ISO 2768: The Complete Guide to General Tolerances in Manufacturing

ISO 2768-mK appears on more engineering drawings than any other general tolerance callout. Yet most articles about ISO 2768 either dump the standard's text without context or skip the actual tolerance values entirely. If you're sourcing CNC machined parts from China, getting these tolerances right is the difference between a smooth production run and a box of non-conforming parts.

Here's what you actually need: the full tolerance tables, what each class means in practice, how to call it out on a drawing, and where engineers consistently get it wrong.

TL;DR / Key Takeaways

• ISO 2768 is a two-part standard that defines general tolerances for machined parts - eliminating the need to tolerance every single dimension on a drawing
• Part 1 (ISO 2768-1) covers linear and angular dimensions in 4 classes: fine (f), medium (m), coarse (c), very coarse (v)
• Part 2 (ISO 2768-2) covers geometrical tolerances - straightness, flatness, perpendicularity, symmetry, runout - in 3 classes: H, K, L
• The most common callout is ISO 2768-mK (medium dimensional, K geometrical) - you'll see this on the majority of CNC machining and sheet metal drawings
• Choosing the wrong tolerance class costs you money: tighter than necessary inflates machining time, looser than necessary causes assembly failures

What is ISO 2768?

ISO 2768 is an international standard that defines general tolerances for machined parts - the default permissible deviations applied to any dimension on a drawing that doesn't have its own explicit tolerance. It was published by the International Organization for Standardization (ISO) and remains the most widely used general tolerancing standard in manufacturing.

Think of it as the safety net for your drawings. Instead of tolerancing every single linear dimension, angular dimension, and geometrical feature individually, you write “ISO 2768-mK” in the title block and the standard does the rest.

The standard has two parts:

• ISO 2768-1 (1989) - General tolerances for linear and angular dimensions
• ISO 2768-2 (1989) - Geometrical tolerances for features without individual tolerance indications

Both parts are typically called out together as a single designation like “ISO 2768-mK” - where the lowercase letter refers to Part 1 (dimensional class) and the uppercase letter refers to Part 2 (geometrical class).

Sidenote. ISO 2768 was first published in 1989 and hasn't been formally revised since. A draft revision (ISO/DIS 2768) reached DIS stage in 2025, with key changes including removal of the rejection rule and restriction of scope to linear and angular sizes only. The 1989 version remains the active standard as of 2026.

What are the ISO 2768 tolerance classes?

ISO 2768 tolerance classes define how much dimensional and geometrical deviation is acceptable for features without explicit tolerances. The tighter the class, the more precision required - and the more machining time and cost involved.

Part 1 - Dimensional tolerance classes:

Class	Designation	Typical Use
Fine	f	Precision instruments, optical components, tight-fit assemblies
Medium	m	General CNC machined parts - the most commonly specified class
Coarse	c	Sheet metal, castings, non-critical structural parts
Very Coarse	v	Flame-cut parts, rough fabrications, weldments

Part 2 - Geometrical tolerance classes:

Class	Designation	Typical Use
H	High precision	Close-fitting assemblies, precision fixtures
K	Standard	General machined parts - the default for most applications
L	Low precision	Non-critical fabrications, large structural parts

The most common combination worldwide is ISO 2768-mK - medium dimensional tolerances with K-class geometrical tolerances. If a drawing doesn't specify a class, most CNC machining shops default to this.

What is ISO 2768-1? Linear and angular dimension tolerances

ISO 2768-1 defines the permissible deviations for linear dimensions, external radii, chamfer heights, and angular dimensions when no individual tolerance is specified on the drawing. All values are in millimetres.

Linear dimension tolerances

This is the core table - the one engineers reference most. It covers external sizes, internal sizes, step dimensions, distances, diameters, and radii.

Nominal length range (mm)	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

To put this in practical terms: a 50mm dimension on a drawing callout of ISO 2768-m has a permissible deviation of ±0.3mm. That means anything between 49.7mm and 50.3mm is within tolerance. For the same dimension under class f, the window shrinks to ±0.15mm.

External radii and chamfer heights

Nominal size range (mm)	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

Notice that fine and medium are identical for radii and chamfers, and so are coarse and very coarse. This makes sense - chamfer accuracy rarely drives part function, so the standard doesn't differentiate as aggressively.

Angular dimension tolerances

Angular tolerances depend on the length of the shorter side of the angle, not the angle value itself.

