GD&T and Related Standards

This information provided by Bryan R. Fischer, of TDP360 LLC.

For more information about GD&T, ISO GPS, Tolerance Analysis, and product geometry management training and consulting services, visit www.TDP360.com.

For more information about MBD and MBE training and consulting services, visit www.AdvantageMBE.com.

Bryan’s contact information

phone +1(503)260-3084

email:  

contact@tdp360.com

contact@advantagembe.com

ASME Y14.5 is the main ASME dimensioning and tolerancing standard. It defines almost 100% of the dimensioning and tolerancing rules, tools, and methods for product definition data sets. Several other standards define related and additional content. See below.

ASME Y14.5-2018 Dimensioning and Tolerancing

This is the main ASME dimensioning and tolerancing and GD&T standard.

ASME Y14.5.1-2019 Mathematical Definition of Dimensioning and Tolerancing Principles

This standard defines mathematical interpretations of dimensioning, tolerancing, and GD&T values and methods in ASME Y14.5. This standard is primarily used by software developers.

ASME Y14.8-2022 Castings, Forgings, and Molded Parts

This standard defines rules, tools, and methods for parts produced using casting, forging, and injection molding processes. It includes examples of GD&T applied to product definition data sets of cast, forged, and injection molded parts.

ASME Y14.41-2019 Digital Product Definition Data Practices

Types of Dimensions

Directly-toleranced dimensions are dimensions that have a tolerance – the tolerance is defined with the dimension, either directly on the drawing or annotated model or from another source. By contrast, basic dimensions do not have a tolerance – ever. Basic dimensions represent perfect, theoretically exact geometry. Directly-toleranced dimensions can have several forms. The name “directly-toleranced” is a little misleading, as the tolerance might not be directly specified with the dimension, but might come from a tolerance code (e.g. Ø25 f6), a standard that defines tolerance values, or it might be a default tolerance that comes from a tolerance block, title block, or general notes. See the following examples.

Note:

The inch and metric tolerance values shown are not equivalent.

Basic Dimensions

Basic dimensions are different than directly-toleranced dimensions. Basic dimensions do not have a tolerance. That is, tolerances are not specified for or applied to a basic dimension. Basic dimensions define perfect geometry. In GD&T, basic dimensions are used to define perfect geometry, and geometric tolerances are applied to control features that are defined by basic dimensions. If a basic dimension is explicitly specified on a drawing or annotated model, that is, if the dimension is shown as annotation, the dimension value is enclosed in a rectangular frame. Often, with model-based product definition data sets, such as minimally-dimensioned annotated models, basic dimensions are not explicitly shown. A rule or note is applied that indicates the model geometry is used to define the product geometry, and the model geometry is basic – the model geometry is equivalent to geometry defined by basic dimensions, even though the dimensions are not shown.

Reference dimensions are intended to provide information that exists and is formally specified somewhere else. In this sense, reference dimensions contain redundant information, such as information that is defined elsewhere in the product definition data set (e.g. on another sheet of the drawing or in another view of an annotated model), in a different product definition data set, in a catalog, on a vendor drawing, in a company or industrial specification, or it may be the sum or difference of multiple dimensions, such as an overall dimension defined by a chain of dimensions. 

Reference dimensions are displayed with the dimension value enclosed in parentheses. Other information, such as text, tolerances, and symbols may accompany the dimension value within the parentheses. As reference dimensions are understood to represent redundant information, a reference dimension does not define a requirement or constraint upon the product. That is, the reference dimension itself should only be included for information only – reference dimensions can be considered as FYI (for your information). They are included to help the reader understand something without having to search for the view or other product definition data set that includes the formally-specified information. Truly, a reference dimension could be removed from the product definition data set and the requirements defined by the specifications would not change.

Examples of Reference Dimensions

Inches    (1.000)    (Ø.375)     (R.50)                 3 examples, dimension values only

(1.000 ±.005)   (Ø.375 ±.010)     (R.50 ±.02)                  3 examples, dimension and tolerance values

Metric     (25)     (Ø10.5)     (R0.8)                 3 examples, dimension values only

(25 ±0.1)     (Ø10.5 ±0.25)     (R12 ±0.5)                 3 examples, dimension and tolerance values

A size dimension is used to define the size of a feature of size. The size dimension is a directly-toleranced dimension. See the section on Directly-toleranced Dimensions for more information.

