Free tools · ISO GPS · mm
Tolerance calculators, with the course behind each one
Fits, tolerance stack-ups, GD&T position and fastener holes: enter your values, read the answer on a diagram that follows them, and open the course text when you want the reasoning.
Pick the standard of your drawings: units, tables, vocabulary and course text follow.
No sign-up. Calculations run in your browser; nothing is sent to MecAgent.
- 01ISO fit calculatorLimits and clearance of a hole and shaft class, such as H7/g6.
- 02Tolerance stack-up calculatorGap of an assembly in worst case, statistically and by Monte Carlo.
- 03Position and MMR calculatorPosition deviation, extra tolerance from size and virtual size of a hole or pin.
- 04Fastener hole calculatorPosition tolerance of bolt holes that always assemble.
- 05Lever arm and locating pinsHow a small tilt or pin clearance grows with distance.
- 06Capability and defect rateCp, Cpk and parts per million from a mean and a standard deviation.
01
ISO fit calculator
Pick a nominal size and two ISO 286 tolerance classes. You get the limits of each part, the extreme clearances and the kind of fit.
Inputs
Common fits
Precise sliding guide
Results
- Hole Ø25 H7
- 25.000 to 25.021 mm
- 0 / +21 µm · IT7 = 21 µm
- Shaft Ø25 g6
- 24.980 to 24.993 mm
- −20 / −7 µm · IT6 = 13 µm
- Minimum clearance
- 7µm
- Maximum clearance
- 41µm
Clearance fit: the shaft always enters, with 7 to 41 µm of clearance.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
A fit is decided by where each part's tolerance zone sits relative to the nominal size. The letter places the zone, the number sets its width.
How it works
Reading a tolerance class
In H7, the letter H is the fundamental deviation: it says how far the zone starts from the nominal size. The number 7 is the tolerance grade: it sets the width of the zone, which grows with the size of the part. Capital letters are holes, small letters are shafts.
The hole-basis system is the default: keep the hole at H (it starts exactly at the nominal size) and move the shaft, which is easier to machine and to measure. From a to h the shaft is below the nominal size and gives clearance. With an H7 hole, js to n usually give a transition fit and p to z an interference fit.
Size does not control form
By default (ISO 8015), a size tolerance is checked between two opposite points. A bent shaft can pass that check and still not enter the hole. For a fit that must assemble, add the envelope requirement Ⓔ after the tolerance, or a form tolerance. ASME Y14.5 works the other way round: the envelope applies by default (Rule #1).
Formulas
- Maximum clearance
- J max = ES − ei
- Minimum clearance
- J min = EI − es
- Tolerance unit (sizes up to 500 mm)
- i = 0.45 · ∛D + 0.001 · D (µm, D in mm)
- Grades
- IT6 = 10 i, IT7 = 16 i, IT8 = 25 i, IT9 = 40 i
Worked example: Ø25 H7/g6
- Range 18 to 30 mm: IT7 = 21 µm, IT6 = 13 µm, deviation g: es = −7 µm.
- Hole 25 H7: 0 / +21 µm, so 25.000 to 25.021 mm.
- Shaft 25 g6: −7 / −20 µm, so 24.980 to 24.993 mm.
- J min = 0 − (−7) = 7 µm and J max = 21 − (−20) = 41 µm: a clearance fit for a precise sliding guide.
Common mistakes
- Counting on the minimum clearance without the envelope requirement: a form error uses it up.
- Choosing a fine grade out of habit: each finer grade cuts the tolerance by more than a third, and often adds an operation.
- Forgetting temperature: 100 mm of aluminum grows 23 µm for 10 °C, more than the whole IT6 tolerance at that size (22 µm).
Standards
- ISO 286-1 and ISO 286-2: limits and fits
- ISO 14405-1: linear sizes and their modifiers
- ISO 8015: independency principle
02
Tolerance stack-up calculator
List the dimensions of the chain and say whether each one opens or closes the gap. The calculator compares the worst case, the statistical result and a simulation, and shows which dimension matters most.
Inputs
Results
- Mean gap
- 0.260mm
- Standard deviation
- 0.0455mm
- Worst case
- 0.000 to 0.520 mm
- ± 0.260
- Statistical, ± 3σ
- 0.124 to 0.396 mm
- ± 0.136
Worst case: some combinations of in-tolerance parts break the requirement. Statistically, about 216 assemblies per million fall outside it.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
The gap is the sum of the dimensions that open it minus the ones that close it. In worst case the tolerances add up; statistically their squares do.
