December 2009 / Volume 61 / Issue 12|
Where taps fear to thread
By Daniel McCann, Senior Editor
If the tap broke it could damage the thread, which would mean scrapping the part—and Dusan Micic wasn’t about to take that chance. Micic, owner of the 3½-year-old job shop Redrox Industrial, Mississuaga, Ontario, specializes in 5-axis milling of aerospace and military parts. Careful planning for such jobs is as essential as skillful machining, and in June 2008 Micic received a work order that prompted him to consult toolmaker Myles Tool Co. Inc., Sanborn, N.Y., which also houses a machine shop.
The part, he explained to Joe Adams, Myles Tool’s cutter grind supervisor, was a camera-mounting plate. Composed of 17-4 precipitation hardened stainless steel heat-treated to a hardness of 45 HRC, the component called for internal threads in a series of holes, two of which—each measuring 0.106" in diameter and ¼" deep—were especially small.
Tapping wasn’t an option. The material was too hard; the risk of the tool snapping too great. “When a tap breaks it can be very difficult to take out, and the hole could be damaged,” Micic said. While a tap is completely embedded in a workpiece as it threads, a thread mill rotates freely inside the drilled hole, sculpting a thread with each turn. The thread mill’s movements are controlled by 3-axis mills using simultaneous helical interpolation (X and Y axes traveling in a circular direction while the Z-axis follows a linear path). Should the tool break, it falls to the bottom where it’s easily retrieved with needle-nose pliers.
Adams suggested threading the holes with a 6-32 thread mill (No. 6 thread at 32 threads per inch). “It’s a submicrograin solid-carbide tool, which has high transverse rupture strength, coated with aluminum titanium nitrate,” Adams said.
Then Micic and Adams calculated the necessary feeds and speeds. “In our machine shop,” said Adams, “we have a hard mill tool for milling up to 62-HRC materials, so I went to that feed and speed chart and then backed the numbers off about 30 percent because the geometry of the 6-32 isn’t like a hard mill; it’s only 0.100" in diameter. Heat-treated material is much more abrasive than material in the soft state. When you machine [hardened steel] you have to be very toolload conscientious; you have to watch how much you’re going to push that tool because it’s only as strong as its smallest diameter.”
Micic programmed his Haas 3-axis VF5 to thread at 2,100 rpm, with a feed rate of 1.5 ipm. He used a fixture plate to hold the workpiece. To minimize vibration and tool load, Micic arced in and out of the hole. Starting at the bottom of the part, he used the climb milling technique, whereby the feed and rotating thread mill revolve in the same direction. The action ensures that chips fall behind the thread mill, which helps provide optimal surface finish and extend tool life.
The 6-32 tool completed the first pass in each hole in about 20 seconds. “You can’t get too aggressive with this material. I did three passes in each hole, a semifinish and two finish passes,” Micic said. “I still do taps, but it all depends on the application. If it’s a very difficult application, I thread mill. It gives me peace of mind.”
Thread milling internal threads in heat-treated steel parts from 40 to 55 HRC has gained ground in recent years as part of a wider trend among shops to machine harder, more resilient materials. Jim Hartford, vice president of Advent Tool and Manufacturing Inc., Lake Bluff, Ill., estimated that during the past 5 years, the percentage of his customers thread milling heat-treated steel has increased about 30 percent.
The trend has been abetted by technological advances such as CNC 3-axis machinery capable of simultaneous, multiaxis helical interpolation, the increased use of solid-carbide thread mills and, not least, shops’ interest in streamlining operations.
Traditionally, companies working with hardened steel threaded it first with either a tap or a thread mill, sent it out for heat treatment, had it shipped back and then performed grinding or whatever was necessary to rectify problems due to heat-related movement in the steel. It was often a cumbersome, time-consuming regimen. “If you buy the material already hardened, all you have to do is machine it,” said Nick Gaten, manager of global milling at Kennametal Inc., Latrobe, Pa. “It’s a lot faster to deliver a part from a hardened piece of steel than it is to do it the traditional way. And, of course, speed is a big advantage when it comes to winning orders.”
Machining hardened steel—and thereby avoiding possible thread movement or distortion due to heat treating—also improves quality, said Don Halas, threading and grooving product manager for Seco Tools Inc., Troy, Mich. “You get a perfectlooking thread and you don’t have to chase anything out [scale from heat treatment] because the finish is exceptionally good. Also, because you thread after heat treating, your positioning is 100 percent accurate.”
