Resources
Choosing datums on a machined aluminium drawing
Published 2026-09-03
When a drawing lands on our desk, the first thing we read is not the tolerance values — it is the datum scheme. A tolerance says how far one dimension may drift; a datum says where that dimension starts. Get the second one wrong and the first one stops meaning anything. This is about choosing datums, placing them, and knowing when to push back on a supplier who wants to choose for you.
A datum is not where you measure from — it is what the part sits on
Plenty of drawings treat datums as a starting point for dimension lines: begin at this edge and work right. The real definition is stricter. A datum is a surface the part is constrained on — in the fixture, on the inspection table, and in the assembly. It answers 'how does this part sit still', not 'where does this dimension begin'.
A part has six degrees of freedom in space. The classic scheme removes them in stages with three mutually perpendicular datums: the primary face seats the part and takes three away, the secondary face pushes against it and takes two more, the tertiary stops the last one. That is why the order in an A|B|C call-out carries meaning — A seats, B aligns, C stops. Reverse the order and the same physical part measures differently, and neither reading is wrong.
So a datum is not a drafting habit, it is a process instruction. The datums you set on the drawing are the faces the part rests on in our fixture and the faces the inspector indicates off. Change the datums and both the fixture and the inspection plan change with them.
Why ten linear dimensions cost more than three datum faces
Measuring from one hole to the next, then to the next, builds a chain. Every link carries its own tolerance, and the real deviation between the ends is those tolerances stacked on top of each other. The longer the chain, the more the far end wanders — every hole inside its own tolerance, the last hole nowhere near where the assembly needs it. Nobody made a mistake; the dimensioning scheme did it.
The more expensive part is the uncertainty. A chained drawing never says which link is the critical one, so the shop has to prepare for the worst case: an extra setup, an extra indicating operation, an extra round of inspection. Reference every hole to the same datum frame instead, and that long chain breaks into a set of short parallel ones — each feature answers to the datums alone, and the tolerances stop compounding.
Inspection gets cheaper too. A part with clean datums is measured in one setup on the CMM. A part with vague datums forces the inspector to guess how it should be seated, and a wrong guess throws away the whole data set. That guessing time always finds its way back into the quote in one form or another.
Pick the faces that talk to the assembly
There is really only one clue worth following: when this part is installed, which faces locate it? Those are your A, B and C. Functional datums, fixture datums and inspection datums should be the same faces — that is what makes a drawing self-consistent. When they diverge, the part is made to one set of rules and used under another.
The classic mismatch is choosing the face that is easiest to measure rather than the face that actually locates. The bottom is flat and sits nicely on a surface plate, so it becomes A — but in service the part is bolted against the frame on two side bosses. Every part then passes inspection and every part sits crooked, because the surface you controlled so carefully is one nobody in the assembly cares about.
The second clue is area and stiffness. The primary datum belongs on the largest, least deflection-prone face you have, so the part genuinely sits still. Put A on a narrow edge or a thin unsupported wall and what you measure is how far that face bent under clamping, not what the part is — worth extra care on thin-wall parts.
Extruded parts: the section gives you no ready-made datum
Extruded-then-machined parts carry a specific problem. The cross-section comes out of the die, so its accuracy is governed by extrusion standards — precision profiles typically to EN 12020, on the order of ±0.1 mm — and along its length the bar also carries twist and bow. Anchor your primary datum on an as-extruded surface and you have tied the accuracy of the whole drawing to extrusion tolerances. No amount of tightening on the machined features downstream wins back what you gave away at the origin.
Usually the better move is to leave a small machined datum on the drawing: a milled pad, a faced end. Let the CNC create the reference first, and start every precision dimension from it. The added area is small and the cutting time short, but it puts a wall between section tolerances and machining tolerances.
If the part genuinely has to locate on an extruded surface — because in the assembly it really does hang off that dovetail — then say so explicitly and accept that this datum inherits extrusion-grade accuracy. That is a perfectly valid choice. It just should not happen by default.
The datum call-outs we keep having to ask about
None of these stop a drawing from being quoted, but each one costs a round of emails. Scan for them before you send and the quote comes back a full loop sooner.
| What the drawing says | Why it stalls |
|---|---|
| Datum points at a theoretical centreline or an internal cavity | Fixtures and gauges need a surface they can physically touch |
| A, B and C are named but not ordered | Order decides how the part seats; change it and the same part reads differently |
| The same datum letter marks different faces on different views | The two do not agree, so the shop stops and asks, and the quote waits |
| Datum sits on a thin wall, a narrow edge, or unsupported material | Clamping deflects it, so you measure the deflection instead of the part |
| Position tolerance references datums but states no material condition | The same hole pattern can pass or fail depending on the reading |
| A tapped hole is a datum with no pitch-diameter or minor-diameter note | Two parties inspect it two different ways and the numbers never match |
When to push back, and when to just send the drawing
If a supplier answers 'we'll pick the datums ourselves', push back once. Picking them in the shop means picking whatever the fixture finds convenient, and convenient is not always the direction the assembly needs. Only you know which faces locate the part in the finished machine — don't let that get reinvented on the shop floor.
The other way round: if you are not yet sure which faces really locate it — completely normal while the part is still changing — you don't have to freeze a datum scheme before you send anything. Send the mating part, the assembly relationship, or simply the whole assembly drawing, and we will work out the origin together.
Every drawing in our flow goes through an engineering review before it is priced, and the datum scheme is one of the first things read. Drawings with clean datums get their feasibility answer quickly; drawings with vague ones get a first reply that is entirely questions about datums — better to settle those before the file leaves your desk.
Keep reading