ISO 2768 Tolerance Guide for CNC Machined Parts

ISO 2768 is widely used on engineering drawings to define general tolerances for dimensions without individual tolerance indications. For CNC machined parts, it provides a practical way to control non-critical dimensions without assigning a separate ± tolerance to every feature.

However, ISO 2768 does not mean that every dimension has the same allowable deviation. The applicable tolerance depends on the selected class, nominal dimension, type of feature, and edition of the standard referenced on the drawing.

This guide explains ISO 2768 tolerance classes, reference values, drawing notations, and practical applications in CNC machining. It also clarifies the status of ISO 2768-2, the role of ISO 22081, and when engineers should specify individual tolerances or geometric requirements.

Quick answer: Under ISO 2768-1:1989, a 50 mm linear dimension controlled by class m has a general tolerance of ±0.3 mm. A 10 mm dimension under the same class has a tolerance of ±0.2 mm. These values apply only where the relevant general tolerance is specified and no individual tolerance overrides it. Functional features may require tighter, separately defined requirements.

What Is ISO 2768 and Why Is It Used in CNC Machining?

ISO 2768 is a general tolerance standard used to simplify engineering drawings. Instead of specifying a tolerance beside every dimension, designers can reference an applicable standard and tolerance class in the drawing notes or title block.

This approach helps define acceptable manufacturing variation while keeping technical drawings easier to read.

For example, a CNC-machined aluminum housing may have several overall dimensions, pocket depths, external profiles, mounting holes, and chamfers. Some features affect assembly or performance, while others only define the general shape of the component.

Applying the same tight tolerance to all these features would often be unnecessary.

A general tolerance note allows non-critical dimensions to follow an established tolerance class. More demanding features can still receive individual tolerances based on their function.

How ISO 2768 Works on an Engineering Drawing

A traditional drawing may include the following note:

General tolerances: ISO 2768-m

Under the 1989 edition of ISO 2768-1, the letter m represents the medium general tolerance class for applicable linear and angular dimensions.

If a dimension has no individual tolerance indication, the relevant general tolerance can be determined from the nominal dimension and its applicable reference table.

Consider a drawing with the following dimensions:

• Overall length: 100 mm

• Overall width: 50 mm

• Pocket depth: 12 mm

• Precision bore: Ø12 H7

If the drawing references ISO 2768-1:1989 class m, the first three dimensions can be evaluated against the applicable general tolerance values, provided they fall within the standard's scope and no other requirement overrides them.

The Ø12 H7 bore, however, has its own fit-based size specification. It must be evaluated against that specific requirement rather than treated as an ordinary untoleranced dimension.

This distinction is essential when preparing CNC manufacturing instructions and inspection reports.

Why General Tolerances Matter to CNC Manufacturers

General tolerances help manufacturers and buyers establish a consistent interpretation of dimensions that are not individually toleranced.

They can support:

• Clearer communication between engineering and manufacturing teams

• More consistent quotation assumptions

• Reduced drawing complexity

• Practical control of non-critical dimensions

• More efficient machining and inspection planning

• Fewer disagreements about dimensional acceptance

However, ISO 2768 is not a guarantee of machining capability.

The fact that a drawing specifies a particular class does not automatically mean every machine, material, or component geometry can meet that requirement economically.

Manufacturers must still consider tool access, material behavior, workholding, part rigidity, and the required inspection method.

For project-specific manufacturing capabilities, see NAITE TECH's custom CNC machining services.

ISO 2768 Standards Status: Part 1, Part 2 and ISO 22081

Understanding the referenced standard edition is especially important when working with existing CNC drawings.

Many technical documents still reference ISO 2768-1 and ISO 2768-2 together, although their current publication status is different.

As of October 22, 2026, the ISO publications have the following status:

Source: ISO official standards catalog. Status checked October 22, 2026.

ISO 2768-1:1989 — General Dimensional Tolerances

ISO 2768-1:1989 establishes four tolerance classes for dimensions covered by its scope:

• f — Fine

• m — Medium

• c — Coarse

• v — Very coarse

The standard includes reference tables for linear dimensions, angular dimensions, and the specified broken-edge dimensions in its 1989 edition.

It is commonly referenced on drawings for machined components and fabricated parts.

When an existing drawing specifies ISO 2768-1:1989, its tolerances should be interpreted according to that edition, together with any applicable drawing notes and contractual requirements.

