True Position Calculator

True position = 2 × √(ΔX² + ΔY²), where ΔX and ΔY are the measured deviations from the nominal target in X and Y. If you have coordinates rather than deviations, ΔX = measured X − nominal X. For 3D true position (including the Z-axis), the formula extends to 2 × √(ΔX² + ΔY² + ΔZ²). The result is a diametrical value that you compare directly to the Ø tolerance in the feature control frame.

MMC bonus tolerance is additional position tolerance earned when a feature’s actual size deviates from its Maximum Material Condition. For a hole at MMC (smallest allowable diameter), bonus = actual hole diameter − MMC diameter. A 10.0 mm MMC hole that actually measures 10.2 mm earns 0.2 mm of bonus tolerance. Combined with the stated position tolerance, the total allowed can be substantially larger than the number printed in the feature control frame. Bonus tolerance under MMC is the single most cost-reducing concept in GD&T for CNC machined parts.

RFS (Regardless of Feature Size, no symbol in the feature control frame) means the position tolerance is fixed, the feature gets no bonus regardless of its actual size. MMC (Maximum Material Condition, Ⓜ symbol) awards bonus tolerance when the feature deviates from its maximum-material extreme: a hole larger than MMC, or a shaft smaller than MMC. LMC (Least Material Condition, Ⓛ symbol) awards bonus when the feature deviates from its least-material extreme. RFS is the default and most conservative; MMC is the most commonly specified on production parts for cost reduction; LMC is used when minimum wall thickness or edge distance controls the design.

Yes, but you will scrap more parts. ± coordinate tolerancing creates a square zone. GD&T position creates a circular (cylindrical) zone of equivalent functional fit that is about 57% larger in area. A hole that falls in the corner of the square zone, within both ± limits, can still be outside the cylindrical position zone at the same nominal tolerance value. Conversely, GD&T position accepts parts in the corners of its cylindrical zone that would fail ± inspection. GD&T position is the functionally correct callout for assembly-critical features and almost always reduces manufacturing cost compared to equivalent ± tolerances.

A standard CNC machining process can routinely hold position tolerances of Ø0.1 mm (0.004″) to Ø0.2 mm (0.008″) at RFS. With MMC on holes, the bonus tolerance often adds another 0.05–0.15 mm of allowance, making these callouts comfortably achievable in production. Tolerances of Ø0.05 mm (0.002″) and tighter require precision fixturing, temperature-controlled inspection, and in many cases, boring or jig grinding rather than standard drilling, significantly increasing cost. For position tolerances tighter than Ø0.05 mm, consult your machine shop during design to confirm feasibility before releasing the drawing.