Guide
How do you pick the primary, secondary and tertiary datums in a datum reference frame?
A datum reference frame is the set of three mutually perpendicular planes, built from the datum features named in a feature control frame and taken in the order they are listed, that fixes a part in space so every toleranced feature can be located and measured from the same origin. The primary datum is contacted first and usually removes the most freedom, the secondary is contacted next, and the tertiary removes whatever freedom is left.
By Saola Manufacturing engineering team · Published · Updated
Most explanations stop at “three planes, 3-2-1 contact.” This guide is about the decision that comes before that: which real surface on a machined part should be A, which should be B, and which should be C, and what happens to the numbers when that order is wrong or left ambiguous. Datum order is not a drafting formality. It decides how the part is clamped on the machine, how it is set up on the inspection plate or coordinate measuring machine, and therefore whether the supplier’s report and your incoming inspection agree. The rules cited come from ASME Y14.5-2018 and ISO 5459; the worked example is arithmetic on a hypothetical plate, not a measurement of any shop’s parts.
On this page
What does each datum in a datum reference frame actually constrain?
Each datum removes the degrees of freedom that the datums ahead of it left free. A rigid part has six, three translations and three rotations, and the order in the feature control frame decides which datum feature gets to remove which of them.
On a prismatic part with three flat datum features, the primary plane takes three degrees of freedom (one translation and two rotations), the secondary takes two (one translation and the last rotation), and the tertiary takes the final translation. That is the familiar three-two-one contact: the part rests on at least three high points of the primary, is pushed against at least two high points of the secondary, and stops against at least one high point of the tertiary. The physical contacts are the datum feature simulators, and on the shop floor they are a fixture, a vise jaw, a granite plate or the probed planes in a measurement program.
The count changes when the primary datum is not a plane. A cylinder used as the primary datum, such as a bearing journal on a shaft, removes four degrees of freedom on its own: two translations and two rotations. A face then becomes the secondary and only has one translation left to stop, and a tertiary is needed only if something on the part has to be clocked around the axis, such as a cross hole or a flat. The table below lists the counts for common primary datum feature types.
How many degrees of freedom does each type of primary datum remove?
A plane or a width removes three, a cylinder four, a sphere three and a cone five, per ASME Y14.5-2018. Whatever the primary leaves free is the job of the secondary and tertiary, and a datum reference that has nothing left to constrain should not be on the drawing.
Use the table as a check when you review a feature control frame. Count what the primary removes, then ask what the secondary can still remove. If a cylinder is primary and the drawing still lists a face and two more features, one of those references is doing nothing, or worse, it tells the inspector to rotate the part to a feature that has no functional reason to control the result.
| Primary datum feature type | Translations removed | Rotations removed | Total removed |
|---|---|---|---|
| Plane (flat face) | 1 | 2 | 3 |
| Width (slot or tab center plane) | 1 | 2 | 3 |
| Cylinder (bore or shaft axis) | 2 | 2 | 4 |
| Sphere (center point) | 3 | 0 | 3 |
| Cone (axis and vertex) | 3 | 2 | 5 |
| Complex surface | 3 | 3 | 6 |
How do you choose which surface is primary, secondary and tertiary?
Pick datums the way the part is held in the assembly: the primary is the surface that seats the part against its mating part and sets its orientation, the secondary is the feature that locates it next, and the tertiary is whatever stops the last movement. If the drawing mirrors the assembly, the supplier can fixture and measure the part the way it will be used.
Four questions settle most cases:
- Which surface bolts down or seats first? On a bracket, a cover or a manifold block, that is usually the largest machined face that sits against the mating part. It becomes A because it sets orientation in the assembly, and its size makes the three contact points stable.
- What locates the part in the plane of that face? If two dowel pins locate it, the dowel holes should be B and C (a hole as B and a hole or slot as C), not the outside edges. Edges make convenient datums on a drawing, but if the assembly never touches them they put the tolerance in the wrong place.
- Is the datum feature big and stable enough to come first? A narrow shoulder used as primary on a long shaft rocks on its high points, and the angular error multiplies along the shaft. On parts that are long compared with their seating face, the long cylindrical feature usually makes the better primary, with the shoulder as secondary.
- Can all three features be reached in one setup? If the primary is on the bottom, the secondary is a bore on the top and the tertiary is on a side face that a fixture would have to cover, the frame is valid on paper but expensive to make and to measure. Move the datum, or accept that the part will need a dedicated fixture.
Machinability is a tiebreaker, never the first criterion. A shop will often propose datums that suit its setup, which is reasonable only when the function is not affected. The ASME companion standard on gages and fixtures, ASME Y14.43, is a useful reference when you want to see how a given datum scheme turns into a physical check fixture.
Why do supplier and customer measurements disagree when datum order changes?
Real datum features are never perfectly square to each other, so the frame lands in a slightly different place depending on which feature it aligns to first. Swap the order and a hole that measured perfect in one frame can use a large share of its position tolerance in the other.
The table works one hypothetical case. A plate is located on face A, with the long edge as datum B and the short edge as datum C. The short edge leans slightly out of square to the long edge. A hole is machined exactly at its basic location in the A-B-C frame. Measured to the same drawing but with B and C swapped, the frame rotates to follow the short edge, and the hole moves.
| Datum order in the frame | Measured X (mm) | Measured Y (mm) | Position result, diameter (mm) |
|---|---|---|---|
| |A|B|C| (as drawn) | 180.00 | 80.00 | 0.00 |
| |A|C|B| (secondary and tertiary swapped) | 179.96 | 80.09 | 0.20 |
The arithmetic is simple: the swap rotates the frame by the out-of-square angle, and the hole moves by that angle times its distance from the new origin. The further a feature sits from the datum corner, the bigger the disagreement. If the hole’s position tolerance is only a little larger than that shift, the same part passes comfortably in one frame and is close to rejection in the other, with nothing wrong with the part.
