Creating Shells

Shelling a feature means emptying it, while keeping a given thickness on its sides. Shelling may also consist in adding thickness to the outside.
This task shows how to create a cavity.
Open the Shell.CATPart document.
  1. Select the face to be removed.

  2. Click Shell . The Shell Definition dialog box appears.
    The selected face becomes purple.

  3.  Enter 15mm in the Default inside thickness field.

  4. Click OK.
    The feature is shelled: the selected face is  left open. This creation appears in the specification tree.

  5. Double-click the shell to edit it.

  6. Decrease the inside thickness value. Enter 4mm.

  7. Click OK.
    The cylinder is now hollowed:

  8.  Double-click the shell again and click the Other thickness faces field.

  9. Select the face as shown.

  10. Double-click the thickness value displayed on this face.

  11. In the dialog box that appears, enter 10mm.

  12. Click OK to confirm and close the dialog box.

  13. Click OK to create the shell feature.
    The length between the selected face and the shell is 10mm.


A Few Notes About Shells

  • The value for the shell must be lower by half than the thickness of the input body. Otherwise, the resulting body may be not valid due to self-intersections. To avoid problems, ensure that the input body is thick enough.
  • In some specific cases, you may need to perform two shell operations consecutively. To avoid problems, the value for the second shell should be lower by half than the value of the first shell.

  • If you need to shell a multi-domain body, perform only one Shell operation : select one face by domain to avoid problems. The specification tree then includes only one Shell feature as illustrated below.

Solving Problems

Ignoring Faces

In some specific cases, the application cannot shell the selected face. An error message appears informing you that the body cannot be built properly. After closing that window, another message appears proposing you to ignore the faces causing trouble. If you accept that solution, the shell is performed and the face causing trouble is removed.

Later on if you edit the shell, the ignored face is previewed and the Reset ignored faces option is then available in the Shell Definition dialog box.

By checking this option, the ignored face is reinitialized and the indication Ignored face in the geometry is deleted. If the check box is unchecked, the previous ignored face is still taken into account for the next feature definition.

Ignoring faces in many cases  avoids a costly and difficult manual rework of the part.

Extracting Geometry

Sometimes, you will need to use Extract to be able to add thickness to a face. The Extract capability lets you generate separate elements from initial geometry, without deleting geometry. This command is available after clicking a dialog box prompting you to deactivate the shell and extract the geometry. Once the operation has been done, the Extracted Geometry (Shell.1) node is displayed in the tree. This category includes the elements created by the application.

The Extract capability is available if only one face was selected to perform the shell operation.

Note also that if you have Generative Shape Design installed, the geometry resulting from the Extract operation is associative.