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Coincident Constraint

In one sentence: Force two points to share the same location, effectively joining the endpoint of one edge to the endpoint (or midpoint) of another.

Overview

Workbench: Sketcher · Menu: Sketch → Sketcher constraints → Coincident Constraint
Toolbar: Sketcher Constraints · Shortcut: C

Coincident is the most fundamental geometric constraint in Sketcher. It merges two points into one, ensuring they always occupy the same coordinates. Every closed profile, every connected chain of lines and arcs, relies on Coincident to form a single continuous wire rather than a collection of disconnected edges.

In FreeCAD 1.0+, the Unified Coincident tool (C) handles both the classic coincident (point-to-point) and the Point on Object case automatically, based on what you select. The older split commands (Sketcher_ConstrainCoincident for point-to-point, Sketcher_ConstrainPointOnObject for point-on-edge) still exist and are exposed in Point on Object.

Intuition

Think of two pen strokes that look like they touch on paper — but under a magnifying glass they are actually separate, with a tiny gap between them. Coincident is the formal statement "these two points are the same point — not close, not nearly touching, but identical." Once the constraint is applied, no other force can move them apart.

This matters because the Sketcher solver treats geometry as exact: a near-coincident vertex still has two degrees of freedom (it can drift). A formally constrained vertex has zero — it is locked to its partner.

When to use it

  • Joining the endpoint of a line to the endpoint of an arc (forming a connected chain).
  • Centring a circle or arc at a specific point (constrain the circle's centre to a vertex or origin point).
  • Closing a polyline by joining the last endpoint back to the first.
  • After Mirror Sketch or Carbon Copy, connecting the imported geometry to the existing sketch.

When NOT to use it

  • You want a point to lie somewhere on a line or arc but not at an endpoint — use Point on Object instead.
  • Two edges should be tangent at their junction — use Tangent in addition to Coincident (Coincident alone does not guarantee tangency).

Step-by-step walkthrough

Point-to-point coincident

  1. Select two points — click the first vertex, then Ctrl-click the second. (Alternatively, select both with a box selection.)
  2. Press C or activate Sketch → Coincident Constraint.
  3. The two points merge to a single location. The solver updates all connected geometry.

Point-to-object (using the unified tool)

  1. Select a point and an edge — click a vertex, then Ctrl-click a line or arc.
  2. Press C. The unified Coincident tool detects a point-to-edge selection and applies a Point on Object constraint instead.

Tip

You can also apply Coincident by selecting elements first, then pressing C — the order of selection does not matter for the result.

Parameters

Coincident has no numeric parameters. It is a pure geometric constraint that removes 2 degrees of freedom (the relative X and Y offset between the two points).

Unified vs split mode in depth

FreeCAD 1.0 introduced the Unified Coincident (Sketcher_ConstrainCoincidentUnified) tool, which replaces two older separate commands:

  • Sketcher_ConstrainCoincident — classic point-to-point
  • Sketcher_ConstrainPointOnObject — point-to-edge

The unified tool picks the appropriate behaviour based on what you select.

Classic Coincident (point-to-point)

Forces two specific vertices to share identical coordinates. Both vertices become one logical point. This removes exactly 2 DoF.

Use when: - Joining endpoint-to-endpoint (connecting edges end-to-end). - Centring a circle at a line endpoint. - Closing a polyline loop.

Watch out for: Applying Coincident to two vertices that are both already fully constrained elsewhere results in a redundant constraint (shown in red). Avoid using Coincident as a substitute for proper structural design — if two points are already determined to be at the same location by other constraints, an extra Coincident is redundant.

Point on Object

Forces a point to lie on a line, arc, or circle (anywhere along its extent, not necessarily at an endpoint). This removes 1 DoF (the point can still slide along the edge). See Point on Object for full details.

Use when: - A midpoint or construction point must lie on an edge without being fixed to a specific location on that edge.

Watch out for: A point constrained to lie on an edge still has 1 remaining DoF (its position along the edge). Add a second constraint (e.g. a distance or another Point on Object to a crossing edge) to fix it completely.

Advanced usage

Centring geometry at the sketch origin

To place a circle's centre at the sketch origin:

  1. Select the circle's centre vertex.
  2. Select the sketch origin point (the special ExternalPoint at coordinate 0, 0).
  3. Apply Coincident (C).

The origin point is accessible via Sketch → Select Origin or by clicking the central cross in the sketch viewport.

Multiple coincidents at a node

A single vertex can be coincident with multiple others. For example, a T-junction (three lines meeting at one point) requires two Coincident constraints: one between lines A and B, one between A and C. All three lines' endpoints then share the same location.

Common mistakes and pitfalls

Sketch shows as over-constrained after Coincident

Cause: Both points were already determined to be at the same location by other constraints (e.g. a Lock Position on each), so the Coincident is redundant.
Fix: Remove one of the Lock Position constraints and let the Coincident define the shared location.

Profile appears connected visually but the solver reports DoF

Cause: Two endpoint vertices appear to touch in the viewport but no Coincident constraint exists. The solver sees them as separate free-floating points.
Fix: Select both vertices and press C to apply the Coincident constraint. Use Validate Sketch to detect all such gaps automatically.

Python API

Minimal example

import FreeCAD as App
import Sketcher
import Part

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

# Add two lines
line0 = sketch.addGeometry(
    Part.LineSegment(App.Vector(0, 0, 0), App.Vector(10, 0, 0)), False)
line1 = sketch.addGeometry(
    Part.LineSegment(App.Vector(10, 0, 0), App.Vector(10, 10, 0)), False)

# Make endpoint of line0 coincident with start of line1
sketch.addConstraint(Sketcher.Constraint("Coincident", line0, 2, line1, 1))
doc.recompute()

Method signature

sketch.addConstraint(Sketcher.Constraint(
    "Coincident",
    geo1,    # int — first geometry index
    vertex1, # int — 1 = start point, 2 = end point, 3 = centre/midpoint
    geo2,    # int — second geometry index (-1 = sketch origin, -2 = X-axis, -3 = Y-axis)
    vertex2, # int — same encoding as vertex1
))

See also