Solidworks MBD - Solidworks 2015 Training [PDF]

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SOLIDWORKS MBD SOLIDWORKS 2015 TRAINING

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SOLIDWORKS® 2015 SOLIDWORKS MBD

Dassault Systèmes SolidWorks Corporation 175 Wyman Street Waltham, MA 02451 U.S.A.

© 1995-2014, Dassault Systèmes SolidWorks Corporation, a Dassault Systèmes S.A. company, 175 Wyman Street, Waltham, Mass. 02451 USA. All Rights Reserved. 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; 8,581,902, 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 Portions of this software © 1986-2014 Siemens Product Lifecycle Management Software Inc. All rights reserved. This work contains the following software owned by Siemens Industry Software Limited: D-Cubed™ 2D DCM © 2014. Siemens Industry Software Limited. All Rights Reserved. D-Cubed™ 3D DCM © 2014. Siemens Industry Software Limited. All Rights Reserved. D-Cubed™ PGM © 2014. Siemens Industry Software Limited. All Rights Reserved. D-Cubed™ CDM © 2014. Siemens Industry Software Limited. All Rights Reserved. D-Cubed™ AEM © 2014. Siemens Industry Software Limited. All Rights Reserved. Portions of this software © 1998-2014 Geometric Ltd. Portions of this software incorporate PhysX™ by NVIDIA 20062010. Portions of this software © 2001-2014 Luxology, LLC. All rights reserved, patents pending. Portions of this software © 2007-2014 DriveWorks Ltd. Copyright 1984-2010 Adobe Systems Inc. and its licensors. All rights reserved. Protected by U.S. Patents 5,929,866; 5,943,063; 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 Portions of this software © 2008 Solversoft Corporation. PCGLSS © 1992-2014 Computational Applications and System Integration, Inc. All rights reserved. Copyright Notices for SOLIDWORKS Enterprise PDM Product Outside In® Viewer Technology, © 1992-2012 Oracle © 2011, Microsoft Corporation. All rights reserved. Copyright Notices for eDrawings Products Portions of this software © 2000-2014 Tech Soft 3D. Portions of this software © 1995-1998 Jean-Loup Gailly and Mark Adler. Portions of this software © 1998-2001 3Dconnexion. Portions of this software © 1998-2014 Open Design Alliance. All rights reserved. Portions of this software © 1995-2012 Spatial Corporation. The eDrawings® for Windows® software is based in part on the work of the Independent JPEG Group. Portions of eDrawings® for iPad® copyright © 1996-1999 Silicon Graphics Systems, Inc. Portions of eDrawings® for iPad® copyright © 2003 – 2005 Apple Computer Inc.

Document Number: PMT1525-ENG

Contents

Introduction About This Course . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Prerequisites . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Course Design Philosophy . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Using this Book . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 2 Conventions Used in this Book . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 About the Training Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 Training Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Windows® 7 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Use of Color . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Graphics and Graphics Cards . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Color Schemes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Lesson 1: What is SOLIDWORKS MBD? What is SOLIDWORKS MBD? . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 8 Steps in the Process. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 Preparing the Part or Assembly . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 View Styles . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 9 Dimensions, Annotations and Tables . . . . . . . . . . . . . . . . . . . . . . 10 Configurations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 10 DimXpert Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 11 Manipulating Annotation Views. . . . . . . . . . . . . . . . . . . . . . . . . . 11 Capturing 3D Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 12 Publishing a 3D PDF and eDrawings . . . . . . . . . . . . . . . . . . . . . . . . . 12 3D PDF Templates . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 13 Setting up SOLIDWORKS MBD. . . . . . . . . . . . . . . . . . . . . . . . . 13

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Lesson 2: Using DimXpert DimXpert . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 16 Features and Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 17 Prismatic and Turned Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 DimXpert Selections. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 18 Other Types of Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 19 Settings for DimXpert. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Block Tolerance vs. General Tolerance . . . . . . . . . . . . . . . . . . . . 20 DimXpert Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 Auto Dimension Scheme . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 22 How the Auto Dimension Scheme Works . . . . . . . . . . . . . . . . . . 22 DimXpert Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 25 DimXpert Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 28 Mapping Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 30 Show Tolerance Status . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 32 Size and Location Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . 33 Imported Geometry. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 35 Exercise 1: Using Auto Dimension Scheme. . . . . . . . . . . . . . . . . . . . 37 Exercise 2: Imported Geometry . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 40 Lesson 3: Adding Size and Location Dimensions Special Selection Techniques . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Compound Selections . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 44 Combining Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 46 Dimensions Between Cylinders . . . . . . . . . . . . . . . . . . . . . . . . . . 47 Intersection Lines . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 48 3D Note Options . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 54 Manually Creating DimXpert annotations . . . . . . . . . . . . . . . . . . . . . 55 Adding Datums . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 55 Adding Geometric Tolerance Symbols. . . . . . . . . . . . . . . . . . . . . 58 Recreating Basic Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . 60 DimXpert Annotations and 2D Drawings . . . . . . . . . . . . . . . . . . . . . 63 Exercise 3: Automatic and Manual Methods 1. . . . . . . . . . . . . . . . . . 66 Exercise 4: Automatic and Manual Methods 2. . . . . . . . . . . . . . . . . . 69 Exercise 5: Using Selection Techniques. . . . . . . . . . . . . . . . . . . . . . . 72

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Contents

Lesson 4: Turned Parts Turned Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 76 Deleting Dimensions and Symbols. . . . . . . . . . . . . . . . . . . . . . . . 79 Deleting the Tolerance Scheme . . . . . . . . . . . . . . . . . . . . . . . . . . 79 Using Plus and Minus . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 80 Tolerance Rule Checking . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 82 Duplicate Datums . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 83 Cylindrical Position . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 84 Collinear Datums . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 86 Non-Coaxial Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88 Exercise 6: Turned Parts 1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90 Exercise 7: Turned Parts 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 93 Exercise 8: Rule Checking . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96 Lesson 5: Annotation Views Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 Why Are Annotation Views Important?. . . . . . . . . . . . . . . . . . . 100 Types of Annotation Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 100 Orthographic Annotation Views. . . . . . . . . . . . . . . . . . . . . . . . . 101 Specialty Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . 101 Manipulating Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . 103 Hiding and Showing Annotation Views . . . . . . . . . . . . . . . . . . . 103 Activating an Annotation View . . . . . . . . . . . . . . . . . . . . . . . . . 104 Orienting an Annotation View . . . . . . . . . . . . . . . . . . . . . . . . . . 105 Dynamic Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . 106 Reassigning Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 108 Other Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 109 Adding a New Annotation View . . . . . . . . . . . . . . . . . . . . . . . . 113 Using Configurations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 116 Copy Scheme . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 118 ‘Hiding’ Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 119 Modifying Dimension Attachments . . . . . . . . . . . . . . . . . . . . . . . . . 119 Lesson 6: Capturing 3D Views Capturing 3D Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 Simulating Drawing Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . 124 3D Views for Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 125 Using Section Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 128 Dimension Size in PDF. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 130 Using Configurations and Display States in 3D Views . . . . . . . 131 3D Views for Assemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 132 Breaking Views. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Model Break Styles. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 134 Model Break Methods . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135 Model Break Properties . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 135

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Using Feature and Reference Dimensions . . . . . . . . . . . . . . . . . . . . 138 DimXpert Annotations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Reference Dimensions and Annotations. . . . . . . . . . . . . . . . . . . 139 Feature Dimensions . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 139 Dimensions in Annotation Views . . . . . . . . . . . . . . . . . . . . . . . . 139 Exercise 9: Capturing 3D Views 1 . . . . . . . . . . . . . . . . . . . . . . . . . . 143 Exercise 10: Capturing 3D Views 2 . . . . . . . . . . . . . . . . . . . . . . . . . 148 Exercise 11: Capturing 3D Views - Assembly . . . . . . . . . . . . . . . . . 152 Lesson 7: Publishing PDF and eDrawings Files Publishing PDF and eDrawings Files . . . . . . . . . . . . . . . . . . . . . . . . 156 Theme . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156 Views to Include . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 156 Output Details . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 Publishing a Part to a 3D PDF . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 157 3D View Manipulation . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160 Mouse Buttons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160 3D Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 160 Publishing a Part to an eDrawings File. . . . . . . . . . . . . . . . . . . . . . . 164 eDrawings Tools . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 164 Publishing an Assembly to a PDF . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Adding 3D Comments . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 170 Publishing an Assembly to an eDrawings File . . . . . . . . . . . . . . . . . 171 Exercise 12: Publishing a Part 1 . . . . . . . . . . . . . . . . . . . . . . . . . . . . 175 Exercise 13: Publishing a Part 2 . . . . . . . . . . . . . . . . . . . . . . . . . . . . 177 Exercise 14: Publishing an Assembly. . . . . . . . . . . . . . . . . . . . . . . . 179 Lesson 8: 3D PDF Template Editor 3D PDF Template Editor . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 184 Template Arrangement . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 184 Components of the Template . . . . . . . . . . . . . . . . . . . . . . . . . . . 185 Text Types . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 186 Modifying a Template. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187 Standard Template Files . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 187 Changing the Logo . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 188 Saving the Template . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 189 Adding Text . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 190 Using The Template . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 191 Exercise 15: Creating a Template . . . . . . . . . . . . . . . . . . . . . . . . . . . 193

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Introduction

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Introduction

About This Course

SOLIDWORKS 2015

The goal of this course is to teach you how to create 3D PDF and eDrawings files using SOLIDWORKS MBD or Model Based Definition software. The SOLIDWORKS MBD application in the SOLIDWORKS software is so robust and feature rich that it is impractical to cover every minute detail and still have the course be a reasonable length. Therefore, the focus of this course is on the fundamental skills and concepts central to successfully publishing 3D PDF files. You should view the training course manual as a supplement to, not a replacement for, the system documentation and on-line help. Once you have developed a good foundation in basic skills, you can refer to the on-line help for information on less frequently used command options.

Prerequisites

Students attending this course are expected to have the following: I I I

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Mechanical design experience. Completed the course SOLIDWORKS Essentials. Familiarity with the Annotations lesson from the course SOLIDWORKS Drawings - ANSI or SOLIDWORKS Drawings - ISO. Experience with the Windows™ operating system.

Course Design Philosophy

This course is designed around a process- or task-based approach to training. Rather than focus on individual features and functions, a process-based training course emphasizes the processes and procedures you follow to complete a particular task. By utilizing case studies to illustrate these processes, you learn the necessary commands, options and menus in the context of completing a design task.

Course Length

The recommended minimum length for this course is 1 day.

Using this Book

This training manual is intended to be used in a classroom environment under the guidance of an experienced SOLIDWORKS instructor. It is not intended to be a self-paced tutorial. The examples and case studies are designed to be demonstrated “live” by the instructor.

Laboratory Exercises

Laboratory exercises give you the opportunity to apply and practice the material covered during the lecture/demonstration portion of the course. They are designed to represent typical design and modeling situations while being modest enough to be completed during class time.

Drafting Standards

SOLIDWORKS software support several internationally accepted drafting standards including ANSI, ISO, DIN, and JIS. The examples, illustrations, and lab exercises in this course were created using the ANSI standard.

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Conventions Used in this Book

Introduction

This manual uses the following typographic conventions: Convention Bold Sans Serif

SOLIDWORKS commands and options appear in this style. For example, Features > means click the Extruded Extruded Cut Cut icon on the Features tab of the CommandManager.

Typewriter

Feature names and file names appear in this style. For example, Sketch1.

17 Do this step

About the Training Files

Meaning

Double lines precede and follow sections of the procedures. This provides separation between the steps of the procedure and large blocks of explanatory text. The steps themselves are numbered in sans serif bold.

A complete set of the various files used throughout this course can be downloaded from the SOLIDWORKS website, www.solidworks.com. Click on the link for Support, then Training, then Training Files, then SOLIDWORKS Training Files. Select the link for the desired file set. There may be more than one version of each file set available. Direct URL: www.solidworks.com/trainingfilessolidworks

The files are supplied in signed, self-extracting executable packages. The default extraction location for the training files will be C:\SOLIDWORKS Training Files. The files are organized by lesson number. The Case Study folder within each lesson contains the files your instructor uses while presenting the lessons. The Exercises folder contains any files that are required for doing the laboratory exercises. Completed lesson files are also included and the files names are followed by “_&” to differentiate them.

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Introduction

Training Templates

SOLIDWORKS 2015

A set of training templates are used throughout the course to standardize the settings for the new files that are created. These templates are also supplied in signed, self-extracting executable packages. They can be downloaded from the same website address as the Training Files and use the same extraction location. These templates are used for all SOLIDWORKS core courses. To access the training templates in SOLIDWORKS: 1. 2. 3. 4.

Click Tools, Options, System Options, File Locations. Choose Document Templates from the drop down menu. Click Add and browse to the Training Templates folder. Click OK and Yes on each of the messages.

Accessing Training Templates

Once the file location has been added, click the Advanced button and the Training Templates tab in the New SOLIDWORKS Document dialog can be used.

Windows® 7

The screen shots in this manual were made using the SOLIDWORKS software running on Windows® 7. If you are not using Windows 7, or if you have a different theme setting, you may notice slight differences in the appearance of the menus and windows. These differences do not affect the performance of the software. The SOLIDWORKS installation paths conform to Windows 7 standards. If you are not using Windows 7, the installation paths will be different.

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Use of Color

Introduction

The SOLIDWORKS user interface makes extensive use of color to highlight selected geometry and to provide you with visual feedback. This greatly increases the intuitiveness and ease of use of the SOLIDWORKS software. To take maximum advantage of this, the training manuals are printed in full color. Also, in some cases, we may have used additional color in the illustrations to communicate concepts, identify features, and otherwise convey important information. For example, we might show the result of an operation in a different color, even though by default, the SOLIDWORKS software would not display the results in that way.

Graphics and Graphics Cards

The SOLIDWORKS software sets a new standard with best-in-class graphics. The combination of a highly reflective material and the realism of RealView Graphics is an effective tool for evaluating the quality of advanced part models and surfaces. RealView Graphics is hardware (graphics card) support of advanced

shading in real time. For example, if you rotate a part, it retains its rendered appearance throughout the rotation. Color Schemes

Out of the box, the SOLIDWORKS software provides several predefined color schemes that control, among other things, the colors used for highlighted items, selected items, sketch relation symbols, and shaded previews of features. We have not used the same color scheme for every case study and exercise because some colors are more visible and clear than others when used with different colored parts. In addition, we have changed the viewport background to plain white so that the illustrations reproduce better on white paper. As a result, because the color settings on your computer may be different than the ones used by the authors of this book, the images you see on your screen may not exactly match those in the book.

