ISO 2768 general tolerances: which class belongs on your drawing?
Not every dimension on a drawing needs its own tolerance. ISO 2768 applies a single rule to every dimension that carries a value but no tolerance. The two letters you put in the title block decide both how the part will be inspected and what it will cost.
What ISO 2768 actually solves
A part carries dozens of dimensions and most of them are not critical: the overall thickness of a face a bolt head sits on, the outer length of a body, the height of a chamfer. Toleranceing each one individually makes the drawing unreadable. ISO 2768 collapses all of them into a single line: you write "ISO 2768-mK" in the title block, and every untoleranced dimension automatically takes its value from the standard’s table.
The standard has two parts. ISO 2768-1 covers dimensional features (lengths, diameters, chamfers, angles) in four classes: f (fine), m (medium), c (coarse), v (very coarse). ISO 2768-2 covers geometrical tolerances (flatness, perpendicularity, symmetry, run-out) in three classes: H, K, L. That is why the title block usually carries two letters together — "ISO 2768-mK" means m for dimensional, K for geometrical.
ISO 2768-1 — permissible deviations for linear dimensions (mm)
| Nominal size | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 – 3 mm | ±0.05 | ±0.1 | ±0.2 | — |
| 3 – 6 mm | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| 6 – 30 mm | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
| 30 – 120 mm | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| 120 – 400 mm | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| 400 – 1000 mm | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
| 1000 – 2000 mm | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
| 2000 – 4000 mm | — | ±2.0 | ±4.0 | ±8.0 |
Read it like this: an 80 mm dimension is allowed ±0.3 mm in class m and ±0.15 mm in class f. Below 0.5 mm the general tolerance does not apply — such a dimension must be toleranced individually on the drawing.
Angles and chamfers
For angles the limit is set by the length of the shorter leg forming the angle, not by the size of the angle itself. The shorter that leg, the larger the same angular deviation appears on the part.
| Shorter leg | f / m | c | v |
|---|---|---|---|
| up to 10 mm | ±1° | ±1°30′ | ±3° |
| 10 – 50 mm | ±30′ | ±1° | ±2° |
| 50 – 120 mm | ±20′ | ±30′ | ±1° |
| 120 – 400 mm | ±10′ | ±15′ | ±30′ |
| over 400 mm | ±5′ | ±10′ | ±20′ |
External radii and chamfer heights are looser: ±0.2 mm for f/m and ±0.4 mm for c/v between 0.5 and 3 mm; ±0.5 / ±1.0 mm between 3 and 6 mm; ±1.0 / ±2.0 mm above 6 mm.
ISO 2768-2 — geometrical tolerances (mm)
A face can be dimensionally correct and still not be flat; a hole can be the right diameter and still not be square to the face. ISO 2768-2 puts a separate limit on both.
| Straightness / flatness — longer side | H | K | L |
|---|---|---|---|
| up to 10 mm | 0.02 | 0.05 | 0.1 |
| 10 – 30 mm | 0.05 | 0.1 | 0.2 |
| 30 – 100 mm | 0.1 | 0.2 | 0.4 |
| 100 – 300 mm | 0.2 | 0.4 | 0.8 |
| 300 – 1000 mm | 0.3 | 0.6 | 1.2 |
| 1000 – 3000 mm | 0.4 | 0.8 | 1.6 |
| Perpendicularity — shorter side | H | K | L |
|---|---|---|---|
| up to 100 mm | 0.2 | 0.4 | 0.6 |
| 100 – 300 mm | 0.3 | 0.6 | 1.0 |
| 300 – 1000 mm | 0.4 | 0.8 | 1.5 |
| 1000 – 3000 mm | 0.5 | 1.0 | 2.0 |
Symmetry stays at 0.5 mm in class H up to 1000 mm; class K runs from 0.6 to 1.0 mm and class L from 0.6 to 2.0 mm. Circular run-out does not depend on size at all: 0.1 mm for H, 0.2 mm for K, 0.5 mm for L.
Why tolerance moves the price
Tightening a tolerance does not simply make the machine run slower — it changes the whole process. A tight tolerance forces a separate roughing and finishing pass, shortens tool life, may require intermediate stress relief because removing material releases internal stress, demands fixturing that will not deflect the part under clamping load, and finally changes inspection: a dimension that a caliper could accept moves to a micrometer, and a geometry a micrometer could accept moves to the CMM.
- Do not tighten non-functional dimensionsIf a face does not mate with anything, the general tolerance is enough. Putting ±0.02 on every dimension is not precision, it is cost.
- Tolerance the critical features individuallyBearing seats, fit diameters, seal grooves, hole patterns — these need their own tolerance, not ISO 2768.
- State the datumsPerpendicularity and symmetry can only be measured against a reference. With no datum, the inspection result is arguable.
- Put the class in the title blockIf the drawing says nothing, the manufacturer applies its own assumption — and that becomes a dispute at acceptance.
Which class is used in practice
In machining the common combination is ISO 2768-mK: medium for dimensions, K for geometry. Welded fabrications and sheet metal parts normally sit at c or v. Class f declares that the whole part is precision work and is usually tighter than needed — toleranceing the critical features individually and leaving the rest at m is both more accurate and more economical.
At Q TECH we read every incoming drawing this way before production starts: which dimensions were left to the general tolerance, which were toleranced separately, and against which datums the part will be measured. Because inspection is in-house — a COORD3 ARES CMM with a Renishaw PH20 head — the tolerance discussion happens before the part ships, not after.
- ISO 2768
- general tolerances
- ISO 2768-mK
- technical drawing
- CMM inspection
- precision machining
- Ankara Ostim
Frequently asked questions
What does ISO 2768-mK mean?
The "m" sets the medium tolerance class for dimensional features and the "K" sets the medium class for geometrical tolerances. Every dimension without its own tolerance is taken from the ISO 2768-1 class m table, and limits such as flatness, perpendicularity, symmetry and run-out are taken from the ISO 2768-2 class K table. It is the most common combination in machining.
How is ISO 2768 different from ISO 286 (h7, H7)?
ISO 2768 is a general tolerance: it applies to dimensions that carry no tolerance on the drawing, and it is symmetric (±). ISO 286 is the fits system; it defines how a shaft and a hole sit together and is written as letter-number codes such as h7, H7 or g6. A bearing seat is never given ISO 2768 — it is given H7.
What happens if my drawing states no tolerance at all?
The manufacturer falls back on its own shop standard. That means there is no document to settle who is right if the part is rejected. The shortest fix is one line in the title block — "ISO 2768-mK" — which defines every untoleranced dimension at once.
How much does a tight tolerance add to the price?
There is no single percentage; it depends on the geometry, the material and the quantity. What raises the price is not the tolerance itself but what it forces: an extra finishing pass, dedicated fixturing, stress relief, more frequent tool changes and CMM inspection per piece. This is why we agree on which features are genuinely critical at the quotation stage.
Does the general tolerance apply below 0.5 mm?
No. The ISO 2768-1 table starts at 0.5 mm. Below that nominal size the tolerance must be written next to the dimension on the drawing.
Send us your technical drawing and quantity; we will prepare your quote with a manufacturability review.
Request a Quote