ISO 2768 Tolerances: Classes, Tables and How to Call Them Out

ISO 2768 is the international standard for general tolerances: the default limits that apply to any dimension on your drawing that has no tolerance of its own. Part 1 covers linear and angular dimensions. Part 2 covers geometry such as flatness, straightness and run-out. You pick one class from each part, write it in the title block (for example ISO 2768-mK), and the shop knows how far every untoleranced feature may wander.

This guide gives you the class tables, a worked example, the drawing note, the limits of the standard and the mistakes that cause rejected parts.

Key takeaways

• ISO 2768-1 has four linear and angular classes: f (fine), m (medium), c (coarse) and v (very coarse). ISO 2768-2 has three geometric classes: H, K and L.
• A callout like ISO 2768-mK means class m for size and class K for geometry. Any dimension with its own tolerance overrides the general note.
• General tolerances are for non-critical features. Fits, seals, bearing seats and datum-related features need individual tolerances.
• The standard is voluntary. It binds you and your supplier only when your drawing or contract invokes it.
• ISO 2768-1:1989 is being replaced by a new edition of ISO 2768. Check the current text before you cite it in a new drawing template.

Table of Contents

• What ISO 2768 covers
• ISO 2768-1 linear tolerances by class
• ISO 2768-2: classes H, K and L
• Reading a callout: what ISO 2768-mK means
• What ISO 2768 does not cover
• When to use individual tolerances instead
• Choosing a class for your process
• ISO 2768 in US production: ASME Y14.5, contracts and GB/T
• Status of the standard
• Perspective: why we ask about the general note first
• Get your drawing checked and quoted
• Common mistakes with ISO 2768
• FAQ
• Sources

What ISO 2768 covers

The standard exists to simplify drawings. ISO 2768-1:1989 gives general tolerances for linear and angular dimensions without individual tolerance indications, so the drawing does not need a plus-minus value on every edge and hole. The standard’s own text says it applies to parts made by metal removal or formed from sheet metal. It is not written for plastics, castings or additive parts, although many buyers apply it to them by contract.

The two parts split the work:

• Part 1: linear dimensions, external radii and chamfer heights, and angular dimensions.
• Part 2: general tolerances for form and position, covering straightness, flatness, perpendicularity, symmetry and run-out, in classes H, K and L.

The idea behind both is that a drawing should be complete. The standard states that nothing should be left to workshop or inspection judgment, and general tolerances are the shortcut that makes this practical.

ISO 2768-1 linear tolerances by class

The permitted deviation is bilateral (plus and minus) and grows with two things: the nominal size range and the coarseness of the class. According to the standard, the 6 to 30 mm range is ±0.10, ±0.20, ±0.50 and ±1.00 mm for f, m, c and v, while 1000 to 2000 mm is ±0.50, ±1.20, ±3.00 and ±6.00 mm. Class f is not defined above 2000 mm, and class v is not defined from 0.5 to 3 mm.

The full set of linear limits, in millimeters:

The extremes run from ±0.05 mm (class f, smallest range) to ±8 mm (class v, 2000 to 4000 mm).

External radii and chamfer heights

The same part has a short table for broken edges. For classes f and m the limit is ±0.2 mm up to 3 mm, ±0.5 mm over 3 to 6 mm and ±1 mm above 6 mm. Classes c and v allow ±0.4 mm, ±1 mm and ±2 mm in the same ranges. These apply to external radii and chamfer heights, not to internal radii you have dimensioned elsewhere.

Angular dimensions

Angular limits depend on the length of the shorter leg of the angle, not on the angle itself. For classes f and m the tolerance is ±1° up to 10 mm, ±0°30′ from 10 to 50 mm, ±0°20′ from 50 to 120 mm, ±0°10′ from 120 to 400 mm and ±0°5′ above 400 mm. Classes c and v are looser, starting at ±1°30′ and ±3° respectively for the shortest legs.

ISO 2768-2: classes H, K and L

Part 2 limits form and position when the drawing has no geometric tolerance of its own. It is shorter than Part 1 because it gives one zone value per size range, not a deviation around a nominal.

