solidworks-mcp

An MCP server that drives a running SOLIDWORKS session over its COM API.

It does not launch SOLIDWORKS, register an add-in, execute arbitrary code, or touch the network. It attaches to a session you already have open and calls the documented API — so if a tool can't do something, neither could a macro.

92 tools: sketching with real relations and driving dimensions, the solid features you actually reach for, reference geometry, assemblies and mates, and — importantly — a feedback channel, including screenshots returned as images so the model can see what it just built.

A sibling server, autocad-mcp, does the same for AutoCAD.

Requirements

• Windows, with SOLIDWORKS installed and already running

• Python 3.10+

Related MCP server: SolidWorks MCP Server

Install

git clone https://github.com/limuzi013/solidworks-mcp.git
cd solidworks-mcp
py -3 -m venv .venv
.venv\Scripts\python.exe -m pip install .

That puts a solidworks-mcp command in the environment, which is what the MCP host runs. uv works too, if you prefer it:

uv tool install --from git+https://github.com/limuzi013/solidworks-mcp solidworks-mcp

Claude Code / Claude Desktop

{
  "mcpServers": {
    "solidworks-mcp": {
      "command": "C:\\path\\to\\.venv\\Scripts\\solidworks-mcp.exe"
    }
  }
}

Codex CLI (~/.codex/config.toml)

[mcp_servers.solidworks-mcp]
command = 'C:\path\to\.venv\Scripts\solidworks-mcp.exe'

Use single-quoted TOML strings so backslashes survive. Restart the MCP host after editing its configuration.

An MCP host can also be pointed straight at a checkout, with nothing installed but the dependencies — server.py at the repository root exists for exactly that:

[mcp_servers.solidworks-mcp]
command = 'C:\path\to\.venv\Scripts\python.exe'
args = ['C:\path\to\solidworks-mcp\server.py']

Configuration

The two ideas that make it usable

1. Units are explicit, always

Every length parameter ends in _mm and every angle in _deg. The COM API underneath is metres and radians; conversion happens once, at the boundary. No tool has ever silently taken metres.

2. Selection is declarative

SOLIDWORKS features read from an implicit global selection set, with per-feature "marks" deciding which selection means what. Exposing that to an agent is hopeless. Instead every tool that needs geometry takes the same selection object, and the server sets the marks:

// list_edges first, then:
{ "selection": { "edges": [4, 6, 9] } }
{ "selection": { "face_edges": [2] } }        // every edge of face 2
{ "selection": { "planes": ["front"] } }
{ "selection": { "sketch_segments": [0, 1] } }
{ "selection": { "points": [{ "x_mm": 30, "y_mm": 0, "z_mm": 20, "type": "FACE" }] } }

Indices come from list_faces / list_edges / list_vertices / list_sketch_segments and describe the current model state — re-list after any geometry change. Under the hood, selection resolves to a point that provably lies on the entity and picks by 3D coordinate, which survives the fact that late-bound Python cannot QueryInterface a Face2 to IEntity.

Tools

Session and documents

Reference geometry

list_reference_planes, create_plane (offset / angle / midplane / three points / parallel-through-point), create_axis.

Sketching

create_sketch (on a plane or a model face), edit_sketch, close_sketch, list_sketches, list_sketch_segments, get_sketch_status.

Geometry: draw_line, draw_centerline, draw_circle, draw_rectangle, draw_arc, draw_3point_arc, draw_ellipse, draw_polygon, draw_slot, draw_point, draw_spline.

Editing: sketch_fillet, sketch_chamfer, sketch_trim, sketch_offset, sketch_mirror, convert_entities, set_construction_geometry.

Parametrics: add_relation, add_dimension, set_dimension, list_dimensions.

Features

boss_extrude, cut_extrude, revolve, fillet, chamfer, shell, draft, rib, simple_hole, sweep, loft, linear_pattern, circular_pattern, mirror_feature, delete_feature, rename_feature, set_feature_suppression.

Inspection — the feedback channel

Assemblies

list_components, insert_component, add_mate, list_mates, set_component_fixed.

Engineering drawings

create_drawing, list_sheets, add_sheet, activate_sheet, insert_standard_views, insert_model_view, insert_projected_view, insert_section_view, insert_detail_view, list_drawing_views, activate_drawing_view, create_drawing_sketch, set_drawing_view, insert_model_annotations, auto_dimension_view, insert_center_marks, insert_centerlines, add_note.

For section and detail views, call create_drawing_sketch after activating the parent view, then use the normal draw_line or draw_circle sketch tools.

A worked example

create_new_document   { "kind": "part" }
create_sketch         { "plane": "front", "name": "Base" }
draw_rectangle        { "x1_mm": 10, "y1_mm": 10, "x2_mm": 70, "y2_mm": 50 }
add_dimension         { "selection": { "sketch_segments": [0] }, "kind": "horizontal",
                        "value_mm": 80, "place_x_mm": 40, "place_y_mm": -10 }
add_dimension         { "selection": { "sketch_segments": [1] }, "kind": "vertical",
                        "value_mm": 50, "place_x_mm": -10, "place_y_mm": 30 }
close_sketch          {}
boss_extrude          { "depth_mm": 20, "name": "BasePad" }

list_edges            { "curve_type": "line", "min_length_mm": 19 }   // find the four verticals
fillet                { "radius_mm": 5, "selection": { "edges": [0, 1, 2, 3] } }
shell                 { "thickness_mm": 2, "selection": { "faces": [4] } }

capture_screenshot    { "view": "isometric" }
get_mass_properties   {}

Notes from the implementation

These are the things that cost real time. They are documented because anyone automating SOLIDWORKS from Python will hit them.

