Machining of Polyurethanes
|
|
Machining Polyurethanes: Introduction
Cast
polyurethanes can be readily turned, sawed, drilled,
ground, or milled. These and other secondary operations
present many similarities to the machining of metal, but
there are also some important differences. This paper is
intended to provide some general guidelines for
machining urethanes, and also focus on the most common
group of machining operations and discuss some specific
tools and techniques.
|
|
It is
important to note the material presented here is a
starting point. The wide variety of urethane compounds
and their respective physical properties and
characteristics creates a wide range of machining
situations. Experimentation and experience will tell you
what speeds, what feed rates, and what types of tools
will work best for the urethanes you machine regularly.
Harder urethanes -90A and up -have a high degree of
machinability. Lathe turning, fly-cutting, grinding,
contouring, and more are easily accomplished on
conventional metal-working equipment by machinists who
are familiar with procedures for handing plastics.
Some different tools and techniques are required for
compounds of 80A durometer and lower. These lower
modulus compounds are typically machined by knifing,
grinding, and sanding. In some cases, however, they can
be worked like higher modulus materials by "freezing"
them in dry ice or liquid nitrogen environments.
SOME KEY POINTS TO REMEMBER IN MACHINING
URETHANE
- Urethanes have much lower thermal conductively
than metals, so heat generated by cutting tools
stays close to the tool and raises the urethane
temperature rapidly. This heat must
be controlled. Melting can occur above 400 degrees
F.
In addition to possible melting, heat generated by
machining causes the part to expand. When that part
cools, it shrinks down and can end up undersize.
- Elastic memory - Elastic
recovery occurs in urethane both during and after
machining. The cutting tool must provide clearance
to compensate for this. With compensation, expansion
of the urethane as it passes the tool will result in
increased friction between the cut surface and the
cutting tool. Excess heat build-up will result.
Elastic recovery after machining can result in
smaller internal diameters and larger external
diameters than were measured during cutting.
- Modulus of elasticity -
Urethanes are resilient and can easily be distorted.
It is possible to alter the shape of a urethane part
by clamping or chucking it with too much force. This
would cause the final machined shape to be distorted
after the cut had been made and the fixturing
pressure was released. Care must be taken to hold
parts securely, but avoid distortion due to holding
or cutting.
- Softening point - Gumming, poor
finishes, and poor dimensional control will occur if
excess heat is generated and allowed to accumulate.
Proper tool geometry, feed rates, and cutting speed,
in conjunction with coolants usually overcome these
problems. Water soluble cutting oils and/or light
machining oils are good coolants for urethanes.
|
Machining Polyurethanes: Sawing &
Shearing
One of the best machines for sawing urethanes is
a band saw. Long blades of 125 to 175 inches are
desirable because they stay cooler and keep the
urethane from melting. A band type that we have
found to work will is a 4 tooth per inch with
raker set. A raker set blade is one that has its
teeth alternating to the left and right of
center.
|
|
Band speeds in the range of 3200 feet per minute
work well on almost all durometers. Feed rate is
controlled by hand, so it is operator dependent.
Any moderate hand feed will suffice, but
do not force the work.
On softer urethanes, a faster blade speed helps
prevent the urethane from pulling down into the
cut, rubbing on the blade, and building up heat.
When cutting thin, low durometer sheet stock,
the work must have some support. A sheet of
cardboard, for example, will help prevent the
workpiece from being pulled through the table
slot by the blade.
If a finer finish is needed, change to a 10
tooth per inch blade with raker set. When
cutting 90A durometer and below, use a spray
mist of water soluble oil (50 – 50 mix) to help
keep the heat down and to improve the finish.
This spray coolant is also helpful on thick cuts
where feeds are slow, and on long cuts where the
blade will contact urethane for a long period.
A good alternative to saw cutting thinner and
lower durometer sheets is a shear. Shearing,
punching, and die cutting are possible on sheet
stock up to 1" thick if the hardness is low and
the tools are sharp. Remember, though, as the
thickness increases, so does the tendency for
the cut edge to have a "dish" due to the
elasticity of the urethane. Shearing and
punching are also possible on 50D to 75D
urethanes, but it's only practical up to 1/4
inch thickness.
|
Machining Polyurethanes:
Turning O.D.'s & Facing
Turning,
boring, and facing operations can be
performed on either a turret or engine
lathe. Tool configuration, geometry, and
placement, as well as rpm are dependent
on what hardness the urethane is and
what the operation is. Another variable
is feed rate – the speed of the tool
with respect to the rpm of the lathe.
