Tutorial 3 — Enclosures, Gears & Sketch-to-CAD

Jump to: 3A Project box · 3B Spur gear · 3C Sketch-to-CAD · Downloads · Video storyboard

Three new skills in about 15 minutes:

• 3A: Project box. fillet → shell → floor hole. Hollow parts with one open face.
• 3B: Spur gear. spur_gear + hub cylinder + union + a bore and a bolt circle of holes.
• 3C: Sketch-to-CAD. Drop a dimensioned drawing on the Designer and let the vision model read it.

You need a signed-in account with alpha access on /design/. If you haven't done Tutorials 1 and 2, start with the Quick Start. Every recipe below was built and checked with design/dsl.py, and every volume is the real result.

Part A — Electronics Project Box (3D print)

A1. Prompt

Rectangular electronics enclosure box 80x50x30 mm, 2.5 mm wall thickness, open on top, with 4 mm outer vertical corner fillets and two 3.5 mm mounting holes on the bottom floor

Set Mode = 3D print and click Generate. Expect PASS with a bounding box of 80 × 50 × 30 mm and a volume of 26,780.5 mm³.

A2. The CADL recipe (box → fillet → shell → hole)

// prompt: Rectangular electronics enclosure box 80x50x30 mm, 2.5 mm wall thickness, open on top, with 4 mm outer vertical corner fillets and two 3.5 mm mounting holes on the bottom floor
// verified with design/dsl.py 2026-10-27, volume 26780.5 mm^3
{
  "plan": "1. Solid block 80x50x30, centred in x/y, z 0..30. 2. Round the 4 vertical outer corners (r 4). 3. Shell inward 2.5 mm with the top face removed. 4. Two 3.5 mm mounting holes through the 2.5 mm floor, 25 mm either side of centre.",
  "units": "mm",
  "issues": [
    {"type": "assumption", "msg": "Mounting holes placed on the long axis at x = \u00b125 mm, y = 0.", "ref": "$hole_dx"}
  ],
  "params": {
    "w": 80,
    "d": 50,
    "h": 30,
    "wall": 2.5,
    "corner_r": 4,
    "hole_d": 3.5,
    "hole_dx": 25
  },
  "steps": [
    {"id": "block", "op": "box", "size": ["$w", "$d", "$h"]},
    {"id": "rounded", "op": "fillet", "target": "block", "radius": "$corner_r", "edges": "vertical"},
    {"id": "hollow", "op": "shell", "target": "rounded", "thickness": "$wall", "open_face": "top"},
    {
      "id": "mounts",
      "op": "hole",
      "target": "hollow",
      "face": "bottom",
      "positions": [["=-$hole_dx", 0], ["$hole_dx", 0]],
      "diameter": "$hole_d",
      "depth": "$wall"
    }
  ],
  "result": "mounts"
}

Why the steps are in this order - Fillet before shell. Rounding the 4 vertical edges of the solid block first means shell offsets the rounded walls inward. You get r4 corners outside and matching r1.5 corners inside (4 − 2.5) for free. Shelling first and filleting second would need two fillets and often fails in the kernel. - shell with open_face: "top" removes the +Z face and hollows everything else inward by $wall. The floor and the walls both end up exactly wall thick. - hole on face: "bottom" with depth: "$wall". Positions on the bottom face are global (x, y). box defaults to anchor: "base", so x and y are centred and [±25, 0] sits on the long axis. Using depth: "$wall" means the holes cut only the floor, and they stay correct when you change the wall thickness.

A3. Tweak it (Rebuild, no LLM)

In the CADL editor, change two params and press Ctrl+Enter or Rebuild (no LLM):

"h": 30 → 40,  "wall": 2.5 → 3.5

The floor holes follow automatically, because their depth is $wall. Other one-number edits to try: corner_r 4 → 8 for softer corners, hole_dx 25 → 30 to spread the holes.

Lid idea: ask Edit with AI to "add a separate 80x50x2.5 lid with a 1.5 mm lip that fits inside the walls". Or reuse the enclosure prompt from Tutorial 1's prompt list.

Part B — Parametric Spur Gear with Hub & Bolt Circle

B1. Prompt

24-tooth spur gear, module 2 mm, 10 mm thick, with a 20 mm diameter x 16 mm tall center hub, an 8 mm through bore, and four 4 mm lightening holes on a 30 mm bolt circle

Expect PASS at 51.98 × 51.98 × 16 mm with a volume of 18,312.5 mm³.

B2. The CADL recipe (spur_gear + cylinder + union + 2 holes)

