Sketcher Workbench¶
The Sketcher workbench is the foundation of parametric solid modelling in FreeCAD. You use it to draw precise 2-D geometry that is then handed off to Part Design (or Part) to become 3-D solids.
What Sketcher is for¶
A sketch is a fully-defined 2-D drawing attached to a plane. Each piece of geometry in the sketch — lines, arcs, circles, splines — can be locked to an exact size and position by applying constraints. When every degree of freedom has been removed (the sketch is fully constrained) the geometry turns green and the sketch is ready to drive a solid feature.
The constraint-based approach is what makes FreeCAD models parametric: change a dimension value and the entire sketch — and every feature that depends on it — updates automatically.
The Sketcher workflow¶
- Open a sketch on a plane (XY, XZ, YZ, a datum plane, or a face).
- Draw geometry — lines, arcs, rectangles, splines, etc.
- Apply constraints — geometric (parallel, tangent, …) then dimensional (distance, radius, angle, …).
- Achieve full constraint — all elements turn green; the constraint counter reads "Fully constrained".
- Close the sketch and use it as input to Pad, Pocket, Revolution, etc.
Constraint colours¶
| Colour | Meaning |
|---|---|
| White / default | Unconstrained (still has degrees of freedom) |
| Green | Fully constrained — no remaining degrees of freedom |
| Red | Over-constrained or conflicting constraints — resolve before closing |
| Blue | Reference (construction) constraint or dimension — does not constrain geometry |
| Yellow | Partially redundant constraint |
Key concepts¶
Degrees of freedom (DoF)¶
Every 2-D point has 2 DoF (it can slide in X and Y). Every line between two points has 4 DoF, and so on. A constraint removes one or more DoF. The Solver panel in the left sidebar counts the remaining DoF in real time: the goal is always zero.
Driving vs reference constraints¶
A driving constraint commands geometry to a specific value. A reference constraint reads the current value without constraining anything — it is a measurement label, not a command. See the individual constraint pages for details.
Construction geometry¶
Any geometry element can be toggled to construction mode (thin dashed line). Construction geometry is used as a scaffolding aid — it participates in constraints but is not included in the profile passed to Part Design. This lets you add helper circles, centre lines, and guide lines without polluting the final shape.
Tools overview¶
| Group | Tools |
|---|---|
| Sketch Lifecycle | New Sketch, Edit Sketch, Leave Sketch, Map Sketch, Reorient, Validate, Mirror, Merge |
| Geometry | Point, Line, Polyline, Arcs, Circles, Conics, Rectangle, Polygon, Slot, Fillet, Chamfer, B-Spline |
| Editing | Trim, Split, Extend, External Geometry, Carbon Copy |
| Geometric Constraints | Coincident, Horizontal/Vertical, Parallel, Perpendicular, Tangent, Equal, Symmetric, Block, Point on Object, Lock |
| Dimensional Constraints | Dimension, Distance, Radius/Diameter, Angle, Snell's Law, Toggle Driving |
| Transforms | Offset, Translate, Rotate, Scale, Mirror, Copy/Clone/Move |
| Analysis | Select tools, Delete all, Remove axes alignment, Toggle internal geometry |
See the Tools index for a complete alphabetical reference.
Relationship to Part Design¶
Sketcher does not build solids — it produces a 2-D profile. Part Design takes that profile and extrudes, revolves, sweeps, or lofts it into a solid. Every Pad, Pocket, Revolution, and similar feature in Part Design requires a Sketcher sketch as its starting point.
If you are new to FreeCAD, the typical learning path is:
- Learn the Sketcher (this workbench) — how to draw and fully constrain a sketch.
- Learn Part Design — how to turn sketches into solids.