Creating Thin Solids

You can add thickness to both sides of the profiles when creating the pads, pockets and stiffeners.

Before you begin:
  • To perform this task, create a simple closed profile.
  • Make sure that the Open dialog boxes with legacy appearance check box available at Me > Preferences > App Preferences > 3D Modeling > 3D Modeling Core > Part Design > Appearance of dialog boxes, is selected.
See Also
About Thin Solids
About Pads
Using the Sub-Elements of a Sketch
Location of Sketches in the Tree (Hybrid Design)
  1. From the Model section of the action bar, click Pad .
  2. Select the sketch containing a closed profile.
  3. Select the Thick check box.

    This opens the whole Pad Definition dialog box. You can now define a thin pad using the options available in the Thin Pad area.

    Important: The options for creating thin solids are not available when you select a surface as the element to be extruded. For more information, see Creating Pads or Pockets from Surfaces.
  4. In the Thickness1 box, enter 18mm.
    A thickness is added to the profile as it is extruded.
  5. Click Preview to see the result.
    The profile is previewed in dotted line.

  6. In the Thickness2 box, enter 10mm.
    Material is added to the other side of the profile.
  7. Click Preview to see the result.


  8. To add material equally to both sides of the profile, select the Neutral fiber check box and click Preview to see the result.
    The thickness you defined for Thickness 1 is evenly distributed: a thickness of 9mm has been added to each side of the profile.

    Tip: This capability can be applied to several profiles contained in the same sketch.