Design for manufacturability is not a checklist you run after the design is finished. It is a set of small drawing decisions that determine whether a part is cut in one setup or four, held in a vice or a custom fixture, measured in ten minutes or two hours. The rules below are the ones that change a quote most often on prototype work. None of them require a different design intent — only a different way of expressing it.
01 — Wall thickness
The problemA 0.5 mm wall looks fine in CAD and behaves like foil on the machine. It deflects under clamping, chatters while being cut, and measures differently every time it is touched.
What to doKeep load-bearing walls at 1.0 mm or more in aluminium and 1.5 mm or more in plastics, and thicken any wall that will be clamped or held in a vice. If the design needs a thin cosmetic wall, say so on the drawing and expect the part to be machined from a larger blank with support material left in place until the last operation. Uniform wall thickness is cheaper than a mix of thick and thin sections, because the cutter can run at one set of parameters instead of backing off at every transition.
02 — Internal corners and fillets
The problemA sharp internal corner cannot be cut by a round cutter. The tool leaves its own radius, so the drawing and the part disagree at exactly the place where stress concentrates.
What to doDraw an explicit fillet at every internal corner, ideally at least one third of the pocket depth and no smaller than the cutter radius you expect the shop to use. A 3 mm corner radius is a safe default for pockets deeper than 10 mm; 1 mm is possible but forces a small cutter, more passes and a higher price. Where a square corner is functionally required, design a relief hole at the corner and call it out — that is cheaper than a broached corner and easier to inspect.
03 — Draft and deep pockets
The problemVertical walls are fine in CNC, but a pocket deeper than three times its width forces a long, slender cutter that deflects. The floor comes out stepped and the wall tapers, even when the program is correct.
What to doKeep pocket depth below four times the cutter diameter where possible. If the geometry needs a deeper cavity, add a corner radius, split the pocket into a stepped shape, or accept a larger radius at the bottom. For moulded or cast derivatives of the same part, add 1–2° of draft now — it costs nothing at the prototype stage and prevents a tooling change later. Mark the deep feature on the drawing so the quote includes the long-reach tooling instead of discovering it at setup.
04 — Minimum hole diameter and depth
The problemA 0.8 mm hole in a 20 mm block is not a hole, it is a drilling project. The drill wanders, the exit burr is unpredictable, and the depth tolerance is difficult to hold without a second operation.
What to doKeep hole depth under four times the diameter for a standard drill, and under eight times only with peck drilling and a starter hole. Holes below 1 mm are better laser-cut, EDM’d or printed depending on the material. Always specify the drill point if the hole is blind: a 118° point adds roughly 0.3 × diameter to the flat-bottom depth, which matters when a screw or a dowel has to seat. Add a chamfer callout on both ends and the deburring cost disappears from the argument.
05 — Threads and thread relief
The problemA thread that runs to the bottom of a blind hole cannot be cut cleanly. The tap bottoms out, the last thread is incomplete, and the fastener binds before it seats.
What to doSpecify a thread relief or an undercut at the end of every blind threaded hole, and keep thread depth at least one diameter shorter than hole depth. For prototypes, a heat-set insert or a threaded insert is often better than a cut thread in plastic — it survives repeated assembly and can be replaced. State the thread standard (M, UNC, NPT) and the class; “M3 thread” without a class leaves the fit to the shop. Avoid threads in thin walls: aim for at least one diameter of material around the thread.
06 — Tolerance stack-up
The problemEvery dimension on the drawing is individually reasonable and the assembly still does not close. The error accumulates across the chain, and the last feature takes the blame.
What to doIdentify the assembly-critical dimension first, then work backwards and add the individual tolerances. If the stack exceeds the gap, tighten one feature rather than all of them — usually the one that is cheapest to measure. Use position or profile tolerances tied to a datum scheme instead of stacking symmetric ± values. On a prototype, it is often cheaper to leave one interface slightly oversize and fit it during assembly than to hold a tight tolerance across five parts.
07 — Surface finish and finishing allowance
The problemAnodising, powder coating and painting all add material. A bore that measures correctly before finishing may not accept its bearing afterwards, and a cosmetic face may lose its edge definition.