Carbide Thread Mills
The tool of choice for threading holes ¾" in diameter and smaller in heat-treated steel is the solid-carbide thread mill. The indexable carbide model is recommended by many toolmakers for larger holes. Indexables are favored because they provide greater cost savings; rather than replacing the entire tool due to wear, only the inserts need to be changed. Hartford of Advent Tool, which makes carbide thread mills, said the company’s tools are fabricated with carbide blends for hardness and added flexibility to provide “a little deflection for the side pressures.”
He added, “We use a special submicron blend with 10 percent cobalt for harder steel, 12 percent cobalt for softer steel and, for diamond-coated tooling, more of a standard-size micron with 6 percent cobalt.”
The company grinds and hones the edge of the thread mill. “Because the high-cobalt blend with a hardness of about 91 HRA might make the tool wear quickly, we use vapor deposition to draw a titanium-aluminum-nitride coating on it to increase hardness,” said Hartford.
X-L Engineering Inc., Niles, Ill., makes medical and aerospace components and, depending on the job, will either mill or tap threads. “We make a lot of internal components used in tools for surgeries,” said Ted Tworek, production manager. “The majority of parts we deal with are 1" in diameter or smaller.”
Aside from material hardness, the amount of clearance at the bottom of a hole can be the deciding factor for choosing whether to thread mill or tap. If the hole is too shallow for a tap’s lead thread length, a thread mill makes more sense. “You hold size better [with the thread mill] compared to a bottom tap, which has a tendency to cut oversize,” said Tworek.
A recent job involved threading for a component used in an air-driven surgical tool. It was a 416 stainless steel part that had been heat treated to 36 to 44 HRC. The job called for a 2-56 thread with a minimum thread depth of 0.125" and a maximum drill depth of 0.150" in a 0.070"-dia. hole.
Tworek used a 2-56 Vardex thread mill set at 9,600 rpm with a feed rate of about 14.5 ipm. He programmed the tool to make four passes, using the climb milling technique. “Because of the harder material, you have a bigger chance of blowing up the tool, so I like to add passes,” he said. Tworek made two passes removing about 0.003" of material each time, and two spring passes to produce a clean finish. “It took less than a minute,” he said. “So there was really no time difference between tapping and thread milling. It all comes down to the value of the part
Climb milling, as practiced by Micic and Tworek, is essential to effective thread milling, said William Durow, senior milling specialist for Sandvik Coromant Co., Fair Lawn, N.J. “When you climb mill, you ensure a thick-to-thin chip,” he said. “Carbide thread mills work very well in compression; when you conventional mill you create tensile stresses, which carbide does not like. [Conventional milling] also creates more heat, and when you are dealing with difficult- to-machine materials the conditions are multiplied.”
Tapping vs. Thread Milling
While X-L Engineering’s Tworek noted that tapping and thread milling run noseto- nose in terms of threading time, tapping has the clear advantage when it comes to certain-sized holes in hardened material. Using a tap is the prudent option when the depth-to-diameter ratio is about 3:1 or greater. Thread mill deflection becomes a greater risk in those cases. “As the thread mill descends a deep hole, it loses rigidity and there’s a push-away effect from the workpiece, so the tool cannot thread effectively,” said Seco’s Halas. “While there’s always the chance that a tap can break, it’s the better option.”
Other than long-hole applications, thread milling’s effectiveness in hardened steel clearly surpasses that of tapping, according to sources for this article. In addition to the capabilities already cited, thread milling provides smaller chips—about 0.3" long—while those produced during tapping can be several times larger, which can present evacuation challenges. Also, thread mills can be programmed to machine holes of varying diameters and pitch, while a tap is limited to a single pitch and hole size. “Let’s say you want to change the pitch diameter, make it larger or smaller,” said Halas. “Well, you can do that with a CNC offset machine—and even make right- and left-handed threads with the same thread mill. You cannot do that with a tap. Whatever tap you buy, that’s what you get. So that’s a big advantage of thread mills.”
And while a thread mill can cost five times or more than a tap, it’s much more likely than a tap to remain intact for multiple threading jobs on hardened material. (A tap for the hole Micic threaded costs about $16, whereas the price of a 6-32 thread mill can run from about $57 to $97.)
Thread mills also provide deeper, stronger threads. “When you tap, you drill the hole first, generally 25 percent larger [than the minor diameter] to make the tapping operation easier,” Halas said. “That means that the thread is not 100 percent; it’s only 75 percent because you lost 25 percent drilling oversize. With thread milling, you do the opposite. You go in undersize, take the material off and get a 100 percent thread on there. What you gain from that is 5 percent to 7 percent more thread strength.”
