Datum Strategy for Functional GD&T

Reading a datum reference frame is one skill. Judging whether it is the right frame is another. At this level, you look at a drawing and ask whether its datums match how the part works, whether they can be measured the same way twice, and whether a CMM program really honors them. A poor datum choice cannot be fixed by careful inspection. It makes good parts fail and bad parts pass, and it starts arguments between suppliers and customers. This is written around the ideas in ASME Y14.5 in plain words. It does not replace the standard. Always work to the edition the drawing names, and take any change to a drawing to the engineer who owns it.

What You Will Be Able to Do

• Pick primary, secondary and tertiary datums from how a part assembles.
• Decide whether a face or a cylinder should lead, using a tilt calculation.
• Choose between RMB and MMB, and work out datum shift.
• Know when to use datum targets and co-datums.
• Spot a CMM alignment that does not match the drawing.
• Review a drawing for common datum problems.

Start From the Assembly

Datums should copy how the part is located in real use. Picture the part going into its assembly, and ask three questions in order.

1. What seats first, and sets the tilt? That is usually the primary.
2. What centers or locates it next? That is usually the secondary.
3. What stops the last motion, such as the spin? That is the tertiary.

Worked example. A pump cover bolts onto a housing. Its flat back face seats on the housing. A short round pilot boss centers it in a bore. A dowel hole near the edge stops it from turning. The natural frame is: face as A, pilot as B, dowel hole as C. The bolt holes and the seal groove are controlled to A, B and C, because that is how the cover sits when it does its job.

A drawing that uses the two outer edges of the cover as datums might be easier to fixture. But those edges touch nothing in the assembly, so the holes could pass inspection and still fail to line up.

Which Leads, the Face or the Cylinder?

When a face and a cylinder both locate a part, one of them has to be primary. Whichever controls tilt in real use should lead. A simple calculation tells you which one does.

Tilt allowed by a pilot = clearance / engagement length

Worked example. A pilot has 0.002 inch of clearance in its bore. The mounting face reaches out 4 inches from the center.

With the short pilot, the part could rock 0.032 inch at the rim, far more than the face will allow. So the face sets the tilt and should be primary, and the pilot only centers it. With the long pilot, the pilot limits tilt to 0.0027 inch, so the bore sets the tilt, and the cylinder should be primary. The face then only stops the part from sliding along the axis.

Length-to-diameter thinking gives you the same answer quickly. A long engagement leads. A short one follows.

Qualify the Datum Features

Everything in a frame is measured from the datum features, so they need controls of their own. If they have none, the drawing has a loose foundation.

The tolerance on a datum feature should be tighter than what depends on it, within reason. A flatness of 0.010 on a face that sets a 0.004 profile zone makes no sense, because the seat varies more than the feature.

Also check that a datum feature is big enough. Two contact points close together let a small error swing the whole frame. A tertiary locator near the center of the part has a poor lever arm for stopping the spin. One out near the edge does much better.

RMB or MMB

When a datum feature is a feature of size, its letter in the frame may or may not carry an (M).

• RMB (regardless of material boundary) is the default. With no modifier, the simulator closes on the feature, so the part is centered with no looseness.
• MMB (maximum material boundary) is shown by an (M) after the datum letter. The simulator is a fixed size, and the part may move on it. That movement is datum shift.

Choose based on how the part mates.

Worked example. A boss, datum B, is Ø 1.000 +/- 0.002, with a perpendicularity of Ø 0.002 (M) to A. It is used at MMB in a position frame.

1. MMC of the boss is 1.002.
2. Its boundary is 1.002 + 0.002 = 1.004, because it has an orientation control to the higher datum.
3. The boss's actual mating size is 0.999.
4. Total looseness is 1.004 - 0.999 = 0.005, so the part may shift 0.0025 in any direction.

The boundary is the key step. If you stopped at 1.002, you would give the part less shift than the drawing allows and might reject a good part. If the boss has no control to the higher datum, the boundary is just its MMC.

Datum Targets

A rough or flexible surface does not make a stable datum. A casting skin has high spots that change from part to part, so a full-surface datum on it cannot repeat. Datum targets name specific points, lines or small areas to contact. The drawing shows them with a target symbol, and they are labeled A1, A2, A3, B1, B2, C1 and so on.

Use them on:

• Castings and forgings, where the surface is rough.
• Sheet metal and large thin parts, which bend if a whole face is forced flat.
• Parts where only certain areas are reliable, such as pads.