Feed is often controlled by hand and is
subject to operator judgement and
"feel".
|
|
In general,
use sharp tools, high turning speed, and
slow to moderate feeds (depending on
hardness). Cutting tools for urethane
must have sharp, carefully honed cutting
edges. Sharpen tools on a honing stone
for a razor sharp edge on the sides,
tip, and top of your tool. We have found
success with both high speed steel and
carbide tools.
Tool clearances must be greater than
those used for metal. The goal is to
have little or no resistance as the tool
travels through the urethane. The chip
(material that is being cut away) should
come off as a continuous strip or
ribbon. A smooth surface on the top of
your tool will aid in chip removal. This
is very important to prevent the chip
from wrapping back around the workpiece.
Good chip removal is also critical for
heat removal and tool life. See figure
1.
Figure
1. TURNING / FACING TOOL
Tool
geometry is very important for
successful machining of urethane. Rake
angles and nose radius will vary
depending on durometer and desired
surface finish. TOP RAKE
determines chip flow. Too little causes
that build-up and poor chip removal. Too
much will cause reduced tool life. 10 to
15 degrees is a good starting point.
SIDE RAKE is the amount
of angle from the cutting edge to the
bottom of the cutting tool 30 degrees is
a good starting point for side rake.
This angle affects surface finish. Too
little allows the tool to rub against
the workpiece. Too much will shorten
tool life. NOSE RADIUS
is the radius of the top edge of the
tool at the tip. Nose radius is the most
important part on a urethane tool
because it significantly affects surface
finish. As a rule, as durometer goes up,
nose radius increases.
High durometer urethanes (95A and up)
can be turned very easily. Smooth
surfaces can be achieved on heavy as
well as light cuts, so roughing cuts are
seldom required. Surface finish is best
when your removal is .050" or more so
your cutting tool gets a good "bite". We
have found that on the harder urethanes,
a speed of 600 to 1000 rpm works well.
Feed rate depends on the desired surface
finish. Typical feeds are in the .005 to
.010 in./sec, range. The faster the feed
rate, the more of a "record effect" you
will have in your surface finish.
For higher durometer urethanes, a
round-nose tool is a good choice. The
radius on the cutting end affects
surface finish. The nose radius should
be about 1/16 with a 10 to 15 degree top
rake and a 30 degree rake around both
sides.
Medium hardness urethanes - 80A to 90A -
require a tool with a smaller nose
radius of 1/32 or less. Side and top
rake should stay about the same. RPM
should be faster than what is used for
harder durometers - in the range of 1000
to 1500 rpm. Feeds are generally faster
- in the range of .050 to .150 in./sec.
This is a rapid "plunge" type feed.
When turning large diameter parts, cuts
of 1/10 to 1/8 inch deep and a light
feed of .003 to .007 inches per
revolution are recommended. Remember
also that centrifugal forces on large,
low hardness parts can cause a "flaring"
type deformation at high turning speeds.
This effect can cause the part to be
machined improperly if it is not
compensated for.
|
Machining of
Polyurethanes: Parting
Another lathe operation that is
a little different than turning
o.d.'s and facing is parting.
Parting, or cut-off, is used to
remove over-pour on higher
hardness parts that are too hard
to knife cut.
Tool that work well for parting
are .060" to .100" wide with a
20 to 30 degree front rake and
no top rake. A small 3/64 radius
is ground into the top of the
tool. Starting on the cutting
edge, some side clearance is
helpful. 3 to 5 degrees is all
that is usually needed. See
figure 2.
|
|
The
proper tool, feed, and speed
allow the chip to exit the cut
with little resistance and heat
build up. Parting yields a good
surface finish and is a useful
variation for facing certain
urethane parts.
Fig 2.
