Splitting Sheet Metal Parts

You can create a multibody sheet metal part using any command that creates multiple bodies from a single body.

Use these commands on the Features toolbar to split a sheet metal part into multiple bodies:

  • Extruded Cut
  • Revolved Cut
  • Swept Cut
  • Lofted Cut
  • Boundary Cut
  • Split

This topic describes the use of the Split command.

To split a sheet metal part using the Split command:

  1. Open the part to be split.
  2. Create a sketch to be used to split the part.
  3. Select Split (Features toolbar).
  4. In the PropertyManager, under Trim Tools, select the sketch.
  5. Click Cut Part.
  6. Under Resulting Bodies, under , specify the bodies for the split operation.
  7. Optionally, click the <None> callout for each body and save it using the Save As dialog box.
    The names appear in the PropertyManager and the callouts in the graphics area.
  8. Click .
    The part now contains multiple sheet metal bodies.

    In the FeatureManager design tree, the bodies in the cut list are named for the split feature.

    When you add a feature to a body, the cut list name changes to the last feature added. Here, when you add an edge flange, the name of the body changes from Split1[2] to Edge-Flange2.