PartDesign Thickness

Description
The Thickness tool works on a solid Body and transforms it into a thick-walled hollow object with at least one open face, giving to each of its remaining faces a uniform thickness. On some solids it allows you to significantly speed up the work, and avoids making extrusions and pockets.



Usage

 * 1) Select one or more face(s) on the active Body.
 * 2) Press the  button.
 * 3) Define the Thickness parameters (see Options).
 * 4) To add more faces to open, press the  button and select a face in the 3D view.
 * 5) To remove a previously select face, press the  button and select a face in the 3D view, or right-click on the Face label in the list and select Remove.
 * 6) Press.

Options

 * Thickness: Wall thickness of the resulting object. Set the desired value.
 * Mode
 * Skin: Select this option if you want to get an item like a vase, headless but with the bottom
 * Pipe: Select this option if you want to get an object like a pipe, headless and bottomless. In this case it may be convenient to select the faces to be deleted before you start the tool. Helping with predefined views buttons or use the numeric keys.
 * Recto Verso:
 * (In case you wonder: Pipe and Recto Verso functionality hasn't been implemented since version 0.13, see 2013 topic and 2021 follow-up)


 * Join Type
 * Arc: removes the outer edges and creates a fillet with a radius equal to the defined thickness.
 * Intersection: when faces are offset outward, sharp edges are kept between faces.
 * Make thickness inwards: when checked, faces are offset inward.

Limitations

 * At least one face to be opened must be selected.
 * If thickness goes inwards, the value must be smaller than the smallest height of the Body.
 * The command may fail with complex shapes. In this context the surface of e.g. a cone has already to be regarded as complex.
 * Additive Pipe or Additive Loft may work better to create complex shapes

Example

 * 1) Create a Pad from the sketch
 * 2) Create a second sketch on the XY plane
 * 3) Create a second Pad from the second sketch

As in the following pictures:







Then
 * 1) Select a circular face
 * 2) Select
 * 3) Add the other circular faces to the selection

Result:

Known Errors

 * BRep_API: command not done
 * BRep_Tool: no parameter on edge
 * Silently Fails