SW_MCP

Origin. SW_MCP continues solidworks-mcp by JIALE LIU (Apache License 2.0), forked at commit 6019ce0 of 2026-08-16 after upstream went quiet. On top of it: fallbacks to earlier COM method variants for older SOLIDWORKS releases (verified on 2016 SP3), sketch tooling (fully_define_sketch, entities without inferencing, origin selections, diameter dimensions, rectangles and slots from lines and arcs), list_open_documents, close_document, silent save and export, and fixes found while driving the server from an automated build pipeline. The Python package and the console script keep the names solidworks_mcp and solidworks-mcp, so existing configurations keep working. The compatibility part was offered upstream as PR #2.

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.

116 tools: sketching with real relations and driving dimensions, the solid features you actually reach for, sheet metal with its flat pattern and DXF export, weldments from 3D sketches, 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 3.12

Related MCP server: solidworks-mcp

Install

git clone https://github.com/d-veloping/SW_MCP.git solidworks-mcp
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/d-veloping/SW_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.

Sheet metal

Every feature-creating tool here is judged by geometry, never by the API's return value: it reports the body volume and bounding box after the feature, because several of the sheet metal API calls raise on return even when they have built the feature, and others return nothing at all when they have not. What a tool asked for is held against the feature's own readback (thickness, bend radius, hem length, corner type and gap, ...), a feature that removes material must have removed some, and a mismatch is ok: false with the feature still in the tree under its reported name, so the caller can inspect it or hand it to delete_feature. Only the leftovers of a call that built nothing are removed again: a 3D sketch whose lines did not all appear, the profile sketches of a failed edge flange, a Weldment feature added for a member that was refused. The boxes of the sheet metal, weldment and list_bodies results come from IBody2::GetExtremePoint (six calls per body, exact on the geometry; for a rotated assembly component list_bodies transforms the two corners, which is exact only without rotation); get_bounding_box keeps GetPartBox, which SOLIDWORKS documents as approximate, so it is for orientation, not for a check, unless it is called with exact: true, which takes the extreme points of every solid body, hidden ones included. sheet_metal_flatten and export_flat_pattern take single-body sheet metal parts only.

Weldments

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, delete_drawing_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, list_drawing_dimensions, hide_drawing_dimensions, arrange_drawing_dimensions.

insert_standard_views, insert_model_view, insert_projected_view and set_drawing_view take display_mode: hidden_lines_removed (SOLIDWORKS' default), hidden_lines_visible (hidden edges dashed, so bores and steps show without a section), wireframe, shaded, shaded_with_edges. The style counts as applied only when it reads back from the view; otherwise the tool returns ok: false with the style each view ended up in. insert_standard_views applies it only to the views it places. A scale on insert_model_view or set_drawing_view counts the same way: it must read back from the view.

Every drawing tool (sw_drawing, all but create_drawing) takes an optional document (the drawing's title). When another document is active, the call is refused with ok: false and active_document, and nothing is changed; the check runs in the same call. A read SOLIDWORKS refuses where the answer proves something (the view chain, cutting lines, the dimension walk) fails the call instead of counting as "none there". A dimension whose model dimension cannot be read is listed with readable: false; one whose visibility or drawing layer cannot be read with visible: null: it may be hidden, counts for no duplicate, and arrange_drawing_dimensions arranges no view that has one.

insert_section_view takes the cutting line as two sheet points or as a model point it passes through (through_model_mm) plus direction, and draws it in the parent view's own sketch, whose coordinates are (sheet - view position) / view scale, not sheet millimetres. Drawn at sheet coordinates the line lies beside the part and SOLIDWORKS still creates a "section view" that cuts nothing (issue #2). The tool succeeds only when the new view is a section with hatched faces; otherwise it deletes the view and its cutting line again and returns ok: false. When SOLIDWORKS returns no view at all, the call fails and the line it drew may remain in the parent (parent_section_lines is read back). The parent must not be rotated; an unreadable position, scale or angle fails the call. delete_drawing_view removes a section view together with its cutting line, which SOLIDWORKS otherwise leaves in the parent. Deletions are read back: DeleteSelection2 also answers true for what stays, so removed and line_removed say what is gone from the drawing afterwards. insert_detail_view converts its circle the same way. list_drawing_views reports each view's outline, hatched faces, section lines and the transform from model to sheet millimetres.

