This page covers the complete ISO 2768 standard: what it is, how to read the tolerance tables, what ISO 2768-mK means on a drawing, how to select the right class for your project, and how it compares to ASME Y14.5.
What is ISO 2768?
ISO 2768 is an international standard published by the International Organization for Standardization (ISO) that defines general tolerances for engineering drawings. Its purpose is straightforward: instead of writing a tolerance value next to every single dimension on a technical drawing, an engineer can add one note to the title block — for example, ISO 2768-mK — and that single callout sets the default permissible variation for all features that do not carry an explicit individual tolerance.
The standard is divided into two parts that work together:
- ISO 2768-1 covers linear and angular dimensions — lengths, widths, heights, diameters, step sizes, external radii, chamfer heights, and angles. It provides four tolerance classes: fine (f), medium (m), coarse (c), and very coarse (v).
- ISO 2768-2 covers geometrical tolerances — straightness, flatness, perpendicularity, symmetry, and circular run-out. It provides three tolerance classes: H, K, and L.
ISO 2768 is the dominant general tolerance standard in Europe and Asia, and is widely recognised by CNC machining suppliers worldwide. It is also published as DIN 7168 in Germany and has equivalents in many national standards bodies.
Why it matters
Without a general tolerance reference in the title block, every machine shop interprets untoleranced dimensions differently. Some default to national standards, others guess. ISO 2768 eliminates that ambiguity with a single, globally understood callout.
ISO 2768 applies to parts produced by metal removal (CNC milling, CNC turning, drilling, grinding) and to parts formed from sheet metal. It does not apply to thread tolerances, surface roughness (Ra values), or dimensions that already carry an explicit tolerance — those always take precedence.
ISO 2768-1: Linear and Angular Dimension Tolerances
The following is the tolerance table corresponding to the 4 class precision levels, you can choose the most suitable one according to machining capabilities and your design requirements.
Table 1 - Linear Dimensions
| Nominal length range (mm) | Tolerance Class Designation (Description) | |||
|---|---|---|---|---|
| F (Fine) | M (Medium) | C (Coarse) | V (Very Coarse) | |
| 0.5 up to 3 | ±0.05 | ±0.1 | ±0.2 | – |
| over 3 up to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6 up to 30 | ±0.1 | ±0.2 | ±0.5 | ±1.0 |
| over 30 up to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120 up to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400 up to 1000 | ±0.3 | ±0.8 | ±2.0 | ±4.0 |
| over 1000 up to 2000 | ±0.5 | ±1.2 | ±3.0 | ±6.0 |
| over 2000 up to 4000 | – | ±2.0 | ±4.0 | ±8.0 |
For nominal sizes below 0.5 mm, the deviations shall be indicated adjacent to the relevant nominal size(s).
Table 2 - External Radii and Chamfer Heights
| Nominal length range (mm) | Tolerance Class Designation (Description) | |||
|---|---|---|---|---|
| F (Fine) | M (Medium) | C (Coarse) | V (Very Coarse) | |
| 0.5 up to 3 | ±0.2 | ±0.2 | ±0.4 | ±0.4 |
| over 3 up to 6 | ±0.5 | ±0.5 | ±1.0 | ±1.0 |
| over 6 | ±1.0 | ±1.0 | ±2.0 | ±2.0 |
For nominal sizes below 0.5 mm, the deviations shall be indicated adjacent to the relevant nominal size(s).
Table 3 - Angular Dimensions
| Permissible deviations in mm for ranges in nominal lengths | Tolerance Class Designation (Description) | |||
|---|---|---|---|---|
| F (Fine) | M (Medium) | C (Coarse) | V (Very Coarse) | |
| up to 10 | ±1º | ±1º | ±1º30′ | ±3º |
| over 10 up to 50 | ±0º30′ | ±0º30′ | ±1º | ±2º |
| over 50 up to 120 | ±0º20′ | ±0º20′ | ±0º30′ | ±1º |
| over 120 up to 400 | ±0º10′ | ±0º10′ | ±0º15′ | ±0º30′ |
| over 400 | ±0º5′ | ±0º5′ | ±0º10′ | ±0º20′ |
ISO 2768-2: Geometrical Tolerances for Form and Position
ISO 2768-2 simplifies drawings by providing general tolerances for geometrical quantities — the shape and relative position of features — in three classes: H, K, and L. These cover straightness, flatness, perpendicularity, symmetry, and circular run-out.
Important: ISO 2768-2 does not cover parallelism, cylindricity, concentricity, profile, or position (true position). Those require explicit GD&T callouts.
