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Version 2010
What's New: Highlights of SolidWorks 2010.....................................................................x Legal Notices..................................................................................................................12 1 Administration..............................................................................................................14
Installation Improvements......................................................................................................................14 SolidWorks Rx.......................................................................................................................................15 Diagnostics for Graphics Card and Driver........................................................................................15 SolidWorks Rx Workflow..................................................................................................................15 Converting Files to SolidWorks 2010.....................................................................................................16
2 User Interface...............................................................................................................17
Heads-Up View Toolbar Customization ................................................................................................17 Context Toolbars....................................................................................................................................17 Instant3D Enhancements.......................................................................................................................17 Mouse Gesture Support ........................................................................................................................18 Mouse Gestures...............................................................................................................................18 PropertyManager Improvements ..........................................................................................................22 Graphics Area Controls Improvements .................................................................................................22 Larger Icons for Windows Vista.............................................................................................................23 Data Migration Tab in CommandManager.............................................................................................23 Touch and Multi-Touch Support ...........................................................................................................23
3 Fundamentals..............................................................................................................25
Documentation for SolidWorks..............................................................................................................25 Web-based Documentation..............................................................................................................25 New Tutorials....................................................................................................................................25 30 Minute Lesson Renamed............................................................................................................26 New Illustration Policy......................................................................................................................26 Display States for Parts.........................................................................................................................26 Custom Properties.................................................................................................................................27 Reference Planes .................................................................................................................................27 Creating Reference Planes..............................................................................................................27 Modifying Reference Planes............................................................................................................28 Selecting Points to Create Planes....................................................................................................28 Viewing Decals in SolidWorks...............................................................................................................30 Saving Multiple Documents...................................................................................................................30 Normal To Command.............................................................................................................................30
4 Application Programming Interface..............................................................................32
5 3D ContentCentral.......................................................................................................34
Self-Service Catalog Publishing............................................................................................................34 My 3D ContentCentral...........................................................................................................................34 Request Content....................................................................................................................................35 3D ContentCentral Community..............................................................................................................35
6 Assemblies...................................................................................................................36
Assembly Visualization .........................................................................................................................36 Assembly Visualization Overview.....................................................................................................36 Activating the Assembly Visualization Tool......................................................................................36 Visualizing the Assembly..................................................................................................................37 Changing the Sorting Property.........................................................................................................39 Creating an Equation for Sorting......................................................................................................40 Mirror Components ...............................................................................................................................41 Making Mirror Selections..................................................................................................................42 Setting Orientation............................................................................................................................42 Creating Mirrored Configurations.....................................................................................................43 Editing a Mirror Component Feature................................................................................................44 Virtual Components ..............................................................................................................................45 Making External Components Virtual...............................................................................................45 Naming Virtual Components............................................................................................................46 Copying Virtual Components............................................................................................................46 Moving Virtual Components.............................................................................................................47 Saving New In-Context Components...............................................................................................48 Component Reference per Instance......................................................................................................49 Display States........................................................................................................................................50 SpeedPak..............................................................................................................................................51 Mates.....................................................................................................................................................51 Relocating Components...................................................................................................................51 Replacing Components....................................................................................................................51 Coordinate System Mates................................................................................................................52
7 CircuitWorks.................................................................................................................53
User Interface........................................................................................................................................53 Updating Assemblies.............................................................................................................................53 Importing Non-CircuitWorks Assemblies from SolidWorks....................................................................53 Selecting the Board Component and Orientation.............................................................................54 Using Silhouette Edges to Determine Component Shape...............................................................54 PADS Support........................................................................................................................................54
8 Configurations..............................................................................................................55
Configuration Publisher .........................................................................................................................55 Starting with Multiple Configurations................................................................................................56 Starting with a Single Configuration.................................................................................................59 Modify Configurations ...........................................................................................................................64
...........................................70 UI Enhancements...75 Bills of Materials....................................................70 Virtual Sharp Check.81 Tables..........66 9 Design Checker..........................................................................................................................................................................................................................................................................................................75 Annotation Attachments...........................................................................................................................................69 Validation Against ANSI/ISO/JIS Drafting Standards............................................................................................................85 Section Views...........................................................................................................................................................................64 Configuring Custom Properties.................................................................................................................................................................................85 Opening Parts and Assemblies from Drawings....................................................................................................................................................................71 Samples of Industry Vertical Custom Checks to 3D ContentCentral.......................................................................................................................................75 Balloons........................................................78 Dimension Palette ................................................................................83 Aligned Section Views...............................77 Cosmetic Threads........................................................................................................................................................................................................................................77 Center Marks....................................................................................................................................................81 Fractional Dimensions......................................................................................................................................................................................82 Drawings........................................83 Component Line Font.........72 11 DFMXpress.........................................................81 Deleting Dimensions..........74 Zoom to Selection.............................74 12 Drawings and Detailing..........................................................................................................................................................................................................................................................................................................71 10 Design Studies...............................................................................................................................................................69 One-Button Push to Correct All Errors.......................................................................................78 Rapid Dimension ....................................................................................................84 Hiding and Showing Edges..............................69 Integration of Design Checker.................................................................................................................................................................................................................................................................................................................82 Title Block Tables in Parts and Assemblies....................................................................................................................................................................................65 Editing a Table View.............................70 Task Scheduler Option for Autocorrection........................................................................................80 Ordinate Dimensions................74 Managing Standard Hole Sizes....................................................................................................................................74 Sheet Metal Validation.........................................................................................85 iv ...........................................................................................................................................................................................................................................................................................................................................................Contents Configuring Material.................................................................................................................................................................................................................................................83 Configurations...........................................................................................................................................................................................................................................................81 Dimension Names..........................81 Notes....................................................................................................84 Drawing Views of Multibody Parts ......................................................................................................................................................78 Dimensions....84 Drawing Templates.........................................................................................76 Blocks...................................................
............95 Setting Up Tasks............104 SMTP Mail Setup.................................................................................................................................................................................................................................................95 Managing Tasks .............................................................................................................................................................................101 Generating Item IDs from File Attributes........................102 Central Assignment of Permissions......................................................................................................86 13 eDrawings...................................................................................................................................................................................................................................................104 v ..............................................................................................................................................................................................................................101 Expanding and Collapsing Item Structure..................................................................96 Executing Tasks......98 Using Toolbox with Enterprise PDM..................................................................93 14 Enterprise PDM.........102 Administration Tool.........................................................................................................100 Changing Column Names and Order in the SolidWorks Add-in....................90 Apple Mac Printing Enhancements.............................................................................98 Enterprise PDM and Toolbox Integration ...........................................................................................................................101 Display Formats for Item BOMs........................................................................................................................................................................................................86 System Properties..............................................................101 Named BOMs for Items.......................................................86 Tangent Edges.............................................................................................................................97 Monitoring Tasks............................................89 Enhanced BOM Support..........................................................97 Task Add-ins..........................101 Optional Parent Node Check Boxes................................................................92 Decals.......................100 Naming Files with Serial Numbers Using Copy Tree .............................................................................................................................................................................................................................102 Extended Export and Import Functionality...................................................102 Add-in and File Format Support..................................................................................100 Drawings with Multiple References Not Automatically Checked Out...........................................................................................................................................................................................................................................99 File Explorer and SolidWorks Add-in.....................................................................................................................................................................................................................................................................................................................................................................................................................................................................................................................................95 Convert and Print Tasks..................................................................................101 Item Management...........................100 Warning when File Is Open in Another Application...........................89 Print Preview.........................................................................................103 Serial Number Enhancements........................................................................................................................................................................................................................................................91 Title Block Tables....100 Cold Storage Versions in Get Version Submenu.........................................................................................................................................................................................................................93 Sketch Pictures.............................91 Display States Linked to Configurations...................................................................................................................................................................................................................................................................................Contents Sketch Pictures.102 API Support for Items......................................................100 Naming Drawings with Model Names Using Copy Tree..................................98 Configuring Enterprise PDM and Toolbox...........................................................................89 Integrated Publisher.................................................100 File Preview Rebuild Warning .........................................................................................................
..............105 Web-based Documentation .........................................................................................................................................114 Force and Motor PropertyManager Enhancements..........................................................................................................................................................117 Features......104 API Support for Items..107 Importing and Exporting Adobe Photoshop Files on 64-bit Computers................................................................................................109 Event-based Motion Analysis .....................................................109 Event-based Motion Analysis........................................................................................................................................................................................................................... or PSD File to a Custom Size...........................................................................116 17 Parts and Features....................................................................................................................................................................................................................................................................................................................................................................104 API Methods for Users and Groups..............................................................115 Contact PropertyManager Name Change............................................107 DXF / DWG Output PropertyManager............................................................................. JPG..................................................................................................................................................................................................115 Contact....................................110 New Proximity Motion Sensor.................108 Importing Adobe Illustrator Files............................................................................................................................119 Pattern and Mirror Preview...................................................................................................................................................................................................................................................................................................................................................................122 Shape Feature........................................................................................................107 Importing Rhino Files on 64-bit Computers.............................108 16 Motion Studies............122 FeatureWorks ..........................................................................................................................................108 Saving a TIF......................................................................................................................................................................................105 15 Import/Export.....................................................................110 Event-based Motion Study............105 Installation...................................................................................104 Dispatch Set Card Variables Command................................................................................................................................................................105 Predefined Data Set Configurations......................................122 Wrap Feature Enhancement...............................................................................114 Structural Simulation Analysis for Motion....................123 Surfaces...........................................................110 Rigid Groups.............................................................................................................................................................................................................................................................107 Importing Autodesk Inventor Files.........................................................................................................117 Hole Wizard......................................................................................115 Setting the Exact Time for Key Points and the Time Bar.........................................................................................................................................................126 vi ...........................................................................................................................................................................................................................................115 Curve-to-Curve Contact.......................................122 Split Lines Enhancements.....................................................................118 Move Face Features .....105 Documentation..........117 Materials and Multibody Parts..........................................................................................................................................................................Contents API...........................................................109 Servo Motors for Event-based Motion Analysis..........115 Contact Groups for Motion............................................................................................................................................................................117 Lip and Groove Enhancements..............................................117 Instant3D Enhancements..............................................................................................................
...................................................................................................................................................................................................................................................................................130 19 Routing........................................................................................................................................................................................................................................................................147 Splitting the Part...........................................................................................................................................................................130 Camera Effects......................................................................................................................................................137 Pipe and Tube Route Export Enhancements........................................................................................................................................................152 Hem Improvements.....................................................................128 Support for Background Images and Custom Environments...........................................................................................................................................................129 Video Tutorials..................157 Simulation Study Tree Enhancements................................................................136 Access to Pipe................................................... or Electrical Harness Coverings..................................................................142 Accessing Sheet Metal Bodies in Multibody Parts..........................................................153 Flat Pattern Improvements..................................................................137 Routing Library Enhancements...........................................................................................................................................................................................................................................137 20 Sheet Metal..............................................................................................136 180-Degree Elbows or Bends for Piping................................................................128 Controlling Scenes..............128 PhotoWorks Decals in PhotoView 360............................................157 vii .................................................141 Locating the Inserted Part..............................................................................................156 SimulationXpress.......................................................................145 Splitting a Sheet Metal Part..........................................................................................136 Multiple CPoint Enhancements.......................................................................................................................................................................................................................................................................................................................139 Creating a Mirrored Sheet Metal Part.................................................................................................................................................................................................................................132 Manufacture-style Flattening .........................................................................136 P&ID Data Import and Modeling Process.......................................................................151 Closed Corner Improvements............................................................................................................................................................................156 Optimization in SimulationXpress.................................................................................................157 NAFEMS Benchmarks.....................147 Preparing to Split the Part............................................132 Manufacture-style Flattening..156 New SimulationXpress Interface..............................136 Piping Drawings....143 Merging Sheet Metal Bodies by Inserting Edge Flanges........................................................................................Contents 18 PhotoView 360...................................148 Inserting a Sheet Metal Part Using a Base Flange.......................................................................................................................................................................................................................................................................157 Simulation Interface.......154 21 Simulation....................................... Tube.......130 Saving Custom Views.......................................................................................................................................................................149 Editing Sheet Metal Bodies......................................................................................................................................................................................................154 Exporting Sheet Metal Parts to DXF or DWG .....139 Multibody Sheet Metal Parts .....................................................................................................................140 Inserting a Part to Create a Multibody Sheet Metal Part...........132 Adding Components and Assembly Fittings to Routes............................................137 Reference Designators........
.................169 Beams.........177 Contact for Nonlinear Studies (Premium)...........................................................................181 Large Sketch Performance.........................................................................................................................................181 Equation-driven Curves.......................................................................................................Contents PropertyManager Enhancements.................................................................................................................................160 Simplifying Assemblies for Nonlinear Studies (Premium)...........................................................................................178 Handling Large Results Files (Premium)...............................................160 Simplified and Enhanced Fatigue Study (Professional)...180 Configurable Number of Instances in Sketch Entity Patterns....................................................................................................................................................................................................................174 Bearing Loads for Circular Holes in Shells..............................................................................................................................................160 General Enhancements.................................................................................160 Expanded Features for Simulation Advisor.............................................170 Connectors.........................183 Selecting a Material........................................................................................................................................................172 Connectors Applied to Hole Series................................................................................................................................................................................................................................................................................................................................174 Mesh..................180 Fit Spline Tool........................................................................................................................................................................................................................................................................................................................................................................................................................................................................................................................175 Mesh Enhancements.............................................................172 Bolt Connectors.........................................................................................................................................................................................................................................................................................................................................................................................182 SolidWorks Sustainability Overview .....................................................................................................185 Setting the Material....................................................................................................................................................................................................................172 Edge Weld Connectors (Professional)..........................182 Designing for Sustainability..............................................................................................................................178 Plot Stress During Time Steps in Motion......................................161 Offsets for Composites (Premium)....................181 23 SolidWorks Sustainability ........................................................................................................................180 Sketch Fillet Tool.....................................................................................................180 Convert Entities Sketch Tool..178 Plot Improvements..........................172 Spring Connectors for Shells..................................................................................................................................................................................................................176 Contact.............................................................................................................184 Comparing Similar Materials................................................159 Simulation Studies.............................................................................................................................................................................184 Setting the Manufacturing and Use Options...............................186 viii ...........................176 Contact Set Enhancements......................180 Linking Sketch Text to File Properties.......................................161 New Design Study ....................................................................175 Shell Definition by Selection of Faces.172 Bearing Connectors Between Parts.............................................................................................................................................................................................................................................................................177 Result Viewing.............................176 Component Contact .........................................................................................................................................................................................178 22 Sketching...................................................................181 Dimensions in 3D Sketches......................
........................................189 Single Part Number per Component Size..................................................................................................................................................193 Location Dimensions........................................197 Support for Virtual Components in SolidWorks Explorer.............................................................................................................................................................................................197 Support for the /3GB Switch...........................................195 Materials in Cut Lists..............191 Auto Dimension Scheme..............190 26 Tolerancing...........................................................................................................195 Property Tab Builder..............................................................195 Drawing Views of Weldments...Contents Creating a Report.........................................................................188 Compare BOM Utility............................................................................................................................191 New Feature Recognition.......................................................................................191 DimXpert........................................................................................................................................................................................189 Configuration-specific Properties in the Configurations Table...............................................................................................................................................................................................................................................................................................189 Custom Property Visibility in the PropertyManager.................................................................................................................................................................................................................................................................................................................................190 Custom Property Creation....................................197 ix .............................................................................189 Australian Standard.......................................................195 Cut List Items...........................................................189 Toolbox Custom Properties ..............................................................................................196 28 Workgroup PDM......................................................................188 Simplify Utility..................................................................187 24 SolidWorks Utilities..................................................................................................................188 25 Toolbox ........................................................................................................................................193 27 Weldments...................................................................................................................................................................................................................................................................................................................................188 Usability Improvements..........................189 Toolbox and Enterprise PDM Integration .........................................................
Throughout this guide. look for the User Interface Fundamentals Assemblies symbol in these areas: Mouse Gesture Support on page 18 Reference Planes on page 27 Assembly Visualization on page 36 Mirror Components on page 41 Virtual Components on page 45 Configurations Configuration Publisher on page 55 Modify Configurations on page 64 Drawings and Detailing Rapid Dimension on page 78 Dimension Palette on page 80 Drawing Views of Multibody Parts on page 84 Enterprise PDM Enterprise PDM and Toolbox Integration on page 98 Managing Tasks on page 95 Motion Studies Parts and Features Routing Sheet Metal Simulation Sustainability Event-based Motion Analysis on page 109 Move Face Features on page 119 Manufacture-style Flattening on page 132 Multibody Sheet Metal Parts on page 139 New Design Study on page 161 SolidWorks Sustainability on page 182 For More Information Use the following resources to learn about SolidWorks: What's New in PDF and This guide is available in PDF and HTML formats. Click: HTML • Help > What's New > PDF x . most in direct response to customer requests.What's New: Highlights of SolidWorks 2010 SolidWorks® 2010 includes many enhancements and improvements. This release focuses on the following themes: • User experience • Reliability • Performance Top Enhancements The top enhancements for SolidWorks 2010 provide improvements to existing products and innovative new functionality.
Provides information about late changes to our products. click Help > What's New > Interactive. Online Help Release Notes Contains complete coverage of our products. click the symbol to display the section of this manual that describes an enhancement. xi . The symbol appears next to new menu items and the titles of new and changed PropertyManagers. and examples. including details about the user interface. To enable Interactive What's New.• Help > What's New > HTML Interactive What's New In SolidWorks. samples.
6.712. 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). and in the license agreement. Concord. 6. and foreign patents pending. DWGgateway. 300 Baker Avenue. PhotoWorks.705. Premium. and SolidWorks 2010 are product names of DS SolidWorks. 7.571. 6. Government Restricted Rights.844.990. or implied by. 7.027. Dassault Systèmes SolidWorks Corporation.219.6184.108.40.206 and JP 3.517. 7. Massachusetts 01742 USA 12 . COMMERCIAL COMPUTER SOFTWARE . and the eDrawings logo are registered trademarks and FeatureManager is a jointly owned registered trademark of DS SolidWorks. TolAnalyst. EP 1. 7. for any purpose without the express written permission of DS SolidWorks. DWGseries. U. SolidWorks Simulation. PDMWorks. Feature Palette. this document or its contents shall be considered or deemed a modification or amendment of such warranties. or disclosure by the government is subject to restrictions as set forth in FAR 52. Concord. eDrawings.Legal Notices © 1995-2009. 01742 USA. FeatureWorks is a registered trademark of Geometric Ltd.S.262.. No material may be reproduced or transmitted in any form or by any means. SolidWorks Flow Simulation.044. a Dassault Systèmes S. 7. duplication.906.643). 6. 6.877. 7. Trademarks and Other Notices for All SolidWorks Products SolidWorks. company.815.NET. DFARS 227.7202 (Commercial Computer Software and Commercial Computer Software Documentation).486.477. All warranties given by DS SolidWorks as to the software and documentation are set forth in the SolidWorks Corporation License and Subscription Service Agreement. All Rights Reserved. FloXpress.g. Patents 5. SolidWorks Enterprise PDM. and Professional Products U.079. and foreign patents. Patent Notices for SolidWorks Standard. 6.898. and XchangeWorks are trademarks of DS SolidWorks. CircuitWorks. electronic or mechanical. The software discussed in this document is furnished under a license and may be used or copied only in accordance with the terms of this license.502. Contractor/Manufacturer: Dassault Systèmes SolidWorks Corporation. Use.S.049.079. (e.154. Other brand or product names are trademarks or registered trademarks of their respective holders.227-19 (Commercial Computer Software Restricted Rights). 3D ContentCentral. 300 Baker Avenue.560. 3D PartStream.PROPRIETARY U.055. 6.558. and nothing stated in. as applicable.603.S.116.725.A. DWGeditor. Mass.
Portions of this software © 1998-2009 Geometric Ltd. Portions of this software are copyrighted by and are the property of UGS Corp. Copyright Notices for SolidWorks Simulation Portions of this software © 2008 Solversoft Corporation. Portions of this software incorporate PhysX™ by NVIDIA 2006-2009. 6. Portions of this software © 2001 . and its licensors.866. Portions of this software © 1986-2009 mental images GmbH & Co. 6.063.S. Portions of this software © 1996-2009 Microsoft Corporation. Adobe. 6. Distiller and Reader are registered trademarks or trademarks of Adobe Systems Inc. Patents Pending.2009 Luxology. All rights reserved.639.929. Patents 5. Inc. Acrobat.502. For more copyright information. 5.364. Copyright 1984-2009 Adobe Systems Inc. All rights reserved.382. Patents Pending.S.289.593. 13 . Inc. 6. All Rights Reserved. PCGLSS © 1992-2007 Computational Applications and System Integration. and other countries. Portions of this software © 1998-2009 3Dconnexion. All rights reserved.2009 DriveWorks Ltd. This software is based in part on the work of the Independent JPEG Group. and Professional Products Portions of this software © 1990-2009 Siemens Product Lifecycle Management Software III (GB) Ltd. Premium. Inc. Other portions of SolidWorks 2010 are licensed from DS SolidWorks licensors.754. © 2009. Portions of this software © 2000-2009 Tech Soft 3D.943. the Adobe PDF logo. in SolidWorks see Help > About SolidWorks. All Rights Reserved. Portions of this product are distributed under license from DC Micro Development. Copyright © 1994-2005 DC Micro Development.563. the Adobe logo. Portions of this software © 2007 . in the U. All rights reserved.Copyright Notices for SolidWorks Standard. KG. Protected by U.
optional installation behavior. • The default workflows are much shorter. The Installation Manager log files have been improved to help resellers and users read them more easily to resolve issues encountered during installation and update. • All optional settings are available from the summary screen (for example. typically one screen for the SolidWorks serial numbers followed by a summary screen in which you can initiate the installation. download files. Error Messages and Log Files The Installation Manager error messages have been rewritten to allow easier diagnosis of installation problems. you are not required to click through multiple screens just to accept the default settings. installation location. indicating the current step in the process.1 Administration This chapter includes the following topics: • • • Installation Improvements SolidWorks Rx Converting Files to SolidWorks 2010 Installation Improvements SolidWorks 2010 contains many improvements to SolidWorks Installation Manager and the installation process. You can now start SolidWorks Installation Manager using the setup.exe file). Installation Manager The SolidWorks Installation Manager process has been redesigned to simplify the workflow and improve ease of use: • The workflow is now displayed on the left. product component selections. and Toolbox options). However.exe file found at the root of the DVD or installation directory (in addition to the sldim\sldim. The log files are located in the SolidWorks application data folder on the computer where you ran the installation: • For Microsoft Windows Vista : C:\Users\username\AppData\Roaming\SolidWorks\Installation Logs\ • For Windows operating system versions prior to Windows Vista: C:\Documents and Settings\username\Application Data\SolidWorks\Installation Logs\ ® ® ® 14 . or remove the installation.
Administration Installation File Sizes and Processing Time The installation and download process now supports patching for more individual product components. download. In the Problem Capture Details dialog box. Parallel Service Pack installations of the same major release on the same computer are not supported. without requiring any other local or downloaded files or a DVD. SolidWorks Rx Workflow The SolidWorks Rx Workflow is improved to create service requests based on the information you provide in the Rx file. a new Download driver button allows you to download the latest SolidWorks certified driver. On the Problem Capture tab. If your driver is out of date. To write an explanation of the problem. • A new Check KB button is added to access the Knowledge Base in the Problem Capture Details dialog box. wizard-based configuration process and eliminates the need for dongles.dll from the Web site. All users at your site can share this full download file set to install on any computer. not just the files required to update the computer on which you are running the installation. 15 . This file set includes all files included on the DVD for that release. Downloading the Full Release File Set Using SolidWorks Installation Manager. type a summary of the problem. SolidWorks Rx cannot access the online graphics card database due to this error. and uninstall actions. SolidWorks Rx Diagnostics for Graphics Card and Driver You can now determine whether your graphics card is supported and your driver is up to date using the Diagnostics tab in SolidWorks Rx. If you encounter problems with downloading a library named GfxDbMash. SolidNetWork License Activation SolidNetWork License Manager now uses SolidWorks license activation technology. Service Pack Installation Changes Beginning in SolidWorks 2010. This problem might be related to a proxy server or certain firewall restrictions. This patch support reduces file sizes and processing time when performing install. click Describe Problem. recreate the problem by clicking Begin Recording. which allows a simple. • A new Troubleshoot tab is added where you can view common solutions to the listed areas using the SolidWorks Knowledge Base. you can now download the full file set for the release. Click Check KB to check the Knowledge Base if similar issues have already been reported. a warning message is displayed. installing a new Service Pack release upgrades the latest version of the corresponding major release. particularly for Service Pack releases. The following enhancements are made to improve the workflow for SolidWorks Rx: • The Diagnostics tab is updated to include links to new graphics card diagnostics.
