Creating a Pocket and Holes

This task shows how to create a pocket and holes, with technological properties.
These features are available on both the board and the manufacturing panel.
Open a CATProduct document containing a board.

  1. Sketch the contour of the pocket.

    To do so:

    1. click the Sketcher button I_SketcherP2.gif (229 bytes)

    2. select the board to define the working plane

    3. click the Profile button I_ContourP2.gif (211 bytes) and draw the contour around the motor

    4. then click the Exit Sketcher button I_CloseP2.gif (214 bytes) to return to the 3D world.

  1. Click Pocket I_PocketP2.gif (230 bytes).

    The Pocket Definition dialog box is displayed and CATIA previews a pocket with default parameters.

  2. Set the Up to last option to define the pocket limit.

    This means that the application will extend the pocket to the last possible face, that is the pad bottom.

  1. Click OK.

  2. Before creating the Hole, right-click the board PartBody and select Define in Work Object so that the PartBody becomes the active product.

  3. Click Hole I_HoleP2.gif (232 bytes).

  4. Select the board to define the working plane.
    The Hole Definition dialog box appears.
    CATIA previews the hole to be created with default parameters.

  5. Enter 4mm for the diameter and click OK.
    The hole is created.

  6. Repeat the steps 5, 6 and 7 for the second hole.

    The pocket and holes are added to the specification tree.
    PocketandHolesNLS.gif (11600 bytes)

  7. Right-click Hole.1 in the specification tree to display the contextual menu.

  8. Select Properties.

    The Properties dialog box opens.
    db_holePropNLS.gif (8838 bytes)

  9. Click More... .

  10. Select Circuit Board.

  11. Switch the Subtype to NPTH (non conductive) and click OK.
    The hole is more than a simple hole: it has a technological property.

  12. Repeat the steps 9 to 13 for the second hole.
    These holes are used for mounting purposes.