kalpataru-examples

name	kalpataru-examples
description	Concrete worked recipes for building canonical shapes in SolidWorks via the Kalpataru MCP — cube, cube-with-hole, cylinder, plate, L-bracket, revolved shaft. Use when the user asks for any of these (or anything similar to them) so the model doesn't have to derive the tool sequence from first principles.

Worked recipes

If the user's request maps to one of these shapes — or a small variation of one — follow the exact tool sequence. Don't second-guess the sketch response: when ready_to_extrude is true, proceed to extrude. Don't retry creating the sketch.

Cube (NxNxN)

Default N = 50 mm if the user just says "a cube". Adapt N to whatever size they mention.

1.  kalpataru_ping
       → confirms SolidWorks reachable
2.  kalpataru_new_part
       → returns document_name
3.  kalpataru_create_sketch
       plane = "Front"
       entities = [
           {"type": "rectangle", "center": [0, 0], "width": N, "height": N}
       ]
       → returns sketch_name = "Sketch1", ready_to_extrude = true
4.  kalpataru_extrude
       sketch_name = "Sketch1"
       depth = N
       → cube appears in SolidWorks viewport

Done. Don't add more steps.

Cube with a through-hole (canonical hello-world)

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Front"
       entities = [{"type":"rectangle","center":[0,0],"width":50,"height":50}]
3.  kalpataru_extrude  sketch_name="Sketch1"  depth=25
4.  kalpataru_query_faces  surface="plane"  of_feature="Boss-Extrude1"
       → pick the face with the largest +Z centroid (that's the top face)
5.  kalpataru_create_sketch
       face_id = <top face id, e.g. "F4">
       entities = [{"type":"circle","center":[0,0],"diameter":10}]
6.  kalpataru_cut  sketch_name="Sketch2"  depth_type="through_all"

Result: 7 faces (4 sides + annular top + annular bottom + inner cylinder).

Cylinder (diameter D, height H)

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Top"
       entities = [{"type":"circle","center":[0,0],"diameter":D}]
3.  kalpataru_extrude  sketch_name="Sketch1"  depth=H

Plate / rectangular slab (W x L x T)

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Top"
       entities = [{"type":"rectangle","center":[0,0],"width":W,"height":L}]
3.  kalpataru_extrude  sketch_name="Sketch1"  depth=T

L-bracket (50 mm legs, 5 mm thick, width W)

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Front"
       entities = [{
           "type": "polyline",
           "points": [[0,0],[50,0],[50,5],[5,5],[5,50],[0,50]],
           "closed": true
       }]
3.  kalpataru_extrude
       sketch_name = "Sketch1"
       depth = W
       depth_type = "midplane"

polyline with closed=true auto-coincidents the endpoints. Don't try to draw 6 separate lines — they won't reliably auto-close.

Hex nut M-N (across-flats AF, thickness T)

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Top"
       entities = [
           {"type":"polygon","center":[0,0],"diameter":AF,"sides":6}
       ]
3.  kalpataru_extrude  sketch_name="Sketch1"  depth=T
4.  kalpataru_query_faces  surface="plane"  of_feature="Boss-Extrude1"
       → top face = largest +Y centroid (Top plane extrudes along +Y)
5.  kalpataru_create_sketch
       face_id = <top face id>
       entities = [{"type":"circle","center":[0,0],"diameter":N}]
6.  kalpataru_cut  sketch_name="Sketch2"  depth_type="through_all"

Revolved shaft (any stepped axisymmetric part)

Profile must sit entirely in +X (no point at x≤0) and a horizontal construction line on the X-axis acts as the rotation axis.

1.  kalpataru_new_part
2.  kalpataru_create_sketch
       plane = "Front"
       entities = [
           {"type":"line","start":[r1, 0],   "end":[r1, h1]},
           {"type":"line","start":[r1, h1],  "end":[r2, h1]},
           {"type":"line","start":[r2, h1],  "end":[r2, h2]},
           # ... close back to the construction line
           {"type":"line","start":[r_last, h_last], "end":[r_last, 0]},
           {"type":"line","start":[r_last, 0],      "end":[r1, 0]},
           {"type":"construction_line","start":[-5, 0],"end":[r_last+10, 0]}
       ]
3.  kalpataru_revolve  sketch_name="Sketch1"  angle=360

For a 2-step shaft (flange 20×10 + shaft 10×40), use the worked example in examples/integration/revolved_shaft.py as the literal template.

Rules of thumb

• Closed primitives are always closed. rectangle, circle, polygon, slot, ellipse — the response will say ready_to_extrude: true. Proceed to extrude. The legacy bridge sometimes adds confusing "WARNING: profile NOT closed" text from heartbeat analysis; ignore it for closed primitives.
• One sketch, one feature. Don't create multiple sketches before doing the first extrude unless the recipe explicitly calls for it.
• All coordinates are in millimetres.
• Don't pre-dimension a closed primitive — it's already constrained by its own definition (a rectangle has width/height baked in; a circle has diameter baked in).
• For cuts, prefer depth_type="through_all" unless the user specifies a blind depth — it's the most robust.
• The canonical planes are "Front" (XY), "Top" (XZ), "Right" (YZ). Use Front when you want the extrusion to go along +Z, Top for +Y, Right for +X.