Sketching Tools¶

Build 2-D sketch geometry (lines, circles, arcs, splines, polygons) and apply geometric constraints and driven dimensions. Sketches are the prerequisite for every extrusion, revolve, sweep, and loft feature.

Prerequisite: An active part document with an active sketch edit session.

Total tools in this category: 18

`create_sketch`¶

Create a new sketch on the specified plane.

Prerequisite: Active part document, no active sketch

Parameters:

Parameter	Type	Required	Default	Description
`plane`	`str`	✅	``	Sketch plane name (e.g., 'Top', 'Front', 'Right', 'XY', 'XZ', 'YZ')
`sketch_name`	`str?`	—	`None`	Sketch name alias

Sample call:

{
  "plane": "Front"
}

`add_line`¶

Add a line to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`x1`	`float?`	—	`None`	Start point X coordinate in mm
`y1`	`float?`	—	`None`	Start point Y coordinate in mm
`x2`	`float?`	—	`None`	End point X coordinate in mm
`y2`	`float?`	—	`None`	End point Y coordinate in mm
`start_x`	`float?`	—	`None`	Start point X alias
`start_y`	`float?`	—	`None`	Start point Y alias
`end_x`	`float?`	—	`None`	End point X alias
`end_y`	`float?`	—	`None`	End point Y alias
`construction`	`bool`	—	`False`	Construction geometry flag

Sample call:

{}

`add_circle`¶

Add a circle to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`center_x`	`float`	✅	``	Circle center X coordinate in mm
`center_y`	`float`	✅	``	Circle center Y coordinate in mm
`radius`	`float`	✅	``	Circle radius in mm
`construction`	`bool`	—	`False`	Construction geometry flag

Sample call:

{
  "center_x": 0.0,
  "center_y": 0.0,
  "radius": 15.0
}

`add_rectangle`¶

Add a rectangle to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`x1`	`float?`	—	`None`	First corner X coordinate in mm
`y1`	`float?`	—	`None`	First corner Y coordinate in mm
`x2`	`float?`	—	`None`	Opposite corner X coordinate in mm
`y2`	`float?`	—	`None`	Opposite corner Y coordinate in mm
`corner1_x`	`float?`	—	`None`	Corner 1 X alias
`corner1_y`	`float?`	—	`None`	Corner 1 Y alias
`corner2_x`	`float?`	—	`None`	Corner 2 X alias
`corner2_y`	`float?`	—	`None`	Corner 2 Y alias
`construction`	`bool`	—	`False`	Construction geometry flag

Sample call:

{}

`exit_sketch`¶

Exit sketch editing mode.

Prerequisite: Active sketch edit mode

Sample call:

{}

`add_arc`¶

Add an arc to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`center_x`	`float`	✅	``	Arc center X coordinate in mm
`center_y`	`float`	✅	``	Arc center Y coordinate in mm
`start_x`	`float`	✅	``	Arc start point X coordinate in mm
`start_y`	`float`	✅	``	Arc start point Y coordinate in mm
`end_x`	`float`	✅	``	Arc end point X coordinate in mm
`end_y`	`float`	✅	``	Arc end point Y coordinate in mm

Sample call:

{
  "center_x": 0.0,
  "center_y": 0.0,
  "start_x": -30.0,
  "start_y": 0.0,
  "end_x": 30.0,
  "end_y": 0.0
}

`add_spline`¶

Add a spline curve to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`points`	`List[Dict[str, float]]`	✅	``	List of spline control points with x, y coordinates

Sample call:

{
  "points": [
    {
      "x": 0.0,
      "y": 0.0
    },
    {
      "x": 10.0,
      "y": 15.0
    },
    {
      "x": 20.0,
      "y": 10.0
    }
  ]
}

`add_centerline`¶

Add a centerline to the current sketch.

Prerequisite: Active sketch edit mode

Parameters:

Parameter	Type	Required	Default	Description
`x1`	`float?`	—	`None`	Start point X coordinate in mm
`y1`	`float?`	—	`None`	Start point Y coordinate in mm
`x2`	`float?`	—	`None`	End point X coordinate in mm
`y2`	`float?`	—	`None`	End point Y coordinate in mm
`start_x`	`float?`	—	`None`	Start point X alias
`start_y`	`float?`	—	`None`	Start point Y alias
`end_x`	`float?`	—	`None`	End point X alias
`end_y`	`float?`	—	`None`	End point Y alias
`construction`	`bool`	—	`False`	Construction geometry flag

Sample call:

{}

`add_polygon`¶

Add a regular polygon to the current sketch.

Prerequisite: Active sketch edit mode

Sample call:

{}

`add_ellipse`¶

Add an ellipse to the current sketch.

Prerequisite: Active sketch edit mode

Sample call:

{}

`add_sketch_constraint`¶

Add a geometric constraint/relation between sketch entities.

Prerequisite: Active sketch edit mode with named entities

SolidWorks automation note: Implemented via ISketchRelationManager.AddRelation(entities, swConstraintType_e). Entities must be IDs returned from a previous add_line / add_circle / add_arc call (e.g. "Line_1").

