Engineering Tolerances Explained: How to Read Limits, Fits & Stack-Up

What an Engineering Tolerance Actually Means

No part is ever manufactured to its exact drawing dimension. Cutting tools wear, machines flex, material springs back, and every measurement carries its own uncertainty. A tolerance is the designer’s statement of how much of that variation is acceptable before the part stops doing its job. When a drawing says 25 ±0.1 mm, it is not asking for 25 mm — it is saying that anything between 24.9 mm and 25.1 mm will function and must be accepted.

That makes a tolerance a contract between three people: the designer who decides what the part needs, the machinist who has to hold it, and the inspector who decides whether it ships. Read it wrong and you either scrap good parts or assemble bad ones. This guide walks through the notation you will see on real drawings, the ISO fit codes that replace it on mating features, how tolerances accumulate across an assembly, and how to pick numbers a workshop can actually hit.

How to Read Tolerance Callouts on a Technical Drawing

Four notations cover almost everything you will meet on a mechanical drawing. They express the same idea — an upper limit and a lower limit — in different ways.

1. Symmetric bilateral: 25 ±0.1

Variation is allowed equally in both directions. Limits are 25.1 mm and 24.9 mm, and the total width of the tolerance is 0.2 mm. This is the default for non-critical features.

2. Unequal bilateral: 25 ^+0.15_−0.05

Both directions are allowed, but not by the same amount. Limits are 25.15 mm and 24.95 mm. The nominal size is no longer the middle of the range — the true centre is 25.05 mm, which matters when you set up the machine.

3. Unilateral: 25 ^+0.021₀

Variation is permitted in one direction only. Limits are 25.021 mm and 25.000 mm. This is standard on features that mate with something else, because it guarantees the part never crosses the nominal line.

4. Limit dimension: 25.021 / 25.000

Both limits are written out and no nominal appears at all. It leaves nothing to interpretation, which is why inspection departments like it.

One more thing to check before you trust any of these: the general tolerance note in the title block. Most drawings carry something like “ISO 2768-m unless otherwise specified”, which silently applies a tolerance to every dimension that has no explicit one. On imperial drawings the same job is often done by decimal places — .X = ±0.05", .XX = ±0.01", .XXX = ±0.005" is a common convention. A dimension written 2.500" instead of 2.5" can therefore be ten times tighter, with nothing else on the drawing to warn you.

Bilateral vs Unilateral Tolerance: When to Use Each

The choice is not stylistic. It changes where the manufacturing target sits and how the part behaves at the extremes of its range.

• Use bilateral for free-standing features — overall lengths, non-mating widths, cosmetic dimensions. Anywhere drift in either direction is equally harmless.
• Use unilateral for mating features — shafts, bores, keyways, spigots. A shaft toleranced ⁰_{−0.02 can only ever be at or below nominal, so a hole cut at nominal will always accept it.}
• Use unequal bilateral when one direction is more dangerous than the other — for example a sealing face that may sit slightly proud but must never sink below flush.

Unilateral tolerancing is also the logic behind the hole-basis system used by ISO fits: the hole is always toleranced from nominal upwards (its lower limit is the nominal size), and the fit is then tuned entirely by moving the shaft. That is deliberate — holes are cut with fixed-size tooling like reamers and drills, while a shaft can be turned to any diameter you like. Adjusting the cheap side of the pair is simply good engineering economics.

How to Calculate Maximum, Minimum, and Tolerance Width

Whatever notation the drawing uses, the arithmetic is the same. Add each deviation to the nominal size, keeping the sign, and the two results are your limits:

• Maximum limit = nominal + upper deviation
• Minimum limit = nominal + lower deviation
• Tolerance width = maximum − minimum
• Mid-limit (target size) = (maximum + minimum) ÷ 2

The mid-limit is the number people forget. Aiming at nominal on a unilateral tolerance puts you hard against one limit before you have made a single part, so the first sign of tool wear produces scrap. Aiming at the mid-limit gives you variation room on both sides.

A tolerance of 21 µm sounds tight until you note that a human hair is roughly 70 µm across — the whole allowed range is under a third of a hair’s width. That is routine for a ground or precision-turned feature and impossible for a saw cut, which is exactly why the number has to match the process.

What ISO Fit Codes Like 25H7/g6 Actually Mean

On mating features, drawings usually drop explicit deviations and use an ISO 286 fit code instead. It looks cryptic but carries exactly the same information in four characters:

• The letter sets the position of the tolerance zone relative to nominal — how far above or below the line it sits. Uppercase letters (H, G, K, P) describe holes; lowercase (h, g, k, p) describe shafts.
• The number is the IT grade, which sets the width of the zone. Lower numbers are tighter. The same grade means a wider tolerance on a big feature than on a small one, because ISO scales grades with size.

So 25H7/g6 reads as: a 25 mm nominal pair, the hole at position H (lower limit exactly on nominal) with grade 7 width, running against a shaft at position g (slightly below nominal) with the tighter grade 6 width. For the 18–30 mm size band, ISO 286 gives IT7 = 21 µm and IT6 = 13 µm, and the g shaft position an upper deviation of −7 µm:

Because the smallest possible hole is still larger than the largest possible shaft, every single combination of parts assembles with clearance. That guarantee — not the individual numbers — is the point of the code.

