name: openclaw-fusion description: Control Autodesk Fusion 360 via the AuraFriday MCP Server add-in. Use when the user wants to create, modify, measure, or inspect 3D CAD models, sketches, assemblies, or manufacturing setups in Fusion 360. Triggers on any Fusion/CAD/3D-modeling request.

Fusion 360 Skill

Control Fusion 360 through the AuraFriday MCP-Link server. The server exposes a fusion360 MCP tool with three execution modes: Generic API calls, Python execution, and documentation lookup.

Connection

MCP-Link SSE endpoint: https://127-0-0-1.local.aurafriday.com:31173/sse

Use mcporter to call tools:

mcporter call fusion360.execute --args '{"api_path": "design.rootComponent.sketches.add", "args": ["design.rootComponent.xYConstructionPlane"]}'

Or configure in config/mcporter.json:

{"mcpServers": {"fusion360": {"url": "https://127-0-0-1.local.aurafriday.com:31173/sse"}}}

Verify connection: mcporter list fusion360 --schema

Three Execution Modes

1. Generic API — Simple operations

{"api_path": "design.rootComponent.sketches.add", "args": ["design.rootComponent.xYConstructionPlane"], "store_as": "sketch1"}

• api_path: Dot-path into Fusion API. Prefix stored objects with $ (e.g., $sketch1.sketchCurves)
• args: Array of arguments. Objects constructed from dicts: {"type": "Point3D", "x": 5, "y": 10, "z": 0}
• store_as: Save result for later use as $name

Supported object types in args:

• {"type": "Point3D", "x": 0, "y": 0, "z": 0}
• {"type": "Vector3D", "x": 1, "y": 0, "z": 0}
• {"type": "ValueInput", "value": 2.5} (cm) or {"type": "ValueInput", "expression": "2.5 mm"}
• {"type": "ObjectCollection"} (empty collection)
• Enum values as integers (e.g., 0 for FeatureOperations.JoinFeatureOperation)

2. Python Execution — Complex workflows

{"operation": "execute_python", "code": "...python code..."}

Pre-injected variables: app, ui, design, rootComponent, fusion_context (stored objects dict), mcp (bridge to other tools).

Full access to adsk.core, adsk.fusion, adsk.cam. Use print() for return values.

3. Documentation Lookup

{"operation": "get_api_documentation", "search_term": "ExtrudeFeature", "category": "class_name", "max_results": 5}
{"operation": "get_online_documentation", "class_name": "ExtrudeFeatures", "member_name": "createInput"}
{"operation": "get_best_practices"}

Always call get_best_practices on first use and get_api_documentation when unsure of API.

Core Workflow: Execute → Verify → Iterate

NEVER trust API return values alone. Visual verification after every geometry operation is mandatory, not optional.

The Verification Loop

Every geometry-changing operation follows this exact sequence:

1. Zoom camera to the target area BEFORE executing (~3× feature size)
2. Execute the Fusion operation
3. Screenshot the viewport immediately
4. Quick vision check — send screenshot to a cheap/fast model (Gemini Flash, ~$0.001/check)
5. Pass/fail — if the check fails, undo and fix immediately. Do NOT proceed.

Use this exact prompt format for quick checks:

I just [OPERATION] in Fusion 360.
Expected: [WHAT SHOULD BE VISIBLE]
Location: [WHERE ON THE MODEL]
Check: Is the change visible? Is it in the right place? Right direction?

Use model="google/gemini-2.0-flash" (or equivalent cheap model) for routine checks. Reserve the main model for design decisions and complex analysis only.

Cost: ~$0.001 per check. 50 checks per session = $0.05. This is essentially free compared to the cost of blind debugging (which wastes 3-5× more API calls fixing compounded errors).

Pre-Operation Checks

Before creating geometry, verify:

1. Which body am I modifying? (confirm it exists)
2. Which sketch plane? (XY/XZ/YZ — see direction table below)
3. Which direction will the extrude go?
4. Will the tool body overlap the target? (bounding box check for booleans)

Sketch Plane Direction Table

This is the #1 source of errors. Memorize or reference before every sketch:

| Sketch Plane | Sketch X → | Sketch Y → | Extrude → | |-------------|------------|------------|-----------| | XY (offset in Z) | Model X | Model Y | ±Z | | XZ (offset in Y) | Model X | Model Z | ±Y | | YZ (offset in X) | Model Y | Model Z | ±X |

⚠️ Offset planes can FLIP axes! XZ plane offset in -Y flips sketch Y → -Z. Always verify with bounding box after first extrude.

