Guide
What do the GD&T symbols mean, and what does each one cost to inspect?
GD&T symbols are the graphic shorthand that geometric dimensioning and tolerancing uses to say how much a feature may deviate in form, orientation, location, profile or runout, and from which datums. Under ASME Y14.5-2018 there are twelve geometric characteristic symbols, down from the fourteen on most older charts, plus a set of modifiers that change what each tolerance zone means.
By Saola Manufacturing engineering team · Published · Updated
This is a working reference for engineers and buyers who read drawings for a living: the full chart, what changed in 2018, the modifiers you will meet inside a feature control frame, and, for each symbol, how it is usually verified. The inspection method matters because it is part of the unit price. Two drawings with identical tolerance values can cost very different amounts to accept, depending on which symbols carry them.
On this page
What are the GD&T symbols in ASME Y14.5-2018?
The 2018 edition groups twelve geometric characteristics into five types: form, orientation, location, profile and runout. Form controls never take a datum, orientation and runout always do, and position and profile usually do.
The type tells you most of what you need to know before you read the number. A form tolerance (straightness, flatness, circularity, cylindricity) compares a feature only with a perfect version of itself. An orientation tolerance (perpendicularity, parallelism, angularity) controls tilt relative to a datum but not where the feature sits. Position controls location of a feature of size, profile controls the true shape and, with datums, location and orientation of a surface, and runout controls how a surface behaves as the part turns on a datum axis. The chart below lists every symbol, the inspection method shops typically use, and a relative inspection effort. The effort column is industry guidance for a single feature on a machined part, not a requirement of the standard.
| Symbol and name | Type | Datum needed? | MMC/LMC allowed? | Typical inspection | Relative effort |
|---|---|---|---|---|---|
| ⏤ Straightness | Form | No | Only on a feature of size (derived median line) | Indicator along a surface plate or straightedge | Low |
| ⏥ Flatness | Form | No | Only on a feature of size (derived median plane) | Indicator or height gauge sweep on a surface plate | Low |
| ○ Circularity (roundness) | Form | No | No | Roundness instrument; V-block readings only as a screen | Medium |
| ⌭ Cylindricity | Form | No | No | Roundness/cylindricity instrument or dense CMM scan | High |
| ⟂ Perpendicularity | Orientation | Yes | Yes, on a feature of size | Square or indicator on a surface plate; CMM for holes | Low to medium |
| ∥ Parallelism | Orientation | Yes | Yes, on a feature of size | Indicator sweep with the datum face on a surface plate | Low |
| ∠ Angularity | Orientation | Yes | Yes, on a feature of size | Sine plate and indicator, or CMM | Medium |
| ⌖ Position | Location | Almost always | Yes | Functional gauge at MMC; CMM otherwise | Low per part with a gauge; medium to high on CMM |
| ⌒ Profile of a line | Profile | Optional | No (datums may use MMB) | Optical comparator, contour tracer or CMM sections | Medium |
| ⌓ Profile of a surface | Profile | Optional | No (datums may use MMB) | CMM or 3D scan compared with the CAD model | High |
| ↗ Circular runout | Runout | Yes (axis) | No | Dial indicator while the part turns on its datum axis | Low |
| ⌰ Total runout | Runout | Yes (axis) | No | Indicator traversed along the surface during rotation | Low to medium |
| ◎ Concentricity (removed in 2018) | Location (2009) | Yes | No | CMM with opposed point pairs and derived midpoints | Highest |
| ⌯ Symmetry (removed in 2018) | Location (2009) | Yes | No | CMM with opposed point pairs and derived midpoints | Highest |
Which symbols did ASME Y14.5-2018 remove, and what replaces them?
The 2018 edition removed concentricity and symmetry, which is why older charts show fourteen characteristics and current ones show twelve. Use position, runout or profile instead, chosen by what the feature actually has to do.
Both removed symbols control derived median points: the midpoints between opposed surface points, which have to sit inside a zone around a datum axis or center plane. That is hard to measure, needs dense coordinate data and a midpoint calculation, and rarely matches design intent, because a lobed or tapered feature can pass while it still wobbles or fails to assemble. The ASME Y14.5 committee dropped both and pointed users to the other controls; the 2018 edition was reaffirmed in 2024 and remains the current US reference.
- A diameter that rotates against a bearing or seal: circular or total runout to the datum axis.
- A pilot, boss or bore that has to assemble: position, usually at MMC, so a fixed gauge can check it.
- A slot or tab centered on a datum plane: position at MMC for fit, or profile of a surface if the two faces must be controlled as shapes.
- Mass balance: a balance specification, not a midpoint tolerance.
