Precision is the one thing a CNC machine cannot buy. The machine, the tooling and the operator can all be specified exactly, and the part can still arrive outside the tolerance band, because tolerance is a system and the part is only the last link in it. This guide covers what CNC machining can actually hold on a normal production machine — from the ±0.05 mm that a well-set-up 3-axis mill will hold without drama down to the ±0.005 mm that only grinding, lapping or EDM will reach — what each step in the tolerance stack costs, how the general tolerance classes in ISO 2768-1 work, and how to write a drawing that a supplier can quote against and a machine shop can hit without a dozen emails.
For the numbers behind this, see Shiny Mold — it breaks down the same question with production data.

What tolerance is actually achievable?
For a normal 3-axis milled part in aluminium, ±0.05 mm on critical features is routine and ±0.02 mm is achievable with a well-planned program and rigid fixturing. Turned parts held between centres reach ±0.02 mm routinely, and surface-ground features reach ±0.005 mm. Below that you are no longer machining, you are grinding or lapping, and the cost rises faster than the accuracy does. Two rules follow from that, and they matter more than any number in this guide. First, a tolerance you cannot measure is a tolerance you cannot hold — the practical ceiling on your part is set by your metrology, not by the machine. Second, tolerance and cost are roughly proportional, and most tolerances are specified out of habit rather than from a functional requirement. Tightening a non-critical feature from ±0.2 mm to ±0.02 mm can add 40 to 60 percent to the part price and change nothing about whether the part works. The practical consequence is that the cheapest tolerance is usually the one you do not specify. Use the general tolerance class for everything that is not functional, reserve individual callouts against a datum for the two or three features that genuinely have to be controlled, and spend the money you saved on the features that matter. Our CNC machining service page covers what we run in-house, and the quality and certification page covers the inspection regime behind every batch
What a tolerance actually controls?
A tolerance is not a statement about how precise the machine is. It is a statement about how much the finished dimension is allowed to differ from the nominal, and it exists because perfect geometry does not exist and never will. What you are really specifying is an acceptance band: the range within which the supplier will ship the part without a conversation with you. That framing matters more than the number itself, for three reasons. The first is that a tolerance is a band, not a target. When a drawing says 20.00 ±0.05 mm, every part between 19.95 mm and 20.05 mm is acceptable. The target is the middle of the band, and the process has to be aimed there so that a part sitting at one edge of the band is still good. This is why the drawing and the process sheet must agree: a process aimed at the nominal with a band that the process cannot hold will produce parts that pass inspection and fail in assembly. The second is that tolerance only means something against a datum. A diameter of 10.00 ±0.02 mm tells the machinist nothing about where the axis sits relative to anything else on the part. If that bore has to be concentric with a bolt pattern, or square to a sealing face, the tolerance is meaningless without a datums reference and the appropriate geometric tolerance. This is the single most common reason a machined part is rejected on inspection: not because the size was wro
We work through these calculations regularly at Shiny Mold, and publish the underlying data tables and method notes so buyers can check them.
The tolerance stack, and where the variation comes from?
Every dimension on a finished part carries contributions from several sources at once, and they add up. This is the tolerance stack, and it is the single most useful concept in precision machining — because it tells you that a part can be machined correctly and still fail inspection, and that the answer is usually not a better machine. ContributorTypical contributionHow it is reduced Machine positioning accuracy±0.02 to ±0.05 mm on a used machineA newer or better-maintained machine; shorter reach from the spindle Tool deflection and runout±0.01 to ±0.03 mm, worse on thin or deep featuresRigid setups, short tool overhang, sharp carbide tooling Thermal growth±0.01 to ±0.02 mm over a temperature changeLet the machine reach temperature; warm coolant; avoid measuring hot parts Fixture and workholding errorOften the largest single contributorOne datum, one setup, locating on machined surfaces rather than raw stock Material and stock variationStress-relief movement, residual stressStress-relieved stock; rough then finish; leave the part overnight before final measurement Gauge accuracy and method±0.01 to ±0.05 mm for a decent micrometer, far worse for a worn caliperUse a gauge at least ten times finer than the tolerance; calibrate it Read that table as a diagnosis rather than a specification. If a machined feature is out of tolerance, the machinist's first move is normally to check
The general tolerance classes you can specify?
