True position calculator

Paste the X/Y and size readings for one hole or a whole pattern from your CMM report. You get each feature's true position, its MMC or LMC bonus tolerance, the tolerance it is allowed, pass or fail, and the virtual condition a functional gauge would be made to. Free, no sign-up, and nothing you type leaves your browser.

ASME Y14.5-2018 / ISO 1101 · 2-D position of holes and pins · worked example verified by script · Updated 16 Nov 2026

FeatureBasic XBasic YMeas. XMeas. YSizeRemove
Hole 115.0015.0015.0815.119.06
Hole 275.0015.0075.1914.939.03
Hole 375.0055.0075.2155.189.15
Hole 415.0055.0014.8655.249.02
Result3 of 4 passHole 4 rejected
Virtual condition (gauge pin)Ø8.500resultant condition Ø9.940
1. Hole 1Ø0.272 vs Ø0.56 (bonus 0.06)Pass
2. Hole 2Ø0.405 vs Ø0.53 (bonus 0.03)Pass
3. Hole 3Ø0.553 vs Ø0.65 (bonus 0.15)Pass
4. Hole 4Ø0.556 vs Ø0.52 (bonus 0.02)Fail
1234zone Ø0.50 · with full bonus Ø0.72

Hole 3 passes only because it earned 0.15 mm of bonus; Hole 4 has almost the same position error but is close to MMC, so it fails.

How do you calculate true position?

True position is twice the distance between where a feature's axis is and where the drawing says it should be. Take the X and Y deviations from the basic (exact) location, find the straight-line distance, and double it, because the tolerance in the feature control frame is a diameter. Then compare it with the tolerance, plus any bonus.

Here and are measured minus basic, in the datum reference frame named in the feature control frame. Three steps, in this order:

  1. Check the size first. A hole outside its size limits is rejected for size, whatever its location.
  2. Compute the position from the formula above.
  3. Work out the allowed tolerance: the stated value, plus bonus if the callout carries Ⓜ or Ⓛ. Pass if the position is no larger.

What is bonus tolerance and how is it calculated?

Bonus tolerance is the extra position tolerance a feature earns when the callout has the MMC modifier (Ⓜ) and the feature is made away from its maximum material size. A bigger hole leaves more room for the bolt, so it can be further off and still assemble. Bonus equals the difference between the actual size and the MMC size.

The feature passes if its position is no larger than the allowed diameter and its size is within its limits.

MMC is the size with the most material: the smallest hole, the largest pin. With Ⓛ (LMC) the logic flips: the bonus grows as the feature moves away from least material (a hole getting smaller, a pin getting larger), which protects a minimum wall or edge distance. With no modifier (regardless of feature size, RFS), the stated tolerance applies at every size.

CalloutBonus for a holeBonus for a pinTypical use
Ⓜ MMCactual − smallest sizelargest size − actualclearance holes, bolts, dowel clearances: the function is assembly
Ⓛ LMClargest size − actualactual − smallest sizeminimum wall, edge distance, a boss that will be machined
none (RFS)00bearing bores, press fits, centring features: location must hold at every size

Worked example: a cover plate on a gearbox housing

A 90 × 70 mm steel cover plate, 8 mm thick, is held on a housing by four M8 cap screws. The plate has four clearance holes of Ø9.00 H13, that is 9.00 to 9.22 mm (ISO 273's medium clearance hole for M8 is 9 mm; H13 at 9 mm allows +0.22). The housing has tapped M8 holes. Because the screw is held by the housing, this is a fixed fastener case:

Split equally, the plate holes get Ø0.5 at MMC and the tapped holes Ø0.5 at MMC with a projected tolerance zone of 8 mm (the plate thickness), so a tilted tapped hole cannot push the screw into the plate. The plate drawing:

Cover plate 90 by 70 mm with four holes at basic positions 15 and 75 from datum C, 15 and 55 from datum B, called out 4X diameter 9.00 to 9.22 with position diameter 0.5 at MMC to datums A, B and C123415601540BCdatum A: mounting face4X Ø9.00–9.22Ø0.5MABC
Basic (boxed) dimensions locate the four holes from datums B and C. Position Ø0.5 at MMC to A, B, C applies to all four.