Straightness and flatness, by length of the shorter side or the feature, in millimeters:

For circular run-out, the standard gives a single value per class: 0.1 mm for H, 0.2 mm for K and 0.5 mm for L. Perpendicularity, symmetry and the rest follow the same logic, and you should read them directly from ISO 2768-2 before you rely on them.

Reading a callout: what ISO 2768-mK means

The designation is the standard number followed by one letter from each part. In ISO 2768-mK:

1. m is the Part 1 class, so a 50 mm dimension with no tolerance may vary by ±0.3 mm.
2. K is the Part 2 class, so a 50 mm long face with no flatness callout must sit within a 0.2 mm zone.

You can also cite one part only, such as ISO 2768-m, when you do not need to control geometry by default. Supplier documentation typically shows the note in or near the title block, worded like “GENERAL TOLERANCE ISO 2768-m”, and dimensions carrying their own tolerance take precedence.

A worked example

Take a machined aluminum bracket, 80 mm long, with a 25 mm wide pocket, a 10 mm boss height and one 4 mm chamfer, drawn with the note ISO 2768-mK.

• The 80 mm length falls in the 30 to 120 range: ±0.3 mm.
• The 25 mm pocket width is in the 6 to 30 range: ±0.2 mm.
• The 10 mm boss height is also 6 to 30: ±0.2 mm.
• The 4 mm chamfer height is 3 to 6 mm: ±0.5 mm.
• The 80 mm top face has no flatness callout, so class K gives a 0.2 mm zone (30 to 100 range).

Now suppose a dowel pin must press into a 6 mm hole. A ±0.2 mm general tolerance is useless there. That hole needs its own fit tolerance, which is exactly the point of the next section.

What ISO 2768 does not cover

General tolerances are a default, not a design tool. Know the exclusions:

• Auxiliary and basic dimensions. The standard does not apply to auxiliary dimensions in brackets or theoretically exact dimensions in rectangular frames.
• Functional features. Supplier guidance commonly separates the two: important functional dimensions are toleranced individually, while dimensions that do not need high precision can use the general note.
• Process-specific limits. Molded, cast and printed parts have their own shrinkage and warpage behavior. For molded parts, see what you can realistically specify in injection molding.

There is a useful nuance in the standard itself. Exceeding a general tolerance does not automatically mean rejection if the function of the part is not impaired. Do not rely on that as a quality plan. A supplier working to your drawing will usually measure to the written limit, so write the limit you actually need.

When to use individual tolerances instead

Use an individual tolerance, or a geometric tolerance per your drawing standard, for:

• Mating features: shafts, bores, slots and tabs that must assemble.
• Sealing faces, bearing seats and press fits.
• Any feature referenced as a datum.
• Dimensions where the general class is looser than your function allows.
• Dimensions where the class is far tighter than you need, since tighter limits on every feature add machining time and inspection effort.

A practical rule: tolerate what matters tightly, and let ISO 2768-m cover the rest. If your assembly fails only when you tighten the whole drawing to class f, you probably have three or four critical features that should have been called out one by one.

Choosing a class for your process

These are starting points for discussion, not guarantees from any shop. Confirm with your supplier what a given class means for your material, thickness and feature type. Our guides on tolerance in machining and explaining tolerance in manufacturing cover the basics behind these choices.

ISO 2768 in US production: ASME Y14.5, contracts and GB/T

US drawings are typically built on ASME Y14.5. NIST notes that a tolerance is formally defined by ANSI Standard Y14.5 on dimensioning and tolerancing. ISO 2768 is an ISO standard and sits alongside it, so mixing the two on one drawing needs care: state which standard governs, and avoid applying a Y14.5 title block tolerance table and an ISO 2768 note at once.

Is ISO 2768 legally required in the United States? No. ASME explains that standards are voluntary unless a contract or regulation incorporates them. That means the note on your drawing, or a clause in your purchase order, is what makes ISO 2768 binding.

