Sketcher is the workbench every Part Design feature secretly relies on. You don't usually open Sketcher directly — you open it from inside Part Design when you click "New Sketch." But everything that makes parametric CAD work — the green-when-fully-constrained behavior, the dimensions that propagate through the whole model when you change one number, the ability to revise a design six months later — comes from Sketcher.

This page is a structured reference. The rule of thumb: spend 10 extra minutes fully-constraining every sketch. You'll save hours of debugging when designs need revisions.

The two kinds of constraints

Sketcher constraints come in two categories:

• Geometric constraints: describe shape relationships. Coincident, horizontal, vertical, parallel, perpendicular, tangent, equal, symmetric. They have no number — they are pure topology rules.
• Dimension constraints: describe sizes. Distance, horizontal distance, vertical distance, length, radius, diameter, angle. Each carries a numeric value you can edit.

A fully-constrained sketch uses both — geometry to lock shape, dimensions to lock size. When the count of constraints matches the degrees of freedom in the geometry, the sketch turns green. Green is the goal.

Geometric constraints — what each does

• Coincident: two points must be at the same location. Most common — line endpoints meeting, etc.
• Point on object: a point must lie somewhere on a line, arc, or curve.
• Horizontal / Vertical: a line or two points must be horizontal or vertical.
• Parallel: two lines must be parallel to each other.
• Perpendicular: two lines must meet at 90°.
• Tangent: a line must be tangent to an arc, or two arcs tangent to each other.
• Equal: two segments must be the same length, or two arcs the same radius.
• Symmetric: two points symmetric about a line or another point.
• Block: lock a piece of geometry in place permanently — useful for imported reference geometry.

Apply geometric constraints first. They lock shape without specifying numbers — the building block before you start dimensioning.

Dimension constraints — what to use when

• Distance: generic distance between two points or along a line. Use when horizontal/vertical isn't precise enough.
• Horizontal distance: X-coordinate difference. Most common for laying out features along an axis.
• Vertical distance: Y-coordinate difference.
• Length: length of a single line segment.
• Radius / Diameter: for arcs and circles. Use diameter for round holes (machinist convention), radius for fillets.
• Angle: angle between two lines, or interior angle of a corner.

Each dimension can hold a formula or reference another dimension. Type Sketch.Constraints.WallThickness * 2 to derive one dimension from another — parametric design's superpower.

Color codes — what FreeCAD is telling you

Color	Meaning	What to do
White	Under-constrained	Add more constraints until green
Green	Fully constrained	Done — close the sketch
Yellow	Conflicting constraints	Some constraint is impossible — find and remove it
Red	Sketch error	Check the Solver Messages panel for details
Light blue	External geometry	Reference geometry from outside the sketch — read-only

Common Sketcher errors and fixes

• "Conflicting constraints": two dimensions try to set the same length to different values, or geometry that can't be both horizontal and at 30° at once. Open the Solver Messages panel — FreeCAD tells you which constraints conflict. Remove one.
• "Redundant constraints": the same dimension is specified twice (e.g., both Length and Horizontal distance on a horizontal line). Remove the duplicate.
• "Cannot solve sketch": usually a coincident-constraint loop — a point coincident with two other points which are coincident with the first. Click the affected geometry to highlight, delete one constraint.
• Dimension flips on edit: when you change a dimension and the geometry "jumps" to the wrong side, you missed a constraint that locks the side. Add a horizontal-distance constraint with a sign to lock orientation.

External geometry — referencing outside the sketch

Sometimes a sketch needs to align to existing 3D geometry — for example, a hole sketched on a face must align with an edge of that face. Use External geometry (the icon with a 3D arrow): pick edges, vertices, or curves from existing solids in the same Body. They appear as light-blue read-only references in the sketch and you constrain to them like any other geometry.

External geometry is what makes Part Design's parametric chain work — change the upstream feature, the sketch's external references update, the downstream features rebuild.

Construction geometry — helper lines

Toggle a line, circle, or point to construction mode (the dashed-line icon or B shortcut). Construction geometry doesn't generate solid output — it exists only to support constraints. Use it for centerlines, symmetry axes, "this dimension is from the part centerline" reference lines.

Sketch hygiene — habits that compound

• One profile per sketch. Don't pile multiple unrelated shapes into one sketch — split them across sketches and use multiple Pad/Pocket operations.
• Sketch on the origin planes when possible. Sketches attached to existing faces break when those faces change. The origin XY/YZ/XZ planes never disappear.
• Use symmetry constraints aggressively. A symmetric design with one constraint fully captures both sides — half the constraint count, twice the robustness.
• Name your sketches. "Sketch001" is useless three months later. Rename in the model tree to "WheelProfile" or "MountingHoles."
• Always close the sketch fully constrained. Tempting to leave it half-constrained because it "looks right" — that's a future bug.

Related workbench guides