Limits, Fits, Tolerances and Gauging

Introduction

Manufactured parts cannot be produced to perfectly exact dimensions. Cutting-tool wear, machine-tool accuracy, thermal effects, elastic deformation, measurement uncertainty and operator technique all introduce variation. Metrology provides the means of specifying, measuring and controlling that variation so that parts remain functional and interchangeable.

Limits, tolerances and fits convert functional requirements into permissible dimensional variation. Gauges then provide a rapid production-control method for determining whether manufactured features fall within those limits. These ideas are central to shafts, holes, bearings, gears, bushes, couplings and almost every mechanical assembly.

A designer must answer four related questions:

1. What dimensions are functionally acceptable?
2. How much variation can each component have?
3. Should mating parts have clearance, transition or interference?
4. How can production parts be inspected quickly and reliably?

Learning Objectives

After studying this chapter, the student should be able to:

• distinguish basic size, actual size, limits, deviation, tolerance and allowance;
• calculate upper and lower limits for holes and shafts;
• select and interpret common ISO system fits;
• calculate worst-case and statistical tolerance stacks;
• explain Taylor’s principle;
• design and evaluate GO/NO-GO, plug, ring and snap gauges;
• identify gauge-maker’s tolerance, wear allowance and measurement limitations;
• apply these principles to an industrial inspection problem.

1. Fundamental Terminology

1.1 Basic size and actual size

The basic size is the theoretical size from which limits are derived. It is commonly the nominal dimension shown on a drawing, such as 40 mm. The actual size is the size obtained by measurement on a manufactured component.

The maximum limit is the largest permissible size, and the minimum limit is the smallest permissible size. A component is conforming when its actual size lies between these limits, subject to the stated inclusion convention.

The total permissible variation is the tolerance:

where T is tolerance, U is the upper limit and L is the lower limit. All three quantities must use the same units, normally millimetres or micrometres.

For example, a shaft specified as 25.000 to 24.980 mm has:

1.2 Deviations

A deviation is the algebraic difference between a limit and the basic size. For a feature with basic size B:

The fundamental deviation is the deviation nearest to the zero line. The zero line represents the basic size. Positive deviations lie above it and negative deviations below it.

1.3 Allowance

Allowance is the intentional minimum clearance or maximum interference between mating parts. For a clearance fit:

For an interference fit, the allowance is commonly expressed as the maximum allowable clearance algebraically, or as the minimum interference using a positive magnitude:

Allowance differs from tolerance. Tolerance describes variation within one feature; allowance describes the designed relationship between two mating features.

1.4 Hole and shaft conventions

In ISO limits and fits, a hole is identified by an uppercase letter, such as H7, while a shaft is identified by a lowercase letter, such as h6 or g6. The number indicates the tolerance grade, called the IT grade. The letter identifies the position of the tolerance zone relative to the basic size.

The hole-basis system uses H holes. For an H hole, the lower deviation is zero, so the minimum hole equals the basic size. Different fits are obtained by changing the shaft zone. The hole-basis system is widely used because standard drills, reamers and gauges make certain hole sizes economical.

The shaft-basis system uses h shafts. For an h shaft, the upper deviation is zero, so the maximum shaft equals the basic size. Different fits are obtained by changing the hole zone. This system is useful when a shaft size is fixed by a standard bar, bearing or other component.

2. Tolerance Grades and ISO Fits

2.1 International tolerance grades

ISO 286 expresses the magnitude of tolerance using grades IT01, IT0, IT1 through IT18. Lower numbers represent finer tolerances. The appropriate grade depends on function, manufacturing process, cost and inspection capability.

For a nominal size range, the standard tolerance unit i, in micrometres, is approximately:

where D is the geometric mean of the relevant diameter range in millimetres. The expression applies to the ISO diameter ranges and gives i in micrometres. Standard IT tolerances are multiples of i; for example, IT6 is 10i and IT7 is 16i over the usual engineering size ranges. Exact values must be taken from the applicable ISO 286 table rather than reconstructed by rounding.

The use of standard tables is important because tolerance values are tabulated by diameter step and include standardized rounding.

2.2 Classification of fits

A fit describes the relationship between mating hole and shaft.

For a hole with limits H_min and H_max and a shaft with limits S_min and S_max:

Here C_max and C_min are maximum and minimum clearance. If C_min is positive, the fit is definitely a clearance fit. If C_max is negative, the fit is definitely an interference fit. If C_min is negative and C_max is positive, the fit is transition.

2.3 Common ISO fit designations

H7/h6 is a close clearance fit often used for accurate sliding or locating applications. H7/g6 gives a larger clearance and is suitable where free movement is required. H7/k6 and H7/n6 are typical transition fits, depending on size. H7/p6 and H7/s6 are interference fits, with the latter generally producing stronger interference.

A designation must never be selected solely from a memorized list. The engineer should consider load, temperature, lubrication, assembly method, rotation, required centring accuracy, material properties and service environment. The exact limits must be obtained from the current ISO standard tables.

Worked Example 1: Limits and fit condition

A 40 H7/g6 fit is specified. For illustration, suppose the relevant standard table gives the following limits:

• H7 hole: 40.000 to 40.025 mm;
• g6 shaft: 39.984 to 39.995 mm.

Then:

Both clearances are positive; therefore the fit is a clearance fit. Its clearance range is 5 to 41 μm. The tolerance of the fit, defined as the total possible variation in clearance, is:

The numerical limits in this example are illustrative; production design must use the applicable ISO table and unit system.

3. Tolerance Stacks

A tolerance stack determines how individual dimensional variations affect an assembly requirement. It is required for axial gaps, bearing preload, gear centre distance, seal compression and positional relationships.

3.1 Worst-case stack-up

For a linear dimension formed by dimensions x₁, x₂, …, xₙ, the nominal result is calculated using the dimension chain. If all dimensions contribute with the same sign, the maximum total tolerance is the sum of individual tolerances:

For a simple additive chain:

where Uᵢ and Lᵢ are the upper and lower limits of each contributing dimension. For subtractive dimensions, signs must be retained in the dimension chain; the tolerance contribution remains positive in the worst-case total.

Worst-case analysis assumes that every dimension simultaneously reaches its unfavorable limit. It is conservative and appropriate where interchangeability and safety require certainty, but it may produce unnecessarily expensive tolerances.

3.2 Statistical stack-up

If variations are independent, centred, approximately normal and represented by standard deviations σᵢ, the root-sum-square estimate is:

For correlated dimensions:

where ρᵢⱼ is the correlation coefficient between dimensions i and j. Statistical stack-up does not guarantee that every assembly will conform; it predicts a distribution under stated assumptions. It must therefore be supported by process capability evidence and appropriate risk analysis.

Worked Example 2: Assembly gap

An assembly gap is:

The dimensions are:

• A = 80.00 ± 0.10 mm;
• B = 30.00 ± 0.05 mm;
• C = 20.00 ± 0.03 mm.

Nominal gap:

Worst-case limits are:

Thus the worst-case gap is 30.00 ± 0.18 mm, and the total tolerance is 0.36 mm. The tolerance sum is 0.10 + 0.05 + 0.03 + 0.05 + 0.03 = 0.26 mm as a one-sided contribution calculation? More directly, the variation from nominal is 0.10 + 0.05 + 0.03 = 0.18 mm on either side, so total gap tolerance is 0.36 mm. This distinction prevents the common error of confusing bilateral half-width with total tolerance.

Under independent statistical assumptions, the standard-deviation-like combined half-width, if the quoted ± values are treated as variation measures of the same type, is proportional to:

This number must not be called a standard deviation unless the input tolerances have been converted to standard deviations using a justified distribution model.

4. Taylor’s Principle and Limit Gauging

Taylor’s principle states that:

• the GO gauge should check the maximum material condition (MMC) of the feature and should check all related dimensions simultaneously as far as practicable;
• the NO-GO gauge should check the minimum material condition (LMC), but should check only one element or dimension at a time.

For a hole, MMC is the smallest hole. Therefore, the GO plug gauge for a hole corresponds approximately to the minimum hole size and has a full-form length. The NO-GO plug corresponds approximately to the maximum hole size and is generally shorter or segmented.

For a shaft, MMC is the largest shaft. Therefore, the GO ring or GO snap-gauge opening corresponds approximately to the maximum shaft size, while the NO-GO member corresponds approximately to the minimum shaft size.