The CMM report for one plate gives these centres and sizes (actual mating size, the largest pin that fits each hole). These are the readings the calculator above starts with:

HoleBasic X, YMeasured X, YΔx, ΔySizePositionBonusAllowedResultWithout Ⓜ
Hole 115, 1515.08, 15.11+0.08, +0.119.06Ø0.2720.06Ø0.56PassPass
Hole 275, 1575.19, 14.93+0.19, −0.079.03Ø0.4050.03Ø0.53PassPass
Hole 375, 5575.21, 55.18+0.21, +0.189.15Ø0.5530.15Ø0.65PassFail
Hole 415, 5514.86, 55.24−0.14, +0.249.02Ø0.5560.02Ø0.52FailFail

Hole 1, step by step. The size, 9.06, is inside 9.00 to 9.22. Position:

Ø0.272 is within Ø0.56: pass.

Holes 3 and 4 tell the real story. They are almost equally far off: Ø0.553 and Ø0.556, both beyond the stated Ø0.5. Hole 3 was drilled at 9.15, 0.15 mm over MMC, so it is allowed Ø0.65 and passes. Hole 4 is 9.02, almost at MMC, so it is allowed only Ø0.52 and fails. Without the Ⓜ, Hole 3 would be scrap too, though a screw fits it with room to spare.

What is virtual condition, and why does it match a gauge?

Virtual condition is the fixed worst-case boundary a feature makes when it is at MMC and uses all of its position tolerance. For a hole, VC = MMC − position tolerance; for a pin, VC = MMC + position tolerance. It is the size of the mating part that always assembles, and the size of a functional gauge pin.

A fixed gauge with four Ø8.50 pins at the basic positions accepts exactly the plates whose holes pass the bonus check. For a hole, the space a pin can use is its size minus its position error: Hole 3 leaves 9.15 − 0.553 = 8.597 mm (above 8.50, gauge enters), Hole 4 leaves 8.464 mm (below, gauge does not enter). Our verifier script confirms the bonus test and the gauge test agree on 2,00,000 random holes and pins.

The other extreme is the resultant condition: the hole at its largest size with all its tolerance used, Ø9.94 here. Use it for minimum wall thickness or edge distance next to the hole.

How do you choose the position tolerance for a bolt pattern?

Use the fastener formula from the appendix of ASME Y14.5. It gives the largest position tolerance at MMC that still lets every screw or bolt assemble, from two numbers: H, the smallest (MMC) hole diameter, and F, the largest fastener diameter.

Total H − F = 1.00 mm: clearance holes Ø0.50 Ⓜ, tapped holes Ø0.50 Ⓜ with a projected zone at least as tall as the clamped part.

  • Floating fastener: both parts have clearance holes and a nut clamps them. Each part gets T = H − F. With M8 bolts in 9.00 mm holes in both plates that is Ø1.0 each. If the holes differ (9.00 in one, a fine-series 8.40 in the other), split T = (H1 + H2 − 2F)/2 = Ø0.7 each.
  • Fixed fastener: one part holds the fastener (tapped hole, stud, press-fit pin), so the two parts share H − F. Splits other than 50/50 are fine as long as T1 + T2 ≤ H − F; tapped holes often get the larger share because they are harder to hold.
  • Projected tolerance zone (Ⓟ) on the tapped or press-fit holes, with a height at least the maximum thickness of the part being clamped. A tapped hole that is in position at its top face but tilted can still push the screw into the mating hole.
  • For F, use the fastener's maximum major diameter. The nominal size (8.00 for M8) is a safe upper bound because metric external threads are made at or below nominal.

These formulas assume zero clearance at the worst case and perfect perpendicularity of the fastener. Engineers usually leave margin for burrs, coatings and screw-head seating, and check the head still covers the hole at the resultant condition.

Why is position better than ± coordinate tolerance?

A ± tolerance on X and Y makes a square zone. A position tolerance makes a round one, and the circle that just contains a square has a diameter of . The function (a bolt fits) is the same in every direction, so the corners of the square were already acceptable. The round zone has times the area of the square, 57% more, so more good parts pass without risking assembly. The square also gives the corners more room than the sides, which has no functional reason. More on this in coordinate vs position tolerance.

