Feature Article
Tips For Better Boring
This set of step-by-step guidelines will help you establish optimal
speeds and feeds for boring operations. The underlying principles
are simple but sound.
By Klaus Lohner
Vice President, Engineering and Sales
BIG Kaiser
Precision Tooling, Inc.
Elk Grove Village, Illinois
In boring operations,
it is important to obtain optimum free cutting conditions; that is,
to run the boring bars at the highest possible speed and to keep the
feed rates on the moderate side. In many cases, especially in new
boring applications, little may be known about the characteristics
of the material or the behavior of the machine.
Proven Steps
The proven way to obtain optimum cutting conditions can be outlined
in the following steps:
1. Make a
preliminary speed selection.
Considering
the material specification, select a speed that allows you to cut
the material without buildup on the cutting edge and without undue
tool wear. You can either consult your carbide manufacturer's instructions,
or use a machining data handbook such as the one published by Metcut
Research Associates. Speeds suggested by carbide manufacturers tend
to run high, so I would start with about 70 percent of their recommended
cutting speed.
When using
triple-coated carbide inserts for steel, you should not go below
450 sfpm. For cast iron, stay within 400 to 450 sfpm, and for aluminum,
start out at about 800 sfpm. In other words, select a speed at which
you obtain safe cutting operation without undue overload, vibrations
or tool wear.
2. Select
a chip load in inches per revolution.
All carbide inserts have an acceptable range with regard to chip
load. For roughing operations, most inserts will start breaking
steel chips from about 0.007 ipr and up. By selecting starting speeds
and feed rates according to these recommendations, you normally
will get reasonable initial cutting conditions.
3. Check
the projection ratio of your boring bar.
In other
words, divide the total bore depth of your tool by the largest boring
bar diameter at the root of the tool. If the ratio obtained is within
4:1, you will virtually never have to worry about vibration or chatter.
If the ratio is 5:1 or greater, you may have to reduce your cutting
speeds progressively to avoid chatter.
 |
| Boring is a critical operation
for many shops, as it is a Bachman Tool & Die in Independence,
Iowa, where this cast-iron arm for a large printing press is
machined on a vertical machining center. By following the principles
for optimum boring performance, bores on this workpiece are
completed with maximum efficiency. |
4. Take a trial cut.
After establishing
steps one, two and three, take a trial cut. Listen to the sound
of the machining. The smoother the noise the better. Look at your
chips. If you get long, curling chips, you must increase your feed
rate. If you get chips that look like corrugated iron, then the
feed rate is too high. The ideal chip form is short Cs, as shown
in Figure 1.
I recommend
using coolant from the beginning, whenever possible. Please remember,
however, if you use coolant, use it with high pressure and high
volume. Don't just splash a little bit of coolant onto the cutting
edge, as this will unfailingly lead to thermal cracks.
Before you
change speed, adjust the chip load accordingly to maintain optimal
chip forms. You can also check the point where the chip makes contact
with the chip groove. If that wear mark is about half-way down the
chip groove, you have selected a good feed rate; if the wear mark
is close to the cutting edge, you will get cratering and premature
failure of the cutting edge. If the chip makes contact beyond the
deepest point of the chip groove, then you have to reduce the feed
rate.
 |
Fig. 1 - When the chips produced
by a boring tool look like these short Cs, the feed rate during
the test cut is just about right.
|
Another way
to verify optimal cutting conditions is to observe the return spiral
made by the inserts. When free cutting conditions are achieved,
the spiral lines on the return groove will be virtually invisible.
If these grooves are very deep, then you are overfeeding the tool
and probably not running fast enough.
Once you
have made a preliminary speed selection, selected a chip load in
inches per revolution, checked the projection ratio of your boring
bar, and made the trial cut, proceed to the next step.
5. Optimize
cutting speeds.
After consulting
your load meter, listening to the chip formation and looking at
the surface finish obtained, you may want to increase your cutting
speed. For safety's sake, do this in steps of about ten percent
each. For steel, especially low-carbon steels, higher cutting speeds
lead to better cutting conditions. Ideally, the heat created by
the cutting action should be carried away by the chip so that the
cutting edge and the workpiece remain cool.
It now becomes
important to watch very carefully for tool wear. If premature tool
wear is visible, you may have to change cutting speed or chip load.
This step can be long and drawn out because it takes quite a bit
of experience to find the optimal speed.
6. Watch
insert wearing in.
