Fusion 360 Solid / Body Operations

Control Fusion 360 3D features and bodies via tools/fusion-solid. All dimensions are mm. Output is JSON.

Orient yourself first

Before creating features, understand the current model:

tools/fusion-solid summary       # world bounds, all bodies, orientation
tools/fusion-solid list           # all bodies with dimensions + provenance
tools/fusion-solid planes         # all construction planes (xy, xz, yz + custom)
tools/fusion-solid center --body Body1   # center point + bounding box of a body

Core workflow: sketch → extrude

# 1. Create a sketch (use fusion-sketch skill)
tools/fusion-sketch create --plane xy --name Base
tools/fusion-sketch rect --sketch Base --c1 0,0 --c2 100,80

# 2. Extrude the profile into a 3D body
tools/fusion-solid extrude --sketch Base --distance 20 --name BasePanel

# 3. Verify the result
tools/fusion-solid list
tools/fusion-solid center --body BasePanel

Feature operations

All features that work from sketch profiles support --op for boolean behavior:

• new_body — creates a separate body (default)
• join — adds material to an existing body (must intersect)
• cut — removes material from an existing body
• intersect — keeps only the overlapping volume

Extrude

# Basic extrude
tools/fusion-solid extrude --sketch S --distance 20

# Extrude as a cut into an existing body
tools/fusion-solid extrude --sketch SlotSketch --distance 15 --op cut --target Panel

# Symmetric extrude (both directions)
tools/fusion-solid extrude --sketch S --distance 10 --dir symmetric

# Extrude with draft/taper
tools/fusion-solid extrude-draft --sketch S --distance 20 --draft 5

Revolve

# Full revolution around X axis
tools/fusion-solid revolve --sketch Profile --axis x

# Partial revolve (90°) around a sketch line
tools/fusion-solid revolve --sketch Profile --axis-sketch AxisSketch --axis-line 0 --angle 90

Loft

# Loft between two sketches
tools/fusion-solid loft --sketches TopProfile BotProfile

# Loft with guide rails
tools/fusion-solid loft --sketches S1 S2 --rails RailSketch

Sweep

# Sweep a profile along a path
tools/fusion-solid sweep --profile-sketch CrossSection --path-sketch SweepPath

# Sweep with twist
tools/fusion-solid sweep --profile-sketch CS --path-sketch P --twist 90

Edge/face modifications

# Fillet edges (round them)
tools/fusion-solid fillet --edges Body1_edge_0 Body1_edge_3 --radius 2

# Chamfer edges (bevel them)
tools/fusion-solid chamfer --edges Body1_edge_0 --distance 1.5

# Boolean combine bodies
tools/fusion-solid boolean --op union --target Body1 --tools Body2 Body3
tools/fusion-solid boolean --op subtract --target Body1 --tools CutterBody

# Shell a body (hollow it out)
tools/fusion-solid shell --body Body1 --thickness 2 --faces 0

# Split a body with a plane
tools/fusion-solid split --body Body1 --tool xz --keep both

Stable entity references

Edge indices (Body1_edge_3) shift after every boolean, fillet, or chamfer. Use spatial references instead — they survive topology changes.

Three reference formats

Format	Example	When to use
Index (legacy)	Body1_edge_3	Quick one-shot before any topology change
Spatial	Body1@170,0,542	Preferred — stable across booleans/fillets
Token	token:abc123...	EntityToken from resolver cache

Spatial reference workflow

# 1. List edges to find midpoints
tools/fusion-solid edges --body Body1
# Output includes midpoint for each edge, e.g.:
#   edge_3: midpoint [170.0, 0.0, 542.0]

# 2. Use the midpoint as a spatial ref — this survives topology changes
tools/fusion-solid fillet --edges "Body1@170,0,542" --radius 10

# 3. After a boolean, the same spatial ref still finds the right edge
tools/fusion-solid boolean --op subtract --target Body1 --tools Cutter
tools/fusion-solid fillet --edges "Body1@170,0,542" --radius 5

The spatial lookup finds the nearest edge within 10mm of the given point. Use midpoints from edges --body for best accuracy.

Primitives — quick body creation

For simple shapes, skip the sketch step entirely:

# Box from two corners
tools/fusion-solid box --c1 0,0,0 --c2 100,80,20 --name Panel

# Box from center + dimensions
tools/fusion-solid box --center 50,40,10 --width 100 --depth 80 --height 20 --name Panel

# Cylinder
tools/fusion-solid cylinder --center 0,0,0 --radius 25 --height 50 --axis z --name Peg

# Sphere
tools/fusion-solid sphere --center 0,0,50 --radius 30 --name Ball

# Hole (cut into existing body)
tools/fusion-solid hole --body Panel --center 50,40,20 --diameter 10 --through

# Box joint helper
tools/fusion-solid box-joint --receiving SidePanel --mating BottomPanel --edge front

Surfaces and stitching

For creating complex geometry from surface patches:

# Create a surface patch from a sketch profile
tools/fusion-solid patch --sketch FaceSketch --name Face1

# Stitch multiple surfaces into a solid (if watertight)
tools/fusion-solid stitch --bodies Face1 Face2 Face3 Face4 --name SolidResult

Polyhedron / faceted geometry

# Arbitrary polyhedron from vertices + triangular faces
tools/fusion-solid polyhedron \
  --vertex V1=0,0,0 V2=100,0,0 V3=50,86.6,0 V4=50,28.9,81.6 \
  --face V1,V2,V3 V1,V2,V4 V2,V3,V4 V1,V3,V4 \
  --name Tetrahedron

# Triangular prism (simpler)
tools/fusion-solid tri-prism --v1 0,0,0 --v2 100,0,0 --v3 50,86.6,0 --height 50 --name Prism

Construction planes

# List all planes
tools/fusion-solid planes

# Offset from a base plane
tools/fusion-solid offset-plane --base xy --offset 50

# Angled plane from point + normal
tools/fusion-solid angled-plane --point 50,50,50 --normal 1,1,0 --name DiagonalPlane

# Angled plane from three points
tools/fusion-solid angled-plane --p1 0,0,0 --p2 100,0,0 --p3 0,100,50

# Plane by rotating around a sketch line
tools/fusion-solid plane-by-angle --base xy --sketch AxisSketch --angle 45 --name Tilted

Body query — understand the model

# List all bodies with dimensions and provenance
tools/fusion-solid list
tools/fusion-solid list --component Carcass

# Edges and faces of a specific body
tools/fusion-solid edges --body Body1
tools/fusion-solid faces --body Body1

# Detailed face geometry (normal, area, angles to world planes)
tools/fusion-solid face-info --body Body1 --face Body1_face_0

# Body center and bounding box
tools/fusion-solid center --body Body1

# Find shared edges between two bodies (miter joints, etc.)
tools/fusion-solid intersections --b1 Panel1 --b2 Panel2

# Select geometry by 3D position
tools/fusion-solid select --point 50,40,10 --type face --tolerance 2

# Full model summary
tools/fusion-solid summary

Body transforms

# Copy a body
tools/fusion-solid copy --body Body1 --name Body1_Copy

# Translate a body
tools/fusion-solid move --body Body1 --translate 100,0,0

# Rotate a body
tools/fusion-solid move --body Body1 --rotate-axis 0,0,1 --rotate-angle 90

# Mirror across a plane
tools/fusion-solid mirror --body Body1 --plane yz

# Rectangular pattern
tools/fusion-solid pattern --body Body1 --dir 1,0,0 --count 4 --spacing 25

# Delete a body
tools/fusion-solid delete --body Body1

Entity ID format

Bodies, edges, and faces support multiple reference formats:

• Body names: whatever Fusion auto-assigns or you specify with --name
• Edges: BodyName_edge_0 (index) or BodyName@x,y,z (spatial — preferred)
• Faces: BodyName_face_0 (index) or BodyName@x,y,z (spatial — preferred)

Use edges --body B or faces --body B to discover IDs and midpoints. Prefer spatial refs (Body@x,y,z) whenever you plan to modify topology afterward.

Unit conversions

All inputs and outputs are mm. Fusion internally uses cm, but the bridge handles conversion.

You give	Fusion gets	Meaning
25.4 mm	2.54 cm	1 inch
12.7 mm	1.27 cm	1/2 inch
19.05 mm	1.905 cm	3/4 inch (standard plywood)

Common mistakes

1. Extrude join that creates an orphan body. The extruded geometry must physically touch the target body. If not, Fusion silently creates a new body. Watch for warning: JOIN_CREATED_ORPHAN_BODY in the output.

2. Wrong extrude direction. On XZ or YZ plane sketches, positive extrude may not go where you expect. Use summary to check body positions after extruding.

3. Edge IDs change after modifying the body. If you fillet/chamfer/boolean a body, the edge indices shift. Use spatial refs (Body@x,y,z) instead of index-based IDs to avoid this problem entirely.

4. Shell without specifying faces to remove. If --faces is empty, you get a fully enclosed shell (no opening). Usually you want to remove at least one face.

5. Boolean with wrong body scope. Bodies in different components may need assembly-context proxies. The bridge handles this, but verify with list if results seem wrong.

Decision guide

I want to...	Command
Turn a sketch into a 3D shape	extrude
Create a round shape from a profile	revolve
Blend between two profiles	loft
Extrude along a curved path	sweep
Add material to an existing body	extrude --op join --target B
Cut material from a body	extrude --op cut --target B
Combine two separate bodies	boolean --op union
Subtract one body from another	boolean --op subtract
Round sharp edges	fillet
Bevel sharp edges	chamfer
Hollow out a solid	shell
Cut a body in half	split
Quick box without sketching	box
Quick cylinder without sketching	cylinder
Drill a hole	hole