GD&T Symbols Chart
Every ASME Y14.5 geometric characteristic, grouped by what it controls, with whether it takes a datum and whether it can carry MMC or LMC. Below that: the modifiers, the datum symbols, and how to read a feature control frame from left to right.
| Symbol | Characteristic | Datum | MMC / LMC | Tolerance zone |
|---|---|---|---|---|
| Form | ||||
| StraightnessHow straight a line element of a surface is, or how straight the derived median line (axis) of a pin or hole is. | Never | Only on a feature of size | Two parallel lines for a surface element; a cylinder (Ø in the frame) for a derived median line. | |
| FlatnessHow flat a surface is, independent of every other feature. | Never | Only on a feature of size | Two parallel planes the tolerance apart; the whole surface must sit between them. | |
| Circularity (roundness)Roundness of each circular cross-section of a cylinder, cone or sphere, checked one slice at a time. | Never | No (RFS only) | Two concentric circles in each cross-section, the tolerance apart radially. | |
| CylindricityRoundness, straightness and taper of a whole cylindrical surface at once. | Never | No (RFS only) | Two coaxial cylinders the tolerance apart radially. | |
| Orientation | ||||
| AngularityOrientation of a surface, axis or center plane at a basic angle to a datum, usually one other than 0 or 90 degrees. | Required | Only on a feature of size | Two parallel planes at the basic angle to the datum; a cylinder when the frame shows Ø and the feature is an axis. | |
| PerpendicularityHow square a surface, axis or center plane is to a datum. | Required | Only on a feature of size | Two parallel planes at 90 degrees to the datum; a cylinder for an axis when the frame shows Ø. | |
| ParallelismHow parallel a surface, axis or center plane is to a datum. | Required | Only on a feature of size | Two parallel planes parallel to the datum; a cylinder for an axis when the frame shows Ø. | |
| Location | ||||
| PositionLocation of a feature of size (hole, pin, slot, tab) relative to its true position, set by basic dimensions from the datums. | Usually | Yes | A cylinder (Ø) around the true position of an axis, or two parallel planes around a true center plane. | |
| ConcentricityWithdrawn in 2018Whether the median points of a feature of revolution sit on a datum axis. | Required | No (RFS only) | A cylinder around the datum axis that must contain every derived median point. | |
| SymmetryWithdrawn in 2018Whether the median points of a slot or tab sit on a datum center plane. | Required | No (RFS only) | Two parallel planes centered on the datum center plane that must contain every derived median point. | |
| Profile | ||||
| Profile of a lineShape of each line element (cross-section) of a surface against its true profile. | Optional | No (RFS only) | Two offset lines along the true profile in each cross-section, equally disposed unless noted. | |
| Profile of a surfaceThe whole surface in 3D against its true profile: form, and with datums, orientation and location too. | Optional | No (RFS only) | Two offset surfaces around the true profile, equally disposed unless the frame carries the U modifier. | |
| Runout | ||||
| Circular runoutWobble of each circular element of a surface of revolution as the part turns on the datum axis. | Required | No (RFS only) | Checked slice by slice: the indicator reading (FIM) at each circular element must not exceed the tolerance. | |
| Total runoutThe whole surface at once as the part turns on the datum axis: straightness, taper, roundness and coaxiality together. | Required | No (RFS only) | Two coaxial cylinders about the datum axis (or two parallel planes square to it for a face). | |
ASME Y14.5-2018 vocabulary. Concentricity and symmetry were withdrawn in the 2018 edition and remain in ISO 1101. Summaries are ours; confirm against the edition your drawing invokes.
- Straightness: Applied to a diameter it controls the axis and overrides Rule #1, so the part may bow past the perfect-form envelope at MMC; the limit becomes a virtual condition.
- Flatness: On a plain surface there is no modifier. Applied to a width (a feature of size) it controls the derived median plane and may take MMC or LMC.
- Angularity: Orientation tolerances do not locate the feature; pair them with a size or location tolerance.
