Creating Multi-Pockets

You can create a pocket feature from distinct profiles belonging to a same sketch and this, using different length values. The multi-pocket capability lets you do this at one time.

Before you begin:

To perform this task, create a pad on which you will sketch six closed profiles similar to the one below.

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

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

  2. Select the sketch that contains the profiles to be extruded.

    Important: All profiles must be closed and must not intersect. In case a profile would be open, the application would not take it into account.

    The Multi-Pocket Definition dialog box appears and the profiles are highlighted in green. For each of them, you can drag associated manipulators to define the extrusion value.

    The red arrow normal to the sketch indicates the proposed extrusion direction. To reverse it, you just need to click it.



    The Multi-Pocket Definition dialog box displays the number of domains to be removed. In our example, the application has detected six domains, as indicated in the Domains section.



  3. Select Extrusion domain.1 from the dialog box. Extrusion domain.1 now appears in blue in the geometry area.

  4. Specify the length by entering a value. For example, enter 10mm.

    Warning: Contrary to a certain number of sketch-based feature dialog boxes, the Edit Formula... contextual command allowing you to manage length values is not available from the Length field.

  5. You need to repeat the operation for each extrusion domain by entering the value of your choice. For example, select Extrusion domain.2 and Extrusion domain.6 and enter 30mm and 40mm respectively.

    Tip: For complex sketches, the Preview button proves to be quite useful.

  6. Note that you can multi-select extrusion domains from the list before defining a common length: multi-select Extrusion domain.3, Extrusion domain.4, and Extrusion domain.5, then enter 50 as the common length value.



  7. Click More>> to expand the dialog box. In the Second Limit box, you can specify a length value for the direction opposite to the direction previously defined. Note that the Thickness section displays the sum of two lengths defined for a given extrusion domain.



    Important: Clearing the Normal to sketch option lets you specify a new extrusion direction. Just select the geometry of your choice to use it as a reference.

  8. Click OK to create the multi-pocket.

    The multi-pocket (identified as Multi-Pocket.xxx) is added to the specification tree.