Resources
How to tolerance CNC-machined aluminium parts — a guide to faster, sharper quotes
Published 2026-07-23
Every ± on a drawing is a promise the workshop has to keep with real process choices — machine, fixturing, inspection. Tolerance a drawing intelligently and the quote comes back fast and honest; tolerance it bluntly and you either get 'not feasible' or pay for precision the part never uses. This guide is about putting tightness exactly where the function needs it.
First, sort every dimension: does the die own it, or the machine?
An extruded-then-machined aluminium part gets its dimensions from two different places. The cross-section — walls, grooves, outer envelope — is fixed in the extrusion die, and its precision is governed by extrusion standards (precision profiles typically to EN 12020, on the order of ±0.1 mm). Holes, threads, end faces and pockets are cut later on the CNC, where fixturing and the machine set the limit — usually far tighter than any press can hold.
Most tolerancing trouble comes from mixing the two: applying machining-grade numbers to the section, which the press cannot hold, or extrusion-grade slack to hole positions, which the assembly cannot accept. Before you dimension anything, assign it to its owner — section dimensions go to the profile standard, machined features to CNC tolerances.
Three layers: a general tolerance underneath, marked criticals on top, datums for relationships
A healthy drawing is layered. Layer one: a general tolerance class in the title block (ISO 2768 class m or f is the usual choice for machined features), which quietly covers every dimension that doesn't drive assembly. Layer two: the few dimensions that genuinely decide fit — rarely more than five — carry their own ± values. Layer three: anything that matters relative to something else (a hole pattern to an edge, face to face) is expressed with datums and geometric tolerances rather than a chain of linear dimensions fighting each other.
A useful sanity check: when more than eighty percent of a drawing rides on the general tolerance and only a handful of dimensions are individually tightened, the estimator can see at a glance where the process effort belongs — and the quote reflects it.
Why 'everything ±0.01' kills a quote
Writing one very tight number into the title block and letting the whole drawing inherit it is the most common red flag on the quoting desk. It forces every chamfer and every non-functional edge through the most demanding process and full inspection — lead time stretches, the price climbs, and nine-tenths of that precision does nothing for the part.
Worse, it hides what you actually care about. Tell us instead which two or three features are tight because something mounts there. Knowing the function, we can often push the other way: point out where a looser value changes nothing, so the precision budget lands where it earns its keep.
Three habits of aluminium: clamping, heat, and coating growth
Aluminium machines beautifully, but three of its habits belong in your tolerancing decisions. First, thin walls deflect under clamping force — the classic failure is a bore that is round while clamped and springs oval when released. Leave the process somewhere to hold the part, or accept engineered supports near critical thin walls.
Second, aluminium expands by roughly 23 µm per metre per °C. On long parts measured across a temperature difference, numbers drift — precision dimensions are referenced to the standard 20 °C inspection temperature, and it is worth saying so on the drawing for long critical lengths.
Third, surface treatment changes size. Anodic films run 8–30 µm (growing roughly half into and half out of the base metal); powder coating adds 60–120 µm. For close-fitting bores and shafts, state whether dimensions apply before or after treatment, and call out masking for threads and precision holes that must stay bare.
The sixty-second check before you hit send
Run the table below before the drawing goes out. Every unchecked line usually costs one extra round of questions before a number can come back.
| Check | Why it matters |
|---|---|
| General tolerance class in the title block (e.g. ISO 2768-m) | Covers the bulk of the drawing so nobody has to guess |
| Individually toleranced criticals — five or fewer | Shows exactly where process effort and inspection belong |
| Datums given wherever features relate to each other | Keeps the tolerance chain clean instead of self-contradictory |
| Stated whether dimensions apply before or after coating | Anodize and powder films eat clearance on close fits |
| Alloy with temper, in full (6061-T6, not just 6061) | Temper sets mechanical properties and machining behaviour |
| Threads complete: size, depth, masking requirement | Threads are the most common source of rework — specify once, make once |
Solve tolerance questions at the quoting desk, not on the line
In our flow, every drawing passes an engineering review before it is priced: what the press can hold, what the CNC should finish, and where a tolerance collides with a surface treatment all get flagged — with a suggested fix — in the reply. The cleaner the drawing, the faster that loop; most well-layered drawings get their feasibility read the same day.
And if you are unsure how to tolerance a feature, don't decide for us — describe the function and the mating part in a note, and we will settle the call-out together.