CNC machining tolerances are not simply a matter of "the smaller the better." Truly valuable tolerance standards enable design, machining, inspection, and purchasing to communicate in the same language: which dimensions are just general machining requirements, which hole-shaft fits must be controlled, which form and position errors will affect assembly, and which surface roughness will affect sealing, sliding, or fatigue life.
This compilation follows internationally accepted standards, Chinese national standards, Japanese JIS, German DIN, American ASME/ANSI, and British BS. It is suitable for CNC parts quotations, drawing review, overseas customer drawing conversion, and supplier quality communication. The values in this document are for engineering selection reference; formal acceptance should still be based on customer drawings, contract versions, and the original standard text.
I. What do CNC tolerance standards mainly cover?
Tolerances in machining drawings are generally divided into five categories:
- Dimensional tolerances:Allowable deviations for dimensions such as length, width, height, groove width, step, hole diameter, and shaft diameter.
- General tolerances:When tolerances are not specified separately on the drawings, the default rules uniformly applied in the title block shall be followed, such as ISO 2768-m.
- Fitting tolerances:Clearance fits, transition fits, or interference fits between holes and shafts, pins and holes, bearing housings and bearing outer rings, such as H7/h6.
- Geometric tolerances:Flatness, perpendicularity, coaxiality, position, profile, circular runout, etc., are commonly referred to as GD&T or ISO GPS.
- Surface texture and roughness:Ra, Rz, processing texture direction, deburring, chamfering, sharp edge treatment, etc.
II. ISO Tolerance System: The Most Common Basic Language in Global Trade
ISO 2768 ISO 2768-1 is the most common general tolerance standard for CNC common parts. It is used for linear and angular dimensions that are not individually specified. Common grades include f, m, c, and v, which can generally be understood as precision, medium, coarse, and very coarse, respectively. Many drawings will be written as "ISO 2768-m" or "ISO 2768-mK". Here, m controls linear and angular dimensions, and K usually corresponds to the geometric tolerance grades in the older version of ISO 2768-2.
ISO 286 It is the core standard for hole-shaft fits and IT tolerance grades. It uses letters to indicate the tolerance zone position and numbers to indicate the tolerance grade, such as H7, g6, and h6. Common combinations include H7/h6 for fine-position clearance fit, H7/g6 for small-clearance sliding fit, H7/k6 for transition fit, and H7/p6 for interference fit. When making bearing housings, locating pins, guide shafts, bushings, and couplings, general tolerances should not be written alone; the fit designation or upper and lower limit dimensions should be clearly specified.
ISO 1101 It is the core standard of ISO geometric tolerances, covering the symbolic language and interpretation rules for shape, orientation, position and runout tolerances. For multi-hole plate parts, pump valve bodies, fixtures, precision housings and multi-reference assemblies, simply using positive and negative dimensional tolerances can easily lead to ambiguity. Position, flatness, perpendicularity and profile are often better able to express functional requirements.
ISO 8015 It is a fundamental principle standard of ISO GPS, used to unify the basic concepts and interpretation principles of geometric product specifications. It reminds designers that requirements for dimensions, shapes, orientations, and positions should be clearly defined, and that a single dimensional tolerance cannot be assumed to automatically resolve all geometric errors.
ISO 22081 It is a newer general geometric specification standard used for the definition and interpretation of general geometric and dimensional specifications. It is important to note that ISO 22081 has replaced ISO 2768-2; for new projects, European clients, or drawings that strictly adhere to the new version of ISO GPS, it is essential to confirm with the client whether they accept ISO 22081, rather than continuing to use the older ISO 2768-2.
ISO 14405 Pay attention to the definition and measurement interpretation of linear dimensions. For "dimensional elements" such as hole diameter, shaft diameter, slot width, and distance between two parallel surfaces, it can help design and inspection clarify whether the measurement is a two-point dimension, an envelope dimension, a minimum circumscribed dimension, or a dimension in a statistical sense.
III. China's GB/T Tolerance System: Commonly Used Correspondences in Domestic CNC Machining
Common standards in Chinese machining drawings include: GB/T 1804、GB/T 1184、GB/T 1800/1801、GB/T 1182、GB/T 4249 GB/T 1804 is mainly used for unspecified linear and angular dimensional tolerances, and its engineering approach is similar to that of ISO 2768-1; GB/T 1184 is used for unspecified geometric tolerances, and its engineering approach corresponds to the older version of ISO 2768-2; the GB/T 1800 and GB/T 1801 series are used for limits and fits.
