A datum is a theoretically exact point, axis, or plane from which the location, orientation, size, or form of features on a part are measured and controlled. The datum is not a physical feature — it is a geometric reference derived from the physical feature designated as the datum feature.
This distinction — between the datum (theoretical) and the datum feature (physical) — is the most misunderstood aspect of datum definition in mechanical engineering, and it is where most inspection errors originate. The flat face of a machined aluminum block is a datum feature. The perfect, theoretical plane that the datum simulator (a precision surface plate or CMM fixture) represents is the datum. You never measure from the physical surface directly; you measure from the theoretical datum that the physical surface establishes through contact with a datum simulator.
This article covers the precise ASME Y14.5-2018 definition of a datum, how the three-datum reference frame is constructed, how datums are selected in practice, and how datum definition directly affects dimensional control in laser-cut and machined parts.
Datum Definition: The ASME Y14.5-2018 Standard
ASME Y14.5-2018 — Dimensioning and Tolerancing — is the governing standard for datum definition in US mechanical engineering practice. Its definition:
A datum is a theoretically exact point, axis, line, or plane from which the location or geometric characteristics of features of a part are established.
Three terms in this definition require precision:
“Theoretically exact”: The datum has no error. A real machined surface has flatness error, waviness, and surface roughness. The datum ignores all of this — it is perfect. The datum is established by how the datum feature contacts its datum simulator (the measurement equipment or fixture), not by averaging the surface.
“Point, axis, line, or plane”: Datums are simple geometric primitives. A cylindrical feature establishes a datum axis (the perfect theoretical axis of the cylinder). A flat surface establishes a datum plane. A spherical feature establishes a datum point. The datum is the simplest geometry the physical feature reasonably represents.
“From which … features are established”: The datum is a reference origin. Tolerances, dimensions, and geometric controls are stated relative to the datum — meaning inspectors and fixture designers must locate parts to simulate the datum before any measurement is valid.
ISO 5459 (the international equivalent for datum definition in ISO-system technical drawings) uses similar language but organizes datum simulation differently. For international work, verify which standard applies — ASME Y14.5 and ISO 5459 are compatible in concept but differ in some annotation practices.
The Datum Reference Frame: Three Mutually Perpendicular Planes
Most engineering parts require more than one datum to constrain their position in space fully. The datum reference frame (DRF) consists of three mutually perpendicular datum planes designated primary, secondary, and tertiary. Together, they constrain all six degrees of freedom of a rigid body (three translational, three rotational).
Primary datum
The primary datum plane contacts the datum feature at at least three high points (three-point contact). It removes two rotational degrees of freedom (the part cannot rock about the X or Y axis relative to the datum plane) and one translational degree of freedom (Z-position is constrained).
Selection rule: The primary datum feature should be the surface that locates the part most functionally, the surface that matters most for the part’s fit in the assembly. For most flat plate parts, this is the largest flat face. For a turned shaft, it is typically the axis (which becomes a datum axis).
Secondary datum
The secondary datum plane contacts the datum feature at at least two high points. It removes one additional rotational degree of freedom (rotation about Z is constrained) and one additional translational degree of freedom (Y-position is constrained).
Selection rule: The secondary datum is typically the surface that controls the next most functionally important location — often an edge, a machined groove, or a specific bore that locates the part laterally.
Tertiary datum
The tertiary datum contacts the datum feature at a single point, removing the final translational degree of freedom (X-position is constrained). All six degrees of freedom are now fully constrained: the part has a unique, repeatable location in the datum reference frame.
Selection rule: The tertiary datum is often a secondary locating feature — a small hole, a pin location, or an end face — that prevents the part from sliding along the secondary datum surface.
Why order matters
The three-point contact of the primary datum → two-point contact of the secondary datum → one-point contact of the tertiary datum is not an arbitrary convention. It reflects how parts are physically seated: a wobbly primary contact creates positional error that cascades into every secondary and tertiary measurement. The rule: seat the part on its primary datum first, then contact the secondary datum without lifting from the primary, then contact the tertiary without lifting from either.
A CMM operator who contacts the secondary datum before the primary is fully seated — because it is physically convenient in the machine setup — produces systematically incorrect measurements. The datum definition in the part drawing specifies the contact sequence as well as the contact features.
