Metal Part Tolerances: A Practical Buyer Guide

Pull a drawing from your archive and look at the title block. There is a good chance it says "ISO 2768-mK" in the corner, and a good chance nobody on the current team can say why "m" was chosen over "f", or whether the "K" still means anything. That inherited block governs every dimension without its own tolerance. On a sheet-metal enclosure or a machined bracket, that can be most of the part. The practical answer to getting tolerances right in metalwork is short. Specify tight limits only where function demands them. Check that the process and the measurement system can repeatedly hold those limits. Let a correctly stated general tolerance cover everything else, and back it with datums so the supplier knows what the numbers are measured from.

The short version

A tolerance is the permitted variation from a nominal dimension. Choose it according to function, fit, material behaviour, manufacturing process, measurement capability and cost, in that order of questioning. Tighter is not automatically better, because every step down in tolerance raises machining, inspection and rejection costs. A tolerance means something in production only when the whole process can achieve it repeatedly and the inspection method can reliably separate good parts from bad.

What does a tolerance mean on a metal part?

A tolerance is the amount a real dimension may differ from its nominal value and still be accepted. It is expressed as limits around the nominal size. The type of tolerance (unilateral, bilateral, fit, geometric or general) tells the supplier which direction the variation may go and which feature it controls.

The vocabulary matters, because suppliers quote against the literal drawing.

• Nominal dimension: the ideal size, for example 40 mm.
• Limit dimensions: the largest and smallest acceptable sizes, for example 40.2 mm and 39.8 mm.
• Bilateral tolerance: variation allowed both ways, equal (40 ±0.2) or unequal (40 +0.3/−0.1).
• Unilateral tolerance: variation allowed in one direction only (40 +0.2/0 or 40 0/−0.2). Use this when a feature must never be smaller, such as a slot that has to accept a fixed-width tab.
• Fits: paired hole and shaft tolerances under ISO 286, such as H7/g6, that define clearance, transition or interference between mating parts.
• Geometric tolerances: controls on form, orientation and location (flatness, perpendicularity, position) under the ISO GPS system, referenced to datums.
• General tolerances: the default block, usually ISO 2768-1, applied to every dimension that carries no explicit tolerance.

Dimensional tolerances say nothing about shape. A 3 mm laser-cut plate can sit inside its length and width limits and still rock on a surface table, and only a flatness callout would reject it. That is why a drawing needs a datum structure and, for anything critical, a stated inspection method, instead of relying on the general block to carry every functional requirement. Our guide to laser cutting and sheet-metal bending tolerances goes further into how this plays out on flat parts.

ISO 2768 general tolerances, and what is changing in 2026

ISO 2768-1:1989 is still the general tolerance standard on most European drawings for linear and angular dimensions. A second edition is approved but, as of September 2026, listed by ISO as under publication. It does not yet replace the 1989 text. ISO 2768-2, the old geometric companion, is withdrawn.

The 1989 standard defines four classes: f (fine), m (medium), c (coarse) and v (very coarse). The permitted deviation widens with size. Take a length between 30 and 120 mm. The standard allows ±0.15 mm in class f, ±0.3 mm in m, ±0.8 mm in c and ±1.5 mm in v. Stretch that to the 120 to 400 mm band and class m opens up to ±0.5 mm. Those numbers are why "m" became the reflex choice. It is loose enough for fabricated work and tight enough that nobody complains.

The revision has a long paper trail. According to the ISO project record, work on the second edition was approved on 4 October 2022. The draft international standard was registered on 18 June 2025, and FDIS registration was approved on 26 January 2026. The status moved to "under publication" on 2 June 2026. The new edition aligns terminology with current GPS practice and limits the scope to linear and angular dimensions. It drops the tolerances for interrupted edges, radii and chamfers, and it removes the rejection rule. It will also apply regardless of material or manufacturing method.

Warning: Do not write "ISO 2768-2 K" on new drawings as though it were a live geometric standard. ISO lists it as withdrawn. If you still need its values for straightness, flatness or perpendicularity, state them explicitly as geometric tolerances or reference the standard contractually, with the edition, so both parties agree what applies.

