Most GD&T disputes on the shop floor are not about the tolerance value — they are about the datum scheme underneath it. A position tolerance is only as meaningful as the datum reference frame it hangs on, and a badly chosen frame quietly converts good parts into rejects. This page collects the seven datum mistakes we see repeatedly in drawings sent for machining, with the consequence of each and the standard-cited fix.
A drawing comes in with a hole pattern controlled by position ∅0.1 mm to datum frame A|B|C. Datum A is the large cast bottom face — unmachined, wavy, and the part rocks on it. The shop does what any reasonable shop does: it machines the top face flat, flips the part, and inspects the holes from the machined face because the cast face is unusable as a reference. Every part “passes” against this substitute frame. The customer’s CMM sets up on datum A exactly as drawn, the holes report out of position by the cast face’s flatness error, and the entire batch is rejected. Nobody machined anything wrong; the datum scheme made agreement impossible.
This pattern — a datum scheme that looks fine in CAD but cannot be physically realized or does not match function — is behind a large share of GD&T rejects. The seven mistakes below cover the recurring failure modes discussed across Practical Machinist, Eng-Tips, and r/Machinists, cross-checked against ASME Y14.5-2018 and ISO 1101:2017.
A datum is a theoretically exact point, axis, line, or plane derived from a physical datum feature, and the datum reference frame (DRF) built from up to three datums is the coordinate system in which every controlled feature is measured. The order in the feature control frame is not cosmetic: it is the order of precedence in which the part contacts its simulators. A primary planar datum constrains 3 degrees of freedom (one translation, two rotations), a secondary typically 2 more, a tertiary the last one.
Consequence: the same feature, the same part, and the same CMM will report different position values under different datum schemes. A 0.05 mm perpendicularity error between the face you used as A and the face the customer used as A becomes a 0.05 mm position error at 100 mm from the datum — invisible in the tolerance value, fully visible in the report. Per ASME Y14.5-2018 §7 (Datum Referencing) and ISO 5459, the datum reference frame defines the measurement; everything downstream inherits its errors.
The most common error: datum A is assigned to an as-cast, as-forged, or rough saw-cut surface because it is “the bottom of the part”. A primary datum feature sits on a theoretically exact simulator — a surface plate, a CMM-constructed plane contacting the high points. A wavy cast face rocks on that simulator, and ASME Y14.5-2018’s datum stabilization rules (a notable 2018 clarification over 2009) allow more than one legitimate resting position for a rocking feature — meaning two inspectors can legally establish different datum A’s from the same part.
| Primary datum choice | What happens on the simulator | Result |
|---|---|---|
| As-cast / as-forged face | Rocks; multiple stable positions; high-point contact varies part to part | Non-repeatable DRF; batch-to-batch scatter in every position value |
| Small or narrow face | 3-point contact on a tiny area; leverage amplifies flatness error | Angular error magnified across the part envelope |
| Machined, flatness-controlled face | Stable, repeatable seating | Repeatable DRF; measurements agree between setups and suppliers |
Engineers often write A|B|C in the order the part is fixtured for machining, or in the order the features were modeled in CAD — not in the order the part seats in assembly. The order of precedence is functional: the primary datum should be the feature the part locates on in use (the mounting face, the mating flange), the secondary the feature that clocks or edges it, the tertiary the feature that stops rotation. Swapping primary and secondary is not a notation detail; it changes which surface’s form error enters the measurement and which is averaged out.
A position ∅0.1 mm to A|B|C where functionally the part bolts down on D and edges against E will pass inspection against a frame the assembly never sees — the classic “good parts that don’t fit” scenario. Forum consensus across r/Machinists and Eng-Tips is blunt: datum selection is based on functionality at assembly, and a datum scheme chosen for machinist convenience is the designer outsourcing a design decision to the shop.
ASME Y14.5-2018 removed concentricity and symmetry from the standard. Both required median-point analysis — finding midpoints of diametrically opposed surface elements — which is data-heavy, rarely done correctly on a production CMM, and was in practice almost always (incorrectly) inspected as runout or position anyway. The 2018 replacement guidance: use position (for the axis location of a feature of size, with a proper datum frame) or runout (for surfaces of revolution relative to a datum axis).
The datum mistake that follows: drawings still circulate with concentricity called to a datum axis, and shops either guess at an inspection method or silently substitute runout — two different controls with different acceptance criteria. There is a second trap here: ISO 1101:2017 retains concentricity and symmetry, so a multinational program can have the same symbol meaning “removed, substitute position/runout” under ASME and “median-point control” under ISO on sister drawings.
A hyphenated datum — A-B — establishes one datum (typically a common axis) from two features treated as a single common datum feature. ASME Y14.5-2018 §7.12 covers patterns of features used this way (the 2009 edition called it a “multiple datum feature” at §4.12; the 2018 edition renumbered datum content into §7 and renamed the concept “common datum feature”). The classic use: two bearing journals establishing one shaft axis, or two bores one housing axis.
