Previously, I provided you with a detailed introduction to ISO 2768 Tolerance Standards. Now, as the new general tolerance standard under the GPS system, ISO 22081:2021 has officially replaced ISO 2768-2. Furthermore, ISO 22081:2021 does not provide a default tolerance table that can directly replace the H, K, L grades. It specifies the definition and interpretation rules for general geometrical specifications and general size specifications, used to reduce repetitive annotations on drawings.
This article will introduce the core rules of ISO 22081:2021, the differences from ISO 2768-2, and how to apply these requirements to CNC machining and inspection through drawing examples. I believe that after reading this, you will have a deeper understanding of it.
What Is ISO 22081:2021?
ISO 22081:2021 is an international standard within the ISO Geometrical Product Specifications (GPS) system that specifies the definition and interpretation rules for general geometrical specifications and general size specifications. It allows designers to centrally express common tolerance requirements in engineering drawings or product definition data, without the need to repeatedly annotate each dimension, thereby simplifying the drawings.
ISO 22081 mainly includes the following categories of general specifications:
| Specification | What It Controls | Typical Drawing Application |
| General geometrical specification | Geometry of applicable surfaces | General surface profile tolerance referenced to a datum system |
| General linear size specification | Linear sizes without an individual tolerance | A general ± tolerance or another defined size tolerance |
| General angular size specification | Angular sizes without an individual tolerance | A general angular tolerance |
| Variable general tolerance | Tolerance changes according to feature size or location | Defined through an additional table or referenced document |
Scope of ISO 22081
ISO 22081 general specifications apply only to integral features, including features of size. They do not apply to derived features or integral lines. For general size specifications, the standard covers linear and angular sizes; other types of dimensions are outside its scope.
How Are General Tolerances Specified Under ISO 22081?
ISO 22081 requires that general tolerance specifications should be clearly defined in the drawing, usually placed near the title block.
For example, a CNC machining drawing can specify:
| Drawing Requirement | Example |
| Standard | ISO 22081:2021 |
| General linear sizes | ±0.10 mm |
| General angular sizes | ±0.5° |
| General geometrical tolerance | Surface Profile 0.20 | A | B | C |
| Critical dimensions | Individually toleranced |
| Critical GD&T | Individually specified |
| Fits and precision holes | Specified separately where required |
Example title-block indication:
General tolerances ISO 22081
General geometrical specification: Profile 0.20 | A | B | C
Linear sizes: ±0.10 mm
Angular sizes: ±0.5°
Note:
The ±0.10 mm, ±0.5°, and 0.20 mm in the above table are only engineering application examples and are not the default tolerance values specified by ISO 22081. You should determine the actual tolerances based on part function, manufacturing capability, assembly requirements, and inspection methods.
ISO 22081 vs. ISO 2768-2: What Changed?
Actually, after ISO 22081:2021 replaced ISO 2768-2:1989, the most obvious change is: as designers or engineers, you no longer need to directly look up general geometric tolerances through H, K, L grades, but instead clearly specify general specifications and their tolerance values. This changed the way drawing expression requirements are presented.
| Comparison Item | ISO 2768-2:1989 | ISO 22081:2021 |
| Scope of Application | General geometrical tolerances not individually indicated | General geometrical specifications and general size specifications |
| Tolerance Values | Determined by tolerance classes (H, K, L) and standard rules | Explicitly specified values, or referenced via clear rules to tables and other documents |
| Geometric Control Method | Specifies general tolerance rules for straightness, flatness, perpendicularity, etc. | General geometrical specifications adopt profile tolerance of a surface |
| Datum Handling | Datum determined according to the rules of the corresponding geometric characteristic | When using general geometrical specifications, the datum system must be clearly specified as required by the standard |
| Drawing Indication | Can reference requirements using tolerance class symbols | In addition to the standard number, the adopted general specification must also be indicated |
| Applicability Determination | Applied per the coverage and exceptions of the legacy standard | Clearly distinguishes applicable features, size specifications, individual geometrical specifications, and related exceptions |
From Tolerance Classes to Explicit Specifications
In old drawings, “ISO 2768-mK” includes two requirements: lowercase m corresponds to the general dimensional tolerance class of ISO 2768-1, and uppercase K corresponds to the general geometric tolerance class of ISO 2768-2.
ISO 22081 does not provide a new grade to directly replace K. You need to determine tolerance values based on the function of the parts, and you must also enable machining and inspection parties to clearly find applicable values. Therefore, when updating drawings, you cannot simply replace “ISO 2768-mK” with “ISO 22081”.
General Geometrical Control Uses Surface Profile
ISO 22081’s general geometrical specification uses surface profile tolerance, in conjunction with theoretically exact geometry and a specified datum system, to express the permissible geometrical deviation for applicable surfaces.
How to Apply ISO 22081 on Your Drawings?
