I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. I have a
0.058" carbide 2 flute end mill. My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". This seems wildly optimistic but I've never worked with end
mills this small before. I'm thinking maybe two passes instead at
0.012" deep with a finish pass 0.004" to clean the floor. The end
mill has a 5/16" max depth of cut so it's fairly stubby. I also have
a 4 flute 0.058" cutter I could use instead. Any comments?

"oldjag" wrote in message
...
I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. I have a
0.058" carbide 2 flute end mill. My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". This seems wildly optimistic but I've never worked with end
mills this small before. I'm thinking maybe two passes instead at
0.012" deep with a finish pass 0.004" to clean the floor. The end
mill has a 5/16" max depth of cut so it's fairly stubby. I also have
a 4 flute 0.058" cutter I could use instead. Any comments?

Yeah right. I run 10,000 RPM on my home CNC mill. I might go for 15.7 IPM
as I cut most everything at 20IPM, but I think I wouldn't try to get more
than about .003 per pass, and more likely .001 or .002 as I would be afraid
of snapping the cutter. And trust me. I have snapped a bunch of cutters.
In 1/16 and smaller a lot more than I have worn out. I think I would also
start several thousandths above the work surface so that an irregularity
doesn't bite you in the dearie aire on the very first pass.. And yes I cut
a fair amount of 6061 T6. I am machining a mold out of .500 thick 6061 T-6
right now.

I tried those feed speed tables and the feed speed calculators, and the
numbers sure don't seem to work for me.

Or as a buddy of mine says... "Push it till you snap a cutter. Then back
it off a little bit."

oldjag wrote:

I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. I have a
0.058" carbide 2 flute end mill. My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". This seems wildly optimistic but I've never worked with end
mills this small before. I'm thinking maybe two passes instead at
0.012" deep with a finish pass 0.004" to clean the floor. The end
mill has a 5/16" max depth of cut so it's fairly stubby. I also have
a 4 flute 0.058" cutter I could use instead. Any comments?

Why did you get an endmill the size of the groove? You don't do that. You use a smaller
diameter endmill and make over lapping passes.

If I'm reading this right, the calculator wants you to take a close to .002 chip with your
end mill? That seems insane.

http://www.practicalmachinist.com/vb...3-64-a-206358/

Go down to message #18 and start reading.

HTH,

Wes
--
"Additionally as a security officer, I carry a gun to protect
government officials but my life isn't worth protecting at home
in their eyes." Dick Anthony Heller

The number one problem in machining is ALWAYS chip removal. Chip bind snaps the cutter, not only tool load. This is especially
important in cutting a groove with an endmill. I always fasten an airgun to the spindle and blast the endmill with compressed air.
It blows the chips everywhere, but it sure works to prevent chip bind.
Steve

"oldjag" wrote in message ...
I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. I have a
0.058" carbide 2 flute end mill. My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". This seems wildly optimistic but I've never worked with end
mills this small before. I'm thinking maybe two passes instead at
0.012" deep with a finish pass 0.004" to clean the floor. The end
mill has a 5/16" max depth of cut so it's fairly stubby. I also have
a 4 flute 0.058" cutter I could use instead. Any comments?

oldjag wrote:
I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. I have a
0.058" carbide 2 flute end mill. My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". This seems wildly optimistic but I've never worked with end
mills this small before. I'm thinking maybe two passes instead at
0.012" deep with a finish pass 0.004" to clean the floor. The end
mill has a 5/16" max depth of cut so it's fairly stubby. I also have
a 4 flute 0.058" cutter I could use instead. Any comments?

I think you can probably get away with it. I would use a smaller end
mill and make three passes, plow the middle of the groove, then climb
milling on the inner and outer face. otherwise, you will get wavy edges
on the sides.

Jon

On Jul 12, 3:19*pm, Jon Elson wrote:
oldjag wrote:
I'd need to cut a 0.058" wide x 0.028" deep circular groove in 6061
aluminum. *The groove is about 1 1/2" diameter and will used as part
of a face type "O" ring gland. *I can only run the spindle on my home
CNC mill to 4500 rpm, so this will limit the feed rate. *I have a
0.058" carbide 2 flute end mill. *My feed calculator shows I can run
this cutter at 15.7 IPM feed or 0.0017" IPT at the full cut depth of
0.028". *This seems wildly optimistic but I've never worked with end
mills this small before. *I'm thinking maybe two passes instead at
0.012" deep with a finish pass *0.004" to clean the floor. *The end
mill has a 5/16" max depth of cut so it's fairly stubby. *I also have
a 4 flute 0.058" cutter I could use instead. *Any comments?

I think you can probably get away with it. *I would use a smaller end
mill and make three passes, plow the middle of the groove, then climb
milling on the inner and outer face. *otherwise, you will get wavy edges
on the sides.

Jon

the smaller end mill, I can increase the groove size to 0.060",
which might help slightly, but I was concerned since this machine is
RPM challenged for a 1/16" end mill anyway, going smaller, to say a
0.030 diameter end mill might actually make the feed rate/chip
clearing situation worse. I guess I'll give the 0.058" 2 flute a try
since and see if it will clear off 0.004 at a time. At least the cut
time won't run to hours. I can leave 0.001" for a climb mill cleanup
on each side of the groove. I was trying to make this groove with a
fly cutter using a boring pass but my fly cutter setup does not seem
to have quite enough rigidity to get a good finish on the groove
bottom. I might go back to the flycutter setup if I can find a source
for pre ground HSS or insert type face grooving tool that will fit one
of my boring heads for this mill. This would be lot faster than the
end mill. For the quantity involved I can't justify spending more
than $150-$250 on tooling.