Guide
Standard machining tolerances: what does a CNC shop hold when the drawing says nothing?
Standard machining tolerances are the default limits a machined dimension must meet when the drawing gives it no tolerance of its own, supplied either by a general tolerance note such as ISO 2768-m or by the decimal-place tolerance block printed in a US title block. There is no single universal standard tolerance: if a drawing carries neither a note nor a tolerance block, the untoleranced dimensions are incomplete under ASME Y14.5, and every shop quietly falls back on its own habit.
By Saola Manufacturing engineering team · Published · Updated
This page answers the questions buyers and design engineers actually ask about default tolerances: which rule applies to an untoleranced dimension, what ISO 2768 and a typical American title block allow, whether a three-place tolerance is tight, what the general note does not cover, and how to write the block so a supplier on the other side of the world reads it the same way you do. The full ISO 2768 linear table and the die-casting side are covered in the ISO 2768 and NADCA tolerances guide, and the cost side of tightening in the guide to what a too-tight tolerance costs; this page links to them rather than repeating them.
On this page
What tolerance applies to a dimension with no tolerance on the drawing?
The tolerance comes from the general note or the title-block tolerance block, and nowhere else. If the drawing has neither, the dimension has no defined tolerance, the drawing is incomplete, and the supplier should ask before quoting rather than assume a value.
The governing rule is in ASME Y14.5-2018: each feature must be toleranced, dimensions identified as reference, maximum, minimum or stock are the only ones exempt, and the tolerance may be applied directly to the dimension, through a feature control frame, by a general note, or in a supplementary block of the drawing format. The standard also requires dimensioning and tolerancing to be complete. It defines how a general note works but does not prescribe the values the note should contain. That is why two US companies can both follow ASME Y14.5 and still print different numbers next to the same “.XXX” in their title blocks.
On ISO drawings the mechanism is the same but the values are standardized. A note such as “General tolerances ISO 2768-m” pulls in a published table, so a drawing that cites the class is complete for every untoleranced linear and angular size. A drawing that cites nothing is a different problem. Under the definitive drawing principle of ISO 8015, only the specifications actually indicated on the drawing are required, so a supplier cannot legitimately invoke a tolerance the designer never wrote down.
In practice, untoleranced drawings still arrive every week, usually as a model with a dimensioned PDF exported from CAD without the company template. When we review a drawing like that, we ask which general standard the designer intended and write the answer into the quote, because a silent assumption on either side is what turns into a rejected first article.
What are the standard machining tolerances in ISO 2768 and a typical US title block?
ISO 2768-1 gives fixed tolerances by size band and class, and class m (medium) is the usual default for machined parts. A US title block instead ties the tolerance to the number of decimal places written in the dimension, and the values are company practice rather than a standard.
The table below is ISO 2768-1 Table 1, the linear values every untoleranced length, width, depth, step and hole diameter falls under once the class is named. Holes and bosses are linear sizes too, so an untoleranced hole diameter under class m takes the same band as any other length of that size. The same standard has two shorter tables. Per ISO 2768-1, external radii and chamfer heights from 0.5 mm to 3 mm may deviate by 0.2 mm either way under classes f and m, and angles are graded by the length of the shorter leg: under classes f and m, an angle whose shorter leg is over 10 mm up to 50 mm may deviate by half a degree either way, and one whose shorter leg is 10 mm or less by a full degree.
Annex A of ISO 2768-1 ties these values to customary workshop accuracy, which is the whole point of a general tolerance: it should cost nothing extra. ISO has also approved a second edition, titled simply ISO 2768 and in the final publication stage as of October 2026, that will replace ISO 2768-1:1989; until a drawing cites it, the 1989 table below is the one most prints refer to, so check which edition your customer means. A general class that is tighter than the shop’s normal accuracy turns every dimension on the print into a controlled one and raises the price of the whole part.
| Nominal size (mm) | f (fine) | m (medium) | c (coarse) | v (very coarse) |
|---|---|---|---|---|
| 0.5 up to 3 | ±0.05 | ±0.1 | ±0.2 | — |
| over 3 up to 6 | ±0.05 | ±0.1 | ±0.3 | ±0.5 |
| over 6 up to 30 | ±0.1 | ±0.2 | ±0.5 | ±1 |
| over 30 up to 120 | ±0.15 | ±0.3 | ±0.8 | ±1.5 |
| over 120 up to 400 | ±0.2 | ±0.5 | ±1.2 | ±2.5 |
| over 400 up to 1000 | ±0.3 | ±0.8 | ±2 | ±4 |
| over 1000 up to 2000 | ±0.5 | ±1.2 | ±3 | ±6 |
| over 2000 up to 4000 | — | ±2 | ±4 | ±8 |
Is .005 a tight tolerance for CNC machining?
