CNC Machining Tolerances: ISO 2768, ISO 286 and GD&T

CNC machining tolerances are the permitted deviations from the nominal values on a drawing. Three systems set them: ISO 2768 general tolerances for every dimension without a tolerance of its own, ISO 286 tolerance classes and fits for sizes that must mate, and geometrical tolerances to ISO 1101 or ASME Y14.5 (GD&T) for form, orientation and location.

What are CNC machining tolerances?

Every machined feature has a size and a geometry. A drawing controls them in layers, from the loosest layer that still works to the tightest, and each layer has its own standard.

Table 1. Tolerance layers on a machined part

Source: ISO catalogue entries listed under Sources; ASME Y14.5-2018 (R2024).

A tighter layer costs more to produce and to inspect, so each layer is applied only where a feature's function needs it.

What does ISO 2768 allow when a drawing says nothing else?

ISO 2768-1:1989 defines four classes, f (fine), m (medium), c (coarse) and v (very coarse), for workpieces made by metal removal or formed from sheet metal. The note "ISO 2768-m" in the title block applies class m to every linear and angular dimension that has no tolerance written next to it.

Table 2. Permissible deviations for linear dimensions, ISO 2768-1, mm

Source: ISO 2768-1:1989, Table 1. Below 0.5 mm the deviation is written next to the dimension.

A 25 mm diameter without its own tolerance, on a drawing marked class m, may therefore measure anywhere from 24.8 mm to 25.2 mm. The standard also gives separate tables for external radii, chamfer heights and angles; they are in the ISO 2768 tolerance tables.

General tolerances suit features where nothing depends on the exact size. They do not suit a bearing seat or a sealing face.

How do ISO 286 IT grades and fits work?

ISO 286-1:2010 defines 20 standard tolerance grades, IT01 to IT18, and ISO 286-2:2010 tabulates the limit deviations for the tolerance classes built from them. A grade fixes the width of the tolerance zone for a size range. A letter fixes its position relative to the nominal size: capital letters for holes, lower case for shafts. H means the zone starts at the nominal size and runs upward, so a Ø25 H7 bore measures 25.000 mm to 25.021 mm.

Table 3. Standard tolerance grades IT6 to IT11 in µm, ISO 286-1

Source: ISO 286-1:2010, Table 1 (values as reproduced on Wikipedia).

A fit pairs a hole class with a shaft class. For Ø25 H7/g6 the hole measures 25.000 mm to 25.021 mm. The shaft class g6 sits 7 µm below nominal and is 13 µm wide (IT6 for 18 to 30 mm), so the shaft measures 24.980 mm to 24.993 mm. The clearance is then 0.007 mm at minimum and 0.041 mm at maximum. H7/g6 is one of the preferred hole-basis fits in ISO 286-1.

Compare that with the general tolerance. At 25 mm, class m allows a band 0.4 mm wide; IT7 allows 0.021 mm, about one nineteenth of it. An IT grade describes the width of a tolerance zone, not what a process can hold. Whether a machine, material and feature combination reaches IT7 is a question for the supplier, per feature. The ISO 286 article covers the fit tables in full.

What do geometrical tolerances add to size tolerances?

A size tolerance does not say how flat, round or square a feature is, or where it sits relative to another. ISO 1101:2017 (edition 4, "Tolerances of form, orientation, location and run-out") defines the symbols and rules for those requirements. ASME Y14.5-2018 plays the same role in the American system, and ASME lists the 2018 edition as in effect after reaffirmation in 2024.

A geometrical tolerance appears in a feature control frame: the characteristic symbol, the tolerance value, and the datum features it refers to. A flatness tolerance of 0.02 mm on a sealing face, for example, controls form only and refers to no datum. A position tolerance that locates a bolt pattern relative to a mounting face names that face as a datum.

The two systems are not interchangeable. ISO 8015:2011 sets the fundamental concepts, principles and rules for interpreting ISO GPS indications on drawings, while ASME Y14.5 carries its own default rules, including how size limits relate to form. A drawing that mixes the two without naming a standard is ambiguous. Name the standard in the title block.

For features without a geometrical tolerance, ISO 22081:2021 gives the rules for general geometrical specifications made under ISO 8015:2011, clause 5.12. It does not replace the H, K and L values of the withdrawn ISO 2768-2. In Germany, DIN has issued a draft, E DIN 2769:2026-09, that supplements DIN EN ISO 22081 with tolerance classes and values.

Which of these standards are current in November 2026?

Table 4. Status of the standards in this article, as of 2026-11-02

Source: ISO catalogue pages, ISS life cycle records and ASME page listed under Sources, read on 2026-11-02.

The new ISO 2768 keeps the number of the old standard. ISO lists it with four tolerance classes and three tables, and it replaces ISO 2768-1:1989. An undated "ISO 2768-m" on a drawing can therefore point to either edition once the new one is published. DIN described the same problem for ISO 2768-2 and ISO 22081 and recommended dating the reference.

