True position is the GD&T control that defines how far a feature may deviate from its exact theoretical location, holding it inside a cylindrical diameter tolerance zone centered on the basic dimensions, relative to specified datums. It answers one question: is the hole where it needs to be to assemble?
Position is the most-used control in all of GD&T because nearly every part has holes and pins that must line up with a mating part. Get position right and things bolt together; get it wrong and they do not, no matter how perfectly round or correctly sized the holes are. This guide goes deep on the mechanics: why the tolerance zone is a diameter rather than a box, how to calculate a true-position value from measured X and Y, how bonus tolerance grows the zone, and how it is inspected. For the wider language it lives in, start with GD&T basics.
What is true position in GD&T?
True position is a location control that specifies a tolerance zone within which the center (axis) of a feature must lie. The exact intended location is defined by basic dimensions, theoretically perfect numbers shown in boxes, carrying no tolerance of their own. The feature control frame then states how far the actual feature axis may stray from that perfect location, and relative to which datums. "True position" strictly refers to the exact theoretical location; the tolerance is the positional tolerance around it, though in everyday shop talk "true position" names the whole control and the calculated deviation value alike.
The key idea is that the tolerance applies to the feature's axis, not to a surface, and it is measured from datums in a defined order. That datum reference is what makes the measurement repeatable: everyone sets the part up the same way and measures location from the same origin, which is why position callouts almost always reference a datum reference frame.
Why is the tolerance zone a diameter, not a box?
The tolerance zone for position is cylindrical because that is how parts actually assemble. A hole functions based on how far its center sits from true position in any direction, a radial distance, so the set of acceptable center locations is a circle, and through the depth of the hole, a cylinder. The diameter symbol in front of the tolerance in the feature control frame is what declares the zone cylindrical rather than a rectangular slab.
Contrast that with plus/minus coordinate tolerancing, which puts a square box around the allowed location. The corners of that box let the center drift farther from true position than the sides do, up to about 1.4 times farther diagonally, so a square zone rejects good parts near the flats and accepts marginal ones in the corners. Switching the same distance limit to a round zone captures exactly the parts that assemble and gives roughly 57 percent more usable tolerance area for the same maximum deviation. That is not a rounding trick; it is the round zone matching the physics of a round hole mating with a round pin.
How do you calculate true position from X and Y?
To check a hole, you measure where its center actually is, compare that to where the basic dimensions say it should be, and convert the miss into a diameter you can read against the tolerance. The formula is:
True position = 2 × √(ΔX² + ΔY²) where ΔX and ΔY are the differences between the measured and the basic (true) coordinates.
The factor of two is the part people forget. The square-root term is the straight-line (radial) distance from true position to the measured center, the hypotenuse of the ΔX, ΔY right triangle. But the tolerance zone is a diameter, so you double that radial distance to get a diameter you can compare directly to the frame value. Here is the calculation as a procedure.
- Find the basic (true) coordinates. Read the exact intended X and Y of the feature from the basic dimensions on the drawing. These are theoretically perfect and carry no tolerance.
- Measure the actual coordinates. Establish the datums in order, then measure the feature's actual center X and Y from that origin, normally on a CMM.
- Compute the deviations. Subtract: ΔX = measured X minus true X, and ΔY = measured Y minus true Y. Sign does not matter because the next step squares them.
- Find the radial distance. Take the square root of (ΔX² + ΔY²). This is how far the center sits from true position in a straight line.
- Double it to a diameter. Multiply by two. The result is the actual true-position value, expressed as a diameter to match the cylindrical zone.
- Compare to the tolerance. If the calculated value is less than or equal to the positional tolerance in the feature control frame (plus any bonus tolerance), the feature passes.
A quick worked example: a hole is called out at basic X = 40.000, Y = 25.000 with a position tolerance of ∅0.20. It measures X = 40.050, Y = 24.960. Then ΔX = 0.050, ΔY = −0.040, the radial distance is √(0.0025 + 0.0016) = √0.0041 ≈ 0.064, and the true position is 2 × 0.064 ≈ 0.128, or ∅0.128. That is inside ∅0.20, so the hole passes on position, with room to spare before any bonus tolerance is even counted.
What is bonus tolerance and how does MMC add to it?
Bonus tolerance is extra position tolerance you earn when a feature is not at its worst-case size, and it is one of the most valuable ideas in GD&T because it keeps good parts from being scrapped. It appears when the positional tolerance carries a material condition modifier, most commonly maximum material condition (MMC), the circled M. At MMC a hole is at its smallest allowed size, which is the tightest case for assembly. As the hole is made larger than that, the extra clearance means the hole could sit slightly farther off position and still fit the mating pin, so that extra clearance is added to the position tolerance as a bonus.
The bonus is exactly the difference between the feature's actual size and its MMC size. If a hole's MMC (smallest) diameter is 10.00 with a position tolerance of ∅0.20 at MMC, and the hole is actually produced at 10.15, it has earned 0.15 of bonus, so the available position tolerance becomes ∅0.35. A hole calculating to ∅0.30 true position would fail against the stated ∅0.20 but pass against the ∅0.35 it actually earned, and it genuinely assembles, so passing it is correct, not lenient. This is why parts controlled at MMC are often checked with functional gauges that physically embody the boundary, bonus and all, and it is covered in depth under bonus tolerance in GD&T.
By the numbers
By the numbers. Position is defined in ASME Y14.5, the recognized U.S. standard for dimensioning and tolerancing, whose current edition is ASME Y14.5-2018; it establishes the position symbol, the cylindrical tolerance zone, basic dimensions, and the material condition modifiers that grant bonus tolerance (ASME, Y14.5 Dimensioning and Tolerancing). The geometry behind the round zone is fixed: a circular tolerance zone inscribed in the equivalent square provides roughly 57 percent more usable area for the same maximum deviation from true position, which is why position tolerancing accepts good parts a plus/minus box would reject. And because the value is a diameter, the true-position formula doubles the radial miss: true position = 2 × √(ΔX² + ΔY²), compared directly against the frame tolerance plus any earned bonus.
How is true position inspected?
True position is usually measured on a coordinate measuring machine (CMM), because the check needs the datums established in their correct order and the feature's actual center located precisely from that origin, something hand gauges cannot reproduce for a multi-datum callout. The CMM probes the datum features first to build the reference frame, measures the hole's actual axis, computes ΔX and ΔY, and reports the doubled radial value as the true-position result, automatically crediting bonus tolerance when the callout is at MMC. For position at MMC on simpler parts, a functional gauge is a fast alternative: a hardened pin at the virtual condition boundary either enters the hole in the fixtured part or it does not, physically testing position and bonus together in one motion.
Either way, the inspection is only as good as the measurement system behind it. A CMM still needs calibration and its own measurement systems analysis and gage R&R because a true-position number from an untrustworthy machine is just a precise-looking guess, and choosing between a CMM and a functional gauge is part of selecting the right gauge for the feature. A position callout is like a surface-roughness callout in one way that matters: both are exact requirements on the drawing that mean nothing until they are measured with a verified instrument and recorded where someone can act on them. When those results are captured live at the point of inspection rather than on a clipboard, a bolt pattern drifting toward the edge of its position zone shows up the same shift, not at the next audit, the shift CLS made with Harmony's quality intelligence and connected-systems modules, from measurements found the next morning to measurements visible while the parts are still on the machine.