A hole pattern that "looks fine" on the height gauge can still be rejected at the customer's CMM, and a hole that is slightly off can still be a good part. Most of these arguments come down to one line on the drawing: the position tolerance and the little circled M after it. If your team reads that line correctly before quoting and setup, you avoid both needless rework and unpleasant surprises at incoming inspection.

What true position actually means

The true position is the exact theoretical location of a feature, set by basic dimensions (the boxed dimensions with no tolerance) from the datums. As GD&T Basics puts it, it is the exact coordinate "that represents the nominal value". The position tolerance in the feature control frame then says how far the actual axis of the hole or pin may wander from that point.

When the tolerance value has a diameter symbol (Ø) in front of it, the tolerance zone is a cylinder, not a square. This matters on the shop floor:

  • A ±0.1 coordinate tolerance gives a square zone of 0.2 x 0.2 mm.
  • A Ø0.2 position tolerance gives a round zone of 0.2 mm diameter, centred on the true position.
  • The corners of that 0.2 x 0.2 square sit about 0.141 mm from the centre, so the circle that just contains it is about Ø0.28. When a designer converts ±0.1 coordinates to a Ø0.28 position, the shop gets more usable area without the part functioning any worse.

How to calculate position from X and Y readings

The CMM or your layout report will give you the measured X and Y of the hole axis. The deviation from nominal in each direction (Δx, Δy) is converted into a diameter using the formula given by Wevolver:

Position = 2 × √(Δx² + Δy²)

The factor of 2 is there because the formula first finds the radial distance from nominal, and the tolerance on the drawing is a diameter.

For example (illustrative numbers): a hole is 0.06 mm off in X and 0.08 mm off in Y. The radial distance is 0.10 mm, so the position deviation is Ø0.20. Against a Ø0.2 tolerance it is just at the limit.

MMC, LMC and RFS: where bonus tolerance comes from

The modifier after the tolerance value changes everything:

  • RFS (no modifier): under ASME Y14.5, regardless of feature size is the default when no modifier is shown. The position tolerance stays the same whatever the hole size, so there is no bonus.
  • MMC (circled M): maximum material condition is the smallest hole or the largest pin within its size tolerance. As the feature departs from MMC, the position tolerance grows.
  • LMC (circled L): least material condition is the largest hole or the smallest pin, often used to protect wall thickness.

The rule from GD&T Basics on MMC is simple: bonus tolerance = the difference between MMC and the actual measured size.

A worked example on a bolt hole

Take this callout (illustrative numbers): hole Ø10.0 +0.2/0, position Ø0.2 at MMC relative to datums A, B and C.

  • MMC of the hole is Ø10.0, so at that size the allowed position is Ø0.2.
  • The hole is measured at Ø10.12. Bonus = 10.12 − 10.00 = 0.12.
  • Allowed position for this hole = 0.2 + 0.12 = Ø0.32.
  • The measured offsets are Δx 0.09 and Δy 0.12, so position = 2 × √(0.0081 + 0.0144) = Ø0.30.
The same hole is a reject if the drawing says RFS and a good part if it says MMC, so read the modifier before you argue with the inspection report.

Note that bonus is calculated from the actual size of that particular hole. Each hole in a pattern gets its own bonus, so record size and location together in the layout report.

Functional gauges and what to clarify before quoting

MMC callouts can be checked with a simple functional gauge. For an internal feature, GD&T Basics gives the gauge pin size as the MMC of the hole minus the position tolerance. In our example that is 10.0 − 0.2 = Ø9.8, which is the hole's virtual condition, the worst-case boundary a mating bolt sees. For volume jobs, a fixed pin gauge on the datum fixture can be quicker than taking every part to the CMM.

Before you quote, check these points on the drawing:

  • Is there a diameter symbol, or is it a square zone?
  • Is the modifier MMC, LMC or blank (RFS)? Blank means no bonus, so plan for tighter process control.
  • Are the datums clear and is the datum order practical for your fixturing?
  • Are all locating dimensions basic? A toleranced dimension combined with position is a conflict to raise with the customer.
  • Is the drawing to ASME Y14.5 or ISO? Ask if it is not stated, because defaults differ.

How SpecReview helps

When you upload a drawing PDF, SpecReview flags unclear GD&T notes, such as a missing modifier or a position callout without clear datums, as spec gaps to clarify before quoting. Its layout inspection plan lists each position and size characteristic so your inspector records the values needed to work out bonus tolerance, and each item is tagged as coming from the spec, the geometry or an assumption.