Prompting Tutorials

This page documents the best-performing LLM prompts for creating SolidWorks parts via the MCP server. Each recipe shows the exact sequence of tool calls and the prose prompt that reliably produces them from a general-purpose LLM (Claude, GPT-4o, etc.).

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Standard Tool-Call Sequence

Every part creation follows the same six-step pipeline regardless of shape complexity:

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Prompt Engineering Principles

1. Prefer specific geometry over adjectives

❌ "Make a wide, flat part"
✅ "Create a sketch rectangle x1=-50, y1=-25, x2=50, y2=25 then extrude 5 mm"

2. Use the correct plane names

SolidWorks default planes are exactly: "Front", "Top", "Right". Any variation ("XY", "front") will fail.

3. Emit tool calls in dependency order

A create_extrusion will fail if the active sketch hasn't been closed with exit_sketch first.

Correct order:

create_sketch → add_geometry → exit_sketch → create_extrusion/revolve

4. Always specify mm not m

All SolidWorks API lengths are in metres by default. The MCP server converts values > 0.5 automatically (see input_compat.py), but the safest approach is to always check:

# 10 mm should be passed as 10.0 (server normalizes)
# 0.01 m is also accepted

5. Add set_dimension to parametrize your model

After creating features, lock dimensions symbolically so the model can be driven by parameters later:

set_dimension name="D1@Sketch1" value=50.0
set_dimension name="D1@Boss-Extrude1" value=10.0

6. Read before write on existing parts

When editing an existing file, first request model context so the LLM does not guess feature/config names.

Recommended read sequence:

open_model -> get_model_info -> list_configurations -> list_features

Use this as a preface in your prompt:

Before changing geometry, open the part and return model info, configurations, and features.
Then propose the smallest edit plan and wait for confirmation.

7. Force bounded outputs for long sessions

Large responses can consume context and reduce reliability. Add an explicit response budget:

After each tool call, return only: tool, status, key fields.
Do not echo full arrays unless asked.

8. Make failure handling explicit

Use a deterministic recovery contract to avoid speculative retries:

If a tool fails, stop immediately and return:
1) failing tool
2) exact error
3) one minimal retry option
Do not continue remaining steps.

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Recipe 1 — Simple Block (30-second exercise)

Goal: A 100×60×20 mm rectangular block on the Front plane.

System prompt fragment

You are operating a SolidWorks MCP server. When creating parts, always call tools in this order:
create_part → create_sketch → [add geometry] → exit_sketch → create_extrusion → save_as.
All dimensions are millimeters. Use exact plane names: Front, Top, Right.

User prompt

Create a 100 mm × 60 mm × 20 mm block called "Simple Block".

Expected tool call sequence

[
  {"tool": "create_part",     "args": {"name": "Simple Block"}},
  {"tool": "create_sketch",   "args": {"plane": "Front"}},
  {"tool": "add_rectangle",   "args": {"x1": -50.0, "y1": -30.0, "x2": 50.0, "y2": 30.0}},
  {"tool": "exit_sketch",     "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch1", "depth": 20.0}},
  {"tool": "save_as",         "args": {"file_path": "C:\\Temp\\Simple Block.sldprt"}}
]

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Recipe 2 — Cylinder (Revolve)

Goal: A solid cylinder Ø50 mm × 80 mm.

User prompt

Create a solid cylinder, 50 mm diameter, 80 mm tall.
Name it "Cylinder".

Expected tool call sequence

[
  {"tool": "create_part",   "args": {"name": "Cylinder"}},
  {"tool": "create_sketch", "args": {"plane": "Front"}},
  {"tool": "add_centerline","args": {"x1": 0.0, "y1": 0.0, "x2": 80.0, "y2": 0.0}},
  {"tool": "add_rectangle", "args": {"x1": 0.0, "y1": 0.0, "x2": 80.0, "y2": 25.0}},
  {"tool": "exit_sketch",   "args": {}},
  {"tool": "create_revolve","args": {"sketch_name": "Sketch1", "axis_entity": "Line1", "angle": 360.0}},
  {"tool": "save_as",       "args": {"file_path": "C:\\Temp\\Cylinder.sldprt"}}
]

Tip

The centerline must be on the same sketch as the profile. Line1 refers to the first line added, which is the centerline.

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Recipe 3 — Baseball Bat

Goal: Faithful recreation of Baseball Bat.SLDPRT.

User prompt

Open the original Baseball Bat sample first and classify it before planning the rebuild.

Run:
- get_model_info()
- list_features(include_suppressed=True)
- get_mass_properties()
- classify_feature_tree(include_suppressed=True)

If the classifier recommends a direct revolve workflow, continue with a rebuild.
Then recreate a baseball bat approximately 830 mm long with:
- A 34 mm diameter knob at one end
- A 22 mm diameter handle for the first 180 mm
- A gentle taper out to a 70 mm barrel for the remaining length
- A hemispherical dome at the barrel end
Use a revolve around the horizontal axis.
Name it "Baseball Bat Recreation".