Practical rule: the first machining fixture should locate on those same targets. If the machinist locates from one set of points and the inspector from another, the difference shows up as a rejected part with nothing wrong with it. Some drawings show a movable target, so a locator slides toward the surface. That is common for angled or curved faces.

Co-Datums

Sometimes two features work together as one datum, and neither one leads. Two bearing journals on a shaft are the classic case. The drawing shows them as a single reference with a hyphen, such as A-B. Both are simulated at the same time, and together they set one axis.

Worked example. A shaft has two journals 6 inches apart, each 1 inch long. Suppose the frame used journal A alone as primary, with a form error of 0.0005 inch across its 1-inch length. The axis from A tilts by that much per inch, so at 6 inches away it has moved about 0.0005 x 6 = 0.003 inch. Journal B would read 0.003 off, and nothing is wrong with the shaft. With A-B, both journals set the axis together, as they do in the bearings.

Telling the Drawing Which Motions Matter

By default, a datum locks every degree of freedom it can. Sometimes that does not match the function. The 2009 and later editions allow a customized frame, which lists in brackets after a datum letter exactly which motions it controls. Few drawings need this. If you see it, read it literally, and do not assume the normal 3-2-1 pattern. If you think one is needed, raise it with the engineer.

Datums Versus CMM Alignments

Here is where correct drawings go wrong in practice. A datum plane comes from contact with the high points of a surface. A CMM's default plane is often a best-fit through the measured points. These are not the same plane.

Worked example. Datum A is a face with a 0.004 bow, crowned in the middle. On a surface plate, it would rest on its high points and rock. A least-squares plane through probe points passes through the middle of that bow, so about 0.002 below the high points. A hole depth measured from that plane reads about 0.002 different from a measurement taken on the plate. For a 0.003 tolerance, that decides pass or fail.

Check these in any CMM program:

Best-fitting a part to its model is useful for development, but it is not a datum frame. A report made that way cannot be used to accept a part against the drawing.

A part that rocks has more than one possible seat. The standard's math companion treats this as a set of candidate datums. Do not choose a seat just because it passes. Write down a method, agree on it with the customer where it matters, and use it the same way each time.

Flexible Parts

Thin parts change shape when held. For these, normal rules may not apply. Two tools help:

• Free state. The (F) modifier says a tolerance applies with the part unrestrained.
• Restraint note. The drawing states how to hold the part for inspection, such as which points get clamped and at what force, often to copy the assembly.

If a flexible part has no restraint note and the frame assumes it is held, ask. Two inspectors holding it in two ways will get two answers, and both will think they are right.

Reviewing a Drawing

When you check someone else's datum scheme, work through these.

Bring these up as questions. A drawing may reflect a reason you cannot see, and the engineer has the final say. Get any answer in writing, and do not reinterpret a drawing on your own.

Common Mistakes

Check Your Understanding

1. A long sleeve slides into a bore for most of its length, and a small shoulder stops it. The drawing makes the shoulder primary. What do you ask?

Whether the long bore really sets the tilt. A long engagement leads and a short one follows, so the cylinder may belong as primary, with the shoulder only stopping travel along the axis.

2. An inspector works out datum shift from a boss's MMC alone and ignores the boss's orientation control. What does that do to the result?

It understates the shift, because the boundary also includes the control to the higher datum. A good part could be rejected.

3. A bore on a spinning flywheel is called out as a datum with an (M). What do you ask?

Whether MMB matches the function. A rotating part centered on its bore should not be allowed to shift, so RMB may be the right choice.

4. A casting has a full-surface datum on its rough top. Readings change every time it is reset. What should you suggest?

Datum targets on stable spots, with the first machining fixture located on those same targets.

5. A supplier's report shows every point in tolerance after the part was best-fit to its CAD model. Can you accept it against the drawing?

No. A best fit is not a datum frame, so the report has not tested what the drawing asks. Ask for results from an alignment that builds the datums in the frame's order.

Key Takeaways

• Choose datums from how the part seats, centers and clocks in its assembly.
• Long engagement leads. Short engagement follows.
• Datum features need their own controls. A loose foundation spoils everything measured from it.
• Use MMB where the part can really shift, and RMB where it centers. The boundary includes any control to a higher datum.
• Use targets on rough or flexible parts, and co-datums where two features act as one.
• A best-fit CMM plane is not a datum. Ask questions about a drawing, and leave changes to the engineer.