True Position & Bonus Tolerance Calculator

Compare the measured centers of circular holes or pins with a diametric drawing tolerance. Enter nominal and measured coordinates in the same established datum frame and choose regardless of feature size or maximum material condition. See how the available allowance changes with entered feature size, plot each reading against the zone boundary, and review the size and position results together.

Dimensional inspection

True position & bonus tolerance

Compare measured centers with the drawing’s diametric zone. See what maximum material condition changes.

Drawing inputs

Use the same established datum frame for nominal and measured centers. The original readings are retained when switching display units.

Measured readings

Use the applicable unrelated mating envelope diameter for bonus tolerance.

Reading 1
Reading 2
Reading 3

Center and tolerance zone

Position error Ø

0.3 mm

Allowable Ø

0.36 mm

Inside zone · Within size limits

MMC diameter 10 mm. Bonus 0.16 mm.

Sample A

Equal axes from −0.2124 to 0.2124 mm relative to the nominal center.

Measured center at ΔX 0.09, ΔY 0.12 mm.

  • Nominal center
  • Measured center
  • Allowable radius 0.18 mm
  • Drawing radius 0.1 mm

This worksheet checks the entered center and size. Feature form, full-axis orientation, datum fitting and measurement uncertainty need a separate inspection evaluation.

Reading comparison

Offsets, diameters and tolerances shown in mm.

ReadingΔXΔYDiameterSizePosition error ØBonusAllowable ØPosition
Sample A0.090.1210.16Within size limits0.30.160.36Inside zone
Sample B-0.060.0810Within size limits0.200.2On boundary
Sample C0.12-0.0510.03Within size limits0.260.030.23Outside zone

How to use this calculator

  1. Select mm or in, Hole or Pin and the Tolerance basis shown on the drawing. The worksheet supports RFS and MMC for one diametric center tolerance.
  2. Enter Nominal X, Nominal Y, the smallest and largest drawing diameters, and the Drawing tolerance Ø.
  3. Enter Measured X and Y from the same established datum frame. With MMC, enter the applicable unrelated mating envelope diameter. Add up to six readings for the same drawing inputs.
  4. Choose a reading above Center and tolerance zone. Compare Position error Ø, Allowable Ø and the plotted center. Review size and position together in Reading comparison.
  5. Use Download position CSV or Show selectable CSV to retain the original quantities, axes, applicable allowances and comparison results.

The Formula

The mathematical logic powering this calculation is:

ΔX = measured X − nominal X and ΔY = measured Y − nominal Y. The radial center offset is √(ΔX² + ΔY²). The diametric position error is 2√(ΔX² + ΔY²), and the allowable zone radius is half its allowed diameter. The worksheet compares the squared diameters using exact fractions. Equality is reported as On boundary.

At RFS, the allowed diameter is the drawing's position tolerance. At MMC, the material condition size is the drawing's smallest allowed hole diameter or largest allowed pin diameter. For a hole, bonus = entered envelope diameter − smallest diameter. For a pin, bonus = largest diameter − entered envelope diameter. The allowable diameter is the drawing tolerance plus bonus. The entered diameter is separately compared with the size limits, including equality. An out-of-range size makes the MMC bonus and allowance unavailable. At RFS, position remains comparable with the drawing tolerance.

Use a circular feature with a diametric center tolerance and coordinates already aligned to the same fixed datum frame. These comparisons use the entered center and a single entered diameter. A full inspection can also depend on tolerance interpretation, feature form, axis orientation, datum establishment, pattern constraints and uncertainty. At MMC, use the effective unrelated mating envelope diameter determined by the applicable inspection method.

One inch is exactly 25.4 mm. Signed coordinates, positive diameters and a nonnegative drawing tolerance accept plain decimal inputs with at most six places and 100,000 mm equivalent magnitude. Converted input displays round to six decimal places and retain the entered quantity and unit until edited. Square roots and chart coordinates are numerical approximations. Position decisions and size decisions use exact entered quantities before display rounding.

Worked Example

If you input:

  • Feature: Hole at MMC
  • Nominal X, Y: 40 mm, 20 mm
  • Diameter limits: 10 mm to 10.2 mm
  • Drawing tolerance Ø: 0.2 mm
  • Sample A measured X, Y and envelope diameter: 40.09 mm, 20.12 mm, 10.16 mm
  • Sample B measured X, Y and envelope diameter: 39.94 mm, 20.08 mm, 10.00 mm
  • Sample C measured X, Y and envelope diameter: 40.12 mm, 19.95 mm, 10.03 mm

Result:

Sample A has a 0.15 mm radial offset and a 0.30 mm diametric error. Its 0.16 mm bonus gives a 0.36 mm allowable diameter, so the center is inside the zone. Sample B is on the 0.20 mm boundary. Sample C has 0.26 mm error compared with 0.23 mm allowable and is outside its zone. All three entered diameters are within size limits.

Frequently Asked Questions

Why does the position error use twice the distance from center?

The center-to-center offset is a radius. The drawing specifies the allowable zone by diameter, so the worksheet doubles that offset when comparing error with the drawing value. The chart shows circles with the corresponding radii.

How do I calculate bonus tolerance at maximum material condition?

Take the difference between the feature’s effective envelope diameter and its maximum material condition in the direction that reduces material. For a hole, subtract the drawing’s smallest size from the entered envelope diameter. For a pin, subtract that diameter from the drawing’s largest size. Add the resulting bonus to the drawing position tolerance.

Which measured diameter should I enter at MMC?

Use the unrelated mating envelope diameter supplied by the applicable inspection method. It is associated with the fitted perfect-form envelope of the feature independent of the drawing datum constraints. An arbitrary local diameter may differ from that envelope. Confirm the diameter definition in your drawing and inspection method.

What changes at RFS?

Regardless of feature size uses the drawing position tolerance as the allowance for every size. Each entered size still receives its own comparison against the drawing's diameter limits.

What happens exactly at the tolerance boundary?

The worksheet reports On boundary when the entered values yield equal squared position and allowance diameters. It compares the exact squared values before rounding the display. A real measurement decision can also depend on uncertainty and the acceptance procedure used by your organization.

Can I compare centers measured from different datums?

First express both sets of coordinates in the same established datum frame. The worksheet takes a difference directly between the entered axes, so the drawing and measured data need shared origins and axis directions.

Why do I still see an error when the MMC allowance is unavailable?

The geometric offset can be calculated from the coordinates alone. This worksheet provides the MMC comparison only when the entered diameter is within its drawing limits. The size column identifies which limit was exceeded.

Similar Calculators