SolidWorks 2015, Simulation, Flow Simulation, eDrawings, eDrawings Professional, Sustainability, Plastics, Electrical, Composer, Enterprise PDM, Workgroup PDM software User guide

PDF

Document

Engineering Design and Technology Series

SAE

®

Design and Analysis

Project with SolidWorks

Software

®

Put Picture Here

Dassault Systèmes SolidWorks Corporation,

175 Wyman Street

Waltham, Massachusetts 02451 USA

Phone: +1-800-693-9000

Outside the U.S.: +1-781-810-5011

Fax: +1-781-810-3951

Email: [email protected]

Web: http://www.solidworks.com/education

Dassault Systèmes S.A. company, 175 Wyman Street, Waltham,

The information and the software discussed in this document are subject to change without notice and are not commitments by

Dassault Systèmes SolidWorks Corporation (DS SolidWorks).

No material may be reproduced or transmitted in any form or by any means, electronically or manually, for any purpose without the express written permission of DS SolidWorks.

The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of the license. All warranties given by DS SolidWorks as to the software and documentation are set forth in the license agreement, and nothing stated in, or implied by, this document or its contents shall be considered or deemed a modification or amendment of any terms, including warranties, in the license agreement.

Patent Notices

SolidWorks

3D mechanical CAD software is protected by U.S.

Patents 5,815,154; 6,219,049; 6,219,055; 6,611,725; 6,844,877;

6,898,560; 6,906,712; 7,079,990; 7,477,262; 7,558,705;

7,571,079; 7,590,497; 7,643,027; 7,672,822; 7,688,318;

7,694,238; 7,853,940, 8,305,376, and foreign patents,

(e.g., EP 1,116,190 B1 and JP 3,517,643).

eDrawings

software is protected by U.S. Patent 7,184,044; U.S.

Patent 7,502,027; and Canadian Patent 2,318,706.

U.S. and foreign patents pending.

Trademarks and Product Names for SolidWorks Products and Services

SolidWorks, 3D ContentCentral, 3D PartStream.NET, eDrawings, and the eDrawings logo are registered trademarks and

FeatureManager is a jointly owned registered trademark of DS

SolidWorks.

CircuitWorks, FloXpress, PhotoView 360, and TolAnalyst, are trademarks of DS SolidWorks.

FeatureWorks is a registered trademark of Geometric Ltd.

SolidWorks

2015, SolidWorks Enterprise PDM, SolidWorks

Workgroup PDM, SolidWorks Simulation, SolidWorks

Flow Simulation, eDrawings, eDrawings Professional, SolidWorks Sustainability,

SolidWorks Plastics, SolidWorks Electrical, and

SolidWorks Composer are product names of DS SolidWorks.

Other brand or product names are trademarks or registered trademarks of their respective holders.

COMMERCIAL COMPUTER SOFTWARE - PROPRIETARY

The Software is a "commercial item" as that term is defined at 48

C.F.R. 2.101 (OCT 1995), consisting of "commercial computer software" and "commercial software documentation" as such terms are used in 48 C.F.R. 12.212 (SEPT 1995) and is provided to the U.S. Government (a) for acquisition by or on behalf of civilian agencies, consistent with the policy set forth in 48 C.F.R.

12.212; or (b) for acquisition by or on behalf of units of the department of Defense, consistent with the policies set forth in 48

C.F.R. 227.7202-1 (JUN 1995) and 227.7202-4 (JUN 1995).

In the event that you receive a request from any agency of the U.S. government to provide Software with rights beyond those set forth above, you will notify DS SolidWorks of the scope of the request and DS SolidWorks will have five (5) business days to, in its sole discretion, accept or reject such request. Contractor/Manufacturer:

Dassault Systèmes SolidWorks Corporation, 175 Wyman Street,

Waltham, Massachusetts 02451 USA.

Copyright Notices for SolidWorks Standard, Premium,

Professional, and Education Products

This work contains the following software owned by Siemens

Industry Software Limited:

Portions of this software incorporate PhysX™ by NVIDIA 2006-

2010.

6,289,364; 6,563,502; 6,639,593; 6,754,382; Patents Pending.

Adobe, the Adobe logo, Acrobat, the Adobe PDF logo, Distiller and Reader are registered trademarks or trademarks of Adobe

Systems Inc. in the U.S. and other countries.

For more DS SolidWorks copyright information, see Help >

About SolidWorks.

Copyright Notices for SolidWorks Simulation Products

Copyright Notices for SolidWorks Enterprise PDM Product

Outside In

Copyright Notices for eDrawings Products

Mark Adler.

The eDrawings

for Windows

software is based in part on the work of the Independent JPEG Group.

Portions of eDrawings

Graphics Systems, Inc.

for iPad

Portions of eDrawings

Computer Inc.

for iPad

Document Number:

Contents

Lesson 1: Introduction . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 1

Using This Book . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

What is SolidWorks Software?

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

Prerequisites

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2

Conventions Used in This Book . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

Before You Begin

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3

Analyzing a Structure Using SolidWorks and SolidWorks Simulation

. . . . . . . . . . . . . . . . . . . . 5

Lesson 2: Using Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 7

Creating Parts In-Context . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

Opening an Assembly with Quick View . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8

Hiding and Showing Components. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9

The Assembly FeatureManager design tree . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12

Working In-Context . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

Edit Assembly Mode vs. Edit Part Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13

In-Context Parts and Virtual Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

Setup for Using Edit Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 14

Creating a New Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 15

Edit Part Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Why do the Colors Change? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Controlling the Display . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16

Understanding the Color Coding. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 21

Extrusions In-Context . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 24

Edit Assembly Mode . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26

Working with Virtual Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 26

Adding Component Instances and Mating

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 27

SolidWorks SAE Design and Analysis Project i

Contents

In-Context Part Editing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30

Opening a Part from an Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 31

Multi-body Materials. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

Reordering Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32

Materials

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 33

Pack and Go

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

Work Flow. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35

Lesson 3: Creating a Weldment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 39

Creating Weldment Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

Planes and Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

Structural Members . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

Weldments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40

Creating a Weldment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 41

Using Different Planes and Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 43

Using 2D Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46

Renaming and Opening a Virtual Part. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 50

Additional Planes and 2D Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 53

Sketching with Pierce Relations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54

Adding Bracing to the Frame

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 58

Using 3D Sketches

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 59

Sketching in the X, Y and Z Directions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60

3D Sketch Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 61

Placing a Component Using Sketch Geometry

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 63

Making Changes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 65

Working With Sub-Assemblies

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

Opening a Sub-assembly from the Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

Rigid vs. Flexible Sub-Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 66

Bracing Sketches

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 68

Remaining Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 69

Weldment Structural Members

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71

Creating Custom Profiles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 71

Adding Structural Members . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 74

Corner Treatments. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 75

Using Trim/Extend

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78

Trimming Boundary . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 78

Using Folders . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 79

Map for Structural Member Types and Trim/Extend . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80

Mirroring Structural Members . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 81

Editing

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82

Editing the Corner Treatment . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82

Using Locate Profile . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 84

ii SolidWorks SAE Design and Analysis Project

Contents

Using Instant 3D . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 87

Checking Clearances . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88

Interference Detection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90

Mounting Plates

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92

Creating a Reusable Sketch. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 92

Pasting the Sketch . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94

Weldment Cut Lists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 99

Cut List Properties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100

Save as External File . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100

Lesson 4: Using Molds and Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101

Molds and Surfaces . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 102

The runner part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103

Features in the Part . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103

Anatomy of a Loft . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 105

Creating Mold Tooling

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106

Surface and Solid Bodies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106

Description of the Bodies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 107

Mold Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108

What Does This Mean? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 110

Using Surfaces. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 113

Making Use of Symmetry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119

Lesson 5: Brake Rotor Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 123

Brake Rotor Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124

SolidWorks Simulation Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125

Transient Thermal Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 127

Thermal Boundary Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128

Convection . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128

Heat Power . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130

Post Processing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 133

Static Study

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134

Temperature Dependent Material Properties. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135

Fixtures

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 136

Braking Force

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 137

Thermal Loading . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 138

Post Processing . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140

Editing Plots . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 140

Chart Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141

Settings . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 141

Conclusions

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 142

SolidWorks SAE Design and Analysis Project iii

Contents

Lesson 6: Frame Analysis. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 143

Torsional Rigidity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 144

Element Types

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 144

Shell Elements. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145

Beam Elements . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 145

Preparing for Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 146

Experimental Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 147

Beam Meshing

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148

Section Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 148

End Conditions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 149

Trusses. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150

Joint Group . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 150

Merging Joints Automatically . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 152

Fixtures . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 153

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 154

Post Processing

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156

Cylindrical Coordinates. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156

Torsional Rigidity . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 158

Beam Stresses . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 159

Cross Section Directions 1 and 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160

Shear and Bending Diagrams . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 161

Conclusion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 162

Lesson 7: Intake Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 163

Intake Manifold Design . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

Model Preparations

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

External Flow Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

Internal Flow Analysis . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164

SolidWorks Flow Simulation Interface . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 165

Lids . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 166

Check Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167

Creating the Project

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167

Engineering Goals . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 174

Post-Processing

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 176

Color Bar . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177

Discussion . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 179

Conclusions

. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 179

iv SolidWorks SAE Design and Analysis Project

Lesson 1: Introduction

When you complete this lesson, you will be able to:



Describe the relationship between Parts, Assemblies and Drawings.



Identify the principal components of the SolidWorks user interface.



Download and extract the required companion files.

SolidWorks SAE Design and Analysis Project 1

Lesson 1: Introduction

Using This Book

The SAE Design and Analysis Project with SolidWorks Software helps you learn the principles of assembly design and structural analysis using SolidWorks and SolidWorks Simulation as an integral part of a creative and iterative design process.

For this project, you will “learn by doing” as you complete modeling and structural analysis lessons.

What is SolidWorks Software?

SolidWorks is design automation software. In SolidWorks, you sketch ideas and experiment with different designs to create 3D models using the easy to learn Windows

® graphical user interface.

SolidWorks is used by students, designers, engineers and other professionals to produce single and complex parts, assemblies and drawings.

Prerequisites

Before you begin the SAE Design and Analysis Project with

SolidWorks Software

you should complete the following tutorials that are integrated in the SolidWorks software:



Lesson 1 - Parts



Lesson 2 - Assemblies



Lesson 3 - Drawings

You can access the tutorials by clicking

Help

SolidWorks Tutorials.

The tutorial resizes the SolidWorks window and runs beside it.

As an alternative, you can complete the following lessons from CAD Student Guide:



Lesson 1: Using the Interface



Lesson 2: Basic Functionality



Lesson 3: The 40-Minute Running Start



Lesson 4: Assembly Basics



Lesson 6: Drawing Basics

2 SolidWorks SAE Design and Analysis Project

Lesson 1: Introduction

Conventions Used in This Book

This manual uses the following typographical conventions:

Convention

Bold Arial

Courier

New

17 Do this step.

Meaning

SolidWorks commands and options appear in this style.

For example, Insert, Boss means choose the Boss option from the Insert menu.

Feature names and file names appear in this style. For example,

Sketch1

The steps in the lessons are numbered in Bold Arial.

Before You Begin

If you have not done so already, copy the companion files for the lessons onto your computer before you begin this project.

Start SolidWorks.

Using the

Start

menu, start the SolidWorks application.

SolidWorks resources.

Click the

SolidWorks Resources

tab and click

Student Curriculum

SolidWorks SAE Design and Analysis Project 3

Lesson 1: Introduction

SolidWorks Content.

Expand the SolidWorks Educator Curriculum folder.

Expand the proper Curriculum <year> folder.

Click

Design Library

to open the design library task pane.

Click the SAE Car Design Project folder.

The lower pane will display an icon representing a Zip file that contains the companion files for this project.

Download the Zip file.

Press

Ctrl

and click the icon.

You will be prompted for a folder in which to save the Zip file.

Ask your teacher where you should save the

Zip file. Usually the C:\Temp folder is a good location.

Click

Tip:

Remember where you saved it.

Open the Zip file.

Browse to the folder where you saved the Zip file in step

Double-click the SAE Project Files.zip file.

Click Extract.

Click

Extract

and Browse to the location where you want to save the files. The system will automatically create a folder named _SAE_Project_ENG in the location you specify. For example, you might want to save it in My Documents.

Check with your teacher about where to save the files.

You now have a folder named SAE Project Files on your disk. The data in this folder will be used in the exercises.

Tip:

Remember where you saved it.

SolidWorks SAE Design and Analysis Project

Lesson 1: Introduction

Analyzing a Structure Using SolidWorks and SolidWorks Simulation

During this session, you will learn how to analyze a structure using SolidWorks and

SolidWorks Simulation.

Once you have had a chance to see how easy it is to use SolidWorks solid modeling software, you will use an assembly to check whether components fit properly.

SolidWorks SAE Design and Analysis Project 5

Lesson 1: Introduction

6 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

When you complete this lesson, you will be able to:



Understand the difference between edit assembly and edit part modes.



Create a virtual, in-context part.



Open a part from the assembly.



Create a new instance from an existing instance.



Set the materials in a part.



Use pack and go to manage the files.

SolidWorks SAE Design and Analysis Project 7

Lesson 2: Using Assemblies

Creating Parts In-Context

A thorough knowledge of how to work with assemblies is critical to success with SolidWorks.

In this example, you will create a virtual part and use incontext techniques to model a brake pad using geometry from both the Rotor - Cast Iron and Brake Caliper components.

The component will copied to create a second instance and it will be mated into the assembly.

Opening an Assembly with Quick View

Clicking the

Quick view / Selective open

when you open an assembly allows you to view only the components that you want to view.

Open Brake&Wheel.

Click

File, Open

and select the assembly Brake&Wheel from the Lesson

2\Brake&Wheel folder

. Select

Mode: Large Design Review

and click

Open

Click

on the

Large Design Review

page.

Note: At the message: Graphics data might be out of date for the

flagged components because these components reference inactive configurations

, click

SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Hiding and Showing Components

Components can be hidden or shown at any time to create an uncluttered display and make working on the assembly faster.

In addition, components that are hidden before opening the assembly are not loaded into memory, further decreasing the load on the machine.

Tip:

The Quick view / Selective open settings are stored in a Display State.

There are many ways to hide and show components. Here are a few useful methods and where they are best used.

Many

Components

Single or Few

Components

Hiding Components

Hide Others- Hides all visible components but the selected component(s).

Hide/Show Components-

Hides the selected visible components.

Showing Components

Show Hidden

Components-

Shows all the hidden components for selection.

Hide/Show Components-

Shows the selected hidden components.

Orientation.

The assembly opens in an Isometric orientation. Click in the graphics area and press

Shift+Arrow Up

to change the view orientation.

Where to Find It



Shortcut Menu: Right-click a component and click

Hide Others

Hide others.

Right-click the Rotor - Cast Iron and select

Hide Others

SolidWorks SAE Design and Analysis Project 9

Lesson 2: Using Assemblies

Where to Find It



Shortcut Menu: Right-click and click

Show Hidden Components

Show hidden.

Right-click in the graphics area and select

Show Hidden

Components

. Click the Brake Caliper component as shown.

Click

Exit Show-Hidden

to complete the command.

Where to Find It



CommandManager:

Large Design Review > Selective Open > Selective Open

Selective open.

Click

Selective Open

Click

All components displayed

and click

Open

These are the only components that we need to view right now.

Message.

A message appears.

Because you used “Selective Open”, hidden components are not loaded into memory. Therefore, when you first show a hidden component you might notice a delay while it is loaded. Also, a new Display State is created corresponding to the

“Selective Open” state.

Click

10 SolidWorks SAE Design and Analysis Project

Display state.

The changes are stored in the original display state

Default_Display_State-1

Lesson 2: Using Assemblies

Save.

Click

File, Save

to save the assembly and parts.

Orientation changes.

Press the

Spacebar

and click the orientation

Isometric from the dialog.

Middle

(wheel)+click

and drag the edge of the Rotor -

Cast Iron

as shown to rotate the geometry.

Zoom.

Click the Brake Caliper component in the

FeatureManager design tree and click

Zoom to

Selection

SolidWorks SAE Design and Analysis Project 11

Lesson 2: Using Assemblies

The Assembly FeatureManager design tree

The assembly is comprised of components and mates. The components can be either part components or assembly components (sub-assemblies). The assembly FeatureManager design tree shows an accurate snapshot of the assembly using icons and text to describe the current settings.

