About Pads

Creating a pad means extruding a profile or a surface in one or two directions. The application lets you choose the limits of creation as well as the direction of extrusion.

By default, the application extrudes the profile normal to the plane used to create the profile. To see how to change the extrusion direction, see Creating Pads not Normal to Sketch Planes

If you extrude a surface, you need to select an element defining the direction because there is no default direction.

This section describes the various options available in the Pad Definition dialog box to create a pad.

In this dialog box, you can define a pad using these options:

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

You can:

• Use profiles sketched in the Sketcher workbench or planar geometrical elements created in the Generative Shape Design workbench (except for lines).

• Select diverse elements constituting a sketch. For more information, see Using the Sub-Elements of a Sketch.

• If you execute the Pad command with no profile previously defined, just click the icon available in the dialog box. You then just need to select a sketch plane to enter the Sketcher workbench and then create the desired profile. As soon as you click , the Running Commands window is displayed to show you the history of commands you have run. This informative window is particularly useful when many commands have already been used, in complex scenarios for example.
• Select Generative Shape Design surfaces, non-planar faces and even V4 surfaces. For more information, see Creating Pads or Pockets from Surfaces.

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

  
  
  

• Clicking Sketch opens the Sketcher workbench in which you can then edit the profile . Once you have done your modifications, you just need to exit the Sketcher workbench. The Pad dialog box then reappears to let you finish your design.

This section provides information on the Pad command.

Keep in mind the following when using Pad .

• The application allows you to create pads from open profiles provided existing geometry can trim the pads. The pad below has been created from an open profile which both endpoints were stretched onto the inner vertical faces of the hexagon. The option used for Limit 1 is Up to next. The inner bottom face of the hexagon then stops the extrusion. Conversely, the Up to next option could not be used for Limit2.

  Profile

  Result

• You can also created pads from sketches including several profiles. These profiles must not intersect. In the following example, the sketch to be extruded is defined by a square and a circle. Applying the Pad command on this sketch lets you obtain a cavity :

  Profile

  Result

  However, if the application can generate an intersection between both profile endpoints, it produces a pad as in the following example. The profile chosen is an arc of circle. Although no existing geometry can trim the pad to be created, the application succeeds in generating a pad.

  Profile

  Result

You can copy and paste a pad using the As specified in Part document option.

When copying and pasting a pad using the As specified in Part document option (for more information, see Handling Representations in a Multi-Representation Environment, if the extrusion direction used does not belong to the same body as the pad, this direction is not taken into account by the Copy and Paste commands.