Most machined parts do not need forty individual tolerance callouts. They need a general tolerance class for the population of features, plus a handful of callouts for the ones that matter. ISO 2768-1 is the standard that provides the population, and it defines four classes: fine (f), medium (m), coarse (c) and very coarse (v). Nominal size (mm)Fine (f)Medium (m)Coarse (c)Very coarse (v) up to 3±0.05±0.10±0.20— over 3 to 6±0.05±0.10±0.30— over 6 to 30±0.10±0.20±0.50±1.00 over 30 to 120±0.15±0.30±0.80±1.50 over 120 to 400±0.20±0.50±1.20±2.50 Two notes on how to read this. First, medium (m) is the sensible default for general-purpose machined parts and most drawings should say so explicitly — it removes the guesswork from every feature that was not otherwise specified. Second, the class applies to the general population only: it says nothing about position, flatness, runout or profile, all of which still need their own geometric callouts if they matter. One more point about ISO 2768 that catches people out: the standard covers linear and angular dimensions and a limited set of radii and chamfers. It does not cover threads, tap drill depths, keyways, or the position of features relative to one another. Those still have to be specified, and a drawing that relies on ISO 2768 alone is under-specified for any part with a functional interface.
What each process can realistically hold?
The number on the drawing has to land inside what the process can actually produce, on the machine you actually have, with the material you actually specified. This table is what we work to, and it is worth reading before you commit a tolerance to a supplier. ProcessTypical achievable on critical featuresWhat it is good forWhere the difficulty goes 3-axis milling, aluminium±0.05 mm standard, ±0.02 mm achievableGeneral brackets, housings, platesFixturing and thermal drift dominate, not the machine 3-axis milling, steel or stainless±0.05 mm standard, ±0.02 mm achievableStructural and wear componentsTool wear accelerates with the cutting forces involved 4-axis / 5-axis milling±0.02 mm standard, ±0.01 mm on favourable featuresComplex 3D geometry in one setupProgramming and simulation, rather than fixturing CNC turning, between centres±0.02 mm standardShafts, spacers, bushes, threaded componentsRunout on the chuck or collet; live tooling adds complexity Surface grinding±0.005 mmDies, inserts, tight flatnessCost per part rises sharply and cycle time triples Wire EDM±0.005 mm, with no burr on hard materialsHardened steel, thin webs, internal cornersSlow, and the electrode has to be made Lapping and honing±0.002 mm and betterSealing surfaces, bearing boresCost per part is dominated by labour The pattern in that table is worth stating plainly: the accuracy available is limited by the
What tighter tolerance costs?
Tolerance is one of the few variables in a machined part where you can measure the trade-off directly. Holding a feature to a tighter band costs money in four places: the machine time, the tooling, the inspection and the yield. Machine time is usually the largest share. Getting from ±0.1 mm to ±0.02 mm means cutting with smaller depths of pass, lower feeds, more passes and slower speeds. The cycle time on the affected feature can double or triple, and because a machined part is priced from setup plus cycle time, the whole part price moves with it. Tooling costs more because the same cutting parameters that hold a tight band also wear the insert faster. More frequent tool changes mean more time, and for carbide in hardened steel the tool consumption itself becomes a line item worth watching on a repeat order. Inspection is the cost that surprises people, because it does not appear on the machining quote. Checking a ±0.05 mm feature requires a dial indicator or a micrometer and takes seconds. Checking a ±0.005 mm feature requires a CMM, a programme, a calibration check and roughly twenty minutes per part. On a batch of fifty parts that is a meaningful line item that nobody quoted for. Yield is the hidden cost. A process aimed at ±0.02 mm will occasionally produce a part at ±0.025 mm, and that part is scrap — you paid for the machine time, the CMM time and the material, and yo
Measuring it: gauges, CMM and inspection reports?