Hidden Sub-assembly

Component

Sub-assembly

Component

Part Component

Component

Instance

Mates

Folder

Hidden

Part

Component

Mate

Where to Find It



CommandManager:

Evaluate > AssemblyXpert



Menu:

Tools, AssemblyXpert

AssemblyXpert.

Click

AssemblyXpert

. The dialog lists the number of parts, unique parts, subassemblies and unique sub-assemblies among other things.

Click

SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Working In-Context

Working in-context means editing a component (part or assembly) while in the context of the assembly. The mode is toggled between

Edit Assembly

and

Edit Part.

Edit Assembly Mode vs. Edit Part Mode

When an assembly is opened, it opens in the default

Edit Assembly

mode. To create or edit a component part in-context,

Edit Part

is used. You can toggle back and forth between the modes using

Edit Component

Edit Assembly Edit Part

Tip:

Colors are used to indicate which mode is currently active. See "Why do the Colors

Change?" on page 16 for more information.

Below is a breakdown of some common actions that are typically performed in each mode:

Edit Assembly Mode

Adding new components

Inserting mates

Moving components

Edit Part Mode

Creating new sketches

Creating sketch geometry

Creating bosses or cut features

SolidWorks SAE Design and Analysis Project 13

Lesson 2: Using Assemblies

In-Context Parts and Virtual Parts

In-Context Parts

are parts that are created or edited in the context of the assembly. In-context part names appear in the

FeatureManager design tree appended with an arrow (In-

Context->

Virtual Parts

are in-context parts that are saved within the assembly rather than as separate part files. Parts can be both incontext and virtual. Virtual part names appear in the

FeatureManager design tree in square brackets

[Virtual_Part^Test]

Why use In-Context and Virtual Parts?

In-context parts reference other parts in the assembly and change automatically when the references change.

Virtual parts are more flexible because they can be renamed, deleted or saved as external

(part) files at any time.

Tip:

If there are no references, do not create the part in-context.

Setup for Using Edit Part

There are settings under system options that can be used to determine how assemblies and virtual parts behave in Edit Part mode.

Where to Find It



CommandManager:

Assembly > Edit Component



Shortcut Menu: Right-click a component and click

Edit Part

Virtual part setting.

Click

Tools, Options, System Options, Assemblies

and clear

Save new components to external files

Do not click

yet.

In-context appearance setting.

Click

Display/Selection

and select

Opaque Assembly

from the pulldown menu under

Assembly transparency for in context edit

Do not click

yet.

In-context part setting.

Click

Colors

and click

Use specified color when editing parts in assemblies

. That color is listed under the

Assembly, Edit Part

setting.

Click

14 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Creating a New Part

Creating an in-context new part requires a few selections including a planar face or plane for use as a sketch plane.

The selected face or plane will establish the orientation and position of the Front plane of the new virtual part. This in turn defines the orientations of the Top and Right planes.

Where to Find It



CommandManager:

Assembly > Insert

Components New Part



Menu:

Insert, Component, New Part

New part.

Click

New Part

and select the face of the Brake Caliper as shown.

SolidWorks SAE Design and Analysis Project 15

Lesson 2: Using Assemblies

Edit Part Mode

Edit Part Mode

is the opposite toggle of

Edit Assembly Mode

and allows the use of sketch and feature tools within the assembly. It is triggered by adding a new part component or editing an existing part in the assembly.

Why do the Colors Change?

Due to the settings made ("Setup for Using Edit Part" on page 14), the appearance of all

the parts remains opaque. The part being edited will appear in the

Assembly, Edit Part

color and all others appear in the

Assembly, Non-Edit Parts

color.

Controlling the Display

The display includes the visibility and colors of the components in the assembly.

Controlling the display is the first step in managing the assembly itself, and the Display

Pane is one of the best tools.

Display Pane

The

Display Pane

is a portion of the FeatureManager design tree that has visual controls and is usually hidden. The columns show the current state of

Hide/Show

Display Mode

Appearance

and

Transparency

and allow you to change them. The options are described below.



Hide/Show

- Toggles between

Hide Component

and

Show Component.



Display Mode

- Sets the display to

Wireframe

Hidden Lines Visible

Hidden Lines Removed

Shaded With Edges

Shaded

, or

Default

Display



Appearance

- Sets the appearance of the component. The lower triangle represents the part appearance while the upper triangle represents the component (assembly level) appearance.



Transparency

- Toggles

Transparency

on and off.

Note: The display pane works independently of the mode.

Where to Find It



Display Pane:

Hide/Show

in the component row

Note: Click

Hide Display Pane

to close the display pane.

16 SolidWorks SAE Design and Analysis Project

Display pane.

Click

Show Display Pane

to expand the display plane and change the appearance of components.

Expand the Brake Rotor Assembly folder.

Click the Rotor - Cast Iron component in the

Hide/Show

column as shown to hide it.

Lesson 2: Using Assemblies

Where to Find It



CommandManager:

Sketch > Convert Entities



Menu:

Tools, Sketch Tools, Convert Entities

Convert entities.

Select the face and click

Convert Entities

Tip:

If you see small green icons on the geometry of the sketch, you are seeing sketch relations.

Click View, Sketch Relations to shut off their display.

SolidWorks SAE Design and Analysis Project 17

Lesson 2: Using Assemblies

Delete.

Delete three entities to open the end of the sketch.

Note: There is one large arc and two small ones connected to it. Only one small arc is

shown here.

Convert edge.

Click

Show Display Pane

and show the Rotor - Cast Iron component.

Select the edge of the Rotor - Cast Iron component and click

Convert Entities

18 SolidWorks SAE Design and Analysis Project

Where to Find It



CommandManager:

Sketch > Sketch Fillet



Menu:

Tools, Sketch Tools, Fillet

Sketch fillets.

Click

Fillet

Fillet Radius

2.5mm

, and select the first set of geometry by selecting the geometry inside of where they would intersect.

Lesson 2: Using Assemblies

Repeat the selections for the similar geometry on the opposite side. Click twice.

View normal to.

Right-click the sketch in the FeatureManager and click

View Normal To

and zoom in as shown.

Delete.

Box select from upper left to lower right as shown to select the three entities.

Delete the three selected entities.

SolidWorks SAE Design and Analysis Project 19

Lesson 2: Using Assemblies

Drag endpoints.

Drag the endpoint of the vertical line outside the geometry as shown.

Repeat for the other vertical line and stop where the endpoints are horizontal.

Tangent Arc.

Click

Tools, Sketch Entities, Tangent Arc

and create the arc between the two endpoints as shown.

Drag and drop.

Drag the centerpoint of the arc to the edge of the circular edge. Drop it on the centerpoint that appears.

Previous view.

Click

Previous View

to go back to previous views and zoom states. Return to the zoomed isometric view.

SolidWorks SAE Design and Analysis Project

Extrude.

Click

Extrude

and set the

Depth

3mm

. Click .

Lesson 2: Using Assemblies

Understanding the Color Coding

The part turns blue when the extrusion is completed. The reason was explained earlier

("Why do the Colors Change?" on page 16) but until there is a solid body, it is difficult to

notice. This is the

Assembly, Edit Part

color and it appears in both the graphics and in the

FeatureManager design tree.

SolidWorks SAE Design and Analysis Project 21

Lesson 2: Using Assemblies

New sketch.

Select the face and click

Sketch

Convert entities.

Select the edge and click

Convert Entities

Where to Find It



CommandManager:

Sketch > Offset Entities



Menu:

Tools, Sketch Tools, Offset Entities

Offset entities.

Hide the Rotor - Cast Iron component. Click

Offset

Entities

and set the

Offset Distance

2mm

. Select the edge, click

Reverse

and click .

Repeat the procedure for the opposite side.

22 SolidWorks SAE Design and Analysis Project

Convert.

Show the Rotor - Cast Iron component. Select the edge as shown and click

Convert Entities

Click .

Lesson 2: Using Assemblies

Drag.

Drag the open endpoints out beyond the converted edge.

Trim.

Click

Trim Entities ,

Power trim

Click+Drag

across the sections of geometry using the paths shown to trim away excess geometry.

SolidWorks SAE Design and Analysis Project 23

Lesson 2: Using Assemblies

Sketch fillets.

Add sketch fillets

Radius 1mm

in four places as shown.

Tip:

If corners are trimmed to a single endpoint, select the endpoint to add the fillet.

Extrusions In-Context

Extrusions can also be created in-context when external features are referenced. In this example, the depth of an extrusion is measured as an offset from an existing face.

Extrude.

Click

Extrude

and set the

End Condition

Offset from

Surface

. Set the

Offset Distance

1.5mm

. Click in

Face/

Plane

field.

24 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Select other.

Right-click the face as shown and select

Select Other

. Click the top selection,

Face@Extrude1@[Brake Rotor Assembly<1>/Rotor - Cast

Iron<1>]

Tip:

The top selection at the cursor is not listed. Why? It is assumed that if you wanted to select that face you would have selected it directly.

Offset distance.

Check the direction and click .

SolidWorks SAE Design and Analysis Project 25

Lesson 2: Using Assemblies

Edit Assembly Mode

Edit Assembly Mode

is the opposite toggle of

Edit Part Mode

and is the default state of the assembly where you can add components and mates. It is triggered by exiting the editing of a part in the assembly or opening of an assembly file.

Edit assembly.

Click

Edit Component

or the confirmation corner to edit the assembly. This returns you to edit assembly mode and all the colors return to their original settings.

Working with Virtual Parts

The virtual part has been stored inside the assembly since it was created. Now that it is nearly complete, we will save it externally and make it a real part.

Renaming a Virtual Part

Rename.

Right-click the [Part1^Brake&Wheel] component and select

Rename Part

Type the name Brake Pad.

Tip:

Although the part has been renamed, it remains a virtual part.

Saving a Virtual Part as an External Part

The virtual part requires a location on disk to store the new *.sldprt file.

Save as external file.

Right-click the part and select

Save Part

(in External File).

The file Brake

Pad.sldprt

is added to the assembly folder.

Click

Same As Assembly

and

Tip:

The part name appears without the square brackets.

SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Adding Component Instances and Mating

Components can be added to the assembly in several ways. If there is already an instance of that component in the assembly, additional instances can be added using control+drag and drop.

Copy an instance.

Click and

Control+drag

the Brake Pad<1> component. Drop the component outside the Brake Caliper as shown.

Hide component.

Click the Rotor - Cast Iron component and click

Hide Components

SolidWorks SAE Design and Analysis Project 27

Lesson 2: Using Assemblies

First mate.

Press

Shift+Up Arrow

key. Click

Insert, Mate

and select the faces as shown. Click

Coincident

and Click .

Second mate.

Press the

Down Arrow

key. Select the faces as shown, click

Coincident

and click

Third mate.

Hide the Brake Caliper component. Select the faces as shown, click

Coincident

and click .

SolidWorks SAE Design and Analysis Project

Show.

Show the Brake Caliper component.

Lesson 2: Using Assemblies

Save.

Click

File, Save

to save the assembly and parts.

Viewing the Mates of a Component

The mates used to constrain a component can be listed and viewed using

View Mates

. It is a useful tool in understanding how components are used in the assembly.

Note: The arrow symbol indicates a path to ground. Mates marked like this are the

ones that hold the component in place.

Where to Find It



Shortcut Menu: Right-click a component and click

View Mates

View mates.

Click the Brake Pad<2> and

View Mates

Note: Click the “

” to close the dialog

SolidWorks SAE Design and Analysis Project 29

Lesson 2: Using Assemblies

In-Context Part Editing

Any component part can be edited in the assembly whether it was created in the context of the assembly or not. Toggling back to edit part mode uses the same command;

Edit Part

Edit part.

Click Brake Pad<1> and

Edit Part

New sketch.

Click the face and click

Insert Sketch

. A new sketch has been created on the face.

Convert edge.

Click the circular edge and click

Convert Entities

Click .

Exit the sketch.

30 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Opening a Part from an Assembly

In this example, we will create a slot to match up with the hole in the

Brake Pad component. The slot will be constructed from an existing hole and makes for easier fit up.

Open Brake Pad.

Click on the Brake Pad<2> in the FeatureManager design tree and select

Open

Part

Edit a sketch.

Right-click on Sketch3-> in the FeatureManager design tree and select

Edit Sketch

Construction.

Click the circle and click

For construction

to make it dashed.

Where to Find It



CommandManager:

Sketch

Straight Slot

Centerpoint Straight Slot



Menu:

Tools, Sketch Entities

Centerpoint Straight Slot

Slot.

Click

Tools, Sketch Entities

Centerpoint Straight Slot

and place the cursor at the center of the circle. Drag the cursor horizontally and click to create the centerline. Drag vertically and click to create the height. Click .

Relations.

Click the circle and a horizontal line of the slot. Add a

Tangent

relation.

SolidWorks SAE Design and Analysis Project 31

Lesson 2: Using Assemblies

Dimension and cut.

Add a

2mm

dimension as shown to fully define the sketch.

Create a cut using a

Through All

end condition.

Multi-body Materials

In order to have different materials in the same part there must be multiple solid bodies

(multi-bodies) within that part.

This part is currently made up of three features; two bosses and one cut feature. They are listed in their order of creation. There is just one solid body because by default new boss features are merged to the current body. The part will be edited to create multi-bodies.

Boss-Extrude1-> Boss-Extrude2-> Cut-Extrude1->

Reordering Features

Features can be reordered in the Feature Manager design tree using drag and drop. The rule to remember is that you cannot reorder a child feature before the parent feature. So how can you determine the parent/child relationships?

Parent/Child Relationships

The

Parent/Child

tool is used to determine the parents and children of any feature. In this case it will be used to determine the limits of where a feature can be reordered.

Parent/child.

Right-click the Cut-Extrude1 feature and select

Parent/Child

. The dialog tells you that the Boss-

Extrude1

and Sketch3 features are the parents of the selected feature. This also means that the

Boss-Extrude2

feature is not. This means that the child can be moved to a position between the boss features. Click

Close

Note: The Sketch3 feature is embedded in the Cut-Extrude1 feature.

32 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Reorder.

Drag the Cut-Extrude1 feature and drop it on the Boss-Extrude1 feature. This places it between the boss features.

Folder.

Click the first feature Boss-Extrude1,

Control+right-click

the second feature Cut-Extrude1 and select

Add to New Folder

Name the folder Backing.

Edit feature.

Click Boss-Extrude2 and

Edit Feature

Merge result

and click . There are now two solid bodies named Cut-

Extrude1

and Boss-Extrude2. Rename them to Plate and

Pad

as shown.

Tip:

The default names were taken from the last feature that was applied to the body.

Materials

Materials can be added to the entire part or to selected solid bodies within the part. In this case we will take advantage of the multi-body format to assign different materials to each body.

Where to Find It



Shortcut Menu: Right-click a component or body and click

Edit Material

SolidWorks SAE Design and Analysis Project 33

Lesson 2: Using Assemblies

Material for the Plate.

Right-click Plate from the body folder in the FeatureManager and select

Material, Edit Material

. Under

Steel,

select

1023

Carbon Steel Sheet (SS)

. Click

Apply

and

Close

Material for the pad body.

Right-click Pad from the body folder in the FeatureManager and select

Material, Edit Material

. Under

Other Non-metals,

select

Ceramic Porelain

. Click

Apply

and

Close

Note: Custom materials and custom material libraries can be

created.

Open assembly.

Press

Control+Tab

and move the cursor to the assembly.

This message appears:

Models contained within the assembly have changed. Would you like to rebuild the assembly now?

Click

Yes

Edit assembly.

Click

Edit Component

. Hide the Brake Caliper and

Rotor - Cast Iron

components.

Display state.

Create a new display state and rename to ALL. Right-click in the graphics area and click

Show Hidden Components

. Window-select all the components and click

Exit

Show Hidden

34 SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Pack and Go

Pack and Go

is utility that can be used to copy all files used by the assembly into a new folder or zip file, consolidating the file set into one location.

New

Folder

Zip

File

Work Flow

The work flow using Pack and Go creates multiple backups, using the last backup to start the next work session.

Creating a Zip File

Creating a zip file is a good way to consolidate the files and generate a backup in one step.

The zip file can be used to start the next session and then be stored away.

SolidWorks SAE Design and Analysis Project 35

Lesson 2: Using Assemblies

Pack and go.

