Dimensional Tolerancing Basics

A dimension on a drawing is a wish; the tolerance says how far the real part may be from that wish and still work. Every manufactured size varies, so the question is never whether to allow variation but how much, in which direction, and how the dimensions are arranged so the variation does not add up. This page covers the vocabulary and the conventions that every other page in the Fits & Tolerances guide builds on. Terms follow the Machinery’s Handbook and ASME B4.1; where ISO differs, it is noted.

The terms

Term	Meaning	Example
Nominal size	The name used for general identification	“1 inch”, “M10”, “25 mm”
Basic size	The size from which the limits of size are derived by applying allowances and tolerances	25.000 mm
Design size	The basic size with any allowance applied; the size the tolerance is added to. With no allowance, it equals the basic size	24.990 mm for a shaft with a 0.010 mm allowance
Limits of size	The largest and smallest sizes permitted for a feature	25.021 and 25.000 mm
Tolerance	The total permitted variation in a size: the maximum limit minus the minimum limit. It has no sign	25.021 − 25.000 = 0.021 mm
Allowance	A prescribed difference between the maximum-material limits of two mating parts: the tightest fit that will occur (minimum clearance, or maximum interference)	Smallest hole minus largest shaft
Deviation	The difference between a limit and the basic size (ISO uses ES/EI for a hole and es/ei for a shaft)	+0.021 and 0
Maximum material limit	The limit of size that leaves the most material: the largest shaft, or the smallest hole	See Modifiers and Material Conditions

The words tolerance and allowance are often swapped in conversation, but they are different things. A tolerance is how much one part may vary. An allowance is the intended difference between two mating parts. A fit is the result of both.

Ways to write a tolerance

Form	Example	Allowed sizes	Notes
Limit dimensions	25.10 25.00	25.00 to 25.10	Clearest to read and inspect: both limits are on the drawing, with no arithmetic. The larger limit is placed on top for external and internal features alike
Unilateral	25.00 +0.10−0.00	25.00 to 25.10	All the tolerance is on one side of the basic size. The Handbook recommends unilateral tolerances for mating surfaces
Bilateral, equal	25.00 ± 0.05	24.95 to 25.05	The tolerance is split evenly. Compact; common for sizes where a deviation in either direction is equally harmful
Bilateral, unequal	25.00 +0.08−0.02	24.98 to 25.08	Both signs, unequal amounts. Used when the design size is not the middle of the range

The Handbook lists three correct ways to express unilateral tolerances on mating parts: state the limiting dimensions only (hole 2.250 to 2.252, shaft 2.249 to 2.247 inch), state one limit with its tolerance (hole 2.250 +0.002 −0.000, shaft 2.249 +0.000 −0.002), or state the nominal size for both parts with a notation for each (hole 2¼ +0.002 −0.000, shaft 2¼ −0.001 −0.003). Whichever you use, use it consistently on the drawing.

Unilateral or bilateral?

The Handbook’s rule is a good starting point: apply the tolerance in the direction that does less harm. If variation in either direction is equally harmful, split it evenly (bilateral). If one direction is worse than the other, put the tolerance in the safe direction (unilateral).

Situation	Use	Why
Mating surfaces: a shaft in a hole	Unilateral	The worst case is easy to control: the smallest hole is the basic size, the largest shaft is the basic size, and the tolerance runs away from them. Also the most economical, because standard tools and stock then give the basic size (see below)
Distance between two holes or two features	Bilateral	Too far and too near are usually equally harmful
Distance between two shafts that carry gears	Unilateral, plus	If the shafts are too close the gears run tight and bind; a slight increase in backlash is seldom important
Non-mating surfaces	Either	Choose the one that suits the process and inspection
Tapered mating surfaces	Depends	Bilateral if a deviation in or out is equally harmful; otherwise unilateral toward the less harmful direction

The Handbook adds a cost rule. The minimum hole should be the basic size wherever standard tools (drills, reamers) make the hole, and the maximum shaft should be the basic size wherever standard purchased stock is used without further machining, even if special tools are needed for the mating part. This is the origin of the hole-basis and shaft-basis systems on the How Fits Work page.