My recommendation for anyone revising a drawing set this year: keep ISO 2768-1:1989 with the edition year written out, and add explicit tolerances to radii and chamfers that matter. Those features lose their default cover under the new edition, and a year-stamped reference removes the argument about which version governs.

Which tolerances can laser cutting, bending and CNC machining hold?

Each process has a different capability, and a supplier's advertised figure is rarely the tolerance you will get on your part. Laser cutting is limited mainly by kerf, heat input and material flatness. Bending is governed by springback and stack-up across flanges. Machining depends on fixturing, tool wear and temperature. Your part's geometry decides which of these actually matters.

This is where I see buyers get caught by what I call the three-tolerance gap. There is the declared tolerance, meaning the figure on a supplier's website, usually measured on a favourable feature in favourable material. There is the standard tolerance, the class a shop holds routinely without special effort. And there is the guaranteed tolerance: the figure the supplier will commit to for your geometry, your material and your inspection method, after reviewing your drawing. Only the third belongs in a purchase order. Machinists on r/Machinists make the same point from the other side. They are interested in what can be held repeatedly in production, and they distinguish that from what one machine achieved once on a good day.

The last row causes more rejections than the others combined. If a drawing does not state whether a fit applies before or after powder coating, the supplier has to guess. Whichever way they guess, one party ends up unhappy. Our capabilities page sets out the process routes; the achievable tolerance for any given part is confirmed from the drawing and RFQ, never from a generic figure.

What factors change the tolerance a supplier can actually hold?

Material, geometry, thermal effects, fixturing and measurement capability decide whether a tolerance is achievable. The same ±0.05 mm is routine on a short turned steel pin and difficult on a long, thin aluminium plate. Specify with the material and the process in mind, not the machine brochure.

Material behaviour comes first. Aluminium expands roughly twice as much as steel for the same temperature change, so a large aluminium part measured warm from the machine can pass and then fail on the customer's inspection bench. Stainless steel work-hardens and springs back more than mild steel in bending, which makes flange angles harder to hold across a batch. Plate from different heats varies in thickness within its own mill tolerance, and that variation feeds straight into bend dimensions.

Then there is deformation during the process itself. Mitsubishi Electric reported in March 2026 that its CNC digital-twin technology cut errors from workpiece deformation under cutting force by up to half in tests run with RWTH Aachen University. That result says something about where error comes from: the part moves under load, even on a rigid machine. Digital twins link machine data, cutting forces, axis positions and measurements for active compensation. That is still an emerging practice. A NIST workshop summary this year named interoperability, model verification and validation, uncertainty quantification, cybersecurity and workforce preparation as open challenges, so treat active compensation as a promising supplement to good fixturing, not a replacement for it.

Software is rarely the bottleneck anymore. Autodesk lists its Fusion standard plan at US$85 a month or US$680 a year, and cites CIMdata's analysis to claim a 15% share of the global CAM market in 2024, though that is the vendor's own framing of the number. Capable CAM is within reach of small workshops. The tolerance problems I see now start on the drawing, not in the toolpath. Engineers on r/MechanicalEngineering say something similar: time on the shop floor teaches more about tolerances than any software, and they warn that 3D printing is no general substitute for close-tolerance machining.

Worked example: a machined bushing and a bent bracket

Two parts show how a tolerance on paper becomes a clearance, or a failure, in assembly. The first is a 20 mm shaft running in a bushing. The second is a sheet-metal bracket with four bends. The numbers below use published ISO 286 fit values and simple arithmetic.

The shaft and bushing come first. The designer wants a precise running fit and specifies 20 H7/g6. Under ISO 286, the H7 hole is 20.000 to 20.021 mm. The g6 shaft is 19.980 to 19.993 mm. The tightest assembly (smallest hole, largest shaft) leaves 0.007 mm of clearance, and the loosest leaves 0.041 mm. So the whole functional range is 34 microns. A turned diameter of that kind needs a micrometer or plug and ring gauges to verify, and a calliper cannot reliably tell 20.021 from 20.025. If the bushing is later zinc plated without masking, a coating of even 8 to 12 microns per side eats the clearance entirely. A single sentence on the drawing prevents that failure: "fit dimensions apply after plating; mask bore."