Click

File, Pack and Go

and click

Save to Zip file

. Using

Browse

, set the location to a temporary folder, name the file Backup_1.zip and click

Save

Unzip.

At the start of the next session, unzip the file to a new folder and begin working. More files may be added from external drives or different folders.

Repeat the process.

At the start of the next session, unzip to a new folder and begin working. Repeat the process each time to keep all the files together.

Adding to File Names

If you want to rename the files with each new backup, the

Add prefix

and

Add suffix

options can be used.

For example, the file name Brake Caliper could become Brake Caliper_2 or

2-Hub Assembly

with a suffix or prefix added.

Note: Using a prefix or suffix changes the name. It is not the same as using the

SolidWorks Data Management product.

SolidWorks SAE Design and Analysis Project

Lesson 2: Using Assemblies

Appending the names.

Use the same settings as in the previous step

but click

Add suffix

and type _1 in the box. Click

Save

Tip:

Virtual parts that have not been saved as external files will appear greyed in the list with

<internal to assembly> as the folder. They are stored within the assembly that was active when they were created.

Save and close all files.

SolidWorks SAE Design and Analysis Project 37

Lesson 2: Using Assemblies

38 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

When you complete this lesson, you will be able to:



Create weldment parts.



Use 3D sketches.



Work with sub-assemblies.



Create custom profiles.



Add structural members.



Trim structural members.



Edit structural members.

SolidWorks SAE Design and Analysis Project 39

Lesson 3: Creating a Weldment

Creating Weldment Parts

The Frame will be built as an in-context

Weldment

using references from existing assemblies. The weldment process includes creating sketches, adding structural members and trimming the structural members.

Planes and Sketches

Planes and sketches, both 2D and 3D, are used to define the locations of the structural members in the weldment.

Structural Members

The structural members, square and round tubes in this example, are added to the lines and arcs of the sketches. After they are added they are trimmed to fit.

Weldments

Weldment

is a multi-body part composed of structural members. The centerlines of the structural members are sketched and profiles are selected from a library and are applied to the sketches.

Tip:

Most of the work to create a weldment is invested in the creation of the weldment sketches.

40 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Creating a Weldment

Creating a typical weldment involves several steps to create and trim the weldment members.

For example, this weldment is made up of five structural members; two of the longer length and three of the shorter length.

The following chart defines the basic steps in creating a weldment part.

Sketch

Create a new sketch that defines the centerlines of the weldment profiles.

The sketch can be a 2D or

3D sketch.

Close the sketch.

Create

Structural

Members

Click Structural

Member and select geometry.

Select a profile from the library for use with the geometry.

Trim and

Extend

Structural

Members

Click Trim/Extend and trim or extend the length of structural members to planes or other structural members.

Some Important Points about Weldments

Here are some important points to remember about weldments:



Weldment parts are multi-body parts. Each structural member is an individual solid body.



The profiles used are selected from a library. You must create your own profiles and library folders if the standard profiles are not what you need.



Weldments can make use of symmetry. Structural members can be patterned using

Mirror

with the

Bodies to Pattern

option.



A Cut-List folder is created to store information about the structural members and their lengths of the structural members. They can also be sorted by equal lengths.



Weldment Cut List

table can be generated in a drawing of the weldment.



The drawing can also have balloons like a BOM.

SolidWorks SAE Design and Analysis Project 41

Lesson 3: Creating a Weldment

Some Details About Weldment Sketches

Weldment sketches are used to define the centerlines of beams used in the weldment.

Continuous beams should be created using single pieces of geometry. If they are not, smaller separate pieces will be created.

Sketches used for weldments may be different than sketches used for other features. For example, the sketch shown here would not be useful for a boss extrude or revolve.

Single Line

Open Frame&Suspension.

Multiple Lines

Click

File, Open

and select the assembly Frame&Suspension from the Lesson

3\Frame&Suspension

folder.

42 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Show sketches.

Open any instance of the A-Arm Spherical Ball component.

Right-click Sketch1 and select

Show

Return to the assembly.

Note: The A-Arm Spherical Ball components can be rotated for a better view

of the sketch.

Using Different Planes and Sketches

In the process of adding a new part in-context, a planar face or plane must be selected.

This plane is used as a sketch plane and a new sketch is opened. In fact, several things happen at once when the plane is selected:



A new in-context part is created.



The new part is being edited.



A new sketch is created on the selected plane.



The new sketch is open.



The selected plane becomes the Front plane of the new part.

The new sketch may not be the sketch you want. Although it is a requirement to select something, you do not have to use the sketch. You can just exit the sketch and create the plane or sketch that you need.

SolidWorks SAE Design and Analysis Project 43

Lesson 3: Creating a Weldment

New part.

Click

Insert, Component, New Part

and select the plane Ground. A new sketch, in

the new part, is automatically started on the selected plane. See "Creating a New Part" on page 15 for more information.

Note: The Ground plane is selected, but in theory any plane or planar face could

have been selected because none of the existing planes or planar faces is sufficient.

Exit sketch.

Right-click in the graphics area and select

Exit Sketch

to leave the current sketch.

You are still editing the new part.

Reference plane.

Click

Insert, Reference Geometry, Plane

Select the plane Front from the active part

[Part1^Frame&Suspension]<1>

and

Parallel

Select the centerpoint of an arc from A-Arm Spherical

Ball

(connected to the A-arm - Upper assembly) as shown. Click and rename the plane Upper_Arm.

44 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Lower plane.

Using the same procedure as the previous step, create a new plane using the plane Front and a centerpoint of an arc from

A-Arm Spherical Ball

(connected to the A-arm -

Lower assembly) as shown. Click and rename the plane

Lower_Arm

SolidWorks SAE Design and Analysis Project 45

Lesson 3: Creating a Weldment

Using 2D Sketches

A series of 2D sketches will be created to form the basic shape of the frame.

3D sketches will be used to fill in much of the bracing and support structure after the basic shapes are complete.

Note: Many of the 2D sketches, like this one, will require the creation of new planes.

New sketch.

Right-click the plane Lower_Arm and

Sketch

Rectangle.

Click

Rectangle

and sketch as shown.

46 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Reference to existing geometry.

Add dimensions between the centerpoint of the arc and the edge of the rectangle as shown. Set the values to

35mm

and

30mm

. Selection of A-Arm Spherical Ball geometry for the dimensions creates external references to that component.

Centering geometry.

Sketch a centerline connecting the midpoint of the line and the origin as shown. Add a

Horizontal

relation.

SolidWorks SAE Design and Analysis Project 47

Lesson 3: Creating a Weldment

Add line and dimension.

Add the line and dimensions

710mm

and

430mm

as shown.

Exit sketch.

Right-click in the graphics area and select

Exit Sketch

to leave the current sketch.

Rename the sketch Main.

New plane.

Control+drag

the plane Lower_Arm downwards. In the

Plane

dialog set the offset to

115mm

. Rename the plane Lower_Frame.

Hide components.

Hide the Steering Wheel and Steering Rack and Shaft Assembly assemblies.

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

New sketch.

Create a new sketch on the plane Lower_Frame. Sketch the lines and a centerline connecting the midpoints of both lines as shown.

Symmetry.

Add a

Horizontal

relation to the centerline. The two angled lines are now symmetric to each other.

Relation to inactive sketch.

Select the centerline of the current sketch,

control+select

the centerline of the inactive sketch and add a

Collinear

relation.

SolidWorks SAE Design and Analysis Project 49

Lesson 3: Creating a Weldment

Complete sketch.

Add the dimensions as shown. Exit the sketch. Rename the sketch Lower_Frame

_Sketch

Renaming and Opening a Virtual Part

It is easier to work on the part outside the assembly provided that the assembly geometry is not being referenced. The part can be opened even though it is a virtual part.

Rename the virtual part.

Right-click the virtual part Part1^Frame&Suspension in the FeatureManager design tree and select

Rename Part

. Type Frame.

Open the virtual part.

Right-click the virtual part Frame^Frame&Suspension and select

Open Part

50 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Why is the View Orientation Different?

When a new part is created in-context, the initial plane or planar face selected defines the position and orientation of the Front plane of the new part. This may cause the new part to an unexpected orientation, different than that of the assembly. Saving a view state is a great solution.

Orientation.

Click

View, Modify, Rotate

and rotate the view orientation so that it looks similar to that of the assembly.

Save a view state.

In order to save the view orientation and zoom, save a view state. Press the

Spacebar

and click the

New View

icon on the

Orientation

dialog.

Type the name ISO and click

The view name ISO will be added to the list and can recalled by double-clicking.

Plane.

Create a new plane using the plane Right and

Parallel

for the

First Reference

and the endpoint of the Main sketch as the

Second Reference

. Rename the plane

Bulkhead1

SolidWorks SAE Design and Analysis Project 51

Lesson 3: Creating a Weldment

Sketch geometry.

Create a new sketch on the plane Bulkhead1. Add lines to the existing endpoints of the Main sketch. Select the centerline, control+select the endpoints and add a

Symmetric

relation.

Note: Endpoints or geometry can be selected for the addition of a symmetry relation.

Dimensions and fillets.

Add the three linear dimensions (

440mm

215mm

and

420mm

) as shown.

Click

Sketch Fillet

and set the

Fillet Radius

100mm

. Select four corners as shown. Click .

Tip:

If this message appears:

At least one segment being filleted has a midpoint or equal length relation. Geometry may have to move to satisfy this relation when the fillet is created. Do you want to continue?

Click Yes.

Close the sketch and rename it to

Bulkhead1_Sketch

52 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Additional Planes and 2D Sketches

A series of small 2D planes and sketches are needed to define the shape of the frame.

Bulkhead3_sketch

Bulkhead2_sketch

Seat_Angle_sketch

Engine2_sketch

Engine1_sketch

Through_Point_Sketch

Bulkhead2

and Bulkhead3 planes and sketches.

Create planes parallel to Right through the endpoints in the Main sketch and create the following sketches.

Bulkhead2_sketch

Bulkhead3_sketch

SolidWorks SAE Design and Analysis Project 53

Lesson 3: Creating a Weldment

Seat position and angle.

Create a new plane using Right and

Parallel

for the

First Reference

and the endpoint of the Lower_Frame_Sketch as the

Second Reference

. Rename to

Seat_Position

Using Seat_Position and the sketch line as shown, create a new plane. Click

Angle

and use

degrees. Rename it to Seat_Angle.

Create the sketch and rename it to Seat_Angle_sketch.

Tip:

Add the 100mm sketch fillets before the 90mm and 500mm dimensions.

Sketching with Pierce Relations

So far, we have connected geometry to endpoints and midpoints. But what if the structural members are connected to an arc or elbow shape? This method utilizes a lesser known relation called

Pierce

. The pierce relation positions an endpoint where the sketch plane intersects (pierces) the selected geometry.

Note: Sometimes it is necessary to create a bracing member in order to create

bulkheads and other sketches. In this case the position of the bracing member is required to sketch the position of a bulkhead.

54 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Edit sketch.

Edit the sketch Bulkhead1_Sketch. Click

Point

add a point near the arc. Add a

Midpoint

relation between the point and the arc as shown. Exit the sketch.

Plane through point.

Create a new plane using Front and

Parallel

for the

First Reference

and the point as the

Second Reference

. Rename to Through_Point.

SolidWorks SAE Design and Analysis Project 55

Lesson 3: Creating a Weldment

Pierce.

Create a new sketch on the Through_Point plane. Sketch a line from the point towards the arc as shown. Select the endpoint and the arc and add a

Pierce

relation.

Rename to Through_Point_Sketch.

Planes.

Create a new plane offset

550mm

from the Seat_Position plane. Rename to

Engine1

. Offset

300mm

from the Engine1 to create Engine2.

56 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Converting a single sketch entity.

Create a new sketch on the Engine1 plane. Click

Convert Entities

and select the centerline in the Seat_Angle_sketch as shown. Click . Click the line and select

Construction Geometry

. Add the lines to the centerline as shown.

Mirror in the sketch.

Click

Tools, Sketch Tools, Mirror

and select the three sketched lines. Right-click and select the centerline and click .

SolidWorks SAE Design and Analysis Project 57

Lesson 3: Creating a Weldment

Collinear with a plane.

Add a

Collinear

relation between the

Through_Point

plane and the top line and add the dimensions as shown. Exit the sketch and rename it

Engine1_Sketch

Converting an entire sketch.

Create a new sketch on the Engine2 plane.

Click

Convert Entities

and select the sketch

Engine1_Sketch using the flyout

FeatureManager design tree as shown. Click .

Close the sketch and rename it

Engine2_Sketch

Adding Bracing to the Frame

Bracing is added between the existing sketches using more sketches. The best practice is to use the type that is most suitable in the situation, 2D or 3D. For more information

regarding 3D sketches, see "Using 3D Sketches" on page 59.

Tip:

All of the previous sketches could have been created as 3D sketches.

58 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Sketch.

Create a new sketch on the Through_Point plane. Add the two centerlines, three lines and two dimensions as shown. Rename to Engine_Mount.

Exit the sketch in an under defined state.

Note: This sketch is another example of a valid weldment sketch that would be

unsuitable for a standard extrusion. For more information, see "Some Details

About Weldment Sketches" on page 42.

Using 3D Sketches

3D sketches are very useful in creating sketch geometry that does not lie on an existing or easily definable plane. Bracing lines that cross through 3D space between existing endpoints are best created using 3D sketches.

Where to Find It



CommandManager:

Sketch > Sketch > 3D Sketch



Menu:

Insert, 3D Sketch

SolidWorks SAE Design and Analysis Project 59

Lesson 3: Creating a Weldment

Sketching in the X, Y and Z Directions

The

Space Handles

that appear in a 3D sketch when creating lines can be used to sketch along the

and

directions. The direction is shown at the cursor.

Note: The space handles can be ignored to sketch between endpoints in 3D space.

How do you know if you are in a 3D sketch?

Look at the

Status Bar

near the bottom right corner of the window. It will say Editing

3DSketch1

for a 3D sketch or Editing Sketch6 for a 2D sketch.

3D sketch.

Click

3D Sketch

and add a line. Start the line at the lower endpoint and end it on the angled line as shown. A

Coincident

relation is added in the process.

60 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

3D Sketch Dimensions

The

Tab

key can be pressed while creating a dimension to switch between the true distance (absolute) and distances along the X, Y and Z axes.

Select the line and place the dimension... (Absolute)

Select the line and...

press Tab once

(Along X) press Tab twice

(Along Y) press Tab three times (Along Z)

Note: Once created, you can use

Edit Sketch

to edit either a 2D or 3D sketch.

SolidWorks SAE Design and Analysis Project 61

Lesson 3: Creating a Weldment

Dimension.

Add an absolute dimension of

350mm

that defines the true length of the line.

Exit the sketch.

Assembly.

Press

Ctrl+Tab

and click the assembly. At the message: Models contained within the assembly have changed. Would you like to rebuild the assembly now?

Click

Yes

Edit assembly.

Edit the assembly by right-clicking in the graphics area and selecting

Edit Assembly:

FrameSuspension

Save.

Save

the assembly and click

Save All

. At the message: This assembly contains unsaved virtual components which must be saved click

Save internally (inside the assembly)

click

Show display state.

There are many components that have been hidden. They will be shown now.

Click the ConfigurationManager tab in the FeatureManager design tree and doubleclick the display state Full_Display State-1. Click the FeatureManager design tree tab .

Hide planes.

If there are planes visible, click

View, Planes

to turn of the display.

SolidWorks SAE Design and Analysis Project

Placing a Component Using Sketch Geometry

The geometry of the Frame, an in-context virtual part, can be used to create mates as well as place and orient components.

Lesson 3: Creating a Weldment

Insert component and mate.

Click

Insert, Component, Existing Part/Assembly

and select the ENGINE part from the Lesson 3 folder.

Mate the Right plane of the ENGINE and the Centerline plane of the assembly using a

Coincident

mate.

Note: Use the

Aligned

and

Anti-Aligned

options to get the mate alignment as shown.

SolidWorks SAE Design and Analysis Project 63

Lesson 3: Creating a Weldment

Concentric mate.

Select the cylindrical face of the engine and the sketch line as shown. Add a

Concentric

mate between them.

Rotate.

Rotate the under defined component as shown.