// prompt: 24-tooth spur gear, module 2 mm, 10 mm thick, with a 20 mm diameter x 16 mm tall center hub, an 8 mm through bore, and four 4 mm lightening holes on a 30 mm bolt circle
// verified with design/dsl.py 2026-10-27, volume 18312.5 mm^3
{
  "plan": "1. 24-tooth module-2 spur gear, 10 thick, z 0..10 (pitch dia 48, tip dia 52). 2. Hub cylinder dia 20 x 16 on the same axis, z 0..16. 3. Union. 4. 8 mm through bore on the axis. 5. Four 4 mm lightening holes on a 30 mm bolt circle.",
  "units": "mm",
  "issues": [
    {"type": "assumption", "msg": "Pressure angle 20 deg (default); hub sits on the gear base and projects 6 mm above the gear face.", "ref": "$hub_h"}
  ],
  "params": {
    "m": 2,
    "z": 24,
    "gear_t": 10,
    "hub_d": 20,
    "hub_h": 16,
    "bore_d": 8,
    "lh_d": 4,
    "bc_d": 30
  },
  "steps": [
    {"id": "gear", "op": "spur_gear", "module": "$m", "teeth": "$z", "thickness": "$gear_t"},
    {"id": "hub", "op": "cylinder", "diameter": "$hub_d", "height": "$hub_h"},
    {"id": "body", "op": "union", "items": ["gear", "hub"]},
    {"id": "bore", "op": "hole", "target": "body", "face": "top", "positions": [[0, 0]], "diameter": "$bore_d"},
    {
      "id": "lightening",
      "op": "hole",
      "target": "bore",
      "face": "top",
      "positions": {"polar": {"count": 4, "radius": "=$bc_d/2", "start_deg": 45}},
      "diameter": "$lh_d"
    }
  ],
  "result": "lightening"
}

How it works - spur_gear builds an involute gear centred on the Z axis from z = 0, with a 20° pressure angle by default. Pitch Ø = m × z = 48. Tip Ø = m × (z + 2) = 52. Root Ø = m × (z − 2.5) = 43. - Hub. The cylinder also starts at z = 0 (anchor base). It overlaps the gear for its first 10 mm and stands 6 mm proud. The union fuses them into one solid. - Bore. A hole on face: "top" at [0, 0] with no depth goes through all 16 mm. - Bolt circle. Instead of listing 4 coordinates, positions uses {"polar": {"count": 4, "radius": "=$bc_d/2", "start_deg": 45}}. The holes sit at 45°, 135°, 225° and 315° on a 30 mm circle. They span r = 13…17 mm, clear of the hub (r 10) and the root circle (r 21.5). - spur_gear also has a built-in bore field. A separate hole step makes the bore a visible, editable step and lets you add a counterbore later (cbore_diameter / cbore_depth).

B3. Tweak it (Rebuild, no LLM)

"z": 24 → 30,  "bore_d": 8 → 10

The rebuild takes seconds. Mating gears need the same m. Their centre distance is m × (z1 + z2) / 2, so a 24T and a 30T gear at module 2 sit 54 mm apart. Keep bc_d / 2 + lh_d / 2 below the root radius when you shrink the tooth count.

Making it: 3D print it in PETG or nylon for prototypes. Or take spur_gear.step to CAM, check feeds & speeds in FeedWhiz and simulate the toolpath in G-code Sim.

Part C — Sketch-to-CAD: Start from a Drawing

C1. Get a sketch

Download sample_sketch_plate.png. It's a top view of an L-shaped mounting bracket: 90 × 70 outline, 30-wide legs, an R10 inside corner and 3 holes 12 mm from the edges. You can also photograph your own pencil sketch. Dark lines on light paper, every number legible, one view per image.

C2. Drop it in

On /design/, drag the image onto the Optional sketch drop zone, click it to choose a file, or paste with Ctrl+V. It accepts PNG, JPEG, WEBP or GIF up to 10 MB. Then type a short prompt that adds only what the drawing lacks:

Make this bracket 6 mm thick with M5 clearance holes

Click Generate. The status first shows describing sketch.

C3. What happens behind the scenes

1. A vision model (qwen2.5vl) reads the image together with your prompt. It writes a factual description: overall shape, every dimension written on the sketch (assumed mm), hole count and positions, fillets. It is told not to invent dimensions and to write "unspecified" instead.
2. That description is appended to your prompt. The usual CADL model then writes the recipe, and it's built and spec-checked like any other job.
3. Anything the sketch and prompt leave open shows up in issues as an assumption. Here that's the M5 clearance = 5.5 mm. Check those first.

A correct result looks like this recipe (verified at 90 × 70 × 6 mm, 23,101.1 mm³):

{"units":"mm","plan":"1. L-shaped plate outline from the sketch (90x70, 60x40 notch at top-right), extruded 6 mm. 2. R10 inside corner. 3. Three 5.5 mm M5-clearance holes 12 mm from the edges.",
"issues":[{"type":"assumption","msg":"M5 clearance = 5.5 mm (normal fit).","ref":"$hole_d"}],
"params":{"t":6,"hole_d":5.5,"r_in":10},
"steps":[{"id":"plate","op":"extrude","sketch":{"points":[[0,0],[90,0],[90,30],[30,30],[30,70],[0,70]]},"height":"$t","anchor":"corner"},
{"id":"corner","op":"fillet","target":"plate","edges":"near","radius":"$r_in","points":[[30,30,3]]},
{"id":"holes","op":"hole","target":"corner","face":"top","diameter":"$hole_d","positions":[[12,12],[78,12],[12,58]]}],
"result":"holes"}

Your generated CADL may use different ids or a slightly different construction. That's fine as long as the bounding box, holes and volume match.

C4. Sketch tips

• Dimension everything you care about. Overall sizes, hole centres from a datum edge, and radii. Unlabelled features get guessed or skipped.
• Put thickness, material, hole standards and "through" vs "blind" in the prompt. A top view can't show them.
• One part per image. Crop away clutter, and keep the lighting even for photos.
• If a dimension is misread, don't regenerate. Fix that one number in the CADL editor and Rebuild.

Downloads

Drop a .cadl file on the Designer's drop zone to open it straight in the CADL editor.

90-Second Video Storyboard — Tutorial 3

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