fusion-sketch - SKILL.md Agent Skill

name: fusion-sketch description: Create and edit sketches in Fusion 360 using the fusion-sketch CLI. Use when the user asks to sketch, draw geometry, create profiles, add constraints, dimensions, patterns, or work with 2D geometry in Fusion 360.

Fusion 360 Sketching

Control Fusion 360 sketches via tools/fusion-sketch. All coords are mm. Output is JSON.

Orient yourself first

Before drawing anything, understand where you are:

tools/fusion-sketch state              # what's focused, selected, timeline position
tools/fusion-sketch list               # all sketches in the design
tools/fusion-sketch info --sketch S1   # curves, points, constraints detail
tools/fusion-sketch graph --sketch S1  # topology of a specific sketch

Core workflow

# 1. Create sketch on a plane
tools/fusion-sketch create --plane xz --name SidePanel

# 2. Draw geometry (sketch coords — read the plane rules below)
tools/fusion-sketch rect --sketch SidePanel --c1 0,-50 --c2 100,0

# 3. Add constraints to lock geometry
tools/fusion-sketch constrain --sketch SidePanel --type horizontal --e1 SidePanel_curve_0

# 4. Add dimensions to make it parametric
tools/fusion-sketch add-dim --sketch SidePanel --type distance --e1 SidePanel_curve_0 --value 100

# 5. Verify profiles formed
tools/fusion-sketch finish --sketch SidePanel

# 6. If gaps exist, diagnose and fix
tools/fusion-sketch gaps --sketch SidePanel
tools/fusion-sketch close-gaps --sketch SidePanel

Plane coordinate rules — MEMORIZE THESE

The sketch 2D coordinate system depends on which plane you drew on:

Plane	Sketch X →	Sketch Y →	Gotcha
XY	World +X	World +Y	None — direct mapping
XZ	World +X	World -Z	Y is inverted! For +Z geometry, use negative sketch Y
YZ	World -Z	World +Y	X is inverted! For +Z geometry, use negative sketch X

The rule: to place geometry at positive World Z, negate the corresponding sketch axis.

Example: panel from Z=0 to Z=50 on XZ plane

# sketch Y = -50 → world Z = +50
# sketch Y = 0   → world Z = 0
tools/fusion-sketch rect --sketch S1 --c1 0,-50 --c2 100,0

Bypass: use world coordinates directly

# rect3d auto-converts world coords to sketch coords for you
tools/fusion-sketch rect3d --sketch S1 --wc1 0,0,0 --wc2 100,50,0

Prefer rect3d when placing geometry at known world positions. Use rect only when you're thinking in sketch-local terms.

Verify coordinates before trusting them

# Convert sketch 2D → world 3D to check your math
tools/fusion-sketch coords --sketch S1 --points 0,0 100,-50

# Get suggested sketch coords for world 3D targets
tools/fusion-sketch suggest --plane xz --wmin 0,0,0 --wmax 100,50,100

Complete command reference

Lifecycle

Command	What it does
`create --plane P [--name N] [--component C]`	New sketch on plane xy/xz/yz/custom
`create-on-face --body B --face F [--name N]`	New sketch on a body face
`finish --sketch S`	Validate: returns profile count + open curves
`delete --sketch S [--component C]`	Delete a sketch
`list`	All sketches with plane info + coordinate mappings

Drawing primitives

Command	What it does
`line --sketch S --start x,y --end x,y [--construction]`	Line segment (optionally construction)
`arc --sketch S --center x,y --radius R --start-angle D --sweep D`	Arc by center+radius+angles
`arc3 --sketch S --start x,y --mid x,y --end x,y`	Arc through 3 points
`circle --sketch S --center x,y --radius R`	Circle
`rect --sketch S --c1 x,y --c2 x,y`	Rectangle in sketch coords
`rect3d --sketch S --wc1 x,y,z --wc2 x,y,z`	Rectangle in world coords (auto-converts)
`spline --sketch S --points x,y x,y ... [--closed]`	Spline through points
`polygon --sketch S --center x,y --radius R [--sides N] [--rotation D]`	Regular polygon (default 6 sides)
`slot --sketch S --c1 x,y --c2 x,y --radius R`	Slot (oblong) shape
`centerline --sketch S --start x,y --end x,y`	Construction line
`point --sketch S --pos x,y`	Sketch point

