CNC Machining Tolerances Explained: ISO 2768 for Buyers
ISO 2768 is a general-tolerance note for untoleranced dimensions on a CNC drawing—not a promise of tight tolerances everywhere. This guide explains the classes, worked examples, cost drivers and what to put on an RFQ.
Direct answer: what CNC machining tolerances and ISO 2768 actually mean
When engineers search “CNC machining tolerances ISO 2768,” they usually want two answers: what a title-block note such as ISO 2768-m actually buys on a machined part, and whether they should tighten it. ISO 2768 is a general-tolerance system for linear, angular and (in part 2) geometrical features that do not carry an individual tolerance. It is not a shop certification, not a promise that every face will come in at ±0.01 mm, and not a substitute for a fit class or a datum scheme on a functional interface.
The usual drawing note is ISO 2768 followed by a class letter, for example ISO 2768-m for medium linear deviations, or ISO 2768-mK when a geometrical class from ISO 2768-2 is added. Medium (m) is the most common default on machined-part drawings. Fine (f) is tighter; coarse (c) and very coarse (v) are looser. The class applies only where you left a dimension untoleranced. If a bore, a seat or a sealing face matters, give that feature its own tolerance.
At JHW Molding (Suzhou Jiahongwei Technology Co., Ltd., founded 2016 in Suzhou), we are a one-stop mold and injection project service provider: DFM, mold design review, project management, mold-trial follow-up and outgoing inspection. Mold making, molding and CNC machining run at production partners we manage—we do not claim “our factory” ownership. CNC machining supports mold components, fixtures and custom metal parts that sit next to a plastics program. It is not positioned as a standalone high-volume metal commodity shop. Verified CNC equipment at manufacturing partner Suzhou Weiyu Mould Industry Co.,Ltd. is listed, with model and quantity, on the Manufacturing Equipment & Facilities page. Machine selection and available capacity are confirmed per project drawing. Common metals for tooling and fixtures include aluminum, steel and brass; grade and availability are confirmed in the quotation, not as a universal catalog.
Tight tolerances are applied only to functional faces, not blanket-applied across the title block. Critical dimensions are identified and checked at first article against the released drawing. Inspection records follow the agreed scope per program. Every RFQ includes free DFM; we aim for DFM notes plus a quote in about 48 hours when the pack is complete. Factory visits and audits are not promised on a cold RFQ. Contact: sales@jhwmolding.com, WhatsApp +86 189 6217 3434. Foreign trade and R&D office: Room 1710, China Automotive Parts Industry Base, No. 19 Aigehao Road, Weitang Town, Xiangcheng District, Suzhou, Jiangsu, China. Production partner (Suzhou): No. 8 Yinyan Road, Suzhou High-Tech Zone. Capability context starts on our CNC machining and mold making pages.
What ISO 2768 is — and what it is not
ISO 2768-1 specifies general tolerances for linear and angular dimensions that have no individual tolerance indication. It covers sizes such as external and internal dimensions, steps, diameters, radii and distances, plus a separate set of deviations for broken edges (external radii and chamfer heights). The four linear classes are f (fine), m (medium), c (coarse) and v (very coarse). The standard is meant to keep drawings readable: you tolerance the features that function, and the class covers the rest.
ISO 2768-2 covers general geometrical tolerances for features without an individual geometrical tolerance—typically items such as straightness, flatness, perpendicularity, symmetry and circular run-out—in classes H, K and L. A combined title-block note such as ISO 2768-mK means medium linear deviations plus geometrical class K. If your drawing says only ISO 2768-m, you have invoked the linear (and angular) general system; do not assume a geometrical class that is not written down.
The general system applies only where no individual tolerance is given. It does not replace theoretically exact (boxed) dimensions, auxiliary dimensions in brackets, or a size that already belongs to another standard. Hole and shaft fits belong to a system such as ISO 286 (for example H7 on a hole), not to a hope that ISO 2768-f is “close enough.” Threads, many tapped holes, and assembly-locating positions usually need their own callouts or a true-position / GD&T scheme.