TYPIC
|
Machining of
Polyurethanes:
Knifing
Knife cutting urethane
to close tolerances can
be done without too much
difficulty. The tool
must be absolutely razor
sharp and be as thin as
possible. When knifing,
the urethane will have
the tendency to pull
into the tool. This
displacement of material
will cause a “dish” on
the finished end of the
part. The thinner the
tool, the less the
pulling effect on the
cut edge.
|
|
A good practice on thick
cuts is to do a rough
cut to remove the bulk
of the material, then
take finishing cut to
remove the final .025 to
.050 of an inch.
The type of fixture used
to hold the part is very
important. Parts with
metal inserts are
usually easy to hold.
Solid urethane parts can
deform if they are held
too tightly. Again, this
would make it impossible
to get a flat cut.
We use 2 types of
knifing tools. High
speed steel is used on
medium to hard urethanes
70A to 95A. This type
of tool must be very
smooth and have a razor
sharp point. All edges
and surfaces behind the
cutting point must be
smooth the prevent the
cut-off material from
being pulled between the workpiece and the tool.
High turning speeds of
600 to 1000 rpm’s with
rapid hand feed will
yield an excellent
surface finish. See
Figure 3.
Carbide blanks .250 x
.125 ground on a
diamond wheel to a razor
sharp edge and point
provide excellent cuts
on low durometer,
hard-to-machine
urethanes. Cuts as thin
as .005 are possible.
The tool must be as long
as the cut is deep.
Turning speeds of 600 to
700 rpm work well with
moderate to rapid hand
feeds.
Figure 3.
KNIFING TOOL FOR
HARDER URETHANES
Figure 3.
KNIFING TOOL FOR
SOFTER URETHANES
|
Machining of
Polyurethanes:
Contouring
O.D.
Machining
tapers,
chamfers,
grooves, and
other surface
configurations
into wheels,
roller, and
other round
parts all fall
into the general
category of
contouring.
Tools for
grooving the
O.D. of hard
urethanes 95A
to 75D all have
the same basic
tool geometry.
We have found
that a 10 to 20
degree front
rake works well
with no top
rake. Use high
rpm (depending
on the diameter
of the work
piece) and
moderately fast
hand feeds.
|
|
The tool works
best when
positioned 0.025
to 0.075 below
the center of
the work piece.
The chip should
come off in a
continuous
ribbon. Try to
keep the chip
from wrapping
around the work
piece.
Large tools work
well on hard
durometers, but
your machine
must be heavy
and have the
horsepower to
maintain
constant rpm
during the
cutting cycle.
See figure 5.
Figure 5.
CONTOURING
TOOL
Fixturing of
parts when
contouring is
very important.
It is possible
to pull
workpieces out
of the machine
if your
fixturing is not
rock solid. When
possible, pinch
the workpiece
between the
chuck and the
tailstock.
Another
possibility
would be to hold
the workpiece on
a fixture in a
lathe chuck or
collet by
bolting a plate
to the fixture
and sandwiching
the part between
the plate and
the fixture.
This type of
fixturing is
especially good
when cuts are
heavy, "plunge"
type.
Contouring and
chamfering
urethane wheels
and rollers is
done with tools
that are ground
and radiused to
the specific
dimensions of
the desired
final shape. For
95A to 75D
durometers, the
contouring tool
needs no top
rake. Coolant
applied with a
brush will help
the surface
finish. The work
must be kept wet
during the
entire cutting
cycle. Remember:
most contouring
tools have large
cutting surfaces
that build up
heat. This heat
must be kept
under control.
When contouring
urethanes softer
than 95A, use a
tool with 15 to
30 degrees of
top rake. Lathe
speed depends on
the o.d. of the
part. In
general, high
RPM works best.
|
Machining
of
Polyurethanes:
Milling
Urethane
ranging
from 90A
to 75D
durometer
can be
successfully
milled
without
much
difficulty.
Attempting
to mill
parts
below
80A is
not
recommended.
Tools
must be
sharp
and the
work
must be
fixtured
securely.
Two-fluted
end
mills
and
single
point
fly
cutters
are
preferred.
Fly
cutters
would
utilize
high
speed
tool
bits
ground
to a
round
nose.
Speed of
the
cutter
should
be 900
to 1300
rpm. A
feed
rate of
15 to 20
inches
per
minute
is a
good
starting
point.
|
|
Milling
is used
on parts
that are
impractical
or
impossible
to
machine
in a
lathe.
