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What's New: Highlights of SolidWorks 2011....................................................................ix Legal Notices..................................................................................................................11 1 User Interface...............................................................................................................13
SolidWorks Search................................................................................................................................13 PropertyManager Icons..........................................................................................................................13 Error Reporting......................................................................................................................................13
2 SolidWorks Fundamentals...........................................................................................15
Application Programming Interface........................................................................................................15 Documentation.......................................................................................................................................16 New Tutorials....................................................................................................................................16 Toolbox Administration Overview.....................................................................................................16
3 3D ContentCentral.......................................................................................................17
Defeature Tool.......................................................................................................................................17 Configuration Publisher..........................................................................................................................17 3D ContentCentral for Suppliers............................................................................................................17
4 Administration..............................................................................................................19
Converting Files to SolidWorks 2011.....................................................................................................19 Installation Improvements......................................................................................................................19 SolidWorks Rx.......................................................................................................................................21 Diagnostics.......................................................................................................................................21 Usability and Workflow Improvements.............................................................................................21 Hardware Benchmarks.....................................................................................................................22 Graphics Card Health Checker........................................................................................................22
5 Assemblies...................................................................................................................23
Assembly Features................................................................................................................................23 Fillets and Chamfers ........................................................................................................................23 Weld Beads .....................................................................................................................................23 Assembly Visualization..........................................................................................................................24 Defeature for Assemblies ......................................................................................................................25 Defeature - Step 1: Components......................................................................................................25 Defeature - Step 2: Motion...............................................................................................................26 Defeature - Step 3: To Keep.............................................................................................................26 Defeature - Step 4: To Remove.......................................................................................................27 Defeature Complete.........................................................................................................................28 Equations...............................................................................................................................................29
Interference Detection............................................................................................................................29 Ignore Hidden Bodies.......................................................................................................................29 Quality and Performance..................................................................................................................30 Mates.....................................................................................................................................................30 Replace Mate Entities.......................................................................................................................30 Mates in Motion................................................................................................................................30 Rebuild Report.......................................................................................................................................30 SpeedPak..............................................................................................................................................31
6 CircuitWorks.................................................................................................................32
User-Defined Coordinates for Component Orientation..........................................................................32 Interface Improvements.........................................................................................................................34 Workflow Improvements........................................................................................................................34 Comparing Boards.................................................................................................................................34 Export to PADS PowerPCB Format.......................................................................................................35
7 Configurations..............................................................................................................36
Configuration Publisher..........................................................................................................................36 3D ContentCentral............................................................................................................................36 Parent/Child Relationships...............................................................................................................37 Modify Configurations............................................................................................................................37 Parameters............................................................................................................................................37 SpeedPak..............................................................................................................................................38
8 Design Checker............................................................................................................39
Design Checker Standards from SolidWorks Files................................................................................39 File Location Check...............................................................................................................................39 Dimension Precision Check...................................................................................................................40 Feature Positioning Check.....................................................................................................................40 Standard Template Check.....................................................................................................................40 Design Checker Report..........................................................................................................................40 Summary Report for Task Scheduler....................................................................................................40 Design Checker Task in Enterprise PDM..............................................................................................41
9 DFMXpress..................................................................................................................42
Injection Molding....................................................................................................................................42 Running an Injection Molding Check.....................................................................................................42
10 Drawings and Detailing..............................................................................................43
Alignment Options for Dimension Palette .............................................................................................43 Auto Arrange Dimensions .....................................................................................................................49 Using Auto Arrange Dimensions......................................................................................................49 Adjusting Spacing.............................................................................................................................50 Bounding Box for Sheet Metal...............................................................................................................50 Cut List Properties in Drawings..............................................................................................................52 Center Marks in Assembly Drawings.....................................................................................................52
...........................................................................................................Contents Cosmetic Threads...........................................................................................................................................................................................................................................................................................................................................................................................................................................................55 Dual Unit Support ..............................................................................62 12 eDrawings..................................................................................................63 Display Enhancements...........53 Display Scale in Orthogonal Views........................................................................................................................................................58 Show Model Colors in Assembly Drawings..........................................70 Group Import from Active Directory............................69 Administration Tool.........................................................................65 Expanded Search Capability..................................................................................................54 Hide Bodies in Drawing View..................................68 Saving eDrawings Markup Files........................................56 Notes..................55 Hole Tables...............................................................................................................................................................................................................................................................................................................................................................................68 Updating Broken File References.............................................................................................................................................................................................................................................................................54 Dual Dimensions for Chamfers..............................................................................63 Triad Manipulation...........70 Collecting Support Information........................................................................................................................................................................................................56 Merge and Unmerge Cells in Tables........................59 Geometric Tolerance Symbols......................................................................................................................................57 Fit Text in Notes...................................................................................63 Native 64-Bit Support.................................................................................................................................................................................................................59 ANSI Drafting Standard....................................................54 Drawing Sheet Format...............................................................................................................................63 Filtering by Component Name.....................................................................................................................................................60 3D Drawing Views.....................................................................................................................................................................................................61 11 DriveWorksXpress.........................................................................................................................................................................................................................................................................................................................................................67 Expanded File Open Capabilities........................................................................................................59 Datum Feature Symbols........65 Enterprise PDM Menus ...71 iv ...............................................................................................................................................................................................................62 Task Pane Interface.........................................................................................................................................................55 Hiding a Body.............58 GB Drafting Standard.....................................................................................................................................................57 Show Dimension Units....................64 13 Enterprise PDM...................................................................57 Pattern Notes.........................................................................................................................................................................................................................................................................71 3DVIA Composer File Format Support......................................................................................................................................65 File Explorer and SolidWorks Add-in.........................55 Showing a Body...........................................................................................................................63 File Synchronization............................................................................................................69 Creating Submenus...69 Restoring Files from Cold Storage...................................................55 Tags....
..................................................................................................................................................89 Adding and Editing an Appearance................................................84 Scenes..................................................80 Walk-through...................................................................................................78 Repairing Sketches After .DXF Files...............................................................................................88 PhotoView Support on 64-bit Computers..............................74 Associating Drawing Types with File Types.............................................................................................DWG or ..................................DXF Import....76 14 Import/Export.........................................................73 Arithmetic and String Functions in Input Formulas........................................................................Contents Design Checker Validation.........................................................................................................71 Aliases in Card Lists......75 API..............................................................................88 Motion...................................................................................................................................................................................................................................................................................................................................................................................................................88 Learning About the DisplayManager..................................................................................................................73 Exported Workflow Links.........................................................88 Working with Appearances and Rendering a Model..................................................................................................................................................................................................................................................................................................................78 Importing Layers from .......................84 DisplayManager .......................76 Updating the BOM Quantity Using the API.....................................................................................................IFC Files.............................................................................81 Grid System..............................DWG or ...................................................77 Importing or Exporting ..............................................................79 Exporting Bend Line Directions....................................................................................................................................87 PhotoView Preview Window..................................................................................87 Lights.................................................82 16 Model Display...........................92 Performing a Final Render..............................89 Adding a Decal.............DWG or ................................................................................................84 Appearances.............................76 SQL-DMO Drivers.............75 Using an Add-in to Define Item Explorer Menu Commands........................................................................................91 Preparing to Render: Working with Lighting and Scenes........78 Filtering Sketch Entities on .......................................................78 Exporting Sheet Metal Parts to DXF or DWG Files.........................................................................IFC Files............................................................................................................................................................................................................................................86 PhotoView 360 ................................79 15 Large Scale Design....................................................................................................................................................................................................................................................................................................................DXF Import...........................................................................78 Defining the Sketch Origin and Orientation on ....................76 Installation.......................................................................79 Exporting a Bounding Box................................................................................................................................................93 v ..............................................................................................................75 Adding Commands to Submenus...................................................85 Decals...............................................................................................................................................................................................................................................................80 Importing or Exporting .......................................................................................................................................................DXF Import.............................................................................DWG or .........................................91 Changing Another Appearance on the Model..................................................................77 DXF DWG Import Wizard.......................................
...................................................107 Surfaces.................................................................................................................................................................................................................................................................125 Mapping Bend Directions When Exporting to DXF/DWG Files........................................................................................................................................................................................................................................................................126 vi .................................................................................................................107 Surface Extrudes From a 2D or 3D Face ...........................................................................96 Function Builder......126 Sheet Metal Properties...................................................................113 Automatic Recognition of Draft Features...........................................................................126 Mirroring Edge Flanges and Miter Flanges.........................................................113 FeatureWorks.116 20 Routing.............................................................................................................................................113 Bosses and Cuts Recognition..........................................................................................................................................................................................................................................................................................................................................................123 Flat Patterns.......................................................................................119 Weld Gaps........................123 Convert to Sheet Metal..125 K-Factor in Configurations..................................................................................................................................................107 Capping an Extruded Surface..................................................................................................................................................................................................................................................................................................................................121 Routing Options in Isolate......................................................................99 Defeature for Parts ..........105 Absorbed Curves....................................................................................................................................................................................................................99 Parts...................................................99 Equations.....................................................................................Contents 17 Mold Design..............................................................................................................................................................................................121 P&ID Report.......................................................................................................................................................................................................................................................................................................................................................................................................94 18 Motion Studies..............................................................................................120 Moving and Rotating a Fitting ..........................................123 Bend Calculation Tables...............................................................................................................................97 19 Parts and Features......................................................................104 Features..........................................97 Motion Along a Path...............................................................................................................................................................................................................................121 21 Sheet Metal........................................................................................................119 Autosize.............................................99 Global Variables............................................................................................................................................................................................................................118 Route Along Existing Geometry................................................................................................................................................................................................................................................................................................................................................................................118 Routing Library Manager...................................94 Manual Mode for Creating Parting Surfaces.......106 Scale.........96 Reflected Load Inertia and Reflected Load Mass...............105 Helix.......105 Revolve........................................................................................116 Combining Like Features During Automatic Feature Recognition...........................................................................................................................................................120 P&ID Import...........................................97 Reference Components for Linear Couplers...............................
Patterns of Edge Flanges and Tab Features.......................................................................................127
22 Simulation...............................................................................................................128
New Simulation Studies.......................................................................................................................128 New 2D Simplification Study..........................................................................................................128 New Response Spectrum Analysis Study (Premium)....................................................................137 Interface...............................................................................................................................................142 Organization of Bodies...................................................................................................................142 Filtering the Simulation Study Tree................................................................................................142 Display Enhancements for Simulation Studies...............................................................................144 Display of Simulation Symbols.......................................................................................................144 Expressions in Input Fields............................................................................................................144 Shells...................................................................................................................................................144 Offsets for Shells............................................................................................................................144 Ply Orientation in Composites (Premium)......................................................................................145 Composite Stack Information (Premium).......................................................................................146 Beams..................................................................................................................................................147 Improved Bonding for Beam Joints................................................................................................147 Non-uniform and Partial Loading of Beams...................................................................................147 Tapered Beams..............................................................................................................................148 Connectors...........................................................................................................................................149 European Standard for Edge Welds (Professional).......................................................................149 Contact.................................................................................................................................................150 Automatic Option for Simplified Bonding........................................................................................150 Mesh....................................................................................................................................................150 Mesh Enhancements......................................................................................................................150 Nonlinear Studies.................................................................................................................................151 Improved Accuracy for Nonlinear fixtures (Premium).....................................................................151 Results.................................................................................................................................................151 Nonlinear Plots (Premium).............................................................................................................151 Heat Power and Heat Energy.........................................................................................................151 Interaction with List Result Tables..................................................................................................151 Probe Callout Enhancements.........................................................................................................152 Sensors for Transient Studies........................................................................................................153 Study Reports.................................................................................................................................153
23 Sketching.................................................................................................................156
Grid System.........................................................................................................................................156
24 Sustainability............................................................................................................158
New Supported Regions......................................................................................................................158 Sustainability Link for Custom Material................................................................................................158
25 SolidWorks Utilities..................................................................................................159
Symmetry Check Utility........................................................................................................................159 Find/Modify/Suppress Feature Selection.............................................................................................160
26 Toolbox ...................................................................................................................161
Opening Models with Referenced Toolbox Components....................................................................161 Gears in the GB Standard....................................................................................................................161
27 Weldments...............................................................................................................162
Cut Lists...............................................................................................................................................162 Cut List Icons..................................................................................................................................162 Reordering and Excluding Cut List Items.......................................................................................162 Weld Beads .........................................................................................................................................162 Weld Bead Display.........................................................................................................................163 Weld Beads in Assemblies.............................................................................................................163 Weld Support in Drawings ..................................................................................................................167 Weld Symbols.................................................................................................................................167 Weld Tables....................................................................................................................................167
28 Workgroup PDM......................................................................................................169
Deleting Unused Documents That Are Not Revision Managed...........................................................169
What's New: Highlights of SolidWorks 2011
SolidWorks® 2011 includes many enhancements and improvements, most in direct response to customer requests. This release focuses on the following themes: • Visualization and collaboration • Design efficiency • Reliability and stability
Top Enhancements
The top enhancements for SolidWorks 2011 provide improvements to existing products and innovative new functionality. Throughout this guide, look for the Assemblies Fillets and Chamfers on page 23 Weld Bead Display on page 163 Defeature for Assemblies on page 25 Drawings and Detailing Alignment Options for Dimension Palette on page 43 Auto Arrange Dimensions on page 49 Dual Unit Support on page 56 Weld Support in Drawings on page 167 Enterprise PDM Model Display Enterprise PDM Menus on page 65 DisplayManager on page 84 PhotoView 360 on page 87 Parts and Features Defeature for Parts on page 99 Sharing Equations Among Models on page 99 Suppression States of Features and Components on page 101 symbol in these areas:
What's New Examples What's New Examples are updated at every major release to provide examples of how to use most top enhancements in the release. To enable Interactive What's New. To open What 's New Examples click Help > What's New > What's New Examples. samples. including details about the user interface. click the symbol to display the section of this manual that describes an enhancement. click Help > What's New > Interactive. Click: • Help > What's New > PDF • Help > What's New > HTML In SolidWorks. Online Help Release Notes Contains complete coverage of our products.Surface Extrudes From a 2D or 3D Face on page 107 Simulation Weldments New 2D Simplification Study on page 128 Weld Beads on page 162 Weld Bead Display on page 163 Fillets and Chamfers on page 164 For More Information Use the following resources to learn about SolidWorks: What's New in PDF and HTML This guide is available in PDF and HTML formats. The symbol appears next to new menu items and the titles of new and changed PropertyManagers. Interactive What's New x . Provides information about late changes to our products. and examples.
906.898.877. 7.044. Educational. company. as applicable. All warranties given by DS SolidWorks as to the software and documentation are set forth in the SolidWorks Corporation License and Subscription Service Agreement.219. Premium. Dassault Systèmes SolidWorks Corporation. TolAnalyst. 7.694.A. Mass. 6. 7. 6.705. this document or its contents shall be considered or deemed a modification or amendment of such warranties. and in the license agreement.712. PDMWorks. 7. Massachusetts 01742 USA 11 .g.190 and JP 3.049.560. 3D PartStream.672. and SolidWorks 2010 are product names of DS SolidWorks. 6. SolidWorks Enterprise PDM.S.477. PhotoWorks.611. SolidWorks Flow Simulation.558.Legal Notices © 1995-2010.844. and foreign patents.S.055. FeatureWorks is a registered trademark of Geometric Ltd. 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). COMMERCIAL COMPUTER SOFTWARE .643.. a Dassault Systèmes S.517. and foreign patents pending. duplication. and XchangeWorks are trademarks of DS SolidWorks. Use. Patents 5. 7.154. Concord. (e. and the eDrawings logo are registered trademarks and FeatureManager is a jointly owned registered trademark of DS SolidWorks.227-19 (Commercial Computer Software Restricted Rights). Government Restricted Rights.262.027. 7.990. 7.NET. 7. for any purpose without the express written permission of DS SolidWorks. or disclosure by the government is subject to restrictions as set forth in FAR 52. EP 1.688. DFARS 227.497. 7.027. Concord. 6.079. and nothing stated in. and Professional Products U. Patent Notices for SolidWorks Standard. 3D ContentCentral. All Rights Reserved.822.7202 (Commercial Computer Software and Commercial Computer Software Documentation). 01742 USA. eDrawings. Other brand or product names are trademarks or registered trademarks of their respective holders.318. 6.079. U.238.116. 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.571. FloXpress. SolidWorks Simulation.219.S. Trademarks and Other Notices for All SolidWorks Products SolidWorks. Contractor/Manufacturer: Dassault Systèmes SolidWorks Corporation. CircuitWorks.590.502.184. 300 Baker Avenue.PROPRIETARY U. 7.643).725. electronic or mechanical. No material may be reproduced or transmitted in any form or by any means. 7. 300 Baker Avenue.815. or implied by. 6. Feature Palette.
382.364. Patents 5. All rights reserved.Copyright Notices for SolidWorks Standard. Portions of this software © 1996-2010 Microsoft Corporation.943.593. Protected by U. Portions of this software are copyrighted by and are the property of UGS Corp. All rights reserved. Premium. 6. and its licensors.502. All rights reserved. 6. Copyright © 1994-2005 DC Micro Development. Portions of this software © 2007 . Portions of this software © 1998-2010 Geometric Ltd. All Rights Reserved. © 2010. the Adobe logo.754. and other countries. KG.2010 Luxology. Educational. 12 . Copyright Notices for SolidWorks Simulation Portions of this software © 2008 Solversoft Corporation. 5.289. Portions of this software © 2001 . All rights reserved. Inc. All Rights Reserved.929. Portions of this software © 2000-2010 Tech Soft 3D. This software is based in part on the work of the Independent JPEG Group. Patents Pending. Copyright 1984-2010 Adobe Systems Inc. Inc. Portions of this product are distributed under license from DC Micro Development. in SolidWorks see Help > About SolidWorks. Portions of this software © 1998-2010 3Dconnexion.639. 6. Other portions of SolidWorks 2010 are licensed from DS SolidWorks licensors. For more copyright information.S.563.063. in the U. Acrobat.2010 DriveWorks Ltd. Adobe. 6. PCGLSS © 1992-2007 Computational Applications and System Integration. and Professional Products Portions of this software © 1990-2010 Siemens Product Lifecycle Management Software III (GB) Ltd. Portions of this software incorporate PhysX™ by NVIDIA 2006-2010. Distiller and Reader are registered trademarks or trademarks of Adobe Systems Inc. Patents Pending. Portions of this software © 1986-2010 mental images GmbH & Co.S.866. Inc. the Adobe PDF logo.
or the community forums. The dialog box lets you do the following: • Send a failure report to SolidWorks. in the SolidWorks Search box type the text to search for. select the location to search and See SolidWorks Help: Search. you can search SolidWorks Help. PropertyManager Icons Icons for labels and buttons in PropertyManagers and dialog boxes are updated for greater consistency with toolbar and FeatureManager design tree icons. 13 . • Include a short description of your actions when the application stopped responding. Error Reporting The SolidWorks Error Report dialog box now allows SolidWorks to gather more information about why the software stopped responding.1 User Interface This chapter includes the following topics: • • • SolidWorks Search PropertyManager Icons Error Reporting SolidWorks Search New search modes have been added to SolidWorks Search. In addition to searching for files and models. the Knowledge Base. • Preview the contents of the report to send to SolidWorks. This information helps SolidWorks Engineering identify stability trends. . • Indicate whether this is a new problem or is similar to a previous problem. On the Menu Bar.