Official reference: ISO 2768-1:1989.

ISO 2768-2:1989 — Withdrawn Geometrical Tolerance Standard

ISO 2768-2:1989 previously defined general geometrical tolerances for features without individual geometrical tolerance indications.

It used three tolerance classes:

• H

• K

• L

These classes appeared in combined drawing notes such as ISO 2768-mK.

ISO withdrew Part 2 in February 2021, with ISO 22081:2021 identified as its replacement.

However, withdrawing the standard does not automatically make every previously issued engineering drawing unusable.

For a legacy drawing, the engineering and purchasing teams should identify the edition originally referenced, establish the contractual acceptance requirements, and confirm whether an updated drawing is needed.

Official reference: ISO 2768-2:1989 — Withdrawn.

ISO 22081:2021 — General Geometrical Specifications

ISO 22081:2021 provides rules for defining and interpreting general geometrical specifications and general size specifications within the ISO GPS system.

It is relevant when engineers want to define general geometrical requirements without placing an individual geometric tolerance indication on every applicable feature.

However, ISO 22081 does not simply recreate the H, K, and L classes from ISO 2768-2.

An existing ISO 2768-mK note should therefore not be automatically replaced with ISO 22081 without reviewing the drawing's geometrical specification strategy.

The designer may need to establish appropriate general geometrical requirements, datum relationships, and individually specified critical characteristics.

Official reference: ISO 22081:2021.

What Is Changing in the New ISO 2768 Edition?

ISO is preparing a revised edition intended to replace ISO 2768-1:1989.

The published revision information identifies changes intended to align the document with the current ISO Geometrical Product Specifications system.

The draft also identifies changes to the scope of the standard, including the removal of the previous general tolerance provisions for broken edges, external radii, and chamfer heights.

At the time of this article's technical review, the revised edition was still marked Under publication.

For new engineering drawings, confirm the edition actually published and required by the customer before adopting revised requirements.

Official status: ISO 2768 — Edition 2.

Engineering takeaway: Do not interpret tolerance values solely from the words “ISO 2768.” The referenced edition, selected tolerance class, and drawing-specific requirements must be clear.

ISO 2768 Tolerance Classes and Reference Tables

ISO 2768-1:1989 defines four general tolerance classes for applicable linear and angular dimensions.

The classes provide different permissible deviations depending on the nominal size or angular feature involved.

ISO 2768-f, m, c and v: What Is the Difference?

These descriptions explain the relative tolerance levels, not the capability of a particular manufacturing process.

A fine-class drawing is not automatically suitable for every precision assembly. Likewise, a medium-class drawing may still contain individually toleranced holes, surfaces, or other high-accuracy features.

The appropriate class should be selected according to the component's functional and manufacturing requirements.

ISO 2768-1 Linear Tolerance Reference

The permissible deviation increases as the nominal dimension moves into larger size ranges.

For example, the following values apply to a 50 mm linear dimension under ISO 2768-1:1989:

Representative example based on the nominal size range over 30 mm up to 120 mm in ISO 2768-1:1989.

This example shows why the tolerance class matters.

A 50 mm dimension does not automatically have a tolerance of ±0.1 mm or ±0.2 mm simply because the drawing mentions ISO 2768.

The selected class determines the applicable deviation.

ISO 2768-m Tolerance Examples

The medium class is frequently encountered on CNC engineering drawings.

The following representative dimensions show how the general permissible deviation changes with nominal size.

Reference: ISO 2768-1:1989, medium class. These are selected examples, not the complete standard table.

For example, consider a machined housing with a nominal overall length of 150 mm.

If the dimension is governed by ISO 2768-1:1989 class m, its applicable general deviation is ±0.5 mm.

The corresponding permissible size range is:

149.50 mm to 150.50 mm

If the assembly requires a substantially tighter overall length, the engineer should specify an appropriate individual tolerance.

For complete size ranges and boundary conditions, consult the applicable published ISO standard rather than relying solely on a shortened online reference.

ISO 2768 Angular Tolerances

ISO 2768-1:1989 also provides general tolerances for applicable angular dimensions.

Unlike linear tolerances, the permissible angular deviation is selected using the length of the shorter side associated with the angle.

For example, under the 1989 edition, for a feature whose shorter side is greater than 10 mm and no more than 50 mm:

These are angular deviations, not millimeter deviations.

They do not directly specify the flatness of a surface or the geometric position of a hole pattern.

