Internal Decision

Of the two most common methods of producing internal threads—tapping and thread milling—tapping is by far the more popular.

Mark Hatch, applications specialist at Emuge Corp., a Northborough, Mass., manufacturer of taps and thread mills, estimated that 85 to 90 percent of all internal threads are produced with taps.

Thread milling, however, has begun to narrow the popularity gap. Recent advancements in CNC technology have spurred the growth of the process, which has been around since the 1950s.

Thread milling involves the application of a specially designed milling cutter to machine an internal or external thread. According to Bryan Young, application engineering manager at Mazak Corp., Schaumburg, Ill., most modern CNCs can precisely move a tool in the X, Y and Z axes simultaneously. This 3-axis movement is a process known as helical, or spiral, interpolation. It allows a thread mill to produce highly accurate threads while allowing the operator to precisely control variables that he couldn’t while tapping.

Deciding whether you should tap or thread-mill a hole depends on a number of factors. These include the machine tool used, hole characteristics, material, desired operational flexibility and control, and, of course, cost.

You must analyze all of these factors, determine how significant they are to your process and then choose a course of action. Below are some guidelines to help you with the selection process.

Machine Tool. Start by assessing the capabilities of your machine tool. As Young points out, most of today’s popular 40-taper machining centers lack geared headstocks. This is the result of the market demanding speedier, more accurate, lower-cost machines.

While these machines are generally fast and possess high positional accuracy, their ability to develop adequate torque drops dramatically when spindle speeds fall below 300 rpm—the traditional speeds at which tapping is performed. Upgrading to a geared headstock could cost thousands of dollars and slow nontapping operations.

Thread milling eliminates low-rpm power problems, since it is a milling process. However, CNCs capable of helical interpolation are relatively new. Older CNCs may not be able to perform thread milling, leaving the tapping process as your only viable option.

When tapping or thread milling, experts recommend that you equip your machine tool with a coolant-through-the-spindle system. This is especially important when threading deep holes to ensure that coolant reaches the workpiece/tool interface. If your machine lacks such a system, have one retrofitted by the builder or a third-party supplier.

Another consideration is the long-term effects the chosen process will have on the machine. Thread milling puts no more stress on the machine than conventional milling does. Tapping, though, can wreak havoc on the spindle.

Emuge helped an automobile manufacturer set up a high-volume tapping operation that involved running 20 standard machining centers continually, three shifts a day. The frequent reversing of the spindle that’s required when tapping caused all of the machines’ spindles to fail prematurely. Each had to be rebuilt within 18 months.

The automaker solved the problem by installing self-reversing tapping heads.

Hole Characteristics. The next area to consider is the hole you intend to thread. Dan Gajdosik, engineering manager at tap manufacturer Besly Products Corp., South Beloit, Ill., recommends tapping any hole up to 4" in diameter. He said that while taps tend to be less forgiving and more problematic than thread mills, he believes that they can be more consistent and cost-effective on long runs once the process is brought under control.

Emuge’s Hatch disagreed. He said that thread milling is cost-effective for many applications, including some high-volume runs.

Thread depth and the required configuration at the bottom of the hole also can affect whether you tap or thread-mill. The vice president of Lake Bluff, Ill.-based Advent Tool & Manufacturing Inc., Jim Hartford, said thread mills are only practical at depths that satisfy the 3-1 ratio rule: Thread depth is limited to three times the major thread diameter.

Another consideration is whether you’re threading a through hole or a blind hole. In a tapping operation, there needs to be clearance at the bottom of the hole for the tool’s cutting edge (chamfer). A tap cannot thread the entire hole depth, due to its chamfered cutting edge.

According to Hartford, this is not a problem for a thread mill, which leaves only a slight undercut at the hole’s bottom.

Material. Standard taps begin to encounter problems when cutting materials hardened above R_C 30 and in production situations if the material has inconsistencies, such as hard spots. Standards can snap, wear quickly or produce inconsistent thread forms. Using special taps, designed to counter these problems, will increase tool costs.

Thread milling may be the only viable method to effectively cut a thread in difficult-to-machine materials such as Inconel, Invar and Monel. Thread mills also may work better on gummy materials, which can collapse around a tap. That won’t happen with a thread mill, because it doesn’t fully engage the workpiece.

Operational Flexibility and Control. When it comes to flexibility, thread mills have an edge over taps. According to Hatch, only minor programming changes are required for a single 1/2-20 thread mill to thread a range of hole diameters—up to 7/8-20. The same tool can also produce UNC, UNF and UNEF threads. This flexibility lowers tool costs and changeover times and frees up pockets in the toolchanger.

The inherent control that thread milling offers can also lower your scrap rate. If you snap a tap during a high-volume production run, the part might be salvaged or scrapped at a tolerable cost. However, if you are in the final steps of threading holes in an aerospace part with 1,500 hours into it, the risk of scrap can be a critical factor in choosing a thread mill over a comparable tap.

The president of Fulton Precision Industries, Walt Barmont, said that his McConnellsburg, Pa., job shop usually generates threads with taps. Occasionally, though, he opts for thread milling because of the extra control and flexibility that the operation provides.

He takes advantage of the ability to make size adjustments to a thread mill when threading a part that’s been distorted during heat treatment or to make a size allowance for a thread that has to be plated. Barmont said that this capability saves him from having to purchase special taps.

Barmont also discussed a downside to thread milling: It takes longer. In one application, he thread-milled a 1˝-12 hole that was 2" deep. He ended up with a high-quality thread, but the thread mill had to make four passes to complete the thread form. Barmont said that the cycle time was 25 to 30 percent longer than if he had tapped the hole.

When comparing dimensional accuracy, taps and thread mills can both produce threads that will conform to design requirements. In high-accuracy situations, though, it’s hard for a tap to compete with a thread mill.

Hatch said that a standard quick-change tap/holder combination will hold a tolerance of ±0.0050". A solid holder tightens the tolerance to ±0.0020". A typical thread mill, however, can meet a tolerance of ±0.0005". That’s similar to the results possible with a boring bar.

Cost. Aside from the relative operational advantages of one process over another, many times a decision boils down to cost. The table below compares the average cost and performance of a 3/8-24 thread mill and two types of taps.

The general-purpose tap is made of HSS. The high-performance tap is coated. In this example, a chromium nitride coating is specified for tapping aluminum and a titanium nitride coating is specified for the steel and titanium applications.

Notice that the hole count does not change significantly between the high-performance tap and the thread mill. Therefore, your decision about whether to tap or thread-mill will probably be based on other variables, such as setup time, tool-pocket limitations, cycle time and hole characteristics.

Taps cost anywhere from $12.37 for a 0-80 tool made of HSS to $1,500 for a 4˝-8 with a TiN coating. Thread mills run from about $200 for a 10-32 tool up to several hundred dollars for a 4˝-8.

An advantage offered by some larger thread mills—those designed for hole diameters of 3/4" or larger—is that they incorporate replaceable inserts. You can run several sizes of a particular pitch by making a programming change, or you can vary thread characteristics by switching to a different type of insert.

Besly’s Gajdosik pointed out that tap resharpening needs to be factored into the total cost of tapping. This expense must be weighed against the cost of inserts for thread mills (above 3/4") vs. the quantity of backup taps needed to keep production running while tools are resharpened.

The decision to tap or thread-mill depends on the variables mentioned above, as well as others. You will have to do some homework before deciding which method is better for a specific threading application.

With the growing sophistication of coatings and CNC technology, you have more options and flexibility than ever before. This flexibility can help you pick the best machine and tool to thread a variety of holes in a myriad of materials.