OneCAD/skills/solidcraft-modeling/reference.md

SolidCraft command reference for agents

These are the shapes of the commands a part build needs, so an agent rarely has to call list_commands. The worked example at the end runs in CI (skill_reference_example_builds_as_documented in crates/mcp/src/tests.rs).

• Lengths are in mm.
• Angles inside expressions take units: "30 deg".
• Any numeric field can be an expression that names parameters: "w/2 - wall - 6".

Sketch planes: where sketch (x, y) lands in the world

plane	sketch x	sketch y	normal (+distance)
"XY"	+X	+Y	+Z
"XZ"	+X	-Z	+Y
"YZ"	+Y	+Z	+X
{origin, x_dir, y_dir}	x_dir	y_dir	x_dir x y_dir

• offset: "expr" on sketch.create moves the plane along its normal and follows parameters.
• Front wall (-Y) of a part centred on the origin:
  • Sketch on {"plane":"XZ","offset":"-d/2"}.
  • Draw a feature at height z at sketch y = -z.
  • A cut with a positive distance goes into the wall.
• Top face: sketch on {"plane":"XY","offset":"h"}.
• Hole direction: solid.hole {sketch} drills from the sketch plane along -normal. A hole sketch at z=0 under a part drills into empty space and still reports success, so put the sketch on the top face.

Ids

• Numbering: every creator returns created: {points, curves, constraints, dimensions}. Ids are stable and numbered per sketch.
• Curves: l1, c1, a1.
• Points: p1, l1.start, l1.end, c1.center, a1.center, and the sketch origin "origin".
• Rectangles: sketch.rectangle.* also returns sides {bottom,right,top,left} and corners {bottom_left,...}.
  • rectangle.center adds 2 construction diagonals, so each corner joins 3 lines. Its centre point is p5.
  • sketch.fillet {point} therefore fails on its corners. Use {a:"l1", b:"l4", radius} or the 3D solid.fillet.
• Slots: sketch.slot.overall and sketch.slot.center_to_center create curves l1, a1, l2, a2 and points p1-p4, a1.center, a2.center.
  • The length role of slot.overall is the overall length. The arc centres are at ±(length/2 - width/2).
  • After length and width, 3 dof remain. To remove them, dimension origin to a1.center horizontally and vertically, and origin to a2.center vertically. For a slot along Y the solver refuses that last dimension as over-constraining; dimension a2.center horizontally instead.
  • sketch.slot.center_point creates no centre point. Dimension an arc centre instead.
• Circles: sketch.circle.center creates c1 and c1.center, and no p point.
• Dimensions share the k counter with constraints.
• Constraints can add curves: a constraint about an axis, such as sketch.constraint.symmetry with line:"y", adds a construction line and so takes the next l id. Read created before you count further.
• Over-constraining is refused with that conflicts with the sketch: neither entity can move to satisfy it. For example, symmetry already makes two circles equal.

Dimensions

{"command":"sketch.dimension","params":{"entities":["origin","c1.center"],"type":"horizontal","value":"w/2 - wall - 6"}}
{"command":"sketch.dimension","params":{"entities":["c1"],"type":"diameter","value":"6"}}
{"command":"sketch.dimension","params":{"entities":["l1"],"value":"w"}}

Distances are unsigned. Draw the geometry on the correct side first, and the dimension keeps it there.

sketch.draw.dimensioned creates a shape and its dimensions in one undo step. The dimension roles depend on the creator:

Creator	Roles
line (exactly 2 points)	length, angle
rectangle.*	width, height
circle.*	radius or diameter
arc.center_point	radius, sweep
slot.center_to_center, slot.overall	length, width
polygon.*	radius

{"command":"sketch.draw.dimensioned","params":{"command":"sketch.rectangle.center","params":{"center":[0,0],"corner":[35,25]},"dimensions":{"width":"w","height":"d"}}}

