PartDesign Thickness

Description
The PartDesign Thickness command works on a solid body and transforms it into a hollow object with at least one open face, giving to each of its remaining faces a uniform thickness. It adds a Thickness object to the document with its corresponding representation in the Tree view.



Add a thickness

 * 1) Optionally activate the Body to apply Thickness to (by double clicking the Tree view item).
 * 2) Select one or more face(s) of the active Body.
 * 3) There are several ways to invoke the Thickness tool:
 * 4) * Press the button.
 * 5) * Select the option from the menu.
 * 6) The Thickness parameters dialog will open in the Task panel and allows to set several options.
 * 7) Click  to validate.


 * Remember:
 * Since there must be at least one face for the feature, the last remaining face in the list cannot be removed.

Edit a thickness

 * 1) There are two ways to reopen the Thickness parameters dialog to edit a Thickness:
 * 2) * Double-click on the Thickness item in the Tree view
 * 3) * Right-click on the Thickness item in the Tree view and select from the context menu.
 * 4) The Thickness parameters dialog will open in the Task panel and allows to set several options.
 * 5) Click  to validate.

Options

 * : Set the desired wall thickness of the resulting object either by editing the value or by clicking on the up/down arrows.
 * : Select this option if you want to get an item like a vase, headless but with the bottom
 * : Select this option if you want to get an object like a pipe, headless and bottomless.
 * (In case you wonder: Pipe and Recto Verso functionality hasn't been implemented since version 0.13, see 2013 topic and 2021 follow-up)
 * (In case you wonder: Pipe and Recto Verso functionality hasn't been implemented since version 0.13, see 2013 topic and 2021 follow-up)
 * (In case you wonder: Pipe and Recto Verso functionality hasn't been implemented since version 0.13, see 2013 topic and 2021 follow-up)


 * : Removes the outer edges and creates a fillet with a radius equal to the defined thickness.
 * : When faces are offset outward, sharp edges are kept between faces.
 * : When checked, faces are offset inward.
 * : When checked, faces are offset inward.

Properties
See also: Property editor.

A PartDesign Thickness object is derived from a Part Feature object and inherits all its properties. It also has the following additional properties:

Data

 * : Base. Sub-link to the parent feature's list of selected edges and faces.
 * : Support Transform. "Include the base additive/subtractive shape when used in pattern features.
 * If disabled, only the dressed part of the shape is used for patterning. Default:.


 * : Add Sub Shape.
 * : Base Feature. Link to the parent feature.
 * : _Body. Hidden link to the parent body.


 * : "Refine shape (clean up redundant edges) after adding/subtracting". Default:.


 * : Value. "Thickness value". Default:.
 * : Mode. (default),  (seems to be useless).
 * ("Recto verso" isn't even listed here...)


 * : Join. "Join type". (default).
 * : Reversed. "Apply the thickness towards the solids interior". Default:.
 * : Intersection. "Enable intersection-handling". Default:.

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