User Interface • View the SolidWorks data privacy policy. To send reports to SolidWorks for every failure. subject to this policy. 14 . select Enable performance feedback in Tools > Options > General. The reports are confidential.
and surface parameter properties Manage line styles in drawings Get the contents of folders in the FeatureManager design tree Create flyout groups in the CommandManager Convert draft quality drawing views to high quality Access a ray-trace rendering engine. templates. properties. and delegates. spline. or part document • After an entity is selected in a part. 15 . or drawing document • Use Design Checker to: • Build checks from existing SolidWorks documents. assembly. such as PhotoView 360.2 SolidWorks Fundamentals This chapter includes the following topics: • • Application Programming Interface Documentation Application Programming Interface Major enhancements are new interfaces. You can now: • • • • • • • • • • • • • • • • • • • Display .NET macro and to the SolidWorks journal file Send notification: • Before a command or PropertyManager page executes or opens • When a BOM or general table is inserted in an assembly. and its options Determine whether the current sketch is a boundary box Get the direction of a bend line Get the boundary-box sketch display data of a flat-pattern drawing view Add and delete material from specific display states in the active configuration of a model Access Presentation Studio to create 3D PDF files of parts and assemblies Add a standard SolidWorks or custom button to the Task Pane Get the name of the active PropertyManager page Get custom and stock render references for a model Get whether a command or PropertyManager page is active Add a line to a C# or VB.NET controls in the SolidWorks user interface Access Pack and Go Get data objects containing curve. methods. drawing. and drawing standards • Check against an existing file • Get summary results and save its report in Microsoft Word format Click Help > API Help > SolidWorks API Help > SolidWorks APIs > Release Notes.
Click Help > SolidWorks Tutorials. and SustainabilityXpress. Event-based Motion Studies. See SolidWorks Help: Toolbox Administration Overview. Click one of the following: • All SolidWorks Tutorials (Set 1) • All SolidWorks Tutorials (Set 2) 3. Toolbox Administration Overview SolidWorks Help contains new Toolbox administration information. 2. To access these tutorials: 1.SolidWorks Fundamentals Documentation New Tutorials SolidWorks 2011 includes the following tutorials: Assembly Visualization. 16 . Select a new tutorial from the list. Mouse Gestures.
A sample of possible configurations is tested. See Model Tests on page 37. You can then share the new file without revealing all the design details of the model. and users can search 3D ContentCentral for the model by part number. Part Numbers Suppliers can use the Configuration Publisher to generate part numbers for a configurable model. For more information. solids without feature definition or history). and multiple parents are allowed.3 3D ContentCentral This chapter includes the following topics: • • • Defeature Tool Configuration Publisher 3D ContentCentral for Suppliers Defeature Tool Use the SolidWorks Defeature tool to remove details from a part or assembly and save the results to a new file in which the details are replaced by dumb solids (that is. Model Tests You can test the health of models before uploading them to 3D ContentCentral. see Defeature for Parts on page 99. You can define parents explicitly. See Part Numbers on page 36. 3D ContentCentral for Suppliers Supplier Services introduces new self-service publishing capabilities for industrial component suppliers. See Parent/Child Relationships on page 37. the parents of controls which you have specified as parents). 17 . Configuration Publisher Multiple Parent/Child Control The Configuration Publisher offers more flexibility when defining data parents for controls. You no longer automatically inherit grandparents (that is. Results are reported in a log file that lists the configurations that were tested and whether they rebuilt successfully.
Defeature Tool Suppliers can enable the rules they have defined in SolidWorks to remove details from configurable models prior to download. See Defeature for Parts on page 99. 18 . See Model Tests on page 37.3D ContentCentral Model Health Suppliers can test configurable models for Model Health in SolidWorks before uploading them to 3D ContentCentral.
• The display of borrowed licenses is improved. License Activation SolidWorks License Activation is enhanced. use Convert Workgroup PDM Files. You can use the SolidWorks Task Scheduler (SolidWorks Professional) to convert multiple files from an earlier version to the SolidWorks 2011 format. SolidNetWork License Manager SolidNetWork License Manager is enhanced. After you convert files to SolidWorks 2011. • You can transfer a license from a computer even if SolidWorks is no longer installed on that computer. • You can activate and transfer licenses for multiple serial numbers in a single step. Click Windows Start > All Programs > SolidWorks 2011 > SolidWorks Tools > SolidWorks Task Scheduler. Installation Improvements SolidWorks Installation Manager and the installation process have significant improvements. In the Task Scheduler: • Click Convert Files and specify the files or folders to convert. You can download and run SolidWorks Activation Wizard from the SolidWorks customer portal to transfer the license. 19 . subsequent opening time returns to normal.4 Administration This chapter includes the following topics: • • • Converting Files to SolidWorks 2011 Installation Improvements SolidWorks Rx Converting Files to SolidWorks 2011 Opening a SolidWorks document from an earlier release can take extra time. For files in a SolidWorks Enterprise PDM vault. use the utility provided with Enterprise PDM. you cannot open them in older versions of SolidWorks. • For files in a SolidWorks Workgroup PDM vault. After you open and save a file.
you can: • Create a 32-bit image on a 64-bit operating system • Create a 64-bit image on a 32-bit operating system • Create 32-bit and 64-bit images on the same operating system Administrative Image Option Editor The interface and workflow for SolidWorks Administrative Image Option Editor are enhanced. • Borrowing a SolidWorks package license now automatically borrows the pre-requisite SolidWorks Standard license.Administration • The list of product licenses available to borrow now shows only what has been purchased and is available on the SolidNetWork License Manager. Installation Manager SolidWorks Installation Manager is enhanced. • The Workgroup PDM and SolidNetWork License Manager installations are more integrated into the SolidWorks Installation Manager workflow. You are notified when downloading is complete and the files are ready for installation. avoiding the overload of a particular server because all the updates take place simultaneously). delay the installation. rather than removing the previous version and then installing the new one. • You can create 32-bit and 64-bit administrative images on both 32-bit and 64-bit operating systems. • You can specify which languages to include in an administrative image. This allows you to manage automatic updates (for example. you can specify whether automatic updating is enabled for one or more machines or groups. • You can manage both 32-bit and 64-bit administrative images using the same Option Editor on either a 32-bit or a 64-bit operating system. Background Downloader You can use SolidWorks Background Downloader to download installation files in the background. or delete the download. • In SolidWorks Administrative Image Option Editor. English is always installed. rather than including all languages in all images. You can choose to install now. You also can specify when the update occurs for specific machines or group of machines. even if you do not specify it during installation. • You can perform all administrative image configuration steps using SolidWorks Administrative Image Option Editor (some of which were handled previously in SolidWorks Installation Manager). 20 . • The Option Editor opens automatically after SolidWorks Installation Manager creates the administrative image. • You can update SolidNetWork License Manager to a new version using SolidWorks Installation Manager. For example.
This button replaces the Re-create the problem dialog box.Administration SolidWorks Rx Diagnostics The improved page design and content on the Diagnostics tab helps you locate and download the correct graphics driver at http://www. A new SolidWorks session starts. the status shows the error icon .solidworks. In the Problem Capture Details dialog box. 1. 2. 4.com/sw/support/videocardtesting. Status shown in the Diagnostics tab for different system and graphics card combinations on your machine: Machine System Certified Status Fields Displayed All system and graphics card related fields Graphics Certified only for Card previous version of SolidWorks Graphics card related information System Not certified Graphics Certified only for Card previous version of SolidWorks All system and graphics card related fields System Graphics Card Certified Out-of-date System Graphics Card Certified Current All system and graphics card related fields If you have no internet connection. Click Record Video. describe the problem and click OK This dialog box has been shortened to improve usability. In the Capturing Problem dialog box. and package the SolidWorks files. On the Problem Capture tab. click Describe Problem. 3. 21 . Usability and Workflow Improvements The Problem Capture tab helps you describe the problem.html. record the video. click Start Recording.
Graphics Card Health Checker Enhancements to the Graphics Card Drivers page help you identify the correct graphics driver. or assembly files. • An updated results chart with color-coded keys that improves readability. 22 .html .0 or later installed on your machine to view this button on the web page. To run the SolidWorks performance benchmark. Record the problem and click Finish Recording. 7. You can determine whether your system is qualified to run SolidWorks effectively. click OK. 6. See http://www. A zipped folder is created. Click Add Files to add parts. save it on your hard disk. 5.solidworks.Administration The floating dialog box stays on top of your SolidWorks session. and populates the information on the web page for you to identify the correct graphics card. Improvements: • A one-click application that profiles your system and graphics card. You need . Hardware Benchmarks The Addins tab now has a link to www. on the Addins tab. drawings.solidworks. and send it to the Technical Support team.com/benchmarks for you to find details about running SolidWorks and computer-related benchmarks.com/sw/support/videocardtesting. click Start the SolidWorks Performance Benchmark. When prompted to shut down the SolidWorks session. You can rename the folder. then click Package files Now.NET 2.
which are useful for weld preparation. As with other assembly features. you can create fillets and chamfers. simple representation of weld beads. Fillets and Chamfers In assemblies. you can propagate these features to the parts they affect. 23 . and weld beads to assemblies. chamfers. see Fillets and Chamfers on page 164. Simplified weld beads provide a lightweight. For a step-by-step example of adding chamfers in an assembly. Weld Beads You can add simplified weld beads to assemblies.5 Assemblies This chapter includes the following topics: • • • • • • • • Assembly Features Assembly Visualization Defeature for Assemblies Equations Interference Detection Mates Rebuild Report SpeedPak Assembly Features Enhancements include the ability to add fillets.
parts only. The File Name and Quantity columns cannot be deleted. see Weld Beads on page 162. Sorting and Column Options You can build more complex sorting scenarios by doing the following: • Adding multiple columns • Adding multiple parameters to the sorting hierarchy • Rearranging column position to change the order in which the parameters are sorted Right-click a column header and select the following: • Add Column. Parts only. Then in the Save As dialog box. you added weld beads as components of the assembly. • Save the Assembly Visualization view as a display state. Deletes the column you right-clicked. The minimum number of columns is three. select Top-level only. Adds a column to the Assembly Visualization list. Enables you to sort by the values in that column. For more information about simplified weld beads. You can then change which property is listed in the new column. Right-click any column header and click Save as. Drag a column header to move a column left or right to move it up or down in the sorting hierarchy. This method is no longer supported. Click the arrow to the right of the column headers and click Add Display State. You can adjust the width of a column to fit the column contents by double-clicking the column separator. 24 . you can: • Export the Assembly Visualization list in top-level only. A sorting widget appears under the column title. Save and Display Options With enhanced save and display capabilities. • Delete Current.Assemblies In previous versions of SolidWorks. the hierarchy of the sort is from left to right. To remove a column from the sort hierarchy. or indented format when saving the list to a separate file. you can still edit existing weld bead components. • Add to Sort Hierarchy. see Weld Beads on page 163. When multiple columns have sorting widgets. right-click it and click Remove from Sort Hierarchy. or Indented. Assembly Visualization Enhancements support complex sorting scenarios and provide additional display and save options. However. For a step-by-step example of adding a weld bead to an assembly.
1. from an oil pump assembly. The PropertyManager has multiple pages. and then click Component Driven or Assembly Driven.sldasm. In this example. 2.Assemblies • Apply the same color to components that have identical values (for example. Defeature for Assemblies With the Defeature tool. Right-click a color slider and click Group Identical. Click Tools > Defeature. Defeature . Click the arrow to the right of the column headers. 25 . you use the Defeature tool to remove all internal components and features. which provides tools for manual and automatic selection of details to keep and remove.Step 1: Components You can specify components to remove from the model. The Defeature PropertyManager opens to Step1: Components. solids without feature definition or history). and some external features. You retain the mounting holes. You can then share the new file without revealing all the design details of the model. • Set the length of the value bars to be calculated as a percentage of the value for the highest-value component or as a percentage of the value for the entire assembly. The software adds sliders as needed to apply a distinct color for each discrete value. Before After Click Tools > Defeature to access the Defeature PropertyManager. you can remove details from a part or assembly and save the results to a new file in which the details are replaced by dumb solids (that is. click Value Bars. Open install_dir\samples\whatsnew\assemblies\oil_pump. when components are sorted by a discrete property such as Vendor or Status).
Step 2: Motion If you want to allow motion in an assembly. For Features to Keep : a) In the graphics area. Under Remove. Click Plane1 6. Defeature . Click Next . you can remove details from groups of components and allow motion between the groups. to view different sections of the assembly. to clear the section view. under Section View. 5. For this example. 4. 3. Defeature . 26 . examine a section view of the assembly. such as mounting holes. Click Next . select the three mounting holes on the cover.Assemblies First. In the PropertyManager. that might otherwise be removed by the Defeature tool. Change Offset Distance . click Plane1 You can see internal details and components. Internal components are removed. select Internal components. skip this step. 1.Step 3: To Keep You can specify features that you want to retain.
2. the cut feature is highlighted.Step 4: To Remove You can specify to remove features that were not automatically removed. In the graphics area. When you rotate the assembly.Assemblies b) Rotate the assembly and select the three mounting holes on the housing. expand Cover and select Rib Cut. Features on the housing are removed to close up the assembly. In the PropertyManager. Rib Cut and its dependent features appear in Items to Remove . Assembly Preview Defeature . In the flyout FeatureManager design tree. The mounting holes you selected are retained. 1. 27 . the preview also rotates. Click Next . The screen splits and a preview of the model appears.
3. Under Results. The part has only one feature. 1. The preview shows that the cut feature is removed. . type oil pump . c) Click Save. Defeature Complete You can save the less-detailed model in a separate part file or publish it to 3D ContentCentral.Assemblies 2. The settings you select in the PropertyManager are saved in the original model. Click . and 28 . Imported1 has no references to the original assembly. Click Next . 2.details removed. b) For Save as type. The assembly is saved as a part. In the Save As dialog box: a) For File name. select Part(*.sldprt). select Save the defeatured model as a separate file.
4. 29 . Ignore Hidden Bodies You can ignore interferences with hidden bodies. change the settings. click Section View > Section View. Defeature tree. with different details removed. (Heads-Up toolbar) or View > Display Equations Equation functionality is enhanced. and save another version of the assembly. In the part window.Assemblies In the assembly. appears near the top of the FeatureManager design You can right-click Defeature . Interference Detection Interference Detection has been enhanced. • You can share equations and global variables among models. • You can use equations to control the suppression state of assembly components. click Edit Feature . • You can configure global variables. See Equations on page 99. The part has no internal details.
For linear/linear coupler mates. Quality and Performance The quality and performance of Interference Detection have been improved. instead of solving individually each time you select a replacement entity. certain mates are now solved relative to other components rather than relative to the assembly origin. • While replacing multiple mate entities. you can choose to not show interferences between the hidden body and other components. a component.Assemblies For example. the software might find interferences that were previously missed. Because of the changes. The reference component information is used in SolidWorks Motion simulations. Select Defer update so that all mates are solved together when you exit the PropertyManager. you specify the appropriate reference components in the Mate PropertyManager. you can postpone the solving of the mates. select Ignore hidden bodies. Mates Replace Mate Entities Replace Mate Entities is enhanced. In an assembly. Click AssemblyXpert (Assembly toolbar) or Tools > AssemblyXpert. Rebuild Report AssemblyXpert now provides a report of the rebuild time for the total assembly. resulting in changes in the number of interferences reported. you create a body for construction purposes and then hide it. Mates in Motion To support more accurate motion simulations. rack and pinion mates. 1. • The Missing Entities popup toolbar is now available while you replace any mate entities. under Options. You must rebuild the assembly during the current session of SolidWorks before generating the report. The reference components for gear mates. and screw mates are detected automatically. not just while you replace a component that includes mate entities. 30 . Click Interference Detection (Assembly toolbar) or Tools > Interference Detection. suppose that in a multibody part. or a Mates folder and click Replace Mate Entities (Assembly toolbar). In the PropertyManager. Select a mate.
in the information-only row about the rebuild report. select Use SpeedPak. in the FeatureManager design tree. The subassemblies switch from the SpeedPak configuration to the SpeedPak's parent configuration. 31 . click Show these Parts . If a subassembly's active configuration has a SpeedPak configuration. right-click one or more subassemblies and click Use SpeedPak. Switching All Subassemblies to SpeedPak Do one of the following: • When opening an assembly. then the SpeedPak configuration is used. If the selected subassembly's active configuration has a SpeedPak configuration. Switching Selected Subassemblies to SpeedPak In the FeatureManager design tree. In the AssemblyXpert dialog box. SpeedPak New commands make it easier to switch between SpeedPak and parent configurations of subassemblies. then the SpeedPak configuration is used. Switching from SpeedPak to Parent Configurations In the FeatureManager design tree. right-click the top-level assembly and click Use SpeedPak. In the Open dialog box. right-click the top-level assembly or one or more selected subassemblies and click Set SpeedPak to Parent.Assemblies 2. click Open (Standard toolbar) or File > Open. • In an assembly that is already open.
CircuitWorks assigns the user-defined coordinate system as the ECAD origin when you export the assembly into CircuitWorks. select SolidWorks Export. click CircuitWorks > CircuitWorks Options. and modify the Import and export components relative to this coordinate system option.6 CircuitWorks This chapter includes the following topics: • • • • • User-Defined Coordinates for Component Orientation Interface Improvements Workflow Improvements Comparing Boards Export to PADS PowerPCB Format User-Defined Coordinates for Component Orientation You can add a SolidWorks user-defined coordinate system to a component that is not modeled with the SolidWorks origin. CircuitWorks interprets the positive Z-direction of a user-defined coordinate system as perpendicular to a circuit board assembly.directions control the angle at which the component is inserted into the assembly. You might obtain such components from a manufacturer website or from other CAD systems.and Y. To assign a name other than CWX to the user-defined coordinate system representing the ECAD origin. The XY plane represents the board surface. 32 . and the X. If you insert components without a user-defined coordinate system into a CircuitWorks assembly. When you name the user-defined coordinate system CWX before inserting the component in the CircuitWorks Library. CircuitWorks assigns SolidWorks origin as the ECAD origin. CircuitWorks assigns the user-defined coordinate system as the ECAD origin and correctly positions the components when you insert them into a circuit board assembly.
CircuitWorks Example: LED Orientation With and Without Coordinates Defined The coordinates of an externally manufactured LED set the Z-direction parallel to the base of the LED. the LEDs are oriented horizontally. 33 . Before adding the component to the CircuitWorks Library. You add the LED to the CircuitWorks Library without defining a coordinate system named CWX. add a coordinate system named CWX to the LED component in SolidWorks. When you insert the LED components into the board assembly after building it in CircuitWorks.
