can an endmill cut longer than it's cutting length using multipass

[parkson]

Im trying to cut a 2in bar of aluminum in the VMC.
I am rounding the corners w/ a 3/4in dia, 3in cutting length endmill
I am getting chatter w/ any feedrate faster than 5ipm
Spindle is 1000rpm

Can I use a 3/4in dia but with a 3/4in cutting lenght for better rigidity and cut the bar using multipasses? Or will the sides of the endmill rub when I cut passed the 3/4in mark?

-Park

[HuFlungDung]

Yes, the shank of the endmill will rub unless you can grind it slightly undersize between where the flutes and and the chucking surface of the shank begins. If you have no facility to do this, you can carefully grind this 'neck' with an angle grinder or something, while the tool is running slowly in the spindle. Move the tool out of the holder a little so you don't mark the holder. Clean up the dust afterwards, and clean the toolholder too.

You don't have to radically undersize the tool, a couple of thousandths will suffice.

[Jason S]

Im trying to cut a 2in bar of aluminum in the VMC.
I am rounding the corners w/ a 3/4in dia, 3in cutting length endmill
I am getting chatter w/ any feedrate faster than 5ipm
Spindle is 1000rpm

Can I use a 3/4in dia but with a 3/4in cutting lenght for better rigidity and cut the bar using multipasses? Or will the sides of the endmill rub when I cut passed the 3/4in mark?

-Park

Try leaving .005 for a finish pass or a spring pass at a slightly faster feedrate.

[chuck5121]

Make sure you are Climb cutting, Leave .005 to .010 for a clean up pass, reducing the neck of the End Mill is a common practice you can use a Bench grinder, Angle grinder or a Cylindrical grinder. Good luck

[little bubba]

For chatter on something like that, toss the convention of slowing it down and taking a smaller finish out the window. Leave more stock for your finish, and feed it harder, leave yourself maybe .025-.030 and feed at .0025-.004 per tooth. Giving the endmill something to do(actually cut) won't let it chatter.

Back to the original question, yes you can, I do it a lot, even though your not supposed to. It kills your finish where the shank rubs. I'd never do it on a part that actually had to be tight on tolerance, or "shiny", then I'll either relieve the shank a bit (which relegates that endmill to that length of cut or longer for life) or Maritool has these cool little guys that are relieved about .005-.010 for the length of the shank so you can hang out as much or little as you need to. I keep a few of these guys on hand also.

http://www.maritool.com/Cutting-Tool...219/index.html

Harvey tool has basically the same thing, but they are relieved back to the next fractional size and are about 5 times the price and as far as the 4 flutes aren't variflutes/helix.