After introducing ISO 22081 and its comparison with ISO 2768-2, how to apply ISO 22081 on drawings is certainly a topic of great concern to you. Below, I will provide you with a detailed introduction, which is also one of the core contents of this article. In fact, to apply ISO 22081 on drawings, you need to clarify the content of general specifications, tolerance values, and scope of application.
For general geometrical specifications, you also need to define a compliant datum system. Simply writing “General tolerances ISO 22081” in the title block cannot fully express the acceptance requirements of the part.
Define Functional Requirements
First, you need to determine which features will directly affect the fit, positioning, sealing, and motion of parts, then set appropriate individual specifications for them. For example, bearing holes require clear dimensional fit requirements, while positioning holes may require position tolerance control, etc.
Then, after completing these functional requirements, you can determine which remaining features are suitable for general tolerances. This way, you can avoid insufficient requirements for critical features of the part, while also avoiding the unnecessary tightening of general tolerances for the entire part just for a few precision areas.
Establish the Datum System
When using general geometrical specifications, you should establish a datum system based on the assembly and positioning method of the parts, and express it clearly according to the relevant rules of ISO 22081.
To give a simple example, when milling brackets, you need to select the mounting base surface and positioning features to establish datums based on the actual installation relationships. The basis for your selection is also based on how these features determine the position and orientation of the part.
But note that, the datum system does not necessarily need to consist of three datums or constrain all six degrees of freedom. It only needs to constrain the degrees of freedom necessary to locate the tolerance zones defined by the general geometrical specification.
Specify the General Tolerance Values
For each part type, you should respectively determine the general geometrical specifications and general size specifications to be adopted:
- General geometrical specifications:Use surface profile, clearly define tolerance values and datum references.
- General size specifications: Clearly define applicable allowable deviations for linear or angular dimensions.
Tolerance values can be given directly or determined through tables or reference documents. If values that vary based on dimensions or other conditions are used, you must clearly state the basis for classification, the limits, and the rules for determining values. When referencing external documents or standards, you must also indicate the document number and applicable version.
Of course, there’s another point to note: when you select values, in addition to considering functional requirements, you must also take into account machining and inspection capabilities.
Add the Indication and Define the Nominal Geometry
In accordance with the annotation rules of ISO 22081, you must clearly indicate “General tolerances” and the standard number in or near the title block, along with the general geometrical specifications, general size specifications, or both that have been adopted.
At the same time, the drawing must also let the reader know what ideal geometry the tolerance is evaluated against. For complex contours, the theoretically correct geometry can also be provided through an explicitly referenced CAD model.
Check Coverage Before Releasing the Drawing
Finally, before releasing the drawings, you must check item by item to ensure that the general specifications cover the intended features, and especially not assume that general surface profile tolerance applies to all surfaces by default. The items to be checked are as follows:
| Inspection Item | What Needs to Be Confirmed |
| Critical Functional Features | Whether fit, sealing, and positioning requirements are fully defined |
| General Specifications | Whether tolerance values, units, determination rules, and reference documents are clearly specified |
| Datum System | Whether datum features, referencing order, and related requirements are clearly stated |
| Applicability Exceptions | Whether existing size specifications, individual geometrical specifications, and datum features are correctly handled |
| Simplified Representation Features | Whether threads, fillets, or edges not included in the CAD model have separately defined requirements |
| Document Consistency | Whether the versions of drawings, models, referenced standards, and inspection documents are consistent |
Of course, you must also remember to confirm with the manufacturer and the inspection agency that they understand the requirements and the verification methods.
What ISO 22081 Means for CNC Machining & Inspection?
For CNC machining and inspection, the main impact of ISO 22081 is to make general tolerance requirements more explicitly integrated into process planning and inspection workflows. Manufacturers need to identify which features of parts are controlled by general specifications, while inspection teams need to evaluate parts according to the same tolerance requirements, theoretically correct geometry and datum systems.
Machining Setups and Datum Alignment
The datum relationships on drawings will affect the clamping methods and machining sequence.
For example, consider a valve block in which the mounting bottom surface, side surface, and end surface establish the datum system. If the applicable surfaces are controlled by a general surface profile tolerance relative to this datum system, then when machining this valve block, it is necessary to consider the positional and orientational relationships between these surfaces and the datums, rather than just ensuring the length, width, and height dimensions separately.
Inspection Beyond Individual Dimensions
In fact, passing dimensional inspection of a part does not prove that it meets surface profile requirements. Calipers or micrometers can check applicable dimensional features, but the deviation of complex surfaces relative to the datum system cannot be completely evaluated based on just a few readings.
The CMM inspection system can compare the measured surface data with the theoretically correct geometry. When formulating the inspection plan, you still need to clarify the following points:
- Which version of drawings and CAD models to use;
- Which features are controlled by general specifications and which belong to applicable exceptions;
- How to establish measurement datums consistent with drawing requirements;
- Whether measurement points or scanning paths can cover the areas that need to be evaluated.
