PartDesign Thickness/ru

The PartDesign Thickness tool transforms a solid body 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.

Base solid (A) → Solid with selected face to be opened (B) → Resulting hollow object (C)

1. Optionally activate the Body to apply the Thickness to.
2. Select one or more faces of the Body.
3. There are several ways to invoke the tool:
   • Press the Thickness button.
   • Select the Part Design → Apply a dress-up feature → Thickness option from the menu.
4. If there is no active Body, and there are two or more Bodies in the document, the Active Body Required dialog will open and prompt you to activate one. If there is a single Body it will be activated automatically.
5. The Thickness parameters task panel opens. See Options for more information.
6. Press the OK 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.

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

• Add face: Add faces to the selection by pressing the Add face button and selecting more faces.
• Remove face: Choose a way to remove faces from the selection:
  • Select one or more faces in the list and press the Del key or right-click the list and select Remove from the context menu.
  • Press the Remove face button. All previously selected faces are highlighted in purple. Select each face to be removed.
• Thickness: Set the wall thickness either by editing the value or by clicking the up/down arrows.
• Mode:
  • Skin: Select this option if you want to get an item like a vase, headless but with the bottom. Only this option can be selected.
  • Pipe: Not implemented. See this forum topic.
  • Recto Verso: Not implemented. See this forum topic.
• Join Type:
  • Arc: When non-tangential faces are offset, new faces that do not intersect are joined by a fillet with a radius equal to the defined thickness.
  • Intersection: When non-tangential faces are offset, new faces that do not intersect are extended to meet at their virtual intersection.
• Intersection: When checked, self-intersections in certain models are avoided. This option is not recommended as it relies on an incomplete OpenCASCADE method.
• Make thickness inwards: When checked, faces are offset inward.

• If thickness goes inwards, the value must be smaller than the smallest height of the Body.
• The tool may fail with complex shapes. Additive Pipe or Additive Loft may work better to create complex shapes.
• Known errors:
  • BRep_API: command not done.
  • BRep_Tool: no parameter on edge.
  • Silently fails.

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:

• ДанныеBase (LinkSub): Sub-link to the parent feature's list of selected edges and faces.
• ДанныеSupport Transform (Bool): 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: false.
• Данные (hidden)Add Sub Shape (PartShape)
• Данные (hidden)Base Feature (Link): Link to the parent feature.
• Данные (hidden)_ Body (LinkHidden): Link to the parent body.

Part Design

• ДанныеRefine (Bool): Refine shape (clean up redundant edges) after adding/subtracting. The default value is determined by the Automatically refine model after sketch-based operation preference. See PartDesign Preferences.

Thickness

• ДанныеValue (Length): Thickness value. Default: 1 mm.
• ДанныеMode (Enumeration): Mode. Skin (default), Pipe or Recto verso. Only Skin is implemented.
• ДанныеJoin (Enumeration): Join type. Arc (default) or Intersection.
• ДанныеReversed (Bool): Apply the thickness towards the solids interior. Default: false.
• ДанныеIntersection (Bool): Enable intersection-handling. Default: false.