PartDesign Chamfer

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Revision as of 08:28, 20 May 2022 by FBXL5 (talk | contribs) (properties added)
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PartDesign Chamfer.svg PartDesign Chamfer

Menu location
Part Design → Apply a dress-up feature → Chamfer
Default shortcut
Introduced in version
See also
PartDesign Fillet


This tool creates chamfers on the selected edges of an object. A new separate Chamfer entry (followed by a consecutive number if there are already existing chamfers in the document) is created in the Project tree.


  • Select a single edge, multiple edges or a face on an object, then start the tool either by clicking the button PartDesign Chamfer.svg Chamfer or using the menu PartDesign → Apply a dress-up feature → Chamfer. In case you selected a face or a 3D object (introduced in version 0.20) all its edges are respected for chamfering.
  • In the appearing Task panel you can define the chamfer in 3 ways:
    • Equal distance: The chamfer edges are equally distanced from the body edge.
    • Two distances: The distances of the chamfer edge to the body edge are specified. The distance direction can be flipped. introduced in version 0.19
    • Distance and angle: One distances of the chamfer edge to the body edge is specified. The second chamfer edge is defined by the angle of the chamfer. The distance direction can be flipped. introduced in version 0.19
  • If you want to add more edges or faces click the Add button and select edges and/or the faces.
  • After clicking the Add button you can add all edges of the object by right-clicking and selecting Add all edges from the context menu. introduced in version 0.20
  • If you want to remove edges or faces
    • either select the edge/face in the list of the dialog and press the DEL key. Note: Since there must be at least one edge for the feature, the last remaining edge or face in the list cannot be removed.
    • or click the Remove button. All edges and faces being previously selected are highlighted in purple. Select the edge or the face to be removed.
    • Ensure the Use all edges checkbox is unchecked or else some widgets in the dialog will be disabled. introduced in version 0.20
  • Click OK to validate.
  • For a chain of edges tangential to one another, one single edge can be selected; the chamfer will propagate along the chain.
  • To edit the chamfer after the function has been validated, either double-click on the chamfer label in the Project tree, or right-click on it and select Edit Chamfer.


  • PartDesign Chamfer should not be confused with Part Chamfer. Unless you know what you are doing, Part Chamfer should not be used on a PartDesign Body. See Part and PartDesign.
  • Chamfers cannot completely consume the adjacent faces.


See also: Property editor.

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



  • 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.


  • DataCamferType (Enumeration): Chamfer Type. "Type of chamfer".Equal distance (default), Two distances.
  • DataSize (QuantityConstraint): Size. "Size of chamfer". Default: 1,00 mm.
  • DataSize2 (QuantityConstraint): Size2. "Second size of chamfer". Default: 1,00 mm.
  • DataAngle (Angle): Angle. "Angle of chamfer". Default: 45,00 °.
  • DataFlipDirection (Bool): Flip Direction. "Flip direction". Default: false.
  • DataUseAllEdges (Bool): Use All Edges. "Chamfer all edges if true, else use only those edges in Base property.
If true, then this overrides any edge changes made to the Base property or in the dialog". Default: false.

Part Design

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

Known issues

See PartDesign Fillet.

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