Furthermore, ISO 22081 does not mandate the use of a CMM, and the inspection agency should be selected based on the characteristics of the part being measured, tolerances, and required measurement capabilities.
Effects on Manufacturing and Inspection Costs
The impact of these factors cannot be overlooked. If general tolerances are set too tightly, more surfaces that do not inherently affect functionality will be subjected to strict control. This will increase the subsequent workload. On the other hand, incomplete requirements for parts can easily lead to differences in quotations.
Therefore, to address these issues, a more reasonable approach for you is to control key functional characteristics individually, and to set general specifications that meet the function for other applicable characteristics. At the same time, during the quotation stage, you should also specify the inspection scope, sampling requirements, and report content.
Checklist for Updating ISO 2768-2 Drawings
When updating old drawings to ISO 22081:2021, you need to re-examine the tolerance requirements and their scope of application, not just replace the standard number in the title block. I have prepared a checklist for you that can be used for review before drawing release.
| Check Item | Specific Action |
| ☐ Confirm the legacy standard reference | Verify the standard number, version, and grade; for “ISO 2768-mK,” identify dimensional and geometric requirements separately. |
| ☐ Review functional requirements | Check fit, location, sealing, and motion features; add individual dimensional or geometrical specifications as needed. |
| ☐ Clarify general specifications | Determine whether general geometrical specifications, general size specifications, or both apply. |
| ☐ Determine tolerance values | Specify the exact values or the rule for referencing tables; do not directly convert H, K, L grades into surface profile values. |
| ☐ Check the datum system | Confirm the datum features and reference order required for general geometrical specifications, based on actual function and locating relationships. |
| ☐ Verify the scope of application | Check for exceptions such as existing size specifications, individual geometrical specifications, and datum features to avoid missing callouts. |
| ☐ Clarify theoretically exact geometry | Confirm whether geometric information comes from the drawing or a specified CAD model, and note the necessary file identification. |
| ☐ Update documentation and inspection plans | Revise drawings, models, referenced documents, and inspection requirements accordingly; record substantive changes between old and new requirements. |
| ☐ Confirm changes and validate | Confirm the effective version with customers, suppliers, and quality personnel; arrange first-piece or first-batch validation based on change risk. |
Summary
Well, that’s all the content about ISO 22081:2021. It can be said that the core of ISO 22081:2021 is to make general tolerance requirements expressed more clearly. When you update old drawings, in addition to replacing the standard number, you also need to clarify tolerance values, datum systems, and scope of application. Besides controlling key functional features separately, you should also set reasonable general specifications for the remaining applicable features.
If your CNC part drawings are adopting or transitioning to ISO 22081, we welcome you to share drawings, CAD models, and key functional requirements with DSR. Additionally, as a professional CNC machining manufacturer, DSR can not only provide you with professional CNC machining services, but also discuss machining feasibility and inspection requirements based on specific parts. Please feel free to contact us with any needs you may have.
* Here, I have specially prepared a PDF file of the DSR ISO 22081:2021 General Tolerance Reference Chart for you to download and use.
FAQ
Q1: What is the ISO standard for GD&T?
A: In the ISO system, the core fundamental standard for GD&T is ISO 1101, complemented by standards such as ISO 5459, ISO 8015, and the ISO 14405 series.
Q2: What are ISO GPS standards?
A: ISO GPS (Geometrical Product Specifications) is a comprehensive ISO standard system used for defining, specifying, interpreting and verifying geometric requirements of products, covering dimensions, tolerances, geometric tolerances, datums, surface texture and measurement rules.
Q3: Are ISO standards used in the USA?
A: Yes. ISO standards are frequently used in American enterprises and engineering projects, especially in global supply chains, aerospace, automotive, medical devices, quality management, and international manufacturing projects.
Q4: What are the four main types of tolerances in engineering?
A: Form tolerances, orientation tolerances, location tolerances and runout tolerances.
Q5: Summary of ISO 22081:2021 requirements for machine tools?
A: ISO 22081:2021 is a general geometric tolerance standard that replaces the traditional ISO 2768-2. It requires comprehensive control over all geometric features without specified tolerances through unified profile tolerances combined with a clearly defined datum system. This approach replaces the previous scattered and vague handling of unspecified form, orientation, and location tolerances.
Q6:What is the US equivalent of ISO?
A:There is no single U.S. equivalent to ISO. ANSI coordinates U.S. national standards, while organizations such as ASME, ASTM, and SAE develop standards for specific engineering fields. For GD&T, ASME Y14.5 is widely used in the United States.
Q7: What are the three categories of tolerance?
A: Limit dimensions, unilateral tolerances, and bilateral tolerances.