Clearance, Transition, and Interference Fits Compared

Change only the shaft letter and the same 25H7 hole produces three completely different mechanical relationships.

Clearance fit — the parts always slide

The shaft is always smaller than the hole. H7/g6 gives 0.007–0.041 mm of clearance: close enough to locate accurately, loose enough to slide by hand. Looser grades like H7/f7 suit plain bearings that need room for an oil film, while H7/h6 is the classic “sliding but snug” location fit.

Transition fit — it depends which two parts you pick

The zones overlap, so some pairs assemble with a small clearance and others with a small interference. H7/k6 (shaft 25.002–25.015) ranges from 0.019 mm clearance to 0.015 mm interference. H7/n6 (shaft 25.015–25.028) leans harder toward interference. Both are used where accurate centring matters more than easy assembly — gears on shafts, dowelled locations — and both normally need a press or a soft mallet.

Interference fit — the parts are always tight

The shaft is always larger than the hole. H7/p6 (shaft 25.022–25.035) gives 0.001–0.035 mm of interference, so the joint is held by elastic deformation of the material and transmits torque without a key. These cannot be pushed together by hand: you press them, or you heat the outer part and shrink-fit it. Be aware that an interference fit puts real hoop stress into the surrounding material — thin-walled hubs can split.

One practical warning: the fit is a property of the pair, not of either part. An in-tolerance hole and an in-tolerance shaft can still give you the loosest assembly in the range, and that worst case is the one your design has to survive.

IT Tolerance Grades vs What Each Machining Process Can Hold

ISO 286 defines twenty IT grades, from IT01 (gauge blocks) to IT18 (rough castings). For the 18–30 mm band, the grades most drawings use come out like this:

• IT5 = 9 µm — precision grinding, high-accuracy bearing seats
• IT6 = 13 µm — ground or fine-turned shafts, the standard partner for an H7 hole
• IT7 = 21 µm — reamed and bored holes; the everyday choice for located features
• IT8 = 33 µm — good general turning and milling
• IT9–IT11 = 52 to 130 µm — general machining, drilled holes, non-critical work

Those numbers only mean something next to what a process can repeatably deliver. Typical capability, in ±mm, assuming a competent shop and a moderate part size:

• Sand casting or flame cutting: ±0.5 to ±1.5
• FDM 3D printing: ±0.2 to ±0.5
• Laser or waterjet cutting: ±0.1 to ±0.3
• General milling and turning: ±0.05 to ±0.13
• Precision CNC turning and boring: ±0.013 to ±0.025
• Cylindrical grinding: ±0.005 to ±0.013
• Honing and lapping: ±0.001 to ±0.005

The rule that follows is simple: never specify a tolerance tighter than the process that will make the feature. A ±0.01 mm callout on a milled surface does not make the shop more careful — it forces a secondary grinding operation, or it gets quietly ignored and the parts pass anyway. Both outcomes cost you something. Ranges also widen with part size and material: the same grade is far harder to hold on a 500 mm aluminium extrusion than on a 25 mm steel pin.

Tolerance Stack-Up: Worst-Case vs RSS Analysis

Individual parts pass inspection and the assembly still does not fit. That is tolerance stack-up — the accumulation of variation along a chain of dimensions. There are two standard ways to add it up, and they give very different answers.

Worst-case (arithmetic) stack-up

Assume every part lands at its worst limit simultaneously, and simply add the tolerances:

This guarantees 100% interchangeability — if the design works at ±0.20, no assembly can ever fail. It is the right method for safety-critical work, for low volumes, and any time a failed assembly is expensive to discover. The cost is that it is pessimistic: with four independent parts, all four hitting the same extreme is vanishingly rare.

Statistical (RSS) stack-up

Root-sum-square treats the variations as independent random variables and adds them in quadrature — the square root of the sum of the squares:

RSS buys back half the tolerance in this example, which is often the difference between a routine part and an expensive one. But it rests on assumptions you must actually check: the dimensions are independent, each process is centred on its mid-limit, and the distributions are roughly normal. A supplier whose parts all sit at one limit — common when a tool is worn or the operator aims at nominal — destroys the statistics, and a small percentage of assemblies will fall outside the RSS range by design. Use RSS on high-volume production where you can afford to rework the tail; use worst-case when you cannot.

Two habits make stack-ups far less painful: keep the dimension chain short by referencing features to a single datum instead of chaining them nose-to-tail, and spend your tight tolerances only on the two or three dimensions that actually drive the critical gap.

