjust over shoots and

undershoots for your trails.

Choose OK to apply your selections.

Next, create an assembly drawing view.

Creating Assembly Drawing Views

An assembly drawing view shows a 2D representation of the 3D assembly.

You use the base part for a base view. Then you create an isometric view of

the entire assembly model. Drawing views are automatically updated when

you change a part or subassembly.

Before you begin, select the Drawing tab to switch to Drawing mode.

Reviewing Assembly Models |519

To create a drawing view

1Use AMDWGVIEW to create a new drawing view.

Context Menu In the graphics area, right-click and choose New View.

2In the Create Drawing View dialog box, specify:

Type: Base

Data Set: Scene: DESIGN1

Scale: Enter .03 (or .75 mm)

Choose OK.

3Respond to the prompts as follows:

Select planar face, work plane or [Ucs/View/worldXy/worldYz/worldZx]:

Enter z

Select work axis, straight edge or [worldX/worldY/worldZ]:

Enter x

Adjust orientation [Flip/Rotate] <accept>

Enter r until the UCS icon is upright

Adjust orientation [Flip/Rotate] <accept>: Press ENTER

Specify location of base view: Specify a point in the left of the title block

Specify location of base view: Press ENTER

520 |Chapter 18 Assembling Complex Models

The base assembly drawing view is displayed.

4Create an isometric view of the assembly.

Context Menu In the graphics area, right-click and choose New View.

In the Create Drawing View dialog box, specify:

View Type: Iso

Scale: Enter 1

Relative to Parent: Select the check box

Choose OK.

5Respond to the prompts as follows:

Select parent view: Select the base view

Specify location for isometric view: Specify a point to the right of the base view

Specify location for isometric view: Press ENTER

An isometric view of the assembly is displayed.

Reviewing Assembly Models |521

6Use AMMOVEVIEW to align the views, responding to the prompts.

Context Menu In the graphics area, right-click and choose Move View.

Select view to move: Select the isometric view

Specify new view location or [Layout]: Align the views and press ENTER

Examine the Browser. The isometric view is listed under the base view.

Now, create a BOM database, and add a parts list and associative balloon callouts.

522 |Chapter 18 Assembling Complex Models

Creating Bills of Material

After you have assembled your parts, you can create a bill of material (BOM)

database. This database contains a list of attributes assigned to each part. The

attributes store information such as manufacturer, description, and vendor

part number.

The attributes are contained in part references that are assigned to each part.

Part references can also be created to reference other geometry in your draw-

ing, such as surfaces. The geometry can then be included in a parts list.

The BOM database counts the number of instances in an assembly and tallies

instances for each part. In the BOM table, defined columns can be edited,

added, deleted, moved, and sorted.

By accessing the information in the BOM database, you can add balloons and

insert parts lists into your drawing. You can edit part references, balloons,

and parts lists. The BOM database is automatically updated.

Because the BOM database is fully parametric, any changes to it update the

information stored in balloons, part references, and parts lists.

To create a BOM database

1Use AMBOM to create the BOM database.

Command AMBOM

In the BOM dialog box, review the parts in the database.

Creating Bills of Material |523

Notice the SUBPULLY definition in the list of parts. The plus sign in front of

it indicates that it is a subassembly.

2Click the plus sign in front of SUBPULLY.

The BOM database now lists all the parts in the assembly, including those in

the subassembly.

Choose OK to exit the BOM dialog box.

3Select the Model tab in the browser. A BOM icon is located under PULLYASM.

By default, the BOM takes the same name as the assembly file. You can

change this setting by editing the name of the BOM directly in the Browser.

To edit the name of a BOM

1Using the Browser, rename the BOM database.

Browser Right-click the BOM icon and choose Rename.

2Change the name to BOM_1.

Customizing BOM Databases

Mechanical Desktop provides symbol standards for major drafting conven-

tions, including ANSI, BSI, CSN, DIN, GB, ISO, and JIS. By modifying the

symbol standards, you can control the way symbols, balloons, and parts lists

are displayed in the drawing, when you create them.

Next, modify the symbol standards to control the number of columns used

in the parts list and the name of one of the columns.

524 |Chapter 18 Assembling Complex Models

To modify symbol standards

1Use AMOPTIONS to access the Mechanical Desktop symbol standards.

Command AMOPTIONS

In the Mechanical Options dialog box, expand the hierarchy of ANSI, and

double-click the icon in front of BOM Support.

2In the BOM Properties for ANSI dialog box, in Columns select Material and

specify:

Caption Alignment: Select the Center Align Text icon

Data Alignment: Select the Center Align Text icon

Creating Bills of Material |525

Choose Apply, then OK.

The Mechanical Options dialog box is still open.

3Choose OK to close the Symbol Standards dialog box.

Save your file.

Working with Part References

When you create a BOM database, each part in the assembly is assigned a part

reference. A part reference is an attributed block that can be modified to

include any information you want to attach to the part. That information is

used by the BOM database and included in the parts lists you generate.

Before you begin, in the Browser, select the Drawing tab to switch to Drawing

mode.

526 |Chapter 18 Assembling Complex Models

To edit a part reference

1Use AMPARTREFEDIT to edit a part reference, responding to the prompt.

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

Menu ➤ Parts List ➤ Part Reference Edit.

Select pick object: Select the part reference for BRACKET (1)

2In the Part Ref Attributes dialog box, double-click in the Name field and enter

Pulley Bracket.

Choose OK.

Creating Bills of Material |527

3Use AMBOM to display the BOM database.

Context Menu In the graphics area, right-click and choose Parts List ➤

BOM Database.

Bom table [Delete/Edit] <Edit>: Press ENTER

Notice that Pulley Bracket is now listed under Note for BRACKET.

Choose OK to exit the BOM dialog box.

Next, add balloon callouts to the isometric view.

Adding Balloons

Balloons are used to reference parts in your drawing to a parts list. They con-

tain the same information as the part reference they are attached to. You can

edit that data by selecting balloons. Changes made to the data associated

with a balloon are reflected in the BOM database and the parts list.

You can control the size and appearance of balloons, using the Symbol Stan-

dards dialog box.

528

To place a balloon callout

1Use AMBALLOON to create balloon callouts for BRACKET, DPULLEY, BUSH-

ING, SHAFT, and NUT3, responding to the prompts.

Desktop Menu Choose Annotate ➤ Parts List ➤ Balloon.

Select part/assembly or [auTo/autoAll/Collect/Manual/One/ Renumber/

rEorganize]: Enter T

Align [Angle/Standalone/Horizontal/Vertical] <Vertical>: Press ENTER

Select pick object: Select the part reference for BRACKET (1)

Select pick object: Select the part reference for DPULLEY (2)

Select pick object: Select the part reference for BUSHING (3)

Select pick object: Select the part reference for SHAFT (4)

Select pick object: Select the part reference for NUT3 (5)

The objects are aligned after you pick them.

Creating Bills of Material |529

Continue on the command line:

Select pick object: Press ENTER

Align Standalone/Horizontal/<Vertical>:

Specify a point between the two drawing views

Next, place the parts list in the drawing.

Placing Parts Lists

A parts list is an associative block of information about your assembly. It dis-

plays information about the parts, according to the settings specified in the

BOM database. Because it is parametric, any changes you make to the BOM

database or symbol standards are automatically reflected in the parts list.

530 |Chapter 18 Assembling Complex Models

To place a parts list

1Use AMPARTLIST to place the parts list under the base view of your assembly,

responding to the prompts.

Context Menu In the graphics area, right-click and choose Parts List ➤

Part List.

The Parts List dialog box is displayed.

2In the Parts List dialog box, in Title, enter the new name Pulley Parts List.

3Choose Apply, then choose OK.

Specify location: Specify a point under the base view

The parts list is placed in the drawing.

NOTE You may need to move the drawing views to make room for the parts

list. Place the parts list first, and then move the views as needed. Because the bal-

loons are associated with the views, they will also move.

Finishing Drawings for Plotting |531

When the parts list is created, a parts list icon is displayed in the Browser.

Save your file.

Finishing Drawings for Plotting

Now that the assembly has been documented, plot the drawing.

Paper drawings are useful for reviewing the entire assembly to make sure that

the design is feasible and can be manufactured. The Parts List on the assem-

bly drawing provides information about the parts needed to manufacture the

assembly. If you wish, add more reference dimensions, fill in the title block,

and add some notes to your drawing before you plot.

This tutorial has demonstrated the flexibility of using subassemblies to create

complex models. Even a complex assembly can be easily modified and doc-

umented, if it is truly a parametric assembly.

532

533

In This Chapter 19

Creating and Editing

Surfaces

This Autodesk® Mechanical Desktop®tutorial

introduces surfaces grouped by function, and provides

instructions for creating the different types of surfaces.

You learn surface types, practice surface modeling, and

work with modeling some typical surfaces.

Once you have completed this lesson, you will

understand the techniques required to surface a more

complex part.

■Creating surfaces—motion

based, skin, and derived

■Joining and trimming surfaces

■Editing surfaces

534 |Chapter 19 Creating and Editing Surfaces

Key Terms

Te r m Definition

augmented line A 3D polyline with vector information at each vertex. An augmented line is a

surface creation tool that allows you to control the curvature and the tangency

of a surface.

base surface A basic underlying surface that carries a shape across a larger area. Can be

trimmed to precise shapes as needed, but the base surface remains intact and

may be displayed.

derived surface A surface that gets some or all of its attributes from one or more base surfaces.

motion-based surface A surface created by moving wires through space.

rail One or more curved lines along which a surface is swept. Rails form the

curvature of a swept surface.

skin surface The surface draped over a wireframe.

surface normal A short line perpendicular to a surface that shows where the surface starts and

which direction is out.

surface primitive Surface created by values you specify. It does not require a wireframe model.

U or V display lines Lines that correspond to rails and wires.

wire Generic term for lines, arcs, circles, ellipses, 2D and 3D polylines, augmented

lines, and splines.

wireframe modeling Wires and surface parts intermixed to construct the basic framework of a 3D

model. The initial step in creating a surfaced model.

wireframe surfacing Covering a wireframe model with surfaces.

Basic Concepts of Creating Surfaces |535

Basic Concepts of Creating Surfaces

Three-dimensional surface modeling can be compared to constructing a

building. You start by establishing the initial shape. Then you cover the

rough framing with siding and roofing.

One approach to surface modeling is to create a 3D framework of wires. Wire

is a generic term for lines, arcs, circles, ellipses, 2D and 3D polylines, aug-

mented lines, and splines, including splines created from existing part edges.

This framework is called a wireframe.

Wires and surface parts can be intermixed to construct the framework of your

3D model. This initial step in creating a surfaced model is called wireframe

modeling.

Once the 3D wireframe model is created, the next step is to cover the frame-

work with a surface. This task is called wireframe surfacing. This technique is

one approach to creating surfaces.

rough frame siding applied

line ellipse polyline

spline augmented line

circle

536 |Chapter 19 Creating and Editing Surfaces

Working with Surfaces

In this tutorial you’ll learn about these types of surfaces:

■Primitive, created by specifying values

■Motion-based, created by moving wires through space

■Skin, applied over a wireframe

■Derived, generated from existing surfaces

Primitive surfaces (cone, cylinder, sphere, and torus) do not require wire-

frames for their construction. To create a sphere surface, for example, you

determine the center of the sphere and then enter a value for its radius. Prim-

itive surfaces are most often used for conceptual design.

You can practice creating primitive surfaces on your own by choosing Surface

➤ Create Primitives.

In this tutorial, you’ll practice working with motion-based, skin, and derived

surfaces you create from wireframes. You’ll also work with simple wireframe

geometry to learn surfacing techniques.

After you create each surface, use the Extents option of the ZOOM command

to redisplay all of the wireframes provided in the drawing file. Then zoom to

enlarge the object you need for the next exercise.

Working with Surfaces |537

To set up your file

1Open the file t_surfs.dwg in the desktop\tutorial folder. The wireframe objects

you need for this lesson are included in this file.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

Surface lines, called U and V lines, indicate the direction of the surface.

Increasing the number of lines increases the density of the surface image.

2Use the Mechanical Options dialog box to change the number of surface

lines used to display surfaces.

Desktop Menu Surface ➤ Surface Options

Choose the Surface tab, and in Surface Properties specify:

U Display Wires: Enter 7

V Display Wires: Enter 7

Choose OK.

NOTE If you shade the surfaces you create to better view them, adjust the

AutoCAD setting that controls back faces. Go to Assist ➤ Options and select the

System tab. Choose Properties, then clear the check box for Discard Back Faces.

Choose Apply & Close, then OK.

You are ready to create your first surfaces.

538 |Chapter 19 Creating and Editing Surfaces

Creating Motion-Based Surfaces

Some surfaces are created by “moving” wires through space. These motion-

based surfaces are revolved, extruded, and swept.

Revolved Surfaces

A revolved surface uses two wires: one establishes the constant shape of the

surface, and the other is the axis about which to spin the shape. The revolved

surface is created by the motion of a wire shape through space.

To revolve a surface

1Use AMREVOLVESF to revolve a spline curve about an axis, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Revolve

Select path curves to revolve: Select spline (1)

Select path curves to revolve: Press ENTER

Specify axis start point or [Wire]: Enter w

Select wire to define axis: Select line (2)

Enter start angle <0>: Press ENTER

Enter included angle (+=ccw, -=cw) <Full circle>: Press ENTER

The curve revolves about the vertical line.

2Use the Zoom Extents option of ZOOM to redisplay all the wireframes and

select the object for the next exercise.

Creating Motion-Based Surfaces |539

Extruded Surfaces

An extruded surface is created by a 3D wire shape moved along a straight line.

You select a line, polyline, arc, or spline to extrude, and you specify the direc-

tion and magnitude of the extrusion.

To extrude a surface

1Use AMEXTRUDESF to extrude a circle into a cylinder, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Extrude

Select wires to extrude: Select circle (1)

Select wires to extrude: Press ENTER

Define direction and length.

Specify start point or [Viewdir/Wire/X/Y/Z]: Enter w

Select wire to define direction: Select line (2) above its midpoint

Enter an option [Accept/Flip] <Accept>:

Press ENTER to accept the extrude direction

Enter taper angle <0>: Press ENTER to accept the default

The extrusion direction is determined by your selection point on the wire.

You selected the upper half of the line to extrude the circle along the length

of the line. To extrude the circle in the opposite direction, select a location

below the midpoint of the line.

540 |Chapter 19 Creating and Editing Surfaces

The extruded surface should look like this.

2For more practice, choose Extrude again. Select the spline and then a location

on the line to determine the length and direction.

Because the line is obscured by the first surface you created, you may have

difficulty selecting it. Press CTRL as you select, to cycle through the objects.

Press ENTER when the line is highlighted.

3Use the Zoom Extents option of ZOOM to redisplay all the wireframes and

select the object for the next exercise.

Swept Surfaces

A swept surface is a wire cross section moved along a curved line called a rail.

You can use multiple cross sections and one or two rails. The lines on the

swept surface in the illustration are U and V display lines. Cross sections can

be dissimilar but you need to select them in order.

In this exercise, you use different combinations of cross sections and rails to

create four swept surfaces.

Creating Motion-Based Surfaces |541

To create a swept surface

1Use AMSWEEPSF to sweep two cross sections along a rail, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select the first cross section (1)

Select cross sections: Select the second cross section (2) and press ENTER

Select rails: Select line (3) and press ENTER

2In the Sweep Surface dialog box, choose OK to accept default settings.

A message tells you that four surfaces will be created. Choose Continue. The

surfaces should look like this.

542 |Chapter 19 Creating and Editing Surfaces

You can select the individual surfaces to see the shape of each one.

Because one of the cross sections has sharp corners, a single surface cannot

be created. Instead, four separate surfaces are created, each corresponding to

one side of the rectangular cross section. For more information, see “To sur-

face polylines with sharp corners” on page 550.

3Use the Extents option of ZOOM to redisplay all the wireframes and select the

object for the next exercise.

To sweep a spline along a rail

1Sweep one spline along a rail, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select spline (1) and press ENTER

Select rails: Select line (2) and press ENTER

2In the Sweep Surface dialog box, choose OK to accept the default settings.

Your surface should look like this.

Creating Motion-Based Surfaces |543

You created a nonuniform rational B-spline (NURBS) surface from a spline.

You can convert a NURBS surface into a part by adding thickness.

NOTE Save a copy of your NURBS surface if you will need it later. When you

thicken a surface, the original surface is consumed and disappears.

To convert a NURBS surface to a solid

1Use AMTHICKEN to convert a NURBS surface to a thin solid, responding to the

prompts.

Desktop Menu Surface ➤ Surface Thicken

Select surfaces to thicken: Select the surface

Select surfaces to thicken: Press ENTER

Select direction to thicken [Flip/Accept] <Accept>:

Flip to point the direction arrow down, and press ENTER

Thickness <1.0000>: Press ENTER

A solid is created, and a new part icon is displayed in the Browser.

2Use the Extents option of ZOOM to redisplay all the wireframes and select the

object for the next exercise.

A swept surface is useful when your design has different shapes at either end.

544 |Chapter 19 Creating and Editing Surfaces

To sweep dissimilar shapes

1Sweep two dissimilar shapes along two nonparallel rails, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select first shape (1)

Select cross sections: Select second shape (2) and press ENTER

Select rails: Select first rail (3)

Select rails: Select second rail (4)

2In the Sweep Surface dialog box, choose OK to accept the default settings.

The swept surface should look like this.

3Use the Extents option of ZOOM to redisplay all the wireframes and select the

object for the next exercise.

Creating Motion-Based Surfaces |545

To sweep multiple cross sections along two rails

1Sweep multiple cross sections along two rails, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections:

Select cross sections (1) through (5) in consecutive order and press ENTER

Select rails: Select first rail (6)

Select rails: Select second rail (7)

2In the Sweep Surface dialog box, choose OK to accept the default scale.

Because the cross sections have rounded corners, a single surface results. If

the cross section had square corners, three surfaces would have been created.

3Use the Extents option of ZOOM to redisplay all the wireframes and select the

object for the next exercise.

546 |Chapter 19 Creating and Editing Surfaces

Creating Skin Surfaces

A skin surface drapes over a wireframe model. After the wireframe is

removed, the surface retains the shape of the wireframe. Skin surfaces are

ruled, planar, lofted U, and lofted UV.

Ruled Surfaces

A ruled surface is a straight, flat shape stretched between two wires of any 3D

shape. You can create a ruled surface between any two nonintersecting wires

that can represent the top and the bottom. The top and bottom can be open

or closed wires. You can create a ruled surface from two augmented lines as

well, and from a single augmented line by adding thickness to it.

To surface two wires

1Use AMRULE to create the ruled surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select line (1)

Select second wire: Select line (2)

Creating Skin Surfaces |547

The ruled surface shows the surface normal, a short vertical line in one corner.

A surface normal shows where the surface starts and which direction is out.

If surface normal indicators are too small, use the DISPSF system variable to

change the size. In the Individual Surface Display dialog box, change the

value in the Normal Length field. Adjust the setting as needed.

You can create a ruled surface from two augment lines, or by adding width to

a single augmented line. Besides using the command method, you can access

AMAUGMENT in the Desktop menu by choosing Surface ➤ Create Wireframe

➤ Augmented Lines.

To create an augmented line on a surface

1Use AMAUGMENT to create an augmented line on the surface.

Command AMAUGMENT

Select surface wire or [Angle/Distance/Spacing]:

Select the leftmost wire of the surface

Select surface wire or [Angle/Distance/Spacing]: Press ENTER

When you use an augmented wire to create a surface, the vectors are ignored.

You specify a value for the width of the surface.

548 |Chapter 19 Creating and Editing Surfaces

To surface an augmented line

1Use AMRULE to create a surface from the augmented wire, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select the augmented line

Enter an option [Next/Accept] <Accept>: Press ENTER

Enter width (or) [Select second wire] <1.0000>: Press ENTER

The surface extends beyond the vectors to the specified width.

You can use this technique to create a ruled surface normal to any existing

ruled surface. First you create a parting line on the surface and project it to get

an augmented line, and then create the ruled surface from the augmented line.

2Undo the surfaces you created so that you can use the two original aug-

mented lines in subsequent exercises.

Desktop Menu Edit ➤ Undo

3Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Creating Skin Surfaces |549

To surface two arcs with different radii

1Create a surface from two arcs of different radii, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select arc (1)

Select second wire: Select arc (2)

The ruled surface should look like this.

2To experiment, use the previous example and select the arcs in a different order.

3Erase the surface you just created.

Desktop Menu Modify ➤ Erase

Select the surface and press ENTER.

If creating the surface was the last command, you can use UNDO.

4Create a surface again, selecting the arcs in reverse order.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select arc (2)

Select second wire: Select arc (1)

surface normal

550 |Chapter 19 Creating and Editing Surfaces

Selecting the arcs in different order changes the surface normal.

5Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

In the next exercise, you surface polylines. A surface follows a spline exactly

but approximates the polyline by a curve. The Polyline Fit default setting of

150 maintains all corners less than 150 degrees as sharp corners. In such

cases, multiple surfaces are created.

To surface polylines with sharp corners

1Use the Mechanical Options dialog box to adjust the Polyline Fit settings:

Desktop Menu Surface ➤ Surface Options

Choose the Surfaces tab and then choose Polyline Fit.

