In GD&T, datums are the foundation for establishing geometric relationships and for defining the orientation and location of tolerance zones. A datum may seem like nothing more than a reference label on a drawing, but in reality, it influences how geometric requirements are interpreted, established, and verified. Therefore, to truly understand and select datums effectively, it is not enough to stop at deciding “which surface” or “which hole” to use; it is also necessary to understand the nature of a datum and the logic behind how it is established.
1.What Is a Datum?
A datum is not the physical surface of a part itself, but a theoretically exact reference established from actual geometric features. Actual surfaces always contain form deviations, so they cannot be directly equated with a datum. What is actually used in the definition of geometric tolerances is the ideal plane, ideal axis, or ideal center plane derived from those actual features.

The role of a datum is to provide a clear reference for the tolerance zone. A datum is not simply a “reference surface” or a “reference hole,” but the basis on which a geometric tolerance can be defined.
2.How Is a Datum Established?
A datum does not exist on its own; it is established through a specific process. This process can generally be understood as:
datum feature → datum feature simulator (simulation / fitting) → datum
A datum feature is a feature that physically exists on the part and is designated for establishing a datum, such as a plane, a hole, an external cylindrical surface, or a slot. Because it is a real feature, it may itself contain deviations.
To obtain a stable and consistent reference from these actual features, a datum is established by means of a datum feature simulator (ASME Y14.5-2009). This process may be achieved either through physical simulators in actual contact with the workpiece, such as a surface plate, mandrel, or V-block, or through mathematical fitting in measurement to obtain the corresponding ideal geometric reference.
For example, a plane may establish an ideal reference plane through a surface plate, while an external cylindrical surface may establish an ideal reference cylinder through fitting or enveloping methods. The figure below takes a cylindrical surface as an example.

In the figure, the external cylindrical surface is the datum feature. The actual external cylindrical surface first establishes a reference through an ideal datum feature simulator, which in this example is represented by the minimum circumscribed cylinder (MCC); the center axis derived from that cylinder is the datum.
3.Types of Datums
Datums can be divided into single datums and common datums.
Single datum: a datum established from one datum feature. For example, one base surface may establish a datum plane, or one hole may establish a datum axis. Its characteristics are a single source and a clear establishment relationship.

Common datum: a single datum established from two or more features together. It is not a case of several datums being used in parallel, but rather multiple features jointly forming one unified reference. The figure below shows one datum formed by two surfaces.

This situation usually appears where multiple features must function together, such as two supporting surfaces jointly determining an installation condition, or two coaxial features jointly forming a reference axis.
A single datum emphasizes “one feature establishes one datum,” while a common datum emphasizes “multiple features jointly establish one datum.”
4.Datum System (Datum Reference Frame)
In practical applications, a single datum is often not enough to fully determine the orientation and location of a tolerance zone in space, so a datum system is needed. A datum system is a reference framework composed of one or more datums arranged in a defined order, used to provide a clear and consistent basis for geometric tolerances.
A datum system does not necessarily have to contain three datums. Depending on the geometric requirement, it may use only one datum, or two or three datums. Only when it is necessary to define the part’s spatial attitude, orientation, and positional relationship more completely is the combination of primary, secondary, and tertiary datums typically used.
In a datum system composed of multiple datums, each datum has a definite order of precedence. The primary datum is established first; the secondary datum further constrains orientation on that basis; and, when needed, the tertiary datum completes the remaining positional relationship. Whether a system uses two datums or three, this order directly affects how the reference is established and therefore cannot be exchanged arbitrarily. The figure below compares the differences before and after the datum order is changed.


