Tutorial 2 — Two Classic Mechanical Parts: a Flanged Bushing and an L-Bracket

▶ Prefer video? Tutorial 2 starts about halfway through the Quick Start walkthrough (MP4). Next: Tutorial 3: Box, Gear & Sketch →

Before you start: do Tutorial 1 first (starter-help-and-tutorial.md). It covers the editor, params, and how Rebuild works. Every CADL listing below passes dsl.validate and builds to STEP with design/dsl.py. The measured results are noted under each listing. The AI may phrase its own result a little differently, but the structure will be the same.

What you'll learn - Part A: a turned (round) part. You'll see two ways to build it, with stacked cylinders or with a single revolve profile, plus how to resize the bore and take the STEP file to CNC. - Part B: a multi-face part. You'll drill holes from two different faces and learn how the hole [u, v] coordinates work on each face.

Part A — Flanged Bronze Bushing (CNC lathe or 3D print)

A1. Prompt

Set Mode to CNC (3-axis) if you'll machine it, or 3D print if you'll print it. Then enter:

Flanged bushing: 30 mm flange diameter, 4 mm flange thickness, 18 mm body outer diameter, 22 mm total height, with a 10 mm through bore and a 1 mm chamfer on the top edge

Click Generate. You should get PASS with a bbox of 30 × 30 × 22 mm.

A2. The CADL recipe (stacked cylinders + union + chamfer + hole)

{
  "units": "mm",
  "plan": "1. Flange: cylinder Ø30 x 4, base centred on the origin (z 0..4). 2. Body: cylinder Ø18 x 22 on the same axis (z 0..22), overlapping the flange. 3. Union. 4. 1 mm chamfer on the outer top edge of the body, picked by a point on that edge. 5. Ø10 bore drilled through all from the top.",
  "issues": [
    {"type": "assumption", "msg": "Only the outer top edge is chamfered; the bore edge stays sharp.", "ref": "top_chamfer"},
    {"type": "assumption", "msg": "The flange sits at the bottom (z = 0).", "ref": "flange"}
  ],
  "params": {"flange_d": 30, "flange_h": 4, "body_d": 18, "total_h": 22, "bore_d": 10, "chamfer": 1},
  "steps": [
    {"id": "flange", "op": "cylinder", "diameter": "$flange_d", "height": "$flange_h"},
    {"id": "body",   "op": "cylinder", "diameter": "$body_d",   "height": "$total_h"},
    {"id": "blank",  "op": "union", "items": ["flange", "body"]},
    {"id": "top_chamfer", "op": "chamfer", "target": "blank", "distance": "$chamfer",
     "edges": "near", "points": [["=$body_d/2", 0, "$total_h"]]},
    {"id": "bore", "op": "hole", "target": "top_chamfer", "face": "top", "diameter": "$bore_d", "positions": [[0, 0]]}
  ],
  "result": "bore"
}

Measured: bbox 30.00 × 30.00 × 22.00 mm, volume 5,652.8 mm³. The STEP file has 3 cylindrical faces, 3 flat faces and 1 cone (the chamfer).

How the params work

Why it's built this way - Cylinders default to anchor: "base", so both start at z = 0 on the same axis. The body overlaps the flange instead of sitting on top of it. That keeps total_h truly the total height and gives the union a solid overlap. - The chamfer uses edges: "near" with a point exactly on the outer top rim, [body_d/2, 0, total_h]. edges: "top" would also chamfer the bore rim, because every edge of the top face counts. - The chamfer comes before the hole. At that point the top face has only one circular edge, so there's no ambiguity. - The hole has no depth, so it goes through all. On face: "top", [0, 0] is the global x, y of the axis.

Alternative: one revolve profile (identical solid, also 5,652.8 mm³). Use this when you want the whole cross-section in one place:

{"units": "mm",
 "params": {"flange_d": 30, "flange_h": 4, "body_d": 18, "total_h": 22, "bore_d": 10, "chamfer": 1},
 "steps": [{"id": "bushing", "op": "revolve", "profile": [
   ["=$bore_d/2", 0], ["=$flange_d/2", 0], ["=$flange_d/2", "$flange_h"], ["=$body_d/2", "$flange_h"],
   ["=$body_d/2", "=$total_h-$chamfer"], ["=$body_d/2-$chamfer", "$total_h"], ["=$bore_d/2", "$total_h"]]}],
 "result": "bushing"}

The profile is a list of [r, z] points: radius out from the Z axis, and height. Starting at r = bore_d/2 instead of 0 leaves the bore hollow, and the diagonal point pair is the chamfer.

A3. Open up the bore: 10 → 12 mm (no AI)

1. In params, change "bore_d": 10 to "bore_d": 12.
2. Click Rebuild (no LLM) or press Ctrl+Enter.
3. Check the result: the bbox stays 30 × 30 × 22 and the volume drops to 4,892.5 mm³. If the bore were bigger than body_d - 2*chamfer, the build would fail and a red error line would appear. Click it to jump to the problem.