What to doState the finish and the expected build on the drawing: anodising adds roughly 2–5 µm per surface, powder coat 60–80 µm, paint 20–60 µm. For a precision bore, mask it or machine it after finishing. Keep sharp cosmetic edges to a small chamfer or radius so the coating does not pull back and expose a bare line. If the part will be bead blasted, specify the Ra range — the same blast parameter produces a different reading on aluminium and on stainless.
08 — Assembly datums and locating features
The problemA part with no clear datum is measured from wherever the inspector decides. Two “identical” parts then fail to interchange, and the argument is about the inspection rather than the machining.
What to doDefine three primary datum features on the drawing — typically a face, a side and a hole — and reference them in every geometric callout. Add locating features that force the assembly orientation: a dowel hole, a keyed edge or an asymmetric boss. For parts that pair with another, dimension the pair from a shared datum rather than from each part’s own centre. A datum scheme drawn once removes most of the ambiguity in a prototype review.
09 — Feature accessibility
The problemA feature that is easy to model can be impossible to reach. An undercut on the fourth face, a slot behind a wall or a hole at the bottom of a narrow channel may require a second setup — or a different process entirely.
What to doLook at the part from the direction of each feature and ask which face the cutter approaches from. Group features by approach direction: one face per setup is cheap, five faces is not. Where an undercut is unavoidable, consider 5-axis machining, a printed prototype or a split design. Tell the shop which features are cosmetic and which are functional; the setup order is planned around that answer, not around the CAD feature tree.
10 — File preparation
The problemA STEP file with no drawing leaves the shop guessing about material, finish, tolerance class and which faces matter. The quote comes back low, and the part arrives wrong.
What to doSend a STEP or IGES for geometry and a PDF or DWG for callouts — both, not one or the other. Put the material, general tolerance class (ISO 2768-m by default), finish and quantity in the title block. Balloon the critical dimensions, state the datum scheme and mark cosmetic surfaces. Name the revision on every file and keep the file name consistent with the drawing number. If a model has changed, send the new revision explicitly rather than overwriting the old one.
Reference — minimum walls and tool reach
The two tables below cover the questions that come up in almost every review. Both are starting points, not guarantees: the achievable value depends on the feature, the fixture and the finish, so confirm the number against your part before designing around it.
| Material | Min wall | Comfortable | Note |
|---|---|---|---|
| Al 6061 | 0.8 mm | 0.8 mm | Watch deflection on tall walls |
| Al 7075 | 1.0 mm | 1.0 mm | Higher strength, more notch-sensitive |
| SS 304 / 316 | 1.0 mm | 1.2 mm | Work-hardens; thin walls chatter |
| Brass | 0.8 mm | 0.8 mm | Free machining, stable |
| POM | 1.0 mm | 1.2 mm | Low friction, stable |
| ABS | 1.2 mm | 1.5 mm | Clamp marks show on thin walls |
| PC | 1.5 mm | 1.8 mm | Stress cracking risk |
| PEEK | 1.5 mm | 1.8 mm | Expensive stock; avoid rework |
| Cutter | 3 : 1 | 6 : 1 | Typical use |
|---|---|---|---|
| Ø 3 mm | 12 mm | 18 mm | Small radii, fine detail |
| Ø 6 mm | 24 mm | 36 mm | General pocketing |
| Ø 10 mm | 40 mm | 60 mm | Deep cavities, faster removal |
| Ø 12 mm | 48 mm | 72 mm | Large pockets, strong walls |
A 6:1 reach is possible but needs a long-reach cutter, lighter passes and more time. Anything beyond that is usually cheaper to redesign than to machine.
How to apply this before you send a file
Print the ten headings and read the drawing against them once. Then check the two things that are not on the list because they are not geometry: the general tolerance class in the title block, and whether the file you are sending is the revision you mean. In our experience, those two omissions cause more rework than any single feature on the list.
If a rule cannot be met because the function requires it, say so on the drawing. A thin wall marked as intentional will be machined with support and inspected with a method that suits it. The same wall unmarked will be quoted as a standard feature and will arrive with a defect that nobody agreed to accept.
Take the checklist to the drawing
The PDF version is the same ten rules with the two reference tables, formatted for printing and marking up.