More about Pockets

Creating a pocket consists in extruding a profile or a surface and removing the material resulting from the extrusion. The application lets you choose the limits of creation as well as the direction of extrusion.

The limits you can use are the same as those available for creating pads. To know how to use them, see Creating 'Up to Plane' Pads, Creating 'Up to Surface' Pads.

If you insert a new body and create a pocket as the first feature of this body, the application creates material as shown below:

This section describes the various options available in the Pocket Definition dialog box to create a pocket.

In this dialog box, you can define a pocket using the following options:

This section provides information on the profiles used to create a pocket.

You can:

• Use profiles sketched in the Sketcher workbench or planar geometrical elements created in the Generative Shape Design workbench (except for lines).
• Create pockets from open profiles provided existing geometry can trim the pockets.
• Create pockets from sketches including several closed profiles. These profiles must not intersect. In the following example, the initial sketch is made of eight profiles. Applying the Pocket command on this sketch lets you create eight pockets:
  
  
  
  
• Select diverse elements constituting a sketch. For more information, see Using the Sub-Elements of a Sketch.
• Instead of selecting profiles, you can select surfaces created in the Generative Shape Design workbench, non-planar faces and even V4. To know how to create a pocket from a surface, see Creating Pads or Pockets from Surfaces.
• If you execute the Pocket command with no profile previously defined, just click the icon to access the Sketcher workbench and sketch the profile you need.

• If you are not satisfied with the profile you selected, note that you can:

  
  
  • Click the Selection box and select another sketch.
  • Use any of these creation contextual commands available from the Selection box:
    

    • Insert Wireframe > Create Sketch: Opens the Sketcher workbench after selecting any plane, and lets you sketch the profile you need as explained in the Sketcher User's Guide.

    • Insert Surfaces > Create Fill: Creates fill surfaces between the boundary segments. For more information, see Generative Shape Design User's Guide: Creating Surfaces: Creating Fill Surfaces.

    • Insert Operations > Create Join: Joins surfaces or curves. For more information, see Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Joining Surfaces or Curves.

    • Insert Operations > Create Extract: Generates separate elements from non-connex sub-elements. For more information, see Generative Shape Design User's Guide: Performing Operations on Shape Geometry: Extracting Geometry: Extracting Elements.

    If you create any of these elements, the application then displays the corresponding icon in front of the box. Clicking this icon enables you to edit the element.

    If you have chosen to work in a hybrid design environment, the elements created on the fly via the contextual commands mentioned above are aggregated into sketch-based features.

You can define a direction while creating a pocket.

Note that:

• By default, if you extrude a profile, the application extrudes normal to the plane used to create the profile. To specify another direction, click More>> to display the whole Pocket Definition dialog box, clear the Normal to profile check box and select a new creation direction in the geometry.

• When copying and pasting a pocket using the As specified in Part document option (for more information, see Handling 3D Shapes in a Multi-Representation Environment), note that if the extrusion direction used does not belong to the same body as the pocket, this direction is not taken into account by the Copy and Paste commands.
• If you extrude a surface, you need to select an element defining the direction because there is no default direction.