Tolerances are not just numbers on a drawing. They are the difference between a part that fits first time and one that ends up in the scrap bin. For small UK workshops, getting tolerances right controls fit, function and cost. Too loose, and your assembly rattles or leaks. Too tight, and you spend hours chasing microns that do not matter. This guide explains the common notation you will see on mechanical engineering drawings and how to apply limits to simple machined components.

Why tolerances drive cost and function

A tolerance is the allowable variation in a dimension. If a drawing says 20 mm, that is a nominal size. The real part will never be exactly 20.000 mm. The tolerance tells you how far off you can be. A shaft turned to 20 ±0.5 mm is cheap. A shaft ground to 20 ±0.005 mm is not. The tighter the tolerance, the more operations, skill and inspection time you need. For a small workshop, that directly affects your hourly rate and your ability to compete.

Function comes first. A pivot pin needs a clearance fit so it rotates. A bearing inner ring needs an interference fit so it does not spin on the shaft. A cover plate needs a loose fit so it bolts down without distortion. Each requirement translates into a specific tolerance band. If you cannot explain why a tolerance is there, question it.

Common notation on drawings

Most drawings use a few standard ways to show limits. Recognise these and you can read any job.

• Limit dimensions: Two numbers, such as 25.00 / 24.95. The part must measure between them.
• Plus/minus: 25 ±0.1 means 24.9 to 25.1. Simple, but it gives the same variation in both directions.
• Unilateral: 25 +0.05 / -0.00. The part can be larger than nominal, but never smaller. Often used for holes that will be reamed.
• ISO fit notation: A letter and number, such as 20 H7 or 20 g6. H means a hole with a lower deviation of zero. g means a shaft with a negative upper deviation. The number is the tolerance grade. Smaller numbers are tighter.
• Geometric tolerances: Symbols for flatness, concentricity, perpendicularity. These control shape and position, not just size. A shaft can be within size but still bent. Geometric tolerances catch that.

For simple components, limit dimensions and ISO fits cover most needs. Geometric tolerances matter when parts must align or seal.

Applying limits to a shaft and hole

Suppose you are making a bush for a pivot pin. The bush has a 12 mm bore. The pin is 12 mm. You want the pin to slide freely but not rattle. Choose a clearance fit.

• Hole: 12 H7. Limits are 12.000 to 12.018 mm.
• Shaft: 12 f7. Limits are 11.966 to 11.984 mm.
• Minimum clearance: 0123456789 = 0.016 mm.
• Maximum clearance: 0123456789 = 0.052 mm.

That gives a smooth sliding fit. Now change to a press fit for a bearing seat. Use 12 H7 hole and 12 s6 shaft. Shaft limits are 12.012 to 12.023 mm. The shaft is always larger than the hole. Interference ranges from 0.012 to 0.023 mm. You will need a press or a warm bearing to assemble it. The function dictates the fit. The fit dictates the tolerance.

Choosing tolerances your workshop can hold

Do not specify a tolerance tighter than your process can deliver. That is the fastest way to lose money. Here are rough capabilities for common operations in a small workshop.

• Turning: ±0.05 mm is comfortable. ±0.025 mm needs a good lathe and sharp tooling. ±0.01 mm requires patience, a rigid setup and often a grinder.
• Milling: ±0.05 mm is typical. ±0.025 mm is possible with care. Below that, consider surface grinding.
• Drilling: ±0.1 mm is normal. For a precise hole, drill undersize and ream to H7.
• Reaming: H7 or H8 is standard. It gives a round, smooth hole.
• Grinding: ±0.005 mm or better. Reserve it for bearing seats, gauge work or hardened parts.

If a drawing calls for ±0.01 mm on a turned diameter, ask whether a grinder is available. If not, redesign the fit or accept a looser tolerance. Communication here saves hours.

Inspection and practical checks

You cannot hold a tolerance you cannot measure. For outside diameters, use a micrometer. For inside diameters, use a bore gauge or plug gauge. Callipers are fine for rough work, but they will not prove a 0.01 mm tolerance. Let parts cool before measuring. Steel expands by about 12 microstrain per degree Celsius. A 100 mm part grows 0.012 mm if it warms by 10°C. That is enough to fail a tight tolerance.

Always measure from the datum stated on the drawing. If the drawing shows a face as datum A, do not measure from the opposite end. Use the same reference for every check. For small batches, make a master sample that you know is good. Compare new parts to it. That is faster than reading a micrometer for every feature.

Rules of thumb for small workshops

• Use standard fits from ISO 286 or BS 4500 tables. Do not invent your own letter and number combinations.
• Only tighten a tolerance where function demands it. Every extra decimal place adds cost.
• Ask your machinist what they can hold before you finalise the drawing. They will tell you the truth.
• Write the fit and its purpose in the drawing notes. "Clearance for sliding pin" prevents guesswork.
• Allow for coating, plating or heat treatment. A plated shaft can grow by 0.01 mm or more.
• Keep a reference part for each critical fit. It is the quickest way to check a new batch.

Good tolerancing is a conversation between design and manufacture. Get it right, and your parts fit, your costs stay sane, and your customers come back. Get it wrong, and you will spend your evenings reworking parts that should have been simple.