No. A three-place tolerance of five thousandths either way gives a total band of 0.010 in, which per ISO 286-1 falls between grades IT12 and IT13 on a one-inch dimension: general-tolerance territory for milling and turning, roughly between ISO 2768 f and m at that size.
The easiest way to judge any title-block tolerance is to convert its total band into an ISO 286 international tolerance (IT) grade at the size you care about. The second table does that for the decimal-place conventions typically printed in American title blocks, at a nominal size of 25 mm (about one inch). The conventions themselves are not a standard; they are the values that typically appear in US company templates, and your own template may differ, which is exactly why the block should always be on the drawing.
As industry guidance, ordinary CNC milling and turning reach somewhere around IT7 to IT11 depending on the feature, the setup and the material, so a five-thousandths three-place tolerance is comfortable and a ten-thousandths two-place tolerance is loose. A four-place tolerance of ±0.0005 in (0.013 mm) is a different matter: per ISO 286-1 its band sits between IT7 and IT8 on a one-inch size, the range of a reamed or bored fit, and it should be placed only on features that need it. The trap is the CAD export that writes every dimension to four places: in a title block that maps four places to half a thousandth, that one setting makes the whole part a precision part.
| Dimension written as | Typical total band (in) | Total band (mm) | Nearest IT grade at 25 mm |
|---|---|---|---|
| Fraction (1/2) | 1/32 to 1/16 | 0.79 to 1.59 | IT15 to IT16-17 |
| Two places (.XX) | 0.020 to 0.030 | 0.51 to 0.76 | IT14 to IT15 |
| Three places (.XXX) | 0.010 | 0.254 | IT12 to IT13 |
| Four places (.XXXX) | 0.0010 | 0.0254 | IT7 to IT8 |
| For comparison: ISO 2768-m, over 6 up to 30 mm | 0.016 | 0.4 | IT13 to IT14 |
| For comparison: ISO 2768-f, over 6 up to 30 mm | 0.008 | 0.2 | About IT12 |
What does a general tolerance note not control?
A size tolerance note does not control fits, threads, surface roughness or, on an ISO drawing, the form of a surface such as flatness. Each of those needs its own callout or its own general note, or the supplier is free to deliver whatever the process naturally produces.
Form is the most common gap. On an ASME drawing, Rule #1 makes the size limits of a feature of size also limit its form, so a toleranced thickness also bounds how far the faces can bow; a single face that is not part of a feature of size gets no flatness control from the title block at all. ISO drawings work the other way: per ISO 8015 the independency principle applies, so size and form are separate unless the envelope symbol is used. The Rule #1 guide walks through the difference.
The ISO tool for general form and orientation used to be ISO 2768-2, with classes H, K and L; for example, per ISO 2768-2 class K allowed 0.1 mm of straightness or flatness on a feature over 10 mm up to 30 mm long. That part was withdrawn in 2021 and replaced by ISO 22081, which uses a general profile specification relative to a datum system instead of the old classes. Notes such as “ISO 2768-mK” still appear on legacy prints and suppliers still read them, but a new drawing should cite ISO 22081 or put explicit geometric tolerances on the faces that matter.
Fits are the second gap. A bearing bore or dowel hole needs an ISO 286 fit class such as H7 or an explicit limit pair, not the general band, as covered in the reamed vs drilled hole guide. Threads take their class from the thread callout, never from the block. Surface roughness has no default value in ASME Y14.36 or ISO 21920-1, which is why many American templates print a default roughness symbol; if the template omits it, roughness is uncontrolled, and the machined surface roughness guide covers which value to write.
When should you tighten a dimension beyond the general tolerance?
Tighten only the dimensions that set a fit, seal, alignment or a stack-up that fails worst case; leave every other dimension on the general tolerance. Each individually tightened dimension adds machining, inspection and documentation cost, so the number of tight features matters more than how tight any one of them is.
