The most expensive tolerance mistake is the one you catch after the first article ships. A 0.05mm callout on a feature that only needs 0.2mm costs you three weeks and a re-tooling charge. A missing GD&T frame on a mating surface costs you an assembly that does not fit. A tolerance tighter than the process capability costs you a 100% inspection upcharge you did not budget.
Most of these failures trace to three root causes: over-tolerancing features that do not matter, under-tolerancing features that do, and specifying tolerances the chosen process cannot hold. All three are visible in the drawing before it leaves your desk. The audit takes 10 minutes. The cost of skipping it is measured in weeks and four-figure invoices.
The three checks
Run these in order. Each one catches a different failure mode.
1. Flag every tolerance tighter than ±0.1mm
Start at the top of the drawing. Scan every dimension. Circle every tolerance tighter than ±0.1mm. Now ask: does this feature mate with another part, locate a fastener, or define a sealing surface? If the answer is no, the tolerance is wrong.
CNC machining holds ±0.05mm without secondary operations. Holding ±0.02mm requires grinding or wire EDM. Holding ±0.01mm requires lapping. Each step down costs time and money. A 0.02mm bore that only needs to clear a shaft with 0.2mm radial play is a process you are paying for but not using.
In our experience across 180+ programs audited in 2024 and 2025, 60% of tolerance-related first-article failures traced to dimensions called tighter than function required. The part met the drawing. The drawing did not match the need.
2. Check mating features for GD&T callouts
Mating features are holes that accept fasteners, pins that locate into holes, and surfaces that press against other surfaces. Every mating feature needs a geometric tolerance. A linear dimension alone does not control orientation, perpendicularity, or concentricity.
ISO 1101 defines the full GD&T framework. The five most common callouts for contract manufacturing are:
| Symbol | Control | When to use |
|---|---|---|
| ⊥ (perpendicularity) | Orientation of a surface or axis relative to a datum | Fastener holes, mounting faces |
| ⌭ (position) | Location of a feature relative to datums | Hole patterns, pin arrays |
| ○ (concentricity) | Alignment of two cylindrical features on a shared axis | Bearing bores, shaft steps |
| ⏥ (flatness) | Variation across a single surface | Sealing surfaces, datum faces |
| ⌒ (profile) | Form of a complex surface | Contoured parts, optical housings |
A hole called as Ø6.0mm ±0.05mm without a position tolerance can land anywhere within ±0.05mm of nominal and still meet the drawing. If that hole accepts a dowel pin that locates the part in an assembly, the assembly will not repeat. The position callout (e.g., ⌭ Ø0.1mm A B C) locks the hole's location relative to the datum structure. The shop knows what matters.
3. Cross-check tolerance against process capability
Every manufacturing process has a natural tolerance band it holds without secondary operations. Calling a tolerance tighter than the process can deliver forces the shop into inspection overhead, secondary machining, or a reject rate you pay for.
Standard process capabilities for the five most common contract manufacturing processes:
| Process | Typical tolerance | Achievable with secondary ops | Notes |
|---|---|---|---|
| CNC milling (3-axis) | ±0.1mm | ±0.05mm (grinding) | Flatness on large surfaces: 0.05mm per 100mm |
| CNC turning | ±0.05mm | ±0.02mm (grinding) | Concentricity: 0.02mm TIR standard |
| Die casting (aluminum) | ±0.3mm | ±0.1mm (machining) | Draft angles required, 1-3° typical |
| Injection molding (thermoplastic) | ±0.2mm | ±0.05mm (machining) | Shrinkage varies by resin, 0.3-0.8% |
| Sheet metal (bending) | ±0.5mm | ±0.2mm (secondary forming) | Bend radius minimum 1× material thickness |
A drawing that calls ±0.02mm on a turned diameter is asking for grinding. A drawing that calls ±0.1mm on a die-cast feature is asking for post-cast machining. Both are fine if you need them. Both cost money and time if you do not. The audit is the moment to decide.
If the tolerance is tighter than the standard process capability, write a note on the drawing: "Critical dimension, secondary ops acceptable" or revise the tolerance to match what the process delivers. Do not leave it ambiguous. The shop will quote the tighter process, and you will pay for it.
What happens when you skip the audit
Three programs from the last 18 months:
Program A: Aluminum housing, CNC milled, 12 features called at ±0.02mm. Only two of those features mated with other parts. The other ten were cosmetic radii and chamfers. First article passed inspection but cost 40% more than the revised drawing would have cost. The operator caught it at quote review. The founder approved it anyway because the timeline was tight. The production run carried the same cost structure. Total overspend: 4,800 euros across 200 units.
Program B: Injection-molded enclosure, ABS, six bosses for self-tapping screws. The drawing called hole positions as linear dimensions ±0.1mm with no GD&T. The mold hit nominal on the CMM but the bosses were not perpendicular to the parting line. Screws cross-threaded on assembly. Mold revision: 2,400 euros, three-week delay. A perpendicularity callout of 0.2mm would have caught it at mold approval.
Program C: Turned brass fitting, Ø12mm shaft, called at ±0.01mm. The shaft located into a Ø12.2mm bore with 0.1mm radial clearance. The ±0.01mm tolerance forced grinding. Lead time went from two weeks to four. The grinding added 6 euros per part. Revised tolerance to ±0.05mm after the first article. The fit still worked. The grinding cost did not come back.
The point
The tolerance audit is not a quality problem. It is a decision-making problem. Tolerances encode what matters and what does not. A drawing without that clarity forces the shop to guess, and the shop will guess conservatively. Conservative guesses cost time and money.
If you are about to send a drawing to a shop, stop. Print it. Run the three checks. Circle every tolerance tighter than ±0.1mm and ask if it is load-bearing. Check every mating feature for a GD&T callout. Cross-check every tight tolerance against the process capability table. Revise what does not hold up. The 10 minutes you spend now buys back the three weeks you would lose later.
This is the kind of upstream work Sendspec does for founders before first article. If you have a drawing that needs a tolerance audit and want a quote-ready revision, request a quote. We turn around marked-up drawings with process recommendations in 48 hours.
See also: Prototype to production: the six-week gap, The fastest quote you can't trust.