- Parallelism: On a flat surface, parallelism also limits its flatness to the same value.
- Position: Datums are normally required; a pattern of features positioned only to each other, or a coaxial set, can omit them.
- Concentricity: Withdrawn in Y14.5-2018. Still found on older prints and in ISO 1101. Modern practice: position, runout or profile.
- Symmetry: Withdrawn in Y14.5-2018. Still found on older prints and in ISO 1101. Modern practice: position or profile.
- Profile of a line: Without datums it controls form only; with datums it also controls orientation and location.
- Profile of a surface: The most versatile control in the standard: with datums it can locate a surface the way position locates a hole.
Have a GD&T drawing to make or inspect? that hold the tolerances and report them.
Modifiers
Modifiers sit in the tolerance cell of the frame, next to a datum letter, or on the leader. They change when or where the tolerance applies.
| Symbol | Modifier | What it means |
|---|---|---|
| Maximum material condition (MMC)M in a circle, after the tolerance value | The stated tolerance applies when the feature holds the most material: smallest hole, largest pin. As the feature departs from MMC the zone grows by the same amount (bonus tolerance). Used where the goal is assembly. | |
| Least material condition (LMC)L in a circle, after the tolerance value | The stated tolerance applies at the least material: largest hole, smallest pin. Bonus comes as the feature moves toward MMC. Used to protect a minimum wall or edge distance. | |
| Regardless of feature size (RFS)No symbol: it is the defaultCircled S is the old RFS symbol seen on 1982-era prints; current editions use no symbol. | The tolerance stays the same whatever size the feature is produced at, so there is no bonus. Rule #2 makes RFS (and RMB for datums) the default when no modifier is shown. | |
| Projected tolerance zoneP in a circle after the tolerance, with the projection height | Moves the zone out of the hole and projects it above the part by the stated height. Used on threaded and press-fit holes so a tilted bolt or pin does not clash with the mating part. | |
| Free stateF in a circle after the tolerance | The tolerance applies with the part unrestrained. Used on non-rigid parts (thin rings, sheet metal, rubber) that are otherwise inspected clamped to a note. | |
| Tangent planeT in a circle after the tolerance | The orientation tolerance applies to the plane that rests on the high points of the surface, not to every point on it. Useful for mounting faces where only the contact plane matters. | |
| Statistical toleranceST in an elongated hexagon | The value came from statistical tolerance analysis, so the feature must be produced under statistical process control. The drawing carries a note saying so. | |
| Unequally disposed profileU in a circle inside a profile frame, followed by a value | Profile zones split equally about the true profile by default. With U, the value after the symbol is the part of the zone on the side that adds material; the rest lies on the other side. | |
| IndependencyI in a circle next to a size dimension | Switches off Rule #1 for that feature: size and form become independent, so the perfect-form envelope at MMC no longer applies. Add a form control if form still matters. | |
| All aroundA small circle on the bend of the leader | The profile tolerance applies all the way around the outline shown in that view, not only to the surface the leader touches. | |
| All overTwo concentric circles on the bend of the leader | The profile tolerance applies to every surface of the part in three dimensions. Common on castings, forgings and molded parts. | |
| BetweenA double-headed arrow between two labeled points, under the frame | The tolerance applies only to the stretch of surface from one labeled point to the other (for example from X to Y). |
Datum feature and datum target symbols
Datum feature symbol
A capital letter in a square box, tied by a short leader to a triangle (filled or open) that sits on the surface or on an extension line. On a surface it names that face; in line with a size dimension it names the feature of size (its axis or center plane). The letters I, O and Q are not used.
Datum target symbol
A circle split by a horizontal line. The lower half holds the datum letter and target number (A1, A2, A3); the upper half holds the target area size when the target is an area, and is left blank for a point or line. Used on castings, forgings and other rough surfaces where only specific spots should touch the fixture.
Datum target point
An X on the view where the target point sits. A target line uses an X in the edge view and a phantom line in the other; a target area is a hatched region inside a phantom outline.