2In the Polyline Fit dialog box, change the angle setting to 0 and change the

length setting to inf (infinity) or a specific length longer than the longest line

segment.

surface

normal

Creating Skin Surfaces |551

Choose OK.

These settings force sharp corners to convert to a smooth curved surface.

3Choose OK to exit the Mechanical Options dialog box.

552 |Chapter 19 Creating and Editing Surfaces

4Use AMRULE to create a curved surface from polylines drawn with sharp cor-

ners, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select polyline (1)

Select second wire: Select polyline (2)

A continuous smooth curved surface is created.

5Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Now use the same polylines, but choose a fit angle to recognize sharp corners.

Use the Polyline Fit dialog box to change the angle setting until the image

tile resembles the angles you want to recognize as corners. Choose a setting

between 150 and 165 to recognize most corners.

Creating Skin Surfaces |553

To create surfaces with sharp angles

1Use AMOPTIONS to reset the fit angle to 150 and re-create the ruled surface.

Desktop Menu Surface ➤ Surface Options

2Erase the surface you just created.

Desktop Menu Modify ➤ Erase

3Use AMRULE to create three ruled surfaces from polylines drawn with sharp

corners, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select polyline (1)

Select second wire: Select polyline (2)

4A message tells you that three surfaces will be created. Choose Continue.

The three surfaces follow the sharp corners of the polylines.

554 |Chapter 19 Creating and Editing Surfaces

5Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Trimmed Planar Surfaces

A planar surface may be constructed from lines, arcs, splines, polylines, or

simply two locations, if the selected objects are closed and on the same plane.

The exterior shape of the 2D wire shape becomes the trimmed edge of the

surface. In this exercise, you create trimmed planar surfaces.

To create a planar trimmed surface using a closed polyline

1Use AMPLANE to create a planar trim surface from a closed polyline, respond-

ing to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar Trim

Specify first corner or [Plane/Wires]: _wire

Select wires: Select object (1)

Select wires: Press ENTER

The planar surface is trimmed, using the closed polyline as the border. The U

and V lines appear inside the border.

2Use the Extents option of ZOOM to redisplay all of the wireframes, and select

the object for the next exercise.

The closed polyline for the next exercise contains two interior circles that are

coplanar. You create a trimmed surface using the polyline and circles.

Creating Skin Surfaces |555

To create a trimmed planar surface using three closed polylines

1Create a planar trim surface from three polylines, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar Trim

Specify first corner or [Plane/Wires]: _wire

Select wires: Select object (1)

Select wires: Select interior circle (2)

Select wires: Select circle (3)

Select wires: Press ENTER

Instead of selecting the objects individually, you could also drag a crossing

window around all of them and press ENTER.

A trimmed planar surface is automatically trimmed to the largest boundary

created by the wire. As in this example, when closed areas exist inside the

boundary, these holes are trimmed out.

2Use the Extents option of ZOOM to redisplay all of the wireframes, and select

the object for the next exercise.

Lofted Surfaces

You can create a lofted surface from one or two sets of wires, each with similar

attributes, such as having approximately the same direction. You must select

the wires in consecutive order.

556 |Chapter 19 Creating and Editing Surfaces

A lofted U surface is stretched between any number of wires that share similar

characteristics. The example contains two sets of wires from which you create

two surfaces. The light blue polylines are approximately horizontal, and the

green lines are approximately vertical. First, you create a surface from the

horizontal polylines.

To create a lofted surface using a set of wires

1Use AMLOFTU to surface a set of vertical wires, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ LoftU

Select U wires: Select lines (1) through (8) in consecutive order and press ENTER

2In the Loft Surface dialog box, choose OK to accept the default settings.

Creating Skin Surfaces |557

3Surface a set of horizontal wires, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ LoftU

Select U wires: Select lines (9) through (18) in consecutive order and press ENTER

4In the Loft Surface dialog box, choose OK to accept the default settings.

The two surfaces, one horizontal and one vertical, should look like these.

5Use the Extents option of ZOOM to redisplay all the wireframes and select the

object for the next exercise.

A lofted UV surface is stretched over two sets of wires. Each wire in one set

crosses every wire in the other set. Two sets of wires can accurately describe

a complex surface.

You can select wires directly, as you did in the previous exercise, or you can

select two groups of wires. In this exercise, you create two groups of wires and

then create a lofted surface from the two groups. The wires in the U direction

are magenta (purple), and those in the V direction are cyan (light blue).

558 |Chapter 19 Creating and Editing Surfaces

To create a single lofted surface from two groups of wires

1Group the magenta U lines.

Command GROUP

In the Object Grouping dialog box specify:

Group Name: Enter uwires

Create Group: Choose New to close the dialog box

Respond to the prompt as follows:

Select objects: Select lines (1) through (7) in consecutive order and press ENTER

In the Object Grouping dialog box, choose OK.

2Press ENTER to repeat the GROUP command.

In the Object Grouping dialog box specify:

Group name: Enter vwires

Create Group: Choose New to close the dialog box

Respond to the prompt as follows:

Select objects: Select lines (8) through (13) in consecutive order and press ENTER

In the dialog box, choose OK.

Creating Derived Surfaces |559

3Use AMLOFTU to loft a surface from two groups of wires, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ LoftUV

Select U wires: Enter g

Enter group name: Enter uwires

7 found

Select U wires: Press ENTER

Select V wires: Enter g

Enter group name: Enter vwires

6 found

Select V wires: Press ENTER

Enter an option [eXit/Loft/Node check] <Loft>: Press ENTER

You have created a surface from the two groups of wires.

4Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Creating Derived Surfaces

Derived surfaces are generated from existing surfaces: blended, offset, fillet,

and corner fillet. Derived surfaces can be trimmed.

Blended Surfaces

You can create a blended surface between two, three, or four wires or surfaces.

The blended surface is tangent to the surfaces or wires from which it is created.

NOTE To create surfaces correctly, select lines at points shown in the illustrations.

560 |Chapter 19 Creating and Editing Surfaces

To create a blended surface

1Use AMBLEND to create a blended surface from two wires, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (1)

Select second wire: Select surface (2)

Select third wire [Weights]: Press ENTER

You have created the first blended surface.

The type of object you select affects the blended surface. When you select sur-

faces or augmented lines, you are prompted for the weight of the surface edge.

2Create the second blended surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (3)

Select second wire: Select surface (4)

Select third wire [Weights]: Press ENTER

Creating Derived Surfaces |561

3Create the third blended surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (5)

Select second wire: Select surface (6)

Select third wire [Weights]: Press ENTER

4Use ZOOM to enlarge the corner area created by the blended surfaces.

5Use AMBLEND to create a corner blended surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend.

Select first wire: Select surface (7)

Enter an option [next/Accept] <Accept>: Press ENTER

Select second wire: Select surface (8)

Enter an option [next/Accept] <Accept>: Press ENTER

Select third wire [Weights]: Select surface (9)

Select fourth wire: Press ENTER

The order in which you select the objects to blend determines the orientation

of the corner created by the blend.

562 |Chapter 19 Creating and Editing Surfaces

Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Next, you create a blended surface from two surfaces and lines. To create a

blended surface from four objects, make the selections in the order shown;

the objects cannot be selected in consecutive order.

To blend surfaces and lines

1Use AMBLEND to create a surface from two surfaces and two lines, responding

to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select surface (1)

Select second wire: Select surface (2)

Enter an option [Next/Accept] <Accept>: Press ENTER

Select third wire [Weights]: Select wire (3)

Select fourth wire: Select wire (4)

The new surface is created between the original surfaces and lines.

2Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Next, you create two surfaces, each blended from two augmented lines.

Creating Derived Surfaces |563

To blend augmented lines

1Use AMBLEND to create a surface from two augmented lines, responding to

the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select line (1)

Select second wire: Select line (2)

Select third wire [Weights]: Press ENTER

2Use ZOOM to redisplay wireframes. Then select the second set of lines.

3Create a surface from the second set of augmented lines, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select augmented line (1)

Select second wire: Select augmented line (2)

Select third wire [Weights]: Press ENTER

Compare these two surfaces to see how the direction of the augmented line

vectors affects the resulting surface.

4Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Offset Surfaces

An offset surface is a duplicate of an existing surface, offset by a specific dis-

tance. When you create an offset surface, you can keep the original or remove

it, as needed.

564 |Chapter 19 Creating and Editing Surfaces

To create an offset surface

1Use AMOFFSETSF to create an offset surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Offset

Select surfaces to offset: Select surface (1)

Select surfaces to offset: Press ENTER

Distance=1.0000 Keep=Yes

Enter offset distance or [Keep] <1.0000>: Enter k

Keep original surface(s) [Yes/No] <No>: Enter y

Distance=1.0000 Keep=Yes

Enter offset distance or [Keep] <1.0000>: Enter 0.5

The new surface is offset from the original surface, which is normal at all

locations.

2Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Creating Derived Surfaces |565

Fillet and Corner Surfaces

In this exercise, you create fillet surfaces between two selected surfaces, and

a corner fillet where three fillet surfaces intersect. You trim the original sur-

faces back to the fillet surfaces.

To create fillet and corner surfaces

1Use AMFILLETSF to create a fillet between two surfaces, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (1)

Select second surface: Select surface (2)

2In the Fillet Surface dialog box, specify:

Fillet Type: Constant

Trim: Both Surfaces

Create To: Surface Trim

Radius: Enter 0.5

Choose OK.

566 |Chapter 19 Creating and Editing Surfaces

3Create a fillet between another two surfaces, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (3)

Select second surface: Select surface (4)

4In the Fillet Surface dialog box, specify:

Fillet Type: Constant

Trim: Both Surfaces

Create To: Base Surface

Radius: Enter 0.75

Choose OK.

The Base Surface option was not available when you created the first fillet

surface. It is available now because the first surface was trimmed and now

differs from the base surface. Next, trim to the base surface, not the trimmed

surface.

Creating Derived Surfaces |567

The next illustration shows both fillets, which you will trim later.

5Create a fillet between another two surfaces, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Fillet

Select first surface or quilt interior edge: Select surface (5)

Select second surface: Select surface (6)

6In the Fillet Surface dialog box, specify:

Fillet Type: Constant

Trim: Both Surfaces

Create To: Base Surface

Radius: Enter 0.6

Choose OK.

The fillets overlap at the corner. You need to trim the overlap with a corner

fillet.

568 |Chapter 19 Creating and Editing Surfaces

To create a corner fillet

1Use AMCORNER to trim the overlapping fillets, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Corner Fillet

NOTE The default is set to trim the corner fillet to the three fillet surfaces. If you

do not want to trim, enter T at the first prompt and change the setting to No.

Trim=Yes

Select first fillet surface or [Trim]: Select surface (7)

Select first fillet surface or [Trim]: Select surface (8)

Select first fillet surface or [Trim]: Select surface (9)

The trimmed corner fillet looks like this.

2Use the Extents option of ZOOM and select the object for the next exercise.

Editing Surfaces |569

Editing Surfaces

As you create models, you need to combine surfaces and trim them where

they overlap. You will learn four surface editing techniques: adjusting sur-

faces, joining surfaces, trimming surfaces at intersections, and trimming

surfaces by projection.

Adjusting Adjacent Surfaces

You can control the tangency of two adjacent surfaces by adjusting them to

create one continuous surface. When you select the edges of two adjacent

surfaces to adjust, the first edge you select is the control surface. You can use

a quilt for the control surface. By default, 20 per cent of the total area of each

surface is adjusted. You can change the percentage for either or both of the

the adjustment areas, depending on which surface shape you need to retain.

To adjust adjacent surfaces

1Use AMADJUST to convert two surfaces into one surface, responding to the

prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Adjust

Select surface edge to adjust: Select the control surface edge (1)

Select surface edge to adjust: Select the adjacent surface edge (2)

570 |Chapter 19 Creating and Editing Surfaces

First surface=20.0000% Second surface=20.0000% cOntinuity=Smooth

Keep=No

Enter an option [First surface/Second surface/cOntinuity/Keep] <Continue>:

Enter s

Enter adjustment for the second surface <20.0000%>: Enter 40

First surface=20.0000% Second surface=40.0000% cOntinuity=Smooth

Keep=No

Enter an option [First surface/Second surface/cOntinuity/Keep] <Continue>:

Enter o

Continuity [Coincident/Smooth] <Coincident>: Press ENTER

First surface=20.0000% Second surface=40.0000% cOntinuity=Coincident

Keep=No

Enter an option [First surface/Second surface/cOntinuity/Keep] <Continue>:

Press ENTER

The two surfaces are adjusted to meet.

Joining Surfaces

You can join multiple surfaces into a single surface. Each surface is indicated

by two surface normal indicators.

To join surfaces

1Use AMJOINSF to join the surfaces you select, responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Join

Select surfaces to join: Select surface (1)

Select surfaces to join: Select surface (2)

Select surfaces to join: Press ENTER

Editing Surfaces |571

The two surfaces are joined. Only one surface normal indicator is shown.

To force two surfaces to join, choose Surface ➤ Surface Options. In the

Mechanical Options dialog box, choose the Surface tab and adjust the Join

Gap Tolerance. Two untrimmed surfaces are joined automatically if they are

within twice the gap tolerance.

2Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Trimming Intersecting Surfaces

You can trim intersecting surfaces, including quilted surfaces, and create a 3D

polyline at the intersection. The 3D polyline can then be used to create

another surface.

A 3D point is created at the intersection of a wire curve and a surface or quilt.

If the wire curve intersects the surface or quilt more than once, points are cre-

ated everywhere an intersection takes place.

When you trim, always make your selections on the portion of the surface

you want to keep.

572 |Chapter 19 Creating and Editing Surfaces

To trim intersecting surfaces

1Use AMINTERSF to trim the surface you want to keep, responding to the

prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Intersect Trim

Select first surface/quilt or wire: Select surface (1)

Select second surface: Select surface (2)

2In the Surface Intersection dialog box, check the options indicated in the fol-

lowing illustration and choose OK.

The first surface you selected is trimmed at its intersection with the second

surface.

Using the Trim options, you can trim neither, one, or both surfaces at their

intersection. As you change these options, the dynamic image in the dialog

box displays the results.

Editing Surfaces |573

3Use UNDO to erase the trim. Then try selecting surfaces at different locations.

4Use the Extents option of ZOOM to redisplay all of the wireframes and select

the object for the next exercise.

Trimming Surfaces by Projection

You can project a wire onto a surface to trim a shape that corresponds to the

wire shape. You select the portion of the surface you want to keep.

In this exercise, you trim a curved surface with a star-shaped polyline.

To trim a surface by a projected wire

1Use AMPROJECT to project the wire to trim the surface, responding to the

prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select polyline (1) and press ENTER

Select target surfaces/quilts: Select surface (2) on the side you want to keep

Select target surfaces/quilts: Press ENTER

574 |Chapter 19 Creating and Editing Surfaces

2In the Project to Surface dialog box, specify:

Direction: Choose Normal

Output Type: Choose Trim Surface

Keep Original Wire: Check the check box

Choose OK.

The polyline is projected onto the curved surface, trimming out the surface

inside the polyline.

3Use UNDO and try different selection points and output types for the

projection.

575

In This Chapter 20

Combining Parts and

Surfaces

In Autodesk® Mechanical Desktop®, surfaces are

valuable features because they can represent complex

curved shapes. When joined to a parametric part, they

cut away an angular surface and replace it with a

sculpted face. A surface may also add material to a part

as a protrusion. In this tutorial, you combine parametric

and surface modeling by creating a camera body with a

sculpted face.

■Creating a part with multiple

features

■Creating a simple surface

■Attaching a surface

parametrically to a part

■Cutting out features

■Creating mounting holes

■Sketching on work planes

■Revising and finishing a design

576 |Chapter 20 Combining Parts and Surfaces

Key Terms

Te r m Definition

base surface A basic underlying surface that carries a shape across a larger area. Can be trimmed

to precise shapes as needed, but the base surface remains intact and may be

displayed.

model view Changes orientation of the viewer so that the object is viewed from a different

position. Individual views can be displayed in multiple viewports. For example, enter

3 at the Command prompt to create three viewports with default views: top, front,

and right isometric.

NURBS Acronym for nonuniform rational B-spline. The SPLINE command creates a true

NURBS curve and can be used to create a surface.

rail One or more curved lines along which surfaces are swept. They form the curvature of

a swept surface.

spline A curved line defined by specified control points that assumes a unique shape. Used

to create curved surfaces. The radius of a spline curve is constantly changing. Splines

are used as the basis of free-form surfaces.

surface cut A feature created when a surface is joined to a part. Where the surface cuts the part

or protrudes, the part face assumes the curved shape of the surface. The surface, like

other features, is parametric; both the surface and the part retain their parametric

relationship whenever either is modified.

wire A generic term referring to lines, arcs, circles, ellipses, 2D and 3D polylines,

augmented lines, and splines.

work plane An infinite plane attached to a part. Can be designated as a sketch plane and can be

included in a constraint or dimension scheme. Work planes can be either parametric,

or non-parametric.

work point A parametric work feature used to position a hole, the center of a pattern, or any

other point for which there is no other geometric reference.

Basic Concepts of Combining Parts and Surfaces |577

Basic Concepts of Combining Parts and

Surfaces

You can use Mechanical Desktop® to create angular-shaped parts. You can

apply 3D surfaces to those parts to create hybrid parts consisting of a mixture

of angular and curved shapes. With Mechanical Desktop you can create

model designs with shapes of varying types.

You can apply surfaces to Mechanical Desktop parts and use those surfaces to

cut material from a parametric part, to create any hybrid shapes that your

design requires.

You can also use surfaces to add material to angular parts.

Using Surface Features

A feature created from surfaces has the shape of a contoured surface. You

either cut away material or add material as a protrusion to join it to a part.

In this tutorial, you cut away an angular face and replace it with a sculpted

surface.

Surfaces must have these characteristics to be used as features on models:

■A contoured surface must have four logical boundaries.

■The curved shape must be a single surface. If you need multiple surfaces

to represent the shape, you must join them into a single surface.

■The surface must be a nontrimmed base surface. Join only base surfaces,

not interior trim edges of trimmed surfaces.

■The surface must extend past the part on all four sides.

■A surface cannot contain sharp corners.

■Surfaces should have a minimum number of internal patches. These sur-

faces work better and faster than complex ones.

before surface cut after surface cut

578 |Chapter 20 Combining Parts and Surfaces

First, sketch the camera from all sides (top, side, front, and isometric views).

With a complete idea, you can decide where to place features on the camera

body.

The camera body, which is common to all other features, is the base feature.

The camera design has many other features, some of which are cutaways

from the body: battery and film compartments and cutouts for their doors;

mounting holes for the film advance and shutter release; and compartments

for the viewfinder and the flash. The lens sheath feature, a sculpted surface,

is joined to the camera face.

battery compartment

shutter release mount film advance mount

film compartment

viewfinder

compartment

flash compartment

lens sheath

door cutout

Creating Surface Features |579

Creating Surface Features

Open the file camera.dwg in the desktop\tutorial folder. The file contains the

settings you need, and the geometry to create the camera body—an extruded

feature and some NURBS curves. You use NURBS to create the surface for the

sculpted camera face.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

You can work on your model in any viewport, moving among views as you

create features.

First, you create two surfaces by sweeping wires along a rail. Then, you join

them into a single surface and extend the surface so that it covers the camera

body.

NOTE If you prefer to use toolbuttons to access commands, choose Surface ➤

Launch Toolbar.

580 |Chapter 20 Combining Parts and Surfaces

To create a swept surface

1Use AMSWEEPSF to sweep a spline along a rail, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: In the front view, choose the right horizontal spline (1)

Select cross sections: Press ENTER

Select rails: Select the vertical spline (2)

Select rails: Press ENTER

2In the Sweep Surface dialog box, specify:

Orientation: Parallel

Choose OK. The first half of the swept surface is created.

3Create the second half of the swept surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select the left horizontal spline (3)

Select cross sections: Press ENTER

Select rails: Select the vertical spline (2)

Enter an option [Next/Accept] <Accept>: Press ENTER

Select rails: Press ENTER

In the Sweep Surface dialog box, specify:

Orientation: Parallel

Choose OK.

3 1

Creating Surface Features |581

4Use AMJOINSF to join the two surfaces, responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Join

Select surfaces to join: Select the right surface (1)

Select surfaces to join: Select the left surface (2) and press ENTER

The two surfaces create a single surface. The resulting surface probably does

not extend beyond the part on all sides, so you need to lengthen the surface.

5Use AMLENGTHEN to lengthen the surface, responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Lengthen

Base edge=Single Extension=Percent Method=Parabolic Value=110.0000%

Select surface edge or spline [eDge/Extend/Keep/Mode/Value]: Enter v

Enter percent <110.0000%>: Enter 105

Base edge=Single Extension=Percent Method=Parabolic Value=105.0000%

Select surface edge or spline [eDge/Extend/Keep/Mode/Value]:

Select the rightmost vertical edge of the surface (1)

Base edge=Single Extension=Percent Method=Parabolic Value=105.0000%

Select surface edge or spline [eDge/Extend/Keep/Mode/Value]: Press ENTER

The surface now extends past the cube representing the camera body.

