by Kip Hanson
Tips on single-point thread cutting from the experts
Without threads, light bulbs wouldn’t screw in and pickle jars wouldn’t stay closed. Threads use the principle of the inclined plane to fasten two components together, or drive one against the other—the adjusting screw on a leveling jack, for example, or the locknut used to tighten it down. Unlike fastening methods such as rivets, welds, and glue, threads are often designed to be temporary. Replacing a tire or bolting a television to the wall would be far more challenging without threaded fasteners. Other threads—those that retain a hip joint, or hold a jungle gym together—will hopefully remain in place throughout their service life.
For the most part, threads are defined by their major, or outside diameter, and pitch. The engine in your snowblower might be secured with a few M10 x 1.5 hex-head bolts. The major diameter of the threads in this case measure just less than 10 mm (0.393 in), and the bolt advances by its pitch, or 1.5 mm (0.059 in) per turn of the wrench. Like many threads, those snowblower bolts probably have a 60° V-form, but there are also 29º Acme threads, 55° Whitworths, square threads, buttress threads, and a host of others.
There’s also a host of manufacturing methods. Threads can be rolled, milled, tapped, formed, ground, moulded, cast, EDM’d, printed, whirled, and single-pointed. For the intent of this article, it’s the last on this list that concerns us. Screw-cutting lathes have been around since DaVinci, but until the invention of CNC machines, single-point threading was tedious work. Chucker lathes use a lead-screw and follower to chase a thread, while engine lathes use complex gearboxes. Both require a steady hand and quick reflexes.
It’s all routine
Thanks to today’s machine controls, programming a screw thread on a CNC lathe is a straightforward exercise. Most employ G76 or comparable automatic threading routines that need only a few parameters to generate the correct toolpath. For Fanuc-compatible controls, these include the thread diameter (X), height (K) and length (Z), its pitch (F), and whether the thread is tapered (I), as in a pipe fitting. There are a lot of details about thread programming, but two of these values are especially worth discussing.
The programmed infeed angle is often overlooked, but is possibly the most important of all threading parameters. By default, this value is set to 0°, which means the tool feeds into the workpiece straight on, perfectly perpendicular to the longitudinal
axis of the thread. Cutting occurs equally on both flanks of the insert, creating extreme tool pressure. This can cause chatter on deep threads, and poor chip evacuation.
As a rule, tooling manufacturers recommend a “modified flank infeed” angle of 30° (half of the 60° thread form). This is the equivalent of tipping the compound rest on an engine lathe, which any veteran lathe machinist knows is the best way to improve tool life and improve thread quality. It minimizes cutting force and allows the chip to flow away from the workpiece. This programming method is important with chipbreaker-style threading inserts, since these are designed to cut on one side of the tool.
Not so fast
Another programming consideration is feedrate. Except on multiple start threads (the cap on my toothpaste tube has a triple-start thread) feedrate is equal to thread pitch—in the program for our snowblower bolt, the “F” value would be 1.5 mm/rev (0.059 in). However, with today’s advanced carbides and coatings, high cutting speeds are the norm, and operating a lathe at 6000 rpm or more isn’t unusual. Cutting a snowblower bolt at this spindle speed, however, requires a Zaxis velocity of 9000 mm/min (354 ipm). Granted, this is far less than the rapid traverse rate of modern CNC lathes, but few of them can accurately control a cutting tool at this heart-stopping speed. The moral? Do the math and understand your machine’s capabilities, or be prepared for scrapped parts.
Successful threading takes more than G-code, however, and the choice of cutting tool is just as important as which parameters are used to program it. Indexable threading inserts are available in two basic styles, laydown or on-edge. Both use a clamp, screw, pin, or combination thereof to force the insert against the walls of a pocket machined in the toolholder.
Laydown inserts, as their name implies, lie horizontally in the toolholder pocket. Most are triangular in shape and have three cutting edges, although variations exist. They usually employ a carbide shim that sits below the insert, tipping it to the correct helix angle for the thread being cut. This may mean an assortment of shims is required—a very fine, 96-pitch thread for a watch stem will almost certainly use a different shim than that used to cut an 8-pitch thread for a trailer hitch ball.
On-edge threaders, also known “stand up” inserts, have two to four cutting edges. So-called “Top Notch” style threading tools have a simple clamp that engages a groove in the top of the insert, pulling it down and back against the pocket. Others use a flush-mounted screw or eccentric pin that mates with a hole in the centre of the insert. Because there’s no shim, some argue this style of insert is simpler to use, while proponents of laydown inserts claim theirs are more secure than their on-edge counterparts. As with anything, your mileage may vary.
Whichever threader style you’re using, there are also several variations in the insert itself. General-purpose V-style inserts cut the thread form and root diameter—the major diameter must be cut with a separate turning tool. This approach offers fine control over the thread’s various dimensions. Also, a single threading tool can be used to cut a wide range of thread pitches and sizes. This makes V-style inserts ideal for low volume work found in many job shops.
A little off the top
Topping and partial profile inserts cut all or most of the thread form at the same time. Unlike a general-purpose tool, a 16-pitch topping insert cannot be used to cut a 12-pitch thread. A dedicated insert is needed for any given thread series, but since topping inserts cut the thread’s major diameter simultaneously with the rest of the thread form, they eliminate the necessity to deburr the top of the thread—the crest—after threading, thus saving time and possibly improving part quality.
Carbide grades are also important. Because of the feedrate limitation explained earlier, thread cutting is often performed at less than optimal surface speed. This leads to built-up-edge (BUE), chipping, and galling, especially on gummy materials such as stainless steel. Tooling manufacturers combat this problem with tough carbide and lubricious coatings such as TiN and TiCN, designed to reduce build up and improve tool life. Some tooling manufacturers recommend polycrystalline diamond (PCD) inserts when threading aluminum and copper, while others offer high speed steel cutting tools for machining plastics.
Whatever the thread form or workpiece material, chances are good there’s an insert to cut it. If not, a custom tool may be the answer. For a slight premium, many cutting tool manufacturers offer special geometries to cut the proprietary thread forms increasingly seen with medical, oil and gas, and aerospace applications.
Thanks to the programming power of CNC lathes, along with the wide variety of threading tools, carbide grades, and coatings, tooling up for a threading job isn’t too tough. Choose the best insert style and geometry for your application, evaluate the cost per edge, apply clean cutting fluid—preferably at high pressure—and take a look at toppers if part volumes are high. You’ll be threading in no time. SMT
Kip Hanson is a contributing editor. [email protected]
David Andrews, Western Ontario regional business manager, Sandvik Coromant Canada, Mississauga, ON
Ken King, COO, Kaiser Tool Company Inc., Fort Wayne, IN
Nathan Preiss, threading product manager, Ingersoll Cutting Tools USA, Rockford, IL