General tolerances (ISO 2768) and H7/g6 fits explained
No part is ever made exactly to size, so every drawing must say how far each size may vary. Critical sizes, such as a bore for a shaft, carry their own tolerance next to the number. All the other sizes — usually the majority — use a general tolerance written once in the title block. "ISO 2768-m" means every size without its own tolerance follows the m (medium) table.
ISO 2768-1: linear dimensions (mm)
For lengths, widths, heights, distances and diameters without an individual tolerance.
| Size range (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 to 3 | ±0.05 | ±0.1 | ±0.2 | – |
| over 3 to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6 to 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30 to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120 to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400 to 1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1000 to 2000 | ±0.5 | ±1.2 | ±3 | ±6 |
| over 2000 to 4000 | – | ±2 | ±4 | ±8 |
Example: a 150 mm plate on a drawing marked ISO 2768-m is acceptable from 149.5 to 150.5 mm.
Chamfers, radii and angles
| Radii and chamfer heights | f / m | c / v |
|---|---|---|
| 0.5 to 3 mm | ±0.2 | ±0.4 |
| over 3 to 6 mm | ±0.5 | ±1 |
| over 6 mm | ±1 | ±2 |
| Length of the shorter side of the angle | f / m | c | v |
|---|---|---|---|
| up to 10 mm | ±1° | ±1°30′ | ±3° |
| over 10 to 50 mm | ±0°30′ | ±1° | ±2° |
| over 50 to 120 mm | ±0°20′ | ±0°30′ | ±1° |
| over 120 to 400 mm | ±0°10′ | ±0°15′ | ±0°30′ |
| over 400 mm | ±0°5′ | ±0°10′ | ±0°20′ |
These are the commonly used ISO 2768-1 values. Where a contract or customer specification applies, follow the edition of the standard it references.
Which class to choose
- m (medium) — the usual default for general turning, milling and laser cutting.
- f (fine) — precision turning or milling; costs more because inspection is tighter.
- c (coarse) — bending, welded frames, sheet parts that do not need a tight fit.
- v (very coarse) — large structures, rough castings.
Do not choose finer than needed: one class tighter can add a lot to part price and inspection time. Put tight tolerances only on sizes that matter for assembly or function.
Fits: the H7 hole-basis system
For holes that take a shaft, use the ISO 286 system, written as a letter and a number such as Ø20 H7. The letter gives the position of the tolerance zone (capital = hole, lower case = shaft) and the number its width (IT grade). Most general work uses the hole-basis system: the hole is always H7, and the shaft is chosen for the kind of fit.
| Fit | Type | Hole Ø20 (mm) | Shaft Ø20 (mm) | Used for |
|---|---|---|---|---|
| H7/g6 | Close running clearance | +0.021 / 0 | −0.007 / −0.020 | Shafts turning in bushes, precise sliding parts |
| H7/h6 | Locational clearance (slides together by hand) | +0.021 / 0 | 0 / −0.013 | Parts that must come apart yet locate accurately |
| H7/k6 | Transition | +0.021 / 0 | +0.015 / +0.002 | Gears and pulleys on keyed shafts, fitted with a soft mallet |
| H7/p6 | Interference (press fit) | +0.021 / 0 | +0.035 / +0.022 | Permanently pressed bushes, assembled with a press or by heating |
These values are for sizes over 18 up to 30 mm; other sizes differ. Always look them up in ISO 286-2, or write the limits on the drawing — for example Ø20 +0.0210 — so the machinist does not need the table.
Putting it on a drawing in DXCAD2D Online
- When exporting a PDF, tick Add drawing frame + title block. The General tolerance field defaults to
ISO 2768-m; change it as needed. - For sizes with their own tolerance there are two ways: place a text (T) such as
H7or±0.05right after the dimension value, or give the dimension a name such as A, B, C and type the tolerance in its Tolerance / note field, which appears in the dimension table — good when many sizes need control. - If most of a part needs tight tolerances, change the general tolerance for the whole sheet rather than tagging every size.
Try it right now — a free 2D CAD in your browser. Nothing to install, no sign-up.
Open DXCAD2D OnlineThings to watch
- General tolerances do not cover form and position — straightness, parallelism, concentricity. Where those matter, add GD&T symbols separately.
- A size in brackets, such as (45), is a reference dimension: not inspected, no tolerance.
- Bending and welding have their own tolerance standards (ISO 13920 for welded structures, for example). Do not put class f on a bent part without asking the maker.
- Always state units and the standards used in the title block — see title blocks and revision control.