Inserting A Body In An Added Volume

This task shows you how to insert a new body in an added volume. From a selected volume in an ordered geometrical set, you are now able to insert some Part Design features.
The created body is always a hybrid body independent of the option set in Tools > Options > Part Infrastructure > Part Document; i.e. selecting or deselecting Enable hybrid design inside part bodies and bodies has no effect.
A volume must have been created.
You can open the VolumeAdd1.CATPart document.
 

  1. Right-click the volume in the specification tree and select Volume.1 object > Insert Added Volume... contextual command.

    The result in the specification tree is an Add operation (Add.2) of a new body (Body.1) within the ordered geometrical set. The new body itself contains an Add feature (Add.1) of the input volume (Volume.1).
    • Add.1 becomes the current object.
    • Add.2 is a modification feature of Volume.1 and absorbs it.
    • The visualization of Volume.1 is absorbed by Add.1 and the visualization of Body.1 is absorbed by Add.2.
    • If you delete the volume, the body will also be deleted, unless you deselect Delete Aggregated Features in the Delete dialog box.
     
    You are now able to create Part Design features within the body. Let's create an edge fillet.

  2. Activate the Part Design workbench.

  3. Click Edge Fillet .

  4. Select the edge as show below:

  5. Click OK to fillet the edge.

    The edge fillet is created within Body.1.
This command is available from the contextual menu of any volume.
  • It is only available in an ordered geometrical set environment.
  • Reordering is not possible on a solid body aggregated by the Add feature.