You can use the SolidWorks Task Scheduler (SolidWorks Professional) to convert multiple files from an earlier version to the SolidWorks 2010 format. After you convert files to SolidWorks 2010. In the Task Scheduler: • Click Convert Files and specify the files or folders to convert. Click Windows Start. then All Programs > SolidWorks 2010 > SolidWorks Tools > SolidWorks Task Scheduler. use the utility provided with Enterprise PDM. use Convert Workgroup PDM Files. • For files in a SolidWorks Workgroup PDM vault. 16 .Administration Converting Files to SolidWorks 2010 Opening a SolidWorks document from an earlier release can take extra time. For files in a SolidWorks Enterprise PDM vault. After you open and save a file. subsequent opening time returns to normal. you cannot open them in older SolidWorks versions.
or reorder the toolbar buttons. • Select the Commands tab to add. To customize the Heads-Up View toolbar. when you click Move with Triad from the shortcut menu. 17 . You can also show or hide the Heads-Up View toolbar by selecting or clearing View > Toolbars > View (Heads-Up). click Tools > Customize and select the Toolbars tab: • Select or clear View (Heads-Up) to show or hide the toolbar. remove.2 User Interface This chapter includes the following topics: • • • • • • • • • Heads-Up View Toolbar Customization Context Toolbars Instant3D Enhancements Mouse Gesture Support PropertyManager Improvements Graphics Area Controls Improvements Larger Icons for Windows Vista Data Migration Tab in CommandManager Touch and Multi-Touch Support Heads-Up View Toolbar Customization You can customize the Heads-Up View toolbar with different setups for modeling and drawing. rulers now appear with the triad so you can move components to a defined location. Context Toolbars Context toolbars appear when you right-click the following entities in drawings: • • • • Components Drawing views Edges Vertices Instant3D Enhancements In assemblies.
down.User Interface You can use the triad to edit a Move Face feature (Translate or Rotate type) that was created with Instant3D triad. Once you learn command mappings. a guide appears. showing the command mappings for the gesture directions. The triad appears when you select the feature in the graphics area. To activate a mouse gesture. right-drag in one of four directions: up. from the graphics area. similar to a keyboard shortcut. Mouse Gesture Support Mouse Gestures You can use a mouse gesture as a shortcut to execute a command. The guide highlights the command you are about to select. Drawings Guide With Eight Gestures Assemblies Guide with Four Gestures 18 . When you right-drag. left or right. you can use mouse gestures to invoke mapped commands quickly.
select All Commands. or assemblies. right-click and drag straight down. To view or edit the current mouse gesture assignments. Mouse Gestures for Sketches and Parts In this example. and sketches. To use mouse gestures with assemblies. drawings. adding a dimension. The mouse gesture guide highlights the rectangle sketch tool icon. The rectangle sketch tool is mapped to the straight down mouse gesture . click Tools > Customize. Click File > New and double-click Part 2. parts. From the Mouse Gestures tab. and from the Mouse Gestures tab. 4. select 8 gestures and click OK. (Sketch toolbar) and select the Front Plane to start the sketch. parts. Before selecting a highlighted command. assemblies. In the graphics area. click Tools > Customize. From the Customize dialog box. Sketching the Part First you open a part and use a mouse gesture to invoke the rectangle sketch tool. Click Sketch . Actions you perform with mouse gestures include: • • • • Sketching a rectangle and a circle Saving the sketch Dimensioning the sketch Changing the view of the extruded part To see the mouse gesture command mappings for sketches. with the cursor inside the guide. select the Mouse Gestures tab. you create a simple part by creating a sketch. and extruding it. To enable eight mouse gesture directions. Drag through the highlighted rectangle sketch tool.User Interface You can customize up to eight gestures each. click Tools > Customize. for drawings. 3. and Show only commands with mouse gestures assigned. 1. you can drag through another command to select it. 19 . right-drag in the graphics area away from components to avoid component rotation or press Alt + right-drag. 5.
2. Invoking the Circle Sketch Tool Next you invoke the circle sketch tool with a mouse gesture. Click to set the radius and complete the circle. Your cursor is a sketch pencil. The circle sketch tool is mapped to the straight right mouse gesture . Invoking the Dimension Tool Next you invoke the dimension tool with a mouse gesture and save the sketch. The Circle PropertyManager appears. 6. 7. Center a circle within the rectangle. The save sketch 1. ready to draw a centered rectangle. through the highlighted circle sketch tool. . Left-click and drag to stretch a rectangle from the center of the graphics area. 8. Click again to complete the rectangle. Right-click and drag straight up through the highlighted dimension sketch tool. 3. The dimension sketch tool is mapped to the straight up mouse gesture tool is mapped to the right diagonal up mouse gesture . 1. 20 .User Interface The Rectangle PropertyManager appears. Right-click and drag to the right. Click Center Rectangle .
User Interface
2. Select the two upper corners of the rectangle and click to place the dimension. 3. Click to close the Modify dialog box.
4. Right-click and drag up in the right diagonal direction to save the sketch.
Extruding the Sketch and Viewing the Part The back view command is mapped to the left diagonal down mouse gesture . Next, to complete the part, you extrude the sketch, using a mouse gesture to display the back view. 1. Click Boss/Base (Features toolbar). The Extrude PropertyManager appears. 2. For Depth , enter 0.40in and click .
User Interface
3. Right-click and drag down in the left diagonal direction to display the back view of the part.
PropertyManager Improvements
PropertyManager improvements include: • Retaining settings, group box visibility, and values between uses of the same command across sessions • Automatically transferring focus from one control to another to facilitate the workflow • Using round numbers as default values
Graphics Area Controls Improvements
When you interact with PropertyManagers, graphics area controls, including the following are applied more consistently: • Right-click OK pointers
User Interface
• Right-click Advance pointers Right-click a graphics area Advance pointer to advance through PropertyManager selections when multiple selections are required.
Larger Icons for Windows Vista
When using Windows Vista, 256 x 256-pixel versions of the SolidWorks application and document icons are available, depending on your Windows icon display settings. Large icons appear in various interfaces in the operating system, including Windows File Explorer.
Data Migration Tab in CommandManager
The new Data Migration tab in the CommandManager contains tools to help you migrate solid or surface data. By default, the tab is not displayed in the CommandManager. To turn on the Data Migration tab, right-click a CommandManager tab and click Data Migration.
Touch and Multi-Touch Support
If you install SolidWorks on a touch-enabled computer, you can use flick touch and multi-touch gestures in SolidWorks.
The back, forward, drag, and scroll flick actions are mapped to SolidWorks view rotations. Commands for all other flick actions, for example, Undo, invoke the same command in SolidWorks. For example, flick back corresponds to the left arrow view rotation (15 degrees, by default). When you do a flick action, the default Windows command icon for the action is displayed, even though the commands are mapped to SolidWorks arrow key view rotations. You can also apply multi-touch gestures for zoom, rotate, pan, roll, right-click, and zoom-to-fit operations.
see the product documentation for your device. see SolidWorks Help: Flick and Multi-Touch Actions. 24 .User Interface To learn how to use touch and multi-touch gestures in touch-enabled computers. For more information about the SolidWorks interpretation of touch and multi-touch gestures.
Select or clear Help > Use SolidWorks Web Help to switch between the local and Web-based versions of the help. You can still choose to use local help files (. including next and previous topic buttons and breadcrumb navigation. • Improved topic navigation. Benefits of Web-based help include: • Improved search functionality. By default.3 Fundamentals This chapter includes the following topics: • • • • • • • Documentation for SolidWorks Display States for Parts Custom Properties Reference Planes Viewing Decals in SolidWorks Saving Multiple Documents Normal To Command Documentation for SolidWorks Web-based Documentation Documentation® is now available on the Web for SolidWorks. for example. when you access help. • Ability to provide feedback directly to the documentation team on individual help topics. and guided navigation to help you identify relevant topics. including improved relevancy ranking. SolidWorks Enterprise PDM. New Tutorials New tutorials are available: • SolidWorks • • • • DimXpert Electrical Routing ™ TolAnalyst SolidWorks API C# 25 . and eDrawings . spelling correction. your Internet connection is slow or unavailable.chm) if. short descriptions in search results views. • Up-to-date documentation without the need to download large compiled help (. the Web version of the documentation is displayed in a Web-based viewer.chm) files.
display mode. by right-clicking in the top right corner of the FeatureManager design tree. New Illustration Policy In response to customer requests. features. for example. curves. Click Simulation > Help > Simulation Online Tutorial to access the SolidWorks Simulation tutorials. parting lines. In the past. our documentation now includes more images than in earlier releases. In this release. Display States for Parts You can now specify display states for parts in the same way that you could specify them for assemblies in previous versions of SolidWorks. hide/show.NET • SolidWorks Simulation ® • Design Check for Assembly with Mixed Mesh • Design Check for Connectors Click Help > SolidWorks Tutorials to access the SolidWorks and SolidWorks API tutorials. Part display states control the appearance. and transparency of bodies. ® Hide/Show Transparency X Appearance X X X X X X X X X X 26 . • Open. the location of an item or the general layout of the UI. 30 Minute Lesson Renamed 30 Minute Lesson has been renamed Introduction to SolidWorks to better reflect its scope. by right-clicking in the display pane and mousing over Activate Display State. we include English illustrations in localized documentation when translated text is not required for understanding the concept. reference geometry.Fundamentals • SolidWorks API Visual Basic • SolidWorks API . Display states allow you to toggle quickly between different visual representations of the part without changing configurations. and parts according to the following chart: Display Mode Part Body (solid and surface) Feature Features you can hide (including sketch. faces. which limited the number and type of illustrations we could provide. you can see them: • When the display pane is: • Closed. and routing points) Face If a part contains multiple display states. all images that contained text were localized.
You select geometry and apply constraints to the geometry to define reference planes. Custom Properties The Custom Properties tab of the Task Pane now supports lightweight components. 2. select the face shown. Click . 4. Reference Planes Creating reference planes is now easier. you can view the component's custom properties in the Task Pane. 27 .sldprt. To add a display state. Click Plane (Reference Geometry toolbar). For First Reference . You can now select which of a part's display states to use in an assembly. The new process lets you create more types of reference planes than were previously possible. When you select a lightweight component of an assembly. The software creates a plane that is offset from the selected face. The Message box indicates that the plane is fully defined. The PropertyManager Message box prompts you to select references and constraints. The software creates the most likely plane based on the entities you select. You cannot save changes to lightweight components. Creating Reference Planes 1. Open install_dir\samples\whatsnew\RefGeom\Bracket. You can adjust the offset distance or select another type of reference to use to create the plane.Fundamentals • In the ConfigurationManager under Display States. If you edit a value. the software prompts you to resolve the component. 3. right-click in any blank area in the ConfigurationManager and click Add Display State. See Display States on page 50.
2. 2. 28 . In the PropertyManager. Click Plane (Reference Geometry toolbar). select the vertex shown.Fundamentals Modifying Reference Planes 1. select Flip. Select the curved face shown. Click Shaded with Edges (View toolbar). 3. 4. 5. For First Reference. The plane type Tangent selected. Right-click the plane you created and select Edit Feature . Selecting Points to Create Planes 1. The software creates a plane tangent to the face. select the cylindrical face shown. is The plane extends to become tangent to both faces. 3. Under Second Reference. Click . for First Reference. The plane flips to become tangent with the opposite side of the cylindrical face.
Fundamentals The software creates a plane coincident to the vertex. 29 . The Rebuild Errors message instructs you to replace the selection with a point or plane. 5. Select the endpoint of the edge. The plane type Coincident is selected. indicating invalid selections. select an edge approximately as shown. The Message box informs you that the current combination of references is not valid. 6. The software creates a plane coincident to both references. select the vertex at the opposite end of the edge. The plane turns red. 4. For Second Reference. For Third Reference.
Viewing Decals in SolidWorks A new menu item lets you see decals in SolidWorks without activating PhotoWorks™. Click . Save Modified Documents. To apply decals. To orient a model normal to the nearest global XYZ coordinates: 30 . 7. The Message box reports that the plane is now fully defined. When saving or closing an assembly or other document that includes modified documents. To display or hide decals. Normal To Command You can use the Normal To command to orient a model normal to the nearest global XYZ coordinates.Fundamentals The software creates a valid plane that is coincident to the three selected references. View Decals (View toolbar) Saving Multiple Documents The dialogs presented when saving or closing multiple documents have been consolidated into a single dialog box. you can do the following from the Save Modified Documents dialog box: • Save all modified documents • Selectively save modified top-level documents • Discard changes to all documents Read-only documents and documents saved by other users during your session are indicated in the dialog box. you must first activate PhotoWorks. as in earlier releases. click one of the following: • View > Decals • Hide/Show Items • View Decals (Heads-up View toolbar).
. double-click Normal To The model aligns with the rotated coordinate system. press the spacebar. the model is aligned normal to the sketch. 31 . see SolidWorks Help: Orientation. with nothing selected. From an open model or 3D sketch. When you apply this method to a 2D Sketch.Fundamentals 1. For more information on the Normal To command. From the Orientation dialog box. 2.
and drawings • When interactive users preselect entities in parts. right-click. methods.4 Application Programming Interface Major enhancements are new interfaces. and C#) when recording a macro • Delay solving of equations until all equations are added • Customize the size of balloons • Hide table columns • Customize tags in hole tables • Get the UV parameters of a curve 32 . VB. You can now: • • • • • • • • Access DimXpert features Include attributes in library features Access tangent lines associated with bend lines in drawings of sheet metal parts Get an array of mates for a component Create generic. 2D parametric. y. and drawings • After all SolidWorks graphics are drawn • Compare two persistent reference IDs to determine if they point to the same SolidWorks data • Create bubble ToolTips for PropertyManager page controls • Add and modify graphics-area dimensions in circular and linear sketch patterns • Get the names of all components in an assembly document before selectively opening the assembly document • Get and set pick points for lofts • Add and purge display states and fire notifications when a display states changes • Create equations for 2D explicit. and z coordinates • Add smart components and insert virtual components in assemblies • Create a new assembly from preselected components • Insert a title block table in a part or assembly • Get sheet and configuration persistent reference IDs • Create a loft body using specified parameters instead of using interactive user selections • Create multiple types of macros (VBA. and 3D curves • Get or set a component reference • Box-select entities • Specify the distance from the section line of the section view • Determine if a sketch is derived • Insert a route line in an explode line or 3D sketch • Rotate or copy 3D sketch entities about a vector or x. properties. and delegates.NET. edges. and vertices in a folded and flattened sheet metal part Fire notifications: • For undo and redo operations in parts. assemblies. and pop-up menus Specify alignment of axes when inserting a coordinate systems mate Find the corresponding faces. assemblies.
and get a component in the context of a subassembly after getting the component in the context of the top assembly • Access feature statistics Click Help > API Help > SolidWorks API Help > SolidWorks APIs > Release Notes.Application Programming Interface • Get a component in the context of the top assembly after getting the component in the context of a subassembly. 33 .
Suppliers get access to their own secure content management system. and review your tags. which makes publishing supplier catalogs fast and easy. comments. To register for a Supplier Services account. browser-based file upload utility. My 3D ContentCentral You can personalize your own workspace on 3D ContentCentral. 34 . You can join this active community of more than a half million CAD users who share and download user-contributed and supplier-certified models and more. Access to these subscription features is online and self service. click Register Now. favorites. and downloads all on your own page.5 3D ContentCentral 3D ContentCentral is a free service for locating. views. and requesting 3D parts and assemblies. or updates. monitor your requests. To register. The Configuration Publisher tool in SolidWorks lets you create rules that define allowable configurations of a model before you upload the model to 3D ContentCentral. downloading. and model preview and edit pages. You can update your profile. and macros. click Register. Click My 3D ContentCentral on 3D ContentCentral to access your personal area. 2D blocks. You can also generate reports about activity in your supplier catalog. This chapter includes the following topics: • • • • Self-Service Catalog Publishing My 3D ContentCentral Request Content 3D ContentCentral Community ® Self-Service Catalog Publishing Supplier Services provides industrial component and OEM suppliers with the tools needed to publish CAD models of their products to the vast 3D ContentCentral community. library features. Click Supplier Services on 3D ContentCentral to explore how to publish your models to the CAD community and to your own Web site. Click 3D ContentCentral to learn more about this service. configuring. add models to your portfolio. See Configuration Publisher on page 55 for more information on how to use the Configuration Publisher tool with 3D ContentCentral.
Click Request Content on 3D ContentCentral to request specific parts. Plus. You can invite colleagues or friends to be your contacts on 3D ContentCentral and stay current with each other's activities in My Updates. Click Updates on My 3D ContentCentral to add contacts and follow your contacts' activities.3D ContentCentral Request Content If you have a specific need. or other content from the community. You can take advantage of the vast user and supplier communities. 35 . assemblies. 3D ContentCentral Community The 3D ContentCentral community is an active group of people who understand design and the advantages of sharing. you can post a request and let the active members respond. you have the ability to request new suppliers.
36 . and volume are available in the tool. In the graphics area. the software applies colors to the components based on the value of the property you are sorting by. Open install_dir\samples\whatsnew\assemblies\visualize\food_processor.sldasm. Properties from SolidWorks Sustainability are also available. You can save the list information in a separate file such as a Microsoft Excel spreadsheet or a text file. density. If you defined noncalculated properties such as Vendor or Status in the component files. Additionally. where subassembly structures are ignored (similar to a parts-only BOM) You can sort the list by one property at a time. you can edit component materials directly from the list. you can access those properties for modification and sorting. Basic calculated numerical data such as component mass. where subassemblies are indented • Flat view. The colors help you to visualize the relative value of the property for each component. you can create customized criteria which are dependent on several numerical values.6 Assemblies This chapter includes the following topics: • • • • • • • Assembly Visualization Mirror Components Virtual Components Component Reference per Instance Display States SpeedPak Mates Assembly Visualization Assembly Visualization Overview Assembly Visualization provides different ways to display and sort an assembly's components in a list and in the graphics area. You can list the components in these ways: • Nested view. ® Activating the Assembly Visualization Tool To activate the Assembly Visualization tool: 1. (See SolidWorks Sustainability Overview on page 182.) If you sort by SW-Material.
(Tools toolbar or Evaluate tab on the The Assembly Visualization tab in the FeatureManager design tree panel contains a list of all components in the assembly. For a complete list of possible icons. 37 . Click Assembly Visualization CommandManager). Visualizing the Assembly To visualize the assembly: 1. The lengths of all the other bars are calculated as a percentage of the highest value. see SolidWorks Help: Assembly Visualization Tab. the longest bar is applied to the component with the highest value. Icons in the list indicate the following: Part Subassembly Description A component with a single instance. sorted initially by file name. A component with multiple instances. all of which are shown. When the value bars Bars are on. where subassembly structures are ignored (similar to a parts-only BOM) / Show/Hide Value Turns the value bars off and on. You can click to change the appearance of the list. where subassemblies are indented • Flat view. At the top of the last column.Assemblies 2. / Flat/Nested View Switches between: • Nested view. click Mass to sort the components by mass.
To return to the original two sliders. You can right-click a color slider and change its color or delete it. The heaviest components are shown in red. the lightest in blue. To add another color to the spectrum: a) Click in the blank area to the left of the vertical bar.Assemblies 2. The vertical bar displays a spectrum of colors from red to blue. click the vertical bar. right-click any slider and click Reset all. 38 . and the others in shades in between. A yellow slider is added to the spectrum. b) In the Color dialog box. In the graphics area. the components change to the color that is beside their entry in the Assembly Visualization panel. You can move the color sliders up and down to modify the spectrum. On the left side of the panel. select (yellow) and click OK. The parts change color in the graphics area. The colors indicate the relative mass of the components. 3.
the heaviest component. Under the column headers. Return the bars to their original positions: a) Right-click the top bar and click Roll to Top. b) Right-click the bottom bar and click Roll to End. 6. In the graphics area. The three components that weigh the least are hidden. Note that the spectrum adjusts to the visible components. gear-caddy. is hidden.Assemblies 4. Changing the Sorting Property You can change the property used to sort components. drag the horizontal bar down and position it below gear-caddy. showing their relative values. 5. At the bottom of the list. You can select custom properties defined in the component files and create equations involving those properties. drag the horizontal bar up and position it above shaft gear insert. 39 .
To change the sorting property: 1. Click the arrow to the right of Mass. The flyout list contains some commonly used properties. You can also select from any other custom properties already defined in the components, as demonstrated in the following steps. 2. Click More. 3. In the dialog box, in Properties, select Cost. Cost appears in Column header. 4. Click OK. Cost appears at the top of the property column, and the components are sorted from highest to lowest cost. In the graphics area, the colors of the parts change accordingly.
Creating an Equation for Sorting
Some components are in the assembly multiple times. For example, there are five rubber feet on the bottom of the base plate. Component rubber feet appears at the bottom of the list because it costs the least.
Now create and sort by an equation that calculates the extended cost for each part. 1. Click the arrow to the right of Cost. 2. Click More. 3. In the dialog box: a) In Properties, select Cost. b) In Column header, type Extended Cost. c) Select Use Formula. Cost appears in the equation box.
d) In the equation box, type *. e) In Properties, select Quantity. The equation defines extended cost as cost multiplied by quantity. 4. Click OK. Extended Cost appears at the top of the property column and the components are sorted from highest to lowest extended cost. Component rubber feet moves up to the middle of the list. In the graphics area, the colors of the parts adjust accordingly.
You can right-click in the header area and select Unit Precision to change the number of decimal places. 5. Save the assembly. The custom column data is saved so it will appear the next time you access Assembly Visualization in this model. You can save the list information in a separate file. 6. In the header area of the list, right-click and click Save as. 7. In the Save As dialog box: a) For Save in, select My Documents. b) For File name, type my_food_processor. c) For Save as type, select Text(*.txt). d) Click Save. The text file contains a list with the information from the Assembly Visualization panel. 8. At the top of the panel, click Exit Visualization The panel closes and its tab disappears. .
Mirror Components
Enhancements: • A MirrorComponent feature is added to the FeatureManager design tree to maintain the position of mirrored components relative to seed components. • You can create an opposite-hand version as a derived configuration of the component you are mirroring. • The Mirror Components PropertyManager includes changes that simplify the workflow.
In this example, you mirror a two-component subassembly. You create opposite-hand versions of the subassembly and one component, and save them as derived configurations. You create a second instance of the other component.
Making Mirror Selections
First you select the mirror plane and the components to mirror. 1. Open install_dir\samples\whatsnew\assemblies\mirror\vise.sldasm.
2. Click Mirror Components (Assembly toolbar) or Insert > Mirror Components. 3. In the PropertyManager: a) For Mirror plane, in the flyout FeatureManager design tree, select Right Plane . b) For Components to Mirror, select the subassembly jaw_and_support.
4. Click Next . A preview of the mirrored components appears.
Setting Orientation
For each component, you specify whether to create an opposite-hand version or just a copy. For copies, you specify orientation.
Because the jaw is symmetrical. In support. The icon appears beside jaw_and_support-1 and each of its components to indicate that you are creating an opposite-hand version for each item. Expand MirrorComponent 4. . you do not need to create an opposite-hand version. 2. Instead. you create an opposite-hand version of support and a copy of jaw. Select Create new derived configuration in existing files. 43 . and to clear the icon . 3. on the ConfigurationManager tab. If a message about mates appears.sldprt. Under jaw_and_support. you create an opposite-hand version of the subassembly jaw_and_support. select jaw-1. expand jaw_and_support-1. and then expand jaw_and_support. to cycle through the four possible orientations and select Correct 6. Click Create opposite hand version . right-click support and click Open Part 5. For its components. click OK. MirrorComponent appears in the FeatureManager design tree. you can create it in a new file or as a new derived configuration in the existing component file. 4. . expand Default. Click Next . Under Orient Components. 1. 3. MirrorDefault is the new opposite-hand configuration you created. 2. Click .Assemblies In this example. The subassembly and the support component appear under Opposite Hand Versions. 1. create a copy of the jaw and orient it as needed. Click Create opposite hand version 5. Under Orient Components. Creating Mirrored Configurations When you create an opposite-hand version of a component. Click Reorient the correct one.
Editing a Mirror Component Feature You can edit a mirror component feature. In the PropertyManager. Click Next . select clamp-1. Close the part and click No when asked if you want to save changes. right-click clamp and click Unsuppress A clamp appears on the model. Click Reorient and if necessary to obtain the correct orientation. you do not need to create an opposite-hand version. select the clamp in the graphics area. Click . Another instance of clamp is added to the assembly. 6. 1. 44 . 7. Because the clamp is symmetrical. . 2. In the FeatureManager design tree. 3. Under Orient Components. 4. for Components to Mirror. 5.Assemblies Default MirrorDefault 6. Right-click MirrorComponent and click Edit Feature .
