PartDesign Fillet

Description
The PartDesign Fillet command creates fillets (rounds) on the selected edges of an object. It adds a Fillet object to the document with its corresponding representation in the Tree view.

Add a Fillet

 * 1) Optionally activate the Body to fillet (by double clicking the Tree view item).
 * 2) There are several ways to select edges to fillet:
 * 3) * Select one or more edge(s) of the active Body individually.
 * 4) * Select one or more face(s) on the active Body to select all surrounding edges at once.
 * 5) * Select the whole active Body to select all its edges at once.
 * 6) There are several ways to invoke the Fillet tool:
 * 7) * Press the button.
 * 8) * Select the option from the menu.
 * 9) The Fillet parameters dialog will open in the Task panel and allows to set several options.
 * 10) Click  to validate.


 * Remember:
 * For a chain of edges tangential to one another, one single edge can be selected; the fillet will propagate along the chain.
 * Since there must be at least one edge for the feature, the last remaining edge or face in the list cannot be removed.
 * Uncheck the checkbox to add or remove edges and/or faces individually.

Edit a Fillet

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

Options

 * : Set the fillet radius either by editing the value or by clicking on the up/down arrows.
 * : Add edges to the selection by pressing the button and selecting more edges or faces.
 * To select all remaining edges right-click in the list and select from the context menu.
 * : Choose a way to remove edges from the selection:
 * Select each edge or face in the list of the dialog and press the key or right-click in the list and select  from the context menu.
 * Press the button. All edges and faces being previously selected are highlighted in purple. Select each edge or face to be removed.
 * : Select all edges by checking the checkbox . This deactivates the selection list and the related buttons.

Properties
See also: Property editor.

A PartDesign Fillet 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.


 * : "Fillet radius". Default:.
 * : Use All Edges. "Fillet all edges if, else use only those edges in Base property.
 * If, then this overrides any edge changes made to the Base property or in the dialog". Default:.


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

Known issues
Fillets, chamfers, and other features that operate on solid bodies depend on the underlying OpenCASCADE Technology (OCCT) kernel that FreeCAD uses. The OCCT kernel occasionally has difficulty handling coincident sharp edges, where two faces meet. If this is the case FreeCAD may crash without an explanation.

If run from the terminal, FreeCAD may output a log like this one after the crash:

This output references functions located in, , etc., which are OCCT libraries. If this type of crashes occurs, the problem may need to be reported and solved in OCCT rather than in FreeCAD.

See the forum threads for more information:
 * Bug Chamfer bigger than 2mm crashes freecad
 * Segfault when using part design fillet

The user is also responsible for the integrity of his or her own model. Depending on the model, it may be impossible to perform a fillet or chamfer if the body is not big enough to support that operation. For example, it wouldn't be possible to create a 10 mm fillet if an edge is separated only 5 mm from the next surface. In that case, the maximum radius for a fillet would be 5 mm; trying to use a larger value may result in a shape that doesn't compute, or even a crash. If using the exact limit of 5 mm doesn't work, it may be possible to use a very close approximation, like 4.9999 mm, to produce the same visible result.

Topological naming
Edge numbers are not completely stable, therefore it is advisable that you finish the main design work of your solid body before applying features like fillets and chamfers, otherwise edges could change name and filleted edges would likely become invalid. When the property  is  there is some protection from this. Because in such cases all the edges of the base object are used and there is no dependence on individual edge names.

Read more in topological naming problem.

Scripting
The tool can be used in a macro, and, from the Python console using the following function:


 * 3 = radius
 * Box.Edges[2] = Edge with its number

Example: