Datums and Datum Reference Frames
Where every GD&T measurement starts: datum features and simulators, the six degrees of freedom, how to choose datums, datum targets, and datum shift at MMB.
A datum is where every measurement on a GD&T drawing starts. It is what turns “how far is this hole from that edge?” into a question with exactly one answer. This page explains datums, datum features and the simulators that stand in for them, how a datum reference frame holds a part in all six degrees of freedom, how to choose datums, datum targets for rough or flexible parts, and how material condition at a datum feature creates datum shift. It is part of the GD&T guide and follows ASME Y14.5-2018, with ISO 5459 differences noted.
Datum, datum feature and simulator
Four terms are easy to mix up, and the whole subject depends on keeping them apart.
| Term | What it is | Example |
|---|---|---|
| Datum (theoretical) | A perfect plane, axis or point that exists only in theory. Measurements are made from it. | The perfectly flat plane that the bottom of a block would sit on |
| Datum feature | The real feature on the part that is identified with a datum feature symbol. It is imperfect: rough, bowed, a little out of round. | The actual bottom face of the block, with its machining marks and any bow |
| Datum feature simulator | The equipment that stands in for the datum during inspection, or that touches the part in the machine: a surface plate, a gage pin, a chuck, an angle plate. | The granite surface plate under the block; a ⌀20.00 gage pin in a datum hole |
| Datum reference frame (DRF) | The set of up to three mutually perpendicular planes (or axes and points) built from the datums in order of precedence. It is the coordinate system for the measurements. | The three planes A, B and C that the bracket is pressed against |
The idea behind the table: you never measure from the real datum feature itself, because it is imperfect and the answer would depend on which spot you touched. You make the datum feature touch a simulator, which is accurate, and measure from the simulator. A flat but slightly bowed face rests on a surface plate at its high points, and that contact fixes the datum.
The datum feature symbol
- The symbol is a capital letter in a square frame, joined by a leader to a triangle that touches the feature. ASME allows the triangle to be filled or empty.
- On a surface or its extension line (not in line with a dimension line), the surface is the datum feature and the datum is a plane. Placing the symbol on the dimension line of a feature of size, in place of one arrowhead, makes the axis or center plane of that feature the datum.
- Letters. ASME skips I, O and Q because they look like numbers, and after Z continues AA, BB, CC. Use letters in the order the drawing needs them, not necessarily A, B, C by importance.
- One letter per datum feature. A feature can only be one datum on a drawing, and a datum letter must be defined by a datum feature symbol somewhere on the drawing before it is referenced.
- A datum feature symbol can sit on a feature control frame for the feature it controls, so a feature that is both toleranced and a datum is shown once.
Six degrees of freedom
A free body can move along three axes (translation in X, Y and Z) and turn about three axes (rotation about X, Y and Z): six degrees of freedom. A datum reference frame removes degrees of freedom one datum at a time until the part is held in the way the drawing needs.
| Datum | Minimum contact | Degrees of freedom removed | Left over |
|---|---|---|---|
| Primary plane A | 3 points (high points of the surface) | 1 translation (normal to A) + 2 rotations (about the two axes lying in A) = 3 | 3: slide in A (2) and spin about the normal to A (1) |
| Secondary plane B | 2 points | 1 translation (normal to B) + 1 rotation (about the normal to A) = 2 | 1: slide along B |
| Tertiary plane C | 1 point | 1 translation (normal to C) = 1 | 0: fully located |
This is the 3-2-1 principle shown on the GD&T overview page. Real parts do not have to use three flat faces. A cylindrical datum feature gives an axis, and an axis removes four degrees of freedom at once:
| Datum scheme | What each datum removes | Total |
|---|---|---|
| A = bore or shaft (axis) | 2 translations + 2 rotations perpendicular to the axis = 4 | 4 |
| B = shoulder or end face (plane perpendicular to A) | 1 translation along the axis = 1 | 5 |
| C = a hole, slot or flat that fixes the angle | 1 rotation about the axis = 1 | 6 |
You only need to constrain the degrees of freedom that matter for the measurement. If a bolt circle has no angular requirement to anything, datum C is not needed: leaving the rotation free is correct, and the pattern is still fully defined. Adding an unnecessary datum makes the part harder to inspect and can reject good parts.
Order of precedence
Datums are listed in the feature control frame in order of precedence: primary first, then secondary, then tertiary. The order is not a matter of taste: it tells the inspector which datum feature gets to rest on its simulator first, and which one is only allowed to touch what is left.
