About Pads

Creating a pad means extruding a 2D profile or a surface in one or two directions. The app lets you choose the limits of creation as well as the direction of extrusion. There are a few things that you need to know when creating pads.

This page discusses:

See Also
Creating Pads
Using the Sub-Elements of a Sketch
Creating Pads Using Limiting Plane
Creating Pads Using Limiting Surface
Location of Sketches in the Tree (Hybrid Design)

Pad Definition Options

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

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

Type

By default, the app specifies the pad's length (Dimension). Here are the different types of limits you can set:

  • Dimension.
  • Upto to next : The app detects existing material for trimming the pad.
    Profile

    Result

  • Up to last: The last face encountered by the extrusion trims the pad.
    Profile

    Result

  • Up to plane: The selected plane trims the extrusion.
  • Up to surface: The selected surface trims the extrusion.
    Profile

    Result

If you set Up to plane or Up to surface, the Offset box becomes available to let you define an offset from the selected plane or surface.

If you set Up to plane, contextual commands creating new planes you may need are then available from the Limit box:

  • Insert Wireframe > Create Plane: For more information, see Creating Planes.
  • Insert Wireframe > XY Plane: The XY plane of the current coordinate system origin (0,0,0) becomes the limit.
  • Insert Wireframe > YZ Plane: The YZ plane of the current coordinate system origin (0,0,0) becomes the limit.
  • Insert Wireframe > ZX Plane: The ZX plane of the current coordinate system origin (0,0,0) becomes the limit.

If you set Up to surface, contextual commands creating new surfaces you may need are then available from the Limit box:

If you create any of these elements, the app 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.

Reverse Side

The button applies for open profiles only. This option lets you choose which side of the profile is to be extruded. When designing Creating Thin Solids, this option is meaningless.

Direction

you can create a pad along a specified reference direction by specifying the reference element in the Direction box.

Contextual commands creating the directions you need are available from the Reference box:

  • Insert Wireframe > Create Line: For more information, see Creating Lines.
  • Insert Wireframe > Create Plane: For more information, see Creating Planes.
  • Insert Wireframe > X Axis: The X axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Insert Wireframe > Y Axis: The Y axis of the current coordinate system origin (0,0,0) becomes the direction.
  • Insert Wireframe > Z Axis: The Z axis of the current coordinate system origin (0,0,0) becomes the direction.

If you create any of these elements, the app then displays the line or the plane icon in front of the Reference. Clicking this icon enables you to edit the element.

About Profiles

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

You can:

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

  • Select diverse elements constituting a sketch.

  • If you execute the Pad command with no profile previously defined, click the icon available in the dialog box. You then need to select a sketch plane to enter the Sketcher app 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 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 Creating Fill Surfaces.

      • Insert Operations > Create Join: Joins surfaces or curves. For more information, see Joining Curves or Surfaces.

      • Insert Operations > Create Extract: Generates separate elements from unconnected sub-elements. For more information, see 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 app in which you can then edit the profile . Once you have done your modifications, you just need to exit the Sketcher app. The Pad.x dialog box then reappears to let you finish your design.

More about the Pad Command

This section provides information on the Pad command.

Keep in mind the following when using Pad .

  • The app 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 with 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

Copy and Paste a Pad

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.