Metal removal rates are faster today than
ever before. What was considered high speed machining just a few years ago
is regarded as conventional today. Many factors are driving shops to faster
metal cutting rates. These include better and more capable machine tools and
CNC processors that allow the machine to accurately cut at increasingly
higher speeds and feeds.
Commercial considerations are also driving
shops toward higher rates of productivity. The need to put more work across
machine tools has shops looking constantly to improve metalcutting
While much of the discussion about high
speed machining tends to focus on the role played by the machine tool, the
cutter is its partner in high speed machining. And, that's the focus of this
article. We're going to look at what a shop needs to know about specifying
cutting tools for their high speed applications.
To get perspective on tooling
considerations for high speed machining, we contacted
North Carolina) to discuss high speed cutting tools.
What's High Speed?
A generic definition of high speed
machining is elusive. High speed is relative. What's very fast for one
industry segment seems glacial to another.
Machining speed is very application
specific. Calling a machining process high speed draws a comparison between
its current and previous performance capabilities. For example, high speed
might mean changing from an HSS tool to solid carbide, which allows you to
bump up machine feeds and speeds. Because carbide cutters, in many
applications, can remove metal faster than HSS, a shop using carbide is
machining faster compared with HSS rates. But it's relative because another
shop, using cermet or ceramic cutters, can cut faster than carbide.
So, we're not going to assign a definitive
value to high speed. Suffice it to say high speed machining means cutting
metal faster that is customary for your operation.
Some Basics -- SFM And
Elusive as high speed machining is to
define, there are measurements used for machining speed. These allow
comparison between different rates and help a shop determine its place in
the machining speed continuum.
To quantify how fast a machine
actually cuts metal, spindle rpm needs to be converted into something more
useful. According to Dan Spanovich, application specialist for
figure is expressed as surface feet per minute (sfm).
Likewise, feed rate for the machine tool
is usually measured in inches per minute (ipm). But for cutting tools, it is
expressed as inches per tooth (ipt). Working from the optimum sfm and ipt
for workpiece material, a machine tool's rpm and ipm can be determined and
These two measurements are dependent on
each other to determine the speed at which a workpiece can be maintained.
For example, titanium can be cut effectively at about 250 sfm. That's using
a chip load of 0.005 ipt. However, some shops report machining titanium at
close to 500 sfm, but to do that, lighter chip loads are taken.
Depending on the cutter material, chip
load and surface speeds can be adjusted to deliver the best combination for
a shop's application. If heavy metal removal is the goal, cranking up the
chip load and sfm will maximize the cutting efficiency. For better finish,
backing off the chip load while keeping sfm up will give good surface
There are no specific formulas to
determine the best combinations and results. It takes a little
experimentation to find optimum feeds and speeds for a specific application.
A cutting tool material has specific
attributes that make it usable in a metalcutting application. Because
applications vary so widely, there are many cutting material combinations
from which to choose.
But in general, only two performance
criteria are used to determine the applicability of a cutter. These are
toughness or resistance to fracture (ductility) and thermal hardness
(resistance to heat). A myriad combination of coatings, substrates and base
materials can be created to deliver specific proportions of toughness and
thermal hardness to fit various applications.
Cutting tool materials can be classified
into five general categories. The materials are arranged from best toughness
characteristics to best thermal hardness:
- Tungsten carbide (uncoated and coated),
- Ceramics, and
- Diamond and CBN.
Starting with HSS and progressing to
diamond and CBN coatings, a scale can be built progressively from best
toughness characteristics to best thermal hardness. High speed steels take a
pounding but can't take much heat. Ceramics and diamond coated cutters can
take the heat but fracture easily.
Generally, tungsten carbide cutters have a
working range of 100 to 1200 sfm, according to Mr. Spanovich (HSS goes up to
approximately 100 sfm). Ceramics, including silicon nitride, push the
envelope up to 4,000 sfm. Polycrystalline diamond and CBN coated tools push
sfm above 4,000. These rates are at chip loads of 0.003 to 0.030 ipt.
These rates represent optimum cutting
potential for the right combination of workpiece material and cutter
material. However, there are other factors that must be considered before a
shop can hope to approach these kinds of cutting speeds.
