3mf-to-fusion

3MF / STL to Fusion 360 Analytical Reverse-Engineering Skill

When asked to copy, reverse-engineer, or recreate a .3mf or .stl file in Autodesk Fusion 360, follow this deterministic analytical pipeline.

THE CAD REVERSE-ENGINEERING MANDATE

[!IMPORTANT] STRICTLY FORBIDDEN: Never use Fusion 360's built-in "Convert Mesh to Solid" (MeshToBREP or bRepBodies.addByMesh).

Converting mesh facets directly into BRep creates tens of thousands of planar triangular faces that freeze the viewport, cannot be filleted or chamfered, break downstream CAM/drawings, and destroy all parametric design intent.

MANDATORY: Dissect the mesh mathematically ("slice and dice"), extract its 2D cross sections and geometric primitives (slots, circumscribed holes, counterbores, turned profiles, rectangular patterns), and construct 100% native parametric solid bodies in the Fusion 360 timeline using sketches, driving user parameters, extrusions, revolves, and pattern features.

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Phase 0: Pre-Flight Safety Gate (Mandatory)

Before processing files, verify that Autodesk Fusion 360 and its MCP server are live:

1. Canary Probe: Call fusion-mcp tool execute_api_script:

   def run(context):
       import adsk.core, adsk.fusion
       app = adsk.core.Application.get()
       if not app:
           raise RuntimeError("Autodesk Fusion 360 application instance not found.")
       design = adsk.fusion.Design.cast(app.activeProduct)
       if not design:
           raise RuntimeError("No active Fusion 360 design document open.")
       print("FUSION_MCP_READY")
   

2. Fail-Fast Abort Rule:

   • If the call fails or times out, STOP immediately.
   • Do NOT run extraction scripts or CAD commands.
   • Instruct the user to open Fusion 360, ensure the add-in is started, and open an active document.

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Phase 1: Slice, Dice & Classify (Metrology Engine)

[!IMPORTANT] Workspace Isolation Rule: Never output extraction files into the main repo root (e.g. ./extracted_cad is forbidden). Always ensure a dedicated model folder exists under models/<NN>_<Model_Name>/ (scaffold with scaffold_text_model.py "<Model_Name>" if new), and route all slice/dice outputs into models/<NN>_<Model_Name>/workspace/extracted_cad.

1. Execute the deep metrology engine into the model's isolated workspace:

   python3 <path_to_skills>/3mf-to-fusion/scripts/inspect_3mf.py <path_to_file.3mf_or_stl> --out-dir models/<NN>_<Model_Name>/workspace/extracted_cad
   

2. Read models/<NN>_<Model_Name>/workspace/extracted_cad/manifest.json.

3. Check the archetype and detected features for each part:

   • Type A: Prismatic / Stepped CAD: Planar base extrusion + pocket cuts + hole arrays.
   • Type T: Turned / Axisymmetric: Collinear circular slices along Z axis. Modeled using a single half-profile sketch + 360° RevolveFeature.
   • Type B: Multi-tier Enclosure / Shell: Stepped construction planes + thin-wall extrusions + shell.
   • Type C: Organic Freeform Sculpture: High non-planar curvature ($> 15$ tiers). Immediately alert the user:

     "This part is a continuous organic sculpture without discrete planar faces or prismatic sketches. Reconstructing it using planar sketches will generate a stepped staircase approximation rather than a smooth organic sculpt."

4. Present a summary table to the user:

   Part ID	Archetype	Bounding Box ($X \times Y \times Z\text{ mm}$)	Tiers	Key Primitives / Patterns Detected

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Phase 2: Metrology Mathematics & Rules

1. Unit Conversion (cm = mm / 10.0):
   • Fusion 360's internal database (adsk.core.ValueInput.createByReal()) strictly uses centimeters (cm).
   • Define at the top of every script:

     def mm(val): return adsk.core.ValueInput.createByReal(float(val) / 10.0)
     

2. Circumscribed Circle Compensation (Chord Error):
   • STL tessellations approximate circular holes with inscribed polygons whose edges cut inward along chords.
   • Never use the inner minimum diameter. Always use radius_mm from manifest.json["primitives"]["circles"] (95th-percentile circumscribed radius) rounded to the nearest $0.05\text{ mm}$.
3. Slot / Obround Recognition:
   • When loops have two parallel straight lines and two semicircular ends, model them as a seed slot (sketchLines + sketchArcs) rather than a multi-segment polygon.
4. Pattern Recognition (Grid / Polar):
   • When manifest.json["patterns"] detects a regular pitch ($\Delta X, \Delta Y$), model one master seed cutout and duplicate it using comp.features.rectangularPatternFeatures. Do not draw repetitive identical geometry by hand.

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Phase 3: Pure Parametric Fusion 360 Reconstruction

Execute CAD generation via execute_api_script. Reconstruct each part using clean timeline features:

Step 1: Occurrence & User Parameters

transform = adsk.core.Matrix3D.create()
occ = root.occurrences.addNewComponent(transform)
comp = occ.component
comp.name = part_name

# Add Driving Parameters
params = design.userParameters
params.add(f"{part_name}_width", mm(width_mm), "mm", "Base width")
params.add(f"{part_name}_length", mm(length_mm), "mm", "Base length")
params.add(f"{part_name}_height", mm(height_mm), "mm", "Base height")

Step 2: Primary Solid Geometry

• If Type T (Turned): Sketch half-profile on comp.xZConstructionPlane and call comp.features.revolveFeatures.add(prof, comp.zConstructionAxis, adsk.fusion.FeatureOperations.NewBodyFeatureOperation).
• If Type A/B (Prismatic): Sketch base outline on comp.xYConstructionPlane (centered at origin) and extrude base solid.

Step 3: Secondary Cutouts & Patterns

• Draw master seed cutout (slot, counterbore, or pocket).
• Apply comp.features.extrudeFeatures.add with adsk.fusion.FeatureOperations.CutFeatureOperation.
• Apply comp.features.rectangularPatternFeatures.add across comp.xConstructionAxis and comp.yConstructionAxis.

Step 4: Finishing Touches

• Apply corner fillets (comp.features.filletFeatures) and chamfers (comp.features.chamferFeatures).

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Phase 4: Reference Ghost Overlay & In-CAD Inspection

To verify mathematical and dimensional alignment without polluting the final model:

1. Ghost Reference Mesh (Optional): If detailed visual alignment is needed, import the raw mesh into a separate temporary reference occurrence:

   # Import mesh as reference backdrop
   ref_occ = root.occurrences.addNewComponent(transform)
   ref_occ.component.name = "Reference_Mesh_Ghost"
   # Set transparent visual style
   

2. Visual & Interference Inspection:
   • Check that the parametric solid completely encompasses and aligns with the mesh envelope.
   • Once verified, hide or remove ref_occ.

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Phase 5: Timeline Health & Visual Self-Verification Gate

1. Timeline Feature Verification: Ensure zero mesh bodies exist in the reconstructed part:

   assert comp.bRepBodies.count > 0, "No solid bodies produced!"
   assert comp.meshBodies.count == 0, "Forbidden MeshBody detected in component!"
   assert comp.sketches.count > 0, "No sketches found in timeline!"
   

2. Visual Inspection: Call get_screenshot(view="iso-top-right", width=1024, height=1024) to visually verify the clean parametric solid model and the clean timeline tree.