Geometric Dimensioning and Tolerancing (GD&T): A Complete Guide

Geometric dimensioning and tolerancing (GD&T) is a standardized system of symbols and rules used on engineering drawings and 3D models to define how much a part's form, orientation, location, and profile can vary while still functioning correctly. Unlike traditional plus-or-minus dimensions, which mainly control size, GD&T describes each feature's geometry and how it relates to the rest of the part, giving designers, machinists, and inspectors one shared language.

No manufacturing process produces perfect geometry. Holes drift slightly, surfaces aren't perfectly flat, and shafts are never perfectly round. GD&T defines exactly how much imperfection is acceptable. In this guide, we'll cover why GD&T matters, how to read a feature control frame, how datums work, what each symbol controls, and how to apply GD&T effectively.

Why GD&T Matters

Traditional plus-or-minus dimensioning is simple, but it doesn't clearly define where measurements start and can be interpreted differently by different people. It also creates tolerance zones that don't always match how parts function.

Hole position is a classic example. Plus-or-minus coordinate dimensions create a rectangular tolerance zone, yet a bolt fits just as well whether a hole drifts horizontally, vertically, or diagonally by the same distance. GD&T position tolerances use a cylindrical tolerance zone that matches this functional requirement more closely, which can provide more usable positional tolerance than coordinate tolerancing for the same fit requirement. As a result, more good parts pass inspection.

The benefits include clearer communication, tolerances based on function, more manufacturing flexibility, consistent inspection, and less scrap and rework.

GD&T Standards: ASME Y14.5 and ISO GPS

ASME Y14.5 is the dominant standard in North America, with the 2018 edition being current. ISO GPS (Geometrical Product Specifications), including ISO 1101 for geometric tolerancing, is widely used in Europe and international supply chains.

Both share core concepts but differ in symbols, terminology, and default rules. ASME Y14.5-2018 removed the concentricity and symmetry controls. ISO GPS standards retain related requirements, but their definitions and application are not always identical to older ASME editions, so the applicable ISO standard should be consulted directly.

The standards also treat size and form differently by default. Under ASME's Rule #1 (envelope principle), a feature's size limits also control its form, while ISO's independency principle controls size and form separately unless the envelope requirement is specified. Every drawing should state which standard and edition applies.

Key GD&T Terms

Feature of size: a feature with a measurable size, such as a hole, pin, or slot.

Basic dimension: a theoretically exact dimension shown in a box. It locates features or defines profiles, while the allowable variation comes from the geometric tolerance.

Tolerance zone: the space within which a feature must lie, such as two parallel planes for flatness or a cylinder for hole position.

Datum: a theoretically exact reference, such as a plane or axis, from which measurements are made.

How to Read a Feature Control Frame

GD&T requirements appear in a feature control frame, a rectangular box attached to a feature, read from left to right:

1. Geometric characteristic symbol: the type of control, such as flatness or position

2. Tolerance value: the size of the tolerance zone, with a diameter symbol (Ø) when the zone is cylindrical, followed by any modifiers that apply to the toleranced feature

3. Datum references: the primary, secondary, and tertiary datums, listed in order of precedence

For example, Position | Ø0.1 Ⓜ | A | B | C means the feature's axis must lie within a 0.1 mm diameter cylindrical tolerance zone. The Ⓜ modifier means the tolerance applies at the feature's maximum material condition, and datums A, B, and C establish the datum reference frame in that order of precedence, with the zone located by basic dimensions.

Datums and the Datum Reference Frame

Datums make measurements repeatable. They're placed on real features, such as a mounting face or locating hole, and identified with a lettered datum feature symbol.

Together, datums form a datum reference frame that locates the part for manufacturing and inspection. A common introductory way to explain this is the 3-2-1 principle: the primary datum is often a large, stable surface that the part rests on, the secondary datum orients it further, and the tertiary datum completes its location. This is a simplified model. In practice, how datums constrain a part depends on the datum feature geometry, such as planes, holes, or shafts, and on the rules of the applicable standard.

Good datums reflect how the part is actually located and assembled, not just what's convenient to measure.

The GD&T Symbols Explained

Form Controls

The four form controls define a feature's shape on its own and do not use datum references.

• Straightness: how straight a line or axis must be, often on shafts and pins

• Flatness: how flat a surface must be, common on sealing and mounting faces

• Circularity: how round each cross section must be

• Cylindricity: controls the entire cylindrical surface, combining roundness, straightness, and taper

Orientation Controls

Orientation controls define how a feature is angled relative to a datum, so they require a datum reference.