Open install_dir/samples/whatsnew/assemblies/virtual/conveyor. 2. Click Insert > Component > Existing Part/Assembly.sldprt. open rod_clevis. 1. select Make Virtual. and click to place it in the graphics area. 3. Under Part/Assembly to Insert. In the PropertyManager. The assembly contains two components: a rail subassembly and a pin.sldasm.Assemblies Virtual Components Making External Components Virtual You can make externally saved components virtual. You can make components virtual while you insert them or after you insert them into the assembly. under Options. 4. Existing references are ignored and the component is renamed. 45 . click Browse. which breaks the link to the external component file.
The name of the pin is changed to [Copy of pin . When you move or copy a virtual component to another assembly. The virtual component is renamed [pin_special^conveyor]. Click OK. Open install_dir/samples/whatsnew/assemblies/virtual/support_assembly_2. The software warns you that making a component virtual breaks the link to the external file. In either the FeatureManager design tree or the graphics area. select [bumper^support_assembly_2] and drag it to the graphics area of conveyor. Partn.sldasm are visible. Naming Virtual Components The name of a virtual component now always includes its parent assembly's name. 1. In the FeatureManager design tree of support_assembly_2. 2. 1.0^conveyor]. right-click the pin and click Make Virtual. The format of the default name for virtual components remains the same: [Partn^Assembly_name] However. In the FeatureManager design tree.0^conveyor] and click Rename Part. now you can rename only the first name.sldasm.75x3.Assemblies The software warns you that making a component virtual breaks the link to the external file. Assembly_name.sldasm.sldasm. Existing references are not copied.sldasm and support_assembly_2.75x3. and not the surname. 7. Click OK. Now make the pin a virtual component. Click Window > Tile Horizontally so that both conveyor. Type pin_special and press Enter. right-click [Copy of pin . The copy is not linked to the original virtual component. The part is added to the assembly as a virtual component named [Copy of rod_clevis^conveyor]. 46 . 6. 5. the surname changes to reflect that assembly's name. The assembly contains a virtual component named [bumper^support_assembly_2]. 3. which ensures that the name of the virtual component is unique. and the copy is given a new name. Copying Virtual Components You can copy virtual components between assemblies. 2.
In the graphics area. 1. b) Select [shaft^RH_rail].sldasm.sldasm and maximize the window for conveyor. 2. select the shaft and try to drag it. The component is renamed to [Copy of shaft^conveyor] to reflect that it is now a component of conveyor. In the FeatureManager design tree: a) Expand the subassembly RH_rail. Close support_assembly_2. Existing references are ignored and the component is renamed. The Assembly Structure Editing dialog box appears. Click OK. drag it down.Assemblies The software warns you that copying a virtual component to another file breaks the link to the original file. and drop it when the pointer changes to . select the shaft and drag it. Click OK. In the graphics area. 47 . 4. the component will be renamed and links to the original component will be broken. 4. 6. 5. 3.sldasm and is renamed [Copy of bumper^conveyor]. You cannot move the shaft because it is a virtual component created in the context of the subassembly RH_rail. It informs you that the shaft's InPlace mate will be deleted and its in-context sketch will go out of context.sldasm. The software warns you that if you move a virtual component to another assembly. The part is copied into conveyor. It is constrained by an InPlace mate and its sketch contains references to another component in the subassembly. Click Move. Moving Virtual Components You can move virtual components within the hierarchy of the FeatureManager design tree.
bolt holes. In the dialog box. The new part. type gasket1 and click Save. 3. saves new in-context components in the assembly file as virtual components.sldasm.Assemblies The shaft moves because it is no longer constrained by its Inplace mate and in-context sketch. Open install_dir/samples/whatsnew/assemblies/virtual/flanges. Click Tools > Options and click Assemblies. appears in the FeatureManager design tree. for File name. Click Insert > Component > New Part. Now you select a face on which to position the new part. Click OK. 2. Select the face of the three-bolt flange. Editing focus changes to the new part and a sketch opens on the selected face. Saving New In-Context Components You can specify the default behavior for saving new in-context components as: • External files (same as in SolidWorks 2007 and earlier) • Virtual components (same as in SolidWorks 2008 and 2009) A new option in System Options . 7. 4. 8. Select Save new components to external files. prompts you to name and save new in-context external files components to external files. If cleared. The Save As dialog box appears so you can save the new part to an external file. gasket1. To save new in-context components in external files: 1. and center hole. 5. Use Convert Entities to create sketch entities that reference the edges of the flange.Assemblies sets the default behavior: Save new components to If selected. 6. 48 .
you can also link the value of a component reference to the text of a balloon. if you want to change the default behavior back to saving as virtual components. click Component Properties . return to System Options . you can assign a different value for Component Reference for each instance of a component in an assembly. right-click a component. For example. you can use Component Reference to store the reference designators for an electrical harness or printed circuit board assembly. 49 . Extrude the sketch to a depth of 10 to create the part. In drawings. Click in the Confirmation Corner to return editing focus to the assembly. 11.Assemblies and clear Save new components to external files. The value appears in braces { } at the end of the component name string in the FeatureManager design tree. 10. and set a value for Component Reference. Close the sketch. After completing the above example. Component Reference per Instance In the Component Properties dialog box. you can show the instances as separate line items in a BOM.Assemblies 9. When different instances of the same component have different values for Component Reference. In assemblies.
In assemblies or drawings.Assemblies In SolidWorks Routing. To link balloons to component reference values. You can now assign display states to parts. you can now specify which of a component's display states to use in the assembly. You can override the default for each instance of the component. when inserting a column in a BOM. In drawings. each instance of a component (part or subassembly) is shown in the display state that was current when the component was last saved. You can use different display states for each instance. when inserting balloons. The override is stored in the parent assembly's display state. Display States While editing an assembly. select COMPONENT REFERENCE for Column type. the drawing must contain a BOM with a COMPONENT REFERENCE column. right-click a highlighted component and click Component Display State > display_state_name. select Component Reference for Balloon text. By default. See Display States for Parts on page 26. without changing the instance's configuration. To specify a different component display state. do one of the following: • In the Display Pane. 50 . you can assign values automatically when importing a P&ID document.
View Mates now appears in a separate window. select from the list of display states currently available in the component. In the Mated Entities PropertyManager: 51 .Assemblies • In the Component Properties dialog box. Mates Relocating Components View Mates now indicates which mates are in the path to ground. under Referenced Display State. A new icon. to help you understand which mates you need to modify to be able to relocate the component. Replacing Components More guidance is provided to let you know which mate references need to be replaced. . you can now select a replacement component from a list of open files. A horizontal bar separates the positioning mates from other mates. indicates mates that are in the path to ground. SpeedPak You can now create a SpeedPak configuration for an assembly even when the assembly contains subassemblies that have SpeedPak configurations active. These positioning mates are shown first on the list. In the Replace PropertyManager.
The pointer indicates a potential mate between two coordinate systems or between a coordinate system and an origin. or show the entire assembly. you can select Align axes on the popup toolbar. you can: • Show the replacement part alone. • Toggle mate alignments. • Skip mates. show the replacement part with related parts. you can select coordinate systems and origins as reference entities and choose to align axes. • Delete mates. 52 .Assemblies • A popup toolbar helps you to navigate through existing mates as you replace mate references. From the popup toolbar. Coincident Mates You can create coincident mates between a coordinate system and an origin. You can use SmartMates to create mates involving coordinate systems and origins. • Undo selections and operations. • A view of the original component is displayed in a separate window. The missing mate entity is highlighted. When you drop a component to create a coordinate system SmartMate. Mate References SmartMates For mate references. Coordinate System Mates Mates involving coordinate systems have been enhanced.
Previously. • To display the CircuitWorks feature tree. which replaces the Edit Component Information dialog box. . CircuitWorks rebuilt the entire assembly for any change. This chapter includes the following topics: • • • • User Interface Updating Assemblies Importing Non-CircuitWorks Assemblies from SolidWorks PADS Support User Interface The CircuitWorks user interface has been enhanced to better integrate with SolidWorks. the CircuitWorks feature tree is now available in SolidWorks. • To display the Annotate Components PropertyManager. For example. Also. deleting. or moving components. which replaces the Locate Components dialog box. right-click a feature in the CircuitWorks feature tree and click Properties. To update an assembly. See CircuitWorks Help for details about these changes. click the CircuitWorks tab. • To display the Properties dialog box. and click Build Model See CircuitWorks Help: Updating Assemblies. make changes to the corresponding data file in CircuitWorks. 53 . which replaces the Annotate Components dialog box. Importing Non-CircuitWorks Assemblies from SolidWorks Importing SolidWorks PCB assemblies that were not created in CircuitWorks has been improved. CircuitWorks now displays build progress in a pane at the bottom of the CircuitWorks window instead of in a separate window.7 CircuitWorks Available in SolidWorks Premium. Updating Assemblies CircuitWorks can now update an assembly that is open in SolidWorks when you make minor changes in CircuitWorks such as adding. click Annotate Components (CircuitWorks toolbar). open the assembly in SolidWorks.
® 54 . select an option for If no correctly named sketches are found. click the CircuitWorks application menu and click Options • In SolidWorks. . Select the top face of the board component and click Continue. you can specify the assembly orientation by selecting the planar face that represents the top of the board component. CircuitWorks can use silhouette edges to determine component shapes. To control silhouette edge recognition. click Export to CircuitWorks If the assembly was not created by CircuitWorks. click CircuitWorks > CircuitWorks Options.SolidWorks Export. do one of the following: • In CircuitWorks. click Import Model (Tools toolbar).CircuitWorks Selecting the Board Component and Orientation When exporting from SolidWorks. See CircuitWorks Help: Export Rules and CircuitWorks Options . Using Silhouette Edges to Determine Component Shape If appropriate sketches are not available. • From SolidWorks. See CircuitWorks Help: Exporting SolidWorks Models to CircuitWorks. (CircuitWorks toolbar). PADS Support The CircuitWorks reader for Mentor Graphics PADS ASCII (. do one of the following: • From CircuitWorks. On the SolidWorks Export page of the CircuitWorks Options dialog box.asc) now imports files faster and supports plated holes. the Select Orientation dialog box appears. To import an assembly into CircuitWorks.
Other enhancements: • You can configure custom properties. You set attributes for each control in the pane on the right. You upload models to 3D ContentCentral directly from the dialog box. now you can create a single-row design table that includes all the variables you need. In addition to its previous functionality.8 Configurations This chapter includes the following topics: • • Configuration Publisher Modify Configurations Configuration Publisher The Create PropertyManager dialog box has been renamed to Configuration Publisher. you drag controls (list boxes. • You can create PropertyManagers for assemblies. you can still build a PropertyManager that enables you to select a configuration when you place the model in an assembly. Alternatively. You can now use rules to define the configurations of a model. In the dialog box. In the Configuration Publisher dialog box. Then. 55 . As in previous releases of SolidWorks. you define the interface for specifying configurations. Your model must contain a design table (single or multiple rows). you create rules to define the configurations. On 3D ContentCentral. You assign values for the variables and define relationships between them. in the Configuration Publisher dialog box. it contains only the configuration they specified. your end users select values to build the configuration they want. and check boxes) from the palette on the left into the pane in the center. When they download your model. you can now use the dialog box to prepare models for uploading to 3D ContentCentral. you can define all the configurations in a multiple-row design table. number boxes. As in previous releases of SolidWorks.
outside diameter. At the top of the ConfigurationManager tab. Because the design table has multiple rows.sldprt so you do not overwrite the example file. Building the PropertyManager Now create a PropertyManager for selecting the length. Open install_dir\samples\whatsnew\configurations\rod_multiple. The Configuration Publisher dialog box appears and the design table opens in a separate window. In some configurations. 56 . and hole diameter of the part vary among configurations. right-click the part name and click Configuration Publisher. a control appears in the palette for each parameter in the design table. outside diameter. the model has multiple configurations which are defined in a design table. 1. 3. Accessing the Dialog Box To create a PropertyManager: 1. 2.sldprt.Configurations Starting with Multiple Configurations In this example. The length. Save the part as my_rod_multiple. the hole is suppressed. and hole diameter. hole suppression state. Click the Edit tab in the center pane.
In Name. type Hole. 5. Under Control Visibility: a) In Visibility Parent. PropertyManager appears in the ConfigurationManager. b) For Show. 11. d) For Hole Diameter. In the PropertyManager preview: a) For Outside Diameter. double-click in Name and type Length.5. c) Select Hole. 3. Drag Hole Diameter@Sketch2 from the palette and drop it below Hole in the center pane. Click Apply. 8. 6. Configuration changes to Rod-10M-H45. List1 appears in the center pane and its control attributes appear in the right pane. Under Control Attributes. the part changes to the selected configuration. Click Update Model. 1.Configurations 2. under Control Attributes. 4. In preview mode. Drag Rod-Diameter@Sketch1 from the palette to the center pane. The PropertyManager is saved. Previewing the SolidWorks PropertyManager You can preview the PropertyManager to see how it will appear in SolidWorks. double-click in Name and type Outside Diameter. select 20. In Name. select 10. there might be a delay as you select values. click the SW Preview tab. In the center pane. 3. The interface as it will appear in the SolidWorks PropertyManager is displayed. select Hole. In the right pane. set: • Checked to • Unchecked to The Hole Diameter control will be available only when Hole is selected. Drag Rod-Length@Rod from the palette and drop it below Outside Diameter in the Edit pane. Outside Diameter appears on the control in the center pane. 9. b) For Length. 7. 2. In the graphics area. select 4. 10. 57 . Drag $STATE@Hole from the palette and drop it below Length in the center pane. Now make the Hole Diameter control available only when Hole is selected. Now add the check box that controls the suppression state of the hole. type Hole Diameter.
When you have a real model to upload. select 10. c) Clear Hole. 2. 3. Click Update Model. the part changes to the selected configuration. 4.Configurations Previewing the 3D ContentCentral Interface You can preview the interface to see how it will look in 3D ContentCentral. and Configuration changes to Rod-10L-N. select 10. Click the Edit tab. b) For Length. 1. Click Close and click Yes to save. Click the 3DCC Preview tab. click Upload to 3D ContentCentral to log in to your account and initiate the upload process. 5. In preview mode. In the 3D ContentCentral preview: a) For Outside Diameter. there might be a delay as you select values. In the graphics area. 58 . The interface as it will appear in 3D ContentCentral is displayed. The Hole Diameter control disappears. Do not upload the example model.
the software asks if you want to autocreate it. At the top of the ConfigurationManager tab. You create rules to define the configurations. you must have a Supplier Services account registered on 3D ContentCentral. see Register Now on www. Save the part as my_rod_single.sldprt. generic controls for List. Open install_dir\samples\whatsnew\configurations\rod_single. Supplier Services accounts are free. • For more information about Supplier Services accounts. Accessing the Dialog Box The Configuration Publisher process requires a design table. To create a PropertyManager: 1. Because the design table has only a single row. see Supplier Services on www. right-click the part name and click Configuration Publisher.3dcontentcentral. • To register for a Supplier Services account. The design table contains a single row of values for the parameters of the model.sldprt so you do not overwrite the example file. You assign values for the variables and define relationships between them.3dcontentcentral. the model has a single configuration which is defined in a design table. If your model does not contain a design table. The Configuration Publisher dialog box appears and the design table opens in a separate window. 2. 3.Configurations Before uploading a model.com. and Checkbox appear in the palette. Starting with a Single Configuration In this example. Number. 59 .com.
5. under Control Attributes: a) Double-click in Name and type Outside Diameter. select Rod-Diameter@Sketch1. List1 appears in the center pane and its control attributes appear in the right pane. Drag a List control from the palette to the center pane. outside diameter. type the following in the cells: 60 . c) In Type. hole suppression state. d) In Range Requirements. You also specify the increment between values in each range. In the right pane. 4. 2. and hole diameter. In Range Requirements. Now define the range of values for rod length that correspond to each outside diameter. b) In Design Table Variable. 3. Under Control Attributes: a) Double-click in Name and type Length. Drag a Number control from the palette and drop it below Outside Diameter in the center pane. Click Edit in the center pane. type the following in the cells: You can press Tab and Shift + Tab to move between cells. c) In Data Parent. select Rod-Length@Rod. select List.Configurations Building the PropertyManager Now create a PropertyManager for selecting the length. b) In Design Table Variable. select Outside Diameter. d) In List Values. a table appears with rows for each value of Outside Diameter. 1.
11. type the following in the cells: Now make the Hole Diameter control available only when Hole is selected. Drag a List control from the palette and drop it below Hole in the center pane. you want the check box to be available when Outside Diameter is set to 5. The Hole check box will not be visible when Outside Diameter is set to 7. Under Control Attributes: a) In Name. In this example. e) In List Values. Under Control Attributes: a) In Name. Under Control Visibility. b) For Show. select Hole. Because the check box is not needed. c) In Type. select None. you can specify that it not be visible. 9. 7. Drag a Checkbox control from the palette and drop it below Length in the center pane. set: • Checked to 61 . select Outside Diameter. type Hole Diameter. c) In Data Parent. 10. 6. select Hole-Diameter@Sketch2. select List. Under Control Visibility: a) In Visibility Parent. in Visibility Parent. d) In Data Parent. you want the hole to be unavailable for all configurations with Outside Diameter set to 7. b) In Design Table Variable.Configurations Now add a check box to control the suppression state of the holes. 10. A table with a column for each value of Outside Diameter appears. but not when it is set to 7. select $State@Hole. Clear the check box for 7. 12. or 13. select Outside Diameter. type Hole. b) In Design Table Variable. In this example. 8. Now define the values for the hole diameter.
In the PropertyManager preview: a) For Outside Diameter.5. type 20. appears below the Length box. Click Apply. Click Update Model. The PropertyManager is saved. Click the SW Preview tab. d) For Hole Diameter. there might be a delay as you select values. 2. PropertyManager appears in the ConfigurationManager. Previewing the 3D ContentCentral Interface You can preview the interface to see how it will look in 3D ContentCentral. 10-50(by increments of 10). 3. The range of acceptable length values and increments.Configurations • Unchecked to The Hole Diameter control will be available only when Hole is selected. In the 3D ContentCentral preview: a) For Outside Diameter. 62 . 1. c) Select Hole. appears below the Length box. 20-80(by increments of 15). b) For Length. Click the 3DCC Preview tab. the part changes to the selected configuration. select 10. In the graphics area. In preview mode. The range of acceptable length values and increments. there might be a delay as you select values. select 4. select 5. 13. 2. In preview mode. Previewing the SolidWorks PropertyManager You can preview the PropertyManager to see how it will appear in SolidWorks. 1.
The Configure Component PropertyManager opens. 3. Placing the Part in an Assembly 1. d) For Hole Diameter. 3. c) Select Hole.Configurations b) For Length. Click Close. Click . select 5. 63 .5. Under Parameters: a) For Outside Diameter. 4. the part changes to the selected configuration. Do not upload the example model. type 70. 2. 5. select my_rod_single and click in the graphics area to place the part. In the Begin Assembly PropertyManager. b) For Length. Click Update Model. type 20. c) Clear Hole. select 13. Save the part. In the graphics area. Click the Edit tab. The specified configuration of the part appears in the assembly. 6. but do not close the file. 4. Open a new assembly.
5. Save the assembly as rod.sldasm. In the Save Modified Documents dialog box, click Save All. In my_rod_single.sldprt, the configuration you specified in the assembly appears in the ConfigurationManager as Default_New2.
Modify Configurations
The Modify Configurations dialog box has been enhanced. You can: • • • • • • • • Rename features and dimensions. Add and remove feature parameters from the table. Configure the material of parts. Create, edit, and delete configuration-specific custom properties. Unconfigure parameters. Save views of the table. Rearrange columns in the table. Edit and navigate the table similarly to how you would in Microsoft Excel. For more information about editing and navigating tables, see Tables on page 82.
Configuring Material
1. Open install_dir\samples\whatsnew\configurations\flange_1.sldprt. The part has three configurations.
2. In the FeatureManager design tree, right-click Material and click Configure Material . The Modify Configurations dialog box appears with a Material column. 3. Under Material, select a material for each configuration:
Configuration 12.5 20 25 4. Click Apply. 5. Click <Enter Name> and type Material. 6. Click Save table view .
Material Brass Copper Plain Carbon Steel
The table is saved in the Tables folder on the ConfigurationManager specified materials are applied to each configuration. Do not close the dialog box yet.
tab. The
Configuring Custom Properties
1. At the bottom of the Modify Configurations dialog box, click Hide/Show Custom Properties . The Custom Properties column appears, and contains a New Property column. 2. Right-click New Property and click Rename. 3. Type Supplier and press Enter. 4. Type values for each configuration: Configuration 12.5 20 25 Supplier ABC Co. XYZ Co. BCD Co.
Now configure some existing properties. 5. Click at the top of the Custom Properties column and select Cost and LeadTime.
You can create additional new properties by selecting **New Property from the list. 6. Click in a blank area of the dialog box. Columns appear for Cost and LeadTime. 7. Type values for each configuration:
Configuration 12.5 20 25 8. Click Save table view 9. Click OK. .
Cost 6.00 7.00 8.00
LeadTime 3 days 4 days 5 days
Editing a Table View
In this example, you edit a saved table view and: • • • • Rename a sketch feature Add a sketch dimension Move a column Unconfigure a parameter
1. In the ConfigurationManager, expand Tables . The table you just created (Material) appears with two others that were saved previously. 2. Right-click Base and click Show Table. The table view opens in the Modify Configurations dialog box. It contains three dimensions from Sketch1. 3. In the dialog box, double-click Sketch1.
4. Type Base Sketch and press Enter. The sketch name changes to Base Sketch in the dialog box.
5. Click Apply. The sketch name updates in the FeatureManager design tree. Now add another sketch dimension. 6. Beside Base Sketch, click , select J, and click in a blank area. A column for J appears, and the dimension appears in the graphics area.
67 . Click Apply. Click Save table view 13. . The dimension appears in the graphics area. Now unconfigure a parameter. 12. The active configuration's value for N is applied to all configurations. 11. Under J: a) For 20. Select the column heading J. drag the column and drop it to the left of column L. Now rearrange columns in the table. Click OK. b) For 25. 10.Configurations 7. 8. type 90 and press Enter. 9. Right-click column heading N and click Unconfigure. Click column heading N. type 100.
5 20 25 68 .Configurations 12.
When you select a related command. 69 . Validation Against ANSI/ISO/JIS Drafting Standards The following enhancements have been implemented: • Drafting standards (ANSI. Click Tools > Design Checker. provided you have installed it and are running SolidWorks Professional or SolidWorks Premium. GOST and GB) are provided with a set of built-in drafting standard files. DIN. ISO. The Design Checker tab is added to the Task Pane. You can load any of the provided drafting standards in SolidWorks Design Checker to view its customized document settings. You can set the location of Design Checker files in Options > File Locations . BSI. The file location of the drafting standards is install_dir\dsgnchk\Data. Validation using these files ensures that the SolidWorks document conforms to the corresponding drafting standard. the add-in loads dynamically. A Design Checker toolbar button is added to the Evaluate tab of the CommandManager. User defined. JIS. in the Dimensioning Standard Check dialog box lets you specify a name for the user-defined drafting standard. This chapter includes the following topics: • • • • • • • Integration of Design Checker Validation Against ANSI/ISO/JIS Drafting Standards One-Button Push to Correct All Errors UI Enhancements Virtual Sharp Check Task Scheduler Option for Autocorrection Samples of Industry Vertical Custom Checks to 3D ContentCentral Integration of Design Checker The user interface for SolidWorks Design Checker has been fully integrated into toolbars and menus of the SolidWorks software. • A new check box.9 Design Checker Available in SolidWorks Professional and SolidWorks Premium.
swstd file. your preferred values override the default autocorrection values specified in the selected *. Activate Virtual Sharp under Document Checks . • The Update and Recheck button is removed. Virtual Sharp Check The Virtual Sharp check verifies that your document uses the correct style of virtual sharp. When you select Auto Correct All. Selective correction of failed entities is available with the Correct Selected option. Recheck Document. allows you to revalidate your document without running a correction. Auto Correct All. and specify the desired values under Preferred auto correction values.Design Checker One-Button Push to Correct All Errors A new tool. • A new tool. Select a criticality factor among Critical . • Only the list of failed checks is shown. The parameters that support checks are automatically corrected according to the selected *. UI Enhancements Enhancements for the Design Checker interface include: • You can now specify your preferred correction values for parameters that support checks. or Low .swstd drafting standard file. The active document passes the check when it satisfies the specified virtual sharp style criterion. 70 . Create a parameter check in the Design Checker module. Medium . High . The criticality factor icon is displayed next to each check definition. lets you correct all of the errors shown in Design Checker. • A new criticality factor box is added to the user interface.
