Guide
What does a too-tight tolerance cost on a machined part?
A too-tight tolerance is a limit on a drawing that is narrower than the function of the part requires. It costs money twice: once in the extra machining, inspection and scrap needed to hold it, and again when a feature that never mattered gets flagged, questioned or rejected.
By Saola Manufacturing engineering team · Published · Updated
This guide uses the ISO 286 system of IT grades as a common scale, so a tolerance can be judged by how hard it is rather than by how small the number looks. It then covers where the cost sits, why inspection grows faster than cutting, and a checklist for relaxing dimensions before a drawing goes out for quotation. It describes general practice and published standards, not any shop’s capability or pricing.
On this page
Why do tighter tolerances cost more to machine?
Every machining process has a natural spread of sizes, and a tolerance band that is narrow compared with that spread forces the shop to slow down, control more variables and check more parts. The cost does not rise in a straight line: each step tighter removes margin the process was using to absorb tool wear, heat and setup error.
Think of the tolerance band as a budget. Tool wear, heat growth, clamping distortion and measurement uncertainty all draw on it. On a loose tolerance, all of those together use a small share of the band and the part is made at full speed with occasional checks. On a tight one, the same effects use most of the band, and every one of them has to be managed.
Managing them is where the time goes: lighter finishing passes, more frequent offsets and tool changes, warm-up cycles before the first good part, parts left to cool before measuring, and a higher share of parts measured. Past a certain point, the feature moves off the lathe or mill to a different process altogether, typically grinding, honing or lapping, which adds a second setup and a second route through the plant.
A bearing seat, a sealing bore or a locating pin earns its tolerance. The cost problem is the tolerance copied from an old drawing, set by a CAD default, or tightened “to be safe” on a face that touches nothing.
How do ISO 286 IT grades show how hard a tolerance is?
ISO 286-1 defines standard tolerance grades, IT01 through IT18, that scale with the nominal size, so the same grade means the same level of difficulty on a small pin and a large bore. Reading a tolerance as an IT grade shows whether it is ordinary machining or precision work far better than the raw number does.
| Nominal size (mm) | IT5 | IT6 | IT7 | IT8 | IT9 | IT10 | IT11 |
|---|---|---|---|---|---|---|---|
| over 6 up to 10 | 6 | 9 | 15 | 22 | 36 | 58 | 90 |
| over 18 up to 30 | 9 | 13 | 21 | 33 | 52 | 84 | 130 |
| over 30 up to 50 | 11 | 16 | 25 | 39 | 62 | 100 | 160 |
| over 80 up to 120 | 15 | 22 | 35 | 54 | 87 | 140 | 220 |
Per ISO 286-1, the grades from IT6 upward follow a geometric series: each grade is about 1.6 times wider than the one before, and the band grows tenfold every five grades. So moving a diameter from IT9 to IT7 is not a small refinement. It takes away well over half of the band the process had to work with.
To use the table, convert the drawing tolerance to a total band and find the grade that matches at that size. Per ISO 286-1, a 40 mm diameter with a 26 µm total band sits right at IT7 for that size range. A band that narrow on a turned diameter is reviewed feature by feature; see the CNC turning page. Per ISO 2768-1 Table 1, the medium general tolerance class gives a total band of 600 µm for sizes over 30 mm up to 120 mm, which per ISO 286-1 is close to IT14 at 40 mm.
Those two comparisons frame most drawings. The general tolerance note covers the bulk of the part at a coarse grade that any competent shop holds without special effort. The individually toleranced features are where the grade jumps, and every jump of two or three grades is a feature a quoting engineer will look at closely. When one part carries dozens of IT6 or IT7 callouts, the price reflects each of them.
The grade also hints at the route. As typical industry guidance, IT9 to IT11 is ordinary turning and milling, IT7 to IT8 is careful finish machining, and IT6 and finer on a diameter often points toward grinding. Exact limits depend on the material, the feature length, the wall thickness and the machine, which is why a supplier reviews tight features one by one.
Where does the extra cost of a tight tolerance actually go?
Most of it goes into time around the cut rather than the cut itself: setup and warm-up, slower finishing, in-process checks, final inspection and the parts that are scrapped. A second process such as grinding, when it becomes necessary, adds its own setup and handling on top.
- Setup and first-article approval. A tight feature takes longer to dial in, and the first good part arrives later in the run. On small batches that fixed time is spread over few parts.
- Cycle time. Finishing passes get lighter and slower, and the program may add probing or a spring pass to take out deflection.
- Tooling. Inserts are changed on a schedule set by size drift rather than by edge breakdown, so fewer parts come off each edge.
- Inspection. Sampling plans get denser, and some features move from a hand gauge to a coordinate measuring machine in a controlled room.
- Scrap and rework. When the band is narrow relative to process spread, more parts land outside it, and their cost is carried by the good ones.
- Secondary operations. Grinding, honing or lapping means another machine, another fixture and another move between departments.
Material matters too. Aluminum moves more with temperature than steel, thin-walled parts deflect under clamping, and parts with heavy stock removal can relieve stress and change shape after they come off the machine.
Why does inspection get expensive at tight tolerances?
Because the measurement itself starts to use up the tolerance: every instrument has an uncertainty, and under the decision rules of ISO 14253-1 a part is only proven conforming when its measured value sits inside the limits by at least that uncertainty. The tighter the band, the larger the share taken by measurement, and the better (and costlier) the measuring method has to be.
The arithmetic is simple. Per ISO 14253-1, if a 16 µm band is checked with an expanded uncertainty of 2 µm, the zone in which a supplier can prove conformance shrinks to 12 µm, a quarter of the band gone before a single chip is cut. The NIST guidelines on evaluating and expressing measurement uncertainty describe how that expanded uncertainty is built up and reported, usually with a coverage factor of 2. A shop that wants margin has to measure better, which means better instruments, a controlled environment and more time per part.
