Guide
What are the differences between ASME Y14.5 and ISO GPS on a drawing?
ASME Y14.5 is the American standard for dimensioning and tolerancing: one document that defines the symbols, rules and defaults for geometric dimensioning and tolerancing (GD&T) on drawings and models. ISO GPS (geometrical product specifications) is a family of ISO standards that covers the same ground in many separate parts, anchored by ISO 8015 for its fundamental principles and ISO 1101 for its symbol language.
By Saola Manufacturing engineering team · Published · Updated
The two systems share most of their symbols, which is exactly why they cause trouble. A feature control frame drawn to one standard looks almost identical when read under the other, yet the part it allows can be different. This guide sets out the differences that change what a supplier makes and inspects, shows how to tell which system a drawing uses, and ends with a short checklist for engineers and sourcing managers who send drawings to shops abroad. It describes the standards themselves; it is not a substitute for the documents, which are sold by ASME and ISO.
On this page
What is the biggest difference between ASME Y14.5 and ISO GPS?
The default relationship between size and form: under ASME Y14.5, Rule #1 (the envelope principle) makes a feature of size perfectly formed when it is at maximum material condition, while ISO 8015 applies the principle of independency, so a size tolerance controls size alone and form must be toleranced separately.
Take a turned pin with a plain diameter tolerance and no geometric callout. Under ASME Y14.5, that pin may not be bent or lobed beyond a boundary of perfect form at its largest permitted diameter. If every cross-section measures at the upper limit, the pin must be straight. The size tolerance quietly limits straightness, roundness and flatness as well.
Under ISO 8015:2011, the same callout controls the size of the pin and nothing else. A banana-shaped pin whose local sizes all sit inside the limits conforms, unless the drawing adds a straightness tolerance, a general geometrical tolerance, or the envelope requirement. For a pin that must slide into a bore, that difference decides whether the part assembles.
Each system can switch to the other’s behavior. An ISO drawing applies the envelope to one feature with the circled E modifier after the size tolerance, and a note can apply it more widely. An ASME drawing relaxes Rule #1 for a feature with the independency symbol, a circled I, or with a note that perfect form at maximum material condition is not required. So the question to ask of any drawing is not only which standard it cites but which default governs each fit-critical feature.
Material condition modifiers show the same split in another form. Under ISO 2692:2021, the maximum and least material requirements tie size and geometry together for features where assembly or minimum wall thickness depends on both. In our reading, applying one of them to a feature therefore sets independency aside for that feature. In ASME practice, the same circled M reads as a bonus tolerance on top of a Rule #1 envelope that was already there.
How does each standard define the size of a feature?
ISO 14405-1 makes the two-point local size the default and offers a menu of size modifiers, such as least-squares or maximum inscribed size, while ASME Y14.5 checks a feature of size against its limits with local measurements plus, by default, the Rule #1 envelope.
The current edition, ISO 14405-1:2025, sets out the default specification operator for linear size on cylinders, spheres and two parallel opposite planes, and defines a special operator as well. Its 2016 predecessor went further and listed the family of size types a drawing may call for with a modifier: local sizes such as two-point and spherical, global sizes such as least-squares, maximum inscribed and minimum circumscribed, and rank-order sizes such as the average or range of sizes. A diameter followed by a small code in the tolerance tells the inspector which of those to measure.
ASME drawings rarely carry such codes. The inspector checks the actual local size at each cross-section against the limits and, because of Rule #1, also checks the feature against a perfect-form boundary, often with a go gauge or a functional check. The practical upshot for a buyer: an ISO size modifier left on a drawing sent to a shop used to ASME conventions may simply be ignored, and an ASME drawing sent to an ISO shop may be measured with two-point readings alone, missing a form error Rule #1 was meant to catch.
The size of fits is shared ground. Both systems accept tolerance classes from the ISO fit system, such as H7 or g6, and ISO 286-2:2010 gives the limit deviations for those classes. What differs is how the resulting size is interpreted, which is the point above.