The Add Multiple Components wizard assists you in adding SolidWorks models to the CircuitWorks library. 34 . • The option Check component library data for errors highlights any missing SolidWorks components in the component tree (rather than simply removing them as in previous releases). only the components on the board were compared. • CircuitWorks offers to overwrite zero-height components in the library if it later encounters the same component with a defined height. • Components managed through SolidWorks Workgroup PDM or SolidWorks Enterprise PDM are marked with this icon . • You can now save library data to a database for backup or data migration. • The Add Parts from Folder function has been renamed Add Multiple Components and moved to the Files menu. Interface Improvements The CircuitWorks library is enhanced. Comparing Boards You can use the Compare command to identify differences between boards (their shape. Improvements to menus. • When you set the Add components to the library when exporting from SolidWorks option. for example).CircuitWorks The LEDs are properly oriented when you insert them into the board assembly. You can then remove or repair them. Workflow Improvements New options improve the CircuitWorks workflow. and the library display include: • Commands to import and export library data are grouped more logically on the Tools menu. CircuitWorks adds records to the library for any new component it encounters when exporting a SolidWorks assembly to CircuitWorks. You can set the Overwrite any existing 2D models in the Library with 3D model option to apply this action automatically. In previous releases. options.
CircuitWorks When differences are identified. Open two boards in CircuitWorks and click Tools > Compare . you can choose whether to replace the board or selected components in the SolidWorks assembly. Click > Save As and select PowerPCB 2007 File (*asc). Export to PADS PowerPCB Format You can export Circuitworks data to the PADS PowerPCB 2007 (*. 35 .asc) format.
In the Configuration Publisher. Your customers can search for the model by part number. On the 3DCC Preview tab. create a column with the header $PARTNUMBER. enter a part number for each configuration by typing or using Microsoft Excel functions. In the design table of the model. To include a part number with the model: 1. use Microsoft Excel functions such as CONCATENATE to make the value of the cell reflect the model's part number based on values in other columns. Part Numbers A part number can be displayed with your model on 3D ContentCentral. the part number updates to reflect the current selections. a part number is generated for each possible configuration. On 3D ContentCentral: 36 . Click Upload to 3D ContentCentral and click Yes to save the model. • For multiple-row design tables. the list contains the part numbers you entered for each configuration in the design table. As you change selections. Under $PARTNUMBER: • For single-row design tables. 2. Supplier part number displays the part number of the selected configuration. 4. based on the rules and values you defined in the Configuration Publisher. add controls. 3. The software generates a list of part numbers and stores it within the model in a format that is accessible to the 3D ContentCentral software.7 Configurations This chapter includes the following topics: • • • • Configuration Publisher Modify Configurations Parameters SpeedPak Configuration Publisher 3D ContentCentral The Configuration Publisher has new capabilities for 3D ContentCentral suppliers. and values. rules. • For multiple-configuration models. • For single-configuration models.
• You can search for the model by part number or partial part number. To test a model before uploading it: 1. click Test. You can view the log file for more details.) • Cosmetic threads (See Cosmetic Threads on page 53. Then you can add multiple data parents to the third or later controls. specify the sample size and where to store the log file. In the Configuration Tester dialog box. on the 3DCC Preview tab. 2. the parents of controls which you have specified as parents). Parameters You can configure parameters in the following areas. and multiple parents are allowed. or Configure Material. one Parent field is initially visible. Results are reported in a log file that lists the configurations that were tested and whether they rebuilt successfully. • Scale features (See Scale on page 107. and click Begin Test.) 37 . A sample of possible configurations is tested. You can define parents explicitly. • The All Parameters option has been moved from the table view drop-down list to a separate button . Right-click an item and select Configure dimension.) • Global variables (See Global Variables on page 104. even if it is used in several features. In the Configuration Publisher.Configurations • On the Configure & Download page. Each linked dimension appears in the list only once. Configure component. In the Configuration Publisher. Parent/Child Relationships The Configuration Publisher offers more flexibility when defining data parents for controls. under Data. Configure feature. Model Tests You can test the health of models before uploading them to 3D ContentCentral. You must have at least two controls already defined. the part number appears at the bottom of the Configure area and updates as you change selections. The dialog box reports the percentage of the samples that succeeded. You no longer automatically inherit grandparents (that is. • Linked dimensions are grouped in a column labeled Linked Dimension instead of appearing in columns for individual features. Modify Configurations The Modify Configurations dialog box has been enhanced. To add others. click Add Parent .
38 .Configurations SpeedPak New commands make it easier to switch between SpeedPak and parent configurations of subassemblies. see SpeedPak on page 31. For more information.
8 Design Checker
SolidWorks Design Checker is available in SolidWorks Professional and SolidWorks Premium. This chapter includes the following topics: • • • • • • • • Design Checker Standards from SolidWorks Files File Location Check Dimension Precision Check Feature Positioning Check Standard Template Check Design Checker Report Summary Report for Task Scheduler Design Checker Task in Enterprise PDM
Design Checker Standards from SolidWorks Files
Design Checker now supports the creation of standard files (*.swstd) from the following file formats, in addition to the *.dwg file format: • • • • • Part (*.sldprt, *.prt) Assembly (*.asm, *.sldasm) Drawing (*.drw, *.slddrw) Template (*.prtdot, *.asmdot, *.drwdot) Drafting Standard (*.sldstd)
Click Tools > Design Checker > Check Against Existing File to specify a file for the creation of the standard file. The program creates the standard file based on your selection, validates the active document, and displays results in the Task Pane.
File Location Check
You can use the File Location check to verify that your document templates are located in the correct file path. The current document is checked against the settings in Tools > Options > System Options > File Locations. Click File Location under Document Checks to add to the Build Checks.
The check also contains three new options for auto-correction: • Add missing paths. During autocorrection, Design Checker adds the file paths in the preferred values list to the list of actual values at the system level. • Remove extra paths. During autocorrection, Design Checker removes the file paths that are not present in the preferred values list from the list of actual values at the system level.
Design Checker
• Check for order. Design Checker checks for the file path order in the actual and preferred lists.
Dimension Precision Check
The Dimension Precision check now includes the expected precision for dimensions, angles, and tolerances. You set the level of precision by selecting the number of digits after the decimal point or by setting the value. The current document is checked against the settings in Tools > Options > Document Properties > Dimensions. The check also contains two new options for auto-correction: • Modify all length dimension & tolerance precisions in document • Modify all angle dimension & tolerance precisions in document Click Dimension Precision under Dimension Checks to add to the Build Checks.
Feature Positioning Check
The Feature Positioning check verifies that the active document has no 2D or 3D sketches positioned with references to fillet or chamfer edges. Click Feature Positioning under Feature Checks to add to the Build Checks.
Standard Template Check
The Sheet Format check is renamed to Standard Template check. This check verifies the sheet size properties of the drawing and the type of projection used for the views' layout. Click Standard Template Build Checks. under Drawing Document Checks to add to the
Design Checker Report
The Design Checker report is now formatted for better readability. You can also save the report as a Microsoft Word document. The report includes information for autocorrected entities when a Design Checker task is executed from the SolidWorks Task Scheduler or SolidWorks Enterprise PDM. The new format summarizes the failure instances according to criticality level and lists the autocorrected parameters with their initial and corrected values.
Summary Report for Task Scheduler
Design Checker creates a summary report when run on multiple files through SolidWorks Task Scheduler. You can access the summary report under the Status of the Design Checker task. To view the detailed Design Checker report for a file, in the Task Scheduler summary report, select the report file path.
Design Checker
Design Checker Task in Enterprise PDM
You can use the new Design Checker task inside the Administration Tool of Enterprise PDM to validate selected SolidWorks documents in the vault using standards files (.swstd) created in Design Checker. See Design Checker Validation on page 71.
click Tools > DFMXpress. Running an Injection Molding Check 1. Under Manufacturing Process. 2. select Injection Molding. set Minimum wall thickness and Maximum wall thickness. Click Settings. 3. You set the Minimum wall thickness and Maximum wall thickness parameters that DFMXpress uses to validate manufacturability. With a part open. Click Run. 4. Under Rule Parameters. The Manufacturing Process: Injection Molding report displays a list of rules passed and rules failed.9 DFMXpress This chapter includes the following topics: • • Injection Molding Running an Injection Molding Check Injection Molding DFMXpress supports injection molded parts. 42 . 5.
select dimensions and move the pointer over the Dimension Palette rollover button . 43 .10 Drawings and Detailing This chapter includes the following topics: • • • • • • • • • • • • • • • • • • Alignment Options for Dimension Palette Auto Arrange Dimensions Bounding Box for Sheet Metal Cut List Properties in Drawings Center Marks in Assembly Drawings Cosmetic Threads Display Scale in Orthogonal Views Drawing Sheet Format Dual Dimensions for Chamfers Hide Bodies in Drawing View Hole Tables Merge and Unmerge Cells in Tables Notes Show Dimension Units Show Model Colors in Assembly Drawings GB Drafting Standard ANSI Drafting Standard 3D Drawing Views Alignment Options for Dimension Palette Alignment tools are available on the dimension palette when you select more than one dimension. To display the dimension palette.
Auto Arrange Dimensions Automatically arranges selected dimensions. 44 .Drawings and Detailing The following alignment tools are on the dimension palette. See Auto Arrange Dimensions on page 49. These tools are also available on the Align toolbar.
between the closest and furthest selected dimensions from the part. linearly or radially. Linear Before Radial After Before After 45 .Drawings and Detailing Space Evenly Linear/Radial Equally spaces all dimensions.
Before After 46 . or radially. Before After Align Stagger Staggers linear dimensions.Drawings and Detailing Align Collinear Aligns dimensions horizontally. vertically.
Before After 47 . Before After Bottom Justify Dimension Text Bottom justifies linear dimension text.Drawings and Detailing Top Justify Dimension Text Top justifies linear dimension text.
48 . Before After Right Justify Dimension Text Right justifies linear dimension text.Drawings and Detailing Left Justify Dimension Text Left justifies linear dimension text. Before After You can adjust the spacing between dimensions using the thumbwheel in the dimension palette or by manually dragging the dimensions.
• The Dimension Spacing Value is the scaling factor for the spacing. if necessary Using Auto Arrange Dimensions To use Auto Arrange Dimensions: 1. Auto Arrange Dimensions The Auto Arrange Dimensions tool positions dimensions quickly and easily.Drawings and Detailing • The thumbwheel appears in the dimension palette only when spacing options are available. Box select all of the dimensions. 5. The dimensions are automatically arranged. the selected dimensions are placed as Spaced from smallest to largest Aligned and centered. For example. 3.SLDDRW. to display the 49 . 2 increases the spacing by a factor of 2. Open install_dir\samples\whatsnew\drawings\Auto_arrange. or doubles it. Move the pointer over the Dimension Palette rollover button dimension palette. 4. Click in the graphics area off of the dimension palette. 2. When you use Auto Arrange Dimensions follows: • • • • • . Click Auto Arrange Dimensions .Dimensions Adjusted to avoid overlapping Staggered. if possible Spaced with the offset distances defined in Document Properties .
Bounding Box for Sheet Metal You can display a bounding box that fits a flat pattern for sheet metal parts and bodies. 2. Move the thumbwheel to the right and left to adjust the Dimension Spacing Value. Select the horizontal dimensions at the top of the drawing and display the dimension palette. 50 . with or without grain direction.Drawings and Detailing Adjusting Spacing To adjust the horizontal spacing in the dimensions at the top of the drawing: 1.
In the Drawing View Properties dialog box. Click in Grain Direction. 2. edit the Flat Pattern feature. Select an edge or sketch line to define the grain direction. In the part. Right-click a drawing view and click Properties. 4.Drawings and Detailing No Bounding Box To display the bounding box: Bounding Box 1. Click . select Display bounding box. 2. To set grain direction: 1. 3. 51 .
fillets . 2. click Options Options. select from: • Center marks . On the Document Properties tab.assembly • Center marks . 3. To insert the cut list properties: 1.assembly • Center marks . click Detailing. Center Marks in Assembly Drawings You can insert center marks automatically in assembly drawings. Click to place the list in the graphics area. In an assembly drawing document. Under Auto insert on view creation. or slots automatically in assembly drawing views: 1.holes .assembly (Standard toolbar) or Tools > 52 .slots . In the graphics area. 2. right-click the flat pattern view and click Annotations > Cut List Properties.Drawings and Detailing Cut List Properties in Drawings You can insert the cut list properties as an annotation when you insert a flat pattern view of a sheet metal part in a drawing. To insert center marks on holes. fillets.
Drawings and Detailing
Cosmetic Threads
You can configure callouts for cosmetic threads. Cosmetic thread callouts are editable, and therefore configurable, only when Standard is set to None in the Cosmetic Thread PropertyManager. Use one of the following methods: PropertyManager Under Thread Callout, click Configurations and specify the configurations to which the callout applies. Design Table The column header for controlling the callout of a cosmetic thread uses this syntax: $THREAD_CALLOUT@cosmetic_thread_feature_name Example:
Drawings and Detailing
Display Scale in Orthogonal Views
You can display the scale of an orthogonal view if the scale is different than the default drawing scale. Previously, you could only display the scale of a detail, section, or auxiliary view in a drawing. To display the scale of an orthogonal view: 1. 2. 3. 4. In a drawing, click Options (Standard toolbar) or Tools > Options. On the Document Properties tab, expand View Labels and click Orthographic. Select Show label if view scale differs from sheet scale. Click OK.
Scale Displayed
Scale Not Displayed
Drawing Sheet Format
The default location for storing drawing sheet formats is now at: Windows XP Windows 7 Windows Vista C:Documents and Settings\All Users\Application Data\SolidWorks\version\lang\language\sheetformat C:ProgramData\SolidWorks\version\lang\language\sheetformat C:ProgramData\SolidWorks\version\lang\language\sheetformat
To change the default location, click Tools > Options > System Options > File Locations. In Show folder for, select Sheet Formats.
Dual Dimensions for Chamfers
You can display dual units in chamfer dimensions. For example, you can display the chamfer dimensions in inches and centimeters. To display dual dimensions for all chamfers in a drawing, click Tools > Options > Document Properties > Dimensions > Chamfer. Under Dual dimensions, select Dual dimensions display. To display units, select Show units for dual display.
Drawings and Detailing
To display dual dimensions for a particular chamfer, select the chamfer dimension and then in the Dimension PropertyManager, select Dual Dimension.
Hide Bodies in Drawing View
In addition to hiding components in a drawing view, you can now hide a body in a drawing view.
Hiding a Body
To hide a body: In the drawing view, right-click the body and click Show/Hide, then Hide Body.
Showing a Body
To show a body: 1. In the FeatureManager design tree or graphics area, right-click the drawing view and click Properties. 2. In the Drawing View Properties dialog box on the Hide/Show Bodies tab, select the body to view and press Delete. 3. Click OK.
Hole Tables
You can renumber the tags when you add or delete holes from a hole table. Renumbering All Tags To renumber all tags: Right-click the hole table in the graphics area or in the FeatureManager design tree and select Renumber All Tags. Renumbering a Series To renumber a series: Right-click any row in the series and select Renumber Series. In this example, hole A3 is removed and the corresponding A series is renumbered.
you can display the size of a hole in millimeters and inches. Merge and Unmerge Cells in Tables You can merge and unmerge cells in a table using tools from the Table pop-up toolbar. Select the cell.Drawings and Detailing Before renumbering series After renumbering series Dual Unit Support You can display dual units in hole tables. (Table pop-up toolbar). select Show units for dual display. click Tools > Options > Document Properties > Tables > Hole. select Dual dimensions display. Select the cells. To display dual dimensions in hole tables. 2. 56 . You can also right-click a hole table and click Show dual dimensions. 2. When dual dimensions are displayed. To merge cells: 1. Click Unmerge a Cell (Table pop-up toolbar). To display units. you can right-click the hole table and click Show units for dual dimensions. For example. Click Merge Cells To unmerge cells: 1. Under Dual dimensions.
In a drawing. (Annotations toolbar). To create a circular note pattern. set the options. 5. In the PropertyManager. 4. 57 . double-click each note and enter the text. then create the linear or circular pattern of the note. 2. click Circular Note Pattern or click Insert > Annotations > Circular Note Pattern. Pattern Notes You can display notes in linear or circular patterns in drawings. it was available only when you edited notes. 1. click Note (Annotation toolbar) or Insert > Annotations > Note. To edit the notes.Drawings and Detailing Notes Fit Text in Notes The Fit Text tool is available in the PropertyManager and pop-up toolbar when you create notes. First create a note. In the PropertyManager. Previously. 3. set the options for the note and place it in the drawing.
click Tools > Options > Document Properties > Detailing. 3. 1. Show Model Colors in Assembly Drawings You can view the model colors of a part or assembly in a drawing in HLR/HLV. click Options (Standard toolbar) or Tools > Options. In a drawing. On the Document Properties tab. Assembly with colors Drawing with colors 58 . Click OK. Select Use model color for HLR/HLV in drawings. click Dimensions and select Show units of dimensions.Drawings and Detailing Show Dimension Units You can show dimension units in drawings. To show model colors. 2. Any assigned layer overrides this setting.
In Tools > Options > Document Properties > Dimensions: • Arrow length increased from 3. Click Datum Feature (Annotation toolbar) or Insert > Annotations > Datum Feature Symbol.08mm. along the model line extension. click Leader . Attachment to Linear Dimensions You can attach datum feature symbols to linear dimensions. Horizontal Text. In the PropertyManager. Datum Feature Symbols Leaders You can use leaders for datum feature symbols that you apply to planar surfaces. The datum is placed in the center of the dimension. • Extension line: • Gap changed from 1mm to 0mm. puts the ANSI Drafting Standard The SolidWorks software supports some of the requirements of ASME Y14. chamfer dimension in line with the model edge. In the PropertyManager. Click Datum Feature (Annotation toolbar) or Insert > Annotations > Datum or No Leader Feature Symbol.3mm to 4.Drawings and Detailing GB Drafting Standard Additional requirements of the GB drafting standard are supported. In Tools > Options > Document Properties > Dimensions > Chamfer. • Beyond dimension line changed from 1mm to 2mm. under Leader. 59 . then select a linear dimension to which you want to attach the symbol. • Arrows changed from hollow to solid. set the options. a new Text position option.5-2009.
click All Over Leader . the symbol is placed as shown. Click Geometric Tolerance (Annotation toolbar) or Insert > Annotations > Geometric Tolerance. 60 . under Leader. Geometric Tolerance Symbols Leaders All Over is available as a new leader type. In the PropertyManager.Drawings and Detailing If you attach the symbol to a dimension that is centered between its extension lines.
3D Drawing Views You can use the 3D Drawing View pre-defined view orientations. set the options. In the Properties dialog box. Diameter and Square You can use the Diameter when applying a Flatness Unequally Disposed Profile and Square tolerance. If you click Exit its original orientation. When you rotate the model or set a . Click Save the view a View name. In the Symbols dialog box. select Modifying Symbols. Click Geometric Tolerance (Annotation toolbar) or Insert > Annotations > Geometric Tolerance.Drawings and Detailing Material Conditions The following material conditions are available. under Text. click More. you exit 3D Drawing View mode and the model returns to You can save the view orientation to use it in other views. symbol symbols You can use the Unequally Disposed Profile in geometric tolerance symbols. then select a symbol. type 61 . . Independency Continuous Feature Click Geometric Tolerance (Annotation toolbar) or Insert > Annotations > Geometric Tolerance. in Symbol library. tool to save a 3D drawing view or to select Click 3D Drawing View (View toolbar) or View > Modify > 3D Drawing View and access the options in the pop-up toolbar. and click OK. . In the PropertyManager. the orientation different view orientation from View Orientation is kept. The OK button has changed in functionality. Symbols The following symbols are available in the symbol library. then click OK .