The bracket is next. It has four flanges, each dimensioned from the previous bend (chain dimensioning), each at ±0.5 mm. In the worst case, the distance from the first edge to the last flange can be off by ±2.0 mm. That happens even though every individual dimension passes inspection. If the bracket must bolt to a frame with holes at fixed spacing, some parts in the batch will not fit. The remedy costs nothing to specify. Dimension every flange from a single datum edge, so each position carries its own ±0.5 mm and none inherits the others' error. Tightening each dimension to ±0.2 mm would have cost more at the press brake, and it still leaves a worst-case error of ±0.8 mm.

How do you check that a part meets its tolerances?

Verification means measuring the feature the tolerance controls, from the datums the drawing names, with an instrument whose uncertainty is small relative to the tolerance. A common working rule is that measurement uncertainty should consume no more than about a tenth of the tolerance band. Agree the inspection method before production, not at goods-in.

Four terms get confused here, and they are not interchangeable:

• Dimensional accuracy: how close a measured size is to nominal.
• Repeatability: how consistently the process produces the same size across a batch.
• Geometric accuracy: whether form, orientation and position are correct, independent of size.
• Measurement uncertainty: how much doubt the measurement itself carries.

A process can be repeatable and inaccurate, making the same wrong size every time. That is easy to correct. An accurate but unrepeatable process is harder, because each part is a gamble.

The instrument should match the requirement. Callipers suit general fabricated dimensions and micrometers suit turned diameters. Go/no-go gauges are fast for bores and threads in series work. Height gauges on a surface plate handle hole positions and flange heights. Optical systems measure flat laser-cut profiles without contact. Coordinate measuring machines are for positional tolerances, complex datums and first-article reports. If your drawing calls up a position tolerance of 0.1 mm relative to three datums, ask whether the supplier will report it from a CMM. Checking with a calliper from a convenient edge does not measure the same thing.

How do tolerances affect fit, function and cost?

Tolerances decide whether parts assemble, how they wear and what they cost. Each tighter step adds machining time, inspection effort and scrap risk. The right tolerance is the widest one that still guarantees function. Anything tighter costs money and returns nothing.

Over-tolerancing also narrows your supplier base. The wider European picture makes that expensive. Eurostat puts the value of EU industrial production sold at €6,090 billion in 2025, up from €5,869 billion the year before. Inside that total the demand and supply sides diverged. Machinery and equipment output rose 3.3% in real terms, while production of fabricated metal products fell 1.4%. The Eurostat category is broad, so do not read it as a CNC-specific indicator, but the direction is clear. Demand from equipment builders grew while the metalworking base that supplies them shrank. The machine-tool makers saw a similar split. Spain's AFM reported that metal-cutting machine-tool turnover grew 1.56% in 2025, while metal-forming turnover fell by almost 12%.

The monthly figures are no steadier. The same statistics office recorded total EU market production in December 2025 up 1.2% year on year, yet industrial production down 0.8% from November. When capacity is uncertain, you will more often find yourself quoting with suppliers who have never seen your parts before. A drawing full of unnecessary ±0.02 mm callouts gets no-quoted, or quoted with a risk premium, by exactly the shops you most want to compare. A drawing that separates critical from general features gets quotes you can compare line by line.

A drawing checklist before you send an RFQ

As a build-to-print metal manufacturer, we see the same omissions again and again. Most tolerance disputes trace back to one of these items missing from the drawing:

1. Units stated, metric throughout.
2. Nominal values on every functional dimension.
3. Plus/minus or limit values on critical features. Use unilateral tolerances where a feature must never go undersize or oversize.
4. The general tolerance block with the edition year (ISO 2768-1:1989, class stated).
5. Datums identified, with critical dimensions referenced to them rather than chained.
6. Geometric tolerances (flatness, perpendicularity, position) only where function needs them.
7. Surface finish requirements on functional faces.
8. Material and grade, plus heat treatment if any.
9. Coating or finish, and whether dimensions apply before or after it; masking of threads and fits.
10. Weld requirements and which dimensions apply after welding.
11. Inspection and documentation expected: first-article report, CMM data, material certificates.
12. Drawing revision, quantity, delivery destination and required date.

