Guide
What do ISO 2768 and NADCA tolerances mean on a machined or die-cast drawing?
ISO 2768 is the ISO standard for general tolerances: the default limits that apply to every dimension on a drawing that carries no tolerance of its own. The NADCA Product Specification Standards play a similar role for die castings, with standard and precision tolerance grades that a die caster quotes against.
By Saola Manufacturing engineering team · Published · Updated
This guide explains how to read a general tolerance note, reproduces the ISO 2768-1 linear table, explains how NADCA organizes its die-casting tolerances, converts surface roughness grades, and shows how to call out threads. It is written for engineers and sourcing managers sending machined or die-cast parts to a supplier overseas. The tables show the values published in each standard. They describe the standards, not the capability of any particular shop. None of the figures on this page describes Saola’s own capability; the tolerance a given part can hold is confirmed in its quote.
On this page
What does ISO 2768-mK mean on a drawing?
ISO 2768-mK is a two-part general tolerance note: the lowercase m selects the medium class of ISO 2768-1 for linear and angular sizes, and the capital K selects class K of ISO 2768-2 for form and position features such as flatness, perpendicularity and run-out. Any dimension or feature without its own tolerance falls back to those two classes.
The two letters come from two different documents, and their status is no longer the same. ISO 2768-1:1989, the part that covers linear and angular dimensions, is still current. ISO 2768-2:1989, the part that defines the H, K and L geometrical classes, has been withdrawn and replaced by ISO 22081:2021, which specifies general geometrical tolerances in a different way, as a general specification tied to the drawing’s datum system.
In practice, a great many drawings in circulation still say “ISO 2768-mK”, and shops everywhere read it. The note is still interpretable, because it names the documents it relies on. On a new drawing, decide on purpose which system you want. Either keep the familiar note and accept that the K part points to a withdrawn standard, or cite ISO 2768-1 for sizes alone and control geometry explicitly, or under ISO 22081, with feature control frames. Whichever you choose, write it once in the title block so the supplier does not have to guess.
A suffix you may also see is “ISO 2768-mK-E”. The E invokes the envelope requirement for features of size, which ties form to size so that a shaft at its largest size must also be perfectly straight. It changes how a feature is inspected, so do not add it by habit.
US drawings built on ASME Y14.5 usually do something different: a tolerance block in the title block sets the default by the number of decimal places shown. That block is a company convention, not a table from ASME, so the supplier needs the drawing itself to know what the default is.
What are the ISO 2768-1 linear tolerances for f, m, c and v classes?
Per ISO 2768-1:1989 Table 1, the permitted deviation grows with the nominal size and with the class, from fine (f) through medium (m) and coarse (c) to very coarse (v). The table below reproduces those values in millimeters.
| 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 |
Read the table by row. Per ISO 2768-1, a 50 mm dimension under class m may measure anywhere from 49.7 mm to 50.3 mm, while the same dimension under class f may measure from 49.85 mm to 50.15 mm. A dash means the standard gives no value for that class and size, so a feature in that cell needs its own tolerance. Per ISO 2768-1, sizes below 0.5 mm are always toleranced individually.
ISO 2768-1 also has separate tables for external radii and chamfer heights and for angular dimensions, which this page does not reproduce. The standard describes its general tolerances as the accuracy a workshop can normally reach without special measures. That is the practical point of the note: general tolerances are cheap by design, and the individual tolerances you add on top are where cost comes in.
General tolerances apply to the finished part. For a die-cast part that is later machined, say which faces are machined and which stay as cast, because the as-cast faces follow casting tolerances, not the ISO 2768-1 class.
What tolerances does NADCA specify for aluminum and zinc die castings?
The NADCA Product Specification Standards for Die Castings give each alloy family two grades of linear tolerance, standard and precision, written as an allowance for the first inch of a dimension plus an increment for each additional inch. Precision values are tighter and take more process control to hold, so they belong only on features that need them.
This page does not reproduce the NADCA tables. They are published in the NADCA manual itself (NADCA, Product Specification Standards for Die Castings), which is updated from edition to edition, so the drawing should name the edition it was toleranced against. Aluminum, zinc and magnesium alloys each have their own values.
Beyond the basic linear values, the standards add allowances for dimensions that cross the parting line or that are formed by moving die components such as slides. The reason is physical. As NADCA’s design guidance puts it, flash at the parting line increases its thickness and so alters dimensions measured across it, and critical dimensions should be kept within one die half where possible (NADCA, parting line).
For a drawing sent to a die caster, three habits prevent most tolerance questions:
- Name the grade per feature. Write “NADCA standard” as the default and mark the few features that need the precision grade, instead of calling out precision across the part.
- Mark machined faces. A face that will be machined after casting is toleranced as a machined face; the casting only needs stock on it.
- Keep critical dimensions in one die half. Ask the die caster where the parting line will fall before freezing the drawing, then dimension critical features from the same side.
ISO drawings can use ISO 8062-3 casting tolerance grades instead of NADCA values. Either way, the die casting quote should confirm, feature by feature, which tolerances will be held as cast and which need machining.
How tight can CNC turning hold?
On a CNC turning order at Saola’s lead CNC plant, whether a tight feature can be held and what it costs depends on the material, the feature and how it is measured, so it is reviewed part by part and confirmed in the quote.
What drives cost below a shop’s routine tolerance is typically not the cutting itself but everything around it. Tighter features typically mean slower finishing passes, more frequent tool changes, measurement in a temperature-controlled room, finer gauges, and a larger share of parts measured rather than sampled. Some features typically move to a secondary operation such as grinding or honing, which adds a setup and a second route through the plant.