It should also be noted that a datum system and a common datum are not the same concept. A common datum emphasizes that multiple features jointly form one datum and usually does not reflect any primary-secondary order, whereas a datum system emphasizes that one or more datums form a complete reference framework in a defined sequence.
2. How Datums Affect Machining and Assembly
1) Machining Location
Before CNC machining begins, the part must be clamped, aligned, and assigned a machining coordinate system. That coordinate system is not chosen arbitrarily; it is usually established from a particular surface, hole, or outside diameter. If the datums are selected properly, the part will be more stable during fixturing, the machining coordinates will be easier to keep consistent, and the positional relationships between critical features will be easier to maintain.
2)Assembly Relationship
What matters most in assembly is not whether a single dimension is correct by itself, but whether the relative relationships between critical features are correct. For example, in a housing part, what truly matters is often not the length of one edge, but whether the relationship among the mounting base, locating holes, and side interface meets the assembly requirements. If machining is not based on these function-related datums, a very common situation can occur: every individual dimension looks fine, but the part simply does not assemble properly. This is also why, in the system of geometric dimensions and tolerances, requirements such as position, perpendicularity, and parallelism must all be defined relative to datums. Only with a unified reference can assembly relationships be truly controlled.
3)Tolerance Stack-Up
If a part keeps changing references from one operation to another, errors will gradually accumulate throughout the process. One operation may locate from a raw edge, the next may switch to another side face, and inspection may then use a third reference. Even if every step falls within its own tolerance range, the final critical positional relationship may still end up out of tolerance. The value of datum consistency lies in shortening the error chain as much as possible and reducing unnecessary accumulation.
3. How to Select Datums for CNC Parts
Selecting datums for a part essentially means determining what the part should ultimately reference for machining, inspection, and assembly. Datum selection should not be based only on which surface is larger or which hole is easier to use, but should instead take into account function, assembly, locating stability, and consistency between machining and inspection.
1) Start with the functional relationship
When selecting datums, the first thing to consider is the function of the part. Is it used for support, connection, sealing, or rotational fit? Which positional relationships determine whether it can function properly?
Datums should first serve function, not just machining convenience.
2) Prioritize features involved in assembly and fit
Priority should generally be given to features that actually participate in assembly, locating, and fit, such as mounting surfaces, locating holes, mating outside diameters, or end faces.
In general, machining datums should be as close as possible to assembly datums, so that the resulting dimensions and positional relationships more closely reflect the part’s actual working condition.
3) Prioritize stable and repeatable surfaces or structures
A datum should not only be important, but also stable, rigid, and easy to locate repeatedly. In general, large planes, finished surfaces, and structurally rigid features are better choices for datums, while as-cast or as-formed surfaces, irregular curved surfaces, small bosses, and thin-wall regions should be avoided whenever possible.
4) Pay attention to the hierarchy within the datum system
After identifying which features are suitable as datums, their hierarchy within the datum system must also be determined. In general, the feature that first establishes the basic attitude of the part can serve as the primary datum; the feature that further constrains orientation can serve as the secondary datum; and when the remaining positional relationship still needs to be defined, a tertiary datum can be introduced.
For example, for a mounting block, the bottom surface used to contact the mounting surface can serve as primary datum A; the side surface used to contact a locating edge can serve as secondary datum B; and the end face used to control the assembly distance can serve as tertiary datum C. In this way, the position of a mounting hole can be defined relative to the A-B-C datum system.
5) Minimize the number of setups
Each additional setup adds another round of re-alignment and coordinate re-establishment, and therefore another source of error.
For this reason, as many critical features as possible should be machined under the same reference framework, so as to reduce error accumulation and lower machining cost.
6) Keep machining and inspection references as consistent as possible
Design datums, process datums, and inspection datums should be kept as consistent as possible, or at least highly correlated. Otherwise, if machining is carried out using one reference while inspection is performed using another, dimensional disputes or even misjudgment can easily occur.
4. Practical Examples
1) Housing-Type Part
For this type of housing part, we use the bottom mounting surface as the primary datum A because it is the main reference surface for both assembly and machining location; we use the center axis of the angled circular cavity in the middle as the secondary datum B to control the positional and directional relationship between the cavity, the bottom face, and the related features; and we use the center axis of the hole in the right-side connection port as the tertiary datum C to further define the mounting position and direction of the connection port.
Once these datums are established, the position, orientation, and assembly relationship among the bottom face, cavity, and connection port become much easier to control consistently.

2) Shaft-Type Part
For this shaft-type part, we use the overall center axis as the primary datum A because it determines the coaxial relationship of the various outside diameters and the rotational accuracy; we then use the critical locating shoulder face as the secondary datum B to control the axial mounting position. For this type of rotationally symmetric part, the main functional relationships are usually built around the axis and the shoulder face, so these two datums are sufficient to control concentricity, runout, and assembly position effectively.

Conclusion
Datum selection essentially answers one question: what should this part ultimately reference for machining, inspection, and assembly?
Only when the right datum is chosen can dimensions, tolerances, and assembly relationships be truly aligned. If the wrong datum is selected, even high machining accuracy may fail to land where it matters. For parts that require CNC machining, the datum is not a secondary detail to be considered later, but a prerequisite that determines whether the machining result is truly effective.