GDT: Two-Dimensional
 Design Home Fundamentals Introduction 2D Datums 2D Hole/Shaft 2D Bonus Tolerance 2D Bon Tol Example 2D Virtual Condition 3D Datums 3D Hole 3D Bonus Tolerance 3D Virtual Condition 3D Functional Gauge Reference Symbols Parallel vs Flat Cylindrical Specs Acceptance Resources Bibliography
 Home Membership Magazines Forum Search Member Calculators
 Materials Design Processes Units Formulas Math

2D Hole Positioning
In 2D Datums we have rigorously defined how we fixture the part for dimensioning features, we can now define where the hole is.
Figure 2.6
Figure 2.6 shows two dimensions which show where the hole is with respect to datums A and B. Plus/minus tolerances are also shown, as is a square tolerance zone within which the center of the circle must lie. Although it may seem that we are not using GDT here, without the GDT datums, the two dimensions shown are ambiguous.

However, the plus/minus tolerance zone is not clearly defined since we do not know what is meant by the "center of the circle". In addition, a square tolerance zone is typically not what is needed for defining the position of a hole with respect to a mating shaft as shown below:

Figure 2.7 illustrates the equivalent GDT tolerancing of the hole position. The tolerance zone within which the center of the circle must lie is circular rather than rectangular.

Figure 2.7
We will later learn how the size and position of this circular zone is defined based upon the symbols shown. In GDT, the "center of the circle" is defined as the center of the best-fit circle determined by the actual hole. Coordinate Measuring Machine (CMM) equipment typically uses at least three points on an actual hole to define the best-fit circle, as illustrated in Figure 2.7b. Figure 2.7c shows the CMM probe touching the side of the hole for a data point. The CMM machine of course uses the A and B functional datum planes as its position and orientation references.
 Figure 2.7b Figure 2.7c
A big advantage of GDT is that the circular tolerance zone contains 57% more area than an equivalent square tolerance zone. The largest deviation from true position occurs on the diagonals of a square, and the circle meets this, while providing 40% more possible deviation along the vertical and horizontal. Therefore, more parts can be accepted by inspection. With the square tolerance zone, parts that can fit are rejected since typically only the vertical and horizontal location deviations are checked.

The 7.5 and 3.0 dimensions in Figure 2.7 do not have attached tolerances for a reason. They are called basic dimensions and represent the exact position of the center of the circular tolerance zone within which the center of the circle must lie. They can be recognized as basic dimensions because they are box framed. The diameter of the circular tolerance zone comes from the feature control frame which is below the 2.5 hole diameter dimension. The diameter of the tolerance zone in the feature control frame is 0.7 inches. The first symbol in the frame designates the tolerance as a positional tolerance. The -A- and -B- are the GDT datums to which the zone refers. For a two dimensional problem, the importance of -A- and -B- is not apparent, but we will see in the 3D example how they come into play. For now, let us notice that the tolerance zone location is located via -A- and -B-. The ±0.2 tolerance on the 2.5 hole diameter allows the diameter of the hole to vary from 2.3 to 2.7, but the center of the hole must still lie within the circular tolerance zone described above. The ± 0.2 tolerance will be discussed further under bonus tolerancing.

There is another way in which the circular tolerance zone for the hole can be interpreted. Figure 2.8 shows this tolerance zone as being the annular "racetrack" formed by two circles centered at 7.5, 3.0, nominally 2.5 in diameter, and ±.2 above and below 2.5 in diameter.

Figure 2.8
If the actual hole profile is within this "racetrack", it is very similar to its center being within the 0.7 diameter circular tolerance zone. This interpretation of hole positional tolerances is common and probably originated before CMM machines allowed finding the center of the best fit circle. This interpretation lends itself to inspection with calipers, gauge pins, and the like. However, in cases where extreme precision and the utmost certainty of geometry are required, the true GDT (ANSI Y14.5) definition should be used.

Now that we have observed how GDT can clearly define hole position, let us move on to bonus tolerancing. If you would like to skip bonus tolerancing for now and move on to the 3D case of what we have discussed, see 3D Datums.