Modeling Tools¶

Create and manipulate SolidWorks parts, assemblies, and drawings. These are the foundational tools for any CAD workflow — opening files, creating features (extrude, revolve), and querying/setting driven dimensions.

Prerequisite: An active SolidWorks session. Most feature tools require an open Part document.

Total tools in this category: 12

Measured change¶

create_extrusion, create_revolve and create_cut_extrude report what the feature actually did. Their success reply carries a measured_change block with volume_before_mm3, volume_after_mm3 and volume_delta_mm3; the bounding-box size before and after; and the solid-body count before and after. If the feature reports success but the volume did not change, the reply also has a warning: that is how SolidWorks shows a feature it accepted without doing anything. Measuring never fails the feature; any value that can't be read is null with a note. Finish a build with verify_model (see Analysis tools).

Which way a cut goes. A one-way create_cut_extrude (Blind or ThroughAll) goes along the sketch plane's normal. From a sketch on a face, or on a plane that touches the body on one side only (a Top Plane sketch under a block extruded up from it), that direction can point away from the material. The tool then cuts the other way and its reply has cut_extrude.direction_flipped: true, so there's no need to guess reverse_direction. For a sketch on a plane through the middle of a body, use ThroughAllBoth (or ThroughAll with both_directions: true) to cut both sides. If neither direction removes material, the error is feature_not_built: change the sketch, its plane or the depth rather than retrying the same call.

`open_model`¶

Open a part, assembly or drawing from disk and make it the active document.

Prerequisite: SolidWorks running

Parameters:

Parameter	Type	Required	Default	Description
`file_path`	`str`	✅	``	Full path to the SolidWorks file (.sldprt, .sldasm, .slddrw)

Sample call:

{
  "file_path": "C:\\Temp\\mcp_demo\\part.sldprt"
}

`create_part`¶

Create a new, empty part document and make it active, ready for create_sketch.

Prerequisite: SolidWorks running

Parameters:

Parameter	Type	Required	Default	Description
`name`	`str`	✅	``	Name for the new part
`template`	`str?`	—	`None`	Template file path for the new part
`units`	`str?`	—	`None`	Document units
`material`	`str?`	—	`None`	Material name

Sample call:

{
  "name": "MCP_Demo_Part"
}

`create_assembly`¶

Create a new, empty assembly document and make it active, ready for insert_component.

Prerequisite: SolidWorks running

Parameters:

Parameter	Type	Required	Default	Description
`name`	`str`	✅	``	Name for the new assembly
`template`	`str?`	—	`None`	Assembly template file path
`components`	`List[str]`	✅	``	Component list

Sample call:

{
  "name": "MCP_Demo_Part",
  "components": []
}

`create_drawing`¶

Create a new, empty drawing document and make it active.

Prerequisite: SolidWorks running

Parameters:

Parameter	Type	Required	Default	Description
`name`	`str`	✅	``	Name for the new drawing
`template`	`str?`	—	`None`	Drawing template file path
`model_path`	`str?`	—	`None`	Source model path
`sheet_format`	`str?`	—	`None`	Sheet format template

Sample call:

{
  "name": "MCP_Demo_Part"
}

`close_model`¶

Close the active document, saving it first only if asked.

Prerequisite: An active open document

Parameters:

Parameter	Type	Required	Default	Description
`save`	`bool`	—	`False`	Save the model before closing

Sample call:

{}

`create_extrusion`¶

Extrude the sketch you just closed into a solid boss, added to the active part.

Prerequisite: Active part with an active sketch (exit sketch first with exit_sketch)

Parameters:

Parameter	Type	Required	Default	Description
`sketch_name`	`str`	✅	``	Sketch name to extrude
`depth`	`float`	✅	``	Extrusion depth in millimeters
`direction`	`str`	—	`blind`	Extrusion direction
`reverse`	`bool?`	—	`None`	Reverse direction alias
`draft_angle`	`float`	—	`0.0`	Draft angle in degrees
`reverse_direction`	`bool`	—	`False`	Reverse extrusion direction
`both_directions`	`bool`	—	`False`	Extrude in both directions
`thin_feature`	`bool`	—	`False`	Create as thin wall feature
`thin_thickness`	`float?`	—	`None`	Thickness for thin wall feature in mm
`end_condition`	`str`	—	`Blind`	End condition type
`merge_result`	`bool`	—	`True`	Merge with existing geometry

Sample call:

{
  "sketch_name": "Sketch1",
  "depth": 25.0
}

`create_revolve`¶

Revolve the sketch you just closed around the centreline drawn in it, adding a solid to the active part.

Prerequisite: Active part with an active sketch containing the profile and axis

Parameters:

Parameter	Type	Required	Default	Description
`sketch_name`	`str`	✅	``	Sketch name to revolve
`axis_entity`	`str`	✅	``	Axis entity for the revolve
`angle`	`float`	✅	``	Revolve angle in degrees
`direction`	`str`	—	`one_direction`	Revolve direction
`reverse_direction`	`bool`	—	`False`	Reverse revolve direction
`both_directions`	`bool`	—	`False`	Revolve in both directions
`thin_feature`	`bool`	—	`False`	Create as thin wall feature
`thin_thickness`	`float?`	—	`None`	Thickness for thin wall feature in mm
`merge_result`	`bool`	—	`True`	Merge with existing geometry

Sample call:

{
  "sketch_name": "Sketch1",
  "axis_entity": "Line1",
  "angle": 360.0
}

`get_dimension`¶

Read one dimension of the active model by its full name, e.g. "D1@Sketch1".

