Prompt-Driven Design with SolidWorks MCP¶

You know SolidWorks. This guide shows you how to describe what you want to build in plain language, let an LLM translate that into the right tool calls, and have SolidWorks build it — without clicking through menus.

The examples below use real SolidWorks sample parts as targets. Because the finished .SLDPRT files already exist, you can open them and check the feature tree to confirm whether your prompts produced the right result. That makes them ideal for learning the workflow before applying it to your own designs.

What You Need¶

• SolidWorks installed and open
• MCP server running (.\dev-commands.ps1 dev-install then .\dev-commands.ps1 dev-run if needed)
• Claude Code (this tool) or VS Code with Copilot Chat
• Python environment activated: .\.venv\Scripts\python.exe

The Core Workflow¶

Every design session follows the same loop:

flowchart LR
    D(["1 · Describe\nWhat to build\n+ dimensions"])
    P(["2 · Plan\nLLM proposes\nMCP call sequence"])
    R(["3 · Review\nYou approve\nthe plan"])
    E(["4 · Execute\nClaude Code runs\nMCP tools"])
    C(["5 · Check\nVisual or\nfeature-tree"])
    I(["6 · Iterate\nRefine dimensions,\nadd features"])

    D --> P --> R --> E --> C --> I
    I -->|"new idea or fix"| D

    style R fill:#f0f4ff,stroke:#4a6cf7
    style C fill:#f0f4ff,stroke:#4a6cf7

Steps 3 (Review) and 5 (Check) are yours. The LLM handles 2 and 4.

Step 1 — Describe What You're Building¶

Be specific about shape and size. Adjectives like "wide" or "thin" are ambiguous. Geometry and dimensions are not.

Good description¶

I want to create a paper airplane shape.
It should be a flat delta-wing profile — like looking down at a paper airplane from above.
The nose points right at (80, 0), the two wing tips are at (0, 60) and (0, -60),
and everything connects back to the origin.
Extrude it 0.5 mm — just enough thickness to represent folded paper.

What not to say¶

Make me a flat airplane shape, kind of thin.

No dimensions. No plane. No feature type. The LLM will guess, and the guess will be wrong.

Plane names (must be exact)¶

SolidWorks default planes are case-sensitive. Use these exactly:

Step 2 — Let the LLM Plan the Tool Sequence¶

After your description, ask for a plan before executing anything. This is the most important habit — reviewing a text plan takes seconds; undoing a bad extrusion takes longer.

Prompt to use¶

Based on this description, write the exact sequence of SolidWorks MCP tool calls
to build it from scratch. Rules:
- Plane names exactly: "Front", "Top", or "Right"
- All dimensions in millimetres
- Dependency order: create_sketch → add geometry → exit_sketch → create feature
- Named arguments on every call
- If any step needs a VBA macro (loft, sweep, shell, sheet metal), say so and write
  the generate_vba_part_modeling call instead of a direct tool call

Show me the numbered list. Do not execute anything yet.

The LLM returns a numbered list. Read it. If step 5 says create_extrusion(depth=500) and you wanted 5 mm, fix it before running.

Step 3 — Execute the Plan¶

Once the plan looks right, tell Claude Code to run it:

That looks correct. Execute each step using the SolidWorks MCP server.
Confirm each step succeeds before moving to the next.
If any step fails, stop and show me the error.

Claude Code calls each MCP tool in sequence. SolidWorks builds the part live.

Step 4 — Check the Result¶

Visual check¶

Ask Claude Code to export an image:

Export an isometric view: export_image(file_path="my_part.jpg", format_type="jpg")
Then show me the image.

Drag the image into the chat or open it in Photos. Does it look right?

Feature tree check (for sample parts)¶

If you're building one of the SolidWorks sample parts, open the original:

open_model(file_path=r"C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2026\samples\learn\Paper Airplane.SLDPRT")
list_features()
close_model(save=False)

Compare the feature families and order, not just one matching name. If the original tree shows sheet metal, flanges, bends, or unfold/fold operations, a single matching sketch or extrusion is not enough.

Step 5 — Iterate¶

Design is never one-shot. Common iteration patterns:

Change a dimension¶

The wing is too narrow. Change the wing tip Y coordinates from ±60 to ±80
and re-extrude. Keep everything else the same.

Add a feature¶

Add a 2mm fillet to all the outer edges of the extrusion.

Fix an error¶

The extrusion failed with "sketch not closed". Show me the current sketch geometry
and identify which lines are missing to close the profile.

Tutorial 1 — Paper Airplane Audit¶

Sample file: Paper Airplane.SLDPRT SolidWorks feature: Sheet metal workflow with a base flange and downstream bends What you'll learn: Why the feature tree must drive delegation before you attempt a rebuild

Your starting prompt¶

Open the original Paper Airplane sample and inspect it before planning a rebuild.

Run `open_model`, `get_model_info`, `list_features(include_suppressed=True)`,
and `get_mass_properties()`. Then answer:

1. What is the first real modeling feature after the reference planes?
2. Does the tree indicate sheet metal, bends, or unfold/fold states?
3. Which downstream features depend on that first feature?
4. Should this be executed with direct MCP modeling tools, a VBA plan, or both?

Expected conclusion¶

The Paper Airplane sample is not a good first "single sketch + extrude" lesson.
Its tree must be treated as a sheet metal sequence rooted in a base flange.
Delegate reconstruction planning to the part reconstructor and preserve the
feature-family ordering instead of approximating the silhouette.

