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Circles and Ellipses

In one sentence: Draw complete circles or ellipses — by specifying their centre and a point on their perimeter, or by specifying three points that the curve passes through.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Circle / Ellipse
Toolbar: Sketcher Geometries (Conic dropdown) · Shortcut: G, C (default: Circle from Center)

The Conic group provides four tools for drawing closed conic sections:

Tool Shortcut Description
Circle From Center G, C Two clicks: centre, then a point on the rim
Circle From 3 Points G, 3, C Three clicks on the circumference
Ellipse From Center G, E, E Three clicks: centre, major-axis end, minor-axis end
Ellipse From 3 Points G, 3, E Three clicks: two on the ellipse, one to set minor radius

Intuition

A circle is the simplest closed curve — all points equidistant from the centre. Circle From Center is the most natural approach: place the centre where you want it, then drag out to set the radius. Circle From 3 Points is useful when you know three points the circle must pass through (e.g. three hole centres that define a bolt circle) and don't want to compute the centre yourself.

An ellipse is a stretched circle — it has a long axis (major) and a short axis (minor). Ellipse From Center asks you to place the centre, then click to establish the major axis direction and length, then click again for the minor axis.

When to use it

  • You need a circular boss, hole profile, slot end-cap, or any round feature.
  • You need an elliptical extrusion or decorative oval shape.
  • Three existing geometry points define the circle you need (Circle From 3 Points).

When NOT to use it

Step-by-step walkthrough

Circle from Center

  1. Press G, C or select Circle From Center from the toolbar dropdown.
  2. Click the centre point.
  3. Click a point on the circumference (or type a radius in the toolbar input field). The full circle appears.
  4. Constrain the circle — add a Radius/Diameter constraint to fix its size, and a Coincident or Lock Position constraint to fix its centre.

Circle from 3 Points

  1. Press G, 3, C or select Circle From 3 Points.
  2. Click three points on the desired circumference. FreeCAD computes the unique circle through these three points.
  3. Constrain if needed — the circle's radius and centre are already defined by the three points, so additional radius constraints are redundant unless those points are themselves unconstrained.

Ellipse from Center

  1. Press G, E, E or select Ellipse From Center.
  2. Click the ellipse centre.
  3. Click the end of the major axis (sets major radius direction and length).
  4. Click a point to set the minor radius (drag perpendicular to the major axis).
  5. Constrain the major and minor radii with Radius/Diameter constraints.

Parameters

Circle

Parameter Type Applied via
Radius Distance Radius/Diameter
Centre position Coordinate Lock Position or Coincident

Ellipse

Parameter Type Applied via
Major radius Distance Radius/Diameter applied to the major-axis edge
Minor radius Distance Radius/Diameter applied to the minor-axis edge
Major axis angle Angle Angle or Horizontal
Centre position Coordinate Lock Position or Coincident

Ellipse

An ellipse in Sketcher is stored as a Part::GeomEllipse with two focus points that are exposed as special construction vertices. The focus points can be constrained to specific positions if you want to drive the ellipse eccentricity by specifying the focal distance rather than the minor radius.

For many practical use cases (oval boss, decorative shape) simply constrain the major and minor radii directly and position the centre.

Common mistakes and pitfalls

Diameter vs radius confusion

Cause: When you apply a Radius/Diameter constraint to a circle, the tool auto-selects whether to show radius or diameter based on the circle's current appearance. Entering 10 when diameter mode is active gives a circle of diameter 10 (radius 5), not radius 10.
Fix: Check the constraint label — R 10 means radius 10, Ø 10 means diameter 10. Use the R (radius) shortcut K, R or Ø (diameter) shortcut K, O to force the mode you want.

Ellipse focus-point constraints conflict with radius constraints

Cause: Adding coincident constraints to the focus points while also constraining major and minor radii can over-constrain the ellipse.
Fix: Constrain either the foci or the radii — not both. For most designs, constrain the radii and leave the foci unconstrained.

Python API

Minimal example — circle

import FreeCAD as App
import Sketcher
import Part

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

# Draw a circle radius 15 centred at (20, 10)
circle = Part.Circle(App.Vector(20, 10, 0), App.Vector(0, 0, 1), 15)
idx = sketch.addGeometry(circle, False)

# Fix the radius
sketch.addConstraint(Sketcher.Constraint("Radius", idx, 15.0))
# Fix the centre with X/Y distance constraints from origin
sketch.addConstraint(Sketcher.Constraint("DistanceX", idx, 3, -1, 1, 20.0))
sketch.addConstraint(Sketcher.Constraint("DistanceY", idx, 3, -1, 1, 10.0))
doc.recompute()

Key geometry properties

Part.Circle returned from sketch.Geometry[idx]:

Property Type Description
Center App::Vector Circle centre coordinates
Radius float Radius in mm

Part.Ellipse has additional MajorRadius, MinorRadius, AngleXU (major axis angle).

See also