Modifications

Command	What it does
`fillet --sketch S --c1 CURVE_ID --c2 CURVE_ID --radius R`	Fillet between two curves
`trim --sketch S --curve CURVE_ID --point x,y`	Trim curve at point
`extend --sketch S --curve CURVE_ID --point x,y [--from-start]`	Extend curve toward point
`offset --sketch S --curves ID ... --dist D --dir x,y`	Offset curves by distance
`mirror --sketch S --curves ID ... --line LINE_ID`	Mirror curves about a line
`pattern-rect --sketch S --curves ID ... [--xn N --yn N --xs D --ys D]`	Rectangular pattern
`pattern-circ --sketch S --curves ID ... --center x,y [--count N --angle D]`	Circular pattern

Constraints

Command	What it does
`constrain --sketch S --type TYPE --e1 ID [--e2 ID]`	Add geometric constraint
`coincident --sketch S [--tolerance T]`	Auto-apply coincident constraints at close endpoints
`list-constraints --sketch S`	List all constraints

Constraint types: coincident, horizontal, vertical, perpendicular, parallel, tangent, equal, concentric, midpoint, fix, collinear

Single-entity types (no --e2): horizontal, vertical, fix

Dimensions

Command	What it does
`dims --sketch S`	List all dimensions with values + expressions
`dim-edit --sketch S --dim INDEX [--value V] [--expr E]`	Edit dimension value or expression
`add-dim --sketch S --type TYPE --e1 ID [--e2 ID] [--value V] [--pos x,y]`	Add dimension

Dimension types: distance, diameter, radius, angular

Analysis & repair

Command	What it does
`gaps --sketch S [--tolerance T]`	Find unclosed gaps between curves
`close-gaps --sketch S [--tolerance T] [--max-gap M] [--dry-run]`	Auto-close small gaps
`recreate --sketch S [--new-name N] [--delete-orig]`	Recreate as proper closed polygon

Query & coordinate helpers

Command	What it does
`profiles --sketch S`	Profile list with areas and world bounds
`info --sketch S`	Detailed sketch: all curves, points, constraints
`coords --sketch S --points x,y ...`	Sketch 2D → world 3D conversion
`suggest --plane P --wmin x,y,z --wmax x,y,z`	World 3D → sketch 2D suggestion
`graph [--sketch S]`	Topology graph (LOCAL_GRAPH)
`state [--compact]`	Navigation state snapshot

Import & text

Command	What it does
`import-svg --path FILE [--plane P] [--body B] [--name N] [--scale S]`	Import SVG into sketch
`text --text T [--sketch S] [--plane P] [--font F] [--height H] [--pos x,y]`	Add text to sketch

Entity ID format

Curves and points use a predictable naming scheme:

SketchName_curve_0, SketchName_curve_1, ... (index-based)
SketchName_point_0, SketchName_point_1, ...
SketchName_dim_0, SketchName_dim_1, ...

Use info --sketch S to see all entity IDs.

Reading the output

Every command returns JSON. Key fields to watch:

finish — the most important check:

{"success": true, "is_valid": true, "profile_count": 1, "open_curves": 0}

is_valid: false means no closed profiles → can't extrude
open_curves > 0 means geometry doesn't close → run gaps

profiles — what you'll extrude:

{"profiles": [{"profile_index": 0, "area_mm2": 5000, "sketch_bounds": {...}}]}

profile_index is what you pass to extrude later

info — full detail for planning:

{"curves": [{"curve_id": "S_curve_0", "type": "SketchLine", "start": [0,0], "end": [100,0], "length_mm": 100}]}

Common mistakes

Forgetting the Y inversion on XZ plane. Geometry ends up at -Z. Use rect3d to avoid this entirely.
Drawing open geometry then trying to extrude. Always finish and check profile_count > 0 before moving on.
Sketch coords in mm but thinking in inches. Everything is mm. A 1" panel is 25.4mm.
Not naming sketches. Always use --name on create. Unnamed sketches get auto-names that are hard to reference later.
Drawing on the wrong plane. XY = horizontal (floor). XZ = vertical front-facing. YZ = vertical side-facing.
Not adding constraints. Unconstrained sketches drift when you edit dimensions. Use constrain to lock geometry relationships, then add-dim to make it parametric.

Decision guide: which plane?

I want to make...	Plane	Extrude direction
A horizontal panel (floor/shelf)	XY	+Z (up) or -Z (down)
A vertical front panel	XZ	+Y (into model) or -Y (toward viewer)
A vertical side panel	YZ	+X (right) or -X (left)
A panel at an offset	Create offset plane first, then sketch on it
A shape on an existing body face	Use `create-on-face` instead of a plane