Execute and check¶

Execute the plan. After the extrusion, run:
export_image(file_path="paper_airplane_gen.jpg", format_type="jpg")

Then open the real sample for comparison:

open_model(file_path=r"C:\Users\Public\Documents\SOLIDWORKS\SOLIDWORKS 2026\samples\learn\Paper Airplane.SLDPRT")
list_features()
close_model(save=False)

The useful check here is whether your audit identified the correct feature family and dependency chain. Do not validate this sample by looking for a single Boss-Extrude1.

Tutorial 2 — Baseball Bat¶

Sample file: Baseball Bat.SLDPRT SolidWorks feature: Half-profile sketch + revolve 360° What you'll learn: How to describe a revolved part and specify the centerline

Your starting prompt¶

I want to build a baseball bat in SolidWorks.

Shape: a symmetric bat profile revolved 360° around its long axis
Sketch plane: Right
Dimensions:
  - Total length: 830 mm
  - Revolution axis: centerline along the X axis from (0,0) to (830,0)
  - Knob at handle end: small arc, radius ~17mm centered at (0, 17)
  - Handle: thin cylinder ~17mm radius from x=0 to x=150
  - Taper from handle to barrel: radius increases from 17mm to 35mm, x=150 to x=680
  - Barrel: constant 35mm radius, x=680 to x=790
  - Barrel end cap: small arc closing the top
  - The half-profile connects back to the centerline at both ends

Part name: "Baseball Bat"

Write the MCP tool call sequence. Do not execute yet.

What to watch for in the plan¶

The plan should include:

1. create_sketch(plane_name="Right")
2. add_centerline(...) — the revolve axis
3. Multiple add_line and add_arc calls tracing the half-profile
4. exit_sketch()
5. create_revolve(sketch_name="Sketch1", axis_entity="Line1", angle=360.0)

If the LLM skips add_centerline or tries to use a construction line as the axis without naming it, correct before running:

Step 3 is missing the centerline. Add:
add_centerline(start_x=0, start_y=0, end_x=830, end_y=0)
before the profile lines, and use that as the axis_entity in create_revolve.

Tutorial 3 — U-Joint Assembly¶

Sample files: U-Joint/ directory — 9 parts SolidWorks feature: Multi-part assembly with coincident and concentric mates What you'll learn: How to describe assemblies and mates, and when to use VBA

The U-Joint is the most complex sample and the best model for assembly workflows. Build each part separately first, then assemble.

Part 1 of 9: Spider¶

The spider is the cross-shaped centre piece. Start here because it's the assembly anchor.

I want to build the spider component for a U-Joint.

Shape: a cross — four cylindrical arms extending from a central sphere
Sketch plane: Front
Approach: revolve a plus-sign half-profile 360°, or use VBA if needed
Dimensions:
  - Central hub: 15mm radius sphere
  - Four arms: each 8mm radius, 25mm long, pointing in +X, -X, +Y, -Y from hub centre
  - Arms are symmetric

Part name: "spider"

Write the MCP tool call sequence. Flag if VBA is required.

Assembly prompt (after all parts are built)¶

Create a U-Joint assembly.

Components (all in the same directory):
  crank-shaft.sldprt, yoke_male.sldprt, yoke_female.sldprt,
  spider.sldprt, bracket.sldprt, pin.sldprt, crank-arm.sldprt, crank-knob.sldprt

Assembly mates needed:
  1. crank-shaft long axis coincident with yoke_male bore axis
  2. spider centre coincident with yoke_male rotation centre
  3. spider pin arms fit into yoke_male ear bores (concentric)
  4. yoke_female mirrors yoke_male on the other spider axis pair
  5. bracket fixes to the frame reference

Use generate_vba_assembly_insert and generate_vba_assembly_mates.
Write the sequence — do not execute yet.

Using the Agent CLI for Planned Runs¶

For repeatable, logged runs — especially when testing a new part concept before running in SolidWorks — use the smoke test CLI. Results are saved to .solidworks_mcp/agent_memory.sqlite3.

# Plan a reconstruction using the reconstructor agent
.\.venv\Scripts\python.exe -m solidworks_mcp.agents.smoke_test `
  --agent-file solidworks-part-reconstructor.agent.md `
  --github-models `
  --schema reconstruction `
  --prompt "Baseball bat: half-profile on Right plane, revolved 360 degrees. 830mm long, 17mm handle radius, 35mm barrel radius. Plan the MCP reconstruction."

This returns a validated ReconstructionPlan JSON — a structured, typed plan you can hand back to Claude Code for execution.

# Get a manufacturability check on your design before committing
.\.venv\Scripts\python.exe -m solidworks_mcp.agents.smoke_test `
  --agent-file solidworks-print-architect.agent.md `
  --github-models `
  --schema manufacturability `
  --prompt "ABS baseball bat handle, 17mm radius, 150mm long. Bambu X1C printer (256x256x256). Print orientation and support strategy?"

Iteration Cheat Sheet¶

Common Errors¶

What's Next¶

• Sample Models Guide — pre-written feature sequences for every learn sample part
• Prompting Best Practices — detailed prompt engineering for MCP tools
• Agents and Testing — full agent CLI reference
• Tools Overview — complete MCP tool catalogue

Planned: Full Reverse-Engineering Workflow¶

A future guide will document the automated reverse-engineering loop: open an existing part programmatically, read its feature tree and mass properties, feed that data to the solidworks-part-reconstructor agent to generate a ReconstructionPlan, execute it, and compare outputs via pixel diff and mass property matching. This is tracked in docs/planning/ROADMAP_2026_2027.md.