Why Tighter Tolerances Cost More Money

Tolerance cost does not rise smoothly — it rises in steps, because each step demands a different manufacturing reality:

• A new operation. Going from ±0.05 to ±0.01 mm can mean adding a grinding pass after turning: another setup, another machine, another queue in the shop.
• Slower cutting. Lighter finishing passes, more spring passes, and lower feeds mean fewer parts per hour.
• More inspection. Loose tolerances get sampled; tight ones often get 100% inspected, sometimes on a CMM with its own queue and its own operator.
• Better metrology. A tolerance you cannot measure reliably is not controlled. Tight callouts pull in gauges, fixtures, and calibration you may not own.
• Higher scrap. As the tolerance band narrows toward the process capability, the fraction of parts falling outside it climbs sharply — and scrap on a finishing operation throws away all the value added before it.
• Environmental control. At single-digit micron levels the shop itself has to be temperature-stabilised.

The discipline that follows is worth building into every drawing review: for each tight tolerance, ask what physically fails if it is doubled. If nobody can answer, it is probably a habit rather than a requirement. Tight tolerances inherited by copy-paste from an old drawing are one of the most common avoidable costs in mechanical design.

GD&T vs Plus/Minus Tolerancing: What Geometric Tolerances Add

Plus/minus tolerancing controls size. It says nothing about whether a face is flat, whether two bores are parallel, or where a hole pattern sits relative to the surfaces that actually locate the part. Geometric Dimensioning and Tolerancing (GD&T), defined by ASME Y14.5 and ISO 1101, fills that gap by adding controls for form, orientation, location, and runout, all referenced to explicitly named datums.

The clearest illustration is hole location. Tolerancing a hole ±0.1 mm in X and Y creates a square 0.2 × 0.2 mm zone of acceptable positions. A GD&T position callout creates a round zone instead. The circle that circumscribes that square is ø0.283 mm — and it has about 57% more area, meaning parts that were functionally fine but failed the square check now pass. Same function, more yield, no extra manufacturing cost.

GD&T also introduces the maximum material condition bonus: when a hole is made larger than its tightest size, the extra material removed can be traded for additional position tolerance, because a bigger hole genuinely tolerates more misalignment. For a drawing reader, the practical takeaway is that a feature control frame is not simply a stricter version of a ± dimension — it controls a different property, and the two coexist on the same feature.

How Temperature, Measurement, and Setup Distort Real Tolerances

A tolerance is only real if it survives the conditions in which the part is measured and used.

Temperature

ISO 1 defines 20 °C as the standard reference temperature for all dimensional specifications, and for good reason. Steel expands about 11.7 µm per metre per °C; aluminium roughly 23. A 200 mm aluminium part measured 10 °C above reference is 200 × 23 × 10⁻⁶ × 10 ≈ 0.046 mm longer — larger than many tolerances on the drawing. A part machined warm and inspected cold can fail against nothing but physics, and a steel shaft in an aluminium housing changes its fit across the operating temperature range.

Measurement uncertainty

Your gauge consumes part of the tolerance band. The classic rule of ten says the measuring instrument should be about ten times more precise than the tolerance being checked; modern practice often accepts 4:1. Checking a 0.02 mm tolerance with a caliper that resolves 0.02 mm means you are not really measuring it — you are guessing, and both false accepts and false rejects follow.

Fixturing, burrs, and finish

Thin walls deflect under clamping and spring back once released, so a part can be in tolerance in the vice and out of tolerance on the bench. A burr adds material exactly where a caliper touches. And on a rough surface, a micrometre anvil rides the peaks while a bore gauge finds the valleys — below about 10 µm of tolerance, surface finish stops being cosmetic and becomes part of the dimension.

Common Mistakes When Reading or Specifying Tolerances

• Ignoring the general tolerance block. Every unmarked dimension still has a tolerance, and it is not always the one you assume.
• Machining to nominal on a unilateral tolerance. On 25 ^+0.021₀ the nominal sits on a limit; aim for the mid-limit instead.
• Treating nominal as the centre of an unequal bilateral tolerance. On 25 ^+0.15_−0.05 the true target is 25.05 mm.
• Adding tolerances along a chain. Five chained dimensions at ±0.1 give ±0.5 at the far end. Reference to a datum instead.
• Copying tolerances from an old drawing. Inherited tightness with no functional reason is pure cost.
• Specifying tighter than the process. A ±0.005 mm callout on a laser-cut edge cannot be met.
• Forgetting that fit is a property of the pair. Two in-tolerance parts can still land at the worst combination in the range.
• Mixing hole-basis and shaft-basis systems in one assembly, which quietly changes what the fit codes mean.
• Assuming RSS applies. If the supplier’s process is off-centre or the dimensions are correlated, statistical stack-up understates the real variation.

Run the Numbers on Your Own Dimensions

The arithmetic behind limits and fits is not difficult, but it is easy to slip a sign or a decimal place when you are converting micron-level deviations into millimetres at the end of a long day. Our free tolerance calculator works out maximum and minimum limits, tolerance width, and mid-limit for a single part, and for a shaft-and-hole pair it identifies whether the result is a clearance, transition, or interference fit along with the maximum and minimum clearance.

Specify what the part actually needs, match the number to a process that can hold it, and check the stack-up before anything is cut. Do those three things and most fit problems disappear before they reach the shop floor.