O-RING GROOVE IN STEEL PLATE

As long as you don't overdo it with chip load, it should be fine. Turn the profit (feed) knob down if in doubt.

Later, Charlie

seems a bit fast, thats a 116 surface feed, chipload seems to be ok at .0007 per tooth (on an 8 flute) Is it carbide tipped? if its just HSS, I would back the SF down to 70-80, and maybe start with a .0005 chip load per tooth and listen to it..

Randy, Looks OK to me, I've done similar without a problem.

Best, Steve

M42 Cobalt MSC #40607053 6 flute

just got it, shank necks down to 0.125" looks real skinny!

I'm at 116 SFM, 0.0010" FPT maybe I will back it down, with the flood coolant I won't hear anthing.

Thank You, Randy

Remove 333 from email address to reply.

Randy:

This is probably too late, but if it's an unusual operation on a one off, that CAN'T be screwed up, I try to test the operation in a piece of scrap material that has the the same or "worse" machinability rating. That way it limits those "Opps" surprises.

Then slow the hell down. personally I'd run fast as hell and take lite cuts. But if breaking your tool is more important than wasting 50-75 bucks an hour in shop labor, do it old school. Real slow rpm, real slow feed, large cut, and sulfur based cutting oil. I wouldn't spiral either. Give a leadin with a slow feed, and increase it when it starts the circle. I like your feedrates and rpm, but if breaking the tool is the most important, go sloooow. Maybe 3 or 400 rpm, and 1 or 2 inches per minute. and hand brush on the stinky black oil.

Don't forget that chip load may be based on center of cutter path, not the actual diameter of your groove. If'n I only had one tool, I'd do it twice, once to .515 dia., and then again to .625 dia.

Thank you for all the replies and advice, it worked. I did hear the cut, sounded like chips were being recut, I could not get a good angle on the coolant to wash them out. Started at 1018 RPM and 4.89 IPM, I ended up at 1018RPM and 2.50 IPM. ( feed at 60%) Works out to 100 SFM and .0004" fpt.

As for starting on a scrap peice I wasn't really worried about scraping a peice of CRS, I was worried about breaking the $40.00 tool.

Thanks again.

Thank You, Randy

Remove 333 from email address to reply.

Glad to hear it all worked out :)

Tom

your feed is probably way too fast unless you are using g41--with straight g2 /g3 you need to remember to calculate feed from the tool diameter not from centerline.