Article — True Position Calculator (GD&T)
True Position Calculator — GD&T Position Tolerance per ASME Y14.5
True position is the GD&T tolerance that defines a cylindrical zone around the theoretically exact location of a feature, usually a hole or pin. The formula is TP = 2 × √(Δx² + Δy²) — the factor of 2 converts radial deviation into the diameter of the zone.
True position replaces the older plus/minus dimensions for locating features. The change matters because a plus/minus tolerance creates a square zone — and the corners of a square are farther from the center than the sides. A 0.10 mm plus/minus tolerance allows 0.1414 mm error at the corners but only 0.10 mm on the axes. GD&T position uses a circular zone that is uniform in every direction, saving tolerance for actual function.
What is true position
True position is a callout on engineering drawings (per ASME Y14.5 and ISO 1101) that defines where a feature must lie relative to a datum reference frame. The feature control frame looks like a small grid with a target symbol, the tolerance value (a diameter), and a stack of datum letters (primary, secondary, tertiary).
The feature passes inspection if its center axis lies inside a cylindrical tolerance zone of the specified diameter, centered on the basic (theoretically exact) location. Basic dimensions are usually shown in boxes on the drawing and are not tolerated themselves — they are the ideal, and the position tolerance defines how close to that ideal the part must come.
The true position formula
For a 2D position (X-Y plane): TP = 2 × √((x_actual − x_nominal)² + (y_actual − y_nominal)²). The factor of 2 is the most-forgotten part of the calculation — students often report TP as the radial deviation rather than the diameter. The drawing specifies a diameter; the formula must produce a diameter.
Example: a hole that should be at (10.000, 20.000) is measured at (10.030, 19.960). Δx = 0.030, Δy = −0.040. Radial deviation = √(0.030² + 0.040²) = √(0.0025) = 0.050. True position = 2 × 0.050 = 0.100. If the drawing calls out a 0.10 diameter zone, this hole just barely passes.
The factor of 2 in the true position formula is the single most common GD&T mistake. Beginners report TP as radial deviation (0.050 in the example above), which makes a borderline part look perfect. Always double-check by comparing your result against the printed tolerance — they must be in the same units (diameter).
Cylindrical vs square tolerance zones
A plus/minus dimension creates a square tolerance zone. ±0.05 in both axes allows error from 0 to 0.0707 (the corner of the square) — about 41% more tolerance at the corners than on the axes. The square zone wastes tolerance because the corner positions are usually not functionally important; the part still mates whether the hole is off in X, Y, or diagonally.
True position uses a cylindrical zone — circular in 2D — that is uniform in every direction. A 0.10 diameter zone allows 0.05 error in any direction. The numerical value looks tighter than plus/minus, but the functional tolerance is similar to ±0.05 because the corner cases are eliminated. Most companies allow a slightly larger numerical value (e.g., 0.14 diameter ≈ ±0.05 square) for the same fit.
MMC and bonus tolerance
The Ⓜ (M-circled) modifier in a feature control frame applies the position tolerance only at maximum material condition. A 10 mm hole has MMC = 9.9 mm (smallest, most material), LMC = 10.1 mm (largest, least material). If the position tolerance is 0.10 at MMC, that 0.10 is mandatory only when the hole is at its smallest.
As the hole grows toward LMC, bonus tolerance equal to the size deviation becomes available. A hole measured at 10.0 mm gets 0.10 bonus on top of the 0.10 baseline = 0.20 total. A hole at LMC (10.1 mm) gets 0.20 bonus = 0.30 total. The principle: a bigger hole gives more room for the bolt, so positional accuracy can be looser.
MMC bonus turns a tight 0.10 callout into an effective 0.20-0.30 mm of usable position tolerance when the part is at LMC. This is a free gift for the shop — manufacturers love MMC modifiers because they reduce the cost of meeting position specs.
True position datum references
A position tolerance has no meaning without datums. The feature control frame lists primary, secondary, and tertiary datums (usually labeled A, B, C) in priority order. The part must first be aligned to A (usually a flat reference surface), then constrained by B (a perpendicular surface or edge), then by C (the final orientation reference).
Datum order matters. A position tolerance "0.10 |A|B|C" means the part is leveled against A, then rotated against B, then translated against C — in that exact sequence. Reversing the order changes which inspection measurements pass and fail. The drafter should specify datums based on how the part actually mates in assembly, not arbitrarily.
Measuring true position
A coordinate measuring machine (CMM) is the standard tool. The operator establishes the datum reference frame by probing the reference surfaces, then probes the feature (usually 4-8 points around a hole) to fit a cylinder or center point. The CMM software reports the deviation from the basic coordinates and multiplies by 2 to give the diameter, which is compared directly against the print tolerance.
For low-volume or shop-floor inspection, fixed gauges (functional gauges) replicate the worst-case mating part. If the part fits over the gauge pin (size = MMC bolt − position tolerance), it passes. Functional gauging is faster than a CMM but gives only pass/fail, not the actual deviation value.
Common true position mistakes
The most common error is forgetting the factor of 2 — reporting TP as the radial deviation rather than the diameter. The second most common is applying MMC bonus when the modifier is not on the print. RFS (Regardless of Feature Size, the default) gets zero bonus regardless of actual size.
The third most common: using the wrong datum frame. Two different inspection setups can give two different TP values for the same physical part, simply because they leveled and rotated the part differently. Always use the datum order on the print.
- TP formula = 2 × √(Δx² + Δy²), always a diameter
- 0.10 diameter zone = ±0.05 deviation in any direction
- Square zone corners = 41% looser than circular zone of same nominal value
- MMC bonus = |actual size − MMC size|, free tolerance
- Datum order = primary, secondary, tertiary, applied in that sequence
- 3D true position = same formula plus a Δz² term under the radical