Know What You're Tapping

The key to successful tapping is knowing the true size of the drilled hole.

While many factors contribute to tap failure or breakage, one basic, obvious factor is often overlooked - the size of the drilled hole. The problem is, that factor can’t be calculated accurately using traditional tap/drill charts.

Many changes have taken place in the years since tap/drill charts were first developed - programmable machinery, rigid tapping, synchronous tapping, better toolholders, specialized tapping fluids, and premium high-grade taps.

Most importantly, the drills used to make the holes to be tapped have improved. Advanced drillpoint geometries, new flute shapes, coolant holes, improved HSS and carbide grades, and coatings like TiN and TiCN have done much to improve the quality and size of the drilled hole.

As drill recommendations were being developed for standard-size coarse (UNC) and fine (UNF) series threads, drill sizes were selected based on tests showing that a standard, general-purpose, jobber-length drill - having a standard 118° point angle - will produce a hole size larger than the measured drill diameter. This became known as the "probable hole size," which is often listed on tap/drill charts next to the decimal equivalents of the drill sizes (Table 1). For example, a No. 7 (0.2010"-dia.) drill will, on average, produce a hole that is 0.0038" larger than the drill’s diameter. This would result in a drilled hole size of 0.2048", approximately 70% of thread height. Compared to the minor-diameter specifications for a 1/4-20 UNC-2B tap (0.1960"- to 0.2070"-dia.), the finished hole size is near the high limit, 0.0022" under the maximum minor diameter (Table 2). The drill is removing as much material as possible from the hole, reducing the load on the tap. This makes tapping easier and reduces the possibility of tap breakage. And staying below the maximum minor diameter prevents the production of threads that are too shallow.

Today’s advanced drills - powered by more accurate, higher speed machine tools - are producing holes much closer to the actual measured size of the drill, or even smaller than the drill diameter. Producing smaller pretapped holes substantially increases the workload on the tap. Changing to one of these advanced drills could result in tap breakage where none existed before. The standard No. 7 drill may no longer be the correct drill size for a 1/4-20 UNC-2B thread. It may require a 13/64, No. 6 or even a No. 5 drill to produce a hole that’s 70% of thread height.

Determining Drill Size

Table 1: Typical tap/drill chart, featuring probable hole sizes.

If tap/drill charts are not adequate for today’s machining practices, then how do you establish proper drill size? For a start, keep in mind these factors:

The drilled hole must be within the specification for the class of thread. The drill selected should produce a hole size that falls between the minimum and maximum minor diameter for the class of thread. For example, for a 1/4-20 UNC-2B thread, any drill that produces a hole between 0.1960" and 0.2070" in diameter could be used. Once the hole is drilled, it is important to gage the hole to verify the size using pin or plain plug gages matching the minimum and maximum minor-diameter specifications. Dimensions for the minimum and maximum minor diameter of screw threads are available in many publications. The ASME industry standard B1.1 is one of the best sources for this information.

Remove as much material with the drill as possible for a given length of engagement to make tapping easier. Along with lowering cutting forces and reducing tap breakage, this strategy will also benefit the drilling operation. Larger drills are less fragile and have a lower depth-to-diameter ratio, and their larger flutes ease chip evacuation.

Table 2: Minor diameters and pitch diameters for 1/4-20 UNC threads.

Length of Engagement

While it is best to use the largest drill size possible, doing so may adversely affect the strength of the threaded assembly in some situations. If, for instance, the internally threaded part or nut were made of something thin, such as heavy-gage sheet metal, the one or two threads in the nut might not be strong enough to support the load when the screw is tightened. Therefore, for thin parts the smallest drill size is recommended for the highest percentage of thread to keep the threads as strong as possible.

As the length of the thread engagement between the nut and screw, also known as the length of engagement becomes longer, there are a greater number of threads contributing to the strength of the assembled nut and screw; therefore, the hole size can be enlarged. In summary, drill close to the minimum minor diameter in thin parts and near the maximum minor diameter in longer assemblies.

To determine the proper hole sizes that maximize strength for various lengths of engagement, consult the ASME standard or other commercial manuals containing this information. Looking at the recommended hole sizes for a 1¼4-20 UNC-2B thread (Table 3), the lengths of engagement are listed in terms of thread diameters. In other words, "1/3d" indicates the length of engaged threads between the nut and bolt when assembled. One-third of 1/4" thread diameter is 0.083". This means that if a 3/4"-long bolt were threaded into a 0.083"-thick nut, it would be said to have a length of engagement of 1/3 of the diameter (1/3d). Notice that for this short length of engagement, the hole-size range recommended for a class 2B thread is 0.1960" to 0.2020", or near the low limit.

Now look at the longer lengths of engagement. As the engagement increases, the recommended drilled hole size before tapping gets larger. From 2/3d to 1 1/2d, the predrilled hole size recommended is 0.2020" to 0.2070", or near the high limit. This range is often referred to as a "1-diameter" length of engagement. Tap/drill-chart recommendations are generally based on this length.

Table 3: Recommended hole-size limits for various lengths of engagement for 1/4-20 UNC threads.

In extreme cases in which the length of engagement is greater than 1 1/2 times the thread diameter (1 1/2d), the hole size can be enlarged to 0.2100", or 0.0030" larger than the maximum minor-diameter limit of 0.2070". The additional threads in the engagement allow the height of threads to be reduced while maintaining the assembly strength. However, caution should be taken before applying this rule. It is the engagement between the two parts that allows the use of the larger hole size, not the depth of the tapped hole. If the tapped hole were 3/4" deep and the screw were only 1/4" long, the engagement would be 1 diameter and this rule would not apply.

Long lengths of engagement with high percentages of thread (small drilled-hole sizes) do not significantly increase the strength of the fastened threads. In fact, in some cases, it has been proven that long lengths of engagement can actually reduce assembly strength because of accumulated thread errors that are more likely to occur with high percentages of thread. So resist the urge to use longer fasteners and high-percentage threads in an attempt to strengthen threaded assemblies.

Thread-Forming Taps

Thread-forming taps use drill diameters that are larger to allow for the displacement of part material. The material displaces inward, generating the finished minor diameter of the thread. Table 3: Recommended hole-size limits for various lengths of engagement for 1/4-20 UNC threads

For example, the recommended drill size for a 1/4-20 UNC thread is a No. 1 (0.228"-dia.) on a tap/drill chart. However, the principle of oversize drilling or probable oversize applies to these recommendations as well. Since high-performance drills produce smaller holes, the drill diameter may have to be enlarged to prevent tap breakage or rough threads due to excessive material displacement. As with holes drilled for thread-cutting taps, the size of the hole is far more important than the diameter of the drill used to make it.

Whether cutting or forming threads, the practice of using the tap to produce the minor diameter of the thread is not recommended. While using taps to produce the minor diameter is not a good idea, taps can be used to help eliminate "spin-down" burrs formed below the minor diameter in the part during tapping. Taps used for this purpose are called "controlled root" taps. The minor diameter of the tap is controlled to the size of the drilled hole in the part. During tapping, burrs produced at the minor diameter are "clipped off" by the tap’s minor diameter, leaving the thread smooth. Burrs generally are small and should have little effect on the cutting force. If, however, the tap is called upon to remove more material than small burrs, the cutting or forming force could exceed the breaking torque of the tap.

Although many factors influence tap breakage and affect tap performance, establishing the proper hole size is often overlooked or taken for granted. While drill diameter is important, it is finished hole size that is most critical. Use whatever drill size gives you the optimal hole size for best results.

About the Author

David Miskinis is product specialist with Greenfield Industries, Evans, GA.