If an angular relationship is functionally important, an individual angular or geometrical specification may be more appropriate.

Chamfers and Edge Radii Under the 1989 Edition

ISO 2768-1:1989 includes a separate reference table for certain broken-edge dimensions, including external radii and chamfer heights.

The permissible deviations in that table differ from the general linear dimension table.

For example, under the 1989 edition, a nominal chamfer height of 2 mm covered by the broken-edge provisions has a general deviation of ±0.2 mm for class m.

This should not be confused with the ±0.1 mm deviation applicable to an ordinary 2 mm linear dimension under the same class.

Engineers should also distinguish between:

• Chamfer height or size

• Chamfer angle

• External edge radius

• Internal corner radius

• General deburring or edge-breaking instructions

These are not necessarily controlled in the same way.

Because the revised ISO 2768 edition changes the treatment of broken-edge tolerances, designers should identify the referenced edition before applying any historical chamfer or radius values.

For functional chamfers, sealing edges, assembly lead-ins, and closely controlled radii, specifying the required dimensions directly is usually clearer.

What Do ISO 2768-m and ISO 2768-mK Mean on a Drawing?

Two common drawing notes are ISO 2768-m and ISO 2768-mK.

Although they look similar, they historically referred to different combinations of tolerance requirements.

ISO 2768-m: General Dimensional Tolerances

The notation ISO 2768-m is traditionally used to identify the medium class of general dimensional tolerances under ISO 2768-1.

It provides the applicable general tolerances for linear and angular dimensions covered by the referenced standard.

It does not mean that every dimension is controlled to ±0.1 mm.

For example:

• 10 mm → ±0.2 mm

• 50 mm → ±0.3 mm

• 150 mm → ±0.5 mm

These examples are based on ISO 2768-1:1989 class m.

The nominal dimension determines which permissible deviation applies.

ISO 2768-mK: Dimensional and Legacy Geometrical Tolerances

On traditional drawings, ISO 2768-mK combines two elements:

m: Medium dimensional tolerance class under ISO 2768-1:1989.

K: Geometrical tolerance class under the former ISO 2768-2:1989.

Historically, this notation allowed an engineer to identify both general dimensional and certain general geometrical tolerance requirements in a compact drawing note.

However, ISO 2768-2 has since been withdrawn.

If a customer sends a legacy drawing marked ISO 2768-mK, the manufacturer should not silently reinterpret the K class using ISO 22081.

Instead, confirm the original standard edition and whether its historical geometrical provisions remain contractually applicable.

Where the drawing is being revised, the design authority should establish an appropriate current specification strategy.

Example: Reading a CNC Drawing Title Block

Consider the following simplified drawing information:

In this example, the general tolerance note controls applicable dimensions without individual tolerance indications.

It does not override the bore tolerance, defined hole-position requirements, or other separately specified characteristics.

When reviewing old engineering drawings, remember that a note in the title block is part of the drawing specification, not simply a manufacturing suggestion.

Any proposed changes should be agreed with the customer or design authority before production.

Practical Example: ISO 2768 on a CNC Machined Aluminum Housing

To illustrate how general tolerances should be used, consider a hypothetical 6061-T6 aluminum housing manufactured by CNC milling.

The component contains an external profile, a machined pocket, a precision bore, mounting holes, and a sealing or locating surface.

The drawing references ISO 2768-1:1989 class m for applicable dimensions without individual tolerances.

This is an illustrative engineering example, not a documented customer project or an actual NAITE TECH inspection result.

Example Dimensions and Tolerance Requirements

The first three dimensions are examples of ordinary linear dimensions governed by the selected general tolerance.

The remaining features require additional engineering consideration.

General Dimensions: Overall Size and Pocket Depth

For the overall length:

60 ±0.30 mm

The acceptable size range is:

59.70–60.30 mm

For the housing depth:

20 ±0.20 mm

The acceptable depth range is:

19.80–20.20 mm

These are valid examples under the stated edition and class, assuming no more specific drawing requirement applies.

A manufacturer can use them to identify the dimensional acceptance range when planning production and inspection.

However, if the part must fit inside a closely controlled assembly envelope, even the overall housing dimensions may need individual tolerances.

General tolerance selection should therefore follow the product's function.

Precision Bores Need Individual Specifications

Suppose the housing contains a bore used to locate a bearing or alignment component.

