Every engineered part that gets manufactured carries a question at its core: how close is close enough? A drawing dimension of 50mm rarely means exactly 50.000mm — it means somewhere within an acceptable range. Define that range too tightly, and manufacturing costs climb. Define it too loosely, and parts fail to assemble or function as intended. Getting this balance right is what tolerance standards are designed for, and ISO 2768 is the one most widely used across global manufacturing.

ISO 2768 is the international standard that defines general machining tolerances for linear dimensions, angular dimensions, and geometric form — providing a default set of acceptable deviations for any feature on a drawing that doesn't carry its own individual tolerance callout. Whether you're producing a CNC-machined enclosure, a die cast bracket, or a sheet metal assembly, understanding what each ISO 2768 class means — and when to apply it — is one of the most practical skills an engineer or product designer can develop.

This guide covers both parts of the standard in full detail: what each tolerance class means, how to read the tables, what the common callout ISO 2768-mK actually tells your manufacturer, and how to avoid the over-tolerancing mistakes that quietly inflate manufacturing costs from prototype all the way to full production.

What Is ISO 2768?

ISO 2768 is an international standard published by the International Organization for Standardization that defines general tolerances for engineering drawings. Its core purpose is straightforward: instead of writing a specific tolerance value next to every single dimension on a technical drawing, an engineer can place one concise note in the drawing's title block — for example, ISO 2768-mK — and that single callout establishes the default permissible variation for all features that do not carry an explicitly specified individual tolerance.

The standard is divided into two complementary parts. ISO 2768-1 covers linear and angular dimensions — lengths, widths, heights, diameters, step sizes, external radii, chamfer heights, and angles. ISO 2768-2 covers geometrical tolerances, controlling the shape and relative position of features such as flatness, straightness, perpendicularity, symmetry, and circular run-out. Together, the two parts give manufacturers and design teams a shared, globally understood language for dimensional accuracy without the overhead of tolerancing every feature individually.

The standard primarily applies to parts produced by material removal processes — CNC milling, CNC turning, drilling, and grinding — as well as to parts formed from sheet metal. It is the dominant general tolerance standard across Europe and Asia, recognized by CNC machining suppliers worldwide, and serves as the foundation for most internationally sourced mechanical components.

Why General Tolerances Matter on Engineering Drawings

Without a general tolerance reference in the title block, every machine shop interprets untoleranced dimensions differently. Some default to national standards, others apply their own shop floor conventions, and some simply make their best judgment. This ambiguity creates real risk: parts that don't fit, assemblies that don't align, and inspection disputes that delay delivery. ISO 2768 eliminates that ambiguity with a single, globally understood callout that every qualified manufacturer can apply consistently.

There's also a cost dimension that engineers often underestimate. Specifying tolerances that are tighter than necessary inflates machining time, requires slower feed rates, demands more rigorous inspection, and increases the likelihood of scrap or rework. Specifying tolerances that are too loose, on the other hand, can cause assembly failures that are far more expensive to resolve once parts are in the field. ISO 2768 gives engineers the framework to calibrate this tradeoff deliberately — matching the level of precision to the functional requirement of each feature, rather than defaulting to a single tight standard across the board.

ISO 2768 Part 1: Linear and Angular Tolerance Classes

Part 1 of ISO 2768 defines four tolerance classes for linear and angular dimensions, each identified by a letter designation. The permissible deviation for any given dimension depends on both the tolerance class selected and the nominal size of the dimension — larger features carry proportionally wider tolerance bands. Here is a breakdown of what each class means in practice.

Class f – Fine

The fine class applies to high-precision components where tight dimensional control is genuinely required by function. For a nominal dimension in the 30–120mm range, for example, the permissible deviation under class f is ±0.15mm. This class is appropriate for bearing housings, sealing surfaces, precision mating interfaces, and critical alignment features. Because achieving fine tolerances requires careful process control, slower machining parameters, and more rigorous inspection protocols, specifying this class increases part cost and lead time. It should be reserved for the features where precision genuinely changes whether the part works — not applied broadly to a whole drawing.

Class m – Medium

The medium class is by far the most commonly used across general manufacturing, and for good reason. It strikes the optimal balance between precision and manufacturing cost, making it appropriate for the majority of CNC machined enclosures, brackets, structural housings, and non-critical mating components. For a 30–120mm nominal dimension, the permissible deviation under class m is ±0.3mm. Most standard CNC machining operations can meet medium tolerances without special fixturing, slower cycle times, or exceptional inspection effort, which keeps costs predictable. When a drawing specifies ISO 2768-mK, the 'm' refers to this class.

Class c – Coarse

The coarse class is suited to larger industrial components, structural parts, and features where dimensional variation has minimal impact on fit or function — for example, rib walls that provide structural reinforcement rather than dimensional alignment, or mounting surfaces that allow for adjustment. For a 30–120mm nominal dimension, the permissible deviation under class c is ±0.8mm. Coarse tolerances also apply to castings or formed parts before secondary machining operations, where the raw process naturally produces wider variation. Using this class where it's appropriate reduces cost without compromising part performance.

