ISO 2768-mK Tolerance Chart: Meaning, Classes & Limits

ISO 2768-mK combines class m general linear and angular tolerances from ISO 2768-1 with legacy class K geometric tolerances from the now-withdrawn ISO 2768-2. The ISO 2768-1 chart below applies only to eligible dimensions that do not already have an individual tolerance.

Use the tables as a drawing-review aid, then confirm the licensed edition and contract requirements. An mK note does not define every critical interface, datum or inspection condition. For new or revised drawings, set functional dimensions and geometric controls deliberately instead of copying an old mK or fH title-block note. Our sheet metal tolerance capabilities explain the manufacturing review that should accompany those decisions.

For an OEM RFQ, send the revision-controlled drawing, nominated tolerance class, functional datums and the state in which each feature is inspected. Press-brake formed sheet-metal parts and assembled OEM sheet-metal components require different inspection boundaries even when the same general tolerance note appears on both drawings.

Current ISO 2768 status in 2026

The official ISO catalogue is the right place to check status:

• ISO 2768-1
  remains published. ISO says it was reviewed and confirmed in 2022, and a replacement revision is under development.
• ISO 2768-2
  is withdrawn. Its H, K and L classes still appear on legacy drawings, but withdrawal matters when creating or revising controlled documentation.
• ISO 22081
  is the published successor identified on ISO’s own lifecycle pages. It defines rules for general geometrical and general size specifications; it should not be assumed to translate every legacy K, H or L note automatically.

That does not make every existing ISO 2768-mK drawing unusable. It means the buyer should preserve the approved drawing basis, avoid silently changing interpretation, and state which revision or successor GPS standard governs new work.

Does ISO 22081 automatically replace ISO 2768-mK on my drawing?

No. ISO identifies ISO 22081 as the successor to withdrawn ISO 2768-2, but changing the title block can also change which features and geometrical specifications are controlled. The design authority must compare the approved legacy interpretation with the intended new specification and release the drawing revision before manufacturing.

For an unchanged legacy order, preserve the contractually approved note and clarify ambiguity with the buyer. For a new or revised design, state the selected dimensional standard, geometric standard, drawing edition, applicable features and inspection basis explicitly.

What ISO 2768-1 controls

ISO 2768-1 is intended to simplify drawings by assigning general tolerances to dimensions that do not carry an individual tolerance. It covers four classes:

Class	Meaning	Typical drawing intent
f	Fine	Features that need closer general dimensional control
m	Medium	General commercial dimensions where process capability supports the class
c	Coarse	Fabricated or less critical dimensions
v	Very coarse	Large, non-critical dimensions

The standard applies to eligible linear dimensions, angular dimensions and broken-edge dimensions. It does not override an explicit dimension tolerance, a framed theoretically exact dimension, another governing standard or a customer-specific requirement.

The practical hierarchy on a drawing should be clear:

1. A feature-specific tolerance or GD&T control governs that feature.
2. A customer or product standard governs where the contract says it does.
3. ISO 2768-1 applies only to eligible dimensions left without individual tolerances.

ISO 2768-1 linear tolerance table

The values below are a working reference for nominal linear dimensions. The purchased standard and the contract revision remain authoritative.

Nominal length (mm)	f	m	c	v
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	+/-1.0
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 1,000	+/-0.3	+/-0.8	+/-2.0	+/-4.0
Over 1,000 to 2,000	+/-0.5	+/-1.2	+/-3.0	+/-6.0
Over 2,000 to 4,000	-	+/-2.0	+/-4.0	+/-8.0

For example, a 50 mm untoleranced dimension under class m has a general tolerance of +/-0.3 mm. That does not mean every relationship involving that feature is controlled: hole position, profile, flatness and perpendicularity may require separate geometric controls.

Angular dimensions and bent sheet metal

For angular dimensions, the tolerance band depends on the length of the shorter side forming the angle.

Shorter side length (mm)	f / m	c	v
Up to 10	+/-1 degree	+/-1 degree 30 minutes	+/-3 degrees
Over 10 to 50	+/-30 minutes	+/-1 degree	+/-2 degrees
Over 50 to 120	+/-20 minutes	+/-30 minutes	+/-1 degree
Over 120 to 400	+/-10 minutes	+/-15 minutes	+/-30 minutes
Over 400	+/-5 minutes	+/-10 minutes	+/-20 minutes

This table is frequently misused on press-brake parts. An angular tolerance alone does not control the final flange-tip position. Material thickness, inside radius, springback, bend deduction and the distance from the bend to the measured point all affect the resulting linear location.

For a mating flange, the drawing may need a functional hole position, profile or finished envelope requirement rather than only a general bend-angle class. Our press brake bending guide explains the manufacturing side of that decision.

What mK and fH mean on legacy drawings

On a legacy note such as ISO 2768-mK:

• m refers to the medium linear/angular class from ISO 2768-1.
• K refers to the medium geometric class from the now-withdrawn ISO 2768-2.

Likewise, fH historically combined fine dimensional and fine geometric classes. These codes remain important search terms and still appear in supply chains, but a supplier should not guess how a legacy geometric class interacts with newer ISO GPS rules.

For an existing approved drawing, record the exact drawing revision and standard basis during contract review. For a new drawing, the design authority should choose current dimensional and geometric standards and state them explicitly.

A better title-block approach

For new work, a controlled note should identify the actual requirement rather than rely on shorthand alone. A possible structure is:

General linear and angular tolerances:
ISO 2768-1:1989, class m, unless otherwise specified.

