PartDesign Fillet/tr

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



Usage

 * Select a single or multiple edges or a face on an object, then start the tool either by clicking its icon or going into the menu. In case you selected a face all its edges are respected for filleting.
 * In Fillet parameters in the Task Panel, set the fillet radius either by entering the value, or by clicking on the up/down arrows. The applied fillet is shown in real time.
 * If you want to add more edges or faces click first the Add ref button and then select the edge or the face.
 * If you want to remove edges or faces click the Remove ref button. All edges and faces being previously selected are highlighted in purple. Select the edge or the face to be removed.
 * Click OK to validate.
 * For a chain of edges tangential to one another, one single edge can be selected; the fillet will propagate along the chain.
 * To edit the fillet after the function has been validated, either double-click on the Fillet label in the Project tree, or right-click on it and select Edit Fillet.

PartDesign Fillet VS. Part Fillet
The PartDesign Fillet is not to be confused with its  Part workbench counterpart. Although they share the same name, they are not the same, and are not used the same way. Here is how they differ from each other:
 * The PartDesign Fillet is Parametric. After a fillet has been applied, its radius can be edited; this is not possible with the Part Fillet.
 * Edges must be selected on an object before activating the PartDesign Fillet. With the Part Fillet, the tool can be started, then a solid is selected, then edges.
 * The PartDesign Fillet creates a separate Fillet entry (followed by a sequential number if there are already existing fillets) in the Project tree. The Part Fillet becomes the parent of the object it was applied to.
 * The PartDesign Fillet offers a live preview of the fillet applied to the object before validating the function.
 * The Part Fillet supports variable radii (with a start radius and an end radius). The PartDesign fillet doesn't.

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 desgin 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.

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 :