Dewey Wu General Manager & senior mechanical engineer at EPOC CRAFTER, 15 years in design engineering, quality, and metallurgy. Hands-on across CNC machining, metalwork, sheet metal, and prototyping (subtractive + 3D printing).
A CNC tolerance costs what it costs because of the process, machine, and inspection the number forces at a given size, not because of the ± value on the drawing. Move from ±0.1 mm down through ±0.05, ±0.025, ±0.01, and ±0.005 mm, and each step crosses a point where the shop switches tools, adds a finishing operation, or moves inspection from a caliper to a CMM. Figures put that jump at roughly 1.5x to 3x per tier once a feature crosses into reaming, boring, or grinding. The real multiplier is a quote question, set by material, geometry, feature type, process route, fixturing, surface finish, quantity, and inspection method. One rule frames the rest: a ± value or an IT grade means nothing until you attach it to a nominal size. IT7 is 0.015 mm on a 10 mm bore and 0.035 mm on a 100 mm bore, the same grade at more than double the band.
1. What each tolerance tier costs
The table pairs each tolerance tier with the process it forces, how the feature gets verified, and the cost relative to a ±0.1 mm baseline. Read the cost column as a direction, not a quote, since the multiplier depends on the eight factors above.
Table 1. Tolerance tier to process, inspection, and relative to a ±0.1 mm (ISO 2768-medium) baseline.
| ±0.1 mm | IT12 to IT14 | Standard milling or turning, as-machined | Vernier caliper | 1.0x (baseline) |
| ±0.05 mm | IT10 to IT11 | Finish milling pass | Micrometer | ~1.1 to 1.3x |
| ±0.025 mm | IT8 to IT9 | Turning on diameters, finish boring | Micrometer, dial indicator | ~1.3 to 1.6x |
| ±0.01 mm | IT7 | Reaming, precision boring, or jig grinding | CMM | ~1.8 to 2.5x |
| ±0.005 mm and tighter | IT5 to IT6 and below | Grinding, lapping, or honing | Full CMM, air gauge | ~2.5 to 4x and up |
Two patterns drive most tolerance-cost decisions. Cost steps rather than climbs: ±0.1 mm to ±0.05 mm stays inside one milling operation, while ±0.025 mm to ±0.01 mm adds a second operation and a move to CMM inspection, which is where the multiplier roughly doubles. The expensive jumps sit at the process boundaries. Inspection is a cost line of its own: three features at ±0.025 mm take a few minutes per piece, while twenty on a CMM can run past half an hour per piece, a separate inspector at volume. Section 2 shows why the same IT7 callout is not one physical band.
2. Why an IT grade or ± value means nothing without nominal size
A tolerance is a band, and the band grows with the size of the feature it sits on. The ISO system sets the width with an IT number, scales that width with the nominal size, and locates the band with a letter. Skip the size and you cannot know what a callout costs, because the same number lands on a different process at a different diameter.
2.1 IT is a width, and it scales with size
Place one callout, ±0.01 mm, which is a 0.02 mm total band, on four diameters. The physical band stays fixed, but the IT grade it represents tightens as the part grows, and so does the process needed to hold it.
Table 2. The same ±0.01 mm callout (0.02 mm total band) across nominal size, against standard IT7 values from ISO 286-1.
| Ø10 mm | 0.015 mm | Looser than IT7, near IT8 | Finish milling or reaming |
| Ø25 mm | 0.021 mm | About IT7 | Reaming or precision boring |
| Ø50 mm | 0.025 mm | Between IT6 and IT7 | Precision boring or jig grinding |
| Ø100 mm | 0.035 mm | Between IT5 and IT6 | Grinding |
A single ±0.01 mm note across a drawing does not buy uniform precision, it buys rising cost as features grow: a reamer holds it on a 10 mm bore, a grinder is needed on a 100 mm bore. Set the band per feature, sized to what that feature does.
2.2 Why H7 is not ±0.0105 mm
A fit callout does not center the band on nominal, which is the mistake behind translating H7 into a symmetric ±. For a 25 mm bore, ISO 286 gives H7 as +0.021 / 0, so the bore runs from 25.000 mm to 25.021 mm and never below nominal. Write ±0.0105 mm instead and you allow 24.9895 mm, which lets the bore run undersize and bind the shaft it should clear.