Boolean Pre-Check

Before any boolean cut, verify tool/target overlap:

t_bb = tool_body.boundingBox
b_bb = target_body.boundingBox
overlap = (t_bb.maxPoint.x > b_bb.minPoint.x and t_bb.minPoint.x < b_bb.maxPoint.x and
           t_bb.maxPoint.y > b_bb.minPoint.y and t_bb.minPoint.y < b_bb.maxPoint.y and
           t_bb.maxPoint.z > b_bb.minPoint.z and t_bb.minPoint.z < b_bb.maxPoint.z)
if not overlap:
    print("WARNING: No overlap — boolean will fail!")

Section Views for Internal Geometry

Cuts, pockets, bore holes — anything inside a body — need a section view to verify:

planes = rootComponent.constructionPlanes
inp = planes.createInput()
inp.setByOffset(rootComponent.xYConstructionPlane, adsk.core.ValueInput.createByReal(offset_cm))
plane = planes.add(inp)
section = rootComponent.analyses.createSectionAnalysis(plane)
# ... screenshot + verify ...
section.deleteMe()
plane.deleteMe()

Camera Control

cam = app.activeViewport.camera
cam.eye = adsk.core.Point3D.create(ex, ey, ez)
cam.target = adsk.core.Point3D.create(tx, ty, tz)
cam.upVector = adsk.core.Vector3D.create(0, 0, 1)
cam.viewExtents = 5.0  # cm — ~3× feature size
cam.isSmoothTransition = False
app.activeViewport.camera = cam
app.activeViewport.refresh()

Screenshot Helper

Combine camera + screenshot + viewport save in one Fusion call:

# Zoom to area, screenshot, return path
cam = app.activeViewport.camera
cam.eye = adsk.core.Point3D.create(ex, ey, ez)
cam.target = adsk.core.Point3D.create(tx, ty, tz)
cam.upVector = adsk.core.Vector3D.create(0, 0, 1)
cam.viewExtents = extent
cam.isSmoothTransition = False
app.activeViewport.camera = cam
app.activeViewport.refresh()
path = '/tmp/fusion-verify.png'
app.activeViewport.saveAsImageFile(path, 1920, 1080)
print(f'SCREENSHOT:{path}')

Then: cp /tmp/fusion-verify.png ~/clawd/fusion-verify.png and use image tool with cheap model.

Load references/verification-checklist.md for the full checklist with failure examples from real builds. Load references/visual-feedback.md for camera presets and section view patterns.

Common Operations Reference

Load references/operations.md for detailed patterns covering:

• Sketches (lines, circles, arcs, rectangles, splines, constraints, dimensions)
• Features (extrude, revolve, fillet, chamfer, shell, draft, loft, sweep)
• Boolean operations (join, cut, intersect)
• Assembly (joints, as-built joints)
• Patterns (rectangular, circular, mirror)
• Construction geometry (planes, axes, points)
• Model tree navigation
• Measurement

Key Gotchas

• Units are cm in the API. Always convert: 10mm = 1.0 in API.
• store_as is essential for multi-step operations. Store sketches, profiles, bodies, features.
• Profile selection: After creating a sketch, profiles are auto-generated. Access via $sketch.profiles.item(0).
• Extrude distance uses ValueInput: {"type": "ValueInput", "expression": "10 mm"} or {"value": 1.0} (cm).
• Boolean operations: Set operation type as integer in ExtrudeInput — Join=0, Cut=1, Intersect=2, NewBody=3, NewComponent=4.
• Thread safety: All calls are queued to Fusion's main thread automatically. No concurrency issues.
• Error handling: Check response for success field. On failure, read the error message and adjust.
• Python mode is preferred for complex multi-step operations — fewer round trips, access to loops/conditionals.