FREE TOOL
True Position Calculator (GD&T) with MMC and LMC Bonus
Enter the basic location, the measured location, and the position tolerance from the feature control frame. Add MMC or LMC to include bonus tolerance from the feature's actual size. The calculator shows diametral position, allowed tolerance, and pass or fail.
True position calculator
The percentage shows how much of the allowed tolerance the measured position uses.
| Step | Formula | Value |
|---|---|---|
| X deviation | Δx = 25.03 − 25 | 0.0300 |
| Y deviation | Δy = 39.96 − 40 | -0.0400 |
| Diametral position | ⌀ = 2·√(Δx² + Δy²) = 2·√(0.0300² + -0.0400²) | 0.1000 |
| Bonus tolerance | |actual size − MMC size| = |8.04 − 8| | 0.0400 |
| Allowed position tolerance | 0.1 + 0.0400 | 0.1400 |
Formulas used
- Deviation from true position
- Δx = x_actual − x_basic; Δy = y_actual − y_basic
- Diametral position
- ⌀ position = 2·√(Δx² + Δy²)
- Bonus at MMC
- bonus = |actual size − MMC size|
- Bonus at LMC
- bonus = |actual size − LMC size|
- Allowed tolerance
- allowed = stated tolerance + bonus; pass if position ≤ allowed
Assumptions and limits
- Two-dimensional position of a feature axis or centre, with a cylindrical (diametral) tolerance zone.
- Basic dimensions and measured coordinates are in the same datum reference frame.
- Bonus tolerance uses the actual size you enter. For MMC this should be the actual mating envelope, not a single two-point reading.
- Datum feature shift (mobility from datum features referenced at MMC/LMC) is not included and can add further tolerance.
- A measured size outside its limits is rejected: the feature fails on size before position is considered.
Worked example
An ⌀8.00–8.08 mm hole is located at basic X 25.000, Y 40.000 with position ⌀0.10 at MMC. The CMM reports the hole at X 25.030, Y 39.960 with an actual mating size of ⌀8.040.
| Step | Formula | Value |
|---|---|---|
| X deviation | Δx = 25.03 − 25 | 0.0300 |
| Y deviation | Δy = 39.96 − 40 | -0.0400 |
| Diametral position | ⌀ = 2·√(Δx² + Δy²) = 2·√(0.0300² + -0.0400²) | 0.1000 |
| Bonus tolerance | |actual size − MMC size| = |8.04 − 8| | 0.0400 |
| Allowed position tolerance | 0.1 + 0.0400 | 0.1400 |
Result: Position ⌀0.100 mm against an allowed ⌀0.140 mm: PASS.
How to calculate true position
Position is a diameter, not a distance
A position tolerance of ⌀0.10 defines a cylinder 0.10 wide centred on the true (basic) location. The axis may move up to 0.05 in any direction. Doubling the radial distance, 2·√(Δx² + Δy²), lets you compare the result directly with the tolerance in the feature control frame.
Bonus tolerance at MMC
When the position tolerance carries the MMC modifier, the zone grows as the feature departs from its maximum material size. A hole at MMC is at its smallest; a pin at its largest. Every 0.01 the hole grows beyond MMC adds 0.01 to the allowed position.
This reflects assembly: a larger hole can be further off location and still accept its mating pin.
LMC and RFS
LMC works the other way: the tolerance grows as the feature departs from least material size, which is used to protect minimum wall thickness. RFS (regardless of feature size) means no bonus. The stated tolerance applies whatever the size.
Reporting results
Report the measured position, the bonus, the total allowed, and the percentage used. The CSV export captures all of them with the inputs, ready for an inspection report or FAI form.
Common mistakes
- Reporting radial instead of diametral position. √(Δx² + Δy²) is the radial offset. Position must be doubled before comparing with a ⌀ tolerance.
- Taking bonus when the frame says RFS. Bonus only exists when the feature control frame shows the MMC or LMC modifier.
- Using the wrong size for bonus. Bonus at MMC is based on the actual mating envelope. A caliper reading at one point can overstate the bonus on an out-of-round hole.
- Mixing datum frames. Measured coordinates must be taken in the datum reference frame named in the feature control frame, not in machine or part-zero coordinates.
- Ignoring a size failure. A hole outside its size limits is rejected before position is checked. Extra bonus does not rescue it.
Frequently asked questions
How do you calculate true position?
Subtract the basic coordinates from the measured coordinates to get Δx and Δy, then compute 2·√(Δx² + Δy²). Compare the result with the position tolerance plus any bonus tolerance.
What is bonus tolerance in GD&T?
Extra position tolerance allowed when a feature controlled at MMC (or LMC) departs from that size. It equals the difference between the actual size and the MMC (or LMC) size.
Is the hole MMC its smallest or largest size?
Smallest. Maximum material condition is the state with the most material left in the part: the smallest hole or the largest pin.
Does this calculator include datum shift?
No. Datum feature shift from datums referenced at MMC or LMC depends on the datum features' actual sizes and the pattern, and needs a separate analysis.
Can I use inches?
Yes. Select inches and enter all coordinates, sizes, and the tolerance in inches.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing — position tolerance, MMC/LMC modifiers, and bonus tolerance.
- ISO 1101, Geometrical product specifications (GPS) — Geometrical tolerancing — Tolerances of form, orientation, location and run-out.
- ISO 2692, Geometrical product specifications (GPS) — Geometrical tolerancing — Maximum material requirement (MMR), least material requirement (LMR) and reciprocity requirement (RPR).
Results are computed in your browser from the published formulas named above. They are an engineering aid, not a substitute for the governing standard, your drawing, or your customer's requirements.