How it works
Drawing the chain
Start from one face of the gap. On that part, go to the face that touches the next part, and write the dimension between the two. Jump to the next part through the contact and repeat until you reach the other face of the gap. A good chain crosses each part once: every extra dimension spends tolerance.
Before any calculation, turn each dimension into a mean value and a half-range: 15 0/−0.12 becomes 14.94 ± 0.06. Components you buy (bearings, circlips, seals) come with tolerances you cannot negotiate: read them in the catalog.
Worst case or statistics
Worst case assumes every dimension sits at its limit at the same time. It needs no assumption and guarantees every assembly, but the tolerance left for each part shrinks as 1/n. Use it for three dimensions or fewer, for safety functions and for small series.
The statistical method adds variances. With normal, centered processes it gives the root sum of squares (RSS), which is narrower and accepts a small, known share of bad assemblies. It only holds if production really is centered and capable: ask for a Cpk on the dimensions of the chain.
Monte Carlo simulation draws each dimension from its own distribution. It is the method to use when a dimension is not normal (a purchased part of unknown spread is closer to uniform) or when the geometry is not a simple sum.
Formulas
- Chain
- J = Σ (dimensions that open) − Σ (dimensions that close)
- Worst case
- T = Σ tᵢ
- Statistical (RSS)
- T = √( Σ tᵢ² ) with tᵢ = 3 σᵢ
- Standard deviation for a half-range t
- normal t/3 · triangular t/√6 · uniform t/√3
- Share of a dimension
- Cᵢ = σᵢ² / Σ σ²
Worked example: A bearing, a spacer and a gear in a housing
- J = A − B1 − B2 − B3, with A = 50 ± 0.10, B1 = 14.94 ± 0.06, B2 = 19.80 ± 0.05 and B3 = 15.00 ± 0.05.
- Mean gap: 50 − 14.94 − 19.80 − 15.00 = 0.26 mm.
- Worst case: ± (0.10 + 0.06 + 0.05 + 0.05) = ± 0.26, so 0.00 to 0.52 mm.
- Statistical: ± √(0.10² + 0.06² + 0.05² + 0.05²) = ± 0.136, so 0.124 to 0.396 mm.
- The housing alone carries 54% of the variation: halving its tolerance narrows the gap by 23%, halving the gear's by 5%.
Common mistakes
- Adding nominal values that are not centered (15 0/−0.12 is 14.94, not 15).
- Using RSS without asking production for a capability: the assumption binds no one.
- Leaving a dimension of the chain under a general tolerance: it is often the largest contributor.
- Tightening every tolerance instead of shortening the chain or adding an adjustment.
Standards
- ISO 8015: fundamental rules
- ISO 22514-2: process capability
03
Position and MMR calculator
Enter the size limits, the position tolerance and what you measured. The calculator gives the tolerance really available at that size, and tells you whether the feature passes.
Inputs
Results
- Measured position, Ø
- 0.200mm
- Allowed position, Ø
- 0.220mm
- Bonus from size
- 0.120mm
- Virtual size
- Ø 9.900mm
In tolerance: the axis is Ø 0.200 off for Ø 0.220 allowed.
Gauge: a Ø 9.900 pin at the theoretical position must enter the hole.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
A position tolerance defines a zone centered on the theoretically exact position. With Ⓜ, that zone grows as the feature moves away from its maximum material size.
How it works
From coordinates to a position value
The zone is a cylinder of diameter t around the theoretically exact position, which is fixed by theoretically exact dimensions (TED: boxed, without tolerance) from the datums. The axis may be anywhere inside. A measured offset (dx, dy) therefore counts as a diameter: twice the radial distance.
A round zone is fairer than ± coordinates. A ± 0.1 square accepts 0.141 on its diagonal but refuses 0.12 along one axis; the Ø 0.283 circle accepts the same largest error in every direction, with 57% more area.
What Ⓜ changes
The maximum material requirement (MMR) replaces two separate limits with one boundary the surface must not cross: the maximum material virtual condition. Its diameter, the virtual size, is the smallest hole minus the tolerance; for a pin, the largest pin plus the tolerance. A larger hole can be further off and still clear the same boundary: that extra is often called the bonus.
Use Ⓜ when the function is assembly with clearance: bolts, covers, loose pins. Leave it out when position matters at any size: press fits, precise locating, gear centers, sealing, balance. Use Ⓛ when the critical case is thin material: wall thickness or edge distance.
Formulas
- Measured position (zone diameter)
- 2 · √( dx² + dy² )
- Virtual size, hole at Ⓜ
- smallest hole − t
- Virtual size, pin at Ⓜ
- largest pin + t
- Tolerance available at Ⓜ
- t + | measured size − maximum material size |
Worked example: Hole Ø10 +0.2/0, position Ø0.1 Ⓜ
- Maximum material size: 10.0 (smallest hole). Virtual size: 10.0 − 0.1 = 9.9.