You can move easily between designing models in SolidWorks and automating their production in DriveWorksXpress. 62 .11 DriveWorksXpress This chapter includes the following topics: • Task Pane Interface Task Pane Interface DriveWorksXpress is now available from the SolidWorks Task Pane.
a watermark displays a warning and suggests that you rebuild the part in SolidWorks. 63 . Filtering by Component Name You can filter the assembly tree to show component names that contain text you specify. You can also enter values to specify position. eDrawings now displays DWG files more accurately.12 eDrawings This chapter includes the following topics: • • • • • Display Enhancements File Synchronization Triad Manipulation Filtering by Component Name Native 64-Bit Support Display Enhancements The performance of display and printing in SolidWorks eDrawings is significantly improved for some documents. Gradient hatches are supported. Click Tools > Move Component and select Use triad or enter values. translation. type your search text in Enter text to filter list . or rotation. click View > Show Warning Watermark. To control the display of the watermark during the session. This feature was previously available only in eDrawings for Mac®. In the Component tree . Triad Manipulation You can manipulate components of an assembly with greater control and precision. and the handling of overlapping entities more closely matches the display order used in AutoCAD. When you open a potentially outdated component. File Synchronization eDrawings can now detect when the graphics data for a component may not be in sync with a later version modified and saved within a SolidWorks assembly. You can use the triad tool to constrain component movement to a coordinate axis or plane and to rotate components about a coordinate axis.
64 .eDrawings Native 64-Bit Support SolidWorks eDrawings software can now run as a native 64-bit application on a 64-bit Microsoft® Windows® operating system. which permits larger documents to be opened.
All commands are grouped into four Enterprise PDM menus at the top of the file view pane. Click Actions to access actions you can perform such as checking files in or out. The commands available depend on your selection.13 Enterprise PDM This chapter includes the following topics: • • • • File Explorer and SolidWorks Add-in Administration Tool API Installation File Explorer and SolidWorks Add-in Enterprise PDM Menus New menus for the SolidWorks Enterprise PDM client make the commands that you use most frequently easier to find. the most frequently used commands are still available by right-clicking. The new menus reduce the length of the shortcut menu. However. 65 .
66 . such as changing a file's state. or view its properties. Click Display to control how vault information is displayed in the file view pane. Display also lets you view a selected document's history. open it in the SolidWorks Enterprise PDM File Viewer.Enterprise PDM Click Modify to access commands that let you make modifications. The Options submenu lets you choose display options such as Set focus to active configuration and Show bitmap for SolidWorks files.
the Report Generator.Enterprise PDM Click Tools to access tools such as Search. On Windows 7 systems. Copy Tree. To display them. click Get help on the Windows Explorer toolbar or select Help > SolidWorks Enterprise PDM Help on the Windows Explorer menu bar. click Organize > Layout and select Menu bar. Windows Explorer menus are suppressed by default. or the Administration tool. Expanded Search Capability You can use new options on the History tab of the Complete Search card to search the vault based on text in file/item names and configuration/sheet names. To access the File Explorer online help. the Notification Editor. 67 .
Click Tools > Update References. Click (Search dialog box toolbar). • You can replace existing references. Expand (menu bar) and click Complete Search. To access the new search options: 1. 68 . 4. 2. an assembly) and click the Contains tab. To update the references. The referenced files are listed. Select a file that references other files (for example. you can preview files by selecting them on the Contains or Where Used tabs. select the folder to search. 5. listing all references and identifying those that are missing. 4. navigate to a folder in an Enterprise PDM vault. 2. 2. Expanded File Open Capabilities In the SolidWorks Open dialog box. 3. In SolidWorks and other applications. update the references. Warning messages appear when you try to check files with broken references into the vault. and click Next. • You can repoint references to existing files in the vault. To use the Contains tab to preview and open files: 1. On the History tab. Select a file with broken references. Files matching the search appear in the middle pane of the Search dialog box. 3. 3. In the Find Files wizard. type the text to search for. The Update Reference dialog box opens. you can locate them. Updating Broken File References You can use the Update References command to repair broken file references. double-clicking a file on the Contains or Where Used tabs opens the file in the application. click Open (Standard toolbar) or File > Open. In the Open dialog box. 4. and add the files to the vault. In the Text to find in history field.Enterprise PDM Administrators must use the Card Editor to add the new options to search cards created before SolidWorks Enterprise PDM 2011. In SolidWorks. specify how the search should be performed. click Find Files (Update References toolbar). Select a referenced file. select Look in file/item names or Look in configuration/sheet names. cancel the check in and complete the following procedure: 1. Double-click the referenced file to open it in SolidWorks. The preview in the Thumbnail window shows the referenced file. • If the referenced files are outside the vault. If a warning indicates that a file cannot be found.
2. Menu options in the Update References dialog box let you: • • • • • Save the file list as a CSV file Open the file list in Excel Change the view of columns Replace a selected reference Add a file to the vault if it is found outside the vault Saving eDrawings Markup Files SolidWorks eDrawings markup files saved from the Save Markup dialog box are automatically added to the vault. Restoring Files from Cold Storage You can retrieve files from cold storage for any archive server to which you have access if your administrator has granted you permission. you cannot restore them. In the submenu. in eDrawings. markup has been added to the list of files that are always saved to the vault. Select a file and click Actions > Get Version. select the files to update. expand the list and select the file to use. You can only restore files that were removed from the vault by moving archive files to a folder outside the archive. The file is restored to the folder containing the non-cold stored versions. including the restoration date and user name. To see the added file type in the Administration tool: 1. You may want to retrieve files from cold storage if a design's functional specification has changed or if you need to access an older archived design change. 5. 7. Under Review files to update. You can use submenu support to organize items you create in File Explorer. If your administrator set up cold storage to delete archive files. Expand Users. and click Finish. On the Adding Files tab of the Settings dialog box. Click Update to save the reference paths that are shown in the Found In column to the parent file. click File > Save Markup. The restored file's history contains a comment that the file was restored from cold storage. and click Settings. 69 . To restore files from cold storage: 1. Creating Submenus The Enterprise PDM API now supports submenus. such as Search Favorites. expand Versions in Cold Storage and select the cold stored version to use. 2. To save markup files to the vault automatically. If the Found in column indicates that there are multiple matches.Enterprise PDM Files that meet your search criteria are listed. right-click your user name. Click Tools > EPDM Administration to open the Administration tool. 6.
select users who can see the favorite. select the search type to use. In the SolidWorks Enterprise PDM Search dialog box.dll files. version numbers of all installed Enterprise PDM . • Include special instructions or problem descriptions. The wizard creates a single package that you can send to technical support. The backup is not added to the package. type submenu_name\favorite_name . Click Search (Enterprise PDM menu bar). When you view the Search menus. the new favorite will be listed in the submenu: Administration Tool Collecting Support Information You can run the Collect Support Information wizard to collect information about a vault. and all installed add-in packages. registry and environment information. 5. • Create a backup of the SQL database. database statistics. 4. The . Click Add to Favorites (Search dialog box toolbar). for Favorite name. The Collect Support Information wizard lets you: • Specify logs and settings to collect. Enterprise PDM client. 3. and local event logs. • Select folders and files to include in the support package. 2. In the Add to Favorites dialog box. • Specify the location where the support information package is saved. Options include archive server.exe and . 70 .zip file created by the wizard maintains the archive server folder structure if you include archives. Add search criteria to define the search. This input is saved as AdditionalInformation.Enterprise PDM To create a submenu for your favorite searches: 1. and click OK. You must be logged in as the Admin user to run the wizard. You must provide the backup manually to technical support.txt in the package.
htm. you can now import groups.solidworks.smg and . The 3DVIA Composer Player is available as a free download from http://www. which is installed when you create a vault using the Default setup. As with other previews. You can import Active Directory groups: • When you add or edit a group • When you add a new user New users are added to Enterprise PDM groups with the names they have in the Active Directory groups. Importing groups from Active Directory lets you quickly set up the Enterprise PDM environment to be the same as the environment throughout your organization. you can use the 3DVIA Composer Player tools to manipulate the model. Design Checker Validation You can use the new Design Checker task to validate selected SolidWorks documents in the vault using standards (.Enterprise PDM Group Import from Active Directory If you have defined the Archive server login type as Windows login.smgxml. group memberships. The 3DVIA Composer data card. 71 . lets users view file information. 3DVIA Composer File Format Support SolidWorks Enterprise PDM now recognizes the 3DVIA Composer file formats .com/sw/support/downloads. on the 3DVIA Composer tab. Users can preview embedded 3DVIA Composer files if the 3DVIA Composer Player is installed. and email addresses from Microsoft Windows Active Directory®.swstd) files created in the SolidWorks Design Checker add-in.
then click OK. In the left pane. and notifications. Select the files to check. To initiate the task in File Explorer: 1. the Design Checker status appear on the document's data card. After a design check. You can initiate the Design Checker task: • For selected files in File Explorer • From the Add Task button of the Task List dialog box in the Administration tool • By changing a file's workflow state When the task runs. who has permissions to run the task. • Reports list the criteria used to evaluate the document and show failed checks. 72 . Select the user whose permissions are used when the task is run. 1. You configure the Design Checker task in the Administration tool to specify the computer the task is run on. On the Add-in screen. Click Success Notification and Error Notification to create notification messages and select users and groups to be notified. you can modify the documents you check to meet the design standards. click Add Task. To initiate the task in the Administration tool: 1. click Execution Method and select how the task is initiated and the computer on which the task is run. 2. whether to auto-correct failed checks. select Design Checker. In the Task List dialog box. the Design Checker card is selected as the input card. and where to store reports and logs. Click Permissions and select users and groups that are allowed to initiate the task. Configuring the Design Checker Task You configure the Design Checker task from the Tasks node of the Administration tool. By using auto-correct. materials. you complete the Design Checker card to specify the standards file to use. 6. and sketches to ensure that SolidWorks documents meet pre-defined design criteria. • Log files list the selections made when the task is run and the results of task execution. Click Menu Command and specify whether and how the command appears to users in File Explorer. 4.Enterprise PDM SolidWorks Design Checker verifies design elements such as dimensioning standards. In the Add Task dialog box. fonts. Expand Tasks and double-click Design Checker. 3. 5. Click Actions > Design Checker. Click Tasks > Task List. You can also set up design checks to be performed during workflow transitions by specifying that the Design Checker task is performed as a transition action. 4. Running the Design Checker Task You can run the Design Checker task in File Explorer or from the Administration tool. 3. such as success or failure checking files out and in. Use the Select Files and Folders for Design Checker dialog box to select the files to check. 2. 2.
variables have been reorganized on a second flyout menu. Select Variables to display a list of variables that you can use in the formula. 2. when the task runs. 2. • Where reports and logs generated by the Design Checker task are saved. 2. 4. 73 . To use an alias list in a data card: 1. Add one of the following controls: • Listbox • Droplist • Combobox • Combolist 3. • Whether to auto correct failed checks. CSV files. Arithmetic and String Functions in Input Formulas You can now add arithmetic and string functions to input formulas for data card edit boxes. The standards file must be checked in to the vault. Aliases let you truncate values for display and for use in input formulas. Under Input formula. Aliases in Card Lists A new Text with Alias card list data type lets you add aliases when you create card lists to display variable values in data cards. In the dialog box. type the alias to use for the displayed value when the list is used. Open the card in the Card Editor. 4. In the Data list. Under Items.Enterprise PDM In both File Explorer and the Administration tool. to the right of the field. For easier access. click . right-click under Displayed Value or Alias and click Paste. you can copy and paste them to easily create card lists with aliases. The arithmetic and string functions are available as input formula selection choices that are organized on a flyout menu. To create an alias list: 1. To add arithmetic and string functions to an input formula: 1. If you have existing lists of associated variable values and aliases in spreadsheets or other documents. 4. Add an Edit control. type the value. select Special value. In the card list. the Design Checker template card displays to let you specify: • The . for Displayed Value. Open or create a data card in the Card Editor. 2. type the List name and select Text with Alias as the Data type. For Alias. 3.swstd file to use. 3. Select the alias list to use. Right-click Lists (for cards) and click Add New. Open the source document and copy the values. or Word tables: 1. To use existing lists of paired display values and aliases from spreadsheets.
5. The workflow link is maintained. create two workflows. 2.cex files when you export a workflow from SolidWorks Enterprise PDM 2011 or higher. 6. Right-click in the first workflow. Save the modified card.Enterprise PDM For easier access. 7. create vaults A and B. In vault A. In an Enterprise PDM archive.cex file. Select the variable to add. 3. 5. Export both workflows to a . the variables list is now divided into alphabetically-arranged sublists. Enterprise PDM maintains any links between workflows. Workflow links are only maintained in . Exported Workflow Links When you export workflows as . Save the workflows. Import the . View the workflows in the Workflow editor. Select the second workflow as the workflow to link to.cex file into vault B. 4. and select New Workflow Link.cex files and then import them into a vault. Select Functions to display a list of arithmetic and string functions to use. 74 . 6. To see this functionality: 1. 8. Select the function to add.
Click OK. In the task's Properties wizard. To access the guide. users see: 75 . This functionality replaces two options on the File Type Properties dialog box in previous versions of Enterprise PDM: • Do not show "sub-parents" for this file type • Show this file type as a "sub-parent" (drawing) API For information on using the Enterprise PDM API. drawings that are sub-parents to the . Expand File Types. You do not need to do this programmatically. To add the file type drw. Adding Commands to Submenus You can now structure add-in commands so that they appear in submenus.Enterprise PDM Associating Drawing Types with File Types You can improve performance by modifying file type properties to specify the types of drawings that are checked for references when you check specific files out or in.sldprt files: 1. The reference check determines if a drawing is a sub-parent of the file you are checking out or in.sldprt file appear in blue above the . The file type slddrw is listed by default. For example. so that the field reads slddrw. for Menu command. see the SolidWorks Enterprise PDM Programmer's Reference Guide. This example describes how to specify the drawing types to check for references to . You can structure cascading menus by adding backslashes to menu strings. Do not include periods (.sldprt file so you can choose to check them out or in.) 4.drw. Double-click sldprt.) and type drw. when you configure a task. right-click Add-ins and click Programmer's Reference Guide. When you check a . on the Menu Command screen. type Tasks\command_name . you can make the task command appear to users in a Tasks submenu by writing the menu command with a backslash. In File Explorer.sldprt file out or in. type a comma (. Enterprise PDM looks for references to the file in all files of type slddrw and drw. In the Check Out or Check In dialog box. under This file can have drawing nodes with the following extensions. 3. 2. specify the file types to be checked for references. In the File Type Properties dialog box.
Enterprise PDM Using an Add-in to Define Item Explorer Menu Commands You can define menu commands to be used in Item Explorer. items. 76 . Enterprise PDM components now communicate with SQL Server 2008 or SQL Server 2005 using ODBC. Installation SQL-DMO Drivers It is no longer necessary to install SQL-DMO drivers when deploying Enterprise PDM clients using an administrative installation image. and folders • The Item Explorer Tools menu • The Item Explorer toolbar Updating the BOM Quantity Using the API You can now update the BOM quantity using the API without having a pre-defined BOM view. You can add commands to: • Shortcut menus for files.
IFC Files.IFC Files You can import Industry Foundation Classes . 77 . 4. For more information. Navigate to the correct folder and enter a file name. 2.ifc files: 1. (Standard toolbar). click Open for File of type select IFC 2x3 and select a file to open. To import .ifcxml model files into SolidWorks. Click Save. the file geometry is imported but the resulting SolidWorks model has essentially no features. For Save as type. 3. select IFC 2x3.IFC Files DXF DWG Import Wizard Exporting Sheet Metal Parts to DXF or DWG Files Importing or Exporting . select the OmniClass and units. ™ Click Options.ifc files into SolidWorks.ifc or .ifc format. To export SolidWorks models as . and click OK. You can also export SolidWorks models to . 5. Click File > Save As.14 Import/Export This chapter includes the following topics: • • • Importing or Exporting . When you import .ifc files into SolidWorks. see SolidWorks Help: .
select Import to a new part as and 2D sketch. 2.dwg or . Select other options and click Finish. select Rotate about the origin and enter the angle of rotation. In the DXF/DWG Import wizard.DWG or . Select other options and click Finish. you can launch the SolidWorks Repair Sketch tool from the DXF/DWG Import Wizard to fix gap or overlap errors after import. Click Next.dwg or . Open a . click Undo Remove Entities 6. Adjust the origin values and click Apply.dwg file. Select part document options and click Next. Defining the Sketch Origin and Orientation on .dxf file as a 2D sketch for a part. . you can create a new sketch for each layer in the file. select entities to remove and click Remove Entities.dxf file as a 2D sketch for a part. 5. To undo this action. Open a .DXF Import When importing a . you can define the model origin and orientation. In the DXF/DWG Import wizard.dxf file as a 2D sketch for a part. Repairing Sketches After . Select Import each layer to a new sketch. In the preview. 7. 78 .dxf file as a 2D sketch for a part. Select part document options and click Next.DWG or . 4. 3.DXF Import When importing a .dwg file. Click Next. In the DXF/DWG Import wizard. 2. Click Define Sketch Origin and click a point in the sketch preview to define the origin. 5.Import/Export DXF DWG Import Wizard Importing Layers from .dwg or . 4. select Import to a new part as and 2D sketch. 3. Open a . 1.dwg file.DXF Import When importing a . you can filter out unnecessary entities. 1. select Import to a new part as and 2D sketch.dwg file with layers. 3. 6. 5. To change the model orientation about the origin. 1. Click Next.DXF Files When importing a . Open a . Select other options and click Next or Finish.DWG or .DWG or .dwg or . 1. 4. 2. Filtering Sketch Entities on . 8.
Select other options and click .Import/Export 2.dxf or . For file type. 5. 3. select Bounding box. 6. • Map other properties. 5. Select other options and click Finish. 5. in sheet metal drawings with up and down bend directions. In the SolidWorks to DXF/DWG Mapping dialog box: • Assign layers to entities. select .dwg. you can map the different bend line directions to separate layers when you export the drawing. Click File > Save As. To export and map bend line directions for a sheet metal part: 1.dwg file. • Click OK. For file type. In the DXF/DWG Import wizard. In the DXF/ DWG Output PropertyManager. Select part document options and click Next. Click Options. 79 . 4. 3. under Entities to Export. select . Click Options. under Entities to Export. In the SolidWorks to DXF/DWG Mapping dialog box: • Assign layers to entities. you can export the bounding box and assign the bounding box to a specific layer. Exporting Sheet Metal Parts to DXF or DWG Files Exporting a Bounding Box When exporting a sheet metal part as a . You can map bend line directions for exported sheet metal parts or drawings. For example. Click File > Save As. Select other options and click .dwg. 2.dxf or . set export options. Select Run Repair Sketch. and click OK. In the DXF/ DWG Output PropertyManager. Exporting Bend Line Directions You can map bend line directions to specific layers when you export sheet metal models as . 3. 2. 6. To assign the bounding box sketch to a layer: 1.dxf or . set export options. 6. select Bend lines.dxf or . • Map other properties. Click Next. and click OK. 4. • Click OK. 4. select Import to a new part as and 2D sketch.dwg files.
