CNC Machining Tolerances: A Field Guide for Engineers and Sourcing Managers

CNC Machining · Tolerances Deep Dive CNC Machining Tolerances: A Field Guide for Engineers and Sourcing Managers Tolerance is where a drawing becomes either a cheap, repeatable part or an expensive argument with your supplier. This guide explains what tolerance actually means, how it drives cost along a non-linear curve, how GD&T and Cpk turn a wish into a verifiable requirement, and how to specify only the precision your part genuinely needs — so you stop paying for microns you cannot use. Request a quoteWhat tolerance means What tolerance actually means A tolerance is the permitted variation between the dimension on a drawing and the physical part. A bore called out at 12.000 ±0.005 mm may measure anywhere from 11.995 to 12.005 mm and still be a conforming part. Outside that band, it is scrap or rework — no argument, no "close enough." The tolerance is the contract between design intent and manufacturing reality, and everything downstream — cost, lead time, inspection method, scrap rate — is set by how wide or narrow that band is. Two conventions govern how the band is written. A bilateral tolerance splits the variation on both sides of the nominal (±0.005 mm). A unilateral tolerance allows variation in one direction only, typically for fits: a shaft might be 12.000 +0⁄−0.008 mm so it always runs under size. Underneath both sits the international system of IT grades (ISO 286), which classify tolerances from IT01 — laboratory-grade — through IT18 — loose clearance work. Most general CNC work falls around IT9 to IT11; precision work reaches IT5 to IT7; grinding and wire EDM reach IT4 and tighter. The ASM Handbook documents the material and process side of these grades in detail. ASM Handbook reference. Standard vs tight tolerance bands The single most useful frame for a buyer is the tolerance ladder. Each step down costs more and demands more process control, so the job is to land on the step the function needs — not the step the shop is proudest of. The table below is a planning guide, not a guarantee: a given shop's actual floor depends on its machines, thermal control and metrology. Tolerance bandTypical useHow it is heldRelative cost ±0.1 mmClearance holes, non-critical envelopesStandard milling/turning, no special controlBaseline (1×) ±0.05 mmGeneral machined featuresStandard process with basic inspection~1.5× ±0.02 mmFits, locating featuresCareful setup, in-process checks~2–3× ±0.01 mmBearing seats, sealing facesFinish pass, controlled environment~4–6× ±0.005 mmPrecision bores, journalsFinish pass + CMM verification~6–10× ±0.002 mm or tighterGround or wire-EDM featuresGrinding / wire EDM, full inspection10× and up Cost multipliers are indicative. The real curve is process-specific, but the direction is always the same: tighter never gets cheaper. How tolerance drives cost: the tolerance-cost curve For a sourcing engineer. The relationship between tolerance and cost is not linear — it is an accelerating curve, and understanding its shape is the highest-leverage cost knowledge a sourcing manager can hold. At the loose end, tightening a tolerance costs little because the process already lands inside it with slack to spare. But as the band approaches the machine's natural capability limit, every extra micron demands a disproportionate investment: slower feeds, dedicated setups, temperature control, and — the hidden driver — more inspection and a higher scrap allowance. There is a hard floor at the bottom. No machine can hold a tolerance tighter than its own thermal drift, spindle runout and positioning error, and no inspection can certify what it cannot resolve. When the band drops below roughly ±0.005 mm on milling and turning, the only path forward is a different process — grinding or wire EDM — which is slower and more expensive by design. The curve therefore has a kink: cost rises smoothly through the machining range, then steps up when you cross into grinding territory. The buyer's lever is to keep every feature on the cheap, flat part of the curve except the handful that genuinely need to sit on the steep part. Where machining cost actually goes. GD&T basics: true position, flatness, concentricity Plus-minus dimensions control size. Geometric dimensioning and tolerancing controls relationships — and relationships are what make assemblies work. Three symbols cover the vast majority of tolerance work in practice. True position (⊕) locates a feature — most often a hole — relative to datums, inside a cylindrical or rectangular zone. A hole called out at position ∅0.1 mm means its axis must fall within a 0.1 mm diameter zone around the perfect location, regardless of where the part edges happen to be. It is the correct way to tolerance holes that must line up, and it is what lets a shop use the full available location band instead of stacking plus-minuses. Flatness (▱) controls how far a surface deviates from a perfect plane, independent of orientation. It matters on sealing faces, where a gasket or O-ring must compress evenly, and on any face that locates against another part. A face called flat to 0.01 mm cannot be satisfied by thickness alone — it must be measured as a surface, which is why flatness pushes inspection toward a CMM. Concentricity (◎) — and its more practical sibling, runout — controls how a rotating feature shares its axis with a datum axis. It is the tolerance behind bearing journals, spindles and any shaft that must spin true. In practice most engineers now specify circular or total runout instead of concentricity, because runout is directly measurable on the shop floor while concentricity is a derived value that is harder to verify. The point is the same either way: the feature must revolve around the intended axis, not merely be round. The full GD&T symbol set. Tolerance by process: what each method can hold Process sets the ceiling on tolerance, so a smart drawing assigns each feature to the process that can hold it at the lowest cost. The hierarchy below is the practical reality on a well-run floor. ProcessAchievable toleranceBest forNote CNC milling±0.005 mmPrismatic parts, pockets, bores, facesThe workhorse; most features live here CNC turning±0.005 mmRound parts, shafts, journals, threadsExcellent concentricity in one setup Precision grinding±0.002 mmBearing seats, flat faces, tight finishesFiner surface finish and tighter size Wire EDM±0.002 mmHardened steel, sharp internal cornersNo cutting force; cuts any hardness The discipline is sequencing: machine to near-net on the mill or lathe, then grind or wire-EDM only the features that need the last step. Reserve the slow, expensive process for where it earns its cost — a ground bearing seat, a wire-cut slot in hardened tool steel — and let the mill do the bulk. That is the difference between a part that costs what it should and one that pays a grinding premium on every feature. When grinding earns its cost. · Wire EDM explained. Thermal effects: the invisible error in every tolerance Every material expands as it warms, and at tight tolerance that expansion is not a rounding error — it is the dominant source of measurement failure. A steel part 100 mm long grows roughly 1 µm for every 1°C of temperature change; aluminum grows about twice that. A part machined warm and measured cold, or measured on a hot afternoon against a drawing written at a 20°C reference, can drift in and out of tolerance for reasons that have nothing to do with the machine or the operator. A serious shop manages thermal error in three ways. First, it lets the machine and the part reach thermal equilibrium before finish cuts, so the size cut is the size that ships. Second, it keeps the metrology area temperature-controlled, because a CMM reading taken at 28°C on an aluminum part is not comparable to the 20°C drawing. Third, it measures the part and its reference standard under the same conditions and records the temperature, so the report means something. When you qualify a supplier, the thermal question — "how do you control temperature during finishing and inspection?" — separates a precision floor from a machine shop that happens to own precise machines. How we control the environment. How tolerance is verified: the CMM and the first-article report For a quality lead. A tolerance that cannot be measured is not a tolerance; it is an opinion. For single-digit-micron work the standard instrument is the coordinate-measuring machine, which probes a part in three dimensions against the CAD model and reports size, position, form and profile — turning the GD&T callouts on the drawing into measured numbers. The output is a first-article report: a document tied to the lot, the drawing revision and the machine, listing every controlled feature, its measured value and whether it passes. That report, not the machine list, is what proves a supplier can hold tolerance. Supporting instruments close the gaps a CMM leaves: a profilometer for surface finish, a laser microscope or optical comparator for small and fine features, and X-ray fluorescence to confirm the material is what the drawing says. The metrology chain matters because the number on the report is only as trustworthy as the least-calibrated instrument in it. When you compare quotes, compare inspection evidence, not adjectives. The inspection floor in detail. Cpk and process capability: precision that repeats One part that measures in tolerance proves nothing; it could be luck. What a buyer actually needs is a process that stays inside the band across the whole run, and the number that captures this is Cpk. It folds two ideas into one figure: Cp, how wide the process spread is relative to the tolerance, and Ca, how centered that spread is on the target. A process can have a wide tolerance and a narrow spread (high Cp) but sit off-center (poor Ca), so Cpk — which penalizes both — is the honest score. A Cpk of 1.67 or higher is the conventional bar for a key characteristic, with 1.33 accepted for general ones. Numbers make it concrete. Critical characteristics are held to Cpk above 1.67, general features to Cpk ≥ 1.33 — verified by SPC, not by a single lucky part. That is the difference between a shop that can machine one good part and one that can machine a thousand that all stay in tolerance. It is also the number you should ask for in a qualification audit. The measured capability baseline. DFM: don't over-tolerance the part For a manufacturing engineer. The most expensive error on a machining drawing is not a missing dimension — it is a tight tolerance on a feature that does not need one. Over-tolerancing raises cost on every feature it touches, inflates scrap, and forces a shop to inspect and control surfaces that no one cares about. The corrective is a design-for-manufacturing pass that asks one question per feature: what is this feature doing, and how tight does it really need to be? The answer sorts features into two clean piles. A short list needs genuine precision: bearing bores and journals, sealing faces, locating dowels and slots, and pilot diameters that align a mating part. Everything else — clearance holes, cosmetic surfaces, wrench flats, the part body — can run loose, often at ±0.1 mm or looser. A useful habit is to tolerance clearance holes by their function: a through-hole for a bolt needs a clearance band, not a positional micron, and no one ever measured a wrench flat on a CMM. FeatureWhat it needsWhat it does not need Bearing bore / journal±0.005 mm, roundness, runoutCosmetic finish on the OD Sealing faceFlatness, controlled finishTight thickness everywhere else Locating dowel / slotTrue position to datumsTight tolerance on the body Clearance holeA clearance band on sizePosition to microns, CMM inspection Thread (non-locating)Standard thread classFine-pitch precision where a coarse thread fits The payoff of a good DFM pass is asymmetric: it removes cost and scrap risk while adding zero engineering risk, because the features that drive function keep their tight tolerance and only the dead weight is released. A shop that reads your drawing and flags over-tolerance before quoting is saving you money on the spot. The DFM checklist. Material effects on achievable tolerance The material quietly sets the floor on what tolerance is practical. Aluminum (6061, 7075) machines fast and holds tight tolerance well, but its high thermal expansion means temperature control matters more, not less. Stainless (303, 304, 316) is harder to cut but dimensionally stable — the default for instruments and medical parts. Brass and copper cut beautifully and suit precision electrical and fluid parts. Titanium and nickel alloys hold tolerance well but cut slowly and load the tool, so they cost more per micron. Plastics such as PEEK and acetal can be machined precisely but move far more with temperature and clamping pressure than any metal, so a tolerance that is trivial in brass becomes a fight in a soft polymer. The rule is the same as everywhere in this guide: pick the material for the function first, then tolerance it to what that material will reliably hold. Choosing the material. Tolerance stack-up: why a conforming part can still fail One more concept earns its place before you finalize a drawing: a part that passes every individual tolerance can still fail its assembly, because tolerances add up. Put three parts in a stack, each within ±0.05 mm, and the worst-case combined error is ±0.15 mm — three times the per-part band. A fit that works with two nominal parts binds the moment every part lands on the same side of its tolerance. This is tolerance stack-up, and it is the most common reason a “correct” drawing produces an assembly that only sometimes goes together. The fixes are cheap and belong on the drawing, not in the machine. Tolerance the stack, not just the part: run a worst-case or statistical (RSS) stack analysis across the mating chain and set the individual bands so the total lands inside the functional limit. Then use GD&T to loosen non-functional features, which gives the stack room without weakening the fit. A shop that reads your drawing and asks “what does this feature mate with?” is doing stack-up thinking with you — and saving you a batch of parts that pass inspection and still fail assembly. The Nex-G capability baseline: what our floor actually holds At Nex-G in Dongguan Hengli, tolerance is a documented capability, not a sales phrase. The floor — 6,800 m², 100+ staff, operating since 2006 — runs 80+ CNC machines across Mazak, Brother, TSUGAMI and Sodick platforms, and the process split follows the hierarchy above: ±0.005 mm on CNC milling and turning, ±0.002 mm on precision grinding and wire EDM. The quality system is