Maximum material condition (MMC) is the size at which a feature holds the most material: the smallest allowed hole or the largest allowed pin. A circled M after a geometric tolerance means that tolerance applies at MMC and grows, as bonus tolerance, as the feature is made away from MMC. That bonus is what makes MMC the usual choice for parts that just need to assemble.
The idea is simple. A hole at its smallest size is the hardest case for a bolt to pass through, so that is where location must be tightest. Make the hole bigger and it can sit further off-centre while still clearing the same bolt. MMC writes that into the tolerance: bonus = how far the actual size is from MMC.
For a hole, MMC is the lower size limit. For a pin or shaft, MMC is the upper size limit. Write it down before you calculate anything; mixing them up is the commonest error.
MMC also defines the virtual condition, the worst-case boundary that a mating part must clear. For a hole it is MMC size minus the geometric tolerance; for a pin it is MMC size plus the tolerance. That boundary is what a functional gauge pin or ring is made to.
MMC does not create a new zone shape. It changes the size of the zone of the control it modifies, usually position, perpendicularity or axis straightness.
The chart shows the result for a Ø10.0–10.2 hole with position Ø0.1 at MMC: allowed tolerance rises one-for-one with hole size, from Ø0.1 at 10.0 to Ø0.3 at 10.2.
MMC is a modifier, not a control, so it has no datum of its own. When a datum feature of size is referenced with a circled M (shown after the datum letter), it means the datum applies at its maximum material boundary (MMB) and the part may shift on it, giving extra movement called datum shift.
| Modifier | With maximum material condition (mmc) |
|---|---|
| Applies to | Only features of size: holes, pins, slots, tabs, bosses. Never to plain surfaces. |
| Used with | Position, orientation controls on a feature of size, and straightness or flatness of a derived median line or plane. |
| Not allowed with | Runout, circularity, cylindricity, profile tolerances and surface form controls. |
Example: a Ø10.0–10.2 mm hole with position Ø0.1 at MMC
Result: The hole passes. A Ø9.9 mm functional gauge pin at the true position will enter every hole that passes.
Every GD&T symbol page: GD&T symbols chart
For a hole, MMC is the smallest allowed size. For a shaft or pin, MMC is the largest allowed size. Both are the condition with the most material on the part.
Bonus = the difference between the actual size and the MMC size. Add it to the tolerance in the frame. A Ø10.0–10.2 hole made at 10.15 with Ø0.1 at MMC is allowed Ø0.25.
The worst-case boundary from size plus geometric tolerance at MMC. For a hole: MMC − tolerance. For a pin: MMC + tolerance. Mating parts designed to it always assemble.
Position, orientation controls applied to features of size, and straightness or flatness of a derived median line or plane. Not runout, profile or surface form controls.
The datum feature applies at its maximum material boundary (MMB). If it is made away from that boundary, the part can shift relative to the datum, which adds movement to the controlled features.
COPLAIN AI PLATFORM
Coplain turns bonus tolerance rules into plain inspection steps: measure size, compute the allowance, record the result.
Generate yours automatically with Coplain →Related Tools & Templates