Geometric tolerances (GD&T) per ISO 1101
Evaluate position tolerances: from the measured deviations in x and y follow the position deviation, the available tolerance including bonus under maximum or minimum material condition and the utilisation per measuring point – for single holes or complete hole patterns. Plus a filterable reference of the 14 tolerance types per ISO 1101.
True position calculator
Measuring points
| # | dx in mm | dy in mm | d in mm | T_tot in mm | Utilisation | Verdict | |
|---|---|---|---|---|---|---|---|
| 1 | 0.2000 | 0.2500 | 80 % | pass |
d is the diameter-based position deviation (d = 2·√(dx² + dy²)); the radial offset is d/2.
Tolerance zone and actual positions (equal aspect)
Blue circle: zone Ø t. Dashed circle: largest available zone Ø T_tot (bonus). Dots: actual positions (green pass, red fail).
Symbol reference: the 14 tolerance types per ISO 1101
Quick overview of all form, orientation, location and runout tolerances with tolerance zone and typical applications. For binding drawing rules the standards ISO 1101, ISO 5459 and ISO 2692 apply.
Straightness
Limits how far a line or axis may deviate from an ideal straight line.
Tolerance zone: Two parallel lines or planes at distance t; with Ø a cylinder around the axis.
Application: Guide ways; with Ø on the axis of long shafts for assemblability.
Flatness
Limits the deviation of a surface from an ideal plane.
Tolerance zone: Two parallel planes at distance t.
Application: Sealing and mounting faces, support surfaces.
Roundness (circularity)
Limits the deviation of each cross section from an ideal circle.
Tolerance zone: Two concentric circles with radial distance t per cross section.
Application: Bearing seats, O-ring sealing seats, pistons.
Cylindricity
Limits the total deviation of a cylindrical surface from an ideal cylinder; combines roundness, straightness and parallelism of the surface lines.
Tolerance zone: Two coaxial cylinders with radial distance t.
Application: Precision bores, hydraulic cylinders, guide bushings.
Profile of a line
Limits the deviation of an arbitrary contour from its nominal shape, per cross section; with a datum it also acts as an orientation or location tolerance.
Tolerance zone: Envelope of circles of diameter t along the nominal contour.
Application: Cam contours, cam discs, sealing lips.
Profile of a surface
Limits the deviation of a surface from its nominal geometry; the most universal symbol, with a datum also usable for orientation and location.
Tolerance zone: Envelope of spheres of diameter t over the nominal surface.
Application: Free-form surfaces, styling surfaces, 3D sealing faces.
Parallelism
Limits the orientation deviation of a feature relative to a datum for a theoretically parallel course.
Tolerance zone: Two parallel planes or lines at distance t, parallel to the datum; with Ø a cylinder.
Application: Opposing functional faces, centre distances of gearbox shafts.
Perpendicularity
Limits the orientation deviation relative to a datum for a theoretically right angle.
Tolerance zone: Two parallel planes at distance t or a cylinder Ø t, perpendicular to the datum.
Application: Stop faces, hole axis perpendicular to a seating face.
Angularity
Limits the orientation deviation for an arbitrary nominal angle to the datum defined as a basic dimension.
Tolerance zone: Two parallel planes at distance t at the theoretically exact angle to the datum.
Application: Tapered and inclined faces, vee guides.
Position
Limits the deviation of the actual location from the theoretically exact nominal location – the calculation core of this tool, combinable with Ⓜ/Ⓛ.
Tolerance zone: Cylinder Ø t, sphere SØ t or two parallel planes, centred on the nominal location.
Application: Hole patterns, flange bolt circles, pin and tapped holes.
Coaxiality / concentricity
Limits the deviation of an axis (coaxiality) or a centre point (concentricity) from the datum axis; demanding to measure, runout is often the better choice.
Tolerance zone: Cylinder Ø t around the datum axis or circle Ø t around the datum point.
Application: Shaft steps relative to each other, bearing seats on a common axis.
Symmetry
Limits the deviation of a median plane or median line from the datum median plane.
Tolerance zone: Two parallel planes at distance t, symmetric to the datum.
Application: Keyways relative to the shaft centre, clevises, slots.
