The GD&T mistakes that get parts rejected are rarely exotic. They are datums chosen because they were easy to dimension from, hole locations toleranced with plus-minus, positions with no basic dimensions, the wrong material condition modifier, and tolerances tighter than the shop can hold. Each one either lets two people measure the same part and get different answers, or asks for something the process can't deliver. Below are seven of them, what each looks like on the drawing, why it causes trouble, and the fix under ASME Y14.5-2018, the current edition, which ASME reaffirmed in 2024.
If you manage a design or quality team, use this as a checklist on your next drawing release. Pull three recent prints and look for each item.
1. Datums picked for convenience instead of function
What it looks like: datum A is the face the drafter happened to start dimensioning from, or the edge that was easiest to pick in CAD. Datum B is a chamfered corner or a short edge. None of them are the surfaces the part actually sits on or locates from in the assembly.
Why it causes rejects: the datum reference frame tells inspection how to hold the part. If it doesn't match how the part is held in the assembly, you can get parts that pass inspection and don't fit, and parts that fail inspection and would have worked fine. The second case is the expensive one, because it turns into scrap, a deviation request, or an argument with the supplier.
The fix: choose datum features by function. Ask how the part mounts. The primary datum feature is usually the largest mating surface that establishes orientation, such as the face that bolts down. The secondary is often a bore or pin hole that locates it. The tertiary stops rotation. Then check the order in each feature control frame. A|B|C and B|A|C are different set-ups and can give different results on the same part.
2. Datum features that inspection can't simulate
What it looks like: a datum feature symbol attached to a centerline, a datum on a narrow ledge or a surface hidden behind another feature, or datum features that have no form or orientation control of their own.
Why it causes rejects: inspection has to physically contact the datum features, with a surface plate, a fixture, a pin, or a CMM alignment that mimics one. A centerline can't be touched. A tiny or inaccessible surface gives an unstable set-up, so two inspectors rock the part differently and report different numbers. If datum feature B is not controlled to datum A, nothing guarantees the set-up is repeatable.
The fix:
A quick test for any drawing: hand it to someone in inspection and ask how they would fixture the part. If the answer takes more than a minute, the datums need work.
3. Plus-minus tolerances on hole locations
What it looks like: a bolt pattern with holes located by dimensions like 2.000 plus or minus 0.005 in X and 1.500 plus or minus 0.005 in Y, measured from part edges.
Why it causes rejects: plus-minus location has two problems. First, it creates a square tolerance zone. A hole off by 0.005 in both X and Y passes, even though its center is 0.0071 from true position. A hole off by 0.006 in X alone fails, even though it is closer and would assemble just as well. Second, it doesn't say which edges to measure from or in what order, so the part can be set up several ways, and each way reports a different location.
The first problem is simple geometry. A 0.010 by 0.010 square zone has a diagonal of 0.0141. A round zone of diameter 0.0141 passes through the corners of that square, so it accepts every hole the square accepts. Its area is 3.1416 / 4 x 0.01414 x 0.01414 = 0.000157 square inches, against 0.000100 for the square, about 1.57 times as much. Holes in that extra area are good parts that plus-minus throws away.
The fix: locate the holes with basic dimensions from a datum reference frame, and control them with a position tolerance using a diameter symbol, for example a diameter 0.014 position tolerance relative to A, B, and C. The zone now matches how a round bolt fits a round hole, and the datums tell everyone how to set the part up.
4. Missing or conflicting basic dimensions
What it looks like: a position or profile tolerance on a feature whose location dimensions are toleranced, or plain dimensions that fall under the title block tolerance. Sometimes the drawing has both a plus-minus location and a position callout on the same hole.
Why it causes rejects: a basic dimension is the theoretically exact value, shown in a box, and the feature control frame supplies the tolerance. If the location dimension carries its own tolerance, or the title block tolerance applies to it, the feature now has two location requirements. The supplier and your inspector can each pick one, and both can claim they followed the drawing.