SOLIDWORKS members are inconsistently exposed to pywin32. Most are declared in the type library as PROPGET with arguments. Late-bound pywin32 may resolve such a member on plain attribute access by invoking it with no arguments. IBody2.GetFaces then returns a bound method that looks like a one-element result — which is why an extruded box reported exactly one face. Worse, ModelDocExtension.AddDimension invoked that way crashes SOLIDWORKS outright. sw_core.flag_methods() calls _FlagAsMethod on every member the server invokes with arguments, and sw_core.value() invokes zero-argument callables rather than returning the method object.

Modal dialogs deadlock the server. AddDimension2 pops the "Modify" box whenever Input dimension value is enabled — which is the default. A modal dialog blocks the COM call that opened it, and with it the whole server, until somebody clicks. Dimension tools turn the preference off and restore it after. If a tool ever hangs, look for a dialog behind the SOLIDWORKS window.

Return values lie. SketchTrim returns False on success. The Create* sketch APIs return arrays whose truthiness is unreliable. SketchAddConstraints takes a magic string and silently ignores one it does not recognise. So the drawing tools judge success by the sketch's segment count, sketch_trim by whether the sketch actually changed, and add_relation uses the typed ISketchRelationManager.AddRelation and verifies via the relation count — and on failure reports which relations that selection would accept.

Most failures are silent. SOLIDWORKS returns null far more often than it raises. Every feature tool therefore rebuilds and reports ModelDocExtension.GetWhatsWrong, and check_errors exposes it directly.

sketch_trim needs its target selected. Pass the segment in selection; the point alone only tells SOLIDWORKS which piece to discard.

Multi-reference features want distinct marks. InsertRefPlane reads its first, second, and third reference from marks 0, 1, 2 — not from selection order. Selecting all of them with mark 0 silently produces nothing, which is why create_plane selects each reference with its own mark and documents that references are consumed in written order.

Two unit traps. IPartDoc.GetPartBox(False) returns document units, not metres, so it reads 1000x large if you treat it like the rest of the API; pass True. And swSketchLINE is 0, so folding a segment type through or turns every line into "unknown".

Known limitations

• One SOLIDWORKS session, one COM apartment: tool calls are serialised. Two clients driving the same session at once will deadlock it.

• Snapshot indices from list_faces / list_edges are invalidated by any geometry change. Re-list; do not cache.

• A modal dialog opened by SOLIDWORKS for any other reason will still block the server until dismissed.

• rib is picky about its profile. InsertRib returns void and simply builds nothing unless the open profile reaches material at both ends and the extrusion direction can get there. The tool defaults to parallel_to_sketch (right for a cross-section profile) and retries the other direction automatically, reporting which one worked. A profile that overlaps an existing rib still fails, and the tool says so rather than pretending.

• Only the first insert_projected_view off a given parent succeeds; subsequent projections from the same parent return nothing, through re-activation and rebuild alike. Use insert_standard_views for a full orthographic set.

• Detail-view scale is absolute (model to paper), not relative to the parent. On a 1:4 sheet, 2:1 makes the detail eight times the parent view and it overflows the sheet. Pick a scale near the sheet scale.

• Standard-plane and model-view display names are localized. Use front, top, and right for reference planes, and use names returned by list_drawing_views for drawing views; do not hard-code English UI labels.

• through_all_both is translated internally to a two-direction feature with through_all in both directions. Passing swEndCondThroughAllBoth as a single-ended feature silently cuts only one side in SOLIDWORKS 2026.

• circular_pattern cannot pattern a feature that built a separate body (merge: false) — SOLIDWORKS rejects the feature scope. Merge the body, or pattern the body instead.

• save_document cannot overwrite a file SOLIDWORKS currently has open, even with overwrite: true. The error says so when that is the cause.

Testing

The useful tests are live SOLIDWORKS tests: the COM behaviour that matters here cannot be mocked faithfully. With SOLIDWORKS already running, run:

.\.venv\Scripts\python.exe tests\live_p0_regression.py

It verifies the P0 geometry/constraint regressions, including the full-volume through_all_both cut.

Every tool has been exercised against SOLIDWORKS 2026 SP3.2 on a Simplified Chinese install. Where a result could be checked numerically it was: the revolved ring, swept rod and lofted cone match their closed-form volumes; a 5-degree draft removes exactly the expected wedge; rib produces exactly the triangle under its profile; through_all_both removes the full cylinder rather than half of it. The limitations above are what survived that pass.

Layout

tools/tlb_probe.py is worth knowing about before you add a tool. The published API reference disagrees with the shipped type library often enough to matter — FeatureFillet3 takes 14 arguments here, not the documented 7 — so check first:

python tools/tlb_probe.py methods '^IFeatureManager$' '^FeatureFillet3$'
python tools/tlb_probe.py enums '^swMateType_e$'

Adding a tool means writing one decorated function; the registry does the rest.

@tool("my_tool", "What it does. Lengths are millimetres.",
      {"depth_mm": {"type": "number"}}, ["depth_mm"])
def my_tool(args: dict[str, Any]) -> dict[str, Any]:
    _, doc = require_part()
    ...
    return result(True, "Did the thing.")

License

Apache License 2.0 — see LICENSE. Copyright 2026 JIALE LIU.

Use it, change it, ship it in a commercial product; that is all allowed. What the license does require, if you redistribute this or anything derived from it, is that you keep the copyright notices, pass on a copy of the NOTICE file, and state which files you changed.