Runout (circular/axial)
Limits the variation during rotation about the datum axis per single section; captures form and location deviation combined.
Tolerance zone: Per measuring position two concentric circles (radial) or two circles in the axial direction at distance t.
Application: Rotating shaft steps (radial runout), thrust collars (axial runout).
Total runout
Like runout, but evaluated over the whole surface simultaneously – stricter than single-section runout.
Tolerance zone: Two coaxial cylinders or two parallel planes perpendicular to the datum axis.
Application: Complete cylindrical or end faces of high-speed rotors.
Formulas and fundamentals
The tolerance zone of a position tolerance with a Ø modifier is a cylinder of diameter t centred on the theoretically exact position (basic dimension). From the coordinate deviations dx and dy follows the radial offset of the actual position r = √(dx² + dy²); the diameter-based position deviation is twice that value: d = 2·√(dx² + dy²). The factor 2 is the most frequently forgotten step in practice – the tolerance is a diameter while the offset is a radius.
Under the maximum material condition Ⓜ (ISO 2692) the distance of the actual diameter from the maximum material size may additionally be consumed as position deviation. For a hole the maximum material size is the lower limit (bonus B = actual size − lower limit), for a shaft it is the upper limit (B = upper limit − actual size). Under the minimum material condition Ⓛ the distance from the minimum material size applies analogously. The available tolerance is T_tot = t + B, the acceptance criterion is d ≤ T_tot, the utilisation η = d / T_tot · 100 %.
There is no negative bonus: if the actual size lies outside the size limits, the feature has already failed the size check. Without a modifier (RFS) there is no bonus at all. For hole patterns every measuring point receives the bonus from its own actual diameter; the overall verdict is pass only if every point stays within its available tolerance.
Worked example
Hole Ø 10 +0.15/0 (lower limit 10.00 mm, upper limit 10.15 mm) with position tolerance Ø 0.2 Ⓜ. Measured: actual diameter 10.12 mm, dx = 0.12 mm, dy = 0.09 mm. Position deviation d = 2·√(0.12² + 0.09²) = 0.3000 mm – without the modifier the part would be scrap because 0.30 > 0.20.
With Ⓜ the bonus becomes B = 10.12 − 10.00 = 0.12 mm, hence T_tot = 0.2 + 0.12 = 0.32 mm. Since 0.30 ≤ 0.32 the hole passes with a utilisation of 93.8 %. The size surplus of the oversized hole rescues the position deviation – exactly what assemblability means.
Frequently asked questions
Why does the formula contain the factor 2?
A position tolerance with the Ø symbol specifies the diameter of the cylindrical tolerance zone, but dx and dy first yield the radial offset of the actual position. For the actual axis to lie within a zone of diameter t, twice that offset must not exceed t: d = 2·√(dx² + dy²) ≤ t.
What is the bonus tolerance under Ⓜ (MMC)?
Assemblability depends on size and position together. If a hole is produced larger than its maximum material size (the lower limit), it offers the mating part more clearance; exactly this size surplus may additionally be consumed as position deviation. The available tolerance grows to T_tot = t + bonus.
How do hole and shaft differ for the MMC size?
Maximum material means as much material as permitted: a hole contains the most material when it is as small as allowed (MMC size = lower limit), a shaft when it is as large as allowed (MMC size = upper limit). The bonus therefore uses actual size minus lower limit for holes and upper limit minus actual size for shafts.
What happens if the actual size is outside the size limits?
Then the feature has already failed the size check and the point is judged as fail regardless of its position. A negative bonus does not exist; the bonus is clamped to zero at the bottom and to the full size tolerance at the top.
Does the bonus also apply when Ⓜ follows the datum letter?
No. Ⓜ after the datum allows the whole pattern to shift relative to the datum (datum shift) when the datum feature departs from its maximum material size. This is one common transformation of all points and must not be added as an extra per-point bonus – simple calculators that do so judge too optimistically.
How are coordinate (±) tolerances and position tolerances related?
A ± dimension in x and y creates a square zone; the round position zone through its corner points has the diameter of the square's diagonal (factor 2·√2 ≈ 2.83 per ± value). The round zone offers about 57 % more area than the square and reflects the function (assemblability) more realistically.