Guides / Process

Swiss Machining Tolerances: Typical Ranges and What They Cost

September 20, 2026

Most disagreements about a Swiss machined part start with a tolerance that nobody discussed. The drawing says ±0.005 mm, the quote comes back high, the buyer assumes the shop is padding and the shop assumes the buyer measured nothing. Both are usually wrong.

This guide gives typical tolerance ranges on Swiss-type lathes, explains what makes each one harder or easier and shows how to tolerance a drawing so the price reflects what your part actually needs.

Why Swiss machines hold tight diameters

Three things in the machine design work in your favor.

The guide bushing supports the bar within a few millimeters of the cutting edge, so the part cannot deflect away from the tool the way a long overhang does on a conventional lathe. Deflection is the usual reason a slender part tapers.

Everything on the front end is cut in one chucking. The part never comes out and goes back in, so diameters turned in the same cycle sit on the same axis by construction, not by careful re-clamping.

The machines are built small and stiff for small parts. Spindle runout, slide resolution and thermal behavior are all scaled to work where a few microns matter.

That is why a 3 mm pin can hold its diameter end to end. It is also why the tolerance question is really about which feature, over what length, in what material.

Typical ranges

The numbers below are typical of production work on modern Swiss-type lathes, in free machining materials, on features of modest length. Treat them as a starting point for conversation, not a promise from any shop.

Feature	Typical production tolerance	Notes
Turned diameter, short length	±0.005 to ±0.013 mm	Tightest on the machine. Free machining grades
Turned diameter, long length	±0.013 to ±0.025 mm	Widens as L/D grows
Length and shoulder position	±0.025 to ±0.05 mm	Cut off and back end pickup add variation
Drilled hole diameter	±0.025 to ±0.05 mm	Reaming or boring tightens it
Concentricity, same chucking	0.005 to 0.013 mm TIR	Nearly free, cut on one axis
Concentricity, front to back	0.013 to 0.05 mm TIR	Depends on sub spindle pickup
Cross hole position	±0.05 mm	Indexing plus drill wander
Turned surface finish	Ra 0.8 to 1.6 µm	Normal parameters, no extra step
Fine surface finish	Ra 0.4 µm and below	Slower passes, more tool changes

Ask any shop for its own numbers on your specific material and geometry. A shop that answers with a single figure for every case has not thought about your part.

What makes a tolerance harder

Length of the toleranced feature

A diameter held over 3 mm of length and the same diameter held over 40 mm are different jobs. Over the longer length the tool cuts for longer, heat builds and the insert wears measurably within the pass. Always show where on the length a tight diameter applies, using a dimension with limits at a stated position rather than a blanket callout.

Material

Free machining grades such as 303 stainless, C360 brass and 2011 aluminum cut cleanly, break chips and let the machine settle into a stable process. Gummy or work hardening grades behave differently. 316L tears rather than shears, titanium springs back elastically after the tool passes, 17-4 PH is hard enough to wear tooling faster. On these, expect the achievable tolerance to widen or the price to rise, sometimes both. The materials guide goes through the grades one by one.

Wall thickness and section

Thin walls flex. A tube with a 0.4 mm wall can measure in tolerance on the machine and out of tolerance on the bench, because the gauge itself deflects it or because stress relaxed after cut off. If your part has a thin section, say what the measurement method should be.

Front to back relationships

Any tolerance that ties a front end feature to a back end feature depends on how cleanly the sub spindle picked the part up. This is the most common place where a drawing asks for more than the process gives naturally. It is achievable, but it is a deliberate choice that shows in the quote.

Heat treatment and plating

Parts move during heat treatment and grow under plating. A 17-4 PH part hardened after machining will not hold a machined tolerance unless the shop machined it with that movement predicted. A plated diameter grows by the plating thickness, which is often the same order as the tolerance. State whether the dimension applies before or after these steps. Missing this is one of the most common causes of a rejected first article. See secondary operations for how these steps fit into the job.

Tolerance stacks on assemblies

A part that passes every callout on its own drawing can still fail in the assembly. This happens when several tolerances add up in the same direction.

A typical case: a pin with a shoulder locates against a housing face, and a retaining groove sits a nominal distance from that shoulder. The shoulder position carries a tolerance, the groove position carries a tolerance and the housing carries its own. In the worst case all three land at the same extreme, and the retaining ring no longer seats.

Two habits prevent most of this:

Dimension from the datum that matters. If the groove position is functionally measured from the shoulder, dimension it from the shoulder rather than chaining it through two other features. Every intermediate dimension in a chain adds its tolerance to the result.

Decide where the slack lives. Somewhere in an assembly there has to be a feature that absorbs variation. Choose it deliberately and give it the loose tolerance, rather than tightening every feature and hoping.

On Swiss parts this matters more than on larger components, because the absolute tolerances are small and a stack of three or four is easy to build accidentally in CAD.

What tight tolerances cost

Tightening a callout adds cost in four places.

Cycle time. A tight diameter needs a separate finishing pass at lower feed. That pass is seconds, and seconds repeat across every part in the order.

Tooling. Sharper inserts, changed sooner. An insert that would run 800 parts at a loose tolerance may get replaced at 300 to keep a tight one in band.

Gauging during the run. Someone measures parts at intervals and adjusts tool offsets as the insert wears. Tighter bands mean shorter intervals and more adjustments.

Inspection and scrap. Final inspection samples more parts, and parts that drift out of band become scrap rather than usable stock.

None of that is padding. It is why a part with one tight feature and a sensible general block quotes well below the same part toleranced tightly everywhere, even though both are the same shape.

How to tolerance a Swiss part drawing

1. Find the features that control function. Usually two or three: a bearing fit, a sealing diameter, a thread fit, a critical length.
2. Tolerance those properly, with limits and a stated length. This is where effort should go.
3. Put everything else in a general block. A standard such as ISO 2768 medium, or your own block, covers the rest without argument.
4. State datums where relationships matter. If a runout matters relative to a specific diameter, say which one.
5. Say when each dimension applies. Before or after heat treatment. Before or after plating or passivation.
6. Name the measurement method for anything unusual. Thin sections, soft materials and deep bores can measure differently on different equipment.
7. Add a note on what you will inspect. If you plan to check three dimensions on receipt, the shop knows where its report must be solid.

Ask this question in your RFQ

A useful sentence to include with any Swiss RFQ: which callouts on this drawing drive the price, and what would you relax first?

A shop that runs Swiss machines every day will answer it concretely. You get a list of the two or three items that matter, and often a suggestion you can accept without changing how the part works. It costs you nothing and it tells you a lot about who you are dealing with.

Verifying what you receive

Tolerances only mean something if somebody measures them. Agree before the first order on what the first article report covers, how often production is sampled and whether you want measurement data with each lot. A first article that checks every dimension once tells you the process can make the part. In-process data tells you it keeps making it. Both belong in the conversation, and the guide to inspection and quality covers how shops handle them.

Getting a quote you can trust

Send the STEP file and a drawing that marks its critical features clearly through the RFQ form. Tell us the material, the largest diameter, the yearly volume and which tolerances are functional. We match the part with up to three shops that run Swiss-type lathes and reply within 24 business hours. If a callout on your drawing is the reason every quote comes back high, you will hear that too.

Before you finalize the print, the guide to design for Swiss machining covers the geometry choices that sit alongside these tolerance decisions.

Frequently asked questions

Keep reading

• Design for Swiss Machining: Drawing Choices That Move the Price
• Guide Bushing vs Guide Bushing-Less Swiss Turning