ISO 2768 defines how general tolerances apply when a CNC drawing does not specify exact limits. Many engineers rely on it every day, yet misunderstand what it really controls and where its limits begin.
Last Updated on April 28, 2026 by DZ Making Team
In CNC machining, tolerance decisions affect far more than dimensional accuracy. They influence machining methods, inspection effort, production cost, and even whether a part functions as intended. Misapplying ISO 2768 often leads to rework, supplier disputes, or unnecessary cost increases.
In this guide, you will learn how ISO 2768 works in real CNC production, how to choose the right tolerance class, and how to avoid common mistakes that impact manufacturability and performance.
What Is ISO 2768?
ISO 2768 is an international standard that defines general tolerances for dimensions and geometrical features when no specific tolerances are indicated on a technical drawing. Its purpose is to provide a clear default rule so engineers do not need to tolerate every single dimension.
In CNC machining, ISO 2768 acts as a shared reference between designers and manufacturers. When a drawing specifies ISO 2768, both sides understand the acceptable variation for unspecified dimensions, which reduces ambiguity and keeps drawings clean and readable.
The standard is divided into two parts:
- ISO 2768-1 covers general tolerances for linear and angular dimensions
- ISO 2768-2 covers general geometrical tolerances for features such as flatness and perpendicularity
These rules apply across industries, including mechanical engineering, industrial equipment, and custom CNC parts manufacturing. A critical point is that ISO 2768 only applies where tolerances are not explicitly defined. Any specified tolerance on the drawing always takes priority over ISO 2768.
ISO 2768 does not define functional fits or high-precision interfaces. Standards like ISO 286 or GD&T handle those requirements. Because of this, ISO 2768 works best as a communication framework rather than a precision tool. When used correctly, it simplifies drawings and accelerates CNC production. When misunderstood, it creates false expectations about achievable accuracy and part performance.
Why Does ISO 2768 Matter in CNC Machining?
The CNC machining industry depends on ISO 2768 because most CNC parts are highly customized. Unlike standard components, custom parts vary widely in geometry and application. Specifying tolerances for every dimension would overcomplicate drawings and slow down engineering and production.
In global CNC projects, the designer and the manufacturer are usually different parties. Engineers create drawings, while CNC suppliers interpret and produce them. In this setup, default tolerance rules become critical. ISO 2768 provides a shared reference that ensures consistent interpretation across borders and reduces miscommunication.
From a manufacturing viewpoint, ISO 2768 directly affects how a CNC job is handled. It influences quoting, since general tolerance levels impact machining time and cost assumptions. It also guides machining strategy, including setup planning and finishing requirements. Finally, it defines inspection effort, helping quality teams decide which dimensions need verification.
A Practical Overview of ISO 2768
ISO 2768 establishes a unified system for applying general tolerances in CNC machining without overloading technical drawings. Once referenced, it automatically defines acceptable variation for all unspecified dimensions and geometrical features. This approach allows engineers to focus on critical requirements while giving CNC manufacturers clear baseline limits.
ISO 2768-1: Linear and Angular Dimensions
ISO 2768-1 defines general tolerances for linear and angular dimensions when no individual limits are specified on a drawing. In CNC machining, this section governs most everyday dimensions, including lengths, widths, heights, diameters, chamfers, radii, and angles on non-functional features.
For custom CNC parts, ISO 2768-1 works as a default safeguard. It keeps overall part size, hole spacing, and wall thickness within reasonable variation, even when the designer does not tolerance each dimension explicitly. This approach is especially effective for structural or non-critical features where tighter control would increase cost without improving performance.
To understand how ISO 2768-1 applies in practice, it helps to look at its three main tolerance categories: linear dimensions, external radii and chamfer heights, and angular dimensions. Together, these tables define the baseline expectations CNC manufacturers use during machining and inspection.