There are only a few legitimate uses of directly-toleranced dimensions, and defining the size of features of size is one of them. As discussed in the section on Features and Types of Features, features of size are an important class of features and a size dimension and tolerance that defines the size of a feature of size invokes the envelope principle (Rule #1).  The envelope principle (Rule #1) only applies to features of size. We will explain what the envelope principle (Rule #1) mean in the section on Features and Types of Features. We will include introductions to feature and feature of size here so we can recognize size dimensions.

In ASME GD&T, a feature is a surface of a part or an assembly. 

In a product definition data set, such as an engineering drawing or annotated model), features are depicted in their perfect state: perfect form, perfect size, perfect relationship to other perfect features (e.g. perfect orientation and location). While we can view or visualize theoretically perfect features on drawings and in CAD models, we cannot touch them. They only exist in theory.

On actual manufactured parts and assemblies, features are imperfect. Actual manufactured features do not have perfect form, perfect size, or perfect relationship to other perfect features (e.g. they do not have perfect orientation and location relative to one another). All features on actual manufactured parts are imperfect. This is why size tolerances and geometric tolerances were invented. The features that we can touch in the real world, the features we can feel when we pick up a part or assembly, are imperfect. The imperfection is often small, and we might not be able to see it. The part we hold in our hand and its features may be manufactured very well, and the imperfection may be visible without magnification. On some parts, especially very large parts, the imperfection is often easy to see with the naked eye. For example, look at lumber. Stock lumber is often twisted, warped, chipped, and has different sizes at different locations along its length. These same issues apply to all stock materials, but the magnitude of the imperfections is usually much smaller for machined and other precision manufactured parts.

To recap, a feature in in GD&T is a surface. As there are other types of features in the product lifecycle, the term feature means different things to different people performing different activities, in the context of GD&T, I often call features in GD&T tolerancing features. 

For a feature to be a feature of size (actually called a regular feature of size in ASME GD&T), the feature must have the right geometry (it must be a cylinder, a sphere, or a pair of opposed parallel planes), and it must be defined by a directly-toleranced dimension. Thus, not only must a feature be a certain shape (cylinder, sphere, opposed parallel planes), it’s size must be defined using plus and minus tolerancing. Cylindrical features are very common in most industrial applications, such as cylindrical holes, shafts, fastener shapes, pins, etc. Opposed parallel plane features are also common, such as keys and keyways. Spherical features are less common in most parts.

                                                                                         (Inches)                                                                        (Metric)                                                                                                (Metric)                                                                                                 

The geometry in each feature of size example has the right shape and the size is defined by a directly-toleranced dimension. Thus, the dimensioned features in these examples are features of size. We will cover features of size and why they are important in later sections.

In MBD, it is common to use model geometry to represent product geometry. This is common in many industries, but most common in industries that design and manufacture parts with complex geometry and/or use certain manufacturing processes, such as casting, injection molding, complex formed sheet metal, such as for automotive body and aerospace fuselages, and more recently, additive manufacturing. In fact, some of the earliest examples the author experienced where CAD model geometry was used to represent product geometry was for cast and injection molded parts. Cast and injection molded parts often have complex shaped surfaces which cannot be dimensioned easily or completely. This has been a problem for centuries if we consider the hulls of boats and ships. At best, if we try to dimension such shapes, we dimension a series of points on the surface (that represent only a subset of the surface), and provide manufacturing with a cloud of points at specified intervals, such a grid of  X, Y, and Z dimensions for points. Manufacturing and inspection get the grid of points, they get the views of the desired shape on the drawing, and they must interpolate and/or guess what the intermediate X, Y, and Z coordinates on the surfaces are. This is a long-standing problem.

In the late 20th century, 3D CAD became mainstream and designers began using 3D CAD to define complex surfaces. They realized that while it was impossible to completely dimension a complex surface, as it would require an infinite number of dimensions, they could provide a CAD model or neutral 3D model that represented the complete complex surface to manufacturing and inspection. This practice is common today. While this practice brings new challenges, providing a digital model of the entire surface is so much better that companies are never going back to trying to define complex shapes with grids of dimensions.