Length of shorter side (mm)	f (fine)	m (medium)	c (coarse)	v (very coarse)
up to 10	±1°	±1°	±1°30′	±3°
over 10 up to 50	±0°30′	±0°30′	±1°	±2°
over 50 up to 120	±0°20′	±0°20′	±0°30′	±1°
over 120 up to 400	±0°10′	±0°10′	±0°15′	±0°30′
over 400	±0°5′	±0°5′	±0°10′	±0°20′

Again, fine and medium are identical for angular tolerances. The meaningful differentiation only kicks in at coarse and very coarse classes.

What is ISO 2768-2? Geometrical tolerances for features

ISO 2768-2 handles what Part 1 doesn't: form, orientation, and location tolerances for features that lack individual GD&T callouts. These are the tolerances that control straightness, flatness, perpendicularity, symmetry, and circular runout.

Straightness and flatness tolerances

Nominal length range (mm)	H	K	L
up to 10	0.02	0.05	0.1
over 10 up to 30	0.05	0.1	0.2
over 30 up to 100	0.1	0.2	0.4
over 100 up to 300	0.2	0.4	0.8
over 300 up to 1000	0.3	0.6	1.2
over 1000 up to 3000	0.4	0.8	1.6

For a 200mm-long surface under class K, the flatness tolerance is 0.4mm. Under class H, it tightens to 0.2mm - which typically requires a finishing pass on the CNC and potentially surface grinding for critical faces.

Perpendicularity tolerances

Nominal length range (mm)	H	K	L
up to 100	0.2	0.4	0.6
over 100 up to 300	0.3	0.6	1.0
over 300 up to 1000	0.4	0.8	1.5
over 1000 up to 3000	0.5	1.0	2.0

Symmetry tolerances

Nominal length range (mm)	H	K	L
up to 100	0.5	0.6	0.6
over 100 up to 300	0.5	0.6	1.0
over 300 up to 1000	0.5	0.8	1.5
over 1000 up to 3000	0.5	1.0	2.0

Circular runout tolerances

Unlike the other geometrical tolerances, runout isn't range-dependent - it's a single value per class.

Class	Runout tolerance (mm)
H	0.1
K	0.2
L	0.5

Runout at class K (0.2mm) is generous enough for most non-critical rotating assemblies. But if you're machining a shaft that mates with a bearing, 0.2mm runout will cause vibration - you'll need an explicit runout callout tighter than what ISO 2768-2 provides. For precision turned parts, consider working with factories that specialise in small precision turned parts and Swiss machining.

What does ISO 2768-mK mean on a drawing?

ISO 2768-mK is a combined designation that calls out both parts of the standard simultaneously.

Here's how to read it:

• ISO 2768 - the standard being referenced
• m (lowercase) - tolerance class from Part 1 (medium), applied to all linear and angular dimensions without explicit tolerances
• K (uppercase) - tolerance class from Part 2 (standard geometrical), applied to all form, orientation, and location features without explicit GD&T callouts

So when a drawing title block says “General tolerances ISO 2768-mK,” it means: every untoleranced linear dimension follows the medium class table, every untoleranced angular dimension follows the medium class angular table, and every untoleranced geometrical feature follows the K class tables for straightness, flatness, perpendicularity, symmetry, and runout.

Other common combinations you'll encounter:

Designation	Part 1 Class	Part 2 Class	Typical Application
ISO 2768-fH	Fine	High	Precision CNC parts, instruments, tight-fit assemblies
ISO 2768-mK	Medium	Standard	General CNC machining, sheet metal fabrication
ISO 2768-mH	Medium	High	CNC parts with critical flatness or perpendicularity
ISO 2768-cL	Coarse	Low	Rough fabrications, welded structures
ISO 2768-fK	Fine	Standard	Precision dimensions but standard geometrical tolerances

How do you apply ISO 2768 to engineering drawings?

Applying ISO 2768 correctly is straightforward, but there are rules engineers frequently miss.

Step 1: Add the callout to the title block. Write the full designation - for example, “General tolerances ISO 2768-mK” - in or near the title block of the drawing. This single line replaces hundreds of individual tolerance annotations.