582 |Chapter 20 Combining Parts and Surfaces

Attaching Surfaces Parametrically

Next, you create a work plane and work point and then dimension the work

point to the part. This dimension establishes a parametric relationship

between the surface and the part. The position of the surface is controlled by

the work point, and its orientation is controlled by the work plane associated

with the work point. Later, if you modify the position of the work point, the

surface location moves accordingly.

To position the work plane and work point easily, work in the isometric view.

To attach a surface to a part

1Use AMWORKPLN to create a work plane.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

In the Work Plane Feature dialog box, specify:

1st Modifier: Planar Parallel

2nd Modifier: Offset

Offset: Enter 1

Create Sketch Plane: Select the check box

Choose OK.

2Position the offset work plane on the part, responding to the prompts.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the front face of the camera (1)

Enter an option [Next/Accept] <Accept>:

Choose n to cycle to the front face, or press ENTER

Enter an option [Flip/Accept] <Accept>:

Choose f to flip the direction arrow away from the camera body, or press ENTER

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Verify that the UCS icon is upright and press ENTER

Attaching Surfaces Parametrically |583

You have created a parallel work plane offset from the front face of the part.

3Use AMWORKPT to place a work point on the work plane, responding to the

prompts.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Point.

Workpoint will be placed on the current sketch plane.

Specify the location of the workpoint: Specify a location (2)

You have created a work point on the sketch plane.

4Use AMPARDIM to constrain the work point to the camera body, responding

to the prompts.

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

➤ New Dimension.

Select first object: Select the work point (3)

Select second object or place dimension:

Select the right edge of the camera body (4)

Specify dimension placement: Place the horizontal dimension (5)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<1.3316>: Enter 1

Solved underconstrained sketch requiring 1 dimensions or constraints.

584 |Chapter 20 Combining Parts and Surfaces

5Continue on the command line.

Select first object: Select the work point

Select second object or place dimension:

Select the bottom edge of the camera body

Specify dimension placement: Place the vertical dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.8898>: Enter 1

Solved fully constrained sketch.

Select first object: Press ENTER

The work point is fully constrained.

Save your file.

Cutting Parts with Surfaces

Now that the surface is positioned relative to the camera body, you can use

it to cut away material from the planar camera face.

To cut away from a part

1Use AMSURFCUT to create a surface cut, responding to the prompts.

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

Features ➤ Surface Cut.

(Type: Cut)

Select surface or [Type]: Select the surface

Select work point: Select the work point

Specify portion to remove: [Flip/Accept] <Accept>:

Verify the direction arrow points away from the camera body and press ENTER

Cutting Parts with Surfaces |585

One side of the part is cut away, leaving the curved face of the surface. Your

model shows the modified block and the splines used to create the surface.

2Use REGENALL to regenerate the drawing views.

Desktop Menu View ➤ Regen All

3Remove the three splines used to create the surface.

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

➤ Erase.

4Select the three splines and press ENTER.

Save your file.

586 |Chapter 20 Combining Parts and Surfaces

Creating Extruded Features

The film compartment at the back of the base feature has two features—the

compartment and the door.

The camera back is a flat plane. You specify it as the sketch plane, sketch the

profile, and extrude it directly into the camera body.

To sketch the film compartment

1Use AMSKPLN to create a new sketch plane, responding to the prompts. Work

in the isometric view.

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

Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the back face of the camera (1)

Enter an option [Accept/Next] <Accept>:

Choose n to cycle to the back face, or press ENTER

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Select the bottom edge of the camera (2)

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Verify that the X axis is pointing to the left and press ENTER

The back of the camera has been specified as the sketch plane. In the isomet-

ric view, the UCS icon is displayed with the X axis pointing left.

Next, change the view to see the back of the camera. If needed, zoom out to

see the entire back of the camera.

2Change the front view to a back view.

Desktop Menu View ➤ 3D Views ➤ Back

Creating Extruded Features |587

3Use RECTANG to sketch a rectangle to the left on the camera back.

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

➤ Rectangle.

4Use AMPROFILE to create a profile from the sketch.

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

➤ Single Profile.

You need to place four dimensions or constraints: two to define the sketch

size and two to specify the sketch location on the camera body.

To add dimensions and constraints to the film compartment sketch

1Use AMPARDIM to dimension the width of the rectangle, responding to the

prompts.

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

➤ New Dimension.

Select first object: Select the bottom horizontal line of the sketch (1)

Select second object or place dimension: Specify a location (2)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<3.7546>: Enter 4

Solved underconstrained sketch requiring 3 dimensions or constraints.

2Define the height of the rectangle.

Select first object: Select the left vertical line of the sketch (3)

Select second object or place dimension: Specify a location (4)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<2.6011>: Enter 2.5

Solved underconstrained sketch requiring 2 dimensions or constraints.

Select first object: Press ENTER

588 |Chapter 20 Combining Parts and Surfaces

3Make the isometric view active.

To see the dimensions and the profile sketch more clearly, rotate the isomet-

ric view until the back of the camera faces you.

Desktop Menu View ➤ 3D Views ➤ Back Left Isometric

Define the distance between the top of the sketch and the top of the camera

back.

4Use AMPARDIM to constrain the rectangle to the camera body, responding to

the prompts.

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

➤ New Dimension.

Select first object: Select line (1)

Select second object or place dimension: Select line (2)

Specify dimension placement: Specify a location (3)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.2355>: Enter .1626

Solved underconstrained sketch requiring 1 dimensions or constraints.

5Define the distance between the right side of the sketch and the right edge

of the camera back.

Select first object: Select line (4)

Select second object or place dimension: Select line (5)

Specify dimension placement: Specify a location (6)

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.8583>: Enter .8426

Solved fully constrained sketch.

Select first object: Press ENTER

Next, cut the film compartment from the camera body.

3 2 1

Creating Extruded Features |589

To cut the film compartment

1Use AMEXTRUDE to cut the film compartment from the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Blind

Distance: Enter 1.2

Flip: Point the direction arrow into the camera body

Choose OK.

The cut-out compartment is displayed in all four views.

590 |Chapter 20 Combining Parts and Surfaces

2Activate and then restore the viewports to the original orientation.

Upper right viewport: Front Right Isometric View

Lower left viewport: Front View

Cutting the door is similar to cutting the film compartment. You sketch a

rectangle on the right side of the camera and blindly extrude it as a cut into

the camera body.

To sketch the film compartment door

1Use AMSKPLN to create a new sketch plane, responding to the prompts. Work

in the isometric view.

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

Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the side face of the camera (1)

Enter an option [Accept/Next] <Accept>:

Verify that the side face is highlighted and press ENTER

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Verify that the Z axis points away from the camera and press ENTER

Creating Extruded Features |591

2Set the UCS origin to the lower-left corner of the right side of the camera,

responding to the prompts.

Desktop Menu Assist ➤ New UCS ➤ Origin

Specify new origin point <0,0,0>: Enter end

of: Specify a point near the lower-left corner of the side view

NOTE If the UCS icon does not snap to the lower-left corner of the camera,

set the AutoCAD system variable UCSICON to On.

3In the side view, zoom in on the camera face.

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

4Hold down the left mouse button to size the view, and then press ENTER to

end the command.

5Sketch a rectangular shape for the door cutout.

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

➤ Rectangle.

6Create the profile sketch.

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

➤ Single Profile.

You need four dimensions or constraints to solve the sketch. Add constraints

that define the location of the profile on the camera side.

592 |Chapter 20 Combining Parts and Surfaces

To constrain the film compartment door

1Use AMADDCON to make the bottom edge of the profile sketch collinear with

the bottom line of the film compartment, responding to the prompts.

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

Constraints ➤ Collinear.

Valid selection(s): line or spline segment

Select object to be reoriented: Select line (1)

Valid selection(s): line or spline segment

Select object to be made collinear to: Select line (2)

Solved underconstrained sketch requiring 3 dimensions or constraints.

2Make the right side of the profile sketch collinear with the right edge of the

camera body.

Valid selection(s): line or spline segment

Select object to be reoriented: Select line (3)

Valid selection(s): line or spline segment

Select object to be made collinear to: Select line (4)

Solved underconstrained sketch requiring 2 dimensions or constraints.

Valid selection(s): line or spline segment

Select object to be reoriented: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

Creating Extruded Features |593

3Use AMPARDIM to dimension the width and height of the profile sketch,

responding to the prompts.

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

➤ New Dimension.

Select first object: Select a horizontal profile edge

Select second object or place dimension: Place the horizontal dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.6840>: Enter .6

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Select a vertical profile edge

Select second object or place dimension: Place the vertical dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<2.3218>: Enter 2.5

Solved fully constrained sketch.

Select first object: Press ENTER

The horizontal dimension makes the width of the profile equal to half the

depth of the film compartment and the height of the profile equal to the

height of the compartment.

For practice, express the width and height of the profile as equations.

To cut the film compartment door

1Use AMEXTRUDE to cut the profile from the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Blind

Distance: Enter .1574

Flip: Point the direction arrow into the camera

594 |Chapter 20 Combining Parts and Surfaces

2Choose OK to create the extrusion.

Save your file.

The battery compartment also has a cutout for a door. The order in which

you create these features does not matter, but the natural order would be to

create the film compartment first.

The cutout for the battery compartment is more complicated because of its

shape. The key to creating this feature is to locate the sketch plane properly

on the bottom left side of the camera body.

NOTE Watch the UCS icon in the isometric view and make sure it is positioned

on the bottom of the camera.

To sketch the battery compartment

1Change the top view to a bottom view.

Desktop Menu View ➤ 3D Views ➤ Bottom

2Use AMSKPLN to create a new sketch plane, responding to the prompts. Work

in the isometric view.

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

Plane.

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Select the bottom face of the camera (1)

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Verify that the Z axis arrow points down, away from the camera body

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Verify that the X axis points to the left and press ENTER

Creating Extruded Features |595

3Use PLINE to sketch the profile of the battery compartment on the bottom of

the camera body. Work in the bottom view.

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

➤ Polyline.

4Use AMPROFILE to create the profile sketch.

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

➤ Single Profile.

The sketch needs seven to nine dimensions or constraints, depending on

how precisely you drew the sketch. If you need more than seven constraints,

you need to add some missing geometric constraints.

To constrain the battery compartment

1Use AMSHOWCON to view the current geometric constraints.

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

Constraints ➤ Show Constraints.

2Add any missing geometric constraints.

Typically, the radial (R) constraints and one of the tangent (T) constraints are

missing from the arcs.

NOTE When you add constraints, the sketch shape might become distorted,

but you can restore it when you complete the dimensions. Dimension the largest

vertical dimension and the arcs before you dimension smaller objects.

596 |Chapter 20 Combining Parts and Surfaces

3Use AMPARDIM to add the following dimensions.

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

➤ New Dimension.

The sketch is fully constrained.

To cut the battery compartment

1Use AMEXTRUDE to cut the profile from the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Blind

Distance: Enter 2.4

Flip: Point the direction arrow into the camera body

Choose OK.

The door opening of the battery compartment is located on the same plane

as the battery compartment. Therefore, you need only to sketch and con-

strain a rectangle, cutting it into the camera body to the proper depth.

Creating Extruded Features |597

To sketch and constrain the battery compartment door

1Use RECTANG to sketch the profile of the cutout. Work in the bottom view.

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

➤ Rectangle.

2Use AMPROFILE to create the profile sketch.

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

➤ Single Profile.

The sketch requires four dimensions or constraints.

3Use AMADDCON to constrain the sketch to the bottom of the camera body.

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

Constraints ➤ Collinear.

Select lines that make the outside edges of the sketch collinear with the out-

side edges of the camera body.

4Use AMPARDIM to dimension the length and width of the profile sketch,

responding to the prompts.

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

➤ New Dimension.

Select first object: Select the narrow side of the rectangle

Select second object or place dimension: Place the horizontal dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<0.7463>: Enter .76

Solved underconstrained sketch requiring 1 dimensions or constraints.

Select first object: Select the long side of the rectangle

Select second object or place dimension: Place the vertical dimension

Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace]

<1.1274>: Enter 1.3

Solved fully constrained sketch.

Select first object: Press ENTER

The sketch is fully constrained.

598 |Chapter 20 Combining Parts and Surfaces

To cut the battery compartment door

1Use Extrude to cut the door opening from the camera body. Make sure the

direction of the cut is into the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Blind

Distance: Enter .1574

Flip: Point the direction arrow into the camera body

Choose OK.

Save your file.

Creating Holes

Both the shutter release and the film advance mounts are counterbored holes

that you can create as placed features.

To create shutter release and film advance mount holes

1Change the upper-left viewport to a top view.

Desktop Menu View ➤ 3D Views ➤ Top

2Zoom in to enlarge the view as needed, and then activate the isometric view.

3Use AMHOLE to place the holes for the shutter release and the film advance.

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

Features ➤ Hole.

Creating Holes |599

In the Hole dialog box, select the Counterbore hole type icon and specify:

Termination: Blind

Placement: 2 Edges

Dia: Enter .5

Depth: 1.0

Pt. Angle: Enter 180

C’Dia: Enter .65

C’Depth: Enter 1

Choose OK.

4Respond to the prompts as follows:

Select the first edge: Select the top, back edge in the isometric view (1)

Select the second edge: Select the top, left edge in the isometric view (2)

Specify the hole location: Specify a location (3)

Enter the distance from first edge (highlighted) <0.4146>: Enter .5

Enter the distance from second edge (highlighted) <4.3456>: Enter 4.25

Select the first edge: Press ENTER

600 |Chapter 20 Combining Parts and Surfaces

A hole is created for the film advance component.

5Press ENTER to redisplay the Hole Feature dialog box. Specify:

Operation: C’Bore

Termination: Blind

Placement 2 Edges

Drill Size: Custom, enter .2 diameter, 1.0 depth, and 180 degrees point angle

C’bore/Sunk Size: Enter .3 diameter and .1 depth and choose OK

6Respond to the prompts as follows:

Select the first edge: Select the top, back edge in the isometric view

Select the second edge: Select the top, left edge in the isometric view

Specify the hole location: Specify a location

Enter the distance from first edge (highlighted) <0.6946>: Enter .85

Enter the distance from second edge (highlighted) <1.7487>: Enter 1.6

Select the first edge: Press ENTER

A hole is created for the shutter release mount.

Save your file.

Creating Features on a Work Plane |601

Creating Features on a Work Plane

The camera body is complete except for features on the camera face. Unlike

the previous features, you sketch these features on a work plane parallel to

the front of the camera. You extrude the features from the work plane and

into the camera body to the correct depth.

You sketch on the work plane because 2D sketches cannot be drawn and pro-

filed on a NURBS surface.

The lens sheath, a hollow cylinder joined to the face of the camera, has two

features: a solid cylinder and a circle used to cut out the center of the

cylinder.

To extrude the lens sheath on a work plane

1Use AMWORKPLN to create a new work plane on which to locate the sketch

plane.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Work Plane.

In the Work Plane Feature dialog box, specify:

1st Modifier: Planar Parallel

2nd Modifier: Offset

Offset: Enter 1.25

Create Sketch Plane: Select the check box

Choose OK.

602 |Chapter 20 Combining Parts and Surfaces

2Respond to the prompts as follows:

Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]:

Specify a point (1)

Enter an option [Next/Accept] <Accept>:

Press ENTER when the front of the camera is selected

Enter an option [Flip/Accept] <Accept>:

Verify that the work plane is offset from the camera front and press ENTER

Plane = Parametric

Select edge to align X axis or [Flip/Rotate/Origin] <Accept>:

Point the Z axis away from the camera front and press ENTER

The work plane is created in front of the camera face. Because the sketch

plane is specified on the work plane, the UCS icon is also displayed on the

work plane.

3Use CIRCLE to sketch a circle in front of the camera face. Work in the front

view.

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

➤ Circle.

4Use AMPROFILE to create the profile sketch.

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

➤ Single Profile.

Creating Features on a Work Plane |603

To position the circle, you need three dimensions or constraints: a diameter

and two dimensions to locate the circle on the sketch plane relative to the

camera body.

5Use AMPARDIM to dimension the sketch with the following values.

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

➤ New Dimension.

6Use EXTRUDE to extrude the profile to create the outer cover of the lens

sheath. Work in the isometric view.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Join

Termination: Blind

Distance: Enter 1.25

Flip: Point the direction arrow into the camera body

Choose OK.

The lens sheath is complete. Now, cut a smaller cylinder to hollow out the

sheath.

604 |Chapter 20 Combining Parts and Surfaces

To hollow out the lens sheath

1Activate the front view, and sketch a circle on the work plane.

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

➤ Circle.

2Profile the sketch.

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

➤ Single Profile.

Three dimensions or constraints are needed to solve the sketch.

3Use AMADDCON to constrain the sketch to be concentric with the lens

sheath, responding to the prompts.

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

Constraints ➤ Concentric.

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Select the small circle

Valid selection(s): arc, circle, ellipse, or work point

Select object to be made concentric to: Select the large circle

Solved underconstrained sketch requiring 1 dimensions or constraints.

Valid selection(s): arc, circle, or ellipse

Select object to be reoriented: Press ENTER

Enter an option

[Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix]

<eXit>: Press ENTER

4Use AMPARDIM to dimension the sketch to the value shown.

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

➤ New Dimension.

5Make the isometric view active and use AMEXTRUDE to extrude the sketch to

hollow out the lens sheath.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

Creating Features on a Work Plane |605

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Through

Flip: Point the direction arrow into the camera body

Choose OK.

Save your file.

Next, you create the viewfinder compartment, a filleted rectangle that is cut

from the camera face.

To cut the viewfinder compartment

1Use RECTANG to sketch a rectangle on the sketch plane above the lens sheath.

Work in the isometric view.

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

➤ Rectangle.

2Use FILLET to define the fillet for the corners of the rectangle, responding to

the prompts.

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

➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.5000

Select first object or [Polyline/Radius/Trim]: Enter r

Specify fillet radius <0.5000>: Enter .1, and choose OK.

3Press ENTER to restart FILLET. Apply the fillet, responding to the prompts.

Current settings: Mode = TRIM, Radius = 0.1000

Select first object or [Polyline/Radius/Trim]: Enter p

Select 2D polyline: Specify the rectangle

606 |Chapter 20 Combining Parts and Surfaces

4Use AMPROFILE to create the profile sketch.

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

➤ Single Profile.

You need five or more dimensions or constraints to solve the sketch. Add the

dimensions for the length and width of the shape, one dimension for the fil-

lets, and two dimensions to locate the sketch in relationship to the camera

body.

5In the front view, zoom in to enlarge the model as needed.

6Use AMPARDIM to add the following dimensions.

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

➤ New Dimension.

7Use AMEXTRUDE to cut the sketch through the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Through

Flip: Point the direction arrow into the camera body

Choose OK.

The last feature is the flash compartment. It has a shape similar to the view-

finder but is larger and located in the upper-right corner of the camera face.

Creating Features on a Work Plane |607

To cut the flash compartment

1Sketch a rectangle to the right of the viewfinder.

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

➤ Rectangle.

2Define a fillet for the corners of the rectangle, responding to the prompts.

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

➤ Fillet.

Current settings: Mode = TRIM, Radius = 0.5000

Select first object or [Polyline/Radius/Trim]: Enter r

Specify fillet radius <0.5000>: Enter .1

3Press ENTER to restart FILLET. Apply the fillet, responding to the prompts.

Current settings: Mode = TRIM, Radius = 0.1000

Select first object or [Polyline/Radius/Trim]: Enter p

Select 2D polyline: Specify the rectangle

4Create the profile sketch.

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

➤ Single Profile.

You need five or more dimensions or constraints to solve the sketch, just as

you did when you sketched the viewfinder. Dimension the length, width,

and the fillets, and locate the sketch in relationship to the camera body.

Zoom in on the front view as needed.

5Use AMADDCON to make the top and right edges of the sketch collinear with

the upper-right corner of the film compartment.

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

Constraints ➤ Collinear.

608 |Chapter 20 Combining Parts and Surfaces

6Add the following dimensions.

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

➤ New Dimension.

7Extrude the sketch to cut it through the camera body.

Context Menu In the graphics area, right-click and choose Sketched &

Work Features ➤ Extrude.

In the Extrusion dialog box, specify:

Operation: Cut

Termination: Through

Flip: Point the direction arrow into the camera body

Choose OK.

Save your file.

Modifying Designs |609

Modifying Designs

As with all projects, designs change during the development process. For

example, you might want to scale the camera to a smaller size and change

the dimension that positions the camera face on the solid model. Because

you want both the surface and the camera body at the same scale, you first

resize them.

In this exercise, you specify a percentage of the camera’s current size. Then,

to position the surface on the camera proportionately, you modify the para-

metric dimension.

To scale the camera body and face

1Zoom in to magnify the isometric view.

2Use SCALE to reduce the scale of the part, responding to the prompts.

Desktop Menu Modify ➤ Scale

Select objects: Select the camera and press ENTER

Specify base point: Select the rear corner of the camera

Specify scale factor or [Reference] <1.0000>: Enter .9 and press ENTER

The camera and surface are resized to 90 percent of their original size. The

surface and other features retain their original geometric relationships.

full-scale camera body scaled camera body

610 |Chapter 20 Combining Parts and Surfaces

To reposition the camera face

1Use AMEDITFEAT to edit the surfcut feature, responding to the prompts.

Context Menu In the graphics area, right-click and choose Edit Features

➤ Edit.