64 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Making Changes

With the addition of the ENGINE, we can see that it appears to be too close to the

Engine1_sketch

(inside right box). One solution may be to pull the attachment point back by shortening the length of a line in the Engine_Mount sketch (inside left box).

Change dimension value.

Return to the part by pressing

Ctrl+Tab

and clicking the part.

Double-click the Engine_Mount sketch in the FeatureManager design tree and change the dimension to

50mm

as shown. Click

Rebuild

Return to the assembly.

Press

Ctrl+Tab

and click the assembly. With the change in the sketch geometry, the engine has been pulled back to a better position within the frame as shown.

SolidWorks SAE Design and Analysis Project 65

Lesson 3: Creating a Weldment

Working With Sub-Assemblies

Large assemblies often have multiple sub-assemblies within them.

This is good practice and helps make the assembly easier to work with by shortening the FeatureManager design tree and breaking the components into logical groups.

This section will show how to open a sub-assembly from the main assembly and set Component Properties.

Opening a Sub-assembly from the Assembly

Sub-assembly components can be opened directly from the assembly FeaureManager design tree like part components.

Tip:

Right-clicking a component part in the sub-assembly and trying to open it will open the part only.

Open sub-assembly.

Right-click the sub-assembly Rear Axle Assembly from the FeatureManager design tree and select

Open assembly

Rigid vs. Flexible Sub-Assemblies

All sub-assemblies have the option of being solved as

Rigid

Flexible

Where to Find It



Shortcut Menu: Right-click a sub-assembly and click

Component Properties

Change the

Solve as

option to

Rigid

Flexible

Rigid

Rigid treats the entire sub-assembly as a single rigid component when used as a subassembly. Rigid is the default condition for all sub-assemblies.

Flexible

Flexible allows the components that can move or rotate in the assembly to move or rotate when used as a sub-assembly.

66 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Test component.

The assembly is designed so that the

Sprocket

is free to move along the axis CL

Rear Axle

. Move it a small amount to test it.

Close the sub-assembly without changes and return to the main assembly. Click

Discard

Warning.

To line up the Sprocket with the engine output, select the faces indicated and try to add a

Coincident

mate. A warning saying that the coincident mate cannot be added will appear. Click .

Why Does the Warning Appear?

The sub-assembly is solved as the default rigid condition which does not allow components in the sub-assembly to move independently.

Component properties.

Right-click the Rear Axle Assembly and select

Component Properties

Flexible

and

Solve as

, click

Using the same procedure as in step

, add the

Coincident

mate.

SolidWorks SAE Design and Analysis Project 67

Lesson 3: Creating a Weldment

Bracing Sketches

There are several more planes and sketches required to complete the Frame geometry.

Open part.

Open the virtual part Frame.

Pierce relation sketches.

Create a new plane through the endpoint indicated and

Parallel

to Front plane. Use the plane to create two new sketches.

In the each sketch, use one

Coincident

and one

Pierce

relation.

Note: The pierce relation in the first sketch uses an arc, the second uses a line.

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Remaining Sketches

The remaining sketches are all 3D sketches and will be presented with a brief description and an image as shown below.

Two lines and

Coincident relations.

Two lines,

Coincident

and

Midpoint

relations.

SolidWorks SAE Design and Analysis Project 69

Lesson 3: Creating a Weldment

One line and

Coincident relations.

Four lines and

Coincident relations.

Why is the Bracing One Sided?

The resulting structural members will be mirrored across a plane to create the bracing on

the opposite side. For more information, see "Mirroring Structural Members" on page 81.

70 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Weldment Structural Members

Weldments use standard profile shapes that are applied to sketch geometry to create structural members. Each structural member is a separate solid body in the multi-body part.

Weldments also track the quantities and lengths of the structural members using a weldment cut-list.

A Quick Look at the Standard Profiles

The weldment profiles are divided into two

Standard

folders: ansi inch and iso.

Profiles must be library features and be present in the folders to be used. The standard profiles use these shapes: angle iron c channel pipe rectangular or square tube s section

sb beam

Weldment Cut List

The

Weldment Cut List

tracks the structural member types and lengths.

Creating Custom Profiles

We need two profiles: a round (pipe) tube and a square tube each with an outside measurement of

25.4mm

. This size is different than the standard sizes, so they will need to be created and placed in the proper folders.

Note: The weldment profiles are set to specific folders by the

option

Tools, Options, File Locations

and

Weldment Profiles

Open a new part.

Open a new part with mm units.

SolidWorks SAE Design and Analysis Project 71

Lesson 3: Creating a Weldment

Sketch.

Create a new sketch on the Front plane and sketch a

25.4mm

circle and dimension as shown.

Add an offset of

2.4mm

as shown and exit the sketch.

Save as library feature.

Select the sketch Sketch1. Click

File, Save As

Select the

Save as type Lib Feat Part (*.sldlfp)

, type the file name 25.4mm Dia, and click

Save

For

Save in

, navigate to the default weldment library folder located in the

C:\Program Files\SolidWorks Corp\SolidWorks\lang\english\ weldment profiles

folder.

Note: If you receive a message that you are not allowed to save in that folder, try

saving the file in a local folder and moving the file to that folder. Also, the full path used in this lesson is based upon the default installation on SolidWorks onto the C drive. If SolidWorks has not been installed using the default settings, then the path will require some adjustment.

72 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Library Feature Folders and Icons

The library feature is a different file type and uses different icons for the top level component and the sketch.

Close library feature.

Close the library feature part.

Create new Folders.

Adding the weldment profile to the weldment profiles folder is not enough to make use of it.

Create a new folder FSAE in the

<Install Directory>\Program Files\SolidWorks Corp/

SolidWorks\lang\english\weldment profiles

folder. Open that folder and create two folders named Square Tubes and Round Tubes.

Move the 25.4mm Dia.SLDLFP file into the Round Tubes folder.

Move existing file.

Move the existing 25mm Sides.SLDLFP file into the Square Tubes folder.

Note: The file can be found in the Lesson 3 folder.

Why Do Some Profiles Contain Points?

Profiles formed using lines typically contain points at the corners like this tube. They are useful in moving the profile to a position other than the centerline.

SolidWorks SAE Design and Analysis Project 73

Lesson 3: Creating a Weldment

Adding Structural Members

Adding the structural members is the simplest part of the process. Selecting the existing sketch geometry gives the structural members position and length.

It is helpful to keep all the related features together in the FeatureManager design tree for

future editing. In order to do this, it is best to rollback. See "Using Folders" on page 79 for

more information.

Move the rollback bar to a position after the sketch feature that you want to use for creating structural members.

Select the geometry of inactive sketches to define the centerlines of the structural members.

Add only structural members of the same type in the same feature.

Rollback.

In the Frame part, right-click the Bulkhead2 plane and select

Rollback

This will place the Structural Member feature just after the

Bulkhead1_Sketch

sketch, near the related plane.

Structural member.

Click

Insert, Weldments, Structural Member

and the following options:

Standard FSAE

Type Round Tubes

and

Size 25.4mm Dia

Select all the lines and arcs as shown and click .

Rename the structural member feature to Structural

Member_Bulkhead1

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Corner Treatments

The

Corner Treatments End Miter , End Butt1

End Butt2

are used to determine the trimming of the members meeting at a corner within the same feature.

All

Corner treatments are applied to all corners in the

Structural Member dialog and individually.

Individual corner treatments can be set by clicking the circular corner markers and setting the dialog that appears.

Rollback.

Drag the rollback bar to a position after the

Bulkhead2_sketch

Note: The

Weldment

feature is added to the part automatically.

This defines the part as a weldment part.

SolidWorks SAE Design and Analysis Project 75

Lesson 3: Creating a Weldment

Structural member.

Click

Insert, Weldments, Structural Member

and the following options:

Standard FSAE

Type Square Tubes

and

Size 25mm Sides

Make sure

Apply corner treatment

and

End Miter

are clicked. In this example, all corner treatments will remain as end miters.

Select all the lines of the sketch as shown and click .

Using Groups

The

Group

option allows you to select multiple “groups” of edges in the same dialog. The structural members of each group are automatically trimmed against each other; for example the members of Group1 are trimmed by the members of Group2.

Group1

Group2

Note: The use of groups may limit the selection of corner treatments.

SolidWorks SAE Design and Analysis Project

Rollback.

Drag the rollback bar to a position after the Main-> sketch.

Lesson 3: Creating a Weldment

Structural member.

Click

Insert, Weldments, Structural Member

and the following options:

Standard FSAE

Type Square Tubes

and

Size 25mm Sides

These selections are added to Group1.

Group.

Click

New Group

and select the three remaining edges for Group2. Click

SolidWorks SAE Design and Analysis Project 77

Lesson 3: Creating a Weldment

Using Trim/Extend

The

Trim/Extend

tool is used to trim the end of a structural member against a face/ plane or one or more other structural members.

It is helpful to keep the related trim/extend features together with the in the

FeatureManager design tree. In order to do this, it is best to rollback first similar to adding

structural members. See "Using Folders" on page 79 for more information.

Move the rollback bar to a position after the Structural Member feature that you want to trim.

Add one trim/extend feature for each end of the structural member. In the simplest cases, the trim/extend feature may include both ends of the structural member.

Trimming Boundary

The trimming boundary can be either a

Face/Plane

or other

Bodies

. Options with other bodies include

Simple cut between bodies

and

Coped cut between bodies

Bodies

Simple cut between bodies

Bodies

Coped cut between bodies

Face / Plane

Tip:

The Trim/Extend tool eliminates interferences between solid bodies by shaping the ends and creating the correct fit. Interferences between solid bodies in the multibody part can be

checked at the assembly level. For more information, see "Checking Clearances" on page

88.

78 SolidWorks SAE Design and Analysis Project

Trim.

Drag the rollback bar to a position after the Structural

Member_Bulkhead1

feature.

Click

Trim/Extend

and click

End Trim

Select the

Bodies to be Trimmed

and

Trimming Boundary

Bodies

as shown.

Click

Simple cut between bodies

and .

Lesson 3: Creating a Weldment

Bodies to be Trimmed

Trimming

Boundary

The

Bodies to be Trimmed

is shortened using the

Trimming Boundary

body.

Using Folders

Rollback was used in the previous steps to place the trim/extend feature just after the structural member being trimmed. This allows us to group a series of related features into a

Folder

, effectively reducing the length of the FeatureManager design tree.

Note: Features can also be dragged and dropped into the folder but they must remain

in the same sequential order.

Add folder.

Shift+select

the sequence of features as shown. Right-click and select

Add to New

Folder

, naming the folder Bulkhead_1 Folder.

SolidWorks SAE Design and Analysis Project 79

Lesson 3: Creating a Weldment

If this procedure is used throughout the FeatureManager design tree it will significantly shorten the length of the tree.

Map for Structural Member Types and Trim/Extend

The structural member types are either

FSAE, Round Tubes, 25.4mm

Dia

or . Create them and add the trimming and folders using the map below or the included eDrawings files (below). Use

End Trim Trimming Boundary Bodies

for all features.

80 eDrawings File for Member Types and

Trim/Extend

Double-click the eDrawings file

Frame.eprt

or the html file

Frame.html

. This will open an eDrawing or browser that can be zoomed, scrolled and rotated using the same tools as in SolidWorks.

Use the eDrawing to visually determine the type of structural member used for each sketch and how it is to be trimmed.

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Mirroring Structural Members

Mirror

can be used to pattern features, faces or bodies across a plane. In this example solid bodies will be mirrored to complete the frame.

Mirror bodies.

Click

Insert, Pattern/Mirror, Mirror

and click the Top plane as the

Mirror Face/Plane

. Click

Bodies to Mirror

and select the bodies shown in blue. Click .

Note: Mirroring the bodies after trimming eliminates the need to trim the mirrored

bodies.

SolidWorks SAE Design and Analysis Project 81

Lesson 3: Creating a Weldment

Editing

A big advantage of creating geometry in SolidWorks is the editing capability. You can edit sketches and features to change the design at any time. In this section, several types of changes will be introduced.

Editing the Corner Treatment

The corner treatments used on some of the earlier structural members may seem inadequate after all the bracing is added. In this case, an open end makes the connection with the brace difficult.

Zoom in.

Zoom in on the area as shown. This area shows a potential problem where the brace member connects to an open face of a square tube.

Edit structural member feature.

It is not necessary to know the name of the feature. Right-click on a face of any structural member of the feature and select

Edit Feature

82 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Corner treatment.

Click the corner marker as shown. In the

Corner Treatment

dialog, set the

Trim Order

and click . Repeat the process for the other corner and click in the main dialog. This changes the selections to mitered corners.

Note: The potential changes that can be made are limited by how the feature was

created. This feature was created using groups so miters are the only other choice.

Editing the Trimming

With the changes to mitered corners, the trimming can now be changed. In this case a planar face will be used instead of a body.

Edit trim feature.

Right-click the face of the structural member shown and select

Edit Feature

Trimming Boundary

, click

Face / Plane

and select the face as shown. Click .

SolidWorks SAE Design and Analysis Project 83

Lesson 3: Creating a Weldment

Editing the Type of Structural Member

The standard type or size of the structural member can be changed. In this example, structural members that will have plates attached will be changed to square profiles.

Edit feature.

Right-click the face of the structural member shown and select

Edit Feature

Click

FSAE

Type Square Tubes

and

Size 25mm Sides

. Click .

Using Locate Profile

In creating all of the structural members so far, the profiles have been placed directly at the default center position.

Consider a case where structural members of the same type and size are stacked on top of one another. Is it necessary to sketch a centerline offset by the exact amount?

Locate Profile

allows you to place the profile within the

sketch using the points built into the profile. For more information see "Why Do Some

Profiles Contain Points?" on page 73.

Find the parents.

Right-click a face of the structural member as shown and select

Parent/Child

. The

Parents

and

Children

of the feature are listed. Click

Close

Show sketch.

Right-click the Lower_Frame_sketch in the dialog and select

Show

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

New sketch.

Right-click the top face of the structural member and select

Sketch

Convert.

Click

Convert Entities

and select the centerline of the visible sketch.

Drag the endpoints outside the structural members and exit the sketch.

Add relations to span the full width as shown.

Close the sketch.

Locate profile.

Click

Insert, Weldments, Structural Member

and the following options:

FSAE

Type

Square Tubes

and

Size 25mm Sides

. Select the line and click

Locate Profile

. Click the point at the lower center position on the profile and click .

SolidWorks SAE Design and Analysis Project 85

Lesson 3: Creating a Weldment

Measure.

Click

Tools, Measure

and select the two faces shown.

Repeat the measurement on the opposite side to ensure that the structural member is centered.

Save.

Save the part and close it. Return to the assembly and click

Yes

to rebuild the assembly.

86 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Using Instant 3D

Instant 3D can be used to make dynamic changes to a model by dragging or directly changing dimensions.

Single-click a dimension to change the value.

Drag the dimension handle near the ruler to lock onto whole number ruler values.

Where to Find It



CommandManager:

Assembly > Instant 3D

Change dimensions.

Click

Instant 3D

and double-click the feature shown. Right-click the Frame part and select

Edit Part

. Double-click the feature and drag the handles on the dimensions to resize them to the values

80mm

and

300mm

as shown.

SolidWorks SAE Design and Analysis Project 87

Lesson 3: Creating a Weldment

Double-click the feature and change the dimensions to resize them to

350mm

and

530mm

as shown.

Checking Clearances

What is the minimum clearance between the Sprocket and Frame? This question can be answered using

Clearance Verification

tool.

Edit the Assembly.

Click confirmation corner to edit the assembly.

Clearance.

Click

Tools, Clearance Verification

Click

Selected Items

and select the Sprocket and Frame.

Type

0mm

Minimum Acceptable Clearance

and click

Calculate

. The clearance is close to

18mm

. Click .

Note: A visual check shows that there is no interference between the Sprocket and

Frame

components, but they can be checked. For more information, see

"Interference Detection" on page 90.

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Fully Defining a Component

The ENGINE component remains under defined, still able to rotate freely. It should be fully defined to prevent inadvertent movement.

Open the ENGINE.

Right-click the ENGINE component and select

Open Part

Add new plane.

Click

View, Temporary Axes

. Add a

Parallel

plane between the selected face and the temporary axis through the hole as shown.