User Interface Appearance

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Throughout the development of the software, there have been some cosmetic User Interface changes, intended to improve visibility, that do not affect the function of the software. As a policy, dialog images in the manuals which exhibit no functional change from the previous version are not replaced. As such, you may see a mixture of current and “old” UI dialogs and color schemes.

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Introduction

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SOLIDWORKS 2015

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Lesson 1 What is SOLIDWORKS MBD?

Upon successful completion of this lesson, you will be able to:

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Understand how to prepare geometry for a 3D PDF file.

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Understand how DimXpert is used.

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Understand the role of annotation views.

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Understand the concept of a 3D view.

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Understand the concept of publishing to a 3D PDF.

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Lesson 1

SOLIDWORKS 2015

What is SOLIDWORKS MBD?

What is SOLIDWORKS MBD?

SOLIDWORKS Model Based Definition or MBD is a tool used to present product and manufacturing information (PMI), formerly included in traditional 2D drawings, in the drawingless file formats 3D PDF and eDrawings. This PMI includes geometric dimensioning and tolerancing (GD&T) data; specifically 3D dimensions and annotations.

The part and assembly PMI includes many types of information: I I I I I I I I I I I

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Views Configurations Display States Custom Properties Exploded Views Tables Annotations Reference Dimensions DimXpert Annotations Annotation Views 3D Views

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SOLIDWORKS 2015

Lesson 1 What is SOLIDWORKS MBD?

Steps in the Process

The process of creating interactive 3D PDF or eDrawings files requires plenty of preparation within the part or assembly followed by the use of specific MBD tools.

Part and Assembly Preparation Steps

Prepare the part or assembly using appearances and DimXpert tools.

Model Based Definition Steps

Create the 3D PDF or eDrawings file using MBD tools.

Preparing the Part or Assembly

Preparing a part for use in an interactive file format includes the considerations of which descriptive views are needed to define the geometry. In order to imitate some of the views used in traditional 2D drawings, additional geometry may be required.

View Styles

Various types of standard views can be added as 3D views. In addition, many familiar drawing view types can be added using existing SOLIDWORKS tools.

1. Create the appropriate views, configurations, display states, tables, exploded views, and custom properties. 2. Use DimXpert tools create annotations, including datums, dimensions, and geometric tolerances. 3. Optionally, manipulate annotation views to group the annotations. 4. Use configurations, display states, standard views and annotation views. 5. Optionally, create or modify 3D PDF templates. 6. Publish to a 3D PDF or an eDrawings file.

For example, a Section View can be used to create a ‘cutaway’ type of view.

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Lesson 1

SOLIDWORKS 2015

What is SOLIDWORKS MBD?

Dimensions, Annotations and Tables

Multiple sources of dimensions and annotations can be utilized to populate 3D views. Feature, reference and DimXpert annotations can all be displayed in 3D views. The same is true for annotations and tables.

Configurations

Configurations can be leveraged to form 3D views by creating alternative sizes, suppressing specialized cut features, or select an exploded view.

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SOLIDWORKS 2015

Lesson 1 What is SOLIDWORKS MBD?

DimXpert Tools

DimXpert tools can be used to create annotations that define the geometry. The geometry of the part, not the SOLIDWORKS features, is used when creating the annotations and dimensions. The tolerance status is displayed using colors.

Manipulating Annotation Views

Annotation Views are created automatically to organize dimensions.

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The annotations and dimensions in these can be parallel to standard reference plane directions or oblique faces in the model. Some are also flat to the screen for storage of notes and tables.

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Lesson 1

SOLIDWORKS 2015

What is SOLIDWORKS MBD?

Capturing 3D Views

3D Views can be captured by leveraging multiple elements of the model including view orientations, configurations, exploded views, tables, annotations, dimensions, tolerances, and annotation views.

Publishing a 3D PDF and eDrawings

3D PDF files can be published using 3D views, text and custom properties drawn from the part or assembly with a 3D PDF template.

Publish an eDrawings file directly from the part or assembly.

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SOLIDWORKS 2015

Lesson 1 What is SOLIDWORKS MBD?

3D PDF Templates

3D PDF Templates can be

Setting up SOLIDWORKS MBD

The SOLIDWORKS MBD product can be purchased from the Technical Communication set.

copied to create user defined templates for use in publishing a 3D PDF file.

It can be installed along with the SOLIDWORKS installation or after by modifying the installation using the Control Panel. 1. 2. 3. 4.

Purchase SOLIDWORKS MBD. Obtain a serial number for SOLIDWORKS MBD. Install SOLIDWORKS. Add the SOLIDWORKS MBD serial number during the installation. 5. Show the SOLIDWORKS MBD CommandManager.

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Lesson 1

SOLIDWORKS 2015

What is SOLIDWORKS MBD?

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Lesson 2 Using DimXpert

Upon successful completion of this lesson, you will be able to:

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Recognize DimXpert annotations and selections.

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Generate tolerance schemes automatically.

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Analyze the state of constraint.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

DimXpert

The DimXpert software is used to tolerance a model by adding tolerance features and the associated 3D annotations. These 3D annotations (datums, dimensions, and geometric tolerances) are used to partially or fully define the geometry. In this lesson, the DimXpert Auto Dimension Scheme will be used. Manual DimXpert tools will be discussed in Lesson 3: Adding Size and Location Dimensions. The results can also be used for: I I I I I

SOLIDWORKS Model Based Definition Partner CAM applications Partner tolerance analysis applications Metrology (measurement) applications Creating dimensioned and annotated drawing views

SOLIDWORKS model features and topology are recognized to create Features such as fillets, chamfers, patterns, extrudes and hole wizard holes. The associated Annotations (dimensions and tolerances) can be added automatically or manually to complete the process.

DimXpert Feature

Dimensions and Features

Note

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SOLIDWORKS MBD supports industry standards such as Military-Standard-31000A, ASME Y14.41, ISO 16792, and DIN ISO 16792.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

Features and Annotations

DimXpert tools create features and annotations such as datums, size dimensions, location dimensions, and geometric tolerances. They are organized in the DimXpertManager, a tree structure similar to the FeatureManager design tree.

As the annotations are created, they are automatically oriented in 3D space to match the source feature orientations and the default orthographic planes of the model. They are organized into annotation views (see Annotation Views on page 100); annotations that share the same orientation. Note

Feature and reference dimensions and annotations created in the model are also organized in annotation views. For more information, see Using Feature and Reference Dimensions on page 138.

Introducing: DimXpertManager

The DimXpert tree organizes the tolerance features and dimensions that comprise what is considered the Tolerance Scheme in the DimXpertManager. Colors are applied to faces are used to help visualize the status of the tolerance. For more information, see Show Tolerance Status on page 32.

FeatureManager Design Tree

Where to Find It

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DimXpertManager Design Tree

DimXpertManager: Right-click the top level component and click Tree Display and click Feature Based Tree, Annotation Based Tree or Flat Tree

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Prismatic and Turned Parts

Both Prismatic and Turned part (Lesson 4: Turned Parts) types can be toleranced. A comparison between the types is listed below. Prismatic

DimXpert Selections

Turned

DimXpert Selections are specific to the geometry. For instance, a

selected internal cylindrical face could be classified as a cylinder, hole or compound hole. For details on using these and other selections, see Special Selection Techniques on page 44. Some of the common selections are shown below.

Compound Cylinder

Width Feature

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A Compound Cylinder is used to identify a cylindrical face that is broken into multiple faces by other geometry. A Compound Hole can also be selected using a set of coaxial cylinders with the same radius.

A Width Feature is used to identify parallel planar faces that define a width dimension on the part. The planar faces must have opposing surface normals.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

The Compound Plane is used to identify a planar face that is broken into multiple faces by other geometry. Compound Plane

features are recognized from simple or hole wizard holes. A cut using a circular sketch is also considered a hole.

Pattern

Pattern

Note

These parts can be found in the Lesson02\Case Study\Examples folder.

Other Types of Annotations

The annotation types Datum Target, Surface Finish, Weld Symbol, Note and Smart Dimensions are available on the SOLIDWORKS MBD CommandManager, but they do not create DimXpert annotations. They are reference dimensions and they appear in the standard black color. For more information, see Using Feature and Reference Dimensions on page 138.

Tables

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The table types General Table, Bill Of Materials, Design Table and Title Block Table are available from the SOLIDWORKS MBD CommandManager, and they do not create DimXpert annotations. By default they are added to the Notes Area annotation view that remains flat to the screen at all times. For more information, see Specialty Annotation Views on page 101.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Settings for DimXpert

Settings exist for DimXpert to define the style and appearance of the annotations and tolerances. There are several topics that control specific types of annotations. I I I I I I

Size Dimension Location Dimension Chain Dimension Geometric Tolerance Chamfer Controls Display Options

Block Tolerance vs. General Tolerance

Under Tools, Document Properties, DimXpert there are Methods settings for Block Tolerance or General Tolerance.

Block Tolerance

Block Tolerance creates tolerances based on the precision of each dimension. In order to use it, click Document Properties, Dimensions and set Trailing zeroes to Standard.

General Tolerance

If General Tolerance is selected, individual settings for each feature type are available using the following sections.

DimXpert Properties

The DimXpert dialog in Document Properties allows you to set the tolerance types and values for annotations. These values are used by all DimXpert dimension and annotation commands.

Size Dimension

The Size Dimension option has settings for symmetric, bilateral or block tolerancing for several styles of dimension including diameter, depth and fillet radius.

Location Dimension

The Location Dimension option have settings for symmetric, bilateral or block tolerancing for distance and angle dimensions.

Chain Dimension

The Chain Dimension option has settings for the dimension method for holes and pockets. It also sets patterns, and the distance between features to either symmetric, bilateral or block tolerancing.

Geometric Tolerance

The Geometric Tolerance option has tolerance settings for datums, positions, runout, and surface profiles. It also toggles the automatic creation of basic dimensions.

Chamfer Controls

The Chamfer Controls option determine what is recognized as a chamfer as well as the tolerances.

Display Options

The Display Options controls the appearance of slot, geometric tolerance, hole callout, datum and linear dimensions. The display of redundant dimensions are also controlled.

Note

The Drafting Standard, Annotations, and Dimensions settings also have an impact on the annotations.

Where to Find It

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Menu: Tools, Document Properties, DimXpert

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

1

2

Open the part cover plate. Open the part cover plate from the Lesson02\Case Study folder.

Standard and methods.

Click Tools, Options, Document Properties, Drafting Standard, set the Overall Drafting Standard to ANSI. 3

Create basic dimensions.

Click Tools, Options, Document Properties, DimXpert, Geometric Tolerance and click Create basic dimensions as shown.

Do not click OK yet. 4

Redundant dimensions.

Click Display Options and click Eliminate duplicates and Show instance count as shown. Click OK.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Auto Dimension Scheme

Auto Dimension Scheme

offers an automated method for creating a tolerance scheme by creating datums, size dimensions, location dimensions, and geometric tolerances. In this example, the primary, secondary and tertiary datums will be identified along with selected faces of the part.

How the Auto Dimension Scheme Works

Using Auto Dimension Scheme, the geometry is broken down and identified as separate features. User selections identify datums and features of interest. A dimensioning scheme is generated automatically. I

Types of Schemes

Either Prismatic or Turned Part Types can be used depending on the geometry of the part. I

Datums

You identify the Primary, Secondary and Tertiary Datums by selecting planar or cylindrical faces of the model. I

Features identified

The part geometry is examined and features are identified and recognized through the selection of faces. I

Scheme created

A geometric tolerancing scheme, including toleranced dimensions, datums and geometric tolerancing symbols is created. Introducing: Auto Dimension Scheme

The Auto Dimension Scheme option is used to automate the process of recognizing features and adding functional tolerances. Starting with datum selection, additional faces can be added to define the scope of the scheme. See Special Selection Techniques on page 44 for more information.

Where to Find It

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Menu: Tools, DimXpert, Auto Dimension Scheme CommandManager: SOLIDWORKS MBD >

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DimXpertManager: Click Auto Dimension Scheme

Auto Dimension Scheme

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

5

Datum selections.

Click Auto Dimension Scheme and click Prismatic and Geometric. Select the Primary, Secondary and Tertiary planes as shown. Secondary Tertiary

Primary

Use a right-click

Note 6

to move between datum selections.

Scope.

Click in the Scope section and click Selected features. Select one of the holes. The selection popup dialog allows you define the selection as a Pattern and all four of the holes highlight.

Do not click OK yet. Note

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The pop-up appears when there are multiple selection options available. In this example, the cylindrical face can be recognized as a cylinder, hole or a pattern of holes.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

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Planar faces.

Select the two planar faces opposite the datums as shown. These selections are used to define the width and depth of the body. Click OK.

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Tolerance features.

The features created include datums, dimensions and symbols. Show Tolerance Status on page 32 is toggled on automatically.

Note

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This example uses annotation and dimension fonts that were set to 14 point text prior to using Auto Dimension Scheme. To set the fonts, click Tools, Options, Document Properties, Annotations and Dimensions.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

DimXpert Features

DimXpert Features are used to describe the geometry of the part.

many of these features are recognized directly from the topology of faces and edges. The types of features are listed below. Plane features are recognized from

planar faces

in the model.

Plane

Surface features are recognized from non-planar, non-cylindrical faces in the model.

Surface

Cone features are recognized from tapered cylindrical faces in the model. Cone

Cylinder features are recognized

from full or partial (arc) cylindrical faces in the model. Cylinder

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Boss features are recognized from

cylindrical faces in the model. A can be recognized instead of a circular boss.

Cylinder

Boss

Fillet features are recognized from

Fillet

filleted faces . A Fillet Pattern is a collection of fillets of the same size but disconnected. A Fillet Chain is linked directly to a SOLIDWORKS fillet feature.

Chamfer features are recognized from chamfered faces . Chamfers can be patterned and chained like fillets. Chamfer

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

Simple Hole features are recognized

Simple Hole

from cylindrical cut faces that lie within the edge boundaries of the body. They are dimensioned to the geometric center. A Cylinder can be recognized instead of a simple hole.

Counterbore features are

Counterbore

Countersink

recognized from cylindrical cut faces . They lie within the edge boundaries of the body and are dimensioned to the geometric center.

Countersink features are recognized from cylindrical and cone cut faces . They lie within the edge boundaries of the body and are dimensioned to the geometric center. They are a combination of a countersink and simple hole features. Slot features are recognized from

Slot

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internal cut features with two parallel plane faces . Slot features are dimensioned to the geometric center and include a label indicating the overall length and width. They may be blind or through.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Notch

Notch features recognized from cuts defined by parallel plane faces, open at one end and closed at the other with planar or cylindrical faces . Notch features are dimensioned for width and length and located to the geometric center.

