solidworks-mcp

An MCP server that drives a local SOLIDWORKS installation to build and modify parametric solid models.

Verified against SOLIDWORKS 2026 SP0 (revision 34.0.0) on Windows 11.

How it works

MCP client  ──stdio──►  solidworks-mcp  ──COM──►  SLDWORKS.exe

SOLIDWORKS exposes a classic COM automation API. The server attaches to a running instance (or launches one), and every tool maps onto that API.

All lengths are in millimetres and all angles in degrees. The SOLIDWORKS API is metric-SI internally; conversion happens at the tool boundary.

Requirements

• SOLIDWORKS installed and licensed, on the same machine.
• Python 3.12+, 64-bit — it must match SOLIDWORKS' architecture or COM will not bind.
• uv for dependency management.

Install

uv sync

Register with an MCP client

For Claude Code:

claude mcp add solidworks -- uv --directory E:\solid run solidworks-mcp

For a client that reads a JSON config:

{
  "mcpServers": {
    "solidworks": {
      "command": "uv",
      "args": ["--directory", "E:\\solid", "run", "solidworks-mcp"]
    }
  }
}

Tools

Session and documents — solidworks_status, new_part, open_part, save_part, close_part

Sketching — list_planes, start_sketch, start_sketch_on_face, sketch_line, sketch_centerline, sketch_circle, sketch_rectangle, sketch_arc, sketch_polygon, sketch_ellipse, add_sketch_dimension, add_sketch_relation, finish_sketch

Features — extrude, cut_extrude, revolve, fillet, select_entity, clear_selection

Parametric control — list_features, list_dimensions, set_dimension, add_equation, list_equations, rebuild

Inspection — get_measurements, capture_view

A worked example

Building a 80 × 50 × 10 mm plate with a hole, then driving it parametrically:

new_part
start_sketch(plane="front")
sketch_rectangle(0, 0, 80, 50)
add_sketch_dimension(entities=[[40, 0]], value=80)   -> "D1@Croquis1"
add_sketch_dimension(entities=[[0, 25]], value=50)   -> "D2@Croquis1"
finish_sketch
extrude(depth=10)

start_sketch(plane="front")
sketch_circle(40, 25, 8)
finish_sketch
cut_extrude(depth=10, end_condition="through_all", reverse=True)

fillet(radius=5, edges=[[0,0,5], [80,0,5], [80,50,5], [0,50,5]])

set_dimension("D1@Croquis1", 120)   -> the solid rebuilds to 120 mm wide
get_measurements                    -> bounding box 120 x 50 x 10 mm
capture_view("isometric")

Things worth knowing

Sketches created through the API have no dimensions. SOLIDWORKS only adds driving dimensions when you ask for them, so a sketch drawn with sketch_* alone has nothing to drive. Call add_sketch_dimension while the sketch is still open if you intend to change the geometry later.

Cut direction follows the sketch normal. A sketch on the Front Plane cutting a solid that was extruded away from it needs reverse=True, otherwise the cut travels into empty space and fails.

Reference plane names are localised. A Spanish install names features Croquis1 and Saliente-Extruir1. Tools accept the logical aliases front/top/right and resolve them by position in the feature tree, so they work regardless of UI language. list_planes reports the real names.

SOLIDWORKS must be running. There is no supported headless mode. The server launches the application if it is not already open.

Modal dialogs deadlock COM. add_sketch_dimension temporarily disables the "input dimension value" preference, which would otherwise pop a modal box and hang the call, and restores it afterwards.

Implementation notes

Two pywin32 behaviours shape the code and are easy to trip over:

• Zero-argument COM members are auto-invoked on attribute access. Under late binding doc.GetTitle returns the title string; doc.GetTitle() raises TypeError: 'str' object is not callable. Members taking one or more arguments are called normally.
• Typed nulls and in/out parameters need explicit VARIANTs. Optional interface arguments reject a bare None with "Type mismatch" and need VARIANT(VT_DISPATCH, None); error and warning out-parameters need VARIANT(VT_BYREF | VT_I4, 0), with the result read back from .value.

COM objects live in a single-threaded apartment, so com_bridge.py funnels every call through one dedicated thread. Enum values in constants.py were read from swconst.tlb rather than transcribed from documentation, because some differ from commonly quoted values — swEndCondThroughAllBoth is 9, not 8.