Set Tight Tolerances Only Where the Assembly Needs Them

Justify each tight callout

A tolerance is a functional requirement, not a precision flex: it exists to guarantee fit and performance, nothing more¹³.

So the first pass over a drawing is not "how tight can this be" but "does anything fail if this is loose." Cost is driven by the process changes a tolerance forces, not by the number itself.

A limit the machine cannot hold in its normal pass triggers slower speeds, extra offsets and extra setups, and that is where the money goes³. A mating bore drawn at ±0.005" is justified because a loose fit fails assembly⁴.

A nonfunctional face drawn at the same ±0.005" adds cost with no performance gain, because nothing in the assembly reads that surface³. The two callouts look identical on the drawing and behave completely differently in the quote.

Before specifying anything tighter than ±0.005", ask whether the assembly actually requires it or whether it is a default carried over from a previous drawing¹³. That question alone removes the most common avoidable cost driver.

Tight tolerances are generally needed where a part feeds a secondary assembly process, and loose tolerances there can lead to a failure in acceptable assembly⁴. Everywhere else, general tolerances can be used³.

Go feature by feature and mark only the ones whose function depends on the band. If you cannot name the assembly that reads a dimension, that dimension does not need a tight limit.

Where the standard band ends

Below the standard band the part can no longer be held in one normal pass, so the route gains semi-finishing, finishing, secondary grinding and repeat setups — each added operation is a separate cost and a separate queue. The table shows what each band adds to the process.

Will it survive the run?

A tight limit that passes on the first article can still fail on part 400. Holding a tight band consumes tool life, so on a long run the machine stops for tool changes and offsets far more often — the per-part time rises even though the cycle itself looks unchanged.

A new tool might initially meet a ±0.001" standard with ease, but maintaining that level of precision becomes challenging over repeated use⁶. Producing numerous parts to those standards may require frequent tool changes or adjustments in the machining process, leading to longer production times and elevated costs⁶.

This is why the quantity on the RFQ changes the answer: a tolerance that is merely expensive on ten prototypes becomes a scheduling problem on a mass-production batch, where tool wear is particularly critical⁶. that tighter tolerances can increase machining time by 5–20× per feature and drive up QA costs as well²⁰.

That figure is per feature, not per part, which is the part buyers miss: ten tight features multiply the penalty ten times. The practical test is to ask what the tool does over the whole order, not over the first piece.

If a callout only survives because the operator babysits it, the run will show it. Put the tight band on the features that need it and let the rest run at the default, so the tool changes land where they buy something.

Pick the route, not the rate

Every additional setup re-clamps the part and stacks a new positioning error onto the last, so a route that reaches the tolerance in one setup removes both the error and the handling time.

Each setup change in a 3-axis process adds a small positioning mistake, and those errors stack up across many operations until the final part drifts outside the tolerance range²⁴. A 5-axis process holds tighter tolerances because the reference chain is never broken²⁴.

The counter-intuitive part is the price. A 5-axis machine carries a higher hourly rate, yet total project cost 20–40% lower, with savings on labor, fixtures and wasted material²⁵.

The same source reports an aerospace wing rib example where cycle time fell from 48 to 33 minutes — a 30% reduction — from fewer setups and less handling²⁵. So a higher rate is not automatically the more expensive quote; a multi-setup route that needs rework to hold true position usually is.

There is one exception worth knowing: a tighter tolerance is occasionally free if the feature is small and the machine can hold it in the same pass as a looser tolerance elsewhere, but that is the exception, not the rule¹². Do not build a drawing on the exception.

If your part has features on five or six sides, compare the single-setup route before you accept the cheaper hourly rate.

Budget the inspection it pulls in

Inspection is the cost that appears after the quote, because the gauge that was adequate at the default stops being adequate as the band narrows. Any tolerance below 0.01 mm often implies additional inspection — CMM or manual gauge²⁰.

Holes at ±0.01 mm typically require boring and reaming, which is a machining change as well as a measuring one²⁰. Tight tolerances also push the shop toward slower machining speeds, additional setups, more precise workholding, extra tool offsets and longer inspection cycles such as CMM or first-article inspection³.

Note where the effort scales: it grows with the number of tight features, not the number of parts, so a drawing with every dimension marked critical carries that burden on every unit³. A tolerance below ±0.0005" adds more frequent in-process inspection on top of the final check¹³.

That is the difference between a quote that names final inspection only and one that includes in-process checks — and it is often not clearly defined at quotation³. Ask which of the four scopes applies: in-process, final only, FAI, or sampling³.

If your drawing has one ±0.0005" bore, the answer changes the price you actually pay.

Confirm before the RFQ

Inspection scope is the line item most often left undefined at quotation, so an unagreed scope surfaces later as an unexpected charge or a hold at goods-in.

• ✓Name the assembly or function that reads each tight dimension; drop the callout if there is none.
• ✓Check whether the quote covers in-process inspection, final inspection only, FAI, or sampling.
• ✓Confirm whether CMM reports or FAIR documentation are required, and in what format.
• ✓Freeze the drawing revision before placing the order and agree a formal change process.
• ✓Flag any feature tighter than ±0.0005" and ask what operation holds it.
• ✓Ask for a DfM review before the order, since early review often prevents unnecessary tolerance tightening.

Set the default block first

A title-block default that matches what the process holds at normal speed keeps the drawing honest, and every callout tighter than that default becomes a deliberate, costed decision. A ±0.005" tolerance is achievable on most standard 3-axis work at normal speed, and it is also the standard tolerance for metal parts^10,13.

Plastic parts sit at ±0.01"¹⁰. Those two numbers belong in the default block, not repeated on every dimension.

Then the exceptions stand out: push a feature to ±0.0005" and you are often looking at secondary grinding, more frequent in-process inspection and multiple setups just to hold the number¹³. Material changes the default too.

Getting tighter tolerances requires more work on the material, and that extra work is very difficult for materials that are already hard to machine¹⁰. So a hardened steel part and an aluminium part should not share one blanket tolerance.

One caution on the numbers: the ±0.005" metal default and the 0.01 mm inspection threshold are different units describing different things, and the sources do not reconcile them into a single table — treat each as the band its own source states.

Write the default block, list the exceptions, and make each exception earn its place.

What the sources do not establish

• No cost multiplier curve at specific tolerance tightening thresholds
• No Cpk values or scrap-rate correlation for CNC operations
• No consolidated standard-tolerance table by process (milling vs turning)
• No lead-time penalty in days or weeks per tolerance band
• No inspection time shift quantified by tolerance band
• No formal general-tolerance standard with its grade table