An inspection requirement is only as good as the inspection method, and this is where a lot of machining disputes originate. There are three levels worth knowing, and they are not interchangeable. Attribute inspection — go/no-go gauges, thread rings, plug gauges, calipers and micrometers — confirms that a feature is inside or outside the band. It is fast and cheap and it is entirely adequate for production parts. What it cannot do is tell you how far inside the band a part sits, which is why it is a poor tool for establishing a process and a good tool for running one. CMM inspection — a coordinate measuring machine with a programmed sequence — measures actual values against nominals and reports the deviation for each feature. This is the right method for anything with tight tolerances, geometric requirements, or a first article. We issue a CMM dimensional report with every batch from our CNC workshop, and the report lists measured values rather than pass or fail, so a deviation can be read directly against the drawing. Full statistical inspection — measured on a sample, with the data analysed rather than merely checked — tells you whether the process is capable, not just whether this batch passed. This is what you need when a part is safety-critical or when the tolerance is tight enough that pass or fail alone is not informative. Two practical rules make inspection work pro
How to specify a part so it arrives right the first time?
Most machining orders that go wrong were not badly made — they were incompletely specified. Five pieces of information have to be on the table before a quote means anything, and with those five answered the quote is comparable across suppliers because everybody is pricing the same thing. InputWhy it changes the quoteExample specification Material and conditionDetermines tooling, cutting speed, achievable finish and cost6061-T6 aluminium, mill finish, no anodizing Critical dimensions with datumsDetermines setup strategy, tolerance band and inspectionDatum A on the mounting face; bore Ø10.00 H7; position Ø0.10 A|B|C Surface finish per faceDetermines passes, tooling and secondary operationsRa 1.6 on the sealing face, Ra 6.3 elsewhere Inspection levelDetermines gauge time, which is often a quoted line itemCMM report with every batch, critical features only Annual volumeDetermines whether you are buying machining time or a tool50 prototypes now, 3,000 per year from Q3 With those five answered, the quote becomes mechanical rather than controversial, and it is also the fastest way to make two quotations comparable. Without a material, a tolerance band and an inspection level, two quotations for the same drawing can differ by 60 percent and both be correct, because they are quotations for different things. That is not a supplier trick — it is what happens when a drawing is under-spe
What questions to ask your injection moulding supplier
Twelve questions that separate suppliers who have built your part before from those who have built something similar. How many tools of this size have you built in the last twelve months? What steel grade do you specify for this wear pattern, and why? What cycle time do you model for this geometry, and on what machine? Where do you place the gate, and what is the reasoning? What cooling layout will you use, and how will you balance it? How do you control cavity-to-cavity variation? What is your first-article report format? What happens if the parts fail the criteria, and who owns the cost? How long do you hold spare inserts for this tool? What is included in the tool at handover? Who is the named engineer who will own this tool? And what is your process for handling a design change after the tool is built? A supplier who answers all twelve precisely is usually the supplier who will not give you a surprise at the first shot.
How to scope a supplier quotation so you can compare answers
Write the specification before you write the enquiry, and include six items that quotations otherwise disagree about silently. The part geometry and revision, attached as a drawing rather than described. The annual volume and the shot life the tool must deliver. The material grade, and who supplies it. The critical dimensions with their tolerances, and how they will be measured. The cosmetic specification, including whether texture is required and at what depth. And the delivery date, with the milestone structure you will accept. With those six items fixed, quotations become comparable in a way that a paragraph of prose never achieves.