insert_model_annotations puts the same model dimension into several views, also with duplicate_dimensions: false and also when called view by view (measured on 2016 SP3: 3 to 41 duplicates per part). list_drawing_dimensions lists every visible dimension of every sheet (not those hidden or on a hidden layer) with its sheet, view, layer, model dimension and text position and names the duplicates within a sheet. The value key follows the model dimension's kind: value_mm for a length, value_deg for an angle, value for an integer such as a pattern count. hide_drawing_dimensions hides a list of them in one selection and one call (the part stays unchanged), and arrange_drawing_dimensions auto-arranges one view's dimensions, all or none, and reports how many texts moved. Both activate the view's sheet for that and the previous sheet again afterwards. A section label already used on the sheet is refused. A dimension is selected by its selection name: IAnnotation.Select3 does not select drawing dimensions.

For hand-made section and detail views, call create_drawing_sketch after activating the parent view, then use the normal draw_line or draw_circle sketch tools; their coordinates are the view sketch's, as above.

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.

A sketch that cannot solve is not an error to SOLIDWORKS. SetSystemValue3 stores a dimension value the solver then rejects: the sketch is left no_solution, nothing moves, the rebuild returns true and GetWhatsWrong is empty. So set_dimension reads the value back after the rebuild (it reverts to the old one) and reads the owning sketch's GetConstrainedStatus, which works on a closed sketch, and fails on either signal. add_dimension does the same for a new dimension in the open sketch: it fails when a requested value does not read back, when the sketch is left (or already was) unsolved, and when the sketch's state cannot be read (verified: false). A new dimension that would over-define the sketch, a duplicate say, is not refused either: SOLIDWORKS creates it driven, a reference dimension, and the sketch still solves. So add_dimension also reads the new dimension's DrivenState and fails on driven: true, and on a state it cannot read (driven: null, verified: false). The new dimension stays in the sketch in every case, named by full_name. check_errors reads the same state for every sketch when asked with sketches: true; that is one pass over the feature tree, so it is off by default. Measured on 2016 SP3.

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.

• The sheet metal tools work on single-body sheet metal parts. A multibody sheet metal part has one Flat-Pattern feature per body; sheet_metal_flatten and export_flat_pattern refuse such a part instead of reporting one body as the whole.

• 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.

• A .sldlfp holds only the features selected when it is saved; saved with nothing selected it carries no profile, and a structural member with it fails (measured on 2024 SP3). save_document therefore selects every 2D sketch of the part before it saves a .sldlfp.

• Sheet metal (measured on 2016 SP3): the K-factor cannot be changed through the API — ISheetMetalFeatureData and ICustomBendAllowance accept the value and keep the document default — so sheet_metal_info reports what the flat pattern actually uses. tear_drop and double hems are not accepted. With the profile this tool draws, InsertSheetMetalEdgeFlange2 builds the same flange whatever dimension type it is given: the outer virtual sharp reads back length + t·tan(angle/2) for the same geometry, and the bend tangent builds nothing; so sheet_metal_edge_flange offers no length reference and measures from the inner virtual sharp. Options that the feature definitions do not read back on 2016 (all measured 2026-10-08), which are therefore passed and left to the geometry: flip and relief_type of the edge flange, trim_side_bends of the miter flange, depth_mm of the base flange, position of the hem, every parameter of the corner relief (its feature has no definition at all), gap_mm and coped_cut of the trim, thickness_direction and location of the gusset. The end cap's reverse flag is not offered: it reads back as set and moves nothing. export_flat_pattern needs a saved part, because ExportToDWG2 takes the model path; ExportFlatPatternView is not used because it opens a file dialog. A gauge table is refused on this install's templates (SetUseGaugeTable answers "not enabled on template"), and the 2016 material database carries no sheet metal parameters, so neither route sets the K-factor either.

