A drawing with no tolerance on a dimension is not an untoleranced drawing. It is a drawing that has quietly handed the decision to whatever general tolerance note sits in the title block, or to the machinist if there is no note at all. That is where most dimensional disputes on machined parts begin.
In practice, the general standard for machined metal parts is ISO 2768 class m, which allows around plus or minus 0.1 mm on a 6 to 30 mm dimension. Shops in North America often work to a default of plus or minus 0.005 inch, roughly 0.13 mm, which is close but not identical. Tighter individual features can reach plus or minus 0.005 mm on suitable geometry. This guide covers the full charts, what changed in the standard recently, and how to decide which features genuinely need a tight band.
The four levels of CNC machining tolerances
| Level | Typical band | Where it fits | Relative cost |
| Coarse (ISO 2768-c) | Around ±0.5 mm (0.020 in) | Weldments, non-critical brackets, cosmetic covers | Lowest |
| Standard (ISO 2768-m) | Around ±0.1 to ±0.3 mm | Most machined parts, the sensible default | Baseline |
| Fine (ISO 2768-f) | Around ±0.05 to ±0.15 mm | Assemblies with stacked dimensions | Modest increase |
| Precision (individual) | ±0.025 mm down to ±0.005 mm | Bearing seats, sealing faces, mating bores | Steep increase, feature by feature |
The important distinction is that the first three are general tolerances applied to every dimension without its own callout. The fourth is applied dimension by dimension, and it always overrides the general note.
ISO 2768-1 linear tolerance chart
This is the table your general tolerance note actually points to. Values are permissible deviations in millimetres, with inch equivalents in brackets for reference.
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
| 0.5 to 3 | ±0.05 (0.002) | ±0.1 (0.004) | ±0.2 (0.008) | Not defined |
| Over 3 to 6 | ±0.05 (0.002) | ±0.1 (0.004) | ±0.3 (0.012) | ±0.5 (0.020) |
| Over 6 to 30 | ±0.1 (0.004) | ±0.2 (0.008) | ±0.5 (0.020) | ±1.0 (0.039) |
| Over 30 to 120 | ±0.15 (0.006) | ±0.3 (0.012) | ±0.8 (0.031) | ±1.5 (0.059) |
| Over 120 to 400 | ±0.2 (0.008) | ±0.5 (0.020) | ±1.2 (0.047) | ±2.5 (0.098) |
| Over 400 to 1000 | ±0.3 (0.012) | ±0.8 (0.031) | ±2.0 (0.079) | ±4.0 (0.157) |
| Over 1000 to 2000 | ±0.5 (0.020) | ±1.2 (0.047) | ±3.0 (0.118) | ±6.0 (0.236) |
| Over 2000 to 4000 | Not defined | ±2.0 (0.079) | ±4.0 (0.157) | ±8.0 (0.315) |
Notice how the band widens with size. A 20 mm feature at class m gets plus or minus 0.2 mm, while a 300 mm feature gets plus or minus 0.5 mm. That is deliberate, because thermal growth and fixturing error both scale with length. It also means a long part with a stacked chain of general dimensions can accumulate more variation than a designer expects.
External radii and chamfer heights
| Nominal size (mm) | f and m | c and v | Note |
| 0.5 to 3 | ±0.2 | ±0.4 | Applies to break edges and chamfers |
| Over 3 to 6 | ±0.5 | ±1.0 | Generous by design |
| Over 6 | ±1.0 | ±2.0 | Tolerance individually if the radius is functional |
These bands are wide because radii and chamfers are rarely functional. If a radius controls a seal, a fillet stress concentration or a mating clearance, it needs its own tolerance rather than the general one.
Angular tolerances
Angular general tolerances in ISO 2768-1 are set by the length of the shorter side of the angle, not by the angle itself. A 45 degree feature on a 15 mm face carries plus or minus 30 minutes at class m, while the same angle on a 200 mm face carries only plus or minus 10 minutes. Short features get loose angular control, which surprises people who assume the tolerance follows the angle value.
The part of ISO 2768 that no longer exists
This is where many tolerance guides are now out of date. ISO 2768 was published in two parts. Part 1 covers linear and angular sizes and remains in force. Part 2 covered general geometrical tolerances through classes H, K and L, and it was withdrawn and replaced by ISO 22081:2021, which brings general geometrical specification into the wider GPS framework. You can confirm the status directly on the ISO record for ISO 2768-2.