Pocket features are recognized from

internal cut faces . They are irregularly shaped cuts without draft. They may be blind or through all. Pocket

DimXpert Annotations

Size Dimension

DimXpert Annotations include the standard drawing annotations

datums, dimensions and geometric tolerance symbols. They can be created using auto dimension scheme or manually using individual tools. The types of annotations are listed below. Size Dimensions are used to define the overall sizes of geometry. For example, an overall dimension between planar faces would be a size dimension.

Location Dimensions are used to

Location Dimension

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define the distances between features. For example, a dimension between a hole center and a planar face would be a location dimension.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

Datums

Datums are used to define the primary, secondary and tertiary datums of the part. They are placed on planar or cylindrical faces.

Geometric Tolerances are applied to dimensions and are used to communicate tolerances. Geometric Tolerance

Linked Patterns use the SOLIDWORKS features. Manual Patterns use a selection list of individual features, typically of the same type.

Pattern Feature

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Collection Patterns use a selection list of individual features, not necessarily of the same type, for the placement of a symbol such as a geometric tolerance.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Mapping Features

DimXpert features map directly to the annotations in the model. I I I I I

Tip

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Datum A with a flatness tolerance.Datum B perpendicular to Datum A.Datum C perpendicular to Datums A and B. A Hole Pattern1 with four Simple Hole features. Diameter1to define the hole and pattern. Position1 between the pattern and datums A, B and C. Distancebetween1 and Distancebetween2 dimensioning between the datum planes and selected planes.

Click an annotation in the DimXpertManager tree to highlight it in the graphics.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

DimXpertManager Viewing Options

The DimXpert annotations and associated features can be listed in several ways in the DimXpertManager. I I I

The Feature Based Tree lists DimXpert features such as Simple Hole1 first with the associated annotations under them. The Annotation Based Tree lists DimXpert annotations such as Diameter1 first with the features under them. The Flat Tree lists all DimXpert annotations and the associated features at the same level.

Feature Based Tree

Renaming Annotations

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Annotation Based Tree

Flat Tree

The annotations and features in the DimXpertManager can be renamed to make them easier to find and utilize.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

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DimXpertManager.

Click the DimXpertManager . It contains the tree that lists all the tolerancing features and annotations that have been generated. They map directly to the geometric features in the model. For more information, see Mapping Features on page 30.

Show Tolerance Status

The use of DimXpert tools provides definition to some or all of the geometric features of the model. Color coding of faces is used as a key to the current state of constraint. I I I I

Not Constrained = original color Over Constrained = red Under Constrained = yellow Fully Constrained = green

Fully Constrained Under Constrained

Over Constrained

Not Constrained (original color)

Note

Use Tools, Options, System Options, Colors to change the colors using DimXpert, Under Constrained, DimXpert, Fully Constrained, and DimXpert Over Constrained.

Where to Find It

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Menu: Tools, DimXpert, Show Tolerance Status CommandManager: SOLIDWORKS MBD > Show Tolerance Status

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

10 Constraint Status. Click Show Tolerance Status

. The green faces indicate fully constrained geometry. The original color remains on those faces that were not selected in the tolerance scheme, for example the filleted corner faces.

Size and Location Dimensions

To add further constraint to the geometry, add Size and Location Dimensions. Although they appear similar, there are subtle differences in the usage of these dimensions. Location Dimensions

Size Dimensions

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

Size Dimensions

Size Dimensions are for ‘features of size’ and can be used to measure a width, radius or diameter dimension. They are represented by the bottom set of diameter, radius, and linear dimensions.

Location Dimensions

Location Dimensions

Note

For more information, see Lesson 3: Adding Size and Location Dimensions.

Note

The Smart Dimension tool can create DimXpert location dimensions, DimXpert size dimensions, and Reference dimensions.

Where to Find It

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are for ‘features without size’; or everything except size dimensions. They are represented by the upper linear dimension.

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CommandManager: SOLIDWORKS MBD > Location Dimension CommandManager: SOLIDWORKS MBD > Size Dimension CommandManager: SOLIDWORKS MBD > Smart Dimension and select DimXpert location dimension, DimXpert size dimension or Reference dimension

11 Size Dimension. Click Size Dimension

and add a dimension to

the large fillet as shown. A single dimension prefixed with ‘4X’ is created.

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SOLIDWORKS 2015

Lesson 2 Using DimXpert

12 Status. Click Show Tolerance Status

. The part remains under defined, and may remain that way. It is only necessary to fully define those features that require specific tolerances.

Imported Geometry

DimXpert annotations and features can be created whether a part contains multiple SOLIDWORKS features or if it has been imported as a single piece of geometry.

DimXpert tools, such as Auto Dimension Scheme, use selected model features (fillets and hole features for example) as well as the topology of the part in creating the DimXpert annotations and features. The method is similar to what is used by FeatureWorks to identify individual features from topology. In this example a STEP file will be opened and used with the Auto Dimension Scheme tool.

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Lesson 2

SOLIDWORKS 2015

Using DimXpert

1

2

Open the STEP file Imported.STEP. Click Open and select the file Imported.STEP from the Lesson02\Case Study folder. Diagnostics.

Run Import Diagnostics and Attempt to Heal All. The part contains only a single feature, the imported body Imported1. 3

Auto.

Click Auto Dimension Scheme and select the cylinder as the Primary Datum and the circular planar face as the Secondary Datum as shown.

4

Scope.

For the scope, click All features and click OK. 5

DimXpertManager.

The DimXpertManager shows that many DimXpert features have been recognized including: bosses, planes, cones, holes, pockets, notches, fillets, chamfers, cylinders, and patterns.

6

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Save and close all files.

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SOLIDWORKS 2015

Exercise 1 Using Auto Dimension Scheme

Exercise 1: Using Auto Dimension Scheme

Create DimXpert annotations with Auto Dimension Scheme using this part. This lab reinforces the following skills: I I I

1

2

DimXpert on page 16. Auto Dimension Scheme on page 22. Size and Location Dimensions on page 33.

Open the part Using Auto Dimension Scheme. Open the part Using Auto Dimension Scheme from the Lesson02\Exercises folder. Auto Dimension Scheme

Click Auto Dimension Scheme and click Prismatic and Geometric. 3

Primary datum.

Select the cylindrical face as the Primary Datum.

4

Secondary datum.

Select the underside planar face as the Secondary Datum.

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Exercise 1

SOLIDWORKS 2015

Using Auto Dimension Scheme

5

Scope.

Under Scope, click Selected Features and select the 4 faces shown. Click OK.

6

Add size dimensions.

Arrange the annotations as shown. Add a Size Dimension to one of the fillet faces as shown. All of the fillets are selected as a single dimension.

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SOLIDWORKS 2015

Exercise 1 Using Auto Dimension Scheme

7

FeatureManager.

Click the FeatureManager design tree tab. Double-click the Boss-Extrude1 feature. Change the values of the three feature dimensions to 50mm, 75mm, and 120mm as shown. The DimXpert annotations update accordingly.

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Save and close all files.

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Exercise 2

SOLIDWORKS 2015

Imported Geometry

Exercise 2: Imported Geometry

Create DimXpert annotations for this imported geometry. This lab reinforces the following skills: I I

1

Auto Dimension Scheme on page 22. Imported Geometry on page 35.

Open the file Import_Part.STEP.

Open the STEP file Import_Part.STEP from the Lesson02\Exercises folder. Run Import Diagnostics and Attempt to Heal All.

2

Unit system.

Set the Unit System to MMGS. 3

Create basic dimensions.

Using Tools, Options, Document Properties, DimXpert, Geometric Tolerance and click Create basic dimensions as shown. 4

Datums.

Click Auto Dimension Scheme. Select the notch as the Primary Datum and the underside planar face as the Secondary Datum.

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SOLIDWORKS 2015

Exercise 2 Imported Geometry

5

Scope.

Select the pocket, notch pattern, and upper planar face. Click OK.

6

DimXpertManager.

Click the DimXpertManager and expand the features. Click Show annotation based tree to display the datums.

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Save and close all files.

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Exercise 2

SOLIDWORKS 2015

Imported Geometry

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Lesson 3 Adding Size and Location Dimensions

Upon successful completion of this lesson, you will be able to:

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Understand the use of special selection techniques.

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Manually create DimXpert annotations including datums, dimensions, and geometric tolerances.

I

Create a 2D PDF with DimXpert annotations.

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Lesson 3

SOLIDWORKS 2015

Adding Size and Location Dimensions

Special Selection Techniques

When creating datums, size dimensions, location dimensions, and geometric tolerance symbols, there are special, compound selection techniques that use multiple faces. These techniques are required because only faces can be selected. For example, if a virtual edge is required, it is generated as an intersection of faces.

Note

These selections were introduced in DimXpert Selections on page 18.

Compound Selections

Compound selection types include Compound Cylinders and Compound Planes. They are used to combine multiple face selections into a single feature.

Compound Cylinders

The Compound Cylinder selection can be used to select multiple coradial circular faces for a datum or as a selection for a Size Dimension. 1. Click Datum circular face.

and select a

2. Click Create Compound Cylinder and select all of the coradial faces.

3. Click OK and place the datum.

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SOLIDWORKS 2015

Lesson 3 Adding Size and Location Dimensions

Compound Planes

The Compound Plane selection can be used to select multiple coplanar faces for a datum or as a selection for a Size Dimension. 1. Click Datum

and click a planar face.

2. Click Create Compound Plane and select the coplanar faces.

3. Click OK and place the datum.

Note

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These parts can be found in the Lesson02\Case Study\Examples folder.

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Lesson 3

SOLIDWORKS 2015

Adding Size and Location Dimensions

Combining Dimensions

Combine a group of similar dimensions,

Note

When multiple faces are created by the same feature, such as a single fillet, they are generally combined automatically.

such as a set of fillet dimensions that share the same radius value, into a single dimension.

Use the following steps to combine dimensions. 1. Expand the features in the DimXpertManager. Select all of the dimensions to be combined. Or, graphically Control+select the dimensions.

2. Right-click Combine Dimension.

Combining Fillet Dimensions

Fillets and rounds may be combined automatically, but it depends on how the geometry was created. Consider a plate shaped part with rounded outer edges, some created using an extruded sketch that contains Sketch Fillet, others were created using a (solid) Fillet feature. When adding a Size Dimension, the faces resulting from the sketched geometry will require individual dimensions and they will not be combined. The dimensions resulting from solid fillet will be automatically combined. If using Auto Dimension Scheme, they will combine if they are selected together.

Note

46

The combined dimension can be broken down to the original dimensions using Break Combined Dimension.

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SOLIDWORKS 2015

Lesson 3 Adding Size and Location Dimensions

Dimensions Between Cylinders

Location dimensions created between cylindrical faces can create angular or linear dimensions.

Note

Cylindrical faces includes cylinders, holes, counterbores, and countersinks.

Angular Dimensions

1. Click Location Dimension . 2. Click the cylindrical faces and click Angular Dimension .

Linear Dimensions

1. Click Location Dimension . 2. Click the cylindrical faces and click Linear Dimension .

Note

The linear dimension can be adjusted using DimXpert Dimension Directions on page 49.

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Lesson 3

SOLIDWORKS 2015

Adding Size and Location Dimensions

Intersection Lines

Intersection Lines can be used to create location dimensions. These are used at virtual corners, where fillets or chamfers have removed the physical corner.

In this example, the virtual corner is used to create a location dimension between two filleted corners. Use the following steps to create intersect lines for a dimension. 1. Click Location Dimension

.

2. Click the planar face. 3. On the popup menu, click Create Intersection Line .

4. Click the upper planar face and click OK.

5. Repeat selections on the opposite side of the part and place the dimension.

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SOLIDWORKS 2015

Lesson 3 Adding Size and Location Dimensions

DimXpert Dimension Directions

DimXpert dimension between intersect lines have multiple direction options. The direction can be along the X, Y or Z axis, normal (default), or along a user defined direction. The user defined direction requires the selection of an edge for direction. I

Normal To

I

Along X

I

Along Y

I

User Defined

A selection to define the direction of the dimension is required.

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Lesson 3

SOLIDWORKS 2015

Adding Size and Location Dimensions

Intersection Lines for Edges

Intersection Lines are also used with a location dimension to dimension to an edge where actual model edges cannot be selected directly. 1. Click Location Dimension

. 2. Select the angled face and click Create Intersection Line .

3. Select the lower face and click OK.

The intersection line is created at the intersection. 4. Select the planar face as shown and place the dimension.

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Lesson 3 Adding Size and Location Dimensions

Intersection Circles

Intersection Circles are used with a size dimension to dimension to a

virtual circular edge. 1. Click Size Dimension . 2. Select the conical face and click Create Intersection Circle .

3. Select the planar face and click OK.

4. Place the dimension.

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Lesson 3

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Adding Size and Location Dimensions

Intersection Points

Intersection Points are also used with a location dimension to

dimension to an edge as actual model edges cannot be selected directly. 1. Click Location Dimension

. 2. Select the circular face and click Create Intersection Point .

3. Select the planar face. Click OK and a point is placed at the intersection.

4. Select the circular and planar faces to create another intersection point and place the dimension. The dimensions can be adjusted using DimXpert Dimension Directions on page 49.

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Lesson 3 Adding Size and Location Dimensions

Arc Conditions with Dimensions

Arc Conditions is a standard dimension properties tool for dimensions to cylindrical faces that also works with DimXpert annotations. It can set each dimension attachment to the Center, Minimum, or Maximum position. 1. Click Location Dimension . 2. Click the cylindrical face. and click Cylinder .

3. Click the cylindrical face. and place the dimension as shown.

4. Select the dimension and choose the Arc Condition.

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Lesson 3

SOLIDWORKS 2015

Adding Size and Location Dimensions

3D Note Options

3D Notes can have multiple

attachments and geometric tolerance symbols.

The attachment can be moved to another face or edge by dragging the arrow to a different face or edge.

Multiple attachments for a Note can be created by Control+dragging the arrow to an additional face or edge. Attachments can be deleted by clicking the arrow and pressing the Delete key.

Note

Geometric Tolerancing symbols can also be added to the note using

Add Symbol . the More symbols option opens a larger set of categories including Modifying Symbols.

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Lesson 3 Adding Size and Location Dimensions

Manually Creating DimXpert annotations

DimXpert annotations can be created manually using 3D annotations such as datums, size dimensions, location dimensions and geometric tolerances.

Note

The most efficient method may be the hybrid approach of using both automated (Auto Dimension Scheme on page 22) and manual methods to add 3D dimensions and annotations.