For nominal sizes below 0.5 mm, the widely used ISO 2768-1:1989 linear table does not give a general deviation—put a tolerance next to that size. Cite the edition on the drawing. Most title blocks still mean ISO 2768-1:1989 when they write ISO 2768-m; if a customer specifies a later edition, that text governs. The worked examples in this article use the widely published 1989 linear values. ISO 2768 is a drawing contract, not a quality-system certificate and not a claim about JHW or any production partner.
How to read the classes (worked examples, not a substitute for the official tables)
General deviations depend on the nominal size of that dimension, not on the overall size of the part. A 25 mm length and an 80 mm overall length on the same housing do not share one band.
Under ISO 2768-m, a linear size over 6 mm up to 30 mm has a general deviation of ±0.2 mm. A 25 mm length with no individual tolerance is then acceptable from 24.8 mm to 25.2 mm. The same 25 mm under class f is ±0.1 mm; under class c it is ±0.5 mm. That is why switching a whole drawing from m to f is not a free upgrade: every untoleranced size in that range just became twice as tight.
Larger features are looser under the same class. Over 30 mm up to 120 mm, class m is ±0.3 mm, so an 80 mm length is not held to the 25 mm band just because both sit on one part. Over 120 mm up to 400 mm, class m opens to ±0.5 mm. A common reading error is the boundary: 30 mm belongs to the “over 6 mm up to 30 mm” row, not to the next row. When a size sits on a boundary, read the official table for the edition you cited.
Broken edges have their own, usually looser, general deviations. A small chamfer or external radius under ISO 2768-m is not held as tightly as a linear size of the same nominal length. If a break-edge, chamfer or blend is functional—clearance, safety, or a sealing lead-in—tolerance it individually rather than leaving it to the general broken-edge row.
These figures are worked examples from the widely published ISO 2768-1:1989 linear values, not a complete official table and not a substitute for the standard. Use the official ISO 2768 text for the full linear, angular and geometrical values, including ranges this article does not walk through. The drawing and the edition it cites take priority over any handbook or this page.
When a general class is not enough
Mating fits, bearing seats, dowel holes, press fits and sliding fits need an individual tolerance or an ISO 286 fit class. A title-block ISO 2768-f still leaves a 25 mm hole with a general band of ±0.1 mm, which is not a controlled fit. If the bore must locate a pin or a bearing, write the limit or the fit on that feature.
Datums, the flatness of a sealing face, or the perpendicularity of a locating boss belong in a GD&T or individually toleranced scheme when function cares. ISO 2768-2 general geometrical classes are a backstop for features you did not single out. They are not a substitute for a datum frame on a critical interface.
Cosmetic or tight-tolerance faces should be called out rather than applied to the whole part. That is the same rule stated on our CNC machining capability page: tight tolerances belong on functional faces, and a general title-block tolerance is a weak contract if it is the only control you have. Mark the faces that assemble, seal, or show, and leave clearance stock on a realistic general class.
Do not copy a metal CNC general-tolerance note onto a plastic injection-molded part by habit. Shrink, warp and process capability are different; a band that is routine on an aluminum bracket can be unrealistic on a molded housing. If a molded part needs a general class, agree it as a plastics drawing decision. For process choice between machining and molding, see our CNC vs injection molding note.
How CNC machining tolerances drive cost
A blanket tight title block—“all dimensions ±0.05 mm,” or a default ISO 2768-f on a large, deep-pocketed housing—taxes every surface, including ones that only need to clear a cover. Tighter general classes usually mean more finishing passes, more conservative feeds, more fixturing or operations, and more inspection time. The cost shows up in machining hours and inspection scope, not in a published rate card.
Call out only the tolerances that function. Leave the rest on a realistic general class—often ISO 2768-m on machined parts, when that matches the function. If one face must be flat or one bore must fit a bearing, tighten that feature and leave non-functional stock sizes alone. This is the same advice as in our CNC machining cost factors note: setup, material, tolerance and finish should be readable as separate assumptions in the quotation.
Material changes what a tight band costs. Aluminum typically machines faster than steel, so the same close tolerance is not the same cycle. Grade and availability are confirmed per project rather than from a universal metal catalog; our CNC machining materials note covers aluminum, steel and brass in tooling and fixture work. Name the grade when you ask for a close band.
