cadkit — Onshape MCP

A 2 inch pipe flange, generated by Claude Opus 4.8.

Two Model Context Protocol servers for driving Onshape from an LLM:

• `cadkit` — the focus of this fork. A part-modeling server built around one idea: every

part should come out idiomatic, fully-defined, and variable-driven — the way a careful human models, not a pile of absolute coordinates. One sketch carries its entities, geometric constraints, and driving dimensions; it's grounded to the origin and parameterized by variables; downstream features select edges and faces by meaning (concave edge, cylindrical face) rather than by transient ids that break when topology shifts.

• `onshape_mcp` — the upstream server this repo forked from (hedless/onshape-mcp),

kept intact. Broader and assembly-focused (mates, instances, interference, export). Reach for it when you're assembling parts rather than authoring one.

Why two servers? onshape_mcp is wide; cadkit is opinionated. cadkit deliberately emits a narrower, stricter shape of geometry so that what you get back is parametric and editable, not just present. See PLAN.md for the thesis and roadmap.

Why cadkit models the way it does

A few hard-won principles are baked into the tools (the full list is in PLAN.md):

• Grounded + dimensioned, or it warns. cad_sketch_close reports whether the sketch is

grounded to the origin and dimensioned; require_well_formed=true refuses to ship an under-defined sketch instead of letting the solver place it unpredictably.

• Variables drive geometry, but only where they earn it. A dimension, an extrude depth, a

hole diameter, a fillet radius — all accept a number or an expression / #variable. Use a variable when a value travels beyond one sketch or is derived (#leg_len - #thick); use a geometric constraint (equal, symmetric) when the relationship lives between entities; use a literal for a true one-off.

• Select by meaning, not by id. cad_find_edges / cad_find_faces return deterministic ids

chosen by geometry (concave edges for fillets, a cylindrical face by radius), so a feature keeps referring to the right thing after the model changes.

The cadkit tools (35)

A sketch is one session: cad_sketch_begin(plane=… | face=<id>), add entities, add geometric constraints + driving dimensions, then cad_sketch_close. cad_pattern / cad_mirror take the featureIds of the features to repeat (e.g. an extrude or hole) plus a direction/axis/plane.

A small example (L-bracket, parametric)

cad_set_variable("leg", "2 in"); cad_set_variable("thick", "0.25 in")
sk = cad_sketch_begin(plane="Front")
#   draw the L profile with cad_sketch_polyline / line, then:
cad_sketch_constrain("ground_origin", a="ln1.start")   # pin to origin
cad_sketch_dimension(kind="length", target="ln1", value="#leg")
# ... fully define ...
cad_sketch_close(require_well_formed=true)              # refuses if under-defined
cad_extrude(sketchFeatureId=sk, depth="#thick", operation="NEW")

Variable-driven centers (no bolt-circle macro needed)

A center moves with a variable only if a dimension references that variable. To place a hole at (#hx, #hy), dimension its center from the origin:

cir = cad_sketch_circle(center=[2, 1], radius=0.25)    # nominal spot; the dims drive it
cad_sketch_dimension(kind="diameter", entity=cir, value="#bore")
cad_sketch_dimension(kind="position", entity=cir+".center", value=["#hx", "#hy"])  # H + V dims

kind="position" emits a horizontal and a vertical distance from the origin (null skips an axis); kind="distance" with direction="horizontal"|"vertical" does the same between any two entities. A bolt circle is then just a circular pattern (cad_sketch_pattern / cad_pattern) of one hole whose seed sits on a construction circle dimensioned to #bcd — no dedicated feature required.

Install

Both servers live in this one repo and share the same Onshape client.

git clone https://github.com/saltyeg/cadkit-mcp.git
cd cadkit-mcp
python -m venv venv && source venv/bin/activate
pip install -e .

Credentials

You need an Onshape API access key + secret key from the Onshape Developer Portal. cadkit resolves them in this order:

1. ONSHAPE_ACCESS_KEY / ONSHAPE_SECRET_KEY environment variables, else
2. the onshape MCP server entry already in your ~/.claude.json (so if you've configured the

onshape_mcp server, cadkit reuses those keys — you never paste them twice).

See .env.example for all supported variables.

OAuth2 (bring your own account)

cadkit also supports OAuth2 — authenticating as the user via their own Onshape account instead of API keys. This is the architecture behind the "bring-your-own-agent" model and the path to an App Store listing whose calls are exempt from the per-user annual quota. It's optional; API keys remain the default and nothing changes if you don't use it.

