ISO 286 Tolerance & Fit Guide: How to Select Shaft/Hole Fits for Machining

What ISO 286 Is and Why It Exists

ISO 286 is an international standard that defines a system of limits and fits for mating parts. It answers a fundamental question in manufacturing: if I make a shaft in one shop and a hole in another shop, what dimensions should each be held to so that they fit together the way I need?

Before standardized tolerance systems, every shop defined fits their own way. A "slip fit" in one shop might be a "light press fit" in another. Drawings would say "grind to fit" or "machine to match," which meant the parts had to be made together and couldn't be interchanged. ISO 286 (and its predecessor ISA/BS systems) solved this by defining tolerance zones relative to the nominal size, using a letter-number code that any machinist anywhere in the world can interpret.

The system has two components: the fundamental deviation (a letter that defines where the tolerance zone sits relative to the nominal size) and the IT grade (a number that defines how wide the tolerance zone is). Together, they create a tolerance zone. A shaft tolerance like g6 means the shaft will be slightly undersized (fundamental deviation "g") with a tight tolerance band (IT grade 6). A hole tolerance like H7 means the hole will be at or slightly above nominal (fundamental deviation "H") with a moderate tolerance band (IT grade 7).

The beauty of the system is that fits are standardized. An H7/g6 fit produces the same type of clearance whether the nominal size is 10mm or 100mm. The actual tolerance values scale with size, but the fit characteristic remains consistent.

Understanding Tolerance Notation

An ISO 286 tolerance is written as a letter followed by a number: H7, g6, k5, P7, js6, etc. The letter indicates the fundamental deviation — how far the tolerance zone is shifted from the nominal (basic) size. The number indicates the IT grade — how wide the tolerance zone is.

Fundamental deviation letters for holes (uppercase): Letters A through H define holes that are larger than nominal (positive deviation). H is the most common — it means the hole's minimum size equals the nominal size. Letters J through N straddle nominal (some of the tolerance zone is above, some below). Letters P through ZC define holes that are smaller than nominal (negative deviation), used for interference fits.

Fundamental deviation letters for shafts (lowercase): Letters a through h define shafts that are smaller than nominal (negative deviation). h means the shaft's maximum size equals the nominal size. Letters j through n straddle nominal. Letters p through zc define shafts that are larger than nominal, used for interference fits.

The H/h baseline: H (hole at nominal minimum) and h (shaft at nominal maximum) are the baseline references. An H/h fit means the hole is at or above nominal and the shaft is at or below nominal — there is always clearance (or zero clearance at the extreme). Most fit specifications use an H-basis system, meaning the hole tolerance is fixed at H and the shaft letter is varied to achieve the desired fit type.

When you see a fit specified as H7/g6, it means: the hole is machined to H7 tolerance (at or slightly above nominal with IT7 precision) and the shaft is machined to g6 tolerance (slightly below nominal with IT6 precision). The combination of these two tolerance zones determines the minimum and maximum clearance (or interference) of the assembled fit.

Clearance, Transition, and Interference Fits

Every fit between a shaft and a hole falls into one of three categories based on whether there is always clearance, always interference, or sometimes one and sometimes the other.

Clearance fit: The shaft is always smaller than the hole. There is always a gap (clearance) between the two parts when assembled. The shaft can slide or rotate within the hole. Examples: H7/f6 (free running fit for bearings and pulleys), H7/g6 (sliding fit for precision slideways), H11/c11 (loose fit for agricultural and rough machinery). Clearance fits use shaft letters a through h paired with hole letter H.

Transition fit: The tolerance zones overlap. Depending on where in the tolerance band each part falls, the assembly might have a slight clearance or a slight interference. The fit is somewhere between sliding and light pressing. Examples: H7/k6 (locational transition — may need light tapping with a soft hammer), H7/n6 (tighter transition — usually requires a press or light heating). Transition fits use shaft letters j through n.

Interference fit (press fit): The shaft is always larger than the hole. Assembly requires pressing, heating the outer part, or cooling the inner part. The parts are held together by friction from the elastic deformation of the material. Examples: H7/p6 (light press fit for locating pins), H7/s6 (medium press fit for bearing seats), H7/u6 (heavy press fit for permanent assemblies). Interference fits use shaft letters p through zc.

The practical significance: if you specify the wrong fit type, the parts either won't go together (too much interference for your assembly method) or won't stay together (too much clearance for the application). A bearing that needs a light press fit on the shaft will spin and fret if you accidentally specify a clearance fit. A piston that needs a sliding fit will seize if you specify a transition fit.

Common Fit Selections with Real-World Examples

Here are the fits you'll encounter most often in industrial work, organized by application:

H7/g6 — Sliding fit: The workhorse of precision fits. Used for slideways, locating pilots, spigots, and any application where parts must slide or be positioned by hand but without noticeable play. Typical clearance is 0.005 to 0.030mm depending on the nominal diameter. This is the fit most machinists mean when they say "close sliding fit."

H7/f7 — Free running fit: Used for journal bearings, idler pulleys on shafts, and rotating parts that need lubrication clearance. The extra clearance (compared to g6) allows an oil film to form. Typical clearance is 0.020 to 0.060mm.

H7/k6 — Locational transition: The go-to fit for dowel pins and locating features where you want a snug fit that can be assembled and disassembled by hand (sometimes with a light tap). About half the time there's a slight clearance; half the time a very light interference.

H7/p6 — Light press fit: Used for bearing inner races on shafts, locating pins that must not move under load, and semi-permanent assemblies. Requires an arbor press or light hydraulic press to assemble. Can usually be disassembled without damage.