Table 1: ISO 2768-1: Linear Tolerances
| Nominal Dimension (mm) | Fine (f) | Medium (m) | Coarse (c) | Very Coarse (v) |
| 0.5 – 3 | ±0.05 mm | ±0.10 mm | ±0.20 mm | – |
| >3 – 6 | ±0.05 mm | ±0.10 mm | ±0.30 mm | ±0.50 mm |
| >6 – 30 | ±0.10 mm | ±0.20 mm | ±0.50 mm | ±1.00 mm |
| >30 – 120 | ±0.15 mm | ±0.30 mm | ±0.80 mm | ±1.50 mm |
| >120 – 400 | ±0.20 mm | ±0.50 mm | ±1.20 mm | ±2.50 mm |
| >400 – 1000 | ±0.30 mm | ±0.80 mm | ±2.00 mm | ±4.00 mm |
| >1000 – 2000 | ±0.50 mm | ±1.20 mm | ±3.00 mm | ±6.00 mm |
| >2000 – 4000 | – | ±2.00 mm | ±4.00 mm | ±8.00 mm |
According to ISO 2768-1, when a basic dimension is less than 0.5 mm, its allowable deviation isn’t covered by the general tolerance tables. Instead, any permissible limits for these extremely small features must be specified directly next to the relevant dimension on the technical drawing. This avoids ambiguity and ensures all parties know exactly what precision is required for such fine details.
Table 2: ISO 2768-1: External Radii and Chamfer Heights Tolerances
| Nominal Size (mm) | Fine (f) | Medium (m) | Coarse (c) | Very Coarse (v) |
| ≤ 3 | ±0.20 | ±0.20 | ±0.40 | ±0.40 |
| >3 – 6 | ±0.30 | ±0.50 | ±0.60 | ±1.00 |
| >6 | ±0.50 | ±1.00 | ±1.50 | ±2.50 |
These tolerances apply specifically to external radii and chamfer heights as outlined in ISO 2768-1. For linear dimensions of chamfered parts (including the rounding of corners), the permissible deviations are structured by tolerance class and nominal size, ensuring clarity during design and inspection.
Note:
- For basic dimensions below 0.5 mm, the permissible deviations should be indicated directly adjacent to the relevant dimension.
- The values above are in millimeters and are intended as general guidelines for standard machining and fabrication processes.
- When working with components requiring tighter control, always specify the required tolerance class on the technical drawing.
This table helps streamline the tolerance selection process, making it easier to align with industry standards and ensuring consistent part quality across manufacturing projects.
Table 3: ISO 2768-1: Angular Tolerances
| Length of Angle Legs (mm) | Fine (f) | Medium (m) | Coarse (c) | Very Coarse (v) |
| ≤ 10 | ±1.0º | ±1.0° | ±1º30′ | ±3.0° |
| >10 – 50 | ±0º30′ | ±0º30′ | ±1.0° | ±2.0° |
| >50 – 120 | ±0º20′ | ±0º20′ | ±0º30′ | ±1.0° |
| >120 – 400 | ±0º10′ | ±0º10′ | ±0º15′ | ±0º30′ |
| >400 | ±0º5′ | ±0º5′ | ±0º10′ | ±0º20′ |
ISO 2768-2: General Geometrical Tolerances
ISO 2768-2 defines general geometrical tolerances for features without explicitly specified geometric controls, using three tolerance ranges: H, K, and L. In CNC machining, these ranges set default limits for shape and orientation when designers choose not to apply detailed GD&T controls.
In CNC production, ISO 2768-2 typically applies to features such as flat surfaces, cylindrical walls, straight edges, and perpendicular relationships that are not functionally critical. It provides a baseline for shape control when designers choose not to specify stricter requirements such as those in GD&T (geometric dimensioning and tolerancing).
The tolerance range (H, K, or L) reflects the required level of geometric control. H is the tightest, K is the most commonly used, and L allows the largest variation. In CNC production, K is often selected as a practical balance between functional stability and machining efficiency. The tables below summarize the general geometric tolerance limits commonly referenced in machining practice.
