GD&T · Lesson 2 of 4 · ~13 min read

Datums and the datum reference frame

Learning outcomes

• You’ll be able to tell a datum feature, its datum feature simulator and the datum apart on a real part and its inspection setup.
• You’ll be able to say which degrees of freedom the primary, secondary and tertiary datums remove, using the 3-2-1 model for flat faces.
• You’ll be able to show how changing the datum order changes a measured value, and pick datum features from how a part mounts.

Prerequisites: Lesson 1: Reading engineering drawings

Example part used in this lesson: AH-101 mounting bracket (fictional, Rev C: Lesson 1’s Rev B geometry with datum features added). All values are decimal inches.

Axes used throughout: X runs along the 3.00 length, Y runs front to back, Z runs up.

What it is

Lesson 1 left you with a question: the first hole is 1.25 from the upright’s outer face, but measured from where on that face, and with the part sitting how? A real face is never perfectly flat or square, so two inspectors can set the part down two ways and get two answers. Datums fix that.

• A datum feature is a real surface (or hole, or pin) on the part that the drawing names as a starting point. On AH-101, the bottom face of the base.
• A datum feature simulator is real, very accurate equipment that the datum feature rests against, such as a granite surface plate, an angle plate or a fixture. On a CMM it can also be software. The bottom face sits on the plate and touches it at its high points.
• A datum is the perfect plane, axis or point that the simulator stands in for. You measure from the simulator, never from the bumpy part surface (Figure 2.1).

In ASME Y14.5-2018 terms, the perfect shape is the true geometric counterpart, and the plane you actually get from the plate is the simulated datum. For this lesson, the three layers above are enough.

Three mutually perpendicular datum planes make a datum reference frame (DRF): a fixed 3D coordinate system the part is locked into before anything is measured. The order you lock it in matters, as you’ll see in Example 3.

Where you’ll see it on the job

• A quality intern setting up a coordinate measuring machine (CMM) has to touch off datum features in the drawing’s order before measuring any hole. Get the order wrong and every result shifts.
• A manufacturing intern planning a fixture puts locating pads on the same faces the drawing calls datums, so the machined part matches how it will be inspected.
• A design intern in a design review is asked why the mounting face is datum A. The answer should be about how the part bolts down, not which face was easiest to draw.
• An intern handling a supplier question finds that the supplier measured the hole from a different face. Their numbers and yours disagree, and the datum scheme decides who is right.

Step-by-step how-to

Use these six steps whenever a drawing references datums.

1. Find the datum feature symbols. A datum feature symbol is a capital letter in a square box. A short line joins it to a triangle on the surface, or on an extension line from it. The triangle can be filled or open, and the letters I, O and Q are skipped because they look like 1, 0 and 9. Each symbol names a datum feature (Figure 2.2). It does not add a tolerance by itself.
2. Find the datum order. The order comes from the feature control frame (FCF), the boxed tolerance callout from Lesson 1. Its datum letters read left to right as primary, secondary and tertiary. Lesson 3 covers how to read it. The letters are labels, so A is not automatically first.
3. Picture the simulators. For each datum feature, picture what it would rest against. Use a surface plate for a flat face, an angle plate or stop for a side face, and a pin or chuck for a hole or shaft.
4. Constrain in order (3-2-1). A free part has six degrees of freedom (DOF): three slides (X, Y, Z) and three rotations (about X, Y, Z). Set the primary datum feature on its simulator first; it touches at three or more points and removes three DOF. Push the secondary against its simulator, keeping the primary seated; it touches at two or more points and removes two more. Slide the part along both until the tertiary touches its simulator at one or more points; that removes the last one. 3-2-1 is a model for three flat datum faces, used by fixture and inspection people. The standard itself talks about which DOF each datum removes, not point counts. With a hole or pin as a datum, the split is different (see the FAQ on features of size).
5. Measure from the simulated datums. Every location is now a distance from a simulator plane, not from the part’s own surface. On a CMM, the software fits a datum plane to the points you probed. It has to use a fit that stays outside the material, like a plate would; a plain average (least-squares) plane can give a different answer.
6. Check the scheme against function. Ask whether the datum features match how the part mounts and mates. A datum scheme that follows the assembly gives measurements that predict fit.