A general ISO 2768-m tolerance may be too broad to establish the intended fit.

Instead, the drawing should specify the required bore size tolerance, such as an appropriate ISO limits-and-fits designation, selected according to the mating component and assembly requirements.

The corresponding location or orientation of that bore may also need geometric control.

The relevant manufacturing process might include precision boring, reaming, or another finishing operation.

The supplier should verify that the selected process can achieve the required result and that an appropriate measuring method is available.

Mounting Hole Positions and Datum References

Consider four mounting holes in the aluminum housing.

If these holes simply provide generous screw clearance, relatively broad variation may be acceptable.

If they align the housing with a precision assembly, the hole positions may require more rigorous control.

A datum-based position specification can communicate the intended relationship between the hole pattern and functional reference surfaces.

The designer should establish suitable datums based on how the housing is assembled and located.

It is not sufficient to assume that ISO 2768 general dimensional tolerances alone establish every required hole-position relationship.

Sealing and Mating Surfaces

A sealing face may require both flatness and surface-texture control.

These requirements are different from the general tolerance on the overall housing height or length.

For example, a designer may need to define:

• Flatness of a mounting or sealing face

• Parallelism relative to a functional datum

• Surface texture appropriate to the sealing method

• Critical distance between assembled surfaces

The exact values should be selected based on the mating component, seal design, operating conditions, and inspection method.

Applying an arbitrary tight tolerance without understanding the function can increase machining cost without improving the assembly.

For complex housings with pockets, mounting faces, and precision holes, CNC milling services should be evaluated together with the drawing's functional tolerance requirements.

Engineering takeaway: Use general tolerances where practical, but apply individual dimensional and geometrical specifications to features that determine fit, alignment, sealing, and performance.

When ISO 2768 Is Not Enough: Fits, GD&T and Critical Features

ISO 2768 provides a useful framework for general tolerances, but it cannot replace a complete functional tolerance strategy.

CNC components frequently contain features whose performance depends on more than their nominal size.

Hole and Shaft Fits

Bearing seats, dowel pin holes, bushings, precision shafts, and press-fit interfaces should be designed around their required mating conditions.

A nominal diameter and a general tolerance class may not define whether a fit will provide the necessary clearance, transition, or interference.

For these features, engineers should select appropriate limits and fits based on the actual assembly design.

The mating component's requirements must also be considered.

Geometrical Dimensioning and Tolerancing

Geometrical dimensioning and tolerancing, commonly called GD&T, provides a more specific way to define allowable variation in form, orientation, location, and other geometric characteristics.

Typical requirements include:

• Flatness

• Straightness

• Perpendicularity

• Parallelism

• Position

• Profile

• Circularity

• Runout

For example, a hole can meet its diameter tolerance but still be incorrectly located relative to the mounting datums.

Likewise, a sealing face can meet an overall thickness requirement while having unacceptable flatness.

General dimensional tolerances do not necessarily prevent these conditions.

Where function requires control of these geometric relationships, designers should use appropriate specifications under the applicable geometrical tolerancing system.

Critical Features Should Be Defined Separately

A practical CNC drawing distinguishes between three groups of requirements.

The goal is not to add more tolerance symbols to every drawing.

The goal is to describe the required manufactured condition without ambiguity.

For broader design recommendations, read NAITE TECH's CNC machining tolerance design guide.

How ISO 2768 Affects CNC Machining Cost and Inspection

Tolerance requirements influence more than the acceptable finished dimensions.

They can affect machining strategy, workholding, production time, inspection methods, and the risk of rejected components.

General Tolerances and Manufacturing Cost

For non-critical features, a suitable general tolerance can help avoid unnecessary machining and inspection work.

For example, there is usually little value in assigning the same tight tolerance to a cosmetic housing edge and a precision bearing bore.

The two features serve different purposes.

A tight bore may require careful setup, specialized cutting operations, and controlled measurement.

A non-functional edge may need only a practical dimensional allowance and an appropriate edge-finish requirement.

Using a consistent, function-based tolerance strategy helps the manufacturer focus resources where they contribute to the finished part's performance.

Does ISO 2768-f Always Cost More Than ISO 2768-m?

Not necessarily for every feature or component.

Class f allows smaller deviations than class m for many dimensions, but the actual manufacturing cost depends on whether those requirements approach the practical capability of the selected process.

A short, rigid aluminum part with accessible features may be relatively straightforward to machine.