A4. To CNC: STEP → CAM → feeds & speeds → simulate

1. Download part.step. It holds true cylinders and a true cone, which CAM needs for clean toolpaths. Open it in Fusion, FreeCAD Path or another CAM program.
2. Work out spindle speed and feed for bronze (e.g. 932/SAE 660 bearing bronze) and your tool in the Feeds & Speeds calculator at spinstop.com/engine/.
3. Post-process to G-code and load it into G-code Sim at /gsim/ with Open file, or with Save to account and My programs…. Pick a flavor (e.g. milling (LinuxCNC)), choose path + stock, and press ▶. You can color the path by speed to spot slow moves.
4. If you're 3D printing instead: click Save to account → Open in Mesh / Slicer → Slice to G-code → Open in Simulator.

⚠️ gsim simulates milling and printer G-code. It does not show lathe (turning) toolpaths, so check lathe code in your CAM program.

Part B — L-Bracket with Holes in Two Faces

B1. Prompt

L-bracket 50 mm wide, base leg 60 mm long and 6 mm thick, vertical wall 45 mm tall and 6 mm thick, with two 5 mm holes in the base and two 5 mm holes in the vertical wall

You should get PASS with a bbox of 60 × 50 × 45 mm.

B2. The CADL recipe (box + box + union + hole on top + hole on left)

{
  "units": "mm",
  "plan": "1. Base: box 60(x) x 50(y) x 6(z) with its corner at the origin. 2. Wall: box 6 x 50 x 45 with its corner at the origin, so it overlaps the base at x 0..6, z 0..6. 3. Union. 4. Two Ø5 holes down through the base from the top face at x=38, y=12.5 and 37.5. 5. Two Ø5 holes through the wall from the left face (-X) at y=12.5 and 37.5, z=30.",
  "issues": [
    {"type": "assumption", "msg": "Base holes are at x = 38, 12.5 mm in from each side.", "ref": "$base_hole_x"},
    {"type": "assumption", "msg": "Wall holes are at z = 30 mm, well above the base.", "ref": "$wall_hole_z"}
  ],
  "params": {"w": 50, "base_l": 60, "t": 6, "wall_h": 45, "hole_d": 5, "edge": 12.5, "base_hole_x": 38, "wall_hole_z": 30},
  "steps": [
    {"id": "base",    "op": "box", "size": ["$base_l", "$w", "$t"],  "anchor": "corner"},
    {"id": "wall",    "op": "box", "size": ["$t", "$w", "$wall_h"],  "anchor": "corner"},
    {"id": "bracket", "op": "union", "items": ["base", "wall"]},
    {"id": "base_holes", "op": "hole", "target": "bracket", "face": "top", "diameter": "$hole_d",
     "positions": [["$base_hole_x", "$edge"], ["$base_hole_x", "=$w-$edge"]]},
    {"id": "wall_holes", "op": "hole", "target": "base_holes", "face": "left", "diameter": "$hole_d",
     "positions": [["$edge", "$wall_hole_z"], ["=$w-$edge", "$wall_hole_z"]]}
  ],
  "result": "wall_holes"
}

Measured: bbox 60.00 × 50.00 × 45.00 mm, volume 29,228.8 mm³. The STEP file has 4 cylindrical faces (the four holes).

B3. How [u, v] works on each face

A hole's face sets the drilling direction. Its positions are global coordinates in mm on the two other axes:

• Base holes (face: "top"). [38, 12.5] means x = 38, y = 12.5. "Top" means the top of the whole bracket's bbox (z = 45, the top of the wall). Because a hole with no depth goes through all, it still cuts cleanly down through the 6 mm base. Keep base_hole_x greater than t (6), or you'll drill into the wall.
• Wall holes (face: "left"). The wall is the −X side of the bbox (x 0..6), so [12.5, 30] means y = 12.5, z = 30. Keep wall_hole_z greater than t, or you'll hit the base.
• Why not front? The front (−Y) face is the 50 mm edge of the L, so holes from there would run lengthwise through the part. Pick the face whose normal is the hole's axis.

B4. Try these edits (Rebuild, no AI)

• "hole_d": 5 → 5.5 for M5 clearance.
• "wall_h": 45 → 60. The wall grows, and the wall holes stay at wall_hole_z. You could make that a formula: "wall_hole_z": "=$wall_h*2/3".
• "t": 6 → 8. The base and the wall both thicken, because both boxes use $t.
• With AI: type add a 5 mm inside fillet where the base meets the wall in Edit with AI. The usual result is a fillet step ("edges": "near", "points": [[6, 25, 6]], radius 5) placed before the holes. This version was checked and builds.

B5. Export

part.step for CAD/CAM. part.stl → Open in Mesh / Slicer for printing; print it on its side so the layers run along the bend for strength.

90-Second Video Storyboard — Tutorial 2

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