A practical decision rule for the drawing is four questions per dimension. Does it mate with another part? Use a fit class per ISO 286 or an explicit limit pair. Does it carry a seal, a bearing or a sliding surface? Add the size, a form control and a roughness value. Does it sit in a chain whose sum must close? Run the stack, as in the stack-up guide, and tighten only the links that the stack needs. Is it a datum feature? Give it form control. If the answer to all four is no, the general tolerance is the right answer, even if it feels loose.
Cost rises steeply rather than linearly as tolerance narrows, because each step tighter can add a finishing pass, a slower process such as reaming or grinding, temperature control during measurement and a higher inspection sampling rate. The tight-tolerance cost guide breaks those drivers down; the point here is that a general class one step finer, such as f instead of m, tightens every untoleranced dimension at once and is usually a worse choice than tightening three named features.
What should the tolerance block or general note say on an RFQ drawing?
State one general tolerance system explicitly, with its class or its decimal-place values and units, and make sure the dimension precision in the CAD export matches what that system means. A complete block also names the governing standard, the default angle tolerance, the default roughness and how edges are treated.
For an ISO drawing, a complete note reads along the lines of “General tolerances ISO 2768-m; general geometrical specification ISO 22081; dimensions in mm; ISO 8015 applies.” For an ASME drawing, the block should list each decimal-place tolerance, the angle and fraction tolerances, the units, “Interpret per ASME Y14.5-2018”, the default surface roughness and a break-sharp-edges note. Mixed-unit drawings need the block to state which unit each tolerance applies to, because a three-place metric dimension and a three-place inch dimension are very different requirements.
Before sending the RFQ, check three things that cause most quote questions: the CAD template actually printed the block onto the PDF, the dimension precision setting did not round values or add extra decimal places, and the model and the drawing agree. When a drawing reaches us for CNC milling or CNC turning, those are the first things we check, and anything ambiguous goes back to the buyer as a written question with the quote rather than as an assumption. Drawings can be sent through the quote form.
Frequently asked
What is the standard tolerance for CNC machining?
There is no single universal standard. ISO drawings usually cite ISO 2768-m, and American drawings rely on the company title block, where three-place dimensions commonly carry plus or minus five thousandths of an inch. If your drawing states neither, the supplier is guessing, so put one on the print.
What does “unless otherwise specified” mean in a title block?
It means the block values apply to every dimension that has no tolerance written next to it. A tolerance placed directly on a dimension or a fit class overrides the block for that feature, and a basic dimension in a box or a reference dimension in parentheses is not governed by the block at all.
Does ISO 2768 apply to hole diameters?
Yes. ISO 2768-1 covers all linear sizes, including internal ones, so an untoleranced hole takes the band for its size and class. Holes that receive a pin, bearing or shaft should carry an ISO 286 fit class instead.
Is ISO 2768-mK still valid?
The m part, from ISO 2768-1, is current. The K part, from ISO 2768-2, was withdrawn in 2021 and replaced by ISO 22081. Suppliers still understand the legacy note, but new drawings should cite ISO 22081 or apply explicit geometric tolerances.
Can a supplier apply its own default tolerances?
Only if you agree to it in writing. A supplier’s house tolerance is not part of your drawing, so if a part is later disputed, the drawing without a tolerance block gives neither side a basis. Ask for the assumed values to be written into the quote, or better, add the block.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions without individual tolerance indications, ISO, 1989
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances for features without individual tolerance indications, ISO, 1989 (withdrawn 2021)
- ISO 22081:2021, GPS — General geometrical specifications and general size specifications, ISO, 2021
- ISO 286-1:2010, GPS — ISO code system for tolerances on linear sizes — Part 1: Basis of tolerances, deviations and fits, ISO, 2010
- ISO 8015:2011, GPS — Fundamentals — Concepts, principles and rules, ISO, 2011
- ASME Y14.36-2018, Surface Texture Symbols, ASME, 2018
- ISO 21920-1:2021, GPS — Surface texture: Profile — Part 1: Indication of surface texture, ISO, 2021
- ISO 2768, GPS — Dimensional tolerancing — Tolerance limits for general specification of linear and angular sizes, ISO, edition 2, 2026 (under publication; replaces ISO 2768-1:1989)