Two cautions. A released drawing that cites Y14.5-2009 keeps its meaning, so its concentricity callout is still valid and must be inspected as written unless the buyer approves a substitute check in writing. And ISO 1101:2017 still uses the bullseye and symmetry symbols, with definitions based on extracted median features, so a European drawing showing them is current and should not be “corrected” to an ASME reading. The separate concentricity, runout and position guide works through shaft examples.
What do the modifier symbols in a feature control frame mean?
Modifiers change the size, shape or condition of the tolerance zone, and each one changes how the feature is inspected. When no material condition modifier is shown, the tolerance applies regardless of feature size, and datum features apply regardless of material boundary.
That default is Rule #2 per ASME Y14.5, and it is why an unmodified position callout usually goes to a CMM: the zone stays the same whatever the actual size, so a fixed pin gauge cannot represent it. Add the circled M and the tolerance grows as a hole departs from its smallest size, which is what lets a functional gauge accept the part in seconds. The MMC bonus tolerance guide shows the arithmetic. The modifiers you will meet most often are below.
| Symbol | Meaning | Effect on inspection |
|---|---|---|
| Ⓜ Maximum material condition (MMC) | Tolerance applies at the size with the most material; bonus as size departs | Allows a fixed functional gauge; size must still be measured |
| Ⓛ Least material condition (LMC) | Tolerance applies at the size with the least material, protecting wall or edge distance | No simple gauge; usually CMM with size-adjusted evaluation |
| No modifier (RFS / RMB) | Zone is fixed regardless of feature size; datum simulators adjust to the datum feature | Expanding or adjustable fixtures, or CMM |
| Ⓟ Projected tolerance zone | Zone extends above the part, typically for threaded or press-fit holes | Gauge pin or thread plug extended out of the hole and measured |
| Ⓕ Free state | Tolerance applies with the part unrestrained, for flexible parts | Measure before clamping; restrained checks need a separate note |
| Ⓣ Tangent plane | Controls the plane contacting the high points, not every surface point | Measure on a plate or rest; local dips are ignored |
| Ⓤ Unequally disposed profile | Profile zone offset toward one side of the true profile | CMM or scan with the offset entered in the evaluation |
| ↔ Between, ◯ all around, all over (two concentric circles) | Extent of a profile callout; the all over symbol dates from the 2009 edition | Larger surface to measure, often a full scan |
| ▷ Translation (datum) | Datum simulator may move to contact the datum feature | Fixture with a sliding locator |
| CF continuous feature, ST statistical tolerance | Treat interrupted surfaces as one feature; tolerance assumes statistical process control | Single gauge across gaps; capability data instead of 100% checks |
| Boxed dimension (basic) | Theoretically exact value that locates or shapes a tolerance zone | Not measured on its own; checked through the related tolerance |
How do you read a feature control frame from left to right?
Read the characteristic symbol first, then the tolerance with any diameter sign and modifier, then the datums in order of precedence. The datum order tells the inspector how to set the part up, and it is as much a part of the requirement as the number.
Take a hole pattern called out as ⌖ | ⌀0.25 Ⓜ | A | B | C in a
millimeter drawing. In words: the axis of each hole must lie inside a cylindrical zone of that diameter,
centered on its basic location, when the hole is at its smallest allowed size; larger holes get bonus
tolerance; and the part is set up resting on A, then against B, then against C. Swap B and C and you
have a different requirement on the same part, because the fixture contacts change.
Three more patterns worth recognizing on sight:
⏥ | 0.05on a face: flatness only, no datum, no location. It adds nothing if the same face already carries a tighter profile or parallelism callout.⟂ | ⌀0.02 | Aon a bore: the bore axis must sit in a cylinder perpendicular to A. Without the diameter sign the zone would be two parallel planes.⌓ | 0.4 | A | B | Con a cast surface: the whole surface must lie within a band around the CAD shape, located from the datum reference frame. One profile callout often replaces several size, location and form dimensions.
Values above are illustrations only; units come from the drawing’s general note, and that note should also name the standard and its edition.
Which GD&T callouts cost the most to inspect?
Callouts that need dense coordinate data or a full surface scan cost the most: legacy concentricity and symmetry, cylindricity, profile of a surface and unmodified position on many holes. Flatness, parallelism, runout and position at MMC with a gauge are usually the cheapest.
Inspection cost is roughly the time per check multiplied by how often the check is made. A runout or flatness reading takes an operator a short time at a bench and can be logged on every part. A CMM program for a profile or a large hole pattern has to be written once, then run with the part fixtured, and the report reviewed. A functional gauge for position at MMC flips the economics: it costs design and manufacturing time up front, then checks each part almost instantly, which pays at volume and rarely on a short run.