When we review drawings for Build-to-print metal parts and assemblies, the first conversation is usually about items 5 and 9, because those decide whether a tolerance can be held and proven. See our page on parts made to technical drawings for how that review fits into quoting.

Bottom line

Tolerance only what matters, and dimension it from datums. Keep ISO 2768-1:1989 with its year until the new edition is formally published and your contracts reference it. Ask each supplier for the tolerance they will guarantee on your part, not the one they advertise. For a quotation, send a STEP file as the authoritative 3D model. Add a separate, dimensioned PDF drawing covering critical dimensions and tolerances, material and grade, threads, weld requirements, finish or coating, inspection and documentation needs, quantities, drawing revision, delivery destination and required date. Feasibility and delivery dates are confirmed from that drawing and the RFQ.

Frequently asked questions

What does tolerance mean in metal machining?

A tolerance is the permitted variation from a nominal dimension, stated as limits the finished feature must fall within. For example, 40 ±0.2 mm accepts anything from 39.8 to 40.2 mm. Tolerances can control size (dimensional), shape and position (geometric), or the fit between mating parts. Features without an explicit tolerance usually fall under a general tolerance block such as ISO 2768-1.

What is the difference between unilateral and bilateral tolerances?

A bilateral tolerance allows variation in both directions from nominal, such as 25 ±0.1 or 25 +0.2/−0.1. A unilateral tolerance allows variation in one direction only, such as 25 +0.2/0. Use unilateral tolerances when a feature must never be undersize or oversize, for instance a slot that must always accept a mating tab or a pin that must always enter a hole.

Is ISO 2768-1 still valid in 2026?

Yes. ISO 2768-1:1989 remains the reference on most drawings. A second edition was listed by ISO as under publication from 2 June 2026, so it has not formally replaced the 1989 text. ISO 2768-2 is withdrawn. Write the edition year on drawings so supplier and buyer agree which version applies.

What tolerances are usual for sintered metal gears?

Gear accuracy is normally specified through gear quality grades, for example under ISO 1328, not simple plus/minus sizes. Achievable grades for sintered gears depend on the powder, compaction, sintering shrinkage and whether a sizing or machining operation follows. Ask the sintering supplier for the grade they guarantee for your module and diameter, and specify machining for bores or faces that need tighter control.

How do I check whether a part meets its tolerances?

Measure each controlled feature from the datums named on the drawing, using an instrument whose uncertainty is small relative to the tolerance. Callipers suit general dimensions and micrometers and gauges suit turned diameters and bores. Height gauges and CMMs handle positional and geometric tolerances. Agree the inspection method and report format with the supplier before production starts.

Why does a tighter tolerance cost more?

Tighter tolerances need slower machining, more careful fixturing, more frequent measurement and better instruments, and they raise the scrap rate. They can also push a part onto a different process, such as grinding after turning. Specify the widest tolerance that still guarantees function, and reserve tight limits for fits, sealing faces and locating features.

Related Reading

• Prelucrarea metalelor de la debitare la finisare: servicii integrate pentru industrie
• 7 criterii pentru alegerea serviciilor de îndoire tablă la comandă
• How Do Laser Cutting Services Support Prototypes and Repeat Series?
• Costuri excesive la îndoirea tablei? Soluții pentru reducerea prețului
• Producători români de piese din tablă pentru proiecte industriale
• Preț debitare laser tablă: factori care influențează oferta finală
• Ghid pentru alegerea debitării laser industriale în proiecte complexe
• Top 8 instrumente pentru proiectare și prelucrare metalică precisă
• Debitare laser metal | Piese la comanda | HABA Research
• Indoire tabla CNC | Piese metalice la comanda | HABA

Build-to-print metal parts and assemblies

Explore Build-to-print metal parts and assemblies