Just about every machine shop makes parts out of one aluminum alloy or another. Just about every shop also threads holes in those parts using taps. While taps are a highly efficient way to make threads in a hole, they come with potential problems, such as poor or inconsistent thread finishes, thread galling, and the ultimate nightmare — a tap broken off in a part. Here are some common mistakes to avoid and a few tips that have helped me.

I have found that the softer the aluminum, the tougher it is to tap because the material acts like chewing gum if not properly lubricated. Just like when machining aluminum, keeping the chip hardened is important to prevent a myriad of problems. The use of oil or flood coolant helps with preventing galling. Inversely, the harder the alloy, the easier it is to tap.

Proper toolholding also goes a long way in preventing downtime caused by tap failure, in whatever mode it presents itself. Toolholder choice is usually dictated by factors involved in the tapping operation such as the number of holes to tap, the machine being used to do the tapping, as well as the capabilities and limitations of your shop, among others.

For example, if you are about to thread a lot of parts with holes drilled by a different machine, we use a Tapmatic tapping head as it has radial play to allow for better alignment of the tap to the hole, along with an internal clutch to automatically reverse the rotation of the tap as you lift it back out of the part. Most of the time, the drilling and tapping will occur in the same machine and the same setup, so rigid tapping or power tapping with the tool in the spindle, as in a milling machine or CNC mill, is an obvious choice.

A common problem that presents itself is the cutting tool selection, and the use of the wrong tap for the job. There is, after all, an enormous list of different taps, grades of substrate, classes of fit, etc., from which to choose. Each of these facets need to be considered when selecting a tap for a particular part.

Let's take blind holes as an example. The selection of a gun tap or spiral point tap may be the types to avoid in this case. When you need to reach further down, and when you want to prevent chips from compacting in the bottom of the hole and causing premature tap failure, consider switching to a spiral-fluted tap, which is designed to bring the chips up and out of the hole. The chip evacuation helps extend the tool's life and reduces the chances of tap breakage.

Another common mistake machinists make is to assume that "aluminum is almost too easy to tap," and they get too aggressive with speeds and feeds or they prolong the use of a dull tap way beyond its useful lifespan. Most aluminum alloys contain a percentage of silicon, magnesium and chromium. While those amounts may be minuscule (less than 1%), they are abrasive all the same and can play havoc with tap lifespan.

Pressing a dull tap into service beyond its useful life is a ticking time bomb. Aluminum, while one of the easiest metals to work with, still poses significant pitfalls if you become too complacent with tapping it. Dull taps only exacerbate this situation by leaving either a galled or inconsistent finished thread. They also take exponentially more torque to turn and complete the thread as a sharp one takes, and that leads to a higher probability of poor finish and/or a broken tap. The moral of this story is that saving the few dollars to press a dull tap into service right now may end up costing you a pile of money in scrapped parts or tap removal. The abrasive properties of aluminum listed above only add to the trouble lurking in the shadows.

Tap drill size

The formula that I have always used for determining a tap drill size is tap diameter minus 1/N, where N is threads per inch. For example, let's use 3/8-16 UNC. The formula would look like this: 0.375" - 0.0625" = 0.3125" tap drill size. This will result in a 75% thread engagement, which is enough for any standard application of a threaded hole. If you are having trouble with surface finishes or it takes an inordinate amount of effort to turn the tap, the above formula may be too tight of a fit. Especially so in tough or troublesome alloys.

In our shop, the common practice is to move either one drill size larger, or 0.015" larger, depending upon the thread size. The loss of engagement is negligible and the strength is still there. It is surprising how much of a difference those extra few thousandths of an inch can make. We also take the extra few seconds to leave a healthy chamfer at the beginning of any threaded hole. I realize that time is money, and not every shop can afford the cumulative time it would take to chamfer every hole on numerous parts, but the cost savings it brings could more than pay for any time lost in process from chamfering. Chamfering the holes pre-thread can take as much as 25% off of the forces seen by the tap as it engages the hole and cuts the threads.

Whenever possible, we power tap in the same machine setup as the drilling. This ensures proper alignment of the spindle centerline with that of the hole. We also make use of our CNC mill to rigid tap because the CAM software we use generates the feeds that are perfect for any given tap we use. For example, we tap a lot of ¼-20 UNC holes in one of our legacy parts, an aluminum housing. To find the pitch, divide 1 by threads per inch, in this case 1/20. This tap advances 0.050" for every full revolution. We spin the tap at 500 rpm, so 500 rpm ÷ 20 threads per inch = 25" per minute infeed. This puts the perfect load on the tap to prevent excess torque or stretching of the tap. All modern CNC vertical machining centers have stable and strong rigid tapping cycles.