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 and edges.

It includes:

Open the RemoveFace1.CATPart document.

  1. Click Remove Face/Edge  in the Operations toolbar (Trim-Split sub toolbar).

    The Remove Face /Edge Definition dialog box appears.

  2. In the Faces/Edges to remove box, select the faces or edges to be removed.

    These elements are highlighted in purple.
    • The Support box is automatically filled in with the surface whose face belongs to. To modify the
      support, you need to remove all faces first.
    • The Faces to remove box displays the following contextual commands:
      • Clear Selection: removes all selected faces/edges from the selection.
      • Tangency Propagation: Includes all faces/edges tangent to the selected faces from the selection.
      • Fillet Propagation: Includes all tangent continuous filleted faces of the selected face in the selection. This option is available if faces are selected in the Faces/Edges to remove box.
        • Fillet propagation stops at sharp edges.
        • The fillet propagation cannot be performed on variable radius fillet.
      • Auto Propagation: Includes edges connected by point propagation to edges in the selection. This option is available if edges are selected in the Faces/Edges to remove box.

  3. In the Faces to keep box, select the faces or edges to be kept.
    These elements are highlighted in blue.

  4. Select the Show all faces to remove check box 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.


     

    • You can deactivate the Remove Face feature, if it fails at the time of creation. In this case, a warning message is issued asking whether you want to deactivate the feature or not, and the face which is causing the error is highlighted in red color.
    • You can edit the deactivated feature to provide the valid input element.
 

Create a Remove Face feature Using Limiting Elements
  You can partially remove some faces using limiting elements. This particularly helps you to locally modify a fillet.

  1. Click Remove Face/Edge  and select the face as shown to remove it, in the Remove Face Definition dialog box.

  2. Click More>> to define limiting elements for the removal of the face.

    The Remove Face/Edge Definition dialog box is expanded.

  3. Right-click the Faces to Limit box and select Create to determine a face to limit.

    The Face to Limit dialog box appears.
     

  4. In the Face to limit box, select the face as shown.

    The face to limit cannot be a removed face (select the Show all faces to Remove check box to see what are the removed faces).

  5. In the Limiting element box, select the plane as shown.
    The arrow indicates the side of the face to be removed.
    Note: You can click Reverse Direction to reverse the direction of the face to be removed.

  6. Click OK to confirm the first limiting element.

  7. Repeat step 3 to 5 to create another limiting face as shown.

     

    The Faces to limit box displays the following contextual commands:
    • Reframe on: reframes the view on the created limiting face.
    • Edit: edits the limiting face created.
    • Remove: deletes the selected face to limit.
    • Clear all: clears all the selections made.
    • In this command, you can select only one face to limit.
    • The face to limit can only be split once.

  8. Click OK to confirm the second limiting element.
    The face is partially removed up to the limiting elements depending on the defined direction. The new feature identified as RemoveFace.XXX is added to the specification tree.


 
 

Topology
  The Remove Face/Edge does not create any new face. The capability is valid for existing topology extrapolation.
This is why the following pink face cannot be removed:

 

However, this one can be removed because there is a possible trimming face that can be used by the application.

Before After
   
 

Self-Intersecting Volumes
The Remove Face/Edge capability may produce self-intersecting volumes as illustrated in the following example:
 
Initial Geometry

The 3D shape is composed of a shelled pad. Two fillets (in lavender) were created on two of its edges.
 

Resulting remove face feature

Removing the internal fillet feature generates an inconsistent shape.

To analyze self-intersecting volumes, we recommend you use the Split capability which most of the time provides a better view of the problems:

 

Removing the appropriate face

By removing the external fillet first there is no self-intersecting volumes, the resulting geometry is satisfactory.