The reason is functional: a part at MMC contains the greatest amount of material and is most likely to interfere with its mating part. A full-form GO gauge checks size and, to a practical extent, form and alignment. A NO-GO gauge is deliberately restricted so that it does not reject a part merely because several independent dimensions are at permissible combinations.

A GO gauge must pass through or over the feature under specified conditions. A NO-GO gauge must not pass. Gauges do not normally provide the actual measured size; they provide a conformity decision.

5. Gauge Types and Design Principles

5.1 Plain plug gauges

A plain plug gauge inspects holes. It commonly has two ends: GO and NO-GO. The GO end should enter the hole completely or to the specified inspection depth using light hand pressure. The NO-GO end should not enter beyond the permitted amount.

Plug gauges may be double-ended, progressive or separate. Progressive gauges combine steps of different sizes on one member, but they require careful handling and clear identification.

5.2 Ring gauges

A ring gauge inspects external cylindrical features such as shafts. A GO ring should pass over the shaft; the NO-GO ring should not pass. Fixed limit rings are robust and quick, while adjustable rings offer flexibility but require calibration and locking arrangements.

5.3 Snap gauges

A snap gauge has fixed or adjustable anvils and is particularly suitable for high-volume inspection of shafts, widths and thicknesses. A double-ended snap gauge often has GO and NO-GO openings. The GO opening checks the maximum material condition; the NO-GO opening checks the opposite limit.

5.4 Gauge tolerances and wear allowance

A gauge itself is not perfectly accurate. Its manufacturing tolerance must be smaller than the workpiece tolerance. A common allocation is to assign a specified fraction of the work tolerance to the gauge, but the exact value must follow the governing gauge-design standard, company practice and measurement-risk analysis.

Wear allowance is normally applied to the GO gauge because it is used more frequently. For a GO plug gauge, wear increases its effective diameter and could cause undersize holes to be accepted if not controlled. A practical design therefore places the initial GO gauge near the material limit with a specified wear allowance toward the permissible wear direction. NO-GO gauges generally receive no comparable production wear allowance because they should not be used as working gauges.

Gauge design must distinguish:

• workpiece limits;
• gauge-maker’s manufacturing tolerance;
• wear allowance;
• calibration uncertainty;
• temperature reference, usually 20 °C;
• permissible gauging force and contact condition.

5.5 Gauge design example

Suppose a hole has limits 50.000 to 50.025 mm. Ignoring a particular national gauge standard for this illustration, let the GO plug manufacturing tolerance be 0.004 mm and the permitted wear allowance be 0.002 mm. The GO plug is intended to represent the lower hole limit. Its nominal size is therefore near 50.000 mm, with the manufacturing and wear zones placed according to the selected gauge standard. The NO-GO plug is intended to represent 50.025 mm, with its own gauge tolerance but normally no working wear allowance.

This example demonstrates the design logic, but it does not justify a universal numerical placement rule. Gauge dimensions must be calculated from the current standard because the direction and distribution of gauge-maker’s tolerance affect consumer and producer risk.

6. Measurement, Uncertainty and Good Practice

A limit-gauge decision is meaningful only when the gauge, part and environment are controlled. Steel components and gauges should approach the reference temperature because thermal expansion changes size. For a uniform component:

where ∆L is dimensional change, α is the coefficient of linear thermal expansion in K⁻¹, L₀ is the reference length and ∆T is temperature change in kelvin or degrees Celsius.

For a 100 mm steel dimension with α = 11.5 × 10⁻⁶ K⁻¹ and a 10 °C temperature increase:

This is significant when the tolerance is only a few micrometres. Parts and gauges should be clean, free from burrs, and checked without excessive force. A gauge should never be forced through a part. Gauges must be calibrated at defined intervals and verified more frequently where wear, contamination or high usage is expected.

Limit gauging is efficient but cannot diagnose the amount or direction of error. Variable instruments such as bore gauges, micrometers, air gauges and coordinate measuring machines are needed for process adjustment, capability studies and root-cause analysis.

7. Applied Case: Inspection of a Bearing Housing

Background

This illustrative case concerns a bearing housing with a 60 H7 bore and a shaft intended to rotate in the bearing. The bore must accept a standard bearing outer ring without damaging the bearing or producing excessive looseness.