In domestic supply chain communication, common headings include phrases like "Unspecified tolerances are in accordance with GB/T 1804-m," "Unspecified geometric tolerances are in accordance with GB/T 1184-K," and "Unspecified chamfer C0.5, deburring sharp edges." If exporting parts to European or American customers, it is recommended to retain the customer's original standards and avoid arbitrarily modifying ASME or ISO drawings to GB/T standards before processing.
IV. Common Standards: JIS, DIN, ASME/ANSI, BS
JIS B 0405 It is a common general tolerance standard in Japanese drawings, used for linear and angular dimensions that are not separately marked, and its system is close to ISO 2768-1.JIS B 0401 Limits and fits used in ISO systems are commonly found in bearings, shafts, molds, and precision equipment parts.
DIN ISO 2768 This is very common in German and European drawings, and many older drawings still use DIN 7168 or DIN ISO 2768-mK. For CNC machining plants, when seeing DIN ISO 2768-mK, it is important to understand both the general dimensional tolerances and the general geometric tolerances, and not just quote prices based on linear dimensions.
ASME Y14.5 It is the core standard of American engineering drawings and GD&T, covering rules for symbols, datums, shapes, orientations, locations, profiles, and runouts. The ASME system is similar to ISO GPS in many symbols, but the default principles, modifiers, and interpretation methods are not entirely the same, especially in the interpretation of maximum physical conditions, inclusive principles, positional degrees, and profile degrees, which need to be implemented according to the standards specified in the drawings.
ASME B4.1 This standard is used for the selection of limits and fits for cylindrical parts in the imperial or US system, suitable for cylindrical fit scenarios such as shafts, holes, bushings, and pins. Both it and ISO 286 serve the purpose of "hole-shaft fits," but the units, grade systems, and tables cannot be simply substituted one-to-one.
BS 8888 It is the framework standard for British technical product documentation and engineering drawings, organizing many ISO technical product specifications into a single British standards system. When dealing with drawings from British clients, BS 8888 often doesn't provide a single dimensional tolerance table, but rather tells you which ISO/GPS rules should be followed to interpret the entire drawing.
V. Comparison Table of Major Tolerance Standards
| Standards system | Common Standards | Main uses | CNC Machining Focus | Typical drawing format |
|---|---|---|---|---|
| ISO International Standard | ISO 2768-1 | Linear and angular dimension tolerances not specified | Suitable for general machining dimensions, but critical mating dimensions cannot rely solely on it. | ISO 2768-m |
| ISO International Standard | ISO 286 | Hole and shaft limits and fits | For use in H7/h6, H7/g6, etc., it is necessary to consult tables or process according to customer limits. | Ø20 H7 / Ø20 h6 |
| ISO International Standard | ISO 1101 | Geometric tolerance symbols and explanations | Controlling functional errors such as position, flatness, perpendicularity, and profile. | Position degree ⌀0.05 ABC |
| ISO International Standard | ISO 22081 | General geometric specifications and general dimensional specifications | The new drawings need to be confirmed to determine whether they will replace the old ISO 2768-2. | General GPS ISO 22081 |
| China GB/T | GB/T 1804 | Linear and angular dimension tolerances not specified | Commonly used in domestic machining, grades such as m, c, and v are common. | Unspecified tolerances GB/T 1804-m |
| China GB/T | GB/T 1184 | No geometric tolerance noted | General controls for flatness, perpendicularity, symmetry, etc. | Unmarked geometric shapes GB/T 1184-K |
| Japan JIS | JIS B 0405 | General dimensional tolerances | Japanese customer drawings are common, and the design concept is similar to ISO 2768-1. | JIS B 0405-m |
| German DIN | DIN ISO 2768 | General dimensional and geometric tolerances | Old European blueprints often use combinations such as mK and fH. | DIN ISO 2768-mK |
| American ASME | ASME Y14.5 | GD&T Drawing Language | This term should not be confused with ISO GPS; you must refer to the title bar. | Per ASME Y14.5 |
| American ASME | ASME B4.1 | Preferred fit of cylindrical parts | Commonly used for inch-based hole-shaft fits; cannot be directly fitted with ISO 286. | Class fit / limits |
| UK BS | BS 8888 | Technical Product Documentation Framework | Drawings are typically interpreted using ISO/GPS rules. | Drawing to BS 8888 |