Design Checker Task Scheduler Option for Autocorrection A new task in SolidWorks Task Scheduler (SolidWorks Professional) allows Design Checker to automatically correct all errors. Design Checker can correct all failures for which it supports autocorrection. Click Design Checker on the SolidWorks Task Scheduler sidebar. 71 . Samples of Industry Vertical Custom Checks to 3D ContentCentral Design Checker provides samples of industry vertical custom checks which are added to 3D ContentCentral. The corrected document is saved at the location of the original document for ease of comparison.
Previously. For example. discrete values 30mm. The Design Study iterates on the values specified for L. and Volume. Optimization You specify values for each variable. you specify values of 75mm. and 80mm for the height (H). R. 30mm. For a constraint. and 80mm for the height (H). 72 .10 Design Studies You can evaluate and optimize models by using a Design Study. The software runs iterations of the values and reports the optimum combination of values to meet your specified goal. You specify a Volume sensor to monitor the volume of the water body. the Design Study functionality was available only in SolidWorks Simulation as Design Scenarios and Optimization studies. and a range of 10mm to 20mm for the radius (R). and reports the optimum combination to produce minimum mass. For example. You use sensors as constraints and as goals. The software runs the study using various combinations of the values and reports the output for each combination. for this multibody model of a water bottle. you use a Mass sensor and specify to minimize the mass of the bottle. 100mm. You can now run Design Studies in SolidWorks. There are two main modes for running a Design Study: Evaluation You specify discrete values for each variable and use sensors as constraints. you specify a Volume sensor to keep the volume of the water body between 299000mm^3 and 301000mm^3. H. and 10mm and 20mm for the radius (R). either as discrete values or as a range. 55mm. and 150mm for the length (L). for the model above. The Design Study results report the volume of the water for each combination of L. and H. 55mm. R. For a goal. you specify a range of 75mm to 150mm for the length (L).
select a scenario or iteration on the Results View tab. 73 . SolidWorks Standard SolidWorks Professional SolidWorks Premium SolidWorks Simulation Professional SolidWorks Simulation Premium Mass Properties Dimension Simulation Data To create a study. see New Design Study on page 161. the model updates with the values for that scenario or iteration. For information about Design Studies in SolidWorks Simulation. After running a study. A Design Study tab appears at the bottom of the graphics area. In the graphics area.Design Studies Different sensors are available for use in Design Studies depending on your SolidWorks license and whether you are running an Evaluation study or an Optimization study. click Design Study (Tools toolbar) or Insert > Design Study > Add.
See DFMXpress Help: Sheet Metal Rules. Under Standard Hole Sizes. hole-to-edge distances. New rules validate hole diameter-to-thickness ratios.11 DFMXpress This chapter includes the following topics: • • • Sheet Metal Validation Managing Standard Hole Sizes Zoom to Selection Sheet Metal Validation DFMXpress now validates sheet metal parts. right-click a failed instance and click Zoom to Selection. Under Manufacturing Process. click Settings. Zoom to Selection You can easily view a failed instance by zooming the SolidWorks graphics area. and bend radii. 74 . click Settings. select Sheet metal. In the DFMXpress pane. click Edit. After running DFMXpress. Managing Standard Hole Sizes You can manage the list of standard hole sizes used by DFMXpress to validate parts. In the DFMXpress pane. See DFMXpress Help: Standard Hole Sizes. hole-to-hole spacing.
Supported annotations include geometric tolerance symbols. You can then import the balloons into a drawing.12 Drawings and Detailing This chapter includes the following topics: • • • • • • • • • • • Annotation Attachments Balloons Bills of Materials Blocks Center Marks Cosmetic Threads Dimensions Notes Tables Title Block Tables in Parts and Assemblies Drawings Annotation Attachments It is now easier to attach annotations to one another. and surface finish symbols. you can set the balloons to follow the item numbering of a selected BOM in the assembly under Balloon text source in the Balloon PropertyManager. 75 . datum feature symbols. You can: • Attach annotations to dimension extension lines • Move annotations around dimension extension lines • Use handles to detach annotations from dimension extension lines Balloons Use Numbering from Specified BOMs When you insert balloons and stacked balloons into an assembly. See SolidWorks Help: Balloon PropertyManager.
Formatting of linked BOMs is independent. You can exclude items from BOMs by right-clicking a component in the assembly structure column and clicking Exclude from BOM. right-click a component in the assembly structure column and click Component Options. under BOM Options. Custom Balloon Sizes You can set the balloon size to any value using either the Balloon PropertyManager or Tools > Options > Document Properties > Annotations > Balloons. To link BOMs. You can edit the original assembly BOM or the copied drawing BOMs. Custom sizes are available in balloons. select Copy existing table and Linked. You can also: • Edit the display of child components • Change how the part number is defined • Control how the quantity is calculated To access these options. The text did not update parametrically. column width. You need to create a new BOM to re-link the BOMs. 76 . then group the text with the balloon. Changes in one BOM update the other BOM. Formatting items include row height. only the data is linked. but you cannot reestablish the link. in the Bill of Materials PropertyManager. In previous versions you had to add text outside of the balloon. Component References You can display component references for balloons in the Balloon PropertyManager. Bills of Materials Assembly Options You can set options for specific assembly components directly from the BOM. and text direction. auto balloons. font size and color. Linked BOMs You can link drawing BOMs copied from a previously created assembly BOM using the Bill of Materials PropertyManager. You can unlink the drawing and assembly BOMs at any time.Drawings and Detailing Parametric Quantities You can set a quantity value in the Balloon PropertyManager that updates parametrically. See also Component Reference per Instance on page 49. and stacked balloons.
Highlighting is also supported in BOMs of eDrawings. If a component's preview does not appear when you hover over its icon. Use in bill of materials. but does not alter their values. a gap appears.Drawings and Detailing Descriptions In parts and assemblies. selecting a component in the graphics area. Selecting an item in a BOM highlights it in the graphics area of an assembly or in a drawing view. or FeatureManager design tree highlights it in the BOM. Highlighting It is easier to visualize items that are represented in BOMs. the text is used as the description in the BOM. drawing view. Similarly. The text takes precedence over any configuration-specific or custom properties. then hover over the icon again. Center Marks When you add a center mark to a hole that you have already dimensioned. a gap appears between the center mark and the dimension's extension line. When you type text for the Description and select Use in bill of materials. the Configuration Properties PropertyManager contains the option. Similarly. A thumbnail preview is available for each item in a BOM when you hover over its icon in the assembly structure column. See Enhanced BOM Support on page 90. 77 . open and save the component. if you dimension a hole that already has a center mark. Moving BOMs to Different Sheets You can move BOMs to different sheets by dragging them to: • Sheet tabs • Sheet icons in the FeatureManager design tree • Different windows of the same drawing Blocks You can change the style and size of arrowheads on block leaders by right-clicking the handle on the arrowhead.
When you select the edge for the cosmetic thread. Dimensions Rapid Dimension You can use the rapid dimension manipulator to place dimensions so they are evenly spaced and easier to read. When the rapid dimension manipulator creates dimensions on a symmetric centerline. use the: • Tab key to switch to the different manipulator locations • Spacebar to place the dimension in a suitable location outside of the model geometry You can control the spacing used by rapid dimension in Tools > Options > Document Properties > Dimensions under Offset distances. The rapid dimension manipulator appears when you insert dimensions in drawing views. any dimensions that might overlap are staggered for drawings in the ANSI standard.Drawings and Detailing SolidWorks 2009 SolidWorks 2010 Cosmetic Threads You can define cosmetic threads using international standard sizes in the Cosmetic Thread PropertyManager. the new dimension is spaced evenly between them. Thread callouts can also be created automatically. Use the manipulator to place dimensions at evenly spaced intervals. The callouts are populated with the appropriate text from the calloutformat. To place dimensions quickly.txt file. For example. you can select a dimensioning standard and size. if you insert a dimension between two dimensions. 78 .
79 . Open install_dir\samples\whatsnew\detailing\dimension. 5. Click one of the circular edges. 7. The dimension is placed below the selected edge. 2. Click Smart Dimension > Smart. 6. Click the lower portion of the rapid dimension manipulator. Click the two edges as shown.Drawings and Detailing Using Rapid Dimension To use rapid dimensioning: 1. 3. Repeat step 5 for the two edges shown. (Dimensions/Relations toolbar) or Tools > Dimensions The rapid dimension manipulator appears as: 4. Click the edge shown. then click the lower portion of the rapid dimension manipulator.slddrw.
In the Style portion of the palette. text. The dimension appears in the lower right corner. and other formatting options in the palette without going to the PropertyManager.Drawings and Detailing The rapid dimension manipulator appears as: 8. you can select any of the formatting settings that you applied to other dimensions in the drawing. You can change the tolerance. Press Tab three times to switch dimension locations and press the spacebar to place the dimension. If you select more than one dimension. Dimension Palette The dimension palette appears when you insert or select a dimension so you can easily change the dimension's properties and formatting. style. the properties and formatting that you set in the palette apply to all of the dimensions. 80 . precision. which saves you time when formatting dimensions.
Double prime marks on Double prime marks off Deleting Dimensions If you delete a dimension or remove text from a dimension. click View > Dimension Names or. the dimensions continue in detail views.General dialog box. select any portion of the note and select a border in the Note PropertyManager. When inserting or editing a note. The Show Dimension Names setting is removed from the System Options . The detail view uses the existing 0 point in the parent view. To show dimension names. the software can automatically readjust the space among the remaining dimensions. Dimension Names The Show Dimension Names setting is now controlled and saved per document instead of for all documents as a system setting.Drawings and Detailing Ordinate Dimensions When you insert ordinate dimensions in parent views. 81 . when you insert ordinate dimensions in detail views and apply ordinate dimensions in parent views. Click Tools > Options > System Options > Drawings and select Adjust spacing when dimensions are deleted or text is removed. Conversely. the parent view uses the 0 point from the detail view. Notes You can apply borders to portions of notes. Fractional Dimensions You can turn off the double prime marks (") in fractional dimensions. from the Heads-up View toolbar. click Hide/Show Items > View Dimension Names. Click Tools > Options > Document Properties > Dimensions and set the options under Fractional display.
Drawings and Detailing
Three new borders are also supported: square, circle in square, and inspection.
You can edit and navigate in tables as you do in Microsoft Excel. You can: • Control vertical cell padding • Navigate using the Enter, Tab, Arrow, Shift + Enter, Shift + Tab, Shift + Arrow, Home, Ctrl + Home, End, and Ctrl + End keys • Select a cell, type data, and view the data immediately in the cell, overwriting existing data • Press F2 in a highlighted cell to activate the cell for editing and move the cursor to the end of the text in the cell • Double-click a cell to move the cursor to the position where the cell was double-clicked • Press Alt + Enter to add multiple lines of text in a cell • Press Delete to erase all text from a cell without activating the cell for editing • Press Backspace to erase all text from a cell and activate the cell for editing • Select multiple rows or columns and change their heights or widths by dragging or using the formatting tools • Lock row heights and column widths • Copy cells from Microsoft Excel and paste them into SolidWorks tables
Title Block Tables in Parts and Assemblies
You can now generate a title block table in a part or assembly document as an aid for paperless manufacturing. You cannot add title block tables to drawings. In drawings, use the title blocks that are part of the drawing sheet format. You can base a title block table on a sample template supplied by SolidWorks or a template you create yourself. If you define custom properties for the part or assembly and use a template that references those properties, SolidWorks populates the table values from the custom properties automatically. To add a title block table to a part or assembly, click Insert > Tables > Title Block Table. In the Title Block Table PropertyManager, define the size and borders of the table or click to browse to an existing table template with the file extension .sldtbt. After inserting the table, click the upper left corner to open the Title Block Table PropertyManager, which provides a scaling control that lets you resize the table proportionally.
Drawings and Detailing
See SolidWorks Help: Title Block Tables.
Aligned Section Views
You can now dimension across aligned section views.
Component Line Font
The Component Line Font dialog box has been reorganized for ease of use. To access the dialog box, right-click a drawing edge and click Component Line Font. You can also access the Line Color from the context menu. , Line Thickness , and Line Style tools
Drawings and Detailing
You can change drawing view configurations in drawing view PropertyManagers. Previously, you had to go to the Drawing View Properties dialog box.
Drawing Templates
Additional drawing templates are included for supported drawing standards.
Drawing Views of Multibody Parts
You can create Standard 3 Views and model views of multibody parts. For flat patterns of multibody sheet metal parts, you can use one body per view. Displaying Drawing Views of Multibody Parts 1. Open install_dir\samples\whatsnew\drawings\multibody.slddrw. 2. Select the drawing view. 3. In the PropertyManager, under Reference Configuration, click Select Bodies. Multibody.sldprt opens. 4. Select the two bodies shown and click .
Multibody.slddrw opens and the drawing view shows the two selected bodies.
and Show Edge buttons are merged into one button: Hide/Show Edge Selection You can use the following methods to select edges when using the Hide/Show Edges tool: • Click individual edges. This is available under Section Depth in the Section View PropertyManager. Opening Parts and Assemblies from Drawings When you right-click a component in an assembly drawing. Tangent Edges New options in the Hide/Show Edges PropertyManager help you to hide and show different types of tangent edges. the diameter symbol appears in the dimension.Drawings and Detailing Hiding and Showing Edges Toolbar Button The Hide Edge Edges . Section Views Section Depth You can now set the depth of section views in parts by specifying how far beyond the section view line you want to see. The section cut must be through the center of the diameter. Previously. you can open the part or assembly. Diameter Dimensions When you insert diameter dimensions in section views. excluding edges that were previously unselected. • Box selection. you could open the part only. • Alt + Box selection to clear edges fully enclosed in the box selection. 85 . See Display Options on page 86. In previous versions. • Shift + Box selection to select edges fully enclosed in the box selection. including edges that were previously unselected. this functionality existed in assembly drawings only.
The color applies to Tangent Edges Use Font only. (Line Format toolbar) to access these options (except for 86 . Display Options New options are available for filtering tangent edges in drawing views with hidden lines removed or hidden lines visible. Tangent Edges Colors You can set the color of tangent edges.Drawings and Detailing Sketch Pictures If you insert a sketch picture in a part or assembly. Model Tangent Edges and set the color. System Properties There are two new system properties for drawing documents: SW-View Name and SW-View Scale. These properties are similar to the system properties SW-Sheet Name and SW-Sheet Scale. Click Tools > Options > System Options > Colors. the picture appears in the associated drawing views. Click Hide/Show Edges Hide Ends). In Color scheme settings. select Drawings.
Before After Right-click a drawing view and click Tangent Edge > Hide Ends. Hide Hides Non-Planar tangent Edges edges that border non-planar faces. 87 .Drawings and Detailing Option Hide Ends Hides the start and end segments of tangent edges.
Drawings and Detailing Hide Hides tangent Blend edges that: Edges • Border on planar faces which are normal to the viewing direction • Have second order continuity (C2) at the boundary of two faces Hide edges shorter than Hides tangent edges that are less than a specified length. 88 .
You can publish an eDrawings file and animate directly within eDrawings. You can also preview multiple sheets without having to exit Print Preview. With the Current screen image option selected. 89 . You no longer need to load the eDrawings add-in manually. in the Save flyout ® As part of this integration. To publish to eDrawings.13 eDrawings This chapter includes the following topics: • • • • • • • • Integrated Publisher Print Preview Enhanced BOM Support Apple Mac Printing Enhancements Display States Linked to Configurations Title Block Tables Decals Sketch Pictures Integrated Publisher The ability to publish to eDrawings is now fully integrated into SolidWorks toolbars and menus. Close the preview by clicking Hide Preview. See SolidWorks Help: SolidWorks eDrawings. the eDrawings Animate button has been eliminated in the SolidWorks software. you can pan and zoom to fine-tune your selection before printing. you select a portion of the drawing to print. Print Preview With eDrawing's Print Preview. Click File > Print and click Show Preview to fine-tune your selection. you can see your drawing or model exactly as it will be printed. Within the Print dialog box. eliminating wasted paper and time. click File > Publish eDrawings File ( toolbar).
you can explicitly save the design containing a BOM as an eDrawings file. eDrawings displays BOMs in native SolidWorks documents. publish a part or assembly containing a BOM to eDrawings just as you publish any SolidWorks design to eDrawings.eDrawings See SolidWorks eDrawings Help: Print. and reposition them. show. eDrawings already supports BOMs in drawings. In SolidWorks. Click Options and in the Export Options dialog box. and this functionality is unchanged. or show the corresponding components or to make them transparent.easm. From SolidWorks. as well as in eDrawings files saved from SolidWorks. In earlier releases. you can hide. select Save Table Features to eDrawings file. Now. In SolidWorks. Enhanced BOM Support Bills of Materials (BOMs) for parts and assemblies have enhanced support in eDrawings.eprt or . hide. 90 . you could view BOMs created in SolidWorks assemblies. by clicking File > Publish eDrawings File ( in the Save flyout toolbar). click File > Save As and save to an eDrawings format. Select individual rows to highlight. .
In the Save Configurations to eDrawings file dialog box. create a configuration and publish the part or assembly containing the configuration by clicking File > Publish eDrawings File ( in the Save flyout toolbar). You can print an entire sheet or what is currently displayed. You can choose to link a display state to a configuration or to keep the display states independent from configurations. Clear Link Display States to Configurations to toggle the display states so that they are independent from configurations. 91 . Click File > Print to use the new print controls.eDrawings See SolidWorks eDrawings Help: Bills of Materials. You can now print in color or grayscale rather than just black and white. Apple Mac Printing Enhancements Apple Mac printing for eDrawings is enhanced. and you can also set a scale factor. in eDrawings. select the configurations to be saved to the eDrawings file. To link display states to configurations. From SolidWorks. ® Display States Linked to Configurations eDrawings now supports assigning display states to configurations as in SolidWorks. open the Configurations tab and select Link Display States to Configurations.
and this functionality is unchanged. and reposition title block tables. See SolidWorks eDrawings Help: Title Block Tables. hide. eDrawings supports title block tables in drawings. create a title block table and publish the part or assembly containing the table by clicking File > Publish eDrawings File ( in the Save flyout toolbar). as well as in eDrawings files saved from the SolidWorks software. You can show.eDrawings See SolidWorks eDrawings Help: Configurations. eDrawings displays title block tables in native SolidWorks documents. 92 . expand Tables and click the title block table to display the table's handle. From SolidWorks. Title Block Tables Title block tables for parts and assemblies are visible in eDrawings. in the component design tree. In eDrawings.
Add a sketch picture to a SolidWorks part.eDrawings Decals PhotoWorks decals applied to SolidWorks models are now visible in eDrawings. assembly. 93 . or drawing and publish by clicking File > Publish eDrawings File ( in the Save flyout toolbar). Apply a PhotoWorks decal in SolidWorks and publish the part. The decal must be visible when the model is saved to an eDrawings file. The model or drawing is displayed with the sketch pictures shown in eDrawings. in the Save flyout toolbar). eDrawings displays decals in SolidWorks parts and assemblies. assembly. The model is Sketch Pictures Sketch pictures applied to SolidWorks drawing sheets and parts are now visible in eDrawings. or drawing by clicking File > Publish eDrawings File ( displayed with the decal in eDrawings. and also in eDrawings files saved from SolidWorks.
eDrawings Drawing view of a part with a part-level sketch picture and a sketch picture on the sheet format. Model with sketch picture. 94 .
Administrators can configure tasks to run on a specific computer or distribute them to both client computers and dedicated servers. or triggered by a SolidWorks Enterprise PDM workflow. A SolidWorks Print or Convert task can be initiated on any computer that is running Enterprise PDM. To enable tasks: • Include the Convert and Print task options when you create a new vault and specify the vault's configuration details. as long as the computer where the task is executed has SolidWorks installed. Administrators can define tasks to be interactive. programmers can also extend the functionality to support custom tasks. they can set all options so that the task runs silently. The task framework lets administrators and users execute tasks on demand. • Enable the execution of tasks on host computers.14 Enterprise PDM This chapter includes the following topics: • • • • • • • • Managing Tasks Enterprise PDM and Toolbox Integration File Explorer and SolidWorks Add-in Item Management Administration Tool API Installation Documentation Managing Tasks The new Tasks feature in the Administration tool makes it easy to perform tasks such as converting and printing SolidWorks documents. See SolidWorks Enterprise PDM Administration Tool Help: Permitting Task Execution. without requiring user input. based on a schedule. Using the task API and templates provided in the Enterprise PDM software. • Configure the Convert and Print tasks. 95 . Setting Up Tasks You use the Administration tool to install and configure Enterprise PDM tasks. See SolidWorks Enterprise PDM Administration Tool Help: Creating a Vault. letting users initiate the task and choose task options. Alternatively.
For example. For example.Enterprise PDM These tasks. for example. For example. or assemblies • Which versions to print . • Initiate and monitor tasks using the Task List dialog box.none. Use the Task List dialog box to monitor tasks and to view information about completed tasks. • Convert a multisheet drawing to a multipage . you can create a transition action that converts parts and drawings to . Convert tasks lets you convert SolidWorks files using the output formats and options supported by SolidWorks. See SolidWorks Enterprise PDM Administration Tool Help: Launching a Task Using a Workflow. Use Add Task in the Task List dialog box to immediately launch a task. you add tasks supported by the add-in to the Tasks feature by creating new tasks. you can: • Print all drawings in an assembly when the assembly state changes to Reviewed. • Create new tasks using the Task wizard. parts. which are supported by the SolidWorks Task Add-in. If you use the Enterprise PDM API to program a task add-in. you can: • Specify how converted files are named. Specify the following for source files with references: • Which references to print . For example. drawings. are listed under Tasks in the Administration tool. you can create a silent configuration that does not require user input and a second user-initiated configuration that lets users modify task settings. For example. 96 . • Save converted files to the vault or another destination such as a directory used by an Enterprise Resource Planning (ERP) application.the latest version or the version referenced the last time the source file was built You can initiate either a Print or Convert task by adding it to a workflow transition. using the source file name and revision number. Set permissions so that users can print files to a printer near them. so that user computers are not tied up.pdf file. Convert and Print Tasks The Tasks feature in the Administration tool lets you configure task properties. The Convert and Print tasks are available if you select them when you create the vault. • Convert only specifically named drawing sheets such as sheet metal flat patterns. Print tasks are also performed on SolidWorks files.pdf files when an assembly is ready for review. • Map variables from the source file data card to the output file data card to transfer attributes such as Description and Part Number. Direct output to printers based on paper size requirements. you can: • • • • Print drawings to a print server. You can copy an existing task and modify it so that you have multiple task configurations. • Include task execution in workflow transitions.
see SolidWorks Enterprise PDM Administration Tool Help topics: • Configuring the Convert Task • Configuring the Print Task Executing Tasks The task infrastructure provides multiple ways to initiate tasks. including tasks that are currently running and tasks that are scheduled or waiting to run. you can specify options for the newly created files such as file names. Monitoring Tasks The primary tool for monitoring tasks is the Task List dialog box. monitor tasks that are running. who initiated the task. and view information about completed tasks. which you display from the Tasks feature in the Administration tool. You can also initiate tasks from this dialog box. you can: • Trigger tasks using a workflow transition For example. you can view its details to see an error message and error code. Task List Options let you specify the number of task records to retain in the Completed Tasks list. you can automatically generate . These codes are also reported in error logs that are created for failed tasks. users with permissions to perform tasks can select files and use right-click menu options to convert or print them.Enterprise PDM • Convert all drawings in an assembly to . you can see the task progress. If you select a pending task or a task that is executing and click Details. • Schedule task execution If you create custom tasks using the APIs. You can also use notifications to inform users of the success or failure of tasks. As an administrator. and the files on which the task is being executed. • The Pending tasks list shows the task queue. • Configure tasks so that they can be initiated by users With File Explorer.pdf format when the state changes to Released. You can suspend and resume pending tasks. you can include the task scheduling infrastructure so that tasks can be performed when task hosts are available. properties. lets you identify tasks that are pending. 97 . • The Completed tasks list shows the status of completed tasks. For instructions on configuring tasks. and destination folders. or cancel them completely. As part of task setup. • Use the Task List dialog box to execute an on-demand task On-demand task execution lets you initiate the printing of SolidWorks files from an Enterprise PDM client that does not have the SolidWorks software installed.pdf files when SolidWorks files reach a state such as Released. If a task fails. You can set up notification messages to be sent to users and task initiators when a task succeeds or fails. The Task List dialog box.
