Guide
What is Rule #1 in GD&T, and why do ISO drawings not follow it?
Rule #1 is the default in ASME Y14.5 that ties form to size: when a feature of size carries only a size tolerance, its surface may not cross a boundary of perfect form at maximum material condition, so the size limits also cap straightness, flatness and roundness. That is what engineers mean when they search for “rule 1 GD&T”, and it is also called the envelope principle. ISO drawings default to the opposite idea, the principle of independency in ISO 8015, where size controls size and nothing else.
By Saola Manufacturing engineering team · Published · Updated
The side-by-side comparison of the two standards is covered in the ASME Y14.5 vs ISO GPS guide. This guide stays on one rule and works it through: what the envelope actually requires at each size, how much bend or taper a size tolerance quietly permits under each system, where Rule #1 stops applying, how an inspector proves it, and the exact notes to put on a drawing and an RFQ so a supplier on the other side of the world reads the size tolerance the way you meant it.
On this page
What exactly does Rule #1 require of a feature of size?
It sets two limits at once: the whole feature must fit inside a perfect-form envelope at its maximum material size, and every cross-section must still measure no smaller than the least material size for a shaft, or no larger for a hole.
A feature of size is a cylinder, a sphere, or a pair of opposed parallel surfaces such as a slot or a tab. For an external feature like a pin, maximum material condition (MMC) is the largest allowed size; for an internal feature like a bore, it is the smallest. Rule #1, as written in ASME Y14.5, makes MMC a boundary of perfect form. A pin produced exactly at its upper limit along its full length must therefore be perfectly straight and round. As the pin is made smaller, the gap between its actual size and that boundary becomes room for form error.
The rule has a second half that is easy to forget. At least material condition (LMC) there is no envelope: the standard checks the actual local size of each cross-section against the limit, one section at a time. A pin made at the bottom of its tolerance can be bowed by the full size tolerance and still conform, because it would still slide into a hole made at the pin’s MMC. That asymmetry is deliberate. Rule #1 exists to guarantee assembly, and assembly is only threatened at the tight end.
It applies by default to every individual regular feature of size, internal or external. A form tolerance on the surface, such as surface straightness or cylindricity, can only tighten it, never loosen it. Nothing on the drawing has to invoke it beyond the note that the drawing follows ASME Y14.5. That is the source of most cross-border confusion, because a drawing that never mentions form is still controlling form.
How much form error does a size tolerance allow under each rule?
Under Rule #1, the allowed form error equals how far the feature has moved from MMC, so it grows from zero at MMC to the full size tolerance at LMC. Under ISO 8015 independency, the size tolerance places no limit on form at all, and the limit comes only from a form tolerance or a general geometrical tolerance.
Take a pin of nominal diameter 12 with the fit class h7, which per ISO 286-2 gives limits of 12.000 mm and 11.982 mm, mating with a bore of class H7 whose lower limit per ISO 286-2 is also 12.000 mm. The pin is 40 mm long, which matters because per ISO 2768-2 the general straightness tolerance grows with length. The table shows what each reading of the same callout permits. The values are the arithmetic of the standards applied to an illustrative part, not measured data.
| Actual local size of pin (mm) | Form error allowed by Rule #1 (mm) | Worst-case envelope, Rule #1 (mm) | ISO 8015, size callout only | ISO 8015 plus ISO 2768-K straightness: approximate worst-case envelope (mm) |
|---|---|---|---|---|
| 12.000 (MMC) | 0.000 | 12.000 | Form not limited by size | 12.200 |
| 11.995 | 0.005 | 12.000 | Form not limited by size | 12.195 |
| 11.990 | 0.010 | 12.000 | Form not limited by size | 12.190 |
| 11.982 (LMC) | 0.018 | 12.000 | Form not limited by size | 12.182 |
Read across the rows and the point is plain. Under Rule #1 the envelope never exceeds the MMC size, so a pin that passes inspection always enters a bore that passes inspection, with zero clearance as the worst case. Under independency with only a general straightness class, a pin can be bowed by an order of magnitude more than its size tolerance and still conform, and it will not enter the bore. Neither part is wrong. The drawing simply did not say what the assembly needed.
The same logic runs the other way for the bore. Its envelope sits at its smallest size, so a bore made at its lower limit must be perfectly straight and round, and a bore made at its upper limit can carry form error up to the full size tolerance. The fits guide covers how clearance classes are chosen; Rule #1 is what makes the chosen clearance real.
What does ISO 8015 independency do to the same callout?
It makes the size tolerance a pure size check, measured by default as a two-point local size, and leaves form to its own specification. To get envelope behavior on an ISO drawing, the designer must ask for it, either feature by feature with the circled E or with a general note.