Enter an option [Sketch/surfCut/Toolbody/select Feature] <select Feature>:

Enter c

Select surfcut feature: Select a curved edge of the surface

The original sketch, work plane, and work point are displayed.

2Use AMMODDIM to modify the dimension that positions the surface to the

work point, responding to the prompts.

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

➤ Edit Dimension.

Select dimension to change: Select the horizontal dimension

New value for dimension <0.9>: Enter .75

Select dimension to change: Press ENTER

3Use AMUPDATE to update the part.

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

The surface is repositioned on the camera with the new value.

Finishing Touches on Models |611

Finishing Touches on Models

The finishing touch for the camera body is to fillet the corners where the dif-

ferent sides meet.

To finish the camera body

1Use AMVISIBLE to hide the work plane from your display.

Desktop Menu Part ➤ Part Visibility

2In the Desktop Visibility dialog box, select the Part tab and choose Work

Planes and Hide. Choose OK.

3Use ISOLINES to increase the number of isolines. Change the value to 8 to

show more detail on the model. The display will change when you edit your

model.

4Use AMFILLET to fillet the camera body.

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

Features ➤ Fillet.

5In the Fillet dialog box, specify Constant using a fillet radius of .05. Select

Return to Dialog and choose Apply.

NOTE To speed up filleting a complex model, select only a few lines at a time.

Repeat the command with more lines until the filleting is finished.

612 |Chapter 20 Combining Parts and Surfaces

6Fillet the outside corners and edges of the camera body. When you are

finished, choose Done.

The camera body is finished.

613

In This Chapter 21

Surfacing Wireframe

Models

This Autodesk® Mechanical Desktop® tutorial introduces

wireframe surface modeling, one of the key uses for

surface modeling. You learn how to develop a strategy for

a surfacing project, and how to achieve the design intent.

The tutorial provides instructions for surfacing a

wireframe model of a pump housing. The wireframe is

the outline of a pump housing, and the only data you

have to work with.

You should already know how to create surfaces before

you begin this tutorial. If you do not, complete the

exercises in chapter 19, “Creating and Editing Surfaces.”

■Studying the design intent and

developing a strategy

■Identifying logical surface areas

■Identifying base surface areas

■Using creative techniques to

surface a wireframe model

■Verifying surfacing results

614 |Chapter 21 Surfacing Wireframe Models

Key Terms

Te r m Definition

base surface A basic underlying surface that carries a shape across a larger area. Can be trimmed

to precise shapes as needed, but the base surface remains intact and may be

displayed.

logical surface area An area that can be described by a single surface.

projected wire A 2D line that represents an opening on a surface and trims a hole in the surface.

Can also be a 3D polyline that represents the extents of the opening in the

wireframe.

watertight Surfaces conform to the wireframe model; gaps between surfaces are within

allowable tolerances.

Basic Concepts of Surfacing Wireframe Models |615

Basic Concepts of Surfacing Wireframe

Models

A completely surfaced model is a single electronic master suitable for engi-

neering and manufacturing activities, such as:

■Generating accurate sections for engineering and packaging studies.

■Providing input for finite element modeling and analysis.

■Producing shaded renderings for marketing.

■Providing input for rapid prototyping equipment.

■Supplying rotated surfaces for tool, mold, and die design.

■Supplying surfaces for numerical control machining of models and tools.

In this tutorial, building on your knowledge of surface types, you examine

the wireframe to be surfaced and determine which surface will produce the

best results.

Discerning Design Intent

Because wireframe models have complex shapes, they are usually made up of

many surfaces joined together. For a model like the pump housing, you will

use many different individual surfaces to completely define it. When you sur-

face a wireframe model, you complete its design.

Before you begin, analyze the design and then plan how you can achieve

your design goals. This process of planning before you begin modeling can

help you avoid errors. For example, you usually follow these steps for wire-

frame modeling:

■Study the data to understand the design intent.

■Identify the location and extent of each surface area.

■Identify the base surface area(s) that can be trimmed later to adjacent sur-

faces and wires.

■Determine where you can use trimmed planar (flat) surfaces.

■Decide on the best surface types and approach for combining them.

■Create additional geometry as needed to resolve problem areas.

■Verify your surfacing results.

■Add the finishing touches to a watertight model.

616 |Chapter 21 Surfacing Wireframe Models

Review the wireframe in detail, to determine where you will have design

challenges.

Consider the following:

■The complexity of the surfaces you need to create. For example, what

curvature is required of surfaces? Is it sufficient to have surfaces with no

curvature (such as ruled surfaces), or do you need surfaces with multiple

curvatures?

■How you can simplify shapes. Surfaces created from polylines or splines

with a large number of points are complex and greatly increase computa-

tion time.

■Which surfaces are continuous. Continuous surfaces are smoother and

take less time to compute. You can set preferences so that lines with breaks

or changes in curvature aren’t converted to splines.

■Are default preference settings appropriate for the model. Allow as much

tolerance as is practical to avoid converting polylines to splines. Splines

take longer to compute than polylines—a factor that becomes more

important with complex models.

Identifying Logical Surface Areas

Once you determine the intent of the pump design, you get an idea of the

requirements for creating its shape and for constructing it. Identify the loca-

tion and extent of each logical surface area—an area that can be described by

a single surface.

A surface must be smooth and free of sharp breaks. Often, an individual sur-

face area is clearly-defined because it is surrounded by sharp break lines on

all sides. The pump top is a surface because it is surrounded by sharp edges

on three sides. The fourth edge is the end of the part.

Basic Concepts of Surfacing Wireframe Models |617

Likewise, the side of the top part of the pump constitutes a single surface.

Each of these two surface areas requires a surface because no single surface

could cover both.

Surfaces can contain multiple wires.

All lines inside the four boundaries share the same smooth curvature as the

boundary edges. There are no abrupt curvature changes, so the goal is to sur-

face the entire area with a single surface, using the additional wires to con-

strain the surface shape.

Identifying Base Surface Areas

The bottom of the pump housing appears to be a smoothly-curved area.

However, at the top edge, there is an almost 90-degree bend. Also, a flanged

area is formed by a slot opening in the otherwise smooth area.

The primary guideline in wireframe surfacing is to create an acceptable sur-

face first. Later, add a hole by trimming the surface with the shape of the

hole.

wireframe surface

pump housing close-up

top edge

618 |Chapter 21 Surfacing Wireframe Models

In general, use only smooth wires to create surfaces. When you use a wire

with sharp corners, those sharp areas do not produce an acceptable surface.

You need to find some other way to surface the area. Consider the design

intent again. A second look at the area reveals a flat surface on the front of

the pump housing that intersects a smoothly curved surface at the bottom.

How do you know that the front surface is flat? One way to check is to look

at the top line in another view. The approach to surfacing that area is to cre-

ate the smooth bottom surface and the flat surface. Then intersect one with

the other and create a wire at their intersection. If the new wire is the same

as the existing wire, you confirm your observation and surfacing approach.

Next, consider the bottom surface. You already know that you cannot use the

top wire because it has an abrupt corner. A good approach is to use only the

bottom wire as a rail, and the far edge as a cross section.

wireframe unacceptable surface

rail section

surface

Basic Concepts of Surfacing Wireframe Models |619

A surface like this one is a basic surface that carries a shape across larger areas.

This surface is referred to as a base surface. Even after many areas of the sur-

face are trimmed away, the underlying base surface remains intact and may

be displayed at any time with the Surface Display dialog box.

Identifying base surfaces is an important part of wireframe surfacing.

Another approach is to categorize surfaces by type and eliminate those you

won’t need.

To get shapes you can use for creating surfaces, you may need to break poly-

lines into segments. Then combine selected segments to form boundaries for

individual surfaces.

Using Trimmed Planar Surfaces

Use a trimmed planar surface for an area that you know is a flat plane. By

glancing at the pump model, you can see areas that appear to be flat and can

be surfaced with trimmed flat planes.

base surface trimmed surface

620 |Chapter 21 Surfacing Wireframe Models

If you are in doubt about whether a given area is flat, try to make a planar

surface. A planar surface requires a single closed wire as its boundary.

If the wire is not a closed single loop, you can see the breaks in the wire when

you select it.

You can join line segments into a closed wire that forms the boundary of a

planar surface. The surface is trimmed to the boundary shape.

NOTE When joining line segments, set tolerances to compensate for imper-

fect wireframe data that would otherwise cause the surface to fail.

Determine if an area is meant to be flat. If it is flat within the tolerance, create

a flat surface and adjust the edges.

Choosing a Surfacing Method

Which type of surface is best suited for a given area may not be clear.

wire planar surface

closed wire multi

le wires

top area

Basic Concepts of Surfacing Wireframe Models |621

In this example, the top area of the pump is not suitable for a single surface

because there are abrupt changes in its smoothness. The center area is curved

in one direction but straight in the other. When you have a surface area that

can be defined by a straight line between two curves, you can create a ruled

surface between the two curves.

Look beyond the obvious visible surface to find a workable solution. Because

the inlet at the right top area of the pump extends from the surface, consider

making the base surface first and then trimming it to the correct shape.

With the inlet shape removed, you can see possibilities for surfaces. The

shape created by the four wires contains a sharp corner. Avoid creating a

surface from these four wires because they might produce a surface that is

not smooth.

possible surface wire

inlet

abrupt corner

622 |Chapter 21 Surfacing Wireframe Models

You can see that each end of the area beneath the inlet is described by lines

with curvatures in both directions. This offers you a choice of surfacing

methods, such as a swept surface or a lofted UV surface.

In most cases, there is more than one way to surface an area. Try both methods

here, compare the results, and choose the one that produces the best result.

■Swept surfaces give you more control over the shape of the mid portion of

the surface.

■Lofted UV surfaces have fewer controls but risk is minimized.

Once you create a base surface to cover an area, trim the surface back to the

wire with the abrupt edge.

Use trimmed surfaces to create smooth underlying base surfaces that remain

a permanent part of a surface definition. Trim to constrain the edges and you

achieve smoothness in a base surface that contains no abrupt corners in its

boundary wires, yet creates a logical surface bounded by different edges. The

logical surface can contain any number of sharp corners, which have no

effect on the smoothness of the base surface.

The opposite side of the pump top area may also be surfaced several ways.

Again, the surface is really a larger surface cut short by an intersecting area of

the pump. This time, the wire that terminates the surface has no abrupt cor-

ners, so it could be used as one of four sides of a swept or lofted UV surface.

swept surface lofted UV surface

base surface trimmed surface

Basic Concepts of Surfacing Wireframe Models |623

The easiest method is to use a single rail and a single section to surface the

entire area, then trim the base surface to the intersecting part of the pump.

This choice might not always be correct. As you gain experience, you can pre-

dict which approach yields the most accurate results. In the previous exam-

ple, verify that the surface created without the top line matches the top line

within a reasonable tolerance.

Always check the fit between a newly created surface and existing wires to be

sure that you are not deviating too far from the wireframe data. If the new

surface is not within tolerance to the existing top line, the surface does not

accurately reflect the wireframe. You can re-create it using all four wire edges.

Verifying Surfacing Results

As you gain experience, you will see the importance of learned skill and judg-

ment. Your challenge is to produce smooth surfaces that fit the wireframe

closely; the surfaces should be as simple as possible.

You can judge the smoothness of surfaces several ways:

■Analyze a surface and view its color-shaded display to detect small devia-

tions in surface smoothness.

■Create and review flow lines in different rotated views.

■Cut sections through a complete set of surfaces, and then examine the

ends to see how closely they match at the edges.

■On the surface create augmented flow lines with long vectors and examine

the smoothness of the vector ends. The ends of the vectors exaggerate the

smoothness of the surface; areas where it is not smooth become apparent.

rail

section

surface trimmed surface

624 |Chapter 21 Surfacing Wireframe Models

Surfacing Wireframe Models

Now that you have analyzed approaches to surfacing the pump housing and

practiced surfacing techniques, you are ready to surface the pump.

A surface modeling project may begin with a wireframe, whether it is a DXF

or an IGES file from a client, or a 2D or 3D CAD design you created yourself.

In order to describe the 3D object, most designers begin with a 2D drawing.

In this lesson, you create surfaces for an actual part, a wireframe model of a

hydraulic pump. The surfaced model provides the manufacturer with infor-

mation to create prototypes or to NC-machine patterns, molds, and tooling.

To set up a drawing file

1Open the file t_pump.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.

2Use AMOPTIONS to set the surfacing options.

Desktop Menu Surface ➤ Surface Options

In the Mechanical Options dialog box, select the Surfaces tab. In Surface

Properties specify:

U Display Wires: Enter 5

V Display Wires: Enter 5

In Surface/Spline Options, specify:

Polyline Fit Length: Enter 1

Polyline Fit Angle: Enter 150

Choose Model Size.

3In the Approximate Model Size dialog box, choose Measure Model.

The Model Size is 4.7223. Choose Apply & Close.

Surfacing Wireframe Models |625

Notice that the values have changed in the Mechanical Options dialog box.

These settings affect the visual representation of the surfaces and the size of

the surface normal. Choose OK to exit.

NOTE If you shade the surfaces you create to better view them, adjust the

AutoCAD® setting that controls back faces. Go to Assist ➤ Options and select the

System tab. Choose Properties and clear the check box beside Discard back

faces. Choose Apply & Close, then OK.

The labeled parts of the pump are on separate layers. As you work on a part,

you make its layer current and freeze the other layers to make them inactive.

4Use LAYER to set up your current layer.

Desktop Menu Assist ➤ Format ➤ Layer

5In the Layer Properties Manager dialog box, highlight layer 10 and click Make

Current.

6Select layer 20, then press SHIFT and select the last layer. In the second col-

umn, click the sun icon under Freeze to freeze all selected layers. Then freeze

layer 0.

All layers except Layer 10 should be frozen (snowflake icon). Only Layer 10 is

thawed (sun icon). Choose OK.

outlet

body

inlet

top

base

support

626 |Chapter 21 Surfacing Wireframe Models

Creating Trimmed Planar Surfaces

Begin by surfacing the top section of the pump model, creating the individ-

ual surfaces. Top A is a planar surface because it is flat with sharp edges. Tops

B and C are swept surfaces, bounded by curved wires. Top B uses two curves

and two rails, and top C uses one curve and one rail. You trim the top C sur-

face where it extends beyond the wireframe boundary.

As you gain experience using the menu selections that correspond to com-

mands, you may want to use shortcuts. For a list of shortcuts that automate

the selection of menu options and commands, see “Accelerator Keys” in the

online Command Reference.

NOTE For a trimmed planar surface, the surface must be a single polyline that

lies in a single plane. If the wireframe is composed of multiple polylines, join

them into a single polyline before you create the surface.

To create a trimmed planar surface

1Use ZOOM to enlarge the view, responding to the prompt.

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

[All/Center/Dynamic/Extents/Previous/Scale/Window] <real time>:

Press ENTER

2Use AMPLANE to create the top A surface, responding to the prompt.

Desktop Menu Surface ➤ Create Surface ➤ Planar Trim

If you use the command line method, enter w at the prompt before continu-

ing to the following prompt.

top G

top C

top D

top A

top E

top F

top B

top A

Creating Trimmed Planar Surfaces |627

Select wires: Select wire (1) and press ENTER

A planar surface, trimmed to the boundary of wire (1), is created on the top

of the model.

To sweep a surface on two wires and two rails

1Use AMSWEEPSF to create the top B surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select wire (2)

Select cross sections: Select wire (3) and press ENTER

Select rails: Select wire (4)

Select rails: Select wire (5)

In the Sweep Surface dialog box, specify:

Transition: Scale

Keep Original Wire: Check the check box

Choose OK.

628 |Chapter 21 Surfacing Wireframe Models

To sweep a surface on one wire and one rail

1Use AMSWEEPSF to create the top C surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select wire (6) and press ENTER

Select rails: Select wire (7) and press ENTER

In the Sweep Surface dialog box, in Orientation select Normal. Choose OK.

The surface extends beyond the far side of the top. You will trim it later.

2Move surfaces A, B, and C to the TOP layer, responding to the prompts.

Command CHPROP

Select objects: Select surfaces (A), (B), and (C) and press ENTER

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Enter La

Enter new layer name <10>: Enter top

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Press ENTER

The surfaces are now on the TOP layer. Because the TOP layer is frozen, you

cannot see the surfaces, although the wireframe is still visible.

Save the file.

The D and E surfaces are ruled surfaces.

Creating Trimmed Planar Surfaces |629

To create a ruled surface between wires

1Use AMRULE to create the top D surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

2Use BREAK to separate line segment (4) from polyline (3), responding to the

prompts.

Desktop Menu Modify ➤ Break

Select object: Enter end

of: Select polyline (3)

Specify second break point or [First point]: Enter @

Unless you enter @, the adjoining portion of the polyline is deleted. The @ sym-

bol breaks the polyline at the specified location and retains both segments.

3Use AMRULE to create the top E surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (4)

Select second wire: Select wire (5)

4Move the top D and top E surfaces to the TOP layer, responding to the

prompts.

Command CHPROP

Select objects: Select surface (D)

Select objects: Select surface (E) and press ENTER

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Enter La

Enter new layer name <10>: Enter top

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Press ENTER

Save the file.

630 |Chapter 21 Surfacing Wireframe Models

Next, break and join lines that are needed to create the top F planar surface.

To create a planar surface with a joined polyline boundary

1Use BREAK to break polyline (1) where it intersects polyline (2), responding

to the prompts.

Desktop Menu Modify ➤ Break

Select object: Select polyline (1)

Specify second break point or [First point]: Enter f

Specify first break point: Enter int

of: Select polyline (2) at the intersection

Specify second break point: Enter @

To check that the polyline has broken correctly, select it. Grip points should

appear only for the line segment you select. Press ESC to exit Grip mode.

The break creates a line segment you use as part of the boundary for the next

surface.

2Use AMJOIN3D to join the polylines that form the boundary of top F.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

trimmed planar surface

Creating Trimmed Planar Surfaces |631

3In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Gap Tolerance: Enter .004

Choose OK.

4Respond to the prompts as follows:

Select start wire or: Select polyline (1)

Select wires to join: Select polylines (2) through (5)

Select wires to join: Press ENTER

Reverse direction? [Yes/No] <No>:

Press ENTER to accept the direction of the new wire

To confirm that the segments are joined, select the polyline and check the

grip points.

632 |Chapter 21 Surfacing Wireframe Models

5Use AMPLANE to create the top F surface from the joined polyline, responding

to the prompt.

Desktop Menu Surface ➤ Create Surface ➤ Planar Trim

If you use the command line method, enter w at the prompt before continu-

ing to the following prompt.

Select wires: Select the joined polyline and press ENTER

You have created the trimmed planar surface. Save the file.

For the top G surface, extrude a polyline along a straight line, and then trim

the surface to the desired shape.

To create a surface with an extruded polyline

1Change to a front left isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Left Isometric

2Us AMEXTRUDESF to extrude the polyline (1) down the wire (2), responding

to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Extrude

Select wires to extrude: Select polyline (1) and press ENTER

Define direction and length.

Specify start point or [Viewdir/Wire/X/Y/Z]: Enter w

Select wire to define direction: Select polyline (2)

Enter an option [Accept/Flip] <Accept>:

Enter f to flip the direction arrow down, or press ENTER

Enter taper angle <0>: Press ENTER to accept the default

Creating Trimmed Planar Surfaces |633

Your selection point determines the extrusion direction. Select a point on

polyline (2) close to polyline (1). If you select a point beyond the midpoint of

polyline (2), the direction of the extrusion is reversed.

Your drawing should look like this.

3Move top F and top G to the TOP layer, responding to the prompts.

Command CHPROP

Select objects: Select surface (F)

Select objects: Select surface (G) and press ENTER

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Enter La

Enter new layer name <10>: Enter top

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Press ENTER

4Choose Assist ➤ Format ➤ Layer.

Thaw the TOP layer to see all the surfaces you have created.

5Use AMINTERSF to trim top G and top C at their intersection, responding to

the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Intersect Trim

Select first surface/quilt or wire: Select surface (1)

Select second surface: Select surface (2)

634 |Chapter 21 Surfacing Wireframe Models

6In the Surface Intersection dialog box, specify:

Type: Trim

Trim: Select both First Surface and Second Surface

Clear the checkbox for Output Polyline

Choose OK. The surfaces are trimmed where they intersect.

Save the file.

Joining Surfaces on Complex Shapes

Next, you surface the inlet portion of the pump. Because the inlet has a com-

plex shape, you will need five surfaces to represent its shape.

■Inlets A and C are ruled surfaces because they follow two polylines.

■Inlet B is an extruded surface that is trimmed to its final shape.

■Inlet D is surface blended to surfaces B, C, and E.

■Inlet E is a trimmed planar surface created from joined lines that form its

boundary.

Joining Surfaces on Complex Shapes |635

NOTE Be sure to select surfaces and lines where indicated on the illustrations.

To select precisely, zoom in as needed.

To create the inlet A ruled surface

1From the Desktop menu, choose Assist ➤ Format ➤ Layer.

In the Layer Properties Manager dialog box, thaw layer 20 and make it cur-

rent. Then freeze layer 10 and TOP.