Class v – Very Coarse

The very coarse class permits the widest dimensional variation under ISO 2768 Part 1 and is used for parts where geometry is only loosely constrained by function — large castings, rough-formed structures, or features with no assembly or alignment role. For a 30–120mm dimension, the permissible deviation is ±1.5mm. Note that this class does not apply to nominal dimensions below 6mm, so it is unsuitable for small or detailed features. Very coarse is the appropriate starting point for parts that will undergo significant downstream processing or where form is secondary to material volume.

External Radii, Chamfers, and Angular Dimensions

ISO 2768 Part 1 also defines separate tolerance tables for external radii and chamfer heights, and for angular dimensions. For external radii and chamfers, the tolerance values are wider relative to linear dimensions at the same size range — a reflection of the inherent difficulty in holding tight edge geometry. For angular dimensions, the tolerance is expressed in degrees and minutes, with the applicable deviation based on the length of the shorter side of the angle. Importantly, for angular dimensions in the fine and medium classes, the permitted deviation values are identical across multiple size ranges, meaning these two classes converge at larger nominal sizes.

ISO 2768 Part 2: Geometrical Tolerance Classes H, K, and L

Where Part 1 governs the size of individual dimensions, Part 2 governs the shape and relative position of features. It covers five geometric characteristics: straightness, flatness, perpendicularity, symmetry, and circular run-out. The three tolerance classes are designated H, K, and L — representing increasing permissive deviation in that order.

Class H is the tightest geometrical class and applies to high-precision applications where form and position control are critical. A flat surface up to 100mm across, for instance, must lie within a 0.2mm zone under class H. This is appropriate for precision instrument housings, medical device components, and precision sealing faces.

Class K is the most common geometrical tolerance class in everyday manufacturing — the geometric counterpart to the 'm' class in Part 1. It provides practical form control for general CNC machined and sheet metal parts without imposing the cost of high-precision surface verification. A flat surface up to 100mm under class K must lie within a 0.4mm zone. Most well-controlled machining operations can achieve this as standard.

Class L permits the widest form variation and is appropriate for castings, weldments, and components where geometric form is less critical to function. It is less commonly specified in CNC machining drawings but relevant for formed or fabricated assemblies.

One important note: ISO 2768 Part 2 does not cover parallelism as a separate table. Instead, the standard defines parallelism tolerance as equal to the greater of the size tolerance or the flatness/straightness tolerance from Part 2. It also does not cover cylindricity, concentricity, profile, or true position — those require explicit GD&T callouts and are outside the scope of this standard.

What Does ISO 2768-mK Mean on a Drawing?

ISO 2768-mK is the most common general tolerance callout you will encounter on CNC machining and sheet metal drawings worldwide. It combines one class from each part of the standard: m from ISO 2768-1 (medium dimensional tolerance) and K from ISO 2768-2 (medium geometrical tolerance). Together, this single title-block notation tells the manufacturer: for every dimension on this drawing that doesn't carry its own individual tolerance, apply the medium class for size and the K class for form and position.

This pairing is the de facto industry default because it represents the sweet spot between cost and accuracy for the majority of general-purpose machined components. It is reproducible on standard CNC machining centres without special process controls, it keeps inspection straightforward, and it gives enough dimensional control for the vast majority of enclosures, brackets, housings, and structural components. Other valid combinations exist — ISO 2768-fH for high-precision work, ISO 2768-cL for rough castings — but mK is the starting assumption for most supplier relationships unless the drawing specifies otherwise.

How to Choose the Right Tolerance Class

Selecting a tolerance class is fundamentally a question of matching manufacturing precision to functional requirement — not defaulting to the tightest option available. Over-specifying tolerances is one of the most common ways product teams inflate CNC machining costs without improving part performance. The key is to distinguish between features that genuinely require dimensional control for fit, alignment, or sealing, and features whose primary purpose is structural, cosmetic, or simply spatial.

A practical framework works like this: start with ISO 2768-mK as your drawing baseline for all untoleranced features. Then identify the specific features where function demands tighter control — bearing bores, precision mating faces, sealing grooves, press-fit holes — and add explicit individual tolerances for those features on the drawing. This hybrid approach gives you the cost efficiency of general tolerances for the majority of your geometry while ensuring that the dimensions that actually determine whether the part works are controlled precisely.

Industry also plays a role in what class is appropriate. Components for aerospace or medical applications frequently require fine tolerances on critical features due to safety and reliability demands, whereas general industrial brackets or consumer electronics enclosures can comfortably operate within medium or coarse classes across most of their geometry. Material and process matter too: tighter tolerances are easier to achieve consistently in CNC machining than in casting or sheet metal forming, so the manufacturing process itself often dictates the practical floor for what's achievable without added cost.

ISO 2768 vs. ASME Y14.5: What's the Difference?