Milling
is also
used
where
close
tolerances
and a
good
surface
finish
are
required.
Again,
work
should
be held
so that
it is
not
deformed
by
excessive
chucking
pressure.
Of
course,
work
must be
held
securely
enough
so that
it
does not
come
loose
during
machining.
|
Machining of Polyurethanes: Grinding
Urethanes 55A to 80A durometer can be ground successfully in an engine lathe using a tool post grinder. Use low turning speeds - below 150 rpm, with the lathe running in reverse. Start with the grinder feed rate set for .005 inches per revolution. Use a slower feed rate to improve surface finish or to remove more material by taking a deeper grind.
|
|
In cases where larger amounts of material must be removed, turn the piece down with a cutting tool to within .020 of the finished dimension before grinding.
We have found that a Radiac Por-OS-Way 46 grit wheel with slight radius on the leading edge works well. RPM of the wheel should be in the 2250 to 3250 range. Again, low workpiece turning speed of 150 rpm is a good starting point. Fine abrasives can be used for final polishing.
Urethane above 80A durometer usually requires some type of coolant, however it can sometimes be ground dry. Water is good coolant, and can be applied with a brush or with a fine spray mist. Apply spray coolant on long traverse grinds. On a plunge grind where the part width is less than the wheel width, apply water with a brush to keep the urethane wet.
We recommend that the grinder be equipped with a dust collector or the operator wear an approved dust mask when grinding or sanding urethane.
|
Machining of Polyurethanes: Drilling
Slow, spiral drills perform best because the large flute area permits free discharge of chips with a minimum of binding and heat build-up.
Frequent retraction of the drill aids in eliminating chip blockage of the flutes. Break-out tearing at the exit side can be reduced by slowing the drill at the bottom of the hole, or by backing with another material.
|
|
When drilling a series of small holes, inserting a pin in each completed hole prevents the force of the drill from pushing material into adjacent holes and causing subsequent distortion.
Sharp cutting edges will minimize elastic deformation as the chip is formed. Polished flutes should be used to aid in chip clearance and coolant is required for good drilling performance. The rake angle should be reduced to 0 degree or negative angle and a generous lip clearance, (approximately 16 degrees) provided for proper relief.
The point angle is governed by the final wall thickness. Sharp points of 90 to 110 degrees are best for heavy walls and large diameters, while blunt angles of 115 to 130 degrees are better for thin walls. Close tolerances call for feed ranges of 0.004 to 0.006 ipr. Feed rate of 0.015 ipr can be used where tolerances permit.
Figure 6. TOOL FOR DRILLING
|
Machining of Polyurethanes: Safety Considerations
When performing any machining or other secondary operations on urethane, we recommend that all appropriate safety equipment as well as personal protective devices be utilized at all times. To fully address all of the safety issues applicable to a machine shop is beyond the scope of this paper. Good judgement and a thorough understanding of machining procedures is essential.
|
|
Eye protection should consist of approved safety glasses with side shields or full goggles. A full face shield is recommended whenever chip pieces or workpieces could fly out and strike the operator in the face.
In our coverage of fixturing and chucking or workpieces, we said too much hold pressure can distort the urethane and cause machining errors. Fixturing is an extremely important aspect of machining urethane. Never attempt to start machining until you are positive that the fixturing is safe and secure. Improper fixturing during plunge cuts and contouring can cause the workpiece to come out of the machine and injure the operator or a bystander.
Loose machine parts, handles, hand tools, etc. should not be left on or near a machine during operations. If a ribbon-type urethane chip wraps back around the workpiece, these loose items can be caught or thrown and cause a serous injury.
CAUTION ! Excessive heat can be generated by improper machining practices. If smoke is generated by machining, the method must be immediately corrected. DO NOT inhale the smoke or grinding dust from urethane or any elastomer.
When grinding or sanding urethane and generating dust, a dust collector should be utilized. If this is not possible, the operator should properly don and wear an approved dust mask and be sure that a good face seal is achieved.
|
|
Information courtesy of
Polyurethane Products Corporation
|
|
|
|
|
|
|
|
|
|
|
SEND ME MORE POLYURETHANE INFORMATION
|