2Change to a right isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

3Use AMRULE to create the inlet A surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

The ruled surface is created on the top of the inlet.

inlet E

inlet D

inlet A

inlet B

inlet C

inlet A

636 |Chapter 21 Surfacing Wireframe Models

4Move the inlet A surface to the INLET layer, responding to the prompts.

Command CHPROP

Select objects: Select inlet A surface and press ENTER

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Enter La

Enter new layer name <20>: Enter inlet

Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]:

Press ENTER

Inlet B is an extruded partial cylinder, trimmed to its final shape by a closed

wire. The surface is extruded across the inlet wireframe.

The direction of the extrusion is determined by where you select the wire.

You can flip the direction of the extrusion.

Next, you create a ruled surface for inlet B.

NOTE To select the wires, you might need to reorient the view. Use icons on

the Mechanical View toolbar, or options from the View ➤ 3D Views menu.

To create the inlet B extruded surface

1Use AMEXTRUDESF to extrude polyline (1) along line (2), responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Extrude

Select wires to extrude: Select polyline (1) and press ENTER

Define direction and length.

Specify start point or [Viewdir/Wire/X/Y/Z] Enter w

Select wire to define direction: Select polyline (2) near (1)

Enter an option [Accept/Flip] <Accept>:

Enter f to flip direction arrow into part or press ENTER

Enter taper angle <0>: Press ENTER

Joining Surfaces on Complex Shapes |637

A close look at the inlet reveals that the extruded surface extends beyond the

wireframe. You trim the inlet B surface to the boundary of surface D.

2Use AMPROJECT to project the edge of inlet D to trim the inlet A surface,

responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select line (1) and press ENTER

Select target surfaces/quilts: Select surface (2) and press ENTER

3In the Project to Surface dialog box, specify:

Direction: Normal

Output type: Trim surface

Keep Original Wire: Check the check box

Choose OK.

You have trimmed inlet B by projection, keeping the wire you used to trim

the inlet surface.

Next you create inlet C, a ruled surface between two wires.

638 |Chapter 21 Surfacing Wireframe Models

To create the inlet C ruled surface

1Use AMRULE to create the inlet C surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

Your model should look like this.

2Use CHPROP to move inlet B and C surfaces to the INLET layer.

Save the file.

Next, you create inlet D, a surface blended from the edges of inlet B and C

surfaces and the polyline that defines the edge of inlet E. You may need to

rotate the model to show the intersection clearly.

Joining Surfaces on Complex Shapes |639

To create the inlet D blended surface

1Use BREAK to break the polyline into two line segments, responding to the

prompts.

Desktop Menu Modify ➤ Break

Select object: Select polyline (1)

Specify second break point or [First point]: Enter f

Specify first break point: Enter int

of: Select polyline (2)

Specify second break point: Enter @

Check the grip points of the line segments after you break the polyline.

2Use AMBLEND to create the inlet D surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Blend

Select first wire: Select wire (1)

Select second wire: Select wire (2)

Select third wire: Select wire (3)

Select fourth wire: Select wire (4)

Make selections in order, selecting opposite wires in pairs.

640 |Chapter 21 Surfacing Wireframe Models

The blended surface should look like this.

3Use CHPROP to move the surface to the INLET layer.

Join the lines to form the boundary of inlet E, and then create a trimmed planar

surface from the joined lines. Zoom in as needed to make line selection easier.

To create the inlet E trimmed planar surface

1Use AMJOIN3D to join selected lines to form the boundary for the inlet E sur-

face.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Gap Tolerance: Enter .01

Choose OK.

2Respond to the prompts as follows:

Select start wire or: Select polyline (1)

Select wires to join: Select wires (2) through (4)

Select wires to join: Press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER

Joining Surfaces on Complex Shapes |641

This procedure joins lines regardless of their original direction and converts

arcs and splines into polylines. You may need to reset the gap tolerance to

correctly join the polylines.

3Use AMPLANE to create a trimmed planar surface from the joined lines,

responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar Trim

If you choose the command line method, enter w at the prompt before con-

tinuing to the following prompts.

Select wires: Select polyline (1)

Select wires: Press ENTER

Your surface should look like this.

4Use CHPROP to move inlet E to the INLET layer.

Now you can trim top D by projecting the edge of the inlet. First, thaw layers

to show the inlet and top sections of the pump. Then, break a polyline into

segments and join one segment with other polylines. The joined polylines

form the shape of the projection that cuts material where the two surfaces

intersect.

To make selection easier, zoom and rotate the view as needed.

642 |Chapter 21 Surfacing Wireframe Models

To create a shape on a surface using joined wires

1Thaw layers 10 and 20.

2Change to the front right isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

3Use BREAK to break the polyline, responding to the prompts.

Desktop Menu Modify ➤ Break

Select object: Select polyline (1)

Specify second break point or [First point]: Enter f

Specify first break point: Enter end

of: Select polyline (2)

Specify second break point: Enter @

NOTE Use 3D Orbit and Zoom Realtime to rotate the view and zoom in to

show the lines clearly. If you prefer, use VPOINT to set a precise viewpoint. In this

case, set the coordinates 4,-6,1 to show the lines you need for the next step.

4Break the upper part of the polyline into segments, responding to the

prompts.

Desktop Menu Modify ➤ Break

Select object: Select polyline (1)

Specify second break point or [First point]: Enter f

Specify first break point: Enter int

of: Select polyline (2)

Specify second break point: Enter @

Joining Surfaces on Complex Shapes |643

5Use AMJOIN3D to combine three polyline segments.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Gap Tolerance: Enter .004

Choose OK.

6Respond to the prompts as follows:

Select start wire or: Select polyline (1)

Select wires to join: Select wire (2)

Select wires to join: Select wire (3) and press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER

The segments are joined together. Later, you will project the joined line onto

the top surface.

644 |Chapter 21 Surfacing Wireframe Models

To trim a surface using a projected wire shape

1Freeze layer 10 and thaw the TOP layer.

2Return to the front right isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

3Use AMPROJECT to cut top B where the inlet fits, responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select wire (1) and press ENTER

Select target surfaces/quilts: Select surface (2) and press ENTER

4In the Project to Surface dialog box, specify:

Direction: Normal

Output Type: Trim Surface

Keep Original Wires: Remove the check from the check box

Choose OK.

Top B is cut open for the inlet. The top and inlet are complete. Save the file.

Creating Swept and Projected Surfaces |645

Creating Swept and Projected Surfaces

For the main body of the pump, you continue building and trimming sur-

faces to their correct shapes.

■Body A, B, and C are swept surfaces created from curves and rails.

■Body D is a surface created from the boundaries of Body A, B, and C

surfaces.

To create the body A, B, and C swept surfaces

1Thaw layer 30 and make it current. Freeze layers 10, 20, and TOP.

2Use AMSWEEPSF to create the body A surface on the right side of the model.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

body A

body C

body B

body D

646 |Chapter 21 Surfacing Wireframe Models

Respond to the prompts:

Select cross sections: Select wire (1)

Select cross sections: Select wire (2) and press ENTER

Select rails: Select wire (3)

Select rails: Select wire (4)

3In the Sweep Surface dialog box, specify:

Transition: Scale

Keep Original Wires: Check the check box

Choose OK

4Use AMSWEEPSF to create the body B surface on the left side of the model,

responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

NOTE To repeat the previous command, press ENTER or the SPACEBAR.

Select cross sections: Select wire (5) and press ENTER

Select rails: Select wire (6) and press ENTER

Creating Swept and Projected Surfaces |647

5In the Sweep Surface dialog box, under Orientation, specify Normal. Leave

Keep Original Wires checked, and choose OK.

6Create the body C surface near the bottom of the model, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select wire (7) and press ENTER

Select rails: Select the wire (8) and press ENTER

7In the Sweep Surface dialog box, under Orientation, specify Normal. Verify

that Keep Original Wires is checked, and choose OK.

Your model should look like this.

8Thaw layer 20 to reveal the inlet wires.

648 |Chapter 21 Surfacing Wireframe Models

To trim a surface with a projection wire

1Use AMPROJECT to trim the body surface with the inlet edge, responding to

the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select wire (1)

Select wires to project: Press ENTER

Select target surfaces/quilts: Select surface (2)

Select target surfaces/quilts: Press ENTER

2In the Project to Surface dialog box, specify:

Direction: Normal

Output Type: Trim Surface

Verify that Keep Original Wires is checked, and choose OK.

The projected wire cut away a portion of body A surface, but the wire was not

deleted.

Creating Swept and Projected Surfaces |649

3Freeze layer 20.

Cut out the surface areas on body C where body D and the outlet (to be sur-

faced later) extend onto body C.

body surface removed

650 |Chapter 21 Surfacing Wireframe Models

To trim the body C surface with projection wires

1Change to the front view of your model.

Desktop Menu View ➤ 3D Views ➤ Front

2Trim Body C with the lower curve of the flat surface (1), responding to the

prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select wire (1)

Select wires to project: Press ENTER

Select target surfaces/quilts: Select surface (2)

Select target surfaces/quilts: Press ENTER

3In the Project to Surface dialog box, specify:

Direction: Normal

Output Type: Trim Surface

Verify that Keep Original Wires is checked, and choose OK.

Creating Swept and Projected Surfaces |651

Your model should look like this.

4Change to the front left isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Left Isometric

NOTE To set the viewpoint precisely, use VPOINT to specify coordinates. For

example, this viewpoint is -5,-10,3.

5Trim the body B surface with the curve that defines the upper edge of the out-

let. Repeating steps 2 and 3, project wire 3 onto surface 4.

652 |Chapter 21 Surfacing Wireframe Models

6Trim body C with the curve that defines the lower edge of the outlet,

responding to the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select wire

Select wires to project: Press ENTER

Select target surfaces/quilts: Select surface (6)

Select target surfaces/quilts: Press ENTER

7In the Project to Surface dialog box, specify:

Direction: Normal

Output Type: Trim Surface

Verify that Keep Original Wires is checked, and choose OK.

Your model should look like this.

8Use CHPROP to move surfaces A, B, and C to the BODY layer.

Next, you edit the wireframe to join the lines that form the boundary of body

D. You use the polyline to create a planar surface.

Before you begin, set DELOBJ to delete original objects.

Toolbutton On the Surfacing toolbar, use the DELOBJ toolbutton to set

delete original objects.

Creating Swept and Projected Surfaces |653

To create the body D planar surface

1Use AMJOIN3D to join the polylines that define the boundary of body D.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join 3D dialog box, specify:

Mode: Automatic

Output: Polyline

Choose OK.

2Respond to the prompts as follows:

Select start wire or: Select the wire (1)

Select wires to join: Select wires (2), (3), and (4)

Select wires to join: Press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER

3Use AMPLANE to create a planar surface from the joined line, responding to

the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar

Specify first corner or [Plane/Wires]: Enter w

Select wires: Select wire (5) and press ENTER

654 |Chapter 21 Surfacing Wireframe Models

Your model should look like this.

4Use CHPROP to move body D to the BODY layer. Save the file.

The pump body surfaces are complete.

Creating Complex Swept Surfaces |655

Creating Complex Swept Surfaces

Next, you create the surfaces for the outlet on the side of the pump.

Outlet A is a swept surface that blends dissimilar cross sections.

To create the outlet A swept surface

1Thaw layer 40 and make it current, and then freeze all other layers.

2Change to the left isometric view to make lines easier to select.

Desktop Menu View ➤ 3D Views ➤ Front Left Isometric

3Use AMSWEEPSF to Sweep three cross sections along two rails, responding to

the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select wires (1), (2), and (3)

Select rails: Select wires (4) and (5)

outlet F

(back side) outlet E

outlet C

outlet A

outlet B

outlet D

656 |Chapter 21 Surfacing Wireframe Models

4In the Sweep Surface dialog box, in Transition, specify Scale. Choose OK.

Outlet A should look like this.

5Use CHPROP to move outlet A to the OUTLET layer.

Next create a ruled surface for outlet B. The difference between this surface

and the one you just completed is that outlet A is curved in two directions,

and outlet B is curved in one direction and flat in the other.

To create the outlet B ruled surface

1Use AMRULE to create the outlet B surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

Creating Complex Swept Surfaces |657

Outlet B should look like this.

2Use CHPROP to move outlet B to the OUTLET layer.

Next, you create another swept surface and another ruled surface.

To create the outlet C and outlet D surfaces

1To make selections easier, rotate the model to the left with the Desktop View

icons, or set specific coordinates (6,-8,1) with VPOINT, responding to the

prompts.

Desktop Menu View ➤ 3D Views ➤ VPOINT

Current view direction: VIEWDIR=-1.0000,-1.0000,1.0000

Specify a view point or [Rotate] <display compass and tripod>: Enter 6,-8,1

2Use AMSWEEPSF to create outlet C swept surface.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

658 |Chapter 21 Surfacing Wireframe Models

Respond to the prompts:

Select cross sections: Select wire (1)

Select cross sections: Select wire (2) and press ENTER

Select rails: Select wire (3)

Select rails: Select wire (4)

3In the Sweep Surface dialog box, under Transition, specify Scale. Choose OK.

4Use AMRULE to create outlet D ruled surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (5)

Select second wire: Select wire (6)

Your model should look like this.

5Use CHPROP to move both of the surfaces to the OUTLET layer.

Next, you join lines to form the boundaries of outlet E and outlet F. From the

newly created polyline, you create planar surfaces for the outlet.

Creating Complex Swept Surfaces |659

To create the outlet E planar surface

1Use AMJOIN3D to join the polylines.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Choose OK.

2Select the polylines, responding to the prompts.

Select start wire or: Select wire (1)

Select wires to join: Select wires (2), (3), and (4), and press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER to accept the join direction

3Use AMPLANE to create the outlet E surface from the joined polyline, respond-

ing to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar

Specify first corner or [Plane/Wires]: Enter w

Select wires: Select wire (1) and press ENTER

To create the outlet F planar surface

1Use AMJOIN3D to combine lines that form the boundary for outlet F.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join 3D dialog box, specify:

Mode: Manual

Output type: Polyline

Choose OK.

660 |Chapter 21 Surfacing Wireframe Models

2Select the polylines to join, responding to the prompts.

Select start wire or: Select wire (5)

Select wires to join: Select wire (6) and press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER to accept the join direction

NOTE Use the Manual mode to join lines even if they are far apart. It joins all

the lines you select in the order you choose them.

3Use AMPLANE to create outlet F from the lines you just joined, responding to

the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar

Specify first corner or [Plane/Wires]: Enter w

Select wires: Select wire (6) and press ENTER

Your model should look like this.

4Use CHPROP to move the surfaces to the OUTLET layer.

Save the file.

Using Projection to Create Surfaces |661

Using Projection to Create Surfaces

Next, you use projection to create ruled and planar surfaces for the base of

the pump.

To create the base A surface

1Thaw layer 50 and make it current. Then freeze all other layers.

2Change to the left front isometric view.

Desktop Menu View ➤ 3D Views ➤ Front Right Isometric

3Use AMRULE to create the base A surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

base A

base B

base C

662 |Chapter 21 Surfacing Wireframe Models

The illustration shows the ruled surface fit to the flat areas and corner curves.

4Use CHPROP to move base A to the BASE layer.

Next, you join the lines needed to create a planar surface on the bottom of

the pump. Then you copy the surface and trim it.

To create the base B and C surfaces

1Use AMJOIN3D to create a polyline from two wires.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Choose OK.

2Select the wires, responding to the prompts:

Select start wire or: Select wire (1)

Select wires to join: Select wire (2) and press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER

Using Projection to Create Surfaces |663

3Create a planar surface on the bottom of the base, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Planar

Specify first corner or [Plane/Wires]: Enter w

Select wires: Select wire (1) and press ENTER

The planar surface is created.

4Use COPY to copy the last surface, responding to the prompts.

Desktop Menu Modify ➤ Copy

Select objects: Select surface (1) and press ENTER

Specify base point or displacement, or [Multiple]: Enter end

of: Select point (2)

Specify second point of displacement or <use first point as displacement>:

Enter end

of: Select point (3)

Next, project a wire onto the base C surface to trim it.

664 |Chapter 21 Surfacing Wireframe Models

To trim the base C surface

1Use CHPROP to move the bottom surface to the BASE layer.

2Project the curve of the body onto the top surface of the base, responding to

the prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select polyline (1) and press ENTER

Select target surfaces/quilts: Select surface (2) and press ENTER

3In the Project to Surface dialog box, specify:

Direction: Normal

Output type: Trim Surface

Choose OK.

Your model should look like this.

4Use CHPROP to move the surfaces to the BASE layer.

Save the file.

Using Advanced Surfacing Techniques |665

Using Advanced Surfacing Techniques

Next, you create the support rib from the surfaces. Using the techniques you

have already learned, surface the support rib from these general instructions.

Save a copy of your drawing before you begin working on your own.

To create the support rib

1Thaw layer 60.

2Create a ruled surface on the left side of the support rib (rib A).

3Create a ruled surface on the right side of the support rib (rib B).

4Move the surfaces to the SUPPORT_RIB layer.

5Create a swept surface for rib C.

6Move the surface to the SUPPORT_RIB layer.

7Add the support rib to the body and base surfaces.

If you need to, follow these specific instructions to create the support rib.

rib C

rib B

rib A

666 |Chapter 21 Surfacing Wireframe Models

To create the rib A and rib B surfaces

1Thaw layer 60 and make it current. Then freeze all other layers.

2Use AMRULE to create a ruled surface on the left side of the support rib,

responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (1)

Select second wire: Select wire (2)

3Create a ruled surface on the right side of the support rib, responding to the

prompts.

Desktop Menu Surface ➤ Create Surface ➤ Rule

Select first wire: Select wire (3)

Select second wire: Select wire (4)

The surfaces should look like this.

4Use CHPROP to move the surfaces to the SUPPORT_RIB layer.

Using Advanced Surfacing Techniques |667

To create the rib C surface

1Use AMSWEEPSF to create the rib C surface, responding to the prompts.

Desktop Menu Surface ➤ Create Surface ➤ Sweep

Select cross sections: Select wire (1) and (2)

Select cross sections: Press ENTER

Select rails: Select wires (3) and (4)

2In the Sweep Surface dialog box, under Transition, specify Scale. Choose OK.

Your surface should look like this.

3Move the surface to the SUPPORT_RIB layer.

4Use AMJOIN3D to join the lines defining the boundary of the support rib.

Desktop Menu Surface ➤ Edit Wireframe ➤ Join

5In the Join3D dialog box, specify:

Mode: Automatic

Output: Polyline

Choose OK.

6Select the lines.

Select start wire or: Select wire (1)

Select wires to join: Select wires (2), (3), and (4), and then press ENTER

Reverse direction? [Yes/No] <No>: Press ENTER

The support rib wires are joined and ready to project onto the pump.

668 |Chapter 21 Surfacing Wireframe Models

To add the support rib

1Thaw the BODY and BASE layers.

2Use AMPROJECT to project the support rib onto the pump, responding to the

prompts.

Desktop Menu Surface ➤ Edit Surface ➤ Project Trim

Select wires to project: Select wire (1) and press ENTER

Select target surfaces/quilts: Select surface (2)

Select target surfaces/quilts: Select surface (3) and press ENTER

3In the Project to Surface dialog box, specify:

Direction: Normal

Output: Trim Surface

Choose OK.

The support rib is projected onto the body and the base.

Save your file.

body surface removed

Viewing Completed Surfaced Models |669

Viewing Completed Surfaced Models

To view the completed model, freeze all layers except BASE, BODY, INLET,

OUTLET, SUPPORT_RIB, and TOP.

Use the Zoom Extents option of ZOOM to view the entire wireframe model.

One half of the pump housing is complete. You can mirror the surfaces to cre-

ate a complete model.

670

671

In This Chapter 22

Working with Standard

Parts

Standard parts is the term used for the vast selection of

real-world reusable 2D and 3D parts, holes, features, and

structural steel profiles that are available to you in

Autodesk® Mechanical Desktop® 6 with the power pack.

These standard parts are provided in many different

base standards.

In this tutorial you select standard parts to insert

through holes on a 3D part, using two different

positioning methods. You also add a screw connection

to a 3D assembly model using standard parts.

Run Mechanical Desktop with the power pack to

perform this tutorial.

■Selecting standard parts

■Inserting holes using the cylinder

axial placement method

■Inserting holes using the cylinder

radial placement method

■Inserting a screw connection

■Creating a drawing view with 2D

standard parts

672 |Chapter 22 Working with Standard Parts

Key Terms

Te r m Definition

base standard Predefined drafting standard that conforms to International Drafting Standards

ANSI, BSI, CSN, DIN, GB, ISO, and JIS.

cylinder axial Option for placement when you insert a standard part or hole parallel to a

cylinder axis.

cylinder radial Option for placement when you insert a standard part or hole radial into a

cylinder.

hole Geometric feature with a predefined shape: drilled, counterbore, or countersink.

parallel Being an equal distance apart at every point.

standard part Reusable 2D and 3D parts, holes, features, and structural steel profiles available in

Mechanical Desktop 6.

tangent Touching at a single point or along a line, but not intersecting.

through Termination method by which a feature extends from its sketch plane through the

part.

Tutorial at a Glance |673

Tutorial at a Glance

This tutorial is an introduction to the standard parts and calculations func-

tionality in Mechanical Desktop 6. You will become familiar with some of the

intelligence and automation built into this functionality as you perform

exercises to insert

■A through hole using the cylinder axial placement method.

