Skip to content
MecAgentMecAgent

Free tools · ASME Y14.5 · inch

ASME tolerance calculators, with the course behind each one

Inch fits per ANSI B4.1, tolerance stack-ups, true position with MMC and fastener holes per ASME Y14.5: 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.

Open the calculators

No sign-up. Calculations run in your browser; nothing is sent to MecAgent.

01

ANSI B4.1 fit calculator

Pick a basic size in inches and a standard fit of ANSI B4.1: running, locational or force. You get the limits of the hole and of the shaft, the extreme clearances and the kind of fit.

Inputs

in

Close running: accurate machinery, moderate speeds and loads

Common fits

Results

Hole Ø1 RC4
1.0000 to 1.0012 in
0 / +1.2 thousandths
Shaft Ø1 RC4
0.9984 to 0.9992 in
−1.6 / −0.8 thousandths
Minimum clearance
0.0008in
Maximum clearance
0.0028in

Clearance fit: the shaft always enters, with 0.0008 to 0.0028 in of clearance.

Live diagramTolerance zones around the basic size
Deviation, 0.001 in+1.20−0.8−1.6clearance0.0008 inclearance0.0028 inHole RC4Shaft RC4basic size: Ø 1
The course behind this calculatorHow it works, formulas, a worked example, common mistakes and the standards to cite.

ANSI B4.1 names a fit by what it does: run, locate or hold by force. The class number sets how much clearance or interference, and the tables give the limits of both parts in thousandths of an inch.

How it works

Reading a fit designation

RC4 is a running fit of class 4. The letters give the family: RC for running or sliding, LC, LT and LN for locating with clearance, transition or interference, FN for force or shrink. Within a family, a higher number means more clearance for RC and LC, and more interference for LN and FN.

Every fit is hole-basis: the hole starts at the basic size and goes up, and the shaft sits below, across or above it. The designation is for choosing the fit, not for the drawing: write the limits of size on each part, for example 1.0000 to 1.0012 for the hole.

On millimeter drawings, ASME B4.2 uses the ISO classes (H7/g6 and so on): switch this page to ISO for those.

Rule #1: size also controls form

Under ASME Y14.5, the limits of size of a regular feature of size also limit its form (Rule #1, the envelope principle): at maximum material condition the feature must have perfect form, and form error is allowed only as the size departs from MMC. A shaft at its largest size cannot be bent, so the minimum clearance of the fit is real.

Rule #1 does not control the relationship between features (coaxiality, perpendicularity), and it does not apply to stock sizes or to parts measured in the free state. The independency symbol Ⓘ switches it off for one dimension. ISO drawings work the other way round: size and form are independent unless Ⓔ is added.

Under Rule #1, a bent shaft at its largest size is rejectedWith the independency symbol Ⓘ0.5000.530Local sizes are 0.500 everywhere: accepted.It occupies 0.530: it will not enter a 0.502 hole.Rule #1 (the default)perfect form at MMC: Ø 0.500The shaft must fit inside a perfect Ø 0.500 cylinder.Form error is allowed only as the size leaves MMC.
Rule #1: the limits of size also control form.

Formulas

Maximum clearance
largest hole − smallest shaft
Minimum clearance
smallest hole − largest shaft
Interference
a negative clearance: shaft larger than hole
Table values
limits in 0.001 in, added to the basic size

Worked example: Ø1.0000 RC4

  1. Size range over 0.71 up to 1.19 in. RC4: hole +1.2 / 0, shaft −0.8 / −1.6 thousandths.
  2. Hole: 1.0000 to 1.0012 in.
  3. Shaft: 0.9984 to 0.9992 in.
  4. Clearance from 1.0000 − 0.9992 = 0.0008 in to 1.0012 − 0.9984 = 0.0028 in: a close running fit for accurate machinery.

Common mistakes

  • Writing RC4 on the drawing: the shop needs the limits of size, not the designation.
  • Using an LN fit to transmit torque: locational interference fits locate, force fits (FN) hold.
  • Reading the B4.1 symbols such as H8/f7 as ISO classes: the inch values come from their own tables.
  • Forgetting temperature: 4 in of aluminum grows about 0.0005 in for 10 °F, close to the whole hole tolerance of an RC1 fit at that size (0.0006 in).

Standards

  • ASME B4.1: preferred limits and fits for cylindrical parts (inch)
  • ASME B4.2: preferred metric limits and fits
  • ASME Y14.5: Rule #1, the envelope 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

Share of the variation53%
Share of the variation21%
Share of the variation13%
Share of the variation13%
in
in

Results

Mean gap
0.0275in
Standard deviation
0.00183in
Worst case
0.0170 to 0.0380 in
± 0.0105
Statistical, ± 3σ
0.0220 to 0.0330 in
± 0.0055

Worst case: some combinations of in-tolerance parts break the requirement. Statistically, about 21.5 assemblies per million fall outside it.

