← AskMachinist · Guides · Calculator · 🔎 Search

How to Calculate True Position (With MMC Bonus Tolerance)

Guide · Updated October 28, 2026

A position tolerance in GD&T defines a cylindrical zone around the exact (basic) location of a hole. The hole axis must fall inside it. Because the zone is round, you cannot just compare X and Y separately; you combine them into one position value and compare it with the zone diameter, adding any bonus tolerance the material condition modifier allows.

Step by step

1. Read the callout: Note the position tolerance, the modifier (M for MMC, none for RFS) and the datums.
2. Set up on the datums: Locate the part on datum A, B and C as the feature control frame says.
3. Measure the hole center: Find the actual X and Y of the hole axis from the datums with a CMM, height gage with a pin, or DRO and coaxial indicator.
4. Find the deviations: ΔX = measured X − basic X; ΔY = measured Y − basic Y.
5. Calculate position: Position (diameter) = 2 × √(ΔX² + ΔY²).
6. Add bonus if MMC: Bonus = actual hole size − hole MMC size (the smallest allowed hole). Allowed position = stated tolerance + bonus.
7. Compare: The hole passes if the calculated position is no larger than the allowed position.

Worked example 1: a hole that passes

A 0.257 +0.004/−0.000 in hole is located at basic X = 1.000, Y = 0.750 in, with position Ø0.010 at MMC. It measures X = 1.003, Y = 0.7485 in and 0.259 in diameter. ΔX = 0.003, ΔY = −0.0015. Position = 2 × √(0.000009 + 0.00000225) = 2 × 0.00335 = Ø0.0067 in. The bonus is 0.259 − 0.257 = 0.002 in, so the allowed position is Ø0.012 in. The hole passes, and it would pass even without the bonus.

Worked example 2: the bonus saves the part

Another hole measures X = 1.005, Y = 0.753 in, still 0.259 in diameter. ΔX = 0.005, ΔY = 0.003. Position = 2 × √(0.000025 + 0.000009) = 2 × 0.00583 = Ø0.0117 in. That exceeds the stated Ø0.010, so it would fail if the callout were RFS (no modifier). With MMC it gets the 0.002 in bonus, the allowed position is Ø0.012 in, and the hole passes.

Why the factor of 2

ΔX and ΔY give the radius from the true location to the actual axis. The tolerance zone is stated as a diameter, so the radius is doubled. A common mistake is to compare √(ΔX² + ΔY²) directly with the zone diameter, which accepts holes that are twice as far off as allowed. Another is to compare ΔX and ΔY each with half the tolerance as a square zone; a round zone is about 57% larger in area than the square that fits inside it.

Measuring the hole center

On a manual mill, use a coaxial indicator to center on the hole and read the DRO. On a surface plate, put a close-fitting gage pin in the hole and measure to its top and side with a height gage, subtracting half the pin diameter. Check the height gage on a gage block stack at about the same height first. A CMM fits a circle at the hole depth stated by the drawing; for deep holes, the axis tilt can matter as much as the center at the top.

Tips

• GD&T: GD&T basics.
• Height gage: height gage use.
• Bores: indicating a bore.

FAQ

What is the true position formula?

Position = 2 × √(ΔX² + ΔY²), compared with the diametral tolerance.

What is MMC bonus tolerance?

For a hole, the amount the actual size is larger than its smallest allowed size, added to the position tolerance.

Does RFS get a bonus?

No. With no modifier, the stated tolerance applies at any size.

Why multiply by 2?

The zone is a diameter; the deviation is a radius.

How do I measure hole location?

CMM, height gage and pin, or a coaxial indicator and DRO, from the datums.

Related guides and calculators

• GD&T Basics for Machinists
• How to Use a Height Gage for Layout
• How to Indicate a Bore True
• Blueprint Reading Basics for Machinists
• ISO 286 Hole-Basis Fits Explained (H7/g6, H7/h6, H7/k6, H7/p6)
• How to Calculate Press Fit Pressure and Pressing Force
• All free machinist calculators

General shop information only — follow your machine and tooling manufacturer's instructions and your shop's safety rules.