Geometrical tolerances and drawing interpretation:
Per the project-designated current GPS standard and drawing notes.

This is an example format, not universal drawing language. Aerospace, automotive, medical and customer-controlled programs may require a different edition, ASME Y14.5, ISO 1101, a company standard or explicit feature controls.

Sheet metal example: what the note does and does not settle

Consider a laser-cut and bent electronics enclosure with a 200 mm body length, 80 mm flange depth and a connector cutout.

Under ISO 2768-1 class m, the general size tolerances can be read from the applicable ranges. However, the following questions still need drawing decisions:

• Is the connector cutout located from the flat blank or the finished bent datum?
• Does the lid need profile control to maintain a gasket gap?
• Is flange-tip position more important than the nominal bend angle?
• Does coating thickness affect a slot, hinge or insert fit?
• Is flatness measured before or after welding and finishing?

A real inspection plan follows assembly function. It does not simply measure every number against a general table and assume the product will fit.

Worked m-class example for a formed enclosure

Consider an untoleranced 80 mm linear feature on a drawing that expressly invokes ISO 2768-1 class m. The over 30 to 120 mm range gives a planning reference of +/-0.3 mm, so the dimensional interval is 79.7 to 80.3 mm if no other drawing requirement overrides it.

That arithmetic does not define hole true position, gasket-land flatness, coating buildup, free-state distortion or a relationship to a mating assembly. If the dimension is measured only after bending or welding, the drawing must also define the formed datum, restraint condition and inspection stage. Use the sheet-metal tolerance and inspection planning page to review those manufacturing questions before requesting a quote.

When fit is determined only after panels, rails, hinges or purchased hardware come together, define the functional datums and acceptance state at assembly level. The sheet metal assembly service page explains the commercial review scope for BOM boundaries, tolerance stacks and completed-interface inspection; ISO 2768 alone does not define those controls.

Turn the tolerance note into an enclosure RFQ

For a cover, formed body and mounting-plate kit, send the individual part drawings together with the assembly view. A general tolerance class is only one input to the quotation. Identify the interfaces that must work when the kit is assembled:

Interface	Add to the controlled drawing or inspection plan
Display or connector opening	Functional datum, individual location control where required, and the stage at which size is checked
Removable cover and body	Mating-part revision, finished gap or fit requirement, and any restraint used during measurement
Inserted standoff or bracket	Hardware part number, locating datum, installation side and the final assembly interface to check

For medical device sheet metal housings, the same package should distinguish housing components from the complete equipment enclosure. The OEM releases the interface requirements; the supplier confirms the fabrication and inspection scope before quoting. Our precision sheet metal fabrication services connect that review to the required cutting, forming, joining and finishing operations.

Formed parts, welded assemblies and process capability

ISO 2768 is a drawing-tolerance framework, not a promise that every process can hold every class. The supplier still needs to assess:

• Material grade, temper and thickness variation.
• Laser or punch feature capability.
• Press-brake tooling, bend sequence and springback.
• Weld shrinkage and fixture access.
• Coating buildup and masking.
• Measurement method and datum access.

A fine class can increase setup, fixturing, inspection or secondary machining, but there is no universal cost multiplier. The effect depends on which features are tight, how they are measured and whether the selected process is stable for the required quantity.

Common drawing mistakes

Writing only ISO 2768

The class is missing, so the general tolerance is incomplete. State the part, edition and class required by the drawing-control system.

Treating mK as a universal default

It may be appropriate on an approved legacy drawing, but the withdrawn status of ISO 2768-2 means new drawings need a deliberate geometric-tolerancing decision.

Mixing standards without an interpretation rule

Combining ISO general tolerances, ASME GD&T and customer notes can create conflicting defaults. The title block should say which standard controls each aspect.

Applying a general class to critical interfaces

Sealing faces, rail datums, bearing seats, connector patterns and multi-part stackups usually need explicit functional tolerances.

Ignoring inspection feasibility

If the datum is inaccessible after welding or the measurement condition is undefined, two inspectors can reach different conclusions. Define the state of the part, fixture method and sampling requirement before production.

RFQ and drawing review checklist

Before releasing a sheet metal drawing, confirm:

• The exact ISO 2768 part, edition and class are identified.
• Legacy mK, fH or cL notes have an agreed interpretation.
• Critical dimensions carry explicit tolerances or GD&T controls.
• The datum scheme matches how the part functions and can be inspected.
• Coating, welding and assembly state are included in acceptance conditions.
• Tolerance stackups have been checked for mating parts.
• The supplier has identified any feature that needs a different process or gauge.
• The first-article report format and sampling plan are defined.

ISO 2768-mK bottom line

On a legacy drawing, ISO 2768-mK means class m general dimensional tolerances plus the historical class K geometric framework. Preserve the approved drawing basis and resolve ambiguous features with the design authority; do not silently translate the note into a newer standard.

On a new or revised drawing, identify the governing standards and editions, apply explicit controls to functional interfaces and define the inspection state. For formed or assembled parts, send the drawing for a sheet-metal tolerance review so process capability, datums and measurement access can be checked before quotation.

Official references

• ISO 2768-1
  catalogue and scope
• ISO 2768-2
  withdrawn status and lifecycle
• ISO 22081
  general geometrical and size specifications

Public catalogue pages confirm status and scope. Use the licensed standard text and the contractually specified edition for production acceptance. A useful RFQ package includes the 2D drawing, 3D model, material, thickness, finish, mating-part information and critical-feature list; the design authority retains final responsibility for functional tolerances and drawing approval.