certified to ISO 9001, IATF 16949 (with the clause 8.3 design exclusion — we manufacture to your design, we do not own the design) and ISO 14001, with the next URS audit due in 2027. The number that matters is capability. We target Cpk ≥ 1.67 on key characteristics and ≥ 1.33 on general ones, and we publish the evidence rather than asserting it: critical characteristics are held to Cpk ≥ 1.67 and general features to Cpk ≥ 1.33. Lead times run 3 days for prototypes, 7 days for standard parts and 30 days for complex production, and there is no minimum order — MOQ is one part, so a prototype runs on the same machines and the same process as the production run that follows. The full capability sheet. On the floor the checks are concrete rather than aspirational. Every BOM line is cross-checked against the drawing and the purchase spec before release, so a 6061 callout cannot silently become 5052. Critical stock is bought through a cross-checked second source with a matching mill test certificate, and each incoming lot is confirmed by XRF / PMI before it reaches a machine. For aerospace programs we run FAI per AS9102 so the first article is dimensionally signed off before the run begins. Specifying tolerance on your drawing: a practical checklist Reference the temperature. Tight tolerances are only meaningful at the 20°C reference they were written for; state it and let the shop control to it. Use GD&T for relationships. Position, flatness and runout express function better than a stack of plus-minuses, and they let the shop quote tight where it matters and loose where it does not. Put the tight band only on functional features. Bearing bores, sealing faces and locating features earn their microns; the part body does not. Specify the process only when it matters. Call out grinding or wire EDM where the tolerance demands it, and leave the mill to do the rest. Ask for the report, not the promise. Require a first-article CMM report tied to the drawing revision, and a Cpk number on the key characteristics. The short version: tolerance is a system — machine, workholding, thermal control and metrology — and the drawing is where that system is either set up to win or set up to waste money. How to select the partner. Frequently asked questions What tolerance is standard for CNC machining?General CNC milling and turning hold around ±0.05 mm without special effort, and ±0.005 mm on a precision floor with finish passes and CMM verification. Anything tighter on those processes moves into grinding or wire EDM territory. What tolerance can Nex-G hold?±0.005 mm on CNC milling and turning, and ±0.002 mm on precision grinding and wire EDM, verified on CMMs. Key characteristics are held to Cpk ≥ 1.67. Why does a tighter tolerance cost so much more?The cost curve is non-linear. As the band approaches the machine's capability limit, every micron demands slower feeds, more setups, thermal control, more inspection and higher scrap — and below a point it forces a switch to grinding or EDM. What is a good Cpk for machining?Cpk 1.67 or higher is the accepted bar for a key characteristic, and 1.33 for general ones. It measures both spread (Cp) and centering (Ca), so it is the honest score of whether a process stays in tolerance across a run. How do I stop over-paying for tolerance?Run a DFM pass: put tight tolerances only on bearing bores, sealing faces and locating features, and let clearance holes, bodies and cosmetic surfaces run loose. A good shop flags over-tolerance before quoting. How do you prove a part is in tolerance?With a first-article CMM report tied to the drawing revision and the lot, listing every controlled feature and its measured value, plus SPC data across the run. Critical characteristics are held to Cpk ≥ 1.67. Do you need a minimum order to hold tight tolerance?No — MOQ is one part. A prototype runs on the same machines and process as production, so the first-article data transfers directly to the volume run. Does temperature really change a tolerance check?Yes. Aluminum grows roughly 2 µm per 100 mm per 1°C, steel about half that. A part machined warm and measured cold can fail for thermal reasons alone, which is why serious shops control temperature through finishing and inspection. What is tolerance stack-up, and how do I prevent it?Stack-up is the way individual part tolerances add together across an assembly — three parts at ±0.05 mm can combine to ±0.15 mm of worst-case error, binding a fit that works only at nominal. Prevent it by tolerancing the mating chain, not just each part, and by loosening non-functional features so the stack has room. Specifying tolerance on a real part?Send the drawing to [email protected] — we will confirm what we can hold on the features that matter, flag any over-tolerance, and quote the precision your part actually needs.Request a quote Related articlesGD&T ExplainedPrecision CNC MachiningCNC Machining Cost in China