The importance of rigid fixturing cannot
be overemphasized in high speed machining applications. While the goal of
any fixturing or clamping setup is to hold a workpiece securely and allow
for repeatable location of subsequent parts, high speed requirements magnify
any imperfections in a workholding setup.
In high speed machining applications, the
fixture should support the workpiece on a solid base and have enough mass to
help damp cutter-induced vibrations. Fixtures for high speed need not be
overly complex but should follow good shop practice.
For example, a good vise is adequate if it
supports the workpiece securely. It is recommended that positive stops be
used to prevent torquing or movement of the workpiece in response to cutter
The Force Is With You
Proper selection of a cutting tool,
especially an indexable cutter that is rated to spin at elevated speeds, is
important. Not to put too fine a point on it, but we're talking potentially
serious or even fatal accidents if a shop tries to exceed tooling speed
The reason is simplecentrifugal force. For
the same reason tire manufacturers have speed ratings for radials, tooling
manufacturers put a "not to exceed" rpm on cutters. The force created by
rotating a body is exponential to the speed of rotation. That force is
trying to rip the inserts away from their seats. Any part of a cutter flying
off at 10,000, 15,000 or 20,000 rpm poses a risk to life and limb.
Indexable insert tools for high rpm are
different than tools for conventional rotating speeds. Inserts are secured
differently to the cutter body for high speed indexable tools. According to
Mr. Spanovich, a simple setscrew clamp is not adequate for high rotation.
Inserts are secured to the cutter body with a pin that fits into a detent
molded in the insert. It is anchored on the cutter body in a direction
perpendicular to the centrifugal forces generated by rotation.
At elevated cutting speeds and feeds,
coolant may be less necessary than at conventional speeds. Heat is the
by-product of machining. Generally it's the enemy of metalworkers.
Increasingly however, heat is being used to help the cutting process.
In an ideal cut, workpiece material,
machine feeds, spindle speeds and cutter are all making their respective
contributions in optimum fashion. As the cutter creates a chip, the heat
generated by that action is transferred to the chip. When the chip breaks
and leaves the cutting zone, the heat is carried away with it.
A big advantage of high speed machining is
that at elevated rates of speed and feed, the chip is cut and evacuated so
fast it tends to transfer little or no heat to the green workpiece. At
conventional machining speeds, there is time for heat to move from chip to
uncut metal and create a work-hardening condition. This increases the force
needed to create a chip, which creates more heat, and on it goes. Coolant
mitigates the cycle by reducing the temperature in the cut zone and flushing
away the chips.
But at very high rpm, the tool rotation
throws coolant away from the cut zone so without very high pressure or
through-the-tool piping, it never reaches the cutting zone. "In some cases,"
says Mr. Spanovich, "trapped chips can remain in the cut, allowing them to
be recut by the tool. We've found an air blast is very efficient for
evacuating chips in high speed applications."
Thermal shock is another consideration for
users of high speed tools--especially ceramic and harder cutting edges.
Irregular distribution of coolant in the cut can create an unstable heat
zone for these cutters. Designed to operate at elevated temperatures, the
cutter material can undergo successive heat and chill cycles in the cutting
zone that can create premature failure from thermal shock.
The Right Angle
Cutter speed is the major influence in
creating heat at the cutting edge of the tool. Maintaining a high chip load
or feed is how heat is dissipated. Correct ipt, combined with the right
cutter rake angle for the material being machined, produces a chip of
sufficient density to carry heat from the cutting zone so work hardening can
Chip load is feed rate for each cutting
edge of the tool. For indexable insert tools, it's the load against each
insert. On solid body cutters, chip load is rated against each tooth.
According to Mr. Spanovich, a good working range of chip load is generally
between a minimum of 0.003 ipt to a maximum of 0.012 ipt.
The angle of attack for the cutter edge,
its rake angle, influences the chip load for a cutter. Rake angles vary from
positive through neutral to negative. Positive rake angles present a sharper
edge to the workpiece. It's also a weaker edge. Positive rake tools tend to
pull the workpiece toward them during the cut. They also tend to push chips
up and away from the cutting zone.
Negative rake tools have a much stronger
leading edge and tend to push against the workpiece in the direction of the
cutter feed. This geometry is less free cutting than positive rakes and so
consumes more horsepower to cut.