Worked examples

All three use AH-101 Rev C (Figure 2.2). Adding datum features changed the drawing, so the revision block now ends “C | ADDED DATUM FEATURES A, B, C”. As in Lesson 1’s Step 7, check you hold Rev C before you set up. The datum features are A (bottom face), B (upright’s outer face) and C (front face), referenced in the order A, B, C.

Example 1: Check the datum choice against function

Given: AH-101 bolts down through its two holes, bottom face flat against structure. Note 4 masks that face from anodize and chem-films it so it bonds electrically.

• Find the datum feature symbols: A is on the bottom face, B on the upright’s outer face, C on the front face.
• Check the scheme against function: The bottom face is clamped to structure and must conduct, so it controls how the bracket sits. It should be primary. B and C are harder to justify: nothing in the assembly mates against them.

Answer: A on the bottom face is the right primary: it’s the mounting and bonding face. In a real design the bolted holes would often become the next datum, since they locate the bracket. We use the flat faces B and C here because this lesson sticks to flat datums; later lessons show holes as datums.

Example 2: Count the degrees of freedom on the inspection table

Given: The inspector sets AH-101 on a surface plate, pushes it against an angle plate, then against a stop.

• Find the datum order: A, then B, then C.
• Picture the simulators: A on the surface plate, B against a vertical angle plate square to the plate, C against a stop square to both.
• Constrain in order (3-2-1):
  • On the plate, A removes Z travel and rotation about X and Y. That’s 3 DOF.
  • Against the angle plate, B removes X travel and rotation about Z. That’s 2 more.
  • Only Y travel remains, so the part can still slide front to back. The stop on C removes it.

Answer: A removes 3 DOF, B removes 2 and C removes 1, for all 6 (Figure 2.3). With only A and B, the part can still slide in Y.

Example 3: Same part, two datum orders, two answers

Given: On one AH-101, the upright’s outer face leans out by .006 in at its top over the 1.50 in height. Treat the face as perfectly flat, just tilted, and the bottom face as flat, with the hole square to it. At the face’s bottom edge, the first hole’s center is 1.255 in from the face.

This is a thought experiment. A plus-or-minus dimension can’t tell an inspector which face to seat first, which is exactly the problem. On a real drawing the 1.25 would be a basic dimension, controlled by a position tolerance that references A, then B, then C (Lessons 3 and 5). We keep the ±.01 limits (1.24 to 1.26) here so the arithmetic is familiar.

• Find the datum order: The drawing states A, then B. We’ll also see what happens if an inspector seats B first.
• Constrain in order (3-2-1):
  • A first: the base sits flat. The angle plate comes in and touches the upright at its top edge, the point that leans out furthest.
  • B first: the upright face sits flat on the angle plate, and the base tilts slightly.
• Measure from the simulated datums:
  • A first: plane B is .006 in outside the face at base level, so the hole reads 1.255 + .006 = 1.261 in.
  • B first: the face is on plane B, so the part tilts by .006/1.50 = .004 rad. The hole center sits about .125 in up (mid-thickness of the base), so it moves .125 × .004 ≈ .0005 in. Reading ≈ 1.2555 in.

Answer: The stated order is A, then B, so the valid reading is 1.261 in. The part fails. An inspector who seats B first reads about 1.2555 in and wrongly passes it. The part didn’t change; the setup did. That’s why the order has to be on the drawing, and followed (Figure 2.4).

Easy mistakes

Measuring from the part instead of the simulator

Calipers on the part feel direct, so people measure from the bumpy face itself. Measure from the plate, angle plate or CMM plane that simulates the datum.