To create a task add-in. To configure the 2010 Enterprise PDM and Toolbox integration: 1. From the Enterprise PDM Administration tool. 98 .Net.Enterprise PDM • If a conversion task succeeds. they add the tasks it defines to the Tasks node by creating new tasks. After administrators install the add-in to the vault.html. Enterprise PDM automatically: • • • • Checks Toolbox parts out and in as needed so the latest versions are used Adds missing Toolbox parts to the vault Redirects assembly references to Toolbox parts in the vault Replicates the Toolbox files and database (if replication servers are configured) Enterprise PDM still supports the SolidWorks pre-2010 Toolbox integration. see SolidWorks Enterprise PDM Administration Tool Help: Configuring Toolbox. You can program the task add-in to: • • • • • Send parameters and data to the task executor as part of the task instruction ® Execute any MS-DOS /Windows command Start up any Windows program with an arbitrary number of parameters Give commands to any Windows program Access and send command to installed resources like printers and plotters ® Enterprise PDM and Toolbox Integration Enterprise PDM can now manage SolidWorks Toolbox part files and the Toolbox database entirely in an Enterprise PDM vault. A task add-in extends the capabilities of the task executor. Check the Toolbox root folder (SolidWorks Data by default) into the Enterprise PDM vault. If you have SolidWorks 2010. you need to program in Visual Basic . Users point SolidWorks to the Toolbox vault folder and use Toolbox as before. For example. C#. See the description of the API in the SolidWorks Enterprise PDM Programmer's Reference Guide. the new integration is recommended. and see the file's history. or C++. view the file's properties. 2. Programmers can use the Enterprise PDM API to create an add-in to execute tasks unique to their environment. where the master Toolbox library is outside the vault and Enterprise PDM creates copies in the vault as parts are used. the notification contains links to the converted files. Configuring Enterprise PDM and Toolbox An administrator must configure Enterprise PDM and Toolbox before users access Toolbox. Enterprise PDM includes the task executor add-in SWTaskAddIn. so that you open a file in the Enterprise PDM File viewer. a task add-in could open files in Microsoft Word and save them to another format such as . Task Add-ins Tasks are defined by task executor add-ins. double-click Toolbox and set configuration options. which enables conversion and printing of SolidWorks files. For details about this procedure. • If a task fails. the notification contains a link to the error log.
the Clear Local Cache dialog box appears. you can clear the Enterprise PDM cache. Enterprise PDM creates a new version of the master part file containing the new configuration. Have all users set their SolidWorks Hole Wizard and Toolbox folder to the Toolbox vault folder. Enterprise PDM checks the cache and retrieves the latest file if necessary. 4. which affects performance. These permissions determine what operations you can perform. If the size does not already exist. You cannot create new sizes when working offline. use Get Latest on the Toolbox vault folder. To reduce disk space. which removes local files. Enterprise PDM displays a message if you do not have permission to perform an operation. Enterprise PDM operations are performed using your Enterprise PDM permissions or the permissions of a designated user. Search Paths SolidWorks always searches for Toolbox parts in the Enterprise PDM vault first. In File Explorer. If Toolbox is configured to create part files for each new size. Enterprise PDM caches files again when needed. From SolidWorks. As you continue to use Toolbox. Permissions Depending on how your administrator has configured Toolbox integration. You do not need to add the vault folder to your System Options . if you have read access to Toolbox but no permission to check out files. For example. You can remove cached Toolbox files by clearing Do not remove Toolbox files. When you clear the cache from the vault root folder (from File Explorer. right-click the vault and select Clear Local Cache). 99 . click Tools > Options > Hole Wizard/Toolbox: a) Set Hole Wizard and Toolbox folder to match the setting from the Enterprise PDM Administration tool. b) Click Configure to configure Toolbox using the Toolbox configuration tool. Enterprise PDM automatically creates a new file in the vault without first checking the local cache. but there are some details to be aware of. If Toolbox is configured to add configurations to the master part file. Using Toolbox with Enterprise PDM Enterprise PDM's management of Toolbox is mostly transparent to users. Local Cache When you first insert a Toolbox component into an assembly. Automatic Part Creation Toolbox detects when assemblies contain configurations that do not exist in the library and can automatically create missing sizes for you. Enterprise PDM manages your cache automatically.Enterprise PDM 3. you can use existing component sizes but not create new sizes.File Locations folder list. Enterprise PDM caches the latest version of the part file in your local vault view. Working Offline You can work with Toolbox parts when you do not have access to the vault by caching the parts locally before going offline.
select Check In or Check Out. and drawings in the SolidWorks add-in options are used. This happens when referenced parts or subassemblies have been modified but the selected drawing or assembly has not been opened and resaved in SolidWorks. See SolidWorks Enterprise PDM File Explorer Help: Copying Files with References. in SolidWorks. By default. from the Enterprise PDM Administration tool. and click OK. For Affected operation. Right-click a file and click Copy Tree. In the Copy Tree dialog box. Drawings with Multiple References Not Automatically Checked Out Enterprise PDM no longer automatically checks out or retrieves drawings referencing more than one file when you check out or retrieve a referenced part or assembly. you can perform operations from the add-in without closing the file. the serial numbers set up for naming parts. do one of the following: • Click Transform > Rename with Serial Number. If the file is open in SolidWorks and the Enterprise PDM add-in is installed. 100 . but you can select any serial number. on the View Setting tab. In the Properties dialog box. In the Enterprise PDM Options dialog box. In the Copy Tree dialog box. Close the file in the other application and retry the Enterprise PDM operation. click Warnings. expand Users or Groups and double-click a user or group. this condition blocks check-ins and check-outs. clear The file is open in another application. Naming Drawings with Model Names Using Copy Tree The Copy Tree command can copy drawings using the same names as their associated assembly or part files. By default. type a new Caption. • Right-click a file in the file list and click Rename with Serial Number. See SolidWorks Enterprise PDM File Explorer Help: Copying Files with References. This change addresses issues where drawings remained checked out after the referenced file was checked in. Warning when File Is Open in Another Application File Explorer now warns you if you check in. assemblies.Enterprise PDM File Explorer and SolidWorks Add-in Naming Files with Serial Numbers Using Copy Tree The Copy Tree command can now automatically name copied files using serial numbers. click Enterprise PDM > Options. To rename a column. File Preview Rebuild Warning The Preview tab now displays a warning if a drawing or assembly needs to be rebuilt. Right-click a file and click Copy Tree. under Display Information. check out. select Name drawings after their models. Changing Column Names and Order in the SolidWorks Add-in You can now rename and reorder the columns in the Enterprise PDM SolidWorks client. or edit the data card of a file that is open in another application. To make this condition nonblocking.
click Get Versions > Versions in Cold Storage. In the Administration tool. Versions in Cold Storage is available only if at least one version is in cold storage. three. In Item Explorer. File / Variable must be the first column. which shortens the main list to only versions you can retrieve. Named BOMs for Items Named bills of materials (BOMs) are now supported for items. filter. Item Management Generating Item IDs from File Attributes Enterprise PDM can now generate item IDs from file attributes. Display Formats for Item BOMs You can now control which items display in item BOMs. Enterprise PDM uses the item serial number to generate the ID. drag a column header (caption) to a new location. click Expand Levels (toolbar) and click a command. such as part number. and compare BOMs. or all levels of hierarchy. • Top Level Only displays only top-level items. right-click a file and click Get Versions > Versions in Cold Storage. Cold Storage Versions in Get Version Submenu The Get Version command now lists cold storage versions in a submenu. When generating an item from a file. click BOM Display the following: • Indented displays all items in the BOM hierarchically. and click one of Expanding and Collapsing Item Structure You can now expand all items displayed in the Item Explorer main pane to display their content. expand a vault and double-click Items.Enterprise PDM To reorder columns in the SolidWorks Enterprise PDM task pane. > Save as BOM. change position numbers. • Parts Only displays only items without child items. 101 . In Item Explorer. In Item Explorer. Enterprise PDM defaults to an existing item if there is an item with the same ID. You can create one or more BOM views and sort. If variable mapping is not enabled or if the variable has no value. On the Item ID page. See SolidWorks Enterprise PDM Administration Tool Help: Configuring Items. and collapse all levels of hierarchy. for Item ID Variable. click Save BOM See SolidWorks Enterprise PDM Item Explorer Help: Named BOMs. An administrator selects which data card variable to map to. two. You can expand one. select a variable or select <Do not read the ID from a variable>. on the Bill of Materials tab. From the SolidWorks add-in. on the Bill of Materials tab. From File Explorer. otherwise the item ID defaults to the mapped value. A user can choose to generate a different ID.
these bulk selection check boxes were always displayed. You can export data cards for: • • • • • Files Folders Items Searches Templates You can export all cards in the vault.cex file by right-clicking the vault name and clicking Export. or turn them off to simplify the user interface.cex) files. serial numbers.Enterprise PDM See SolidWorks Enterprise PDM Item Explorer Help: Expanding and Collapsing Items and Folders. Extended Export and Import Functionality The Administration tool export functionality has been expanded for Enterprise PDM 2010 to make it easier for you to move settings from one vault to another. 102 . click Import. When you import a data card. In the Generate Item dialog box or Link Files to Item dialog box. Administration Tool Add-in and File Format Support The SolidWorks add-in and file formats for Enterprise PDM 2010 have been updated to support SolidWorks 2010. To import administrative export files. and card lists. See API Support for Items on page 104. You can also export all settings in a vault to a single . API Support for Items Enterprise PDM now provides an API for items.cex file. Data Card Export and Import You can export a data card created using the card editor to a . such as variables. right-click the vault name. Optional Parent Node Check Boxes When generating items from files with references.cex file into another vault. Use these check boxes to make selections more efficiently. Previously. See SolidWorks Enterprise PDM Item Explorer Help: Bulk Selecting References in Dialog Boxes. all cards of a specific type. and navigate to the location of the .cex file and import the . you can now choose whether to display bulk selection check boxes for parent nodes. You can now export all configurable features to administrative export (. are also imported. all card dependencies. right-click in the file list box and select or clear Show Parent Node Check Boxes. or individual cards.
To make it easier to locate and display the permissions to set.cex file into another vault. variables. To export an individual template. right-click the template. bills of materials. Access to the dialog boxes has not changed. all files included with the add-in are also imported. Group settings are included in export files for templates. expand Add-in. When you import an API add-in. including permissions for search cards. To export an individual add-in. right-click the add-in. Tasks. and click Export. all template dependencies such as input forms. Central Assignment of Permissions The Properties dialog boxes for users and groups now provide a central place to assign all permissions. and click Export. Bills of Materials. the tabs used in previous releases have been replaced by a left pane list of controls that link to the permission pages.cex file and import the . When you import a template. right-click Add-in and click Export. 103 . and serial numbers are also imported. To export all registered API add-ins in a vault. For example. right-click Templates and click Export. The following graphic shows the new Group Properties dialog box controls. User settings are not. highlighting the Search Cards. you still expand Groups and double-click a group to display its Properties dialog box. Template Export and Import You can export a template created using the template wizard to a . expand Templates.cex file into another vault. and Template links. To export all templates in a vault. You can export a single add-in or all the currently registered add-ins.cex file and import the .Enterprise PDM Add-in Export and Import You can export an API add-in to a . and templates.
modifying. and creating items Generating items from files Reading. modifying. In the Card Editor. If there are errors in your settings. Previously. if you set up serial numbering. select Default overwrites and type the names of the configurations from which to exclude default values. and other external systems • Importing items into Enterprise PDM • Accessing information to generate reports • Customizing item numbering Specific API capabilities include: • • • • • Reading. The API lets you create applications to perform custom tasks such as: • Synchronizing items between Enterprise PDM and Enterprise Resource Planning (ERP). type the name of an email recipient and click OK to send the test message. In the Test Settings dialog box. on the SMTP tab. Materials Requirements Planning (MRP). and creating item links to child items and files Reading and modifying item bills of materials (BOMs) Finding items and opening them in Item Explorer API Methods for Users and Groups The existing API methods for users and groups have been extended. Enterprise PDM also: • Generates default values when you create new SolidWorks configurations • Preserves card values when you rename a configuration SMTP Mail Setup You can now quickly verify your SMTP mail settings by performing an email test to validate them. right-click Add-ins and click Programmer's Reference Guide. To access the guide. With SMTP selected in the Message System dialog box. default values were generated for all configurations. when adding most controls. API Support for Items Enterprise PDM now provides an API for items. see the SolidWorks Enterprise PDM Programmer's Reference Guide. API For information on using the Enterprise PDM API. click Test Settings. You can now use the API to: • Copy permissions and settings from an existing user 104 . Enterprise PDM returns a detailed error message to help you find the problem. You can now configure data cards to specify configurations for which default values will not be generated.Enterprise PDM Serial Number Enhancements You have more control over how Enterprise PDM handles serial numbers for added or renamed files.
configurations. Administrators can select and configure the Set card variables command and add it to an action. right-click the server name in the Administration tool and click Create new vault. To access the Set card variables command: 1. In the Select command dialog box. workflows. you can browse to it and import it. right-click Dispatch. enabling companies installing Enterprise PDM for the first time to quickly use the software in a production environment. 3. Installs the data set from previous versions of Enterprise PDM.Enterprise PDM • • • • Assign folder permissions for users and groups Add users to and remove users from existing groups Delete existing users and groups Check folder permissions for users and groups Dispatch Set Card Variables Command The Dispatch module includes the new command Set card variables. To select a configuration. click Add. 4. On the Configure vault screen. To make it easier to begin using Enterprise PDM. which makes it easier to import or create objects such as data cards and workflows. data card variable. Installs a simple data set with predefined groups and permissions. This command sets file and folder data card variables to user-specified values. and variable value • Specify the variable value as a static string or as a parameterized string constructed using Dispatch variables Installation Predefined Data Set Configurations Enterprise PDM provides multiple predefined configurations that consist of data cards. 2. when you create a vault. Documentation Web-based Documentation Documentation for SolidWorks Enterprise PDM is now available on the Web. In the Edit Action dialog box. If your company already has a customized data set based on an administrative export file. 105 . select one of the standard configurations shipped with Enterprise PDM: Empty Default SolidWorks Quick Start Creates a data folder with no files. you can choose which configuration to import. Configurations are defined using . templates.cex files. click Add. and bill of materials (BOM) column sets. Use the Set Card Variables dialog box to: • Configure the command to specify the target file or folder. and click Administrate Actions. In the Administrate Actions dialog box. Expand Add-ins. select Set card variables.
You can still choose to use local help files (. for example. The SolidWorks Enterprise PDM Programmer's Reference Guide is available as a locally installed . right-click Add-ins and click Programmer's Reference Guide. short descriptions in search results views. including improved relevancy ranking. and guided navigation to help you identify relevant topics. including next and previous topic buttons and breadcrumb navigation.Enterprise PDM By default. To access it. 106 . the Web version of the documentation is displayed in a Web-based viewer. spelling correction.chm) files. • Ability to provide feedback directly to the documentation team on individual help topics.chm file only. Select or clear Use SolidWorks Web Help on all SolidWorks Enterprise PDM Help menus to switch between the local and Web-based versions of the help. • Up-to-date documentation without the need to download large compiled help (. • Improved topic navigation. when you access help. your Internet connection is slow or unavailable. Benefits of Web-based help include: • Improved search functionality. in the Administration tool.chm) if.
A preview shows what you have selected so that you can remove entities. Restrictions are listed in SolidWorks Help. see SolidWorks Help: DXF / DWG Output PropertyManager. See SolidWorks Help: Adobe Photoshop (*. 107 .3dm format) on 64-bit computers.dxf or . For more information about this PropertyManager.psd format) on 64-bit computers.dwg file type • Selecting one or more planar faces and clicking Export to DXF / DWG • In the FeatureManager design tree for a sheet metal part.dwg file type • Selecting one or more planar faces. you could import Rhino files on 32-bit computers only. open the PropertyManager by: • Saving the part (File > Save As) to a . In earlier releases. right-clicking Flat-Pattern and clicking Export to DXF / DWG After you click Save. In earlier releases. An expanded set of geometrical entities is available when you export a sheet metal flat pattern. the PropertyManager appears. With a part open. JPG.psd) Files. or PSD File to a Custom Size DXF / DWG Output PropertyManager The new DXF / DWG Output PropertyManager lets you export any planar face or named view from a part file to one or more DXF or DWG files. Importing and Exporting Adobe Photoshop Files on 64-bit Computers You can import and export Adobe® Photoshop® files (in . Importing Rhino Files on 64-bit Computers You can import Rhino files (in . you could import Photoshop files on 32-bit computers only.dxf or . clicking File > Save As. See SolidWorks Help: Rhino Files.15 Import/Export This chapter includes the following topics: • • • • • • DXF / DWG Output PropertyManager Importing Rhino Files on 64-bit Computers Importing and Exporting Adobe Photoshop Files on 64-bit Computers Importing Autodesk Inventor Files Importing Adobe Illustrator Files Saving a TIF. and choosing a .
you can choose to import the object as a single body or import it with its features. Inventor must be installed on your computer to import features. select the file format from the Save as type list. In the Export Options dialog box. When you import an Inventor file.Import/Export Importing Autodesk Inventor Files When you import an Autodesk® Inventor® part or assembly file. or PSD File to a Custom Size When you save a part or assembly in . JPG. Saving a TIF. see SolidWorks Help: TIFF. version CS3 or later of Illustrator must be installed on your system. or . Photoshop. You can import geometry with Inventor Viewer installed.jpg. you can save the image to a custom size by specifying dots per inch (DPI) or paper size. click Options to specify the print capture size. Importing Adobe Illustrator Files To import an Adobe® Illustrator® file into SolidWorks. .tif. you are prompted to select an import type. In the Save As dialog box. 108 . Importing by feature provides more detailed information about the original model. For more information.psd format. and JPEG Export Options.
or torques. • Previous tasks in the event schedule • Start and finish times for task actions Task actions define or constrain the motion of one or more components in the assembly. You can define task triggers based on time. or toggle or change values for motors. constant force. Task triggers are the events that drive the motion action for a task. or change the value of a constant speed motor. or sensed values. The tasks can be sequential or can overlap in time. Detects motion of a body crossing a line. Event-based motion requires a set of tasks. This chapter includes the following topics: • • • • • • Event-based Motion Analysis Rigid Groups Structural Simulation Analysis for Motion Force and Motor PropertyManager Enhancements Contact Setting the Exact Time for Key Points and the Time Bar Event-based Motion Analysis Event-based Motion Analysis With SolidWorks Simulation® Professional added in.16 Motion Studies Available in SolidWorks Premium. You can define actions to toggle mates. constant torque. stop motion. Detects the relative position of components from dimensions. forces. you can use Motion Analysis to calculate the motion of an assembly that incorporates event-based motion control. previous tasks. You can create triggers from: • Sensors: Interference detection Proximity Dimension Detects collisions. such as component position. stop. Each task is defined by a triggering event and its associated task action that controls or defines motion during the task. You can define a task action to: • Start. or a servo motor • Stop the motion 109 .
and range of a line that senses when a body in motion crosses it. From a Motion Analysis motion study. To create a sensor. click Motor motor in the Motor PropertyManager. Servo Motors for Event-based Motion Analysis You can use servo motors to implement control actions for event-based motion analysis. if you are not already in an event-based view. you examine an event-based motion study of a welding robot. Click the next task row. . • Add in SolidWorks Motion. servo motors control the motion of a component. right-click the Sensors and click Add Sensor. click Event-based Motion View (MotionManager toolbar). You can create the following types of linear or rotary servo motors: • Velocity • Acceleration • Displacement When triggered. use proximity sensors to model laser position detectors. Specify the triggers and corresponding motor parameters in the Event-based Motion View To create a servo motor. folder Event-based Motion Study In this tutorial. Creating a Task Create the required sensors. or forces before setting up the study. motors. 110 . You can specify the location. in the FeatureManager design tree. For example. you must: • Obtain a SolidWorks Simulation Professional license. 2. 3. • Select Motion Analysis for the motion study type. torques. direction. Enter the task description and specify the trigger and control action for the task. To create an event-triggered motion task for a Motion Analysis study: 1.Motion Studies • Suppress a selected mate To use event-based motion. (MotionManager toolbar) and specify the servo New Proximity Motion Sensor You can use proximity sensors to trigger actions in event-based motion analysis.
• Task 6: Begin welding when the robot is in position. • Task 7: Activate the servo motors to move the robot back to its original position. This motion study is set up for the following tasks: • Task 1: Use a position sensor to stop the motion of a plate at a given location after . Place your pointer over the MotionManager time slider and drag it all the way to the left. 1.sldasm. you examine values for the motors and the sensor in this study. • Task 5: Activate the servo motors to move the robot to its welding X. to check the time 111 . you open the model and examine some components. Each servo motor is set to move in one of the three spatial directions. Viewing Motor and Sensor Parameters Next. You must have a SolidWorks Simulation Professional license and you must add in SolidWorks Motion to run this tutorial.Motion Studies Event-based motion requires a set of tasks. Open install_dir\samples\whatsnew\motionstudies\weldingrobot\weldingrobot. The tasks can be sequential or can overlap in time. 1. Y. 2. Z position. Notice there are four linear motors listed in the MotionManager and one sensor listed in the FeatureManager design tree. Select the Motion Study 1 tab.01 seconds. • Tasks 2-4: Turn on three displacement servo motors. Each task is defined by a triggering event and its associated task action that controls or defines motion during the task. Opening the Model First.
1. double-click Sensor1. torques. Right-click the sensor in the FeatureManager design tree and click Edit Sensor. 3. 1. 2. or toggle or change values for motors. Event-based key points appear in the timeline as the events take place. double-click LinearMotor4. or forces. You can also apply an action that stops the motion altogether. Do not change the trigger selection and click OK to close the dialog box. such as component position. 2. The Trigger dialog box appears with Sensor1 selected. 112 . Task actions define or constrain the motion of one or more components in the assembly.Motion Studies This step places the assembly components in their initial positions and initializes the motor values. • You can specify triggers from sensors or tasks. Notice the constant velocity is set to 75 mm/s. with LinearMotor4 selected. the position sensor is in place to indicate when the plate to weld has reached its required location. or you can specify time-based triggers. You can specify actions by activating or changing motors. 2. You can define task triggers based on time. sensing the position of an assembly component in motion. The Action dialog box appears. You can define actions to toggle mates. In the Trigger column. Click Calculate (MotionManager toolbar) to see the motion events in a (MotionManager toolbar). 4. forces. or by toggling mate suppression. the trigger for Task1. or sensed values. • You can click Add Sensor to create a new sensor trigger. or torques. 4. Next. previous tasks. Right-click LinearMotor4 in the MotionManager and click Edit Feature to view the motor parameters. you calculate the event-triggered robot motion. stop motion. Notice this is a proximity type sensor. Calculating the Motion Next. In the Feature column for Task1. Repeat Step 2 for the other motors in this study and observe that these are displacement servo motors. For this model. Do not change the action selection and click OK to close the dialog box. you open the Trigger and Action dialog boxes to better understand the event-triggered motion setup. 3. Viewing Trigger and Control Actions Task triggers are the events that drive the motion action for a task. Click Timeline View timeline.
. Change the motor velocity to 35 mm/s and click . Hover over the MotionManager timeline slider. 5.6776 seconds. 3. The simulation takes 3. Hover over the MotionManager timeline slider. you calculate the motion after changing the profile of the servo motor displacement. 113 . Right-click LinearMotor8 in the MotionManager and click Edit Feature 4. 2. The welding task does not begin until the plate is properly placed. Select Motion Study 2. the duplicate study. Click Calculate (MotionManager toolbar). 1. you duplicate the study and change the linear motor speed. Right-click the Motion Study 1 tab of the motion study and click Duplicate. Changing the Linear Motor Speed Next. The simulation takes 2. 6. the duplicate study. Changing the Servo Motor Profile Next.Motion Studies Hover over a key point to view information about the event for a given component. due to the slower motor speed of Task1. 2. 3. Notice that changing the speed with which the plate moves into place does not affect the overall simulated motion.2566 seconds. Select Motion Study 3. 1. Right-click the Motion Study 1 tab of the motion study and click Duplicate.
Select the Harmonic profile for LinearMotor9 in Task6. Click Calculate (MotionManager toolbar). To add a component or subassembly to a rigid group. 7. stress analysis duration and start time. Rigid Groups You can reduce the Motion Analysis simulation time by selecting components and grouping them into a rigid group. 4. If a rigid group contains one fixed component. • Mates between components in the group are ignored. Adjust the column widths under Actions so that you can view the feature names and their profiles. you can perform stress. 6. The required loads are obtained automatically from a calculated Motion Analysis study. 114 . 5. 9. Change the duration for tasks 8-11 to 0. Rigid groups of components behave like a single component in motion calculations: • Motion between components in the group is ignored. Structural Simulation Analysis for Motion With SolidWorks Simulation added in.5 seconds. Notice that all of the motors have a linear profile. Select the Constant Acceleration profile for LinearMotor11 in Task8. • All group components contribute to the mass and moment of inertia of the rigid group. factor of safety. Close the assembly and click No if you are prompted to save the document. the rigid group is considered fixed for motion calculations.4566 seconds. right-click the component or subassembly in the MotionManager tree. and click Add to New Rigid Group.Motion Studies 3. Hover over the MotionManager timeline slider. The simulation takes 2. or deformation analysis of components without setting up loads and boundary conditions. 8. Click Simulation Setup (MotionManager toolbar) to select a part. The servo motor profile specifies the displacement path of the motor. and the mesh for each result.