ISO 2768 and ASME Y14.5 both address tolerancing on engineering drawings, but they serve different purposes and are dominant in different regions. ISO 2768 is the standard for general tolerances — it sets a default baseline for every unspecified dimension using a single drawing-level callout, and it is the dominant standard in Europe, Asia, and most global supply chains. ASME Y14.5 is a comprehensive Geometric Dimensioning and Tolerancing (GD&T) system primarily used in North America, which provides a rich symbolic language to precisely control the form, orientation, and location of individual features.

The practical difference is one of scope and specificity. ISO 2768 is a broad tool that efficiently sets acceptable variation across an entire drawing. ASME Y14.5 is a precise instrument for controlling exactly how a specific feature must behave — useful when a part interfaces with many other components or when function depends on the geometric relationship between features. The two standards are not mutually exclusive: a common best practice, particularly for parts sourced internationally, is to use ISO 2768-mK as the general drawing standard and then add explicit individual GD&T callouts only for the two or three features where precise geometric control genuinely matters. This gives you the simplicity of ISO 2768 with targeted precision where needed.

If your customer base or supply chain is predominantly in North America, ASME Y14.5 may be the expected default. For European and Asian supply chains — including most rapid prototyping and manufacturing partners in China and Southeast Asia — ISO 2768 is the universally understood standard, and drawings that rely solely on ASME GD&T symbols risk being misread without additional guidance.

What ISO 2768 Does Not Cover

Understanding the limits of ISO 2768 is as important as understanding what it does cover. The standard explicitly does not apply to thread tolerances, surface roughness (Ra values), or any dimension that already carries an explicitly stated individual tolerance — individual callouts always take precedence over the general standard. It also does not apply to features manufactured by processes other than material removal unless specifically examined for compatibility with the standard's tolerance zones.

Within ISO 2768 Part 2, several geometric characteristics fall outside the scope of the standard entirely: cylindricity, concentricity, profile of a line or surface, and true position are not covered. If your design requires control over any of these characteristics — common in precision rotating assemblies, complex multi-component fits, or safety-critical structures — those features need explicit GD&T symbols and feature control frames on the drawing, regardless of the ISO 2768 callout in the title block.

Common Tolerancing Mistakes and How to Avoid Them

Several tolerancing errors show up repeatedly across manufacturing drawings, and each one either adds cost unnecessarily or creates quality problems downstream. The most expensive habit is applying a fine tolerance class across an entire drawing when only a handful of features actually need it. Tighter tolerances mean longer cycle times, more setup steps, higher inspection requirements, and a greater chance of scrap — and those costs multiply across every part in a production run. Apply fine tolerances selectively, only where function demands them.

A second common error is specifying no general tolerance callout at all. Without a reference in the title block, every manufacturer is left to interpret untoleranced dimensions according to their own conventions or national defaults. This leads to inconsistent results between suppliers, disputes at inspection, and the risk that a part technically meets the shop's internal standard while failing to assemble with its mating components. Always include a general tolerance designation.

Third, engineers sometimes forget to account for tolerance stack-up in assemblies. Each feature's permissible variation adds to the cumulative dimensional deviation across an assembly. If your design has a chain of several features all toleranced to the outer edge of the class m range, the assembly-level gap or interference could exceed what the design can accommodate — even though every individual part technically passes inspection. Reviewing tolerance accumulation during the design phase is especially important for multi-part assemblies with close-clearance fits.

Applying ISO 2768 with NICE Rapid

Understanding ISO 2768 tolerance classes is most valuable when it translates into better part drawings — drawings that communicate your precision requirements clearly, keep manufacturing costs in check, and produce parts that actually fit and function. At NICE Rapid, we work with engineering teams at every stage of this process, from early prototype to high-volume production, across a full portfolio of manufacturing processes.

For teams developing parts through CNC machining, specifying the right ISO 2768 class for your drawing baseline is one of the most direct levers you have over both cost and quality. The same discipline applies when parts move from prototype into tooled production — whether through plastic injection molding, pressure die casting, or sheet metal fabrication. Each process has its own natural dimensional capability, and aligning your tolerance class to that capability avoids unnecessary secondary operations and inspection overhead.

For teams working through rapid prototyping phases, NICE Rapid's 3D printing and vacuum casting services can produce functional prototypes that help validate tolerance requirements before committing to production tooling. Getting tolerance specifications right during prototyping means fewer drawing revisions and less rework as parts scale toward low volume, mid volume, and high volume manufacturing.

Conclusion

ISO 2768 is one of the most practical tools available to engineers designing for manufacture. By setting clear, globally understood defaults for dimensional and geometric variation, it eliminates ambiguity between design intent and shop floor execution — reducing cost, preventing assembly failures, and enabling consistent quality across international supply chains. The key is using it strategically: defaulting to ISO 2768-mK for the majority of your drawing geometry, applying fine tolerances only where function demands them, and adding explicit individual callouts for the critical features that fall outside the scope of the general standard.

Whether you're refining tolerance specifications for a CNC machined prototype or locking down drawing standards ahead of a full production run, the investment in getting tolerancing right at the drawing stage pays dividends at every subsequent step. Parts that meet their tolerance requirements reliably are parts that go together, work as designed, and don't generate rework costs that quietly erode project margins.