OrcaSlicer/docs/design_tab.md

The Design tab

A parametric CAD modeller inside the slicer. Draw a sketch, turn it into a solid, refine it, and send it straight to Prepare — without leaving for another application and coming back through an STL.

The model is a recipe, not a mesh. Every action becomes a feature in a tree that is replayed from the start whenever anything changes, so editing a dimension you set twenty steps ago rebuilds everything downstream. The geometry kernel is OCCT, which the slicer already ships for STEP import.

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Getting started

1. Open the Design tab.
2. Pick a plane — XY, XZ or YZ — and press Sketch.
3. Draw a closed profile, then press ✓ to finish the sketch.
4. Select the sketch and press Extrude (Shift+E).
5. Press Commit to Plate to hand the solid to Prepare.

The status line under the toolbar is the thing to watch: it says what the current tool is waiting for, and it is where a refusal explains itself.

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Sketching

A sketch is a closed (or open) 2D profile on a plane or on a flat face of an existing body.

Entities: line, polyline, rectangle (corner / centre / oblique / rounded), circle (centre-radius / 2-point / 3-point), arc (centre-point / 3-point / tangent), ellipse and elliptical arc, polygon (inscribed / circumscribed), slot (straight / arc), spline, point, and text.

Editing: move, rotate, scale, trim, extend, offset, mirror, and linear or polar arrays.

Constraints: coincident, horizontal, vertical, parallel, perpendicular, tangent, equal, concentric, midpoint, symmetric, fix, plus dimensional radius, diameter, distance and angle. The solver reports the remaining degrees of freedom and tells you when a sketch is fully constrained — or when a constraint conflicts with one already there.

Sketches stay editable. Selecting one in the feature tree reopens it with its dimensions live.

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Building solids

Grouped in the toolbar by what they do, one concept per drawer.

Add material

Tool	Shortcut	What it does
Extrude	Shift+E	Extrude a profile, or push/pull a face already on a body
Revolve	Shift+R	Revolve a profile about an axis
Sweep	Shift+W	Sweep a profile along a path — including a helix, for springs and augers
Loft	Shift+L	Skin between two or more profiles
Thicken	—	Offset a solid face into a thin plate as a new body
Rib	—	Grow a stiffening wall from an open sketch line, fused to a body

Extrude offers blind, symmetric, two-sided, through-all and up-to-face end conditions, plus a draft angle on the side wall, and can add, subtract, intersect or start a new body.

Surface

Sheet bodies — surfaces with no thickness — for shapes that are easier to build as skins and solidify afterwards.

Tool	Shortcut
Surface Extrude	Shift+G
Surface Revolve	Shift+J
Surface Loft	Shift+O
Surface Fill	Shift+Q
Surface Offset	Shift+U
Thicken Surface	Shift+V

Thicken Surface is how a sheet becomes a printable solid.

Dress-up

Tool	Shortcut
Fillet / Chamfer	Shift+F
Draft (taper a face)	Shift+D
Shell	Shift+K
Delete Face	—

Delete Face removes faces and heals the solid — useful for stripping a feature off an imported part.

Holes

Hole (Shift+H) drills simple, counterbored or countersunk holes, with an ISO/ANSI standards table so you can ask for an M6 clearance hole instead of computing a diameter. Thread (Shift+T) cuts a real helical thread into a bore or onto a shaft.

Placement

Operations that move a body without changing its shape: Transform (Shift+Y), Mirror (Shift+Z), and Mate for assemblies.

Combining

Boolean (Shift+B) unions, subtracts or intersects two bodies. Cut (Shift+X) splits a body with a plane. Pattern (Shift+N) repeats a body linearly, in a circle, or along a curve.

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Reference geometry

Datum features carry no material; they exist to give later features something to attach to.

• Plane (Shift+P) — offset, tilted, midplane, tangent, through two edges, or coincident
• Axis (Shift+A) — two points, a face normal, a cylinder centreline, the intersection of two planes, or along an edge
• Coord Sys (Shift+C) — a full frame, from a world point or from a face plus a direction edge
• Helix — a helical curve to sweep along
• Project — project a body's edges onto a plane as sketch geometry

On the Coord Sys tool, picking a direction edge is worth the extra click: without one the frame takes its X from the face's first edge, which is deterministic but not necessarily the direction you meant.

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Assemblies

Mate aligns two coordinate systems and moves one body onto the other. Five kinds:

Kind	Leaves free
Fastened	nothing — 6 DOF locked
Planar	sliding in the plane
Revolute	rotation about the axis
Slider	sliding along the axis
Cylindrical	rotation and sliding

Check interference reports every overlapping pair of solids with the overlapping volume, so a clash is a number rather than an impression. Bodies that merely touch enclose no volume and are not reported.

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Variables and expressions

Define named variables and drive dimensions from them. Any numeric field accepts an expression — width/2, wall*3 — and everything re-evaluates on recompute. Change one variable and the whole model follows.

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Import and export

Import STEP brings in a real B-rep solid, not a mesh: its faces and edges can be filleted, shelled and cut like anything modelled here.

Import mesh (STL/OBJ) converts triangles to a B-rep body and tells you honestly what it got — whether the result is a closed solid or an open shell, with the boundary and non-manifold edge counts. A large mesh becomes a large number of faces, which is slow to edit; the importer warns before you commit to it.

Export STEP writes the model out for another CAD tool.

Commit to Plate sends the solid to Prepare for slicing. The whole feature recipe is saved inside the 3MF, so reopening the project restores the editable model rather than a frozen mesh.

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View controls

Section view hides half the model so you can see inside — PageUp/PageDown move the plane, Flip shows the other half, Delete removes it. Place on Face (F) lays a picked face flat on the bed. The bed and its grid can be toggled off when they get in the way, and origin planes and world axes can be shown while you orient yourself.

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Known limitations

Being straight about the edges, so nobody discovers them the hard way:

• Rib needs a sketch containing an explicit open line. A parametric rectangle sketch carries no individual entities, so Rib cannot use one.
• Surface Loft and Surface Fill have kernel tests but have not been exercised by hand.
• Two kernel tests are known-broken and excluded from the suite: a tangent-constraint case that aborts inside the vendored solver, and an internal-thread groove volume below its asserted threshold. Both are tracked, neither is fixed.
• Mate resolves by composing transforms directly. There is no 3D assembly solver, so mates are applied in order rather than solved simultaneously, and mate limits are not implemented.
• Move-face and replace-face are not implemented — OCCT offers no clean primitive for them.

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Where the code lives

Path	Role
src/libslic3r/CadDocument.*	the feature recipe and its replay
src/libslic3r/GeometryEngine.*	OCCT wrapper — faces, edges, booleans, healing
src/libslic3r/SketchEngine.*	profile → wire → solid
src/libslic3r/SketchSolver.*	constraint solving, over the vendored solver
src/libslic3r/slvs/	vendored 2D constraint solver (GPLv3)
src/slic3r/GUI/DesignPanel.*	the tab: toolbar, cards, feature tree
src/slic3r/GUI/DesignCanvas.*	viewport integration
src/slic3r/GUI/DesignSketchTool.*	in-canvas sketching

Build with -DSLIC3R_CAD=ON (the default). With it OFF the tab is not compiled and the deps prefix matches upstream exactly — see cad_dependency_weight.md.