While ASME Y14.5-1994 does not include a definition for pattern in Section 1.3, it does define the use of multiple (a pattern of) features of size as shown in both options A and B, and discusses such applications as a pattern. See ASME Y14.5M-1994, Paragraphs 4.5.8 and 5.4.1.5. ASME has corrected this omission in the ASME Y14.5-2009 Standard.

Your comment brings up an important point in using a pattern of features of size as a datum feature. Y14.5M-1994 technically permits two practices for interpreting such applications. While both interpretations are mathematically equal, a CMM may report differences depending upon which method is used. In the text, you’ll find that the datum axis is defined as being the axis of each datum feature at the feature’s true position. This is the most accurate method for a CMM.

In option B, you’ll notice that all of the basic dimensions originate from the upper left hole. Basic dimensions do not have a tolerance accumulation where chain dimensioning is used, because they always originate from a datum. Effectively, the datum axis from the upper left hole should be used as the source of measurements, with the other holes simulated to orient the part and define allowable datum shift values.

Where a feature is shown in the center of the pattern of features of size, the interpretation shown in ASME Y14.5M-1994, Figure 4-22 may be applied. This permits all of the holes to produce a best fit center. This practice is only appropriate for simple symmetrical patterns of features of size. Where the pattern consists of stepped features, or features at odd angles to each other, this dimensioning practice should be avoided.

Because CMMs use algorithms to calculate this center, and not all CMM software uses the same algorithms, differences in measurement can be found using this practice with a CMM. Where the drawing uses this practice to indicate a basic zero dimension to the center of a pattern of datum features, an inspection plan can be helpful in documenting which hole the inspector is to use to produce more repeatable measurements and improve validation between supplier and customer.

Alex

Thanks,
Don Webb
Robert Bosch LLC

You would be correct if datum B was just the lower right hole only. In this case, however, datum B is not just the lower right hole; it is all 4 holes. This is indicated by the datum B symbol attached to the feature control frame placed beneath the size dimension that applies to all 4 holes, and by the “4X” in front of the size dimension.

When inspecting the profile tolerance, you must rest on datum A, and all four holes are used to locate the part and stop rotation on datum plane A. Since datum B is referenced at MMC in the profile callout, a functional gage may be used to check the profile tolerance. The part would have to fit around four virtual condition size gage pins for datum B and rest on datum plane A. The outside edges must lie within the profile tolerance zone.

The part can be shifted on the gage based on the amount of clearance between the four holes and their gage pins to get the outside edges to fit within their tolerance zones. All four edges must fit within the profile tolerance zone at the same time.