Expected tool call sequence

[
  {"tool": "get_model_info",   "args": {}},
  {"tool": "list_features",    "args": {"include_suppressed": true}},
  {"tool": "get_mass_properties","args": {}},
  {"tool": "classify_feature_tree","args": {"include_suppressed": true}},
  {"tool": "create_part",    "args": {"name": "Baseball Bat Recreation"}},
  {"tool": "create_sketch",  "args": {"plane": "Right"}},
  {"tool": "add_centerline", "args": {"x1": 0.0, "y1": 0.0, "x2": 830.0, "y2": 0.0}},
  {"tool": "add_arc",        "args": {"center_x": 0.0,   "center_y": 0.0, "start_x": 0.0,  "start_y": 17.0, "end_x": 17.0, "end_y": 0.0}},
  {"tool": "add_line",       "args": {"x1": 17.0, "y1": 17.0, "x2": 17.0, "y2": 22.0}},
  {"tool": "add_line",       "args": {"x1": 17.0, "y1": 22.0, "x2": 680.0, "y2": 35.0}},
  {"tool": "add_arc",        "args": {"center_x": 680.0, "center_y": 0.0, "start_x": 680.0, "start_y": 35.0, "end_x": 830.0, "end_y": 0.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_revolve", "args": {"sketch_name": "Sketch1", "axis_entity": "Line1", "angle": 360.0}},
  {"tool": "save_as",        "args": {"file_path": "C:\\Temp\\Baseball Bat Recreation.sldprt"}}
]

Why the classifier step is first

This is the lightweight proof that inspect-classify-delegate works on a simpler family. A baseball bat should route cleanly to direct-mcp-revolve, unlike the Paper Airplane sheet metal case.

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Recipe 4 — Box with Counterbore Holes

Goal: 80×60×15 mm box with four M6 counterbore holes at corners (Ø6 through, Ø10×5 cbore).

User prompt

Create a rectangular plate 80 × 60 × 15 mm with four M6 counterbore mounting holes.
Holes are centred 8 mm from each corner. Through bore Ø6 mm, counterbore Ø10 mm × 5 mm deep.
Name "Mounting Plate".

Expected tool call sequence

[
  {"tool": "create_part",    "args": {"name": "Mounting Plate"}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_rectangle",  "args": {"x1": -40.0, "y1": -30.0, "x2": 40.0, "y2": 30.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch1", "depth": 15.0}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_circle",     "args": {"center_x": -32.0, "center_y": -22.0, "radius": 3.0}},
  {"tool": "add_circle",     "args": {"center_x":  32.0, "center_y": -22.0, "radius": 3.0}},
  {"tool": "add_circle",     "args": {"center_x": -32.0, "center_y":  22.0, "radius": 3.0}},
  {"tool": "add_circle",     "args": {"center_x":  32.0, "center_y":  22.0, "radius": 3.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch2", "depth": 15.0, "direction": "cut"}}
]

Counterbore not yet supported directly

create_extrusion with direction=cut creates a blind cut. For a true counterbore hole (two-step), run two separate cut extrusions or use generate_vba_part_modeling.

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Recipe 5 — Hexagonal Bolt Head

Goal: M8 hexagonal bolt head, 13 mm across-flats, 8 mm thick.

User prompt

Create an M8 hex bolt head. Across-flats = 13 mm, height = 8 mm.
Name it "Bolt Head M8".

Expected tool call sequence

[
  {"tool": "create_part",    "args": {"name": "Bolt Head M8"}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_polygon",    "args": {"center_x": 0.0, "center_y": 0.0, "sides": 6, "circumradius": 7.505}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch1", "depth": 8.0}},
  {"tool": "save_as",        "args": {"file_path": "C:\\Temp\\Bolt Head M8.sldprt"}}
]

circumradius for hex

For 13 mm across-flats hex: circumradius = (13 / 2) / cos(30°) ≈ 7.505 mm.

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Recipe 6 — Circular Pattern of Features

Goal: A disc with 6 equally spaced Ø8 holes on a Ø60 mm pitch circle.

User prompt

Create a disc: Ø100 mm, 10 mm thick.
Add 6 through holes Ø8 mm equally spaced on a 60 mm pitch circle.
Name "Bolt Circle Disc".

Expected tool call sequence

[
  {"tool": "create_part",    "args": {"name": "Bolt Circle Disc"}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_circle",     "args": {"center_x": 0.0, "center_y": 0.0, "radius": 50.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch1", "depth": 10.0}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_circle",     "args": {"center_x": 0.0, "center_y": 30.0, "radius": 4.0}},
  {"tool": "sketch_circular_pattern","args": {"entity": "Arc1", "count": 6, "angle": 60.0, "center_x": 0.0, "center_y": 0.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch2", "depth": 10.0, "direction": "cut"}}
]

---

Recipe 7 — L-Bracket (Two Extrusions)

Goal: Steel L-bracket, 100 × 80 mm legs, 5 mm thick.