Table 4: ISO 2768-2: Straightness and Flatness Tolerances
| Nominal Length (mm) | H | K | L |
| ≤ 10 | 0.02 | 0.05 | 0.10 |
| >10 – 30 | 0.05 | 0.10 | 0.20 |
| >30 – 100 | 0.10 | 0.20 | 0.40 |
| >100 – 300 | 0.20 | 0.40 | 0.80 |
| >300 – 1000 | 0.30 | 0.60 | 1.20 |
| >1000 – 3000 | 0.40 | 0.80 | 1.60 |
Table 5: ISO 2768-2: Perpendicularity Tolerances
| Nominal Length (mm) | H | K | L |
| ≤ 100 | 0.20 | 0.40 | 0.60 |
| >100 – 300 | 0.30 | 0.60 | 1.00 |
| >300 – 1000 | 0.40 | 0.80 | 1.50 |
| >1000 – 3000 | 0.50 | 0.80 | 2.00 |
Table 6: ISO 2768-2: Symmetry Tolerances
| Nominal Length (mm) | H | K | L |
| ≤ 100 | 0.50 | 0.60 | 0.60 |
| >100 – 300 | 0.50 | 0.60 | 1.00 |
| >300 – 1000 | 0.50 | 0.80 | 1.50 |
| >1000 – 3000 | 0.50 | 1.00 | 2.00 |
Table 7: ISO 2768-2: Run-out Tolerances
| H | K | L |
| 0.10 | 0.20 | 0.50 |
ISO 2768 Tolerance Classes (f, m, c, v)
ISO 2768-1 defines four tolerance grades for general linear and angular dimensions:
- f (fine)
- m (medium)
- c (coarse)
- v (very coarse)
These grades accommodate a wide range of CNC manufacturing needs. Class f provides tighter dimensional control and typically requires more stable machining conditions and inspection effort. Class m is the most commonly used option for industrial CNC parts, offering a practical balance between accuracy and cost. Classes c and v allow larger variation and are suitable for non-functional or rough features where precision does not affect performance.
Typical ISO 2768 Tolerances for CNC Metal Parts
ISO 2768 is most commonly applied to metal CNC parts used in industrial equipment, machinery, and structural assemblies. In these applications, the standard provides predictable limits for non-critical dimensions while allowing manufacturers to machine parts efficiently.
In practice, the actual outcome of ISO 2768 tolerances depends on material type, part geometry, and machining method. Aluminum, steel, and stainless steel all behave differently under cutting forces, thermal load, and tool wear. ISO 2768 accounts for this by allowing reasonable variation rather than forcing unnecessary precision.
For most CNC metal parts, ISO 2768 tolerances work well for:
- Overall part dimensions
- Wall thickness and spacing
- Non-critical hole locations
- External profiles and covers
They are not intended for press fits, bearing seats, sealing surfaces, or motion-critical interfaces.
The table below summarizes typical applications of ISO 2768 tolerances in CNC metal machining, based on common industry practice.
| Material | Common CNC Application | Typical ISO 2768 Class | Notes |
| Aluminum alloys | Housings, brackets, frames | m | Stable machining, good cost balance |
| Carbon steel | Structural parts, plates | m / c | Higher cutting forces, thermal effects |
| Stainless steel | Covers, supports | m | Tool wear affects tight tolerances |
| Tool steel | Non-functional features | c | Precision features should be specified |
| Brass | Bushings, fittings | m | Good machinability, stable results |
How to Select the Right ISO 2768 Tolerance Grade in CNC Production?
Selecting the right ISO 2768 tolerance grade is a manufacturing decision, not a formatting choice. The grade you choose sets expectations for machining effort, inspection scope, and cost. In CNC production, the goal is to apply the loosest tolerance that still guarantees function.
Define Part Function First
Start by assessing each feature independently, not the part as a whole. Ask whether the part will still function if the dimension reaches the ISO 2768 limit. If the answer is no, that feature requires an explicit tolerance.
Features such as bearing seats, press fits, sliding surfaces, sealing faces, and datum-related interfaces should never rely on general tolerances. Small deviations in these areas directly affect performance and assembly. ISO 2768 works best for non-functional features like outer profiles, covers, ribs, and structural dimensions. General tolerances control size consistency, not functional behavior.
