Moket Help

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.

Drawings ​

A drawing is a document of its own that draws a part or an assembly (its source, at the latest revision) on sheets: views, dimensions and annotations whose values come from the model. When the part changes, the drawing follows. On a drawing use inspect_drawing and get_view; the part tools answer only on parts.

Read Working with plans first.

Standard, sheets and template ​

  • A drawing follows ISO (A4 to A0 sheets, first angle projection) or ASME (ANSI A to E sheets, third angle), and shows millimeters or inches (inspect_drawing: standard, units). Change them with drawing.update, and the sheets' size and projection with sheet.update, in one plan. Use ASME and inches when the user works in inches. Dimension values in inspect_drawing stay in mm whatever the drawing shows.
  • Sheets are drawn on a template: the standard's own (ISO 7200 or ASME Y14.1, with zones) unless drawing.update names a template document of the project ({"kind":"document","documentId":...}); list_projects lists each project's templates and create_drawing takes a templateId.
  • Title block fields are typed per sheet with sheet.update titleBlock, by the template's field keys (title, number, material, checker, approver, ...); empty ones come from the part and the account. Revisions go in drawing.update revisions ([{rev, description, date, by}], the whole list); the revision table lists them and the latest goes in the title block.
  • sheet.update also sets scale ("1:2"), size, orientation, projection, generalTolerance ("ISO 2768-m") and generalSurface.

Views ​

  • Orientations: front (looks along +Y, Z up), back, top (looks down, Y up), bottom, right, left, iso.
  • A view's position is where the part's origin lands on the sheet, in mm from the lower left. Projected views name their parent and stay aligned with it; the sheet's projection method decides on which side they go.
  • The views.standard helper places the standard views of the source, laid out by the projection method and scaled to fit:
json
{
  "summary": "Front, top, right and iso views of the plate",
  "steps": [
    {
      "label": "Views",
      "commands": [
        { "type": "views.standard", "views": ["front", "top", "right", "iso"] }
      ]
    }
  ]
}
  • view.create, view.update (orientation, scale, hidden lines, tangent edges, label, breaks), view.move and view.delete change single views.
  • Sections show what is inside: views.section cuts a front, top or side view along a line across the part (straight, half, or in steps for an offset section), hatches the cut faces and places the section beside its parent with its letter (A-A). Use one where hidden lines would cross, or the inside matters (bores, pockets, tapped holes), and dimension inside features on the section, on the cut edges get_view lists for it.
  • Details (views.detail) show small features larger; auxiliary views (views.auxiliary) show an inclined face at its true size; breaks (view.update breaks) shorten a long view. Dimension on them like on any view; values stay true.

Dimensions and annotations ​

Annotations reference edges by the topological names get_view returns for that view; their values come from the model, never from you.

json
{
  "type": "annotation.create",
  "id": "$width",
  "annotation": {
    "kind": "dimension",
    "view": "<front view>",
    "type": "horizontal",
    "refs": [
      { "kind": "edge", "name": "<left edge from get_view>", "at": "start" },
      { "kind": "edge", "name": "<right edge from get_view>", "at": "start" }
    ],
    "offset": [0, -12]
  }
}
  • Dimension types: horizontal, vertical, aligned (one line edge gives its length, two edges the distance between them), radius and diameter (a circle seen face on), angular, chamfer, ordinate (from a datum along an axis), arcLength. offset places the dimension line in sheet mm from the middle of its edges; 10 to 15 mm away from the view reads well. "text":"4x <value>" adds words around the value. Dimensions with the same set move together (baseline or chain).
  • Hole callouts: {"kind":"holeCallout","view":<view>,"ref":<a circle of the hole seen end on>,"position":[x,y]} writes the hole as the part makes it (count, drill, depth, counterbore, countersink, thread: 4x M4 - 6H ↧ 8). A through hole has no depth: ISO writes only its diameter (2x Ø5.5), ASME adds THRU. Use one on every hole and tapped hole instead of a plain diameter.
  • Tolerances on a size: {"type":"symmetric","value":0.1}, {"type":"deviation","upper":0.1,"lower":-0.05}, {"type":"limits",...}, {"type":"fit","hole":"H7"} or "shaft":"g6" (ISO 286, deviations from the tables), {"type":"basic"} for GD&T, {"type":"reference"}.
  • GD&T: datums ({"kind":"datum","letter":"A",...} on an edge seen edge on, or on a dimension) and feature control frames ({"kind":"featureControlFrame","characteristic":"perpendicularity","zone":{"value":0.02},"datums":[{"letter":"A"}],...}). Form tolerances take no datum; orientation and location need one; M and L only on a dimension. Broken rules show as GDT_INVALID.
  • Surface texture: {"kind":"surfaceSymbol","ref":<edge of the surface>,"process":"removal","parameters":["Ra 1.6"],...}, and generalSurface on the sheet for every other surface.
  • Center marks, centerlines and notes: centerMark, centerline, note.
  • A dimension whose edge is gone is dangling and shows no value: reattach it with annotation.update (new refs), or delete it.

Dimensioning a part completely ​

Unless the user asks for less, dimension a drawing so someone can make the part from it without measuring the model:

  1. The overall size in all three directions.
  2. Every hole by a hole callout, and its position from the part's edges or from a datum.
  3. Angles by angular dimensions, chamfers by chamfer dimensions, fillet radii.
  4. Every boss, slot and step; patterns with count and spacing (4x <value>).
  5. A fit on every size that mates with another part (a bore for a shaft or a bearing H7, a shaft g6, or as the user says), and the general tolerances in the title block (ISO 2768-m unless asked).
  6. A datum on the face or feature a fit is measured from, and a frame (perpendicularity or position) tying the fit to it; surface texture on fitted faces and a general symbol for the rest.
  7. A section view where hidden lines would cross inside the part.

Each size once, in the view that shows its shape best. Before you answer, check inspect_drawing:

  • missingSizes, missingCallouts, unfittedBores, crowded and gdtProblems must be empty. missingSizes lists overall and circle sizes no dimension shows yet; it cannot see positions, so check those yourself. crowded lists texts a line or another text runs through: move those annotations clear of the views and of each other.
  • No dimension may be dangling: reattach or delete one you leave behind, and say so.

Drawings of assemblies ​

Refs also name the component ({"kind":"edge","name":...,"component":...}). A parts list is {"kind":"partsList","sheet":<sheet>,"source":<assembly source id>} (above the title block, item 1 at the bottom), and balloons {"kind":"balloon","view":<view>,"component":<component>,"position":[x,y]} point at components.

Drawing commands ​

document.rename, drawing.update, sheet.update, view.create, view.update, view.move, view.delete, annotation.create, annotation.update, annotation.delete, and the helpers views.standard, views.section, views.detail, views.auxiliary. Read them with describe_commands.

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