What is true position in GD&T?

True position — called simply position in ASME Y14.5 and marked with the position symbol (a circle with a crosshair) — is the GD&T control that locates the axis or center of a feature, such as a hole or boss, relative to specified datums. Unlike a plus/minus coordinate dimension, position defines a single cylindrical tolerance zone centered on the basic (theoretically exact) location. As long as the feature’s real axis falls inside that cylinder, the part passes.

The cylindrical tolerance zone

A position callout states a diameter — for example a Ø0.3 zone. That diameter is the full width of a cylinder whose centerline sits exactly at the basic dimensions taken from the datums. The feature’s actual axis can lean or shift in any direction, but it must stay within that round cylinder. Because the zone is round, the allowed error is the same in every direction, which is exactly how a round pin fits a round hole.

The true position formula

To check a feature, you measure how far its actual center is from the basic location in two perpendicular directions, ΔX and ΔY. The actual position deviation is:

TP = 2 · √(ΔX² + ΔY²)

The square-root term, √(ΔX² + ΔY²), is the straight-line (radial) distance from the basic point to the actual center. The factor of 2 converts that radius into a diameter, because the position tolerance is always expressed as a diameter. The feature passes when this computed TP is less than or equal to the callout — and never confuse the radial distance with the diametral zone; forgetting the 2 is the most common true-position mistake.

Worked example

Suppose a hole is measured ΔX = 0.1 mm and ΔY = 0.1 mm off its basic location, against a Ø0.3 position callout:

TP = 2 · √(0.1² + 0.1²) = 2 · √(0.01 + 0.01) = 2 · 0.1414 = 0.283 mm

The actual deviation is 0.283 mm, which is inside the 0.3 mm zone, so the hole passes — but only by 0.017 mm. (This is exactly what the calculator returns for these inputs.) You can use the true position calculator to run your own X/Y deviations and get the same pass/fail check instantly.

Round zone vs. square ± box

Position is usually preferred over plain coordinate (±) tolerancing because of the shape of the zone. A coordinate dimension of ±x in both X and Y defines a square tolerance box, side 2x. The largest round zone that still guarantees the same minimum clearance is the circle inscribed in that square — but the round position zone that delivers equivalent fit is actually the one whose diameter spans the square’s diagonal:

Ø = 2 · x · √2

Switching from the inscribed-square thinking to the diametral round zone gives roughly 57% more usable area for the feature’s center to land in, all while keeping the same worst-case fit. That extra area means more good parts pass inspection without loosening the assembly — the practical reason GD&T position is the standard way to locate holes. The corners that the square allowed (where error in X and Y stack up) were never really safe for a round-on-round fit anyway, so the round zone is both more permissive and more honest about real clearance.

Material condition and bonus tolerance

Position is often combined with a material condition modifier. The most common is MMC (Ⓜ) — maximum material condition — which is the size at which the feature contains the most material (the smallest hole or the largest pin). When the callout carries the MMC modifier, the part earns bonus tolerance: any departure of the actual feature size from MMC is added to the allowed position tolerance.

The logic is geometric, not a loophole. A hole made larger than its MMC size has extra clearance around the mating pin, so its axis can wander further and the part still assembles. The amount of extra wander it can tolerate equals exactly how much bigger the hole is than MMC. To work the numbers — feature size, MMC, and the resulting bonus added to the geometric tolerance — see the MMC bonus tolerance calculator.

Reading the callout

A position feature control frame reads left to right: the position symbol, the diameter of the tolerance zone (a Ø prefix tells you the zone is round), any material condition modifier such as MMC (Ⓜ), and then the datum references — primary, secondary, and tertiary — that establish the coordinate system the basic dimensions are measured from. The basic location dimensions themselves are usually boxed elsewhere on the drawing and carry no tolerance, since the position zone is the only thing that bounds the error. If the symbols and datum letters are unfamiliar, the how to read GD&T symbols guide walks through each part of the frame.

Common pitfalls

• Dropping the factor of 2. The √(ΔX²+ΔY²) term is a radius; the callout is a diameter. Always double it.
• Ignoring bonus tolerance. With an MMC (Ⓜ) modifier, a feature can exceed its nominal geometric tolerance and still pass once the size departure is added.
• Measuring from the wrong origin. ΔX and ΔY must be taken from the basic location in the datum reference frame, not from a nearby edge or the part’s rough center.

Frequently asked questions

How do you calculate true position?

Measure how far the feature’s actual center is from its basic (theoretically exact) location in X and Y, then compute TP = 2·√(ΔX² + ΔY²). The factor of 2 turns the radial error into a diameter, because the position tolerance zone is a diameter, not a radius.

Why is a position tolerance better than a ± coordinate tolerance?

A square ±x box inscribes a round Ø = 2·x·√2 zone of the same minimum clearance, which has about 57% more area. The round zone matches how a round hole actually accepts a round pin, so position accepts more good parts without loosening the fit.

What is bonus tolerance at MMC?

When the callout carries an MMC (Ⓜ) modifier, any departure of the feature size from its maximum material condition is added to the stated position tolerance. A hole made larger than MMC has more clearance, so it earns extra position tolerance equal to that size departure.

Last reviewed: 2026-05-29.