About tolerances, GD&T and DT
Scope of this document is to compare two methodologies to dimension a drawing: Geometrical Dimensions & Tolerancing (GD&T) and Dime
nsional Tolerances (DT). In particular the proper way of communicating tolerances information across the company and outside is discussed. Different applications of GD&T and DT are shown with practical examples, using a tolerance analysis tool: eM-TolMate by Tecnomatix, This document does not describe how to use GD&T and/or DT.
2 Tolerances: what is, why?
The most traditional way of dimensioning a drawing is by simply defining an origin and a target. This method is commonly used when measuring the size of the backyard (from the fence to the back of the house) or the size of your workbench (from the left side to the right side, right there where there is a vise). The same concept also applies to mechanical drawings. Leonardo Da Vinci (14521519) used ordinary dimensions in his fantastic mechanical sketches: helicopters, tanks, and submarines. Ordinary dimensions have existed for as long as man has had product ideas. In 1935, with the publication of the American Standards Association’s "American Drawing and Drafting Room Practices," the first recognized standard for engineering drawings was established. Steady progress was made, in the United States and abroad, throughout the World War II years to define and specify the symbols and terms used in functional dimensioning. In mechanical drawing, in addition to a simple dimension, there is also the concept of tolerance.
What is a tolerance? According to the Webster dictionary: the allowable deviation from a standard; especially : the range of variation permitted in maintaining a specified dimension in machining a piece. Why do we need to have a tolerance when “machining a piece”? Why “shop-floor” workers are not able to machine a “perfect” piece? Why Mechanical machines (lathe or mill or other) cannot machine a piece as designed? The reason is not because we do not have “good skilled workers” any more or because we use “lousy equipment”. The real reason is that life is not perfect and also “manufacturing” is not. Whenever we try to drill a hole of 10 mm of diameter, we end up drilling a hole that is slightly bigger or slightly smaller than 10 mm. This “slightly” amount is what it is called “variation”. The maximum allowed amount of variation that still guarantee fit, function and form to the part is called “tolerance”. The difference between nominal, actual (machined) and the tolerance range (variation) is shown below.
3 What is a D&T?
The easiest to understand type of tolerance, is the one applied directly to the dimensions:
This type of tolerance is what is commonly called Dimensional Tolerances (DT) or it is also known as Plus and Minus dimension (PLMI). Basically there are three different applications: ? Linear ? Angular ? Size The 3 above tolerances define the size, the location and the orientation of part features. Here after some examples.
A linear tolerance specifies a tolerance on a linear dimension. In this case the distance between the two sides of the L-shaped block vary from 74.9 to 75.2. The volume where the two faces can be found is shown with the dotted lines (drawing not in scale).
75 +0.2 –0.1
An angular tolerance specifies a tolerance on an angular dimension. In this case the angle can vary from 74° 30’ to 75° 30’. The volume where the two faces can be found is shown with the dotted lines (drawing 75? +/- 30’ not in scale).
A size tolerance specifies a tolerance on a size dimension, such as a diameter. In this case the hole can vary its size from 9.9 to 10.1. The hole envelope is shown with the dotted lines (drawing not in scale).
?10 +/- 0.1
4 What is a GD&T?
GD&T is a precise symbolic language that describes the size, form, orientation, and location of part features. It’s also a design-dimensioning philosophy that encourages designers to define a part based on how it functions in the final product. Through the use of functional dimensioning, tolerances are assigned to a part by the designer based on the part’s functional requirements, often resulting in a larger tolerance for manufacturing. The techniques and principles of GD&T consider the actual design requirements of the part and, without impairing the quality and function of the part, allow for maximum tolerances at all stages of the manufacturing process. The use of GD&T as part of a co-ordinate dimensioned drawing clarify design requirements, provide much more complete information for manufacturing and inspection and help to reduce cost and improve quality. Here is an example of a GD&T application.
4.1 GD&T symbols
The symbols used in GD&T are very simple and do need to be translated into other languages. Here is a list of the most used symbols and their characteristic. For a description and example of usage of the GD&T symbols please refer to ASME Y14.5M-1994, ISO 1101 or ANSI Y14.5M-1982 standards.
Characteristic Flatness Straightness Circularity Cylindricity Profile of a Line Profile of a Surface Perpendicularity Angularity Parallelism Circular Runout Total Runout Position Concentricity Symmetry
5 Why GD&T? A brief history of GD&T
In the late 50's and early 60's in the US, Europe and throughout the world, many major manufacturing companies had their own form of drawing and manufacturing standards. Alongside these company standards, each of the industrial sectors, aerospace, automotive and military had developed their own. It became clear that some form of national and international standard was required. To this end a committee was set up in the USA with members from all the various industries and education with the goals of: ? providing a single standard for practices in the USA. ? updating existing practices in keeping with technological advances and extend the principles into new areas of application. ? establishing a single basis and voice for the United States in the interests of international trade. Alongside this work in the USA, the International Standards Organization (ISO) was doing similar work with similar goals for the rest of the world. This work continues and the most recent American standard ASME Y14.5 1994 is now much closer to the ISO Standard. It also includes new definitions and practices as a direct result of the global shift towards electronic product definition. Advances in product sophistication, manufacturing technology and the increase in joint ventures have ensured and will continue to ensure the growth, development and increasing adoption of GD&T.