1. Register a Connected desktop app (OAuth application) in the

Onshape Developer Portal with:

• Redirect URI http://localhost:8910/callback (must match exactly)
• Scopes read, write, delete (OAuth2Read OAuth2Write OAuth2Delete)

1. Put the issued credentials in .env (or your environment):

   ONSHAPE_OAUTH_CLIENT_ID=…
   ONSHAPE_OAUTH_CLIENT_SECRET=…

1. Run the one-time browser handshake:

   cadkit-auth login     # opens the browser, stores tokens at ~/.cadkit/onshape_token.json
   cadkit-auth status    # show token + expiry;  cadkit-auth logout to revoke locally

Once a token is stored, the cadkit server prefers it over API keys automatically (with silent refresh). Caveat: until the app is published in the App Store it's a private OAuth app, so calls still count against the 2,500/yr quota exactly like API keys — OAuth buys the right architecture, not quota relief, until launch.

Register with Claude Code

Add to ~/.claude.json (or ~/.claude/mcp.json). The cadkit entry can omit keys if the onshape entry already has them:

{
  "mcpServers": {
    "onshape": {
      "command": "/abs/path/to/onshape-mcp/venv/bin/python",
      "args": ["-m", "onshape_mcp.server"],
      "env": { "ONSHAPE_ACCESS_KEY": "…", "ONSHAPE_SECRET_KEY": "…" }
    },
    "cadkit": {
      "command": "/abs/path/to/onshape-mcp/venv/bin/python",
      "args": ["-m", "cadkit_mcp.server"]
    }
  }
}

Use the absolute path to the venv's Python. Restart Claude Code after editing the config or after any change to the server code (a running server holds the old module until restart).

API quota — read this before testing

The Onshape free / standard / education-student tiers allow 2,500 _successful_ API calls per user per year (limits doc). Only 2xx/3xx responses count — 4xx/5xx are free; 429 is a separate short-term burst limit; 402 means the annual budget is spent. A naive live test suite drains this fast.

cadkit's development practice is built around that constraint:

• Offline-first tests. tests/test_cadkit_builders.py asserts on the **JSON the builders

emit — parameter ids, enum strings, constraint structure — with zero** API calls. This catches the bug class that actually costs debugging time (a wrong/hidden parameterId).

• `cadkit_mcp/devkit.py` — quota-frugal live helpers: ScratchStudio reuses one part studio

across checks; measure_fs returns bbox / volume / count / sketch bbox / named variables in a single FeatureScript eval (SOLID-body filtered, inch-converted).

• One on-demand live smoke (~6–8 calls), run by hand before a release — only for truths

offline can't prove (a variable actually drives geometry; a concave edge actually fillets).

# offline builder tests — free, run anytime
venv/bin/python -m pytest tests/test_cadkit_builders.py -o addopts="" -q

Layout

cadkit_mcp/
├── server.py     # the cadkit tools + feature JSON builders
├── sketch.py     # SketchSession: entities, constraints, grounding, diagnostics
├── selection.py  # semantic edge/face finders (FeatureScript-backed)
├── quota.py      # successful-call counter behind cad_api_calls
├── hole_template.json  # 160-param native Hole feature template
└── devkit.py     # quota-frugal live verification helpers
onshape_mcp/       # inherited upstream server (assemblies, mates, export) — see git history
tests/            # offline builder tests (zero-API)
PLAN.md           # cadkit thesis + roadmap (P0–P3)

Roadmap

cadkit is ordered so the parametric core is correct before feature breadth — see PLAN.md. Shipped (P0–P2): the sketch session, idempotent variables, parametric scalars everywhere, extrude/revolve/fillet/chamfer/shell/hole, sketch-on-face, feature-based pattern/mirror, semantic edge/face selection, plus inspection/lifecycle/IO — cad_measure, cad_get_variables, cad_delete_feature, cad_suppress, cad_edit_feature, cad_export. In progress (P3): richer semantic selection (largest/smallest/extreme/adjacency/on-plane done; by-tag next) and sketch ergonomics (slots, center-point arcs, fillets, construction geometry done; in-sketch mirror live-verified; in-sketch pattern emits geometric copies). Deferred: cad_rollback, mass/COM in cad_measure, and tapped threads on the native Hole feature.

Notes

Not tested on assemblies yet, only individual parts

Credits

Forked from hedless/onshape-mcp; the onshape_mcp server and its assembly tooling are upstream's work. Built on the Model Context Protocol and the Onshape REST API. MIT License.