Step 2: Understand what it covers. ISO 2768 applies to:

• Linear dimensions (external, internal, step, distances, diameters)
• Angular dimensions
• External radii and chamfer heights
• Straightness, flatness, perpendicularity, symmetry, and circular runout

Step 3: Understand what it does NOT cover. This is where most mistakes happen. ISO 2768 does not apply to:

• Dimensions that already have an explicit tolerance on the drawing
• Threaded features
• Dimensions governed by other standards (e.g., ISO 286 for fits and shaft/hole tolerances)
• Features with specific GD&T callouts (e.g., a flatness callout of 0.05mm overrides the Part 2 table)
• Reference dimensions (marked REF or in parentheses)

The rule is simple: if a feature has its own tolerance, ISO 2768 steps aside. It only governs the untoleranced features.

How does ISO 2768 compare to ASME Y14.5?

If you're working across international borders - sourcing parts from China for a US-designed product, or vice versa - you'll encounter both ISO 2768 and ASME Y14.5. They solve a similar problem but approach it differently.

Aspect	ISO 2768	ASME Y14.5
Origin	International (ISO)	United States (ASME)
Scope	General tolerances for untoleranced features	Full GD&T framework including general and specific tolerances
Default tolerances	Yes - 4 dimensional classes, 3 geometrical classes	Yes - Rule #1 (envelope principle) provides default form control
Drawing callout	“ISO 2768-mK” in title block	Title block reference to ASME Y14.5
Approach to form	Separate geometrical tolerance classes (H, K, L)	Envelope principle: form controlled by size tolerance by default
Symmetry and position	ISO uses symmetry tolerance	ASME uses position tolerance (symmetry deprecated in 2009)
Adoption	Europe, Asia, most international manufacturing	Primarily North America

The practical difference matters when you send a drawing with ASME conventions to a factory using ISO standards - or the other way around. A Chinese factory receiving an ASME drawing may interpret tolerance zones differently than intended, particularly for form tolerances where the envelope principle doesn't apply under ISO. For more on navigating these differences, see our FAQ on sourcing CNC machined parts from China.

Sidenote. If your drawing references ISO 2768 and the manufacturing happens in the US, add a note clarifying the standard. Don't assume the machine shop knows ISO conventions - many US shops default to ASME Y14.5 interpretations.

How does ISO 2768 affect manufacturing costs?

Every step tighter on the tolerance class costs more. That's not a vague rule of thumb - it directly drives machining time, tool selection, and inspection requirements.

The relationship between tolerance and cost is exponential, not linear. According to industry analysis of machining quotes, halving a tolerance (e.g., moving from ±0.1mm to ±0.05mm) typically increases the cost of that feature by 1.5-2x. Pushing to ±0.01mm can mean a 4-8x cost multiplier, because you're now requiring secondary operations like precision grinding.

Here's how that maps to ISO 2768 classes:

• Class v (very coarse): Achievable with flame cutting, waterjet, or a single rough machining pass. Minimal inspection. Lowest cost per part.
• Class c (coarse): Standard CNC machining with no special setup. Basic caliper inspection. This is where most non-critical parts live.
• Class m (medium): Requires controlled CNC parameters - proper feeds, sharp tooling, and stable fixturing. Inspection with calibrated instruments. The sweet spot for most functional parts.
• Class f (fine): Often requires finishing passes, tighter machine calibration, and potentially temperature-controlled environments for large parts. CMM inspection typical. Expect a meaningful cost premium over class m for complex parts.

The same principle applies to geometrical tolerances. Moving from class K to class H for flatness on a 300mm surface might mean adding a grinding operation - which can double the cycle time for that feature. For a detailed breakdown of how tolerancing affects CNC machining costs, including hourly rates and per-part pricing in China, that's worth reading separately.

The takeaway: don't specify tighter tolerances than your application actually needs. “ISO 2768-fH everywhere” isn't precision engineering - it's wasted money.

What are common mistakes when specifying ISO 2768?