A thin-wall housing, deep pocket, or large component may be more sensitive to material stress, cutting forces, tool deflection, and fixturing.

The same tolerance class can therefore create different manufacturing challenges on different parts.

During quotation, the supplier should evaluate the actual geometry instead of estimating cost from the tolerance class alone.

How General and Critical Dimensions Are Inspected

Inspection methods should be selected according to the characteristic being verified.

These are possible methods, not mandatory instruments for every part.

The actual measurement plan should consider tolerance magnitude, accessibility, measurement uncertainty, part condition, and contractual requirements.

For precision housings with multiple datums and hole patterns, CMM inspection can provide useful verification of geometric relationships.

Why First Article Inspection Matters

Before repeat production, a first article inspection can help confirm that the selected manufacturing process produces parts meeting the approved drawing requirements.

An inspection plan may include:

• General dimensions

• Individually toleranced critical features

• GD&T requirements

• Thread specifications

• Surface finish

• Material information

• Required documentation

The inspection scope should be agreed before manufacturing.

Not every project requires the same reporting level, and the applicable customer or industry requirements determine whether a formal first article inspection report is necessary.

For more information, see the First Article Inspection (FAI) guide for CNC machined parts.

NAITE TECH supports drawing-based dimensional inspection, including CMM and other measurement methods, according to the agreed project requirements.

Learn more about quality control and inspection capabilities.

Common ISO 2768 Drawing Mistakes and How to Avoid Them

Many tolerance-related manufacturing problems arise from unclear drawings rather than insufficient machine accuracy.

A drawing may contain the correct nominal geometry but leave important questions unanswered about the applicable standard, tolerances, and inspection requirements.

The following issues are worth checking before releasing a CNC machining RFQ.

1. Treating ISO 2768 as One Fixed Tolerance

A common mistake is assuming ISO 2768 always means ±0.1 mm or ±0.2 mm.

In reality, the permissible deviation depends on the selected class, dimension range, and feature category under the applicable edition.

Better approach: Confirm the exact standard edition, tolerance class, and nominal-size range.

2. Using General Tolerances for Precision Fits

General tolerances are not a substitute for selecting the proper clearance or interference fit.

Better approach: Specify critical bores and shafts individually using appropriate functional size requirements.

3. Continuing to Use ISO 2768-mK Without Checking the Edition

The K class comes from the withdrawn ISO 2768-2 standard.

A legacy drawing may still reference it, but the applicable historical requirements and contractual interpretation should be established.

Better approach: Confirm the original specification for legacy work. For new drawings, review the current geometrical tolerancing framework.

4. Confusing Dimensional and Geometrical Tolerances

Meeting the diameter tolerance of a hole does not necessarily mean its position or orientation is acceptable.

Better approach: Define functional geometric relationships separately where required.

5. Applying Tight General Tolerances to Every Feature

Selecting a strict tolerance class without considering component function can increase manufacturing and inspection effort.

Better approach: Evaluate whether tighter requirements are needed for the entire component or only selected critical features.

6. Using Ambiguous Drawing Notes

Notes such as “standard tolerance,” “normal machining tolerance,” or “high precision required” do not establish complete acceptance criteria.

Better approach: Identify the applicable standard, edition, tolerance class, and individual requirements clearly.

7. Ignoring the Effects of Surface Finishing

Anodizing, plating, coating, and other secondary operations can change finished dimensions.

Better approach: Specify which dimensional requirements apply to the final delivered condition and identify any relevant inspection stages.

8. Not Agreeing on Inspection Requirements

A manufacturer may produce a dimensionally acceptable component but still fail to provide the documentation expected by the customer.

Better approach: Confirm inspection scope, measurement requirements, sampling, and reporting before production.

CNC Drawing Review Checklist

Before submitting a drawing to a manufacturing supplier, confirm the following:

A drawing review completed before quotation can help identify unnecessary precision, missing specifications, and features that may be difficult to manufacture or inspect.

Need a review of your CNC drawing tolerances? NAITE TECH can evaluate your STEP model and 2D drawing to identify general and critical tolerance requirements, discuss machining feasibility, and prepare a project-specific quotation.

Explore our CNC machining capabilities.

Frequently Asked Questions About ISO 2768

What is ISO 2768 tolerance?

ISO 2768 provides general tolerancing rules for dimensions covered by the applicable standard and referenced on an engineering drawing. Under ISO 2768-1:1989, four classes—f, m, c, and v—define different permissible deviations for applicable linear and angular dimensions without individual tolerance indications.