Scrap is the other driver. When a tolerance band is narrow compared with normal process variation, more parts fall outside it, and the price of those parts is spread over the good ones. That is why the most effective way to lower a turned-part price is to hold tight tolerances only where the part mates, seals or locates, and leave every other diameter at the general tolerance.
If a fit is the reason for a tight diameter, call it as an ISO 286 fit, such as H7/g6, or state the mating part. The supplier then sees the intent as well as the limits, and can suggest a cheaper way to reach the same fit.
How do surface roughness grades convert?
Roughness grade numbers N1 to N12 are shorthand for fixed Ra values, and each grade roughly doubles the Ra of the grade before it. The table converts each grade to Ra in micrometers and in microinches.
| Grade | Ra (µm) | Ra (µin) |
|---|---|---|
| N12 | 50 | 2000 |
| N11 | 25 | 1000 |
| N10 | 12.5 | 500 |
| N9 | 6.3 | 250 |
| N8 | 3.2 | 125 |
| N7 | 1.6 | 63 |
| N6 | 0.8 | 32 |
| N5 | 0.4 | 16 |
| N4 | 0.2 | 8 |
| N3 | 0.1 | 4 |
| N2 | 0.05 | 2 |
| N1 | 0.025 | 1 |
The N-grade scale comes from older editions of ISO 1302. The current ISO standard for indicating surface texture on drawings, ISO 21920-1:2021, replaced ISO 1302 and does not use N-grades, so on a new drawing write the Ra value with its unit. N-grades still turn up on older prints, which is when the table above is useful.
Older US drawings often give roughness as RMS. Per ASME B46.1, that parameter is Rq, which is not the same measurement as Ra, so ask the designer which one is meant before quoting a surface to it. Either way, call out roughness only on the surfaces where it matters, such as seals, bearing seats and sliding faces, and let the general note cover the rest.
How should threads be called out?
Name the thread standard, size, pitch and class so the gauge is unambiguous: tapered pipe threads as NPT per ASME B1.20.1, and metric threads with an ISO 965-1 tolerance class, such as 6H for an internal thread and 6g for an external one.
A complete pipe-thread callout reads like “1/4-18 NPT”: nominal size, threads per inch and the form. If the joint must seal without sealant, the dryseal form, NPTF per ASME B1.20.3, is a different thread with its own gauges, so write it only when you need it. A complete metric callout reads like “M8x1.25-6H”: diameter, pitch and tolerance class. For inch threads that are not pipe threads, write the series and class per ASME B1.1, such as 1/4-20 UNC-2B.
Add the full-thread depth for blind holes and say whether the thread is gauged with a go/no-go plug or ring. Threads that follow a published standard are checked with standard gauges, which keeps inspection simple; a custom thread form means a custom gauge set, which the supplier has to price in.
What should a tolerance note look like on a drawing sent to an overseas shop?
State the governing standard and its edition in the title block, give one general tolerance class, and add individual tolerances only where the part mates, seals or locates. A shop in Vietnam, Mexico or anywhere else can then price the drawing as written instead of sending questions first.
- One default. Either an ISO 2768-1 class or your company tolerance block, not both.
- One unit system. Say whether the drawing is in inches or millimeters; ISO 2768-1 tables are metric, so an inch drawing that cites them forces a conversion on every dimension.
- Castings named separately. NADCA grade or ISO 8062-3 grade for as-cast features, with the machined faces marked.
- Tight features flagged. List the features tighter than the general class in the RFQ, so they are reviewed on purpose rather than discovered after the quote.
The RFQ package guide covers the rest of what to send with the drawing. When the package is ready, send it for a quote; tolerances that need discussion are called out in the reply, feature by feature.
Frequently asked
Does ISO 2768 apply to inch drawings?
It can be cited on any drawing, but its tables are metric, so an inch drawing that cites it forces a conversion. Many US drawings use a decimal-place tolerance block instead. Either works, as long as the drawing states which one governs.
Is ISO 2768-mK still valid now that ISO 22081 exists?
ISO 2768-1 is still current. ISO 2768-2, the source of the K, was withdrawn and replaced by ISO 22081:2021. Drawings that cite mK are still read the way they were written; on a new drawing, decide which system you want and name it.
Can you quote a die-cast part to NADCA precision tolerances?
Send the drawing with the precision features marked. Whether a feature can be held as cast depends on the alloy, its size and where the parting line falls, so the written quote answers feature by feature and lists any that need machining.
Should I use an N-grade or an Ra value?
Use an Ra value with its unit, per ISO 21920-1 or ASME B46.1. If an older drawing gives an N-grade, the conversion table above gives the matching Ra.
What is the flatness tolerance under ISO 2768?
Flatness sits in Part 2 of the standard, ISO 2768-2, which sets general geometrical tolerances in three classes, H, K and L, with the allowed value growing with the length of the feature. In a note such as ISO 2768-mK, the "m" is the Part 1 class for linear and angular dimensions and the "K" is the Part 2 class that covers flatness and straightness.
Sources
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions, ISO, 1989 (reviewed and confirmed 2022)
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances, ISO, 1989 (withdrawn)
- ISO 22081:2021, General geometrical specifications and general size specifications, ISO, 2021
- Product Specification Standards for Die Castings, NADCA, accessed September 2026
- Parting line design guidance, NADCA, accessed September 2026
- ISO 21920-1:2021, Surface texture: Profile — Part 1: Indication of surface texture, ISO, 2021
- ASME B46.1-2019, Surface Texture (Surface Roughness, Waviness, and Lay), ASME, 2019
- ASME B1.20.1, Pipe Threads, General Purpose (Inch), ASME, 2013 edition