Three tolerance errors account for roughly 80% of first-article failures in our audit history. All three are invisible to the person who drew the part because they know what they meant. All three are obvious to the machinist who has to hold the tolerance because the drawing does not say what the designer thinks it says.
The 10-minute audit below catches these three before the drawing leaves your desk. It is not a complete drawing review. It is a targeted sweep for the errors that cost the most money when they reach the shop floor.
The three errors
1. Tolerance stack without a datum scheme
A part has six dimensions, all toleranced to ±0.1mm. No datum features are called out. The machinist machines each feature to nominal, holds each tolerance independently, and the part does not fit the mating assembly because the cumulative error across the chain exceeds the assembly clearance.
This is the most common error. It happens when a designer thinks in terms of individual features rather than functional relationships. The drawing communicates six independent requirements. The assembly requires a relationship between feature A and feature F that the drawing does not define.
2. Tighter tolerance than the process can hold
A turned shaft specifies ±0.02mm on a diameter. The shop's standard turning capability is ±0.05mm. The machinist can hit ±0.02mm with a second operation (grinding), but the drawing does not call for grinding and the quote assumed single-op turning. The part comes back out of tolerance or the shop asks for a change order mid-run.
This happens when a designer copies a tolerance from a previous project without checking whether the new part's manufacturing process can hold it. It also happens when a designer applies a default tolerance block (e.g., "unless otherwise specified: ±0.1mm") to a part that includes features the default does not fit.
3. GD&T callout with missing or ambiguous datum reference
A hole is toleranced for position with a feature control frame that references datum A. Datum A is identified on the drawing but the datum feature itself is a surface with no obvious measurement point. The machinist interprets datum A as the center of the surface. The designer intended datum A as the edge of the surface. The hole is out of position by half the datum feature's width.
This is the GD&T version of error 1. The callout is syntactically correct but semantically ambiguous. It passes a drawing checker that looks for missing datum letters but fails when a human has to set up the part on a CMM.
The 10-minute audit
Run this checklist on every drawing before it goes to a supplier. The checklist is ordered by frequency of error, not severity. Do the first check first because it catches the most problems.
| Check | What to look for | Fix if missing |
|---|---|---|
| Datum scheme exists | At least one datum feature is identified. Dimensions that define position or orientation reference a datum. | Add datum features. Convert at least the primary locating surface to a datum. Reference it in positional tolerances. |
| Tolerances match process | Every tolerance is achievable by the process called out in the notes or implied by the material/geometry. | Loosen tolerances to process capability or add a note specifying the tighter process (e.g., "grind to ±0.02mm"). |
| Datum features are unambiguous | Every datum feature has a clear measurement point or reference surface. Planar datums are flat. Cylindrical datums are turned or bored, not cast. | Replace ambiguous datum features with machined features. If a cast surface must be a datum, call out flatness and add a note. |
| Tolerance stack is closed | For every assembly interface, the cumulative tolerance from the datum to the mating feature is less than the assembly clearance. | Add intermediate datums or tighten critical dimensions. If the stack does not close, the part will not assemble. |
| GD&T modifiers are specified | Feature control frames that allow maximum material condition (MMC) or least material condition (LMC) include the modifier symbol. | Add the modifier or confirm that regardless of feature size (RFS) is intended. RFS is the default per ASME Y14.5-2018 but many shops still assume MMC. |
| Surface finish is called out where it matters | Mating surfaces, seal surfaces, and bearing surfaces have a roughness value (Ra in μm). | Add surface finish callouts. If no value is available, use Ra 3.2 μm as a default for functional surfaces and Ra 6.3 μm for non-functional. |
The first three checks catch the three errors above. The last three catch secondary problems that show up less often but still cause delays when they appear.
What the audit does not catch
This is not a substitute for a full drawing review. It does not check for missing views, incorrect material callouts, missing hardware specifications, or any of the other fifty things that can be wrong with a drawing. It checks for the three tolerance errors that cause the most first-article failures in our experience.
It also does not check whether the tolerances are correct for the application. It only checks whether the tolerances are achievable and unambiguous. A part can pass this audit and still be over-toleranced or under-toleranced for its function. That is a design review problem, not a drawing review problem.
The point
The tolerance error is not a machining problem. It is a communication problem. The designer knows what the part is supposed to do. The machinist knows what the machine can hold. The drawing is the interface between those two bodies of knowledge. When the drawing is ambiguous, the machinist guesses. When the machinist guesses wrong, the part fails first article and you lose two weeks.
If you are about to send a drawing to a supplier, stop. Run the six checks above. Fix what fails. Budget 10 minutes per drawing. The time cost is trivial. The failure cost is not.
This is the kind of upstream work Sendspec does for founders before first article. If you have a drawing package that needs review and want a tolerance audit with specific process recommendations, request a quote. We turn around drawing audits in 48 hours.
See also: CNC machining, injection molding, die casting.