A position tolerance in a feature control frame defines a cylindrical zone, centred on the basic location, within which the axis of the feature must lie. "True position" is the shorthand for how far the actual axis is from that basic location, expressed as a diameter so that it compares directly with the zone size on the drawing. If the axis is off by Δx in one direction and Δy in the other, the radial error is √(Δx² + Δy²) and the true position is twice that:[1]
The factor of two is the source of most disagreements between a machinist's coordinate check and a CMM report. A hole that measures 0.003 off in X and 0.002 off in Y feels like it is "within 0.003," but its true position is 0.0072, and against a Ø0.010 zone it has used 72% of the tolerance.
When the feature control frame carries the M modifier, the stated position tolerance applies only when the feature is at its maximum material condition: the smallest hole or the largest pin. As the feature departs from MMC toward its other size limit, the location can be off by that same amount more and the mating part will still assemble, so the position tolerance grows by the departure. That growth is the bonus tolerance.[1][2]
| Feature | MMC size | Bonus at MMC |
|---|---|---|
| Hole or slot (internal) | Minimum size limit | Measured size − minimum size |
| Pin or boss (external) | Maximum size limit | Maximum size − measured size |
The L modifier works the other way, protecting a minimum wall or edge distance: the tolerance applies at least material condition and grows as the feature approaches MMC. With no modifier (regardless of feature size, RFS) the zone is fixed at the stated diameter no matter what size the feature measures. The calculator applies all three.
What the calculator does not do is datum shift: when a datum feature is itself referenced at MMC, the datum can float by its own departure and the whole pattern gains a further allowance. That needs the datum feature's size and modifier, and is left to a full GD&T analysis.
A Ø0.250 through hole, size limits 0.250 to 0.255, is located with a position tolerance of Ø0.010 at MMC. The CMM reports the axis 0.0045 off in X and 0.0030 off in Y, and the hole measures 0.253.
| Step | Value |
|---|---|
| True position = 2 × √(0.0045² + 0.0030²) | 2 × 0.00541 = 0.0108 |
| Against the stated zone alone (RFS) | 0.0108 > 0.010: fails |
| Bonus = measured size − MMC size = 0.253 − 0.250 | 0.003 |
| Allowed = 0.010 + 0.003 | 0.013 |
| Against the bonused zone (MMC) | 0.0108 ≤ 0.013: passes, 83% of the tolerance used |
The same hole drilled at the bottom of its size limit, 0.250, would have no bonus and would be rejected. That is the practical meaning of MMC: a hole cut a little larger buys location tolerance, exactly as much as the mating pin needs.
Older drawings locate holes with ± dimensions, which define a square tolerance zone. A position tolerance defines a circle. The circle that passes through the corners of a ±t square has a diameter of 2√2 × t, about 2.83t; going the other way, the largest square that fits inside a Ø z circle is ±0.354z. Converting a ±0.005 coordinate callout to Ø0.014 position keeps every previously acceptable hole acceptable and adds the corners of the circle, 57% more area, which is why the conversion is a free gift to manufacturing.[1][3]
C&W measures position, bonus, and datum shift on calibrated CMMs and delivers AS9102 first-article reports with the numbers behind every pass.