Datum Features and Datum Simulators
The datum feature is the physical surface, axis, or point on the actual part that establishes the datum. The datum simulator is the precision surface, gauge pin, or CMM reference that contacts the datum feature to simulate the theoretically exact datum.
| Datum feature type | Datum established | Common datum simulator |
|---|---|---|
| Flat machined surface | Datum plane | Precision surface plate, CMM fixture plate |
| External cylinder | Datum axis | V-block, collet, CMM cylinder scan |
| Internal cylinder (bore) | Datum axis | Precision gauge pin, expanding mandrel |
| Flat end face + bore | Datum axis + plane | Combination fixture: face plate + pin |
| Sphere | Datum point | Precision socket, CMM sphere scan |
| Two parallel planes | Datum center plane | Gauge blocks contacting both faces |
The datum simulator must have a flatness, roundness, or straightness error significantly smaller than the tolerance being simulated — typically at least 10:1 (gauge ratio). A surface plate used as a primary datum simulator for a 0.05 mm flatness tolerance should itself have a flatness better than 0.005 mm across the workpiece contact area.
Datum shift: When a datum feature is not perfect — when a hole used as a secondary datum has some size error within its tolerance — the position of the datum axis can shift relative to the perfect theoretical axis by the amount of the datum feature’s departure from perfect form. This datum shift is a real tolerance that can be usable or harmful depending on the drawing specification. ASME Y14.5-2018 distinguishes between datum features referenced at Regardless of Feature Size (RFS), Maximum Material Condition (MMC), and Least Material Condition (LMC), with datum shift permitted only in the MMC and LMC cases.
Read More: Tolerance Definition
Selecting Datums for Laser-Cut and Sheet Metal Parts
Datum selection for laser-cut flat parts, formed sheet metal, and machined plate follows specific conventions driven by the part’s function and the manufacturing process.
Primary datum on laser-cut flat parts
For a laser-cut flat plate, the primary datum is almost always the flat face — the surface that was lying on the laser cutting table during processing. This surface has the smallest flatness error (gravity ensures it conforms to the table surface during cutting) and is the functional mounting surface in most applications.
Exception: If the part mounts on its edge or on a machined feature that is added after laser cutting, the functional mounting surface should be the primary datum regardless of the cutting setup.
Secondary datum for rectangular plates
The secondary datum for a rectangular laser-cut plate is typically the longest straight edge. On a fiber laser-cut part, all four edges have similar geometric quality, but the longest edge provides the most stable two-point contact for secondary datum simulation. The second-longest edge is the tertiary datum.
The implication for inspection: When measuring the location of a hole in a laser-cut bracket, the inspector must seat the part on its primary datum face first (surface plate contact), then contact the secondary edge (using a precision stop or gauge block), then contact the tertiary edge. The measured hole position is only meaningful relative to this correctly established datum reference frame. An inspector who simply clamps the part in a convenient orientation and measures from the clamp faces introduces a systematic datum error.
Datum selection for turned and bored parts
For parts with cylindrical features — flanges, hubs, nozzles, tube fittings — the datum is typically:
- Primary: The bore axis (the functional centerline that mates with a shaft or pin) — established as a datum axis
- Secondary: The flat face perpendicular to the bore (the mounting face) — established as a datum plane
- Tertiary: A keyway, cross-hole, or timing feature that prevents rotation — established as a point or plane
This sequence reverses the flat-part convention: the bore axis precedes the flat face because concentricity of the outer features to the bore is the primary functional requirement. Machining the part with the bore as the primary datum — in a lathe or on a mandrel — ensures that all features are coaxial to the functional centerline.
Common Datum Definition Errors in Practice
Understanding the definition of a datum is straightforward in theory. Applying it correctly in a production environment is where errors accumulate.
Error 1: Measuring from the datum feature instead of the datum
An inspector places a part on a surface plate and measures from the surface plate correctly. Another inspector clamps the same part in a fixture and measures from the clamp reference. If the clamp does not precisely simulate the primary datum plane, the two measurements are taken from different datums and will disagree, even if both inspectors are competent.
Consistent datum simulation throughout the manufacturing process — same fixture for machining, same fixture family for CMM inspection — is the physical implementation of datum definition. The drawing defines the datum; the fixtures ensure the same datum is used at every stage.
Error 2: Reversing primary and secondary datum order
A part is fixtured on its secondary datum surface for machining convenience, then inspected using the correct primary datum. The machining operations were performed relative to a different datum than the inspection. Features that appear to be in tolerance relative to the machining datum may be out of tolerance relative to the inspection datum.
This error is particularly common when laser-cut blanks are subsequently machined in a mill vice that contacts the edges (secondary/tertiary datums) rather than the flat face (primary datum). The resulting edge features are accurately positioned relative to the edges — but the drawing likely calls for them to be positioned relative to the face.
