Putting a value on cutting speed
The
cutting speed of any material is based on the speed of the material
passing over the cutting tool. This speed is measured as SFPM –
surface feet per minute.
The measurement is based on the
circumference size of the part or cutter. The circumference of a
circle is the distance around the periphery. With milling, this is
the peripheral speed of the cutter acting on a stationary workpiece.
With turning, this is the peripheral speed of the workpiece material
acting on a stationary cutting tool.
The speed that the surface of the part or
cutter moves each minute is measured in feet, not inches.
Constant surface speed (CSS) is applied to
cutting tools to provide the correct machining conditions. The use
of a constant surface speed (sfpm) results in a spindle speed being
relative to the part diameter (turning) or to the cutter diameter in
milling.
The correct sfpm values for machining are
available for each particular material type. A first-class machinist
must develop a knowledge of the various sfpm values for each
material type. There are many variables in the choice of the correct
sfpm. Here are factors to consider: material type, rigidity of the
machine, material hardness, type of cutting tool material, coolant
type.
Programming considerations: One of the
major benefits of using a CNC lathe is the G96 command that engages
the constant surface speed mode. The formulas for the correct rpm
for a specific sfpm are easy to calculate:
| rpm
= |
sfpm
x 3.82 |
|
| part
diameter or cutter diameter |
| |
|
| sfpm
= |
rpm
x part diameter or cutter diameter |
|
| 3.82 |
|
|
| rpm
= |
sfpm |
|
| part
diameter or cutter diameter x 0.262 |
|
|
| sfpm
= |
rpm
x part diameter or cutter diameter x 0.262 |
|
A word of caution regarding G50/G92 code: Do not exceed speed. When
you are facing to the centerline of the part, the spindle of a CNC
lathe will attain the maximum possible RPM available on that
machine. There is a standard G code that must be programmed to
prevent accidents. The standard G50/G92 code must be set at a
specific speed prior to the control reading the G96 command for css.
If you are facing on a machine with a 5000-rpm spindle, the machine
will attain that maximum rpm unless you specify a safer, lower
spindle speed.
This must be considered prior to running
the program. We must limit the machine’s maximum speed with a
sensible G50/G92 command prior to running the part. There is a
danger any time a large-diameter part is run or there are any
compromises in the workholding. Excessive rpm can overcome the
chucking force, resulting in the part flying out of the chuck.
Always consider the centrifugal force. Set
the G50/G92 to a safe maximum speed.
When facing to centerline, you will produce
a dull finish at the centerpart of the face. This is caused by the
css reducing as the tool approaches centerline.
You can calculate the diameter that the
machine will attain at the maximum rpm. Once that diameter is
calculated, you can reduce the facing feedrate in an attempt to
improve the surface finish. Use this formula:
|
Diameter
at maximum rpm = |
sfpm
x 3.82 |
|
| Machine
maximum rpm |
Here’s an example: face an 8” diameter part to centerline at 600
sfpm. A g50/G92 command of 2000 has been programmed.
| Starting
rpm at 600 sfpm = |
600
x 3.82 |
|
|
= 279 rpm |
| 8.2 |
|
| |
|
|
| Diameter
at maximum rpm = |
600
x 3.82 |
|
|
= 1.146” diameter |
| 2000 |
|
|