• Perpendicularity: how close a surface or axis is to 90° from a datum

• Parallelism: how parallel a surface or axis is to a datum

• Angularity: controls a surface or axis at any specified angle

Location Controls

Position is the most widely used GD&T control. It defines a tolerance zone, usually cylindrical for holes and pins, within which a feature's axis or center plane must lie.

ASME Y14.5-2018 removed concentricity and symmetry, recommending position, profile, or runout instead. ISO GPS standards include related controls with their own definitions.

Profile Controls

Profile of a line controls individual cross sections, while profile of a surface controls an entire surface in 3D. Profile is highly versatile: on its own it can control form, and when datum references are included, it can also control orientation and location.

Runout Controls

Runout controls apply to rotating parts and reference a datum axis. Circular runout checks each cross section as the part rotates, while total runout controls the entire surface at once. Both are common on shafts, pulleys, and rotating components.

Material Condition Modifiers and Bonus Tolerance

Material condition modifiers change how a tolerance applies based on a feature's actual size:

• MMC (Maximum Material Condition): the feature contains the most material, such as the smallest hole or largest pin

• LMC (Least Material Condition): the feature contains the least material, such as the largest hole or smallest pin

• RFS (Regardless of Feature Size): the tolerance stays the same regardless of size, and is the default in ASME Y14.5

When position is specified at MMC, a feature gains bonus tolerance as it departs from its MMC size. For example, a hole dimensioned Ø10.0–10.2 mm with a position tolerance of Ø0.1 at MMC has Ø0.1 mm of position tolerance at 10.0 mm. If produced at 10.2 mm, it gains 0.2 mm of bonus tolerance, for a total of Ø0.3 mm. A larger hole gives the bolt more room, so the hole can be slightly further out of position and still assemble.

Other common modifiers include the projected tolerance zone, used for threaded holes and press-fit pins, and free state, used for flexible parts that deform when unrestrained.

How GD&T Is Inspected

Coordinate measuring machines (CMMs) are widely used for complex features and position tolerances, while functional gauges can quickly verify MMC-based tolerances. Simpler controls like flatness and runout can often be checked with surface plates and dial indicators, depending on the inspection setup. Because GD&T defines datums clearly, results are more consistent across suppliers.

GD&T in CAD and Model-Based Definition

Most CAD software includes tools for adding datums and feature control frames to 2D drawings, and many support adding them directly to 3D models as product manufacturing information (PMI). This is the foundation of model-based definition (MBD), where the 3D model becomes the primary manufacturing reference. STEP AP242 can carry PMI between CAD systems, although successful transfer depends on the software, export settings, and receiving system. 

How to Apply GD&T Effectively

Start with function. Understand what each feature does and how it interacts with mating parts before adding tolerances.

Choose meaningful datums that reflect how the part is located and assembled.

Use the right control: position for holes and pins, flatness for sealing faces, runout for rotating parts, and profile for complex shapes.

Avoid over-tolerancing. Tight tolerances everywhere add cost without improving function.

Use MMC for clearance fits to gain bonus tolerance and reduce manufacturing cost.

Design for manufacturability. Tolerances should match what the process can achieve; see What Is DFM?

Avoid common mistakes, such as adding datum references to form controls, omitting basic dimensions, or mixing ASME and ISO rules on one drawing.

Frequently Asked Questions

How many GD&T symbols are there?

Earlier ASME editions used 14 geometric characteristic symbols. ASME Y14.5-2018 removed concentricity and symmetry, leaving 12. ISO GPS standards define their own set of geometric tolerances, so refer to ISO 1101 for ISO drawings.

What is the most common GD&T symbol?

Position, especially for locating holes and pins.

What is the difference between MMC and RFS?

At MMC, tolerance can increase as the feature departs from its maximum material size. At RFS, it stays the same regardless of size.

Is GD&T required on every drawing?

No. It's most valuable for features that affect fit, function, and assembly.

Conclusion

GD&T gives engineers a precise, shared language for defining how parts must be made and inspected. By understanding feature control frames, datums, the five symbol categories, and material condition modifiers, you can create drawings that reflect real function, reduce scrap and rework, and give manufacturers more flexibility. Detailed drawings should always follow the specific standard and edition they invoke.

For a detailed breakdown of the differences between STEP file formats and how AP203, AP214, and AP242 compare in practice, read our article on STEP File Formats: AP203, AP214 and AP242.