Adding Datums

Datum feature symbols (datums) can be added manually to faces of the model. It is created in the same way as the annotation datum symbol. Multiple datum sets can exist to create more than three datums.

Note

Datum names are case sensitive.

Where to Find It

I I

1

2

Menu: Tools, DimXpert, Datum CommandManager: SOLIDWORKS MBD > Datum

Open the part bracket single. Open the part bracket single from the Lesson03\Case Study\ Wheel assembly folder. Datums.

Click Datum and add the datums A, B and C as shown.

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Lesson 3

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Adding Size and Location Dimensions

3

Size dimension.

Click Size Dimension dimension as shown.

, select a hole, Pattern

and place the

For a review of Size Dimension, Size and Location Dimensions on page 33.

Note 4

Hole.

Add another Size Dimension. Select the upper hole, click Hole place the dimension as shown.

56

and

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SOLIDWORKS 2015

Lesson 3 Adding Size and Location Dimensions

5

Check status.

Click Show Tolerance Status . The color of the faces shows geometry in a variety of constraint states.

6

Dimension the base feature.

Add another size dimension between the B datum face and the selection. opposite, parallel face using the Create Width Feature Repeat the procedure to add another dimension between the C datum and the opposite face as shown.

Note

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For a review of selections, Special Selection Techniques on page 44.

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Adding Size and Location Dimensions

7

Size of boss.

Add another size dimension to the outer cylindrical face as shown.

Adding Geometric Tolerance Symbols

The Geometric Tolerance symbol can be added to a face or dimension of the model. It uses the same dialog as the annotation geometric tolerance symbol.

Where to Find It

I

CommandManager: SOLIDWORKS MBD >

I

Geometric Tolerance Menu: Tools, DimXpert, Geometric Tolerance

8

Geometric tolerance.

Click Geometric Tolerance datums as shown.

Note

58

and set the Symbol, Tolerance and

A datum name must exist before using it in a geometric tolerance symbol.

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Lesson 3 Adding Size and Location Dimensions

9

Place symbol.

Click the diameter dimension and OK. The geometric tolerance symbol is attached to the diameter dimension and is applied to all of the holes in the pattern.

Note

Rebuild may be necessary to see the addition of the symbol. 10 Additional geometric tolerances.

Repeat the procedure for the 32mm circular boss by creating the symbol and selecting the dimension to add it as shown. Do not click OK yet. For the final geometric tolerance symbol on the 15mm concentric hole, edit the dialog box and select the dimension as shown. Note

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To edit only the geometric tolerance symbol, right-click it and click Properties or double-click it.

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Adding Size and Location Dimensions

Position of the Geometric Tolerance

The geometric tolerance symbol can be below the dimension text or it can be dragged to other positions as shown. It can also be dragged back into position below the dimension text.

Recreating Basic Dimensions

Basic dimensions can be created automatically with the tolerance features if the Create basic dimensions option was selected. If not, they can be added after the fact for a Position feature. The basic dimensions can also be recreated after the fact using the position feature.

1. Expand the DimXpertManager and the Hole Pattern3 feature.

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Lesson 3 Adding Size and Location Dimensions

2. Right-click the Position1 feature and click Recreate basic dim.

11 DimXpertManager.

Change the DimXpertManager Tree Display to Show annotation based tree. The position features represent the holes and circular boss features. 12 Recreate basic dimensions.

Right-click the hole pattern position feature Position1 from the DimXpertManager and click Recreate basic dim. Three dimensions are added.

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Adding Size and Location Dimensions

13 Repeat.

Repeat the procedure of adding basic dimensions for the remaining two position features; the cylindrical boss and concentric hole. Dimensions and features are added.

Note

Some of the dimensions are duplicates. 14 Combine duplicates.

Combine the duplicate 65mm dimensions as shown. See Combining Dimensions on page 46 for more information.

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Lesson 3 Adding Size and Location Dimensions

15 Hiding DimXpert annotations. Right-click the Annotations folder and clear Show DimXpert Annotations. Click Show Tolerance Status .

DimXpert Annotations and 2D Drawings

The dimensions and annotations generated when dimension schemes are created are considered DimXpert Annotations. These annotations, combined with the planes that hold them, are very useful when creating 2D drawing views.

1

2

Open the part DimXpert_Annotations. Open the part DimXpert_Annotations from the Lesson03\ Case Study folder. Dimension scheme.

The part has the existing dimension scheme shown below.

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Lesson 3

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Adding Size and Location Dimensions

The annotation views *Right and *Front are found in the Annotations folder of the FeatureManager design tree. All the dimensions created in the dimension scheme are automatically organized in one of theses annotation views based on their orientation.

Annotation Views

Drawing views use the annotation views and the dimensions organized in them. They are marked in the View Palette with a prefix (A). This topic will be discussed in detail in Lesson 5: Annotation Views. 3

Make drawing.

Click File, Make Drawing from Part. and select the A (ANSI) Landscape drawing template. Select Import Annotations, DimXpert Annotations and Include items from hidden features.

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Lesson 3 Adding Size and Location Dimensions

4

View.

Drag and drop the (A) Front (annotation) view from the View Palette to the drawing sheet.

To include all annotations that may be in annotation views other than the default Front, Top and Right, select Include items from hidden features on the View Palette. If this option is not selected, the annotations for the back side boss and hole pattern would not appear.

Note

5

Create PDF.

Click Save As and select the type Adobe Portable Document Format (*.pdf). Name the file 2D PDF.

6

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Save and close all files.

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Exercise 3

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Automatic and Manual Methods 1

Exercise 3: Automatic and Manual Methods 1

Create DimXpert datums and annotations using automatic and manual methods. This lab reinforces the following skills: I I I

1

2

Auto Dimension Scheme on page 22. Special Selection Techniques on page 44. Manually Creating DimXpert annotations on page 55.

Open the part base. Open the part base from the Lesson03\Exercises folder.

Datums.

Click Auto Dimension Scheme and set the Primary, Secondary and Tertiary (using Create width feature) datums as shown.

3

Compound.

Under Scope, and select these two planes using the Create compound plane selection technique.

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Exercise 3 Automatic and Manual Methods 1

4

Width.

Select these two planes using the Create Width Features selection technique.

5

Plane.

Select the plane and click OK.

6

Move dimensions.

Move the dimensions as shown.

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Exercise 3

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Automatic and Manual Methods 1

7

Length.

Add a Size Dimension using the Create Width Feature selection technique to create the length dimension shown.

8

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Save and close all files.

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SOLIDWORKS 2015

Exercise 4 Automatic and Manual Methods 2

Exercise 4: Automatic and Manual Methods 2

Create DimXpert datums and annotations using automatic and manual methods. This lab reinforces the following skills: I I I

1

Auto Dimension Scheme on page 22. Special Selection Techniques on page 44. Manually Creating DimXpert annotations on page 55.

Open the part jaws.

Open the part jaws from the Lesson03\Exercises folder. 2

Datums.

Click Auto Dimension Scheme and set the Primary (using Create compound plane), Secondary and Tertiary (using Create width feature) datums as shown below.

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Exercise 4

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Automatic and Manual Methods 2

3

Scope.

Under Scope, select the three planar faces as shown. Click OK.

4

Status.

View the tolerance status.

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Exercise 4 Automatic and Manual Methods 2

5

Location dimension.

Create a Location Dimension using the Create Intersection Lines selection technique and a planar face as shown. Check the status.

6

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Save and close all files.

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Exercise 5

SOLIDWORKS 2015

Using Selection Techniques

Exercise 5: Using Selection Techniques

Create DimXpert datums and annotations using selection techniques. This lab reinforces the following skills: I I I

1

2

Auto Dimension Scheme on page 22. Special Selection Techniques on page 44. Manually Creating DimXpert annotations on page 55.

Open the part Sheet Metal. Open the part Sheet Metal from the Lesson03\Exercises folder.

Datums and dimensions.

Use Auto Dimension Scheme to create the datums (primary = bottom face, secondary = slot). For Scope, select the parallel inside face.

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Exercise 5 Using Selection Techniques

3

Location dimensions.

Using Location Dimensions with Create Intersection Line and a planar face, add the dimensions as shown.

4

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Save and close all files.

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Exercise 5

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Using Selection Techniques

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Lesson 4 Turned Parts

Upon successful completion of this lesson, you will be able to:

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Use DimXpert with a turned part.

I

Create plus and minus style tolerances.

I

Understand tolerance rule checking.

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Lesson 4

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Turned Parts

Turned Parts

The DimXpert software has been seen to generate a toleranced model with features and the associated annotations created from SOLIDWORKS geometry. The Turned option in the auto dimension scheme tool is used to tailor the annotations and dimensions for a turned style of part with diameters in place of lengths. The tolerance type Plus and Minus, with Linear and Polar options, is also introduced. 1

2

Open the part Turned with pattern. Open the part Turned with pattern from the Lesson04\Case Study folder.

Turned.

Click Auto Dimension Scheme and click Turned and Geometric. Select the Primary and Secondary datum faces as shown.

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Lesson 4 Turned Parts

3

Scope.

Click Selected features. Under Scope, select the five faces, including a hole pattern, as shown. Click OK.

4

Move annotations.

Move the 3D annotations and dimensions as shown.

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Turned Parts

5

Tree display.

Right-click the DimXpertManager and click Tree display, Show annotations based tree.

6

Position feature.

Right-click the position feature that is associated with the hole pattern and click Recreate basic dim.

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SOLIDWORKS 2015

Lesson 4 Turned Parts

Deleting Dimensions and Symbols

Individual DimXpert annotations can be deleted manually using the Delete key or all at once by deleting the scheme using Delete All Tolerances. many of the dimensions, geometric tolerances, and datums are combined. If the geometric tolerance is deleted from the dimension, the dimension remains.

If the dimension is deleted, the geometric tolerance remains.

The same is true for datums. If the geometric tolerance is deleted, the datum remains.

Deleting the Tolerance Scheme

The Tolerance Scheme includes all of the DimXpert annotations and features. The name is listed after the part name in the DimXpertManager. For example, .

Where to Find It

I

7

Menu: Tools, DimXpert, Delete All Tolerances

Delete scheme.

Click Delete All Tolerances and click Yes. The DimXpertManager is cleared of the scheme and all features, dimensions, and tolerances.

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Lesson 4

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Turned Parts

Using Plus and Minus

The Tolerance option Plus and Minus can be used to create toleranced dimensions without tolerancing. The Pattern Dimensioning option allows for Linear or Polar style dimensioning.

8

Plus and minus.

Click Auto Dimension Scheme, Turned, Plus and Minus and Pattern Dimensioning Linear. Select the Primary and Secondary planes as in step 3 on page 77. For the Scope, click Selected features and select the hole pattern. Click OK.

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Lesson 4 Turned Parts

9

Delete scheme.

Click Delete All Tolerances

and click Yes.

10 Polar. Click Auto Dimension Scheme, Turned, Plus and Minus and Pattern Dimensioning Polar. Select the Primary and Secondary planes as in step 3 on page 77.

For the Scope, click Selected features and select the hole pattern. Click OK.

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Lesson 4

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Turned Parts

Tolerance Rule Checking

The DimXpert tool not only creates 3D dimensions and tolerance features but it also automatically runs Tolerance Rule Checking. For example, if a cylindrical symbol is used with a non-cylindrical feature, warnings will appear in the DimXpertManager and the feature in question will appear in the warning color.

Note

To change the warning color, click Tools, Options, Colors, Dimensions, Danging color.

The warnings will also appear in the DimXpertManager and can be viewed using the What’s Wrong? technique. However, the warnings do not appear in the FeatureManager design tree.

Note

An geometric tolerance or datum feature that is attached to a dimension may trigger the warning even though the dimension itself is correct. In this section, some of the most common conditions will be introduced and repaired. I I I I

82

Duplicate Datums Cylindrical Position Collinear Datums Non-Coaxial Features

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SOLIDWORKS 2015

Lesson 4 Turned Parts

Duplicate Datums

The Duplicate Datums warning appears when two or more datum features use the same letter. The solution is to edit a datum and change the letter. 1

2

Open the part duplicate datum identifier. Open the part duplicate datum identifier from the Lesson04\ Case Study\Rule Checking folder. Conflict.

There are two datum features of the same name displayed in the warning color.

3

Rename datum.

Click the upper datum and change A to B. Click OK. The colors change with the repair.

Note

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Rebuild may be needed to see the warning.

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Lesson 4

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Turned Parts

Cylindrical Position

The Cylindrical Position warning appears when a diameter symbol is used inappropriately, usually a non-cylindrical feature. The solution is to edit the geometric tolerance symbol and remove the diameter symbol. 4

5

Open the part cylindrical position applied. Open the part cylindrical position applied from the Lesson04\ Case Study\Rule Checking folder. The geometric tolerance symbol attached to the dimension is displayed in the warning color.

Dimension.

Click on the dimension. The dimension is referenced to the highlighted rectangular notch feature.

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Lesson 4 Turned Parts

6

Edit the geometric tolerance.

Double-click the geometric tolerance symbol. The warning, Cylindrical position applied to feature Notch1, refers to the diameter symbol that is applied to a rectangular notch feature.

7

Edit symbol.

Click in Tolerance 1 and click the Diameter symbol to clear it. Click OK. The color changes with the repair.

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Lesson 4

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Turned Parts

Collinear Datums

The Collinear Datums warning occurs when two cylindrical datums share the same axis. The solution is to delete one of the datums and remove references to the deleted datum. 8

9

Open the part tertiary collinear primary. Open the part tertiary collinear primary from the Lesson04\ Case Study\Rule Checking folder.

DimXpertManager.

Another way to investigate an warning is to see it in the DimXpertManager tree. Open the DimXpertManager and expand the Hole Pattern1 feature. Float the cursor over the Position1 feature to see the message.

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Lesson 4 Turned Parts

10 Show tree.

Right-click the top level feature and click Tree Display, Show annotations based tree. Expand the datum features A and C to see the associated features Simple Hole1 and Boss1.

11 Delete,

Graphically select just the datum C. Click the Delete key.

12 Edit the geometric tolerance.

Double-click the geometric tolerance symbol. The message indicates that datum C is not defined; in fact it was just deleted. Remove the reference to datum C and click OK. Click Rebuild.

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Turned Parts

Non-Coaxial Features

The Non-Coaxial Features warning occurs when two cylindrical features do not share the same axis have tolerancing symbols that specifies coaxial. The solution is to either: I I

Change the tolerancing symbols, or Edit the geometry and make the cylinders coaxial.