Table 3. A 25 mm clearance fit written three ways. Deviations from ISO 286-2 in millimetres.
| Ø25 H7 (hole) | 0 | +0.021 | Bore never undersize |
| Ø25 g6 (shaft) | -0.020 | -0.007 | Shaft always clears the bore |
| H7/g6 fit | n/a | n/a | Clearance from 0.007 to 0.041 mm |
| Ø25 ±0.0105 (wrong substitute) | -0.0105 | +0.0105 | Bore may run undersize and bind |
The fit letters carry design intent that a symmetric ± throws away, and they cost less to hold, because the machinist works to one edge of the band and lets tool wear walk the dimension in the safe direction. When a feature has to slide, press, or rotate against another, reach for a fit class, not a raw ±. The full set of clearance, transition, and interference pairs sits in the guide to ISO 286 shaft and hole fits.
EPOC CRAFTER engineering note. A ±0.01 mm note dropped on every dimension of a 120 mm plate is the most common way a drawing over-buys precision, since most of those features never touch another part. The fix is a drawing decision made before the RFQ: default the plate to a general class and tighten only the bores that locate something.
3. The general-tolerance baseline you get for free
Most drawings ride on one line in the title block, and that line is the 1.0x baseline. ISO 2768-medium fills in a permissible deviation for every dimension you did not tolerance by hand, and standard milling and turning hold it as-machined with a caliper check, so nothing in this class carries a premium.
Table 4. ISO 2768-1:1989 permissible deviations for linear dimensions, classes f, m, c. Values in millimetres.
| 0.5 up to 3 mm | ±0.05 | ±0.1 | ±0.2 |
| over 3 up to 6 mm | ±0.05 | ±0.1 | ±0.3 |
| over 6 up to 30 mm | ±0.1 | ±0.2 | ±0.5 |
| over 30 up to 120 mm | ±0.15 | ±0.3 | ±0.8 |
| over 120 up to 400 mm | ±0.2 | ±0.5 | ±1.2 |
Two facts decide whether upgrading the general class is worth anything. Upgrading the whole drawing from m to f is a weak lever, because the f class only tightens linear sizes, while external radii, chamfers, and angular dimensions read the same in both columns. And no general class reaches a fit: class m on a 25 mm feature allows ±0.2 mm, roughly IT14, against the 0.021 mm an H7 bore needs. Leave the drawing on a general class, then spend the tier premiums only on the features that locate, seal, or fit. The full class tables and the ISO 22081 change that retired the old geometrical half sit in the reference on ISO 2768 general tolerance classes.
4. The process ladder: milling, boring, grinding, lapping
Each tolerance tier maps to a machining operation, and the cost steps from Section 1 are the moments you climb from one to the next. A finer surface finish rides along, because both come from the same slower pass.
Table 5. Process to as-machined tolerance, IT band, and surface finish.
| Milling, as-machined | ±0.05 mm | IT10 to IT11 | 1.6 to 3.2 µm | Default for prismatic features |
| Turning on diameters | ±0.025 mm | IT8 to IT9 | 0.8 to 1.6 µm | Round features that rotate about one axis |
| Reaming, precision boring | ±0.01 mm | IT7 | 0.4 to 1.6 µm | A bore that has to hold a fit |
| Grinding, jig grinding | ±0.005 to ±0.002 mm | IT5 to IT6 | 0.2 to 0.4 µm | Hardened parts or sub-0.01 mm size |
| Lapping, honing | ±0.0025 to ±0.001 mm | IT3 to IT5 | 0.05 to 0.1 µm | Sealing, sliding, or gauge-grade surfaces |
Two patterns change how you read a tight callout. Turning holds a tighter diameter than milling holds a prismatic size at the same nominal, because the part rotates about a fixed axis while a milled wall depends on tool deflection, so a ±0.02 mm band that needs grinding on a milled slot can come off a lathe. If a feature can be a turned diameter instead of a milled boss, it often drops a cost tier for free. Surface finish is a separate lever: a loose size with a tight Ra still climbs the ladder, because reaching Ra 0.4 µm needs the same finishing pass a tight size needs. The Ra each process delivers sits in the chart of surface roughness Ra by process. A drawing that defaults to a general class and names a fit on two bores maps onto the CNC machining capabilities EPOC CRAFTER runs, at ISO 2768-m by default and ISO 2768-f on request.