• You can specify a component for motion relative to the motor. click Contact (MotionManager toolbar). Define contact groups in the Contact PropertyManager.Motion Studies Click Calculate Simulation Results analysis results after setting them up. Curve-to-Curve Contact For Motion Analysis studies. • You can specify a phase shift for oscillating motors. • You can specify motor location and direction from the same section of the Motor PropertyManager. Create contact groups to reduce computation time for motion of assemblies with contact considerations. you can define curve-to-curve contact between 115 . you can create two groups of components to analyze component contact across the groups and ignore contact among components within the groups. • You can use linear interpolation for interpolated motors or forces. (MotionManager toolbar) to calculate stress Click a simulation result flyout option (MotionManager toolbar) to display a plot of the results after successful calculation: • Stress Plot • Deformation Plot • Factor of Safety Plot • No Plot • Delete Simulation Results Force and Motor PropertyManager Enhancements The Force and Motor PropertyManagers are more consistent and easier to use: • Force and Motor functions have preview graphs. A contact group is treated as a single component in contact force calculations. Contact Groups for Motion For Motion Analysis studies. • You can specify a servo motor for event-based motion control. • The Force PropertyManager is now called the Force/Torque PropertyManager. when your assembly includes components that make contact during motion. when you can model component contact in your assembly with two curves that touch during motion. To open the PropertyManager. Contact Contact PropertyManager Name Change The 3D Contact PropertyManager is now called the Contact PropertyManager.
Click . . select Curves always touch. In the Contact PropertyManager. 1. to rescale 4. curve-to-curve contact applies contact forces to the components. under Contact Type. Click Contact (MotionManager toolbar). 2. click Curves When the curves are in continual contact throughout the motion. To set exact key point time: 1. right-click the time bar. To specify an exact time for the time bar. and click Move Time Bar. click the spin buttons. • Select Offset to shift the current key point time by a value. under Selections. When the two components make intermittent contact during the motion analysis. From the lower right corner of the MotionManager. • Select Exact Time to enter the exact key point time. Drag the dial. Right-click a key point and click Edit Key Point Time . Setting the Exact Time for Key Points and the Time Bar You can specify the exact time for key points and the time bar in nanoseconds or other units. click Zoom to Fit the timeline view if necessary. 116 . 3. or enter a value for the key point time or offset. preventing them from moving through each other.Motion Studies the two components. You can also constrain the continual contact of two components with curve-to-curve contact. 2.
The Hole Wizard creates a 2D sketch unless you select a nonplanar face or explicitly request a 3D sketch. Features Hole Wizard Hole Wizard Creates 2D Sketches by Default When creating a Hole Wizard hole. select a Instant3D Enhancements In assemblies. Previously. Click Hole Wizard (Features toolbar) without preselecting a face. On the Positions tab of the Hole Wizard PropertyManager. select them before right-clicking. click Straight Tap Standard. and for Type select Straight Pipe Tapped hole. In the Hole Wizard PropertyManager. rulers now appear with the triad so you can move components to a defined location. For more information. 117 . The material assignments are used by mass properties. you no longer have to preselect a planar face to create a 2D sketch. See SolidWorks Help: Hole Wizard Overview. To affect several bodies.17 Parts and Features This chapter includes the following topics: • • Materials and Multibody Parts Features Materials and Multibody Parts You can assign different materials to individual bodies in a multibody part. the Hole Wizard supported straight pipe tapped holes for the DIN standard only. under Hole Type. drawing section views. and SolidWorks Simulation. see SolidWorks Help: Materials and Multibody Parts. . right-click a body and click Material. in the Solid Bodies folder. Straight Pipe Threads Added for All Standards The Hole Wizard now includes straight pipe tapped holes for all standards. when you click Move with Triad from the shortcut menu. In the FeatureManager design tree. click 3D Sketch before clicking a planar surface to create a 3D sketch.
for example. select the new Jump Gaps option to allow ribs to adjoin lip and groove faces. • Allow for adjacent geometry. where ribs join the sidewalls of the part. In the PropertyManager. for a mouse hole or a gap in the parting line. You can now: • Create a lip and groove feature when the interface between the lip and groove contains multiple faces. Lip and Groove Enhancements The lip and groove feature now covers more geometry and is more robust for cases where there are tiny faces around the parting line. 118 .Parts and Features You can use the triad to edit a Move Face feature (Translate or Rotate type) that was created with Instant3D triad. The triad appears when you select the feature in the graphics area. for example.
Right-click any CommandManager tab and click Direct Editing to activate this tab. 2. • The shortcut menu now contains the Move Face command. 4. Several other enhancements support Move Face creation and editing. • On the Direct Editing CommandManager tab. The triad appears. Creating Move Face Features Access to the Move Face tool has been enhanced.sldprt. • The Select Connected Faces pop-up toolbar now supports Move Face features. 5. • The new Direct Editing CommandManager tab contains tool buttons such as Move Face. In the PropertyManager. under Move Face. select Translate. A graphical pop-up toolbar appears to help you select connected faces. Move Face is available when you are not in any command and right-click on a face. 3. 119 . Do one of the following: • Right-click the face and click Move Face. Open install_dir\samples\whatsnew\I3D\MoveFace. Click the pop-up toolbar image shown to select all co-planar faces.Parts and Features Jump Gaps cleared Jump Gaps selected Move Face Features • The new Copy option in the Move Face PropertyManager uses Instant3D functionality to edit copied faces. click Move Face and select the face. Creating Translated Move Face Features 1. You cannot create disjoint bodies using the Copy option.
Select Move Face (Direct Editing CommandManager tab). Click . 7. 2. 3.Parts and Features If the pop-up toolbar does not appear. Creating Rotated Move Face Features 1. A ruler appears to help you drag a discrete distance. The selected faces are translated by that distance. Rotate the model and select the face shown. 120 . Drag the triad arm shown away from the face. clear the selected face and reselect it. 6. Click Front (Standard Views toolbar).
Parts and Features 4. In the PropertyManager. The triad appears when you select the feature in the graphics area. A preview of the rotated face appears. You can use the triad to edit a Move Face feature (Translate or Rotate type) that was created with Instant3D triad. 5. A protractor appears to help you rotate the face by a discrete angle. Drag the blue-colored triad ring to rotate the face. 121 . Click . Rotate is selected under Move Face.
Parts and Features Pattern and Mirror Preview Full preview is now available for pattern and mirror features. Wrap Feature Enhancement You can now project a wrap feature onto multiple faces. This method is useful for creating items such as decals. Use the freeform feature instead. Creating and editing the shape feature is not supported in SolidWorks 2010. Split curves on multiple bodies with one command. Split Lines Enhancements You can now: • • • • Select multiple contours from the same sketch to split. Existing shape features are still supported unless you change their parent features. 122 . Shape Feature The shape feature is removed from the SolidWorks software. Create split lines using sketched text. Pattern split line features that were created using projected curves. The preview supports the Up to Surface end condition for patterns and mirrors.
Menu and Toolbar Location The user interface for FeatureWorks has been fully integrated into regular toolbars and menus of the SolidWorks software. The enhanced messages appear when the following features are not recognized: • • • • • • • Chamfer Fillet Hole Boss Extrude Cut Extrude Boss Revolve Cut Revolve Bosses and Cuts Interactive Recognition of Bosses and Cuts Interactive recognition of extrude features (bosses and cuts) has been enhanced. • Click Recognize Features (Data Migration tab of the CommandManager). During interactive recognition of boss extrude features and cut extrude features. FeatureWorks can now recognize dissimilar features if they have a face that is parallel to the selected face. the add-in loads dynamically if you have installed it and are running SolidWorks Professional or SolidWorks Premium. The message also includes a link to a help topic. if the software fails to recognize a feature. open a part that contains imported features and do one of the following: • Click Recognize Features or Options (Features toolbar). Diagnostic Messages Error messages that appear when a feature cannot be recognized have been enhanced. select Check parallel faces. In addition to recognizing similar features. • Click Insert > FeatureWorks and then click Recognize Features or Options. a detailed error message appears to explain the reason for the failure and to suggest possible solutions. During interactive recognition. 123 .Parts and Features FeatureWorks Available in SolidWorks Professional and SolidWorks Premium. To access FeatureWorks commands. When you select a related command.
FeatureWorks recognizes four boss extrude features: Automatic Recognition of Bosses and Cuts Automatic recognition of extrude features (bosses and cuts) has been enhanced to recognize more features. the software automatically executes interactive recognition algorithms for extrude features. In the graphics area. Yes. In the graphics area. select Prompt. 124 . Draft In interactive recognition mode. Child Features Child Features of Recognized Features You can now use Edit Feature to recognize child features of features that have already been recognized. Direct Edit of Bosses and Cuts You can now use Edit Feature to recognize extrude features (bosses and cuts). right-click an unrecognized child feature of a feature that has already been recognized and click Edit Feature . for Automatically recognize child features when using Edit Feature. If an imported body remains after automatic recognition is complete. when you select one face. on the Resize Tool page. you can now recognize child features of the face. right-click an unrecognized extrude feature on an imported body and click Edit Feature . Child Features in Imported Bodies While using Edit Feature to recognize a face on an imported body. In the FeatureWorks Options dialog box.Parts and Features In this example. All types of extrude features (bosses and cuts) that are recognized by FeatureWorks are supported. you can recognize all the fillets and drafts associated with a selected neutral face in one step. or No.
or. select Standard features. select Holes under Automatic Features. sketches. FeatureWorks recognizes two separate hole features. Previously. select the holes in Recognized Features and click Combine Features. Combining Holes You can combine holes on the same plane into a single feature. you had to delete such features before proceeding with recognition of the part. FeatureWorks recognizes all the fillets and drafts associated with that face in one step.Parts and Features Previously. Use automatic recognition mode to recognize the holes. you had to use one step to recognize the fillets and then more steps to recognize each of the different drafts. Holes on Nonplanar Faces You can recognize holes on nonplanar faces. right-click the face of an unrecognized hole feature and click Edit Feature . In automatic recognition mode. Then in the Intermediate Stage PropertyManager. Sketches. select Draft and then Recognize filleted. Features supported for re-creation but not for recognition include: • Sketches: • 2D Sketch • 3D Sketch • Features: 125 . in the graphics area. Reference Geometry. and Surface Features FeatureWorks recreates (but does not recognize) some reference geometry. In interactive recognition mode. When you select the neutral face. Use automatic or interactive recognition modes. and surface features. Holes Intersecting Holes You can recognize intersecting holes. For Feature type.
Trim Surface Feature Enhancements Copies of trimmed bodies are no longer stored when you create standard trim surface features. In the PropertyManager. Select Gap Control to control which gaps are knitted closed and which remain open. resulting in smaller file sizes and improved performance. The Minimal adjustment option is removed from the Knit Surface PropertyManager for all new knit surface features. To create standard trim surface features: 1. under Trim Type. 2. Select other trim surface options and click . 3. For more information see SolidWorks Help: Knit Surface PropertyManager .Gap Control. Surface Extend Feature Enhancements Tangent surfaces no longer fray when you extend them. Click Insert > Surface > Trim.Parts and Features • Delete Face • Move Face • Surface features: • Surface-Offset • Reference Geometry features: • Plane • Axis Surfaces Knit Surface Features The Knit Surface PropertyManager has new options: • Select Merge entities to merge faces that have the same underlying geometry type. select Standard. 126 .
127 .Parts and Features To extend surface features. click Insert > Surface > Extend.
Controlling Scenes You can orient the floor of a scene relative to a model. you can now see PhotoWorks decals that were applied in SolidWorks and that were visible when the part or assembly was saved. This chapter includes the following topics: • • • • • • PhotoWorks Decals in PhotoView 360 Controlling Scenes Support for Background Images and Custom Environments Video Tutorials Saving Custom Views Camera Effects PhotoWorks Decals in PhotoView 360 In PhotoView 360. you must use SolidWorks with PhotoWorks added in to edit. create. or delete a decal. make changes on the Environment Settings tab. or a background image. the floor.18 PhotoView 360 Available in SolidWorks Professional and SolidWorks Premium. Up Axis = Y Up Axis = Y. You can also display or hide the environment. On the Settings dialog box. As in earlier releases. Axis Flipped 128 .
The following image is rendered with the 3 Point Beige environment and a custom 2d background: For more information about controlling backgrounds in PhotoView. Click Settings. • Click Load Environment Image. see PhotoView 360 Help: Settings Dialog Box . On the Environment Settings tab: • Click Load Background Image. see PhotoView 360 Help: Settings Dialog Box . • Select Show Background or Show Environment to show or hide either type of image. but you can show only one at a time. You can also load High Dynamic Range Images (HDRI) to replace the current environment.Environment Settings Tab. 129 .PhotoView 360 Up Axis = X Up Axis = Z For more information about controlling environments in PhotoView. Support for Background Images and Custom Environments You can now include 2D background images for display behind the model. You can hide both.Environment Settings Tab. Loading a custom HDRI image changes the background. reflections. and lighting of the rendering.
The tutorials are available on the Gallery site. and select a view from the list. Click Settings. Display a view that you saved earlier to ensure that the rendering has a specific orientation. Camera Effects The camera now supports additional effects. 130 . • Depth-of-field controls let you create renderings where part of the image is in focus and other parts are not in focus.Output Settings Tab and Settings Dialog Box . • You can switch between perspective and orthogonal views. Saving Custom Views You can now save custom view orientations in PhotoView 360. Make changes on the Output Settings tab in the Image Processing section and on the Camera Settings tab. Right-click in the workspace. and name the view. • You can add a bloom effect to the final render to create a glow for emissive appearances or areas of very bright environment reflections.PhotoView 360 Video Tutorials New video tutorials are available for PhotoView 360. Example: Effect of Changing the Focal Length Focal length = 50 mm (default) Focal length = 35 mm For more information about camera settings. Click Help > Online Tutorials to get started. right-click in the workspace. click Recall Custom View. To restore a saved view.Camera Settings Tab. see PhotoView 360 Help: Settings Dialog Box . click Save Custom View.
PhotoView 360 Example: Effect of Setting Bloom Image without bloom Image with bloom 131 .
right-click the flattened route in the FeatureManager design tree and click Edit Flattened Route. you open an electrical route and create a flattened drawing to scale. Scaled Drawing of an Electrical Route In this example. You can use the manufacture-style flattened route when designing electrical cable routes for manufacturing. To edit a manufacture-style flattened route. Select Manufacture in the Flatten Route PropertyManager to create a manufacture-style flattened route. This chapter includes the following topics: • • • • • • • • • • Manufacture-style Flattening Adding Components and Assembly Fittings to Routes 180-Degree Elbows or Bends for Piping Piping Drawings Access to Pipe. or Electrical Harness Coverings Multiple CPoint Enhancements P&ID Data Import and Modeling Process Reference Designators Pipe and Tube Route Export Enhancements Routing Library Enhancements Manufacture-style Flattening Manufacture-style Flattening A manufacture-style flattened route unfolds a route to scale and defines the boundary of a formboard in which to place the flattened route. Tube. You can edit: • Segment curvature • Segment angle • Flattened route center You cannot apply manufacture-style flattening to ribbon cables.19 Routing Available in SolidWorks Premium. 132 .
Routing Opening and Saving the Model First you open the routing subassembly and save it with another name. Flattening the Route Next you flatten the route subassembly. 133 . 2. and rename the file to my_5connector.sldasm. Click File > Save As. 1. Open install_dir\samples\whatsnew\routing\manufactureflatten\5connector. browse to a new directory on your computer.sldasm.
when prompted. In the next procedure.Routing 1. 134 . Right-click ManufactureFlattendRoute1 in the FeatureManager design tree and click Edit Flattened Route. In the PropertyManager. Editing the Flattened Route Next you edit the flattened route to change the curvature of a cable. In the PropertyManager. Viewing the Drawing Next you check the drawing and decide whether to edit the flattened route. 2. and clear all other drawing options. Click . 1. Select the top right segment of the harness. Examine the drawing to decide whether to edit the flattened route. Select the curved spline as shown. . 3. click Save All and Save. you change the curvature of one of the cables. select Manufacture. 2. 1. The selected segment is listed in the Flatten Route PropertyManager. 3. Click Routing > Electrical > Flatten Route 2. Close the drawing and. select Drawing Options and Connector table.
4. 6. 5. Change the Radius to 20 mm. View the changes before clicking . 135 . 3. click Save All. Click File > Save As and save the flattened route assembly to a file name of your choice. the Bend Angle to 10 degrees. and click Apply. 7. Close the flattened route assembly and in Save Modified Documents.Routing The spline is listed in the selection box under Editing Tools in the Edit Flattened Route PropertyManager. Click Adjust Curvature .
• Drag elbows onto flanges. or electrical harnesses from the Covering Library. a gasket. From the Save Components to Library page of the Routing Component Wizard. To create a piping drawing. Tube. and other fittings. and another flange into a route to insert a gasket between flanges. or Electrical Harness Coverings You can access coverings for pipes. and a BOM in an isometric view. you can drag an assembly consisting of a valve with four flanges into a pipe. pipes. In the wizard. Multiple CPoint Enhancements When you drag a routing component with multiple CPoints to create a route. You can also create custom coverings with fixed diameters. You can also right-click a CPoint in the graphics area to add or remove it from a route. Piping Drawings Piping drawings of routes include fittings. select Select CPoints to select which CPoints to route. provided the component is set up for multiple CPoint selection. valves. Click Coverings (Routing Tools toolbar) to access or add library coverings. dimensions.Routing Adding Components and Assembly Fittings to Routes You can: • Make fitting to fitting connections: • Drag flanges onto elbows. • Drag a flange. you can control the treatment of multiple CPoints when creating or editing routing components. 136 . tubes. 180-Degree Elbows or Bends for Piping You can use 180-degree elbows or create 180-degree bends in pipes. valves. • Drag entire assemblies with appropriate references into a pipe. • Create branch lines in a pipe by dragging a tee into the pipe. Access to Pipe. • Split a run of pipe by dragging a fitting or a pair of flanges into the pipe. and other fittings. click Pipe Drawing (Piping toolbar). you can select CPoints to include in the route from the Multiple CPoints dialog box. For example.
Export routing components such as formed bends and penetrated pipes.pcf file. right-click the route and select Export Pipe/Tube Data. see Documents and Settings\All Users\Application Data\SolidWorks\SolidWorks_Version\design library\routing\piping\pnid sample. and click Import P&ID. Select the assembly origin at the origin point for the . Reference Designators You can use a component property called a Component Reference to store reference designators in an electrical harness. For an example. from You must import the P&ID data file in . sample equipment parts. select the P&ID file.Routing P&ID Data Import and Modeling Process You can import a Piping and Instrumentation Diagram (P&ID) file created with an external system and use that file as a guide in building route assemblies. These references are added automatically when you import from a from-to list or a P&ID file. 137 . You can assign a different Component Reference value for each instance of a component.xml. You must show hidden files to view this folder. import schematics from a P&ID file to design a piping route: • The piping design matches the connectivity and pipe sizes in the schematic.xml format. • Design validation tools warn of any deviation from the schematic. common component SKEY codes are supported to improve the routing of in-line fittings. To access pipe and tube route data export options.pcf files. To import route specifications from a P&ID file. You can: • View component references in the FeatureManager design tree.pcf files. and valve components are in the Routing Library. • Select Highlight Search from the Task Pane to search for component references. Export separate routes to different . As a best practice. • Include component references in drawings and BOM tables. click Piping and Instrumentation the SolidWorks Task Pane. The path to the Application Data folder depends on your operating system. Pipe and Tube Route Export Enhancements You can: • • • • Specify the file name and location for . Routing Library Enhancements New fittings. In addition.
Routing 138 .
Cut Lists In the FeatureManager design tree. 139 .20 Sheet Metal This chapter includes the following topics: • • • • • Multibody Sheet Metal Parts Closed Corner Improvements Hem Improvements Flat Pattern Improvements Exporting Sheet Metal Parts to DXF or DWG Multibody Sheet Metal Parts SolidWorks multibody part functionality has been extended to sheet metal to allow you to create complex sheet metal designs. • Insert one or more sheet metal. weldment. or using the Move/Copy Body command. mirroring the body. Insert Bends. or other bodies into an existing sheet metal part. In addition. the main tree lists each body and its features in the order in which you add them. • Split a single sheet metal part into multiple bodies. • Duplicate a sheet metal body in a part by creating a linear or circular pattern. To create a multibody sheet metal part: • Create new bodies in an existing sheet metal part using Base Flange. and Lofted-Bend commands. with a flat pattern specific to the body. Multibody sheet metal parts can consist of multiple sheet metal bodies or a combination of sheet metal and other bodies such as weldment bodies. a cut list contains a separate representation for each body. Convert to Sheet Metal.
You can use the body-related properties in bills of materials and drawings. You can copy the features of the original part to the mirrored part by breaking the link to the original part. a new part is created. 2. 140 . including the ability to automatically organize and update sheet metal bodies. In the Insert Part PropertyManager: a) Under Link.Sheet Metal Multibody sheet metal cut lists offer the same features as weldment cut lists. The source part is visible in the graphics area. When you mirror a sheet metal part. and view sheet metal properties. Merging Sheet Metal Bodies You can merge sheet metal bodies of the same thickness by: • Using the Up to Edge and Merge option when inserting an edge flange between two bodies with parallel linear edges. click Break link to original part. 3. A new part opens. The copied sheet metal features are added to the FeatureManager design tree of the new part. Creating a Mirrored Sheet Metal Part The Mirror Part command now supports sheet metal parts. To create a mirrored sheet metal part: 1. • Using the Merge result option when adding a base flange that overlaps the profiles of multiple bodies with coplanar faces. Select the Front Plane and click Insert > Mirror Part.sldprt. Open install_dir\samples\whatsnew\Sheetmetal\corner.
In the Heads Up View toolbar. You can also access the features by expanding Cut list(1) Body-Move/Copy1. The features of the original part are displayed and are fully editable.sldprt. c) Click to close the Locate Part PropertyManager. 6. the resulting sheet metal body has its own sheet metal definition. click View Orientation > Front . In the FeatureManager design tree. Keep this part open for use in the next section. When you insert a body and break the links to the source part. expand corner_Mirrored Features1. 141 . 4.Sheet Metal b) Click . You can: • • • • Edit the features of the body Give each body its own material definition and custom properties Isolate and flatten a selected body Display bodies individually in drawings To create a multibody part by inserting a part: 1. Save the part as corner_mirrored. 5. The part appears in the graphics area mirrored around the plane. > Inserting a Part to Create a Multibody Sheet Metal Part The Insert Part command now lets you create a multibody sheet metal part by inserting a sheet metal body into another sheet metal part.
In the Heads Up View toolbar. type 4. 5. if the Locate Part PropertyManager opens to Mate Settings.Sheet Metal 2. click View Orientation > Right The parts are aligned back to back.sldprt.00in. move the translucent image of corner. You do not have to select anything in the model. The image of the inserted part moves four inches to the left. In the graphics area. 2. skip to step 3. Expand Translate. Locating the Inserted Part To locate the inserted part: 1. For Delta Z .prt. Click Insert > Part. If the PropertyManager opens to Translate. Under Link. 142 . under Locate Part. In the PropertyManager. Click to place the part in the graphics area and open the Locate Part PropertyManager. select Break link to original part. 4. select corner. select Launch move dialog. 6. 4.prt until it aligns with corner_mirrored. 3. and click Open. 3. click Translate/Rotate. To separate the parts.
expand corner_Mirrored Features1 to view the features of the mirrored body.Sheet Metal 5.sldprt. Click . Accessing Sheet Metal Bodies in Multibody Parts You can access the bodies of a multibody sheet metal part in the main FeatureManager design tree or in a cut list added to the top of the tree. 7. In the Heads Up View toolbar. Save the part as corner_multipart. 1. 143 . 6. which was the original body in the part. click View Orientation > Isometric . In the FeatureManager design tree.
Body-Move/Copy1 flattens and the second body is hidden. 4. Near the top of the tree. expand the cut list The cut list shows two bodies: .Sheet Metal 2. Expand Body-Move/Copy1. The features listed are the same as the features under corner_Mirrored Features1. Right-click Body-Move/Copy1 and click Flatten . 144 . Body-Move/Copy1 and Body-Move/Copy2 3.
You can unlock flange. Body-Move/Copy1 appears in a transparent state. Click Exit Isolate. Body-Move/Copy1 is hidden. You can also click Exit Flatten in the Confirmation Corner. Both bodies are completely visible. the angle to override the calculation to extend or shorten the connecting To merge the sheet metal bodies in corner_multipart. 6. Right-click Body-Move/Copy1 again and click Exit Flatten to restore the body to its folded state. click Visibility of Removed Bodies Transparent . select the outside front edge of corner Features1. 2. Both bodies are visible. 145 . for Edge. and select 8. 9. and must belong to different bodies. Click Edge Flange (Sheet Metal toolbar). Click again and click Hidden. The Up to Edge and Merge option calculates the angle between the edges automatically. The option is available if you select a single edge under Flange Parameters. under Flange Parameters. part of the sheet metal part base.sldprt: 1. The edges must be the same thickness. Right-click Body-Move/Copy2 and click Isolate. In the Edge-Flange PropertyManager.Sheet Metal 5. In the Isolate dialog box. Only Body-Move/Copy2 is visible. Merging Sheet Metal Bodies by Inserting Edge Flanges The new Up to Edge and Merge option in the Edge Flange Property Manager connects two parallel edges in a multibody part. 7.
