How to read GD&T symbols and the feature control frame

Geometric Dimensioning and Tolerancing (GD&T), defined by ASME Y14.5, is a symbolic language for telling a machinist exactly how much a feature is allowed to wander in form, orientation and location. Every control is packed into a small rectangle called the feature control frame. Once you can read that frame left to right, the rest of the drawing falls into place.

Feature control frame anatomy

The frame is divided into compartments that are always read in the same order, left to right:

1. Geometric characteristic symbol — which of the 14 controls applies (the position symbol, the flatness symbol, the perpendicularity symbol, and so on).
2. Tolerance compartment — the total width of the tolerance zone. If the zone is cylindrical, a diameter symbol (Ø) comes first, then the value, then any material condition modifier such as the MMC modifier (the circled M, Ⓜ).
3. Datum references — the primary, then secondary, then tertiary datum, each in its own compartment, with its own modifier if one is needed.

Written out in words, a typical position callout reads: position | Ø0.25 (M) | A | B | C. In plain English that is: the axis of this feature must lie within a cylindrical tolerance zone 0.25 mm in diameter, the zone is allowed bonus tolerance at maximum material condition, and that zone is located from datum A (primary), then B (secondary), then C (tertiary). The order of the datum letters is the order in which the part is constrained — it is not alphabetical by accident; A is simply the datum you list first.

The 14 geometric characteristics

ASME Y14.5 defines 14 characteristics in five families. Form controls stand alone; the rest reference datums. The tolerance-zone shape tells you what the value in the frame is measuring.

Family	Characteristic	Datum?	Tolerance-zone shape
Form	Straightness	No	Two parallel lines, or a cylinder for an axis
	Flatness	No	Two parallel planes
	Circularity (roundness)	No	Two concentric circles in a cross-section
	Cylindricity	No	Two concentric cylinders
Profile	Profile of a line	Usually	Two offset curves about the true profile (2D)
	Profile of a surface	Usually	Two offset surfaces about the true profile (3D)
Orientation	Perpendicularity	Yes	Two parallel planes (or a cylinder) at 90°
	Angularity	Yes	Two parallel planes at the basic angle
	Parallelism	Yes	Two parallel planes parallel to the datum
Location	Position	Yes	Cylinder (or two planes) around the true position
	Concentricity	Yes	Cylinder about the datum axis
	Symmetry	Yes	Two parallel planes about the datum centre plane
Runout	Circular runout	Yes	Two concentric circles in one cross-section (full revolution)
	Total runout	Yes	Two concentric cylinders over the whole surface

Concentricity and symmetry are rarely used in practice — they are hard to verify and most designers replace them with a position or runout control. The flatness calculator handles the simplest of the form controls, and the cylindricity & runout calculator covers the runout family.

Material condition modifiers

A modifier in the tolerance compartment changes how the tolerance is applied as the feature's size changes:

• MMC — maximum material condition (Ⓜ, the circled M): the stated tolerance applies when the feature contains the most material — the smallest hole or the largest pin.
• LMC — least material condition (Ⓛ, the circled L): the tolerance applies at the least material — the largest hole or the smallest pin.
• RFS — regardless of feature size: no symbol. This is the ASME Y14.5 default — the tolerance is fixed and the feature earns no extra allowance as it changes size.

The reason MMC matters is bonus tolerance. When a position control carries the MMC modifier, any departure of the feature from its maximum material size is added straight onto the position tolerance. For example, a hole called out at Ø10.0 mm MMC with a Ø0.25 mm position tolerance: if the hole is actually produced at Ø10.3 mm, it is 0.3 mm away from MMC, so the position tolerance grows to 0.25 + 0.30 = 0.55 mm. The looser the hole, the more position error it can absorb and still assemble. That bonus is exactly what the true position calculator adds for you; for a deeper walkthrough of the position formula see what is true position.

Datums and the datum reference frame

A datum is a theoretically exact reference — a point, axis or plane — that a feature is measured from. Datums are labelled with capital letters (A, B, C…) in a datum feature symbol, and called up in the frame as the primary, secondary and tertiary references.

Together they build a datum reference frame: three mutually perpendicular planes that fully fix the part in space using the 3-2-1 rule. The primary datum sits on three high points and removes three degrees of freedom (one translation and two rotations). The secondary datum touches on two points and removes two more. The tertiary datum touches on one point and removes the last one, leaving the part fully constrained — six degrees of freedom locked with 3 + 2 + 1 contacts. That is why datum order is load-bearing: A, B and C in a different sequence would seat the part differently and move the tolerance zones with it.

Reading example callouts in plain English

Put the pieces together and any frame becomes a sentence.

• flatness | 0.05 — “this surface must lie between two parallel planes 0.05 mm apart.” No datum, because flatness is a form control, and no diameter symbol, because the zone is a slab of space, not a cylinder.
• perpendicularity | 0.1 | A — “this surface (or axis) must stay within a 0.1 mm-wide zone that is exactly 90° to datum A.” One datum, because orientation is always relative to something.
• position | Ø0.25 (M) | A | B | C — “the axis of this hole must lie in a cylindrical zone 0.25 mm across, located from datums A, B and C, with bonus tolerance allowed as the hole departs from maximum material condition.” The Ø tells you the zone is round; the circled M unlocks the bonus.

Location and fit go hand in hand: once a hole's position is under control you still need its size to mate with its shaft, which is where the hole & shaft fit calculator comes in. Read the frame in order — symbol, tolerance, datums — and GD&T stops being a wall of glyphs and becomes a precise, checkable specification.

Frequently asked questions

What order do the boxes in a feature control frame go in?

Left to right: the geometric characteristic symbol, then the tolerance compartment (with a diameter symbol Ø if the zone is cylindrical, followed by the tolerance value and any material modifier), then the datum references — primary, secondary and tertiary in that order, each with its own modifier if needed.

What does the circled M after a tolerance mean?

The circled M is the maximum material condition (MMC) modifier. It says the stated tolerance applies when the feature is at its maximum material size; as the feature departs from MMC, it earns extra "bonus" tolerance equal to that departure. A circled L is LMC. With no modifier, the tolerance is regardless of feature size (RFS), the ASME Y14.5 default.

Which characteristics do not need a datum?

The four form controls — straightness, flatness, circularity and cylindricity — are self-referencing and never take a datum. Profile, orientation, location and runout controls reference one or more datums.

Last reviewed: 2026-05-29.