Creating Remove Face Features

When parts are far too complex for finite elements analyses, there is a way of making them more simple. This task shows you how to simplify a part by removing some of its faces.
Open the Update.CATPart document. As the Remove Face capability only deals with the geometry of the part, not the history of its design, you can use it for imported parts, like in the following scenario, or Version 4 parts.

  1. Click Remove Face  .
    The Remove Face Definition dialog box appears.

  2. Select the inner face as the face to be removed.
    The face turns purple indicating that it will be removed.

  3. Click the Faces to keep field and select both faces as shown.
    The faces turn blue, indicating that they will not be removed.

  4. Check the Show all faces to remove option to preview all the faces adjacent to the purple face that will be removed.

  5. Click OK to confirm.
    All of the faces have been removed. The new feature identified as RemoveFace.XXX is added to the specification tree.

  6. Launch the command again and select the faces as shown as the faces to be removed.


    Two contextual commands are available from the Faces to remove field:

    • Clear selection: removes all selected faces from the selection.
    • Tangency propagation: includes all faces tangent to selected faces in the selection
  From the Faces to keep field, only the Clear selection contextual command is available.
 

  1. Click OK to confirm.
    All selected faces have been removed. The new feature identified as RemoveFace.XXX is added to the specification tree.