How do you decide which tolerance a feature needs?

Start from what each feature does in the assembly.

• A feature that mates, seals or locates another part gets an ISO 286 class or a tolerance on its limits, for example a bearing seat Ø52 H7 (0 to +0.030 mm, IT7 for 50 to 80 mm).
• A feature whose orientation or position matters for assembly, such as a bore axis relative to a mounting face, gets a geometrical tolerance with a datum.
• Every other dimension stays on the general tolerance.

Test the general tolerance at its extreme: if a part at the edge of the class limit would still work, the feature does not need its own tolerance. If it would not, it does.

Dimensions are specified at the standard reference temperature of 20 °C. NIST reports that the 2016 revision of ISO 1 left that value unchanged, and ISO 1:2022 is the current edition. A tolerance in the IT6 to IT7 range is therefore checked against the 20 °C condition, and buyer and supplier should agree how the supplier measures and compensates for it.

What should the drawing state for a supplier?

A supplier can quote and inspect only what the drawing states. Before a drawing goes out:

• The general tolerance class and its edition are in the title block, for example "ISO 2768-m (ISO 2768-1:1989)".
• Fits are written as ISO 286 classes, such as H7 or g6, with the nominal size.
• The drawing names its geometrical tolerancing standard, ISO 1101 or ASME Y14.5.
• Datum features are marked on the part, not only in the frame.

Our network works to ISO 2768-m as standard on CNC milling and CNC turning, and tighter where the drawing specifies it. The technical drawing checklist lists the other title block entries a supplier needs.

Frequently asked questions

What is the standard tolerance for CNC machining?

There is no single one. A drawing sets it through its general tolerance note. With ISO 2768-m, which our network applies as standard, a linear dimension over 6 up to 30 mm may deviate by ±0.2 mm and one over 30 up to 120 mm by ±0.3 mm. Features that need more carry their own tolerance.

What is the difference between ISO 2768 and ISO 286?

ISO 2768 sets general tolerances for dimensions that have no tolerance of their own. ISO 286 defines tolerance classes such as H7 and g6 that you write after a dimension for features that must fit together. For a 25 mm size, ISO 2768-m allows ±0.2 mm and H7 allows 0 to +0.021 mm.

What is the IT7 tolerance for a 25 mm bore?

25 mm lies in the range over 18 up to 30 mm, where IT7 is 21 µm (ISO 286-1:2010). A bore of Ø25 H7 therefore measures between 25.000 mm and 25.021 mm.

Is ISO 2768-2 still valid?

No. ISO 2768-2:1989 (classes H, K, L for geometry) was withdrawn in 2021. ISO 22081:2021 covers general geometrical specifications but does not contain the H, K and L values, so drawings that cite part 2 should name the 1989 edition.

Is ISO 1101 the same as ASME Y14.5?

No. Both define geometrical tolerancing, but ISO 1101 belongs to the ISO GPS system and ASME Y14.5 is a separate American standard with its own rules. The drawing has to name the one it follows, and the supplier has to inspect to that one.

Sources

1. ISO 2768-1:1989, General tolerances, Part 1 (ISO catalogue, stage 90.92, reviewed 2022)
2. ISO 2768, edition 2, linear and angular sizes (ISO catalogue, stage 60.00, under publication)
3. ISO 2768 edition 2, life cycle record (ISS mirror of the ISO catalogue)
4. ISO 2768-2:1989, life cycle record, withdrawn 2021-02-04 (ISS mirror of the ISO catalogue)
5. ISO 2768-1 linear dimension table, as reproduced by AMESWeb (the standard text is paywalled)
6. ISO 22081:2021, General geometrical specifications and general size specifications (ISO catalogue)
7. E DIN EN ISO 22081:2021-12, note on the replacement of ISO 2768-2 (DIN Media)
8. E DIN 2769:2026-09, general tolerances supplementing DIN EN ISO 22081 (DIN Media)
9. ISO 286-1:2010, ISO code system for tolerances on linear sizes, Part 1 (ISO catalogue)
10. ISO 286-2:2010, Part 2, tables of tolerance classes and limit deviations (ISO catalogue)
11. ISO 286-1:2010 Table 1, standard tolerance grades IT01 to IT18 (reproduced on Wikipedia)
12. ISO 286-2 shaft limit deviations, class g6 (Roy Mech tables)
13. ISO 1101:2017, Geometrical tolerancing (ISO catalogue, confirmed 2022)
14. ISO 8015:2011, GPS fundamentals, concepts, principles and rules (ISO catalogue, confirmed 2021)
15. ASME Y14.5-2018 (R2024), Dimensioning and Tolerancing (ASME)
16. The 2016 revision of ISO 1: standard reference temperature remains 20 °C (NIST)
17. ISO 1:2022, Standard reference temperature (Genorma catalogue entry)

Questions on a drawing? sales@ertas.engineering

Related guides