OrcaSlicer/docs/CAD/design_tab.md

The Design tab

Object-driven parametric CAD inside the slicer. Point at geometry; the geometry offers the verbs that apply to it. Selection comes first and the tool consumes it. Draw a sketch, constrain it, 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. Click a face or a reference plane in the viewport, then press Shift+S (Sketch). The offer opens with the sketch tools on it.
3. Draw a closed profile, then press ✓ Confirm in the floating action bar.
4. With the sketch selected, press Shift+E (Extrude).
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. When no plane is picked it reads "Click a face or a reference plane in the viewport, then a sketch tool"; once one is picked it reads "Sketching on — pick a tool". It is also where a refusal explains itself.

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Selecting

• One left-click selects what is under the cursor. There is no click-cycling through face → edge → body.
• A click near a corner takes the corner, not the face behind it.
• Left-drag sweeps a rubber band, and a rubber band takes the whole body.
• An open sketch line can be clicked, even where it bounds a region.
• Double-click a sketch stroke to edit it — the gesture belongs on the geometry.
• Editing a dimension's value updates that dimension instead of adding a second one next to it.
• The floating chrome that belongs to a sketch leaves with the sketch when it ends.
• Sketching happens on the face you clicked, first click.
• A sketch whose entities form no wire fails instead of extruding a default box. A subtraction that removes nothing is reported as an error instead of a silent success.

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The offer

Right-click on the geometry, released without moving the mouse (an 8 px budget — a right-drag that orbits the camera does not open it). Left-click still only selects, so pointing at things stays quiet.

The offer also opens by itself the moment you press Sketch on a face or plane, showing the sketch tools — the app hands you the tools directly.

Eight families, always in this fixed order: Create, Add material, Remove, Dress-up, Repeat, Transform, Reference, Modify.

• A family with at least one applicable verb shows it. Several applicable verbs collapse into a submenu under the family name.
• A family with nothing applicable is shown greyed in place, with the reason — e.g. "Create — Click a face or a reference plane in the viewport, then a sketch tool". It is not hidden. A control that cannot be used still says what it is and what you would have to do first.
• Inside a sketch the offer shows the sketch verbs; outside it shows the feature verbs.

Document-level actions never enter the offer, because they act on the document and not on a selection: Import STEP, Import mesh, Text, SVG, Export STEP, Commit to Plate, Undo, Redo, Variables, Section view, Origin planes, World axes. They live in the toolbar.

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Keyboard

Single letters drive sketch tools while a sketch is open; Shift+letter drives feature tools and single letters drive view toggles when no sketch is open. The two maps are selected by the mode, not by whether a sketch session is running.

Sketch (while a sketch is open)

Key	Tool
L	Line — click start, then end
R	Rectangle — click two opposite corners
C	Circle — click centre, then radius
A	Arc — click start, end, then a point
S	Slot — two centreline ends, then width
E	Ellipse — centre, major end, minor point
B	Spline — click control points
P	Point — click to place
G	Polygon — click centre, then a vertex
D	Dimension — click 2 points or an entity
T	Trim — click a segment to trim it
X	Extend — click a line/arc to extend it
O	Offset — pick an entity, drag the distance
M	Mirror — pick axis, then entities
F	Fillet — pick two lines, set the radius
H	Chamfer — pick two lines, set the distance
K	Constrain — finish the live sketch and enter constrain
Q	Construction toggle — draw the next entity as construction geometry
Del	Delete the selected sketch entity
Esc	Cancel the live tool

Feature (when no sketch is open)

Key	Tool
Shift+S	Sketch
Shift+E	Extrude — extrude a profile, or push/pull a picked face
Shift+R	Revolve
Shift+W	Sweep
Shift+L	Loft
Shift+N	Pattern
Shift+G	Surface Extrude
Shift+J	Surface Revolve
Shift+O	Surface Loft
Shift+Q	Surface Fill
Shift+U	Surface Offset
Shift+V	Thicken Surface
Shift+P	Plane
Shift+A	Axis
Shift+C	Coord Sys
Shift+Y	Transform
Shift+Z	Mirror
Shift+B	Boolean
Shift+X	Cut
Shift+F	Fillet / Chamfer
Shift+D	Draft
Shift+K	Shell
Shift+H	Hole
Shift+T	Thread
Shift+I	Import STEP
Shift+M	Import mesh

View toggles (single letters, when no sketch is open)

Key	Action
Home	Axonometric view, fitted to the model
P	Origin planes on/off
A	World axes on/off
X	Section view on/off

While the section is on: PageUp / PageDown move the cut plane, F flips which half is kept. With no section on, F is Place on Face — lay the picked face flat on the bed.

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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. Press Shift+S, click the face or plane you want to sketch on, and draw. The toolbar and the offer both carry the sketch tools.

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 (X) hides half the model so you can see inside — PageUp/PageDown move the plane, F flips which half is kept. Place on Face (F, when section is off) lays a picked face flat on the bed. Origin planes (P) and world axes (A) can be toggled on 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.
• Card wiring for 9 of the 16 late-wired tools has never been click-tested.
• 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.
• There is no automated GUI test in CI. Every behaviour above is traced to code and to a hand pass, not to a synthetic click.

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Where the code lives

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