Introduction
Administration
User Interface
SolidWorks Fundamentals
Moving from 2D to 3D
Assemblies
CircuitWorks
Configurations
SolidWorks Costing
Design Checker
Design Studies in SolidWorks
Drawings and Detailing
DFMXpress
DriveWorksXpress
FloXpress
Import and Export
Large Scale Design
Model Display
Mold Design
Motion Studies
Parts and Features
Routing
Sheet Metal
Comparing Sheet Metal Design Methods
Using Sheet Metal Tools
Using Forming Tools with Sheet Metal
Converting Solid Bodies to Sheet Metal
Bend Types
Creating a Sheet Metal Part by Converting a Solid Body
Converting a Solid Part to a Sheet Metal Part
Converting an Imported Part to a Sheet Metal Part
Using Rip Sketches with Convert to Sheet Metal
Convert To Sheet Metal PropertyManager
Example of Keep Body Option
Creating a Sheet Metal Part Using Sharp Bends
Creating a Sheet Metal Part Using Round Bends
Creating Sheet Metal Parts with Conical Faces
Adding Walls to a Sheet Metal Part
Sheet Metal Features
Flattening Sheet Metal Bends
Sheet Metal Parts
Multibody Sheet Metal Parts
Using Sheet Metal Bend Parameters
Simulation
SimulationXpress
Sketching
Sustainability Products
SolidWorks Utilities
Tolerancing
Toolbox
Weldments
Workgroup PDM
Troubleshooting
Glossary
Hide Table of Contents Show Table of Contents

Converting a Solid Part to a Sheet Metal Part

The Convert to Sheet Metal command lets you specify the thickness, bends, and rips necessary to convert a solid part to a sheet metal part.

To convert a solid part to a sheet metal part:

  1. Create the solid part.

  2. Click Convert to Sheet Metal (Sheet Metal toolbar) or Insert > Sheet Metal > Convert To Sheet Metal .
  3. In the PropertyManager, under Sheet Metal Gauges, set options if you want to use a gauge table:
    1. Select Use gauge table.
    2. In Select Table , select a gauge table to use, or click Browse and browse to a gauge table.
  4. Under Sheet Metal Parameters:
    1. Select a face as the fixed face for the sheet metal part.
    2. Set the sheet thickness and default bend radius.
    3. Select Keep body if you want to keep the solid body to use in another Convert to Sheet Metal feature. When cleared, the body is consumed by the Convert to Sheet Metal feature.
  5. Under Bend Edges, select the model edges that will form bends.

    Change the display style to Hidden Lines Visible to make it easier to select edges.

    The rips required are automatically selected and listed under Rip Edges found.

    In the graphics area, callouts are attached to the bend and rip edges if you selected Show callouts in the PropertyManager. You can use the callouts to change the bend radii and rip gaps.

    You can restore the default value by right-clicking the bend edge or rip edge and selecting Restore Default Value.

  6. Under Corner Defaults, set the rip options. To override these defaults by setting options for individual rips:
    1. Under Rip Edges found, select Show callouts.
    2. In the graphics area, click Default in the gap callout.

    3. In the pop-up window, set the rip options.
    4. In the graphics area, right-click and click OK .
  7. Under Custom Bend Allowance, set a Bend Allowance Type and value.
  8. To add relief cuts for the inserted bends, under Auto Relief, select the type of relief cut: Rectangular, Tear, or Obround.

    Tear reliefs are the minimum size required to insert the bend.

    If you select Rectangular or Obround, specify a Relief Ratio.

  9. Click .
  10. Click Flatten (Sheet Metal toolbar) to flatten the part using the bends and rips you specified.



Related SolidWorks Forum Content

Provide feedback on this topic

SolidWorks welcomes your feedback concerning the presentation, accuracy, and thoroughness of the documentation. Use the form below to send your comments and suggestions about this topic directly to our documentation team. The documentation team cannot answer technical support questions. Click here for information about technical support.

* Required

 
*Email:  
Subject:   Feedback on Help Topics
Page:   Converting a Solid Part to a Sheet Metal Part
*Comment:  
x

We have detected you are using a browser version older than Internet Explorer 7. For optimized display, we suggest upgrading your browser to Internet Explorer 7 or newer.

 Never show this message again
x

Web Help Content Version: SolidWorks 2012 SP05

The search functionality within the web help is in a beta test phase and you may experience periodic delays or interruptions in its performance. These are the normal and ordinary features of a beta test and shall not under any circumstances give rise to any liability on the part of DS SolidWorks or its licensors. The topics within the Web-based help are not beta topics; they document SolidWorks 2012 SP05.

To disable Web help from within SolidWorks and use local help instead, click Help > Use SolidWorks Web Help.

To report problems encountered with the Web help interface and search, contact your local support representative. To provide feedback on individual help topics, use the “Feedback on this topic” link on the individual topic page.