■Through holes using the cylinder radial placement method.

■A screw connection using the automated screw connection feature.

■A standard related 2D-Representation of standard parts.

Basic Concepts of Standard Parts

A large selection of standard parts are made available to you in Mechanical

Desktop 6. These standard parts are provided in many different base stan-

dards. You make your selections from lists of standard parts as you work. For

example, when you select a screw, you can choose from different types of

screws and from different configurations of threads. Using the standard parts

and calculations functionality, you can insert complete screw connections

including screws, holes, and nuts in one automated process.

The software is intelligent, and prevents you from assembling parts that do

not fit. For example, if you select a screw with a metric thread, only metric

threads are added with any additional parts or features, such as threaded

holes or nuts. If you select screws, holes, and nuts from varying standards,

the software determines if those parts will work together.

674 |Chapter 22 Working with Standard Parts

Inserting Through Holes

It is no longer necessary to insert a workpoint on the cylinder face,

dimension it, and insert a hole on the workpoint. Instead, the standard hole

function automatically defines a workpoint at the location you select,

dimensions it, and places the hole you specify. You can also define the inser-

tion point dynamically.

Using Cylinder Axial Placement

In this exercise, you insert a standard through hole using the cylinder axial

placement method. Use this method to insert holes parallel to the axis of a

cylinder. You enter specifications and select a size from a list of standard

holes, and the hole is inserted automatically.

Open the file md_ex01.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.

Inserting Through Holes |675

To insert a hole using cylinder axial placement

1Use AMTHOLE3D to define the hole to insert.

Menu Content 3D ➤ Holes ➤ Through Holes

In the Select a Through Hole dialog box, select ISO 273 normal.

2In the Hole Position Method First Hole dialog box, specify:

Placement: Cylinder Axial

Choose OK.

3On the command line, respond to the prompts as follows:

Select circular edge: Select the upper circular edge (1)

676 |Chapter 22 Working with Standard Parts

4Continue on the command line.

Select radius: Press SHIFT and in the graphics area, right-click and choose Midpoint

5Select the midpoint of the upper horizontal edge (2).

6Continue on the command line.

Select insertion method

[Angle to plane or edge/parallel to Line/plane Normal/plane Parallel] <plane

Parallel>: Enter A

Select straight edge, work plane or planar face to add angular constraint

to: Press ENTER

Select angle: Select an angle of approximately 135° (3)

Enter angle [Associate to/Equation assistant] <145>: Enter 135

Radius [Associate to/Equation assistant] <90>: Press ENTER

Hole termination [toPlane/Thru] <Thru>: Press ENTER

Inserting Through Holes |677

7In the ISO 273 normal - Nominal Diameter dialog box, specify:

Select a size: M10

Choose Finish.

The through hole is inserted in the size and location you selected.

Save the file as md2_ex01a.dwg.

Using Cylinder Radial Placement

In this exercise, you insert a through hole using the cylinder radial method.

Use this method to insert holes radial to a cylinder face.

678 |Chapter 22 Working with Standard Parts

To insert a hole using cylinder radial placement

1Use AMTHOLE3D to define the hole to insert.

Menu Content 3D ➤ Holes ➤ Through Holes

In the Select a Through Hole dialog box, select ISO 273 normal.

2In the Hole Position Method First Hole dialog box, specify:

Placement: Cylinder Radial

Choose OK.

3On the command line, respond to the prompts as follows:

Select cylindrical face: Select the upper cylindrical face (1)

Continue on the command line.

Specify hole location [Line/Plane]:

Press SHIFT and in the graphics area, right-click and choose Midpoint

Inserting Through Holes |679

4Select the midpoint of the upper vertical edge (2).

5Respond to the prompts as follows:

Enter distance from base plane [Associate to/Equation assistant] <15>:

Press ENTER

Select drill direction

[Angle to plane or edge/parallel to Line/plane Normal/plane Parallel]

<plane Parallel>: Enter A

Select straight edge, work plane or planar face to add angular constraint to:

Press ENTER

Select angle: Select an angle of approximately 180° (3)

Continue on the command line:

Enter angle [Associate to/Equation assistant] <181>: Enter 180

Hole termination [toPlane/Thru] <Thru>: Press ENTER

680 |Chapter 22 Working with Standard Parts

6In the ISO 273 normal - Nominal Diameter dialog box, specify:

Select a size: M10

Choose Finish.

The through hole is inserted. Your drawing should look like this:

Save the file as md2_ex01b.dwg.

Inserting Screw Connections |681

Inserting Screw Connections

In this exercise, you begin with a drawing of two parts that need a screw con-

nection. Using the screw connection feature, you select the screw, holes, and

nut that you want to use.

You define the size of the screw in a dialog box. Then you insert the screw

connection in the assembly. With this method, there is no need to create two

separate holes before you insert the screw with the nut. The screw connec-

tion function does this for you automatically.

Open the file md_ex02 in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing contains two parts of a housing.

682 |Chapter 22 Working with Standard Parts

To insert a screw connection

1Use AMSCREWCON3D to choose and define the screw to insert.

Menu Content 3D ➤ Screw Connection

In the Screw Connection dialog box, select Screws.

Next, define the type of screw.

Inserting Screw Connections |683

2In the Please select a Screw dialog box, select Socket Head Types.

Select the screw IS2401.

The Screw Connection dialog box is displayed again.

3Repeat steps 1 and 2 to select and define each of the following parts:

Hole ➤ Through Cylindrical ➤ IS1602 normal

Nut ➤ Hex Nuts ➤ ISO842

After you select and define the parts for the screw connection, select a size for

the diameter.

684 |Chapter 22 Working with Standard Parts

4Select M10 for the diameter.

Choose Finish.

The Hole Position Method First Hole dialog box is displayed.

5In the Hole Position Method First Hole dialog box, specify the hole position-

ing method as follows:

Placement: 2 Edges

Choose OK.

Inserting Screw Connections |685

6On the command line, respond to the prompts as follows:

Select first edge or planar face: Specify the first edge (1)

Select second edge or planar face: Specify the second edge (2)

Continue on the command line.

Specify the hole location: Specify a point on the face, offset from the two edges

Enter distance from first geometry (highlighted) [Associate to/Equation assistant]

<15.06>: Enter 20

Enter distance from second geometry (highlighted) [Associate to/Equation

assistant] <23.05>: Enter 20

Hole termination [toPlane/Thru] <Thru>: Press ENTER

686 |Chapter 22 Working with Standard Parts

7In the Hole Position Method Next Hole dialog box, specify:

Placement: Workpoint UCS

Choose OK.

8Respond to the prompt as follows:

Select next part to drill through: Select the lower part (3)

Continue on the command line:

Hole termination [toPlane/Thru] <Thru>: Press ENTER

Inserting Screw Connections |687

The screw connection is inserted. Your drawing should look like this:

You have completed this tutorial.

Save the file as md6_ex17b.dwg.

688

689

In This Chapter 23

Creating Shafts

The shaft generator in Autodesk® Mechanical Desktop® 6

is an automated feature that eliminates the need for

many of the manual steps previously required to create

shafts.

In this tutorial, you learn how to design shafts using the

shaft generator. You create a shaft with segments of

different shapes, and add threads and a profile. Then

you edit the shaft and add standard parts to it. Finally,

you check your design in front and isometric views with

wireframe and shaded displays.

Run Mechanical Desktop with the power pack to

perform this tutorial.

■New in this tutorial

■Using the Shaft Generator

■Creating shaft geometry

■Adding thread and profile

information to a shaft

■Editing a shaft

■Adding standard parts to a shaft

■Shading and displaying 3D views

690 |Chapter 23 Creating Shafts

Key Terms

Te r m Definition

bearing calculation Calculates limiting value, dynamic and static load rating, dynamic and static

equivalent load, and fatigue life of bearing in revolutions and hours.

centerline Line in the center of a symmetrical object. When you create centerlines, you

specify the start and end points.

chamfer A beveled surface between two faces or surfaces.

dynamic calculation Calculation required for a revolving bearing. The result is the Adjusted Rating Life.

This is the life of the bearing associated with 90% reliability with contemporary,

commonly used material, and under conventional operating conditions. With the

number of revolutions you get the life in working hours.

dynamic dragging The act of determining the size of a standard part with the cursor while inserting

it into a side view. The standard part is displayed dynamically on the screen and

can be dragged to the next possible size and length. The values (sizes) are taken

from the Standard parts database.

shaft generator Tool to draw rotationally symmetric parts.

UCS User coordinate system. Designated by arrows that signify the XY coordinates.

Establishes a construction plane and simplifies location of 3D points. Provides

visual reference for positioning a surface.

Tutorial at a Glance |691

Tutorial at a Glance

It is no longer necessary to create a cylinder manually and define new sketch

planes and work planes in order to create a shaft. Instead, you make selec-

tions in the 3D Shaft Generator dialog box, and enter values to further define

your selections.

In this tutorial you use this automated feature to

■Create a shaft with cylindrical and conical sections.

■Add threads and a profile to the shaft.

■Edit the shaft.

■Add standard parts to the shaft.

■Shade and display 3D views of the shaft.

Basic Concepts of the Shaft Generator

The shaft generator is an automated feature for creating shafts of many con-

figurations, including outer and inner shaft contours for hollow shafts, You

define the different segments of a shaft using the options in the 3D Shaft

Generator dialog box.

As you select and define each segment, it is generated automatically and

added to the shaft. Usually, you work from left to right as you add different

types of segments, such as cylinders, cones, thread, profiles, and grooves.

Shaft segments can be inserted, deleted, or edited.

Each element of a shaft is generated from the segment preceding it. When

you delete a shaft element, you also delete the shaft elements that follow.

As you create shaft segments, corresponding icons for the work features and

shaft contours are displayed in the Desktop Browser.

While you are creating the shaft, it is helpful to display front and isometric

views using two viewports. Toggling between wireframe and shaded displays

also makes it easier to visualize your design.

692 |Chapter 23 Creating Shafts

Using the Shaft Generator

You use the 3D Shaft Generator dialog box to select a type of shaft segment,

such as a cylinder or a cone, and then you define that segment. The shaft

generator creates the segment automatically and adds it to the previous

segment.

Getting Started

In order to work through this tutorial chapter, the ISO standard system has

to be installed at your system.

Moreover, you need to set your measurement units to metric. This can easily

be done by selecting an appropriate drawing template. Open the drawing

template acadiso.dwt.

To open a drawing template

1Open a new template.

Menu File ➤ New

Command NEW

The AutoCAD Mechanical Today window is displayed.

2In the AutoCAD Mechanical Today window, in the section My Drawings,

change to the tab Create Drawings, and select the template acadiso.dwt.

Now, you are working with the selected template.

Using the Shaft Generator |693

Creating Shaft Geometry

You start creating the shaft by defining the segments that govern its shape.

In the 3D Shaft Generator dialog box, you select the first segment type and

then you define that segment. You continue adding segments until the con-

tour of the shaft is complete.

To create a shaft using the shaft generator

1Use AMSHAFT3D to define the shaft.

Menu Content 3D ➤ Shaft Generator

Respond to the prompts as follows:

Specify start point or [Existing shaft]: Select a point in the drawing

Specify centerline endpoint: Drag a line to the right, and select a point

Specify point for new plane <parallel to UCS>: Press ENTER

The 3D Shaft Generator dialog box is displayed.

Define the shaft contour, starting with the segment at the left, and working

to the right.

2Verify the Outer Contour tab is selected, then choose the lower Cylinder icon.

Respond to the prompts as follows:

Specify length or [Associate to/Equation assistant] <50>: Enter 10

Specify diameter or [Associate to/Equation assistant] <40>: Enter 74

694 |Chapter 23 Creating Shafts

3Choose the Slope icon, and respond to the prompts as follows:

Specify length or [Dialog/Associate to/Equation assistant] <10>: Enter 7

Specify diameter at start point or [Associate to/Equation assistant] <74>:

Press ENTER

Specify diameter at end point or [Slope/aNgle/Associate to/Equation assistant]

<72>: Enter 48

NOTE If the 3D Shaft Generator dialog box hides your shaft, move the dialog

box to another position on the screen.

4Choose the lower Cylinder icon again, and respond to the prompts as follows:

Specify length or [Associate to/Equation assistant] <7>: Enter 20

Specify diameter or [Associate to/Equation assistant] <48>: Enter 40

5Choose the Slope icon again, and respond to the prompts as follows:

Specify length or [Dialog box/Associate to/Equation assistant] <20>: Enter 10

Specify diameter at start point or [Associate to/Equation assistant] <40>:

Press ENTER

Specify diameter at end point or [Slope/aNgle/Associate to/Equation assistant]

<36>: Enter 32

6Choose the lower Cylinder icon once more, and respond to the prompts as

follows:

Specify length or [Associate to/Equation assistant] <10>: Enter 28

Specify diameter or [Associate to/Equation assistant] <32>: Press ENTER

You have created a shaft consisting of three cylindrical and two conical seg-

ments. Your drawing should look like this.

Next, you add thread information to the shaft.

Using the Shaft Generator |695

Adding Threads to Shafts

The 3D Shaft Generator dialog box provides the option to add threads to a

shaft. You define the thread information in the Thread dialog box, and the

thread is added to the shaft automatically.

To add threads to a shaft

1In the 3D Shaft Generator dialog box, select the Outer Contour tab and

choose the Thread icon.

2The Thread dialog box is displayed. Select ISO 261 from the available thread

types.

696 |Chapter 23 Creating Shafts

3The Thread ISO 261 dialog box is displayed. Specify:

Nominal Diameter d [mm]: M 32 x 1.5

Length l=: Enter 12

4Choose OK.

NOTE If you have previously chosen a thread standard, the Thread dialog box

opens directly to the Nominal Diameter selection screen (illustrated above).

There is no need to choose the same standard again. To return to the standard

selection list in the Thread dialog box, choose Standard.

Mechanical Desktop Power Pack calculates the thread and adds it to the

shaft, then returns you to the 3D Shaft Generator dialog box.

Following the thread segment, you need to add another cylindrical segment

with a diameter smaller than the threaded section.

5Choose the lower Cylinder icon, and respond to the prompts as follows:

Specify length or [Associate to/Equation assistant] <28>: Enter 2

Specify diameter or [Associate to/Equation assistant] <32>: Enter 25

The new segment is added, and you are ready to add a profile to your shaft.

Using the Shaft Generator |697

Adding Profile Information to Shafts

The 3D Shaft Generator dialog box provides the option to add a profile to a

shaft. You further define the profile information in the Shaft dialog box.

Add a profile segment to connect a drive to the shaft.

To add a profile to a shaft

1In the 3D Shaft Generator dialog box, choose the Profile icon.

2In the Profile dialog box, select ISO 14.

3In the Splined Shaft dialog box, specify:

Nominal Size n x d x D [mm]: 6 x 26 x 30

Length l=: Enter 30

Choose OK.

The profile is added to the shaft.

Add another small cylindrical segment to the end of the shaft.

4In the 3D Shaft Generator dialog box, choose the lower Cylinder icon again,

and respond to the prompts as follows:

Specify length or [Associate to/Equation assistant] <30>: Enter 5

Specify diameter or [Associate to/Equation assistant] <30>: Enter 25

698 |Chapter 23 Creating Shafts

5Close the 3D Shaft Generator dialog box.

The shaft contour is complete. Your drawing should look like this.

Save your drawing as shaft.dwg.

Next, you edit the shaft.

Editing Shafts

You can make changes to simple shaft segments such as cylinders and cones.

It is recommended that you delete a more complex segment, such as a gear,

and create a new one. In this exercise, you add a chamfer to a segment and

you add a groove to another segment.

First, add a chamfer to the end segment of your shaft.

Using the Shaft Generator |699

To add a chamfer to a shaft segment

1Activate the shaft generator.

Menu Content 3D ➤ Shaft Generator

Command AMSHAFT3D

2On the command line, respond to the prompts as follows:

Specify start point or [Existing shaft]: Enter E

Select shaft: Select the shaft

3In the 3D Shaft Generator dialog box, select the Outer Contour tab. Choose

the chamfer icon, and respond to the prompts as follows:

Select edge for chamfer: Select the edge (1)

Specify length (max. 5) or [Associate to/Equation assistant] <2.5>: Enter 2.5

Specify angle (min 0.0001, max 78.69) [Distance/Associate to/Equation

assistant] <45>: Enter 45

Enter an option [Revolve/Chamfer] <Revolve>: Press ENTER

The chamfer is created on the shaft end.

In the next step, you use the 3D Shaft Generator dialog box to insert a groove

for a retaining ring on a section of the shaft. This groove will be used for posi-

tioning a bearing.

700 |Chapter 23 Creating Shafts

To insert a groove on a shaft segment

1Choose the Groove icon, and respond to the prompts as follows:

Select cylinder or cone: Select the third cylindrical section (1)

Select position on cylinder or cone [Line/Plane]: Specify the point (2)

Specify direction or [Flip/Accept] <Accept>: Press ENTER

Enter distance from base plane [Associate to/Equation assistant] <11.4>:

Enter 25

Specify length or [Associate to/Equation assistant] <5>: Enter 1.5

Specify diameter <50>: Enter 29

The groove is inserted and displayed on the shaft.

The edits to the shaft are complete.

2Close the 3D Shaft Generator dialog box.

Save your file.

Now that you have finished the shaft, you add standard parts to it.

Using the Shaft Generator |701

Adding Standard Parts to Shafts

In Mechanical Desktop Power Pack, standard parts such as bearings, seals,

circlips, keys, adjusting rings, and undercuts are available. You can select and

insert these standard parts using the shaft generator.

When you insert a standard part on a shaft, the standard part is not con-

sumed by the shaft. You are actually building an assembly. An icon for each

new part is displayed in the Browser under the assembly icon.

To add a bearing to a shaft

1Use AMSHAFT3D TO add a standard part to the shaft.

Menu Content 3D ➤ Shaft Generator

Command AMSHAFT3D

2On the command line, respond to the prompts as follows:

Specify start point or [Existing shaft]: Enter E

Select shaft: Select the shaft

3The 3D Shaft Generator dialog box is displayed. Choose Std. Parts.

4In the Select a Part dialog box, choose Roller Bearings ➤ Radial ➤ ISO 355.

Respond to the prompts as follows:

Select cylindrical face: Select a point on the third shaft segment (1)

Specify location on cylindrical face [Line/Plane]:

Select the left plane of the third shaft segment (2)

Enter distance from base plane [Associate to/Equation assistant] <0>:

Press ENTER

Choose insertion direction [Flip/Accept] <Accept>: Press ENTER

702 |Chapter 23 Creating Shafts

5In the ISO 355 dialog box, verify Geometry is selected and specify:

Inner Diameter: 40

Choose Next to continue.

You use the ISO 355 dialog box for the bearing calculation.

6In the ISO 355 dialog box, verify Calculation is selected and specify the val-

ues as shown below.

By choosing dynamic calculation, Mechanical Desktop is calculating the

adjusted rating life of the bearing.

Choose Next.

The possible bearings are calculated and the results are displayed in the ISO

355 dialog box in Result. Two tabs are provided so you can check both your

input and results.

Using the Shaft Generator |703

7In the ISO 355 dialog box, select the Result tab, and then select 2BC - 40 x 62

x 15.

Choose Finish.

Use dynamic dragging to size the bearing on the screen.

8Respond to the prompt as follows:

Drag size [Dialog] <10>:

Drag the bearing, and click when 2BC - 40 x 62 x 15 is displayed in the status bar

The bearing is inserted and your drawing should look like this.

Insert a second bearing, starting from the groove at the left of the fifth

segment of the shaft.

704 |Chapter 23 Creating Shafts

To add the second bearing

1In the 3D Shaft Generator dialog box, choose Std. Parts.

2In the Select a Part dialog box, choose Roller Bearings ➤ Radial ➤ ISO 355.

3Respond to the prompts as follows:

Select cylindrical face: Select a point on the fifth shaft segment (1)

Specify location on cylindrical face [Line/Plane]:

Select the right plane of the fifth shaft segment (2)

Enter distance from base plane [Associate to/Equation assistant] <25>:

Press ENTER

Choose insertion direction [Flip/Accept]: Enter f

4Use the default values for the calculation, and select the bearing ISO 355 2BD

- 32 x 52 x 14.

5Place the bearing by responding to the prompt as follows:

Drag size [Dialog] <10>:

Drag the bearing, and click when 2BC - 32 x 52 x 14 is displayed in the status bar

Close the 3D Shaft Generator dialog box. Your drawing should look like this.

Save your file.

Using the Shaft Generator |705

Displaying and Shading 3D Views

You can split your screen to display the front and isometric views of the shaft

in separate viewports. You can activate a viewport by clicking inside its

border.

To display front and isometric views in a split screen

1On the command line, enter 2, and press ENTER.

Your drawing area is split to display front and isometric views in separate

viewports.

2Click a viewport to activate it.

3Use AMDT_TOGGLE_SHADWIREF to add shading to the shaft.

Menu View ➤ Shade ➤ Gouraud Shaded

4Activate the second viewport and toggle to shading.

For better visualization, you can change the color properties of a single part,

such as the bearing.

706 |Chapter 23 Creating Shafts

To change the color of a single part on a shaft

1In the Desktop Browser, right-click a bearing and choose Properties ➤ Color.