This chapter includes the following topics: • • • Walk-through Importing or Exporting . in the PropertyManager.15 Large Scale Design Large Scale Design helps you use the tools that the SolidWorks software offers for creating equipment. click Record . You can also use the arrow keys and the mouse to maneuver through the system. and use the controls to maneuver through the system. click View > Lights and Cameras > Add Walk Through. Define your starting point. To use the mouse. such as the camera height. The keyboard controls are: 80 . and plants. left-click to manipulate the view. Define motion constraints and other parameters. You can save what you see and play it back for further study. facilities. To activate the function. and click Capture Motion to open the control panel. You "see" the geometry of the system as you maneuver through it. You may eventually find that a combination of mouse and keyboard controls allows you to maneuver through the system most efficiently.IFC Files Grid System Walk-through You can use the Walk-through function to explore or create a video of the 3D geometry of plants or other systems.
Lock to constraint. or right. You can also export SolidWorks models to . Increase or decrease speed.Large Scale Design Arrows Shift + arrows Control + arrows Alt + arrows Home Z. or right. down. Importing or Exporting . Set speed. 1-9 Scroll Lock Page Up Page Down R Space Esc M Move forward or back. Reset "view" direction. To import . Previous constraint. Next constraint.ifc or . Toggle map view. Look up. . Press the Alt and arrow keys simultaneously. Turn up or down.ifc) files into SolidWorks.ifc files: 81 (Standard toolbar).ifcxml model files into SolidWorks. Move up. turn left or right. Zoom out or in. left. down.ifc format. Cancel. Pause.IFC Files You can import Industry Foundation Classes (. left. click Open for File of type select IFC 2x3 and select a file to open. To export SolidWorks models as . Shift + Z +. Record.
Multiple users can use the grid system and work from the same baseline. select IFC 2x3. select the OmniClass and units. The sketch is replicated for every floor in the structure. To reduce clutter. The grid system is useful when creating welded structures. 2. 3. Click File > Save As. When you use the Grid System tool. Grid system sketch Click Grid System System. Navigate to the correct folder and enter a file name. The grid system is also helpful when you work with multiple users who use different third-party applications to make grids. You can create a grid to help specify the location of key elements in structures. You can then specify the number of floors for the structure and the distance between each floor. Grid System You can use the Grid System tool to lay out a grid system for large structures. Display options are available to help you visualize the grid structure and to ensure correct grid inferencing. ™ Click Options. you can hide and show the geometry. For more information. 4. Balloons are attached to the grid items to help with orientation.Large Scale Design 1.IFC Files. 82 . see SolidWorks Help: . For Save as type. Grid system with weldments applied (Features toolbar) or Insert > Reference Geometry > Grid See SolidWorks Help: Creating a Grid System. Click Save. and click OK. you create a sketch to represent the grid. 5. The graphics area can appear cluttered when the grid system creates a lot of geometry or if you create multiple grid systems.
83 . right-click Grid System and click View Grid Components. such as Normal To . in the FeatureManager design tree. In the View Grid Components dialog box.Large Scale Design To access the display options. select an item and click a display option.
On the DisplayManager tab. You can also save custom appearances in SolidWorks Standard. and Walk Through.16 Model Display This chapter includes the following topics: • • • • • • DisplayManager Appearances Scenes Decals PhotoView 360 Working with Appearances and Rendering a Model DisplayManager The SolidWorks DisplayManager is the central location for managing appearances. including controls previously available only in PhotoView or PhotoWorks. lights. scenes. edit. The DisplayManager lists the appearances applied to the currently active model. click View Appearances . Appearances All appearance functionality. click the DisplayManager tab . 84 . and delete display items applied to the current model. cameras. is now available in SolidWorks Standard. decals. Use the DisplayManager to view. On the Manager Pane.
control the background or environment. You can use the Edit Scene PropertyManager to add a background image to the scene. Background images in legacy models are discarded and are not displayed. Lights and Cameras Scenes are simplified and now consist of the following: • A spherical environment based on a preset scene or image you select is mapped around the model. To save a custom scene. . • A 2D background that can be a single color. The DisplayManager lists the background and environment applied to the currently active model. and save custom scenes. lets you size the floor. a gradient of color. Scenes Scene functionality is enhanced to allow full control of the scene that is visible behind the model. On the DisplayManager tab. 85 . click View Scenes. • A 2D floor on which you can see shadows and reflections. The Insert Picture functionality is removed. available from the View Scene pane in the DisplayManager. You can change the distance of the model from the floor.Model Display See SolidWorks Help: Appearances. The new Edit Scene PropertyManager. You can also turn off the background and show the spherical environment instead. elements of the environment are reflected in the model. Although partially obscured by the background. or an image you select. click Save Scene on the Advanced tab of the Edit Scene PropertyManager.
Use the DisplayManager to view and manage decals applied to the current model. 86 .Model Display Office Space scene Rooftop scene Warm Kitchen scene See SolidWorks Help: Scenes. click View Decals . On the DisplayManager tab. Decals Decals are now part of SolidWorks Standard.
PhotoView 360 PhotoView 360 is now the standard photorealistic rendering solution for SolidWorks. Add in PhotoView 360 and select actions from the PhotoView 360 menu or from the Display tab of the CommandManager. click PhotoView 360 > Preview Render. 87 . Rendering capabilities are the same as in previous releases. With PhotoView 360 added in. The underlying technology has been updated to enhance the user experience and the final results. See SolidWorks Help: PhotoView Preview Render Window. PhotoView 360 is available in SolidWorks Professional and SolidWorks Premium.Model Display See SolidWorks Help: Decals. PhotoView Preview Window The PhotoView Preview window lets you anticipate how changes to a SolidWorks model affect the final rendering of the model. PhotoWorks is no longer supported.
Scene lighting is not possible in RealView. you make further adjustments to lighting and scenes before completing a final render. You typically need additional lighting in PhotoView to illuminate an occluded space in the model. lighting is off in PhotoView. Lights and Cameras See SolidWorks Help: Lights. . PhotoView Support on 64-bit Computers Native support for the PhotoView 360 application on 64-bit platforms lets PhotoView use all available system memory. you use the Display Manager. Controls for shadows and fog now provide a stronger integration with PhotoView.Model Display Lights The DisplayManager is the central location for managing all aspects of lighting. and Cameras pane of the DisplayManager have the following meanings: Directional1 On in SolidWorks Off in PhotoView Spot1 Off in SolidWorks Off in PhotoView Point1 Off in SolidWorks On in PhotoView On the DisplayManager tab. so you often need to illuminate models manually. 88 . Lights. Light intensity is controlled with wattages. Right-click the Motion Study tab and click Create New Motion Study. Lighting controls are separate for SolidWorks and PhotoView 360. change appearances on a model. including lighting controls that are available only when PhotoView is added in. The icons for specific lights in this image from the Scene. you can take advantage of the realistic lighting provided by scenes. point. Working with Appearances and Rendering a Model In this example. and directional lights are on in SolidWorks. If you have installed SolidWorks Professional or Premium. The DisplayManager lists the lights applied to the currently active model. click View Scenes. SolidWorks By default. With lights off. and add a decal. Motion Animations are rendered using PhotoView. PhotoView By default. spot.
Why do you open the part in its own window? 89 . Expand Face.SLDASM. The DisplayManager catalogs the appearances cameras applied to the model. click View Appearances . 4. 5. right-click the black box and click Open Part (Context toolbar). and scenes. Expand the black appearance to see where it is applied. In Sort order. select Hierarchy. Under the DisplayManager tab. Open the box part in its own window. decals . lights. Adding and Editing an Appearance In this section. The black appearance is applied to faces of the box. 2.Model Display Learning About the DisplayManager To start working with the model: 1. 1. you add an appearance to a part in the model and edit the appearance. In the graphics area. and 3. . In the Manager Pane. click the DisplayManager tab. Open install_dir\samples\whatsnew\display\tractor_in_box.
In the Task Pane. d) Click . appearances are applied to components.10 to create a matte appearance that reflects almost no light. click Appearances > Plastic > Textured. Because the faces are highest in the hierarchy. b) Expand Parts/Assemblies and Face. You edit the part to gain more control over where to apply the appearance. c) On the Illumination tab. Alt + double-click PW-MT11010 to apply it to the entire part and to open the Appearance PropertyManager. b) Click Advanced. under Color. edit the appearance: a) On the Color/Image tab. In the PropertyManager. • In a subsequent step. 5. on the Appearances/Scenes tab . black. 2. The entire part has the PW-MT11010 appearance.Model Display • You want to change the appearance of the inside of the box only. set Specular Amount to 0. not to assemblies. change the color to medium grey. 3. Review your work: a) On the Appearances pane of the DisplayManager. you apply a decal. 4. overrides the appearance at the part level. We recommend applying decals to parts. in Sort order. overriding part appearances. select Hierarchy. By default. 90 . In the bottom pane. their appearance. in assemblies.
. 91 . 4.SLDASM. In the Decals PropertyManager. Zoom in to the small rectangular panel inside the front of the box. 2. The decal adjusts to fit the rectangle. you can add decals without loading any add-in applications. If you are prompted to rebuild the model. Changing Another Appearance on the Model Return to the assembly and apply an appearance to the tractor. click Decals. you add a decal to the part. on the Mapping tab: a) Select Fit height to selection. Zoom in to the tractor.Model Display Adding a Decal In this section. where you will place the decal. 1. click Yes. In the Task Pane. Drag the logo decal to the rectangle. 2. b) Click . on the Appearances/Scenes tab 3. Click Window > Tractor_in_box. 1. In SolidWorks 2011.
a) In the Task Pane. . b) Drag burnished chrome to the rightmost stack. If you have installed SolidWorks Professional or SolidWorks Premium. By default. 92 . select Keep light when scene changes. click Assembly. c) Right-click Point2 and select Edit Point Light to increase the brightness of the light. Press F to fit the entire assembly in the graphics area. and spot lights unless you select Keep light when scene changes on the PropertyManager for each light. Change the appearance of the rear exhaust pipe: a) In the Task Pane. 1. b) Expand Lights. If you are not satisfied with the lighting provided by a scene. on the Appearances/Scenes tab > Chrome. In preparation for rendering. 4. e) On the PhotoView tab. d) On the Basic tab. add in PhotoView and use the Preview window to anticipate the effect of further changes. 4. Changing the scene removes all directional. then PhotoView 360 is available and you can continue to the next steps. and click OK. click Scenes > Basic Scenes. point. The PhotoView icon next to Point2 is enabled to indicate that the point light is on in PhotoView. 2. Change the scene to affect lighting and highlights. click View Scenes. 3. Right-click Point2 and click On in PhotoView. you have performed all steps in the SolidWorks software without adding in PhotoView 360. While it is open. Lights and Cameras . the Preview window remains on top of the SolidWorks window. on the Appearances/Scenes tab. The Preview window updates. select PhotoView 360. Adjust the lighting: a) In the DisplayManager. click Appearances > Metal c) On the popup toolbar. Preparing to Render: Working with Lighting and Scenes So far. lights are off in PhotoView because scene lighting is usually sufficient to illuminate the model.Model Display 3.3. Arrange or resize the Preview window so that you can see the graphics area. Click PhotoView 360 > Preview Render. The image in the graphics area does not change because your action does not affect SolidWorks. you can either adjust the lights in the current scene or try a new scene. f) Click . The light inside the box is too dim. set PhotoView brightness to 0. Click Tools > Add-Ins.
93 .Model Display b) From the bottom pane. type a file name. Performing a Final Render You are now ready to perform the final render. The Render Frame dialog box opens and rendering begins. 2. 4. Click Save. 3. Browse to the directory. Click Save Image. drag Backdrop . and select the type of image to save. The Preview window updates. 1. Click PhotoView 360 > Final Render.Studio Room into the graphics area.
To further modify the surface. In the second image the surface has been fixed. Manual Mode lets you override the defined parting surface direction and manually create a portion of the surface. right-click an inner vertex and select Start fill surface region or End fill surface region. which lets you modify surface direction. The first image below shows an irregular parting surface. 94 . Select Manual Mode in the Parting Surface PropertyManager to display handles that you can manipulate to adjust the parting surface.17 Mold Design This chapter includes the following topics: • Manual Mode for Creating Parting Surfaces Manual Mode for Creating Parting Surfaces You can create parting surfaces using Manual Mode.
Mold Design 95 .
or any result as the independent variable. You can also use the Function Builder to define a motor or force profile from a mathematical expression or from interpolated functions along connected segments. This chapter includes the following topics: • • • • Function Builder Reflected Load Inertia and Reflected Load Mass Reference Components for Linear Couplers Motion Along a Path Function Builder For Motion Analysis studies.18 Motion Studies Available in SolidWorks Premium. For motor profiles. cycle angle. 96 . you can specify time. you can use the Function Builder to define motor or force profiles from an imported data set.
For Category. For more information. To define a path mate motor: 1. see SolidWorks Help: Motion for Components Mated with Linear Couplers. Reflected Load Inertia and Reflected Load Mass For Motion Analysis studies. select a path mate. For the first selection component tree. select a rotary motor from the MotionManager . click Motor (MotionManager toolbar) and in the PropertyManager. Motion Along a Path For Motion Analysis studies. for Motor Type.Motion Studies To open the Function Builder from a Motion Analysis type study. You can also access the Function Builder from the Force PropertyManager. select Other Quantities. For Path Mate . From a Motion Analysis study. or acceleration values as a body moves along a path. select reference components when you specify linear/linear coupler mates in the Mates PropertyManager. you can define a path mate motor to specify displacement. . To create reflected load inertia results: 1. click Motor . . 5. you can compute and plot the reflected load mass for linear motors and the reflected load inertia for rotary motors. 2. Select Plot Results options and click Reference Components for Linear Couplers You can select reference components for components mated for linearly coupled motion. under Mates in the FeatureManager design tree. click Results and Plots 2. When required. For Subcategory. For more information. From a Motion Analysis study. click Create New Function. velocity. 3. 97 . Select the motor profile. 3. see SolidWorks Help: SolidWorks Motion Function Builder. select Reflected Load Inertia 4.
click Reverse Direction . click Create New Function.Motion Studies To define the motor profile from a function or from data. Select options and click . for Mates/Direction. To reverse the motor direction. 4. 98 .
Equations Sharing Equations Among Models You can share equations and global variables among models. Alternatively. see Defeature for Assemblies on page 25. You can then share the new file without revealing all the design details of the model. solids without feature definition or history). 99 . Click Tools > Defeature to access the Defeature PropertyManager. Then you import information from the text file into other models. Before After For a step-by-step example. which provides tools for manual and automatic selection of details to keep and remove. You export selected equations and variables from a model to an external text (. you can build the text file manually using an application such as Notepad. you can remove details from a part or assembly and save the results to a new file in which the details are replaced by dumb solids (that is. so that changes you make in the text file update the equations and variables in the models.txt) file. You can choose to link models to the text file.19 Parts and Features This chapter includes the following topics: • • • • Parts Features Surfaces FeatureWorks Parts Defeature for Parts With the Defeature tool.
sldprt. Open install_dir\samples\whatsnew\parts\backplate_01. Five equations are imported into the model. type my_equations. In the Equations dialog box: • Under Active.Parts and Features Exporting Equations In this example. Because Link to file was selected. 5. If prompted to rebuild. 100 . In the Save As dialog box. All the equations are listed in the Equations Export dialog box. The text file is available to import into other parts and assemblies. Click Save. The equations are saved in a text file. displays the path to the external file. changes you make in the text file are propagated to the model. 1. all the equations are selected for export. 3. Linked File 7. click Import. • At the bottom of the dialog box. 2. Link to file is selected as well. Open install_dir\samples\whatsnew\parts\frontplate_01. 4. 6. Importing Equations Now import the equations from the text file to another part. c) Click Open. 3.sldprt. for File name. click Yes. the icon indicates equations that are linked to the external file. In the Equations dialog box. Click OK. 8. Click Export. Under Active. Click Tools > Equations. Click Save. 4. the icon indicates equations that are linked to the external file. 1. 2. In the Equations dialog box: • Under Active. Save the part. The Equations dialog box lists five equations. you export equations from a part to a text file. In the Open dialog box: a) Select my_equations. b) Select Link to file. Click Tools > Equations.txt.
Parts and Features • At the bottom of the dialog box. 6. displays the path to the external file. In the FeatureManager design tree. right-click Equations and click Add Equation. The syntax of the Visual Basic IIf function is: iif(expression. 7. Save the part. Click OK. Click Rebuild (Standard toolbar). truepart. you use the Visual Basic IIf function to specify when to suppress or unsuppress a feature or component. Open frontplate_01. To suppress the feature: 1.sldprt from the previous example. In the Add Equation dialog box. click the linear pattern feature LPattern1. so you define an equation to suppress or unsuppress the linear pattern feature depending on the part length. you suppress a hole in a plate when the length of the plate is less than 40 mm. "LPattern1" appears in the Add Equations dialog box. The hole you want to suppress is part of a linear pattern. Linked File 5. Suppression States of Features and Components You can use equations to control the suppression state of part features and assembly components. The Equations and Add Equations dialog boxes open. In the FeatureManager design tree. The equations are applied to the model. 3. 101 . 2. falsepart) where: • expression is the expression you want to evaluate • truepart is the value to use if expression is true • falsepart is the value to use if expression is false Defining a Feature Suppression Equation In this example.
The external equations file is checked for changes and the length of the part is updated from 100 to 35.txt again. 6. and change "overall length" back to 100. "suppressed". LPattern1 is unsuppressed. which triggers the suppression of the linear pattern feature. 2. Because the length is now less than 40 mm. 5. In the dialog box. The external equations file is checked for changes and the length of the part is updated from 35 to 100. 102 . complete the equation: "LPattern1" = iif ("overall length"<40. Save the text file. change 100 to 35.Parts and Features If Instant 3D is active.txt. LPattern1 is suppressed. you need to click-pause-click LPattern1. expand Equations in the FeatureManager design tree and click "overall length"=100. The second click adds it to the Add Equations dialog box. 4. click the suppress and unsuppress buttons in the dialog box. Testing the Feature Suppression Equation Now decrease the length of the part to 35 mm. which is defined in the linked external file. The first click selects the linear pattern. • To insert "suppressed" and "unsuppressed". Click OK. 6. 3. "unsuppressed" ) You can type the entire equation or use the following tips to enter various pieces: • To insert global variable "overall length". Click Rebuild (Standard toolbar). Save and close the text file. Because the length is now greater than 40 mm. Edit my_equations. 5. 7. Click Rebuild (Standard toolbar). Open my_equations. For "overall length". Click OK. The new equation is added to the Equations dialog box. 4. To trigger the suppression state equation: 1. The length of the part (length@outline) is controlled by the global variable "overall length". which eliminates the second hole.
