About Pockets

Creating a pocket consists of extruding a profile or a surface and removing the material resulting from the extrusion. The app 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 Pads Using Limiting Plane, Creating Pads Using Limiting Surface.

This section describes various options available in the Pocket.x dialog box.

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 app or planar geometrical elements created in the Generative Shape Design app (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.
• Instead of selecting profiles, you can select surfaces created in Generative Shape Design, 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 can click the Pocket command with no profile previously defined, just click the icon to access the Sketcher app 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 app 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 unconnected 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 app 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 app extrudes normal to the plane used to create the profile.

  To specify another direction, Select a new creation direction in the geometry in the Direction box.

  Important: The option to select the direction which is not normal to the profile is only available in the MDG role. In the restricted TDD license, a pocket will be created in the direction normal to the profile.

• 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.