ISO 8015:2011 states that each geometrical specification is met independently of the others unless a standard or a special indication says otherwise. It also makes the whole GPS system apply as soon as a drawing uses any GPS indication, so a drawing does not escape independency by leaving ISO 8015 out of the title block. The default size is the two-point size defined in ISO 14405-1, and the envelope requirement is the circled E written after the size tolerance, as in “Ø12 h7 Ⓔ”.
Older drawings complicate the picture, and a buyer reviewing a legacy package should know three patterns:
- “ISO 2768-mK-E”. The trailing E applies the envelope to every single feature of size on the sheet, which turns the drawing into a Rule #1 drawing in effect. The class letters are explained in the ISO 2768 and NADCA tolerance guide.
- German drawings without an ISO 8015 note. The older DIN 7167 convention applied the envelope by default, so a drawing made to that practice expected Rule #1 behavior even though it cited no ASME standard. A note reading “Tolerancing ISO 8015” was the switch to independency.
- General geometrical notes. ISO 22081:2021 replaced the general geometrical tolerances of ISO 2768-2. It sits inside the ISO GPS system, so independency still applies: a general geometrical note limits form loosely, but it does not recreate the envelope.
Material condition modifiers also bring size and form back together for the feature that carries them. The maximum material requirement in ISO 2692:2021 is the ISO way of protecting assembly through a geometrical tolerance, and the MMC bonus tolerance guide works an example of it.
Where does Rule 1 GD&T stop applying?
Rule #1 controls the form of one feature against its own size and nothing more. It does not control orientation or location between features, and ASME Y14.5 lists cases where it is switched off by default or by the drawing.
- Relationships between features. Two diameters on a stepped shaft can each satisfy Rule #1 and still be tilted or offset relative to each other. Perpendicularity of a bore to a face, coaxiality of two journals, and the position of a hole all need their own feature control frames. A buyer who reads “Rule #1 applies” as “the part is geometrically controlled” is reading too much into it. The runout and position guide covers the controls that do this job.
- Stock as supplied. Bar, sheet, tube and structural shapes made to an industry or government standard follow that standard’s own straightness and flatness, not Rule #1, unless the drawing says the raw surface must meet it. This matters on a turned part that keeps an unmachined bar diameter.
- Free-state variation. Thin-walled or flexible parts that distort once released from the fixture are exempt from Rule #1 in the free state, and are normally specified in a restrained condition instead.
- Straightness of the axis or median plane. When a drawing applies straightness to the derived median line of a pin, Rule #1 no longer applies to that feature, and the MMC envelope is replaced by a boundary equal to the size limit plus the straightness tolerance (the virtual condition when the straightness is modified at MMC). This is the deliberate way to allow a long pin some bow while keeping a predictable mating boundary.
- Independency on purpose. In ASME Y14.5-2018 the circled I after a size tolerance (the independency symbol) removes the envelope for that feature; earlier editions did the same with the note “PERFECT FORM AT MMC NOT REQUIRED”. It is used for long slender parts, for features that are straightened in assembly, and for sizes that only matter as local thickness.
Edition matters too. The current Y14.5 edition is the 2018 one, reaffirmed in 2024 according to ASME, and earlier ANSI and ASME editions also carried the envelope rule. What changed over the editions is the wording of the exceptions and the symbols for switching it off, so state the edition on the drawing.
How is the envelope verified in inspection?
By checking both halves of the rule: a full-form gauge or an equivalent computed fit proves the MMC envelope, and local two-point measurements prove that no cross-section breaks the LMC limit. A caliper or micrometer alone only proves the second half.
This is the old Taylor principle of gauging. A go gauge should be a full-form counterpart of the mating part: a ring gauge for a pin, a plug gauge for a bore, long enough to cover the feature’s length, so a bowed or lobed part is caught the way the assembly would catch it. A no-go check should be a two-point contact, so a single undersize section is caught. The design and tolerancing of such gauges is set out in ASME Y14.43. Where a coordinate measurement is used instead, the software must evaluate the minimum circumscribed cylinder for a pin, or the maximum inscribed cylinder for a bore, against the MMC limit. A program that only reports average diameters will pass parts that Rule #1 rejects.
The common failure in overseas sourcing is not a bad part but a mismatched check. A shop used to ISO drawings may report two-point diameters only, which is correct under independency and incomplete under Rule #1. A shop used to ASME drawings may not apply an ISO size modifier at all. Both problems are solved before production by writing the expected method into the RFQ and the inspection plan, and by asking that the first article report show the envelope result next to the local size.