- The primary datum feature touches its simulator at the three highest points (for a plane). It gets the best, most stable contact.
- The secondary datum feature touches its simulator after the primary has been set, and the simulator is held at the correct angle to the primary. If the real secondary face is a little out of square, it touches at only two high points.
- The tertiary datum feature touches last, at one point, with its simulator square to both of the others.
- Swapping the order changes the answer. | A | B | and | B | A | hold the part differently, so the same part can pass with one and fail the other. This is exactly why an order is always written, and why the primary datum should be the surface that really seats the part in its assembly.
Choosing datum features
Good datums come from how the part is used, not from what is convenient on the drawing. Work through these questions for every candidate:
- Function. Which features locate the part in its assembly? The face that bolts to the frame, the bore that a shaft runs in, the pin that locates it. These are the datums, because the mating part sees the same references.
- Stability. Is it large enough and well enough shaped to hold the part steady? A long flat face makes a good primary; a tiny pad does not. A short bore is a poor datum axis because it can rock.
- Accessibility. Can the inspector and the machine both reach it? A datum hidden inside a cavity is hard to use.
- Repeatability. A reasonably flat, clean surface gives the same set-up every time. If the datum surface is rough or bowed, add a flatness control to it, or use datum targets.
- Manufacturing order. Machine the datum features first, in one set-up, so everything else is cut relative to them, and the drawing’s datum scheme matches the way the shop holds the part.
Typical datum schemes
| Part | A (primary) | B (secondary) | C (tertiary) | Why |
|---|---|---|---|---|
| Bracket or plate | Mounting face | Long edge or dowel hole | Short edge or second hole | Seats on the machine frame, then locates in the plane |
| Flange | Mounting face | Pilot bore or spigot (axis) | One bolt hole, only if the angle matters | Mates face to face, centers on the pilot |
| Shaft | Both bearing journals together (A-B) | Shoulder against a bearing | Keyway, only for angle | Runs on its bearings, so they define the axis |
| Housing | Mounting face | Main bore (axis) | Dowel hole or side face | Bolts down, then centers the rotating part |
| Sheet-metal part | Flat face (often with targets) | Edge or hole | Second edge or hole | Flexible: datum targets give a repeatable set-up |
| Casting | Datum targets on the base (A1-A3) | Targets on a side (B1-B2) | One target on an end (C1) | Rough surfaces, so only small spots are controlled |
Common datums (A-B)
Sometimes one datum is created by two features working together, for example a shaft that runs on two separated bearing journals. The datum letters are written in one compartment of the frame with a dash, A-B, and the two features together establish a single common datum axis. Neither has priority over the other: both simulators are applied at the same time.
- Use it when the function really is “the axis through both journals”, such as a shaft, a two-bore housing, or a gear on two bearings.
- Why it matters. Using only one journal as the datum would let the other journal’s misalignment count as part of the error of every other feature, and a short datum axis can tilt. The common axis is the same axis the bearings use.
- Two bores on one datum also works: an in-line pair of bores at either end of a housing gives a long, stable axis, much better than a single short bore.
- In ISO 5459 the same idea is a “common datum” written A-B, with the same meaning.
RMB, MMB and datum shift
When a datum feature is a feature of size (a hole, a pin, a slot, a tab), its size varies within the size tolerance, and the drawing has to say how the simulator treats that. There are three choices, written after the datum letter in the frame:
| Reference | Written as | The simulator… | Datum shift? |
|---|---|---|---|
| RMB (regardless of material boundary) | A (no modifier: this is the default) | adjusts to the actual size of the datum feature: it expands into a hole or closes on a pin until it touches. Think of an expanding mandrel or a self-centering chuck. | No: the datum axis follows the actual feature |
| MMB (maximum material boundary) | A Ⓜ | is fixed at the maximum material boundary size. A feature smaller than MMB (for a pin) or larger (for a hole) can float on it. | Yes |
| LMB (least material boundary) | A Ⓛ | is fixed at the least material boundary size, which is the other end of the size range. | Yes |
The boundary used by MMB or LMB is the size limit itself, unless a geometric tolerance on the datum feature makes it bigger or smaller (then it is the virtual condition; see Modifiers and Material Conditions).
What datum shift is
Datum shift (total, on diameter) = actual size of the datum feature − MMB size (for a hole)
Datum shift (total, on diameter) = MMB size − actual size (for a pin or shaft)
Datum shift is a bonus that only exists because the feature is not at its worst-case size. It is how a functional gage works: the gage has a fixed pin at the MMB size, and a part with a larger-than-minimum hole simply has some clearance to move on it.