Filtering the FeatureManager Design Tree

The FeatureManager design tree filter can be used to filter by name. Typing a name into the filter will result in a list of only the features, sketches, components or mates that use those characters.

Filter.

Return to the assembly. Click in the filter at the top of the

FeatureManager design tree and type engine.

Right-click Engine1_sketch and select

Show

Click “

” to stop the filter.

SolidWorks SAE Design and Analysis Project 89

Lesson 3: Creating a Weldment

Mate.

Add a

Coincident

mate between the plane and the line in the sketch.

Interference Detection

is useful in finding interferences or clashes, between static component parts in the assembly. The results show the interfering volumes in red.

Tip:

To check interferences between solid bodies in the same multibody part, select the multibody part only and click Include multibody part interferences.

90 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Interferences.

Click

Tools

Interference Detection

By default, the entire assembly is selected for interference detection, so right-click in the

Selected Components

field and select

Clear Selections

Select the ENGINE and Frame components and click

Calculate

A total of four interferences are found combined into two symmetrical sets. Click .

Edit sketch.

Click in the filter at the top of the FeatureManager design tree and as before type engine

. Right-click the under defined (-) Engine_Mount and select

Edit Sketch

. Click “

” to stop the filter.

Tip:

This is a shortcut that puts you in Edit Part and Edit Sketch mode directly.

Drag.

Drag the open endpoint short of the ENGINE component.

SolidWorks SAE Design and Analysis Project 91

Lesson 3: Creating a Weldment

Dimension.

Add a dimension between the edge of the ENGINE and the endpoint as shown.

Edit assembly.

Click

Edit Component

to exit the sketch and return to edit assembly mode.

Note: The sketch name has changed to Engine_Mount-> denoting that it is fully

defined and contains external references.

Mounting Plates

The Frame is currently placed with reference to the suspension points, but it is not attached. To create an actual attachment, mounting tab plates are required.

Creating a Reusable Sketch

The mounting tabs used to attach the suspension to the Frame are plates that are rounded on one end. Although all the tabs have a similar shape, the length and ends may vary. For this reason, creating a sketch that can be easily copied and modified is a good solution.

New part.

Open a new part with units mm. Create a new sketch on the Front plane.

92 SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Geometry and dimensions.

Create the geometry and dimensions using these guidelines:

Create a centerline from the origin on a slight angle.

Offset the centerline with the bi-directional option (add dimensions off) to create the sides.

Add a tangent arc to close the upper end.

Add a line between endpoints to close the lower end.

Add a circle.

Add dimensions.

Note: The centerline is on a slight angle (not horizontal or vertical) and under defined

to make the placement flexible.

Drag.

Drag the lower corner endpoint. The under defined sketch should rotate but maintain the shape.

Save.

Save the part as TAB_Sketch.

Exit the sketch but do not close the part.

SolidWorks SAE Design and Analysis Project 93

Lesson 3: Creating a Weldment

Copy sketch.

Select the Sketch1 feature in the FeatureManager design tree and

Edit, Copy

Pasting the Sketch

After editing the Frame part, the sketch will be pasted onto the face of a structural member.

Tip:

A common mistake in this situation is to paste the sketch before editing the part. The sketch can be pasted, but is only useful as an assembly feature. An assembly feature is a feature that exists only at the assembly level and can only be used to create a cut.

Edit part.

Return to the assembly, right-click the Frame part and select

Edit Part

Paste.

Select the face of the structural member as indicated. Click

Edit, Paste

94 SolidWorks SAE Design and Analysis Project

Edit sketch.

Right-click an edge of the sketch and select

Edit Sketch

Lesson 3: Creating a Weldment

Temporary axes.

Show the temporary axes by clicking

View, Temporary Axes

. Select the centerline and the temporary axis and add a

Parallel

relation.

SolidWorks SAE Design and Analysis Project 95

Lesson 3: Creating a Weldment

Concentric.

Select the circular edge and the circle and add a

Concentric

relation.

Extrude.

Extrude the sketch

3mm

as shown.

Note: This part has been marked as a weldment

option in extrude remains cleared.

, so the

Merge Result

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Repeat procedure.

Select the bottom face and create a new sketch. Convert edges from the previous body to create the sketch and extrude the sketch

3mm

as in the previous step.

Repeat for the remaining tabs on the same side and mirror.

Paste sketch.

Show Engine1_sketch. Select the face, click

Edit, Paste

and edit the sketch. Add a

Concentric

relation between the arc and circular edge as shown.

SolidWorks SAE Design and Analysis Project 97

Lesson 3: Creating a Weldment

Point.

Add a point on the centerline. Add a

Coincident

relation between the centerline and the point. Use the point to add a

Pierce

relation between the point and the inactive sketch line.

Trim and extrude.

Create the front edge of the structural member using

Convert Entity

. Trim the geometry leaving the centerline and point intact as shown.

Extrude the sketch

3mm

Plane.

Click

Insert, Reference Geometry, Plane

, select the faces and click

Mid Plane

. Rename the plane Centered.

Mirror.

Mirror the body using the in-context plane.

SolidWorks SAE Design and Analysis Project

Lesson 3: Creating a Weldment

Weldment Cut Lists

The Cut list folder list of all structural members in the weldment.

Note: In a non-weldment multi-body part the folder is named Solid Bodies.

Updating the folder.

Open the part Frame.

Right-click the Cut list folder and select

Update

to group similar structural members in folders.

SolidWorks SAE Design and Analysis Project 99

Lesson 3: Creating a Weldment

Cut List Properties

The

Cut-List Properties

can be used to view detailed information about the individual structural members including lengths and angles. Right-click a

Cut-List-Item

folder and select

Properties

For example, Cut-List-Item11 the following property values and are listed:

LENGTH

= 184.21

ANGLE1

= 45.00

A drawing of the structural member would look like this:

Save as External File

The virtual part can be saved externally, creating a part file outside of the assembly file.

Note: You cannot create a drawing of the virtual part until it is

saved to an external file.

Edit the Assembly.

Return to the assembly.

Click confirmation corner to edit the assembly.

Save external.

Right-click the virtual part and select

Save Part (in External File)

. Click

Same As

Assembly

and

Note: The name changes slightly. The braces surrounding the name ([,]) are

removed.

Save and close all files.

100 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

When you complete this lesson, you will be able to:



Understand the loft feature.



Describe the bodies created using the mold tools.



Use surfaces to add to the mold tools.



Use symmetry to create additional molds.

SolidWorks SAE Design and Analysis Project 101

Lesson 4: Using Molds and Surfaces

Molds and Surfaces

The Mold Tools commands can be used to create the mold tooling for a part. The mold tooling is created using a set of surface and solid bodies in the same part. Like the weldment, it is a multibody part.

Open assembly.

Open the assembly Intake Assembly from the Mold folder.

plenum restrictor runner intake connection boot

Open assembly.

Open the assembly Frame&Suspension from the

Lesson 3\Frame&Suspension

folder. This is the assembly used in the previous lesson.

Add the Intake Assembly assembly to the main assembly. Mate the sub-assembly using one concentric and two coincident mates.

102 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Open runner.

Right-click one of the instances of the part runner and select

Open Part

The

runner

part

The actual runner part is created in two pieces, a right and a left, that are later assembled into one. Each piece requires a mold.

Features in the Part

The model of the runner part is created using three main boss features: the Bell, the

Straight Boot Section

and the Center Guide Curve.

SolidWorks SAE Design and Analysis Project 103

Lesson 4: Using Molds and Surfaces

The revolve feature named Bell is used to connect the runner components to the plenum.

The extrude feature named Straight Boot Section is used to connect the runner components to the intake connection boot components.

This feature must fit inside the intake connection boot.

The loft feature named Center Guide Curve smoothly connects the revolve and extrude features.

For more information about loft features, see "Anatomy of a Loft" on page 105.

104 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Anatomy of a Loft

The loft feature is used to transition between different profile shapes. In this example, the starting profile is a slot shape that transitions to a circular shape.

Profiles

Profiles represent the starting, ending and optionally intermediate shapes along the loft.

They are closed contour sketches or curves.

Guides

A centerline is a guide used to orient the profiles in transition. A guide curve is used to shape the loft. Guide curves are open contour sketches or curves.

Loft with Guide Loft without Guide

SolidWorks SAE Design and Analysis Project 105

Lesson 4: Using Molds and Surfaces

Creating Mold Tooling

SolidWorks contains a series of mold tools that can be used to analyze and create mold tooling starting with the molded part.

If carbon fiber is used, the cavity solid body is the desired mold. When the carbon fiber is created, the thickness will be applied to the inside maintaining the outside dimensions that fit into the intake connection boot components.

This example assumes carbon fiber is used.

Surface and Solid Bodies

The mold tool procedure creates multiple bodies, including sets of both surfaces and solids, in a single part file. For more information see

"Surface and Solid Bodies" on page 106.

Surface Bodies

Solid Bodies

Note: A multibody part, like a weldment, is created.

106 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Description of the Bodies

Each of the resulting solid and surface bodies are created for a specific purpose. They are described below.

Molded Part Parting Surface

Cavity Solid Cavity Surface

Core Solid Core Surface

SolidWorks SAE Design and Analysis Project 107

Lesson 4: Using Molds and Surfaces

Mold Tools

The mold tools are designed for use with plastic injection molding, but they can be adapted for use with other manufacturing methods. The sequence shown here is typically used. The result is a multibody part with bodies representing the molded part, the core, and the cavity.

Scale

Scales the molded part to account for shrinkage in some materials. Not used

in this example.

Analysis Tools

Split Line

Parting Lines

Shut-off Surfaces

Parting Surfaces

Surfaces

Tooling Split

Draft Analysis Undercut

Analysis

are used to see if the part can be removed from the mold.

Parting Line Analysis

is used to visualize potential parting lines.

Breaks up model faces by adding edges.

Uses model geometry to define the parting line edges that define the parting surface.

Adds surfaces to close holes in some molded parts. Not used in this

example.

Surfaces created from the parting lines to separate the mold cavity from the core.

Many surfaces types can be used to supplement or replace the parting surface depending on the complexity of the model.

Creates both the core and cavity solid bodies by splitting a solid.

Note: The options scale and shut-off surfaces are not used in this example.

Tip:

Most of these tools are on the Mold Tools tab of the CommandManager. Right-click an existing tab and select Mold Tools to display the tab.

108 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Configuration.

Create a new configuration, Mold, to hold all the mold features.

Make sure that

Suppress features

under

Advanced Options

is checked. The new features will be suppressed in the Default configuration.

Add the Mold Tools Tab.

Right-click an existing tab on the CommandManager and click

Mold Tools

. The Mold Tools tab is now displayed on the

CommandManager.

Draft analysis.

Click

Draft Analysis

from the Mold Tools tab in the

CommandManager and select the Right plane. Set the

Draft

Angle

1deg

and click .

SolidWorks SAE Design and Analysis Project 109

Lesson 4: Using Molds and Surfaces

What Does This Mean?

This means that the angle between the Right plane and the yellow faces is

1deg

or less. It is in fact

0deg

because they are perpendicular.

Note: This small undrafted area is not a problem using carbon fiber,

but it would cause problems for other materials.

Display off.

Click

Draft Analysis

Undercut Analysis.

Click

Undercut Analysis

and select the Right plane. Click

. This confirms that the mold should be created in two pieces.

Split line.

Click

Split Line

and click

Intersection

. Select Right plane and the faces that intersect that plane. Click .

110 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Parting line.

Click

Parting Lines

Right

plane and set the

Draft Angle

1deg

Click

Draft Analysis

Edge selections.

Select the starting edge as shown.

Click

Select Next Edge

(or type “n”) and then

Add

Selected Edge

(or type “y”).

Continue the selections using the selection tools.

SolidWorks SAE Design and Analysis Project 111

Lesson 4: Using Molds and Surfaces

Continue selecting edges to complete the loop of selections as shown. Click .

Parting surface.

Click

Parting Surfaces

and select

Perpendicular to pull

. Set the

Distance

30mm

and click

Knit all surfaces

. Click

Sharp

and click .

112

Note: The parting surface is not always large enough to be able to

split the mold.

SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Using Surfaces

Surfaces often must be used to fill in or complete the surface geometry started by parting and shut-off surfaces. Here is a partial list of surface tools found on the

Surfaces

tab of the CommandManager.



Extruded Revolved



Swept Lofted



Planar



Ruled



Knit



Filled



Extend Trim



Offset

Extend edges.

Click

Extend Surface

and select three edges as shown. Click

Distance

, set the value to

30mm

and click .

Repeat the process for five edges on the opposite end.

SolidWorks SAE Design and Analysis Project 113

Lesson 4: Using Molds and Surfaces

Planes.

Create planes offset

170mm

from the Front and

60mm

from the Top as shown.

Trim.

Click

Trim Surface

and select

Standard

. Select the Plane3,

Keep selections

and select inside the plane. Click . Repeat the process for the opposite end.

114 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Sketches.

Click the parting surface and select

Sketch

. Using converted entities and lines, create the two sketches as shown. Exit both sketches.

Planar surfaces.

Click

Planar Surface

and select a sketch. Press

Enter

to repeat the command and repeat the procedure for the other planar surface.

SolidWorks SAE Design and Analysis Project 115

Lesson 4: Using Molds and Surfaces

Knit surface.

Click

Knit Surface

and select the three surfaces. Click

Merge entities

and click .

Drag and drop.

Drag and drop the Surface-Knit1 body into the Parting Surface Bodies folder as shown.

Note: The surface must be moved because it was created manually using extend,

planar and knit surfaces.

116 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Tooling split sketch.

Click

Mold Tools > Tooling Split

and select the knitted surface as the sketch plane.

Create the sketch and dimensions as shown.

Tooling split sizing.

Exit the sketch. Set the

Depth In Direction1

and

Depth In

Direction2

50mm

as shown. Click .

SolidWorks SAE Design and Analysis Project 117

Lesson 4: Using Molds and Surfaces

Test measurements.

Right-click the first (Parting Line1) solid body in the Solid Bodies folder and select

Isolate

. Click

Tools, Measure

and measure the distance between endpoints as shown. The key dimension is

Dist 56.45mm

as shown.

Exit isolate.

Click

Exit Isolate

on the

Isolate

dialog.

Isolate cavity solid.

Right-click the third solid body in the Solid Bodies folder and select

Isolate

. The key dimension is the again

Dist 56.45mm

as shown.

118

This shows that the outside faces are used to create the mold. Click

Exit Isolate

SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

Making Use of Symmetry

Individual bodies can be saved into new part files. This creates an external reference from that single body to the part file.

The other half of the mold is symmetric to the current one. It can be created using a mirrored part. The mirrored part is derived from the original part but mirrored using a plane or planar face. runner -> mirrored part

runner-> runner-Cav_1-> runner-Cav_2-

Note: If the other mold is not symmetrical to the first, a similar procedure can be

followed using slightly different selections in the Parting Line feature.

Stock feature.

Right-click the cavity solid body in the Solid Bodies folder of the FeatureManager design tree and click

Insert into New Part

. Use the name runner-Cav_1. A stock feature Stock-runner-1 is created.

SolidWorks SAE Design and Analysis Project 119

Lesson 4: Using Molds and Surfaces

Mirror part.

Select the back face of runner-Cav_1 as illustrated. Click

Insert

Mirror Part...

Click . Save the part as runner-Cav_2.

Holes.

Return to the runner-Cav_1 part. Select the outer face and click

Insert, Features, Hole, Wizard

10mm

through all holes placed as shown and select the two mold bodies with the

Feature Scope

. Click .

120 SolidWorks SAE Design and Analysis Project

Lesson 4: Using Molds and Surfaces

New assembly.

Create a new assembly and add the runner-Cav_1 and runner-Cav_2 parts.

The holes have been transferred to these parts using the external references.

Save and close all files.

SolidWorks SAE Design and Analysis Project 121

Lesson 4: Using Molds and Surfaces

122 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

When you complete this lesson, you will be able to:



Set up and run a thermal analysis.



Post process thermal results.



Set up and run a static analysis.



Apply thermal loading to structural analysis.



Post process static analysis.

SolidWorks SAE Design and Analysis Project 123

Lesson 5: Brake Rotor Analysis

Brake Rotor Design

When a vehicle is in motion, it is said to have kinetic energy. Brakes are designed to stop the vehicle by absorbing the kinetic energy of the vehicle and dissipating it in the form of heat.