- Measured Ø10.12: bonus 0.12, so Ø0.22 is allowed.
- Measured offsets 0.06 and 0.08: position = 2 · √(0.06² + 0.08²) = Ø0.20. The hole passes.
- Without Ⓜ the same hole fails: Ø0.20 for Ø0.10 allowed.
Common mistakes
- Comparing the radial offset with the tolerance: the tolerance is a diameter, so double the offset.
- Putting Ⓜ on a press fit or a precise locating feature: there is no clearance to trade.
- Adding the play of a datum at Ⓜ to the tolerance of every hole of a pattern: it moves the whole pattern, once.
- Writing a position tolerance without theoretically exact dimensions or without datums.
Standards
- ISO 1101: geometrical tolerancing
- ISO 2692: maximum and least material requirements
- ISO 5459: datums
04
Fastener hole calculator
Choose the screw and its clearance hole. The calculator gives the position tolerance each part can take so that every screw goes in, for a bolt and nut or for a tapped hole.
Inputs
Results
- Clearance to share, H − F
- 0.600mm
- Clearance holes
- Ø 0.300mm
- Tapped holes
- Ø 0.300mm
On the drawing
The clearance is shared: Ø 0.3 for the clearance holes and Ø 0.3 for the tapped holes, projected over 10 mm.
Not to scale: deviations are exaggerated.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
Screws assemble when the position errors of the two parts fit inside the clearance between screw and hole. With a nut, each part gets all of it; with a tapped hole, the two parts share it.
How it works
Floating and fixed fasteners
Floating fastener: the screw passes through clearance holes in both parts and a nut closes the joint. The screw can move in both holes, so each part may use the whole clearance H − F as its position tolerance.
Fixed fastener: the screw is held by one part, in a tapped hole, as a stud or as a pressed pin. Only one hole has clearance, so the two parts share H − F. Give the larger share to the part that is harder to machine accurately.
Why the tapped hole needs a projected zone
A screw extends the axis of its thread outside the part. A tilt that is acceptable inside the thread becomes a much larger offset where the screw crosses the cover. The projected tolerance zone Ⓟ moves the zone out of the tapped part, over the thickness of the cover, where the clearance is really needed. Without it, the tapped hole's tolerance has to shrink by the factor 1 + 2P/D.
Write the tolerances at maximum material Ⓜ on clearance holes: a larger hole then earns a bonus. A thread has no usable bonus, so the tapped hole keeps its stated value.
Formulas
- Floating fastener
- T = H − F for each part
- Fixed fastener
- T1 + T2 = H − F
- Fixed fastener without a projected zone
- H = F + T1 + T2 · (1 + 2P / D)
Worked example: Cover held by M6 screws in tapped holes
- F = 6.0. Medium clearance hole per ISO 273: H = 6.6. Clearance to share: 0.6.
- Equal split with a projected zone: Ø0.3 Ⓜ on the cover's holes, Ø0.3 Ⓟ on the tapped holes.
- Without a projected zone, cover 10 mm thick, 9 mm of engagement: 0.3 / (1 + 20/9) = Ø0.093 for the tapped holes.
- A cover hole made at Ø6.82 earns 0.22 of bonus: Ø0.52 available.
Common mistakes
- Using the floating formula for a tapped hole: the parts get twice the tolerance the joint can absorb.
- Forgetting the projected zone on tapped holes, studs and pressed pins.
- Not checking that the screw head or washer still covers the hole in its extreme position.
Standards
- ISO 273: clearance holes for bolts and screws
- ISO 1101: projected tolerance zone
- ISO 2692: maximum material requirement
05
Lever arm and locating pins
Two effects that dominate real stack-ups: an orientation error acting far from its seat, and the rotation a part can take inside the clearance of its two locating pins.
Inputs
Results
- Displacement at the point
- ± 0.250mm
- Sensitivity, h / L
- 5
- Tilt
- 2.5mrad
- 0.143°
A tolerance of 0.05 mm on the seat becomes ± 0.250 mm at the functional point: 5 times more.
Not to scale: deviations are exaggerated.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
An angle multiplies with distance. A tolerance that looks small on a short seat or in a pin clearance can become the largest contributor far from it.
How it works
Lever arm
An orientation tolerance t over a seat of length L lets the part tilt by ± t / L. At a distance h from the seat the tilt becomes a displacement of ± t · h / L. The ratio h / L is the sensitivity: in two dimensions it is rarely 1, and it is what a one-direction stack-up misses.
