Part Design is the workbench you use 90% of the time in FreeCAD if you're modeling mechanical parts. Sketch a 2D profile, extrude to 3D, add features (holes, fillets, chamfers, threads), edit dimensions later — and the entire model rebuilds. This is the modern parametric workflow comparable to SolidWorks Sketches/Features, Onshape Sketches/Extrudes, or Fusion 360 Sketches/Bodies. If you've used any of those, Part Design will feel familiar in an afternoon.

This page is a structured reference — what each tool does, when to use it, the gotchas that catch beginners. For a step-by-step "first model in 30 minutes" walkthrough see our beginner guide; for the broader workbench tour see all workbenches.

Body — the parametric container

Every Part Design feature lives inside a Body. A Body holds one connected solid plus its construction history. To start: Part Design → Create body. The origin (three planes — XY, YZ, XZ — and three axes) appears inside the Body for sketches to attach to.

Bodies are isolated. Operations inside one Body don't see geometry from another Body unless you explicitly reference it. For multi-part assemblies, create one Body per part and combine them in the Assembly workbench.

Sketches — the input to every feature

Almost every Part Design feature starts with a sketch. Part Design → New Sketch prompts you to pick a plane (or face) to draw on. The Sketcher opens in 2D edit mode. Draw your profile with the Line, Rectangle, Circle, Polygon tools, then add geometric constraints (coincident, horizontal, vertical, parallel) and dimension constraints.

A fully-constrained sketch turns green — every degree of freedom is locked. This is the goal for production work. An under-constrained sketch turns white/yellow and behaves unpredictably under edits. See our Sketcher reference for the full constraint catalog.

Pad — extrude a sketch to 3D

The most common Part Design operation. Close your sketch, click Pad, set a distance, click OK. The sketch becomes a solid. Pad has six variants:

• Dimension: extrude N millimeters (most common).
• To last: extrude until you hit another solid feature.
• To first: extrude until the first intersection.
• Up to face: pick a face to stop at.
• Two dimensions: different distances forward and back from the sketch plane.
• Symmetric: extrude equally in both directions from the sketch plane.

Use Symmetric or Two dimensions when you want the sketch plane to stay at the part's centerline — easier to add symmetric features later.

Pocket — subtract a sketch from a solid

The inverse of Pad: cut material away. Sketch a hole profile on a face, click Pocket, set depth. Pocket has the same six variants as Pad. Use it for holes, slots, recesses, cutouts — anything that removes material from an existing solid.

For round holes the dedicated Hole tool is better than Pocket — it handles tap drills, counterbores, threads, and standardized hole sizes (M3, M4, M5, etc.) with one click.

Revolve and Groove — rotational symmetry

Revolve takes a 2D profile and rotates it around an axis to create the solid — the natural workflow for any rotationally-symmetric part: shafts, knobs, bottles, wheels. Sketch a half-profile, click Revolution, pick the axis, set the angle (default 360°).

Groove is Revolve's subtractive twin — sketch a profile, revolve to cut. Use for snap-ring grooves, decorative rings, sealing surfaces.

Fillet, Chamfer, Draft

After the basic solid is built, add edge treatments:

• Fillet: rounded edges. Pick edges, set radius. Use for stress concentrations and aesthetics.
• Chamfer: beveled edges. Pick edges, set distance and angle. Use for assembly chamfers and hole entries.
• Draft: tapered faces. Pick faces, set angle. Critical for injection-molded parts so they release from the mold.

Apply fillets and chamfers last in the feature tree. Adding a fillet early then trying to add a hole that intersects the filleted edge often fails. Build the rough solid first, refine after.

Patterns — Linear, Polar, Mirror, MultiTransform

Repeat a feature efficiently:

• LinearPattern: repeat in a straight line — bolt rows, rib arrays.
• PolarPattern: repeat around an axis — bolt circles, gear teeth.
• Mirrored: mirror across a plane — left/right symmetry.
• MultiTransform: chain multiple transforms — e.g., mirror then linear pattern.

Patterns are applied to features (Pad, Pocket, etc.), not raw geometry. Edit the original feature and every pattern instance updates.

Booleans — combining and subtracting Bodies

When two Bodies need to merge or one needs to cut another, use the boolean operations: Union, Cut, Common (intersection). These work between Bodies — for operations inside a single Body, use Pad and Pocket instead.

Booleans between Bodies are how multi-body assemblies become single solids when needed — for example, combining a frame and a bracket into one printable STL.

Edit history — the parametric advantage

Every feature you create appears in the Model tree on the left. Double-click any feature to edit its parameters — sketch dimensions, pad depth, fillet radius, hole size — and FreeCAD recalculates the entire model. This is the property that makes parametric CAD different from polygon modelers (Blender, Maya): you can change a base dimension three months later and every dependent feature updates.

The trade-off: feature order matters. A fillet that depends on an edge created by a Pocket will fail if you delete the Pocket. The "topological naming problem" historically caused fillets and chamfers to break unexpectedly when upstream features changed; FreeCAD 1.0 significantly improved this — most rebuilds now succeed cleanly.

Tips for productive Part Design

• Fully constrain sketches. An unconstrained sketch is a future bug. Aim for green.
• Build the rough solid first, refine later. Pad, Pocket, Hole, then Fillet/Chamfer/Draft.
• Reference the origin, not other features. Sketches that attach to existing faces break when those faces change. Sketch on the origin planes when possible.
• Use Spreadsheets for parameters. Drive dimensions from a named parameter table — change one cell, the model rebuilds with the new size.
• Save often. FreeCAD 1.1.3 is stable but parametric rebuilds are CPU-intensive — autosave doesn't always catch a hard crash.

Related workbench guides