Every dimension on a drawing needs a tolerance. Specifying one individually for all of them is laborious and clutters the drawing, so general tolerance standards exist to cover everything not explicitly toleranced.
ISO 2768 is the most widely used of these, and it appears in a title block as something like “ISO 2768-mK”. Many engineers copy that notation from a previous drawing without knowing what it commits them to, which produces two opposite problems: parts made looser than intended, or general tolerances tighter than anything actually requires.
This guide covers what the standard means, what tolerance levels are realistically achievable in machining, and how tolerance choice translates into cost.
What ISO 2768 Does
ISO 2768 provides default tolerances for dimensions and geometry that carry no individual callout. It has two parts.
ISO 2768-1 covers linear and angular dimensions. It defines four classes:
| Class | Description |
| f | Fine |
| m | Moyen |
| c | Coarse |
| v | Very coarse |
Tolerance values within each class vary by the size of the dimension. Larger dimensions receive proportionally wider tolerances, which reflects manufacturing reality since holding an absolute value over a long dimension is harder than over a short one.
ISO 2768-2 covers geometric tolerances such as straightness, flatness, perpendicularity, symmetry and runout. It defines three classes: H, K and L, from tightest to loosest.
A callout of ISO 2768-mK therefore specifies medium linear tolerances and class K geometric tolerances.
Choosing a Class
Fine (f) suits precision components where most dimensions matter. It raises cost across the whole part, since every unspecified dimension is now held tightly.
Medium (m) is the most commonly used class for general machined parts and is a reasonable default.
Coarse (c) suits structural and non-critical parts where dimensions have generous functional allowances.
Very coarse (v) suits rough fabrication work.
The important principle is that the general class should reflect what the majority of unspecified dimensions require, not what the most demanding feature requires. Critical features should carry individual tolerances.
Specifying a fine general class to cover a handful of critical dimensions is a common and expensive error. It applies tight control to everything, including features where it serves no purpose, and the cost of that shows up across the entire part rather than on the few dimensions that needed it.
What Machining Can Actually Hold
Standard machining practice on common metals holds roughly ±0.005 inches, or about ±0.127 mm, without special measures. This is achievable at normal feeds and speeds with routine fixturing and inspection.
Tighter capability is available in stages, and each stage changes the process:
Around ±0.001 inches (±0.025 mm) requires more careful setups, better fixturing, controlled tooling and more inspection. Achievable on standard equipment by a capable shop, at higher cost.
Around ±0.0005 inches (±0.0127 mm) requires precision equipment, temperature stability and rigorous process control. Cost rises substantially.
Tighter than that typically moves the feature out of milling and turning and into grinding, honing, lapping or wire EDM, with inspection in a temperature-controlled environment.
These figures are general and vary by material, feature type and part size. A small bore in aluminium behaves differently from a long slot in stainless. Treat them as orientation and confirm capability against your specific feature.
Why Tolerance Drives Cost
Several mechanisms compound.
Cutting parameters. Tight tolerances require lighter cuts and slower feeds, extending cycle time.
Fixturing. Holding a part rigidly enough to machine precisely may require custom fixturing rather than standard workholding.
Tool wear. As a cutting tool wears, dimensions drift. A tight tolerance means tools must be changed more often, before drift consumes the tolerance band.
Thermal effects. Machining generates heat, and metal expands. On tight tolerances this becomes significant, sometimes requiring the part to stabilise before final passes or inspection.
Inspection. Tighter tolerances demand more measurement, better equipment, and calibrated environments. Measurement uncertainty also consumes part of the tolerance band, so a tolerance close to the measurement system’s capability is effectively tighter than it appears.
Scrap. As tolerances tighten, the proportion of parts falling outside them rises. That scrap is paid for in the price of the parts that pass.
The relationship is not linear. Halving a tolerance can more than double the cost of a feature, particularly near the limits of a given process.
Material Affects Achievable Tolerance
Aluminium machines predictably and holds tolerance well, though it expands more with temperature than steel, which matters for tight work.
