Do you tap or thread-mill?

May 21, 2018 8:49 am

By Kip Hanson

Click Here for a free subscription to Cutting Tool Engineering magazine.

There’s a long-running argument in the machining community: Should I tap or should I thread-mill?

For many, the former is the preferred method of threadmaking on a CNC machining center. It’s fast, easy to program and can even be done offline—on a drill press or with a tapping arm—if the CNC machine is better utilized another way.

Yet others contend that thread milling is more accurate and almost as fast. Plus, there’s no risk of the tap breaking inside the workpiece, which often results in scrapping the part.

BIG KAISER’s MEGA Synchro drives taps securely and compensates for the small synchronization errors common with many CNC machine tools.  Image courtesy of BIG KAISER Precision Tooling.

Which group is right? The answer depends on several factors.

As a rule, thread mills are limited to threads no smaller than 1⁄8″(3.175mm), and because of the high cutting forces and resulting tool deflection, are generally limited to threading holes about 3 diameters deep. On the other hand, taps for #000-120 watch threads are readily available, and an extension tap can reach roughly 20 diameters deep.

Taps suitable for threading a fire hydrant hose are also available, but good luck driving a tool that big. Most CNC machine spindles struggle with tap diameters 1⁄2″ (12.7mm) and larger.

When tapping, there’s no way to adjust the thread’s pitch diameter except by changing to a different “H” size tap. This requires machine downtime and a large tool inventory. When thread milling, size adjustment is a simple offset. What’s more, the thread mill you applied on the 1⁄4″-20 job last week can be used on the 9⁄16″-20 job today, or any other 20-pitch thread that comes along.

Regardless of the workpiece material and preferred threading method, what’s most important is that the job is tooled and programmed properly. Here’s a list of pointers to help you do that:

  • With synchronous, or rigid, tapping, avoid using ER or comparable collet-style toolholders. A number of tooling suppliers offer holders that grip and drive the tap more securely than a collet. These holders also provide a small amount of axial “float” to compensate for the spindle-to-Z-axis synchronization errors common with many CNC machine tools. On a related note, thread mills should be gripped like any other milling cutter: with a well-maintained milling chuck or shrink-fit holder.
  • Some older machining centers don’t have rigid tapping capabilities. For these, a tension-compression holder is a must. Be sure to keep the spindle speed sufficiently low—no more than 500 rpm—so that it can reverse before the toolholder runs out of axial travel. Doing this will prevent breaking the drive pin inside. Here again, several companies provide tap holders equipped with quick-change tap adapters and internal clutch mechanisms that minimize the chance of damaging the holder.
  • A self-reversing tapping head may require installation of a drive dog on the machine’s spindle face, but it can be adapted to almost any machining center. Depending on its size, this type of attachment allows tapping at up to several thousand rpm and avoids the wear and tear that comes with repetitive spindle reversal. If you tap a lot of holes in aluminum, brass and other relatively soft materials, this method blows the doors off thread milling and traditional tapping methods.
  • If you’re unsure about the programming part of all this, you’re in luck. Several tool supplier websites have G-code calculators to generate the necessary toolpaths for thread milling. (Most CAM systems are capable of this as well.) When rigid tapping, use whatever M code is specified in the machine’s programming manual. Be sure to use a G84 or comparable tapping cycle—don’t use a G01 or G81 command, unless you enjoy breaking taps.
  • Don’t forget that much of what was discussed here applies equally to mill-turn centers and multitask lathes, which, thanks to their C-axis capabilities, can thread-mill with ease. These, as well as many 2-axis lathes, also offer rigid tapping—again, be sure to use the correct toolholder for the application.

What about hard materials such as heat-treated 17-4 PH or D2 tool steel? There’s little chance of successfully thread milling metals much above 45 HRC. And if you’re going to try to tap them, be prepared to duck the flying shrapnel when the tap explodes! Internal thread grinding and, on rare occasion, orbiting sinker EDMing are about the only ways to produce good threads in materials harder than 45 HRC.


Click Here for a free subscription to Cutting Tool Engineering magazine.

*This article is reprinted with permission from CUTTING TOOL ENGINEERING Magazine, and is protected under U.S. and international copyright laws. CUTTING TOOL ENGINEERING Magazine is protected under U.S. and international copyright laws. Before reproducing anything from this Web site, call the Copyright Clearance Center Inc. at (978) 750-8400.

Leave a Reply