The sampling plan multiplies all of this. A characteristic checked on every part costs more than one checked on the first article and then at intervals, and a callout marked as a key or critical characteristic usually triggers more frequent checks. The cheapest drawing is not the one with the loosest numbers; it is the one where each tight requirement uses the control that is easiest to verify while still protecting the function. The tight-tolerance cost guide covers the machining side of the same trade-off, and the ASME Y14.43 standard governs how functional gauges and fixtures are toleranced.
What GD&T mistakes show up most on drawings sent for quotes?
The most common are a missing or ambiguous datum reference frame, symbols that conflict with each other or with the stated edition, and tight form controls stacked on features that do not need them. Each one either raises the quote or produces an exception list in the reply.
- No edition named. A drawing that says “GD&T” but not “per ASME Y14.5-2018” or “per ISO 1101” leaves the meaning of several symbols open.
- Concentricity under a 2018 note. The symbol does not exist in that edition, so the supplier has to ask what was meant.
- Datums the part cannot rest on. A small chamfer or a cast surface with draft as primary datum gives an unstable setup and readings that do not repeat.
- Orientation without location. Perpendicularity on a hole with no position callout controls tilt but leaves the location to plus-minus dimensions, which accumulate.
- Redundant form controls. Flatness tighter than the size tolerance can be meaningful, but flatness looser than a profile or parallelism already on that face is noise that still gets measured.
- Runout with MMC. Runout cannot take a material condition modifier; if bonus tolerance is the goal, position is the control.
To see how a CAD system writes feature control frames on the model, the NIST MBE PMI test cases publish fully toleranced example parts using ASME Y14.5 GD&T. NIST states that these test cases are not intended to show best practice in applying GD&T, so use them to check how annotations are written and exchanged, not as a model for your own tolerancing.
What should an RFQ say about GD&T and inspection?
Name the standard and edition, mark which geometric callouts are functionally critical, and say what inspection evidence you expect for each. With those three things, a supplier can price the inspection instead of guessing it.
- Standard and edition in the title block or general notes, and the units.
- Critical characteristics flagged on the drawing, so the inspection plan concentrates on them.
- Evidence per callout: a recorded value, a gauge pass/fail result, or a CMM or scan report. If a callout can only be verified by coordinate measurement, say so, so the method is agreed before the quote.
- Legacy symbols: if the drawing is under Y14.5-2009 and keeps concentricity or symmetry, state whether runout or position may be used as the check.
- Functional gauges: say whether you supply them, approve the supplier’s design, or expect variable data instead.
At Saola, every GD&T callout on a milled part is measured and logged, the first piece off new tooling is measured against every toleranced dimension, and the drawing review reads every tolerance, callout and note and returns a marked-up copy of your own drawing; ISO 9001 is in progress, not held. Datum faces and bores on castings and blanks are cut on CNC milling, and shafts, bushings and fittings on CNC turning. The RFQ guide lists the rest of the package, and the quote form accepts the STEP file and the drawing in one upload.
Frequently asked
Are there 14 or 12 GD&T symbols?
Both answers appear because the editions differ. ASME Y14.5-2009 and earlier list fourteen geometric characteristics; the 2018 edition removed concentricity and symmetry, leaving twelve. ISO 1101 still includes the equivalents of both.
Is true position the same as position?
Yes. “True position” is the older shop name; the standard calls the characteristic position and uses “true position” for the theoretically exact location set by basic dimensions.
Does flatness need a datum?
No. Flatness is a form control and compares the surface only with a perfect plane. If the face must also be parallel or square to something, that needs an orientation control with a datum.
Can a supplier check profile of a surface without a CMM?
Sometimes, with a dedicated checking fixture and indicators at defined points, or an optical comparator for profile of a line. For a complex surface, a CMM or scan against the model is the usual method, so say in the RFQ how you expect it to be verified.
Do ASME and ISO use the same symbols?
Mostly, but not always with the same meaning. Default rules on size and form differ, and ISO uses some symbols ASME removed. The ASME vs ISO GPS guide covers the differences that change a quote.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ASME Y14.5-2009, Dimensioning and Tolerancing, ASME, 2009 (superseded; source of the concentricity and symmetry definitions)
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, 2011 (reaffirmed 2020)
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (reviewed and confirmed 2022)
- ISO 2692:2021, GPS — Geometrical tolerancing — Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR), ISO, 2021
- ISO 5459:2024, GPS — Geometrical tolerancing — Datums and datum systems, ISO, 2024
- NIST MBE PMI CAD models and test cases (ASME Y14.5 GD&T), NIST, 2016 (page updated 2025)