An introduction to geometric dimensioning and tolerancing
Manufacturing tolerances allow parts to deviate from perfection, but only within defined limits.
The amount of tolerance allowed is usually based on part function. The limits allow the part to deviate, but a properly applied tolerance will ensure that parts fit properly and function as intended.
When tolerances were first introduced, they were simple; every dimension had a “±” tolerance. If the drawing dimension stated 2,00″ ± 0,010″, then an acceptable part would measure between 1,990″ to 2,010″ for that dimension. As engineering progressed and parts became more complicated, a new method of implementing tolerances was created – geometric dimensioning and tolerancing (GD&T).
GD&T allows for comprehensive and consistent tolerances with the use of relatively simple tools. A part drawing may include a single GD&T callout, or the drawing may be defined fully using GD&T, depending on part requirements.
Fig. 1: Datums create a reference co-ordinate system for repeatable part locators.
Datum locating principles
A basic understanding of GD&T locating datums is helpful to provide a foundation for locating parts repeatedly in the most consistent way. The advantages of using GD&T over conventional dimensions/tolerances include:
- A concise way to describe a reference co-ordinate system or datums (see Fig. 1) of a component or assembly to be used throughout the manufacturing and inspection processes.
- Reduced number of notes, dimensions and tolerances on a drawing.
- Features like maximum material condition (MMC) allow more manufacturing tolerance while still ensuring proper component function.
Conventionally, datum A in Fig. 1 is the primary, B is the secondary, and C is the tertiary datum. In this picture, it appears that each datum is a planer surface, but this is technically never the case as a perfect planer surface is theoretical and can never be achieved in practice.
Three points define a plane, two points define a line. After the primary datum is located using three points, the secondary datum will typically use two points to define a line. The only degree of freedom remaining can be constrained by a single point on the tertiary (third) datum. Therefore, in a standard datuming scheme, six points locate a part or assembly: three for the primary; two for the secondary and one for the tertiary datums.
Fig. 2: Datum A with three point locators.
Datum A
Imagine that the primary locating datum in Fig.1 is a flat granite surface. Once the part is placed on the surface, only three points will actually contact the granite. No surface can be perfectly flat, which means only the lowest three points of the part will be touching the highest three points of the granite, where these intersect. As no two parts are identical, these three points touching the granite, and therefore locate the part, will not be the same from part to part.
There are ways to control which locations on the parts surface are used to create the reference co-ordinate system. Three distinct locators can be used instead of using a planer surface as the locating feature. By using three “point” locators, the same three areas of every part are used to locate it.
Three point locating targets are used to create the primary datum for a component (see Figs. 2 and 3.)
Fig. 3: Datum A with part.
The locators are considered points because the tops of the green locators are spherical, so the centre is the highest point. Once the B and C datums are added (see Figs. 4 and 5), the primary datum plane formed by this fixture will repeatedly locate off the same three points on the parts. Instead of relying on the lowest three points of a part, this configuration dictates the location of these three points. Notice how far apart the locators are. If the three points are moved to be very close to each other, the part would become unstable and therefore not as repeatable. This principle applies to all part locators – further apart is better.
Datum B
Similar principles apply to datum B. A planer surface can be used to locate datum B, which means that two undefined points touch the planer surface. This may work well in some cases. Two distinct point locators may be used when more control is needed.
Similar principles apply to datum C.
Fig. 4: Datum B with two point locators.
Once a reference co-ordinate system is created with datums, the dimensioning scheme should take advantage of this new co-ordinate system. Without extenuating circumstances, dimensions should go to a datum’s edge, which will produce more consistent parts for no additional cost (see Fig. 6).
Limits of size
Many different GD&T tolerances may be used to control a feature’s position or location. These will include a reference to a datum in the feature control frame. Limits of size, however, do not relate the size of the feature in question to a location or position, so no datum reference is needed. This is how GD&T can be used minimally on a drawing.
Having even one positional GD&T tolerance on a drawing will necessitate datums. Control dimensions in GD&T are slightly different; a rectangular box around the dimension means it is a basic dimension. Basic dimensions do not have conventional tolerances. Instead, they use feature control frames (FCF),shown in Fig. 8 to control the tolerance. The box around the basic dimension serves as a visual cue to search for the tolerance in a feature control frame.
Fig. 5: Datum C with one point locator.
Feature control frames
An FCF is the name of a GD&T tolerance symbol used on a drawing. A sample drawing including two feature control frames is shown in Fig. 7. The upper FCF denotes a flatness tolerance of 0,005″. The FCF does not refer to any datums as this is a limit of size. An important distinction is that all tolerance values shown in FCFs are total tolerances, not plus/minus values. So, in this example, you could think of it as a ±0,0025″ tolerance of flatness. This tolerance only controls how flat this surface is.
GD&T tolerances
Unlike limits of size, tolerances of location must reference at least one datum plane, usually three. An example of this can be seen in Fig. 7. The lower FCF includes a reference to three separate datums. The “target circle” symbol is named position and is usually used for locating holes.
Regarding the position tolerance shown in Fig. 7, notice that the two linear dimensions locating the hole have rectangular boxes around them and are therefore basic dimensions. Basic dimensions are considered theoretically exact dimensions; chained basic dimensions do not create tolerance stacks. Again, basic dimensions have their tolerances in a Feature Control Frame. Take a closer look at the position FCF shown in Fig. 7.
Fig. 6: Drawing with GD&T representing the three datums in Fig. 5.
The first box in a feature control frame contains an identifying symbol, in this case, position. The second box of the FCF contains the total tolerance value. An important distinction is that all tolerance values shown in FCFs are a total tolerance, not a “±” value. The datum callouts start with the third box and continue until there are no more datums to reference.
