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Arcs (Circular, Elliptical, Hyperbolic, Parabolic)

In one sentence: Draw curved arc segments — from simple circular arcs to conic section arcs — that can be joined with lines or other curves to form complex sketch profiles.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Arc
Toolbar: Sketcher Geometries (dropdown) · Shortcut: G, A (default: Arc from Center)

The Arc group contains five arc tools grouped under one toolbar dropdown:

Tool Shortcut Description
Arc From Center G, A Three clicks: center, start angle, end angle
Arc From 3 Points G, 3, A Three clicks: start, end, and a point on the arc
Elliptical Arc G, E, A Elliptical arc section (arc of an ellipse)
Hyperbolic Arc G, H Arc of a hyperbola
Parabolic Arc G, J Arc of a parabola

For most work, use Arc From Center or Arc From 3 Points. The conic arcs (elliptical, hyperbolic, parabolic) are specialised tools for optical and mathematical geometry.

Intuition

A circular arc is a portion of a circle — think of trimming a circle to just the segment you need. Arc From Center specifies where the centre is and the angular sweep; Arc From 3 Points specifies two endpoints and one intermediate point and FreeCAD computes the circle that passes through all three.

The conic arcs follow the same principle but with non-circular curves: an elliptical arc is a portion of an ellipse, a hyperbolic arc is a portion of one branch of a hyperbola, and a parabolic arc is a portion of a parabola.

When to use it

  • You need a rounded corner or curved section in a profile (use Arc From Center or From 3 Points).
  • You are drawing a cam profile, a gear tooth, or any shape whose outline follows a circular arc.
  • You need an elliptical slot or transition curve (Elliptical Arc).
  • You are designing optical elements (mirrors, lenses) that require exact conic sections (Hyperbolic Arc, Parabolic Arc).

When NOT to use it

Step-by-step walkthrough

Arc From Center

  1. Press G, A or select Arc From Center from the toolbar dropdown.
  2. Click the centre point.
  3. Click the arc start point (sets the radius and start angle).
  4. Click the arc end point (sets the end angle; the arc sweeps CCW by default).
  5. Constrain the arc — add radius, centre position, and angular constraints.

Arc From 3 Points

  1. Press G, 3, A or select Arc From 3 Points.
  2. Click the first endpoint of the arc.
  3. Click the second endpoint (the arc will span between these two points).
  4. Click a third point that lies on the arc body between the endpoints. FreeCAD computes the unique circle through these three points and draws the arc.
  5. Constrain as needed.

Elliptical Arc

  1. Press G, E, A.
  2. Click the ellipse centre.
  3. Click a point on the major semi-axis (sets the major radius direction and length).
  4. Click a point to set the minor radius (perpendicular drag).
  5. Click the arc start point and end point to define the angular sweep.

Tip

Use a Symmetry or Equal constraint on the two semi-axes to make the ellipse a circle; or control both radii with Radius constraints.

Parameters

Arc From Center / Arc From 3 Points

Parameter Type Applied via
Radius Distance Radius/Diameter
Centre position Coordinate Lock Position or Coincident
Start / end angle Angle Angle on endpoint reference

Elliptical Arc

Parameter Type Applied via
Major radius Distance Radius/Diameter
Minor radius Distance Radius/Diameter
Major axis angle Angle Angle
Centre position Coordinate Lock Position

Elliptical arc

An elliptical arc is defined by its centre, major axis direction, major and minor radii, and the start/end angles of the arc portion. It is stored as a Part::GeomArcOfEllipse.

Internally, an elliptical arc has two focus points (special geometry attached to the arc). These are visible as small construction points; they participate in constraints and can be used to constrain the eccentricity of the ellipse.

Hyperbolic and parabolic arcs

These are mathematically precise conic sections, not approximations. They are most useful in optical design (parabolic mirrors, hyperbolic lenses) and in architectural geometry (hyperbolic cooling towers, parabolic arches).

Hyperbolic arc is defined by centre, one vertex of the hyperbola, and a point on the arc. Two focus points are also available as constraint handles.

Parabolic arc is defined by the focal point, a point on the directrix, and a point on the parabola. The focus is the primary constraint handle.

Advanced usage

Mixing arcs and lines in a Polyline

Inside Polyline mode, press M to toggle between line and arc sub-modes. The junction between a line and an arc in Polyline mode automatically gets a Tangent constraint, giving you smooth blended corners.

Toggling arc direction

During Arc From Center placement, clicking on the opposite side of the centre from the intended sweep reverses the arc direction (CW vs CCW). After creation, edit the arc endpoints to change which sector is kept.

Common mistakes and pitfalls

Arc is the wrong portion of the circle

Cause: The arc sweeps the larger sector when you expected the smaller one (or vice versa).
Fix: Select the arc, open its properties, and swap the StartAngle and EndAngle; or delete and re-draw clicking in a different order.

Elliptical arc focus points show as red (conflicting)

Cause: The focus points have been over-constrained by coincident or distance constraints that conflict with the ellipse geometry.
Fix: Remove duplicate constraints on the focus points — they are derived from the radii and should generally be left unconstrained unless you specifically want to drive the eccentricity via the foci.

Python API

Minimal example — circular arc

import FreeCAD as App
import Sketcher
import Part

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

# Arc from center (0,0), radius 10, from 0° to 90°
import math
arc = Part.ArcOfCircle(
    Part.Circle(App.Vector(0, 0, 0), App.Vector(0, 0, 1), 10),
    0,           # start angle (radians)
    math.pi / 2  # end angle
)
idx = sketch.addGeometry(arc, False)
# Constrain centre to origin
sketch.addConstraint(Sketcher.Constraint("Coincident", idx, 3, -1, 1))
# Fix radius
sketch.addConstraint(Sketcher.Constraint("Radius", idx, 10.0))
doc.recompute()

Key geometry properties

Property Type Description
Center App::Vector Centre of the parent circle
Radius float Radius in mm
StartAngle float Arc start in radians
EndAngle float Arc end in radians

See also