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

1. Forgetting the Y inversion on XZ plane. Geometry ends up at -Z. Use rect3d to avoid this entirely.

2. Drawing open geometry then trying to extrude. Always finish and check profile_count > 0 before moving on.

3. Sketch coords in mm but thinking in inches. Everything is mm. A 1" panel is 25.4mm.

4. Not naming sketches. Always use --name on create. Unnamed sketches get auto-names that are hard to reference later.

5. Drawing on the wrong plane. XY = horizontal (floor). XZ = vertical front-facing. YZ = vertical side-facing.

6. 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