What is the difference between ISO 2768-f, m, c and v?

The four classes represent fine, medium, coarse, and very coarse general tolerance levels. Class f generally allows smaller dimensional deviations, while class v permits larger deviations. The actual numerical tolerance depends on the nominal dimension and the relevant table in the referenced edition.

What does ISO 2768-mK mean on a drawing?

On traditional drawings, m identifies the medium dimensional tolerance class under ISO 2768-1, while K identifies a geometrical tolerance class from the former ISO 2768-2. Since ISO 2768-2 has been withdrawn, legacy drawings should be interpreted using their applicable editions and agreed requirements.

Is ISO 2768-2 still valid?

ISO 2768-2:1989 was withdrawn in February 2021 and replaced in the ISO catalog by ISO 22081:2021. However, withdrawn standards may still be referenced in legacy drawings and contractual specifications. Their applicability to a particular order should be confirmed with the customer or design authority.

What is the difference between ISO 2768 and ISO 22081?

ISO 2768-1:1989 establishes general dimensional tolerances using classes such as f, m, c, and v. ISO 22081:2021 provides rules for general geometrical specifications and general size specifications. It does not offer a direct, automatic substitution for the former ISO 2768-2 H, K, and L classes.

Does ISO 2768 apply to every dimension on a CNC drawing?

No. General tolerances apply according to the scope of the referenced standard and the drawing's indications. Dimensions with individual tolerances, certain excluded dimensions, and characteristics requiring specific geometrical control must be interpreted according to their applicable requirements.

Is ISO 2768-m suitable for precision CNC machining?

ISO 2768-m can be suitable for non-critical dimensions on many CNC machined parts. However, precision bores, bearing seats, alignment features, and sealing surfaces may require individual tolerances or GD&T. The selected requirements should reflect the part's function rather than relying on one general class for every feature.

When should CNC drawings use GD&T instead of general tolerances?

GD&T should be considered when a feature's position, form, orientation, or relationship to datums affects assembly or performance. Examples include precision hole patterns, mounting faces, sealing surfaces, and rotating components. General dimensional tolerances can remain useful for non-critical features.

Final Takeaway: Specify Clear Tolerances Before CNC Manufacturing

ISO 2768 helps simplify engineering drawings by establishing general tolerances for applicable dimensions without individual tolerance indications.

For CNC machined parts, its value comes from providing a common reference for non-critical dimensions while allowing engineers to define tighter requirements where function demands them.

The most important principles are straightforward:

• Confirm the ISO standard edition and tolerance class.

• Use the applicable reference values rather than assuming one fixed tolerance.

• Specify fits, critical dimensions, and geometric relationships individually where required.

• Review older ISO 2768-mK notes before applying them to new production.

• Agree on manufacturing and inspection requirements before placing an order.

A well-defined drawing can reduce uncertainty during quotation, machining, inspection, and final acceptance.

Request a CNC Machining Quote from NAITE TECH

NAITE TECH provides custom CNC machining for prototypes, low-volume orders, and repeat production, supported by drawing review and project-specific quality requirements.

If your drawing references ISO 2768 or includes critical dimensional and geometrical tolerances, our engineering team can review the requirements and evaluate a suitable manufacturing approach.

For a more accurate quotation, please provide:

• 3D CAD file, preferably STEP or a compatible format

• 2D technical drawing and revision

• Material grade and condition

• Required quantity

• General tolerance note and critical feature requirements

• Surface finishing specifications

• Inspection and documentation requirements

• Requested delivery date and destination

Request a CNC Machining Quote

Standards and Technical References

This guide uses the following official standards as its primary references:

1. ISO 2768-1:1989 — General tolerances, Part 1

2. ISO 2768-2:1989 — Withdrawn geometrical tolerance standard

3. ISO 22081:2021 — General geometrical and size specifications

4. ISO 2768, Edition 2 — Revised standard publication status

Standard status reviewed: October 22, 2026.

The numerical examples in this guide are based on ISO 2768-1:1989 and are provided for engineering explanation. They are not a substitute for the complete published standard, an approved engineering drawing, or a project-specific manufacturing agreement.

The information is intended to support technical understanding and supplier communication. Final manufacturing and inspection requirements should be established using the applicable drawing revision, referenced standards, and contractual specifications.