Time to read: 8 min

Geometric Dimensioning and Tolerancing (GD&T or GD and T) is a language of symbols and standards designed and used by engineers and manufacturers to describe a product and facilitate communication between entities working together to manufacture product. GD&T was first utilized by the US military in the 1940s with the MIL-STD-8 publication (NOTE: MIL-STD-8 has since been cancelled). GD&T has evolved since then and is now commonly utilized across the industry. 

By deepening your knowledge around how to create a well-structured GD&T (aka GDT), you will improve communication with your machine shop and ensure everyone involved is speaking the same language. Understanding the GD&T terminology, as well as learning best application techniques is key to obtaining the best-quality manufactured parts. 

There is a lot to learn when it comes to mastering GD&T, so this post will serve as a launching point to help you understand the most important GD&T basics and concepts, including:

  • CNC machining tolerances
  • The Datum Reference Frame (DRF)
  • Interpreting GD&T Symbols
  • Applying Geometric Symbols to Engineering Drawings
  • The Feature Control Frame
  • Communicating Basic Dimensions
  • Material Condition Modifiers

If you want to go even more in-depth into this topic, check out our on-demand webinar on Conveying Design Intent with GD&T.

Tolerances are like Bacteria: Small, but Powerful

Tolerances in engineering are an allowable amount of variation of a physical dimension. It’s important to keep tolerances on engineering drawings in perspective, so I think of tolerances like bacteria—like bacteria, they’re not visible to the naked eye, but we know they’re there.

Tolerances are one part of GD&T, or Geometric Dimensioning and Tolerancing. GD&T is an acronym for the geometrical product specifications – the ‘G’, the dimensioning – the ‘D’ and the tolerancing – the ‘T’. 

When you look at machined parts, they look flat and straight, but if you were to precisely measure every single cross-section of the part, you would find that there are imperfections all over the parts. These variations (imperfections) are allowed within the tolerance limits (constraints) placed on the parts. In order to understand geometric tolerancing, it helps to think of parts as having varying degrees of imperfection.

To provide some context, let’s consider an average human hair, which is around .005 inches in diameter. In general, tolerances of +/- .005 inch are expected and achieved from today’s CNC mills. However, just because you can hold tolerances smaller than a human hair doesn’t mean you need to.

The engineer or designer should strive to keep tolerances as large as possible while still maintaining the function of the part. Small, or tight tolerances can increase cost in the manufacturing, inspection, and tooling of parts. Tight tolerances are sometimes necessary, but it’s important to keep them in perspective.

Datums and Features

The Datum Reference Frame (DRF) in design engineering is a three-dimensional Cartesian coordinate system against which the part’s tolerances, tolerance symbols, and geometric features are defined. It’s arguably the most important concept in GD&T. The DRF is the skeleton of the geometric system—it’s the frame of reference to which all referenced geometric specifications are related and the origin of all dimensions and geometric specifications related to it.

A DRF establishes Six Degrees of Freedom (DOF), three translational and three rotational. In order to design, manufacture, and verify parts, the necessary DOF must be constrained. Parts are mated to the DRF so measurements, processing, and calculations can be made.

There’s an important distinction between datums and datum features. Datums are points, axes (lines), and planes, or some combination of these components, that make up the DRF. Datum features are the actual, physical features (holes, faces, slots, etc.) on the part. They’re not perfect—they have variation. The illustrations below are provided to emphasize that Datums (left) are theoretical (perfect) and datum features (right) are real (imperfect).

datums (left) and datum features (right) in GD&T

In defining a part, an engineer will identify the datum features on a part that are most important to the functional requirements of the design—usually the features that mount the part in the assembly. Datum features referenced in the end compartments of a feature control frame (see Feature Control Frame), in an order of precedence, will mate the part to the datum reference frame.

GD&T Meaning and Geometric Dimensioning and Tolerancing Symbols

Symbols or Geometric Characteristics are what most often come to mind when people think about GD&T. There are over twenty GD&T characteristics, and the most commonly used symbols that represent them are shown in the symbol “cheat sheet” below.

GD&T is a feature-based system, and parts are composed of features. Geometric tolerances are applied to features by feature control frames. The most frequently used tolerance categories are form, orientation, and location. The remainder of the five geometric dimensioning and tolerancing symbols are runout and profile. 

Form tolerances control the “shape” of features and are often used as a refinement of size.

Orientation tolerances control the “tilt” of feature and are always associated with basic angle dimensions, often used as a refinement to location. If applied to surfaces, orientation tolerances also control form.

Location tolerances control location and are always associated with basic linear dimensions. Position locates and orients the median plane or axis of features of size. Profile locates feature surfaces. GD&T profile is the most powerful characteristic of all which controls orientation and form.

GD&T symbols Chart

Feature Control Frame

GD&T symbols are placed in the first compartment of a feature control frame and define the type of tolerance that is to be applied to the feature. The characteristics are grouped together into types of tolerance: form, orientation, location, runout, and location of derived median points. The primary use and description of each characteristic is also shown.

