Rather than using taps to thread steel prior to hardening, a growing number of shops are opting to thread mill heat-treated steel.

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

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

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.”

Heat-Treated Steel

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.

Milling Stainless

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
and the application.”

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.”

Quality Threads

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@ or (847) 714-


Advent Tool and Manufacturing Inc.
(800) 847-3234

Applied Thermal Technologies Inc.
(866) 998-6029

Kennametal Inc.
(800) 446-7738

Myles Tool Co. Inc.
(716) 731-1300

Redrox Industrial
(905) 670-2277

Sandvik Coromant Co.
(800) 726-3845

Seco Tools Inc.
(248) 528-5200

X-L Engineering Corp.
(847) 965-3030

Making steel hard—but not too hard

in warsaw, ind., Applied Th ermal 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

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.

—D. McCann

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, click on “Machine
Operations, Cutting” and scroll down to
“Where Taps Fear to Th read.”

1. Th read mill is showing accelerated or
excessive wear.
a) Incorrect speed and feed selection.
Solution: verify the correct speed and
feed was selected from the speed
and feed chart.
b) Excessive tool pressure. Solutions:
Decrease the feed per tooth; perform
tool change at quicker intervals; check
the tool for excessive wear—beginning
threads will wear the fastest.
c) Incorrect coating creating built-up
edge. Solutions: Investigate other
coatings; increase the coolant fl ow
and volume.
d) Spindle speed is too high. Solution:
Decrease the spindle speed.

2. Cutting edges are chipping.
a) Incorrect speed and feed selection.
Solution: Verify the correct speed
and feed selection was selected from
the speed and feed chart.
b) Th read mill moved or slipped in
its holding device. Solution: Use
hydraulic clamping chuck.
c) Lack of machine rigidity. Solutions:
Verify the workpiece is being properly
clamped; retighten or increase
stability if needed.
d) Insuffi cient coolant pressure or fl ow.
Solution: Increase the coolant fl ow
and volume.

3. Steps in thread profi le.
a) Feed rate is too high. Solution:
Decrease the feed rate per tooth.
b) Ramp-in is programmed as an
axial move. Solution: Make sure the
threadmill is arcing in the major
diameter instead of making a radial
c) Excessive thread mill wear. Solution:
Perform tool change at quicker
d) Tool is sticking out of the holder too
far. Solution: Make the amount of
overhang in the holding device as
short as possible.

4. Gage difference from part to part
a) Tool is sticking too far out of the
holder. Solution: Reduce the
overhang in the holding device as
much as possible.
b) Incorrect coating creating BUE.
Solutions: Investigate other
coatings; increase the coolant fl ow
and volume.
c) Excessive thread mill wear. Solution:
Perform tool change at quicker
d) Workpiece moving in its fi xturing.
Solution: Verify workpiece is being
properly clamped—retighten or
increase stability if necessary.