After reviewing thousands of engineering drawings, these are the errors that cause the most problems in manufacturing:

1. No ISO 2768 callout at all. The drawing has no general tolerance reference in the title block. The factory has to guess - and every factory guesses differently. Some default to ISO 2768-m, others to their national equivalent (e.g., GB/T 1804 in China, DIN 7168 in older German drawings).
2. Assuming ISO 2768 covers threads. It doesn't. Threaded features need their own tolerance class callout (e.g., 6H for internal threads, 6g for external threads per ISO 965). If you leave threads untoleranced, the factory picks what's convenient - which may not be what you need.
3. Mixing tolerance classes on one drawing. Some engineers write “ISO 2768-fH” in the title block but then add coarse tolerances to non-critical features. That's technically fine - explicit tolerances override the general class. But it confuses the shop floor. If most features need coarse tolerances, call out ISO 2768-cL and add explicit tight tolerances only where needed.
4. Using ISO 2768-fH as a default “because tighter is better.” Fine + High is expensive to manufacture and inspect. Most CNC parts function perfectly under ISO 2768-mK. Specifying fH when mK would suffice inflates your quotes and extends lead times - without improving part function.
5. Forgetting that ISO 2768-2 doesn't cover all geometrical tolerances. Part 2 covers straightness, flatness, perpendicularity, symmetry, and runout. It does not cover parallelism, cylindricity, concentricity, profile, or position. If your part needs these, you must add explicit GD&T callouts.
6. Sending ISO 2768 drawings to shops that use ASME Y14.5. A US machine shop may not recognise “ISO 2768-mK” in the title block. They'll either ignore it (applying their own defaults) or misinterpret the geometrical tolerances. Always confirm which standard your manufacturer follows.

 

Frequently Asked Questions

Is ISO 2768 obsolete?

No. ISO 2768-1:1989 was last reviewed and confirmed by ISO in 2022 (stage 90.92 - “to be revised”), meaning it remains the current active standard. A draft revision (ISO/DIS 2768:2025) is in development, but the 1989 version is still what you should reference on drawings today.

What is the difference between ISO 2768-1 and ISO 2768-2?

ISO 2768-1 covers dimensional tolerances - how much a linear measurement (length, diameter, distance) or angular measurement can deviate from nominal. ISO 2768-2 covers geometrical tolerances - how much a feature's form (straightness, flatness), orientation (perpendicularity), location (symmetry), or runout can deviate. They work together: you specify both as a combined designation like ISO 2768-mK.

When should I use ISO 2768?

Use ISO 2768 on any machined part drawing where you want to simplify tolerancing. It's standard practice for CNC machined parts, sheet metal fabrications, and turned components. Avoid it for castings (use ISO 8062 instead), forgings (use ISO 8015/EN 10243), or purely 3D-printed parts where different tolerance conventions apply.

What tolerance does ISO 2768-mK give for a 100mm dimension?

Under ISO 2768-m, a 100mm nominal dimension falls in the “over 30 up to 120” range, giving a permissible deviation of ±0.3mm. The actual part can measure anywhere between 99.7mm and 100.3mm and still be within general tolerance.

Does ISO 2768 apply to 3D-printed parts?

ISO 2768 was written for machined parts (material removal processes). The achievable tolerances in FDM, SLS, or SLA don't reliably meet even the coarse (c) class for many features.

If you're 3D printing, specify tolerances explicitly or reference ISO/ASTM 52902 for additive manufacturing. For a detailed comparison, see CNC machining vs 3D printing.

What's the Chinese equivalent of ISO 2768?

China's national equivalent is GB/T 1804-2000, which was adopted as an equivalent of ISO 2768-1:1989. The tolerance values are identical across all four classes (f, m, c, v). If your drawing says ISO 2768, a Chinese factory working to GB/T 1804 is following the same tolerance values.

Can I use ISO 2768 and explicit GD&T on the same drawing?

Yes - this is standard practice. ISO 2768 provides the baseline for all untoleranced features, and any feature with an explicit tolerance callout is governed by that callout instead. The two systems complement each other: ISO 2768 handles the 90% of dimensions that don't need special attention, while explicit GD&T handles the 10% that do.

What is the difference between ISO 2768 and ISO 286?

ISO 2768 defines general tolerances for untoleranced features on a drawing. ISO 286 defines tolerance grades (IT grades) for specific fits between shafts and holes - it's what you use when you need an H7/g6 clearance fit or an H7/p6 press fit. They serve different purposes and are often used on the same drawing.

Get your tolerances right before you submit your next RFQ

Specifying the correct ISO 2768 class is one of the simplest ways to get faster, more accurate quotes. Too tight and you're overpaying. Too loose and you'll discover the problem at assembly - after the parts have shipped from the other side of the world.

If you're sourcing CNC machined or sheet metal parts and want to test how your tolerancing affects real factory quotes, submit an RFQ on Haizol with ISO 2768-mK on your drawing and compare what comes back from multiple verified factories.