On the supplier side, the quality page describes a drawing review in which every tolerance, callout and note is read and the buyer receives a marked-up copy of the drawing, and a first-article report that measures every toleranced dimension on the first piece from new tooling. That review is the point at which an unstated size-form default should surface as a question. For long, slender turned parts, ask how the part will be supported along its length instead of cantilevered off a chuck, the setup that keeps a thin shaft straight; the CNC turning page describes turning at our lead CNC plant. A tight size limit only protects the assembly when the drawing also says whether form is bound by it. If your check needs a specific gauge or a computed envelope, say so on the RFQ so the method is confirmed in the written quote.
What should the drawing and RFQ say so a supplier applies the right rule?
Name one standard and edition, then mark every fit-critical feature with the behavior you want, using the symbol of that standard. Do not rely on the supplier inferring the default from the drawing’s origin.
Callout patterns that read unambiguously in either system:
- ASME drawing, envelope wanted (the default): “DIMENSIONING AND TOLERANCING PER ASME Y14.5-2018” in the title block, plain size tolerances on mating diameters, and no circled I on them.
- ASME drawing, independency wanted on one feature: the circled I after that size tolerance, plus a straightness or cylindricity control if the form still matters.
- ISO drawing, envelope wanted on fits: “Ø12 h7 Ⓔ” on each mating shaft and bore, with ISO 8015 and the general specification standard named once.
- ISO drawing, envelope wanted everywhere: a general note applying the envelope to all features of size, or the legacy “ISO 2768-mK-E” if the package already uses ISO 2768.
Common mistakes worth catching at drawing review:
- A metric drawing from a US team that cites ASME Y14.5 but is read as ISO because of the first-angle symbol or decimal commas. The projection guide explains why projection says nothing about the tolerancing standard.
- An ISO drawing with fit classes on shafts and bores but no circled E, where the designer assumed the fit class implied the envelope. Under ISO 8015 it does not.
- A drawing that cites both ASME Y14.5 and ISO 8015 without saying which wins.
- A long slender pin left under Rule #1 that cannot be made straight to its own size tolerance, where a circled I plus a realistic straightness tolerance would have been the honest callout and cheaper to make, as the tight tolerance cost guide explains.
In the RFQ itself, add one line per critical feature: the governing rule, the check you expect, and the data you want back. Something like “Bore B: envelope per ASME Y14.5-2018 Rule #1, verify with plug gauge at MMC plus two-point at LMC, report both” removes the guesswork. The RFQ preparation guide lists the rest of the package, and a drawing prepared this way can go straight to a quote request.
Frequently asked
Does Rule #1 apply to a slot or a tab, not just a cylinder?
Yes. A width between two opposed parallel surfaces is a feature of size, so at MMC the two surfaces must fit between two perfectly flat, parallel planes set at the MMC distance. That limits the flatness and bow of the faces. It does not orient the slot or tab to any other feature; that still needs a geometric tolerance to a datum.
Does Rule #1 control perpendicularity or position?
No. It controls the form of a single feature relative to its own size limits. Orientation and location between features always need their own geometric tolerances, under either standard.
Does an MMC modifier on a position tolerance replace Rule #1?
No. Under ASME Y14.5 the size envelope from Rule #1 still applies to the feature, and the position tolerance at MMC adds a separate virtual-condition boundary for location. Both must be met.
Can a part pass under ISO 8015 and fail under Rule #1?
Yes. A shaft with every local size inside its limits but a bow that pushes its envelope past the maximum size conforms to a plain ISO size callout and fails Rule #1. That is why the governing standard has to be agreed before inspection, not after a rejection.
Should I switch my ASME drawings to independency to lower cost?
Only on features where form does not affect assembly or function, and then with an explicit form tolerance if form still matters at all. Removing the envelope from a fit makes inspection simpler but moves the risk to the assembly line.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 8015:2011, GPS — Fundamentals — Concepts, principles and rules, ISO, 2011
- ISO 14405-1:2016, GPS — Dimensional tolerancing — Part 1: Linear sizes, ISO, 2016 (since replaced by the 2025 edition)
- ISO 286-2:2010, GPS — ISO code system for tolerances on linear sizes — Part 2: Tables of standard tolerance classes, ISO, 2010
- ISO 2768-2:1989, General tolerances — Part 2: Geometrical tolerances, ISO, 1989 (withdrawn)
- ISO 22081:2021, GPS — General geometrical specifications and general size specifications, ISO, 2021
- ISO 2692:2021, GPS — Maximum material requirement, least material requirement and reciprocity requirement, ISO, 2021
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, 2011 (reaffirmed 2020)