In this example, the geometry will be edited. 13 Open the part tolerance feature runout coaxial. Open the part tolerance feature runout coaxial from the Lesson04\Case Study\ Rule Checking folder.

14 What’s Wrong.

Click the DimXpertManager and expand the Boss2 feature. Rightclick the CircularRunout2 feature and click What’s Wrong? to see the details.

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Lesson 4 Turned Parts

15 Edit sketch.

Switch to the FeatureManager and edit the sketch of the BossExtrude2 feature as shown. Exit the sketch.

16 Save and close all files.

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Exercise 6

SOLIDWORKS 2015

Turned Parts 1

Exercise 6: Turned Parts 1

Create DimXpert annotations for this part. This lab reinforces the following skills: I

Turned Parts on page 76.

1

Open the part Turned. Open the part Turned from the Lesson04\Exercises folder.

2

Auto Dimension Scheme. Click Auto Dimension Scheme

3

, click Turned and Geometric.

Datum selections.

For the Primary Datum, select the large cylinder as a boss. For the Secondary Datum, select the small cut as a hole.

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Exercise 6 Turned Parts 1

4

Face selections.

Click selected features and select the 5 faces as shown. Click OK.

5

Move.

Move the 3D annotations and dimensions as shown.

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Exercise 6

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Turned Parts 1

6

Ends.

Note that the flat on the cylinder has a linear dimension from the center and the end face of the large diameter cylinder is under defined. These will be modified.

7

Arc condition.

Click the linear dimension to the flat (3.1mm). In the Dimension properties, click the Leaders tab and click Min. Click OK.

8

Size dimension.

Add a Size Dimension to the large diameter cylinder as shown.

9

92

Save and close all files.

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SOLIDWORKS 2015

Exercise 7 Turned Parts 2

Exercise 7: Turned Parts 2

Create DimXpert annotations for this part. This lab reinforces the following skills: I I

1

2

Adding Geometric Tolerance Symbols on page 58. Turned Parts on page 76.

Open the part turned_cover_plate. Open the part turned_cover_plate from the Lesson04\Exercises folder.

Datums.

Click Auto Dimension Scheme and click Turned and Geometric. Select the Primary (rear planar face) and Secondary (center cylindrical face) Datums.

3

Scope.

For the scope, select the hole pattern and three additional faces as shown.

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Exercise 7

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Turned Parts 2

4

Status.

Check the tolerance status and move the dimensions.

5

Size dimensions.

Click Size Dimension and add dimensions to the two cylindrical faces as shown. Both cylinders remain partially defined.

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Exercise 7 Turned Parts 2

6

Geometric tolerance.

Click Geometric Tolerance and add a symbol to the 75mm cylindrical face, and dimension, as shown. Repeat for the 25mm cylindrical face. Both cylinders are now fully defined.

7

Fillet.

Click Size Dimension and add a dimension to the fillet face as shown.

8

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Save and close all files.

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Exercise 8

SOLIDWORKS 2015

Rule Checking

Exercise 8: Rule Checking

Repair DimXpert annotations for this part. This lab reinforces the following skills: I

1

Tolerance Rule Checking on page 82.

Open the part Repairs.

Open the part Repairs from the Lesson04\Exercises folder.

2

DimXpertManager.

Expand the tree as shown.

3

Error.

Right-click the Perpendicularity1 feature and click What’s Wrong? The message indicates an issue with the geometric tolerance symbol. Warning: The tolerance feature for Perpendicularity1 is not perpendicular to the primary y1 datum.

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Exercise 8 Rule Checking

4

Repair geometric tolerance.

Edit the geometric tolerance symbol and change the Primary datum from B to A.

5

Float over feature.

float the cursor over the CounterBore1 feature as shown. The message indicates that the counter bore feature does not exist. This occurs because the hole features are not concentric.

6

Edit sketch.

Click the FeatureManager Design Tree tab. Edit the sketch Sketch4 and make the circle concentric with the circular edge as shown. Exit the sketch and rebuild the part.

7

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Save and close all files.

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Exercise 8

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Rule Checking

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Lesson 5 Annotation Views

Upon successful completion of this lesson, you will be able to:

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Understand annotation views.

I

Manipulate annotation views.

I

Reassign dimensions to different annotation views.

I

Create new annotation views.

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Annotation Views

Annotation Views

Annotation Views are used to organize annotations

that share the same orientation. Although much of the creation, organization, and naming of annotation views is automatic, annotation views can be edited and new annotation views can be created. The individual annotations can also be moved between annotation views (for more information, see Reassigning Annotations on page 108). Standard annotation views also imply orientations. For example, the *Top annotation view is associated with the Top view orientation. for

more information, see Orienting an Annotation View on page 105. Why Are Annotation Views Important?

Annotation views are critical to the creation of 3D Views (see Lesson 6: Capturing 3D Views), as they are used to define which annotations appear in each 3D View. The 3D views are in turn used to create the final output of SOLIDWORKS Model Based Definition: 3D PDF and eDrawing files. Consider a part that contains annotations created using the DimXpert tools. With all the annotation views visible, it may not be obvious how the annotation views are organized. If the annotations are organized into multiple annotation views, more possible combinations are available with 3D views.

Types of Annotation Views

Annotation views fall into two main categories based on the annotations that they contain: Orthographic and specialty types that are used to organize notes and other dimensions.

Note

Parts with features already have dimensions in annotation views. These are the Feature Dimensions that are created along with the sketches and features. Reference Dimensions may also be included.

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Lesson 5 Annotation Views

Orthographic Annotation Views

Annotations and dimensions are automatically sorted and placed into orthographic annotation views such as *Top, *Bottom, *Front, *Back, *Right and *Left. These are associated with the view orientations of the same names. For example, for annotations parallel to the Front plane of the model, a *Front annotation view will be created and all of the annotations using that same orientation will be organized there. They are all oriented parallel to the Front plane.

Note

Each of the annotations is associated with only one annotation view.

Specialty Annotation Views

The specialty annotation views include both Notes Area and Unassigned Items by default. I

I

Notes Area - An annotation view oriented flat to the screen. Notes annotations without leaders are commonly located in this annotation view. Unassigned Items - Annotation view used to organize annotations that do not exist in any other annotation view. Feature and reference dimensions are often organized in this annotation view.

Other specialty views are created automatically based on the geometry or manually by the user (for more information, see Adding a New Annotation View on page 113). For example, the dimensions parallel to the angled face generate a new annotation view of the form Annotation View N.

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Annotation Views

1

2

Open the part Ortho. Open the part Ortho from the Lesson05\Case Study folder. This part will be used to demonstrate manipulation of annotation views.

DimXpertManager.

Click DimXpertManager to view the tree. Expand the Annotations folder. In this example, the Annotations folder contains six annotation views. Some information can be gathered from looking at the Annotations folder: I I

102

The active annotation view is *Top, as indicated by the arrow . All of the annotation views are currently visible, as indicated by the filled icons .

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SOLIDWORKS 2015

Lesson 5 Annotation Views

Manipulating Annotation Views

Annotation views can be manipulated to control the visibility, activation, and orientation of tolerances and dimensions. This is a critical component in designing 3D views.

Hiding and Showing Annotation Views

Annotation views can be hidden or shown to control the visibility of the annotations organized in them. By hiding an annotation view, all of the dimensions and tolerances associated with that annotation view are hidden.

Where to Find It

I

3

Shortcut Menu: Right-click an annotation view and click Hide.

Hide all annotation views.

In the annotations folder, click Notes Area and Shift+click *Bottom and right-click Hide to hide all annotation views and related dimensions and tolerances except the active one. Only the active annotation view *Top with the associated annotations is shown. For more information on the active annotation view, see Activating an Annotation View on page 104.

Note

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The selections may not highlight but they will be selected. Standard Shift+click or Ctrl+click selection methods can be used.

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Annotation Views

Activating an Annotation View

Like configurations, one annotation view is always active. The active annotation view is indicated with a yellow arrow. When an annotation view is active: I I

The associated annotations are visible. Manually added dimensions and annotations will be added to it.

Note

In the above example, the note is added with the annotation view *Front active. The orientation reflects the Front plane.

Where to Find It

I I

4

Shortcut Menu: Double-click an annotation view in the Annotations folder Shortcut Menu: Right-click an annotation view and click Activate

Activate.

Currently *Top is the active view. Double-click the *Front annotation view to make it active. Only annotations associated with the *Front annotation view are visible.

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Lesson 5 Annotation Views

Double-clicking an annotation view may generate a message asking whether the feature dimensions should be made visible.

Note

Click No and optionally Don’t show again. Orienting an Annotation View

Annotation view dimensions are visible as long as the annotation view is shown, regardless of view orientation (expect when using Dynamic Annotation Views on page 106). You can change the view orientation to match that of the annotation view while also making it active. Although the planes are parallel, there is a difference in the orientation of an annotation in the *Top annotation view and one in the *Bottom.

Where to Find It

I

Shortcut Menu: Right-click the active annotation view and click Orient

I

Shortcut Menu: Right-click an annotation view and click Activate and Reorient

5

Activate and orient.

Right-click the *Top annotation view and click Activate and Reorient. The *Top becomes the active annotation view and the orientation matches it.

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Lesson 5

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Annotation Views

6

Switch orientations.

Right-click the *Bottom annotation view and click Activate and Reorient.

Dynamic Annotation Views

The contents of annotation views can be viewed dynamically using the Dynamic Annotation Views tool. It provides an easier way of showing the contents of each annotation view; much easier than using activate and reorient.

Note

If the orientation does not come close to matching an annotation view orientation, transparent dimensions shown.

Introducing: Dynamic Annotation Views

The Dynamic Annotation Views tool allows you to view the 3D dimensions annotations while rotating the view orientation. When using the tool, the dimensions are only visible as they approach or match the view orientation of an annotation view. Also, the arrow pointer will change as the dimensions of an annotation view appear.

Where to Find It

I

CommandManager: SOLIDWORKS MBD > Dynamic Annotation Views

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7

Heads-up View Toolbar: Dynamic Annotation Views

Show.

In the annotations folder, click Notes Area and Shift+click *Bottom. Right-click Show to view all of the annotations. Change the view orientation to an isometric view.

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8

Dynamic annotation views.

Click Dynamic Annotation Views and use the middle mouse button to rotate the view. The hidden dimensions and tolerances become more visible as you drag the mouse.

9

Rotate.

Rotating close to the Top view orientation makes the *Top annotation view annotations visible. The arrow moves to point at the *Top view.

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Annotation Views

10 Rotate to Bottom.

Rotating close to the Bottom view orientation makes the *Bottom annotation view visible and active.

Reassigning Annotations

Existing annotations can be reassigned to a different annotation view. this effectively moves it the annotation view from one annotation view to another.

Why Reassign?

Placing dimensions and tolerances in the proper annotation view is critical to the creation of 3D Views (see Lesson 6: Capturing 3D Views) that are in turn used to create the final output of SOLIDWORKS Model Based Definition, 3D PDF and eDrawing files.

Where to Find It

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Right-click an annotation and click Select Annotation View Click a 3D annotation, press the ~ (tilde) key and click an annotation view

11 Reassign annotation.

The single 3D annotation in the *Bottom annotation view points to an edge that is not visible in the bottom view. It would be better seen in the *Top annotations folder. Right-click the annotation and click Select Annotation View (*Bottom).

Click *Top from the list and the annotation disappears.

Note

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If there are multiple annotation view options, float over the names in the list to preview the potential orientation changes.

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12 Change orientation. Change to the *Top annotation view. The annotation now appears in the

annotation view.

Other Annotation Views

Annotation views are created based on the geometry of the part. They can also be user created to suit the needs of viewing the dimensions. Two types are automatically created with every part and assembly: they are the Notes Area and Unassigned Items. Additionally, other Annotation views are created as needed based on the geometry of the part. these are used to organize annotations on a plane other than the standard orthographic planes. The associated views are oriented normal to the planes. A sample name is Annotation View 1.

Note

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In this example, there are no annotations in the Notes Area or the Unassigned Items folders. Due to the shape of the part, no additional annotations views were created.

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Annotation Views

1

2

Open the part Other. Open the part Other from the Lesson05\Case Study folder.

DimXpertManager.

Click DimXpertManager to view the tree. Expand the Annotations folder. The Annotations folder contains some additional annotation views named Annotation View 2 and Annotation View 4. These annotation views have automatically been created for dimensions and tolerances on the oblique planes of the model.

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Lesson 5 Annotation Views

3

Dimension by annotation view.

The current arrangement of annotation views and dimensions is shown in these images. Use Dynamic Annotation Views and rotate to each to see the dimensions and view or click View Orientation annotations. *Front

*Top

Annotation View 2

Annotation View 4

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Annotation Views

4

Move.

Click Dynamic Annotation Views . Click the 45mm dimension as shown. Press the ~ (tilde) key and click Annotation View 4.

5

Rotate.

Rotate close to Annotation View 4. The 3D annotation has been moved. Clear Dynamic Annotation Views .

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Lesson 5 Annotation Views

Adding a New Annotation View

Annotation views can be added when another place to organize dimensions and annotations is needed. Additional annotation views are useful in separating the dimensions and annotations when creating 3D views. Consider a part where there are annotation views *Right and *Left, they differ in the direction of the view plane. Therefore, the dimensions in the annotation view *Right are not visible in annotation view *Left. A copy of a *Right annotation view would perform the same function.

Where to Find It

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Right-click the annotations folder and click Insert Annotation View

6

Hide DimXpert annotations.

The DimXpert annotations can be temporarily hidden. Right-click the Annotation folder and clear Show DimXpert Annotations. 7

New view.

Right-click the Annotations folder and click Insert Annotation View. Click Selection and select the face as shown.

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Annotation Views

8

Direction.

Under Horizontal Direction, click the short edge as shown.

9

Orient.

Click Orient View to preview the results and click OK. Right-click the Annotation folder and click Show DimXpert Annotations.

10 Rename.

Click the new annotation view and press F2. Rename the annotation view to Detail A.

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11 Reassign.

Activate and reorient Annotation View 2. Reassign these annotations to Detail A.

‘ 12 Reorient.

Activate and reorient Detail A. Rebuild and drag the annotations.

Note

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To edit an existing annotation view, right-click an annotation view and click Edit Annotation View.

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Annotation Views

Using Configurations

Multiple configurations can be used to create variations of parts and assemblies. When a tolerance scheme is created, it is created for the active configuration only. Other configurations can have tolerance schemes, but they must be created separately or copied from and existing scheme using Copy Scheme. In this Lesson 6: example, an alternate configuration will be created. The configuration will be used to create a 3D View in Lesson 6: Capturing 3D Views. 1

2

Open the part Configurations. Open the part Configurations from the Lesson05\Case Study folder.