Achieving optimal thread milling results usually requires little more than correctly programming thread mill software, which is provided by thread mill manufacturers. “With our guide, you type in the tool you’re using and the kind of material you’re working on and it generates the code for you,” Sandvik’s Durow said. “It gives you your feeds and speeds in a [Microsoft] Word file, you pop it into your program and you’re good to go.”
Problems can occur when companies neglect programming guidelines. “Some people use the software just to pick the tool,” Kennametal’s Gaten said. “But if you don’t use the output feeds and speeds that are on the CNC program that the software generates, you can have trouble.” Companies that forego programming guidelines commonly miscalculate feeds, Gaten continued. “If you have a tool in a hole that’s not much bigger than the tool itself, the tool’s going around the periphery of the thread, but the center of the tool is going around a much smaller diameter. The machine tool is controlling the feed rate of that smaller diameter, and people often work out the feed rate at the cutting edge and forget to compensate it down for the difference in the radius that the tool’s going around compared to the radius that the center of the tool is going around. You end up having horrendously high feeds, and the thread mills chip.”
Also, shops working with hardened materials sometimes need to conduct multiple threading passes to ensure a quality thread, Seco’s Halas said. “Let’s say the length of the thread is 1" and you get three-quarters of the way down and the tool stops,” he continued. “That means the cutter was pushing away; it couldn’t cut the threads large enough and [the threading] actually looks like a bell as it gets narrower toward the bottom. But if you do an extra pass, or sometimes three passes, that helps to alleviate that.”
As for further developments to enhance thread milling’s capabilities, Halas said Seco is experimenting with thread mills made of CBN, a material nearly as hard as diamond. If it proves effective, it will be another step forward for shops interested in thread milling heat-treated steel. “Once shops try thread milling, they’re hooked,” Halas said. “Actually, we’ve seen an increase in thread mill sales since [the economy] slowed down. Previously, most shops were running full kilt. They didn’t have time to try it. So now they are trying thread milling, and they really like it.” CTE
About the Author: Daniel McCann is senior editor of Cutting Tool Engineering. He can be reached at dmccann@ jwr.com or (847) 714- 0177.
Advent Tool and Manufacturing Inc.
Applied Thermal Technologies Inc.
Myles Tool Co. Inc.
Sandvik Coromant Co.
Seco Tools Inc.
X-L Engineering Corp.
Making steel hard—but not too hard
In warsaw, ind., Applied Thermal Technologies Inc. specializes in vacuum heat treating and brazing steels and exotic materials. Equipped with nine vacuum furnaces and eight tempering furnaces, the company serves the orthopedic and aerospace industries, said Micky Bradican, president of Applied Th ermal. “While medical implants are usually made of titanium, surgical instruments are typically stainless steel, and aerospace runs that gamut from Inconels to cobalt alloys, titanium and stainless steels,” he said.
Methods of heat treating the metals to increase hardness and tensile strength vary. Steel, a ferrous metal, generally undergoes a two-step process called “quench and temper hardening.” Depending on the chemistry and size of the part, the steel is heated to 1,400° F or higher for a minimum of 30 minutes. Heating repositions the carbon atoms and strengthens the atomic bonds. Th e steel is then quickly quenched in water, oil or air, locking the carbon atoms in place. Tempering, the next step, involves reheating the steel from 200° F to 800° F to reduce some of the hardness, yet retain enough for the part’s intended use.
While quench and temper is used for most steels, it’s not the sole method of heat treating the material. Th e specifi c chemical composition (percentage of carbon, iron and other alloys) is the determining factor. For instance, the 17-4 PH stainless steel plate for the camera mount cited at the beginning of the main article contains iron, nickel and chromium, and would have required a single-step process (heating at 900° F for 1 hour) to achieve a hardness of 45 HRC.
Troubleshooting common thread mill problems
Myles Tool Inc. Co. has compiled a troubleshooting chart listing the 11 the most common problems and solutions for thread milling. Th e four most prominent problems and corresponding solutions are listed below. To view the entire list, visit www.ctemag.com, click on “Machine Operations, Cutting” and scroll down to “Where Taps Fear to Thread.”
1. Thread mill is showing accelerated or excessive wear.
2. Cutting edges are chipping.
3. Steps in thread profile.
4. Gage difference from part to part.
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.|