The practical consequence matters. A drawing released today that says ISO 2768-mK is still readable, and any competent supplier will interpret the K half against the old table. But the K half now references a withdrawn document, and ISO 22081 deliberately publishes no fixed value table. It asks the designer to state the general geometrical specification explicitly, with a stated datum, rather than inheriting one from a letter class.
Legacy drawings citing H, K or L classes are still interpreted against these values, so the table remains useful for reading existing prints.
| Characteristic and range | Class H | Class K | Class L |
| Flatness, up to 10 mm | 0.02 | 0.05 | 0.1 |
| Flatness, 30 to 100 mm | 0.1 | 0.2 | 0.4 |
| Flatness, 100 to 300 mm | 0.2 | 0.4 | 0.8 |
| Perpendicularity, up to 100 mm | 0.2 | 0.4 | 0.6 |
| Perpendicularity, 100 to 300 mm | 0.3 | 0.6 | 1.0 |
| Circular run-out | 0.1 | 0.2 | 0.5 |
If you are drawing up a new title block, the cleanest options are to state your general geometrical specification explicitly per ISO 22081, or to keep referencing ISO 2768-2 deliberately and knowingly. Either works. What causes problems is an unclear note with no class letter and no date, because that leaves the interpretation open on exactly the dimensions most likely to be argued over. A revised edition of the linear and angular part has also been progressing through ISO/TC 213, so it is worth checking the current status before you standardise a template across a product family.
How to read a general tolerance callout
A note such as ISO 2768-mK carries two separate instructions. The lower case letter selects the linear and angular class from Part 1. The capital letter selects the geometrical class from the older Part 2. So mK means medium general tolerances on untoleranced lengths and angles, plus class K limits on straightness, flatness, perpendicularity, symmetry and run-out.
Three rules follow from that, and they resolve most disputes before they start:
- An individual tolerance always wins. If a dimension carries its own limits or a fit such as H7, the general note does not apply to it.
- General tolerances only fill gaps. They are the floor, not a substitute for functional tolerancing.
- A general note never controls true position or profile. Position still needs explicit geometrical tolerancing with a stated datum reference frame.
What each process can realistically hold
General tolerances for machined parts are only meaningful if the chosen process can hit them. These are typical capabilities on suitable features in a rigid setup.
| Process | Comfortable | Achievable | Limiting factor |
| 3-axis milling | ±0.05 mm | ±0.0125 mm | Setups, tool deflection, part rigidity |
| 5-axis milling | ±0.025 mm | ±0.010 mm | Feature-to-feature accuracy improves with one setup |
| CNC turning | ±0.025 mm | ±0.0075 mm | Diameter control is easier than length control |
| Reaming and boring | H8 | H7 | Hole quality depends heavily on pre-drill and material |
| Surface grinding | ±0.005 mm | ±0.002 mm | Flat and cylindrical geometry only |
| Wire EDM | ±0.005 mm | ±0.002 mm | Conductive materials, 2D and tapered profiles |
Material changes these numbers too. Aluminum machines accurately but expands most with temperature, austenitic stainless work hardens on the finishing pass, and titanium deflects under cutting load. Our comparison of titanium, aluminum and stainless steel for machined parts covers how each behaves. Our precision CNC machining service holds plus or minus 0.005 mm where the geometry and material allow it, and we confirm feature by feature during design review rather than promising it across a whole drawing.
What tolerance actually costs
Tightening a tolerance does not add a fixed percentage. It changes the process. Each step down usually triggers one or more of the following:
- An extra finishing pass, with lighter cuts and slower feeds.
- A fresh tool for the finishing operation so edge wear does not shift the dimension.
- Additional or more rigid workholding, sometimes a custom fixture.
- A secondary process such as grinding, reaming or wire EDM.
- More inspection, including CMM time and a written dimensional report.
- Higher scrap risk, which is priced into the quote whether or not it occurs.
The last two are the ones buyers underestimate. Tight tolerance CNC machining shifts cost away from cutting and toward measuring. A part with forty tight callouts may spend as long on a CMM as it did in the machine, and that time appears on every unit, not just the first article.
This is also why a documented first article matters more as tolerances tighten. If you are unfamiliar with how that process works, our guide to first article inspection in CNC machining explains what the report contains and when to ask for one.