Live diagramWhere the gap can land
min 0.02worst case± 3σ0.0200.0250.0300.035Gap, in
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: 0.625 +0/−0.005 becomes 0.6225 ± 0.0025. Components you buy (bearings, retaining rings, 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.

On an ASME drawing, a tolerance that relies on the statistical method carries the statistical tolerancing symbol ⟨ST⟩, with a note requiring statistical process control on those features.

The gap closes the loop: J = A − B1 − B2 − B3HousingBearingSpacerGearJA = 2.000 ± 0.004same direction as JB3 = 0.600 ± 0.002B2 = 0.750 ± 0.002B1 = 0.6225 ± 0.0025opposite to JWorst case: J = 0.0275 ± 0.0105 in. Statistical: J = 0.0275 ± 0.0055 in. Not to scale.
Dimension chain of the worked example: four links.

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

  1. J = A − B1 − B2 − B3, with A = 2.000 ± 0.004, B1 = 0.6225 ± 0.0025, B2 = 0.750 ± 0.002 and B3 = 0.600 ± 0.002.
  2. Mean gap: 2.000 − 0.6225 − 0.750 − 0.600 = 0.0275 in.
  3. Worst case: ± (0.004 + 0.0025 + 0.002 + 0.002) = ± 0.0105, so 0.0170 to 0.0380 in.
  4. Statistical: ± √(0.004² + 0.0025² + 0.002² + 0.002²) = ± 0.0055, so 0.0220 to 0.0330 in.
  5. The housing alone carries 53% of the variation: halving its tolerance narrows the gap by 22%, halving the gear's by 5%.

Common mistakes

  • Adding nominal values that are not centered (0.625 +0/−0.005 is 0.6225, not 0.625).
  • 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

  • ASME Y14.5: statistical tolerancing symbol ⟨ST⟩
  • ASTM E2281: process capability and performance

03

True position and MMC 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

in
in
in
Material condition
in
in
in

Results

Measured position, Ø
0.0100in
Allowed position, Ø
0.0110in
Bonus tolerance
0.0060in
Virtual condition
Ø 0.3950in

In tolerance: the axis is Ø 0.0100 off for Ø 0.0110 allowed.

Functional gage: a Ø 0.3950 pin at true position must enter the hole.

Live diagramTolerance zone at the measured size
Measured size between its limits0.40.408ⓂⓁstated zone Ø 0.005with bonus Ø 0.011measured axistrue position
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 true position. With Ⓜ, that zone grows as the feature departs from its maximum material condition.

How it works

From coordinates to a position value

The zone is a cylinder of diameter t around the true position, which is fixed by basic dimensions (boxed, without tolerance) from the datum reference frame. 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 ± 0.005 square accepts 0.0071 on its diagonal but refuses 0.006 along one axis; the Ø 0.014 circle accepts the same largest error in every direction, with 57% more area.

RFS, MMC and LMC

Without a modifier the tolerance applies regardless of feature size (RFS, Rule #2): the zone keeps its stated diameter at any size. With Ⓜ the stated value applies at maximum material condition, and the departure from MMC is added to it: the bonus tolerance. The surface then never crosses one constant boundary, the virtual condition: the MMC hole minus the tolerance, or the MMC pin plus the tolerance. That is the size of the functional gage.

Use Ⓜ when the function is assembly with clearance: bolts, covers, loose pins. Stay at RFS 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.

A datum feature of size referenced at Ⓜ (maximum material boundary) lets the whole pattern shift as that datum feature departs from its boundary. The shift moves the pattern as a group: it is not a bonus for each hole.

A feature control frame reads left to right: what, how much, relative to whatØ .005MABCShape and size of the zoneØ: a cylindrical zone of .005 inDatum references, in orderprimary, secondary, tertiaryGeometric characteristichere: positionModifiermaximum material conditionthe leader points to the toleranced feature
Anatomy of a feature control frame. Inch values take no zero before the decimal point.

Formulas

Measured position (zone diameter)
2 · √( dx² + dy² )
Virtual condition, hole at MMC
MMC hole − t
Virtual condition, pin at MMC
MMC pin + t
Tolerance available at MMC
t + | measured size − MMC size |

Worked example: Hole Ø0.400 to 0.408, position Ø0.005 Ⓜ

  1. MMC size: 0.400 (smallest hole). Virtual condition: 0.400 − 0.005 = 0.395.
  2. Measured Ø0.406: bonus 0.006, so Ø0.011 is allowed.
  3. Measured offsets 0.003 and 0.004: position = 2 · √(0.003² + 0.004²) = Ø0.010. The hole passes.
  4. At RFS the same hole fails: Ø0.010 for Ø0.005 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 datum feature shift to the tolerance of every hole of a pattern: it moves the whole pattern, once.
  • Writing a position tolerance without basic dimensions or without datum references.
  • Reaching for concentricity or symmetry: Y14.5-2018 removed them. Use position, runout or profile.