The error is assuming A-B behaves like A then B. It does not: the common datum feature simulator (e.g. one long mandrel or one best-fit axis through both bores) is established from both features simultaneously. Form error and spacing error in the two features both feed the axis — a short span between two imperfect bores gives a poorly defined axis, and every position value referenced to A-B inherits that instability. It is also not interchangeable with A|B|C-style precedence: A-B|C means “the common axis of both features, then C”, while A|B|C means “seat on A, then B, then C” — different frames, different results.
When a datum feature of size is referenced at maximum material boundary (MMB) or least material boundary (LMB) — the (M) or (L) modifier after the datum letter in the feature control frame — the datum simulator is sized at that boundary, and the actual datum feature can shift within the gap between itself and the simulator. This is datum shift (2009 §4.11; 2018 §7.11 material boundaries): extra freedom of the whole controlled pattern relative to the datum axis or center plane. It is emphatically not bonus tolerance — bonus adds to the feature’s own tolerance zone; shift lets the entire pattern translate or rotate together, and the amount varies part to part with the datum feature’s actual size, form, and orientation error.
| Modifier location | Effect | Common misreading |
|---|---|---|
| (M) after the tolerance value | Bonus tolerance: zone grows as the controlled feature departs from MMC | — (well understood) |
| (M) after the datum letter | Datum shift: the datum simulator (e.g. a fixed-size gauge pin at the MMB) lets the whole pattern displace as the datum bore gets larger | Misread as “more bonus” — actually a loosening of the reference frame itself |
| No modifier (RMB default) | Simulator adjusts to the actual feature; no shift available | Assumed tighter — it is, and sometimes that is wrong for the function |
The mistake cuts both ways: designers add (M) to datums “for extra tolerance” on press-fit or sealing bores where the resulting shift destroys the function; or they omit it on clearance-bolt patterns where shift would legitimately rescue parts. The Zeiss CMM forum’s recurring datum-shift threads show the inspection side: the realized shift depends on the form and location error of every datum feature in the frame, so two CMM programs that model shift differently report different numbers for the same part.
ASME Y14.5-2018 and ISO 1101:2017 use nearly identical symbols but differ in the default rules underneath datums — and cross-border machining (a US drawing machined in Asia or Europe, or vice versa) is where those defaults silently bite:
| Topic | ASME Y14.5-2018 default | ISO 1101:2017 / GPS default |
|---|---|---|
| Feature control frames sharing one DRF | Simultaneous requirement applies by default — patterns to the same frame are evaluated together | Independency principle (ISO 8015) — each specification is met independently unless stated |
| Size vs form (envelope) | Rule 1: size controls form by default | No envelope by default; requires the (E) symbol |
| Concentricity / symmetry | Removed in 2018; use position / runout | Retained in ISO 1101:2017 |
| Datum rules location | Inside Y14.5 (§7) | Separate standard: ISO 5459 (datums), with the “situation feature” concept |
The simultaneous-requirement difference is the sneakiest: under ASME, two hole patterns positioned to the same A|B|C frame must hold their relative location as a group; under ISO defaults each pattern is judged alone, so a batch can pass ISO-style inspection and fail ASME-style inspection with identical hardware. Krulikowski’s oft-cited estimate (in Mitutoyo’s CMM/GD&T training material) is that roughly 65% of possible tolerances are specified or interpreted differently between the two systems.
On a large casting, a thin-wall housing, or any part that flexes under its own weight or clamping force, an entire surface used as a datum is an illusion: the part seats differently on every fixture, and clamping strain moves the “datum” after inspection. Classic practice (long predating the current standards and echoed in Eng-Tips casting-datum threads) is to control datum feature flatness when the part is clamped in assembly, add a restraint note (“inspect with datum feature A mounted against a flat surface, bolts torqued to X”), or — better — define datum targets: specific points, lines, or areas with basic locations that every supplier, CMM, and fixture reproduces exactly.
Datum targets are also the only clean answer when the machining datum must come from an unmachined casting: casting design manuals recommend casting in datum target features, and ASME Y14.8-2009 §4.4 requires the casting datum targets to be re-shown on the machining drawing — a “shall”, not a “should”. The Eng-Tips consensus adds the practical reason: the casting supplier and the machine shop must seat the part on identical points, or the two inspect against two different reference frames and both make “good” parts that disagree. Targets called out without basic dimensions (or a controlled CAD model) are a known failure mode — “points close to as-shown on print” means the customer can never exactly duplicate the supplier’s inspection.