High speed tooling geometry, in general,
mirrors the geometry of conventional machining. "What you know about tool
geometry for conventional machining transfers to higher speed applications,"
says Mr. Spanovich. "If there is a trend in high speed, it is toward a
positive lead angle tooling. This lead angle effect allows greater ipt, by
lifting the chip, while maintaining the same chip thickness. This greater
feed rate results in higher speed machining.
"The formation of a sufficiently thick
chip is the goal," says Mr. Spanovich. "The idea is to use chips as a heat
sink. Faster speeds make more heat, so directing that heat into chips
becomes critical in high speed machining applications."
Watch For Wobble
Successful high speed machining is
dependent on static and dynamic rigidity among the many components that
bring together the tool and the workpiece. Critical to this is a highly
rigid connection between the tool, toolholder and the machine tool spindle.
Tool balance becomes a big issue at high
spindle speeds. "We recommend smooth shank tools, for end mills and drills,
held by a hydraulic or roll-lock collet chuck for high speeds," says Mr.
Spanovich. "Balance becomes an issue at 5,000 rpm and up. At those speeds, a
notch shank with setscrew can move the tool enough off-center to induce
vibration--hence chatter." For speeds of 20,000 rpm and up, a custom balance
of tools and toolholder combination is recommended.
The V-flange taper connection is a
potential source for high speed vibration. Until recently, the V-flange
taper and measurement gages used by cutting tool manufacturers were made to
ANSI/ASME B5.10 standards. "Until high speed applications came along, the
ANSI/ASME standard worked well," says David Lewis, staff engineer for
Kennametal and vice
chairman of the ANSI/ASME B5 standard committee.
Taper fit between a tool body and the
machine spindle can be in tolerance (per ANSI/ASME B5.10) and still cause
runout and eccentricity problems for a high speed cutter. Mr. Lewis and
others representing U.S. tooling manufacturers recommend application of the
European ISO 1947 AT3 standard in place of ANSI/ASME B5.10. The ISO standard
has twice the accuracy requirement of ANSI/ASME and results in a better
connection between the spindle taper and the V-flange tool. To make sure the
tooling you purchase for high speed applications is made to the new
standards, specify ISO 1947 AT3 or equivalent from your tooling manufacturer
for toolholders and collet chucks. For machine tool spindles, specify ISO
1947 AT2 (a lower AT number means a better fit). Mr. Lewis recommends gaging
be acquired to check spindle and tool tapers in the shop.
A Word About HSK
Much has been written about HSK or
equivalent tooling as a possible replacement for the V-flange connection in
machining operations. "While there are some advantages to the design
concept," says Mr. Lewis, "its widespread application is being held up in
part by a lack of manufacturing standards."
The primary difference between HSK or
other hollow shank, short taper toolholders is the way the tool fits into
the machine tool spindle. HSK uses a simultaneous fit between the short
taper and the face of the spindle. The connection is very rigid.
"The problem with HSK," says Mr. Lewis,
"is no governing body has established a standard for tooling companies to
manufacture to. There is a German DIN standard that's being considered by
ISO but so far it has not been approved. There are also some challenges to
HSK from Japan, other European countries and the United States. The question
of what HSK will look like is not yet decided.
"In the mean time, shops looking to do
high speed machining on their machining centers may be better off specifying
AT3 or better V-flange tooling than waiting for an HSK standard tooling
configuration," says Mr. Lewis. It could be a while before HSK or an
equivalent standard for tool, spindle and gages comes along.
Why Higher Speed?
Implementing higher speed machining in a
shop has many benefits some obvious but others less so. Obviously, making
parts faster helps satisfy customers' demands for quicker deliveries despite
shorter lead times. There are also benefits derived from increased tool
life. It may seem paradoxical, but machining at high speed with the right
tooling matched to the application can reduce tool wear because of the
diminished cutting forces at high speed.
High speed machining can help a shop
manufacture more accurate parts with better surface finishes. Often, because
a machine tool and workpiece setup must be very rigid for high speed
machining, the results are more consistent workpieces.
A less obvious benefit of high speed
machining for shops moving in that direction is derived from the exercise of
implementing it. Learning to do the things necessary for successful high
speed machining can simultaneously elevate other facets of an enterprise to
equivalent levels of productivity. MMS