True Position Calculator: Formula and Bonus Tolerance
True position is twice the distance between a feature’s measured centre and its exact location: 2 × √(ΔX² + ΔY²). Enter the nominal and measured coordinates below, add the size limits if the callout carries Ⓜ or Ⓛ, and the calculator gives the position, the bonus tolerance and pass or fail.
True position and bonus tolerance
Use one unit throughout, mm or inches. Coordinates are measured from the datums.
| Deviation X / Y | 0.09 / 0.12 |
| True position | Ø0.3 |
| Bonus tolerance | 0.15 (MMC 10, LMC 10.2) |
| Tolerance allowed | Ø0.35 |
| Result | Pass, 0.05 to spare |
What is true position in GD&T?
True position is the exact location of a feature, such as a hole, set by basic dimensions from the datums. A position tolerance in a feature control frame, such as ⌖ Ø0.2 Ⓜ A B C, allows the feature’s axis to sit anywhere inside a round zone of that diameter centred on true position.
Basic dimensions are drawn in a box and carry no ± tolerance of their own; the position callout is the only tolerance on the location. The datum letters tell the inspector which surfaces to measure from, in order. For the other symbols in the frame, see engineering drawing symbols.
What is the true position formula?
True position = 2 × √(ΔX² + ΔY²). ΔX and ΔY are the measured coordinates minus the basic ones. The square root gives the distance from true position, and doubling it turns that radius into a diameter you can compare with the Ø tolerance.
Worked example: a hole is basic at X 25, Y 15 and measures X 25.09, Y 15.12. ΔX is 0.09 and ΔY 0.12, so the distance is 0.15 and the true position is Ø0.3. Against a plain Ø0.2 callout, it fails by 0.1.
How does bonus tolerance work at MMC?
With the Ⓜ modifier, the position tolerance grows as the feature moves away from its maximum material size. For a hole, the bonus is its actual size minus its smallest allowed size; for a pin, its largest allowed size minus its actual size. The bonus adds to the stated tolerance.
In the example, the hole is Ø10.00 to 10.20 and measures Ø10.15, so the bonus is 0.15 and the allowed position is Ø0.35. The measured Ø0.3 now passes with 0.05 to spare. A hole made at Ø10.00 gets no bonus and would still fail. The logic is assembly: a larger hole can sit further off and still clear its bolt.
What is the difference between MMC, LMC and RFS?
MMC (Ⓜ) gives bonus as a feature leaves its maximum material size, which protects assembly. LMC (Ⓛ) gives bonus as it leaves its least material size, the largest hole or smallest pin, which protects wall thickness. With no modifier the tolerance applies regardless of feature size (RFS) and there is no bonus.
Under ASME Y14.5, RFS is the default: a position callout without Ⓜ or Ⓛ gets no bonus, however the feature is made. Bonus also needs the measured size to be inside its own limits first; a hole that is oversize fails on size before position is checked.
How do you convert ± tolerance to true position?
A ±t coordinate tolerance makes a square zone; the round position zone that just holds it has a diameter of 2 × √2 × t, about 2.83 × t. So ±0.1 mm in X and Y becomes Ø0.283 mm, and the round zone gives 57% more area for the same worst-case corners.
| ± in X and Y | Equivalent position zone |
|---|---|
| ±0.05 mm | Ø0.1414 mm |
| ±0.1 mm | Ø0.2828 mm |
| ±0.2 mm | Ø0.5657 mm |
| ±0.005 in | Ø0.0141 in |
| ±0.010 in | Ø0.0283 in |
Going the other way, the largest square that fits inside a Ø0.2 zone is ±0.0707: a part checked to that square is always inside the round zone, which is the safe side when an old ± drawing is redrawn with GD&T.
How is true position measured?
An inspector sets the part on its datums in order, A then B then C, finds the feature’s centre, usually with a measuring machine probing several points, and reads its X and Y from the datums. Those readings, the basic dimensions and the measured size go into the formula above.
On the shop floor, a fixed functional gauge with pins at true position, each made at the hole’s virtual condition (its MMC size minus the position tolerance), checks MMC callouts without any arithmetic: if the part drops on, the holes pass. For how size and location tolerances add up across a part, see tolerance stack-up basics.
Frequently asked questions
What is the formula for true position?
True position = 2 × √(ΔX² + ΔY²), where ΔX and ΔY are how far the measured centre sits from its basic location. A hole 0.09 off in X and 0.12 off in Y has a true position of Ø0.3.
Why is true position multiplied by 2?
The position tolerance is a diameter, the width of the round zone the axis must lie in, while √(ΔX² + ΔY²) is the distance from its centre, a radius. Doubling the distance lets you compare it straight with the Ø value in the feature control frame.
How do you calculate bonus tolerance?
With the Ⓜ modifier, the bonus is how far the feature’s actual size has moved from its maximum material size: for a hole, actual size minus the smallest allowed size; for a pin, the largest allowed size minus actual size. Add the bonus to the stated position tolerance.
What does true position at MMC mean?
It means the stated tolerance applies when the feature is at its maximum material condition, the smallest hole or largest pin, and grows as the feature departs from that size. A bigger hole can sit further off and still clear its mating bolt.
Is true position radial or diametral?
The tolerance in the feature control frame is diametral when it starts with Ø. Some measuring machines report radial deviation, the plain distance from true position; double it before comparing it with the tolerance.
Can true position be calculated in 3D?
Yes. When the tolerance zone is spherical, written SØ, the formula adds the third axis: 2 × √(ΔX² + ΔY² + ΔZ²). Most position callouts on holes are cylindrical, so only X and Y count.
Does the same formula work for ISO drawings?
Yes. ISO 1101 uses the same position symbol and a round tolerance zone for a Ø value, and ISO 2692 gives the Ⓜ requirement, so the calculation is the same. Only the default rules for size and form differ between the standards.
Have a drawing of the part but no CAD model?
Upload the drawing to Drawing to STEP: a PDF, PNG or JPG becomes a 3D STEP model, with files from $29.99. The model puts each hole at its true position; keep the drawing with it, because the drawing carries the tolerances.