How do the two systems compare, default by default?
Most day-to-day differences come from a handful of defaults and modifiers, summarized in the table below. Where a drawing does not state an exception, the default of whichever standard governs it applies.
| Topic | ASME Y14.5 default | ISO GPS default | How to override |
|---|---|---|---|
| Size vs. form | Rule #1: perfect form at maximum material condition | Independency: size and form are separate | ASME: circled I or a note. ISO: circled E after the size |
| Size measurement | Actual local size plus the envelope | Two-point local size | ISO size modifiers (for example GG, GX, GN) |
| Invoking the system | Drawing notes the standard and edition | Using any GPS indication invokes the whole GPS system | State the governing standard in the title block |
| Patterns on the same datums | Simultaneous requirement | Separate requirements | ASME: SEP REQT. ISO: CZ or SIM modifiers |
| Concentricity and symmetry | Removed in the 2018 edition; use position, profile or runout | Still defined in ISO 1101 | Replace with position or runout on mixed drawings |
| Exact dimensions | Basic dimension (boxed) | Theoretically exact dimension, TED (boxed) | Same symbol, different name |
| Datums | Datum feature simulators, degrees of freedom | Association rules and modifiers in ISO 5459 | Name the standard; add datum targets where contact matters |
| Material condition default | Regardless of feature size unless M or L is shown | No material requirement unless M or L is shown (ISO 2692) | Add the circled M or L where function needs it |
Two rows deserve a note. The invocation row reflects how ISO 8015 frames GPS as a system: once a drawing uses a GPS indication, the fundamental principles come with it, whether or not ISO 8015 is named. The concentricity row reflects the 2018 revision of Y14.5, which, as ASME describes it, restructured the standard around profile, orientation and form and emphasized profile for locating surfaces. An old ASME drawing may still show concentricity; the edition in the title block tells you whether it is valid.
Do datums work the same way in ASME Y14.5 and ISO 5459?
The datum letters and reference frames look alike, but the two standards establish a datum from a real, imperfect surface by different rules, so the same datum reference can seat the part differently in inspection.
ASME Y14.5 builds datums from datum feature simulators: the theoretically perfect counterpart of a datum feature, such as a plane contacting the high points of a surface or the largest pin that fits a hole, and it explains the reference frame in terms of the degrees of freedom each datum constrains. The 2018 edition expanded that treatment.
ISO 5459:2024 defines datums through specification operators: rules for associating an ideal feature with the real surface, with modifiers that can change the association or restrict which part of a feature is used. The edition matters here, because the 2011 edition was withdrawn and replaced in 2024.
For a machined or cast part the practical advice is the same under both systems. Pick datum features that are functional and stable, dimension critical features from them, and use datum targets on as-cast or warped surfaces so every inspector contacts the same spots. On a die-cast part that is later machined, show which datum features the machining fixture uses and which ones the final inspection uses, and make them the same where you can.
How can you tell which standard a drawing follows?
Read the title block first: a well-made drawing names the governing standard and its edition, such as ASME Y14.5-2018 or ISO 8015 and ISO 1101. When it does not, a few clues narrow it down, but a clue is not a substitute for asking the designer.
- Projection symbol. The truncated-cone symbol shows first-angle projection, common on European and Asian drawings, or third-angle projection, the North American norm. It hints at origin, not at the tolerancing standard.
- Decimal marker and units. A decimal comma and metric units suggest an ISO-based drawing; inch dimensions with a decimal-place tolerance block suggest ASME. Metric ASME drawings exist, so this is only a hint.
- Modifiers. Circled E after a size, ISO size codes, CZ in a frame, or a general note citing ISO 22081 or ISO 2768 point to ISO GPS. SEP REQT, a circled I, or a note citing Y14.5 point to ASME.
- Symbols that one side dropped. A concentricity or symmetry symbol on a drawing that claims the 2018 ASME edition is a red flag worth querying before the quote.