On a drawing, give the initial clearance as small as the mechanism will permit and the maximum clearance as great as it will tolerate. Setting the first dimension at the exact, tolerance-free value you would use if you could work without tolerances, and then adding tolerance in the safe direction, is the simplest way to avoid mistakes.

Chain or baseline dimensioning

The Handbook gives the rule: only one dimension in the same straight line can be controlled within fixed limits, and it is incorrect to locate any point or surface with tolerances from more than one point in the same line. Dimensions should run between the points that must hold a relation to each other, and it is good practice to establish a common locating point in each plane and dimension from it. The locating points on the drawing, the points used to machine, and the points used to measure should all be the same.

Position from the left edge	Chain, worst case	Chain, RSS	Baseline
Hole 1 (20 mm from the edge)	± 0.10	± 0.100	± 0.10
Hole 2 (40 mm from the edge)	± 0.20	± 0.141	± 0.10
Hole 3 (60 mm from the edge)	± 0.30	± 0.173	± 0.10
Hole 4 (80 mm from the edge)	± 0.40	± 0.200	± 0.10

Every dimension in the example is 20 ± 0.1. In the chain, the position error of hole k is the sum of k tolerances: worst case k × 0.1, or √k × 0.1 if the errors are independent and centered (RSS: root sum of squares, covered on the Tolerance Stack-up Analysis page). From a baseline, each hole is ± 0.1 whatever its distance. The trade-off is that neighboring holes can differ by up to 2 × 0.1 = ± 0.2 from the baseline, while in the chain neighbors are controlled to ± 0.1 directly. Choose the scheme by the relationship that matters: if holes must match a mating part, use the baseline; if they must match each other, dimension them from each other.

Decimal places and conversions

• State the tolerance; do not rely on decimals. The number of decimal places in a dimension does not, by itself, tell the inspector the tolerance, unless a general tolerance note says it does (see General Tolerances and Drawing Notes).
• “0.1” is ambiguous. In a note, “0.1 mm” can mean ± 0.1 (a total band of 0.2) or a total band of 0.1. Always write the sign, or say “total”.
• Converting inch to millimeter. Convert the limits of size, not the tolerance, and round the result inward (toward the middle of the range) so the converted part can never be looser than the original. A tolerance of ± 0.002 in becomes ± 0.0508 mm, which you would write as ± 0.05 mm: slightly tighter, never looser.
• Keep the digits consistent. A size and its tolerance should show the same number of decimal places, for example 25.00 ± 0.05, not 25 ± 0.05.

What “size” means: ASME and ISO

A real cylinder is never perfectly round or straight, so “its size” needs a definition. Under ASME Y14.5 (the US standard), Rule #1 says the limits of size also control form: a feature at its maximum material size must have perfect form, and the actual size at any cross-section must lie within the limits. A shaft toleranced 25.000 to 24.979 therefore cannot be bent beyond a perfect 25.000 cylinder envelope. ISO 8015 works the other way: size and form are independent unless the drawing asks for an envelope. ISO 14405-1 defines the different ways size can be measured (two-point, spherical, calculated and others) and the symbols that select them, with two-point local size as the default. This difference matters whenever a drawing crosses a border; see the Form Tolerances page for Rule #1 in detail.

How tight should it be?

• Start from function. The least clearance that still lets the part assemble or move, and the most that still lets it work, set the combined tolerance of the two mating parts. Split it between the parts in proportion to how hard each is to make.
• Match the process. Each process makes parts within a band of tolerances (the Tolerances by Process and Surface Finish page has the Handbook’s table). Asking for a grade finer than the process can hold means an extra operation such as grinding or honing, with the cost that comes with it.
• Leave room to measure. The gage or instrument should be several times more accurate than the tolerance (a ratio of 4 or 10 to 1 is the usual target). A tolerance too small to measure cannot be enforced.
• Do not tolerance what does not matter. A bracket hole that only needs to clear a bolt does not need the tolerance of a bearing bore.

Worked examples

Example 1: reading a tolerance

A shaft has a maximum limit of 2.000 inches and a minimum limit of 1.990 inches (the Handbook’s own example).

• Tolerance = 2.000 − 1.990 = 0.010 inch.
• As a unilateral tolerance on a 2.000 basic size: 2.000 +0.000 −0.010.
• As an equal bilateral tolerance: 1.995 ± 0.005 (the design size moves to the middle of the range).

