Modifiers and Material Conditions

A feature control frame states what is controlled and how much. Modifiers say when and how the tolerance applies: whether it grows as the feature moves away from its worst-case size, whether it is measured at a plane, in a free state, or on a projection. The most important ones are the material condition modifiers: Ⓜ (maximum material condition, MMC), Ⓛ (least material condition, LMC), and the default of none, which means regardless of feature size (RFS). This page covers all of them with formulas and worked examples. It is part of the GD&T guide and follows ASME Y14.5-2018.

Every modifier and symbol

Symbol	Name	Meaning	Typical use
⌀	Diameter	The zone is cylindrical (a round tolerance zone) instead of a pair of planes	Position or perpendicularity of holes and pins
S⌀	Spherical diameter	The zone is a sphere	The position of a ball center
Ⓜ	Maximum material condition	The tolerance applies at MMC and gains bonus as the feature departs from MMC. Also used on datum features	Clearance fits, fasteners
Ⓛ	Least material condition	The tolerance applies at LMC and gains bonus as the feature departs from LMC	Minimum wall thickness, minimum edge distance
(no symbol)	Regardless of feature size	The tolerance applies at every size, with no bonus. This is the default in ASME Y14.5-2009 and later	Press fits, locating features, runout
Ⓟ	Projected tolerance zone	The zone extends above the surface; the value gives the height	Tapped holes, press-fit pins that carry a mating part
Ⓕ	Free state	The tolerance applies to the part with no restraining forces	Thin, flexible parts such as gaskets and sheet metal
Ⓣ	Tangent plane	The tolerance applies to the plane touching the high points of the surface	Flat surfaces that sit on a mating face
Ⓤ	Unequally disposed profile	The zone is not centered on the true profile; the number after it is the outside part	Profile of a surface
Ⓘ	Independency	Rule #1 (the envelope requirement) does not apply to this size	Features where form is controlled separately
Ⓔ	Envelope	ISO: the envelope requirement applies (the reverse of the ASME default)	ISO drawings that keep the envelope rule
ST	Statistical tolerance	The tolerance may be met by statistical process control	High-volume parts with a capable process
CF	Continuous feature	Features that are physically separate are treated as one	A split or interrupted shaft
4X, 6 HOLES	Number of places	The frame applies to that many identical features, each on its own	Hole patterns
SIM REQT / SEP REQT	Simultaneous / separate requirement	Several frames with the same datums are checked together or on their own	Patterns and two-frame callouts
[ 25 ] (boxed)	Basic dimension	The exact theoretical value; its tolerance comes from the frame	Locating a feature or defining a true profile
( 25 )	Reference dimension	For information only	Overall sizes and conversions

MMC, LMC and RFS

Every feature of size has two extreme sizes, and the one that leaves the most material is its maximum material condition; the one that leaves the least is its least material condition.

Feature	MMC (most material)	LMC (least material)
External: a pin, shaft or boss	The largest size (upper limit)	The smallest size (lower limit)
Internal: a hole or slot	The smallest size (lower limit)	The largest size (upper limit)

Modifier	Where the stated tolerance applies	Bonus tolerance	Use it when
Ⓜ (MMC)	When the feature is at its MMC size	Yes: equal to how far the size departs from MMC	The feature has to fit something (a bolt through a hole). Clearance matters, not exact position
Ⓛ (LMC)	When the feature is at its LMC size	Yes: equal to how far the size departs from LMC	The feature must not break through or leave too little material (wall thickness, edge distance)
RFS (no symbol)	At every size	None	The position or alignment must be controlled exactly, whatever the size (press fits, bearings, balance)

Bonus tolerance (MMC) = |actual size − MMC size|
Total tolerance = stated tolerance + bonus

Virtual and resultant condition

The boundary a feature must stay inside is the virtual condition: the combined effect of its size and its geometric tolerance at the worst case. A gage built to the virtual condition checks every part at once. The opposite, the worst case on the other side, is the resultant condition.