VI. How to choose the ISO 2768 level?
| grade | Common understanding | Applicable parts | Quotation and processing suggestions |
|---|---|---|---|
| f / fine | More precise | Positioning surfaces, precision supports, and parts with tight assembly relationships | It requires stable cutting tools, fixtures, and inspection solutions, resulting in higher costs than conventional machining. |
| m / medium | Medium grade, most common | General CNC aluminum, steel, and stainless steel parts | Suitable as the default tolerance for unspecified dimensions, but critical holes still need to be individually specified. |
| c / coarse | coarse | Non-critical shapes, post-weld machining, rough-machined parts | Suitable for cost reduction, but assembly dimensions should not be used. |
| v / very coarse | Very rough | Large parts, non-mating contours, and blank related dimensions | Suitable for non-functional size requirements, but should be avoided for misuse in mating areas. |
VII. Practical Tolerance Reference for Commonly Used CNC Machining
In the absence of mandatory customer standards, factories often establish empirical values based on processing capabilities and intended use. For ordinary three-axis CNC milling of aluminum alloy parts, non-critical dimensions are commonly referenced to ±0.10 mm to ±0.20 mm; more critical locating surfaces, groove widths, and hole spacing can be controlled to approximately ±0.05 mm; precision holes, bearing housings, and sealing surfaces should be individually confirmed according to fit, tolerance zones, and inspection methods. For stainless steel, titanium alloys, thin-walled parts, long shafts, and post-weld machined parts, due to more pronounced deformation and heat-affected zones, it is not advisable to directly apply the empirical values for aluminum parts.
For procurement, a good request for quotation (RFQ) package should at least include: 3D model, 2D drawings, material grade, heat treatment condition, surface treatment, critical dimensions, acceptance criteria, test report requirements, and batch quantity. Providing only STEP documents without tolerance standards forces suppliers to quote based on standard processing capabilities, easily leading to issues where the material can be manufactured but not assembled.
VIII. Examples of Common Labeling Methods
- Unspecified dimensional tolerances: General tolerances ISO 2768-m.
- Unspecified dimensions and geometric tolerances: General tolerances ISO 2768-mK, commonly seen in older drawings; for new projects, it is necessary to confirm whether to switch to ISO 22081.
- For domestic drawings: unspecified linear and angular dimensional tolerances shall conform to GB/T 1804-m, and unspecified geometric tolerances shall conform to GB/T 1184-K.
- Hole-shaft fit: Ø10 H7, Ø10 h6, Ø20 H7/g6.
- American drawings: Dimensioning and tolerancing per ASME Y14.5.
- Surface roughness: Ra 1.6, Ra 3.2, and indicate whether deburring, chamfering, texture direction or scratching is prohibited.
9. The most common mistakes during drawing review
- Treat general tolerances as fit tolerances:Hole shafts, pin holes, bearing seats, and sealing grooves must be labeled separately.
- Only dimensions are specified, not the reference datum.For multi-hole parts, the reference points A, B, and C need to be clearly defined; otherwise, the inspection coordinate system may be inconsistent.
- Mixing ASME and ISO standards:The two systems should not be assumed to be equivalent simply because the symbols are similar; they should be interpreted according to the standards specified in the title block.
- Ignore material and process deformation:Thin-walled aluminum parts, stainless steel welded parts, and heat-treated parts need to have deformation control plans in place.
- The testing method was not specified.The results from CMM, plug gauge, ring gauge, micrometer, and roughness tester may have different focuses, and the inspection method for critical dimensions should be agreed upon.
- Excessive tolerances led to a surge in costs:Non-functional dimensions should not be uniformly written as ±0.01 mm; high precision should be reserved for dimensions that truly affect assembly and performance.
10. Summary: Recommendations for Selecting Tolerance Standards
For general export CNC parts, ISO 2768-m is usually a more easily understood starting point for communication; if hole-shaft fits are involved, ISO 286 or ASME B4.1 should be used; if assembly position, plane, perpendicularity, coaxiality, or profile are involved, ISO 1101 or ASME Y14.5 should be used; for domestic projects, GB/T 1804, GB/T 1184, and GB/T limit fit systems can be followed; for drawings from Japanese, German, or British customers, the original interpretation rules of JIS, DIN, or BS 8888 should be retained.
For CNC machining plants, tolerance standards are not only acceptance criteria but also a language of cost. Clearly distinguishing between general dimensions, critical fits, geometric tolerances, and surface requirements is essential to ensuring assembly reliability while keeping machining costs within a reasonable range.
Reference standards and materials
- ISO 2768-1: General tolerances, linear and angular dimensions without individual tolerance indications.
- ISO 286-1: ISO code system for tolerances on linear sizes, basis of tolerances, deviations and fits.
- ISO 1101: Geometrical tolerancing, tolerances of form, orientation, location and run-out.
- ISO 8015: GPS fundamentals, concepts, principles and rules.
- ISO 22081: General geometrical specifications and general size specifications.
- ASME Y14.5: Dimensioning and Tolerancing.
- ASME B4.1: Preferred Limits and Fits for Cylindrical Parts.
- BS 8888: Technical product documentation and specification.