Assuming alphabetical order

A, B, C look like a ranking, so students treat A as primary by default. The FCF sets the order; read it every time.

Forcing full contact on the secondary

It’s tempting to push the upright flat against the angle plate. That lifts the base off the plate and quietly swaps the order. Keep the primary seated and let the secondary touch where it touches.

Treating the datum feature symbol as a tolerance

The boxed letter looks like a callout, so people expect limits from it. It only names a feature; tolerances come from FCFs and dimensions.

Choosing datums for convenience

The flattest-looking or easiest-to-probe face is tempting. Pick the faces that mount and mate, or the measurements won’t predict fit.

Expecting the datum feature to be perfect

Datum features have form error like any surface. The simulator absorbs it by touching high points; how flat the feature must be is set by form controls in Lesson 4.

Practice questions with answers

Use Figures 2.2-2.4 unless a question says otherwise.

Q1. Which of these is the datum, rather than the datum feature or the simulator?

A) AH-101’s bottom face
B) The granite surface plate
C) The perfect plane the plate stands in for
D) The boxed letter A

Q2. How many degrees of freedom does the primary datum plane remove on AH-101, and which ones?

Q3. With only A and B engaged, what can AH-101 still do?

A) Rotate about Z
B) Slide in X
C) Slide in Y
D) Nothing

Q4. What is the minimum number of contact points for the secondary datum feature in the 3-2-1 model for flat faces?

Q5. Another AH-101’s upright leans out .008 in at the top. The hole center is 1.250 in from the face at base level. With A primary and B secondary, what does it read, and does it pass 1.24 to 1.26?

Q6. In a design review, a colleague proposes the top end of the upright as datum A because it’s easy to probe. What do you say?

FAQs

Why not just measure from the edges with calipers?

You can for a rough check. But calipers pick up whatever bump they land on, so two people get two answers. A datum setup makes the answer repeatable.

Do the letters have to be A, B and C?

No. They’re labels, and a drawing can use other letters. The order comes from the feature control frame.

What if the datum feature is a hole or a pin?

Then the datum is an axis, and the simulator is a pin, chuck or expanding gauge that fits it. Holes and pins are features of size, features with opposed points you can measure across, like a hole’s diameter or the .250 plate thickness. Datums on features of size bring in ideas such as maximum material boundary (MMB), which a later lesson covers.

Do I need a CMM?

No. Surface plates, angle plates and fixtures simulate datums well. A CMM builds those planes in software, but only if its datum fitting is set to mimic contact.

Do companies do datums differently?

The ideas are shared, but some companies have house rules for datum choice. ISO drawings follow ISO datum rules (ISO 5459), which differ in places from ASME Y14.5. Check your company’s drafting manual.

What comes next?

Lesson 3 covers the feature control frame, where datum letters and their order are written.

Sources (all checked 2026-10-28; used for facts only, no text or figures copied)

• GD&T Basics, Datums, datum features, and datum simulators
• GD&T Basics, How GD&T datums control degrees of freedom and Datums
• GD&T Basics, Feature of size and Feature control frame
• Action Engineering, MBE dictionary: ASME Y14.5 terms (datum feature simulator, simulated datum, true geometric counterpart)
• Hexagon PC-DMIS documentation, How PC-DMIS solves datums and NIST, Datum planes based on a constrained norm (PDF) (CMM datum fitting)
• Five Flute, Building datum reference frames
• NJIT (S. Sengupta course notes), Datum precedence rule
• Enerpac, The 3-2-1 locating principle
• IIT Bombay ME338 notes, Fixturing/workholding (PDF)
• WisTech Open, Blueprint Reading, Print symbols and notes
• Wikipedia, Geometric dimensioning and tolerancing and Degrees of freedom (mechanics)
• ASME, Y14.5 Dimensioning and Tolerancing product page (current edition 2018, reaffirmed 2024)