Chapter vi · Material Condition & Location
There is a way to make your tolerance grow — for free — the moment you start cutting metal. Most people leave that money on the table.
Two identical shops drill the same thousand brackets. One scraps forty; the other ships all thousand — and the only difference on the drawing is a single circle drawn around one letter. Every feature of size lives between two limits. The one with the most material is maximum material condition — MMC. The one with the least material is least material condition — LMC. That sounds simple until you notice the trap: for a hole, most material means the smallest diameter; for a pin, it means the largest. Internal and external features invert.
So MMC is emphatically not "the maximum dimension." It is the maximum metal. A 10.0 mm hole at MMC is the tightest hole the drawing allows; drill it bigger and you have removed material, departing toward LMC.
Hole · internal
MMC = smallest ⌀
Pin · external
MMC = largest ⌀
By default — ASME Rule #2 — a geometric tolerance applies RFS: regardless of feature size. The zone is the stated value, full stop, whatever the part measures. No circled modifier, no bonus.
But add a circled Ⓜ after the tolerance and the contract changes. Now departing from MMC earns you tolerance. The amount is exactly the departure:
bonus = |actual size − MMC| total tol = geometric tol + bonus The logic is purely physical. A hole drilled bigger than MMC has extra clearance around the bolt that will pass through it. Our bracket's clearance hole, drilled 0.1 over its smallest size, has 0.1 of extra slack around the bolt — and that slack is exactly what lets the hole sit 0.1 further off-centre and still drop onto the mating plate's stud. That clearance is slack you can spend on location instead — so the standard refunds it as permission to sit further off-centre. The Ⓜ is the designer saying, in one glyph, "you may keep the change."
Position, RFS (default)
⌀0.2 — always, at any size.
Position at MMC
⌀0.2 plus whatever you depart from MMC.
Drive it yourself. Slide the feature size from MMC toward LMC, flip the modifier on and off, and watch the position cylinder grow — or stay frozen.
- stated tol
- ⌀0.20
- bonus
- +0.00
- total tol
- ⌀0.20
- good parts a ±-only shop scraps
- 0/1000
Notice what the readout calls out: every part sitting in that grown ring is a good part — it fits, it assembles — that a fixed-tolerance shop would scrap for no functional reason. Under RFS that bonus column reads zero, and those parts go in the bin. That is the money on the table. One machinist called the rejected bin "the honest pile" — every part in it would have bolted up fine; it failed a number, not a function.
Datum shift: bonus for the reference, too
The same idea extends to the datums a control references. Put an Ⓜ after a datum letter — ⌀0.2 Ⓜ A B Ⓜ C — and that datum feature, when it departs from its own MMC, allows the whole pattern to shift relative to the datum. It is bonus tolerance for the relationship rather than the located feature: more refunded permission, paid for by clearance somewhere else in the stack.
For the advanced reader → The constant boundary the bonus is really tracking
Bonus is not magic accounting — it is the shadow of a single fixed boundary. Add the geometric tolerance to MMC (for a pin) or subtract it (for a hole) and you get the virtual condition: the one worst-case size a functional gauge is built to. As the feature departs from MMC, its location may wander by exactly enough to keep it inside that constant boundary — which is why the permitted location grows linearly with the departure. The bonus is the room the virtual condition leaves you.
That constant gauge boundary is the whole subject of the next chapter; here it is enough to see that bonus and virtual condition are two readings of one number.
Earn the Bonus
A hole is dimensioned ∅10.0–10.4. Which size is its MMC?
That hole carries position ∅0.2 Ⓜ. A part measures ∅10.3. What is the total position tolerance allowed?
Same hole, but the frame has NO modifier — just position ∅0.2 to A B C. The part measures ∅10.3. What position tolerance applies?
Bonus tolerance is the moment GD&T stops feeling like a rulebook and starts feeling like an economy. A drawing that knows how a part is used can hand back tolerance the instant the metal allows it — and a shop that reads the Ⓜ keeps parts the next bench throws away.
The grammar was never about being strict. It was about being honest with the clearance you already paid for.
Bonus tells you how much you may be off. A gauge tells you whether you actually fit. Chapter vii — position, and the gauge that proves it.