The remedy is in the design, not in the tolerance: lengthen the seat, or bring the datum closer to the functional point.
Two locating pins
Two pins a distance L apart, with diametral clearances c1 and c2, let the part shift by half the smaller clearance and rotate by (c1 + c2) / 2L. Adding the translation and the rotation at the functional point is conservative: both maxima are not reached together.
Two round pins in two round holes also over-constrain the part: the center distances of pins and holes must agree within half the sum of the minimum clearances, usually a few micrometers. The standard answer is one round pin and one relieved (diamond) pin, or a slot, which frees the centre distance and still stops the rotation.
Formulas
- Lever arm
- δ = ± t · h / L
- Rotation on two pins
- θ = (c1 + c2) / (2 L)
- Error at a distance R
- δ = R · θ
- Assembly of two round pins
- | e holes − e pins | ≤ (c1 min + c2 min) / 2
Worked example: Sensor bracket on a 20 mm seat
- Perpendicularity of 0.05 on a seat 20 mm wide; the sensor is 100 mm above it.
- δ = 0.05 × 100 / 20 = ± 0.25 mm: the sensitivity is 5.
- Widening the seat to 60 mm with the same tolerance brings the effect down to ± 0.083 mm.
Common mistakes
- Treating a 2D chain as a simple sum: angles usually dominate.
- Locating a part on two round pins and tolerancing the center distance instead of relieving one pin.
- Putting the locating pins close together: the rotation error is inversely proportional to their spacing.
Standards
- ISO 1101: orientation tolerances
- ISO 5459: datum systems
06
Capability and defect rate
Enter the limits of a dimension and how the process really produces it. The calculator gives the capability indices and the share of parts outside tolerance.
Inputs
Results
- Cp
- 1.67
- Cpk
- 1.33
- Below the lower limit
- < 0.001 ppm
- Above the upper limit
- 31.7 ppm
- Out of tolerance
- 31.7 ppm
- 0.00317 %
Capable: Cpk 1.33 is at or above 1.33.
Cp is 1.67: centering the process alone would raise Cpk to that value.
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.
Cp compares the spread of a process with the tolerance; Cpk also counts how far the process is off center. A statistical stack-up is only as good as the capability behind each dimension.
How it works
Two indices, two questions
Cp asks whether the process could fit in the tolerance if it were perfectly centered: tolerance divided by six standard deviations. Cpk asks whether it does: the distance from the mean to the nearest limit, divided by three standard deviations. Cpk can never exceed Cp, and the gap between them is what centering would win back.
Common targets are Cpk ≥ 1.33 for ordinary characteristics (about 32 parts per million beyond the nearest limit) and 1.67 for critical ones. Six sigma quality means Cp = 2 with the mean allowed to drift by 1.5 σ, which leaves 3.4 parts per million.
Measurement takes its share
Whoever proves conformity carries the measurement uncertainty U (ISO 14253-1): a part is proven good only if its measured value is inside the tolerance reduced by U on each side. For the manufacturer the tolerance really available is the drawing tolerance minus 2 U, so a better gauge gives tolerance back to production.
Formulas
- Potential capability
- Cp = (USL − LSL) / 6σ
- Actual capability
- Cpk = min(USL − μ, μ − LSL) / 3σ
- Share beyond a limit
- p = Φ(−Z) with Z = | μ − limit | / σ
- Proven conformity
- tolerance − 2 U
Worked example: Ø10 ± 0.1 produced at 10.02 with σ = 0.02
- Cp = 0.2 / (6 × 0.02) = 1.67.
- Cpk = (10.1 − 10.02) / (3 × 0.02) = 1.33.
- Upper side: Z = 4, about 32 ppm. Lower side: Z = 6, about 0.001 ppm.
- Centered at 10.00, the same process would reach Cpk 1.67 and well under 1 ppm.
Common mistakes
- Quoting Cp alone: an off-center process can have a high Cp and still make bad parts.
- Estimating σ from a handful of parts, or from a process that is not stable.
- Reading ppm from a normal curve when the data are not normal (tool wear, sorted lots).
Standards
- ISO 22514-2: process capability
- ISO 14253-1: decision rules for conformity
- JCGM 100 (GUM): measurement uncertainty
Use with engineering judgment. These calculators help you reason about tolerances; they do not replace the standards. Check any value that matters against the current edition of the standard and your company's rules before releasing a drawing.
Try it
Put AI to work in your CAD.
Model parts, generate drawings and automate the repetitive work inside your CAD software.