True position is one of the most widely used GD&T (Geometric Dimensioning and Tolerancing) controls in mechanical design — and one of the most misunderstood. If you've ever had a CMM report a true position value and had to decide whether the part passes or fails, this guide is for you. We'll cover what true position measures, how to calculate it from coordinate deviations, and how bonus tolerance at MMC and LMC changes the picture.
What True Position Controls
True position is a location control. It defines how far the actual center of a feature — a hole, a pin, a slot — is allowed to deviate from its theoretically exact (true) position as defined by basic dimensions on the print.
Unlike a ±0.010" coordinate tolerance, which creates a square tolerance zone, true position creates a cylindrical (or circular) tolerance zone centered on the true position. This is more equitable — a hole can be off equally in any direction, not just along the X or Y axis — and it directly reflects whether the feature will assemble with its mating part.
The position tolerance is expressed as a diameter (⌀) in the feature control frame. A callout of ⌀0.010" means the feature's axis must fall within a cylinder of 0.010" diameter centered on the true position.
Calculating True Position from Deviations
When you measure a hole on a CMM, you get an actual X and Y coordinate (and Z if it's a 3D control). To find true position, you calculate the straight-line distance from the measured center to the true position center, then double it to express it as a diameter.
Where ΔX and ΔY are the deviations from the true position in X and Y.
True position callout: ⌀0.020" (no modifier — RFS)
Measured hole center: X = +0.007", Y = −0.005" from basic position
TP = 2 × √(0.007² + 0.005²) = 2 × √(0.000049 + 0.000025) = 2 × √0.000074 = 2 × 0.0086 = 0.0172"
0.0172" < 0.020" → PASS
True position callout: ⌀0.010"
Measured deviation: ΔX = +0.006", ΔY = +0.006"
TP = 2 × √(0.006² + 0.006²) = 2 × √0.000072 = 2 × 0.00849 = 0.0170"
0.0170" > 0.010" → FAIL — even though each individual deviation is only 0.006"
Note: A ±0.007" coordinate tolerance zone would have passed this part. True position correctly catches the diagonal deviation.
Material Condition Modifiers
The feature control frame for true position can include a material condition modifier: MMC (Maximum Material Condition), LMC (Least Material Condition), or nothing (which defaults to RFS — Regardless of Feature Size). The modifier dramatically affects how the tolerance is applied.
RFS — Regardless of Feature Size
The stated tolerance applies regardless of the actual size of the feature. No bonus tolerance is earned. The calculated true position must simply be less than or equal to the stated tolerance zone diameter. This is the strictest interpretation and is the default when no modifier is shown.
MMC — Maximum Material Condition
MMC is the condition where the feature contains the most material: smallest hole (internal feature) or largest pin (external feature). When the part is at MMC, it gets the stated tolerance — the tightest allowance. As the feature departs from MMC toward LMC, it earns bonus tolerance equal to the size departure.
For internal features (holes): Bonus = Actual Diameter − MMC Diameter
Hole: ⌀0.500" +0.010" / −0.000" (so MMC = 0.500", LMC = 0.510")
Position callout: ⌀0.010" ⓜ (at MMC)
Measured actual hole diameter: 0.506"
Bonus tolerance = 0.506 − 0.500 = 0.006"
Total allowed position tolerance = 0.010 + 0.006 = ⌀0.016"
Measured TP = 0.014" → 0.014" < 0.016" → PASS (would have failed at RFS)
The rationale for MMC is assembly-based: a larger hole has more clearance to accommodate positional error and still accept a mating fastener. MMC is the most common modifier for bolt-circle and fastener holes because it directly maps to functional assembly requirements.
LMC — Least Material Condition
LMC is the opposite: largest hole or smallest pin. Bonus tolerance is earned when the feature departs from LMC toward MMC. LMC is less common; it's used when wall thickness or material remaining around a feature is the critical concern — for example, a hole near an edge where a thin wall could break through.
Total Tolerance = Stated Tolerance + Bonus
Summary Table
| Modifier | Bonus Earned When… | Used For… |
|---|---|---|
| RFS (default) | Never — no bonus | Strict location control, no assembly dependency |
| MMC ⓜ | Hole grows larger (or pin gets smaller) | Assembly clearance — fastener holes, bolt circles |
| LMC ⓛ | Hole gets smaller (or pin grows larger) | Wall thickness, edge distance control |
Practical Tips for the Shop
Basic Dimensions Are Not Toleranced
The location of the true position on the print is defined by basic dimensions — dimensions shown in a box (e.g., ⬜1.500). Basic dimensions are theoretically exact. They have no direct tolerance — all the location tolerance is captured in the position feature control frame. Don't add your own tolerance to basic dimensions.
What Datum Reference Matters
True position is always measured from a datum reference frame. Make sure your CMM setup (or fixture) establishes the same datum planes the print specifies, in the same order. A datum reference of A|B|C means primary datum A is established first, then secondary B, then tertiary C. Setting up in a different order changes the measurement results.
Converting from Coordinates to True Position Quickly
In the shop, you can estimate on the fly using the shortcut that TP ≈ 2.83 × the larger of |ΔX| or |ΔY| when both deviations are roughly equal — but always use the actual formula for any documented accept/reject decision. The Machinist Helper measurement calculator handles this automatically.
Summary
True position is a cylindrical tolerance zone centered on the theoretically exact location defined by basic dimensions. You calculate it from coordinate deviations using TP = 2√(ΔX² + ΔY²). When the callout includes MMC or LMC, the effective tolerance zone grows as the feature departs from that material condition — giving you bonus tolerance that reflects real-world assembly function. When there's no modifier, RFS applies and the stated tolerance is absolute. Get the datum setup right, use the formula correctly, and true position is a straightforward pass/fail call.