Hide Table of Contents

Sheet Metal Cut List Commands

When you create a multibody sheet metal part, in the FeatureManager design tree, the main tree lists each body and its features in the order in which you add them. In addition, a cut list contains a separate representation for each body, with a flat pattern specific to the body.

Multibody sheet metal cut lists offer the same features as weldment cut lists, including the ability to automatically organize and update sheet metal bodies, and view sheet metal properties. You can use the body-related properties in bills of materials and drawings.

The name of a body in the cut list is derived from the last feature added to the body.

Right-click the top level of the cut list to display the following commands, which apply to all the bodies in the cut list:

Show Feature History Lists the features that belong to each body.
Isolate  
Delete Bodies Displays the Delete Body PropertyManager, which lists bodies in the Multibody part.
Delete For cut lists containing cut list items, removes all bodies from the cut list items and deletes the cut list items.
Insert into New Part Creates a derived part by inserting the bodies into a new part.

After insertion, the bodies can be manipulated in the new part using Move/Copy Bodies.

To change the features of bodies in a derived part, you must edit the bodies in the original part.

Save Bodies Displays the Save Bodies PropertyManager, where you can save the bodies in the multibody sheet metal part to individual files that you can use to create an assembly.
Automatic When enabled, automatically organizes sheet metal cut list items.

Enabled by default.

If you select Automatic, the Update option is added to the menu, letting you manually update the bodies in the cut list.

fm_cutlist_needs_update.png Indicates that cut list needs to be updated.
Indicates that the cut list is up-to-date.
Go to Displays the Find in FeatureManager Design Tree dialog box, where you can search the text of the design tree for a text string.
Collapse Items Collapses all items in the FeatureManager design tree.
Hide/Show Tree Items Opens the System Options dialog box to the FeatureManager page, to let you change the Hide/Show settings for the FeatureManager design tree.

Available on all right-click menus in the FeatureManager.

Right-click on a body in the cut list to display the following commands:

Flatten Flattens the selected body and hides other bodies.
Create Sub-Weldment Creates a sub-weldment folder containing the selected body.
Create Cut List Item Creates a cut list item containing the selected body.
This option is only available if Automatic is not enabled on the cut list right-click menu. If Automatic is enabled, to create cut list items, click Update.

Right-click the cut list item and click Properties to specify cut list properties.

You specify custom properties for multibody sheet metal parts in the same way that you do for weldments.

Isolate Sets all bodies except the selected body to be hidden or transparent.

In the Isolate dialog box, you can:

  • Change the default behavior of the Isolate command.
  • Toggle between hidden and transparent for bodies other than the selected body.
    When you specify bodies as transparent, you can select geometrical entities.
Material Displays a submenu with these options:
Edit Material Displays the Material dialog box, where you can manage the physical material of the selected body.
Remove Material When the selected body has been assigned a material, removes the material.

To assign a common material to all bodies in the part, you must remove individually assigned materials.

Manage Favorites Displays the Favorites tab of the Material dialog box, where you can modify the material Favorites list.
Material Favorites list Materials you can apply without displaying the Material dialog box.
Body Display Lists display styles you can apply to the selected body.
Delete Body Opens the Delete Body PropertyManager, where you can select bodies to delete.

The deleted body appears in the FeatureManager design tree. You can rollback to redisplay the body.

Insert into New Part Opens a new part document containing the selected body and prompts you to save the part.

The body is saved as a stock part with external references to the multibody part. Changes you make to the body in the multibody part are propagated to the stock part.

Change Transparency Toggles the transparency of the selected body.
Go to Feature (In Tree) Highlights the feature in the main FeatureManager design tree.


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:   Sheet Metal Cut List Commands
*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 2015 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.