Error 3: Incomplete datum specification on the drawing
A drawing that specifies only a primary datum allows the part to rotate about the primary datum axis and translate along the primary datum plane — it has four unconstrained degrees of freedom. A position tolerance applied to a hole location is meaningless relative to a single-datum reference if the part can still rotate.
ASME Y14.5-2018 requires that position tolerances reference a datum reference frame with enough datums to constrain all degrees of freedom relevant to the controlled feature. A hole in the center of a flat plate requires only the primary datum plane to control its Z-position — but to control its X and Y position, the secondary and tertiary datums must be specified.
Frequently Asked Questions About Datum Definition
Q: What is a datum in mechanical engineering?
A datum is a theoretically exact point, axis, or plane from which the location or geometric characteristics of part features are measured and controlled. Per ASME Y14.5-2018, the datum is derived from the datum feature (the physical surface) through contact with a datum simulator (a precision reference surface, pin, or gauge). The datum itself is perfect; the physical datum feature has imperfections. All dimensions and tolerances are measured relative to the theoretical datum, not directly from the physical surface.
Q: What is the difference between a datum and a datum feature?
The datum feature is the actual physical surface, cylinder, or point on the part that designates which feature establishes the reference. The datum is the theoretical geometric entity (perfect plane, perfect axis, perfect point) that the datum feature establishes through contact with a precision datum simulator. A machined flat face is the datum feature; the perfect plane that a precision surface plate represents is the datum. You measure from the datum, not from the datum feature directly.
Q: What are primary, secondary, and tertiary datums?
The three datums form a datum reference frame (DRF) that fully constrains a part’s position in space. The primary datum contacts the datum feature at three minimum points, removing three degrees of freedom. The secondary datum contacts at two minimum points, removing two more. The tertiary contacts at one point, removing the final degree of freedom. Together they constrain all six degrees of freedom (three translational, three rotational). The order of contact during inspection must follow the sequence primary → secondary → tertiary; changing the order changes the established datum reference frame and produces incorrect measurements.
Q: How are datums chosen for sheet metal and laser-cut parts?
For flat laser-cut plate parts, the primary datum is typically the flat face (largest functional surface), the secondary datum is the longest edge, and the tertiary datum is an adjacent edge. For cylindrical features, the primary datum is usually the bore axis (functional mating feature), with the flat mounting face as the secondary datum. Datum selection should reflect functional priority — the features that matter most for fit and function in the assembly should be primary.
Q: What is datum shift in GD&T?
Datum shift is the allowable variation in the location of a datum axis or center plane when the datum feature departs from its maximum material condition (MMC) size. For example, if a 10 mm hole is designated as a secondary datum at MMC (when the hole is exactly 10 mm — the smallest allowed size), the datum axis is perfectly centered in the hole. If the hole is actually 10.2 mm (0.2 mm above MMC), the datum axis can shift by up to 0.1 mm in any direction within the hole. Datum shift effectively increases the usable positional tolerance — a permitted practice called a bonus tolerance at MMC. Datum shift at RFS (regardless of feature size) is zero — no shift is permitted.
References
- American Society of Mechanical Engineers (ASME), ASME Y14.5-2018: Dimensioning and Tolerancing, ASME, New York, 2018. (The governing US standard for datum definition, datum reference frames, primary/secondary/tertiary datum selection, datum simulators, datum shift at MMC and LMC, and GD&T symbology; all datum terminology and definitions in this article derive from this standard.)
- International Organization for Standardization, ISO 5459:2011, Geometrical Product Specifications (GPS) — Datums and Datum Systems, ISO, Geneva, 2011. (The ISO equivalent of ASME Y14.5 datum requirements; establishes datum and datum system definitions for ISO-based technical drawings; used for international comparison and for shops working to both US and European drawing standards.)
- American Society of Mechanical Engineers (ASME), ASME B89.3.1-1972: Measurement of Out-of-Roundness, ASME, New York, 1972. (Roundness measurement methodology for cylindrical datum features; the basis for how datum axes are established from imperfect cylindrical surfaces; datum simulator requirements for bores and shafts used as datum features.)
- Budynas, R.G., and Nisbett, J.K., Shigley’s Mechanical Engineering Design, 11th Edition. McGraw-Hill Education, New York, 2020. (Tolerancing and fits, GD&T introduction, datum reference frame application in mechanical design; design context for datum selection based on functional priority in assemblies.)
Read More: Sheet Metal Bending Calculation K-Factor
- Laser Marking Focus Problems: Symptoms and Solutions - August 31, 2026
- Inline Laser Marking Systems for Automated Production Lines - August 30, 2026
- Laser Safety Requirements for Industrial Laser Marking Machines - August 27, 2026
