CNC machining design guide
The numbers we work to every day: wall thickness, corner radii, hole depth ratios, thread limits and the tolerances that actually move the price. Check them before you finalise the drawing.
Every quotation includes a manufacturability review against these rules. If something in your model falls outside them, we tell you before you commit, not after the first article fails.
Wall thickness
Thin walls chatter under cutting load and spring away from the tool, so the finished dimension drifts. Metal tolerates thinner sections than plastic because it is stiffer and dissipates heat better.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| Minimum wall — metals | 0.8 mm | 0.5 mm | Below 0.8 mm the wall deflects under the cutter and needs a finishing pass at reduced depth; below 0.5 mm it usually distorts on release from the fixture. |
| Minimum wall — plastics | 1.5 mm | 1.0 mm | Plastics soften near the cutting zone and relieve internal stress after machining, so thin sections bow. PEEK and acetal hold better than ABS or nylon. |
| Unsupported rib height | ≤ 8 × thickness | ≤ 12 × thickness | A tall thin rib behaves like a cantilever: the taller it is relative to its thickness, the more it vibrates and the worse the surface becomes. |
Practical notes
- If a thin wall is unavoidable, tell us which face is functional — we can leave stock on the opposite side and machine it last.
- Keep wall thickness consistent across the part. Abrupt changes in section concentrate residual stress and cause warp after the part comes off the fixture.
Internal corner radii
An end mill is round, so an internal corner is always radiused. There is no such thing as a sharp internal corner in milling — the only question is how large the radius is and how hard the tool has to work to produce it.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| Corner radius vs pocket depth | R ≥ depth ÷ 3 | R ≥ depth ÷ 6 | The radius fixes the smallest cutter that can reach the corner, and a cutter can only go about six times its own diameter deep before it starts to deflect. |
| Smallest practical radius | 1.0 mm | 0.5 mm | A 0.5 mm radius needs a 1 mm cutter, which removes very little material per pass. It is achievable but multiplies the cycle time on that feature. |
| Floor radius (pocket bottom) | 0.5 mm or sharp | Sharp achievable | A flat end mill leaves a nearly sharp floor corner. Specifying a floor radius only helps if you also need a ball-nose finish there. |
Practical notes
- Make every internal corner in a part the same radius where you can. One cutter for all corners removes tool changes and cuts the price.
- If a mating part truly needs a sharp internal corner, add a relief slot at the corner instead of tightening the radius.
Holes and threads
Holes are the cheapest feature on a part as long as they use a standard drill diameter and stay within a sensible depth-to-diameter ratio. Threads follow the same logic — standard sizes in through holes cost almost nothing.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| Depth-to-diameter — standard drill | ≤ 4 : 1 | ≤ 10 : 1 | Past 4:1 the drill needs peck cycles to clear chips, which roughly doubles the time per hole. Past 10:1 it needs a gun drill and a separate setup. |
| Hole diameter | Standard drill sizes | 0.8 mm minimum | A non-standard diameter has to be interpolated with an end mill or reamed to size — both are slower than simply drilling it. |
| Blind tapped hole depth | 1.5 × D | 3 × D | Thread engagement beyond 1.5 × diameter adds almost no pull-out strength in metal. Deeper blind threads raise tap breakage risk sharply. |
| Smallest thread | M3 | M2 | Below M2 taps break often enough that we tap those features on a dedicated machine with a torque-limiting holder, which adds a setup. |
Practical notes
- Through holes are cheaper than blind holes, and a through-tapped hole is cheaper than a blind-tapped one. Where the design allows it, break through.
- Put all holes on one face if you can. Every additional face means another setup, and every setup adds both cost and a stack-up of positional error.
Pockets, cavities and undercuts
Cutter reach is the binding constraint on any pocket. The tool has to be long enough to reach the floor and stiff enough not to chatter on the way — and those two requirements pull in opposite directions.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| Pocket depth vs cutter diameter | ≤ 4 × D | ≤ 10 × D | Tool deflection grows with the cube of overhang. At 10 × diameter we have to drop feed and depth of cut enough that the cycle time roughly triples. |
| Undercuts | Standard T-slot / O-ring grooves | Custom profile by quote | Standard undercut cutters come in fixed widths. A custom undercut profile needs a ground form tool, which carries its own lead time and tooling charge. |
| Minimum slot width | 2.0 mm | 1.0 mm | A 1 mm slot means a 1 mm cutter with roughly 3 mm of usable flute length. It works for shallow slots and nothing deeper. |
Practical notes
- A deep cavity is often cheaper as two parts that bolt together. Ask us to compare before you commit to a single-piece design.
Tolerances, text and surface callouts
Tolerance is the single biggest lever on price. Tighten only what actually mates or seals, and leave the rest at the general tolerance — a drawing where every dimension carries ±0.01 mm costs several times one where three do.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| No drawing supplied | ISO 2768-m | ISO 2768-f on request | With only a 3D model we machine to ISO 2768-m (medium) by default. If you need finer as a blanket default, say so in the enquiry. |
| Drawing supplied — general | ±0.05 mm | ±0.01 mm | ±0.05 mm is routine on our machining centres. ±0.01 mm means temperature-controlled setup, in-process probing and 100 % inspection. |
| Engraved text — line width | 0.8 mm | 0.5 mm soft metals | Line width sets the engraving cutter diameter. Below 0.5 mm the tool is too fragile for steel and stainless. |
| Engraved text — depth | 0.25 mm | 0.10 mm | 0.25 mm survives bead blasting and anodising and stays legible. Shallower marks can disappear under a thick coating. |
Practical notes
- Mark the two or three critical dimensions on your drawing explicitly. We inspect those on every piece and report them — the rest go to sampling.
- Remember that anodising adds roughly 5–25 µm per surface. On a close-fitting bore, dimension the part before plating and tell us the final target.
What actually drives the price
Most cost reductions on a machined part come from four or five decisions made at the CAD stage. None of them require compromising on function.
| Parameter | Design to thisNo surcharge, no discussion needed | We can reachAchievable, but affects price or lead time | Where the limit comes from |
|---|---|---|---|
| Number of setups | 1 – 2 | 5+ possible | Each setup adds fixture time and operator handling. Features on five faces usually cost more than the same part machined from two directions on a 5-axis machine. |
| Material removal ratio | < 70 % of stock | > 90 % possible | Machining away 90 % of a billet means you pay for the full block and for the time to turn it into chips. A near-net starting form is often cheaper even if the stock costs more. |
| Quantity break | 25 – 100 pcs | 1 pc to 100,000 | Programming and fixturing are one-off costs. Going from 1 to 25 pieces typically drops the unit price by 50–70 % because that setup is spread across the batch. |
| Surface finish callout | Ra 1.6 (as-machined) | Ra 0.2 by grinding/lapping | As-machined Ra 3.2–1.6 comes free with the cut. Anything below Ra 0.8 needs an extra finishing operation on top of machining. |
Practical notes
- Send the STEP file early, even at concept stage. A ten-minute review before you finalise the drawing is usually worth more than any redesign after the first quote.
Not sure whether your part clears these limits?
Send the STEP file. A manufacturing engineer marks up anything that will be difficult and returns it with the quotation — no charge, no obligation.