Skip to content

Point

In one sentence: Place a standalone reference point in the sketch that can serve as a constraint anchor, a construction aid, or a vertex for other tools.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher geometries → Point
Toolbar: Sketcher Geometries · Shortcut: G, Y

Point creates a single 2-D point in the active sketch. The point has no length or area — it is purely a positional marker. Despite its simplicity, it is useful as a constraint attachment target and as a centre reference for arcs or polygons that you want to position relative to something other than the sketch origin.

Intuition

Think of a pin pushed into a drawing board: the pin has no size but it anchors a position. Other geometry can be constrained to coincide with that pin, and the pin itself can be constrained to a specific coordinate or to lie on an edge.

When to use it

  • You need a named reference point to which other geometry will be constrained (e.g. the centre of a pattern, the pivot of a rotation).
  • You want to place a point that a B-Spline or Polyline will pass through.
  • You are building a construction layout and need intersections that are not naturally produced by existing geometry.

When NOT to use it

  • You want to draw a line that starts from a specific location — draw the line and add a Coincident or Lock Position constraint to its endpoint instead.
  • You want the origin — the sketch origin (at coordinate 0, 0) already exists as a built-in special point; select it with Sketch → Select Origin.

Step-by-step walkthrough

  1. Enter sketch edit mode.
  2. Press G, Y or activate Sketch → Sketcher geometries → Point.
  3. Click in the viewport to place the point. The point appears as a small cross.
  4. Press Esc or right-click to leave point-placement mode.
  5. Constrain the point — add Lock Position or Coincident constraints to remove its remaining 2 degrees of freedom.

Parameters

Parameter Type Default Description
Position (click) 2-D coordinate cursor Where the point is placed; exact position is set by subsequent constraints.
Construction Toggle Off If on, the point is a construction (reference) element and does not contribute to the sketch profile.

Common mistakes and pitfalls

Point adds 2 DoF to the sketch

Cause: Every new point adds two unconstrained degrees of freedom (X and Y). If you place points for reference but do not constrain them, the sketch will be under-constrained.
Fix: Always constrain placed points with at least a Lock Position, two distance constraints, or a Coincident + one more constraint.

Python API

Minimal example

import FreeCAD as App
import Sketcher
import Part

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

# Add a point at (10, 20)
idx = sketch.addGeometry(Part.Point(App.Vector(10, 20, 0)), False)
print(f"Point added at geometry index {idx}")

# Constrain it with absolute X and Y (Lock Position equivalent)
sketch.addConstraint(Sketcher.Constraint("DistanceX", idx, 1, 10.0))
sketch.addConstraint(Sketcher.Constraint("DistanceY", idx, 1, 20.0))
doc.recompute()

Resulting feature properties

A Point geometry element has no special sub-properties beyond its coordinates, which are accessed via sketch.Geometry[idx].StartPoint.

See also