Tolerances are where design meets reality

Every dimension on a drawing is a promise, but the nominal geometry in your CAD model is a fiction. A Ø20 mm shaft is never exactly 20 mm, and a 3 m steel beam is not exactly 3 m long. Tolerance is the language we use to say how much variation the design can absorb before it stops working. Get it right, and parts drop together on site or on the bench. Get it too loose, and assemblies rattle, leak, wear quickly or fail a vibration test. Get it needlessly tight, and you pay for it twice: once in the machining cost and again in rejected parts and awkward conversations with your supplier.

The craft is specifying the widest tolerance band that still does the job — never the tightest number that looks impressive on a drawing.

Limits and fits: the ISO hole-basis system

In the UK, BS 8888 is the standard that governs how we put technical product documentation together, and it points you at the ISO 286 limits and fits system. A fit is written as a pair of toleranced features, for example Ø20 H7/h6. The capital letter is the hole, the lower-case letter is the shaft. Take that pairing literally: the hole runs from 20.000 to 20.021 mm, the shaft from 19.987 to 20.000 mm, so the resulting clearance is anywhere between 0.000 and 0.034 mm.

That single example covers the three families you will use most:

• Clearance fit — the shaft is always smaller than the bore. Sliding spigots, bushes, dowel locations that must be assembled by hand.
• Interference fit — the shaft is always larger. Used to transmit torque, or hold a bearing race; needs a press, a temperature differential, or both.
• Transition fit — could end up tight or loose depending on where each part lands in its band. Good for accurate location with minimal play, but only if you control assembly.

Hole-basis (H) is the sensible default because reamers, drills and bore gauges are more widely available and cheaper than plug gauges. Shaft-basis (h) is the better choice when you are fitting a housing around bought-in ground bar or a standard motor shaft — you cannot change the shaft, so you move the hole.

Building a tolerance stack that tells the truth

A tolerance stack is simply the sum of the contributing dimensions across an assembly, worked out to find the maximum and minimum gap, interference or alignment error at the point that matters. Do it early — a stack on the back of an envelope during concept design is worth far more than a panic calculation after tooling is cut.

Two methods are worth knowing. Worst-case arithmetic adds every contribution at its limit: five stacked features each at ±0.1 mm give ±0.5 mm. That is the honest answer for small batches, safety-critical joints and anything where a single out-of-spec assembly is unacceptable. Statistical (root-sum-square) assumes each dimension is independently and normally distributed, so the same five features give roughly ±0.22 mm. It is defensible for high-volume production where processes are centred and capable, but it is not a way to make a real problem disappear.

Three contributors get forgotten again and again:

• Surface treatment and plating. A hard-anodised or zinc-plated surface can add 0.01 mm per side, which is a fifth of a typical clearance.
• Thermal expansion. Aluminium grows about 23 µm per metre per kelvin, so a 500 mm part is 0.115 mm longer at 30 °C than at 20 °C.
• Assembly and fixture variation. If a part is located by hand against a stop, that stop has a tolerance too.

Geometric controls: form, orientation and position

Size tolerances say nothing about whether a face is flat or a hole pattern is in the right place. That is the job of geometric tolerancing to ISO 1101 — flatness, perpendicularity, position, concentricity and the rest. A position tolerance of Ø0.2 mm at MMC on a bolt hole, referenced to a three-plane datum A|B|C, tells the supplier exactly what to hold and gives you bonus tolerance: as the hole drifts away from its maximum material size, the allowable positional error grows.

The practical rules are short. Choose datums that reflect how the part is measured and how it functions in the assembly. Keep the datum reference frame to three mutually perpendicular planes unless there is a genuine reason for more. And resist over-constraining: every extra control is a measurement someone has to make and a feature the process has to hold.

Specifying what manufacturing can actually hold

Tolerances should be chosen with one eye on the process capability of the method you expect to be used. As rough working figures:

• Laser cutting or waterjet: ±0.1 to ±0.2 mm on sheet profiles.
• CNC milling: ±0.05 mm routinely, ±0.02 mm with care and the right setup.
• Turning: ±0.025 mm as standard, down to ±0.005 mm when ground.
• FDM 3D printing: ±0.3 mm, or ±0.5% of dimension, whichever is greater.
• Injection moulding: tool-dependent, around ±0.1 mm on stable dimensions, with far more variation across a parting line.

Cost climbs steeply once you go much below ±0.05 mm, so reserve tight bands for the features that genuinely need them. Pair them with a sensible surface finish callout — a bearing seat might need Ra 0.8 or better, while a bracket foot does not care. Then put a general tolerance note on the drawing, such as ISO 2768-mK, and dimension only the critical features individually. It keeps drawings readable and gives your supplier room to choose the most economical process.

Checking your work — in CAD and on the drawing

Most modern 3D CAD packages include tolerance analysis tools or allow limits, fits and mate conditions to be attached directly to the model, and model-based definition lets you carry the annotation in the 3D data itself. Whatever the workflow, produce a flat drawing for the critical dimensions and a PDF that a machinist or fabricator can mark up on the shop floor. Walk the tolerance stack in the order the parts are actually assembled, not the order they appear in the feature tree.

Ask a machinist, fabricator or contractor to sanity-check the numbers before you release anything. And for architects coordinating steelwork to BS EN 1090 with cladding, curtain walling or brick coursing, the principle is identical: the model is nominal, the specification carries the tolerance, and generous movement joints and setting-out allowances are far cheaper than forcing the frame to be perfect. Specify the variation you can live with, control only what matters, and let manufacturing do the rest.