Example 2: converting a tolerance

A feature is 2.000 ± 0.002 in. Its limits are 1.998 and 2.002 in, which are 50.749 and 50.851 mm.

• Rounded inward to two decimals: 50.80 − 0.05 … 50.80 + 0.05 gives 50.75 to 50.85 mm, which is the same as 50.80 ± 0.05 mm.
• Check: 50.75 mm is 1.9980 in and 50.85 mm is 2.0020 in, both inside the original 1.998 to 2.002 in range. The metric version is slightly tighter, never looser.

Example 3: how a chain builds up error

A plate has five holes, each dimensioned 25 ± 0.1 mm from the one before it (a chain). The position of the fifth hole, 125 mm from the edge, is the sum of five dimensions.

• Worst case: 5 × 0.1 = ± 0.50 mm.
• RSS: √5 × 0.1 = ± 0.224 mm (assumes independent, centered errors).
• If the fifth hole must be within ± 0.15 mm of the edge, the chain cannot guarantee it. Dimensioning every hole from the edge (a baseline) gives each hole ± 0.1 directly.

Troubleshooting

Symptom	Likely cause	Try
Holes line up with each other but not with the mating part	Chain dimensioning: errors have accumulated	Dimension from a common baseline
Two inspectors disagree	The tolerance is not stated, or “0.1” is ambiguous	Write the sign and the same number of decimals; state limits
Parts bind at the tight end of the tolerance	Bilateral tolerance on a mating surface	Make it unilateral, away from the basic size
Converted drawing rejects good parts	Tolerance converted by rounding the wrong way	Convert the limits and round inward
Supplier says it cannot be made	Tolerance grade is finer than the process	Check the process table; loosen it or add an operation

Related

• Fits & Tolerances: the overview and quick reference.
• General Tolerances and Drawing Notes: what applies when no tolerance is written.
• How Fits Work: clearance, transition and interference, hole and shaft basis.
• Modifiers and Material Conditions: MMC, LMC and bonus tolerance in the GD&T guide.
• Inspection and Tolerance Stack-up: measuring and the basic worst-case and RSS stack.

FAQ

Is a tolerance the same as an allowance?

No. A tolerance is the permitted variation in one size. An allowance is the prescribed difference between two mating parts, such as the minimum clearance. Together they determine the fit.

Should I use bilateral or unilateral tolerances?

Use unilateral for mating surfaces and anywhere one direction of error is worse than the other. Use bilateral for distances between features where too much and too little are equally bad. The Handbook recommends unilateral tolerances on mating surfaces wherever possible.

What is the difference between nominal and basic size?

The nominal size is a general name (1 inch, M10). The basic size is the actual reference value the limits are measured from. For an ISO or ANSI fit they are usually the same number.

Why does the Handbook say “minimum hole = basic size”?

Standard drills and reamers cut holes at fixed sizes, so a hole that starts at the basic size and gets larger only by tool wear is cheap to make. A shaft is easily turned or ground to any size, so it takes the tolerance. This is the hole-basis system.

Do I round a converted tolerance up or down?

Convert the limits of size, then round toward the inside of the range. That way the converted part is never looser than the original.

Is the number of decimals a tolerance?

Only if the drawing says so. Many drawings give a general tolerance by decimal places in the title block, but without that note the decimals mean nothing. See the General Tolerances page.

References

• Machinery’s Handbook, 31st edition, Industrial Press: “Allowances and Tolerances for Fits” (limits and fits: basic dimensions, tolerances, unilateral and bilateral tolerances, application of tolerances, locating tolerance dimensions, direction of tolerances on gages).
• ANSI/ASME B4.1, Preferred Limits and Fits for Cylindrical Parts (definitions of nominal, basic and design size, allowance, tolerance and fit; the 1967 edition, reaffirmed 2009, is listed as out of print in the Handbook).
• ASME Y14.5-2018, Dimensioning and Tolerancing.
• ISO 8015, Fundamentals: concepts, principles and rules; ISO 14405-1, Dimensional tolerancing: linear sizes.

Last reviewed: October 2026. Standards editions change; check the edition named on your drawing.