Datums: how to choose them and why they decide the inspection

Datum feature and datum are not the same thing

A datum feature is a real feature on the part: a face, a bore, a pin, a slot or a set of points. It has imperfections. A datum is the theoretically exact plane, axis or point established from that feature by a datum feature simulator.

The simulator is the surface plate, the mandrel, the chuck or the CMM alignment that contacts the datum feature. The datum is what the simulator establishes, not the average of the real surface. That distinction matters because two different simulators can produce two different datums from the same part.

A datum reference frame is the coordinate system built from the primary, secondary and tertiary datums. Every position, orientation, profile or runout control that names those datums is measured from that frame. If the frame changes, the result can change without the part changing.

Degrees of freedom and the 3-2-1 rule

A free rigid body has six degrees of freedom: three translations and three rotations. A datum reference frame removes them in a fixed order. The primary datum removes three, the secondary removes two and the tertiary removes one.

For a flat primary face, the three removed freedoms are translation normal to the face and the two rotations about axes in the face. The secondary face removes the remaining translation and one rotation. The tertiary removes the last rotation. The order is why the same three features can produce different results when the sequence changes.

A cylindrical primary datum is different. The axis removes four degrees of freedom and leaves translation along the axis and rotation about it. A secondary face can remove one or both, depending on its orientation. This is why a bore and a face are a common pair for a rotating part.

Choose datums from the assembly, not the drawing

The best datum feature is the one that locates the part in service. A housing that sits on a mounting face should use that face as the primary datum. A cover that is positioned by two pins should use the pins or the holes that receive them, not an outside edge that no one touches.

The fixture should copy the same logic. If the assembly clamps on a machined face and two bores, the inspection fixture should also clamp on that face and those bores. A CMM program that aligns to a different set of features is measuring a different part.

This is also the argument for functional gauging. A gauge that reproduces the assembly interface checks the feature in the same relationship as the product. A CMM that aligns to a convenient plane may be more precise and less relevant.

Size and access matter too. A datum feature should be large enough to give a stable contact and reachable with the probe or gauge. A narrow edge can look functional on the assembly drawing and still be a poor datum because the contact repeats within a wide band. If the only functional feature is inaccessible, a datum target or a change to the assembly may be needed.

Datum targets for irregular parts

A cast or forged surface is not flat enough to serve as a whole datum feature. Datum targets solve that by defining specific points, lines or areas on the surface. The simulator contacts those targets, and the datum is established from them.

Targets are also useful on a large thin panel that would rock on a surface plate. Three target points define a stable primary plane. Additional targets can define a secondary or tertiary reference without pretending that the whole surface is in contact.

The drawing must show the target locations and sizes. A note that says the surface is a datum without target definitions leaves the inspector to choose contact points, which defeats the purpose. For a casting, agree the targets with the foundry and the machine shop at the same time.

How datum order changes the answer

Consider a bracket with a large mounting face and two holes. If the face is primary and the holes are secondary and tertiary, the part is located on the face and then positioned by the holes. If a hole is primary, the part is located on an axis first and the face is used for orientation. The two schemes can accept different parts.

The order should follow the assembly sequence. Whatever contacts first and carries the most restraint is the primary datum. Whatever clocks the part is the secondary. Whatever stops the last movement is the tertiary.

A common error is to list three datums without deciding which one is primary. The frame has an order, but the design intent may not. The inspector will follow the frame, and the supplier will quote to it. If the order is wrong, the error is built into every part.

The errors that make a datum unusable

The first is an inaccessible feature. A datum inside a closed housing cannot be contacted without cutting the part. The second is an unstable feature. A small boss or a narrow edge gives a contact that repeats poorly. The third is a datum that moves during measurement because the part is not restrained in the same way as it is in service.

The fourth is a datum feature that is also used for a size control in a way that conflicts with the datum simulation. The fifth is a missing common datum callout for two coaxial or coplanar features that work together. Two bores that act as one axis should be identified as a common datum, not treated as unrelated references.

The sixth is a datum reference at maximum material boundary without checking the clearance to the simulator. That clearance allows datum shift, which is a legitimate allowance but must be understood. If the design assumes no movement, do not invoke the boundary modifier.

• Can the datum feature be contacted in inspection?
• Does the fixture repeat the assembly contact?
• Is the feature stable enough to give a repeatable datum?
• Does the drawing state targets where the surface is irregular?
• Is a common datum needed for features that act together?

A datum checklist for the drawing and the report

On the drawing, mark the datum features with the correct symbol and state the order in every frame that uses them. Show datum targets where applicable. Add a note if the datum feature is to be used at a material boundary, and state the boundary condition.

In the first article report, record the alignment method. Name the simulator, the contact points and the software alignment. For a CMM, keep the alignment program with the report so the next inspector can repeat it. For a hard fixture, record the gauge identity and calibration status.

If the part is measured on a different datum scheme from the one in the drawing, say so. A result from a nonconforming alignment is not evidence of conformity, even if the numbers look good. The datum is part of the requirement, not a setup detail.

1. 01

   Start with the interface

   Identify the surfaces and features that locate the part in assembly.

2. 02

   Assign the order

   Primary takes the first contact and three degrees of freedom, then secondary, then tertiary.

3. 03

   Check access

   Confirm that each datum feature can be contacted by the fixture or the CMM.

4. 04

   Record the method

   Put the simulator and alignment in the first article report.