A guide for AI agents

This page is part of the Moket skill: it is written for AI agents, which read it as Markdown. Values in angle brackets in the examples stand for ids an agent gets from Moket.

Sketches

A sketch (core.sketch) is a 2D drawing on a plane: points, lines, circles, arcs, splines and text, held in place by constraints and dimensions. Its closed regions become profiles for extrude, revolve, sweep and loft, and its points place holes. Dimensions are expressions, so a sketch follows the part's parameters.

Read Working with plans and Parts first.

Sketch templates

Most sketches are a rectangle, circles, hole points, a polygon outline or a slot. The sketch.template plan helper writes them fully constrained, with every size an expression:

json

{
  "type": "sketch.template",
  "id": "$sk",
  "name": "Base",
  "template": {
    "kind": "rectangle",
    "width": "width",
    "depth": "depth",
    "plane": { "kind": "origin", "plane": "XY" }
  }
}

Template	Shape
`{"kind":"rectangle","width":..,"depth":..}`	Centered on the origin; its lines are bottom, right, top, left.
`{"kind":"circles","diameter":"6 mm","centers":[{"x":"0 mm","y":"pitch"}]}`	Circles of one diameter.
`{"kind":"points","points":[{"x":"-30 mm","y":"0 mm"}]}`	Points, for hole centers.
`{"kind":"profile","corners":[{"x":..,"y":..},..],"axis":[[0,0],[0,10]]}`	A closed polygon with every corner dimensioned from the origin; the optional axis is a construction line for a revolve.
`{"kind":"slot","from":{..},"to":{..},"width":"6 mm"}`	A slot between two arc centers; its lines are top and bottom, its arcs start and end.
`{"kind":"polygon","center":{..},"sides":6,"diameter":"10 mm"}`	A regular polygon inscribed in a construction circle, its first side horizontal at the bottom (a hex's flats are `diameter * cos(30 deg)` apart).

The answer lists the entity ids each template made (sketches in the preview), for later plans that constrain, trim or reference them.

Sketch planes

plane is one of:

{"kind":"origin","plane":"XY"|"XZ"|"YZ"}, the default XY. XY: sketch x is the part's X, y its Y, the normal +Z. XZ: x is X, y is Z, the normal -Y. YZ: x is Y, y is Z, the normal +X. Extrudes go along the normal (reversed against it), holes against it.
{"kind":"face","ref":{"kind":"face","name":<topological name>}}: a planar face of a body, from query_geometry or one of your own placeholders (f($base:end)). The sketch follows the face when it moves. Its origin is the part's origin dropped onto the face's plane, sketch x is the part's X laid on the face (the part's Y when the face faces mostly along X), and sketch y is the normal crossed with x, so it depends on which way the face faces:
The face faces Sketch x Sketch y
+Z X Y
-Z X -Y
+Y X -Z
-Y X Z
+X Y Z
-X Y -Z
So hole centers on the top of a flange that faces +Y take the part's Z with its sign changed as y.
{"kind":"plane","feature":<core.plane id>}: a construction plane, offset from a plane or a face. The offset goes along the base's normal: from XZ toward -Y, so a plane at Y = 20 mm is XZ with offset -20 mm.

The face faces	Sketch x	Sketch y
+Z	X	Y
-Z	X	-Y
+Y	X	-Z
-Y	X	Z
+X	Y	Z
-X	Y	-Z

sketch.setPlane moves a sketch to another plane.

Drawing by hand

For shapes no template makes, create a core.sketch with its entities and constraints. Points carry a first guess of their position in mm; the solver moves them to satisfy the constraints. Fix one point (or constrain it to the origin) and dimension the rest until the sketch has no degrees of freedom left (get_sketch says how many remain).

json

{
  "summary": "Triangular gusset 40 x 30, 5 mm thick",
  "steps": [
    {
      "label": "Gusset",
      "commands": [
        { "type": "document.rename", "name": "Gusset" },
        {
          "type": "feature.create",
          "id": "$tri",
          "featureType": "core.sketch",
          "name": "Triangle",
          "params": {
            "plane": { "kind": "origin", "plane": "XY" },
            "entities": [
              { "id": "$p1", "kind": "point", "x": 0, "y": 0, "fixed": true },
              { "id": "$p2", "kind": "point", "x": 40, "y": 0 },
              { "id": "$p3", "kind": "point", "x": 0, "y": 30 },
              { "id": "$bottom", "kind": "line", "start": "$p1", "end": "$p2" },
              { "id": "$side", "kind": "line", "start": "$p1", "end": "$p3" },
              { "id": "$slope", "kind": "line", "start": "$p2", "end": "$p3" }
            ],
            "constraints": [
              { "id": "$h", "kind": "horizontal", "line": "$bottom" },
              { "id": "$v", "kind": "vertical", "line": "$side" },
              {
                "id": "$w",
                "kind": "distance",
                "a": "$p1",
                "b": "$p2",
                "value": "40 mm"
              },
              {
                "id": "$t",
                "kind": "distance",
                "a": "$p1",
                "b": "$p3",
                "value": "30 mm"
              }
            ]
          }
        },
        {
          "type": "feature.create",
          "id": "$plate",
          "featureType": "core.extrude",
          "name": "Gusset",
          "params": {
            "sketch": "$tri",
            "operation": "new",
            "body": "$body",
            "distance": "5 mm",
            "direction": "normal"
          }
        }
      ]
    }
  ]
}