General tolerance notes are a further tell. ISO drawings often set defaults with ISO 22081:2021, which ties general geometrical and size specifications to ISO 8015, or with the older ISO 2768 note. The general tolerances guide covers those notes in detail.
What should a drawing say before it goes to an overseas supplier?
It should name one governing standard with its edition, state which default applies to size and form, and flag every feature where the part depends on an exception. A supplier can then quote and inspect the drawing as written instead of guessing.
This matters more when the supplier works to both systems. A shop in Vietnam or elsewhere in Asia may see drawings built on ISO conventions as well as US drawings built on ASME, and an inspector can carry over the habits of whichever system they see most. A clear title block removes that risk. Use this checklist before release:
- Standard and edition in the title block. Write “Dimensioning and tolerancing per ASME Y14.5-2018” or name the ISO GPS standards, including ISO 8015. Do not cite both unless you say which one wins.
- Size-form default stated for fits. On an ISO drawing, put the circled E on every bore and shaft that must assemble. On an ASME drawing, check that no fit-critical feature carries a circled I by habit.
- Size modifiers explained. If you use ISO size codes, list them in the RFQ so the supplier confirms it can measure them.
- Datum features that the shop can fixture. Datum targets on cast faces, and the same datum reference frame for machining and inspection.
- No retired symbols. Replace concentricity and symmetry with position, runout or profile on ASME 2018 drawings.
- One unit system and one decimal marker. Mixed units are a common source of misreadings.
Tight turned features show why this pays off. A tight tolerance on a feature made on CNC turning only protects an assembly if the drawing also says whether form is bound by the size limits. The RFQ package guide lists the rest of what to send, and a drawing prepared this way can go straight to a quote request, where questions about the standard are raised feature by feature.
Frequently asked
Is ISO GPS stricter or looser than ASME Y14.5?
Neither, as a rule. Under independency an ISO size tolerance alone allows form error that Rule #1 would reject, but a complete ISO drawing adds form tolerances or the envelope where it matters. The risk is an incomplete drawing read under the wrong default.
Can one drawing use both ASME Y14.5 and ISO standards?
It can cite ISO documents for things ASME does not cover, such as ISO fit classes or surface texture, but the tolerancing rules should come from one system. If a drawing cites both, add a note saying which takes precedence.
Does an ISO drawing need to mention ISO 8015?
Under ISO 8015:2011, using any GPS indication invokes the system, so the principle of independency applies anyway. Naming it in the title block still helps, because older national practices sometimes defaulted to the envelope.
Is Rule #1 the same as the ISO envelope requirement?
They express the same idea: perfect form at maximum material size. The difference is that ASME applies it by default to features of size, while ISO applies it only where the circled E or a note calls for it.
Which edition of ASME Y14.5 is current?
ASME lists Y14.5-2018 as the current edition, reaffirmed in 2024. Drawings made to the 2009 or 1994 editions remain valid under the edition they cite, so keep the edition on the drawing.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024), accessed September 2026
- ISO 8015:2011, GPS — Fundamentals — Concepts, principles and rules, ISO, 2011 (reviewed and confirmed 2021)
- ISO 14405-1:2025, GPS — Dimensional tolerancing — Part 1: Linear sizes, ISO, 2025 (replaces the 2016 edition)
- ISO 14405-1:2016, GPS — Dimensional tolerancing — Part 1: Linear sizes, ISO, 2016 (withdrawn; abstract lists the size types)
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (reviewed and confirmed 2022)
- ISO 5459:2024, GPS — Geometrical tolerancing — Datums and datum systems, ISO, 2024
- ISO 2692:2021, GPS — Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR), ISO, 2021
- ISO 22081:2021, GPS — General geometrical specifications and general size specifications, ISO, 2021 (reviewed and confirmed 2026)
- ISO 286-2:2010, GPS — ISO code system for tolerances on linear sizes — Part 2: Tables of standard tolerance classes, ISO, 2010