Which limit is LMC
Least material condition is the size at which the feature contains the least material. Removing metal makes a hole bigger, so for an internal feature LMC is the high limit. It makes a pin smaller, so for an external feature LMC is the low limit. Reading LMC as always meaning the larger number works for holes and fails for every shaft on the drawing.
Once the limit is identified, departure and bonus work exactly as they do at MMC. The departure from LMC and the departure from MMC always sum to the size tolerance, which is a useful check.
What LMC protects
The classic case is a boss or a hole close to the edge of a casting. If the hole grows and moves toward the edge at the same time, the wall between them thins twice over. An MMC modifier would grant more location tolerance exactly when the hole is largest, which is the wrong direction for that failure mode.
LMC reverses it: the tolerance grows as the feature moves away from the least material condition, so the location allowance is smallest exactly when the wall is thinnest. Minimum wall, minimum edge distance and minimum thread engagement are all LMC arguments.
Boundaries at LMC
The virtual condition of an internal feature at LMC is the LMC size plus the tolerance, because the worst case there is the largest space the hole can consume. For an external feature it is the LMC size minus the tolerance. Both are the opposite direction from the MMC case, for the same reason the limits themselves are opposite.
That boundary is what a wall thickness calculation must clear. Using the MMC boundary instead answers a fit question nobody asked, and it does so with a number that looks entirely reasonable.
Why LMC is harder to verify
A functional gauge realises an MMC boundary directly: a pin at the virtual condition size either enters the hole or it does not. The LMC boundary sits on the other side of the material, where no simple fixed gauge can sit.
In practice LMC requirements are verified by measuring the produced size and the location and computing the allowance, which is a coordinate measuring task rather than a go and no go one. That is a real cost, and it is worth spending only where minimum material genuinely governs.
The same hole under both modifiers
A hole toleranced diameter 9.00 to 9.30 mm is produced at 9.18 mm. The two modifiers grant different bonuses from the same measurement.
- Bonus if the frame says MMC
- 0.180 mm
- Bonus if the frame says LMC
- 0.120 mm
- Sum of the two departures
- 0.300 mm
- Size tolerance of the hole
- 0.300 mm
The two departures add to the size tolerance, always. If your two numbers do not, one of them has taken its reference from the wrong limit, and that is worth catching before either reaches a report.