Almost every new engineer and founder-turned-designer picks up the same habit: when in doubt, tighten the tolerance. It feels responsible. It is also one of the most expensive reflexes in hardware, because tolerance cost is not linear. It is a series of cliffs, and each cliff is a change in process, tooling, or inspection method that you pay for on every part forever.
The cliffs are predictable, though. Once you know where they are, you can put tight tolerances where they earn their keep and open everything else up — usually a double-digit percentage off the part price with no functional change.
What a tolerance actually is
A tolerance says how much variation you will accept on a dimension. Every process varies; the tolerance tells the manufacturer how much of its output it may ship. Tighten it far enough and you are no longer specifying a dimension, you are specifying a scrap rate — which is why a shop prices tight tolerances higher for three reasons at once: a slower process, extra inspection, and the parts it expects to scrap.
The cost curve, in real numbers
For a typical machined aluminum part, the relative cost of the same feature at different tolerances looks roughly like this:
| Tolerance | Relative cost | What it takes |
|---|---|---|
| ±0.010 in (±0.25 mm) | 1.0x | Standard machining, no special care |
| ±0.005 in (±0.13 mm) | 1.1x | Still routine on a decent machine |
| ±0.002 in (±0.05 mm) | 1.5x–2x | Careful setup, temperature control, in-process gauging |
| ±0.0005 in (±0.013 mm) | 3x–5x | Grinding or honing, dedicated fixturing, 100% inspection |
| ±0.0001 in (±0.003 mm) | 10x and up | Climate-controlled room, lapping, specialist shop |
What matters is not the multipliers, which vary by shop, but that the first two rows cost essentially the same. Loosening from ±0.005 to ±0.010 saves nothing; tightening from ±0.005 to ±0.001 can double the part price. The money is decided by whether you cross into the third row.
Every process has its own natural capability: injection molding holds roughly ±0.003 to ±0.008 in on small features, die casting is looser, sheet metal after bending looser still, and 3D printing behaves differently again, as explored in why your printed part does not fit. Asking a process to beat its capability means adding a secondary operation — a reamed hole, a ground face — and that operation is the cost, not the number on the drawing.
Is the tolerance driven by fit or by function?
Every tight tolerance on a drawing exists for one of two reasons, and telling them apart is the single most useful audit you can run.
Fit-driven tolerances
The dimension is tight because it mates with something: a bearing bore, a shaft, a dowel pin. Here the tolerance is not about the dimension at all — it is about the clearance or interference between two parts. Standard fit classes exist for exactly this, and using them is cheaper and clearer than inventing numbers, as laid out in sizing a shaft and a bore.
They also have cheaper answers than tightening both parts: make one part adjustable, add a shim, or use a slotted hole, which eliminates a whole stack of tight tolerances for the price of a longer slot.
Function-driven tolerances
The dimension is tight because performance degrades outside it: an optical path length, a sealing surface flatness, a gear center distance. These are real and should stay. But there are usually very few — often three or four dimensions on a part with forty.
And the third category
The one nobody admits to: tolerances that are tight because the title block says ±0.005 on everything and nobody edited it. On a typical first-time drawing, more than half the tight tolerances are these.
Stack-up is why parts that pass still don't fit
Individually conforming parts can still fail to assemble, because variations add. Four parts each at ±0.005 in can produce ±0.020 in of accumulated error — enough to close a gap designed at 0.015 in. Worst-case stacking over-designs the assembly; statistical stacking is more realistic but assumes suppliers are centered on nominal. Either way, do the analysis before you tighten anything; the method is in tolerance stack-up analysis.
The fix is rarely "tighten everything." It is to shorten the chain: fewer parts between the two features that matter, or one part carrying both critical surfaces so their relationship is set by a single machining setup.
GD&T is the cheaper alternative to blanket tightening
Plus-minus dimensioning describes a rectangular tolerance zone and says nothing about form or relationship. Geometric dimensioning and tolerancing describes what actually matters — position, flatness, perpendicularity, profile — relative to defined datums. Three concrete ways GD&T saves money:
- A position tolerance gives a round zone. A hole located by plus-minus dimensions gets a square tolerance zone; the same tolerance expressed as true position gets a round one, roughly 57% larger in area. Same functional result, more parts pass.
- Maximum material condition gives bonus tolerance. A hole larger than its minimum size can sit further off position and still assemble; MMC lets the drawing say so.
- Datums tell the shop how to hold the part. Without them, machinist and inspector may reference different surfaces and disagree about a part that is perfectly good.
Done properly, it opens tolerances on the dimensions that do not matter while controlling the relationships that do. The starting point is GD&T basics and how good drawings cut manufacturing costs.
The inspection bill
Here is the cost nobody quotes separately. Every tight tolerance has to be verified, and verification has its own economics.
A dimension a machinist checks with a caliper costs seconds. One requiring a micrometer costs more. One requiring a coordinate measuring machine means the part leaves the machine, waits for the metrology room, and is measured on equipment costing six figures — see CMM inspection and metrology. Then there is sampling: loose dimensions get checked on a sample, tight ones on every part, and going from an AQL sample to 100% inspection can add more to unit cost than the machining time itself.
Gauge R&R: can you even measure it?
A rule of thumb from measurement systems analysis is that your measurement system's total variation should consume no more than 10% of the tolerance band, and 30% is the outer limit of acceptability. With a ±0.0005 in tolerance, your gauge, operator, and environment together must repeat within about 0.0002 in — which hand calipers cannot do at all. Specify a tolerance your supplier cannot reliably measure and you have not created quality, you have created an argument, in which good parts get rejected and bad ones shipped, essentially at random.
Practical rules to apply this week
- Default the title block to the loosest tolerance the part can live with, then tighten individual dimensions deliberately.
- Mark the three to five genuinely critical dimensions and be able to say why.
- Use standard fit classes instead of invented numbers wherever two parts mate.
- Run a stack-up before tightening anything, and prefer shortening the chain to tightening the links.
- Express location and orientation requirements with GD&T rather than plus-minus, and ask your supplier what their process naturally holds before you commit.
- Verify the critical dimensions properly at first article inspection and then relax the sampling.
Surface finish follows the same economics, so audit it at the same time — a fine Ra callout on a face nobody touches is pure cost, as specifying surface finish explains. Alongside the other drivers in what drives the price of a machined part, tolerance and finish are where a redesign usually finds its savings.
Projects House reviews drawings for tolerance and inspection cost as part of production readiness, routinely taking double-digit percentages out of part prices without changing a functional requirement. Send drawings through our contact form.