Temperature is the other hidden cost. Per ISO 1, dimensions on a drawing are defined at a reference temperature of 20 °C, a convention whose history NIST has documented, noting that steel expands by about 12 millionths of its length per degree Celsius and brass by about 24 (Doiron, NIST, 2007). At those rates, per ISO 286-1 arithmetic, a 50 mm steel diameter measured 5 °C warm reads about 3 µm large, roughly a fifth of its IT6 band, and a brass one about 6 µm, more than a third. On an IT10 feature nobody would notice; on an IT6 feature it decides whether the part passes.
That is why tight features typically bring requirements that loose ones never need: parts soaked to room temperature before measurement, gauges calibrated against traceable standards, and a stated measuring method so that the supplier and the receiving inspector get the same answer.
Which dimensions can usually be relaxed without affecting function?
Any dimension that does not mate, seal, locate, move against another part or carry a calculated load can usually go to the general tolerance. A short review of the drawing against that list, done before the RFQ, is typically the cheapest cost reduction available.
Work through the drawing feature by feature and ask of each individual tolerance:
- Does it touch anything? External faces, cosmetic chamfers, relief grooves, clearance holes and pockets for weight saving rarely need more than the general note.
- Is it a fit? If a diameter exists to fit a bearing, pin or bore, write it as an ISO 286 fit such as H7/g6 and remove any extra tolerance that repeats it. The fit states the intent and lets the supplier see which side of the band matters.
- Is it in a stack-up? If several tolerances add up to one functional gap, check whether all of them need to be tight or whether one adjustable or ground feature can absorb the stack.
- Is the datum the one that matters? A tight position measured from a face the assembly never uses creates inspection work without controlling function. Datum the part the way it is assembled, per ASME Y14.5 or the ISO GPS standards.
- Did the tolerance come from a template? Title-block defaults with too many decimal places, CAD-generated limits and tolerances carried over from a different material or process are the most common sources of unneeded precision.
- Is roughness called out on every surface? Give Ra only where it does work, such as seals, bearing seats and sliding faces.
For a die-cast part that is machined afterward, the same logic applies with one addition: mark which faces are machined. Faces that stay as cast follow casting tolerances, and a tight tolerance on an as-cast face either forces a machining operation or cannot be met. The ISO 2768 and NADCA tolerance guide covers how those general classes work.
How should tight tolerances be flagged when sourcing from an overseas shop?
List every feature tighter than the general class in the RFQ itself, with the reason it is tight and how it will be measured at receiving inspection. A supplier in Vietnam, Mexico or anywhere else can then quote the real requirement instead of pricing in risk for every number it cannot interpret.
Distance changes the economics of a tight tolerance. When a disagreement about a measured size takes an email thread across time zones and a shipment already on the water, the cost of a questionable feature is no longer just machining time. The fix is to agree on the inspection before production: which features are critical, which instrument or gauge checks them, at what temperature, and what the first-article report must show. Both ends then measure the same thing the same way.
It also helps to separate “must hold” from “nice to have”. A short table in the RFQ with each critical feature, its tolerance and its function lets the quoting engineer suggest a cheaper route to the same function, such as a looser diameter with a reamed bore, or a fit instead of paired limits. A note like this usually shortens the question-and-answer round before a firm price, whether the part is turned or goes to CNC milling.
The machining RFQ guide lists the rest of the package. When the drawing is ready, send it for a quote; any tolerance that drives cost is named in the reply, feature by feature, with the reason.
Frequently asked
Is there a formula for how much a tighter tolerance adds to cost?
No single published formula applies to every part. The cost depends on the material, the feature, the batch size and whether the tolerance forces a second process. The reliable signal is the IT grade: each step tighter narrows the band sharply, and features that move to grinding or a controlled-room measurement cost noticeably more.
Should I just use the general tolerance everywhere and let the supplier decide?
No. Features that mate, seal or locate need their own tolerance or a fit, or the part may not assemble. The goal is to tolerance by function: tight where the part does work, general everywhere else.
Does a tighter tolerance make the part higher quality?
Only if the function needs it. A tolerance tighter than the function requires does not make the assembly work better; it raises cost and the number of parts rejected for reasons that do not matter in use.
How do I know which of my tolerances are driving the price?
Ask the supplier. A good quotation response names the features that push the route or the inspection plan, and says what tolerance would remove the extra step. Sending the function of each tight feature with the RFQ makes that answer quicker and more useful.
Are inch tolerances like plus or minus half a thousandth tight?
It depends on the size. Converted to a total band and read against ISO 286-1, the same inch tolerance is a coarse grade on a small pin and a fine grade on a large bore, which is why the IT grade is a better guide than the number of decimal places.
Sources
- ISO 286-1:2010, Geometrical product specifications (GPS) — ISO code system for tolerances on linear sizes — Part 1: Basis of tolerances, deviations and fits, ISO, 2010
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions, ISO, 1989
- ISO 14253-1:2017, Geometrical product specifications (GPS) — Inspection by measurement of workpieces and measuring equipment — Part 1: Decision rules for verifying conformity or nonconformity with specifications, ISO, 2017
- Taylor and Kuyatt, NIST Technical Note 1297: Guidelines for Evaluating and Expressing the Uncertainty of NIST Measurement Results, NIST, 1994
- Doiron, 20 °C — A Short History of the Standard Reference Temperature for Industrial Dimensional Measurements, Journal of Research of NIST, 2007
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)