Creating Pockets

You can extrude a profile or a surface and remove the material resulting from the extrusion to create a pocket.

This task first shows you how to create a pocket, that is a cavity, then you will edit this pocket to remove the material surrounding the initial profile.

Before you begin:

To perform this task, create a pad and sketch a closed profile on one of its faces.

Related Topics
More about Pockets
Using the Sub-Elements of a Sketch
Location of Sketches in the Specification Tree (Hybrid Design)

  1. Select the profile you want to extrude .



  2. Click Pocket in the Sketch-Based Features toolbar (Pockets sub-toolbar).

    The Pocket Definition dialog box appears and the application previews a pocket.

    Tip: Clicking the icon opens the Sketcher . You can then edit the profile to modify your pocket. Once you have done your modifications, you just need to quit the Sketcher. The Pocket dialog box reappears to let you finish your design.

  3. To define a specific depth, set the Type parameter to Dimension, and enter the dimension value you want.



    Tip: Alternatively, select LIM1 manipulator and drag it downwards to the dimension value you want.

  4. Click OK to create the pocket.

    The specification tree indicates this creation. This is your pocket:

  5. Double-click Pocket.1 to edit it. As the application lets you choose the portion of material to be kept, you are going to remove all the material surrounding the initial profile.

  6. Reverse side lets you choose between removing the material defined within the profile, which is the application's default behavior, or the material surrounding the profile. Click Reverse side or alternatively, click the arrow as shown:



    The arrow now indicates the opposite direction.

  7. Click OK to confirm.

    The application has removed the material around the profile.