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Fillet / Chamfer

In one sentence: Round two lines into a smooth arc at their meeting point (Fillet) or clip the corner with a straight cut (Chamfer), in either case adjusting the lines automatically to preserve the overall shape.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Fillet / Chamfer
Toolbar: Sketcher Geometries (Fillet dropdown) · Shortcut: none

Tool Description
Fillet Replace a sharp corner with a circular arc of a specified radius
Chamfer Replace a sharp corner with a straight line at 45° (or custom angle)

Both tools operate on an existing corner (the intersection of two lines). After applying them, the two lines are trimmed and the new transition element (arc or line) is inserted and constrained.

Intuition

When you draw two lines that meet at a corner, the corner is sharp. Fillet "rounds it off" by inserting a small arc, like the rounded corner of a piece of sheet metal bent gently rather than cracked at a sharp fold. Chamfer "cuts the corner" with a straight diagonal line, like the bevelled edge of a machine part.

Both tools trim the original lines back to where the arc or chamfer line begins, then add the transition element with tangency (Fillet) or endpoint (Chamfer) constraints.

When to use it

  • Fillet: Sheet metal forms, injection-moulded parts, any profile where a sharp corner would create a stress concentration.
  • Chamfer: Machined parts where a small angled flat is the standard transition (bolt heads, shaft undercuts).
  • You want to add the transition in 2-D sketch space rather than using the Part Design Fillet or Chamfer dress-up (which works on 3-D edges); the sketch-level tools are better when the profile is the primary design element.

When NOT to use it

  • You need to round a 3-D solid edge — use Part Design Fillet or Part Design Chamfer on the solid instead.
  • You need a fillet between two arcs — the Fillet tool works on line-to-line corners; arc-to-arc transitions require manual arc insertion with tangent constraints.

Step-by-step walkthrough

Fillet

  1. Enter sketch edit mode with the sketch containing the corner you want to round.
  2. Activate Fillet from the Fillet dropdown in the toolbar or menu.
  3. Click the corner point (the vertex where the two lines meet). A circular arc appears, trimming the two lines.
  4. Set the radius:
    • In the task panel input field that appears, type the desired radius and press Enter, or
    • Apply a Radius/Diameter constraint to the arc after creation.
  5. Repeat for other corners, then press Esc to exit the tool.

Chamfer

  1. Enter sketch edit mode.
  2. Activate Chamfer from the Fillet dropdown.
  3. Click the corner point. A short diagonal line appears.
  4. Set the chamfer size:
    • Type the distance value in the task panel input, or
    • Apply Distance constraints to the chamfer line endpoints after creation.

Tip

To produce a 45° chamfer of a specific size, add a Horizontal Distance constraint to one endpoint of the chamfer line and an Equal constraint to force the X and Y offsets to be equal.

Parameters

Fillet

Parameter Type Applied via
Radius Distance Radius/Diameter on the resulting arc

Chamfer

Parameter Type Applied via
Chamfer leg length Distance Distance on either endpoint

Common mistakes and pitfalls

Fillet fails with 'Not enough space for fillet'

Cause: The requested radius is larger than the shorter of the two lines. There is not enough room to trim both lines and still have geometry remaining.
Fix: Use a smaller radius, or extend the lines before filleting.

Fillet arc is not tangent to both lines

Cause: The arc was inserted correctly but a manual constraint deleted or overrode the automatic tangent constraints.
Fix: Check the arc's constraints and re-add Tangent constraints between the arc and each adjacent line if they are missing.

Python API

Minimal example

import FreeCAD as App
import Sketcher

doc = App.activeDocument()
sketch = doc.getObject("Sketch")

# Apply a fillet between geo 0 and geo 1, both lines meeting at point 2/1
# The fillet is applied at the shared vertex.
sketch.fillet(0, 2, 1, 1, 3.0, True, False)
# Args: geo1, vertex1, geo2, vertex2, radius, trim, createCorner
doc.recompute()

Key method signature

sketch.fillet(
    geo1,          # int — index of first line
    vertex1,       # int — vertex on first line (1=start, 2=end)
    geo2,          # int — index of second line
    vertex2,       # int — vertex on second line
    radius,        # float — fillet radius in mm
    trim,          # bool — trim original lines to fillet (True recommended)
    createCorner,  # bool — keep the original corner point (usually False)
)

See also