• Weldments: weldment_trim_extend against a body shortens the trimmed member and grows the trimming member by the same amount, whatever the API's extension option bits say (measured with every combination on 2016), so the part's get_mass_properties does not move and the tool offers no extension switch; list_bodies and the weldment tools report each body's own volume for that reason (the part total is the plain sum of its bodies, overlaps included: two 20 x 20 x 10 boxes overlapping by half report 8000 mm³). The gusset's weld-bead chamfer and sketch-plane offset arguments of InsertGussetFeature3 are accepted and change nothing on 2016, so weldment_gusset does not offer them.

Testing

The useful tests are live SOLIDWORKS tests: the COM behaviour that matters here cannot be mocked faithfully. tools\check.ps1 is the one way to run the check: the server import and the offline tests as in CI, then the live checks one after another, with SOLIDWORKS already running. It stops at the first red step and exits non-zero, so chain the commit on it:

# Windows PowerShell 5.1 (no &&)
powershell -NoProfile -ExecutionPolicy Bypass -File tools\check.ps1; if ($LASTEXITCODE -eq 0) { git commit }

Start it as its own powershell process, as above, rather than as .\tools\check.ps1: a script the execution policy blocks leaves $LASTEXITCODE at its previous value, which may well be 0.

# cmd, Bash, PowerShell 7
powershell -NoProfile -ExecutionPolicy Bypass -File tools/check.ps1 && git commit

The forward slash is deliberate: Bash would swallow the backslash of tools\check.ps1.

Never pipe the check into another command (... | tail): the exit code that counts is then the last command's, and a red live test no longer stops the commit (in Bash only set -o pipefail changes that). -Offline skips the live checks on a machine without SOLIDWORKS, -Python names another interpreter (for a worktree without its own .venv), -SelfTest checks the exit codes of the check itself without SOLIDWORKS. Every tests\live_*.py is either run by the check or listed in it with the reason it is not (measurements that always exit 0, checks that need a saved part as argument); an unlisted one fails the check. If other processes drive the same SOLIDWORKS, run the live part only while you hold their lock.

tests\live_p0_regression.py verifies the P0 geometry/constraint regressions, including the full-volume through_all_both cut. tests\live_sheet_metal.py builds an L profile and a plate with every sheet metal tool and checks the flanges, the flat pattern and the break corner against a closed-form number: flange volumes, the developed length from the K-factor, the material a break corner removes, the bend lines in the exported DXF; the hem, the closed corner and the corner relief are checked by readback, added or removed material and the DXF (32 checks on 2016 SP3, plus 11 for the third part). tests\live_weldment.py does the same for weldments: members measure profile area times length and reach the mitred outer corner, the end cap its inset plate, the trimmed member its new length, the gussets abt/2 with their leg lengths and the polygon with its corner cut, a plane cut into two halves, and a degenerate 3D line leaves no sketch behind; a second pair with butt corners, a turned and mirrored profile and a gap, and end caps with ratio inset and chamfer (volume), and inset by distance and inward (the plate ends flush inside, the recut member is reported), are checked by readback and geometry (41 checks). A third sheet metal part checks an edge flange and a miter flange with every option off its default by readback and reach.

Every tool except the 16 sheet metal and weldment tools and activate_document 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.

Older releases work too, back to at least SOLIDWORKS 2016 SP3, where every tool was exercised the same way on a German install. Where a release lacks the newest numbered method (FeatureCut4, FeatureLinearPattern5, CreateDetailViewAt4, ...) the tool falls back to the earlier variant with the arguments it takes; on newer releases the newest name is always tried first, so nothing changes there. The sheet metal and weldment tools are the exception in both directions: they were measured on 2016 SP3 only (tests\live_sheet_metal.py, tests\live_weldment.py), have not been run against 2026, and call the API names that build on 2016 (InsertSheetMetalBaseFlange, InsertSheetMetalHem, InsertStructuralWeldment4, InsertEndCapFeature3, ...) without a newest-name-first fallback.

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; modifications Copyright 2026 Christian Dengler (d-veloping), see NOTICE.

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.