Which features can hold the tightest limits
Achievable tolerance is a property of the feature, not the machine. A shop that can hold plus or minus 0.005 mm on a bore cannot necessarily hold it across a 400 mm span.
Features that hold tight limits well
- Bores and turned diameters, where the tool geometry defines the size directly.
- Short depths and pocket floors machined in a single setup.
- Ground or wire cut faces on hardened material.
- Features on thick, rigid sections with good workholding access.
Features that resist tight limits
- Long distances between features, especially across more than one setup.
- Thin walls, tall ribs and slender bosses that deflect under cutting force.
- Deep pockets requiring long tools, where deflection grows quickly with reach.
- Anything measured after a coating, since plating and anodizing add thickness.
That last point causes real problems. Type III hardcoat anodizing builds a layer that grows both outward and into the surface, so a bore toleranced tightly before anodizing may fall out of tolerance afterwards. Tight features that will be coated need the tolerance stated for the finished condition, with stock allowed accordingly.
Tolerance, surface finish and position are three different things
These get conflated constantly. Tolerance controls how far a dimension may vary from nominal. Surface finish controls the texture of the face, measured as Ra, and a part can hold a tight dimension with a rough finish or a fine finish with a loose dimension. Choosing them independently is one of the easier ways to control cost, which our overview of machined surface finish options goes into.
Position is different again. A hole can sit perfectly within its diameter tolerance and still be in the wrong place, because no general tolerance note controls where features sit relative to a datum. If hole locations matter for an assembly, they need explicit geometrical tolerancing. Relying on general size limits to control a bolt pattern is one of the most common causes of parts that measure correct but will not assemble.
What to put on your drawing
- Set the general note deliberately. Class m suits most machined work. Class f is reasonable on turned parts and small precise components, but it raises cost across the whole drawing, so use it only if the part genuinely needs it.
- State the geometrical specification explicitly per ISO 22081, or reference the older classes knowingly. Do not leave it blank.
- Tolerance the functional features individually. Bearing fits, sealing faces, mating bores and datum surfaces earn their own limits. Everything else can live on the general note.
- Identify the datums. Geometrical control is meaningless without them, and an unstated datum reference frame is the fastest route to a measurement disagreement.
- State whether tolerances apply before or after surface treatment.
- Say which dimensions are critical and need reporting. That focuses inspection where it matters instead of spreading it evenly.
Getting the tolerance decision right before you quote
The most useful discipline is subtractive. Start from a sensible general note, then tighten only the features that carry a function. Most drawings that quote badly are not over-engineered in geometry, they are over-toleranced across dimensions that never needed control.
If you are unsure which of your callouts are realistic, send the model and drawing together rather than the model alone. The drawing tells a supplier which dimensions are functional, and that changes both the price and the inspection plan. XY Machining returns design-for-manufacturability feedback within 24 hours, flagging callouts that are unachievable on the chosen material or that will add cost without adding function. You can review our CNC machining capabilities or see how inspection is documented on our quality assurance page.
Frequently asked questions
Q: What is the standard tolerance for CNC machined parts?
A: Most machined metal parts default to ISO 2768 class m, which is around plus or minus 0.1 mm on a 6 to 30 mm dimension. North American shops often use plus or minus 0.005 inch instead, which is broadly comparable.
Q: Is ISO 2768 still valid in 2026?
A: Part 1, covering linear and angular sizes, remains in force. Part 2, covering general geometrical tolerances, was withdrawn and replaced by ISO 22081:2021. Existing drawings citing the old H, K and L classes are still interpreted against the original tables.
Q: What does ISO 2768-mK mean on a drawing?
A: Medium general tolerances on any length or angle without its own limits, plus class K general limits on flatness, straightness, perpendicularity, symmetry and run-out. Any individually toleranced dimension overrides both.
Q: How much does a tighter tolerance add to the price?
A: There is no fixed multiplier. Cost rises when the tighter band forces an extra finishing pass, a secondary process such as grinding, custom fixturing or CMM inspection on every unit. A few tight features cost little, a whole tight drawing costs a lot.
Q: Should tolerances be measured before or after anodizing?
A: State it on the drawing. Anodizing and plating add measurable thickness, so a tight bore can drift out of tolerance after treatment. Tight features on coated parts should be toleranced in the finished condition with stock allowed.
