PartDesign Thickness

Draft

Boolean operation

PartDesign

PartDesign Thickness
Menu location
Part Design → Apply a dress-up feature → Thickness
Workbenches
PartDesign
Default shortcut
None
Introduced in version
0.17
See also
Part 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.

The thickness tool applied to a face (B) of a solid (A), resulting in the hollow object (C).

Usage

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

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.

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

• DataBase (LinkSub): Base. Sub-link to the parent feature's list of selected edges and faces.
• DataSupportTransform (Bool): 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: false.

• Data (hidden)AddSubShape (PartShape): Add Sub Shape.
• Data (hidden)BaseFeature (Link): Base Feature. Link to the parent feature.
• Data (hidden)_Body (LinkHidden): _Body. Hidden link to the parent body.

Part Design

• DataRefine (Bool): "Refine shape (clean up redundant edges) after adding/subtracting". Default: true.

Thickness

• DataValue (Length): Value. "Thickness value". Default: 1,00 mm.
• DataMode (Enumeration): Mode. Skin (default), Pipe (seems to be useless).

("Recto verso" isn't even listed here...)

• DataJoin (Enumeration): Join. "Join type".Arc (default).
• DataReversed (Bool): Reversed. "Apply the thickness towards the solids interior". Default: false.
• DataIntersection (Bool): Intersection. "Enable intersection-handling". Default: false.

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:

File:Braga-primoPad.png

File:Braga-secondoschizzo.png

File:Braga-secondo Pad.png

Then

1. Select a circular face
2. Select Thickness
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

Draft

Boolean operation

PartDesign

PartDesign

• Structure tools: Part, Group
• Helper tools: Create body, Create sketch, Edit sketch, Map sketch to face

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• Modeling tools
  • Datum tools: Create a datum point, Create a datum line, Create a datum plane, Create a local coordinate system, Create a shape binder, Create a sub-object(s) shape binder, Create a clone
  • Additive tools: Pad, Revolution, Additive loft, Additive pipe, Additive helix, Additive box, Additive cylinder, Additive sphere, Additive cone, Additive ellipsoid, Additive torus, Additive prism, Additive wedge
  • Subtractive tools: Pocket, Hole, Groove, Subtractive loft, Subtractive pipe, Subtractive helix, Subtractive box, Subtractive cylinder, Subtractive sphere, Subtractive cone, Subtractive ellipsoid, Subtractive torus, Subtractive prism, ‎Subtractive wedge

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• Transformation tools: Mirrored, Linear Pattern, Polar Pattern, Create MultiTransform, Scaled
• Dress-up tools: Fillet, Chamfer, Draft, Thickness
• Boolean: Boolean operation

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• Extras: Migrate, Sprocket, Involute gear, Shaft design wizard
• Context menu: Set tip, Move object to other body, Move object after other object, Appearance, Color per face

User documentation

• Getting started
• Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
• Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate

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• Help: Tutorials, Video tutorials
• Workbenches: Std Base, Arch, Assembly, CAM, Draft, FEM, Inspection, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Start, Surface, TechDraw, Test Framework, Web

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• Addons: Addon Manager, External workbenches, Scripting and macros

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• Hubs: User hub, Power users hub, Developer hub