It is important
to observe how an insert is wearing in. In the first phase, the
cutting edge will wear relatively fast, and diameter adjustments
on the first workpieces may have to be made frequently. Over the
long, middle phase, the insert should remain stable, wearing down
only gradually, so that adjustments for diameter need to be made
less frequently. At the end of the useful tool life, the insert
will wear down rapidly. It is, therefore, important to watch for
that critical point and to change the insert promptly.
General Guidelines
Now, here
is a list of some general guidelines to follow on speeds and feed
rates that we have drawn from our experience:
- As a rule
of thumb, boring operations in steel require approximately one
horsepower per cubic inch of chip per minute. This rule should
allow you to make sure that your machine has enough horsepower.
If you do not have enough horsepower, you may have to slow down
your speed, or better yet, change from balanced cutting to stepped
cutting.
- In low-carbon
structural steels, the ordinary triple-coated inserts allow speeds
between 600 and 750 sfpm and chip loads starting at about 0.007
inch per cutting edge, running up to over 15 thousandths per cutting
edge for larger inserts. For finishing, we recommend Cermet inserts.
These inserts permit speeds of 800 sfpm or more with a chip load
as small as 0.002 inch per cutting edge. For finishing, the chip
form is critical. When you have a small depth of cut, chips breaking
in short Cs may not be possible. What can be achieved with the
right insert is to get half-inch long, small, spring-like curls
that can be easily evacuated.
- For medium
carbon steels, alloyed or not alloyed, we recommend starting with
a normal triple-coated insert at about 550 sfpm; chip loads should
be between 0.007 and 0.009 inch per revolution and cutting edge.
- For higher
strength steel, we recommend consulting the manufacturer's or
supplier's recommendations for that material before starting to
machine.
- For aluminum,
the usual limitation in speed is the maximum rpm of the machine
and the stability of the boring bar, workpiece fixture and machine.
In other words, speeds of 1,000 sfpm and higher are all right.
Generally, when machining aluminum, the higher the speed the better.
For roughing, as a rule, chip loads between 0.010 and 0.020 inch
per cutting edge are recommended. For finishing, the feed rate
is determined by the surface finish that must be attained.
- When interrupted
cuts are encountered, keep the speed up, and reduce depth of cut
and chip load. Following these principles, interrupted cuts can
even be performed with Cermet inserts.
- When machining
a very deep bore, keep your speed moderate, because speed is the
main reason for tool wear. Over a long bore, you can't afford
to lose cutting edge. In addition, let your quill protrude as
far as necessary and feed with the saddle. The boring bar on a
boring mill will hang down. If you feed with the quill, then your
bore will not be straight. Working with the saddle with the boring
bar extended out will eliminate this problem.
 |
At Quality Manufacturing Co.
in Columbus, Ohio, cast aluminum transaxle housings for golf
carts require a tool with total projection of 10.5 inches (top)
to finish two 2.5-inch bores on opposite sides of the hollow
workpiece. They had been running the boring operation on a Cincinnati
Machine T-10 horizontal machining center at a speed of 1800
rpm and a feed rate of 11 ipm. using modular boring tools from
Kaiser - in this case, a twin cutter with modified diamond-tipped
inserts (bottom) they are now running at 6,000 rpm and 40 ipm.
|
 |
Basic Principles
In summary,
keep these guiding principles in mind when establishing speeds and
feed rates for boring:
1. Never
change feed and speed in the same step; that can lead to total confusion.
2. Select
a preliminary speed at which you obtain safe cutting operations
without overload or vibration.
3. Select
a chip load in inches per revolution, permitting C-shaped chip form
or the shortest possible chips.
4. Keep the
projection ratio of your boring bar within 4:1, or as short as possible
5. Make a
trial cut, and optimize the chip form by adjusting the chip load
as necessary.
6. Optimize
the cutting speed, because high cutting speeds usually lead to better
cutting conditions by maintaining the chip load.
7. Use inserts
designed for the lowest possible cutting forces, good chip control,
and unhampered chip evacuation.
8. Pay careful
attention to the way the inserts are wearing in, and change them
before they reach the end of their useful life.
Readily Achievable
Boring tools
seldom amount to more than 10 or 15 percent of all tools involved
in a machining process. But their impact on overall productivity
is much higher. In most cases, precision boring represents one of
the final touches on a workpiece that has accumulated the value
of hours of prior machining. As a consequence, the production of
scrap while finish boring can result in heavy losses.
Therefore,
in both production runs and small-batch jobs, efforts to optimize
boring operations are surely worthwhile. And the best part is, the
principles behind optimum boring are simple and their application
is straightforward. Better boring is readily achievable- don't miss
out. MMS