Align with the Machining Method
The machining process determines how reliably a tolerance grade can be achieved. CNC turning delivers excellent dimensional consistency on round features because the cutting forces are stable and symmetrical. In these cases, ISO 2768-m is usually safe, and selective use of ISO 2768-f may be realistic for short, rigid features.
CNC milling introduces more variability. Multiple setups, tool reach, and fixturing rigidity all affect accuracy. Applying ISO 2768-f across a complex milled part often increases cost without improving repeatability. Five-axis machining can reduce setup error but increases process complexity. Tighter grades should follow functional needs, not machine-capability assumptions.
Account for Material Behavior
Material behavior often determines whether a tolerance grade is stable or risky. Aluminum machines easily but deforms on thin walls and large flat surfaces. Stainless steel resists deformation but generates heat, leading to dimensional drift and tool wear. Engineering plastics relax after machining, changing size once the part is unclamped.
Applying ISO 2768-f to thin aluminum walls or plastic components frequently causes inspection failures, even when machining is done correctly. Medium grades usually deliver better consistency across batches.
Balance Precision and Cost
Tighter general tolerances increase cost across the entire part. They require slower feeds, additional finishing passes, and broader inspection coverage, even on non-critical features. In many cases, tightening one functional dimension explicitly costs less than tightening the overall tolerance grade. This approach keeps manufacturing efficient and drawings clear.
Best practice is to use ISO 2768-m as the default, then selectively override specific dimensions that control fit, alignment, or performance. This strategy delivers predictable quality, stable pricing, and scalable CNC manufacturing without paying for unnecessary precision.
Common Mistakes When Applying ISO 2768 in CNC Machining
ISO 2768 simplifies drawings, but it also introduces risk when applied without intent. Many CNC issues stem not from machining capability, but from how general tolerances are interpreted and used. The following mistakes appear frequently in real production and often lead to avoidable cost, rework, or assembly problems.
Overestimating ISO 2768 Precision Capability
A frequent error is assuming ISO 2768 guarantees CNC precision. In reality, ISO 2768 only defines the allowable tolerance range for unspecified dimensions, not the achievable CNC accuracy. Actual CNC results depend on setup stability, tool condition, machining strategy, and material behavior.
For example, in CNC milling, ISO 2768-m allows ±0.3 mm on a 100 mm feature. This range may be acceptable for CNC-machined housings or brackets, but it is unsuitable for alignment-critical or load-bearing features. Expecting CNC machining to compensate for loose general tolerances often leads to functional failure rather than machining defects.
Applying General Tolerances to Functional Features
Another common CNC design mistake is allowing ISO 2768 to control functional features. In CNC machining, features such as bearing bores, press-fit shafts, sliding guides, datum holes, and sealing grooves define how parts assemble and operate.
When these features rely on general CNC tolerances, parts may pass dimensional inspection but fail during CNC assembly or functional testing. The correct CNC practice is to use ISO 2768 for non-functional features while explicitly tolerancing all CNC features that control fit, motion, or sealing.
Mixing ISO 2768 With Conflicting Tolerances
CNC drawings often combine ISO 2768 with selective explicit tolerances, but without a clear hierarchy. This creates uncertainty for CNC manufacturers when interpreting the drawing and planning machining operations.
In CNC machining, unclear tolerance priority leads to inconsistent quotes, different machining strategies, and uneven inspection results across suppliers. ISO 2768 should act as the default CNC tolerance rule, with explicit tolerances clearly overriding it where necessary and never contradicting it.
Ignoring Material and Machining Process Limitations
ISO 2768 does not account for how materials behave during CNC machining. Thin aluminum walls can deflect under cutting forces, stainless steel can shift due to heat buildup, and plastics often change size after machining stress is released.
Applying tight ISO 2768 CNC tolerances without considering machining method and material response increases scrap and rework. Stable CNC production comes from matching tolerance grades to real CNC process capability, not theoretical limits.
ISO 2768 vs ISO 286 in CNC Manufacturing
ISO 2768 and ISO 286 serve different purposes in CNC manufacturing, yet they are often confused or used interchangeably. In practice, each standard controls a different type of variation, and understanding their roles helps engineers choose the right tolerance strategy for CNC machined parts.