The kinetic energy of a vehicle is given by the following equation:

2 where m is the mass of the vehicle and v is the velocity of the vehicle. If the mass of the vehicle is large, or the velocity is large, this can amount to a large amount of energy dissipated in the form of heat. The braking mechanism must be able to withstand both the temperatures generated by this heating as well as the forces incurred during breaking.

In this lesson, we will investigate the design of the braking rotor. The vehicle will be moving at full speed and will be braked to a complete stop. First, a thermal analysis will be run to calculate the temperature distribution in the brake rotor during braking. Next, a static analysis will be run to see the affect of the thermal load as well as the forces that come with the brake pads.

Open Brake Rotor Assembly.

Click

File, Open

and select the assembly Brake Rotor Assembly. Click

Open

to open the assembly.

Activate the configuration called Split Line. It contains the model with necessary changes so that we can run the analysis properly.

Start SolidWorks Simulation.

Click

Tools

Add-Ins

. Select

SolidWorks Simulation

Click

124 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

SolidWorks Simulation Interface

SolidWorks Simulation functions are accessed in the same way as SolidWorks. When a simulation study is created, a Simulation Study tree appears beneath the FeatureManager design tree. Each new study that gets created is represented by a tab at the bottom of the screen. Like SolidWorks functions, Simulation functions can be accessed from the

Simulation toolbar, CommandManager, or

Simulation

drop-down menu. Additionally, functions can be selected by right-clicking geometry or items in the Simulation Study tree.

CommandManager tab

Toolbar

Simulation

Advisor

Simulation

Study tree

Simulation Study tabs

SolidWorks SAE Design and Analysis Project 125

Lesson 5: Brake Rotor Analysis

Create a study.

From the

Simulation

drop-down menu, select

Study

Select

Thermal

as the

Type

Enter Temperature Distribution as the

Name

Click .

The FeatureManager design tree will split and a Simulation study tree will be created below the FeatureManager design tree.

The setup of the study is done using the Simulation study tree.

Adjust study properties.

Right-click the study name at the top of the Simulation study tree and select

Properties.

Under

Options

, select

Transient

and enter

3 sec

as the

Total time

Click

126 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

Transient Thermal Analysis

This model is run as a transient analysis because we want to study the heat distribution during braking from a speed of 22 m/s to a complete stop. We can easily calculate the time it takes to stop by first calculating the force it takes to stop the vehicle. We know that the vehicle is 275 kg and we assume the coefficient of friction between asphalt and rubber is

0.72. To stop the vehicle in the shortest time, the maximum braking force cannot be larger than the maximum friction force between the tires and the ground, which can be transmitted to the ground. This maximum friction force is calculated as follows.

F f

= =

(

0.72

(



----



= 1942.4N

Now that we know the friction force, we can calculate the average acceleration of the car during braking.

a x

F f

1942.4N

275kg

= 7.06

Finally, we can calculate the time it takes to stop.

v x

= 3s

7.06

Apply material.

Right-click the Parts folder and select

Apply Material to All

Select Gray Cast Iron under Iron as the material. Click

Apply

, then

Close

SolidWorks SAE Design and Analysis Project 127

Lesson 5: Brake Rotor Analysis

Thermal Boundary Conditions

SolidWorks Simulation solves for the temperature distribution in the solid using the conduction equations and boundary conditions applied to the boundaries of the model.

SolidWorks Simulation has several thermal boundary conditions that can be applied to thermal studies.



Temperature

Allows for the definition of a temperature on a certain entity or body.



Convection

Applies a convection boundary condition to the selected faces. The convection coefficient and ambient temperature are specified and the heat lost due to convection is calculated automatically.



Heat Flux

Applies some amount of heat into a face per unit area.



Heat Power

Applies some amount of heat to a vertex, edge, face or component.



Radiation

Allows surface-to-surface or surface-to-ambient radiation.

In our model, we will apply convection to all faces because all of the faces will be exposed to the air. In addition, we will apply a heat power to the faces that the brake pads touch.

Convection

Convection is the transfer of thermal energy between a surface and a fluid. The amount of heat transferred through conduction is proportional to the convection coefficient, h, the surface area, A, and the temperature difference between the surface and the surrounding fluid.

Q convection

–

T f

)

In this lesson, we will assume a convection coefficient of 90 W/m^2.K and an ambient temperature of 20°C, which are approximations. Actual convection coefficients and ambient temperature could be computed by running a CFD analysis in SolidWorks Flow

Simulation or from experiments.

128 SolidWorks SAE Design and Analysis Project

Apply thermal load.

Right-click Thermal Loads in the Simulation Study tree and select

Convection.

Select

Select all exposed faces

in the Convection

PropertyManager. This will choose all of the exposed faces for the convection boundary condition.

Enter

90 W/m^2.K

as the

Convection Coefficient

Enter

293 Kelvin

as the

Bulk Ambient Temperature

Lesson 5: Brake Rotor Analysis

SolidWorks SAE Design and Analysis Project 129

Lesson 5: Brake Rotor Analysis

Edit Time Curve.

Click

Use Time Curve

and select

Edit

Column

denotes the time and column

denotes the multiplication factor that will be applied to the convection coefficient that was entered.

Enter

(0, 1)

and

(3, 1)

in the table. This will represent the convection always being turned ON.

Click

Click .

Note: Similar to the time dependence of the loading using time curves, any thermal

load can be made temperature dependent using temperature curves. Solutions with temperature curves are significantly more time consuming as convergence iterations are required because each finite element can generate a different level of heat power based on its average temperature.

Heat Power

As the vehicle is braked, the rotor is spinning and the brake pads are rubbing against the surface of the rotor, creating friction and heat energy. Much of the kinetic energy of the car is being transferred to thermal energy through the brake pads. The heat power will be applied to the brake rotors in the area that the pads touch.

The amount of heat power can be calculated from the amount of kinetic energy carried by the car. If we assume the mass of the car is 275 kg and the car is travelling at 25 m/s, the kinetic energy of the car is as follows:

) 22





= 66.55kJ

130 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

If we assume all of that kinetic energy is transferred to thermal energy during braking that lasts 3 seconds, we can calculate the heat power.

HeatPower

Δt

66.55kJ

= 22.18kW

Since we will analyze only one pad, and about 60% of the mass of the vehicle will be on the front, the heat power is reduced.

HeatPower

42.95kW 0.60

)

= 6.66kW

Apply thermal load.

Right-click Thermal Loads in the Simulation Study tree and select

Heat Power.

Select the four faces of the rotor that the brake pads touch.

Enter

6660 W

as the

Heat Power

Select

Total.

SolidWorks SAE Design and Analysis Project 131

Lesson 5: Brake Rotor Analysis

Edit Time Curve.

Click

Use Time Curve

and select

Edit

Column

denotes the time and column

denotes the multiplication factor that will be applied to the heat power that was entered.

Enter

(0, 1)

and

(3, 1)

in the table. This will represent the heat power always being turned ON.

Click

Click .

Initial temperature.

Right-click Thermal Loads in the Simulation Study tree and select

Temperature.

Select

Initial temperature

Select the assembly from the fly-out FeatureManager design tree.

Enter

25 C

as the

Temperature

Click .

Mesh the model.

Right-click Mesh in the Simulation Study tree and select

Create Mesh

. Use

Curvature based mesh

and default element size.

Click .

132

Run the study.

Click

Run

from the Simulation drop-down menu.

Note: The study should take several minutes to run. A calculation is performed at

each time step as specified in the study properties. Results will be available for each time step performed.

Tip:

Be careful when specifying the time step magnitude so that accurate resolution of your loading curve is obtained.

SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

Post Processing

We will now look at the various post processing options associated with transient thermal analysis.

Plot Temperature distribution.

Right-click the Thermal1 plot of the temperature distribution and select

Edit Definition

Change the

Units

Celsius

Make sure the

Plot Step

is set as

Click .

Probe.

Right-click on the temperature plot in the Result folder and select

Probe

Select any location on the brake rotor.

Click the

Response

button under

Report Options

A plot of temperature vs. time will appear.

Click .

Note: You can do this with any of your created plots in a transient thermal analysis.

SolidWorks SAE Design and Analysis Project 133

Lesson 5: Brake Rotor Analysis

Plot Resultant Heat Flux.

Right-click Results in the Simulation Study tree and select

Define Thermal Plot

Select

HFLUXN: Resultant Heat Flux

as the

Component

Make sure the

Plot Step

is set as

Click .

Tip:

You can also select Plot Bounds across All Steps from the Plot Step menu. This will look through all solution time steps and plot the maximum or minimum values.

Note: You can also plot the temperature gradient. In addition, you

can plot the directional components of each thermal result quantity. You are encouraged to try these plots.

Static Study

We now know the temperature distribution after the vehicle brakes from 22 m/s to a complete stop. This temperature distribution will be transferred into our static study as a thermal loading condition and the material will be allowed to expand or contract as a result of the temperature distribution. In addition, we will apply a loading condition to simulate the load that the brake pad would apply to the rotor. We want to insure that the brake pad will not warp significantly during this extreme braking situation.

Create a study.

From the

Simulation

drop-down menu, select

Study

Select

Static

as the

Type

Enter Thermal Stress as the

Name

Click .

Apply material.

Right-click the Parts folder and select

Apply Material to All

Select Gray Cast Iron under Iron as the material. Click

Apply

, then

Close

Tip:

You can also copy the materials from the thermal study by selecting the

Parts

folder in the thermal study, then dragging and dropping it onto the static study. Other study parameters can be copied similarly.

134 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

Temperature Dependent Material Properties

Material properties are often temperature dependent. You can make your material properties temperature dependent in SolidWorks Simulation by creating a custom defined material and selecting

Temperature Dependent

under where you enter the parameter value.

Fixtures

The fixtures in your study will represent how the structure is attached to the real world. It is always best to pick the type of fixture that best represents the attachment to the real world. The following type of fixtures are available in SolidWorks Simulation:



Fixed Geometry

Fixes all degrees of freedom. Also known as a rigid support.



Roller/Slider

Specifies that a planar face can move freely in the plane, but is restrained normal to the plane.



Fixed hinge

Can be applied to a cylindrical face and only allows movement about the axis of the cylindrical face.



Advanced Fixtures

Allows for different types of restraints in various directions. Feel free to review the help menu to investigate these types.

Apply fixture.

Right-click Fixtures in the Simulation Study tree and select

Fixed Geometry

Select the face on the inner diameter of the rotor hub where it would be mounted to a shaft.

Click .

Note: We are applying a rigid restraint to the shaft mounting location. With this,

comes the assumption that the shaft will not deform under any applied loading transferred through this mounting location. For this example, we are assuming the shaft is much more rigid than the rotor hub. If we expect the shaft to deform, we would need to include it in the analysis.

SolidWorks SAE Design and Analysis Project 135

Lesson 5: Brake Rotor Analysis

Apply fixture.

Right-click Fixtures in the Simulation Study tree and select

Roller/Slider

Select the split face on one side of the rotor where the fixed brake pad will rub the rotor.

Click .

Discussion

Typically, the brake calipers are designed such that one pad applies a load to the rotor to push it into the other pad. With this restraint, we are simulating the stationary pad and assuming that the pad will not deform under the loading. We will now apply the loading.

Loading

Like the fixtures, the loading in your structure should best represent the in-service loading conditions. The following types of structural loading is available in SolidWorks

Simulation.



Force

Applies a force to an edge, face, or vertex in the direction defined by reference geometry.



Torque

Applies a torque about a reference axis.



Pressure

Applies a pressure to a face.



Gravity

Applies linear acceleration to parts or assemblies.



Centrifugal Force

Applies an angular velocity and acceleration.



Bearing Load

Defined between contacting cylindrical faces.

136 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

Apply load.

Right-click External Loads in the Simulation Study tree and select

Pressure

Select the split face where the brake pad will push against the rotor.

Enter

1e6 N/m^2

as the

Pressure Value

. This value can be known from experiments.

Click .

Braking Force

In addition to the load applied to the rotor through the brake pad, there is also a frictional component of the braking force in the circumferential direction. If we know the normal load applied to the bracket (1 MPa) and the friction coefficient between the rotor and pads

(0.6), the frictional force can be calculated using the area of the pad application.

F f

(

0.6

⋅



×10



= 497N

Note: The frictional coefficient between the pad and rotor can often vary depending

on the temperature. Using 0.6 as the friction coefficient is a simplification made in this example.

SolidWorks SAE Design and Analysis Project 137

Lesson 5: Brake Rotor Analysis

Apply load.

Right-click External Loads in the Simulation Study tree and select

Force

Select the two split faces on the rotor where the brake pads make contact.

Select

Selected Direction

Select Axis1 of the Rotor Hat part as the reference.

Select the

Circumferential

direction and enter

497 N

Click .

Note: When an axis is selected as a reference, the coordinate system changes to

cylindrical coordinates and our load can be applied circumferentially.

Thermal Loading

Now that the structural loadings have been applied, we need to apply the thermal loading.

We want to apply the maximum amount of thermal loading seen during the braking. This is obviously the temperature distribution at the end of the braking. The temperatures solved for in the thermal study will then be transferred to the static study and the material will be able to respond to the change in temperature. This will cause additional displacement and thermal stresses to develop in the structure.

138 SolidWorks SAE Design and Analysis Project

Lesson 5: Brake Rotor Analysis

Adjust study properties.

Right-click the study name at the top of the Simulation study tree and select

Properties.

Select the

Flow/Thermal Effects

tab.

Select

Temperatures from thermal study

and select

Temperature Distribution

Time step 30

as the Thermal study.

Enter

298 Kelvin

as the

Reference temperature at zero strain

Click

The Thermal load will appear in the External Loads folder.

Mesh the model.

Right-click Mesh in the Simulation Study tree and select

Create Mesh

. Use

Curvature based mesh

and default element size.

Click .

Run the study.

Click

Run

from the Simulation drop-down menu.

SolidWorks SAE Design and Analysis Project 139

Lesson 5: Brake Rotor Analysis

Post Processing

We will now learn about the various post processing options available for static studies.

Plot stress.

Activate the Stress1 plot by double-clicking it from the Results folder. It is a plot of the von Mises stress in the model.

Editing Plots

To edit a plot, right click on the plot and select

Edit Definition

The

Display

dialog lets you specify a stress component and units.

The

Advanced Options

lets you choose to plot either a

Node

Element

value. For the nodal values, the stresses are averaged and displayed at the nodes. For the elemental values, the stresses in a given element are averaged and the element is given this averaged stress and it is displayed.

The

Show as tensor plot

option allows you to plot the orientation as well as the magnitude of the stresses.

The

Deformed Shape

dialog allows you to show the deformed shape and to choose the scaling of the graphics window.

140 SolidWorks SAE Design and Analysis Project

Chart Options

The chart options can be accessed by rightclicking on the plot and selecting

Chart Options

or by double-clicking the legend. The chart options control the annotations as well as other options such as the color, type of units

(scientific, floating, etc), and number of decimals shown in the legend.

Settings

The plot settings can be accessed by rightclicking on the plot and selecting

Settings

They are used to control various display options.

Lesson 5: Brake Rotor Analysis

Display model maximum.

Right-click on the plot and select

Chart Options

Click

Show max annotation

Click .

SolidWorks SAE Design and Analysis Project 141

Lesson 5: Brake Rotor Analysis

Discussion

Notice that the maximum occurs in a sharp corner where the mesh is quite coarse. If stresses are of interest in this location, significant mesh refinement would be required. In addition, this may be an area of singular stress due to the boundary conditions and the sharp corner. If this was the case, this stress value could be ignored.

Plot displacement.

Double-click the Displacement1 plot to show the displacement plot.

Conclusions

In this lesson, we did an analysis of a brake rotor. We learned how to set up and run both a thermal and static study. We also learned about some of the post processing options available in SolidWorks Simulation.

In order to perform this analysis, some significant assumptions were made. First of all, the convection was assumed a constant 90 W/m^2.K throughout the analysis. This is a bit of an aggressive assumption due to the fact that as the car slows down, there will be less air flow over the rotor, therefore less heat lost due to convection. As mentioned before,

SolidWorks Flow Simulation could be used to more accurately calculate the convection around the rotor.

