Stainless Machining Tolerances: What a Shop Really Holds in Production

Process / 19 Sept 2026

Machine tool brochures quote positioning accuracy. Shops quote what they hold in production, on your material, with inspection to prove it. Those are different numbers and the gap is where disappointed first articles live.

Here is a realistic picture for machined stainless, and what each band costs.

The bands

For austenitic stainless such as SUS304 and SUS316L, on a part of moderate size in a competent shop:

Tolerance	What it means	Cost
±0.2 mm and looser	General tolerance territory, medium class	Baseline, free
±0.1 mm	Comfortable	Free on most features
±0.05 mm	Standard precision. Careful setup, fresh tooling	Small increase
±0.02 mm	Precision. Dedicated finishing pass, measured inspection	Noticeable. Maybe a separate operation
±0.01 mm	Tight. Grinding or very rigid hard turning, controlled inspection	Significant. Separate operation and fixturing
Under ±0.005 mm	Grinding, lapping, temperature controlled room	Specialist. Expect a long first article

Two observations. The step from ±0.05 to ±0.02 is the first real cost step, because it is where an extra finishing operation and measured inspection enter. The step from ±0.02 to ±0.01 is the expensive one, because it is where grinding enters.

ISO fits in actual numbers

Drawings often use fit designations rather than plus and minus values, and it is worth seeing what they mean in micrometres. For a shaft:

Nominal	h6	h7	h8	g6	f7
10 mm	0 / -9	0 / -15	0 / -22	-5 / -14	-13 / -28
20 mm	0 / -13	0 / -21	0 / -33	-7 / -20	-20 / -41
30 mm	0 / -13	0 / -21	0 / -33	-7 / -20	-20 / -41
50 mm	0 / -16	0 / -25	0 / -39	-9 / -25	-25 / -50
100 mm	0 / -22	0 / -35	0 / -54	-12 / -34	-36 / -71

So h7 on a 20 mm shaft is a 21 micrometre band. That is comfortable turning on a rigid machine with a fresh insert. h6 on the same shaft is 13 micrometres, and that is where shops start reaching for the grinder on stainless, particularly on anything over 30 mm or on a part that has been heat treated.

For holes, H7 on 20 mm is +21 / 0. Reamed or bored, both achievable. H6 usually means a honed or ground bore.

Why stainless is harder than the same tolerance in aluminium

Cutting forces are high. Roughly two to three times those in aluminium for a comparable cut. High force means deflection, in the tool, the part and the fixture. Deflection is a dimensional error that varies through the cut.

The part grows while it is cut. SUS304 conducts at about 16 W per metre kelvin and expands at about 17 µm per metre per kelvin. A 100 mm dimension that rises 20 degC during machining grows about 34 micrometres. That is larger than an h7 band. A part measured warm and shipped cold is a part that fails incoming inspection.

Tool wear is faster and less predictable. An insert that has drifted 15 micrometres through a batch has moved the dimension by that much. Shops running tight tolerances on stainless change tooling on a count, not on failure, and often measure the first and last part of every batch.

Work hardening varies the effective depth of cut. Covered in more detail in work hardening in stainless machining.

What separates a shop that holds ±0.02 from one that does not

Worth asking about directly:

Temperature. Is the shop floor temperature controlled, and is inspection done on a settled part? A shop that measures parts straight off the machine is not holding 20 micrometres reliably, whatever it says
Inspection equipment on site. A CMM, and someone qualified to run it. Subcontracted inspection means a feedback loop measured in days
Tool management. Inserts changed on a schedule, offsets updated systematically
In process measurement. First off, then a sampling plan, not just a final check
Workholding. A part clamped hard enough to distort measures differently clamped and free. On thin or ring shaped parts this is the usual cause of a dispute

How to specify so you get what you need

Tolerance the function, not the feature. The three diameters that locate something need a tolerance. The overall length usually does not. A drawing where every dimension carries ±0.02 mm gets priced as if every dimension mattered.

Use the general tolerance class deliberately. Set it to medium, then tolerance the handful of features that need better. That is almost always cheaper than lifting the general class. The values are in the general tolerance guide.

Say how it is inspected. A dimension checked with a micrometer and one checked on a CMM are different costs. If you need a CMM report, ask for it explicitly on the features that need it.

Say whether the part is measured free or clamped. On thin, long or ring shaped parts this changes the answer. Specify the condition.

Give a temperature reference if the tolerance is tight. The standard reference is 20 degC. Stating it on a drawing with micrometre level tolerances is normal practice and prevents an argument.

Be honest about which features are safety or fit critical. A shop that knows which three dimensions matter will protect those three. A shop looking at forty equally toleranced dimensions will protect none of them in particular.

A worked example

A turned stainless spindle, 20 mm diameter, 120 mm long, two bearing journals.

Specified badly:

All dimensions ±0.02
Ra 0.8 all over
General tolerance JIS B 0405-f

Everything is tight, so everything gets a finishing pass and measured inspection, and the general class adds a further constraint on top.

Specified well:

General tolerances JIS B 0405-m, geometrical JIS B 0419-K
Bearing journals: 20 h6, Ra 0.4, concentric within 0.01 TIR
All other surfaces: Ra 3.2
Measure journals at 20 degC, free standing

The shop now knows there are two critical features, grinds or hard turns those, and runs the rest normally. Same part, considerably less money, and the features that matter are better controlled than they were in the first version.

Have a drawing where you are not sure which tolerances are driving the price? Get a quote. The quote names the features that drive the price, so you can loosen the ones that do not matter. Within 24 business hours.

Questions

What tolerance is normal on a machined stainless part?

Plus or minus 0.05 mm is comfortable production work on most features. Plus or minus 0.02 mm is achievable with care and inspection. Below plus or minus 0.01 mm normally means grinding, temperature controlled inspection, or both.

Can a shop hold h7 without grinding?

Usually yes up to around 30 mm diameter on a rigid turning centre with a fresh tool. Above that, and on any part that has been through heat treatment, plan on grinding.

Why is stainless harder to hold tolerance on than aluminium?

Higher cutting forces mean more deflection, low thermal conductivity means the part grows in the cut, and work hardening means tool wear is faster and less predictable. All three move the dimension.

Does the tolerance have to be the same on every feature?

No, and it should not be. Tolerance the features that carry function and let everything else run on the general tolerance class. That is the cheapest change available on most drawings.

Have a drawing for a stainless part?

Send it and an engineer reads the title block, quotes it within 24 business hours, and if you order we place, manage, inspect and ship the parts on one PO and one invoice.

Get a quote