Constraints: coincident, horizontal, vertical, horizontalPoints, verticalPoints, parallel, perpendicular, equalLength, equalRadius, tangent, pointOnLine, pointOnCircle, midpoint, symmetric. Dimensions, with a value expression: distance, horizontalDistance, verticalDistance, pointLineDistance, radius, diameter, angle, lineOffset, radiusDifference.

Commands on an existing sketch: sketch.add (entities and constraints), sketch.remove, sketch.constrain, sketch.setDimension (a dimension's value), sketch.move, sketch.setConstruction, sketch.setFixed. Construction geometry ("construction": true) guides the shape and makes no profile.

Sketch tools

Commands on a sketch's stored geometry:

sketch.trim: a curve and a point on the piece to remove; it is cut back to the curves that cross it.
sketch.extend: a free end to the next curve.
sketch.offset: curves, a distance expression and its value in mm, side inside, outside or both; linked offsets follow the original. A whole loop is the usual input.
sketch.mirror: curves and a line; the copies stay symmetric.
sketch.fillet: a corner point where two lines meet and a radius; the corner stays as a construction point.
sketch.project: model edges by topological name with their shape on the sketch plane; the rebuild moves them with the edge, and a lost edge leaves SKETCH_PROJECTION_DANGLING. Its ids go in order, per edge: the projection, then its fixed entities (a line: two points and the line; a circle: center and circle; an arc: center, start, end and arc). With "ids":["$proj","$c","$circle"] a later sketch.offset in the same plan takes ["$circle"].

Slots and regular polygons drawn by hand are lines and arcs added with sketch.add, with tangent, equal and point-on-circle constraints.

Splines

A spline is a sketch entity over ordinary points: by fit it passes through them, by control it is shaped by them (add construction lines between control points to constrain its tangents). Constraints go on its points, not on the curve. sketch.setSpline switches between fit and control. Splines work in profiles and in sweep paths.

Text

Text is a sketch entity at a point: an expression height (of a capital letter) and angle, font noto-sans, noto-sans-mono or inter, bold, align left, center or right. Its outlines are closed regions: extrude them to emboss, or cut to engrave. {name} in the text is a parameter's value and {project.name} a project parameter's, so a part number or a size follows the part. sketch.setText changes it.

json

{
  "summary": "Name plate 60 x 20 x 3 with MOKET engraved 0.5 mm deep",
  "steps": [
    {
      "label": "Plate, its top face at Z = 0",
      "commands": [
        { "type": "document.rename", "name": "Name plate" },
        {
          "type": "sketch.template",
          "id": "$outline",
          "name": "Outline",
          "template": {
            "kind": "rectangle",
            "width": "60 mm",
            "depth": "20 mm"
          }
        },
        {
          "type": "feature.create",
          "id": "$base",
          "featureType": "core.extrude",
          "name": "Plate",
          "params": {
            "sketch": "$outline",
            "operation": "new",
            "body": "$plate",
            "distance": "3 mm",
            "direction": "reversed"
          }
        }
      ]
    },
    {
      "label": "Engraving",
      "commands": [
        {
          "type": "feature.create",
          "id": "$label",
          "featureType": "core.sketch",
          "name": "Label",
          "params": {
            "plane": { "kind": "origin", "plane": "XY" },
            "entities": [
              { "id": "$at", "kind": "point", "x": 0, "y": -4, "fixed": true },
              {
                "id": "$text",
                "kind": "text",
                "text": "MOKET",
                "font": "inter",
                "bold": true,
                "position": "$at",
                "height": "8 mm",
                "angle": "0 deg",
                "align": "center"
              }
            ],
            "constraints": []
          }
        },
        {
          "type": "feature.create",
          "id": "$engrave",
          "featureType": "core.extrude",
          "name": "Engrave",
          "params": {
            "sketch": "$label",
            "operation": "cut",
            "targets": ["$plate"],
            "distance": "0.5 mm",
            "direction": "reversed"
          }
        }
      ]
    }
  ]
}

Sketches ​

Sketch templates ​

Sketch planes ​

Drawing by hand ​

Sketch tools ​

Splines ​

Text ​

Sketches

Sketch templates

Sketch planes

Drawing by hand

Sketch tools

Splines

Text