Configuration.

Create a new configuration Extend as shown.

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Lesson 5 Annotation Views

3

Changed values.

Change the values of these dimensions to 2.5” and 6” for This Configuration only.

4

DimXpertManager.

Click the DimXpertManager tab. For the Extend configuration, the DimXpertManager It contains no DimXpert annotations. Change to the Default configuration and check the DimXpertManager. It retains the DimXpert annotations created with the Default configuration.

5

Active configuration.

Make the Extend configuration active and click the DimXpertManager.

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Annotation Views

Copy Scheme

Copy Scheme is used to generate a scheme by coping from a source scheme. The copied scheme includes all of the DimXpert annotations and features from the source. It is generally used when multiple configurations are created.

Note

Only the entire scheme from a different configuration can be copied.

Where to Find It

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6

CommandManager: SOLIDWORKS MBD > Copy Scheme DimXpertManager: Click Copy Scheme

Copy Scheme.

Click Copy Scheme and use the default Scheme Name. Type extend configuration as the Description. Select Default as the source configuration and click OK. All of the contents of the Default DimXpertManager are copied to the new configuration.

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Lesson 5 Annotation Views

‘Hiding’ Annotations

DimXpert features and annotations can be suppressed or deleted, however doing so will cause errors and warnings. To avoid this, ‘hide’ annotations by reassigning them to a different annotation view and hiding that annotation view. The Unassigned Items annotation view can be used in this way. 1. 2. 3. 4. 5.

Modifying Dimension Attachments

Create a new configuration. Make the new configuration active. Copy the scheme. Hide the Unassigned Items annotation view. Reassign dimensions to the Unassigned Items annotation view.

To make dimensions more readable, the dimensions created using the DimXpert can be modified to change the attachment points, arrowheads and extension lines. The readability will make for better 3D views.

7

Change attachment point.

Attachment points can be dragged to model edges or faces. Flip the model over. Select the 1.125 diameter dimension with datum. Drag the endpoint to the circular edge of the hole and drop it as shown.

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Annotation Views

8

Change arrowhead.

This diameter dimensions has a dot arrowhead that is difficult to see. Select the 1.250 diameter dimension and click the Leaders tab in the Dimension PropertyManager. Select a filled arrowhead style and click OK. Also, change the attachment point to the circular edge as shown.

9

Extension lines.

Extension lines do not always attach to the actual edges. Select the 4.500 linear dimension and reattach the extension line to the lower circular edge as shown.

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Lesson 5 Annotation Views

10 Another extension line. Switch to the Default configuration. Move the extension line of the 1.625 dimension to the circular edge as shown.

11 Save and close all files.

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Annotation Views

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Lesson 6 Capturing 3D Views

Upon successful completion of this lesson, you will be able to:

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Create 3D views for parts.

I

Create 3D views for assemblies.

I

Create a broken view.

I

Make use of feature and reference dimensions.

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Capturing 3D Views

Capturing 3D Views

Capture 3D Views is used to record the PMI; view, configuration, display state, and visible annotation views to create a 3D View. The 3D

view is saved under a unique name and is used to create a 3D PDF or an eDrawings file. The 3D Views tab is used to create the and publish the 3D Views.

The PMI saved by the 3D view includes information that was listed in Lesson 1: What is SOLIDWORKS MBD? and has been discussed in the preceding lessons: I I I I I I I I I I

View Configurations Display States Custom Properties Exploded Views Tables Annotations Reference Dimensions DimXpert Annotations Annotation Views

Note

View includes the orientation, display style, zoom, and scroll.

Simulating Drawing Views

Configurations, model break view, and the section view tool can be used to simulate familiar types of 2D drawing views such as detail views, crop views, section views, and broken-out sections.

Where to Find It

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CommandManager: SOLIDWORKS MBD > Capture 3D View Tab: At the bottom of the screen, click the 3D Views tab and Capture 3D View

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Lesson 6 Capturing 3D Views

3D Views for Parts

Create 3D views of a part using view orientations, selected annotation views, section views and configurations. The 3D views are used as PMI for publishing a 3D PDF or an eDrawings file.

3D View Area

1 2

Completed 3D Views

Open the part 3D Views. Open the part 3D Views from the Lesson06\Case Study folder. Move dimensions.

Move the dimensions and tolerances to increase readability.

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Capturing 3D Views

3

Annotations view.

Show all of the annotation views they are not shown already. Expand the Annotations folder and double-click the *Front annotation view to make it active. 4

Tab.

Click the 3D Views tab. The 3D views options are stored in the 3D Views tab in the lower left corner of

the SOLIDWORKS window. 5

Capture 3D view.

The first 3D view will be an Isometric view orientation with all of the DimXpert annotations visible. Click Capture 3D View Views tab.

. This opens the 3D

Type ALL as the 3D View Name and select all of the annotation views. Do not change the Configuration and Display State settings. Click OK.

6

Preview.

A preview of the completed 3D view appears in the bottom pane. Additional 3D views will be added to the right of the current one. This is the first saved 3D view. Additional 3D views will be stored horizontally to the right of this one.

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Lesson 6 Capturing 3D Views

7

Change view orientation.

Activate and reorient to the Front annotation view and clean up the positions of the dimensions and tolerances as shown.

This is they will appear in the final 3D PDF or eDrawings file.

Note 8

3D view Front.

Click Capture 3D View . Type FRONT as the 3D View Name. Clear all of the annotation views except the active annotation view *Front. Click OK.

9

Open a 3D view.

The next 3D view will be a version of the first 3D view. Double-click the 3D view ALL and adjust the orientation slightly as shown.

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Capturing 3D Views

10 Activate annotation view. Expand the Annotations folder and double-click the *Top annotation

view to make it active. Note

If a message asks to turn feature dimensions on, click No.

Using Section Views

Section Views can create ‘section’ and ‘cutaway’ views without the

extra work of creating cuts and configurations. In this example the Zonal method will be used.

Note

The cuts can be made with standard planes or a selected planar face.

Where to Find It

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CommandManager: SOLIDWORKS MBD > Section View Heads-up View Toolbar: Section View

11 Section view. Click Section View and click the Section Method Zonal. Use the following planes at their

default positions. For Section 1, click the Front plane. For Section 2, click the Top plane. For Section 3, click the Right plane.

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Lesson 6 Capturing 3D Views

12 Select zone. Click in Zones selected to be sectioned, select the zone shown and click OK.

13 3D view. Click Capture 3D View

and clear all of the annotation views except the active *Top. Name the SECTION and click OK.

Note

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The color of the cut faces can be edited using Section View and Edit Color, Show section cap, and Keep cap color.

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Capturing 3D Views

14 Test 3D views.

Double-click each 3D view preview to test it.

Note

3D views can be edited, renamed or deleted by right-clicking the preview and clicking Recapture View, Rename, or Delete.

Dimension Size in PDF

The size of the annotations that you see in the graphics area may be different than what you will see in the 3D PDF file. In order to verify the size that will appear in the completed PDF, right-click the Annotations folder and click Details. Clear Always display text at the same size and click OK.

The difference between Always display text at the same size clicked (below left) and cleared (right) can be significant.

Note

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The setting should be cleared before 3D views are captured.

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Lesson 6 Capturing 3D Views

Using Configurations and Display States in 3D Views

Configurations can be used along with the other variables like the view orientation and the visibility of annotation views to capture 3D views.

Note

Display states can also be used to enhance the appearance of parts and assemblies in 3D views.

In this example configurations will used to show a different size version of the part.

15 Configuration 3D view.

Double-click the 3D view ALL. Click Capture 3D View . Name the CONFIG and select the Configuration Extend. Show all of the annotation views. Click OK.

Note

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The Update previews button is used to update the previews of 3D views that have been changed after they were created.

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Capturing 3D Views

3D Views for Assemblies

Create 3D views of an assembly using configurations, display states, and bill of materials tables. The 3D views are used as PMI for publishing a 3D PDF or an eDrawings file. Assemblies cannot use the DimXpert tools, but they can use reference dimensions. For more information, see Reference Dimensions and Annotations on page 139.

BOM

The 3D Tools used with parts are also available for assemblies. See 3D Tools on page 160 for more information.

Note

1

Note

132

Open the assembly Hex Set. Open the assembly Hex Set from the Lesson06\Case Study\ Assembly PDF folder. The assembly includes multiple display states, an exploded view, and a hidden bill of materials.

The bill of materials table is hidden so that it does not appear in the 3D views. It will be used in the final step Publishing an Assembly to a PDF on page 167.

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Lesson 6 Capturing 3D Views

2

Capture.

Click Capture 3D View. Type FULL as the 3D View Name, select the Configuration ANSI and the Display State ANSI_Display State-1. Click OK.

3

Exploded view.

Click Capture 3D View. Type EXPLODED as the 3D View Name, select the Configuration ExplView1 and the Display State ANSI_Display State-1. Click OK.

4

Additional 3D View.

Double-click the FULL 3D view. Click Capture 3D View. Type OPEN as the 3D View Name, select the Configuration ANSI and the Display State Open. Click OK.

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Capturing 3D Views

5

Test 3D views.

Double-click each 3D view preview to test it.

Breaking Views

Broken views can be created in parts and assemblies using Model Break View. The tool ‘breaks’ the geometry using one or more Alignment planes. The break shortens the model, creates a gap, and assigns a break Style to the geometry broken by the planes. In this example, a weldment part using structural steel shapes will be broken.

Model Break Styles

134

The Model Break Styles determine the appearance of the break faces. The Pipe Break is specifically designed for cylindrical sections. Straight Break

Zig-Zag Break

Pipe Break

Single Zig-Zag Break

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Lesson 6 Capturing 3D Views

Model Break Methods

The Model Break Methods determine how the breaks appear when multiple bodies are crossed by the plane. Continuous Break applies the break to each body; Individual Break applies a single break across single or multiple bodies. Continuous Break

Model Break Properties

Individual Break

The Model break properties include the settings that determine the Gap distance, the Shape Intensity and the rotation Angle of the section. Gap

Shape Intensity

Angle

Where to Find It

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CommandManager: SOLIDWORKS MBD > Model Break View Menu: Insert, Model Break View

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Capturing 3D Views

1

2

Open the part Support. Open the part Support from the Lesson06\Case Study folder.

Model break view.

Click Model Break View plane.

136

. Click the Right

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Lesson 6 Capturing 3D Views

3

Adjust.

Click Preview and drag the planes using the arrows. Use the visual intersection of the planes and transparency to locate the planes just off the angled brace members.

4

Break.

Click Apply to create the break. 5

Styles.

Click the Styles tab and select the Single Zig-Zag Break style with the Individual Break method. Click OK.

Using a Model Break View in a 3D View

The Model Break View feature is stored under the current configuration in the ConfigurationManager. It can be used just like an exploded view; as a configuration selection.

Note

Right-click the feature and click Hide Model Break View or Show Model Break View to hide or show the feature. Right-click the feature and Edit Feature to edit it. See Using Configurations and Display States in 3D Views on page 131 for more information.

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Capturing 3D Views

Dimensions and Model Break Views

Dimensions that cross the Model Break View planes in a part are automatically shown as broken dimensions.

Using Feature and Reference Dimensions

Many parts will have Feature and Reference dimensions and annotations in addition to any DimXpert annotations that are created. These dimensions and annotations can also be used to enhance 3D views. DimXpert Dimension

Sketch Dimension

Feature Dimension

Reference Dimension

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Lesson 6 Capturing 3D Views

DimXpert Annotations

DimXpert annotations, like those created in Lesson 2: Using DimXpert and Lesson 3: Adding Size and Location Dimensions, are visible as they are created by default. They must follow standards. Dimensions and annotations are magenta. Click Show DimXpert Annotations to hide or show all of the DimXpert annotations.

Reference Dimensions and Annotations

Reference Dimensions and Annotations are created manually in

Hiding Reference Dimensions and Annotations

Reference dimensions and annotations can be hidden or shown as a group.

sketches or in 3D space. They can be used to create any dimension or annotation. Dimensions are gray, annotations are black.

I I I

Click Show Reference Dimensions to hide or show all of the reference dimensions. Click Show Reference Annotations to hide or show all of the reference annotations. Reassign the dimension or annotation to another annotation view.

Feature Dimensions

Feature Dimensions include both dimensions from existing features

Hiding Feature Dimensions

Feature dimensions can be hidden or shown as a group, by feature or individually.

and dimensions from sketches. Dimensions from a feature are blue, and dimensions from a sketch are black.

I I I I

Dimensions in Annotation Views

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Click Show Feature Dimensions to hide or show all of the feature and sketch or driving dimensions. Use Hide All Dimensions and Show All Dimensions to hide or show all the dimensions in a feature. Use Hide to hide individual dimensions. Reassign the dimension or annotation to another annotation view.

Each of the above dimension types are assigned to an annotation view. The dimensions can be organized, hidden, and shown by annotation view. See Reassigning Annotations on page 108 for more information.

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Capturing 3D Views

1

2

Open the part All Types. Open the part All Types from the Lesson06\Case Study folder.

Settings.

The part is showing some types of annotations. Right-clicking the Annotations folder, click the options Show Feature Dimensions, Show Reference Dimensions, and Show Reference Annotations are all checked.

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Lesson 6 Capturing 3D Views

3

Annotation views.

Expanding the Annotations folder, it is clear that all of the annotation views are visible. 4

DimXpert only.

Right-click the Annotations folder and clear Show Feature Dimensions and Show Reference Dimensions. Only the DimXpert annotations remain.

5

3D view.

Click Capture 3D View and name it DIMX.

6

Reference only.

Right-click the Annotations folder, clear Show DimXpert Annotations and click Show Reference Dimensions.

Click Capture 3D View and name it REF.

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Capturing 3D Views

7

Features only.

Right-click the Annotations folder, clear Show Reference Dimensions and click Show Feature Dimensions.

8

Hide by feature.

Click the FeatureManager tab. Right-click Base-Extrude and click Hide All Dimensions. Repeat for Boss-Extrude1, Cut-Extrude1, and Cut-Extrude3.

9

Hide individual dimensions.

Right-click the radial dimension and click Hide. Repeat for the other diameter dimensions, leaving only the linear dimensions as shown. Click Capture 3D View and name it FEAT.

10 Save and close all files.

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Exercise 9 Capturing 3D Views 1

Exercise 9: Capturing 3D Views 1

Capture 3D views of this part. This lab reinforces the following skills: I I I I

1

2

Reassigning Annotations on page 108. Modifying Dimension Attachments on page 119. Capturing 3D Views on page 124. Using Section Views on page 128.