Table 4 - General Tolerances on Straightness and Flatness
| Ranges of nominal lengths in mm | Tolerance Class | ||
|---|---|---|---|
| H | K | L | |
| up to 10 | 0.02 | 0.05 | 0.1 |
| above 10 to 30 | 0.05 | 0.1 | 0.2 |
| above 30 to 100 | 0.1 | 0.2 | 0.4 |
| above 100 to 300 | 0.2 | 0.4 | 0.8 |
| above 300 to 1000 | 0.3 | 0.6 | 1.2 |
| above 1000 to 3000 | 0.4 | 0.8 | 1.6 |
Table 5 - General Tolerances on Perpendicularity
| Ranges of nominal lengths in mm | Tolerance Class | ||
|---|---|---|---|
| H | K | L | |
| up to 100 | 0.2 | 0.4 | 0.6 |
| above 100 to 300 | 0.3 | 0.6 | 1.0 |
| above 300 to 1000 | 0.4 | 0.8 | 1.5 |
| above 1000 to 3000 | 0.5 | 1.0 | 2.0 |
Table 6 - General Tolerances on Symmetry
| Ranges of nominal lengths in mm | Tolerance Class | ||
|---|---|---|---|
| H | K | L | |
| up to 100 | 0.5 | 0.6 | 0.6 |
| above 100 to 300 | 0.5 | 0.6 | 1.0 |
| above 300 to 1000 | 0.5 | 0.8 | 1.5 |
| above 1000 to 3000 | 0.5 | 1.0 | 2.0 |
Table 7 - General Tolerances on Circular Run-Out
| Ranges of nominal lengths in mm | Tolerance Class | ||
|---|---|---|---|
| H | K | L | |
| 0.1 | 0.2 | 0.5 | |
ISO 2768 General Tolerance Tables — PDF Reference
All 7 tolerance tables (Part 1 & Part 2) in a single printable document · rpproto.com
What does ISO 2768-mK mean?
ISO 2768-mK is the most common general tolerance callout you will encounter on CNC machining and sheet metal drawings. It combines one class from each part of the standard:
- m — medium tolerance class from ISO 2768-1 (linear and angular dimensions)
- K — medium geometrical tolerance class from ISO 2768-2 (form and position)
Together they mean: “For any dimension on this drawing that does not have its own explicit tolerance, apply the medium linear tolerance from Table 1–3 and the K-class geometrical tolerance from Table 4–7.”
Other common combinations and their typical use cases:
| Callout | Dimensional class | Geometrical class | Typical application |
|---|---|---|---|
| ISO 2768-fH | Fine | H (fine) | High-precision optical or medical parts |
| ISO 2768-mK Most common | Medium | K (medium) | General CNC machined parts, enclosures, brackets |
| ISO 2768-cL | Coarse | L (coarse) | Sheet metal, welded structures, castings |
| ISO 2768-m | Medium | Not specified | Drawings using explicit GD&T for all geometry |
Common misconception
The letters in ISO 2768-mK are case-sensitive. Lowercase letters (f, m, c, v) refer to Part 1 dimensional classes. Uppercase letters (H, K, L) refer to Part 2 geometrical classes. Writing ISO 2768-MK or ISO 2768-mk is technically incorrect.
How to indicate ISO 2768 on an engineering drawing
Indicating ISO 2768 correctly on a drawing takes three steps:
Step 1 — Choose your tolerance class combination
Select one dimensional class (f/m/c/v) based on the manufacturing process and the functional requirements of the part. Then select one geometrical class (H/K/L) or omit Part 2 if all geometric tolerances are called out explicitly with GD&T symbols.
Step 2 — Add the general note to the title block
Place the following note in or immediately adjacent to the drawing title block:
GENERAL TOLERANCES: ISO 2768-mK
(Unless otherwise specified)
Some drawing templates use a dedicated “General Tolerance” field in the title block. Either placement is acceptable as long as it is clearly visible.
Step 3 — Override where needed
Any dimension on the drawing that carries its own explicit tolerance — for example Ø 25.00 ±0.02 or a GD&T flatness callout of ⊞ 0.05 — automatically overrides the ISO 2768 general class for that specific feature. The general class applies only to untoleranced dimensions.
Best practice
Only specify tighter tolerances where the function of the part actually requires them — bearing seats, sealing faces, press-fit bores. Applying ISO 2768-fH to an entire drawing when only three features need it is one of the most common ways to inflate CNC machining costs unnecessarily.
Class selection guide: which ISO 2768 tolerance should you use?
Choosing the right class is about matching manufacturing capability to functional need — not defaulting to the tightest option available. Tighter tolerances mean longer cycle times, more setup steps, and higher inspection requirements.