Click OK to dismiss each warning. b) Select Link to file. 5.sldasm. 3. Because the assembly does not contain all the same dimensions as the parts. Click Save. In the Equations dialog box. click Yes. Exporting the Feature Suppression Equation Now add the new equation to the external text file. Open install_dir\samples\whatsnew\parts\plate_assembly_111. 4. The new equation appears at the bottom of the list. 2. import my_equations.txt and click Save. In the Open dialog box: a) Select my_equations. click Import. First. 1. When asked to replace the existing file. Defining a Component Suppression Equation Now use an equation to suppress a component in an assembly. In the FeatureManager design tree.txt. 5. In the dialog box.Parts and Features 8. The feature suppression equation appears in the text file. 103 . click Yes. c) Click Open. select my_equations. 3. right-click Equations and click Edit Equation. 4. 2. warnings about invalid equations appear. Open my_equations. In the Save As dialog box.txt so that you can use the global variable "overall_length" in the component suppression equation.txt. click Export. 6. Click Tools > Equations. If prompted to rebuild. Save the part. Click OK. 1.
Parts and Features
Two equations are imported into the model, including global variable "overall_length". 6. Click OK to close the Equations dialog box. Now add an equation to suppress the second instance of the pin when overall length is less than 40 mm. 7. In the FeatureManager design tree, right-click Equations 8. In the FeatureManager design tree, click pin<2>. "pin<2>" appears in the Add Equation dialog box. and click Add Equation.
9. In the dialog box, complete the equation: "pin<2>" = iif ( "overall length"<40, "suppressed" , "unsuppressed" ) You can type the entire equation or use the following tips to enter various pieces: • To insert global variable "overall length", expand Equations in the FeatureManager design tree and click "overall length"=100. • To insert "suppressed" and "unsuppressed", click the suppress and unsuppress buttons in the dialog box. 10. Click OK. The new equation is added to the Equations dialog box. 11. Click OK. 12. Save the assembly. In the Save Modified Documents dialog box, click Save All . If prompted to rebuild, click Yes. Testing the Component Suppression Equation Now decrease the overall length to 35 mm, which triggers the suppression of the linear pattern feature in the two parts and the suppression of the second instance of the pin in the assembly. 1. In my_equations.txt, for "overall length", change 100 to 35. 2. Save the text file. 3. In part file frontplate_01.sldprt, click Rebuild 4. In part file backplate_01.sldprt, click Rebuild (Standard toolbar). (Standard toolbar).
5. In the assembly, click Rebuild (Standard toolbar). The length of the plates changes to 35 mm and the linear pattern is suppressed. In the assembly, the second instance of the pin is suppressed.
Global Variables
You can configure global variables.
Parts and Features
In a design table, the column header for controlling the value of a global variable uses this syntax: $VALUE@"global_variable_name"@equations In the table body cells, type the value for the global variable. If you leave a cell blank, it inherits the value from the configuration that was active when you opened the design table. Example:
Absorbed Curves
You can now reuse any curve in the FeatureManager design tree in other features. Previously, a curve absorbed into a feature was not available for use in other features.
The PropertyManager and callouts are enhanced. Methods of defining a Variable pitch helix have been expanded. PropertyManager and Callouts The PropertyManager and callouts display more information. • Callouts for Constant pitch cases are now displayed in the graphics area, similar to those that already appear for Variable pitch cases. • The callouts show all parameters, including those that are for information only (shown in gray). • In the PropertyManager, for Variable pitch, the table now shows all parameters, including those that are inactive or for information only (shown in gray).
Parts and Features
Variable Pitch Helix You can define a Variable pitch helix by specifying Height and Revolution. Previously, only Pitch and Revolution and Height and Pitch were available for Variable pitch, and you could use Height and Revolution only when defining a Constant pitch helix. In a part, select a sketch that contains a circle. Click Insert > Curve > Helix/Spiral. In the PropertyManager, under Defined By, select Height and Revolution. Under Parameters, select Variable pitch. Enter values for H and Rev in the table.
More end conditions are available when creating a revolve feature. New end conditions include: • Up To Vertex • Up To Surface • Offset From Surface You can specify separate end conditions for each direction (clockwise and counter-clockwise from the sketch plane). The new end conditions are available when you click the following: • Revolved Boss/Base • Revolved Cut (Features toolbar) or Insert > Boss/Base > Revolve
(Features toolbar) or Insert > Cut > Revolve (Surfaces toolbar) or Insert > Surface > Revolve
• Revolved Surface
In the PropertyManager, under Direction1, in End Condition, select an end condition. Select Direction2 to specify an end condition for the second direction. Example: For this revolved boss, the end condition is Up To Surface for Direction1 and Direction2:
Parts and Features Scale You can configure the X. specify the configurations to which the scale factors apply. 107 . Use one of the following methods: PropertyManager Under Configurations. Design Table The column headers for controlling the X. and Z scale factors. Y. only $X_AXIS@scale_feature_name needs to be defined. Surfaces Surface Extrudes From a 2D or 3D Face You can create extruded surfaces from models that include 2D or 3D faces and knit the extruded surfaces to surrounding features. and Z factors of a scale feature use this syntax: $X_AXIS@scale_feature_name $Y_AXIS@scale_feature_name $Z_AXIS@scale_feature_name Example: For uniform scaling. Y.
Parts and Features Click Insert > Surface > Extrude. • To remove the faces defining the extrude from the model after extruding. In this example. click Delete original faces. or sketch line to define the direction of extrusion . 108 . Both extrudes are created from three contiguous faces: one planar face and two 3D faces. select a plane. To extrude from a 2D face. Select a face: • • • • To extrude from a 3D face. select Knit result . select a 3D face. edge. Select the end condition. you examine a part that has two surface extrudes. press Alt + select the planar face. • To create a single body from the extrude when faces are deleted. 2D face. . Select a plane to define an extrude direction normal to the plane. For 3D faces. • Set other options and click Surface Extrudes from Faces You can create extruded surfaces from models that include 2D or 3D faces and knit the extruded surfaces to surrounding features.
you open the model and examine some components.Parts and Features Opening the Model First. Notice the surface extrude features in the FeatureManager design tree. deleting the original faces. 2.SLDPRT. The two extrusions into and out of the central portion of the model were created by selecting three faces. 109 . Open install_dir\samples\whatsnew\surfaces\multiface-surf-extrude_example. 1. and capping one end of the extrusion.
110 .Parts and Features Viewing the Surface Extrude Options Next. 1. you examine the options used to specify the surface extrude for the model. Click Surface-Extrude2 and click Edit Feature . To view the other faces used to create the surface extrude. select each of them under Faces to Extrude in the PropertyManager. 2. 3. To view one of the 3D faces used to create the surface extrude. select Face<1> under Faces to Extrude in the PropertyManager.
111 . click Front Plane in the PropertyManager. Notice the extrude direction is normal to the front plane. 4. 5. Note the selected options: • Cap end. Knits the resulting extrude to the surface boundary where the original face is deleted. The 3D faces are removed from the model. Close the PropertyManager. Seals the Direction 1 end of the extrude with a translated copy of the selected 3D face.Parts and Features A 3D face defines each end portion of the extude. • Delete original faces . A planar face defines the middle portion of the extrude. To display the plane defining the direction of extrusion. 6. • Knit result . Deletes the faces selected under Faces to Extrude .
you suppress a surface extrude to view the surface before the extrude.6 for Surface-Extrude3. Close the model without saving it. Viewing the Original Surface Before the Extrude Next. The three faces were created by splitting the surfaces with a Split Line feature. Press Ctrl + select the three faces in the middle to view the original surface used to create this model. 112 . ClickSurface-Extrude2 and select Suppress .Parts and Features To examine the other surface extrude created from 3D faces. rotate the model and repeat Steps 1 . 3. 1. 2.
When you cap both ends of an extrude to define an enclosed volume. Click Insert > Surface > Extrude. Bosses and Cuts Recognition Feature recognition is enhanced and new feature types are recognized. Interactive Recognition of Boss and Cut Sweeps FeatureWorks recognizes boss sweep and cut sweep features during interactive recognition when two faces are selected. During interactive recognition of boss sweep features. To seal an end of the extrude. a solid is created automatically. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-BossSweep.x_t. 2. First recognize the upper boss sweep. Boss Sweep 1. You can seal the other end of the extrude by selecting Cap end under Direction 2. under Direction 1 in the PropertyManager.Parts and Features Capping an Extruded Surface You can cap an extruded surface at one end or at both ends. Select End Face1 and End Face 2/Support Face. FeatureWorks Available in SolidWorks Professional and SolidWorks Premium. 113 . recognize the lower boss sweep. select End Face1 and End Face 2/Support Face. Then. 3. select Cap end. Set other options and click .
2. rotate the model. Select End face and then select End Face 1. the Boss-Sweep feature type replaces Base-Sweep. select the face of the cut revolved feature. If necessary. Use interactive recognition and under Feature type. 114 . Cut Sweep 1. Interactive Recognition of Cut Revolve Features FeatureWorks recognizes cut revolve features of the type known as pencil sharpening cuts during interactive recognition. 4. During interactive recognition of cut revolve features.x_t.Parts and Features In the FeatureWorks PropertyManager under Interactive Features. Select End Face 2.x_t. 2. 1. Boss-Sweep recognizes both base and boss sweeps. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-Pencil. 3. select Cut-Sweep. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-CutSweep.
FeatureWorks recognizes one base revolve. 2. Interactive and Automatic Recognition of Bosses and Cuts From Non-Planar Faces FeatureWorks recognizes extrude features (bosses and cuts) that are created from non-planar faces in both interactive and automatic recognition modes. FeatureWorks now recognizes the original boss extrude as well as the four boss extrudes created from the non-planar face. FeatureWorks finds two circular patterns. Verify that Chain revolved faces is cleared.Parts and Features Do not select the top planar face. click Check all filters . Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-NonPlanar_1. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-NonPlanar_2. nine holes. The extrudes must be exact offsets from the supporting face. two chamfers. 115 .x_t. Previously. Use automatic recognition and under Automatic Features. select Extrudes. FeatureWorks maps all of the features automatically. ten cut extrudes.x_t. 2. and 42 fillets. Use automatic recognition and under Automatic Features. FeatureWorks could recognize only the highlighted boss extrude. 1. 1.
chamfers. 2.x_t. 1. select Standard features. In automatic recognition mode. select Standard features. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-CombineFeatures. select Fillets/Chamfers. 2.Parts and Features Original Part Recognized Features Automatic Recognition of Draft Features FeatureWorks recognizes draft features during automatic recognition. Open install_dir\samples\whatsnew\FeatureWorks\FeatureWorks-Draft. or holes of the same geometry into a single feature. Combining Like Features During Automatic Feature Recognition Automatic feature recognition can now combine fillets. Under Automatic Features.x_t. In automatic recognition mode. FeatureWorks maps all of the features automatically. seven fillets with the same radius are recognized as one feature. This reduces the number of features in the FeatureManager design tree and lets you group features together for better readability and smaller file size. 1. For example. Under Automatic Features. 116 . Drafts were previously recognized only in interactive mode. select Drafts and Fillets/Chamfers only.
click FeatureWorks Options (Features toolbar) or Insert > FeatureWorks > Options. Combine Chamfers. To turn off the combine features functionality.Parts and Features Previously. 117 . select or clear Combine Fillets. On the Advanced Controls tab. Now. or Combine Holes. FeatureWorks recognized 36 chamfers in this example. under Automatic Recognition. one chamfer feature appears in the FeatureManager design tree.
To open the Routing Library Manager. click Routing > Routing Tools > Routing Library Manager. 118 . pipes. Click on a tab to open a wizard or tool. It provides access to several existing and new functions.20 Routing This chapter includes the following topics: • • • • • • • • Routing Library Manager Route Along Existing Geometry Weld Gaps Autosize Moving and Rotating a Fitting P&ID Import P&ID Report Routing Options in Isolate Routing Library Manager The Routing Library Manager is a new interface that can be run without launching the SolidWorks application. and equipment. covering. create the geometry of the part and click the Routing Component Wizard tab. Tabs are available for the following functions: • Wizards for creating routing components. To use the wizard. and cable/wire. and electrical component libraries • The Routing File Locations tab for defining library paths • The Administration Tool for managing a database and filtering parts • The Tag Schema Manager for defining the syntax and format of tags in imported schematics The Routing Library Manager provides the following new functionality: • The Routing Component Wizard lets you configure additional types of components such as o-lets and elbows.
Routing • You can use the Tag Schema Manager to define the syntax and format of tags in imported schematics. the name of each field. which allows SolidWorks to interpret the data in P&ID documents. The distance is calculated from the outer surface of the pipe. 119 . using global or joint-specific offset values. • To define when you start a route. This value applies to all weld gaps in the route. select Use weld gaps in the Route Properties PropertyManager and type an offset value in the text box that appears. using a pipe segment or a planar surface or face as a reference. Select Route Along in the PropertyManager and then type the distance in the Modify dialog box. You can define the number of fields in each tag. There are two ways to define the distance: • Use the Smart Dimension tool to define the offset distance. this database is searched for parts that correspond to information available in the schematic and a filtered list appears. You can select a part from this list. You can add part information from the Routing Component Library to the database. You can define weld gaps when you start a route or at any point after you have started it. You can also define the delimiter character. unless the centerline is specified. When you use a P&ID to create a design. Route Along Existing Geometry You can create a route at a defined distance from a surface. and the number of characters in each field. You can also define or change property values and add new properties for parts in the database. • Select the route segment you want to offset and then Ctrl + select the reference object. • The Administration Tool lets you manage the database that is used to select SolidWorks parts when you create a design from an imported P&ID. Weld Gaps You can add weld gaps to routes between pipes and fittings.
You can also right-click a guideline and select Convert Guidelines.Routing • To define after you have created a route. Autosizing also works when editing a pipe. If you drag a fitting onto a pipe. You can also click Weld Gap in the Piping toolbar and select a segment. If a matching size is not located then you are prompted to select a size and configuration. then an attempt is made to obtain the size from a CPoint. See SolidWorks Help: Positioning Parts with the Triad 120 .5%. Type a new value for an individual weld gap in the weld gap label. If the size does not match any available component size. click Tools > Options > Routing and select the option Use triad to position and orient components. right-click a segment and select Weld Gap. To display the triad every time you place a part. Guidelines appear after a part is moved. You can also right-click a part and select Move fitting with triad. See SolidWorks Help: Weld Gaps Autosize When you place a part. +/. or to edit one or more values. it now resizes automatically to match the target equipment or fitting. The size is obtained from the face that the mate reference mates to. After you place the part you are prompted to select a part configuration. the fitting size adjusts to match the diameter of the pipe. or make global changes in the Weld Gap Settings PropertyManager. Click and rotate one of the triad's circles to rotate the part about its axis. Click and drag one of the arrows to move the part. You can use the Auto Route command to convert the guidelines into a route when you have finished positioning the part. Moving and Rotating a Fitting You can use the triad control to rotate or move parts inserted into a route.
If you select Route and direct references then the route and any object it is connected to will be isolated. Symbols and tooltips in the tree identify connections that are missing or have not been successfully created.Routing P&ID Import You can insert inline components into a pipe route after creating it from imported P&ID data. click Report in the Piping and Instrumentation pane. Routing guidelines display without having to first place tees. inline fittings such as valves. Routing Options in Isolate You now have routing-specific actions available in the Isolate command. To generate the report. As an example. Click Tree to see the piping system tree. such as from a Solution Partner. Click Text to see a printable report. Make your selection in the Isolate dialog box. P&ID Report You can generate reports that shows missing components or incomplete connections in a 3D model created from imported P&ID data. Right-click the piping assembly in the FeatureManager and select Isolate. if you select Route only then the route will be isolated. The P&ID Validation Report dialog box displays. the Isolate command is used to isolate a route. You can convert these guidelines to routes as required. SolidWorks identifies required components such as tees and reducers that are not defined in the document and lets you select them from a list. and reducers. 121 . Other options are: • Route and secondary references • Route bounding box • Route segments bounding box In the image below.
Routing 122 .
Gauge Tables You can use gauge tables with the Convert to Sheet Metal tool. In previous releases. and bend deduction methods. In the PropertyManager. in Bend Allowance Type. bend allowance. With bend calculation tables. bend table. Convert to Sheet Metal The Convert to Sheet Metal tool is enhanced. The sheet metal parameters (material thickness. under Sheet Metal Gauges. select Bend Calculation and set the options. under Bend Allowance. and bend calculation method) use the values stored in the gauge table unless you override them. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal. You can specify the file locations for gauge tables in Tools > Options > System Options > File Locations. Click any sheet metal tool where you can select a calculation method for the developed length. select Use gauge table and select a gauge table. In Show folders for. gauge table. select Sheet Metal Gauge Table. 123 . See SolidWorks Help: Bend Calculation Tables. you can define different angular ranges. and calculate the developed length of the part.21 Sheet Metal This chapter includes the following topics: • • • • • • • • Bend Calculation Tables Convert to Sheet Metal Flat Patterns K-Factor in Configurations Mapping Bend Directions When Exporting to DXF/DWG Files Mirroring Edge Flanges and Miter Flanges Sheet Metal Properties Patterns of Edge Flanges and Tab Features Bend Calculation Tables You can calculate the developed length of sheet metal parts using bend calculation tables. you calculated the developed length with K-Factor. bend radius. In the PropertyManager. assign equations to those ranges.
and underlap. See SolidWorks Help: Converting a Solid Part to a Sheet Metal Part. Additionally. You want to keep the solid body to derive another sheet metal body from the same solid body. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal. 124 . Use Convert to Sheet Metal to create the first sheet metal body. Machine with a sheet metal enclosure. Keep or Consume Solid Bodies When using the Convert to Sheet Metal tool. under Corner Defaults. select a rip type and set the options. You can also control individual rip settings by clicking a rip callout in the graphics area. Keep body is selected. In the PropertyManager. you can keep the solid body to use with multiple Convert to Sheet Metal features or specify that the entire body be consumed by the tool. overlap. Available rip types are open butt. you can set the Default overlap ratio for all rips and show or hide callouts in the graphics area.Sheet Metal Rip Types You can define parameters for rip edges and rip sketches created with the Convert to Sheet Metal tool.