Open the part Capture 1. Open the part Capture 1 from the Lesson06\Exercises folder.

Modify attachments.

Modify the attachment points for the following dimensions. The 12mm dimension.

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Capturing 3D Views 1

The 12mm dimension with datum.

The 38mm dimension.

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Exercise 9 Capturing 3D Views 1

3

Reassign dimension.

Reassign the 75mm dimension from the *Front annotation view to the *Top as shown.

4

Test annotation views.

Activate and orient to the *Front, *Top and *Right annotation views. Organize the dimensions and annotations as shown.

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Capturing 3D Views 1

The *Right no longer has any dimensions.

Note

5

Delete annotation view.

Unused annotation views are not needed. Activate the *Unassigned Items annotation view. Right-click and delete the *Right annotation view. 6

Section view.

Change to an Isometric view orientation. Hide all of the annotation views. Create a section view as shown.

Capture 3D Views

146

Using the annotation and section view, capture a set of 3D views as shown. 7

3D view SV. This 3D view uses the section view (step 6 on page 146), hiding all the annotation views.

8

3D view FULL. This 3D view clears the section view and shows all annotation views.

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Exercise 9 Capturing 3D Views 1

9

3D view FRONT. This 3D view shows the *Front annotation view.

10 3D view TOP.

This 3D view shows the *Top annotation view.

11 Test.

Test the completed 3D views.

12 Save and close all files.

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Exercise 10

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Capturing 3D Views 2

Exercise 10: Capturing 3D Views 2

Capture 3D views of this part. This lab reinforces the following skills: I I I I

1

Modifying Dimension Attachments on page 119. Capturing 3D Views on page 124. Using Configurations and Display States in 3D Views on page 131. Using Section Views on page 128.

Open the part Capture 2. Open the part Capture 2 from the Lesson06\Exercises folder.

This part contains two annotation views and two configurations.

2

Note

148

3D view ISO. Create a new 3D view ISO. This 3D view uses the configuration Default. The annotation views can be hidden or shown.

There are no DimXpert annotations for this configuration.

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Exercise 10 Capturing 3D Views 2

3

4

3D view FR. Create a new 3D view FR. This 3D view uses the configuration Simplified and hides all annotation views but the active one.

Orientation.

Change to an isometric view and make the *Right annotation view active. Hide the *Front annotation view. 5

New annotation view.

Create a new annotation view using the *Left view orientation.

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Capturing 3D Views 2

6

Reassign.

Show the *Right annotation view. Reassign the two dimensions shown to the *Left view orientation.

7

Modifying dimension attachments.

Hide the *Right annotation view. Drag the dimension attachment points to reshape the dimensions as shown.

8

150

3D view D1. This 3D view uses the configuration Simplified and hides all annotation views but the active one (*Left).

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Exercise 10 Capturing 3D Views 2

9

3D view S1. Make the *Right annotation view active.

Use the Section View tool to cut the part as shown. This 3D view uses the configuration Simplified and hides all annotation views but the active one. The dimensions have also been reattached as in step 7 on page 150.

10 3D view CUT.

Double-click the preview for ISO. use the section view tool to create the cut as shown. This 3D view uses the configuration Default.

11 Save and close all files.

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Exercise 11

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Capturing 3D Views - Assembly

Exercise 11: Capturing 3D Views Assembly

Capture 3D views of this assembly. This lab reinforces the following skills: I I

1

2

Capturing 3D Views on page 124. Using Configurations and Display States in 3D Views on page 131.

Open the assembly vise. Open the assembly Support Frame from the Lesson06\Exercises\Assembly folder. Add BOM.

Add a new Bill of Materials to the assembly by clicking Insert, Tables, Bill of Materials. Click the options Parts only, Display as one item number, and Display configurations of the same part as separate items. Click OK. 3

Select annotation view.

In the Select Annotation View dialog, Click Notes Area and click OK. Place the table as shown.

4

Hide table.

Right-click the table and click Hide, Table.

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Exercise 11 Capturing 3D Views - Assembly

5

Create 3D views.

Create 3D views using this information: I I I

Display state = Standard, Name = 1 Display state = Transparent, Name = 2 Display state = Hidden, Name = 3

All 3D views use an isometric orientation and are zoomed as shown.

6

Exploded view.

Starting with the 3D view1, create a 3D view using the exploded view configuration ExplView2 and the display state Standard. Name the 3D view X.

7

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Save and close all files.

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Capturing 3D Views - Assembly

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Lesson 7 Publishing PDF and eDrawings Files

Upon successful completion of this lesson, you will be able to:

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Publish a part or assembly to a 3D PDF file.

I

Publish a part or assembly to an eDrawings file.

I

Manipulate a 3D view in a 3D PDF file.

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Publishing PDF and eDrawings Files

Publishing PDF and eDrawings Files

Publishing is the final step in creating 3D PDF and eDrawings files using SOLIDWORKS Model Based Definition software. Publishing is not fully automatic; it requires some user input to shape the file. That input includes the selection of views and output details that include text and properties.

Theme

The Theme is the selection of the template. This includes the standard set and other user defined templates. For more information about templates, see Lesson 8: 3D PDF Template Editor.

Views to Include

Many types of views can exist in a part or assembly, including standard views, user defined named views, and annotation views. They can all be selected for publishing. The Standard (orthographic and pictorial) views are available for section. The Current Model View is the current view orientation of the part or assembly and appear at the beginning of the view list.

Between the current model view and the 3D views are the Named Views that were created in the part or assembly.

The 3D views have been created specifically for publishing (see Capturing 3D Views on page 124) and appear at the end of the view list.

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Lesson 7 Publishing PDF and eDrawings Files

Output Details

The Output Details of the PDF includes a location and text options. The Text Field text types requires typed input before publishing. The Custom Property Field text types require the selection of custom properties before publishing.

Publishing a Part to a 3D PDF

Publish part PMI to a 3D PDF file and generate a standard PDF file that includes 3D views as well as text fields, custom properties and notes. The 3D Views can be manipulated within the Model Area of the PDF. Logo

Text Fields and Custom Properties

List of 3D Views

Type in Notes

Model Area

For more information about 3D PDF Templates, see Lesson 8: 3D PDF Template Editor. Where to Find It

I

CommandManager: SOLIDWORKS MBD >

I

Tab: At the bottom of the screen, click the 3D Views tab and

Publish to 3D PDF Publish to 3D PDF 1 2

Open the part Publish Part. Open the part Publish Part from the Lesson07\Case Study folder. Switch to Full.

Click the 3D Views tab. Double-click the 3D view ALL. Note

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The active 3D view is used to define the configuration when standard views are selected from Views to include.

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3

Publish.

Click Publish to 3D PDF

.

Use the simple part (a4, landscape) template. Under Views to include, click Right View

.

From More views, select ALL, FRONT, SECTION, and CONFIG. Click View PDF after saving. Do not click OK yet.

4

Text fields.

Click Text Fields and type the text Preliminary and ABC as shown. Click Close.

5

Custom property fields.

Click Custom property fields and select the Custom property names PartNo and Material as shown.

Click Close and OK.

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6

Finished PDF.

Click on a thumbnail of the 3D view ALL to show it in the central Model Area.

7

Model View.

Click the 3D view ALL and it will appear in the Model View. Click in the model area and the 3D Tools toolbar appears. Roll the middle mouse button up to zoom in as shown.

Note

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There are many tools available when using the model view area. Those tools will be discussed in 3D View Manipulation on page 160.

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Publishing PDF and eDrawings Files

3D View Manipulation

The 3D Views that were created in SOLIDWORKS and saved in the 3D PDF can be manipulated in the 3D PDF by rotating, zooming, appearance changes and measurements.

Mouse Buttons

Typically, the left mouse button is used with 3D tools within the model view area, however the other buttons can also be used to perform common tasks. I

I I I I

Drag the left mouse button to manipulate the view by rotating, spinning, panning or zooming (see 3D Tools on page 160 for more information). Control+drag the left mouse button to pan. Shift+drag the left mouse button to zoom in and out. Roll the middle mouse button up to zoom in and down to zoom out. Right-click in the Model area to access tools and preferences.

Note

The default left mouse button action is Rotate. To change this, see 3D Tools on page 160.

Where to Find It

I I

3D Tools

Toolbar: Click in the Model View and select an option. Shortcut Menu: Right-click in the Model View and select an option.

Many 3D Tools are available when the Model View is selected. The Tools use the left mouse button and are shown below. Rotates a model in any direction.

Rotate Spin

‘

Turns a model (similar to rotate).

Pan

Moves the model. Also, see Mouse Buttons on page 160.

Zoom

Zooms the model. Also, see Mouse Buttons on page 160.

Walk

‘Walk through’ type options for large models.

Fly Camera Properties

160

Adjust the position and target of the camera.

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Lesson 7 Publishing PDF and eDrawings Files

3D Measurement Tool

Measures model distances and sizes.

Add 3D Comment

Adds text comments with leaders. There are several Snap and Measurement Types available.

The Views and Viewing Options are shown below. Default View

Resets to the default view orientation.

Views

Change the active 3D View with a pull down.

Toggle Model Tree

Use Perspective Projection

Model Render Mode

Transparent Bounding Box

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Solid (Default)

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Transparent

Solid Wireframe

Illustration

Solid Outline

Shaded Illustration

Bounding Box

Transparent Bounding Box Outline

Wireframe

Shaded Wireframe

Transparent Wireframe

Hidden Wireframe

Vertices

Shaded Vertices

Cross Section Properties

Note

162

To view all tools, right-click Tools, and click Expand 3D Tools.

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Lesson 7 Publishing PDF and eDrawings Files

8

Change orientation.

Use rotate, zoom and pan to orient the model as shown.

9

Measure to center.

Click the 3D Measurement Tool

, 3d Snap to Radial Edges

and 3d Point to Point Measurement and clear the remaining filters. Float over the circular edge and click when the center target appears.

10 Place measurement.

Repeat the selection process for the selection of the circular edge on the opposite end as shown. Click to place the dimension as shown.

Note

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The dimension can be selected and deleted.

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Publishing PDF and eDrawings Files

Publishing a Part to an eDrawings File

The 3D Views data can be published to an eDrawings file, a file type familiar to SOLIDWORKS users. The eDrawings file provides plenty of manipulation options, but unlike the 3D PDF it displays them like parts or assemblies; without a ‘drawing sheet’. Toolbars

eDrawings Pane

eDrawings Tools

The eDrawings toolbars share many icons with SOLIDWORKS and many of them perform similar functions.

Note

A SOLIDWORKS part file is published as an *.eprt eDrawings file. 1

Note

164

Return to the part Publish Part. The part was opened at the beginning of the lesson. If it is not already open, click the 3D Views tab.

3D views that use section views are not respected by eDrawings.

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Lesson 7 Publishing PDF and eDrawings Files

2

Publish eDrawings.

Click Publish eDrawings File

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. Click All configurations and OK.

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3

Viewer window.

Clicking 3D Views view CONFIG.

4

Mass Properties.

Click Mass Properties

166

selects a list of the 3D views. Click the 3D

to extract the material, mass and volume.

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Lesson 7 Publishing PDF and eDrawings Files

5

Configurations.

The configuration can be selected independently of the 3D view. Click the 3D View FRONT, click Configurations and click the Extend configuration.

6

Publishing an Assembly to a PDF

Save and close all files.

Publish assembly PMI to a 3D PDF file and generate a standard PDF file that includes 3D views as well as text fields, custom properties, notes, exploded views, and a bill of materials. The process of publishing an assembly PDF is identical to that for a part. See Publishing a Part to a 3D PDF on page 157 for more information.

1

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Open the assembly Publish Assembly. Open the assembly Publish Assembly from the from the Lesson07\Case Study\Publish Assembly folder. Three 3D views have been saved with the assembly.

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2

Publish.

Click Publish to 3D PDF

.

Use the simple assembly (letter, portrait) template. Under Views to include, click Top View, Front View and Right View. Under More views, click FULL, EXPLODED and OPEN. Click View PDF after saving. Do not click OK yet.

3

Text and property fields.

Click Text fields and type the text Set includes 8 hex wrenches and ABC as shown. Click Close. Click Custom property fields. Select Revision from the list.

Click Close and OK.

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Lesson 7 Publishing PDF and eDrawings Files

4

Components to BOM.

Click the Exploded 3D view. Clicking a component highlights it in the BOM. Click the component as shown.

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Publishing PDF and eDrawings Files

5

Measure.

Click the Full 3D view. Click the 3D Measurement Tool

.

Click 3D Snap to Planar Faces and 3D Perpendicular Dimension , clear the remaining filters. Click the opposite faces and place the dimension as shown.

Note

To manipulate the view while measuring: hold down Alt to rotate, Shift to pan, and Alt+Shift to zoom.

Adding 3D Comments

3D Comments allow you to add comment text with a leader, to the

PDF view. The leader is attached to model geometry. 6

Add comment.

Click the Exploded 3D view and zoom in. Click Add 3D Comment and select the edge of the component as shown. Click to place the comment box.

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Lesson 7 Publishing PDF and eDrawings Files

7

Type text.

Type the text ISO? and click OK.

8

Save.

Save and close the PDF.

Publishing an Assembly to an eDrawings File

The 3D Views data can also be published to an eDrawings file. The eDrawings file provides many assembly manipulation options, but unlike the 3D PDF it displays them without a ‘drawing sheet’.

Note

An assembly is published as an *.easm eDrawings file. 1

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Return to the assembly Publish Assembly. The part was opened at the beginning of the lesson. If it is not already open, click the 3D Views tab.

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2

Publish.

Click Publish eDrawings File and create an eDrawings file of the assembly.

3

Exploded view.

Click 3D Views and the 3D view Exploded.

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Lesson 7 Publishing PDF and eDrawings Files

4

Collapse.

Click Explode the view. 5

and clear ExplView1 to collapse

Orientation.

Click View Orientation

6

and Front

Hide.

Click Components

, click the component

shown and click Hide/Show

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.

.

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Publishing PDF and eDrawings Files

7

Reset.

Click Reset 8

to reset back to the original.

Move component.

Click Move and Free Drag component as shown.

9

174

. Select and drag and drop the

Save and close all files.

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SOLIDWORKS 2015

Exercise 12 Publishing a Part 1

Exercise 12: Publishing a Part 1

Create 3D views and publish this part. This lab reinforces the following skills: I I

1

2

Publishing a Part to a 3D PDF on page 157. Publishing a Part to an eDrawings File on page 164.

Open the part Publish a Part 1. Open the part Publish a Part 1 from the Lesson07\Exercises folder. There are four existing 3D views.