Another assumption made in this modeling is that the heat power is applied to the entire rotor surface rather than simply the location the pad touches. In actuality, the heat power is only generated where the pad touches, and as the car moves, this location rotates around the entire surface of the rotor. By applying it to the entire rotor surface, we “smear” the heat power evenly along the surface in what could be considered a conservative assumption. Can you think of a way to apply the heat power to better match the real model?

Additional assumptions were made in this model such as the friction coefficient, material properties, and structural boundary conditions. Therefore, this analysis should serve as a first-pass type of analysis where further testing or investigation could be done for more conclusive results.

142 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

When you complete this lesson, you will be able to:



Set up an analysis using beam elements.



Create truss elements.



Calculate the torsional rigidity of your frame.



Post process results in cylindrical coordinates.



Define beam shear and moment diagrams.



Evaluate your frame design.

SolidWorks SAE Design and Analysis Project 143

Lesson 6: Frame Analysis

Torsional Rigidity

The torsional rigidity is defined as the torsional response

(defined as some deflection angle) of a structure to an applied torque loading. The image to the right shows the deformation of a structure due to some applied torque loading. The torsional rigidity would be mathematically formulated as follows:

TorsionalRigidity

AngularDeflection

With respect to frame design, the torsional rigidity is an important characteristic of the vehicle for several reasons. As we will see, the general rule of thumb for torsional rigidity is “the stiffer, the better.”

Imagine strapping wheels to a mattress and trying to drive the mattress through twists and turns. A mattress car, as you can imagine, would not handle the lateral loading well and it would be very difficult to keep the wheels of the car on the ground. Torsional stiffness drastically affects the car’s handling.

The lateral loading on a vehicle is taken up in two places; the frame and the suspension.

Now, consider tuning the torsional stiffness of your car to drive on different road types.

The suspension can be adjusted, the frame cannot. Ideally then, your suspension will take up much of the lateral loading. Adjusting the stiffness of your suspension will determine how the car handles different types of loading. If the loading is taken by the frame, it will be very difficult to tune the torsional stiffness of your car.

In this lesson, we will use SolidWorks Simulation to evaluate the torsional rigidity of our frame design. Perhaps most importantly, we will also be able to evaluate how design changes affect the torsional rigidity (i.e. is this design stiffer or more flexible than the previous?).

Element Types

To this point, we have used SolidWorks Simulation to analyze the thermal and structural characteristics of our brake rotor using solid elements. Solid elements worked well in the analysis of the rotor because the structure was relatively thick and our computer had the necessary resources to mesh and run the analysis.

In this lesson, we will be analyzing the frame structure that we modeled in a previous lesson. We could use solid elements in this analysis, however we will see another element type that will allow us to greatly simplify our calculations.

144 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

Shell Elements

When the structure becomes thin in one direction, such as a sheet metal part, SolidWorks Simulation can use shell elements to significantly simplify the calculations. The shell element in

SolidWorks Simulation is a two dimensional triangular element.

Each node of the shell element features six degrees of freedom (3 translational, 3 rotational), giving the nodes the ability to transfer moments. The thickness of the geometry is taken into account automatically in the formulation of the element.

Shell elements can be created in SolidWorks Simulation the following ways:



Shell elements are automatically created in SolidWorks

Simulation when a sheet metal part is used.



If any surface geometry exists in your part, SolidWorks Simulation will automatically recognize them as shell elements as well.



To manually define shell elements, you can right-click the solid body from the Parts folder of the Simulation Study tree and select

Define Shell By Selected Faces

Beam Elements

The beam element is another type of structural element available in SolidWorks Simulation. It is a one dimensional element with

2 nodes. Like shells, each node of a beam element has six degrees of freedom. The cross-sectional characteristics of the beam are taken into account in the formulation of the element.

These characteristics are automatically computed in the software, therefore greatly simplifying the model setup.

Beam elements can be created in SolidWorks Simulation in the following ways:



Beam elements are automatically created in SolidWorks

Simulation when a weldment part is used.



Right-click the solid body in the Parts folder of the Simulation Study tree and select

Treat as

Beam

SolidWorks SAE Design and Analysis Project 145

Lesson 6: Frame Analysis

Preparing for Analysis

As previously discussed, the first step in the analysis process is to simplify the model.

Care must be taken when simplifying the model such that we do not remove something that could have a significant effect on our results.

Open Frame.

Click

File, Open

and select the part Frame. Click

Open

to open the part.

This is the Frame part that was created in the previous lesson. There are a couple of modifications to the model in order to make it a bit more convenient for meshing.

Tip:

The model used for finite element analysis is often simplified from its final production state.

Therefore, it is often beneficial to have multiple configurations of your models, one for analysis and one for production.

Add a configuration.

From the ConfigurationManager, right-click the part and select

Add Configuration

Type FEA as the

Configuration name

Click .

The new configuration will be created and activated in the ConfigurationManager. We can now suppress unwanted features in our part that are unnecessary for our analysis.

In addition, there may be features to unsuppress that are not part of the final model, but are necessary to the analysis.

Note: In this model, we are doing an analysis on a part. If we were analyzing an

assembly, it would be necessary to create the alternate configurations at the part level, then have these configurations active or inactive in the separate configuration at the assembly level.

Suppress features.

In the previous lesson, mounting locations were created for the suspension and the engine. In the analysis, these will not have any affect on the torsional stiffness of the vehicle.

Right-click on the Tabs folder and select

Suppress

Right-click on the EngineMount folder and select

Suppress

146 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

Experimental Design

It is important when preparing a finite element model to consider the physical representation of what you are trying to analyze. Loading and fixtures are going to be applied to the model based on the most accurate representation of the physical model.

These boundary conditions will introduce assumptions into the model and it is critical that the assumptions are understood and reasonable with respect to what the model is trying to accomplish.

There are a number of techniques for experimentally measuring torsional rigidity. In the simulation, we will try to most accurately represent the experiment in the analysis setup.

In the experiment, the front and rear wheels are mounted on beams and the suspension components are assumed to be fixed so that all of the load applied is transferred to the frame itself. The rear of the vehicle is held stationary (fixed) while a load is applied to the beam with the front wheels to simulate the torque as shown in the figure below.

Force Force

Note: Our analysis will be setup with respect to this method for measuring torsional

rigidity. Other methods exist and you would want to design your analysis according to the physical setup of the experiment in order to compare the results properly.

Unsuppress features.

In this model, the suspension has not been included in the analysis. We need a location to apply our torque loading as well as a place to measure the angular displacement for calculating the torsional rigidity. For this, beam members have been created to connect the frame to the location where the wheel is mounted.

Right-click on the Rigid_Supports folder and select

Unsuppress

We are now ready to begin the analysis. Make sure that the SolidWorks Simulation

Add-In is active from the

Tools, Add-Ins

menu.

SolidWorks SAE Design and Analysis Project 147

Lesson 6: Frame Analysis

Create a study.

From the

Simulation

drop-down menu, select

Study

Select

Static

as the

Type

Enter Torsional Rigidity as the

Name

Click .

Beam Meshing

As mentioned before, weldment features are automatically treated as beam elements in SolidWorks

Simulation. If solid elements are desired for the analysis, right-click the beam feature in the Simulation

Study tree and select,

Treat as Solid

Examine the Frame folder.

The Frame folder should contain sub-folders that list all the solid bodies that will be meshed as beams. You can tell that bodies the will be beams because of the beam icon next to the body name.

Any Solid Bodies that will be meshed as solids should be excluded from the analysis. To do this, right-click the solid body and select

Exclude from analysis

Section Properties

We mentioned that all of the cross-sectional characteristics of the beam are taken into account automatically by SolidWorks

Simulation. For custom beam profiles, the section properties that are not computed automatically are constants for the torsional shear and shear due to bending calculation. These constants must be entered manually if this information is required from the analysis.

To enter the constants, right-click the beam and select

Edit

Definition

. The required contacts for torsional shear calculations are as follows:



Torsional Constant, K

The value for the torsional constant can be calculated or obtained from literature.



Distance for Maximum Shear

Distance from the center of the section to the point of maximum torsional shear.



Shear Factor

in direction 1

Shear factor to account for non-uniform shear stress in direction 1 of the beam coordinate system.



Shear Factor

in direction 2

Shear factor to account for non-uniform shear stress in direction 2 of the beam coordinate system.

148 SolidWorks SAE Design and Analysis Project

End Conditions

At the end of each beam falls a node that will connect to either another beam joint or a boundary condition. As previously mentioned, the nodes of beams have six degrees of freedom

(three translational and three rotational). These degrees of freedom may be restrained or released to reflect various structural connection configurations. To manually configure these degrees of freedom, right-click the beam and select

Edit

Definition

. The graphics window will show the beam with two ends as shown in the figure.

Lesson 6: Frame Analysis

The following options are allowed for beam end conditions:



Rigid

All six degrees of freedom are tied to the joint. All translational forces and rotational moments will be transferred from the beam element to the joint and vice versa.



Hinge

Three translational degrees of freedom are tied to the joint. All translational forces will be transferred from the beam element to the joint and vice versa. Rotational moments will not be transferred.



Slide

Three rotational degrees of freedom are tied to the joint. All rotational moments will be transferred from the beam element to the joint and vice versa. Translational forces will not be transferred.



Manual

A custom defined connection can be defined.

SolidWorks SAE Design and Analysis Project 149

Lesson 6: Frame Analysis

Trusses

In the same location, the beam can be defined as a

Truss

which can only resist axial loading.

We want to apply the torsional loading to the location where the wheels would mount so that we can best represent the experiment. Weldment features were created that defined this location. We want the loading to be transferred directly to the joints of the frame where the suspension mounts, however, we do not want any moments to transfer, only forces. To only allow the transfer of forces, we will make these members trusses.

Define trusses.

Select one of the truss members in the graphics window. It should highlight the member in the

Frame

folder of the Simulation Study tree.

Right-click the member in the Simulation Study tree and select

Edit Definition

Select

Truss

as the

Type

Repeat this procedure for the seven remaining truss members that mount to the suspension mounting points.

Apply material.

Right-click the Frame folder and select

Apply Material to All Bodies

Select Alloy Steel as the material. Click

Apply

, then

Close

Joint Group

The beam mesh is made out of a series of one dimensional lines that may be connected. The end points of these lines are called joints. SolidWorks Simulation automatically detects the joint positions, however some joints can be very close and it could be desirable to merge them (or un-merge) them. In this case, the joint locations can be modified manually using the Joint Group. We will practice this in this lesson.

The beam joints are shown as yellow or magenta spheres in the graphics window.



joints are connected to two or more beam members.



joints are connected to a single member.

150 SolidWorks SAE Design and Analysis Project

Edit Joint Group.

When a beam is defined in SolidWorks Simulation a folder called Joint Group is created in the Simulation Study tree.

Right-click the Joint Group folder and select

Edit

Lesson 6: Frame Analysis

Examine joints.

Right-click a joint icon to examine the beams that are connected by the joint.

To add or remove a beam member from the list, click the beam in the graphics window.

To save the new joint, simply close the

Select Joint

Members

window.

SolidWorks SAE Design and Analysis Project 151

Lesson 6: Frame Analysis

Edit joint.

Examine the joints in the rear of the vehicle frame.

Notice that at one of the rear suspension mounting points, there may be two joints. This location should only have one joint that connects all of the beams.

Right-click one of the joints and add the omitted beams.

Right-click the other joint and remove all of the beams. This will delete that joint since it is redundant.

Click

Calculate

to recalculate the joints.

Note: This procedure may be repeated as necessary until the joints are calculated

properly. Additionally, this procedure may not be necessary if the joints are initially calculated correctly.

Tip:

Be sure to check your joints to insure that they have been computed accurately by the software. It can be helpful to thoroughly examine the mesh after meshing.

Merging Joints Automatically

The software automatically calculates joint locations based on the ends of beams. At the joint end, a hypothetical sphere is drawn with a diameter chosen automatically with respect to the model geometry. If two joints fall within one sphere, the beam ends will be merged forming one joint. It is possible to modify the diameter of this hypothetical sphere using

Treat as joint for clearance less than

. Re-calculating the joints is necessary to get them to merge.

152 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

Fixtures

SolidWorks Simulation has a number of different fixtures that can be applied to beam joints:



Fixed Geometry

Fixes all six degrees of freedom (translational and rotational).



Immovable (No translation)

Fixes translational degrees of freedom only. Rotational degrees of freedom are left unconstrained.



Use Reference Geometry

The user can specify a reference and choose which degrees of freedom are fixed (translational or rotational) with respect to that reference.

It was mentioned that in the experiment, the rear wheels are held stationary. To measure the torsional rigidity, the entirety of the load must be transferred directly to the frame.

Therefore any components attached to the frame that transfer the load must be assumed to be rigid. If this is the case, it would make sense to fix the rear joints where the rear suspension would attach.

Apply fixtures.

Right-click Fixtures in the Simulation Study tree and select

Fixed Geometry

Select the eight joints at the rear of the frame where the suspension would mount.

Click .

Note: You can tell which degrees of freedom are being

fixed by viewing the arrows. An arrow in a given direction means that the translation in that direction is restrained. If the arrow has a tail, the rotation about that direction is restrained as well.

Fixed Geometry

Immovable

SolidWorks SAE Design and Analysis Project 153

Lesson 6: Frame Analysis

Loading

SolidWorks Simulation allows for the application of forces and torques to beams or beam joints. The force is applied to the beam or joint and the direction is defined by choosing a reference.

As with our fixtures, we will assume that the loading from the experiment is transferred directly to the frame beam joints at the suspension mounting points.

With the wheel structure assumed rigid, the load would be applied to the front axle axis and the frame would rotate about the center of the frame on the front axle axis. This is the location where the angular displacement must be measured about.

Rotation Point

Force

To simplify the analysis, we have not included our suspension components, therefore we must define representative loading condition that will simulate our experiment. The application of our loading to our truss members will transfer the equivalent torque to the frame through the suspension mounting points.

Note: The truss members are used only in the finite element model to directly transfer

the loading. They are not part of the actual frame design.

154 SolidWorks SAE Design and Analysis Project

Apply loading.

Right-click External Loads in the Simulation Study tree, and select

Force

Select

Joints

under

Selection

Select the beam joint at the termination of the truss members.

Select the Front plane as the reference.

Select

Normal to Plane

and enter

169.7 N

Click .

Lesson 6: Frame Analysis

Repeat this procedure for the opposite side.

Make sure that the direction is reversed on the opposite side.

Note: The loading magnitude was calculated such that a 100 N-m torque is applied to

the frame.

Force

0.5892m

Mesh the model.

Right-click Mesh in the Simulation Study tree and select

Create Mesh

The beam mesh will automatically be created.

SolidWorks SAE Design and Analysis Project 155

Lesson 6: Frame Analysis

Note: Truss members are meshed as a single element because they will not have

bending deformation since their nodes only transfer axial forces.

Run the study.

Click

Run

from the Simulation drop-down menu.

Post Processing

After the study is run, the Results folder in the Simulation Study tree will become active and our results are accessible. In this lesson, we will investigate the different post processing options available for beams.

The first result that we would like to compute is the torsional rigidity. To do this, we must know the angular deformation of the frame as a result of the torsional loading.

Cylindrical Coordinates

By default, SolidWorks Simulation plots the results using a cartesian coordinate system. Knowing this, one could convert the results to another, more desirable coordinate system.

SolidWorks Simulation also allows for the plotting of results in cylindrical coordinate. We will use this method to measure the angular deformation of the frame required to calculate torsional rigidity.

To change to cylindrical coordinates, a reference axis must be selected in the

Advanced Options

. When in cylindrical coordinates, the following changes are made to the coordinates with respect to the selected reference axis:



X direction = Radial direction



Y direction = Circumferential direction



Z direction = Axial direction

In addition, the cylindrical coordinate system appears at the bottom right of the graphics window to inform you of your coordinate selection.

156 SolidWorks SAE Design and Analysis Project

7 Plot angular displacement.

Right-click the Results folder and select

Define Displacement

Plot

Select

UY: Y Displacement

as the

Component

Expand the

Advanced Options

and select Axis2 as the reference.

Select the

Automatic

scaling.

Click .

Lesson 6: Frame Analysis

Note: The unit system of this plot is still in mm where we might expect it to have an

angular unit since it is a circumferential displacement. In actuality, the software is taking the angular deformation about the axis and multiplying it by the distance away from the axis. To compute the actual angular deformation, we need to divide by its distance away from the axis.

