Creating Thin Solids 

When creating pads, pockets and stiffeners, you can add thickness to both sides of their profiles. The resulting features are then called "thin solids".

This task shows you how to add thickness to a pad. The method described here is also valid for pockets. To know how to obtain a thin solid from a stiffener, refer to the task Stiffener.

You can create thin solids using the Shaft and Groove capabilities.
Open the GettingStarted.CATPart document and quit the Sketcher.

  1. Click Pad .

  2. Select Sketch.1 if not already done.

  3. Check the Thick option.
    This opens the whole Pad Definition dialog box. You can now define your thin pad using the options available in the Thin Pad frame.
The options for creating thin solids are not available when you select a surface as the element to be extruded. For more information, refer to Creating Pads or Pockets from Surfaces.

  1. Enter 18mm as Thickness1 's value, and click Preview to see the result. A thickness has been added to the profile as it is extruded. The profile is previewed in dotted line.

  1. Enter 10mm as Thickness2 's value, and click Preview to see the result. Material has been added to the other side of the profile.

  1. To add material equally to both sides of the profile, check Neutral fiber 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.

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

Thin Pad options let you extrude profiles from networks

Using the Thin Pad options you can extrude profiles from networks.

Thickness 1 and Thickness 2 are defined.
Checking the Merge Ends option trims extrusions to existing material.

Keep in mind that the creation order of the different elements constituting the profile never affects the resulting extrusion.
If you decide to use the options Up to Plane or Up to Surface, the Merge ends capability is not available.
 

How Extrusions are Trimmed

In the following example, the network goes beyond the edges of the part.

Initial profile is made of two intersecting lines The application trims extrusions to the faces of the pocket