Standards

  • ASME Y14.5-2018: position, MMC, LMC, virtual condition
  • ASME Y14.5.1: mathematical definition of the tolerances
  • ASME Y14.43: gages and fixtures

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

Clearance hole, ASME B18.2.8
in
in
Assembly
in

Results

Clearance to share, H − F
0.0310in
Clearance holes
Ø 0.0155in
Tapped holes
Ø 0.0155in

On the drawing

Clearance holesØ .0155MABCTapped holesØ .0155P.375ABC

The clearance is shared: Ø 0.0155 for the clearance holes and Ø 0.0155 for the tapped holes, projected over 0.375 in.

Live diagramTapped hole: clearance in one part only
clearance0.031 inF = 0.25 in · H = 0.281 in

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.

Without a projected zone, tilt allowed in the thread becomes interferenceCoverHousinginterferencePDWith a projected zone, the toleranceapplies over the height P,where the screw passes.Without it, the tolerance appliesinside the thread, over D.
Projected tolerance zone: section through a screw in a tapped hole.

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 1/4-20 screws in tapped holes

  1. F = 0.250. Normal clearance hole per ASME B18.2.8: H = 0.281 (9/32 drill). Clearance to share: 0.031.
  2. Equal split with a projected zone: Ø0.0155 Ⓜ on the cover's holes, Ø0.0155 Ⓟ on the tapped holes. Round down on the drawing, to Ø0.015 for example.
  3. Without a projected zone, cover 0.375 thick, 0.375 of engagement: 0.0155 / (1 + 2 × 0.375 / 0.375) = Ø0.0052 for the tapped holes.
  4. A cover hole made at Ø0.288 earns 0.007 of bonus: Ø0.0225 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

  • ASME B18.2.8: clearance holes for bolts, screws and studs
  • ASME Y14.5: projected tolerance zone and MMC
  • ASME Y14.5, Appendix B: fixed and floating fastener formulas

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

in
in
in

Results

Displacement at the point
± 0.0100in
Sensitivity, h / L
5
Tilt
2.5mrad
0.143°

A tolerance of 0.002 in on the seat becomes ± 0.0100 in at the functional point: 5 times more.

Live diagramTilt of the seat, seen at the functional point
δh = 4L = 0.8t = 0.002δ = t × h / L0.002 × 4 / 0.8± 0.0100 in

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 ten-thousandths of an inch. The standard answer is one round pin and one relieved (diamond) pin, or a slot, which frees the center 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 0.8 in seat

  1. Perpendicularity of 0.002 on a seat 0.8 in wide; the sensor is 4 in above it.
  2. δ = 0.002 × 4 / 0.8 = ± 0.010 in: the sensitivity is 5.
  3. Widening the seat to 2.4 in with the same tolerance brings the effect down to ± 0.0033 in.

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

  • ASME Y14.5: orientation tolerances and datum reference frames
  • ASME B18.8.2: dowel pins (inch series)

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

in
in
in
in

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.

Live diagramThe process against its limits
mean 0.5008lower limit0.496upper limit0.5040.4960.4980.5000.5020.504
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

A measured value inside the limits is not proof by itself: the gage has its own uncertainty. ASME B89.7.3.1 names the decision rules. The one most shops use is simple acceptance: accept a part whose measured value is inside the tolerance, provided the measurement uncertainty is small against it, typically no more than a quarter of the tolerance (4:1).

When the risk of accepting a bad part must be lower, the contract sets a guard band g: the acceptance zone is the tolerance reduced by g on each side. That reduction comes out of the tolerance left to production, so a better gage gives tolerance back.

A guard band narrows the acceptance zone; simple acceptance uses the whole toleranceLSLUSLrejection zonerejection zoneguard bandacceptance zoneguard bandggggtolerance (specification zone)With a guard band: tolerance − 2 g. Simple acceptance: the whole tolerance.
Decision rules of ASME B89.7.3.1.

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
Acceptance zone with a guard band g
tolerance − 2 g

Worked example: Ø0.500 ± 0.004 produced at 0.5008 with σ = 0.0008

  1. Cp = 0.008 / (6 × 0.0008) = 1.67.
  2. Cpk = (0.504 − 0.5008) / (3 × 0.0008) = 1.33.
  3. Upper side: Z = 4, about 32 ppm. Lower side: Z = 6, about 0.001 ppm.
  4. Centered at 0.500, 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

  • ASME B89.7.3.1: decision rules for conformance to specifications
  • ASTM E2281: process capability and performance
  • 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.