6 Ambiguities of DT
6.1 References or datums
In this example, it seems pretty much complete: dimensions of the block and the position of the holes is quite well defined. But which side of the block has to be taken as reference? Which feature has to be machined first? Which side has to be cut first? What is more important? The distance between the holes or the distance between the holes and the faces? Why so many questions for a simple block with two holes? The reason is that there is no definition of references or, using a GD&T terminology, of datums. A Datum is the origin from which the location or geometric characteristics of features of a part are established. A new concept has to be added: what is my reference? The from/to concept needs to be defined in the drawing. It may be implicit or clear because experience or because some additional written information are on the drawing, but what if the drawing is used in a different country? What if the interpretation of designer and manufacturing engineer is different?
How GD&T can be applied? Here is an example. The datums are defined with a character (A, B, C …) and the symbol is in a square box. Datum A is also the first to be machined therefore is the reference for all other features. From the drawing is clear that the side indicated as datum B Has to be manufactured before the side indicated as datum C. Then the holes are drilled. The position of one hole respect to the other is not important (just a reference) as the position of the holes respect to the datums. Summary: GD&T resolve some ambiguities that may occur in the interpretation on the order of manufacturing, on the reference and on the importance of the critical dimensions.
6.2 Orientation and form control
Referring to the same example as above, the 200 dimension for the width of the part does not give any indication of the variation in shape. ? ? The two sides may have a different orientation and also a different form. With a DT there is no indication of ? ? how to control those two characteristics: orientation and form. ? ? Again, manufacturing is quite “free” to machine the block: anyone of the three is valid. But what about the inspection? Where ? should the inspector check the block? In the third example, the middle ? section is OK but not the top and the bottom. Should the part be considered as a rejected part? ? The common sense suggests that while machining such a part, the parallel sides have to be parallel and squared. GD&T symbols can help in solving these ambiguities. In the example above, the issue about the form of the two sides has been addressed by flatness and straightness symbols. In the same way orientation can be addressed using perpendicularity or parallelism (not shown in the above example). Summary: DT does not fully control orientation and form, leaving manufacturing and inspection pretty free to machine and inspect parts. The common sense is kind of “embedded” in the manufacturing process. GD&T helps to control better the process, defining completely the amount of form and orientation.
6.3 Square zone
Consider the position of the holes in the drawing that uses DT. Di The co-ordinate Dimension 100 dimensioning and DT is creating a square that defines the area in which the centerline of the hole is allowed to fall. Looking at the tolerance zone in more detail, there are some interesting Dimension situations that can arise. 100
The tolerance is ±0.25. This gives a square as shown. The center of the square is the theoretically exact center point of the feature. This type of tolerance zone will cause a point (A) to fail. However, the second point (B) will pass, even though it is further away from the theoretically exact position than point (A). The square tolerance zone allows different amounts of tolerance in different directions (horizontally, vertically rather than diagonally). But the function of the hole cannot be in relation to the co-ordinate direction. Using a GD&T position tolerance zone instead of a co-ordinate dimension helps to recognize and to account for unlimited orientation of round and directions, being more realistic and practical. In most cases geometric tolerancing can specify a circular tolerance zone whose radius is the same as the maximum deviation using the co-ordinate technique. The difference in size of the tolerance zones can be easily calculated: Area of square zone = 0.25 Area of circular zone = 0.39 This is actually a 57% increase.
Summary: GD&T allows bigger tolerance areas allowing fewer parts to be rejected. In addition the function of the feature are evaluated and considered.
One concept typical of GD&T is the Maximum Material Condition (MMC) also known as Bonus Tolerance. Here is a brief description of MMC and some of its application. Maximum Material Condition is the condition that exists when a feature contains the maximum amount of material that is allowed by its size tolerance. When a pin is at its largest allowable size, it contains more material than any other size within its size tolerance. For a hole, the opposite is true. The smaller the hole, the more material it contains. However, it only reaches MMC at its SMALLEST ALLOWABLE size.
If a pin is specified as ?50±0.2 its MMC size is 50.2. If a hole is specified as ?50±0.2 its MMC size is 49.8. From this it follows that MMC can only apply to features that have a size tolerance. When a feature reaches its MMC, it is vital that the positional tolerance for the pin or the hole is not exceeded. If this happens then the parts will simply not fit together. In most cases, traditional co-ordinate dimensions cope with this by calculating the "worst condition" and specifying a tolerance value that will be acceptable at the worst condition. What does this means practically? Let’s analyze the effect of MMC on the Position of a feature of size. The purpose of position tolerancing is to constrain mating parts such that their fit form and function can be assured as well as any interchangeability considerations.