Features

Command	Minimal params	Traps
solid.extrude	distance	profiles defaults to every region, so two concentric circles give a solid disc. Pick regions with [{"point":[x,y]}] or [index]. Other options: operation (new/join/cut/intersect/auto), direction (positive/negative/symmetric), through_all: true, start_offset. A cut that misses reports success.
solid.box	length, width, height	center:[x,y,z] or corner. The quickest way to block out a part.
solid.cylinder	radius or diameter, height	base is the centre of the bottom (default origin), axis defaults to Z. Expressions work in base. Always pass operation.
sketch.slot.overall / sketch.slot.center_to_center	p0, p1 (overall ends / arc centres), width	Ids and dof are in the "Ids" section above.
solid.fillet / solid.chamfer	edges:[[x,y,z]], radius / distance	The pick snaps to the nearest edge, with no distance limit and no error, so check that the face count changed. One pick takes the whole tangent chain: a rounded rim needs 1 point, not 8.
solid.shell	faces:[[x,y,z]], thickness	A point on each face to remove, or its name from body_topology. Fillet first, except an edge of a removed face (see Order in SKILL.md).
solid.hole	position:[x,y,z] on a face + diameter, or sketch (+ points)	clearance:"M3". depth defaults to through all. type is one of simple/drilled/counterbore/countersink. A countersink needs cs_diameter and cs_angle; a counterbore needs cb_diameter and cb_depth. position is a fixed point.
solid.pattern.rectangular	features, dir1, count1, spacing1 (+ dir2, count2, spacing2)	Spacing takes expressions and follows parameters.
solid.pattern.circular	features, axis ("Z" or {origin, dir}), count	angle defaults to 360 deg. A full pattern keeps the COM on the axis, so check its radius with a top-view screenshot.
solid.mirror	features:[names], plane (XY/XZ/YZ, a construction plane, or {origin, normal})	Follows parameters. Mirror and pattern features cannot be mirrored or patterned again.

• Names: name every feature ("name":"Standoff") and keep names unique across sketches and features. timeline.roll_to {"feature":"Plate"} picks the first match, which can be the sketch.

• Counts as parameters: parameters.add {"name":"n","expression":"6","unit":""} creates a unitless parameter, and "count":"n" uses it in a pattern.

• Holes on a parametric bolt circle:

  1. Cut one hole with solid.cylinder {"diameter":6.6,"height":"T + 2","base":["bcd/2",0,-1],"operation":"cut","name":"BoltHole"}.
  2. Repeat it with solid.pattern.circular {"features":["BoltHole"],"axis":"Z","count":"n"}.

  Both the radius and the count follow their parameters.

• Several parameter changes: use one batch of parameters.change steps instead of one set_parameter call each.

• Primitive booleans: a solid.box or solid.cylinder cut that touches curved faces of the target can fail with the exact fallback ... takes planar faces only. Use a sketch profile and an extrude cut instead, for example a slot sketch rather than a box plus 2 cylinders.

Worked example: parametric plate with 4 counterbored holes (1 batch)