H7/s6 — Medium drive fit: Used for permanent bearing seats, gear hubs, and couplings that must transmit torque through friction alone. Requires a hydraulic press or thermal differential (heat the bore, cool the shaft) to assemble. Disassembly usually damages one or both parts.

H11/c11 — Loose running fit: Used for agricultural equipment, rough machinery, and applications with dirt, thermal expansion, or sloppy assembly. Large clearance accommodates misalignment and contamination.

IT Grades Explained: How Tight Is Tight Enough?

The IT (International Tolerance) grade is the number in the tolerance code. It defines the width of the tolerance band — how much variation is allowed. IT grades range from IT01 (tightest, used for gauge blocks) to IT18 (loosest, used for rough castings). The grades commonly used in machining are IT5 through IT11.

IT5-IT6: Precision grinding territory. Tolerance bands are measured in microns (thousandths of a millimeter). IT6 on a 25mm shaft means a tolerance width of 0.013mm (about half a thousandth of an inch). This level of precision requires grinding, honing, or very careful CNC turning with fine finishing passes. Used for bearing journals, precision fits, and high-speed rotating parts.

IT7: The standard grade for reamed holes and precision turned shafts. IT7 on a 25mm dimension is 0.021mm tolerance width. Achievable with carbide boring, reaming, or careful CNC turning. This is the most common grade for the hole in an H7/g6 fit.

IT8-IT9: Standard CNC milling and turning territory. IT9 on a 25mm dimension is 0.052mm (about 0.002 inches). Most CNC machines hold IT8-IT9 routinely without special effort. Used for general-purpose dimensions where fit is not critical.

IT10-IT11: Rough machining, drilling, and stamping. IT11 on a 25mm dimension is 0.130mm (about 0.005 inches). Achievable with manual machines, drill presses, and basic setups. Used for clearance holes, rough bores, and non-critical dimensions.

The key insight is that tighter IT grades cost more money. Going from IT9 to IT7 might double your machining time. Going from IT7 to IT5 might double it again and require grinding. Always specify the loosest IT grade that still meets your functional requirement. Over-tolerancing is the most common engineering mistake on drawings — it wastes machine time and increases scrap rates for no functional benefit.

Reading ISO 286 Tolerance Tables

ISO 286 tolerance tables list the upper and lower deviations (in micrometers) for each letter-grade combination at each nominal size range. To use them, you need three pieces of information: the nominal size, the tolerance code (e.g., H7 or g6), and whether you're looking at a hole or a shaft.

Step 1: Find the nominal size range. ISO 286 groups sizes into ranges: 1-3mm, 3-6mm, 6-10mm, 10-18mm, 18-30mm, 30-50mm, 50-80mm, 80-120mm, etc. A 25mm dimension falls in the 18-30mm range.

Step 2: Look up the hole tolerance. For H7 in the 18-30mm range, the table gives: upper deviation = +21 µm, lower deviation = 0 µm. This means the hole can be 25.000mm (minimum) to 25.021mm (maximum).

Step 3: Look up the shaft tolerance. For g6 in the 18-30mm range: upper deviation = -7 µm, lower deviation = -20 µm. This means the shaft can be 24.980mm (minimum) to 24.993mm (maximum).

Step 4: Calculate the fit. Minimum clearance = hole minimum - shaft maximum = 25.000 - 24.993 = 0.007mm. Maximum clearance = hole maximum - shaft minimum = 25.021 - 24.980 = 0.041mm. So an H7/g6 fit at 25mm nominal produces 0.007 to 0.041mm of clearance.

This process is straightforward but tedious to do by hand for every dimension on a drawing. That's why tolerance calculators exist — you enter the nominal size and fit code, and the calculator returns the actual limit dimensions and the resulting clearance or interference range.

Practical Tips for the Shop Floor

Always machine the hole first. In the H-basis system, the hole tolerance is fixed and the shaft is adjusted to create the desired fit. Since holes are harder to adjust after machining (you can't un-bore a hole), make the hole first, measure it, and then turn the shaft to match. This is standard practice in toolmaking and precision assembly.

Temperature matters for interference fits. A 0.025mm interference fit at 20°C becomes a different interference at 35°C shop temperature because thermal expansion changes the dimensions. For critical interference fits, measure parts at the same temperature or apply thermal expansion corrections. Steel expands about 12 µm/m/°C, so a 50mm shaft changes about 0.009mm per 15°C temperature change.

Surface finish affects functional fit. A ground shaft at Ra 0.8 will slide differently than a turned shaft at Ra 3.2, even if both are within the same tolerance band. For sliding fits, specify surface finish alongside the tolerance grade. As a rule, surfaces in sliding contact should be Ra 0.8 or better; surfaces in interference fits should be Ra 1.6 or better.

Don't mix ISO and ANSI on the same drawing. ANSI/ASME uses a different tolerance system (ANSI B4.1/B4.2) with different notation. RC (running clearance), LC (locational clearance), LT (locational transition), LN (locational interference), and FN (force/shrink fit) classes are the ANSI equivalents. If a drawing uses H7/g6, it's ISO. If it uses Class RC4, it's ANSI. Don't try to cross-reference them directly — the tolerance values differ.

Inspect at the correct points. For shafts, measure the maximum material condition (largest diameter for external, smallest diameter for internal). For fit purposes, the critical dimension is the one that determines whether the parts will or won't assemble. Use multiple measurement points along the length to check for taper or barrel shape, which can make a "within tolerance" dimension produce an out-of-spec fit.