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.
One final thing all shops must consider is the tapping fluid used. All of these other things I’ve mentioned are for naught if your tapping fluid isn’t up to the task. Tap Magic is the standard “go to” for our shop. It is an all-purpose fluid that covers just about every metal that we cut here, from the easiest aluminum to the gummiest and toughest titanium. Everything in between, too. To give you an idea, we have tested Tap Magic against our typical cutting oil while cutting the same thread with each fluid. The Tap Magic reduced cutting forces considerably. It also resulted in the finest finishes on the threads, and it has easily boosted tap life by 50%. The same could be said for the flood coolant in a CNC. So long as your coolant concentrate is properly mixed, it should provide the lubricity necessary to prolong tap life.
Though tapping a hole may seem simple enough, neglecting any of the aspects I’ve covered here can lead to problems in short order. Guard against such complacency, even in a material that could be considered as easy to machine as aluminum. If you keep these pointers in mind — or easily accessible — you can help your shop tap into its potential for threading aluminum.
Related Glossary Terms
- abrasive
abrasive
Substance used for grinding, honing, lapping, superfinishing and polishing. Examples include garnet, emery, corundum, silicon carbide, cubic boron nitride and diamond in various grit sizes.
- alloys
alloys
Substances having metallic properties and being composed of two or more chemical elements of which at least one is a metal.
- aluminum alloys
aluminum alloys
Aluminum containing specified quantities of alloying elements added to obtain the necessary mechanical and physical properties. Aluminum alloys are divided into two categories: wrought compositions and casting compositions. Some compositions may contain up to 10 alloying elements, but only one or two are the main alloying elements, such as copper, manganese, silicon, magnesium, zinc or tin.
- centers
centers
Cone-shaped pins that support a workpiece by one or two ends during machining. The centers fit into holes drilled in the workpiece ends. Centers that turn with the workpiece are called “live” centers; those that do not are called “dead” centers.
- chamfering
chamfering
Machining a bevel on a workpiece or tool; improves a tool’s entrance into the cut.
- computer numerical control ( CNC)
computer numerical control ( CNC)
Microprocessor-based controller dedicated to a machine tool that permits the creation or modification of parts. Programmed numerical control activates the machine’s servos and spindle drives and controls the various machining operations. See DNC, direct numerical control; NC, numerical control.
- computer-aided manufacturing ( CAM)
computer-aided manufacturing ( CAM)
Use of computers to control machining and manufacturing processes.
- coolant
coolant
Fluid that reduces temperature buildup at the tool/workpiece interface during machining. Normally takes the form of a liquid such as soluble or chemical mixtures (semisynthetic, synthetic) but can be pressurized air or other gas. Because of water’s ability to absorb great quantities of heat, it is widely used as a coolant and vehicle for various cutting compounds, with the water-to-compound ratio varying with the machining task. See cutting fluid; semisynthetic cutting fluid; soluble-oil cutting fluid; synthetic cutting fluid.
- galling
galling
Condition whereby excessive friction between high spots results in localized welding with subsequent spalling and further roughening of the rubbing surface(s) of one or both of two mating parts.
- gang cutting ( milling)
gang cutting ( milling)
Machining with several cutters mounted on a single arbor, generally for simultaneous cutting.
- lubricity
lubricity
Measure of the relative efficiency with which a cutting fluid or lubricant reduces friction between surfaces.
- milling
milling
Machining operation in which metal or other material is removed by applying power to a rotating cutter. In vertical milling, the cutting tool is mounted vertically on the spindle. In horizontal milling, the cutting tool is mounted horizontally, either directly on the spindle or on an arbor. Horizontal milling is further broken down into conventional milling, where the cutter rotates opposite the direction of feed, or “up” into the workpiece; and climb milling, where the cutter rotates in the direction of feed, or “down” into the workpiece. Milling operations include plane or surface milling, endmilling, facemilling, angle milling, form milling and profiling.
- milling machine ( mill)
milling machine ( mill)
Runs endmills and arbor-mounted milling cutters. Features include a head with a spindle that drives the cutters; a column, knee and table that provide motion in the three Cartesian axes; and a base that supports the components and houses the cutting-fluid pump and reservoir. The work is mounted on the table and fed into the rotating cutter or endmill to accomplish the milling steps; vertical milling machines also feed endmills into the work by means of a spindle-mounted quill. Models range from small manual machines to big bed-type and duplex mills. All take one of three basic forms: vertical, horizontal or convertible horizontal/vertical. Vertical machines may be knee-type (the table is mounted on a knee that can be elevated) or bed-type (the table is securely supported and only moves horizontally). In general, horizontal machines are bigger and more powerful, while vertical machines are lighter but more versatile and easier to set up and operate.
- milling machine ( mill)2
milling machine ( mill)
Runs endmills and arbor-mounted milling cutters. Features include a head with a spindle that drives the cutters; a column, knee and table that provide motion in the three Cartesian axes; and a base that supports the components and houses the cutting-fluid pump and reservoir. The work is mounted on the table and fed into the rotating cutter or endmill to accomplish the milling steps; vertical milling machines also feed endmills into the work by means of a spindle-mounted quill. Models range from small manual machines to big bed-type and duplex mills. All take one of three basic forms: vertical, horizontal or convertible horizontal/vertical. Vertical machines may be knee-type (the table is mounted on a knee that can be elevated) or bed-type (the table is securely supported and only moves horizontally). In general, horizontal machines are bigger and more powerful, while vertical machines are lighter but more versatile and easier to set up and operate.
- pitch
pitch
1. On a saw blade, the number of teeth per inch. 2. In threading, the number of threads per inch.
- tap
tap
Cylindrical tool that cuts internal threads and has flutes to remove chips and carry tapping fluid to the point of cut. Normally used on a drill press or tapping machine but also may be operated manually. See tapping.
- tapping
tapping
Machining operation in which a tap, with teeth on its periphery, cuts internal threads in a predrilled hole having a smaller diameter than the tap diameter. Threads are formed by a combined rotary and axial-relative motion between tap and workpiece. See tap.
- threading
threading
Process of both external (e.g., thread milling) and internal (e.g., tapping, thread milling) cutting, turning and rolling of threads into particular material. Standardized specifications are available to determine the desired results of the threading process. Numerous thread-series designations are written for specific applications. Threading often is performed on a lathe. Specifications such as thread height are critical in determining the strength of the threads. The material used is taken into consideration in determining the expected results of any particular application for that threaded piece. In external threading, a calculated depth is required as well as a particular angle to the cut. To perform internal threading, the exact diameter to bore the hole is critical before threading. The threads are distinguished from one another by the amount of tolerance and/or allowance that is specified. See turning.
- toolholder
toolholder
Secures a cutting tool during a machining operation. Basic types include block, cartridge, chuck, collet, fixed, modular, quick-change and rotating.
