PartDesign Thickness

Description
The PartDesign Thickness tool 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) Make sure the correct body is active. If required double-click it in the Tree view.
 * 2) Select one or more face(s) of the active Body.
 * 3) There are several ways to invoke the tool:
 * 4) * Press the button.
 * 5) * Select the option from the menu.
 * 6) The  task panel opens. See Options for more information.
 * 7) Press the  button to finish.


 * 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) Do one of the following:
 * 2) * Double-click the Thickness object in the Tree view
 * 3) * Right-click the Thickness object in the Tree view and select from the context menu.
 * 4) The  task panel opens. See Options for more information.
 * 5) Press the  button to finish.

Options

 * : Add faces to the selection by pressing the button and selecting more faces.
 * : Choose a way to remove faces from the selection:
 * Select one or more faces in the list and press the key or right-click the list and select  from the context menu.
 * Press the button. All previously selected faces are highlighted in purple. Select each face to be removed.
 * : Set the wall thickness either by editing the value or by clicking the up/down arrows.
 * : Select this option if you want to get an item like a vase, hollow with only a single opening.
 * : Not implemented. See this forum topic.
 * : Not implemented. See this forum topic.
 * : When non-tangential faces are offset, new faces that do not connect are joined by a fillet with a radius equal to the defined thickness.
 * : When non-tangential faces are offset, new faces that do not connect are extended to meet at their intersection.
 * : This checkbox seems to be obsolete.
 * : When checked, faces are offset inward.
 * : This checkbox seems to be obsolete.
 * : 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

 * : Sub-link to the parent feature's list of selected edges and faces.
 * : "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:.
 * : Link to the parent feature.
 * : Link to the parent body.
 * : Link to the parent body.


 * : "Refine shape (clean up redundant edges) after adding/subtracting". The default value is determined by the preference. See PartDesign Preferences.


 * : "Thickness value". Default:.
 * : "Mode". (default),  or . Only  is implemented.
 * : "Join type". (default) or.
 * : "Apply the thickness towards the solids interior". Default:.
 * : "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