|
Large flange undercut |
I remember when I was machining; I used to get in an
argument with a fellow machinist about metal removal rates on a lathe verses a
mill. He would argue that his milling cutter had 10 inserts. I would come back
saying that I had 100 horsepower and my insert was always in the material.
If you think about it… there are advantages to running more
than a single insert. Applying this concept to a lathe in turning mode can
increase productivity especially on grooves.
Lets think about the difficult situation where the underside
of a flange has to be cut from solid material. You have only got two choices: You
can plunge out the material with the widest grooving tool your machine can
handle or use two opposing tools, one for the topside of the groove and then
changing to a reverse tool to do the bottom side of the groove. The first
option is slow and very noisy because of chatter. Every one in your shop will
run for earplugs. The 2nd option is inferior because it has to take
tiny cuts due to how far the tools are sticking out from the tool post
I’ve tried and tested every possibility known to man to
solve this problem and then I read about chip thinning theory and had a
engineering brainstorm. Button cutters exhibit chip thinning around .03 depth of cut.
What does this have to do with anything?
For the same reason on a mill you can extend a high feed cutter out 7 times
it’s diameter and still run 200 inches per minute. The cutting force is
transferred axially, through the spindle instead of side-to-side reducing
vibration and deflection during the cut.
In reality, we have to stick out our button cutter or prune
tool as it is called on a lathe much farther than 7 times it’s cutting diameter
We need further stiffening. You can only weld supporting steel to the cutter as
wide as the cutter itself otherwise it will obstruct the cut. Since our prune
tool holds a 3/8 button this does not allow for much backing or support.
What if we support our tool with another tool? Now we have
to tools welded together with a ½” gusset in between supporting each other. A
1-½ inch wide double button cutter composed of two 3/8” button prune tool on
each side with a supporting ½” spacer in the middle. Be sure to leave at least
a one inch gap before the button inserts, not extending the support in the
middle past this point.
There is more than extra support that is gained by welding
these tools together. Now every pass that is taken in the Z-axis to remove
material gets to travel 1 ½” less than the groove width. When I explain the
path this tool travels to cut you will see that this is a big savings in time
when converted to inches per minute.
We all know that high feed mills travel at incredible feed
rates. Since this tool follows the same principle it to will travel very fast up
and down. So fast in it will scare the most hardy of operators and pile up
chips like no other groover.
Begin feeding this tool in at an angle. Always keeping .03
depth of cut. On a lathe this equates to .06 in diameter. This is accomplished
by zigzagging up and down. Always moving in. A problem arises when you get to
more than a ¼ depth of the button inserts. The tool no longer is chip thinning
and begins to cut a very wise chip. At this point you will have to slow down
the Z-axis feed .05 before it reaches the corner and then kick it back up when
you change directions.
G01 Z-11.0 X49.0 F.11
G01 Z-11.05 F.020
G01 Z-5.05 X48.94 F.11
G01 Z-5.0 F.02
…
Yes, that is inches per revolution. Rock and roll baby. Let
the chips fly.
|
Large machined groove |