Why the answer is a diameter and not a distance
The axis of a hole can wander in any direction, so the natural zone for it is a cylinder rather than a pair of planes. The drawing states the diameter of that cylinder, which means the measured radial offset of the actual axis has to be doubled before the two numbers can be compared. Radial offset is sqrt(X squared plus Y squared), and true position is twice that.
Comparing a radius against a diameter is the single most common arithmetic error in position work, and it is dangerous in the direction that matters: it makes every feature look twice as good as it is. If a report lists a value that is suspiciously close to half the tolerance on every feature, check which quantity is being reported before congratulating the process.
Basic dimensions define the zone, the frame carries the tolerance
True position only exists once the location is stated with basic dimensions, drawn in a box and carrying no tolerance of their own. All the permitted variation lives in the feature control frame. A drawing that locates a hole with toleranced dimensions and then applies a position tolerance has defined a zone that is itself free to move, and two inspectors can reach two different verdicts on the same part without either being wrong.
The same rule explains why a position tolerance cannot be converted into a coordinate tolerance without losing something. The circular zone reaches into the corners that a square zone rejects, which is roughly fifty seven percent more usable area for the same worst case error.
What regardless of feature size means
An unmodified tolerance compartment means the stated tolerance applies at every produced size. A hole made close to its upper limit gets no more location tolerance than one made at its lower limit. This is the strictest of the three material condition options and the right choice when location matters for its own sake, such as a dowel that positions one casting against another.
Under this default the control is on the derived median line of the feature, so a hole that is bent or tapered can present an acceptable entry point and still fail. That is a real difference from the boundary interpretation a fixed gauge realises, and it is a reason to measure rather than to gauge when the drawing says nothing about material condition.
Reading the result like a process owner
Two numbers make a position result useful: the value itself and the allowance it was judged against. Their ratio is the fraction of the zone consumed, and it is the early warning a pass or fail verdict throws away. A pattern sitting at nine tenths of its zone is passing today and will fail after the next tool change.
Record the signed deviations as well. The magnitude tells you whether the part is good; the direction tells you what to adjust, and it is the only thing that says whether an available datum shift would have helped.
A hole 0.06 mm off in X and 0.08 mm off in Y
A hole toleranced diameter 10.00 to 10.20 mm carries a position tolerance of diameter 0.25 mm with no modifier. It is produced at 10.12 mm and measured 0.06 mm off in X and 0.08 mm off in Y.
- Radial offset of the actual axis
- 0.100 mm
- True position, as a diameter
- 0.200 mm
- Stated tolerance
- 0.250 mm
- Bonus tolerance earned
- 0.000 mm
- Total allowed
- 0.250 mm
- Fraction of the zone used
- 80 percent
The bonus is zero even though the hole is 0.12 mm above its smallest size, because the frame carries no modifier. That single fact is worth more than the rest of the arithmetic: departure from a limit is only an allowance when the drawing says so.