Problem

Production operators report that some housings pass a basic plug gauge but later produce variable bearing fits. Investigation shows that the gauge confirms size but gives little information about taper, ovality, temperature or surface damage.

Analysis

The engineer first obtains the exact ISO limits for the 60 H7 bore. A calibrated full-form GO plug is selected for the lower bore limit, and a NO-GO plug is selected for the upper limit. The bore is also checked at several axial and angular positions with a calibrated variable bore instrument. This separates size error from form error.

The inspection plan identifies four risks:

1. a worn GO plug may accept an undersize bore;
2. excessive force may produce a false gauge decision;
3. a hot housing may contract after inspection and alter the fit;
4. a two-point measurement may miss lobing or taper.

Approach and solution

The company introduces temperature conditioning at 20 °C, cleaning and deburring before gauging, a gauge usage log, periodic calibration and a wear limit for the GO plug. The GO plug checks complete entry, while the NO-GO plug is applied with light hand pressure and must not enter beyond the specified depth. A sampling plan adds variable measurements at three axial sections and two perpendicular directions.

Process data are plotted by machine and tool life. A gradual bore reduction is traced to reamer wear. Tool replacement is scheduled before the GO gauge begins to accept nonconforming parts.

Outcome

The revised system retains the speed of limit gauging while adding variable inspection for process control. False acceptance is reduced, bearing assembly becomes consistent and the inspection records support corrective action rather than merely sorting parts.

Learning points

• A gauge checks conformity, not the complete geometry of a feature.
• Taylor’s principle is functional, not merely a naming convention.
• Gauge wear and temperature can be as important as nominal gauge size.
• Variable measurement is required when process diagnosis or form control is important.

8. Design, Quality and Professional Considerations

Tolerance selection is an economic decision. Tight tolerances may improve interchangeability but increase machining, inspection and scrap costs. Loose tolerances reduce cost only when function permits them. The designer should specify the least restrictive tolerance that guarantees performance.

Drawings should state the applicable standards, units, material condition, datum system, surface texture and temperature reference. Ambiguous drawings cause inconsistent acceptance decisions. Quality systems should control gauge identification, calibration status, traceability, storage, cleaning and out-of-calibration impact assessment.

Digital manufacturing and coordinate measuring machines support detailed analysis, while automated vision and in-process probing can detect trends earlier. Artificial intelligence may assist with tool-wear prediction or anomaly detection, but it does not replace traceable calibration, validated measurement methods or engineering responsibility. Any automated acceptance system must have documented uncertainty, validation data and access control.

Chapter Summary

Limits define the acceptable upper and lower sizes of a feature, while tolerance is the difference between those limits. Deviations locate the tolerance zone relative to the basic size, and allowance defines the intended minimum clearance or maximum interference between mating parts. ISO fits use uppercase hole letters, lowercase shaft letters and IT grades to standardize tolerance zones.

Clearance, transition and interference fits are evaluated from the extreme combinations of hole and shaft limits. Tolerance stacks may be analysed by conservative worst-case addition or by statistical methods when distribution, independence and process capability assumptions are justified. Taylor’s principle requires a full-form GO gauge to assess maximum material condition and a NO-GO gauge to assess the relevant opposite limit without over-constraining the part.

Plug, ring and snap gauges provide rapid production decisions, but their accuracy, wear, temperature, force and calibration must be controlled. Gauging should be supplemented by variable measurement when form, process trends or root causes must be evaluated.

Key Terms

Basic size: The theoretical size from which limits and deviations are derived.

Actual size: The measured size of a manufactured feature.

Upper limit: The largest permissible feature size.

Lower limit: The smallest permissible feature size.

Tolerance: The numerical difference between upper and lower limits.

Deviation: The algebraic difference between a limit and the basic size.

Fundamental deviation: The deviation nearest the zero line.

Allowance: The intentional minimum clearance or maximum interference between mating features.

Hole-basis system: A system in which the hole’s lower deviation is zero.

Shaft-basis system: A system in which the shaft’s upper deviation is zero.

Clearance fit: A fit having positive clearance in all permitted combinations.

Transition fit: A fit that may produce clearance or interference.

Interference fit: A fit having interference in all permitted combinations.

IT grade: An ISO grade defining tolerance magnitude.

Maximum material condition: The condition containing the greatest amount of material.