Highest precision available under ISO 2768. Requires careful process control and increased inspection.
Balances precision and cost. Achievable on standard 3-axis and 5-axis CNC machining without special measures.
Suitable where dimensional accuracy is secondary to form or assembly. Faster and cheaper to produce.
Widest tolerance range. Rarely specified for machined parts; mainly used for large structural weldments.
Geometrical class selection (ISO 2768-2)
| Class | When to use | Example applications |
|---|---|---|
| H Fine | Tight geometric control required; part function depends on form accuracy | Precision bearing housings, optical mounts, valve seats |
| K Medium Recommended | General mechanical assemblies where form variation is acceptable within moderate limits | CNC machined brackets, enclosures, fixture plates |
| L Coarse | Non-precision assemblies; form is not functionally critical | Sheet metal, welded structures, rough machined frames |
RpProto default capability
Our CNC machining service meets ISO 2768-m as standard, with ISO 2768-f available on request for precision components. All parts are inspected in-house per our Quality Control process before shipment.
ISO 2768 vs ASME Y14.5: key differences
If you work with both European/Asian suppliers and US machine shops, you will encounter both standards. Understanding the differences prevents costly miscommunication.
| Attribute | ISO 2768 | ASME Y14.5 |
|---|---|---|
| Origin | International (ISO), widely used in Europe, Asia, China | United States (ASME); dominant in US manufacturing |
| Approach | General tolerance — one title-block callout covers most features | Feature-by-feature — each controlled feature needs an explicit GD&T symbol and datum reference |
| Drawing complexity | Simpler, faster drawings; fewer annotations | More detailed drawings; higher engineering time upfront |
| Geometric control | Limited to 5 geometric characteristics (ISO 2768-2) | Full GD&T suite: position, concentricity, profile, parallelism, cylindricity, and more |
| Ambiguity | Some ambiguity for complex assemblies with critical fits | Highly precise and unambiguous when applied correctly |
| Cost to apply | Low — fast drawing creation | Higher — requires trained GD&T engineers to apply and interpret correctly |
| Best for | General machined parts, international sourcing, prototypes, most CNC components | Complex assemblies, aerospace/defence, parts requiring precise fit and function verification |
When sourcing CNC machined parts from China, ISO 2768 is the preferred and universally understood standard. Most Chinese machine shops are not trained in ASME Y14.5 — a drawing referencing ASME GD&T symbols without explanation will often be misread. If your designs originate in a US GD&T environment, converting the key functional tolerances to ISO 2768 with explicit callouts for critical features is the most reliable approach for international manufacturing.
Practical tip
You can combine both: use ISO 2768-mK as the general note, then add explicit GD&T symbols (⊞, ⌀, ⊙) for the two or three features where precise geometric control genuinely matters. This gives you the simplicity of ISO 2768 with the precision of GD&T where needed.
Common mistakes when using ISO 2768
No general tolerance callout in the title block
The most common problem: the drawing has no ISO 2768 reference at all. Every machine shop then applies its own default — which may be a national standard, a house rule, or a guess. Always include the general tolerance note.
Defaulting to ISO 2768-fH “because tighter is better”
Fine + H is expensive. It increases machining time, fixture complexity, and inspection cost — often with no functional benefit. Most CNC parts work perfectly under ISO 2768-mK. Specify fH only where the part’s function genuinely demands it.
Forgetting that ISO 2768-2 does not cover all geometric tolerances
Part 2 covers five characteristics: straightness, flatness, perpendicularity, symmetry, and run-out. It does not cover parallelism, cylindricity, concentricity, profile, or true position. Engineers who assume their ISO 2768-K callout controls all geometry will get non-conforming parts.
Applying ISO 2768 to features where it doesn’t belong
ISO 2768 does not govern thread tolerances (use ISO 965), surface roughness Ra (specify separately), or interference and clearance fits (use ISO 286). Relying on the general tolerance note for these features leads to assembly failures.
Sending ISO 2768 drawings to ASME-only shops without explanation
A US machine shop unfamiliar with ISO standards may not recognise ISO 2768-mK in the title block and may default to ASME Y14.5 interpretations — or worse, ignore the tolerance note entirely. Always confirm that your supplier understands the standard you are referencing.
Using lowercase and uppercase incorrectly
Dimensional classes are lowercase (f, m, c, v). Geometrical classes are uppercase (H, K, L). Writing ISO 2768-MK or ISO 2768-mk is technically non-standard and may cause confusion with suppliers.
Ready to manufacture your parts to ISO 2768?
Upload your drawing and RpProto’s engineering team will review your tolerance callouts and provide a detailed quote for CNC machining, sheet metal, or injection moulding.