When to use which. Use MMB when the part will assemble onto a pin or into a hole with clearance (a typical bolted joint, or a locating pin), so the function really can use the clearance, and when you want to inspect with a fixed functional gage. Use RMB when the datum feature must center the part exactly, such as a press fit, a bearing seat or a rotating part where runout is measured from the axis.
Datum targets
A whole surface is a poor datum when it is rough, curved, large or flexible: a casting face, a forging, a molded part, a sheet-metal panel. Datum targets pick out specific points, lines or areas on the surface that are to be used as the datum, so the set-up is repeatable. The datum plane is established only by those targets.
| Target | Symbol on the drawing | Minimum for a plane | Typical use |
|---|---|---|---|
| Point | An X on the surface, joined to a circle split in two: the bottom half has the datum letter and number (A1) | 3 targets (A1, A2, A3) | Cast and forged bases that rest on three pads or pins |
| Line | A phantom line with an X at each end, joined to the same circle | 2 targets (one line takes the place of two points) | Rolled edges, a straight edge resting on a rail |
| Area | A cross-hatched area (a circle, usually) with a dashed outline, joined to a circle whose top half gives the size, for example ⌀6 | 3 targets as areas | Pads on a casting or molded part, clamped locations |
- The targets are located with basic dimensions from the other datums, so the position of each target is exact, not toleranced.
- A 3-2-1 scheme with targets is written A1, A2, A3 (the primary plane on three points), B1, B2 (the secondary on two) and C1 (the tertiary on one). The datum feature symbol A then names the whole set of targets A1 to A3.
- Movable datum targets (ASME Y14.5-2018) are targets that move to center or adjust, for example a V-shaped locator that centers a round part. They are drawn with an arrow showing the direction and range of movement.
- Why use them. The inspector rests the part on three small supports at the correct places instead of on a rough surface that may rock, and the foundry and machine shop can agree exactly where the part is held.
Worked examples
Example 1: a flange, and which datums it needs
A flange bolts to a mating flange and centers on a pilot bore. The four ⌀11 holes sit on a ⌀90 bolt circle.
- A = back face. It is the face that seats against the mating flange, so it is the primary: it removes 3 degrees of freedom (1 translation along the axis and 2 tilts).
- B = pilot bore, an axis perpendicular to A. It removes 2 more (the two translations in the plane of A). Total: 5.
- The sixth, a rotation about the bore axis, stays free. The holes are equally spaced on the circle, with no requirement to line up with anything, so no datum C is needed.
- The holes’ frame, position ⌀0.2 at MMC to | A | B |, is enough. If a drawing later needs one hole or a tab at a particular angle, that feature becomes datum C.
Example 2: how much datum shift?
Datum feature B is a hole of size ⌀20.00 to ⌀20.10 and is referenced at MMB. The MMB size of a hole is its smallest size, ⌀20.00, so the pin simulator is ⌀20.00. For several actual hole sizes:
| Actual size of B | Clearance on diameter (datum shift) | Float in any direction | Meaning |
|---|---|---|---|
| 20.00 | 0.00 | ±0.000 | No clearance, so no shift |
| 20.03 | 0.03 | ±0.015 | Part can float; pattern may sit this far off the hole’s own axis |
| 20.06 | 0.06 | ±0.030 | Part can float; pattern may sit this far off the hole’s own axis |
| 20.10 | 0.10 | ±0.050 | Part can float; pattern may sit this far off the hole’s own axis |
So a pattern of holes with position ⌀0.2 relative to | A | B Ⓜ | may, at B = ⌀20.10, be centered up to 0.05 away from the bore’s own axis and still pass, on top of its own tolerance zone. At B = ⌀20.00 the pattern has to be exactly centered on the bore.
Example 3: RMB or MMB for a bearing seat?
A housing has a bore ⌀42.000 to ⌀42.016 that receives a bearing, and two bolt holes that fasten a cover. Datum B is the bore.
- For the bolt holes, referenced to B, MMB is reasonable: the cover just bolts on, with clearance in the screw holes, and a functional gage can check them.
- For the shaft that runs in the bearing (for example a coaxiality or runout control), use RMB: the bearing seat defines the true rotation axis whatever its actual size, so no datum shift may be added.
- The same physical bore can be a datum in two different ways on two different features. The reference modifier on each frame says which applies.