SolidWorks SAE Design and Analysis Project 157

Lesson 6: Frame Analysis

Probe.

Right-click the Displacement plot in the Results folder and select

Probe

Select one of the ends of the trusses where the load is applied.

We now know the angular deformation of the end of the frame.

We must divide this by the distance away from the axis to measure the angle.

3.366mm

589.2mm

= 0.00571rad

Click .

Note: The angular deformation will always be calculated in radians, not degrees.

Torsional Rigidity

We can now calculate the torsional rigidity of the frame.

100Nm

0.00571rad

= 17513

rad

158 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

Beam Stresses

There are a number of different components of stress that develop in beams. Axial, torsional, shear, and bending stresses are all components of stress seen by beams. In

SolidWorks Simulation, you can plot any of these.

By default, SolidWorks Simulation creates a stress plot called

Upper bound axial and bending

which looks at each beam element and plots whichever component of stress is the highest in the plot. This type of plot is useful in evaluating the maximum stress seen in your beams.

Plot stress.

Activate the Stress1 plot that was created by default by SolidWorks Simulation.

This is a plot of the highest stress (axial or bending) in each beam element.

We can view these stress components separately.

Plot axial stress.

Right-click the Results folder and select

Define Stress Plot

Select

Axial

and

Automatic

Click .

Notice that some members are in tension and some members are in compression. You can use this information in design change decisions.

SolidWorks SAE Design and Analysis Project 159

Lesson 6: Frame Analysis

Cross Section Directions 1 and 2

To post process bending and shear stress, the beam directions 1 and 2 must be defined.

SolidWorks Simulation defines direction 1 to be along the longest side of the cross section and direction 2 is it’s perpendicular.

Plot bending stress.

Right-click the Results folder and select

Define Stress Plot

Select

Upper bound bending in DIR1

and

Automatic

Click .

Note: If you probe on one of the truss members, you will see that it has zero bending

stress. This makes sense because the trusses do not transfer moments.

Similarly, the user can plot

Torsional

Shear in DIR 1

and

Shear in DIR 2

stresses.

160 SolidWorks SAE Design and Analysis Project

Lesson 6: Frame Analysis

Shear and Bending Diagrams

SolidWorks Simulation also has the ability to plot shear and bending diagrams in the different beam directions. These can be used to study how the internal bending moments and shear forces vary along the length of the beam.

Plot bending moment.

Right-click the Results folder and select

Define Beam

Diagrams

Select

Moment in Dir1

Under

Selected Beams

, choose

Select

and select the beam member shown at the front of the frame.

Click .

List beam forces.

Right-click on the Results folder and select

List Beam Forces

Click .

A list of the forces in each beam element are listed. You can save this list to be used later.

SolidWorks SAE Design and Analysis Project 161

Lesson 6: Frame Analysis

Conclusion

In this lesson, we evaluated the torsional rigidity of our frame design. We learned how to set up an analysis using beam element. We also learned about the various post processing options available when beams are used.

At this point, it could be advantageous to change the frame design and re-evaluate the torsional rigidity. The most common goal for frame design is a torsionally stiff and light frame. Design changes could include different beam lengths, cross sections, or material properties.

It is important to note that the torsional rigidity was evaluated and set up with respect to the experiment that would be performed once the frame is made. We can only compare experiment to analysis if the boundary conditions are set up in the same manner.

Additionally, assumptions are made in the finite element model that might not reflect the real world situation perfectly. Therefore, it is most advantageous to evaluate different frame designs using the software to decide which is the stiffest, not one that matches the experiment perfectly.

162 SolidWorks SAE Design and Analysis Project

Lesson 7: Intake Analysis

When you complete this lesson, you will be able to:



Set up and run a Flow Simulation.



Post-process a Flow Simulation.

SolidWorks SAE Design and Analysis Project 163

Lesson 7: Intake Analysis

Intake Manifold Design

The common goal of an intake manifold design is even distribution of flow to the piston heads. This is to insure optimum engine efficiency. In this lesson,

SolidWorks Flow Simulation will be used to investigate the design of our intake manifold when the car is moving at 22 m/s (50 mph).

This lesson will introduce the complete set up of a

SolidWorks Flow Simulation project. We will prepare our model for analysis, set up boundary conditions and engineering goals, run our project, and learn to post process our results.

Model Preparations

In structural analysis, it is typically necessary to simplify the SolidWorks geometry to allow the simulation to run. The same is true for flow analysis. A simplified model will result in faster mesh and run times providing you with a quicker result. Part of model preparation is deciding what type of model you will be running. SolidWorks Flow

Simulation categorizes flow analysis in terms of the flow being either internal or external.

External Flow Analysis

This type of analysis involves the study of flow around a region not necessarily bounded by solid geometry. Typically, this is used for the study of flow over aircrafts, automobiles, buildings, etc.

Internal Flow Analysis

Internal flow analysis deals with the study of flow inside a region bounded by solid geometry. A typical example of an internal flow analysis would be the flow through an

HVAC system. In this type of analysis, flow enters the model through some inlet and leaves the model through the outlet. Flow Simulation requires the model to be fully closed to perform an internal analysis, therefore some geometry modifications may be necessary prior to setting up the model. This will be the case in our analysis of the intake manifold.

Open Intake Assembly.

Click

File, Open

and select the part Intake Assembly. Click

Open to open the part.

164 SolidWorks SAE Design and Analysis Project

Start SolidWorks Flow Simulation.

Click

Tools

Add-Ins

. Select

SolidWorks Flow Simulation

Click

Lesson 7: Intake Analysis

SolidWorks Flow Simulation Interface

SolidWorks Flow Simulation functions are accessed in the same way as SolidWorks.

When a simulation study is created, a Flow Simulation analysis tree appears as a tab next to the FeatureManager design tree tab. Each new study that gets created is linked to a specific configuration created in the ConfigurationManager. Like SolidWorks functions,

Flow Simulation functions can be accessed from the Flow Simulation toolbars,

CommandManager, or

Flow Simulation

drop-down menu. Additionally, functions can be selected by right-clicking geometry or items in the Flow Simulation analysis tree.

CommandManager

CommandManager tab

Flow Simulation

Toolbars

Flow Simulation analysis tree

SolidWorks SAE Design and Analysis Project 165

Lesson 7: Intake Analysis

Lids

As mentioned previously, internal analysis requires the geometry of the model to be fully closed. In the intake manifold, there is an opening for the inlet flow and four ports for the flow to the cylinders. We must close these openings with lids. We will then apply the proper boundary conditions to the surface of these lids to tell Flow Simulation how the fluid will be entering or leaving through the lid surface.

Create lids.

From the

Flow Simulation

drop-down menu, select

Tools

Create

Lids

Select the planar faces on the inlet and the four outlet ports that the lid will cover.

Select

Adjust Thickness

and enter

1mm

as the

Thickness

Click .

You’ll notice nine new parts in the FeatureManager design tree. The lids are blind extrusions from the selected planar faces into the openings with a distance that was specified as the

Thickness

. The annular lids can be neglected as they would not come in contact with the internal fluid.

Note: The thickness of the lid for an internal analysis is usually not important

however, the lid should not be so thick that the flow pattern is affected down stream. For most cases, the lid thickness could be the same thickness used to create the neighboring walls.

Tip:

If the lid face is not planar, the lid tool cannot be used. In this case, simply create the lid manually using a mid plane extrusion.

166 SolidWorks SAE Design and Analysis Project

Lesson 7: Intake Analysis

Check Geometry

SolidWorks Flow Simulation has a tool called

Check Geometry

that allows users to check the solid geometry to make sure that it is ready for analysis. We know that the geometry must be fully closed for an internal analysis.

Additionally, we need to make sure that no invalid contacts exist in our model. An invalid contact will cause the

Check Geometry

tool to report zero internal volume and the Flow Simulation will fail to solve. Some examples of invalid contact are shown in the figure.

Check geometry.

From the

Flow Simulation

menu choose:

Tools

Check

Geometry

Select

Internal

under

Analysis Type

Click

Check

The tool should calculate a fluid volume correctly and there should be no invalid contacts.

If invalid contacts exist, you must correct them before beginning the flow simulation project.

Click

Close

when you are satisfied.

Creating the Project

Now that our geometry has been properly modified, we can proceed with the Flow

Simulation project.

Create a project.

From the

Flow Simulation

menu, choose:

Project

Wizard

SolidWorks SAE Design and Analysis Project 167

Lesson 7: Intake Analysis

Create new project.

Under

Configuration

, click

Create new

to create a new configuration.

In the

Configuration name

box, enter

Project 1

Click

Next

Note: SolidWorks Flow Simulation will create and activate a new configuration called

Project 1

when the wizard is finished. All data associated with running the analysis will be stored in a separate folder in the model directory numbered sequentially, i.e. “1”, “2”, “3”... etc. based on how many projects are defined on this model.

Select units.

Select

SI (m-kg-s)

as the

Unit System

for this project.

168

Click

Next

SolidWorks SAE Design and Analysis Project

Select analysis type.

Select

Internal

under

Analysis Type

Lesson 7: Intake Analysis

Click

Next

Select fluid.

Expand the

Gases

tree and double-click

Air

to add it to the

Project Fluids

list.

Click

Next

SolidWorks SAE Design and Analysis Project 169

Lesson 7: Intake Analysis

Select wall conditions.

Accept the default conditions and click

Next

Initial conditions.

Accept the default conditions and click

Next

170 SolidWorks SAE Design and Analysis Project

Results and Geometry Resolution.

Set the

Result Resolution

Click

Finish

Lesson 7: Intake Analysis

Review Flow Simulation analysis tree.

SolidWorks Flow Simulation has created and activated an additional configuration called Project

1. In addition, the Flow Simulation analysis tree tab has been created in the FeatureManager.

Select the Flow Simulation analysis tree tab .

If changes need to be made to the settings of the project, you can right click the Input

Data

folder and select the appropriate option.

In the graphics window, the Computational Domain is shown as a wireframe box enveloping the model.

This is the area where the model will solve the flow simulation. Because this is an internal analysis, the model will be solved inside the solid geometry inside the box.

SolidWorks SAE Design and Analysis Project 171

Lesson 7: Intake Analysis

Insert boundary condition.

In the Flow Simulation analysis tree, under Input

Data

, right-click Boundary Conditions and select

Insert Boundary Condition

Select the inside surface of the lid covering the inlet as shown in the figure.

To access the inner face, right click the outer face of the lid and click

Select Other

. In the

Select Other

window, cycle through the faces by moving the pointer to highlight each face dynamically in the graphics window.

Set up boundary condition.

Under Type select

Flow Openings

Select

Inlet Velocity

Under

Flow Parameters

, click

Normal to Surface

and enter

22 m/s

Click .

172

Insert boundary condition.

In the Flow Simulation analysis tree, under Input

Data

, right-click Boundary Conditions and select

Insert Boundary Condition

Select the inside face of one of the lids covering the outlet ports as shown in the figure.

SolidWorks SAE Design and Analysis Project

Set up boundary condition.

Under

Type

select

Pressure Openings

Select

Environment Pressure

Click .

Lesson 7: Intake Analysis

Set up boundary condition.

Repeat this procedure to create Environment Pressure boundary conditions for the remaining three outlet ports.

SolidWorks SAE Design and Analysis Project 173

Lesson 7: Intake Analysis

Engineering Goals

SolidWorks Flow Simulation contains built in criteria to stop the solution process. In addition, it is best to use your own criteria by using engineering goals. Engineering goals are user specified parameters of interest which users can display while the solver is running and obtain information about after convergence is reached. Goals can be set throughout an entire domain (Global), in a selected area (Surface, Point), or within a selected volume (Volume). Finally, mathematical expressions using other goals can be written in an equation goal.

Surface goal.

In the SolidWorks Flow Simulation analysis tree, rightclick Goals, and select

Insert Surface Goals

To select the inlet surface for the Surface Goals, split the feature pane and in the upper portion click the boundary condition Inlet Velocity 1 item in the Flow

Simulation analysis tree to input the face where the surface goal is to be applied.

In the

Parameter

list, locate

Volume Flow Rate

and check the box.

Click .

Rename goal.

Rename the goal so that it appears as Inlet Volume

Flow Rate

174 SolidWorks SAE Design and Analysis Project

Surface goal.

Repeat the previous steps to apply a surface goal for the volume flow rate at the outlets.

When selecting the Environment Pressure boundary conditions, hold the control key and select all of the outlet conditions.

Click

Create a separate goal for each surface

. This will create a separate goal for each outlet.

Click .

Rename each goal to reflect the outlets.

Lesson 7: Intake Analysis

Equation goal.

Right-click Goals and select

Insert Equation Goal

Select the Outlet Volume Flow Rate 1 surface goal that was defined in the previous step to add it to the

Expression

box.

Click

in the

Equation Goal

window.

Repeat this procedure to sum all of the outlet goals.

Click

Rename goal.

Rename the goal so that it appears as Sum of Outlet Volume Flow Rates

Solve.

In the Flow Simulation analysis tree, right-click the project and select

Run

Make sure that

Load Results

is selected.

Click

Run

with the default settings.

It could take up to an hour to run this study.

SolidWorks SAE Design and Analysis Project 175

Lesson 7: Intake Analysis

Post-Processing

We can begin to post-process the results once the solver is completed. In this part of the lesson, we will learn about various post processing options available in SolidWorks Flow

Simulation. We first must change the transparency of the model so that we can view the results.

Change transparency.

In the

Flow Simulation

menu, select

Results

Display

Transparency

Move the slider to 0.75.

Note: The transparency can also be changed by right-click the parts in the

FeatureManager design tree.

Cut plot.

In the Flow Simulation analysis tree, right-click Cut Plots and select

Insert

Select the Top plane of the plenum assembly.

Click .

176 SolidWorks SAE Design and Analysis Project

Lesson 7: Intake Analysis

Color Bar

In the

Color Bar

dialog box, you can specify a physical parameter for the display. You also have control over various settings of the display. You can access the

Color Bar

double-clicking on the legend in the plot.

Adjust view settings.

Double-click the legend to bring up the

Color Bar

dialog.

Change the

Parameter

Velocity

Change the

Number of colors

110

Click

Hide the Cut Plot when you are through.

SolidWorks SAE Design and Analysis Project 177

Lesson 7: Intake Analysis

Flow trajectory.

In the Flow Simulation analysis tree, right-click Flow Trajectories and select

Insert

Select the Inlet Velocity 1 boundary condition.

Enter

as the Number of Points. Click .

Hide the Flow Trajectories when you are through.

Surface plot.

In the Flow Simulation analysis tree, right-click Surface Plots and select

Insert

Select

Use all faces

Make sure

Contours

is selected and the

Parameter

Pressure

. Click .

178 SolidWorks SAE Design and Analysis Project

Lesson 7: Intake Analysis

Goals plot.

In the Flow Simulation analysis tree, right click Goal Plots and select

Insert

Click

All

in the

Goal Plots

window and click

Show

A table will be automatically created containing information about the goals.

Discussion

As we can see from the goals plot, the inlet volume flow rate matches the outlet volume flow rate. This is a good sanity check in that all the flow entering the model is leaving the model. In addition, we notice the different volume flow rates exiting each outlet condition.

Much of the flow is leaving through one of the outlets in the center. This was also seen with the flow trajectory plot. This could be because the outlet port is slightly off-set from the center of the plenum, causing more flow to leave through one side. Re-design of the plenum could better distribute the flow amongst the outlet ports.

In the real world, each piston would be firing at a different time as the engine is running.

To more accurately represent this situation, a transient study could be set up with the outlet ports turning on and off with respect to when they would fire using time curves. To set this up in SolidWorks Flow Simulation,

Time Dependent

would need to be selected in the

Analysis Type

window of the

Wizard

. In addition, modifications to the outlet boundary conditions would be needed to specify when they turn on (flow is allowed) and off (flow is restricted).

Conclusions

In this lesson, we investigated the design of the intake manifold using SolidWorks Flow

Simulation. We learned how to setup and run a flow analysis. We also learned good postprocessing techniques for evaluating our designs. You are encouraged to continue you investigations of the post-processing options available on your own. In addition, more information in the form of tutorials and technical writings are available through the help menus.

SolidWorks SAE Design and Analysis Project 179

Lesson 7: Intake Analysis

180 SolidWorks SAE Design and Analysis Project