Reading a feature control frame, left to right
- 1. Geometric characteristic (Position symbol): What is being controlled. One characteristic per frame; stack frames to apply two.
- 2. Tolerance (Ø0.25 then M in a circle): Zone shape (Ø means cylindrical), the tolerance value, then modifiers: material condition (M or L), and where used P, F, T, U or ST. Here: a Ø0.25 cylinder when the hole is at MMC, larger as it departs from MMC.
- 3. Primary datum (A): The datum the part meets first and most fully (for a plane, at least three points of contact). A letter can carry its own modifier (M or L for MMB or LMB).
- 4. Secondary datum (B): Constrains the part next, square to the primary (two points of contact for a plane).
- 5. Tertiary datum (C): Removes the last degree of freedom (one point of contact for a plane). Datum order is fixed by the frame, not alphabetical.
Read aloud: the axis of this hole must lie inside a Ø0.25 cylinder at its true position, located by basic dimensions from datums A, B and C, when the hole is at its smallest size; the cylinder grows as the hole is made larger.
Rules worth knowing
Rule #1: size controls form
Where only a size tolerance is given, a regular feature of size may not break a boundary of perfect form at MMC. A pin toleranced Ø9.9 to Ø10.0 must pass a perfect Ø10.0 ring gauge along its length, so a pin made at Ø10.0 has to be perfectly straight. Stock sizes, free-state parts and features marked with the independency symbol are exempt.
Rule #2: RFS is the default
If no modifier is shown, the tolerance applies regardless of feature size and datum features apply regardless of material boundary (RMB). MMC or LMC has to be called out to get bonus tolerance.
Basic dimensions carry no tolerance
A boxed dimension is the theoretically exact distance or angle to the true position or true profile. The allowed variation comes from the feature control frame, not from the title block.
Orientation implies form
Parallelism, perpendicularity or angularity on a flat surface also limits its flatness to the same value, unless the tangent plane modifier is used. Add a tighter flatness callout only if the function needs it.
Frequently asked questions
- How many GD&T symbols are there?
- ASME Y14.5-2009 and earlier define 14 geometric characteristics in five groups: form, orientation, location, profile and runout. Y14.5-2018 withdrew concentricity and symmetry, leaving 12, but both still turn up on older drawings and in ISO 1101. Around the characteristics sit the modifiers (MMC, LMC, projected zone and the rest) and the datum symbols.
- Which GD&T controls never reference a datum?
- The form controls: straightness, flatness, circularity and cylindricity. They compare a feature only to a perfect version of itself. Profile can go either way: without datums it controls form only, with datums it also controls orientation and location.
- When can a tolerance use MMC or LMC?
- Only when it applies to a feature of size (a hole, pin, slot or tab), because the modifier ties the tolerance to the size the feature is actually made at. Position always qualifies. Straightness, flatness and the three orientation controls qualify when applied to a feature of size. Circularity, cylindricity, profile and runout are always RFS.
- What is bonus tolerance?
- With MMC, the tolerance grows by however far the feature departs from its MMC size. A hole sized Ø10.0 to Ø10.2 with position Ø0.1 at MMC gets Ø0.1 when made at Ø10.0 and up to Ø0.3 when made at Ø10.2. Parts that still assemble get accepted instead of scrapped, which is why MMC is the default choice for clearance holes.
- What is the difference between ASME and ISO GD&T?
- Most symbols match, but the defaults differ. Under ASME Rule #1 the size tolerance also limits form (the envelope principle). Under ISO 8015 size and form are independent unless the envelope requirement (circled E) is called out. Check which standard the title block invokes before you inspect or quote.
- Does every drawing need GD&T?
- No. Plenty of parts are fine with plus-minus dimensions and a general tolerance block such as ISO 2768. GD&T earns its keep on the features that locate mating parts: hole patterns, bores, pilots and mounting faces, where it states the function and usually opens up the tolerance a shop can work to.