Three other causes produce the same symptom. The first is a measurement program that fits datum planes by least squares instead of by contact on the high points; per ASME Y14.5 a planar datum is simulated by the high points of the surface, and a least-squares plane through a convex face sits inside the material. The second is a datum feature of size, such as a bore, referenced at maximum material boundary on the drawing but evaluated at regardless of material boundary in the program, or the reverse; the guide to bonus tolerance at MMC explains why that matters. The third is the standard itself: ISO 5459 and ASME Y14.5 handle some datum defaults differently, covered in ASME Y14.5 vs ISO GPS. When two reports disagree, compare the alignment first, before anyone re-cuts a part.
How should datums be chosen on turned parts and shafts?
On a turned part the primary is usually an axis, not a face: either the single bore or journal that locates the part, or a common axis built from two bearing journals. A face becomes secondary to stop axial movement, and a tertiary is only added when a radial feature has to be clocked.
The common mistake is to datum a shaft on its center drill holes because that is how it is held between centers on the lathe. The centers are a manufacturing convenience; the bearings never touch them. If the function is “runs true in two bearings,” call the two journals as a common datum A-B and tolerance everything else to it, as described in the guide to concentricity, runout and position. The shop can still turn on centers, and is then responsible for proving the result against the journals.
The opposite mistake is a bushing whose bore is long compared with its thin flange, where the drawing makes the flange face primary. The face is too small to orient the part, so the bore axis tilts with every setup. If the flange face is what seats in the housing, keep it primary but control its perpendicularity to the bore, or make the bore primary and the face secondary. Saola’s CNC turning page describes bar and tube parts such as bushings, caps, inserts, shafts and threaded fittings turned on CNC lathes, which is where this choice comes up most often.
What datum mistakes cause the most rework on machined parts?
The expensive mistakes are datums with no functional reason, datum order that varies from one feature control frame to the next without intent, and datum features that a coating or a later operation changes. Each one leaves the supplier and the customer free to set the part up differently.
- Datums on non-functional edges. Outside edges that only exist because the blank was sawn are easy to probe but say nothing about how the part fits.
- Inconsistent order. |A|B|C| on one hole pattern and |A|C|B| on another is legal, but it creates two frames. Do it only when the function demands it, and expect two setups.
- A datum on a surface that is finished later. Anodize or plating changes a datum face and a datum bore. State whether the datum and its dependent tolerances apply before or after finishing; the guide to anodizing dimensional change covers the build-up.
- A threaded hole as a datum without saying how. Per ASME Y14.5 a screw thread used as a datum defaults to the pitch cylinder, which is hard to simulate; if you mean the major or minor diameter, state MAJOR DIA or MINOR DIA beneath or next to the datum feature symbol.
- Datum letters that point to the wrong drawing. A machined part made from a casting should not reference datum targets that machining removes; the hand-off between the two frames is covered in setting datums on castings for machining.
What should the drawing and RFQ say so both sides measure the same frame?
Name the standard and its year, put the datum order in every feature control frame, and say how the datums are to be simulated when it is not the default. Then ask the supplier to state on the first article report which alignment was used.
A short drawing note does most of the work, for example: “Dimensioning and tolerancing per ASME Y14.5-2018. Datum features established by contact with their high points, not by least-squares fit. Datum features of size at RMB unless modified.” For model-based definitions the same information belongs in the product manufacturing information on the 3D model, and NIST’s MBE PMI test cases are used to test how CAD software carries that information in STEP AP242 files. In the RFQ, add which features you will check on receipt and how; that lets the supplier choose a method that will reproduce your result. The machining RFQ checklist covers the rest of the package, and a ballooned drawing ties each callout to a line in the report.
On Saola’s side, the CNC milling page asks for one datum scheme used on both the casting and the machining drawing, so that one setup serves both. The quality page lists a first-article inspection report covering every toleranced dimension on your drawing, and says a dimension your drawing marks as a process-capability control point is checked through the run, not only at first article. The inspection tools shown on the factory page are calipers, go/no-go pin gauges, dedicated fixture gauges and a height gauge on a granite plate; neither page lists a coordinate measuring machine. If your acceptance depends on a CMM alignment, say so in the RFQ so the measurement method is agreed before the quote, not after the first article.
Frequently asked
Does every feature control frame need three datums?
No. Reference only the datums needed to remove the degrees of freedom that matter for that tolerance. A perpendicularity callout usually needs only the primary, and a position callout on a coaxial bore may need only an axis.
Can the same datum letters appear in a different order on one drawing?
Yes, but each order is a separate datum reference frame, which means a separate setup or alignment. Use it deliberately and expect it to cost inspection time.
Is a datum feature the same as a datum?
No. The datum feature is the real, imperfect surface on the part. The datum is the theoretical plane, axis or point derived from it through a simulator such as a fixture, a surface plate or probed contact points.
What if the supplier wants to use different datums for machining?
That is fine for the process, as long as the finished part is inspected to the drawing’s frame. Ask the supplier to show the conversion on the first article report rather than changing the drawing to suit the setup.
Do ASME and ISO drawings treat datum order the same way?
The order of precedence in the frame works the same way in both systems, but the rules for fitting a datum to the real, imperfect surface differ. State which standard applies on the title block.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024), accessed October 2026
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures, ASME, accessed October 2026
- ISO 5459:2024, GPS — Geometrical tolerancing — Datums and datum systems, ISO, 2024
- MBE PMI Validation and Conformance Testing, National Institute of Standards and Technology, accessed October 2026