Chamfer¶

In one sentence: Cut a flat angled bevel along selected edges of a solid, replacing each sharp corner with a planar face.

Overview¶

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

Chamfer replaces one or more sharp edges of the active Body's solid with a flat angled face. Three geometric modes are available: equal distance from both adjacent faces, two independent distances, or a distance combined with an angle. Like all dress-up features, Chamfer is fully parametric — changing any dimension updates the solid immediately.

Intuition¶

Imagine filing the corner of a metal bracket at 45 degrees. The sharp edge is replaced by a small flat face set at an angle to both original surfaces. That is an equal-distance chamfer: both adjacent faces are trimmed by the same amount.

In contrast, Two distances mode lets you set different setbacks on each side, creating an asymmetric bevel. Distance and Angle mode lets you control one setback distance and the angle of the chamfer face, which is equivalent to specifying how far back from the edge the bevel starts and how steep it is.

The difference between Chamfer and Fillet is simple: Fillet gives a smooth curved surface; Chamfer gives a flat face. Chamfers are common in machined metal parts (to break sharp edges and allow assembly), while fillets are more common in cast or moulded parts (for strength and mould release).

When to use it¶

You need to break a sharp edge on a machined part for safety or assembly reasons (a 45° chamfer at 0.5 mm is a very common engineering callout).
You are modelling a countersunk screw hole and want the conical lead-in.
You need an asymmetric bevel where different amounts of material are removed from each side of an edge.
You want to combine a distance with an angle — for example, a chamfer that starts 2 mm back from the edge and is inclined at 60°.
You need to add a chamfer to every edge at once (use Use All Edges).

When NOT to use it¶

You want a smooth curved blend rather than a flat cut — use Fillet instead.
The edge is on a sketch profile — add a chamfer geometry directly in Sketcher before padding it.
You are working on a Part workbench solid outside a Body — use Part::Chamfer from the Part workbench.

Step-by-step walkthrough¶

Prerequisite: An active Body with at least one solid feature containing edges.

Select the edges to chamfer. Click one or more edges in the 3-D viewport. Hold Ctrl to add edges to the selection. You may also select a face to pick all its bounding edges. Pre-selection is optional — you can add edges from the task panel.
Open Chamfer. Go to Part Design → Dress-Up Features → Chamfer, or click the Chamfer button in the Part Design Dress-Up Features toolbar.
Choose the chamfer type. In the task panel, select one of:
- Equal distance — one distance value; both sides trimmed equally.
- Two distances — separate Size (first side) and Size2 (second side).
- Distance and Angle — Size controls the setback on the first side; Angle controls the inclination of the chamfer face.
Set the size. Type a value in the Size field. Default is 1 mm.
Set Size2 or Angle if you chose Two distances or Distance and Angle.
Flip direction if needed. For Two distances and Distance and Angle modes, tick Flip direction to swap which adjacent face receives Size versus Size2 (or which side the angle is measured from).
Click OK. The Chamfer feature is added to the model tree.

Tip

Enable Use all edges to apply the same chamfer to every edge on the solid at once, without selecting individual edges.

Parameters¶

Parameter	Type	Default	Description
Type	Dropdown	`Equal distance`	The geometric mode: `Equal distance`, `Two distances`, or `Distance and Angle`. See deep dive below.
Size	Length	`1 mm`	Setback distance on the first (or only) side. Must be > 0.
Size2	Length	`1 mm`	Setback distance on the second side. Active only in Two distances mode. Must be > 0.
Angle	Angle	`45°`	Inclination of the chamfer face. Active only in Distance and Angle mode. Range: > 0° and < 180°.
Flip direction	Toggle	off	Swaps which face receives Size vs Size2 (or the angle reference). Disabled in Equal distance mode.
Use all edges	Toggle	off	Chamfers every edge on the solid; the reference list is ignored.
References (edge list)	Sub-element links	—	Edges to chamfer. Active only when Use all edges is off.

Type in depth¶

The Type dropdown controls the geometry of the chamfer face — specifically, how the two measurements that define the bevel are specified.

Equal distance (default)¶

Both sides of the chamfer set back by the same distance (Size). The chamfer face bisects the angle between the two adjacent faces symmetrically.

Intuition: imagine sanding a 45° bevel where both faces are touched equally — regardless of what angle the original edge subtends, each adjacent face loses the same amount of material.

Use this mode when: - You want a clean symmetric bevel and the setback is the same on both sides - Dimensioning by a single value (callout: "chamfer 1×45°" in machining) - The two adjacent faces meet at 90° (the most common case)

Watch out for: On edges where the two faces meet at an angle other than 90°, "equal distance" still means equal setback, not a 45° angle face. The chamfer face angle will vary depending on the dihedral angle of the edge.

