Tolérances d'usinage CNC : guide pratique pour concepteurs
Ce que coûtent réellement ±0,1 mm, ISO 2768 et ±0,005 mm, quelles tolérances sont gratuites, et comment coter un plan pour que l'atelier chiffre ce que vous vouliez dire.
Rédigé par Engineering Team
La documentation technique est tenue en anglais afin de préserver la précision des termes d'ingénierie.
Tolerance is the single largest cost lever on a machined part that engineers control from the keyboard. A dimension called out at ±0.01 mm where ±0.1 mm would function can raise the price of a part by 30 % or more — not because the machine cannot hold it, but because holding it changes how the part is made, fixtured, measured and inspected.
This guide covers what each tolerance band actually requires, what it costs, and how to specify tolerances so a machine shop quotes the part you intended.
What "tolerance" costs, in practice
Cost does not rise linearly with tightness. It rises in steps, because each step forces a different manufacturing decision:
| Tolerance band | What it requires | Relative cost |
|---|---|---|
| ±0.25 mm (ISO 2768-c) | Standard cutting, no special care | baseline |
| ±0.1 mm (ISO 2768-m) | Standard cutting, routine inspection | baseline |
| ±0.05 mm (ISO 2768-f) | Controlled finishing pass, sampled inspection | +5 – 10 % |
| ±0.02 mm | Single setup, temperature-stable fixture, 100 % inspection | +20 – 35 % |
| ±0.01 mm | Dedicated fixture, spindle probing, climate-controlled measurement | +35 – 60 % |
| ±0.005 mm | Grinding or hard turning after machining, part-by-part verification | +60 – 150 % |
The jump from ±0.05 mm to ±0.02 mm is where most of the cost appears, because that is the point where the shop stops trusting the process and starts measuring every part.
Default tolerances: what happens when you say nothing
If your drawing has no tolerance block, most shops apply ISO 2768-m to linear and angular dimensions. That means:
- Dimensions 0.5 – 6 mm: ±0.1 mm
- Dimensions 6 – 30 mm: ±0.2 mm
- Dimensions 30 – 120 mm: ±0.3 mm
- Dimensions 120 – 400 mm: ±0.5 mm
Notice that the default gets looser as the dimension grows. A 300 mm plate with no tolerance block can legitimately arrive 0.5 mm off nominal. If that matters, say so on the drawing.
Achievable tolerances by process
These are realistic production figures, not marketing numbers:
- 3-axis milling — ±0.01 mm on features within a single setup; ±0.03 mm across setups
- 5-axis milling — ±0.01 mm, with true position across five faces within 0.02 mm
- CNC turning — ±0.008 mm on diameter; concentricity 0.01 mm TIR between spindles
- Swiss turning — ±0.005 mm on diameter, length-to-diameter ratios to 20:1
- Wire EDM — ±0.005 mm positional, internal radii to 0.05 mm
- Surface grinding — flatness 0.003 mm over 300 mm
- Cylindrical grinding — ±0.002 mm on diameter, roundness 0.001 mm
- Lapping — flatness to 0.001 mm on small faces
The three tolerances people forget to specify
Flatness. A face machined to a ±0.05 mm thickness tolerance can still be bowed 0.2 mm across its width. If the face seals, mounts an optic or carries a bearing, call out flatness separately.
Perpendicularity. A bore drilled to H7 can be perfectly round and still sit 0.5° off square to the mounting face. Shafts bind, seals leak and bearings run hot because of exactly this.
Edge condition. "Break all sharp edges" means something different in every shop. Specify 0.2 – 0.4 mm chamfer, or 0.3 mm max radius, and you will get what you expect.
Temperature: the tolerance nobody accounts for
Aluminium expands about 23 µm per metre per °C. A 300 mm aluminium part measured at 26 °C reads roughly 0.04 mm longer than the same part at 20 °C — larger than a ±0.02 mm tolerance band, entirely.
This is why precision inspection happens in a temperature-controlled room, and why a part that measures in tolerance at the supplier may measure out of tolerance in your unheated goods-in area in January. If your tolerance is tighter than ±0.03 mm on a dimension longer than 200 mm, state the measurement temperature on the drawing (ISO 1 specifies 20 °C).
How to mark a drawing so it gets quoted correctly
- Put a tolerance block on the drawing. State the default standard (e.g. ISO 2768-m) once, then only call out the dimensions that differ.
- Balloon the critical characteristics. Five ballooned dimensions tell the shop where to spend inspection time. Thirty ballooned dimensions tell them nothing.
- Use fits, not bands, for mating features. "Ø20 H7" is unambiguous. "Ø20 ±0.01" leaves the shop guessing whether you want a clearance or an interference fit.
- Specify the datum scheme. Without datums, geometric tolerances are unmeasurable and the inspection report will not mean what you think it means.
- Say which dimension wins. If the 3D model and the 2D drawing disagree, the shop needs to know which one governs. Normally the drawing does.
A quick sanity check before you release
Ask three questions about every tight tolerance on the drawing:
- Does the function actually require it? A clearance hole for an M6 screw does not need ±0.02 mm.
- Is it measurable? If you cannot describe how you would inspect it, neither can the shop.
- Does it stack? Five features each at ±0.05 mm can accumulate to ±0.25 mm across an assembly. Tolerance the assembly, not each part in isolation.
Where we can help
Every quotation we issue includes a manufacturability note that flags tolerances driving cost, and suggests where opening a band would save money without affecting function. If you want that review before you release the drawing, send it over — the review is free and takes about a working day.