{"commands":[
 {"command":"parameters.add","params":{"name":"L","expression":"80 mm"}},
 {"command":"parameters.add","params":{"name":"W","expression":"50 mm"}},
 {"command":"parameters.add","params":{"name":"T","expression":"6 mm"}},
 {"command":"parameters.add","params":{"name":"inset","expression":"8 mm"}},
 {"command":"sketch.create","params":{"plane":"XY","name":"PlateSketch"}},
 {"command":"sketch.draw.dimensioned","params":{"command":"sketch.rectangle.center","params":{"center":[0,0],"corner":[40,25]},"dimensions":{"width":"L","height":"W"}}},
 {"command":"sketch.finish","params":{}},
 {"command":"solid.extrude","params":{"distance":"T","name":"Plate"}},
 {"command":"solid.fillet","params":{"edges":[[40,25,3],[-40,25,3],[40,-25,3],[-40,-25,3]],"radius":5,"name":"Corners"}},
 {"command":"sketch.create","params":{"plane":"XY","name":"HolePts","offset":"T"}},
 {"command":"sketch.point","params":{"point":[32,17]}},
 {"command":"sketch.dimension","params":{"entities":["origin","p1"],"type":"horizontal","value":"L/2 - inset"}},
 {"command":"sketch.dimension","params":{"entities":["origin","p1"],"type":"vertical","value":"W/2 - inset"}},
 {"command":"sketch.finish","params":{}},
 {"command":"solid.hole","params":{"sketch":"HolePts","diameter":3.4,"type":"counterbore","cb_diameter":6.5,"cb_depth":3.3,"name":"Hole"}},
 {"command":"solid.pattern.rectangular","params":{"features":["Hole"],"dir1":[-1,0,0],"count1":2,"spacing1":"L - 2*inset","dir2":[0,-1,0],"count2":2,"spacing2":"W - 2*inset","name":"Holes"}}
]}

Expected volume:

• Plate: L*W*T - 4*r²(1-π/4)*T
• Each hole: π*1.7²*(T-3.3) + π*3.25²*3.3
• Total: 23335.2 mm³, with 22 faces.

After set_parameter L=120 the volume is 35335.2 mm³, and the holes stay in the corners.

Reading measure

• Tolerance: analytic and measured volumes agree to about 0.001-0.01%, so treat a gap that small as a match. Long shallow arcs measure worse, about 0.1% (R 1000 mm over 20 degrees).
• Face counts: compare the logical faces, not the larger kernel.faces.
• Reply types: set_parameter returns recomputed as a number. A batch reply echoes every step.
• Boolean warning: a feature warning such as Boolean retry: temporary coincident-face separation up to 2.050000e0 mm per face means the kernel nudged faces that coincide. Examples are a join flush on a face, such as a cylinder joined onto the floor of a shelled box, or a tapered cut that starts on a face. When the volume still matches your number the warning is harmless. When it does not, the retry may have left the geometry wrong, with no error. Seen: on a box with filleted corners, a shell and a rounded rim, a standoff joined and its pilot hole cut as two cylinders, patterned 2x2, left material in the holes at some standoff heights. A boss with its hole as one ring profile (two concentric circles, extrude the ring) built correctly at every height tried (3 to 20 mm). Another kind, tool displacement, moves a tool by about 2e-4 mm.

Reply cost (0.8, plate example)

Call	Size
list_commands {}	Over 100 KB. Never call it unfiltered; filter on a distinctive word such as "hole" or "slot".
body_topology	25-45 KB
inspect_design {}	12 KB, and it grows with the sketches
inspect_design {"measure":false,"sketches":false}	4 KB: parameters, timeline errors, bodies
sketch.inspect	5 KB per small sketch
parameters.list {"filter":"feature"}	3 KB
measure {}	1 KB: volume, bbox, COM, face/edge/vertex counts
sketch.solve	under 100 B: dof, status, profile count
screenshot {"source":"model","width":480,"height":320}	one small image. Without source, a bridged server returns the whole app window and ignores the size.

Errors

Error text	Fix
... is not available right now: no sketch is being edited	Run sketch.create or sketch.edit {sketch} first.
unknown sketch entity 'p1'	Use the ids from created. A circle's centre is c1.center.
the corner must join exactly two lines	It is a rectangle.center corner. Use the {a, b} form.
`cs_diameter` must be a number or an expression	Countersinks need cs_diameter and cs_angle, even with clearance.
unsupported dimension role for this creator	Check the roles table above.
<Feature> cannot be patterned or mirrored yet	Pattern the original feature, for example one 2x2 rectangular pattern.
an edge is a point [x,y,z], {point} or {body, index}	An edge pick contained an expression. Use plain numbers.
boolean Cut: the operation failed ... planar faces only	See "Primitive booleans" above.