GD&T in practice

Why it matters

A drawing that says "hole at 40 ± 0.1 from the edge" seems clear until two inspectors measure the same part and get different answers because they measured from different edges, or until a perfectly good part is rejected because a square tolerance zone was stricter than the assembly needed. Geometric Dimensioning and Tolerancing (GD&T) is a symbolic language that says exactly which features matter, how to measure them, and how much variation is allowed. In the US it is defined by ASME Y14.5 (the current edition is Y14.5-2018); internationally, the ISO GPS standards such as ISO 1101 cover similar ground with some differences. See asme.org and iso.org for the current editions. Checked on 2026-10-23.

Datums: where measurement starts

A datum is a theoretically exact reference (a plane, an axis or a point) established from a real feature on the part, labelled with a letter in a box such as A. Datums are chosen from how the part is located in its assembly: the face that sits on the frame, the bore that goes over a shaft, the edge that butts against a stop.

The datum reference frame uses up to three datums in order of precedence:

• Primary (A): the part rests on it with at least 3 points of contact. It stops 3 degrees of freedom (one translation, two rotations).
• Secondary (B): at least 2 points of contact, perpendicular to A. It stops 2 more.
• Tertiary (C): at least 1 point of contact. It stops the last one.

This is the 3-2-1 rule. The order matters: a part fixtured on A first and then B can measure differently from one fixtured on B first.

Basic dimensions and the feature control frame

GD&T locates features with basic dimensions, shown in a box (for example, a boxed 40). A basic dimension is the theoretically exact distance: it has no tolerance of its own. The tolerance lives in a feature control frame attached to the feature, read left to right:

| position | dia 0.2 (M) | A | B | C |

That reads: "the axis of this hole must lie within a cylinder of diameter 0.2 mm, at maximum material condition, located by the basic dimensions from datums A, B and C."

Position tolerance

With classic ± coordinate tolerances, each direction gets its own band, so the zone is a square. Position uses a cylindrical zone around the true position. A circle that just encloses a ±0.1 mm square has a diameter of 0.2 × sqrt(2) = 0.283 mm, so the round zone accepts about 57 % more area than the ±0.1 mm square while still guaranteeing the part fits (a hole that is 0.14 mm off diagonally fits just as well as one 0.14 mm off in x).

Checking position from measured coordinates:

dx = measured x - basic x,  dy = measured y - basic y
actual position (diameter) = 2 * sqrt(dx^2 + dy^2)

Example: the hole's basic location is (40, 25). A CMM measures its axis at (40.03, 25.04).

dx = 0.03, dy = 0.04
position = 2 * sqrt(0.03^2 + 0.04^2) = 2 * 0.05 = 0.10 mm    (within dia 0.2: accept)

Note the factor of 2: the axis is 0.05 mm from true position, but the zone is specified as a diameter.

Material condition modifiers and bonus tolerance

Maximum material condition (MMC), symbol (M), is the size at which the feature contains the most material: the smallest hole or the largest pin. When position is specified at MMC, the tolerance applies at MMC and grows as the feature departs from MMC. This extra is the bonus tolerance, and it reflects real assembly: a bigger hole can be a little further off and the bolt still fits.

Example: a hole sized dia 10.0 to 10.2, position dia 0.1 at MMC.

MMC (smallest hole)       = 10.0
actual hole size          = 10.15
bonus                     = 10.15 - 10.0 = 0.15
allowed position          = 0.1 + 0.15 = 0.25 mm

Least material condition (LMC), symbol (L), is the opposite (largest hole, smallest pin) and is used when wall thickness or edge distance must be protected. With no modifier, the tolerance is fixed regardless of feature size (RFS, the default in ASME Y14.5).

Other common controls

• Form: flatness, straightness, circularity, cylindricity (no datum needed).
• Orientation: perpendicularity, parallelism, angularity (to a datum).
• Profile of a surface or line: the most versatile control, often used for complex shapes.
• Runout: circular and total runout for rotating parts, measured relative to a datum axis.

Common mistakes

• Choosing datums for convenience. Datums should come from how the part functions and is assembled, then inspection follows them.
• Forgetting the diameter symbol. Without it, a position zone is two parallel planes, not a cylinder.
• Tolerancing everything tightly. Each tight tolerance costs machining time and inspection. Tolerance what the function needs.
• Mixing ASME and ISO rules. Some defaults differ (for example, how size and form interact). State which standard the drawing follows.

Recap

• Datums A, B, C build a reference frame by the 3-2-1 rule, chosen from function.
• Basic dimensions are exact; tolerances live in feature control frames.
• Position = 2·sqrt(dx² + dy²) against a cylindrical zone.
• At MMC, bonus tolerance = departure from MMC size.

Try it

The Do tab has a quiz on reading datums, computing position and finding bonus tolerance.