When parts are rejected and the root cause smells like the datum scheme, the order of investigation matters:
| # | Check | Catches |
|---|---|---|
| 1 | Is the primary datum a machined, flatness-controlled, stable surface — or a cast/rough face that needs datum targets instead? | Mistake 1 |
| 2 | Does the datum precedence order match how the part seats in assembly (first contact = primary)? | Mistake 2 |
| 3 | Is every datum feature physically large and stiff enough to seat the part repeatably? | Mistakes 1, 2 |
| 4 | Any concentricity or symmetry symbols on an ASME Y14.5-2018 drawing? Replace with position or runout. | Mistake 3 |
| 5 | Is each hyphenated datum (A-B) a genuinely shared functional axis with adequate span — not two features with different roles? | Mistake 4 |
| 6 | Every (M)/(L) after a datum letter: does the assembly tolerate pattern-level shift at that datum? | Mistake 5 |
| 7 | Title block names one governing standard with year (ASME Y14.5-2018 or ISO 1101:2017); no mixed conventions? | Mistake 6 |
| 8 | Large, thin-wall, cast, or forged part: datum targets defined with basic dimensions (3-2-1), restraint condition noted if clamped in assembly? | Mistake 7 |
| 9 | Casting + machining drawings: are the casting datum targets re-shown on the machining drawing (ASME Y14.8-2009 §4.4)? | Mistake 7 |
| 10 | Has the shop seen the drawing before release (20-minute DFM review) and confirmed the frame is fixtureable and inspectable as drawn? | All |
Choose the surface the part seats on in assembly — the functional mounting face — provided it is machined, flatness-controlled, and large enough to seat the part stably. The primary datum constrains 3 degrees of freedom and every measurement inherits its errors, so an unstable cast face or a tiny pad as primary guarantees non-repeatable inspection. If the functional seat is a cast or irregular surface, define datum targets (points/areas per ISO 5459 / ASME Y14.5) instead of the whole surface. Never pick the primary datum for machining convenience alone.
A|B|C is precedence order: seat on A first, then B, then C — three separate datums applied in sequence. A-B|C makes A and B a compound (common) datum feature: one datum, typically a shared axis, established from both features simultaneously by a single simulator (e.g. one mandrel through both bores), with C as the next datum in precedence. They produce different reference frames and different inspection results. Use A-B only when the two features genuinely share one functional axis, such as paired bearing journals; use A|B when the features have separate functional roles (ASME Y14.5-2018 §7.12).
It allows datum shift, not bonus tolerance. Referencing a datum feature of size at MMB (the (M) after the datum letter) fixes the datum simulator at the maximum material boundary — for an internal feature, a theoretical pin at its smallest allowed size — so as the actual datum feature departs from that boundary, the whole controlled pattern can translate or rotate relative to the datum axis. Bonus tolerance ((M) after the tolerance value) grows the feature’s own zone; datum shift loosens the reference frame itself, and the realized amount depends on the datum feature’s actual size, form, and orientation error (ASME Y14.5-2018 §7.11). Use it for clearance-bolt patterns; avoid it on sealing, press-fit, or alignment-critical datums.
No — concentricity and symmetry were removed from ASME Y14.5-2018 because their median-point definitions were rarely inspectable correctly in production. The standard’s replacement controls are position (axis location of a feature of size to a datum frame) and runout (surfaces of revolution to a datum axis). Note the cross-border trap: ISO 1101:2017 still retains both symbols, so a symbol that is dead under ASME is alive under ISO — always state the governing standard and year in the title block.
There is no default datum scheme — ask before cutting metal. Without datum feature symbols, only form tolerances and ± dimensions are fully defined; any position or orientation control is ambiguous. In practice shops fall back on the general tolerance block (e.g. ISO 2768) and the most stable machined face, but that is an assumption, not a contract. For anything with a functional hole pattern or mating features, send the drawing back for datum callouts; a 20-minute DFM review is far cheaper than a batch measured against the wrong frame.
Datum targets are specific points, lines, or areas — located by basic dimensions — that define exactly where simulators contact the datum feature, so every supplier and CMM seats the part identically (ISO 5459; ASME Y14.5). You need them when the whole surface cannot serve as a repeatable datum: castings and forgings, large parts (~500 mm+) that sag, thin-wall parts that distort under clamping, and any datum that must be reproduced across a casting drawing and a machining drawing — where ASME Y14.8-2009 §4.4 requires the targets be re-shown on the machining drawing. The classic layout is 3-2-1: three primary targets, two secondary, one tertiary.
The simultaneous requirement. Under ASME Y14.5-2018, feature control frames referencing the same datum reference frame are by default evaluated as a group — patterns must hold their relative location together. Under ISO GPS the default is the independency principle (ISO 8015): each specification is met independently unless stated. Identical hardware can therefore pass an ISO-default inspection and fail an ASME-default one. Other datum-relevant divergences: ASME Rule 1 envelope vs ISO’s explicit (E) symbol, concentricity/symmetry removed in ASME but retained in ISO 1101:2017, and datum rules living in Y14.5 §7 vs the separate ISO 5459. Name one standard and year in the title block; never mix conventions.
Send your drawing for a free DFM review — we check datum precedence, compound datums, datum shift exposure, datum targets, and ASME/ISO standard conflicts before any metal is cut.
Request a Quote