Publish.

Click the 3D Views tab and click Publish to 3D PDF. Select the settings as shown. I I I

Template = simple part (letter, landscape) Views to Include = Trimetric View, Right View More views = SV, FULL, FRONT, and TOP

Click View PDF after saving. 3

Text Fields.

Click Text fields. Under Comments, type Rounds R6mm. Under Designer type your name. 4

Custom property fields.

Click Custom property fields and select PartNo as the Part Number and Material as the SW Material.

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Publishing a Part 1

5

PDF file.

The completed PDF includes all of the selected views.

6

eDrawings file.

Create an eDrawings file using the same part file and configurations of the source.

7

176

Save and close all files.

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SOLIDWORKS 2015

Exercise 13 Publishing a Part 2

Exercise 13: Publishing a Part 2

Create 3D views and publish this part. This lab reinforces the following skills: I I

1

2

Publishing a Part to a 3D PDF on page 157. Publishing a Part to an eDrawings File on page 164.

Open the part Publish a Part 2. Open the part Publish a Part 2 from the Lesson07\Exercises folder. There are five existing 3D views. Publish.

Click the 3D Views tab and click Publish to 3D PDF. Select the settings as shown. I I I I I I

Template = simple part (letter, portrait) Views to Include = Top View and Right View More views = ISO, FR, D1, S1, and CUT Comments = see detail S1 Designer = ABC Part Number = PartNo

Click View PDF after saving.

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Publishing a Part 2

3

eDrawings file.

Create an eDrawings file using the same part file and configurations of the source.

4

178

Save and close all files.

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Exercise 14 Publishing an Assembly

Exercise 14: Publishing an Assembly

Create 3D views and publish this assembly. This lab reinforces the following skills: I I

1

Publishing an Assembly to a PDF on page 167. Publishing an Assembly to an eDrawings File on page 171.

Open the assembly publish assembly. Open the assembly publish assembly from the Lesson07\Exercises\publish assembly folder.

There are four existing 3D views.

2

Publish.

Click Publish to 3D PDF and select the template simple assembly (letter, landscape). Under Views to Include, click the Top View, Front View and Right View. Under More views 1, 2, 3, and X. Return to the 3D view1. 3

Text fields.

Click Text fields. Under Comments, type Hardware galvanized. Under Designer type your name. Click Close. 4

Properties.

Click Custom property fields. Check the settings and click Close.

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Publishing an Assembly

5

View.

Click View PDF after saving and click OK.

6

eDrawings.

Publish an eDrawings file from the same assembly. Click 3D Views and the 3D view X.

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Exercise 14 Publishing an Assembly

7

Wireframe.

Click Display Style

8

Collapse explode.

Click Explode view. 9

and Wireframe.

and clear ExplView2 to collapse the exploded

Orientation.

Click View Orientation to Shaded with Edges.

and Right

. Set the display style back

10 Isolate.

Click Components and type brace to search. Click Corner-1 to highlight it. Click Isolate to show only that component.

11 Save and close all files.

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Lesson 8 3D PDF Template Editor

Upon successful completion of this lesson, you will be able to:

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I

Understand the 3D PDF template editor.

I

Modify a 3D PDF template.

I

Use a 3D PDF template.

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3D PDF Template Editor

3D PDF Template Editor

The 3D PDF Template Editor is used to modify and create templates for use with the Publish to 3D PDF tool. The basic components of a template include the logo, comments, custom properties, text placeholder, table placeholder (assemblies only), thumbnails area and a model area for displaying 3D views.

Note

The 3D PDF template editor tool is an independent program that runs in its own window.

Template Arrangement

The components of the template are arranged in two general ways using the same set of components in portrait or landscape orientations.

Supplied Templates

The supplied 3D PDF templates are stored in the SOLIDWORKS installation directory Program Files\SOLIDWORKS Corp\ SOLIDWORKS\data\themes folder. They are: I I I I I I I I

Note

184

simple simple simple simple simple simple simple simple

assembly (a4, landscape) assembly (a4, portrait) assembly (letter, landscape) assembly (letter, portrait) part (a4, landscape) part (a4 portrait) part (letter, landscape) part (letter, portrait)

Each template requires multiple files and is identified by a folder.

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Lesson 8 3D PDF Template Editor

Creating New Templates

New templates can be created by modifying existing templates or they can be created as new templates from scratch. It is generally easier to modify a template and save it under a new name.

Note

The new template Page Size can be Letter, Legal, various A, B, or custom sizes. It can be oriented in Portrait or Landscape.

Components of the Template

All templates have some common component areas. The areas found on the default template are described below: I

Image Area- This area contains a SOLIDWORKS logo by default,

I

Comments and Custom Properties Area- This ares includes

but a replacement image can be selected.

I I I

I

Image Area

comment text, user input text and custom properties text. Notes Area- This is the only area that allows for user input on the completed PDF. BOM Table Area- This area is only found on assembly templates and it is used to display the Bill of Materials table. Thumbnail Area - This area shows all of the 3D views selected from the model. When they are selected, they appear in the Model Area. Model Area - This area displays the active 3D view that has been selected from the Thumbnail Area. The model view can be manipulated by rotation, shading and many other tools. See 3D Tools on page 160 for more information. Comments and Custom Properties Area

Notes Area

Model Area

BOM Table Area

Thumbnail Area

Note

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Part templates have a single, larger Notes area in place of the BOM Table Area found in assembly templates.

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3D PDF Template Editor

Text Types

A 3D PDF template has multiple text types available. The text type used depends on the information being extracted or entered. For example, text like Notes is not intended to be changed and uses the Template text field type.

Template Text Field

The Template text field is a text string. It is used for titles and headings where it will not change.

Text Field

The Text field is a text box with user defined text. It is filled in by the publisher of the PDF.

Custom Property Field

The Custom property field is a text box that is tied to a Custom Property of the part or assembly. The properties used in the standard templates are: I I I I

PDF Form Field

SW-Part Number SW-Short Date Revision SW Material

The PDF form field is a text box with a fill-in with user defined text. It is filled in by the end user of the PDF. These text types are distributed throughout the template as shown below.

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Lesson 8 3D PDF Template Editor

Modifying a Template

A template can be modified in many ways. The text (see Text Types on page 186) can be moved, modified and new text can be added. In addition, the logo and backgrounds can be changed. In this example, the standard letter sized, portrait oriented template will be modified with a new logo, background and additional text.

Standard Template Files

The standard template files are stored in sub-folders of the Program Files\SOLIDWORKS Corp\SOLIDWORKS\ data\themes folder. Each folder contains the xml and image files that

collectively make up the template. Note

There are separate 3D PDF templates for parts and assemblies.

Where to Find It

I

CommandManager: SOLIDWORKS MBD > 3D PDF Template Editor

1

Open the part Test Template. Open the part Test Template from the Lesson08\Case Study folder. It is a part that includes four 3D views.

2

Open template editor. Click 3D PDF Template Editor

. Minimize the SOLIDWORKS

window. 3

Open template.

Click Open

and select the template

simple part (letter, portrait).

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3D PDF Template Editor

Changing the Logo

The current logo is an image file that has been positioned on the template in the upper left corner. In this example, the current logo (LOGO.png) will be replaced with another image file, be resized, and moved.

Note

Additional image files can be added using Image . The inserted image has the same editing capabilities as a logo image. 4

Logo.

Click the logo, browse, and select the image swlogo1.jpg from the local Lesson08\Case Study folder.

5

Zoom and scroll.

Use the middle mouse button to zoom, use the left mouse button to scroll and the Fit to Window button to see all of the template. When an image is replaced, it may come in distorted. Click Reset to Original Size . To resize an image without distortion, click Lock Aspect Ratio and drag the corner.

Avoiding Distortion

6

Resize.

Select the image. Click Lock Aspect Ratio and drag the corner of the image. Make the depth of the image about the same as the depth of the box surrounding the text. 7

Move and align.

Move the image using the blue guidelines to show where the image is aligned (blue highlights) as shown. Drop the image.

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Lesson 8 3D PDF Template Editor

Saving the Template

Templates are made up of multiple files in a specific folder (see Standard Template Files on page 187). When saving a template, multiple files will be placed in a new folder that uses the template name that you supply. The template folder can be placed with the standard folders or in a user defined location. In this example, we will create a new folder template in the local folder. 8

Save as.

Create a new folder template in the local Lesson08\Case Study folder. Click Save As and name the template new part, logo, letter, portrait and save it to the new folder template. It becomes the active template. The template folder allows multiple templates to be saved in that same location.

Note 9

Background.

Click Background

and the select the image

sheetbackground1.bmp from the local folder.

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3D PDF Template Editor

Adding Text

Text of all types can be edited or added to the template. For more information on selecting which text to use, see Text Types on page 186. In this example, text will be added for a title and for a related custom property. 10 Resize.

Make room for addition text information. Select and resize the text area placeholder text box by dragging as shown.

11 Template text field.

Click Text . Add a Template Text Field and place it on the sheet. Place it below the Comments text as shown. Type Mass: and click OK.

12 Custom property. Drag Text onto the sheet. Add a Custom Property Field

and place it on the sheet as

shown. Type the text as shown and click OK. Resize the text frame.

13 Save and close. Click Save and close the SOLIDWORKS 3D PDF Template Editor. Note

190

The template can be edited after testing to adjust the positions of the text.

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Lesson 8 3D PDF Template Editor

Using The Template

Once the template has been saved, it is ready for use. In this example, a part will be published to test the template. For more information on publishing, see Lesson 7: Publishing PDF and eDrawings Files.

Note

Parts can be used with assembly templates however some properties will not be available and the BOM Table Area will not be used. 14 Publish. Click Publish to 3D PDF and select the new part, logo, letter, portrait template from the

drop down list. Under Views to include, click Right View and from More views, click SV, FULL, FRONT, and CUTAWAY.

15 Text Fields. Click Text fields and type the text shown. Click Close.

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3D PDF Template Editor

16 Custom property fields. Click Custom Property Fields and select Weight as shown. Click Close.

17 Published PDF. Click View PDF after saving and OK. Use the 3D View Manipulation

to work with the views.

18 Save and close all files.

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Exercise 15 Creating a Template

Exercise 15: Creating a Template

Create a new template and publish using a part. This lab reinforces the following skills: I I I I

1 2

3D PDF Template Editor on page 184. Modifying a Template on page 187. Avoiding Distortion on page 188. Using The Template on page 191.

Open the part Plate. Open the part Plate from the Lesson08\Exercises folder. Add property.

Click File, Properties and type a new Property Name surface. For the Value / Text Expression, select Surface Area and click OK.

3

3D views.

Create the 3D views as shown below. 3D view FULL

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Creating a Template

3D view TOP

3D view SECTION

4

Template editor.

Click 3D PDF Template Editor

and open the template

simple part (a4, landscape). 5

Save as.

Click Save As and save the template to the local Lesson08\Exercises folder. Name the template student. 6

Replace logo.

Replace the logo with the image sw.bmp from the local folder. Manipulate the logo and place it as shown.

Note

194

Both Reset to Original Size and Lock Aspect Ratio will be needed.

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Exercise 15 Creating a Template

7

Template text field.

Add a Template text field and type in Surface Area in mm2. 8

Custom property field.

Also, add a Custom property field. Type this: I I I

Field Name: Surface Area Instructions: select surface Custom Property: surface

Place the text as shown. 9

Background.

Set the background image to powdercoat_light.jpg from the local folder as shown.

10 Save and close.

Save the template and close the SOLIDWORKS 3D PDF Template Editor.

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Creating a Template

11 Publish.

Publish to a 3D PDF using the student template. Use the views Front View, Right View, FULL, TOP and SECTION. 12 Text.

For the Custom Text, type this: I I

Comments: All fillets and rounds not noted are 2mm Designer:

13 Custom. For the Custom Property Text, select these names: I I I

Part Number: PartNo SW Material: Material Surface Area: surface

14 Save and close all files.

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Index

Numerics 3D PDF see PDF 3D views 124 assembly 132 capture 124 configurations 131 display states 131 model break view 134 part 125 publishing 156 section views 128 A add 3D views 124 annotation views 100, 113 DimXpert 22, 33 annotation views 100 activating 104 create new 113 dynamic 106 hide and show 103 insert 113 MBD 11 notes area 101 orientation 105 orthographic 101 unassigned items 101 annotations delete 79 feature dimensions 138 geometric tolerance 58 planes 64 reference dimensions 138 views 64 auto dimension scheme 22 automatic tolerancing 22 B break view 134 C capture 3D views 124 color 5 D dimensions combine 46 feature 138 location 33

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recreate basic dimensions 60 reference 138 size 33 sketch 139 dimensions and tolerances move 108 reassign 108 DimXpert 16 annotations 28, 63 auto dimension scheme 22 datums 29 delete dimension 79 delete tolerance scheme 79 dimension directions 49 DimXpertManager 32 drawings 63 features 25 geometric tolerance 58 intersection circles 51 intersection lines 50 intersection lines for virtual edges 48 intersection points 52 location 33 MBD 11 plus and minus 80 polar dimensions 80 prismatic parts 18 properties 20 recreate basic dimensions 60 selections 18, 44 settings 20 size 33 tolerance rule checking 82 tolerance status 32 turned parts 18 DimXpertManager 17 drawings DimXpert 63 driven dimensions 138 driving dimensions 138 dynamic annotation views 106 E eDrawings assembly 171 configurations 167 mass properties 166 part 164 publish 164, 171

G geometric tolerance 58 geometric tolerancing symbols 22 gtol 58 I intersection circles 51 intersection lines 48, 50 intersection points 52 M MBD 3D PDF 12, 156 annotation views 11, 100 annotations 10, 138 capture 3D views 12, 124 configurations 10, 131 dimensions 10, 138 DimXpert 11, 16 PDF templates 13, 184 preparations 9 tables 10, 185 what is MBD? 8 Model Based Definition see MBD model break view 134 method 135 style 134 P PDF 3D PDF 156 3D Tools 160 3D views 156 output options 157 publishing 156 using mouse buttons 160 view manipulation 160 PDF template component areas 185 editor 184 logo 188 modifying 187 saving 189 supplied templates 184 test types 186 PDF template editor 184 planes annotation 64 plus and minus pattern linear 80

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polar 80 PMI 8 R recreate basic dimensions 60 rule checking 82 S section views 128 symbols geometric tolerancing 22 T tolerance rule checking 82 collinear datums 86 cylindrical position 84 duplicate datums 83 non-coaxial features 88 tolerance scheme 17, 79 tolerances 22 training files 3 turned part 76 V view annotation 64 break 134 views dynamic annotation view 106

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