Fillet¶

In one sentence: Round sharp edges of a solid by replacing them with a smooth circular arc of a specified radius.

Overview¶

Workbench: Part Design · Menu: Part Design → Dress-Up Features → Fillet
Toolbar: Part Design Dress-Up Features · Shortcut: none

Fillet selects one or more edges of the active Body's current solid and replaces each sharp edge with a smoothly curved surface whose cross-section is a circular arc. The operation modifies the existing solid in-place — it does not add a separate feature body — and the result remains parametric: changing the radius updates the shape immediately.

Intuition¶

Think of sanding the corner of a wooden block. The sharp 90-degree edge is replaced by a smooth curved surface. The radius of that curve is exactly what you set in the Fillet dialog: a small radius gives a barely-there bevel, while a large radius gives a sweeping curve that eats noticeably into both adjacent faces.

The key constraint is that the radius cannot exceed half the width of either adjacent face — if the fillet circle is too large to fit between the two faces it touches, FreeCAD (and the underlying OCCT kernel) cannot construct a valid solid. A common sign that the radius is too large is the error "Fillet not possible on selected shapes."

The tool works on any combination of straight and curved edges, including edges that form a continuous chain around a pocket or boss. When you select a face instead of individual edges, FreeCAD fillets all edges that bound that face.

When to use it¶

You want to remove sharp corners from a machined part to reduce stress concentrations.
You are modelling a plastic injection moulded part, where all internal and external corners need a blend radius for mould-release and structural reasons.
You need a cosmetic rounded edge on a consumer product model.
You want to fillet all edges of a solid at once (use the Use All Edges option).
You are preparing a model for FEA and need chamfer-free, smooth transitions at stress-critical edges.

When NOT to use it¶

You want a flat, angled cut rather than a curved blend — use Chamfer instead.
The edge you want to round is on a sketch, not on a solid — round the sketch geometry with a Sketcher fillet or constrained arc before padding it.
You need a blend between two bodies — use Part workbench Boolean operations followed by a Part Fillet; PartDesign Fillet only operates on features inside the current Body.

Step-by-step walkthrough¶

Prerequisite: An active Body containing at least one solid feature (a Pad, Revolution, or similar). The solid must have edges to fillet.

Select the edges to fillet. In the 3-D viewport or the model tree, click one or more edges of the solid. Holding Ctrl lets you add edges to the selection. You may also select a face to auto-select all its bounding edges. Alternatively, skip pre-selection and use the task panel's reference list after opening the tool.
Open Fillet. Go to Part Design → Dress-Up Features → Fillet, or click the Fillet button in the Part Design Dress-Up Features toolbar.
The task panel opens showing a Fillet radius field and a list of selected edges.

No edges in the list

If the reference list is empty, click Add Reference in the task panel and then click each edge in the viewport.
Set the radius. Type a value in the Fillet radius field or use the spin box. The preview updates in real time. A radius of 1 mm is the default.
Optionally enable Use All Edges. Tick Use all edges to apply the fillet to every edge of the solid. When this is on, the edge list is ignored.
Click OK to confirm. The Fillet feature appears in the model tree below the feature it modifies.

Tip

Right-click an edge in the reference list to remove it. Right-click the viewport and choose Add all edges to populate the list with every edge on the solid.

Parameters¶

Parameter	Type	Default	Description
Fillet radius	Length	`1 mm`	The radius of the circular arc that replaces each selected edge. Must be greater than zero. Valid range: `> 0` to the maximum length that fits on the narrowest adjacent face.
Use all edges	Toggle	off	When enabled, all edges of the base solid are filleted; the reference list is ignored.
References (edge list)	Sub-element links	—	The individual edges or faces whose edges will be rounded. Active only when Use all edges is off.

Advanced usage¶

Continuous-edge propagation¶

FreeCAD automatically includes edges that are tangentially continuous with the ones you select. If you select one edge of a smoothly rounded pocket, all tangent-connected edges in that chain are filleted together. This is the getContinuousEdges behaviour from the source, and it prevents OCCT from failing at tangent junctions.

Variable-radius fillet¶

PartDesign Fillet applies a constant radius to all selected edges. If you need a variable radius along a single edge (a tapered fillet), use the Part workbench Fillet feature (Part::Fillet), which exposes OCCT's variable- radius API.

Fillet ordering and feature tree position¶

Fillets are applied after all other features above them in the tree. Applying a large fillet before a pocket that cuts through the filleted face can produce unexpected results. As a rule of thumb: add fillets and chamfers last, after all material-adding and material-removing operations are complete.

Common mistakes and pitfalls¶

Fillet not possible on selected shapes

Cause: The radius is too large for the geometry. The fillet arc cannot fit between the two faces adjacent to the edge — it would extend past one of them.
Fix: Reduce the radius, or select fewer edges and fillet them at a smaller radius first.

Resulting shape is null

Cause: OCCT produced an empty result, typically because the combination of edges and radius creates self-intersecting geometry.
Fix: Try filleting edges one at a time, using smaller radii, or avoid filleting edges that meet at very acute angles.

Result has multiple solids

Cause: The fillet operation split the solid into disconnected pieces (rare but possible on thin features).
Fix: Enable Allow Compound in the active Body settings, or redesign the geometry to avoid the problematic edge combination.

Empty fillet created

Cause: You clicked OK with no edges in the reference list and Use all edges was off.
Fix: Re-open the feature (double-click it in the model tree), click Add Reference, and select at least one edge.

Python API¶

Minimal example¶

import FreeCAD as App
import PartDesign
import Sketcher
import Part

doc = App.newDocument()

# Create a body with a simple box (padded rectangle)
body = doc.addObject("PartDesign::Body", "Body")

sketch = doc.addObject("Sketcher::SketchObject", "Sketch")
body.addObject(sketch)
sketch.addGeometry(Part.LineSegment(App.Vector(0,0,0), App.Vector(10,0,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(10,0,0), App.Vector(10,10,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(10,10,0), App.Vector(0,10,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(0,10,0), App.Vector(0,0,0)), False)
sketch.addConstraint(Sketcher.Constraint("Coincident", 0,2, 1,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 1,2, 2,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 2,2, 3,1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 3,2, 0,1))
doc.recompute()

pad = doc.addObject("PartDesign::Pad", "Pad")
body.addObject(pad)
pad.Profile = sketch
pad.Length = 10.0
doc.recompute()

# Add a fillet to all edges
fillet = doc.addObject("PartDesign::Fillet", "Fillet")
body.addObject(fillet)
fillet.Base = (pad, [])          # base feature; edge list populated separately
fillet.Radius = 1.0              # 1 mm radius  # TODO: verify edge selection API
fillet.UseAllEdges = True
doc.recompute()

Resulting feature properties¶

Property	Type	Description
`Radius`	`App::PropertyQuantityConstraint`	The fillet radius in document length units. Minimum: `0`, step: `0.1`.
`UseAllEdges`	`App::PropertyBool`	When `True`, all edges of the base shape are filleted, overriding any edge list in `Base`. Default: `False`.
`Base`	`App::PropertyLinkSub`	Link to the base feature and the list of selected sub-edges or sub-faces. Inherited from `DressUp`.
`SupportTransform`	`App::PropertyBool`	Allow the dress-up to follow pattern transformations. Inherited from `DressUp`.