The fix: every dimension that locates or orients a feature controlled by position, profile, or angularity should be basic. Scan each feature control frame and trace its dimensions back to the datums. Every step in that chain should be a boxed dimension, and none should also carry a tolerance. The title block tolerance does not apply to basic dimensions.
5. The wrong material condition modifier
What it looks like: position tolerances on clearance holes with no modifier, an MMC modifier on a feature that isn't a feature of size, or MMC on a feature where minimum wall thickness is what matters.
Why it causes rejects: in Y14.5-2018, a tolerance with no modifier applies regardless of feature size (RFS), and a datum reference with no modifier applies regardless of material boundary (RMB). That is the strictest reading. For a clearance hole that only has to pass a bolt, RFS rejects parts that would assemble.
With MMC, the tolerance grows as the hole departs from its smallest size. For example, a hole toleranced 0.265 to 0.275 with a diameter 0.010 position at MMC gets 0.010 at 0.265, and 0.020 at 0.275. That extra 0.010 is bonus tolerance, and it costs nothing in function. A hole at 0.275 with 0.020 of position error still has a boundary of 0.255, the same as a hole at 0.265 with 0.010 of error. The part assembles either way, and a functional gage can check it.
The fix:
6. Tolerances tighter than the process can hold
What it looks like: a default title block tolerance of three decimal places on every feature, or a position or flatness value copied from an older part without checking what the feature does.
Why it causes rejects: if the drawing asks for more than the process delivers, some fraction of parts will fail no matter how careful the shop is. You then pay for sorting, scrap, extra operations, or a supplier who quotes high to cover the risk. Worse, people get used to signing deviations, and the tolerances that really matter lose their weight.
The fix:
7. No standard stated, or ASME and ISO mixed
What it looks like: a drawing with no note saying which standard applies, a drawing that mixes ISO-style callouts with ASME conventions, or new drawings still using the concentricity or symmetry symbols.
Why it causes rejects: the two systems read the same symbols differently. By default, ASME Y14.5 applies Rule #1, where the size limits also control form, while ISO GPS applies the independency principle, where each tolerance is met on its own unless the drawing states a relationship. A shaft that passes on an ISO drawing can fail the same callout read under ASME. A supplier in another country may default to the other system.
Concentricity and symmetry were removed from Y14.5 in the 2018 edition. A new drawing that references Y14.5-2018 and uses them is calling for a control the standard no longer defines, and inspection has to guess what you meant.
The fix: state the standard and edition on every drawing, for example "DIMENSIONING AND TOLERANCING PER ASME Y14.5-2018." Replace concentricity with position or runout, and symmetry with position or profile, depending on what the feature needs. If you buy from suppliers who work to ISO, agree up front which standard governs.
A one-page checklist for your next drawing review
| Check | What to look for |
|---|---|
| Datums | Match how the part mounts, in the right order |
| Datum features | Real surfaces or features of size, accessible, qualified |
| Hole locations | Basic dimensions plus position, not plus-minus |
| Basic dimensions | Every locating dimension boxed, no double tolerances |
| Modifiers | MMC to assemble, LMC to protect wall, RFS to center |
| Tolerance values | Set by function and stack-up, checked with the supplier |
| Standard | ASME Y14.5-2018 stated, no concentricity or symmetry |
Run it on a few of your own prints. If you find these issues more than once, the problem is usually shared habits across the team, not one person's drawing, and that is cheaper to fix in a room than one rejected lot at a time.
Fixing it across a team
Our on-site GD&T training is taught on your own drawings, which is where these mistakes live. For teams that already use GD&T, the half-day refresher and drawing review is $2,500 for up to 12 participants, and it works through your own prints against this kind of checklist. Teams that need the full foundation can book the 2-day course, $8,000 for up to 8 participants and $300 for each additional person, up to 16. See all programs on the training page.
If you're an individual engineer working on your own GD&T, one-on-one GD&T tutoring covers the same material at your pace.
To price a session for your team, request a proposal.