Two distances¶

Each side of the chamfer has an independent setback: Size on the first face and Size2 on the second face. The chamfer face is a plane that connects the two setback lines.

Intuition: one side retreats 2 mm and the other retreats 0.5 mm — like a ramp that is steep on one side and shallow on the other.

Use this mode when: - The chamfer must be asymmetric (e.g. more clearance on one side than the other) - Matching a specific engineering callout (e.g. "chamfer 2 × 0.5") - The edge connects faces of different functional importance and each needs its own setback

Sub-parameters active: Size2, Flip direction

Watch out for: FreeCAD assigns "first face" and "second face" based on topological face index, which is not always predictable from the viewport. If the result looks swapped, click Flip direction — this is the correct fix, not changing which edge you selected.

Distance and angle¶

One side is set back by Size and the chamfer face is inclined at Angle from that face. The second side's setback is derived from the geometry.

Intuition: lay a ruler flat on one face, measure Size in from the edge, then tilt a blade up from that point at Angle degrees — the tilted blade face is the chamfer.

Use this mode when: - The chamfer is specified by one distance and one angle (common in machining drawings: "chamfer 1 mm × 30°") - The chamfer needs to reach a specific depth on one face while the angle is the primary design constraint - You are modelling a chamfer that guides a fastener into a hole (60°–90° entry chamfers)

Sub-parameters active: Angle, Flip direction

Watch out for: The angle is measured from the first face to the chamfer surface — not from the edge bisector. If the angle is applied from the wrong face, the result will look correct in angle but incorrect in which face is being measured from. Use Flip direction to change the reference face.

Advanced usage¶

Migration from FreeCAD 0.21¶

Files created in FreeCAD 0.21 with Two distances or Distance and Angle chamfers will have their FlipDirection property automatically adjusted when opened in 1.x because the interpretation of Size and Size2 was reversed. Re-saving in 1.x and re-opening in 0.21 will again produce a different result — this is a known one-way migration.

Common mistakes and pitfalls¶

Size must be greater than zero

Cause: A size value of zero or negative was entered.
Fix: Enter a positive value in the Size (and Size2 if applicable) field.

Angle must be greater than 0 and less than 180

Cause: In Distance and Angle mode, the angle is outside the valid range.
Fix: Enter an angle strictly between 0° and 180°. Typical values are between 15° and 75°; 45° is the most common.

Chamfer result looks correct in one mode but wrong after flipping

Cause: The Flip direction checkbox swaps which face is the reference for Size. In asymmetric modes the visual result changes completely.
Fix: Think of Size as "how far back on the face I first clicked" and Size2 as "how far back on the other face." Use Flip direction if the assignment is reversed.

Failed to create chamfer

Cause: The geometry at the selected edge(s) is incompatible with the chosen chamfer size — often because the size is larger than the adjacent face or the edge is part of a complex curve.
Fix: Reduce the size, select fewer edges, or chamfer edges individually to isolate the problem edge.

Python API¶

Minimal example¶

import FreeCAD as App
import PartDesign
import Sketcher
import Part

doc = App.newDocument()

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(20,0,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(20,0,0), App.Vector(20,20,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(20,20,0), App.Vector(0,20,0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(0,20,0), 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 = 15.0
doc.recompute()

# Equal-distance chamfer on all edges, 1 mm
chamfer = doc.addObject("PartDesign::Chamfer", "Chamfer")
body.addObject(chamfer)
chamfer.Base = (pad, [])         # TODO: verify edge sub-element selection syntax
chamfer.ChamferType = 0          # 0 = "Equal distance"
chamfer.Size = 1.0               # 1 mm setback on both sides
chamfer.UseAllEdges = True
doc.recompute()

Resulting feature properties¶

Property	Type	Description
`ChamferType`	`App::PropertyEnumeration`	`0` = `"Equal distance"`, `1` = `"Two distances"`, `2` = `"Distance and Angle"`. Default: `0`.
`Size`	`App::PropertyQuantityConstraint`	First (or only) setback distance. Minimum: `0`, step: `0.1`. Default: `1 mm`.
`Size2`	`App::PropertyQuantityConstraint`	Second setback distance; used only when `ChamferType` is `1`. Default: `1 mm`.
`Angle`	`App::PropertyAngle`	Chamfer face inclination; used only when `ChamferType` is `2`. Valid range: `0°`–`180°` exclusive. Default: `45°`.
`FlipDirection`	`App::PropertyBool`	Swaps the reference faces for asymmetric types. Default: `False`.
`UseAllEdges`	`App::PropertyBool`	Apply to every edge of the base shape. Default: `False`.
`Base`	`App::PropertyLinkSub`	Link to the base feature and selected sub-edges/faces. Inherited from `DressUp`.