|
Cutting
speed - using our favorite constant
In
working with machinists over the years I’ve noticed that if you
stand in front of a machine tool and ask about speed, most people
think “speed of the spindle” or rpm. The fact that the spindle
is revolving slowly or quickly does not indicate the value of the cutting
speed. In our CNC training classes, it is my goal to have
student think in terms of sfpm
(surface feet per minute). It is a challenge to get people to
think in terms of sfpm and not rpm. We see many machinists who guess
rpm values and keep on guessing until they get it working. Wouldn’t
it be better to just start out with the correct sfpm?
What is sfpm and how is it calculated? Surface feet per
minute is
just that – the distance (measured in feet) traveled by the
cutting tool each minute. This value is determined by
the
following formula.
sfpm = (rpm x
part or cutter diameter) ÷ 3.82
You can re-arrange the formula and calculate spindle rpm.
rpm = (sfpm x 3.82) ÷ part or cutter diameter
The cutting speed is dependant on the spindle speed and the part (or
cutter) diameter. The other piece of the formula is the constant 3.82.
Remember that the math constant 3.82 is derived from 12 divided by Pi
(π). Recall from school days that Pi (π) is the mathematical
constant that represents the ratio of a circle’s circumference to
its diameter. Pi is used to calculate circumference (formula:
π
x diameter = circumference); so when we calculate the movement of a
circular part or tool, we need Pi. The number 12 is used to
convert the inch value of the part diameter into feet. Remember, we
measure our parts in inches but use feet in cutting speed
calculations.
We encourage machinists to use the 3.82 constant. The above formula is
the most popular, although there is another, which uses the reciprocal
of the 3.82 constant, a value of 0.262.
rpm = sfpm ÷ (part or cutter diameter x .262)
Whichever formula used, calculating rpm from a recommended sfpm is
a
must in machining.
Calculating rpm is easy once you have the sfpm – but where
does the sfpm come from? Selecting an ideal sfpm is a combination of
research and experience.
Research a sfpm by reviewing tooling catalogs. Tool suppliers provide
much information on their products, including recommended cutting
speeds for various materials and cutting conditions. Be aware that
these values are based on a short tool life and may be too aggressive
for many machining applications.
Keep in mind that some tools can be run too slowly. Problems can occur
from running both too fast and too slow. Also review your own
experiences or those of your colleagues or company. Each company deals
differently with certain materials, uses different machine tools,
workholding styles, and cutting tools. All of these can impact the
successful selection of cutting speeds. Using all of this information
you can select good working cutting speeds that should be productive.
Once you’ve selected a sfpm and can calculate the rpm, use the CNC
program to set the values chosen. When turning, boring, and grooving
on a lathe we can
program
a G96 command that sets the cutting speed and allows the machine to
calculate the spindle rpm. |
However, when using tools that are designed to cut on the tool point,
such as center drills, spot drills, twist drills, insert drills, taps,
and reamers, we must calculate a cutting speed for the program. This
is the same situation for all tool types used on machining centers.
For example, we know that a specific sfpm works well on a certain
steel. We’ll use 100sfpm for a HSS drill and 28sfpm for tapping.
These known values can be used in our program and the control
calculates the rpm.
Example: S[100*3.82/.4] (spot drill)
S[100*3.82/.312] (twist drill)
S[28*3.82/.375] (tap)
Programming the spindle speed in this manner encourages everyone to
think in terms of sfpm. Remember, using the correct sfpm results in
better tool life, improved chip control, and more predictable
production efficiency.
Using the sfpm in your program for all tool types has got to beat the
rpm guessing game.
Research a sfpm by reviewing tooling catalogs. Tool suppliers provide
much information on their products, including recommended cutting
speeds for various materials and cutting conditions. Be aware that
these values are based on a short tool life and may be too aggressive
for many machining applications.
Keep in mind that some tools can be run too slowly. Problems can occur
from running both too fast and too slow. Also review your own
experiences or those of your colleagues or company. Each company deals
differently with certain materials, uses different machine tools,
workholding styles, and cutting tools. All of these can impact the
successful selection of cutting speeds. Using all of this information
you can select good working cutting speeds that should be productive.
Once you’ve selected a sfpm and can calculate the rpm, use the CNC
program to set the values chosen. When turning, boring, and grooving
on a lathe we can
program
a G96 command that sets the cutting speed and allows the machine to
calculate the spindle rpm.
However, when using tools that are designed to cut on the tool point,
such as center drills, spot drills, twist drills, insert drills, taps,
and reamers, we must calculate a cutting speed for the program. This
is the same situation for all tool types used on machining centers.
For example, we know that a specific sfpm works well on a certain
steel. We’ll use 100sfpm for a HSS drill and 28sfpm for tapping.
These known values can be used in our program and the control
calculates the rpm.
Example: S[100*3.82/.4] (spot drill)
S[100*3.82/.312] (twist drill)
S[28*3.82/.375] (tap)
Programming the spindle speed in this manner encourages everyone to
think in terms of sfpm. Remember, using the correct sfpm results in
better tool life, improved chip control, and more predictable
production efficiency.
Using
the sfpm in your program for all tool types has got to beat the rpm
guessing game. |