Note that datum A references a plane that is perpendicular to the hole’s axis. This is standard practice and this datum reference controls the direction of the hole through the material, usually perpendicular. The next two datum references provide tolerances to the two hole locating dimensions. To verbalise the feature control frame shown in Fig. 8, the hole’s position must fall within a total tolerance zone of 0,005″ relative to datums A, B and C. The datum order does matter. The part must be located on datum A first, then datum B and, finally, datum C.
Fig. 7: Drawing showing GD&T feature control frames (FCFs) and basic dimentions.
Tolerance zone shape
Another difference between standard ± tolerances and GD&T is the shape of the tolerance zone. In conventional tolerances with a ± tolerance in two right-angle dimensions, the tolerance zone is rectangular. This is shown in Fig. 9. If both hole location tolerances are equal, the zone will be square. The phantom line rectangular box in Fig. 9 represents the area in which the circle’s centre may fall and still remain in tolerance.
GD&T tolerance zones are circular in shape, unlike conventional tolerances with rectangular or square zones. When the tolerance value is 0,005″ in a feature control frame, the circle’s centre may move within a circular area with a diameter equal to 0,005″. The tolerance circle’s centre is at the intersection of the basic dimensions. This is a subtle difference but it should be acknowledged, because the same part that fails with conventional tolerances may pass with GD&T tolerances.
Fig. 8: Position FCF with labels.
Notice that a square tolerance zone of ±0,500″ will allow a hole centre location 0,707″ away from the centre if it is located in the squares’ corner (diagonally). Using a GD&T tolerance value of 1,414″ in this case will allow all hole centre locations that pass the conventional test to pass. Using this GD&T callout will allow some hole centre locations which did not pass the conventional test to pass. Below is an illustration of this effect.
To correct this tolerance discrepancy, it is better to err on the side of caution. To convert a ± tolerance to a GD&T tolerance, multiply the ± tolerance by two. But to convert a GD&T tolerance to a ± tolerance, divide the GD&T tolerance by two and then multiply by 0,707. Most holes, pins, bolts, etc. are round, and the round tolerance zone of GD&T is therefore a more logical shape.
Modifying symbols
The second box of a feature control frame may also contain a modifying symbol directly after the tolerance value. These are special symbols that can exist in any FCF box except the first. Some of the modifying symbols are:
Maximum material condition (MMC).
Least material condition (LMC).
Regardless of feature size (RFS).
Projected tolerance zone.
MMC is valuable for allowing more part variance during fabrication while ensuring that the parts will always assemble properly. Projected tolerance zone is used to control the location of a hole beyond the part’s physical edges.
MMC definition, practice
Manufacturing tolerances are used when individual parts are made. When multiple parts must fit together to make an assembly, these individual part tolerances must be controlled properly. If they are not, then the part may not fit into the assembly and must be reworked or discarded. MMC may be used to maximise the allowable manufacturing variability.
Fig. 9: Rectangular shaped tolerance
zone for conventional.
MMC entails the most material. Consider a bolt through a hole. The MMC bolt is of the largest diameter possible within its tolerance. However, an MMC hole is the smallest hole, which also represents the most material. By including the MMC modifying symbol in a feature control frame, the diameter of the hole now comes into play when determining positional tolerance
(see Fig. 10).
The drawing in Fig. 10 represents two plates to be assembled on top of one-another (“top” an “bottom” plate) and a conventional way to dimension and tolerance the parts: ± 0,01″ for hole positions in the bottom plate, and ± 0,01″ for hole positions in the top plate means that the clearance hole diameter must be oversized by 0,02″. A 1/4-20 bolt (bottom plate) is 0,25 maximum diameter + 0,02 equals = 0,27. The hole diameter is 0,28 ±0,01 or 0,27 at the smallest. These parts will always assemble if they are built within tolerance.
These parts will assemble even when the holes are at MMC, or the smallest hole. If both holes in the top plate were made at the large end of the tolerance, Ø 0,29, there would be extra clearance. This is the principle behind allowing extra manufacturing tolerance with MMC – by making the hole larger, its position can drift more.
Fig. 11 represents the GD&T version, with MMC for the two holes in the top plate. Similar tolerances to those in Fig. 10 are used for the hole’s position and diameter, the difference being the circled M in the top plate’s feature control frame. This symbol indicates that MMC applies to these two holes.
MMC is not to be used on threaded or tapped holes, or on male threaded parts as a threaded hole will follow its own strict size and tolerance definitions.
Fig. 10: Conventional dimensions and tolerances – no GD&T.
Projected tolerance zone
Fastening two plates together may require a bolt to fit through a clamped plate hole and to engage a threaded hole in the base plate. When the clamped plate has significant thickness, the angle of the threaded holes in the base plate should be further limited to make sure that assembly is possible. Projected tolerance zones were created for this situation. Instead of controlling the threaded hole location and angle inside the material only, a projected tolerance zone controls the threaded hole axis parameters for a given distance outside the material. This eliminates calculating manually the required angle and adding the two conventional angle dimensions and tolerances.
Fig. 11: GD&T version of Fig. 10. Note the circled M in the second FCF.
Conclusion
GD&T is the modern language of engineering drawings. Its usefulness goes far beyond the topics discussed in this article. It is more involved than conventional tolerances but tends to be more concise and powerful. The proper use of GD&T can save money and time in manufacturing while at the same time improving product yield and quality.
Contact Michael Kremer, Proof Engineering, mkremer@proofengineering.com
Related Articles
BROWSER-BASED E-ZINES
BACK ISSUES
SERVICES
DAILY CARTOON
-