If you source from China, the common issue is that suppliers there may default to the Chinese general tolerance standard (GB/T 1804) when a drawing is silent or ambiguous. We cover that mapping in our ISO 2768 to GB/T crosswalk, and the specific risk on bent parts in managing ISO 2768 coarse risk in sheet metal sourcing.

Status of the standard

ISO 2768-1:1989 was last reviewed and confirmed in 2022, and ISO lists it as due to be replaced by a new ISO 2768. The second-edition ISO 2768, a geometrical product specification (GPS) document, is under publication. Tables you find in older PDFs match the 1989 text. If you adopt the new edition in a template, say which edition the note refers to, because tolerance classes and designations may differ between editions.

Perspective: why we ask about the general note first

When a drawing reaches us, the title block is the first thing our engineers read. In our experience, most tolerance disputes do not come from a machine that cannot hold a limit. They come from a drawing where the buyer and the shop assumed different defaults. A buyer pictures class f, the shop reads class m, and nobody notices until parts are measured.

Our advice is simple. Write the class on the drawing, tighten only the features that carry function, and talk to your project manager about anything that looks unusual before you release the order. We would rather question a note at the quoting stage than discover a mismatch at inspection. Prototypes especially benefit, since a first article is where you learn which “general” features turned out to be critical.

— Nas

Get your drawing checked and quoted

If you have a drawing with an ISO 2768 note and want to know how it will be read in production, upload it for a quote. We manufacture machined parts through our CNC machining service and bent or cut parts through sheet metal fabrication, with no minimum order quantity, ISO-certified production and a dedicated project manager who reviews your tolerances with you.

Common mistakes with ISO 2768

1. No class stated. A drawing that says “general tolerances apply” without a class leaves the default to the supplier.
2. Citing only the number. “ISO 2768” with no letters is incomplete. Add m, mK or the class you mean.
3. Assuming f is free. Fine classes cost more in machine time and inspection on every untoleranced feature.
4. Ignoring bends. On sheet metal, formed dimensions stack up bend by bend, and a single class for the whole part may not suit them.
5. Mixing standards. Combining ASME Y14.5 and ISO 2768 without saying which governs invites arguments.
6. Using it on the wrong process. The standard is written for metal removal and sheet metal forming, not for molded or printed parts.

FAQ

What is the difference between ISO 2768-m and ISO 2768-mK?

ISO 2768-m sets only the Part 1 class, which controls linear and angular dimensions. ISO 2768-mK adds Part 2 class K, which also controls form and position such as flatness and straightness. Use the longer form when geometry matters and you do not want to dimension every face.

Which ISO 2768 class is the default for machining?

There is no official default in the standard; you choose the class. Class m is the most common choice on machined drawings, with K or H added for geometry where needed. Ask your supplier what they can hold economically for your material and part size.

Does ISO 2768 apply to 3D printed or injection molded parts?

The standard’s scope is parts made by metal removal or formed from sheet metal, so it is not a natural fit for printed or molded parts. Many buyers still reference it by contract, but you should agree process-specific limits with the supplier. Molding has its own guidance, linked above.

Is ISO 2768 mandatory in the US?

No. Standards are voluntary unless a contract or regulation incorporates them. The note on your drawing or a purchase order clause is what makes it apply.

Can a part be rejected for exceeding a general tolerance?

The standard says exceeding a general tolerance does not automatically cause rejection if the function is not impaired. In practice, many buyers inspect to the written limit anyway. If a feature matters, give it an individual tolerance.

Sources

• ISO 2768-1:1989 general tolerances, standard page
• ISO 2768-1:1989 online browsing platform text
• ISO 2768-2:1989 online browsing platform text
• ISO 2768 second edition, standard page
• ISO 2768-1 text, Eurotools PDF
• General tolerances for linear and angular dimensions, supplier guidance
• NIST report on dimensional metrology challenges
• ASME standards and certification FAQ

Recommended

• Avoid a Rejected Batch Three Weeks Later: ISO 2768 to GB/T Crosswalk
• Explaining Tolerance in Manufacturing: Engineer’s Guide
• Injection Molding Tolerances: What You Can Specify
• What Is Tolerance in Machining: A Practical Guide