kalpataru-sketch-workflow

name	kalpataru-sketch-workflow
description	How to author a fully-defined SolidWorks sketch via Kalpataru. Geometric entity types, constraints, dimensions, and degree-of-freedom (DOF) tactics.

Sketch workflow

A sketch is "fully defined" when DOF (degrees of freedom) = 0. Until then, SolidWorks will let you extrude it but the resulting feature is fragile — any later parametric change can warp it.

Geometric entity types

kalpataru_create_sketch accepts a list of entity dicts. Each has a type:

Type	Fields	Notes
line	start, end	A straight line. Auto-applies horizontal/vertical constraint if axis-aligned.
construction_line	start, end	A reference line — not part of the boundary.
circle	center, diameter
arc	center, radius, start_angle, end_angle	Angles in degrees.
arc_3point	start, end, point3	Better when you have three known points.
rectangle	center, width, height	Centered rectangle. Most common form.
corner_rectangle	corner1, corner2	Two-corner form.
polygon	center, diameter, sides	Regular polygon (hex, octagon, etc.).
slot	center1, center2, width	Straight slot.
ellipse	center, major_radius, minor_radius, rotation	Rotation in degrees.
spline	points (list of [x,y]), closed	Through-point spline.
polyline	points, closed	Connected line segments.
point	position	Construction point.

All coordinates are 2D [x, y] in millimetres, in the sketch's local coordinate system.

The DOF rule

Every sketch entity adds DOF; every constraint and dimension removes some.

• A line has 4 DOF (x1, y1, x2, y2). A coincident point removes 2. A horizontal/vertical constraint removes 1. A dimension removes 1.
• A circle has 3 DOF (cx, cy, r). Coincident-to-origin: 2. Diameter: 1.
• A rectangle has 4 DOF after auto-constraints (h/v on the sides). Coincident center to origin: 2. Width and height: 2. → fully defined.

If you create a rectangle without anchoring it to the origin and without dimensioning the size, DOF = 4. Anchor first (coincident to origin or a known point), then dimension.

Constraint shorthand

The C# bridge auto-applies these constraints when it can:

• Lines parallel to X-axis → horizontal
• Lines parallel to Y-axis → vertical
• Two lines sharing an endpoint within 0.001mm → coincident
• Two circles with the same center within 0.001mm → concentric
• Symmetric pattern about origin → symmetric

So if you start your rectangle exactly at (−25, −25) and (25, 25), you get horizontal/vertical/coincident-to-origin for free. The dimensions (width: 50, height: 50) finish the constraint.

Inspecting sketch state

kalpataru_create_sketch returns:

• sketch_name — for the next feature call
• dof — should be 0 before extruding
• profile_closed — true for closed boundaries (rectangles, polygons, the four-line outline of a closed shape)
• entities — [{name, type}], gives you names like Line1, Arc2 for later constraint/dimension references
• constraint_status — "fully_defined" / "under_defined" / "over_defined"

If dof > 0, add more constraints. If over_defined, you have conflicting constraints — undo and remove one.

Common patterns

Rectangle centered on origin, 50x50:

entities: [{"type":"rectangle","center":[0,0],"width":50,"height":50}]

Circle concentric to origin, Ø10:

entities: [{"type":"circle","center":[0,0],"diameter":10}]

Polygon, 6 sides, inscribed Ø20:

entities: [{"type":"polygon","center":[0,0],"diameter":20,"sides":6}]

Slot, 30mm long, 10mm wide:

entities: [{"type":"slot","center1":[-10,0],"center2":[10,0],"width":10}]

Closing the loop

For an extrude to work, the sketch boundary must be CLOSED. A rectangle is inherently closed. Four separate lines forming a rectangle ARE closed if the endpoints are coincident (within 0.001mm). The SDK's auto-coincident will normally catch this — but if profile_closed: false is returned, inspect the entities and verify the endpoints meet.