GD&T Symbol Decoder — Read Any Feature Control Frame
Build the frame from the drawing and get back what it actually demands — in plain English, with how it would be inspected and what it does to the cost of the part. It also tells you when a combination is not legal, which is the part most symbol charts leave out.
1. Pick the characteristic
Fill both size boxes to see the bonus tolerance an MMC callout earns you.
The one difference that catches people out
If you take one thing from this page, make it the difference between the two standards on form. ASME Y14.5 applies Rule #1 by default, sometimes called the envelope or Taylor principle: every feature of size must have perfect form at maximum material condition unless the drawing says otherwise. Nothing needs to be written on the drawing to invoke it — it is silently assumed on every feature. ISO does the opposite. Under ISO 8015 the default is independency: size and form are decoupled, and a feature can pass a two-point size check everywhere while being noticeably bowed, tapered or out of round.
The consequence is concrete rather than academic. The same drawing, with the same numbers, means genuinely different things depending on which standard governs it. Read a European ISO print with American assumptions and you may accept a part whose form was never actually controlled. Read an American print with ISO assumptions and you may reject good parts, or add inspection nobody asked for. Each standard provides a symbol to invoke the other behaviour, and they are exact mirror images: ASME has circled I for independency, to switch Rule #1 off for one feature, and ISO has circled E for the envelope requirement, to switch it on. Neither symbol exists in the other standard, because in each case the behaviour is already the default.
The second thing worth internalising is that the modifiers are not free-floating decorations. A great many combinations are simply not legal, and this decoder tells you which. The form controls — straightness, flatness, circularity, cylindricity — never take a datum, because they judge a feature against itself rather than against anything else. Runout is the strictest of all: it never takes a material condition modifier anywhere, not even on the datum reference, because the datum axis has to be derived at RFS by definition. Profile is a subtler case: the tolerance value itself never takes MMC, but a datum letter inside the same frame still can, which produces datum shift rather than bonus tolerance. They are different mechanisms and worth not conflating.
Where modifiers are legal, they are usually worth using, because MMC is the cheapest tolerance on a drawing. Calling a hole position at MMC means the stated zone is the minimum you get, and the feature earns extra allowance as it departs from maximum material — a hole drilled larger than MMC can be further off position and still assemble perfectly, which is exactly the physical truth. Specifying the same position RFS throws that allowance away and buys nothing in return unless the design genuinely requires it. This is one of the most common and most expensive habits we see on incoming drawings.
Finally, the order of the datums is not cosmetic. Reading left to right, they are primary, secondary and tertiary, and they are contacted in that order to build the reference frame — conceptually three points, then two, then one, constraining three, two and one degrees of freedom to fully fix the part. Swapping two letters changes which surface takes priority contact and can change whether a part passes. If a drawing arrives with datums in an order that does not match how the part is naturally located in the fixture, that is worth a conversation before anything is cut.
GD&T symbols — FAQ
How many GD&T symbols are there?
ASME Y14.5-2009 defines 14 geometric characteristics. The 2018 edition withdrew concentricity and symmetry, bringing the official count to 12, because their derived-median-point definitions were difficult to verify repeatably. Both still appear on drawings in circulation and ISO 1101 retains them, so you still need to be able to read them.
Which GD&T symbols cannot have a datum?
The four form controls: straightness, flatness, circularity and cylindricity. They judge a feature against itself rather than against another feature, so a datum reference in a form control frame is an error on the drawing.
What is Rule #1 and how does ISO differ?
Under ASME Y14.5, Rule #1 requires perfect form at maximum material condition by default for every feature of size, with no symbol needed. ISO 8015 defaults to the opposite — independency, where size and form are controlled separately. ASME uses circled I to switch Rule #1 off; ISO uses circled E to switch the envelope requirement on. This is the most consequential difference between the standards.
What is bonus tolerance?
When a geometric tolerance carries an MMC modifier, the stated value is the minimum. As the produced feature departs from maximum material condition, it earns additional tolerance equal to that departure. Bonus = |actual mating size − MMC size|, added to the stated tolerance. It reflects the physical reality that a larger hole can be further off position and still assemble.
Why can runout never use MMC?
Because the datum axis for runout must always be derived at regardless-of-feature-size. That applies to the whole frame, so unlike most other characteristics, runout takes no material condition modifier on the tolerance value or on the datum reference.
Does the diameter symbol change the meaning?
Yes, substantially. A diameter symbol before the tolerance value makes the zone cylindrical, which suits round features because location error can occur in any radial direction. Without it, the zone is the space between two parallel planes, which suits a slot or tab centre plane where the deviation is one-directional.
Send Your Drawing for a Same-Day Quote
Talk directly to the engineers who will machine your parts — no account managers, no trading-company markups. Complimentary DFM review with every enquiry.