Bend Allowance You can select the bend allowance method for the developed length calculation of the part. If you flatten a part that was built prior to SolidWorks 2011. In the FeatureManager design tree. In the PropertyManager. Set the K-Factor values for each configuration. In previous releases. In the PropertyManager. In the Flat-Pattern PropertyManager. select a bend allowance. right-click Sheet-Metal1 and click Configure feature. In the PropertyManager. Rip Edges found. In the FeatureManager design tree. In the dialog box. right-click Flat-Pattern and click Edit Feature. select Recreate flat-pattern.Sheet Metal Use Convert to Sheet Metal to create the second sheet metal body. Callouts You can show or hide callouts for Bend Edges. Keep body is cleared so the solid body is consumed. 125 . Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal. you completed the Convert to Sheet Metal command and then changed the bend allowance in a separate step. under Sheet Metal Parameters. select the variable that corresponds to K-Factor. select or clear Keep body. Flat Patterns The software uses a new calculation method to flatten sheet metal parts. in Sheet-Metal1. K-Factor in Configurations When you use K-Factor as the bend allowance type in sheet metal parts. and Rip Sketches. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal. select or clear Show callouts. under Custom Bend Allowance. under Parameters. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal. you can specify different values for the K-Factor in different configurations. you can apply the new calculation method.
you can map the different bend line directions to separate layers when you export the drawing.dxf or . See Exporting Bend Line Directions on page 79.dwg file. Mirroring Edge Flanges and Miter Flanges You can mirror edge flanges that consist of several flanges attached to different edges. The following properties are calculated in sheet metal parts: Bounding Box Length Bounding Box Width Bounding Box Area Longest side of the bounding box Shortest side of the bounding box Bounding box length x Bounding box width 126 .dxf or . the smallest rectangle in which the flat pattern can fit. When exporting a sheet metal part as a . You can also mirror modified miter flanges where the flanges are shortened so the geometry does not overlap.dwg files. in sheet metal drawings with up and down bend directions. For example. The bounding box is represented by a sketch when you flatten the sheet metal part and is located in the FeatureManager design tree under Flat-Pattern . you can export the bounding box and assign the bounding box to a specific layer.Sheet Metal Mapping Bend Directions When Exporting to DXF/DWG Files You can map bend line directions to specific layers when you export sheet metal models as . Some of the properties that are calculated are based on the bounding box. Part with multiple edge flanges Mirrored edge flanges Sheet Metal Properties New properties specific to sheet metal parts are calculated and displayed in the Cut-List Properties dialog box. See . You can set a grain direction to determine the smallest rectangle that aligns with the grain direction to fit the flat pattern.
expand Cut list . You cannot pattern tab features with attached jogs or sketched bends. Multibody is not supported. See SolidWorks Help: Sheet Metal Properties and Setting the Grain Direction for Bounding Boxes. Patterns of Edge Flanges and Tab Features You can pattern edge flanges and tab features that have additional sheet metal features attached. sketch driven. in the FeatureManager design tree. 127 . The properties are updated whenever you update the cut list or flatten the part. circular.Sheet Metal Bounding Box Area-Blank Cutting Length-Outer Cutting Length-Inner Cut Outs Bends Area of the flat pattern excluding the through cut-outs Outer perimeter of the flat pattern (blank) which is used for calculating the machine's cutting time Sum of the perimeters of internal loops or cut-outs Closed cut outs (through holes) on the flat pattern which are used for calculating the machine's idle time Number of bends in the part To view these properties. Right-click a Cut-List-Item and click Properties. Pattern tools include linear. curve driven. and table driven patterns. The patterns are supported for the same sheet metal body only.
This option is available for static and nonlinear studies. 4. 3. Nonlinear. select Static. no stresses develop normal to the section plane. Enhancements marked with (Professional) are available in SolidWorks Simulation Professional and SolidWorks Simulation Premium. set options and click Types of 2D Simplification You can select from four types of 2D simplification options based on the geometry. nonlinear. select Use 2D Simplification and click . fixtures. loads. This chapter includes the following topics: • • • • • • • • • New Simulation Studies Interface Shells Beams Connectors Contact Mesh Nonlinear Studies Results New Simulation Studies New 2D Simplification Study You can simplify certain 3D models by simulating them in 2D. 2. You can save analysis time by using the 2D simplification option for applicable models. . material properties. In the 2D Simplification PropertyManager. Under Type. Plane stress Simulates thin geometries with no forces acting normal to the section plane. pressure vessel design. or Thermal study. To create a 2D simplification study: 1. 2D simplification is available for static. 2D models require fewer mesh elements and simpler contact conditions compared to their 3D counterparts.22 Simulation SolidWorks Simulation is available in SolidWorks Premium. 128 . For the plane stress assumption. Enhancements marked with (Premium) are available only in SolidWorks Simulation Premium. Under Options. and contact conditions. Click New Study (Simulation CommandManager). and thermal studies.
The figure shows an example of a long block held at a uniform temperature and suddenly exposed to a convection environment. For the plane strain assumption. This option is available only for thermal studies. turning a wrench while tightening a bolt. Extruded Simulates geometries with constant thermal loads along the extrusion direction. Plane strain Simulates thick geometries that extend a long distance on either side of the section plane with no forces acting normal to the section plane. Other examples include a tunnel under pressure and sheet rolling. Other examples include thin plates under pressure. This example shows a dam under water pressure. Plane strain problems are less common than plane stress problems. and snap fit of plastic clips. This option is not available for thermal studies.Simulation This examples shows a bracket under distributed load. no strains develop normal to the section plane. 129 .
130 . 2D Section You create 2D sections from 3D geometries. material properties. loads. or use planar surfaces and 2D closed sketches on the section plane to define the bodies required for analysis. use the top plane to extract the 2D model from the 3D geometry. 3D geometry Modeled section Other examples include vessels under external or internal pressure and many problems encountered in turbine construction.Simulation Axisymmetric Simulates geometries. Sectioning You can create bodies in 2D by splitting solids using a section plane. Solids For the plane stress example of a wrench tightening the bolt shown below. and fixtures that are symmetric about an axis. This example shows a nonlinear contact analysis of an o-ring. You use the 2D Simplification PropertyManager to create the section.
The example shows a three-point bend test on a plate under plane strain with the surface bodies created on the section plane.Simulation 3D model 2D section For the axisymmetric example of a bolt-nut connection. select any plane that sections the solid and the axis of revolution. The head of the bolt and the helical pattern of the threads are not modeled (helical threads are not axisymmetric). 3D model 2D section Using planar surfaces You can create planar surface bodies or 2D closed sketches on the section plane to create 2D sections. 131 .
loads. the applied loads are given in total values (not per radian). For plane stress or plane strain assumptions. Viewing Results You can view the results of a 2D simplification analysis in 2D or 3D. the applied loads are based on a thickness unit you specify. For plane stress and plane strain models. 2D Results Plot 3D Results Plot 132 . Notes on 2D 2D simplification studies: Simplification • For plane stress or plane strain assumptions. For the axisymmetric assumption. • You need to apply fixtures. The results are reported per the thickness unit you specify. the results are the same for all cross sections parallel to the section plane.Simulation Running the Study and Viewing Results Setting up a Setting up a 2D study is similar to setting up a 3D study. and contact conditions on edges rather than faces. • For axisymmetric models. you cannot apply loads Study and fixtures in a direction normal to the section plane. you cannot apply them along the circumferential direction.
the threads are modeled as separate rings of material and not as a continuous helix (this is a simplification. 2D Results Plot 3D Results Plot (rotated 200°) 2D Simplification Analysis of a Bolt-Nut Connection You perform an axisymmetric analysis on a bolt-and-nut assembly to plot the stress results on the threads. By performing a 2D simplification analysis. The bolt head and the clamped members are not modeled. To see the model. open install_dir\samples\whatsnew\2D_Simplification\bolt_nut. To apply 2D simplification. 133 .sldasm. you save time because 2D models require fewer mesh elements and simpler contact conditions compared to 3D models. Creating the 2D Simplification Study You define a 2D simplification study from the 3D model and perform a nonlinear static study. Results are reported in total values (not per radian). you still need to use a 3D model. the results are the same for all cross sections about the axis of revolution. To model the tightening of the joint or sliding of the bolt.Simulation For the axisymmetric assumption. as helical threads are not axisymmetric).
Under Solver. a) For Faces. 7. Click Apply and Close. In the PropertyManager. 2. Under Options. 3. Click . Click . 134 . click Nonlinear . 4. Right-click Connections do the following: and select Contact Set . select the 2D body of the bolt. This is the axis about which the geometry. loads. under Name. The elastic-plastic material properties of Alloy Steel are assigned to the bolt and the nut. select Large strain option. Click New Study (Simulation CommandManager). In the 2D Simplification PropertyManager. for Model Type.von Mises. Edges. For Section plane. 1. In the Nonlinear-Static dialog box. In the PropertyManager. select Plane1 from the FeatureManager design tree. In the Material dialog box. 4. select Direct Sparse and click OK. Right click Parts and select Apply Material to All . 5. 6. select Plasticity. select Axi-symmetric. select Use 2D Simplification. In the Simulation study tree. under Type. 2. 3. Vertices for Set 1 . right-click the bolted connection study folder and select Properties. 6. Applying Material Properties and Contact Sets You define the material properties and contact sets. Under Type. 8. 5.Simulation 1. You select the Large strain option to model plasticity in the bolted connection. 9. select Axis1 from the FeatureManager design tree. 7. For Axis of symmetry. under Geometry nonlinearity options. and fixtures are symmetric. type bolted connection.
c) Under Advanced. . select the 2D body of the nut. for Straight Edges for Fixture bolt and the top edge of the nut as shown. In the PropertyManager. 1. Right-click Fixtures and select Roller/Slider. You then run the bolted connection study. Running the Analysis You apply load to the top edge of the bolt shank and prevent the nut from moving vertically. select the edge of the 2. select Surface to surface. 8. Click .Simulation b) For Faces for Set 2 . No penetration contact without friction is applied between the touching thread regions of the bolt and the nut. 135 .
a) Under Force/Torque. .Simulation 3. select English (IPS). select Plane1. (Simulation CommandManager). In the PropertyManager. for Faces and Shell Edges for Normal Force the edge shown by arrows in the figure. c) For Face. select Along Plane Dir 2 This is the total force acting on the circular face of the bolt shank. and type 3000. the results are the same for any cross section about the axis of revolution. For an axisymmetric analysis. Plane. 136 . Edge. . f) Click 5. Click Run . Viewing the Results You can view the results of a 2D analysis in 2D or 3D. Right-click External Loads and select Force 4. d) For Unit . define the load: . select b) Select Selected direction. from the FeatureManager design e) Under Force. Axis for Direction tree.
a response is read from a design spectrum based on the modal frequency and a given damping ratio. 137 . The values are lower for the subsequent threads. New Response Spectrum Analysis Study (Premium) The new Response Spectrum Analysis study estimates the peak values of your model's response based on a design spectrum specified as a base excitation. 3. You can change the angle in the Stress Plot PropertyManager under Advanced Options. Right-click Stress (-von Mises-) and select Show as 3D plot. the results of a modal analysis are used in terms of a known spectrum to calculate displacements and stresses in the model. In the Simulation study tree. Double-click Stress (-von Mises-) to display the plot. open the Results folder. All modal responses are then combined to provide an estimate of the maximum response of the structure.Simulation 1. Among the contacting threads. the first engaged thread shows a high stress value. you view the results in 2D. 2. In a response spectrum analysis. The result shows plastic deformation on the model. By default. For each mode. By default. the 2D section revolves by 330°.
Takes the absolute value of the response for the mode that exhibits the largest response and adds it to the SRSS response of the remaining modes. wind loads. select Response Spectrum Analysis . Mode Combination Techniques The mode combination options for evaluating the maximum response are: Absolute Sum Assumes that the maximum modal responses occur at the same time for all modes. 138 b) Under Options. jet engine thrust or rocket motor vibrations. a) Under Type. ocean wave loads. equals the maximum absolute value of the relative displacement time history response for each SDOF oscillator. This method is based on random vibration theories. .Simulation Relative displacement response spectrum for a particular damping ratio ξ1. You can use a response spectrum analysis rather than a time history analysis to estimate the response of structures to random or time-dependent loading environments such as earthquakes. It is the most conservative among the modal combination methods. It takes into account the cross-correlation factors between two modes and the modal damping ratios. Natural circular frequency of vibration for each SDOF oscillator. select Linear Dynamic . Click Simulation > Study. Square Root Sum of Squares (SRSS) Complete Quadratic Combination (CQC) Naval Research Laboratory (NRL) Creating a Response Spectrum Analysis Study 1. Estimates the peak response by the square root of the sum of the maximum modal responses squared.
1984). To see the model. 8. You use the design response spectra for horizontal components of ground motion recommended by the Applied Technology Council (ATC-3-06. For more information on Response Spectrum Analysis studies. see Simulation Help: Response Spectrum Analysis. Right-click Result Options and select Edit/Define. You can view the model's maximum response values (stresses. You apply the design response spectrum in one horizontal direction and view the results. or acceleration response spectrum. Define the frequency and response spectrum options of the study. 6. Beams and composite shells are not supported in a response spectrum study. Define material for each body. 3. To define fixtures. open install_dir\samples\whatsnew\Simulation\circuit_board. you can apply multiple response spectra definitions for uniform or selected base excitations. define contact sets and any connectors. velocity. displacements. Under Connections . Right-click Results and select the desired options. 139 . In a response spectrum analysis study. Select the modal combination method to estimate the maximum response. right-click the study icon and click Properties. 9. accelerations) based on the modal combination technique you selected in Step 2. spring and edge welds connector are supported. Tentative Provisions. Response Spectrum Analysis of a Circuit Board You perform a response spectrum analysis on a circuit board assembly. This defines the base excitation (uniform or selected) in terms of a given displacement. 5. In the Simulation study tree. Right-click External Loads and select Uniform Base Excitation or Selected Base Excitation. Select the Naval Research Laboratory mode combination method to evaluate the model's expected maximum response.Simulation 2. velocities. 7. the total response is calculated by the square root of the sum of the squares of the individual responses. 4.sldasm. In case of multiple response spectra definitions. right-click Fixtures and select from the options. Mesh the model and run the study. Bonded contact.
The response spectrum analysis is based on the model's first 30 frequencies for the calculation of the maximum response. select Naval Research Laboratory. contact and mesh definitions from the Frequency study are copied to the new Response Spectrum study. 1. under Type. On the Response Spectrum Options tab. Setting the Study's Properties You select the mode combination method (Naval Research Laboratory) to evaluate the estimated maximum response. 1. and select Properties. Right-click External Loads . You copy the frequency study to the new response spectrum study. and select Uniform Base Excitation. Tentative Provisions. 3. 3.Simulation The assembly document includes a frequency study with material. The design spectrum is recommended by the Applied Technology Council (ATC-3-06. select Acceleration. 140 . To modify the number of frequencies. type Response Spectrum. right-click the response spectrum study icon. fixture. right-click the frequency study icon. Under Linear dynamic study type. Under Acceleration: a) For Unit . 2. 2. Applying Base Excitation You apply a horizontal base excitation in the global X direction defined in terms of an acceleration design response spectrum. The program creates the new Response Spectrum study. Click OK. Click OK. Right-click the response spectrum study's icon and select Properties. In the PropertyManager. 1984). select g. In the Simulation study tree. Under Study Name. and select Copy to New Dynamic Study. fixture and mesh definitions. All material. Set the desired value for Number of frequencies. Creating the Response Spectrum Analysis Study You create a response spectrum analysis study from the existing frequency study and set the study's properties. select Response Spectrum Analysis 4. 2. 3. 1.
cwcur. A plot of the maximum resultant displacement appears. select Hz. 3. Under Variation with Frequency: a) Click Curve. b) In the Function Curves PropertyManager.Simulation b) Click Along Plane Dir 1 . 4. Click Run (Simulation CommandManager). 2. 1. 5. In the Simulation study tree. 6. b) Click Edit. velocity. load the curve library install_dir\Simulation\CWLang\English\response spectra curves. c) Expand Frequency curve and select ATC-3-06-Acceleration (g). e) Click OK twice. d) For Units. 141 . Running the Analysis and Viewing Results After you run the analysis. you can view response plots for the maximum acceleration. right-click Results and select Define Displacement Plot. displacement. Plot the resultant acceleration plot. This excitation is applied to all locations restrained in the global X direction. In the Frequency curve PropertyManager: a) Click Get curve to load the predefined acceleration response spectrum curve. and stress quantities. and type 1. Click .
Absolute Sum. To create sub-folders. You can use a different modal combination method (SRSS.Simulation Note that the maximum displacement and acceleration values occur at different locations of the circuit board. for example: • You can assign the same material properties to the bodies in a sub-folder under the Parts folder. right-click a folder in the Simulation study tree and select Create New Folder. • Cut lists for beams and sheet metal bodies appear in the Simulation study tree. Interface Organization of Bodies Enhancements to the Simulation study tree let you apply simulation features more easily. 142 . • You can drag existing pressure loads to a sub-folder under the External Loads folder. • You can organize bodies into folders in the Simulation study tree. You can then drag entities into the new folder. Filtering the Simulation Study Tree You can use the new Simulation-specific filter tool to filter the Simulation study tree. or CQC) and compare the results. Type text to filter by in the filter tool at the top of the Simulation study tree. All options under the parent folder are available for a newly created sub-folder.
• Recently used searches are stored for usage in other documents.Simulation • Filter by text-based names such as Pressure-3 or properties such as shell thickness or fixed geometry. 143 .
you can type 50*cos(pi/6) for Force in the Force/Torque PropertyManager. and select View Simulation Symbols. such as loads. • When you change a body's material in a Simulation study. the material's appearance updates to the new material when viewing the Simulation study. or bottom faces of the shell. To toggle the display of Simulation symbols. • To reduce the parametric value of density of 7800 kg/m^3 by one-third. Display of Simulation Symbols While editing a Simulation study. The Shell Definition PropertyManager has the following options: 144 . For a list of allowed expressions. Display Enhancements for Simulation Studies Enhancements to the display of parts and assemblies include: • A body that is excluded from an analysis is hidden in the Simulation study. middle. Expressions in Input Fields You can now type expressions in fields that allow numerical inputs. see SolidWorks Help: List of Operators and Functions. you can type an offset value. you can type 7800/3 for User defined value in the Add Parameters dialog box. fixtures.Simulation • Use Filter Graphics View to show only filtered items in the graphics area. Shells Offsets for Shells You can align the mesh to the top. click View > Simulation Symbols or click Hide/Show Items (Heads-Up View toolbar). Examples: • To use a component of a resultant force of 50N oriented at a 30° angle to the selected direction. you can toggle the display of all Simulation-related symbols. and connectors. To align the mesh to a reference surface.
you can create the two surfaces using the Bottom surface option.Simulation Middle surface Top surface Bottom surface Specify ratio Aligns the mesh with the middle surface of the shell Aligns the mesh with the top surface of the shell Aligns the mesh with the bottom surface of the shell Aligns the mesh to a reference surface defined by an offset value that is a fraction of the total thickness. Ply Orientation in Composites (Premium) The options for ply angles of a composite are enhanced. The white arrow shows the ply direction. A striped texture on the composite surface body highlights the ply angle of the selected ply. to model adjacent shells with differing thicknesses such that their bottom faces coincide. The figure shows the texture for a 45° ply angle. under Type. 145 . in the Shell Definition PropertyManager. To access the options. The figure shows the meaning of the positive and negative offset values. For example. select Composite. you can do the following: • Select a row in the Composite shell plies table. Under Composite Options.
