True position is the most commonly specified GD&T (Geometric Dimensioning and Tolerancing) control on machined parts. It defines a cylindrical tolerance zone centered on the theoretically exact location of a feature. Unlike +/- coordinate tolerances, true position allows the full extent of positional error in any direction — and it can be calculated from simple coordinate measurements. This guide explains what true position means, how to calculate it, and how to apply it in practice.
True position defines a cylindrical tolerance zone whose axis is centered on the theoretically exact (basic) location of a hole or feature. The actual feature axis must lie within this cylinder. The diameter of the tolerance zone is specified on the drawing. A callout of ⌀0.010" true position means the hole center must fall within a circle 0.010" in diameter centered on the nominal location. This is different from ±0.005" in both X and Y, which creates a square tolerance zone 0.010" on a side. A circular zone is actually larger in the diagonal direction — a hole can be further from nominal at 45° than at 0° or 90° with ±0.005" tolerances.
True Position = 2 × √(ΔX² + ΔY²). Where ΔX = actual X position − nominal X position, and ΔY = actual Y position − nominal Y position. The factor of 2 converts the radial deviation (distance from nominal) to a diameter — matching the convention that the tolerance zone is specified as a diameter. Example: Nominal position (0.500", 0.750"). Actual position (0.508", 0.743"). ΔX = 0.008", ΔY = −0.007". True Position = 2 × √(0.008² + 0.007²) = 2 × √(0.000064 + 0.000049) = 2 × √0.000113 = 2 × 0.01063 = 0.0213". If the tolerance is ⌀0.020", this hole is OUT of tolerance (0.0213 > 0.020).
True position tolerances are often modified with Maximum Material Condition (MMC), shown as the circled M symbol. MMC means the tolerance zone grows as the feature departs from its maximum material condition (smallest acceptable hole). This provides bonus tolerance equal to the actual size deviation from MMC. Example: A ⌀0.500" hole with ±0.005" size tolerance (MMC = 0.495"). True position tolerance = ⌀0.010" at MMC. If the actual hole measures 0.503" (0.008" above MMC), the bonus tolerance is 0.008". Actual allowed true position = 0.010 + 0.008 = 0.018". MMC callouts are common on bolt holes where the clearance between bolt and hole provides functional tolerance.
Method 1: CMM (Coordinate Measuring Machine). The CMM measures the actual hole center coordinates referenced to the datums specified in the callout. This is the most accurate and traceable method. Method 2: Manual measurement with gauge pins. Measure the distance from a datum surface to the hole center in X and Y using precision measurement tools. Apply the true position formula. Method 3: Go/No-Go functional gauges. A gauge pin of the specified true position size physically checks the tolerance zone. Fast for production but does not provide numerical data. For most machining operations, the shop calculates true position from X/Y deviations measured from a datum edge or machined reference surface.
1) Fixturing: If the part is not properly referenced to the datum surfaces, all holes will be systematically offset. Check datum contact before starting. 2) Tool runout: A drill or boring bar with runout produces holes offset from the programmed path. Check and correct runout before precision hole operations. 3) Thermal growth: CNC machines grow as they warm up. For tight tolerances, run warm-up cycles and verify datum dimensions before cutting. 4) Chip packing in blind holes: Chips in the bottom of a blind hole push the drill off-center. Use peck drilling with chip clearing retract cycles. 5) Worn toolholders: Worn collets or endmill holders contribute runout that accumulates with cutting forces.
True position controls the location of a feature relative to datum reference planes. Concentricity controls the location of a feature's axis relative to a datum axis — it requires that the median points (not just the axis) of the feature lie within a cylindrical tolerance zone. Concentricity is difficult to measure and rarely used in modern GD&T. For most applications where you want to control a round feature's location relative to another round feature, use runout or position with an axis datum instead.
A circular tolerance zone correctly represents the functional requirement for holes: what matters is the radial distance from nominal, not the X and Y deviations separately. A square ±0.005" tolerance zone allows a diagonal deviation of 0.0071" (√2 × 0.005) — 41% more than the stated tolerance. This over-rejects parts that actually function correctly in the diagonal direction, and can under-reject parts near the corners. True position with a circular zone is more precise and less ambiguous.
Yes. A ±X tolerance and ±Y tolerance of equal value converts to a true position tolerance of approximately 2.83× the ± value (2 × √2 × ±value). Example: ±0.005" in X and Y = ⌀0.014" true position (inscribed circle in the square zone). However, you should always use the actual functional requirement to specify tolerance, not convert from legacy ± dimensions. True position with a tighter number is functionally equivalent to the ± callout it replaces.