2Select a different color.

The bearing is displayed in a different color on the shaft. Try changing the

colors of the other parts on the shaft.

Save your file.

707

In This Chapter 24

Calculating Stress on 3D

Parts

Autodesk® Mechanical Desktop® 6 Power Pack includes

a feature called 3D finite element analysis (FEA). FEA is

used to calculate deformation and stress conditions on

3D parts. The 3D FEA calculations feature is a reliable

tool that helps you meet the demands of today’s

sophisticated mechanical engineering.

In this tutorial, you calculate stress on a 3D part using

3D FEA. You create the mesh required to display the

results of the calculations, and then you define the loads

and make the calculations. When you finish, the

calculations are displayed in tables.

Run Mechanical Desktop with the power pack to

perform this tutorial.

■New in this tutorial

■Using 3D FEA calculations

■Defining loads

■Calculating and displaying the

result

708 |Chapter 24 Calculating Stress on 3D Parts

Key Terms

Te r m Definition

distributed force A force that is spread over an area.

FEA Finite element analysis. A calculation routine, or method. Calculates stress and

deformation in a plane for plates with a given thickness, or in a cross section with

individual forces, stretching loads, and fixed and/or moveable supports. The FEA

routine uses its own layer group for input and output.

fixed support A support that is fixed to a part and cannot be moved.

load Forces and moments that act on a part.

mesh Graphical representation of a mesh pattern on a model, required for FEA

calculation and display of the result.

result Results of FEA calculations. Result is displayed in a table, and as surface isoareas on

a model.

stress Force or pressure on a part. Stress is force per area.

surface isoarea Graphic representation of a stress calculation result displayed on the surface of a

model.

Tutorial at a Glance |709

Tutorial at a Glance

The 3D FEA calculations feature is a simple tool that eliminates the need for

the complex programs and calculations previously required to perform stress

and deformation calculations. In this tutorial, you learn to use 3D FEA for

calculations as you

■Start a finite element analysis.

■Define stress loads.

■Generate a mesh.

■Calculate and display the result.

Basic Concepts of 3D FEA

In Mechanical Desktop Power Pack, you use the FEA Calculation 3D dialog

box options to choose the

■Material of your part

■Revolution direction

■Type and quantity of supports and loads

The FEA calculations are dependent upon the definitions you enter for loads

and boundary conditions.

You consider how to reproduce the reality in your model, and how to define

the boundary conditions to achieve the best result. The more precise your

model is, the more useful the results are.

The FEA procedure uses a separate layer group for input and output.

710 |Chapter 24 Calculating Stress on 3D Parts

Using 3D FEA Calculations

To begin calculating the stress conditions on your model, you open the FEA

Calculation 3D dialog box. You work in this dialog box to choose the types

and quantity of loads and supports, and to define the loads and boundary

conditions.

Before you perform the calculation, you create a mesh on your 3D part. This

mesh is required to display the results of the calculation. The calculation is

displayed on your model using isoareas that define the limits of the stresses

and deformations. Tables are automatically created to define the calculations

for each isoarea.

Performing Finite Element Analyses

In the following exercise, you work with a lever that is loaded with a mass

and bolted at two faces. You reproduce these two points on the model as two

face supports, and define the mass as a face load at the front rectangular face.

Open the file md_ex03.dwg in the desktop\tutorial folder.

NOTE Back up the tutorial drawing files so you still have the original files if you

make a mistake. See “Backing up Tutorial Drawing Files” on page 40.

The drawing contains a 3D part, which is the basis for your calculations.

The first step is to open the FEA Calculations 3D dialog box.

Using 3D FEA Calculations |711

To start a finite element analysis

1Use AMFEA3D to perform the FEA calculation.

Menu Content 3D ➤ Calculations ➤ FEA

Respond to the prompt as follows:

Select 3D-Body: Select the 3D part

The FEA Calculation 3D dialog box is displayed.

NOTE If the FEA Calculation 3D dialog box hides your drawing, move the

dialog box to another position on the screen.

Defining Supports and Forces

Next, you define the supports and forces that act on your part. These defini-

tions are used for the FEA calculations.

712 |Chapter 24 Calculating Stress on 3D Parts

To define supports and forces on a part

1In the FEA Calculation 3D dialog box, choose the Face Support icon and

respond to the prompts as follows:

Select a surface: Click the edge (1) of the surface

Specify face [Accept/Next] <Accept>:

Press N to cycle to the surface you selected, then press ENTER

NOTE You may prefer to turn OSNAP off before you create and constrain the

work point. Click the OSNAP button at the bottom of your screen.

The Define Border for Load, Support dialog box is displayed.

Using 3D FEA Calculations |713

2In the Define Border for Load, Support dialog box, choose Whole Face.

Respond to the prompts as follows:

Define insertion point for main symbol:

Specify point or [Dialog]:

Specify a point, other than an edge, on the selected face

NOTE If the support does not act on the whole face, you can define an area

using the different options. See the Help for more information.

3In the FEA Calculation dialog box, choose the Face Support icon again, and

respond to the prompts as follows:

Select a surface: Click the edge (2) of the surface

Specify face [Accept/Next] <Accept>:

Press N to cycle to the surface you selected, then press ENTER

The Define Border for Load, Support dialog box is displayed.

714 |Chapter 24 Calculating Stress on 3D Parts

4In the Define Border for Load, Support dialog box, choose Whole Face, and

respond to the prompts as follows:

Define insertion point for main symbol:

Specify point or [Dialog]:

Specify a point, other than an edge, on the selected face

5In the FEA Calculation dialog box, choose the Face Force icon and respond

to the prompts as follows:

Select a surface: Click the edge (3) of the surface

Specify face [Accept/Next] <Accept>:

Press N to cycle to the surface you selected, then press ENTER

The Define Border for Load, Support dialog box is displayed.

6In the Define Border for Load, Support dialog box, choose Whole Face, and

respond to the prompts as follows:

Define insertion point for main symbol:

Specify point or [Dialog]: Specify a point, other than edge, on the selected face

The Angle type dialog box is displayed. Choose Normal, and respond to the

prompt as follows:

Specify value of load <10 (N/mm^2)>: Enter 2

Using 3D FEA Calculations |715

You have the defined the border conditions for two supports and one force.

Your drawing should look like this:

Calculating and Displaying the Result

Continue in the FEA Calculation 3D dialog box to perform the calculations

and display the results.

Before you can calculate and display the result, you need to generate a mesh.

To generate a mesh

1In the FEA Calculation 3D dialog box, under Run Calculation, turn on Auto

Refining.

2Choose the Run Calculation icon.

The Working dialog box is displayed during the automatic calculation of the

mesh. When the calculation is finished, a mesh is displayed on your model.

Next, define the placement of the mesh.

3Respond to the prompt as follows:

Specify base point or displacement <in boundary>: Press ENTER

This completes the mesh.

716 |Chapter 24 Calculating Stress on 3D Parts

Continue in the FEA Calculation 3D dialog box to calculate surface isoareas

and deformation.

4Under Results, choose the Isolines (Isoareas) icon.

5In the Surface Isolines (Isoareas) dialog box, choose the Isoareas button, and

choose OK.

Your model with isoareas is displayed on the screen beside the model with

mesh.

Respond to the prompts as follows:

Specify base point or displacement <in boundary>: Press ENTER

Specify insertion point or [Paper space]:

Specify a location for the table to the left of the isoareas display

NOTE If necessary, zoom to fit the entire display to your screen before you

place the second table.

6In the Surface Isolines (Isoareas) dialog box, choose the Deformed Mesh icon.

Using 3D FEA Calculations |717

7In the Deformed Mesh dialog box, turn on Automatic, and choose OK.

Respond to the prompts as follows:

Specify base point or displacement <in boundary>: Enter 150,150

Specify second point of displacement: Press ENTER

Specify insertion point or [Paper space]:

Specify a suitable location for the table near the mesh display

8Close the FEA Calculation 3D dialog box.

The calculations are finished, and the results are displayed.

718

In This Appendix

719

Toolbar Icons

Use this appendix as a guide to using the Autodesk®

Mechanical Desktop® toolbar icons. For an overview of

the toolbars and the Mechanical Desktop interface, refer

to “Mechanical Desktop Interface” on page 17 in

chapter 3.

■Desktop Tools toolbar icons

■Part Modeling toolbar icons

■Toolbody Modeling toolbar

icons

■Assembly Modeling toolbar

icons

■Surface Modeling toolbar icons

■Scene toolbar icons

■Drawing Layout toolbar icons

■Mechanical View toolbar icons

720 |Appendix A Toolbar Icons

Desktop Tools

If you are working in the Part Modeling environment, the Desktop Tools

toolbar contains three icons that activate the Part Modeling, Toolbody

Modeling, and Drawing Layout toolbars.

If you are working in the Assembly Modeling environment, the Desktop

Tools toolbar contains four icons that activate the Part Modeling, Assembly

Modeling, Scene, and Drawing Layout toolbars.

Part Modeling

Toolbody Modeling

Drawing Layout

Part Modeling

Assembly Modeling

Scene

Drawing Layout

Part Modeling |721

Part Modeling

The Part Modeling toolbar provides the tools you need for creating and

modifying parts.

Part Modeling ➤ New Part

New Part Flyout

New Sketch Plane Flyout

Launches 2D Sketch Toolbar

Launches 2D Constraints Toolbar

Profile a Sketch Flyout

Sketched Features Flyout

Placed Features Flyout

Work Features Flyout

Power Dimensioning Flyout

Edit Feature Flyout

Update Part Flyout

Part Visibility Flyout

Options Flyout

New Part

Mirror Part

Scale Part

Activate Part

Show Active

Make Base Feature

722 |Appendix A Toolbar Icons

Part Modeling ➤ New Sketch Plane

Part Modeling ➤ 2D Sketching

New Sketch Plane

Sketch View

Highlights Sketch Data

Launches 2D Sketch Toolbar

Construction Circle

Arc 3 Points Flyout

Rectangle

Construction Line

Circle Flyout

Copy Object

Mirror

Offset

Move

Trim

Extend

Fillet

Object Snaps Flyout

Erase

Re-Solve Sketch

Append to Sketch

Launches 2D Constraints Toolbar

Spline

Single Profile

Sketch Flyout

Polygon

Polyline

Line

Part Modeling |723

Part Modeling ➤ 2D Sketching ➤ Arc 3 Points

Part Modeling ➤ 2D Sketching ➤ Circle

Arc Start Center End

Arc 3 Points

Arc Start Center Angle

Arc Start Center Length

Arc Start End Angle

Arc Start End Direction

Arc Start End Radius

Arc Center Start End

Arc Center Start Angle

Arc Center Start Length

Arc Continue

Circle Center Radius

Ellipse Center

724 |Appendix A Toolbar Icons

Part Modeling ➤ 2D Sketching ➤ Object Snaps

Part Modeling ➤ 2D Sketching ➤ Sketch

Snap to Endpoint

Snap to Tangent

Snap to Apparent Intersect

Snap to Center

Profile

2D Path

3D Path

Cut Line

Split Line

Copy Sketch

Copy Edge

Break Line

Project to Plane

Text Sketch

Part Modeling |725

Part Modeling ➤ 2D Constraints

Launches 2D Constraints Toolbar

Tangent

Concentric

Collinear

Show Constraints

Delete Constraint

Parallel

Perpendicular

Horizontal

Vertical

Project

Join

X Value

Y Value

Radius

Equal Length

Power Dimensioning Flyout

Power Edit Flyout

Append to Sketch

Design Variables

Launches 2D Sketch Toolbar

Mirror

Fixed

Re-Solve Sketch

726 |Appendix A Toolbar Icons

Part Modeling ➤ 2D Constraints ➤ Power Dimensioning

Part Modeling ➤ 2D Constraints ➤ Power Edit

Part Modeling ➤ 2D Constraints ➤ Design Variables

Part Modeling ➤ Profile a Sketch

Power Dimensioning

New Dimension

Power Edit

Edit Dimension

Design Variables

Display as Numbers

Display as Equations

Display as Variables

Profile

3D Path

Cut Line

Split Line

Single Profile

2D Path

Re-Solve Sketch

Append to Sketch

Copy Sketch

Copy Edge

Break Line

Text Sketch

Part Modeling |727

Part Modeling ➤ Sketched Features

Part Modeling ➤ Placed Features

Part Modeling ➤ Work Features

Extrude

Face Split

Sweep

Loft

Revolve

Rib

Bend

Hole

Chamfer

Face Draft

Fillet

Rectangular Pattern

Copy Feature

Combine

Part Split

Surface Cut

Polar Pattern

Axial Pattern

Shell

Thread

Work Plane

Work Axis

Work Point

Create Basic Work Planes

728 |Appendix A Toolbar Icons

Part Modeling ➤ Power Dimensioning

Part Modeling ➤ Edit Feature

Part Modeling ➤ Update Part

New Dimension

Power Dimensioning

Edit Dimension

Power Edit

Edit Feature

Suppress by Type

Unsuppress Features

Reorder Feature

Suppress Features

Unsuppress Features by Type

Table Driven Suppression Access

Delete Feature

Update Part

Feature Replay

Update Assembly

Part Modeling |729

Part Modeling ➤ Part Visibility

Part Modeling ➤ Options

Part Visibility

Display All Work Planes

Display All Work Axes

Unhide All

Unhide Pick

Display All Work Points

Display All Cut Lines

Hide All

Hide All Except

Hide Pick

Part Options

Design Variables

List Part

Mass Properties

730 |Appendix A Toolbar Icons

Toolbody Modeling

In the Part Modeling environment, the Toolbody Modeling toolbar contains

the tools you need to create combined parts.

Toolbody Modeling ➤ New Toolbody

Toolbody Modeling ➤ Part Catalog

New Toolbody Flyout

Part Catalog Flyout

Instance

3D Toolbody Constraints Flyout

Assign Attributes

DOF Visibility

Rename Part

3D Manipulator Flyout

Check Interference Flyout

Design Variables

Update Positioning

Toolbody Visibility Flyout

Toolbody Options

New Toolbody

Activate Toolbody

Part Catalog

Detach Toolbody

Replace Toolbody

Where Used?

Input Part Definition

Output Part Definition

Toolbody Modeling |731

Toolbody Modeling ➤ 3D Toolbody Constraints

Toolbody Modeling ➤ Power Manipulator

Toolbody Modeling ➤ Check Interference

Launch 3D Constraints Toolbar

Mate

Flush

Angle

Insert

Edit Constraints

DOF Visibility

Update Positioning

Design Variables

Power Manipulator

List Part Data

Check 3D Interference

Audit External Refs

Update External Refs

Minimum 3D Distance

732 |Appendix A Toolbar Icons

Toolbody Modeling ➤ Toolbody Visibility

Assembly Modeling

In the Assembly Modeling environment, the Assembly Modeling toolbar

provides the tools you need to create and modify assemblies and subassemblies.

Toolbody Visibility

Unhide All

Unhide Pick

Display All Toolbodies

Display All CGs

Display All DOFs

Hide All Toolbody Objects

Hide All Except

Hide Picked Toolbody Objects

New Subassembly Flyout

Assembly Catalog Flyout

Instance

3D Assembly Constraints Flyout

Assign Attributes Flyout

DOF Visibility

Rename Part

3D Manipulator Flyout

Mass Properties Flyout

Design Variables

Update Assembly

Assembly Visibility Flyout

Assembly Options

Assembly Modeling |733

Assembly Modeling ➤ New Subassembly

Assembly Modeling ➤ Assembly Catalog

Assembly Modeling ➤ 3D Assembly Constraints

New Subassembly

Activate Assembly

Replace Part

Detach Part/Assembly

Assembly Catalog

Where Used?

Input Part Definition

Output Part Definition

Launch 3D Constraints Toolbar

Mate

Flush

Angle

Insert

Edit Constraints

DOF Visibility

Update Assembly

Design Variables

734 |Appendix A Toolbar Icons

Assembly Modeling ➤ Assign Attributes

Assembly Modeling ➤ Power Manipulator

Assembly Modeling ➤ Mass Properties

Assembly Modeling ➤ Assembly Visibility

Assign Attributes

Hatch Patterns

Power Manipulator

List Part Data

Mass Properties

Check 3D Interference

Minimum 3D Distance

Audit External Refs

Update External Refs

Assembly Visibility

Unhide All

Unhide Pick

Display All Parts

Display All Assemblies

Display All CGs

Display All DOFs

Hide All Assembly Objects

Hide All Except

Hide Picked Assembly Objects

Surface Modeling |735

Surface Modeling

The Surface Modeling toolbar provides the tools you need to create and mod-

ify 3D wireframe surfaces. To activate the Surface Modeling toolbar, choose

Surface ➤ Launch Toolbar.

Surface Modeling ➤ AutoSurf Options

AutoSurf Options Flyout

Toggles Keep Original

Loft U Surface Flyout

Blended Surface Flyout

Flow Wires Flyout

Object Visibility Flyout

Surface Analysis Flyout

Stitches Surfaces Flyout

Grip Point Placement Flyout

Lengthen Surface Flyout

Extract Surface Loop Flyout

Edit Augmented Line Flyout

Wire Direction Flyout

Swept Surface Flyout

AutoSurf Options

Cylinder Surface

Sphere Surface

Torus Surface

Cone Surface

736 |Appendix A Toolbar Icons

Surface Modeling ➤ Swept Surface

Surface Modeling ➤ Loft U Surface

Surface Modeling ➤ Blended Surface

Swept Surface

Extruded Surface

Tubular Surface

Revolved Surface

Loft U Surface

Loft UV Surface

Ruled Surface

Planar Surface

Planar Trimmed Surface

Blended Surface

Offset Surface

Fillet Surface

Corner Fillet Surface

Surface Modeling |737

Surface Modeling ➤ Flow Wires

Surface Modeling ➤ Object Visibility

Surface Modeling ➤ Surface Display

Flow Wires

Section Cuts

Augmented Line

Copy Surface Edge

Parting Line

Intersection Wire

Projection Wire

Offset Wire

Create Tangent Spline

Object Visibility

Unhide All

Unhide Pick

Hide All

Hide All Except

Hide Pick

Surface Display

Surface Mass Properties

Surface Analysis

738 |Appendix A Toolbar Icons

Surface Modeling ➤ Stitches Surfaces

Surface Modeling ➤ Grip Point Placement

Surface Modeling ➤ Lengthen Surface

Solid Cut

Convert Face

Convert All

Stitches Surfaces

Replace Surface Edge

Adjust

Surface Thicken

Grip Point Placement

Flip Surface Normal

Refine Surface

Intersect and Trim

Project and Trim

Lengthen Surface

Truncate Surface

Break Surface

Join Surfaces

Surface Modeling |739

Surface Modeling ➤ Extract Surface Loop

Surface Modeling ➤ Edit Augmented Line

Surface Modeling ➤ Wire Direction

Extract Surface Loop

Copy Surface Edge

Show Edge Nodes

Project and Trim

Delete All Trim

Edit Augmented Line

Add Vectors

Copy Vectors

Rotate Vectors

Blend Vectors

Vector Length

Twist Vectors

Delete Vectors

Wire Direction

Check Fit

Refine Wire

Fillet Wire

Join Wire

Create Fitted Spline

Unspline

Spline Edit

740 |Appendix A Toolbar Icons

Scene

In the Assembly Modeling environment, the Scene toolbar provides the tools

you need to create, modify, and manage scenes.

Scene ➤ New Scene

New Scene Flyout

Part or Subassembly Explosion Factor

New Trail

Edit Trail

Delete Tweak

New Tweak

Edit Tweak

Suppress Sectioning

Lock Scene Position

Update Scene

Scene Visibility Flyout

Scene Options

Scene Explosion Factor

Delete Trail

New Scene

Activate Scene

Edit Scene

Copy Scene

Delete Scene

Drawing Layout |741

Scene ➤ Scene Visibility

Drawing Layout

The Drawing Layout toolbar provides the tools you need to create, modify,

and annotate drawing views and layouts.

Scene Visibility

Unhide All

Unhide Pick

Display All Parts

Display All Assemblies

Display All Trails

Hide All Scene Objects

Hide All Except

Hide Picked Scene Objects

Mode

New Layout

New View

Multi-Views

Edit View

Move View

Delete View

Tolerance Modeling

List Drawing

Power Dimensioning

Update Drawing View

Drawing Visibility Flyout

Drawing Options

Copy View

742 |Appendix A Toolbar Icons

Drawing Layout ➤ Power Dimensioning

Drawing Layout ➤ Power Dimensioning ➤ Edit Format

Drawing Layout ➤ Power Dimensioning ➤ Welding Symbol

Power Dimensioning

Reference Dimension

Automatic Dimension

Power Edit

Edit Dimension

Move Dimension

Align Dimension Flyout

Welding Symbol Flyout

Line Text Flyout

Annotation Flyout

Dimension Style Flyout

Edit BOM Database

Align Dimension

Join Dimension

Insert Dimension

Break Dimension

Welding Symbol

Surface Texture

Feature Control Frame

Datum Identifier

Datum Target

Feature Identifier

Drawing Layout |743

Drawing Layout ➤ Power Dimensioning ➤ Line Text

Drawing Layout ➤ Power Dimensioning ➤ Annotation

Drawing Layout ➤ Power Dimensioning ➤ Edit BOM Database

Line Text

Multiline Text

Edit Text

Annotation

Leader

Hole Note Flyout

Centerline

Edit BOM Database

Place Balloon

Place Reference

Place Parts List

Part Reference Edit

Edit Part List/Balloon

744 |Appendix A Toolbar Icons

Drawing Layout ➤ Drawing Visibility

Mechanical View

The Mechanical View toolbar provides the tools you need to manage the

view of your design, control 3D viewports, and create rendered views of your

parts and assemblies.

