What Is ISO 2768 General Tolerance?

What Is General Tolerance?
Writing a tolerance on every dimension of a drawing is inefficient. A general tolerance is the permissible deviation applied across the board to dimensions with no individual tolerance specified. If the title block says ISO 2768-m, every dimension without a tolerance callout is controlled by the tables in this standard.
Put the other way, a dimension with no tolerance is not one that only needs to be "roughly right." It is a dimension that must fall within the range set by the general tolerance class. If you do not understand this one line, you are reading only half of the drawing's tolerance system.
How to Read the Designation: Anatomy of "ISO 2768-mK"
The general tolerance designation has two parts.
Part | Applies to | Class |
|---|---|---|
ISO 2768-1 (lowercase) | Linear dimensions, angles, chamfers | f (fine) / m (medium) / c (coarse) / v (very coarse) |
ISO 2768-2 (uppercase) | Geometric tolerances (flatness, perpendicularity, runout, etc.) | H / K / L (H is the tightest) |
ISO 2768-mK means "class m (medium) for linear dimensions and angles, class K for geometric tolerances." It is the combination seen most often on production drawings in Korea.
Linear Dimension Tolerance Table (ISO 2768-1)
Permissible deviations are in mm (±).
Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
0.5 ~ 3 | ±0.05 | ±0.1 | ±0.2 | — |
3 ~ 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
6 ~ 30 | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
30 ~ 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
120 ~ 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
400 ~ 1000 | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
1000 ~ 2000 | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
2000 ~ 4000 | — | ±2.0 | ±4.0 | ±8.0 |
Two points to note when reading the table.
General tolerances do not apply to dimensions under 0.5 mm. An individual tolerance must be specified.
Within the same class, the permissible deviation grows as the dimension grows. Class m is ±0.3 for a 100 mm dimension but ±0.5 for 300 mm.
Chamfers and Radii (External Radius and Chamfer Height)
Nominal size (mm) | f · m | c · v |
|---|---|---|
0.5 ~ 3 | ±0.2 | ±0.4 |
3 ~ 6 | ±0.5 | ±1.0 |
Over 6 | ±1.0 | ±2.0 |
The permissible deviation for chamfers is much larger than for linear dimensions. A C0.5 chamfer that comes out anywhere from C0.3 to C0.7 is still within class m general tolerance. If chamfer size affects function (assembly lead-in, O-ring insertion face, etc.), specify an individual tolerance.
Angles
Angular tolerance is based on the length of the shorter leg.
Shorter leg length (mm) | f · m | c | v |
|---|---|---|---|
Up to 10 | ±1° | ±1°30′ | ±3° |
10 ~ 50 | ±0°30′ | ±1° | ±2° |
50 ~ 120 | ±0°20′ | ±0°30′ | ±1° |
120 ~ 400 | ±0°10′ | ±0°15′ | ±0°30′ |
Over 400 | ±0°5′ | ±0°10′ | ±0°20′ |
Standard History: ISO 2768-2 Has Been Withdrawn
ISO 2768-2:1989, which covers geometric tolerances, has been withdrawn and replaced by ISO 22081:2021. To specify general tolerances for flatness, perpendicularity, and runout on a new drawing, the current standard is ISO 22081. ISO 2768-1, which covers linear and angular tolerances, remains current and has been adopted in Korea as KS B ISO 2768-1.
In shop-floor practice, however, the ISO 2768-mK designation is still widely used, and most machine shops interpret it without difficulty. When reading an older drawing, you can decode the H/K/L classes as they are; when creating a new drawing, take care over which standard you cite.
Class m (Medium) Is the Practical Default
Class m is the level a typical CNC process meets without any extra effort. ±0.2 for a 6~30 mm dimension is achieved naturally in ordinary milling and turning. For that reason, from a quoting and machining standpoint, class m general tolerance has almost no effect on cost.
Here is the practical feel for each class.
f (fine) — Parts with many precision assembly features. Applying it across the whole drawing increases the process and inspection burden, so it is better to specify individual tolerances only for the dimensions that need them.
m (medium) — The standard for general machined parts. This is the default unless there is a separate requirement.
c (coarse) — Non-fit areas such as welded structures and bent sheet metal.
v (very coarse) — Non-functional dimensions on large cast or welded structures.
Cost Impact: One Class Changes the Process
Moving the general tolerance class from m to f is not "the numbers getting slightly better." It means the inspection criterion for every untoleranced dimension on the drawing becomes twice as tight. The results show up as follows.
Change | Effect on machining and inspection |
|---|---|
Added finishing pass | A finishing operation is added to dimensions that rough cutting alone used to satisfy |
More inspection items | Every dimension becomes subject to inspection against the tighter limit |
Higher rework and scrap rate | The probability of going out of tolerance rises on every dimension |
Longer lead time | Added process and inspection steps accumulate |
The key point is that the cost arises across the entire drawing, not only where it is needed. Usually only a few dimensions need to be precise for functional reasons, but raising the general tolerance class makes the dozens of other dimensions more expensive too.
Where to Tighten and Where to Relax
The standard approach is clear: keep the general tolerance at class m and specify individual tolerances only for functional dimensions.
Where individual tolerances are needed — Fit features such as bearing seats and pin holes (fit tolerances such as H7), position dimensions that mate with other parts, and dimensions tied to sealing faces
Where general tolerance is enough — Overall dimensions, dimensions that only affect weight or clearance, and non-functional features such as pocket depth
The principle is the same as with surface roughness: avoid blanket specifications and tighten only the functional surfaces. Over-specification does not raise quality; it only raises cost.
Frequently Asked Questions
What happens if the drawing has no general tolerance note at all?
The usual practice is for the shop to machine to its own standard (typically equivalent to ISO 2768-m). But practice is not a contract. If a dimensional dispute arises there is no basis for judgment, so we recommend stating ISO 2768-mK as one line in the title block.
Can general tolerance produce a fit?
No. The ±0.1~0.2 of class m falls far short of the precision a fit requires (a few µm to a few tens of µm). Bearing, pin, and bushing seats must always have an individual fit tolerance such as H7/g6.
Why not specify class f for everything?
The machining itself is possible. However, the inspection criterion for every dimension becomes tighter, inspection labor and rework rates go up, and this flows straight into the quote. Specifying individual tolerances only for the dimensions that need precision is the way to get the same quality at lower cost.
What does the K in 2768-mK mean?
It is the medium class of geometric tolerance (ISO 2768-2). For example, under class K, perpendicularity of a face up to 100 mm is controlled to 0.4 mm, and flatness to roughly 0.05~0.6 mm depending on the size range. For a new drawing, the current standard for this part is ISO 22081.
Summary
A dimension with no tolerance is not a free dimension; it is governed by the general tolerance
ISO 2768-mK= linear and angular class m + geometric class KClass m is the practical default and has almost no effect on cost
Raising the class raises the cost of the whole drawing, so the standard practice is to specify only functional dimensions individually
Fits are outside the scope of general tolerance; individual specification such as H7/g6 is required
ISO 2768-2 is withdrawn (→ ISO 22081); 2768-1 is current
Upload a drawing to see how the general tolerance class and individual tolerance specifications are reflected in the quote.
Have a part to machine?
Upload a drawing to see your quote.