The feature control frame states the requirements or instructions for the feature to which it is attached. Simply put, the feature control frame controls features. Each feature control frame contains only one message (requirement); if two messages for a feature are necessary, two feature control frames are required.

feature control frame in GD&T

The first compartment of a feature control frame contains one of the geometric characteristic symbols. Only one of the symbols can be placed in a feature control frame; if there are two requirements for a feature, there must be two feature control frames or a composite tolerance. The symbol will specify the requirement for the feature, such as, “this feature must be flat,” or “this feature must be positioned.”

The second compartment of a feature control frame contains the total tolerance for the feature. The feature tolerance is always a total tolerance, never a plus/minus value.

If the tolerance is preceded by a diameter symbol (), the tolerance is a diameter or cylindrical shaped zone, as in the position of a hole. If there is no symbol preceding the tolerance, the default tolerance zone shape is parallel planes or a total wide zone, as in the position of a slot or profile of a surface.

Following the feature tolerance in the feature control frame, a material condition modifier, such as MMC or LMC (see Material Condition Modifiers) may be specified if the feature has size, such as a hole. If the feature has size, and no modifier is specified, the default modifier is RFS (Regardless of Feature Size). If the feature has no size, such as a plane surface, then the modifier is not applicable.

The third and following compartments of a feature control frame contain the datum feature reference(s) if they are required. For example, if a form tolerance, such as GD&T flatness or straightness, is specified, then no datum feature reference is allowed. However, if a location tolerance like position is specified, the datum feature references are usually specified.

The alphabetical order of the datum references has no significance—the significance is their order of precedence, reading from left to right as primary, secondary, and tertiary. The primary is the first feature contacted (minimum contact at 3 points), the secondary feature is the second feature contacted (minimum contact at 2 points), and the tertiary is the third feature contacted (minimum contact at 1 point). Contacting the three (3) datum features simultaneously establishes the three (3) mutually perpendicular datum planes or the DRF. The DRF is created by so-called Datum Simulators which are the manufacturing, processing, and inspection equipment, such as surface plate, a collet, a three-jaw chuck, a gage pin, etc.

In certain situations, the datum feature modifiers Maximum Material Boundary (MMB) or Least Material Boundary (LMB) may be applied to the datum feature. The default modifier is Regardless of Material Boundary (RMB). Since the datum feature has size (it can get larger and smaller), information is necessary on the size condition of the datum feature to which the datum feature reference applies. The modified condition of the datum feature (MMB, LMB, RMB) defines the size or condition of the datum feature simulator.

GD&T Basic Dimensions

Basic dimensions are theoretically exact numerical values used to define form, size, orientation, or location of a part or feature. Basic dimensions are usually shown on a drawing enclosed in a box, but they can also be invoked by referencing a standard or by a note on the drawing. The CAD model itself can also be defined as basic. Permissible variations from basic dimensions are usually defined in the GD&T feature control frame or by notes on the drawing. Any default tolerances in the title block of a drawing do not apply to basic dimensions. Often, basic dimensions are not utilized for quality inspection purposes (pass/fail criteria).

Material Condition Modifiers

In specifying geometric controls, there’s often a need to state that a tolerance applies to a feature at a particular feature size. The terms Maximum Material Condition (MMC) and Least Material Condition (LMC) allow an engineer to communicate that intent.

These material condition modifiers are used in a feature control frame in the feature tolerance compartment and follow the feature tolerance. The application of the MMC and LMC modifiers provide additional geometric tolerance beyond the specified tolerance as the features departs from the specified condition.

Maximum Material Condition (MMC) – The condition where the feature contains the maximum material with the stated limits of size. (ex: largest pin and/or smallest hole)

Least Material Condition (LMC) – The condition where the feature contains the least material within the stated limits of size. (ex: smallest pin and/or largest hole)

In the illustration below, the MMC of the hole is 19.5mm and the LMC of the hole is 20.5mm. As another example, consider a pattern of holes dimensioned to 20+/-0.5mm with a position tolerance of 0.6mm at MMC. The MMC for the holes are 19.5mm diameter. If the holes depart (get larger) from their MMC size, they are allowed additional position tolerance equal to the amount of their departure from their MMC size of 19.5mm. If the hole comes in at 20.0mm, the diameter position tolerance allowed is 1.1mm. This is the concept of bonus tolerance.

bonus tolerance in GD&T

Main Takeaways

GD&T is an entirely new way of describing the dimensions and tolerances compared to traditional plus/minus tolerancing. Fundamentally, the engineer designs a part with perfect geometry in CAD, but the produced part is never perfect. Proper use of GD&T can improve quality and reduce time and cost of delivery by providing a common language for expressing design intent.

The benefits of Geometric Dimensioning and Tolerancing (GD&T) are:

  • A standardized design language
  • A clear and precise way for the customers, suppliers, and production teams to communicate
  • A method for calculating the worst-case mating limits
  • Production and inspection processes are repeatable
  • Assembly is assured from qualified production parts

This article covered the key concepts for its application, including Datums and Features, Symbols, Feature Control Frames, Basic Dimensions, and Material Condition Modifiers. If you’re interested in reading more about conducting a tolerance analysis, read our post on the topic. To go deeper, check out our on-demand webinar on Conveying Design Intent for GD&T!