In the figure below, both tolerances of size and position are applied to two holes. The mating condition simulated here is where gauge quality pins (at their maximum material condition) are located at the basic dimension specified. The mating condition shown represents the maximum offset between pin and hole and can be described as the nominal state.
The figure below shows when each hole is on the maximum permissible limits of the 0.2 tolerance zone in opposing directions. The important fact here is that the holes are still at their MMC size and as can be seen the mating condition is still correct. This picture could be considered as the worst case.
The figure below shows what can be achieved when the holes are on their maximum limit, i.e. a diameter of 10.075mm (Least Maximum Condition). The concept of MMC describes that when moving away from the MMC size, the difference between the actual and that MMC size may be added to the nominal positional tolerance . This is where the term bonus tolerancing comes from, as the addition due to actual size is indeed the bonus. As can be seen in the diagram the mating conditions between pins and holes is still achieved even through the holes are 0.35mm out of position.
Summary: the concept of MMC is not found in the traditional DT. Application of MMC results in a bigger tolerance zones for an easier functional fitting.
7 GD&T and DT application using eM-TolMate
A tolerance analysis tool can show the above concepts and highlight the difference between GD&T and DT. For this purpose eM-TolMate, a tolerance analysis tool by Tecnomatix has been used. EM-TolMate uses a Monte Carlo method to simulate the randomness of the variation. For the analysis the following geometry, modeled with the CAD system Unigraphics, will be used.
The following two tolerance scheme will be compared: one using only DT and the other using GD&T. The tolerance scheme does not intend to be complete but rather it has all the tolerances necessary for the discussion. Below the DT tolerance scheme used.
Below the tolerance scheme using GD&T symbols.
Using eM-TolMate the angle between the two side planes is calculated. The pictures below show eM-TolMate embedded in UG and how results are presented.
As discussed before, the DT tolerance scheme does not have any orientation control. The side planes are free to assume different orientation inside the tolerance zone. Variation between the opposite planes is calculated to be 0.22 degrees.
Using a GD&T with perpendicularity and flatness callout, the orientation and the form are totally controlled. This results in a less variation of the angle formed by the two side planes. In this case the variation is calculated to be about 0.08 degrees.
Summary: although both schemes are valid from a dimension point of view and also for any tolerance analysis, the GD&T better defines and control effects like orientation and form.
7.2 Square zone
The same above tolerance schemes are used to show the difference between defining a positional square zone by DT and a circular area by GD&T. In this case eM-TolMate shows the difference of the distance between the two holes. The calculated variation in case of co-ordinate tolerances is about 1.41 mm.
The calculated variation in case of usage of positional tolerance is 1.60 mm (an increase of 15%) The GD&T scheme allows more variation due to the fact that the overall area is bigger and it is independent from the coordinate direction.
Summary: also in this case both tolerance schemes are valid but they bring to two different results. The different approach between usage of DT and GD&T is generating different variations. The user will determine which tolerance scheme is more suitable for his situation.
In this case, the GD&T scheme uses also the concept of MMC applied to the position tolerance for the two holes.
The effect of the MMC, bonus tolerance, results in a bigger variation than the DT scheme and of course also than the position tolerance with no MMC condition. Using MMC condition the calculated variation becomes 2.14 mm, compared to 1.41 mm with co-ordinate tolerances and 1.60 with positional tolerance and no MMC condition.
EM-TolMate is also able to identify the tolerances contributing to the variation and their percentage of contribution to the variation. It is therefore possible to identify that for the variation of the two holes, there is a contribution of the two position tolerances but also a quite significant contribution (20% each) for the diameter size of the hole. This is due to the fact that variation of the diameter size is considered as MMC condition for the position tolerances.
Summary: MMC concept, applicable only with GD&T, results statistically in bigger variation, as the position is also function of the size of the holes. A positive side effect of this bigger variation is a less expensive manufacturing process and a better assemblability and interchangeability.
Co-ordinate dimensional drawings have been used successfully for many years. Aircraft can fly, cars can drive with absolute great success. Still a lot of current drawings use the traditional DT. But co-ordinate drawings by their very nature, can be ambiguous, language dependent and can be prone to various and different interpretations and sometime to misinterpretation. In addition , parts can be manufactured and passed off to the drawing but for some reason do not fit, or do not perform exactly as they should. This leads to costly rework, engineering drawing changes and an increase in assembly delivery time and costs. The opposite is also true, parts may fail inspection to drawing but would in fact fit and perform as required. GD&T usage provides a better a clear communication between designers, engineers and inspectors. In addition larger tolerance zone that consider the fit function of the parts can be used turning in cost savings and better quality. A tolerance analysis tool, like eM-TolMate, can use both schemes in calculating the combined effect of the tolerances. However different results are obtained, because different assumptions are related to the different tolerance schemes.