If the Mechanical View toolbar is not visible on your desktop, choose View

➤ Toolbars ➤ Mechanical View. You can also right-click any toolbar, and

choose Mechanical View from the list.

Drawing Visibility

Unhide All

Unhide Pick

Display All Viewports

Display All Parts Lists

Display All Balloons

Display All Reference Dims

Display All Parametric Dims

Hide All Drawing Objects

Hide All Except

Hide Picked Drawing Objects

Zoom Realtime Flyout

Sketch View Flyout

Restore View #1 Flyout

Pan Realtime

3D Orbit Flyout

Toggle Shading/Wireframe Flyout

Mechanical View |745

Mechanical View ➤ Zoom Realtime

Mechanical View ➤ 3D Orbit

Zoom Realtime

Zoom All

Zoom In

Zoom Out

Zoom Previous

Zoom Window

3D Orbit

3D Continuous Orbit

3D Swivel

3D Adjust Distance

3D Adjust Clip Planes

Front Clip On/Off

Back Clip On/Off

New Rotation Center

Select Rotation Center

Lighting Control

3D Pan

3D Zoom

746 |Appendix A Toolbar Icons

Mechanical View ➤ Sketch View

Mechanical View ➤ Restore View #1

Sketch View

Top View

Bottom View

Left View

Right View

Front View

Back View

Left Front Isometric View

Right Front Isometric View

Left Back Isometric View

Right Back Isometric View

Restore View #1

Restore View #2

Restore View #3

Save View #1

Save View #2

Save View #3

Named Views

Single Viewport

Two Viewports

Three Viewports

Four Viewports

Mechanical View |747

Mechanical View ➤ Toggle Shading/Wireframe

Toggle Shading/Wireframe

2D Wireframe

3D Wireframe

Hidden

Flat Shaded

Gouraud Shaded

Flat Shaded, Edges On

Gouraud Shaded, Edges On

748

749

Index

active part variables,362

adjusting surfaces,569

ambient light on images,304

Angle type dialog box,714

angular dimensions,92

annotations,337

Approximate Model Size dialog box,624

array features, editing,223

assemblies

analyzing,506

completing,497

restructuring,479, 504

thumbnail previews,483

updating,509

Assembly Catalog,377, 400, 403, 482

Assembly Mass Properties dialog box,419, 510

assembly modeling

checking interference,418, 506, 510

concepts,401, 479

constraints,407, 414, 438, 486, 497

creating instances,502

drawing layouts,309, 428

files,400

mass properties,419

scenes,400, 421, 513

structures,478, 504

trails,400, 423

trees,400

assumed constraints,50, 97

attaching reference files,400

augmented lines,534, 548, 623

axial patterns,221

balloons,308, 338, 527

base features,122, 123, 254, 257, 578

base parts,444

base standards,672

base surfaces,534, 566, 576, 614, 617, 619

base views,308, 310, 380, 386, 478

bearing calculations,690

Bend dialog box,164

bend features,46, 163

bills of material (BOM),522

blended surfaces,559, 638

BOM databases,478, 522, 523

BOM dialog box,522

Boolean modeling,122, 444

border conditions, load,713

break lines, creating,80

breaking polylines,642

Browser command access,37

calculation result,708, 715, 717

callouts,338, 527

centerlines,336, 690

centermarks,336

Chamfer dialog box,204

chamfers,186, 204, 690

closed loop sketches,42

closed loop wires,620

closed profiles,42

collinear profile sketches,592

combine features,444, 457, 458

combining features,186, 227

combining parts, concepts,445

command access methods,37

complex parts,444

constraint symbols,50, 90

constraints

adding,591

assembly,438, 440, 497

assumed,50, 97

between features,276

concepts and tips,85

copied features,226

750 |Index

constraints (continued)

dimension,94

displaying,96

displaying symbols,90

equal length,110

fix,51, 88, 97

flush,478

geometric,84, 88, 94, 272

hiding,51

insert,400

mate,400, 407

missing,113

modifying,91, 414, 438

path sketch,111

project,107, 276

radial,102

sketch,42, 49, 86, 128, 175, 260

techniques,119

toolbody parts,454

construction geometry,42, 105

controlling tangency,115

dimensioning circles,118

in path sketches,111

lines,107

consumed sketches,122, 254

Context Menu command access,37

converged radial shapes,346

Copy Definition dialog box,378, 452

corners

fillets, blending,561

surfaces, filleting,565

counterbored holes, placing,598

Create Drawing View dialog box,310, 380, 429,

519

Create Scene dialog box,421

cross-section views,72, 317

cubic loft,122

cut lines, creating,42, 72, 74

cutting

features,350, 586, 605

planes,317

solids with surfaces,576, 584

cylinder axial placement,675

data exchange,6

default thicknesses,346

Define Border for Load, Support dialog box,713

definitions

assembly,509

copying,449

part,400, 444

renaming,400

degrees of freedom (DOF),84, 87, 406

derived surfaces,534, 559

design variables,362

active part,234, 239, 242

concepts,235

deleting,249

examining,247

global,234, 239, 246, 250

modifying,244

moving,248

table driven,234

Design Variables dialog box,240, 364

designs

changing,609

planning,615

reviewing,348

Desktop Browser,47, 254

changing part colors,416

copying parts,415

hierarchy,369

positioning,38

Desktop Menu command access,37

Desktop Visibility dialog box,143, 236, 323

detaching assembly files,400

detail views,314

dialog boxes

3D Pipe Path,69

3D Shaft Generator,693

3D Spline Path,71

Angle type,714

Appropriate Model Size,624

Assembly Catalog,377, 403, 482

Assembly Mass Properties,419, 510

Bend,164

BOM,522

Chamfer,204

Copy Definition,378, 452

Create Drawing View,310, 380, 429, 519

Create Scene,421

Define Border for Load, Support,713

Design Variables,240, 364

Desktop Visibility,143, 236, 323

Edge Properties,316, 329

Edit Drawing View,312, 316, 328

External Part Save,438

Extrusion,126, 262, 448, 492, 589

Extrusion, for thin features,138

Face Draft,194

FEA Calculation 3D,709, 711

Fillet,199

Fillet Surface,565

Helix,66, 242

Hole,189, 300, 475, 599

Hole Position Method,675

Join3D,631

Layer Properties Manager,125, 625

Lights,305

Loft,144

Index |751

Loft Surface,556

Mechanical Options,49, 524, 624

Mechanical Options, Part,54

Nominal Diameter,677

Note Symbol,334, 335, 394, 395

Object Grouping,558

Page Setup,426

Part Catalog,444, 449

Part Ref Attributes,526

Paste Special,397

Pattern,216

Please select a Screw,683

Plotter Configuration Editorial,427

Polyline Fit,550

Power Dimensioning,330

Power Manipulator,422, 516

Project to Surface,574, 637

Properties for ANSI,524

Revolution,150, 176, 289

Rib,136

Screw Connection,682

Select a Part,701

Select a Through Hole,675

Shaft,697

Shell Feature,209, 350

Splined Shaft,697

Surface Intersection,572

Surface Isolines (Isoareas),716

Sweep,156

Sweep Surface,541, 580

Table Driven Setup,364

Text Sketch,141

Trail Offsets,424, 518

Unsuppress by Type,375

View,238, 351, 448

Work Plane,171

dimensional constraints,84

dimensions

adding,97, 118, 275, 292

angular,92

as constraints,94

as equations,94

as parameters,384

attributes, changing,330

displaying,294

formatting,275

hiding,322, 324, 385

modifying,104, 280, 303

moving,325, 387

parameters,294

parametric,109, 260, 308

power,390

power editing,330

reference,308, 390, 432

direct light on images,304

distributed forces,708

DOF (degrees of freedom),84, 87, 406

draft angles,122, 186

drawing layouts

assembly,428

multiple,309

Drawing mode,308

drawing views

cleaning up,322, 384

concepts,309

creating,379, 425, 518

cross-section,317

detail,314

enhancing,330

isometric,320, 430

modifying,312, 340, 342

orthographic,313, 314, 318, 382

planning,309

plotting,426, 531

relocating,340

dynamic calculation,690, 702

dynamic dragging,690, 703

dynamic rotation,238

Edge Properties dialog box,316, 329

Edit Drawing View dialog box,312, 316, 328

emboss features,140

equal length constraints,110

equations for dimenions,94

excluded faces on shells,346, 353

exploded views,478, 513

External Part Save dialog box,438

external parts

attaching,403, 495

creating features,436

editing,434, 469, 508, 525

referencing,400, 403, 478, 483

reloading,509

extraneous dimensions, hiding,322, 324

extraneous lines in views, hiding,328

extruding

blindly, features,590

features,124, 138, 262, 270, 586, 605

parts,297

profiles,172, 282, 447, 492, 604

ribs,133

sketches,122, 589

surfaces,539, 636

text on parts,140

thin walls,136

weight reduction,465

Extrusion dialog box,126, 138, 262, 448, 492,

589

extrusion direction,539, 633

extrusions, weight reduction,471, 474

752 |Index

Face Draft dialog box,194

face drafts,186, 194

faces on shells,346

excluding,353

faces, splitting,152

FEA Calculation 3D dialog box,709, 711

features,42, 122

appending to tables,373

arrays, editing,223

base,122, 123, 254, 257, 258, 578

bend,46, 163

chamfering,204

combine,444, 457, 458

combining,186, 227

controlling shapes of,235

copying,224

creating from surfaces,577

cutting,350, 605

embossing,140

extruding,124, 130, 182, 262, 586

filleting,186

hole,188, 598

lofting,122, 143, 145

modifying,130, 149, 151, 155, 263, 303

patterns, creating,186, 214

placed,186, 254, 492, 598

positioning,179, 610

revolved,122, 150, 175, 284

rib,46

scaling,609

shelling,186, 209, 346, 347

sketching,121, 122, 123, 254, 601

suppressing,362, 371

surface cuts,212

swept,58, 122, 155, 244

symmetrical,290

thin,46

unsuppressing,375

files assembly, detaching,400

reference, attaching,400

tutorial, copying,40

Fillet dialog box,199

Fillet Surface dialog box,565

filleting

corners,99, 561

features,186, 199, 605

modifying,202

surfaces,565

finishing details,611

finite element analysis (FEA),708, 710

fix constraints,51, 88, 97

fixed support,708

flow lines, augmented,623

flush constraints,478

forces, distributed,708

generating shafts,690, 693

geometric constraints,84, 88, 94

global variables,362

graphics exchange,6

helical sweeps,122, 157, 234

Helix dialog box,66, 242

hidden lines,308

Hole dialog box,189, 300, 475, 599

hole notes,333, 335, 393

Hole Positon Method dialog box,675

hole, positioning,684

holes,186, 672

counterbored,302

creating,188, 598

drilled,300

modifying types,192

positioning,467, 474, 677

standard through,674

weight reduction,465

insert constraints,400

instancing parts,403, 444, 496

interference, checking,418, 506, 510

intersecting surfaces, trimming,572, 633

isoareas, surface,708

isolines, setting,146, 237

isometric views,320, 430

Join 3D dialog box,631

joining

lines,653, 660

surfaces,570, 579

wires,660

Layer Properties Manager dialog box,125, 625

layers,625, 628

layouts, multiple,309

lighting and shading images,304

Lights dialog box,305

linear loft,122

linesaugmented,534

joining,653, 660

Index |753

loads on parts,708

local parts,400, 478, 481

Loft dialog box,144

Loft Surface dialog box,556

lofted features,122, 143

lofted surfaces,555

lofting

cubic,145

linear,143

logical surface areas,614, 616

Manual mode vs. automatic,660

mass properties, calculating,419, 510

mate constraints,400, 407

Mechanical Options dialog box,49, 54, 524,

624

mesh, calculation,708

missing constraints,113

Model mode,308

model views,576

modeling, wireframe,534

motion-based surfaces,534, 538

multiple drawing layouts,309

nested loop sketches,42, 56

Nominal Diameter dialog box,677

nonorthogonal rectangular patterns,217

Note Symbol dialog box,334, 335, 394, 395

NURBS,576

Object Grouping dialog box,558

offset surfaces,563

open profiles,42, 46

orthographic views,313, 314, 318, 382

overriding wall thicknesses,346, 354, 356, 359

Page Setup dialog box,426

parallel,672

parametric dimensions,109, 308

parametric surfaces,582

parametrics,84, 168

parent views,308, 478

part definitions,52, 111, 115, 377, 400, 444,

449

design variables,362

faces, default thicknesses,346

faces, splitting,152

files,445

instances,444, 502

part (continued)

references,478, 525

supports and forces,711

toolbody,444

versions, displaying,366, 371, 375, 379

Part Catalog,444, 449

Part Ref Attributes dialog box,526

partsaligning,454

assembling,406

attaching,403, 495

base,444

calculating stress,708

combining with surfaces,577

combining, concepts,445

complex,444

copying,377, 415

creating,45, 255, 447, 491

cutting with surfaces,584

editing,434, 508

externally referencing,400, 403, 478, 483,

495

extruding,447

grounded,410

instancing,403, 496

local,400, 478, 481

rotating,238

shading,237

shading and lighting,304

splitting,229

standard, using,672

table driven,361, 367

thumbnail previews,450, 483

tweaking,400, 422, 515

versions,362

visibility of,611

parts lists,478, 529

Paste Special dialog box,397

path sketches,42, 58, 71, 111

Pattern dialog box,216

pattern features,186, 214

axial,221

polar,218

rectangular,215

rectangular, nonorthogonal,217

spacing,215, 217

pitches for paths,234

placed features,186, 254, 492, 598

concepts,187

planar surfaces,658

trimmed,554, 619, 627, 640

Please select a Screw dialog box,683

Plotter Configuration Editorial dialog box,427

plotting, drawing views,426, 531

754 |Index

polar patterns,218

Polyline Fit dialog box,550, 552

polylines,619, 629, 642, 643

power dimensioning,330, 390

Power Dimensioning dialog box,330

Power Manipulator dialog box,422, 516

preferences, surface,624

profile planes,234

profile sketches,71, 127, 258, 270, 282, 586,

588

closed,46

collinear,592

constraining to work points,181

construction geometry,105

examining,96

extruding to plane,172

open,46

revolving,175

single,597

text-based,45

profiles, adding to shafts,697

project constraints,107, 276

Project to Surface dialog box,574, 637

Project Trim,642, 644, 648, 650, 652, 664, 668

projected wires,614, 648

Properties for ANSI dialog box,524

radial constraints,102

rails,534, 540, 576

reclaimed faces on shells,346

rectangular patterns,215

reference dimensions,308, 332, 432

reference files, attaching,400

referencing parts externally,403, 478, 508

relief toolbodies,451, 461

reloading external references,509

replaying designs,348

restoring saved views,238

restructuring assemblies,504

result, calculation,708, 715, 717

Revolution dialog box,150, 176, 289

revolved features,122, 150, 284

revolved surfaces,538

Rib dialog box,136

rib features,46, 133

rotating parts,238

rough sketches,49, 51

ruled surfaces,546, 628, 635, 638, 656, 662

scaling features and surfaces,609

scenes,400, 420, 513, 515

Screw Connection dialog box,682

screw connections, inserting,681

Select a Part dialog box,701

Select a Through Hole dialog box,675

shading and lighting images,304

shading parts,237

Shaft dialog box,697

Shaft Generator, 3D, dialog box,693

shafts

contours, defining,693

editing segments,699

generating,690, 693

parts, changing colors,706

profiles, adding,697

standard parts, adding,701

thread, adding,695

views and shading,705

shapes

custom,46

dissimilar,544

distorted,595

sharp corners, surfacing,542, 550

Shell Feature dialog box,209, 350

shell features,186, 209, 346

concepts,347

cutting,350

editing,352, 355

multiple thicknesses,356

overriding wall thicknesses,346, 354, 359

Single Part mode,445, 446

sketch planes,122, 168, 254, 267, 590, 594

sketches,42

appending,100

consumed,122, 254

copying,471

extruding,589, 604

solving,49, 53, 58

using PLINE,44, 52

sketching

analyzing,47, 51, 255

break line,80

closed loop,42

closed profile,46

concepts,43, 123

constraints,86, 260, 272, 472

cut line,42, 72, 74, 76

dependencies,86

dimensions,275

dissimilar shapes,544

editing,54, 263, 280

features,121, 122, 123, 254, 258, 590, 604

geometry, interpreting,49

helical,65

nested loop,42, 56

open profiles,46

open shape,58

parametric,41

path,42, 58, 111

pipe path,67

Index |755

sketching (continued)

on planes,594, 601

process,255

profile,42, 96, 105, 127, 270, 586, 588,

592

restoring shapes of,595

rough,49

rules,47, 55

single profiles,106, 597

spline path,70

split line,42, 77

text sketch profiles,42, 45

tips,44

tolerances,42, 54

skin surfaces,534, 546

Splined Shaft dialog box,697

splines,576

split lines,42, 77, 154, 229

spreadsheets

linking,362

pasting into drawings,396

standard parts,672

adding to shafts,701

holes, through,674

standards, base,672

start angles for paths,234

stress on parts,708

analyzing,710

calculating and displaying,715

defining,711

structures of assemblies,478

subassemblies,478

constraining,498

creating,494

renaming,400

supports and forces, part,711

supports, fixed,708

suppressing features,362, 371

surface cuts,186, 212, 576

Surface Intersection dialog box,572

surface isoareas,708

Surface Isolines (Isoareas) dialog box,716

surface modeling,613

areas, logical,616

complex,616

concepts,535

corners,542

creating features,579

methods,620

polylines with sharp corners,550

primitives,534

wireframe,534

surface normals,534

surfaces

adjusting tangency,569

attaching parametrically,582

base,534, 566, 576, 614, 617, 619

surfaces (continued)

blended,559, 638

changing layers,628

complex,655

continuous,616

creating features from,577

derived,534, 559

editing,569, 581, 610

extruding,539, 633, 636

filleting corners,565

intersecting, trimming,572

joining,186, 570, 579

lofted,555

motion-based,534, 538

offset,563

planar,658

planar, trimmed,554, 619, 627, 640

planning designs,615

preferences for,624

projected wire trimmed,573

projection,661

resizing to scale,609

revolved,538

ruled,546, 628, 635, 638, 656, 662

scaling,609

skin,534, 546

smoothness,623

swept,540, 545, 576, 580, 645, 657, 667

trimming,622, 642, 644, 648, 650, 652,

664, 668

trimming intersecting,633

wireframe,613

Sweep dialog box,156

Sweep Surface dialog box,541, 580

sweeps, helical,122, 234

swept

dissimilar shapes,544

features,58, 122, 244

multiple cross sections,545

paths, construction geometry in,111

profiles,122

splines,542

surfaces,540, 645, 655, 657, 667

wires,540

symbols, constraint,50, 90

symmetry in features,290

table driven parts,361

concepts,363

Table Driven Setup dialog box,364

table driven variables,234

tables

conflicts, resolving,369

editing,367, 373

part versions,362

tangency, controlling,115, 672

756 |Index

taper angles for sweeps,234

Text Sketch dialog box,141

text sketch profiles,42, 45

thickness overrides,346, 356

thin features,46, 136

thread, defining,695

three-dimensional

edge paths,160

helical paths,65, 157

path sketches,62, 71

pipe paths,67, 161

spline paths,70, 162

through termination,672

tips constraining,86

sketching,44

title blocks, inserting,428

toolbodies,444

attaching,449

combining,453, 458, 463

constraining,462

consumption of,444

copying definitions,451

localizing external,451

nested,461

rollbacks,444

Toolbutton command access,37

Trail Offsets dialog box,424, 518

trails,400, 423, 478

trimming surfaces,622, 644, 648, 650, 652,

664, 668

tutorial drawing files,40

tweaking parts,400, 422, 478, 515

two-dimensional path sketches,59

U and V display lines,534, 540

Unsuppress by Type dialog box,375

user coordinate system (UCS),591, 690

variables, design,234

View dialog box,238, 351, 448

view scales,308, 312

views

base,308, 310, 380, 478

creating,518

cross-section,72

drawing,379

exploded,421, 478, 513

isometric,430

model,576

parent,308, 478

restoring,238

visibility

features,448

parts,611

work features,236

wall thickness overrides,354, 356, 359

watertight,614

weight reduction,465, 471, 474

wireframe modeling,534, 613

concepts,615

wires,534, 535, 576

closed loops,620

joining,653, 660

projecting,573, 614

sharp corners,617

work axes,168, 174, 254, 264

work features,254, 264

hiding,236

Work Plane dialog box,171

work planes,168, 254, 265, 576, 582

creating,58, 170

modifying,173

parametric, nonparametric,168

sketching,601

work points,168, 254, 576, 582

creating,179

modifying,182

Autodesk Auto CAD Mechanical Desktop 6.0 Instruction Manual Autocad 6 En

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