How Tight a Tolerance Does Your Stainless Part Need?

September 21, 2026

Tolerance is the dimension of a quote that buyers control most directly and use least carefully. On stainless it costs more than on most materials, for reasons that are worth understanding before you fix the numbers.

The bands, and what each one means in the shop

These are general figures for a typical machined feature in a common austenitic grade. Small features are easier, large ones are harder, and any specific part can differ.

Tolerance	What it takes	Relative cost
±0.25 mm	Falls out of normal machining	Baseline
±0.1 mm	Standard practice, no special effort	Baseline
±0.05 mm	Routine, a little care on setup	Slightly above
±0.02 mm	Dedicated finishing pass, fresh tooling, controlled setup	Noticeably above
±0.01 mm	Process control, thermal settling, dedicated inspection	Substantially above
Below ±0.01 mm	Grinding, honing or lapping, often a second supplier	Different conversation

The steps are not linear. Going from ±0.1 to ±0.05 mm costs little. Going from ±0.02 to ±0.01 mm can double the price of a feature, because it moves the part from being machined to being controlled.

Why stainless is harder than the same feature in aluminium

Heat stays in the part. Stainless conducts heat roughly a third as well as carbon steel and far worse than aluminium. The part grows while it is being cut, so a dimension measured hot is not the dimension you get cold. On a tight feature the shop has to let the part settle before final measurement, and settling is time.

Work hardening changes the cut. A finishing pass on a hardened surface removes a different amount than the same pass on fresh material. See work hardening.

Residual stress releases. Bar and plate arrive with stress from the mill. Remove material asymmetrically and the part moves. On a thin or asymmetric part this alone can exceed a tight tolerance, and the fix is rough, stress relieve, then finish, which is two setups and a furnace cycle.

Ageing and welding move parts further. 17-4 PH shrinks when aged and weldments move by millimetres. Any tolerance applied before those operations is not the tolerance you get.

Measurement itself gets harder. At ±0.01 mm the measurement has to happen at a controlled temperature, because stainless expands about 16 micrometres per metre per degree. A 200 mm part measured 3 degrees warm reads about 10 micrometres long.

Where the money actually goes

A tight tolerance buys you four things you are paying for whether you wanted them or not:

1. An extra operation. Roughing and finishing separated, sometimes with a settling period between.
2. Fresh tooling. A tight feature gets a new insert, and the cost of that insert lands on your batch.
3. Inspection. CMM time, a temperature controlled room and a report. On a small batch this can be a large share of the unit price.
4. Scrap risk, priced in. If one part in twenty misses, the other nineteen carry it.

Spend the tolerance where it does something

The discipline is simple and it is rarely applied.

Identify the features that mate with something. Bores that take a bearing, faces that seal, spigots that locate. Those get tight tolerances.

Everything else gets the general note. Overall length, cosmetic steps, clearance holes, the outside of a housing. These do not need to be controlled and often nobody ever measures them.

On a typical part this is the difference between four tight dimensions and forty. Shops see drawings with a ±0.02 mm title block note every week, and the resulting quote reflects it.

Use GD&T where it actually describes the requirement. Position, concentricity and flatness often express a functional need more cheaply than a stack of tight linear dimensions, because they allow the shop to hold the relationship rather than every absolute. A true position callout with a material condition modifier gives back tolerance as the feature moves away from its worst case size.

Do not stack tolerances by accident. Three dimensions in a chain, each at ±0.05 mm, give a worst case of ±0.15 mm across the chain. Dimension from a common datum instead and the chain disappears.

A note on fits

If a bore takes a bearing, specify the fit rather than inventing numbers. H7 on a bore and h6 or k6 on a shaft are standard, understood everywhere and already sized against the function. A shop reading H7 knows exactly what to do. A shop reading 25.00 to 25.02 has to guess whether that was intended as H7 or whether there is a reason for the difference.

What to put on the drawing

1. A sensible general tolerance, typically ±0.1 mm on linear dimensions, or a standard such as ISO 2768-m
2. Tight tolerances only on features that mate, marked individually
3. Standard fits where a standard fit is what you mean
4. GD&T where it describes the function better than a linear tolerance
5. A datum scheme that reflects how the part is used and that survives later operations
6. Whether inspection is required, on which features, and whether a report is needed

That last point is worth stating explicitly. A full dimensional report on a 40 dimension part is hours of work. A report on the six critical features is a fraction of that and tells you the same thing. The RFQ checklist covers where this sits alongside material and finish, and what drives the cost puts tolerance next to the other levers.

Frequently asked questions

Figures in this guide are published specification limits or published typical values for the alloy, not measurements of any part. Machinability is rated against free-machining carbon steel B1112 at 100 and PREN is chromium plus 3.3 times molybdenum plus 16 times nitrogen. The conventions are set out in thereference section and the editorial standards.

Keep reading

• Why Five Stainless Parts Cost Nearly as Much as Fifty
• Where the Money Goes in a Stainless Machining Quote