In the FeatureManager design tree Cut List. Click . 146 . The edge flange merges the two bodies. select Up to Edge and Merge. To make selection easier. Edge-Flange6. 5. 4. Right-click Edge-Flange6 and click Flatten The merged part flattens. move over an edge and press G to magnify the area. from the Length End Condition list. . . Under Flange Position. select the outside front edge of corner_mirrored You must select corresponding edges (for example. click Bend Outside 6. Under Flange Length. there is now only one body.Sheet Metal 3. For the reference edge Features1. . the outer edges) on both bodies for Flatten to work. 7.
Click Sketch (Sketch toolbar). 2. 6. for Orientation. Select the front plane. select Vertical. 5. Preparing to Split the Part Create the sketch to use to split the part. and other features that can cut a body into pieces. 4. Sketch a vertical line through the midpoints of the face.sldprt. You can separately edit and flatten the bodies that are created. Extend it beyond the model face. In the Confirmation Corner. to restore the body to its folded Splitting a Sheet Metal Part You can now split a sheet metal part to create a multibody part. To create the sketch: 1. You can split sheet metal parts using extruded/revolved cuts. click Exit Flatten state. 3. Click Line > Line (Sketch toolbar). Open install_dir\samples\whatsnew\Sheetmetal\casing_base_part. This example describes the use of the Split feature.Sheet Metal 8. split line. In the Insert Line PropertyManager. 147 .
select the sketch. double-click the first body. under Trim Tools. 148 .sldprt and click Save. Exit the sketch. for File name. Splitting the Part To split the sheet metal part: 1. The name appears in the PropertyManager and in the Body 1 callout. Repeat steps 4 and 5 to assign Body 2 the name casing_right. 6. Under Resulting Bodies. 4. In the PropertyManager. 5. type casing_left. 2.sldprt. Click Insert > Features > Split .Sheet Metal 7. Click Cut Part. In the Save As dialog box. 3.
expand Cut list (2). In this case. 10. Split1[1] and Split1[2] are separate parts. In the FeatureManager design tree. Both bodies are visible. the last feature added is the split feature. Right-click Split1[2] and click Flatten. The Split1[2] flattens and Split1[1] is hidden. Click . 8. The software names bodies in the cut list according to the last feature added to the body. Right-click Split1[2] and click Exit Flatten to restore the body to its folded state. the cut list names change. Inserting a Sheet Metal Part Using a Base Flange You can use the commands that create sheet metal parts to create new bodies in an existing sheet metal part. As you add features. 9. The part now contains two sheet metal parts. These include: 149 .Sheet Metal 7.
7. In the Heads Up View toolbar. Select Insert > Reference Geometry > Plane. select the face of the flange. click View Orientation 4. 1. Click Base Flange/Tab (Sheet Metal toolbar). Exit the sketch.Sheet Metal Convert to Sheet Metal Lofted Bend Insert Bends Base Flange/Tab This procedure illustrates the use of the Base Flange/Tab command to insert a tab without merging it with another body in the part. Click Corner Rectangle (Sketch toolbar) and draw a rectangle extending from the lower corner of the flange to the right. 2. 150 . . Extend the plane to the right. 6. b) Select Coincident c) Click . In the PropertyManager: a) For First Reference. 5. > Front . A sketch opens on the plane. 3.
b) Under Flange Length. click the intersection point of the top of the edge flange and Tab1. clear Merge result. All the editing options are available for both selection methods. select the right edge of the base flange. 1. for Edge. Right-click the Edge-Flange4 feature and click Edit Sketch . In the PropertyManager: a) Under Flange Parameters. 151 .00. 3. Click . To edit the flange feature from the cut list. The Base-Flange1 feature appears at the bottom of the FeatureManager design tree and in the cut list. under Sheet Metal Parameters. Editing Sheet Metal Bodies In a multibody sheet metal part. 4. click Material Outside d) Click . c) Under Flange Position.Sheet Metal 8. 5. expand the cut list and expand the Edge-Flange4 body . Click Edge Flange (Sheet Metal toolbar). 2. . 9. In the graphics area. set the Length End Condition to Blind and the Length to 35. you can edit a feature of an individual body by selecting the feature in the FeatureManager design tree or from the body's folder in the cut list. In the Base Flange PropertyManager.
9. The edge flange is resized. to 10. 8. Click Exit Sketch Closed Corner Improvements You can now use the existing Closed Corner command with a greater variety of sheet metal parts. Click the intersection point of the bottom of the edge flange and Tab1. . You can use the Closed Corner command to add material between sheet metal features: 152 . to 55. In the PropertyManager: a) Under Parameters. set the X Coordinate b) Click .Sheet Metal 6. 7. set the X Coordinate b) Click . In the PropertyManager: a) Under Parameters.
you can now edit the hem profile to control the length.Sheet Metal • When there is a cut across flanges • With large radius bends • When the part is created using Insert Bends or Convert to Sheet Metal • With faces that are part of a larger corner The new Automatic propagation option controls automatic recognition of matching faces. If you delete a face from one of the face set selection boxes. You can build the hem according to design requirements. 153 . It is enabled by default. the option turns off to let you make manual selections. even when it is not applied to the whole edge. Hem Improvements Improved sheet metal hem functionality lets you design more complex sheet metal parts. When you add a hem to a sheet metal part edge. You can also add hems to selected nonlinear edges.
Flat Pattern Improvements Graphical highlighting of self-intersecting flat patterns makes it easier to recognize areas that need improvement for manufacturing. This minimizes the weldment gap for manufacturing of rolled sheet metal parts with cut extrudes and produces a flat pattern with different outlines for the inner and outer faces of the cut. You can also turn off the Normal cut option. With a sheet metal part open. 1. and forming tools. You can also export entities such as bend lines.Sheet Metal You can: 1. sketches. open the PropertyManager by doing one of the following: 154 . Exporting Sheet Metal Parts to DXF or DWG The new DXF/DWG PropertyManager exports sheet metal bodies to . A preview shows your selections and lets you remove unwanted entities such as holes or cutouts. Change the size of the hem feature.dwg files. 2.dxf or . Add hems to edges on different levels.
Click Save. To remove entities. The PropertyManager appears. • Right-clicking the Flat-Pattern feature and clicking Export to DXF/DWG. Cancel the preview and return to the PropertyManager if you want to make changes. 5. 155 . The DXF/DWG Cleanup preview window appears. Select the bodies and entities to export and click . 2.Sheet Metal • Saving the part (File > Save As) to a dxf or dwg file type. 3. 4. select them and click Remove Entities.
Enhancements marked with (Premium) are available in SolidWorks Simulation Premium.21 Simulation Available in SolidWorks Premium. The wizard interacts with Simulation interface components. to guide you through the simulation workflow. such as the Simulation study tree and PropertyManagers. Click SimulationXpress Analysis Wizard or Tools > SimulationXpress and follow the prompts. Enhancements marked with (Professional) are available in SolidWorks Simulation Professional and SolidWorks Simulation Premium. 156 . provide better guidance to new users. This chapter includes the following topics: • • • • • • • • SimulationXpress NAFEMS Benchmarks Simulation Interface Simulation Studies Connectors Mesh Contact Result Viewing SimulationXpress New SimulationXpress Interface SolidWorks SimulationXpress is redesigned to reduce screen clutter. The new wizard uses elements of the full Simulation Professional and Premium interface to make the transition to Simulation easier. The following enhancements are available in SolidWorks Simulation. and allow experienced users to create simulations more quickly.
To access the benchmarks. 157 . or maximum resultant displacement. Frequency. Thermal. and Linear Dynamic studies. SimulationXpress allows you to perform optimization. You can minimize the mass by varying one model dimension. NAFEMS Benchmarks New National Agency for Finite Element Methods and Standards (NAFEMS) benchmarks are added for Static. in the Help menu. such as the force values and bolt types. so you can quickly learn to use the new design study feature. maximum von Mises stress.Simulation Optimization in SimulationXpress After running a simulation on a body and reporting the results. click SolidWorks Simulation > Validation > NAFEMS Benchmarks. Nonlinear. SimulationXpress uses the New Design Study on page 161 interface with certain restrictions. You can define one constraint. Simulation Interface Simulation Study Tree Enhancements • Simulation study tree feature names are now more descriptive and provide more information. which can be the factor of safety.
158 . and connectors into folders. Simulation displays details of the feature. • Fixture icons in the tree now indicate the type of fixture.Simulation • When you move the cursor over a feature in the tree or its symbols in the graphics area. loads. • You can now organize fixtures.
such as connectors. while the pushpin is active connectors that you create into a separate folder. when applying a force to a group of faces. or External Loads in the Simulation study tree and select Create New Folder. When you click connectors. Edit the properties. the software groups PropertyManager Enhancements • You can now select an entity in two different selection areas of a PropertyManager. fixtures.Simulation Right-click Connections. . the properties are applied in all of the selected 159 . Drag corresponding connections. • In the Connectors PropertyManager. to edit common input. or external loads to the folder. you can select one of these faces as a reference geometry. right-click. For example. Fixtures. and select Edit Definition. or right-click the folder name and select an item to create in the folder. . Select several connectors of the same type. • You can select multiple features.
click Backup/Recover and select Save auto-recover info after meshing and after running a simulation study. • Body icons appear in the fatigue study tree to allow you to define S-N fatigue curves. Mesh and Solver Window Improvements The Mesh Progress and Solver Status windows now include memory usage information. you choose constant or variable amplitude. The redesigned Solver Status window now shows memory usage. On the System Options tab. the number of components that failed to mesh. 2. minimized Simulation study tooltip allows you to track the solver status without having to show a separate solver window.Simulation Simulation Studies General Enhancements Enhanced Auto-Recover Capability SolidWorks backup and recover settings now apply to Simulation. elapsed time. and progress. not in the associated studies. solver information. 1. • When creating a fatigue study. Simplified and Enhanced Fatigue Study (Professional) Fatigue study enhancements include: • S-N material curves are now defined in the fatigue study. and progress. You have the option to back up and recover file information after meshing and running a study. • You can now use stress results at a particular solution step from nonlinear and linear dynamic studies. Click Options (Standard toolbar) or Tools > Options. Expanded Features for Simulation Advisor The Simulation Advisor is enhanced with a new interface that interacts with the Simulation PropertyManagers to help new users create. elapsed time. • Damage is shown as a percentage instead of as a fraction in Damage plots. define. The Mesh Progress window shows memory usage. solve. Move the pointer over the Simulation study tab of a running study to see the status of the study. A new. and view the results of Static studies. The Change Event Type command is removed. in addition to information shown in previous versions. You can view other material properties in a fatigue study. 160 .
In a nonlinear study tree.Simulation Fatigue Check Plot (Professional) The Fatigue Check plot alerts you if certain regions of your model are likely to fail due to repeated loading and unloading over infinite time. right-click the body and select one of the available options: Exclude from Analysis. For more information about how the Fatigue Check plot is calculated. The Fatigue Check plot shows the model in two colors: • Blue regions indicate that the stress levels are so low that fatigue should not be a concern with the specified loading. You can assess in advance the safety of your model due to fatigue. You can plot the updated bodies and the calculated results for different iterations or scenarios by clicking their columns on the Results View tab. Simplifying Assemblies for Nonlinear Studies (Premium) You can simplify assemblies and multibody parts in nonlinear studies by treating selected bodies as rigid. After you run a static study. The Fatigue Check plot is not available for composite shells or beams. • Red regions indicate that the specified loading will consume a percentage of the part's life. fixing them in space. or excluding them from the analysis. and select Define Fatigue Check The plot is based on a single constant-amplitude fatigue event with a fully-reversible or zero-based loading. without running a fatigue study. These options can save you computational time when analyzing large assemblies. see Simulation Help: Fatigue . It is recommended to run a fatigue study to assess in detail the safety of your model's design. The new Design Study interface consolidates the earlier interfaces for optimization studies and design scenarios. click Design Study (Tools toolbar) or Insert > Design Study > Add. New Design Study You can now create the Design Study to evaluate or optimize models. Make Rigid.Check Plot. right-click Results Plot. or Fix. based on results from static studies. To create a study. 161 . A Design Study tab appears at the bottom of the graphics area.
Different sensors are available for use in Design Studies depending on your SolidWorks license and whether you are running an Evaluation study or an Optimization study. on the Design Study tab. You can use all Simulation parameters and driving global variables.Simulation You can also right-click a study tab and select Create New Design Study. use the Variable View tab to set up the parameters for the Optimization Design Study. SolidWorks Standard SolidWorks Professional SolidWorks Premium SolidWorks Simulation Professional SolidWorks Simulation Premium Mass Properties Dimension Simulation Data Optimization Design Study To perform an optimization. If you choose to define Variables as a Range or define Goals. 162 . Define the variables as Range. you can minimize the mass of an assembly with density and model dimensions as the variables. For example. select the Optimization check box. or Range with Step. run them. Use the Table View tab to manually define certain scenarios with all discrete variables. the program automatically selects the Optimization checkbox. Discrete Values. You can use the Design Study in SolidWorks for models without Simulation results. • Variables: You select from a list of predefined parameters or define a new parameter by selecting Add Parameter. and find the optimal one among the defined scenarios. and volume as the constraint. In most cases.
• Constraints: You select from a list of predefined sensors or define a new sensor. When using Simulation results. • Constraints: You can select from a list of predefined sensors or define a new sensor. If you define only discrete variables.Simulation You can define a combination of discrete and continuous variables. The Design Study runs the selected Simulation studies. Evaluation Design Study The module lets you evaluate certain scenarios and view their results without performing an optimization. and tracks the sensor values for all iterations. If you select Range. Define the following items to set up the Evaluation Design Study: • Variables: Select from a list of setup parameters or define a new parameter by selecting Add Parameter. FeatureManager design tree Design Study tab • Goals: You use sensors to define the goals. Selecting a scenario on the Results View tab updates the model in the graphics window. Use the Table View tab only to specify each scenario manually or clear certain scenarios if required before running the study. Define the variables as Discrete Values or Range with Step. the program finds the optimal scenario only from the predefined scenarios. select the Simulation study associated with the sensor. a tip deflection of 1mm with cantilever length as the variable. Scenarios are highlighted in different colors. You can also define exact goals. the program uses the Optimization Design Study. for example. Viewing the Results of the Design Study Click the Results View tab to see the results. Use the Variable View tab to allow the program to automatically define the scenarios based on all possible combinations of defined discrete variables. 163 .
Optimization Design Study Variable Type High Quality Continuous (Range) Study Quality Fast Results Operation Finds the optimal solution Finds the optimal solution using using many iterations and few steps and displays the initial displays the initial scenario. the optimal scenario and all iterations. You plot local trend graphs for variables. You display the plots and updated bodies only for the optimal and initial scenarios. You plot local trend graphs for variables. Results You display the plots and updated bodies for all iterations in the Results View tab.Simulation Scenario Color Green (available only for optimization mode) Red Background color Gray text with background color Meaning Indicates the best or optimal scenario Indicates violation of one or more constraints by the scenario Indicates current scenario and all scenarios that are not optimal or faulty Indicates failure to rebuild the scenario or interpolate the results for the scenario when using a low quality study with discrete variables You can plot simulation results on the model and display graphs depending on the combination of variables and the quality of the design study. 164 . Design Study Outcomes The tables summarize the expected results for different combinations of variables and study quality. and optimal scenarios.
Results You display the plots and updated bodies for all iterations. It finds the optimal solution among the If you use continuous scenarios. You display the plots and updated bodies for initial and optimal scenarios. Calculates initial and optimal scenarios accurately. Operates on a continuous space even for discrete variables while finding the optimal solution. Evaluation Design Study 165 . Local trend graph plots include interpolated results. You plot design history graphs and local trend graphs for variables. and interpolates the results for the remaining scenarios. You plot local trend graphs for variables. You plot design history graphs for variables. You plot local trend graphs for variables. Finds the optimal solution using many iterations and displays the initial scenario.Simulation Discrete (Discrete Values and Range with step) Operation Fully calculates the results for each scenario. Resolves back to the discrete space while reporting the optimal solution. and only updated bodies for the remaining scenarios. Finds the optimal solution using few steps and displays the initial and optimal scenarios. the optimal scenario and all iterations. You display the plots and updated bodies only for the optimal and initial scenarios. Resolves back to the discrete space while reporting the optimal solution. the program fully calculates the results for all iterations. Results You display the plots and updated bodies for all scenarios. It finds the optimal solution among the defined scenarios. Combination Operation Operates on a continuous of continuous space even for discrete and discrete variables while finding the optimal solution. variables.
the Design Study runs the Simulation study to determine the factor of safety. Click the Ready_Torsion study tab to review the Simulation study. You plot design history graphs for variables. A gray column indicates interpolated results. because discrete scenarios cannot be defined with a range of variable values. Minimizing the mass saves the cost of the part by reducing material while meeting your validation constraints. You plot history graphs and local trend graphs for variables.sldprt. You display the plots and updated bodies for fully calculated scenarios. right-click its column heading and select Run. and goals. Design Study of a Knob You explore the new Design Study interface by solving this example. Do not use continuous variables with an Evaluation Design Study. You perform an optimization of a knob to minimize its mass by defining the variables. for each scenario. At each iteration of this example. It applies a torque to the handle and does not allow the yellow faces to twist. open install_dir\samples\whatsnew\Optimization\knob. To fully calculate an interpolated result. You display the plots and updated bodies for all scenarios. To see the model. You display only updated bodies for the scenarios with interpolated results. constraints.Simulation Variable Type Discrete Study Quality High Quality Fast Results (Discrete Values and Results Range with step) Operation Fully calculates the results Interpolates the results for certain scenarios. The study subjects the knob to torsional loading. 166 .
Simulation Defining the Variables You can select Simulation parameters and driving global variables for Variables. but also increase the mass of the knob. For Cyl_Ht. 2. 1. in Constraints. You can also use driven global variables for the constraints. 6. For FOS. select High quality (slower) and click . in Variables. select FOS. 7. In Variables. select Range. In the PropertyManager. Defining the Constraints and Goals Use sensors to define constraints and goals for the design study. 4. click Options . For Rib_Thickness. On the Variable View tab. 8. The parameter represents the height of the cylinder defined by the Boss-Extrude1 feature. Ribs increase resistance to torsional loading. feature. 3. 167 . For Min. For Min. For Min. type 15mm. select Cut_Depth. type 11mm and for Max. For Cut_Depth. select Cyl_Ht. type 1mm and for Max. On the Variable View tab. type 3mm. under Design Study Quality. type 10mm. See SolidWorks Simulation Help: Design Study Outcomes. In Variables. To open the part and define the variables for the design study: 1. The parameter represents the depth of the cut defined by the Extrude3 You can save mass by increasing the depth of the cut. In this example you vary different model dimensions within a certain range to optimize the mass of the knob. type 1mm and for Max. The variable uses the tracked value from the factor of safety (FOS) sensor in the FeatureManager design tree. select Range. On the Optimize study tab. The program finds the optimal solution using many steps without compromising the accuracy of the solution. select Rib_Thickness. select Range. The parameter represents the thickness of the three ribs defined by the Rib4 feature. 5. 2. select Ready_Torsion.
select Minimize. See SolidWorks Simulation Help: Properties for the Optimization Design Study for a description of the method. 3. The study updates the body to correspond to the optimal variables in the graphics window. 3. For Mass1. You require the optimal knob design to carry at least two times its operational load. In Goals. and finds the optimal solution. Click Run. 2. 168 . select is greater than and for Min. Click the Optimal column highlighted in green. You want to reduce the mass of the knob as much as possible.Simulation The design study updates the sensor value at each iteration by running the Ready_Torsion study. For condition. Running the Optimization Design Study 1. Review Iteration1. FOS < 2. Iterations that do not satisfy the constraints are highlighted in red. invokes the Simulation study at each iteration. without violating the constraint on the FOS. 4. Here. select Mass1 from the list of sensors. 5. The program selects the variables using a Design of Experiments method. type 2.
as the program always located the surface at the mid-plane of the laminate. Previously. For example. while creating a model. The figure shows the meaning of the negative and positive offset values. The Shell Definition PropertyManager for composites now has these options: Middle Surface Top Surface Bottom Surface Specify Ratio Positions the middle of the stack on the surface body (as in the previous release).8646g.Simulation 4. The initial mass of the knob was 49. The optimal mass of the knob is now 33. Positions the bottom of the stack on the surface body. you had to account for clearance between surfaces with different shell thicknesses. Review the Optimal column. Positions the top of the stack on the surface body. a reduction of 32%. Positions the portion of the stack defined by an offset value that is a fraction of total thickness measured from the mid-surface to the reference surface. consider a hollow stepped shaft made of two different composite stacks. 169 . Offsets for Composites (Premium) You can now control the position of a composite laminate or stack relative to its surface.8779g.
Simulation Create two surfaces using the inner radius of the shaft and select the Bottom Surface option. In the Apply/Edit Beam PropertyManager. This eliminates the necessity to redefine the geometry every time you change the number of layers or thickness of the laminates. under Section Properties. right-click the beam definition select Define Beam Neutral Axis. distance for max shear stess. and shear factor depend on the shape and dimensions of the beam's cross section. see Simulation Help: Apply/Edit Beam. . The torsional constant. similar to Static studies. Select the shear force and its direction in Component For more information on beam properties. Beams Support for Beams in Nonlinear Studies (Premium) You can now define beams in nonlinear studies (static and dynamic) and combine them with solids and shells. To modify the direction of a beam's neutral axis. To list beam shear forces. 170 . the identification of neutral axes for short structural members (those with a length-to-width ratio < 3) was not always accurate. Improved Neutral Axis Detection Previously. Simulation supports all post-processing features and plots for beams. . right-click Results and select Define Beam Diagrams. set the appropriate options. Editing Torsional Rigidity and Shear Factor for Beams You can now input the torsional constant and shear factor of beams that are used in calculating the torsional and shear stresses. respectively. and Select an edge from the beam body parallel to the desired direction of the neutral axis. A new feature called Define Beam Neutral Axis lets you override the neutral axis of beams selected by the program.
analysis. The feature is available for static. • Select or clear Include beam forces and Include beam stresses. right-click the plot and select Save As. To include beam information in a report: 1. Beam Information in Reports You can include beam information in reports and save beam results to an eDrawings file. right-click Results Save All Plots as eDrawings. 2. In Results.eprt). In Results. 2. The program uses beam element sizes compatible with the surface mesh sizes. In the dialog box under Report format settings: • In Included sections. The software automatically bonds beams to curved surfaces that have touching geometries or are situated within reasonable clearance. frequency.Simulation Beam Stiffeners for Curved Surfaces You can now bond beams (straight or curved) that act as stiffeners to curved surfaces of shells or sheet metal bodies. To save all beam result plots to eDrawings files. Click Simulation > Report. Improved Bonded Contact for Beam Stiffeners The accuracy of the bonded contact between faces of solids or shells and beams that act as stiffeners has been improved. In Save as type. • Select Joints or Entire Length. and buckling studies. select eDrawings Files (*. To save beam results to an eDrawings file: 1. select Beams. and select 171 . double-click the plot to display it. 3.