Steel and stainless are dimensionally stable but harder on tooling, so wear-driven drift needs managing.
Titane generates heat and work-hardens, making tight tolerances more demanding.
Plastiques move considerably with temperature and humidity, absorb moisture in some cases, and are less rigid under cutting forces. Tolerances achievable in metal are often not achievable in plastic, and specifying them regardless is a frequent error.
For plastics, always confirm achievable tolerance with the supplier rather than transferring a metal specification.
Practical Tolerancing Strategy
1. Default to the general class most dimensions need. Usually medium for machined parts.
2. Individually tolerance only functional features. Bearing bores, mating faces, sealing surfaces, features controlling assembly.
3. For each tight tolerance, ask what fails without it. If you cannot answer, relax it.
4. Consider tolerance stacking. Chained dimensions accumulate tolerance. Where several dimensions combine to control a critical relationship, either tolerance that relationship directly or use GD&T to reference features to common datums.
5. Use unilateral tolerances where the direction matters. A hole that must clear a shaft can be toleranced +0.05/-0.00 rather than ±0.025, which grants the machinist the same total band positioned where it is useful.
6. Match tolerance to inspection. A tolerance you cannot verify is not a specification, it is a hope. Confirm the supplier can measure what you specify.
Standard Reference Tolerances
Beyond ISO 2768, other standards appear on drawings and are worth recognising.
ISO 286 covers limits and fits for shafts and holes, using the H7, g6 style notation. This is the standard route for specifying fits between mating cylindrical parts, and it is more precise and more economical than inventing plus-minus values.
Thread standards define tolerance classes for threaded features. Specifying a standard class is better than dimensioning threads individually.
Using established standards where they exist is generally better than custom tolerancing, because both parties understand them and inspection methods are established.
Common Errors
Copying a title block without reviewing it. The most common source of inappropriate general tolerances.
Tightening the general class to cover a few critical features. Applies cost everywhere instead of where needed.
Specifying tolerances tighter than the process can hold, then being surprised by cost or rejection rates.
Transferring metal tolerances to plastic parts without checking achievability.
Ignoring tolerance stacking across chained dimensions.
Specifying tolerances that cannot be verified with available inspection equipment.
Symmetric tolerances where the requirement is one-sided, giving away usable band.
Getting the Balance Right
Tolerance specification is the largest single lever on machining cost, and it is entirely within the designer’s control. A drawing reviewed with cost in mind before release frequently reveals several features toleranced tightly out of habit rather than requirement.
That review costs an afternoon and typically changes the quoted price by more than switching suppliers would. Our guide to CNC machining cost drivers covers the other design decisions that move a quote.
Elite Mold Tech provides DFM review before quoting, including specific comments on which tolerances are driving cost and where they could be relaxed without functional consequence. Sending a drawing produces that feedback alongside the quote rather than a price alone.
Questions fréquemment posées
Q: What does ISO 2768-mK mean?
A: Medium class general linear tolerances under ISO 2768-1, combined with class K general geometric tolerances under ISO 2768-2. It applies to dimensions that carry no individual tolerance callout.
Q: What tolerance can CNC machining hold as standard?
A: Around ±0.005 inches, or about ±0.127 mm, is achievable at normal cutting parameters on common metals. Tighter capability exists but requires more careful process control and raises cost.
Q: Why does tightening a tolerance increase cost so much?
A: Several effects compound: slower cutting, better fixturing, more frequent tool changes, thermal management, more inspection and higher scrap. The relationship is not linear, particularly near a process limit.
Q: Should I use the fine general tolerance class?
A: Only if most unspecified dimensions genuinely require it. Tightening the general class to cover a few critical features applies cost across the whole part rather than where it is needed.
Q: Do plastic parts hold the same tolerances as metal?
A: Generally no. Plastics move with temperature and humidity, some absorb moisture, and they are less rigid under cutting forces. Confirm achievable tolerance with the supplier rather than transferring metal specifications.
