our digital manufacturing ecosystem
Global Manufacturing Network
People on the ground
3D Printing Materials
Urethane Casting Materials
Digital Manufacturing Resources
Learn about fictiv
2020 State of Manufacturing Report
GD&T 101: An Introduction to Geometric Dimensioning and Tolerancing
How to Accelerate Your Engineering Builds (and Ensure You Get Parts That Fit)
Thank you for subscribing!
Geometric Dimensioning and Tolerancing (GD&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 produce something.
By deepening your knowledge around how to create a well structured GD&T, you will improve communication with your machine shop and ensure everyone involved is speaking the same language.
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 concepts, including:
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 an allowable amount of variation. 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.
When you look at machined parts, they look flat and straight, but if you were to view the parts with calipers, 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 preserving the function of the part. Small 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.
The Datum Reference Frame (DRF) in design engineering is a three-dimensional Cartesian coordinate system. 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).
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.
Symbols or Geometric Characteristics are what most often come to mind when people think about GD&T. There are a total of fourteen GD&T characteristics, and the symbols that represent them are shown in the symbol “cheat sheet” below.
These 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.
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; therefore, the ten associated symbols are the most utilized of the fourteen total GD&T symbols.
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. Profile is the most powerful characteristic of all, and also controls orientation and form.
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.
The first compartment of a feature control frame contains one of the fourteen 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. 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 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.
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 be also be defined as basic. Permissible variations from basic dimensions are usually defined in the 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.
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.
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:
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, and to go deeper, check out our on-demand webinar on Conveying Design Intent for GD&T!