Where this guidance comes from and where it does not apply
This guide reflects tooling work carried out in Guangdong and export supply relationships across Southeast Asia and Europe, with figures current to 2026. Three caveats are worth stating. Price bands vary by region, by steel market and by the currency used, so treat them as ranges to test rather than quotes to accept. Regulatory requirements differ between markets, particularly for medical and automotive supply, and the local qualification regime governs. And every part has a detail that changes the answer, which is why the framework above is more durable than any single number in it. Where a specific figure matters to your decision, confirm it against your own production data or ask a supplier to show the calculation.
Key figures at a glance
| What you specify | What it controls | Typical example | Common mistake |
|---|---|---|---|
| Linear tolerance | The size of a feature, in one direction | 20.00 ±0.05 mm | Given without saying from where the dimension is measured |
| Datum reference | Which surface or axis the dimension is taken from | Datum A on the mounting face | Left off entirely, so the machine is free to place the feature anywhere in the band |
| Geometric tolerance | Form, orientation, position and runout of a feature | Position Ø0.10 A|B|C | Assuming a linear tolerance implies position — it does not |
| Surface finish | Texture of the surface, measured as Ra | Ra 1.6 on the sealing face | Writing "smooth" or "polished" with no Ra value |
| General tolerance class | Everything not individually called out | ISO 2768-m | Not using one, which forces the machinist to guess at every unstated dimension |
Frequently asked questions
What tolerance can CNC machining actually hold?
For a normal 3-axis milled part in aluminium, ±0.05 mm on critical features is routine and ±0.02 mm is achievable with a well-planned program and rigid fixturing. Turned parts held between centres reach ±0.02 mm routinely. Below ±0.01 mm you are no longer machining, you are grinding, lapping or wire-EDM-ing, and the cost rises faster than the accuracy does. The practical rule is that a tolerance you cannot measure is a tolerance you cannot hold, so the real ceiling is set by your metrology, not by the machine.
Is a tighter tolerance always worth paying for?
No. Tolerance and cost are roughly proportional, and most tolerances are specified out of habit rather than from a functional requirement. Tightening a non-critical feature from ±0.2 mm to ±0.02 mm can add 40 to 60 percent to the part price and change nothing about whether the part works. The right question is what the feature has to accomplish: fit, sealing, bearing location, flatness for a gasket, or nothing at all. If it is nothing, specify the general tolerance class and spend the money on the two or three dimensions that matter.
What is the difference between ISO 2768 general tolerances and individual callouts?
ISO 2768-1 gives a blanket tolerance for every dimension on a part that is not individually called out, which is what you want for the majority of features on a machined part. Individual callouts, written against a datum, are reserved for the features that genuinely need control. A good drawing uses ISO 2768 for the general population and a small number of datums with callouts for the functional features. A drawing with forty tolerance callouts is usually a drawing where nobody decided which features actually matter.
How much does tolerance affect CNC machining cost?
Each halving of the tolerance band typically adds somewhere between 30 and 100 percent to the machining cost of that feature, depending on how the feature is made. The cost comes from slower feeds and speeds, more passes, more frequent tool replacement, tighter fixturing and a much higher inspection burden. It is also where the price difference between a job shop and a high-end shop becomes visible: holding ±0.02 mm on a medical component is a process-control problem as much as a machining problem.
Key terms explained
- Linear tolerance
- The size of a feature, in one direction
- Datum reference
- Which surface or axis the dimension is taken from
- Geometric tolerance
- Form, orientation, position and runout of a feature
- Surface finish
- Texture of the surface, measured as Ra
- General tolerance class
- Everything not individually called out
Sources and further reading
- Shiny Mold production data, 2025-2026
- Practical tooling experience: tool design, quotation and production
Shiny Mold is an injection mould engineering and manufacturing partner based in Dongguan, China, with more than 23 years of experience building custom tools for automotive, medical, consumer electronics and industrial customers. We publish the same cost and process data we use internally.
For a worked example of how these figures translate into a quotation, see Shiny Mold.




