Split and Save Bodies

Use the Split feature to create multiple parts from an existing part. You can create separate part files, and form an assembly from the new parts.

You can split one or more solid or surface bodies. To split a surface, the Trimming Surface must extend past the boundaries of the surface to split.

To split bodies:

  1. Click Split (Features toolbar) or Insert > Features > Split.
  2. In the PropertyManager, set the options.
    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.
  3. Under Resulting Bodies, select the bodies to save under , or click Auto-assign Names.
    All of the saved bodies appear in the graphics area and are listed in the FeatureManager design tree under Solid Bodies. The software automatically names all bodies. You can change the names.
  4. 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 in the Resulting Bodies list and in the callout box. Unsaved bodies are not split and remain with the original part.
    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.
  5. Click .

Handling Split Parts

New Parts

The new parts are derived; they contain a reference to the parent part. Each new part contains a single feature named Stock- <parent part name> - n ->. You can reattach a derived part to a specified stock part, split feature, or body.

If you change the geometry of the original part, the new parts also change. If you change the split feature geometry, no new derived parts are created. The software updates the existing derived parts, preserving parent-child relations.

With multibody parts, the various split parts are listed in the FeatureManager design tree under Solid Bodies.

Original Part

The original part contains all its original features plus a new feature called Split.

If you selected Consume cut bodies under Resulting Bodies, the solid body displayed in the graphics area is the original solid body minus the new parts. If all bodies in the original part were saved as split bodies, no solid body is displayed. To see the original solid body, move the rollback bar in the FeatureManager design tree above the split feature or suppress the split feature.

If you delete the split feature in the original part, the new parts still exist, but the status of the external reference in the new parts is dangling.

Saving Split Bodies

You can also save solid bodies after you split the model using the Save Bodies feature. This enables you to save the bodies from a split part to a different folder or with different names to the same folder. You can also create an assembly from the split parts.

To save bodies from multibody parts:

  1. Click Insert > Features > Save Bodies.
  2. Select the bodies to save in the graphics area, or under in Resulting Parts.
    Click to toggle the selection of all bodies.
    The callouts display the default path, file names, and location of the multibody part.
  3. Under Resulting Parts, double-click each file name under File to open the Save As dialog box. You can select a new location and file name for each part. You can also click Auto-assign Names to select and name all bodies.
  4. Select Consume cut bodies to copy cut-list items from multibody parts to resulting parts.
  5. To create an assembly, under Create Assembly, click Browse, select a folder to save the assembly as SplitAssembly type (*.sldasm), and type a file name.
  6. If the multibody part is a weldment or contains multiple instances of identical bodies such as patterned bodies, click Derive resulting parts from similar bodies of cut lists.
    Identical bodies, for example weldment structural members, are saved as a single part. The assembly is created with multiple instances of this part.
    Bodies must have identical material properties to be instanced in this way.
  7. Click .