Virtual condition, external feature (pin) at MMC: VC = MMC size + geometric tolerance
Virtual condition, internal feature (hole) at MMC: VC = MMC size − geometric tolerance
Resultant condition, external: RC = LMC size − (geometric tolerance + the size departure)
Resultant condition, internal: RC = LMC size + geometric tolerance + the size departure

Tolerance versus size

A hole ⌀10.0 to 10.2 with a stated position tolerance of ⌀0.1. The tolerance that is actually available at three different sizes depends on the modifier:

Hole size	RFS ⌀0.1	MMC ⌀0.1 Ⓜ	LMC ⌀0.1 Ⓛ
10.0	0.1	0.1	0.3
10.1	0.1	0.2	0.2
10.2	0.1	0.3	0.1

• RFS never changes: 0.1 at every size.
• MMC grows as the hole gets larger: 0.1, 0.2, 0.3. The extra comes free because a larger hole leaves room for the position error.
• LMC goes the other way: biggest when the hole is smallest (0.3, 0.2, 0.1 as the hole gets larger).

LMC: protecting wall thickness

MMC is for fit; LMC is for strength. Applying Ⓛ to a hole’s position means that the smaller the hole is than its LMC size, the more the hole may move, because a smaller hole leaves more wall. It guards a minimum wall thickness at the thin side.

Projected tolerance zone

A fastener in a tapped hole stands up out of the part, carrying the mating part. If the hole is tilted, the top of the screw is displaced far more than the hole’s own position suggests. The projected tolerance zone (Ⓟ) moves the position zone out of the hole and up to the height of the mating part, so the tolerance is controlled where it matters.

• Frame: the position frame, then Ⓟ, and the projection height is given beside the frame or in a note.
• Height: the thickness of the mating part (plus any washer or gasket) for a bolt, or the length of a pin above the surface.
• Use: tapped holes, press-fit pins and dowels. See the Position and Location page for a full worked example.

Tangent plane, free state, independency

Modifier	What it does	Example
Tangent plane Ⓣ	The flatness or orientation tolerance applies to the plane touching the high points of the surface, not to the surface itself. A bumpy face that sits flat on a mating part passes	Perpendicularity 0.1 Ⓣ to A: the tangent plane, found with a surface plate, must be square
Free state Ⓕ	The part is measured with no clamping or restraint. Flexible parts spring out of shape when clamped, so the tolerance may need to be met in the free state, then again when restrained	A thin ring: circularity 1.0 Ⓕ; restrained, 0.2
Independency Ⓘ	Cancels Rule #1: size and form are checked separately. A part may then exceed the perfect-form envelope at MMC	A flexible part whose form is controlled by its own frame
Envelope Ⓔ (ISO)	ISO 8015 default is independency; Ⓔ asks for the envelope requirement	An ISO drawing that wants a perfect-form boundary

Statistical tolerance and continuous feature

Statistical tolerance (ST). A tolerance marked ST may be met by statistical process control rather than by every part. It lets a wider tolerance be used in a stack-up because the likelihood that all parts are at their extreme is small. It requires a process in control and is used with caution; see the Inspection and Tolerance Stack-up page for RSS and worst case.

Continuous feature (CF). When a feature of size is made of several parts that are physically separate (a shaft with an interrupted groove, or two coaxial bores separated by a web), CF in the frame tells the reader to treat them as one feature. It saves writing “2 SURFACES” or putting a common datum on each.

Worked examples

Example 1: MMC bonus on a pattern

Four holes ⌀6.0 to 6.2 have position ⌀0.2 at MMC to A | B | C. A part is measured at ⌀6.15 with an axis 0.14 from true position (a diametral zone of 0.28).

• Bonus = 6.15 − 6.0 = 0.15.
• Total tolerance = 0.2 + 0.15 = 0.35.
• The axis is 0.14 from the true position, so it is using a diameter zone of 2 × 0.14 = 0.28, which is inside the available 0.35. Pass. Without the modifier (RFS) the same hole would be allowed only 0.2 and would fail.