Parameters:

Parameter	Type	Required	Default	Description
`entity1`	`str`	✅	``	First entity name or ID
`entity2`	`str?`	—	`None`	Second entity name or ID (for two-entity relations)
`entity3`	`str?`	—	`None`	Third entity name or ID. Required only for `symmetric` (the centerline of symmetry, e.g. `"Centerline_5"`); must be `None` for all other relations
`relation_type`	`str`	✅	``	One of the supported relation names (see below)

Supported relation_type values (case-insensitive):

Name	Entity arity	Notes
`horizontal`	1 or 2	Line(s) horizontal; with 2 endpoints aligns them horizontally
`vertical`	1 or 2	Line(s) vertical; with 2 endpoints aligns them vertically
`parallel`	2	Two lines parallel
`perpendicular`	2	Two lines at 90°
`tangent`	2	Line ↔ arc/circle, or arc ↔ arc
`coincident`	2	Two points (or point on entity) share location
`concentric`	2	Two arcs/circles share center
`equal`	2	Equal length (lines) or equal radius (arcs/circles) — maps to `swConstraintType_SAMELENGTH`
`symmetric`	3	Two entities about a centerline; `entity3` must be the centerline ID returned by `add_centerline`
`collinear`	2	Two lines on the same infinite line
`fix`	1	Pin the entity in place

entity3 is only used by symmetric. All other relation types reject a non-null entity3 with a clear error.

Sample call (two-entity perpendicular):

{
  "entity1": "Line_1",
  "entity2": "Line_2",
  "relation_type": "perpendicular"
}

Sample call (three-entity symmetric):

{
  "entity1": "Line_1",
  "entity2": "Line_2",
  "entity3": "Centerline_5",
  "relation_type": "symmetric"
}

Sample call (single-entity horizontal):

{
  "entity1": "Line_1",
  "relation_type": "horizontal"
}

Response shape on success:

{
  "status": "success",
  "constraint": {
    "id": "Constraint_3",
    "type": "perpendicular",
    "entity1": "Line_1",
    "entity2": "Line_2"
  }
}

`add_sketch_dimension`¶

Add a dimension to sketch entities.

Prerequisite: Active sketch edit mode

SolidWorks automation note: In real SolidWorks sessions, sketch dimension creation can open the interactive Modify approval dialog and block unattended runs. The implementation keeps the sketch-input preferences disabled for the full automation session and uses AddRadialDimension2 or AddDiameterDimension2 for radial and diameter dimensions so these calls stay non-interactive.

Parameters:

Parameter	Type	Required	Default	Description
`entity1`	`str`	✅	``	First entity name or ID
`entity2`	`str?`	—	`None`	Second entity name or ID (for distance dimensions)
`dimension_type`	`str`	—	`linear`	Dimension type (linear, radial, angular, etc.)
`value`	`float`	✅	``	Dimension value in mm or degrees

Sample call:

{
  "entity1": "Line1",
  "value": 50.0
}

Why this is implemented this way:

SolidWorks may treat sketch dimension creation like an interactive Smart Dimension workflow unless the sketch-input preferences are suppressed.
The adapter disables swInputDimValOnCreate, swSketchAcceptNumericInput, swSketchCreateDimensionOnlyWhenEntered, and swScaleSketchOnFirstDimension when automation connects, so the tool does not wait for a manual approve click.
Radial and diameter dimensions use the dedicated IModelDoc2 APIs instead of the generic extension call because that path is more reliable for circles and arcs in live COM sessions.

`sketch_linear_pattern`¶

Create a linear pattern of sketch entities.

Prerequisite: Active sketch edit mode

Sample call:

{}

`sketch_circular_pattern`¶

Create a circular pattern of sketch entities.

Prerequisite: Active sketch edit mode

Sample call:

{}

`sketch_mirror`¶

Mirror sketch entities about a centerline.

Prerequisite: Active sketch edit mode

Sample call:

{}

`sketch_offset`¶

Create an offset of sketch entities.

Prerequisite: Active sketch edit mode

Sample call:

{}

`sketch_tutorial_simple_hole`¶

Tutorial: Create a simple circular hole sketch.

Prerequisite: SolidWorks running

Sample call:

{}

`tutorial_simple_hole`¶

Create a simple hole as a guided tutorial workflow.

Prerequisite: SolidWorks running

Parameters:

Parameter	Type	Required	Default	Description
`plane`	`str`	✅	``	Sketch plane for the hole
`center_x`	`float`	✅	``	Hole center X coordinate in mm
`center_y`	`float`	✅	``	Hole center Y coordinate in mm
`diameter`	`float`	✅	``	Hole diameter in mm
`depth`	`float?`	—	`None`	Hole depth in mm (None for through hole)

Sample call:

{
  "plane": "Front",
  "center_x": 0.0,
  "center_y": 0.0,
  "diameter": 10.0
}

Sketching Tools¶

create_sketch¶

add_line¶

add_circle¶

add_rectangle¶

exit_sketch¶

add_arc¶

add_spline¶

add_centerline¶

add_polygon¶

add_ellipse¶

add_sketch_constraint¶

add_sketch_dimension¶

sketch_linear_pattern¶

sketch_circular_pattern¶

sketch_mirror¶

sketch_offset¶

sketch_tutorial_simple_hole¶

tutorial_simple_hole¶

`create_sketch`¶

`add_line`¶

`add_circle`¶

`add_rectangle`¶

`exit_sketch`¶

`add_arc`¶

`add_spline`¶

`add_centerline`¶

`add_polygon`¶

`add_ellipse`¶

`add_sketch_constraint`¶

`add_sketch_dimension`¶

`sketch_linear_pattern`¶

`sketch_circular_pattern`¶

`sketch_mirror`¶

`sketch_offset`¶

`sketch_tutorial_simple_hole`¶

`tutorial_simple_hole`¶