Creating a Shell

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 VolumeShell1.CATPart document.

  1. Click Shell .

    The Shell Definition dialog box is displayed.

  2. Select the Face to remove.

    The Support Volume field is filled with the volume owning the selected face.

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

  4. Click OK.

    The feature is shelled: the selected face is left open.
    This element (identified as Shell.xxx) is added to the specification tree.

  5. Double-click the shell to edit it.

  6. Click the Other thickness faces field.

  7. Select a face.

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

  9. In the dialog box that appears, enter 10mm and click OK.

    The length between the selected face and the shell is now 10mm.

  10. Click More>>.

      

  11. Select the Smoothing mode under the Deviation parameters section.

    There are three types of smoothing modes:
    • None: No smoothing is applied. This is the default option. The Max deviation field and Constant thickness option are disabled.
    • Manual: Allows you to enter a maximum deviation. The default value is 0.1 mm. The Constant thickness option is enabled to allow you to apply a constant thickness.
    • Automatic: Smoothing is applied automatically. The Max Deviation field is grayed out. However, the Constant thickness option is enabled to allow you to apply a constant thickness.

  12. Click OK.

For further information about shells, please refer to Creating Shells in Part Design documentation.