Taylor’s principle: The functional rule governing GO and NO-GO limit gauges.

Plug gauge: A gauge used primarily to inspect holes.

Ring gauge: A gauge used primarily to inspect external cylindrical features.

Snap gauge: A gauge with fixed or adjustable anvils for rapid external inspection.

Gauge-maker’s tolerance: The permitted manufacturing variation of a gauge.

Review Questions

Short Answer Questions

1. Define basic size, actual size and tolerance.
2. Distinguish allowance from tolerance.
3. What is the difference between a hole-basis and a shaft-basis system?
4. State Taylor’s principle for GO and NO-GO gauges.
5. Why should gauges and workpieces be temperature-conditioned?

Long Answer Questions

1. Explain clearance, transition and interference fits, including the limit conditions that distinguish them.
2. Describe ISO tolerance grades and the meaning of a designation such as H7/g6.
3. Explain worst-case and statistical tolerance stack-up and state the assumptions of each.
4. Describe the construction and application of plug, ring and snap gauges.
5. Discuss gauge-maker’s tolerance, wear allowance, calibration and measurement uncertainty.

Analytical / Application Questions

1. A hole has limits 30.000–30.021 mm and a shaft has limits 29.990–30.005 mm. Calculate maximum clearance, minimum clearance and classify the fit.
2. An assembly dimension is Y = A − B − C, where A = 100.00 ± 0.08 mm, B = 45.00 ± 0.04 mm and C = 20.00 ± 0.02 mm. Determine the nominal value and worst-case limits of Y.
3. Design an inspection plan for a precision bore that uses a full-form GO plug, a NO-GO plug and variable measurements. Explain how you would control temperature, gauge wear, calibration and false acceptance.

Multiple Choice Questions with Answers

Question 1

A shaft has limits 25.000 mm and 24.980 mm. What is its tolerance?

A. 0.002 mm

B. 0.020 mm

C. 0.200 mm

D. 24.990 mm

Correct Answer: B. 0.020 mm

Question 2

For an H hole in the hole-basis system, which deviation is normally zero?

A. Upper deviation

B. Mean deviation

C. Lower deviation

D. Fundamental shaft deviation

Correct Answer: C. Lower deviation

Question 3

A fit has a minimum clearance of 0.005 mm and a maximum clearance of 0.041 mm. What type of fit is it?

A. Interference

B. Transition

C. Clearance

D. Unclassified

Correct Answer: C. Clearance

Question 4

For a hole, the GO plug gauge approximately represents which material condition?

A. Minimum material condition

B. Maximum material condition

C. Mean material condition

D. Zero material condition

Correct Answer: B. Maximum material condition

Question 5

Which gauge is primarily used to inspect an external cylindrical shaft?

A. Plain plug gauge

B. Ring gauge

C. Bore gauge only

D. Thread tap gauge

Correct Answer: B. Ring gauge

Question 6

If independent dimensions have standard deviations σ₁ and σ₂, their root-sum-square combined standard deviation is:

A. σ₁ + σ₂

B. σ₁σ₂

C. √(σ₁² + σ₂²)

D. σ₁² − σ₂²

Correct Answer: C. √(σ₁² + σ₂²)

Question 7

A gap is G = A − B − C, with nominal A = 80 mm, B = 30 mm and C = 20 mm. What is the nominal gap?

A. 10 mm

B. 30 mm

C. 50 mm

D. 130 mm

Correct Answer: B. 30 mm

Question 8

What is the principal purpose of a NO-GO gauge?

A. To measure the exact size numerically

B. To check that a feature has not exceeded the opposite permissible limit

C. To correct the machine tool

D. To measure surface roughness

Correct Answer: B. To check that a feature has not exceeded the opposite permissible limit

Question 9

For a uniform component, dimensional thermal expansion is represented by:

A. ∆L = αL₀∆T

B. ∆L = α/(L₀∆T)

C. ∆L = L₀/(α∆T)

D. ∆L = α + L₀ + ∆T

Correct Answer: A. ∆L = αL₀∆T

Question 10

Why is variable measurement often added to limit gauging?

A. To eliminate all tolerances from the drawing

B. To diagnose size trends and form errors

C. To make calibration unnecessary

D. To replace the need for a datum system

Correct Answer: B. To diagnose size trends and form errors