Quantity and process also move the number. A one-off prototype carries the full setup; a batch spreads it. For plastic parts at higher volume, a production mold is often the piece-price path, while CNC remains the process for many metal interfaces and fixtures even when the plastic is molded. Tolerance decisions and process choice should be made together, not after a tool is already committed. Setup, material, quantity and finish move the same quotation; our CNC machining cost factors guide walks through that full stack, not only the tolerance line.
Inspection, first article and measurement method
A tolerance is only as useful as the method used to check it. Agree what will be measured, with what, and against which released revision. A general class without an inspection scope leaves both sides arguing about a caliper reading on a burr or a fillet the inspector was never asked to include.
As published on our CNC capability page, functional and critical dimensions are identified and checked at first article against the released drawing. Inspection records follow the agreed scope per program. That is the contract you can enforce—not an unspoken hope that every untoleranced size was chased to the fine class.
Partner metrology at Suzhou Weiyu Mould Industry Co.,Ltd. is listed on the Manufacturing Equipment & Facilities page, including digital calipers, a height gauge and an automatic vision measuring machine. Do not assume a method that is not in the agreed scope. For example, do not assume a full coordinate-measuring-machine report if the program was quoted to a drawing-based first-article check with the listed instruments. If you need a specific report format, name it in the RFQ.
Burrs, broken edges, surface finish and temperature can move a measured size. A tight bore checked as-machined with a burr still on the edge is not the same feature the assembly will see. If a coating or anodize is in the process, say whether the tolerance applies before or after finish. Outgoing inspection is coordinated as part of the project service; the exact record format is agreed per program. We do not claim any management-system certification in this article.
DFM and RFQ tips for CNC machining tolerances
Send STEP (preferred) plus a 2D drawing with datums, the general-tolerance note and its edition, and individual tolerances on fits and functional faces. Mark cosmetic or tight faces. A model without a drawing, or a drawing that says only “tolerance tight,” is not a complete pack.
Name the material grade, the quantity (prototype versus batch), and the finish: as-machined, deburr only, polish, or a coating. Finish is its own line in the quotation so it can be accepted or declined. Say which dimensions are critical and how you expect them to be inspected at first article.
Every JHW RFQ includes free DFM; we aim for DFM notes plus a quote in about 48 hours when the pack is complete. We will comment where a blanket tight class could be relaxed, and where an individual callout is missing on a fit. Open assumptions get clarifying questions first, not a fake firm price. Start from the quote page when files are ready; engineering context also sits on our DFM review page.
FAQ: CNC machining tolerances and ISO 2768
Q: What does ISO 2768-m mean on a CNC drawing? A: It invokes the medium general-tolerance class for dimensions that have no individual tolerance. Under the widely used ISO 2768-1:1989 linear values, a size over 6 mm up to 30 mm then carries ±0.2 mm, and a size over 30 mm up to 120 mm carries ±0.3 mm. Features you care about should still have their own tolerances. Cite the edition on the drawing.
Q: Is ISO 2768-f always better? A: No. Fine is tighter, and therefore usually slower and more expensive to machine and inspect, on every untoleranced size in the class. Use f when the untoleranced features truly need it. Otherwise keep a realistic general class and tighten only the functional callouts.
Q: Does ISO 2768 replace GD&T or hole fits? A: No. Fits belong to an individual tolerance or a system such as ISO 286. Datums, flatness of a seal and true position of locating holes need their own scheme. ISO 2768-2 geometrical classes are only a general backstop when written on the drawing.
Q: What CNC machining tolerance can JHW hold? A: There is no single published number for every part. Tight tolerances are applied to functional faces and confirmed against the drawing, material, quantity and inspection scope in the quotation. Critical dimensions are checked at first article. We do not advertise a blanket ± value or treat ISO 2768 as a capability badge.
Q: Does a title-block ISO 2768 note mean JHW or the partner is “ISO 2768 certified”? A: No. ISO 2768 is a drawing standard for general tolerances, not a management-system certification. We do not claim any certification in this article. The note is a contract on the drawing you release.
Q: Can I visit the production partner on a cold RFQ? A: Visits and audits are not promised on a cold RFQ. If your program requires an on-site path, state it early so commercial and schedule assumptions stay honest.