General Tolerances vs Fit Tolerances
ISO 2768 defines general tolerances for unspecified dimensions in CNC drawings. It controls overall size, shape, and orientation where tight control is not critical. This approach keeps CNC drawings readable and avoids over-tolerancing.
ISO 286, by contrast, defines fit tolerances for mating features, such as holes and shafts. It specifies how parts assemble, slide, or press together in CNC applications. ISO 286 focuses on functional relationships, not general size variation. In CNC machining, ISO 2768 manages background variation, while ISO 286 controls interfaces.
Simplicity vs Precision
From a CNC design perspective, ISO 2768 favors simplicity. A single reference applies tolerances across many dimensions, reducing drawing clutter and speeding CNC programming.
ISO 286 prioritizes precision. Each fit is explicitly defined using tolerance classes such as H7, g6, or h6. This precision is essential for repeatable CNC assembly but increases drawing complexity and inspection effort. Simplicity supports efficiency; precision supports function. CNC engineers must decide which matters more for each feature.
Cost Efficiency vs Functional Control
ISO 2768 often lowers CNC machining cost by allowing wider variation on non-critical features. It reduces machining time, inspection scope, and setup sensitivity.
ISO 286 increases cost but delivers predictable functional performance. Tight fits require controlled CNC processes, slower cutting parameters, and more detailed inspection. In CNC manufacturing, applying ISO 286 only where function demands it is usually more cost-effective than tightening general tolerances across the entire part.
When to Use Each Standard
The table below shows how ISO 2768 and ISO 286 are typically combined in CNC machining.
| CNC Feature | ISO 2768 | ISO 286 | Practical CNC Reasoning |
| Overall part size | ✔ | – | Function not affected by minor variation |
| Structural brackets | ✔ | – | Alignment tolerance is forgiving |
| Cosmetic covers | ✔ | – | Appearance more important than fit |
| Bearing seats | – | ✔ | Fit directly affects performance |
| Sliding shafts | – | ✔ | Clearance controls motion |
| Press-fit pins | – | ✔ | Interference must be controlled |
In CNC manufacturing, ISO 2768 sets the foundation, while ISO 286 defines the interfaces. Combining them deliberately results in clear drawings, stable machining, and reliable assembly.
Conclusion
ISO 2768 is most effective when it is used as a deliberate tolerance framework in CNC machining, not as a shortcut for engineering decisions. It helps control general variation, keep drawings clear, and support efficient CNC production, but it cannot replace functional tolerances or fit standards where performance matters. The real value of ISO 2768 comes from knowing when it is sufficient and when it must be overridden based on part function, material behavior, and machining process.
In practice, applying ISO 2768 correctly often requires manufacturing insight beyond the standard itself. At DZ Making, we support engineers with custom CNC parts by combining ISO-compliant tolerances, practical DFM feedback, and stable machining processes. If you are developing custom CNC parts and want tolerances that match function, cost, and manufacturability, share your drawings with us for a professional CNC tolerance review and production support.
FAQs
1. Is ISO 2768 suitable for precision CNC parts?
No. ISO 2768 defines general tolerances and is not suitable for precision CNC features such as fits, sealing surfaces, or alignment-critical geometry. These require explicit tolerances or standards like ISO 286.
2. What does ISO 2768-mK mean on a CNC drawing?
The “m” specifies the medium tolerance class for linear and angular dimensions (ISO 2768-1). “K” specifies the medium tolerance range for geometrical features (ISO 2768-2).
3. Can ISO 2768 be used together with ISO 286?
Yes. ISO 2768 controls general, non-critical CNC dimensions, while ISO 286 defines fits for mating features such as holes and shafts. They are commonly combined on the same CNC drawing.
4. Does ISO 2768 affect CNC machining cost?
Yes. Tighter ISO 2768 grades increase CNC machining time and inspection effort. Using ISO 2768-m by default and tightening only critical features helps control cost.
5. Is ISO 2768 accepted worldwide for CNC manufacturing?
Yes. ISO 2768 is widely recognized in global CNC manufacturing and commonly used in international sourcing and cross-border production projects.
