This article is part of the CNC Tolerances & Quality Control Guide: GD&T, CMM, Cpk, PPAP on CNX Precision.
In precision assembly, location controls everything. When holes, bosses, and slots miss their intended coordinates, fasteners bind and parts fail to fit. The positional tolerance MMC callout solves this problem directly on engineering drawings. It fixes where a feature must sit and, through the maximum material condition modifier, grants additional allowable error as the feature departs from its tightest material state. This guide explains what position tolerance controls, how bonus tolerance accumulates, and how design and manufacturing teams apply these rules correctly.
What Position Tolerance Controls
Position tolerance defines where a feature of size must sit relative to datums. The drawing states basic dimensions from datum planes or axes to the true position of the feature. Around that true position, the tolerance builds a zone inside which the derived axis of the feature must fall. For a round hole, the zone is a cylinder whose diameter equals the stated tolerance value, which is why the feature control frame carries a diameter sign ahead of the number.
Position replaces older coordinate tolerancing because the zone is round rather than square. A square zone lets error accumulate toward the corners, while a cylindrical zone reflects how a fastener actually engages a hole. The same callout can control orientation too when the tolerance zone must stay perpendicular to a datum plane. When applied to a pattern of holes, position keeps both spacing and location of the whole pattern inside one boundary. Datums anchor every measurement, so designers must select them to match how the part locates during assembly, not just how it looks on the page.
How the Maximum Material Condition Modifier Works
Maximum material condition describes the state in which a feature contains the most material within its size limits. For a hole, that means the smallest acceptable diameter. For a pin or boss, it means the largest. When the MMC symbol follows a position tolerance, the stated tolerance applies only at that condition. As the manufactured feature moves away from MMC, the part earns bonus tolerance equal to the amount of departure. That interaction is what separates positional tolerance MMC from a fixed position callout. The combined limit defines the worst case boundary that the feature must never violate if the mating part is to fit.
A simple example shows the math. A drawing calls a hole 10.0 to 10.2 mm in diameter with a position tolerance of 0.2 mm at MMC. At the MMC size of 10.0 mm, the allowable position error is 0.2 mm. If the drilled hole measures 10.2 mm, the feature gained 0.2 mm of bonus, so the allowable position error grows to 0.4 mm. The same logic runs in reverse for external features. A pin at its largest size holds the tightest position zone, and every step below that size adds bonus. Inspectors combine measured size and measured deviation to judge the part, which is why a coordinate measuring machine records both values for every hole it checks.
Applying Positional Tolerance MMC on Engineering Drawings
A correct positional tolerance MMC callout lives inside a feature control frame. The frame reads left to right: the position symbol, the diameter sign with the tolerance value, the MMC modifier symbol, then the datum letters in order of precedence. Basic dimensions locate the true position from those datums, and they carry no plus or minus values of their own. Any tolerance riding on the basic dimensions would defeat the scheme, so drafters keep them boxed and clean. It is the first thing our engineers check when a new drawing arrives.
Interpreting the callout follows a fixed sequence. First, establish the datum reference frame from the part features. Second, measure the actual mating size of the feature. Third, compare the measured axis location against the true position. Fourth, add the bonus allowance to the stated tolerance and judge the result. Assembly-focused drawings often add a note that fastener holes are inspected at virtual condition, which pairs the MMC boundary of the hole with its position error into one worst case limit for mating.
Why Bonus Tolerance Helps Fastener Assemblies
Fastener holes exist to receive bolts, pins, or screws. A hole at its largest size already gives the fastener extra clearance, so demanding a tight position zone at that size buys nothing for assembly. Positional tolerance MMC formalizes that logic. It holds the strictest position requirement where the material is tightest and relaxes the requirement exactly in step with the extra clearance the part already gained.
The payoff shows up in production yield. Parts that would fail a fixed coordinate tolerance pass under MMC rules, which lowers scrap without weakening the joint. Yield gains concentrate on the larger hole sizes, which are also the fastest to drill and the gentlest on tooling. Functional gauges reflect the same philosophy. A pin gauge sized to the virtual condition of the hole pattern checks fit in one pass, mirroring how the real fastener behaves. For floating fastener assemblies, where both joined parts carry clearance holes, the bonus approach also supports a shared tolerance split between the two parts. That makes interchangeability practical across suppliers, which matters for any B2B program that sources components from multiple CNC shops.
How CNC Shops Verify Position Requirements
Verification starts with the same data the drawing demands. A coordinate measuring machine probes each hole, records the actual diameter, and reports the position deviation from true position. Software then applies the bonus allowance automatically and flags only the parts that fail the combined requirement. Shops without a CMM can use functional gauge plates for high volume work, since the gauge embodies the worst case boundary directly. Because positional tolerance MMC judgment depends on measured size, calibration of size instruments matters as much as position measurement.
At CNX Precision, we review these callouts before machining begins. Our engineers confirm datum accessibility, check that tooling can hold the required size range, and match the inspection method to the production volume. First article reports list size and position for every controlled hole, so customers trace each measurement back to the drawing. That discipline keeps assembly lines moving and prevents disputes over parts that sit near the limit. Clear data beats opinion when a borderline part comes up for review.
Frequently Asked Questions
How do you calculate bonus tolerance at MMC?
Subtract the MMC size from the actual size for an internal feature. For the 10.0 to 10.2 mm hole example, a hole measuring 10.15 mm earns 0.15 mm of bonus. Add that value to the stated position tolerance to get the total allowable deviation for that individual part.
Can positional tolerance MMC apply to slots and bosses?
Yes. The modifier applies to any feature of size, including slots, bosses, and tabs. For a slot, bonus derives from the width departure from MMC, and the position zone grows accordingly in the controlled directions while the basic dimensions stay fixed.
When should you avoid the MMC modifier?
Avoid it when the feature does not mate with a counterpart, or when wall thickness, balance, or appearance matter more than assembly fit. In those cases, a fixed position tolerance without a modifier gives clearer and safer control of the geometry.
For related information, see our guide to tolerance stack-up.