The figure shows a spring connection between cylindrical faces of the solid and surface bodies. right-click the folder containing the series and select Dissolve Bolt Series. This easy-to-use connector estimates the appropriate size of a weld needed to attach two metal components. Create a bolt for one hole in a hole series. Model (surfaces are at the ends and solid along the entire length of the cylinder) Zoomed-in cross section Edge Weld Connectors (Professional) Simulation now supports edge weld connectors between two faces. To restore the series. 172 . You can restore the bolt series after you dissolve it. To dissolve a bolt series. Bolt Connectors Simulation selects Alloy steel from the SolidWorks Material library as bolt material by default. Click Yes to propagate bolts to all holes. The spring connector enhancement is available for static. A new folder containing the set of bolts appears in Connections . The program calculates the size of a weld at each node location along the welding edge. Editing any one bolt in the group applies to all bolts in the series. • You can dissolve the bolt series and break the link to allow editing each feature on its own. Spring Connectors for Shells You can now define a spring connector with entities (faces or edges) belonging to surfaces and sheet metal bodies. A dialog box opens to let you propagate the bolt to all the holes in the series. right-click the same folder and select Reestablish Bolt Series. and buckling studies. frequency.Simulation Connectors Connectors Applied to Hole Series The following enhancements are available: • The software automatically groups connectors based on a hole series in a separate folder.
normal force. the weld edge is shown in red (unsafe). see Simulation Help: Connector . A face of a shell. Double-Sided Fillet. shear-surface normal force.Weld Check Plot. Right-click Results and select Define Weld Check Plot.Simulation Right-click Connections • • • • Fillet. Four weld types are available: Set the properties of the weld connector: Face for Set 1 Face for Set 2 Intersecting Edges A face of a shell or sheet metal body. weld throat size. Otherwise. The software automatically selects the welding edge for touching faces of terminated and mating parts. If the estimated weld size is larger than the calculated maximum weld size. Electrode Estimated weld size Viewing Results for Edge Weld Connectors After you run a Simulation study. To specify a user-defined weld strength. Otherwise. Double-Sided Groove. select Custom Steel or Custom Aluminum. you select it manually. shear-weld axis force. you can assess the adequacy of the weld connectors in bonding the selected parts. Material for the electrode with predefined weld strength. sheet metal. 173 . and bending moment. Single-Sided Groove. An edge that belongs to the terminated part where the welding seam is applied. The weld check plot is only available for static studies. For more information about the check plot of edge weld connectors. Single-Sided and select Edge Weld. Right-click Results and select List Weld Results. the weld edge is shown in green (safe). or solid body. Checks the adequacy of the weld connectors when viewing results. You can also view weld results along the weld seam such as: weld size.
click Plot results PropertyManager).Simulation To graph weld size and weld throat values along the weld seam. You can select the housing faces in the Connectors PropertyManager. in the Bearing Loads for Circular Holes in Shells You can now define bearing forces on the following entities: • Circular shell edges • Cylindrical shell faces The bearing force acts normal to the selected edges or faces and has the following distributions: 174 . (Edge-weld Bearing Connectors Between Parts You can now define a bearing connector between split cylindrical faces of a shaft and cylindrical or spherical faces of a housing. Create split faces on the shaft representing the contact areas before defining a bearing connector. right-click Fixtures Simulation study tree and select Bearing Support. The exploded view shows the cylindrical face of a shaft connected to a spherical face of the housing. To define a bearing between the shaft and the ground.
Interference detection is only available when you define bonded contact with compatible mesh.855 6 Solver time (in sec) 433 288** Current Previous * Mesher aborts with insufficient memory. Mesh Mesh Enhancements • The curvature-based mesher supports compatible meshing between touching solid faces. The table shows a comparison of memory management for an h-adaptive analysis between the current and previous releases on a Windows XP machine with a 32-bit operating system and 3 gigabytes (GB) of physical memory. you can generate a larger mesh with smaller element sizes than in earlier versions. As a result. Note that the applied load has a vertical component. • The mesh at the common boundary between shells and beams that acts as a stiffener is now compatible. Make sure to resolve all interferences before you mesh again. 175 . the load is transferred only to the right side of the shell. meshing stops and you can access the Interference Detection PropertyManager to view the interfering parts. Release Successful number of loops run 5 4* Degrees of freedom (x 10 ) 2. • The curvature-based mesher can now mesh models with small features that previously failed to mesh. • The mesher's memory usage is improved.963 1. • The curvature-based mesher can check for interference between bodies before meshing.Simulation • Sinusoidal • Parabolic For the case shown below. If interferences are detected.
When many thin solid bodies are in an assembly. or top-level assemblies to let the program automatically find contact sets between the selected components. in a single user interface. 176 . • Use the new option Find contacts with the rest of the assembly to select a single component or body and let the program find the contact sets for touching faces of neighboring components. You can group the faces with common properties into separate subfolders in the study tree. You can: • Mesh thin solid bodies as shells. you can save analysis time by defining them as shells.Simulation ** Time is shown for 4 loops. surface. Contact The contact workflow has changed. You can assign different shell thicknesses and material properties to faces that belong to the same body. bodies. such as No penetration or Bonded. Contact Set Enhancements • You can select contact sets (manually or automatically) and fully define their types. Right-click on a solid. These changes help you intuitively set up the proper contact conditions for your model and ensure that forces are correctly transferred between components and bodies. set the option for a manual or automatic selection. Shells are suitable for thin solid bodies. Under Contact. or sheet metal body in the Simulation study tree and select Define Shell by Selected Faces. The figure shows three different shell definitions created from a single surface body. Shell Definition by Selection of Faces You can select faces of solid. Right-click Connections and select Contact Set. You can select components. • Create multiple shell definitions for a surface or sheet metal body. as they are two-dimensional elements. The original bodies are excluded from analysis. • You can use the automatic detection tool to find contact sets for touching faces or non-touching faces within a defined clearance. sheet metal. and surface bodies to define them as shells.
• You can apply No-penetration contact to both sides of a shell. Right-click Connections and select Component Contact. you need to previously define a contact type. select the entire assembly and set Contact Type to Bonded (No clearance). To apply No Contact to components or a top-level assembly. error icons conflicting contact sets. • You can drag contact definitions from static studies to nonlinear studies and vice versa. and top-level assemblies. components or bodies you select in the Component Contact PropertyManager do not penetrate each other during simulation. Use contact set definitions to apply No Penetration contact between selected bodies. • The No Contact option overrides existing component contacts.Simulation Select Automatically find contact sets to activate this option. • To apply a global contact behavior. • In the Simulation study tree. 177 . New contact sets override previously defined contact sets. By default. Make sure that these contact definitions are available to both study types. bodies. next to contact set definitions indicate Move the pointer over a conflicting contact set to see the message. Resolve any conflicting contacts before running the simulation. Contact for Nonlinear Studies (Premium) Enhancements include: • The No-penetration and Bonded mortar contact options are now available for nonlinear studies. bodies do not penetrate themselves if the deformation during simulation is sufficient to cause self-intersection. Under Contact Type. select the desired contact behavior. Component Contact The Component Contact tool defines contact types for selected components. Mortar contact definitions provide continuous and more accurate stress results in regions of contacting surfaces with incompatible meshes. Component Contact features include: • For the No Penetration contact. The No Penetration component contact option is not available for nonlinear studies. regardless of their initial contact condition.
Stress. You can compute the finite element results at the specified time step.Simulation Result Viewing Handling Large Results Files (Premium) The time to load and view result plots for the first time from a linear dynamic or nonlinear dynamic study has been reduced considerably. Plot Stress During Time Steps in Motion You can compute stress. factor of safety. mil. or the entire time range. In the Chart Options PropertyManager. • The units available for displacement plots match the units provided in the SolidWorks application. 178 . and Settings PropertyManagers. and select Use 1000 Separator (. cm.). m.). displacement. The units are am. nm. mm. in. select floating or general. • Plots with floating or general values for Number Format now support a 1000 comma separator (. under Position/Format. micron. micron. and ft. and factor of safety results at the chosen time steps or ranges are displayed on the parts during the motion simulation. Chart Options. in Number Format. and deformation results on selected parts as you perform a Motion Analysis study. • You can now control the width of beam plots for better visibility. Plot Improvements • You can use ksi units in stress plots. • You do not need to display a plot to modify the Edit Definition.
179 .Simulation In the Motion Analysis study. after finite element setup and analysis. The figure shows the stress plot on a four-bar linkage mechanism at a time step during the motion simulation. click Display Stress and select from the list of options.
In the Fit Spline PropertyManager. • The fillet preview shows virtual intersections between entities. entity selection before and after starting the tool. • You can specify multiple fillets in a single Sketch Fillet operation. extending the entities in the preview if necessary to show fillets that are possible for the selected entities. Linking Sketch Text to File Properties You can link sketch text to file properties using those properties to display sketch text values in the sketch and to create configurations in design tables. This parameter can be displayed and used to change the pattern directly. and curvature comb. Configurable Number of Instances in Sketch Entity Patterns You can now use the Number of Instances parameter for sketch entity patterns to create configurations (for example. 180 . Fit Spline Tool In the Fit Spline tool. Adjusting the tolerance dynamically updates spline previews. in design tables). including a preview mode. and an enhanced PropertyManager. you can now preview the spline and its inflection points.22 Sketching This chapter includes the following topics: • • • • • • • • Sketch Fillet Tool Fit Spline Tool Configurable Number of Instances in Sketch Entity Patterns Linking Sketch Text to File Properties Convert Entities Sketch Tool Equation-driven Curves Dimensions in 3D Sketches Large Sketch Performance Sketch Fillet Tool The Sketch Fillet Tool contains numerous enhancements. • You can set the fillet radius in the PropertyManager before or after selecting the entities. • While previewing fillets. you can use a horizontal slider to adjust the Tolerance value. Fillets are not created until you click OK in the PropertyManager. you can drag fillets to adjust the radius. maximum curvature.
Large Sketch Performance Selecting a large number of sketch entities to create blocks is now much faster. • You are no longer required to preselect the correct entity types before starting. the property reference appears under Text in the Sketch Text PropertyManager. You now can drag equation-driven curves. or to create custom and configuration-specific properties and values. Equation-driven Curves You can now create parametric (in addition to explicit) equation-driven curves in both 2D and 3D sketches.Sketching In the Sketch Text PropertyManager. You can select entities after opening the PropertyManager. you can specify Select Chain. 181 . and then select the After you link the sketch text to the property. • You can select multiple entities for conversion. you can click File Properties in the Link to Property dialog box to specify values for existing file properties such as Author. which enables you to convert contiguous sketch entities. Dimensions in 3D Sketches You can now use Smart Dimensioning to create point-to-point and Along X/Y/Z dimensions in 3D sketches and configure those dimensions. and Subject. If the file properties or their values are not yet specified. which are transformed into a loop and then converted into sketch entities. Title. • You can select a face and a number of edges on the internal boundaries of that face. click Link to Property property in the Link to Property dialog box. Copy and Paste is also faster. • There is now a Convert Entities PropertyManager. Convert Entities Sketch Tool The Convert Entities Sketch Tool has been improved to become more consistent with other sketch tools. • In the PropertyManager.
Available as a separate product. from within the SolidWorks application. Life Cycle Assessment By integrating Life Cycle Assessment (LCA) into the design process. You can compare results from similar materials to produce the optimal sustainable design. 182 . and incineration All the transportation that occurs between and within each of these steps. you can see how decisions about material. expanded reporting. LCA includes: • • • • • • • Ore extraction from the earth Material processing Part manufacturing Assembly Product usage by the end consumer End of Life (EOL) – Landfill. Other functionality includes configuration support. and location (where parts are manufactured and where they are used) influence a design's environmental impact. Two products are available: SolidWorks SustainabilityXpress Handles part documents (solid bodies only) and is included in the core software. To begin working with SustainabilityXpress. recycling. SolidWorks Sustainability Handles parts (solid bodies only) and assemblies. and expanded environmental impact options. do one of the following: • Click SustainabilityXpress (Tools toolbar or Evaluate CommandManager tab) • Click Tools > SustainabilityXpress The application opens in the Task Pane. manufacturing.23 SolidWorks Sustainability This chapter includes the following topics: • • SolidWorks Sustainability Overview Designing for Sustainability SolidWorks Sustainability Overview SolidWorks® Sustainability lets you do "sustainable design" easily. You specify various parameters that SolidWorks Sustainability uses to perform a comprehensive evaluation of all the steps in a design's life.
You can generate customizable reports to share the results. manufacturing. such as carbon monoxide and methane. resulting in algae blooms and the eventual death of plant and animal life.the drive sled that holds drives in the computer case. resulting in global warming. Energy Consumed Air Acidification Water Eutrophication SolidWorks Sustainability provides real-time feedback on these impact factors in the Environmental Impact Dashboard. Acidic emissions. All forms of nonrenewable energy consumed over the entire life cycle of the product. resulting in algae blooms and the eventual killing of all sea life in certain coastal regions. eventually leading to acid rain. The software measures the environmental impact based on these parameters: 183 . contributing to global warming. which updates dynamically with any changes.SolidWorks Sustainability Environmental Impact Factors SolidWorks Sustainability assesses all the life cycle steps based on your material. Contamination by fertilizers that travel through rivers to coastal waters. Air pollution primarily due to the burning of fossil fuels. such as carbon monoxide and methane. which eventually lead to acid rain. Designing for Sustainability This example demonstrates using SustainabilityXpress to perform an environmental impact analysis of a part. You analyze a common part used in computers . and location input. such as sulfur dioxide and nitrous oxides. SolidWorks Sustainability distills the results into environmental impact factors. Carbon Emissions Carbon dioxide and equivalents. Energy Consumption Air Acidification Water Eutrophication Contamination of water ecosystems by waste water and fertilizers. which it measures and totals. All forms of energy consumed over the entire life cycle of the product. that are released into the atmosphere. that are released into the atmosphere primarily by burning fossil fuels. Sustainability measures these areas of environmental impact: Carbon Footprint A measure of carbon dioxide and equivalents.
in Process. 184 . For Region. 2. Japan has its own region. b) In Name. 1.SolidWorks Sustainability • • • • Material used Manufacturing process and region Transportation and use region End of life Follow these steps to analyze parts: Selecting a Material You start by activating the application and selecting a material. select Injection Molded. select Plastics. Under Material: a) In Class. Open install_dir\Samples\WhatsNew\Sustainability\Drive Sled. Do one of the following: • Click SustainabilityXpress (Tools toolbar or Evaluate CommandManager tab) • Click Tools > SustainabilityXpress The application opens in the Task Pane. Setting the Manufacturing and Use Options Select the manufacturing process and the regions where the part is manufactured and used. select North America on the map. The Environmental Impact dashboard at the bottom of the Task Pane provides real-time feedback about the environmental impact of your design. 3. The software displays the part's weight.sldprt. 1. select PC High Viscosity. Under Manufacturing. 2.
SolidWorks Sustainability 3. 3. select North America. using the Environmental Impact dashboard. Under Material. Under Transportation and Use. To filter the list. select Acrylic (Medium-high impact). select the checkbox Show only selected . Comparing Similar Materials Now you set the baseline material and compare it with other materials. to try to minimize the environmental impact. 185 . The Baseline bar for each environmental impact adjusts to show the values for the selected material. Click Find Similar next to the list in the dialog box. Data is not available for all regions. 1. 2. Next you try to find a similar material that is a better environmental choice. next to the materials to list and click 5. Under the Materials column. Regions that contain data are highlighted when you hover over them. A list of similar materials appears. Set these values: Property Density Tensile Strength Condition ~ (Approximately) > (Greater than) 4. Click Set Baseline at the bottom of the Task Pane. The Environmental Impact dashboard at the bottom of the dialog box gives you intermediate feedback on your selections. PC High Viscosity. for Use Region. The dialog box displays the current material with values for multiple parameters. You select materials from this list to compare them to the original material. click Find Similar.
In the Task Pane. The pie chart colors represent the parameters used to measure the environmental impact. Click Accept. Setting the Material Now you set Plastics Nylon 101 as your material in the model and review the results in the Environmental Impact dashboard. In the Task Pane. Hover over the pieces of the pie charts. The pie charts in the Environmental Impact dashboard are updated. You can modify the Manufacturing Process using the menu next to the pie charts. 7. 1. Acrylic (Medium-high impact). 6. Now select Nylon 101 from the list to see how it compares to the original material. PC High Viscosity. 2. The size of the pieces represent the percentage contributed by the parameters to the total environmental impact. Plastics Nylon 101 is the current material. The bars and pie charts are updated. The dialog box closes. click Set Material. is a better environmental choice than the original material.SolidWorks Sustainability In the dialog box's Environmental Impact dashboard. The visual cues indicate that this material is an even better choice than Acrylic (Medium-high impact). You decide to accept this material. a green bar for Selected appears above the black bar for Original for all four impact areas. Nylon 101 becomes the active Material in the FeatureManager design tree. under Material. The pie charts are updated. under Material. The bar's green color and shorter length indicate that the selected material. 186 . The model updates in the graphics area.
including comparisons between the final material and the baseline material. The software saves the results with the model. 4. 187 . Save the report. Scroll through the document and note the detailed information about each type of environmental impact. and water.SolidWorks Sustainability 3. Save the model and click to close the Sustainability Task Pane. Click and at the bottom of the Task Pane to scroll through detailed reports of the selected material's environmental impact on carbon. energy. Click Generate Report at the bottom of the Task Pane. 2. 1. air. Links after each section bring you to the SolidWorks Sustainability web site where you find more information about this product. The report opens as a separate document. Creating a Report You can create a report that provides details about the environmental impact of your design. 3.
see SolidWorks Help: Viewing Compare Results. • The look and feel of the Results list is more consistent with the SolidWorks FeatureManager design tree. The user interface has also been remodeled to improve usability. For more information about the Compare BOM utility.24 SolidWorks Utilities Available in SolidWorks Professional and SolidWorks Premium. Usability Improvements The user interface for SolidWorks Utilities is now fully integrated into regular toolbars and menus of the SolidWorks software. • The user interface resizes better when you resize the Task Pane. click Tools > Compare > BOM. • Find/Modify/Suppress Features are combined into one Task Pane. Compare Features. click a utility from the Tools toolbar or Tools menu. To access this utility. and Compare Bill of Materials. You can also select Bill of Materials under Items to compare from any Compare Task Pane. Compare Geometry. Simplify Utility When you unsuppress a feature. This chapter includes the following topics: • • • Compare BOM Utility Simplify Utility Usability Improvements Compare BOM Utility The new Compare BOM utility compares Bill Of Material (BOM) tables from two SolidWorks assembly or drawing documents. • All Compare utilities are combined into one Task Pane: Compare Documents. and failed rows. the new Unsuppress child features option lets you unsuppress its child features. extra columns and rows. 188 . • You can more easily recompare results because you no longer need to switch between input and result panes. When you select a related command. the add-in loads dynamically if you have installed it and are running SolidWorks Professional or SolidWorks Premium. The results list missing columns and rows. • Window tiling has been improved when you display results. To access utilities.
From the SolidWorks menu. select or clear Show in PropertyManager. click Toolbox > Configure. From the Toolbox configuration tool. This chapter includes the following topics: • • • Toolbox and Enterprise PDM Integration Australian Standard Toolbox Custom Properties Toolbox and Enterprise PDM Integration Enterprise PDM can now fully manage SolidWorks Toolbox. Previously. which you can download from SolidWorks Content in the Design Library task pane. Customize your hardware. Custom Property Visibility in the PropertyManager You can now control whether a custom property appears in the component PropertyManager in SolidWorks. custom properties always appeared in the PropertyManager. click Toolbox > Configure. Additionally. you had to specify a part number for each length. From the SolidWorks menu. For details. Under Custom Properties. click Add new Custom Property or select a custom property and click Modify Custom Property . Previously. click 1. see Enterprise PDM and Toolbox Integration on page 98. 189 . Toolbox Custom Properties Toolbox provides more control over custom properties. each size of the structural members from the Australian standard is published as a weldment profile. Australian Standard Toolbox now includes the Australian standard. In the Custom Property Definition dialog box. Single Part Number per Component Size For components with editable length properties. click 2.25 Toolbox Available in SolidWorks Professional and SolidWorks Premium. you can now specify a single part number for a component size regardless of length. From the Toolbox configuration tool. Select your hardware and select AS .
From the Toolbox configuration tool. click 2. click Add new Custom Property . click Add new Custom Property . define a Textbox or List custom property. click Toolbox > Configure. Customize your hardware. The property appears as a column in the configuration table and you can type values. Under Custom Properties. 190 . select Add as configuration specific property. you could only enter values from the SolidWorks PropertyManager. click Toolbox > Configure. Custom properties appear on the Custom tab of the Summary Information dialog box. Configuration-specific Properties in the Configurations Table Configuration-specific text properties now appear in the table of configurations. clear Add as configuration specific property. In the Custom Property Definition dialog box. Custom properties are added when a new configuration is created (or a copied part is generated). In prior releases. and click OK. click 2. you had to create custom properties manually by opening the Toolbox file in SolidWorks. Under Custom Properties. Custom Property Creation You can now create custom properties that are not configuration-specific in Toolbox. click 2. In the Custom Property Definition dialog box. click Toolbox > Configure. Customize your hardware. Select a component that has an editable length property. select the new custom property. Select or clear Use single Part Number per size. Previously.Toolbox From the SolidWorks menu. Customize your hardware. and click OK. From the Toolbox configuration tool. regardless of length. From the SolidWorks menu. To see custom properties in SolidWorks. such as structural steel. From the SolidWorks menu. Under Custom Properties. open the part and click File > Properties. You can type values directly in the table or export the table to Microsoft Excel. define a Textbox custom property. From the Toolbox configuration tool. Apply this custom property to a folder or individual component.
To show the reference circle created by DimXpert. 191 .26 Tolerancing This chapter includes the following topics: • DimXpert DimXpert New Feature Recognition The following features are now recognized by DimXpert tools. click View > Curves. Patterns of Boss Features DimXpert supports dimensioning and tolerancing of patterns of boss features. Intersect Circles An intersect circle is a circle derived at the intersection of a cone and plane.
192 .Tolerancing Patterns of Cone Features Patterns of cones are supported as long as the included angle is the same. Patterns of Width Features Use the Pattern Feature tool to recognize width features.
counterbore holes. 193 . Use the polar dimension scheme to apply DimXpert patterns with axial features to define a bolt circle. slots. simple holes. the layout of dimensions has been improved The example below is the same part.Tolerancing Auto Dimension Scheme Polar Plus and Minus Dimension Schemes You can use Auto Dimension Scheme to apply polar plus and minus dimension schemes. . but each sketch is extruded along a different axis: X-axis Y-axis Z-axis Location Dimensions You can apply location dimensions between pairs of axes and lines that are skew (non-intersecting and non-parallel). Supported feature types include cylinders. In the Auto Dimension Scheme PropertyManager. and intersect lines. set the Minimum number of holes to recognize as a pattern. Dimension Layout When you use Auto Dimension Scheme to account for the sketch direction. cones. countersink holes.
Tolerancing 194 .
letting you navigate to any of the Cut-List-Item folders. Shows a preview of how the cut list will look in a drawing. Materials in Cut Lists Weldment cut lists recognize materials when determining whether bodies are identical. and the entities in the folder are highlighted in the graphics area. Cut List Table To display the Cut-List Properties dialog box. Click each property to display the property's value for every item in the cut list. under Balloons. edit. 195 . right-click the cut list folder and select Properties. • The dialog box contains three tabs to manage. • Modify a Value / Text Expression. you can select any of the cut list tables associated with the model. and view all Cut-List-Item properties: Cut List Summary Manages a cut list. and the Evaluated Value updates. Drawing Views of Weldments You can link a drawing view to a cut list table to control the information displayed in balloons. See SolidWorks Help: Drawing View Properties. In the Drawing View Properties dialog box. it appears as <Not Specified>. Properties Summary Shows the unique Cut-List-Item properties in a weldment part. you could edit only one Cut-List-Item at a time. If a Cut-List-Item does not have a unique property assigned.27 Weldments This chapter includes the following topics: • • • • Cut List Items Drawing Views of Weldments Materials in Cut Lists Property Tab Builder Cut List Items The Cut-List Properties dialog box is enhanced for ease of use and efficiency: • Select a Cut-List-Item in the dialog box. In previous versions. You can now manage all Cut-List-Items from one dialog box. even if the view references a different configuration than the cut list.
Weldments When you create a weldment part. they are placed in separate folders in the cut list. Property Tab Builder You can use Property Tab Builder to create custom properties tabs for Weldment cut list items. See SolidWorks Help: Weldment Cut Lists. the cut list includes Material as a property that links to the material applied to the body. If two bodies are geometrically identical but have different materials applied to them. When you apply a material to a body. 196 . the cut list automatically updates by placing the body in the appropriate folder.
com/whdc/system/platform/server/PAE/PAEmem. select a document and click SolidWorks Rename or SolidWorks Replace on the Mini Toolbar. Consider using this switch for large vaults. In the Rename Documents or Replace Documents dialog box. On the References/Where Used tab. This chapter includes the following topics: • • Support for Virtual Components in SolidWorks Explorer Support for the /3GB Switch Support for Virtual Components in SolidWorks Explorer The SolidWorks Explorer Rename Document and Replace Document dialog boxes can display virtual components and update their reference paths. The check-in operation is disabled for virtual components. For details about the /3GB switch. select Virtual components.28 Workgroup PDM Available in SolidWorks Professional and SolidWorks Premium.mspx 197 . select Include virtual components. In SolidWorks Explorer. under Look for. you can choose to include virtual components during rename and replace operations. Support for the /3GB Switch Workgroup PDM now supports the Microsoft Windows /3GB switch. on the File Explorer tab in the left pane. See SolidWorks Workgroup PDM Help: Rename or Replace Document and SolidWorks Workgroup PDM Help: Where Used. visit the Microsoft website: http://www.microsoft. You can also display virtual components in the Where Used tab. Because including virtual components degrades performance. Click Options (SolidWorks Explorer toolbar). You cannot manage virtual components in a Workgroup PDM vault.