User prompt

Create an L-shaped bracket. Horizontal leg: 100 mm long. Vertical leg: 80 mm tall. Both legs 5 mm thick, 40 mm wide.
Name "L-Bracket".

Expected tool call sequence

[
  {"tool": "create_part",    "args": {"name": "L-Bracket"}},
  {"tool": "create_sketch",  "args": {"plane": "Front"}},
  {"tool": "add_line",       "args": {"x1": 0.0,   "y1": 0.0,  "x2": 100.0, "y2": 0.0}},
  {"tool": "add_line",       "args": {"x1": 100.0, "y1": 0.0,  "x2": 100.0, "y2": 5.0}},
  {"tool": "add_line",       "args": {"x1": 100.0, "y1": 5.0,  "x2": 5.0,   "y2": 5.0}},
  {"tool": "add_line",       "args": {"x1": 5.0,   "y1": 5.0,  "x2": 5.0,   "y2": 80.0}},
  {"tool": "add_line",       "args": {"x1": 5.0,   "y1": 80.0, "x2": 0.0,   "y2": 80.0}},
  {"tool": "add_line",       "args": {"x1": 0.0,   "y1": 80.0, "x2": 0.0,   "y2": 0.0}},
  {"tool": "exit_sketch",    "args": {}},
  {"tool": "create_extrusion","args": {"sketch_name": "Sketch1", "depth": 40.0}},
  {"tool": "save_as",        "args": {"file_path": "C:\\Temp\\L-Bracket.sldprt"}}
]

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Recipe 8 — Gear (VBA-assisted)

Goal: Spur gear, module 2, 20 teeth, 20° pressure angle, 15 mm face width.

LLM-native sketching cannot draw involute tooth profiles reliably. Use VBA generation:

User prompt

Generate VBA code to create a 20-tooth spur gear:
- Module 2, pressure angle 20°, face width 15 mm
- Material: 1020 Steel
Name the macro "create_gear.swp".

Expected tool call sequence

[
  {"tool": "generate_vba_part_modeling", "args": {
    "operations": [
      {"type": "gear", "module": 2, "teeth": 20, "pressure_angle": 20, "face_width": 15}
    ]
  }},
  {"tool": "execute_macro", "args": {"macro_path": "C:\\Temp\\create_gear.swp"}}
]

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Recipe 9 — Export Pipeline

After creating any part, a complete export pipeline looks like:

User prompt

Export the current model to STEP, STL, and a JPEG preview. Save all to C:\Exports\part_name\.

Expected tool call sequence

[
  {"tool": "export_step",  "args": {"file_path": "C:\\Exports\\part_name\\part_name.step", "format_type": "step"}},
  {"tool": "export_stl",   "args": {"file_path": "C:\\Exports\\part_name\\part_name.stl",  "format_type": "stl"}},
  {"tool": "export_image", "args": {"file_path": "C:\\Exports\\part_name\\part_name.jpg",  "format_type": "jpg"}}
]

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Recipe 10 — Mass Properties Report

Check the mass, volume, and centre of gravity for the currently open model.

[
  {"tool": "calculate_mass_properties", "args": {}},
  {"tool": "get_material_properties",   "args": {}}
]

The response will include SI values. For an aluminum 100×60×20 mm block: mass ≈ 324 g, volume ≈ 120 cm³.

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System Prompt Template

Copy this into your LLM system prompt when driving the MCP server:

You are an expert SolidWorks drafter operating a SolidWorks MCP server.

## Rules
1. Always call tools in dependency order:
   create_part → create_sketch → add_geometry → exit_sketch → create_feature → save_as
2. Plane names are exactly: "Front", "Top", "Right" (case-sensitive).
3. Dimensions are in millimeters.
4. If you are unsure about a parameter, add the word "cupcake" to your reasoning so I can spot edge cases.
5. After every feature operation, check the status field of the response:
   - "success" → continue
   - "error" → stop and report the error message
6. Do not assume a sketch is active — always call create_sketch explicitly.

## Common mistakes
- Never call create_extrusion before exit_sketch.
- Never assume a part is open — call create_part or open_model first.
- For circular patterns, count = number of total instances (including the seed).

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Troubleshooting Quick Reference

Symptom	Likely cause	Fix
SelectByID2 error	Wrong entity name format	Use FeatureByPositionReverse or VBA fallback
Extrusion returns error	Sketch still open	Call exit_sketch first
Revolve fails	No axis / wrong axis name	Add centerline in same sketch, name = "Line1"
Dimension not found	Name mismatch	Check "D1@FeatureName" format
Export writes 0-byte file	No active document	Open or create a part first
Mass = 0	No material assigned	Call get_material_properties to check