Hide Table of Contents

Split and Save Bodies PropertyManager

The Split PropertyManager appears when you click Split (Features toolbar) to create multiple bodies from a part.

Trim Tools

Trimming Surfaces Select entities to use to trim the part into multiple bodies.
  • Reference planes (Planes extend infinitely in all directions.)
   
  • Planar model faces (Faces extend infinitely in all directions.)
   
Original Part Revised Original Part New Part
   
  • Sketches (Sketches extrude through all in both directions.)
   
Original Part Revised Original Part New Part
   
  • Reference surfaces and non-planar model faces (These do not extend their boundaries. Internal holes on reference surfaces or non-planar model faces are closed when splitting the part.)
   
Original Part New Parts
  Cut Part Cuts the part into multiple bodies using the Trimming Tools geometry. Split lines appear on the part, showing the different bodies formed by the split.
Callout boxes appear in the graphics area for up to 10 bodies at one time. Click Next 10 or Previous 10 to scroll through all the callout boxes for a part.

Resulting Bodies

Lists the split bodies in the part after you click Cut Part.

Select the bodies to save You can also click Auto-assign Names to name the bodies as Body< n >.sldprt and save them.
  File After you split the bodies, they are listed in the FeatureManager design tree under Solid Bodies. Double-click the body name under File, type a name for the new part in the dialog box, then click Save. The new part name appears under File and in the callout box. The bodies that you do not save are not split. They remain with the original part. You can also save bodies from a multibody part using the Save Bodies PropertyManager.
 
If you clear the check box for a split part after you save it, that part is no longer saved as a separate entity. It remains with the original part.
  Consume cut bodies Removes the body from the part. Consumed bodies are not listed in the FeatureManager design tree under Solid Bodies.
  Origin location Places the origin of the split body at the vertex you select.
  Copy custom properties to new parts  

Template Settings

Lets you override the default template from Tools > Options > System Options > File Locations.

Override default template settings Specifies to use an alternate template. The selected template is applied to all new part or assembly files you create during the current Split or Save Bodies operation.
Part template Lists the selected part template. Click to browse to a different template.
Assembly template (Available when you create an assembly in the Save Bodies PropertyManager.) Lists the selected assembly template. Click to browse to a different template.


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:   Split and Save Bodies PropertyManager
*Comment:  
*   I acknowledge I have read and I hereby accept the privacy policy under which my Personal Data will be used by Dassault Systèmes

Print Topic

Select the scope of content to print:

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 2013 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.

0.20.48