Milling a groove in aluminum with a 1/16" end mill

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?
Reply to
oldjag
Loading thread data ...

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."

Reply to
Bob La Londe

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.

formatting link
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

Reply to
Wes

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

Reply to
Steve Lusardi

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

Reply to
Jon Elson

Re: 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.
Reply to
oldjag

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.