EPOC CRAFTER engineering note. The jump that surprises buyers is reaming to grinding, not milling to turning. Reaming and boring stay in the machining center that cut the part, so the cost is a tool and a slower pass; grinding is a separate machine, setup, and inspection, which is why cost roughly doubles at the ±0.01 mm to ±0.005 mm boundary rather than climbing in even steps.
5. The inspection ladder: caliper, micrometer, CMM
Inspection is priced per piece, and it climbs on two axes: how tight each feature is, and how many tight features the part carries. The gauge you need sets a floor under every band you specify, on top of the cutting cost in Section 1.
Table 6. Gauge to the tolerance it can verify and the per-piece cost it carries.
| Vernier caliper | 0.02 to 0.05 mm | ±0.1 mm and looser | Seconds, on the machine |
| Micrometer, dial indicator | 0.001 to 0.01 mm | ±0.05 to ±0.025 mm | A minute or two per feature |
| CMM | Sub-micron | ±0.01 mm and tighter | Minutes per part, off the machine |
| Air gauge, gauge blocks | Sub-micron | ±0.005 mm and tighter | Dedicated setup per feature |
The gauge has to resolve finer than the tolerance it checks. A standard gauge R&R practice wants the measurement system to resolve to about a tenth of the band, so a caliper reading to 0.05 mm cannot verify a ±0.01 mm bore, and any feature tighter than about ±0.025 mm pulls the part onto a CMM whether the machining needed it or not. Feature count multiplies the time, and a ±0.005 mm feature often escalates from first-article to sampled or 100 percent inspection. Real inspection routines on finished parts show up in the inspection commentary from production runs. The lever here is count, not depth: dropping a drawing from twenty tight features to three does more for unit cost at volume than loosening those three a tier, because most dimensions go back onto hand gauges.
6. What tightening one tier actually costs
The cost of a tolerance is set by the tightest feature on the part, because that feature chooses the process route and the gauge for the whole job. That is why deleting a tight callout saves more than relaxing it a tier. Published CNC cost breakdowns put a fit-grade feature at more than double a general-class one, and sub-0.01 mm work at up to triple the baseline. The expensive mistake is precision where nothing needs it: a ±0.025 mm band written across a 50 mm length that carries no fit runs about 1.8x the general-class cost and buys nothing.
Table 7. Two ways to tolerance the same aluminum housing.
| Fit where it matters | ISO 2768-m default, Ø25 H7 on the one locating bore | Standard milling, ream the bore, CMM the bore only | Baseline |
| Tight everywhere | ±0.01 mm on every dimension | Finishing pass on every feature, CMM most of them | Roughly 2x and up |
Both drawings make a working part; the second pays a fit-grade premium and CMM time on features that would function at a general class. The rule is short: tighten only the two or three features that locate, seal, slide, press, or rotate against another part, and leave the rest on the general class.
7. Why the same tier costs more on 316L or titanium
The same ±0.01 mm band is a different job in aluminum, stainless, and titanium, because machinability sets how well a process holds a tolerance. That material factor stacks on the tolerance-tier multiplier from Section 6, it does not replace it.
Table 8. Material effect on the cost of holding the same tolerance tier, relative to Al 6061-T6.
| Al 6061-T6 | Cuts clean, sheds heat, holds tight bands with standard feeds | 1.0x (baseline) |
| SS 316L | Work-hardens under a dull edge, gummy chips, slower feeds, faster tool wear | ~1.5 to 2x |
| Ti-6Al-4V | Low thermal conductivity keeps heat in the tool, rapid wear, low speeds and flood coolant | ~2.5 to 4x |
The alloy changes the feeds, the tool life, and the passes needed to reach the same band. Al 6061-T6 holds a fit-grade bore with standard tooling; SS 316L needs sharper tooling and slower feeds, and Ti-6Al-4V wears the tool fast enough that a one-pass aluminum feature takes several passes in titanium. The machinability data that separates these alloys sits in the material machinability data reference. Geometry moves the band as much as material does: a wall under about 1 mm flexes under cutting force and springs back after the pass, a deep bore with a long tool stickout chatters, and thin walls drift as residual stress releases off the fixture. Read tolerance, material, and geometry as one specification: a ±0.005 mm band on a titanium thin wall is a different order of cost than the same band on an aluminum boss. The material multiplier and the geometry penalty compound rather than average, so when a feature has to be tight, thin, and in a hard alloy, ask whether it can move to a stiffer area or a friendlier material.
