Datums on a drawing: what they are and how to choose them

Before a part can be measured it has to be set against something. A datum states what that something is. When a drawing names no datum, the manufacturer and the customer clamp the part differently, get different numbers, and both are right — because nothing was agreed.

A datum is not the datum feature

This distinction is the key to the whole subject. A datum is a theoretically perfect reference: a point, an axis, a line or a plane. It has no roughness, no form error and no size, because it is not real.

The datum feature is the actual surface on the part: that machined face, that bore, that edge. It is rough, slightly out of true, and it has a size. During inspection the part rests on the real feature, and the perfect datum is derived from those contact points.

On the drawing, a letter in a box (A, B, C) attached to a triangle marks the datum feature — it says "take the reference from this surface".

The 3-2-1 rule: how a part is locked down

A free body has six degrees of freedom: three translations and three rotations. All six have to be removed before anything can be measured. Three datums share the work:

1. Primary datum (A) — three points of contact. The part settles onto the surface. One translation and two rotations are removed: three degrees of freedom.
2. Secondary datum (B) — two points of contact. The part is pushed against a perpendicular face. One more translation and one more rotation go; five in total.
3. Tertiary datum (C) — a single point of contact. The last sliding motion stops. The part is now fully constrained and the origin of the coordinate system is fixed.

On the shop floor this is a surface plate (A), an angle plate (B) and a pin (C). On a CMM the logic is identical; only the contact is made by the probe.

Order matters: A|B|C is not A|C|B

This is the point most drawings overlook, and it causes half of all inspection disputes. The order of the letters in the feature control frame decides which surface the part rests on first. The first surface sets the attitude of the part; the others align to it.

So A|B|C and A|C|B fixture the part differently and produce different numbers for the same hole — even on a perfect part. What counts is the order inside the feature control frame, not the order the letters happen to appear on the drawing: the first letter is always primary.

Which face should be the primary datum?

• Pick the face that has a functionWhatever the part sits on in the assembly is what it should sit on during inspection. Datum selection is not arbitrary; it imitates the job the part does.
• Make the largest face primaryThe further apart the three contact points are, the more stable the attitude. A 4 mm land as a primary datum makes the part rock and the measurement will not repeat.
• Use a stable, machined surfaceAn as-cast skin, a deburred edge or a flexible region is not a reference.
• Use datum targets on irregular partsWhere full surface contact is impractical, specific contact points are defined and marked with an X on the drawing. Common on castings and thin sheet parts.

Which tolerances need a datum and which do not

There is a practical split: tolerances that constrain the shape of a feature on its own need no reference; tolerances that constrain a feature relative to something else do.

You do not need a reference to ask whether a face is flat; it either is or it is not. But to ask whether it is square to something, the question "square to what?" has to be answered. The datum is that answer.

Three mistakes seen again and again

• No datum at allA perpendicularity or position tolerance is given with no reference. That tolerance cannot be measured; the manufacturer has to assume.
• Datums given but the order not consideredThe letters are there but nobody decided which is primary. If the largest face has been put second, the measurement becomes unstable.
• A datum feature with no functionA surface that touches nothing in the assembly has been chosen as the reference. The part passes inspection and then does not sit properly.

Datum systems are defined by ISO 5459 on the ISO side and ASME Y14.5 in the United States. The two differ in some details of notation but the underlying logic is the same: constrain the part first, then measure it.

At Q TECH we read incoming drawings this way before production: are the datums stated, does their order match how the part sits in the assembly, is the primary face large enough to carry the measurement. Because inspection is in-house, we plan the fixturing together with the process.

• datum
• GD&T
• datum reference frame
• 3-2-1 rule
• ISO 5459
• technical drawing
• CMM inspection
• Ankara Ostim