Prerequisite: Active document with named dimensions

Parameters:

Parameter	Type	Required	Default	Description
`name`	`str?`	—	`None`	Dimension name (e.g., 'D1@Sketch1', 'D1@Boss-Extrude1')
`dimension_name`	`str?`	—	`None`	Dimension name alias

Sample call:

{}

`set_dimension`¶

Change one length dimension of the active model, in mm, and rebuild.

Prerequisite: Active document with named dimensions

Parameters:

Parameter	Type	Required	Default	Description
`name`	`str?`	—	`None`	Dimension name (e.g., 'D1@Sketch1', 'D1@Boss-Extrude1')
`dimension_name`	`str?`	—	`None`	Dimension name alias
`value`	`float`	✅	``	New dimension value in millimeters
`units`	`str?`	—	`None`	Units alias

Sample call:

{
  "value": 50.0
}

`set_units`¶

Set the active document's length units: mm, cm, m, in or ft.

Prerequisite: Active document

Parameters:

Parameter	Type	Required	Default	Description
`unit_system`	`str`	✅	``	Linear unit system: mm, cm, m, in, or ft

Sample call:

{
  "unit_system": "in"
}

`rename_feature`¶

Rename a feature in the active model's feature tree.

Prerequisite: Active document containing the named feature

Parameters:

Parameter	Type	Required	Default	Description
`old_name`	`str`	✅	``	Current feature name, e.g. 'Fillet1'
`new_name`	`str`	✅	``	New feature name, e.g. 'MountingEdgeFillet'

Sample call:

{
  "old_name": "Fillet1",
  "new_name": "EdgeBreak"
}

`select_feature`¶

Select a feature, sketch, plane or component by name in the active document.

Prerequisite: Active document containing the named entity

Parameters:

Parameter	Type	Required	Default	Description
`feature_name`	`str`	✅	``	Feature, sketch, plane or component name, e.g. 'Boss-Extrude1', 'Sketch1', 'Front Plane' (an '@Part1' suffix is ok)
`append`	`bool`	❌	`false`	Add to the current selection instead of replacing it

Sample call:

{
  "feature_name": "Boss-Extrude1"
}

`select_face_edges`¶

Select every edge of one face of the active part, ready for add_fillet or add_chamfer with no edge names.

The edges become the live selection, so a following add_chamfer / add_fillet with an empty edge_names acts on exactly them. Anything that changes the selection in between — including a click in SolidWorks — changes what is used. The response reports the face chosen (data.face: centre, normal, area) and each edge (data.edges: curve type, endpoints/length or centre/radius), so you can switch to point if side picked a different face than intended.

Prerequisite: Active part document

Parameters:

Parameter	Type	Required	Default	Description
`point`	`list[float]`	❌	`null`	A point on the face, `[x, y, z]` in mm
`side`	`str`	❌	`null`	`+X`/`-X`/`+Y`/`-Y`/`+Z`/`-Z` or `right`/`left`/`top`/`bottom`/`front`/`back`
`plane`	`str`	❌	`null`	Reference plane name, e.g. 'Front Plane'
`edge_type`	`str`	❌	`all`	`all`, `linear` or `circular`
`append`	`bool`	❌	`false`	Add to the current selection instead of replacing it

Sample call (then chamfer the selected hole rims with add_chamfer({"distance": 0.5, "edge_names": []})):

{
  "side": "top",
  "edge_type": "circular"
}

`rebuild_model`¶

Rebuild the active model and report each feature that fails, with the reason and a fix.

Prerequisite: Active document

Parameters:

Parameter	Type	Required	Default	Description
`top_level_only`	`bool`	❌	`false`	Rebuild only the top level of an assembly

Sample call:

{}

Sample error response (abridged):

{
  "status": "error",
  "message": "Rebuild left 1 feature error(s): Boss-Extrude2. See data.errors for each cause and hint.",
  "data": {
    "error_count": 1,
    "errors": [
      {
        "feature": "Boss-Extrude2",
        "type": "Extrusion",
        "code": 1,
        "code_name": "swFeatureErrorUnknown",
        "severity": "error",
        "parents": [{"name": "Sketch2", "type": "ProfileFeature", "segment_count": 0}],
        "hint": "Parent sketch 'Sketch2' has no geometry. Add a closed profile to it (or delete this feature)."
      }
    ]
  }
}

`create_reference_point`¶

Add a reference point on an edge (at a distance or percentage along it) or at the centre of a face.

Prerequisite: Active part with the target edge/face

Parameters:

Parameter	Type	Required	Default	Description
`mode`	`str`	✅	``	`along_curve` or `face_center`
`x`	`float`	✅	``	X of a point on the target edge/face, in mm
`y`	`float`	✅	``	Y of a point on the target edge/face, in mm
`z`	`float`	✅	``	Z of a point on the target edge/face, in mm
`distance`	`float?`	—	`None`	along_curve only: offset from the edge start in mm
`percent`	`float?`	—	`None`	along_curve only: 0–100 of the edge length

Sample call:

{
  "mode": "along_curve",
  "x": 25, "y": 0, "z": 10,
  "percent": 50
}

Modeling Tools¶

Measured change¶

open_model¶

create_part¶

create_assembly¶

create_drawing¶

close_model¶

create_extrusion¶

create_revolve¶

get_dimension¶

set_dimension¶

set_units¶

rename_feature¶

select_feature¶

select_face_edges¶

rebuild_model¶

create_reference_point¶

`open_model`¶

`create_part`¶

`create_assembly`¶

`create_drawing`¶

`close_model`¶

`create_extrusion`¶

`create_revolve`¶

`get_dimension`¶

`set_dimension`¶

`set_units`¶

`rename_feature`¶

`select_feature`¶

`select_face_edges`¶

`rebuild_model`¶

`create_reference_point`¶