The Ply surface mapping technique that uses the UV coordinates shows curved Orientation stripes on the shell.txt formats. For example. Inappropriate The figure shows a face created using the surface fill operation. You can then reload the stack information for future use. The surface mapping creates inconsistent across Faces orientation for a 45º ply angle across the faces. you can now save the stack data in .csv or . The first ply angle is always absolute. if ply angle 1 is 45° and the absolute value of ply angle 2 is 60°. Surface mapping Planar mapping using XY plane Inconsistent The figure shows consistent ply orientation across multiple faces with Orientation the planar mapping option.Simulation • Select Ply angles relative to ply 1. Ply angles are defined relative to its first ply. then the relative value of ply angle 2 with respect to ply angle 1 is 15°. • Use the Planar Mapping option to define a common zero degree ply angle reference for a group of planar shell faces or if you encounter problems with the default Surface Mapping option. You can use the planar mapping technique by selecting the XY plane and projecting the desired ply orientation. Planar mapping using XZ plane Surface mapping Composite Stack Information (Premium) When defining a composite shell. 146 .
Centered Applies the force or moment you specify at the center of the beam. You can specify table driven force values at different locations of the beam. under Type select Composite and set the different Composite Options. The source entity for the bonded contact set has to be a beam joint. or sheet metal body is improved. Select one of the following options: Total Load Distributes the total force or moment you specify along the length of the Distribution beam. select Nonuniform Distribution. or you can select from predefined load distributions such as In the Force/Torque PropertyManager.Simulation As a best practice. In the Shell Definition PropertyManager. Click Load stack from file to load a saved composite stack file. 2. Loads Load decrease on either side of the center according to the selected distribution. Non-uniform and Partial Loading of Beams You can now define non-uniform loads or loads that are defined on a part of the beam. A finer mesh is created at the area of the beam joint. The software imprints the beam's actual cross-section on the target solid face or surface to create an accurate bond joint. or elliptical. you should edit the stack information in the Shell Definition PropertyManager. Editing the file in an external editor is not recommended. Beams Improved Bonding for Beam Joints The bond connection of a beam to a solid. To save or load the composite stack information: 1. No loads are applied at the ends of the beam. Bonded contact between beam joint and shell Simulation imprints the cross-sectional area of the beam on the shell face. shell. and creates finer mesh at the imprinted area. 147 . Click Save stack to file. triangular. Distribution and are defined per unit length. 3. The shape of the distribution can be parabolic. No loads are applied at the ends of the beam.
Tapered Beams You can now treat tapered geometries as beams with varying cross-sectional sizes along their length. Tapered geometries should have the same cross-sectional profile along their length to be treated as beams. You can select between linear and cubic interpolation schemes for intermediate locations not specified in the table. In the Simulation study tree. The tapered beam is represented by a straight line (neutral axis) connecting the two end joints. The figure shows a tapered I-section beam with cross sectional size that decreases linearly along the direction shown. You can save the table as a .txt or . where the beam is divided into a number of tapered beam elements represented by cylinders. if the solid body has a taper along its length. The lower image shows the mesh. right-click a solid body and select Treat as Beam.Simulation Table Driven Load Distribution Applies the force values at specific locations along the length of the beam. Each element 148 . You specify the locations either as percentages or distances from one end of the beam. A tapered beam icon appears in the study tree.csv file for future use.
but with varying sizes. In the PropertyManager. To use the European standard: 1. the solid body should maintain its cross-sectional profile along its axis. select EN 1993-1-8 : 2002 Standard. Right-click Connections and select Edge Weld. under Weld Sizing. Set the properties of the weld connector: Material of weaker joined part Select the material of the attached metal component with the lesser tensile strength value. If a solid body does not qualify as a tapered beam. 2. The mesh and the results give you a visual indication of the taper along the beam length.Simulation consists of two nodes having cross-sectional areas of the same shape but different sizes.Eurocode 3 for edge weld calculations. To qualify as a tapered beam. 149 . You can also select Custom to define the tensile strength value of the weld. This example shows a body with a twist along its length that does not strictly qualify as a tapered beam. a warning recommends that you do not treat the body as a tapered beam. Connectors European Standard for Edge Welds (Professional) You can now use the European standard EN1993-1-8:2002.
Eurocode 3 Standard. Right-click the Simulation study's icon and select Properties. 150 .1. select Automatic. For correlation factors of different types of joints. Table 4. Estimated weld size Type the value of the weld size. the value is populated automatically. under Mesh Parameters. For other selections. In the Mesh Control PropertyManager.Simulation Ultimate Tensile Strength Type the value of the tensile strength for the custom weld material. Contact Automatic Option for Simplified Bonding The solver now selects the surface-based or node-based bonding contact based on certain performance criteria. • You can control the mesh size of beams. • The default mesher is now the curvature-based mesher. For correlation factors of different material grades. • The curvature-based mesher supports the option Remesh failed parts with incompatible mesh. Buckling. • Mesh diagnostics is incorporated in the Mesh Advisor. Frequency. the solver switches to node-to-surface bonding automatically. Edge weld calculations determine whether this size provides adequate resistance to the applied loads. select Number of elements or Element Size. see EN1993-1-8:200 . see EN1993-1-8:200 . Table 2. The new option for automatic bonding contact is available for Static. Correlation Factor Type the correlation factor used to determine whether the resistance of the weld is sufficient. Partial Safety Factor Type the partial safety factor used to determine whether the resistance of the weld is sufficient. Specify the total number of elements or the element size. Under Incompatible bonding options.Eurocode 3 Standard. and Linear Dynamic Studies. Mesh Mesh Enhancements • Solid and shell meshing performance has been improved because SolidWorks Simulation now takes advantage of your computer's multi-processors for meshing surfaces. If the default surface-to-surface bonding slows down the solution considerably. which guides you to resolve meshing issues like meshing failed bodies.1.
The new method avoids numerical convergence difficulties encountered by the penalty method and improves accuracy and speed for most nonlinear studies. select First. Second. The performance improvement is more prominent (up to 20% gain in analysis time) for nonlinear studies with many restraint definitions and higher mesh densities. Heat Power and Heat Energy You can more easily and accurately find out the heat power generated or dissipated through selected entities for steady-state and transient thermal studies. the corresponding connector or beam is highlighted in the graphics area and Simulation study tree. or Third Principal Strain in Component . In the Strain Plot PropertyManager. Interaction with List Result Tables When you highlight a row in the Pin/Bolt/Bearing or List Beam Forces dialog box. 151 .Simulation Nonlinear Studies Improved Accuracy for Nonlinear fixtures (Premium) An exact method rather than an approximate penalty method is used to apply fixtures in nonlinear studies. Right-click Results and select List Heat Power/Energy. Results Nonlinear Plots (Premium) You can plot elemental principal strains for nonlinear studies. Heat energy is available for transient thermal studies only and for a specified time interval.
under Annotations.Simulation Probe Callout Enhancements Probe callouts contain more information and can be relocated in the graphics area. 152 . In the Probe Result PropertyManager. Z Location are cleared. Show Value is selected and Show Node/Element Number and Show X. In this example of a thermal study. select or clear the results-specific annotations. Y. • You can move probe results to different locations in the graphics area. coordinates. Before After • You can customize the callouts to display annotations such as ID numbers (node numbers). and results-specific information like von Mises stress or temperature.
if you select Model Max for Criterion . click Simulation > Options. select Simulation Data. You can define these sensors to track values across all steps. drop test. select one of the following: Across All Steps Tracks the Simulation data value across all steps for the entire model or for the selected entities and reports a single value. In the Sensor PropertyManager. or at a specific mode. click Report and select a report style from Report formats. On the Default Options tab. at a specific plot step. Specifies the mode number at which the sensor tracks the result. for Step Criterion. select or clear Report sections. and transient thermal studies. For example. Image Capture Enhancements You can include annotations for fixtures and loads when capturing the image for a report. To select specific sections for a report type. the solution step is listed. linear dynamics. the sensor reports the maximum value in the model across all steps.Simulation • When probing an envelope plot for a transient study. for Sensor Type . You can control the number of plot steps and the step interval using the Result Options folder in the Simulation study tree. 153 . At Specific Plot Step Tracks the Simulation data value at the specified plot step based on the plot number you specify. Sensors for Transient Studies You can now define sensors to track the results of nonlinear. • Reports are available for all study types. At Specific Mode Shape This option is available only for the frequency and buckling sensors. Under Properties. After selecting a report format. Study Reports Report Styles and Sections • Different report styles are available and the included sections are customized to the study type.
and select Publish. • To add the image to a report. the Curve Data graph is included with the material properties. In this example. You can move the callouts to different positions. add the image to the report's folder.Simulation • After creating a report. Graphs for Material Properties Related graphs are included along with material properties. select Annotations and select or clear features under Feature Name. right-click the report in the Report folder. in the Simulation study tree. right-click Report and select Include Image. 154 . Click to add the image to the Images folder. To display the annotations. Set the parameters.
155 .Simulation SimulationXpress Study Reports SimulationXpress study reports are generated as Microsoft Word documents.
You can then specify the number of floors for the structure and the distance between each floor. Grid system sketch Click Grid System System. Multiple users can use the grid system and work from the same baseline. Grid system with weldments applied (Features toolbar) or Insert > Reference Geometry > Grid 156 .23 Sketching This chapter includes the following topics: • Grid System Grid System You can use the Grid System tool to lay out a grid system for large structures. Balloons are attached to the grid items to help with orientation. When you use the Grid System tool. You can create a grid to help specify the location of key elements in structures. The grid system is also helpful when you work with multiple users who use different third-party applications to make grids. The sketch is replicated for every floor in the structure. you create a sketch to represent the grid. The grid system is useful when creating welded structures.
To reduce clutter. To access the display options.Sketching See SolidWorks Help: Creating a Grid System. Display options are available to help you visualize the grid structure and to ensure correct grid inferencing. you can hide and show the geometry. in the FeatureManager design tree. select an item and click a display option. such as Normal To . The graphics area can appear cluttered when the grid system creates a lot of geometry or if you create multiple grid systems. In the View Grid Components dialog box. 157 . right-click Grid System and click View Grid Components.
This is done by linking your custom material to a material with similar characteristics in the default SolidWorks Materials database. Click OK. Australia. Only materials with a link to the Sustainability database are listed. click Select. 5. 158 . In the Material dialog box.24 Sustainability This chapter includes the following topics: • • New Supported Regions Sustainability Link for Custom Material New Supported Regions SolidWorks Sustainability and SustainabilityXpress support these additional regions: South America. In the Properties tab. Click Apply and Close. The analysis is then performed using the Sustainability characteristics of the SolidWorks material. Sustainability Link for Custom Material You can perform a sustainability analysis using custom materials. and India. 4. select your custom material. In the Match Sustainability Information dialog box. select the material that is most similar to your custom material. in a custom materials library. 3. To link your custom material to a similar material: 1. You can specify the regions as Manufacturing or Transportation and Use regions. 2. in Material properties.
159 . This chapter includes the following topics: • • Symmetry Check Utility Find/Modify/Suppress Feature Selection Symmetry Check Utility You can use the Symmetry Check Utility to check component symmetry about a selected plane. and to identify symmetric and asymmetric components in an assembly. To run a part or assembly symmetry check with respect to a plane.25 SolidWorks Utilities Available in SolidWorks Professional and SolidWorks Premium. select the plane in the FeatureManager design tree and click Symmetry Check (Tools toolbar).
To find. components that are symmetric with respect to the selected plane appear blue and asymmetric components are pink. modify.SolidWorks Utilities By default. For more information. see SolidWorks Help: Find/Modify/Suppress Feature Selection. see SolidWorks Help: Symmetry Check Utility. For more information. or suppress part features based on properties of a selected feature. select the feature and click Find/Modify Features (Tools toolbar). 160 . after running a symmetry check on an assembly. Find/Modify/Suppress Feature Selection You can select a part feature to match when using the Find/Modify/Suppress utility.
3. Select the required GB gears and clear the unnecessary ones. click GB. for example. To set SolidWorks to search the Toolbox folder for referenced Toolbox components: 1. Power Transmission. This chapter includes the following topics: • • Opening Models with Referenced Toolbox Components Gears in the GB Standard Opening Models with Referenced Toolbox Components When you open an assembly. From the Select Hardware page. even if the assembly is created from a separate Toolbox installation. from a Hole Wizard/Toolbox system option. 4. click All Programs > SolidWorks version > SolidWorks Tools > Toolbox Settings. 3. 2. 2. If you clear the system option. SolidWorks automatically finds references to Toolbox components in your Toolbox folder. Click Hole Wizard/Toolbox. Click Options (Standard toolbar). 161 . Gears in the GB Standard Toolbox administrators can include GB standards gears in Toolbox. and Gears. Select Make this folder the default search location for Toolbox components. from outside your company. You can set this behavior.26 Toolbox Available in SolidWorks Professional and SolidWorks Premium. which is applied to all new SolidWorks installations by default. To include GB standard gears in Toolbox: 1. Close Toolbox Settings. SolidWorks does not automatically find Toolbox component references in the Toolbox folder. From the Windows Start menu.
To exclude Cut-List-Item folders from cut lists: • Right-click a folder in the FeatureManager design tree and click Exclude from cut list. and multibody parts. • Use the Cut-List Properties dialog box to select Exclude from cut list on the Cut List Summary and Cut List Table tabs. • Use the Cut-List Properties dialog box to drag and drop folders on the Cut List Summary or Cut List Table tabs. The reordering propagates to the cut lists in the part and drawing. You can also exclude Cut-List-Item folders from cut lists. 162 .27 Weldments This chapter includes the following topics: • • • Cut Lists Weld Beads Weld Support in Drawings Cut Lists Cut List Icons New icons appear in the FeatureManager design tree under Cut list. To reorder the Cut-List-Item folders: • Drag and drop folders in the FeatureManager design tree. Weld Beads You can add simplified weld beads to weldment parts and assemblies. you can apply a customized order to the cut list. See SolidWorks Help: Excluding Folders from Cut Lists. The icons are based on the type of body in the model: • Sheet Metal • Weldment or structural members • Other bodies Reordering and Excluding Cut List Items You can reorder Cut-List-Item folders. Because the order of the Cut-List-Item folders drives the cut list entries. You should finish modeling the part before modifying the cut list items. You may lose changes to the cut list if you change the geometry after modifying the cut list.
163 . Weld Bead Display Weld beads are displayed as graphical representations in models. Weld Beads in Assemblies Weld Beads You can add simplified weld beads to assemblies. In an assembly.Weldments Benefits of simplified weld beads: • • • • • • • • Uniform implementation in parts and assemblies Compatiblity with all types of geometry. you can set properties for Weld Sub Folders. click Insert > Assembly Feature > Weld Bead. including bodies with gaps Lightweight. The weld beads are lightweight and do not affect performance. including: • • • • • Weld material Weld process Weld mass per unit length Welding cost per unit mass Welding time per unit length Click Weld Bead (Weldments toolbar) or Insert > Weldments > Weld Bead. simplified weld bead display Inclusion of weld bead properties in drawings using weld tables Smart Weld selection tool for face selection of weld bead paths Association of weld bead symbols with the weld beads Handles that assist in defining weld paths (lengths) Inclusion in the Weld Folder in the FeatureManager design tree Additionally.
for Edges and Faces or Vertex . Adding a Chamfer to an Assembly Component First. 164 . you can propagate these features to the parts they affect. Open install_dir\samples\whatsnew\assemblies\plate_assembly. add a chamfer to the plate on the right. you added weld beads as components of the assembly. you can still edit existing weld bead components. or click Insert > Assembly Feature > Chamfer. Then you add a simplified weld bead. Fillets and Chamfers In assemblies.Weldments In previous versions of SolidWorks. Click Assembly Features (Assembly tab on the CommandManager) and click Chamfer . In the PropertyManager. which are useful for weld preparation. Example: Adding Chamfers and Weld Beads to an Assembly In this example. 2. you add chamfers to two plates to prepare them for welding. This method is no longer supported. However. you can create fillets and chamfers. under Chamfer Parameters.sldasm. As with other assembly features. 1. 3. do the following to select the edge of plate01: a) Right-click the top edge between the two plates and click Select Other.
Adding a Chamfer to a Second Component Now add a chamfer to the other plate. you can select Propagate feature to parts if you want to add the chamfer to the plate's part file. b) Set Distance c) Set Angle to 5. 165 . 5. Click . A preview of the chamfer appears. Select the edge of the plate. The chamfer appears. Under Feature Scope. select Edge@[plate01<1>]. Under Chamfer Parameters: a) Select Angle distance.Weldments b) In the dialog box. 1. to 45. 4.
• Click Insert > Assembly Feature > Weld Bead. (Assembly tab on the CommandManager) and click • Click Assembly Features Weld Bead . Adding a Weld Bead Now add a weld bead to the assembly. The chamfer appears in the second plate. Do one of the following: • Click Weld Bead (Weldments toolbar). A preview of the chamfer appears. Click Assembly Features (Assembly tab on the CommandManager) and click Chamfer . under Settings: a) For Weld selection. 3.Weldments 2. 2. In the PropertyManager. click . 166 . In the PropertyManager. 1. select the faces of the two chamfers in the graphics area.
click Welds or Weld Bead. click Welds. Click Insert > Model Items and under Source/Destination. Weld Tables You can insert weld tables in a drawing. 3. By default. Weld bead features that have identical properties are stored together in subfolders. weld tables include: • • • • • Weld size Symbol Weld length Weld material Quantity 167 .Weldments b) Set Bead size to 15. and end treatments for weld beads in specific views. caterpillars. • You can insert weld symbols. Move the pointer to highlight a weld path and click to place the annotation. In the FeatureManager design tree. you can insert bi-directional weld symbols that are attached to weld paths. Weld Bead1 is the weld you just created. Weld Support in Drawings Weld Symbols • In drawings. Click Insert > Model Items and under Annotations. The weld bead appears in the graphics area. You can also select weld bead features from the FeatureManager design tree while in the Model Items command. Click . click Selected feature for Source. Weld Folder appears. Under Annotations.
and save it as a template for future use. click Weld Table (Table toolbar) or click Insert > Tables > Weld . In the PropertyManager. In a drawing view.Weldments You can add other properties to the table such as weld cost and weld time. Table. set the options and click 168 .
The Cleanup unused non-revision managed documents dialog box lists documents that are not used and lets the administrator select those to delete. the vault administrator can grant permission to users to delete these unused documents. 169 . Users with appropriate permissions can manually select unused documents in the vault tree and delete them. select Allow user to delete not referenced non-revision managed documents.28 Workgroup PDM Available in SolidWorks Professional and SolidWorks Premium. This chapter includes the following topics: • Deleting Unused Documents That Are Not Revision Managed Deleting Unused Documents That Are Not Revision Managed Documents can be removed from the vault when they are unused and have references that are not revision managed. On the Vault Settings tab. a vault administrator can initiate a cleanup from the Standard Libraries tab by clicking Cleanup under Check for unused documents. and select Delete. right-click on it. Users with permission to delete unused documents can navigate to an unused document in the task pane. Using the VaultAdmin tool. The vault administrator can search for and remove unused documents from the entire vault. Under Global Settings.
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