Example 2: MMC on the datum feature

A pattern is located to a datum B at MMC (Ⓜ on the datum reference). B is a bore ⌀20.0 to 20.1 with a form tolerance of 0.

• The datum feature is simulated by a gage at its virtual condition. Since B’s MMC is 20.0 (smallest hole) and its geometric tolerance is 0, the simulator is a fixed ⌀20.0 pin.
• When the bore is at ⌀20.1 it can move 0.1 around the pin (shift), so the pattern may shift by up to 0.1 in addition to its own tolerance.
• The shift is not free: it is allowed because the part clears the pin. That is why datum modifiers in the frame reduce inspection cost: a fixed pin gage is enough.

Example 3: choosing RFS for a press fit

A bearing seat is ⌀25.000 to 25.021 and must be coaxial with a shaft datum A to 0.02. Why not use MMC?

• With a press fit the part does not float: bonus tolerance would let the bearing sit off-axis on a seat that is larger than its minimum.
• The axis must be where it is, whatever the size, so the position is RFS (no modifier) and measured with a CMM or a runout fixture.
• The rule: if the mating part can move, use MMC; if it is clamped, pressed or must stay exactly aligned, use RFS.

Troubleshooting

Symptom	Likely cause	Try
Parts assemble in some batches and not others	Position is RFS but the fit needs MMC	Put Ⓜ on the position and on the datum features that float
Gage accepts, CMM rejects the same part	The CMM is not applying bonus	Enter the modifier; calculate the tolerance from the measured size
Walls crack at a drilled hole	MMC lets the hole drift toward an edge as it gets larger	Use LMC (Ⓛ) on the position, or add an edge-distance control
Tilted screws cause the mating part not to fit	The position zone is only in the tapped part	Add the projected tolerance zone Ⓟ at the mating part’s thickness
A thin part fails when measured clamped	The part changes shape under restraint	Specify free state (Ⓕ) and a restrained tolerance

Related

• GD&T: the overview and quick reference.
• Position and Location: MMC and bonus on patterns, and fastener formulas.
• Datums and Datum Reference Frames: material condition on datum features and datum shift.
• Form Tolerances: Rule #1 and the envelope.
• Inspection and Tolerance Stack-up: functional gages at virtual condition.

FAQ

Is MMC always the smaller size?

No. For a hole it is the smallest size, because that leaves the most material. For a pin or boss it is the largest size.

Is “regardless of feature size” still written as a symbol?

Not in ASME Y14.5-2009 and later: it is the default, so no symbol is needed. The older circled S symbol is not used.

Can I use MMC with flatness or straightness of a surface?

No. Material condition modifiers apply to features of size (holes, pins, slots, tabs). A flat surface has no size, so a modifier makes no sense.

What is the difference between virtual condition and MMC?

MMC is the size limit. Virtual condition combines that limit with the geometric tolerance, so it is the real boundary the feature must stay inside.

When should I use LMC?

When you must keep a minimum wall or edge distance, or a minimum thickness of material around the feature, or to keep a part from breaking through.

Does bonus tolerance apply to a datum feature?

A datum feature modified with Ⓜ or Ⓛ gains “datum shift”: the pattern may move as the datum feature departs from its material condition. See the datums page.

Do ISO and ASME treat modifiers the same way?

Mostly. ISO 2692 defines Ⓜ, Ⓛ and the reciprocity requirement Ⓡ. The default size and form relationship differs (ISO 8015 independency versus ASME Rule #1).

References

• ASME Y14.5-2018, Dimensioning and Tolerancing (material condition modifiers, virtual and resultant condition, projected tolerance zone, tangent plane, free state, statistical tolerance, continuous feature).
• ISO 2692, Geometrical product specifications: Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR).
• ISO 8015, Fundamentals: concepts, principles and rules.
• Meadows, J. D., Geometric Dimensioning and Tolerancing: Applications, Analysis, Gaging and Inspection, CRC Press.

Last reviewed: October 2026. Check the symbols and rules against the edition your drawing names.