Example 4: datums for an L-bracket
An L-bracket bolts its base to a machine and its upright face locates a sensor. Mounting holes in the base and a slot in the upright are toleranced.
| Datum | Feature | Reason |
|---|---|---|
| A | Underside of the base | It is the face that seats on the machine, so it is the primary. Flatness 0.05 added to make it a good datum. |
| B | Back edge of the base | A long edge that the bracket is pushed against when assembled. Perpendicularity 0.1 to A makes it a reliable secondary. |
| C | Side edge of the base | A short edge that stops sliding along B. One point of contact is enough for the tertiary. |
Every toleranced feature on the bracket then refers to | A | B | C |, which is the order the shop clamps it in and the way the bracket is assembled.
Troubleshooting
| Symptom | Likely cause | Try |
|---|---|---|
| Two inspectors get different results | Datum order missing or ambiguous, datum feature not clearly marked, or a datum scheme that does not match how the part is held | Check every frame for a complete, ordered datum list; mark datum features clearly; agree the set-up before measuring |
| The part rocks on its primary datum | Primary surface is bowed or rough, so it touches only at the high points | Add a flatness tolerance to the datum feature, or use datum targets |
| The pattern only passes in one orientation | A degree of freedom is not constrained, typically the rotation, because a tertiary datum is missing | Add the tertiary datum that really fixes the angle, if the function needs it |
| Good parts fail in the gage | Datum referenced RMB where MMB was intended, so the gage does not allow the clearance | Decide what the mating part does, and state MMB when there is clearance to use |
| Datum feature keeps moving between set-ups | A short bore or a tiny pad is an unstable datum | Use a longer feature, a common datum A-B, or a larger surface |
| A datum letter is not defined | A frame refers to a letter that has no datum feature symbol on the drawing | Add the symbol, or correct the letter |
Related
- GD&T: the overview, symbols and a quick reference to the 14 characteristics.
- Form Tolerances: controls with no datum at all.
- Orientation Tolerances: the first controls that always need a datum.
- Position and Location: locating features from the datum reference frame.
- Workshop Safety and Shop Tools: surface plates and measuring set-ups.
FAQ
Do I always need three datums?
No. Use only the datums the function needs. A single flat face may be enough for a flatness or parallelism control; a bolt pattern may need just a face and a bore. Extra datums cost money and can reject good parts.
What is the difference between a datum and a datum feature?
The datum is the perfect plane, axis or point of theory. The datum feature is the real, imperfect surface or feature that is used to find it. The datum feature touches a simulator, and the simulator represents the datum.
Does the order of the datums really matter?
Yes. The primary datum feature seats first, the secondary is then held square to it, and the tertiary is held square to both. A different order holds the part in a different way and can give a different measurement of the same part.
Can a datum feature have its own tolerance?
It should usually have one. A flatness tolerance on a primary surface, or perpendicularity on a secondary, tells the shop how good the datum surface must be, because a poor datum makes every measurement from it unreliable.
What does “A-B” in one box mean?
Two datum features that together establish a single common datum, for example two bearing journals that define one axis. They are applied at the same time, with no priority between them.
Is RMB really the default?
Yes, in ASME Y14.5 since the 2009 edition: if a datum feature of size has no modifier, its simulator adjusts to the actual size of the feature (RMB). Older drawings sometimes assumed MMB, so check which edition applies.
What is the difference between datum shift and bonus tolerance?
Bonus tolerance enlarges the tolerance zone of a feature when that feature leaves its MMC. Datum shift lets the whole part move on the datum simulator when the datum feature leaves its MMB. Both come from clearance, and both are only available when the matching modifier is written.
Why are the datum letters I, O and Q not used?
They are too easy to read as the numbers 1 and 0. ASME skips them, and some company standards also avoid X, Y and Z because they are axis names.
References
- ASME Y14.5-2018, Dimensioning and Tolerancing (datum features, datum reference frames, datum targets and material boundary modifiers).
- ASME Y14.43, Dimensioning and Tolerancing Principles for Gages and Fixtures (simulators and functional gages).
- ISO 5459, Geometrical product specifications (GPS): Geometrical tolerancing: Datums and datum systems.
- Krulikowski, A., Fundamentals of Geometric Dimensioning and Tolerancing, Cengage.
- Meadows, J. D., Geometric Dimensioning and Tolerancing: Applications, Analysis, Gaging and Inspection, CRC Press.
Last reviewed: October 2026. Always read the standard that your drawing names; rules differ between ASME editions and between ASME and ISO.