What this calculator does not cover

  • Datum shift. If a datum feature of size is referenced at MMB (for example a bore as datum B with Ⓜ after it), the whole pattern may move as a group. That shift is not added to each hole; it needs a pattern best-fit, which a CMM does. Ignoring it, as this calculator does, is conservative.
  • 3-D axis error. A deep hole can be in position at the top face and out at the bottom. The calculator takes one X/Y point per feature; for a full check, enter the worse of the two ends, or trust the CMM's cylinder fit.
  • Composite and multiple single-segment frames, where a second tolerance controls the holes relative to each other. See composite vs multiple single-segment feature control frames.
  • Size measurement. Bonus uses the actual mating size (the largest inscribed cylinder for a hole), not a single two-point caliper reading. An oval hole earns less bonus than its average diameter suggests.
Learn GD&T on real drawings

Skill-Lync's GD&T course teaches datums, MMC, bonus and virtual condition on industry drawings, the way design and quality interviews ask them.

Frequently asked questions

How do you calculate true position?

Measure how far the feature's axis is from its exact (basic) location in X and Y, then double the straight-line distance: position = 2 × √(Δx² + Δy²). The result is a diameter, so compare it directly with the diameter in the feature control frame. A hole 0.08 mm off in X and 0.11 mm off in Y has a position of Ø0.272.

What is bonus tolerance in GD&T?

Bonus tolerance is extra position tolerance a feature earns when the callout has the MMC modifier and the feature is made away from its maximum material size. For a hole, bonus = actual size − MMC size; for a pin, bonus = MMC size − actual size. It can never exceed the size tolerance, and a feature outside its size limits is rejected whatever its position.

What is the difference between MMC, LMC and RFS for position?

With MMC (Ⓜ) the position tolerance grows as the feature departs from its maximum material size: used for clearance holes and bolts, where assembly is the function. With LMC (Ⓛ) it grows as the feature departs from least material: used to protect a minimum wall. With no modifier (RFS since ASME Y14.5-2009), the stated tolerance applies at every size and there is no bonus.

What is virtual condition in GD&T?

Virtual condition is the constant worst-case boundary a feature generates when it is at MMC and at the full position tolerance. For a hole, VC = MMC − position tolerance; for a pin, VC = MMC + position tolerance. A functional gauge pin made at the hole's virtual condition accepts exactly the holes that pass the bonus check.

Is the true position tolerance a radius or a diameter?

On drawings that show the Ø symbol in the feature control frame, the position tolerance is the diameter of a cylindrical zone, so a Ø0.2 zone lets the axis move 0.1 mm in any direction. CMM reports quote the position as a diameter too (2 × radial deviation). Comparing a radial deviation with the diameter value is the most common error, and it passes parts twice as far off as allowed.

What is the floating and fixed fastener formula?

Floating fastener (bolt and nut through clearance holes in both parts): T = H − F, where H is the hole's MMC diameter and F the fastener's maximum diameter, applied to each part. Fixed fastener (one part tapped or press-fit): T1 + T2 = H − F, often split equally as (H − F)/2, with a projected tolerance zone on the tapped holes.

Does datum shift add to bonus tolerance?

No, not to each hole directly. When a datum feature of size is referenced at MMB, the whole hole pattern may shift and rotate together as that datum departs from its MMB size. It relaxes the pattern's location relative to the datum, not the holes relative to each other. This calculator ignores datum shift, which is conservative.

Related on Skill-Lync

Sources

  • ASME Y14.5-2018, Dimensioning and Tolerancing: position tolerance, MMC/LMC/RFS, virtual and resultant condition, projected tolerance zone; nonmandatory appendix on the floating and fixed fastener formulas (H = F + T; H = F + T1 + T2).
  • ISO 1101:2017 (position) and ISO 2692:2021 (maximum and least material requirements), the ISO equivalents.
  • ISO 273:1979, Fasteners — Clearance holes for bolts and screws (M8: fine 8.4, medium 9, coarse 10 mm); ISO 286-1 IT13 = 0.22 mm for sizes over 6 up to 10 mm (from the table behind our limits and fits calculator).
  • Worked example and all its numbers: Skill-Lync, recomputed by scripts/verify/true_position.py (pure Python; gauge identity on 2,00,000 random cases, seed 20261116; square-vs-circle share by Monte Carlo 63.7% vs 2/π = 63.7%) and cross-checked against this page's calculator code at build time. The CMM readings are illustrative.
Design and quality careers

Talk to a counsellor.

True position, bonus tolerance and stack-ups come up in every design and quality engineer interview at automotive and product companies. We'll map the right program to the job you want.

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.

Talk to a career counsellor

Talk to a career counsellor

Free 20-minute call. We'll map the right course to where you want to work.

By submitting you agree to our Terms and Privacy Policy.