8. How to spec so you don’t overpay
Most of the cost you control is decided on the drawing, before anyone quotes it, and the tolerance callouts, not the geometry, are where a simple part turns expensive. Run this checklist before you release a drawing:
- Default the title block to ISO 2768-m, and reserve ISO 2768-f for a part where most features are small and precise.
- Mark every feature that locates, seals, slides, presses, or rotates against another part, usually two or three.
- Call out a fit class such as Ø25 H7 or Ø25 g6 on each mating feature, not a raw ±.
- Size each tight band to its nominal, since an IT grade widens with size, so do not copy one ± value across features of different sizes.
- Set a fine Ra only where a surface needs it, since a tight roughness callout is its own finishing pass.
- Before you tighten a feature past about ±0.025 mm, ask whether a fixture, a go/no-go gauge, or a functional test can verify it instead of a CMM on every piece.
- Flag any feature that combines a tight band, a thin wall or deep bore, and a hard alloy, because those three compound the cost.
- Send the drawing for a DFM review before you commit, since the callouts that move the quote are visible at review.
The framework for which features earn an individual tolerance, which stay under the general class, and where geometry needs GD&T is set out in how to tolerance a CNC drawing. The upstream design moves that keep a part cheap to hold, such as wall thickness, bore depth, and feature access, sit in the DFM design guidelines.
A drawing that names a fit on the two bores that matter and leaves the rest on ISO 2768-m gets a lower number back than a drawing that asks for precision everywhere, and it does it without changing the part.
9.Frequently Asked Questions
How much more does ±0.01 mm cost than ±0.1 mm on a CNC part?
Breakdowns put a fit-grade feature at more than double a general-class one, and sub-0.01 mm work at up to triple. The jump is not smooth: it lands when the feature crosses from milling into reaming, boring, or grinding, and from a caliper onto a CMM. The figure moves with size, material, and feature count, so a ±0.01 mm bore on a small aluminum part sits near the low end and a large or titanium one near the high end.
Is ±0.005 mm possible with CNC machining?
Yes, on the right feature, with grinding or lapping and a CMM or air gauge to verify it. As-machined milling and turning do not reach ±0.005 mm, so the feature moves to a separate grinding or lapping operation, which is a second setup and its own inspection. Size and material decide whether it is routine or hard: ±0.005 mm on a small hardened-steel diameter is standard grinding work, while the same band on a large span or a thin wall needs temperature control and stress management.
Does a tighter tolerance always need grinding?
No. Grinding starts around ±0.005 mm and below, while ±0.01 mm is usually reachable by reaming or precision boring inside the same machining center that cut the part. The move to grinding is the expensive step, because it adds a machine, a setup, and separate inspection, so a reamed ±0.01 mm feature stays far cheaper than a ground ±0.005 mm one.
What tolerance applies if I don’t specify one?
The general class in the title block applies, and if the drawing carries none, the shop falls back on its own house default, which you cannot predict. Writing ISO 2768-m sets a known band on every unstated dimension and costs nothing extra, because standard machining holds it as-machined. A blank title block is the one case where you lose control of both the tolerance and the price.
Why does the same tolerance cost more on 316L or titanium than on aluminum?
The alloy changes how many passes, how much tool wear, and how slow a feed the shop needs to hold the same band. Al 6061-T6 sheds heat and cuts clean, so a fit-grade bore comes off with standard tooling. SS 316L work-hardens and Ti-6Al-4V holds heat in the cutting zone, so both need slower feeds and more tool changes for the identical band, which is 1.5x to 4x material premium.
Related Resources
Related Capability: the CNC machining service page. The standard tolerances, materials, and finishes EPOC CRAFTER holds, and what moves to a fit grade on request.
Related Article: H7, g6, and interference fit selection. How to pick the fit class for a shaft and hole instead of writing a raw ± on a mating diameter.
Related Standards Reference: the ISO and ASME standards library. Full deviation tables and the standards EPOC CRAFTER machines to, including ISO 2768 and ISO 286.
Related Case Study: quality events and inspection commentary. How general and individual tolerance callouts play out on real production runs.
Ready to Quote Your CNC Prototype?
Upload your STEP file and get a DFM review + quote within 12 hours.
No tooling cost. Minimum 1 part.
