face mill speed and feed

[dustinwassner]

using my speed and feed formulas, for a face mill that was say 2" from point to point of the carbide cutters and had 4 of them would i be able to plug this in and get correct numbers? I have been away from this for about 2 years and am finding that i have forgotten alot.

[RICHARD ZASTROW]

Does this mean a 2" dia. face mill with 4 cutting teeth? If so you can use the carbide manufacturers feed per tooth X 4 with the recommended surface speed for the material you're milling.

You should also remember to keep at least one tooth engaged at all times and face 3/5 of cutter width. These are general recommendations and there are always exceptions. Of course, these are from my Kennametal class in 1968 LOL

Dick Z

[dustinwassner]

i suppose thats what the dia. would be. the ones i used were 4 insert cutters and when looking at it from the bottom we would measure from one cutter to the one across it from point to point to get the "dia" of the tool to find rpm. is there a way you would know if more than 1 tooth was not engaged at any time? is there a max depth of cut to step over ratio associated with these?

[Pondo]

There are so many variables that it's impossible to give definitive #'s.
A good starting point for a 2" 4-flute face mill in a 40 taper machine is 1000 RPM (500 SFM) and 40 IPM (.012 chipload) and .050-.075 DOC.
That's conservative. Increase the SFM for softer materials, the feed and DOC depending on the rigidity of the machine, the power of the machine, the rigidity of the setup, and the length of the holder.
I run a 2" mill on 4140PH @1000 RPM and 45 IPM, .060 DOC.
Soft CRS @1221 RPM and 80 IPM, .080 DOC.
So it can vary a lot.

[dustinwassner]

what about step over?

[Pondo]

Originally Posted by dustinwassner what about step over?

The more the better. I run 1.5" stepover on a 2" mill whenever possible. If the machine or setup is not rigid and chatter develops, then less. I will go to a smaller dia mill if that happens to me though.

[dustinwassner]

wouldnt you get chatter from just going to the smaller dia? and if you were milling a slot and decided to go 1/3 dia. then couldn't you run a deeper cut? How do people arrive at their radial and axial depths of cut relative to each other and overall? I know there are many variables, but just setting up a normal low carbon steel or common aluminum, how does one arrive at their numbers? deeper cut = less step over? and the opposite?

[Pondo]

There's no need to overthink it. Start at the low end of the recommended speed and chipload and work from there. It's usually on a sticker right on the pack of inserts. For a 2" mill, start at .050 DOC for a basic 40 taper machine and a rigid setup like a vice. Keep the chipload over .010/tooth and increase the feed from there.
There is no formula for figuring it out, there are too many variables. When I am running a lot of 1's and 2's I keep it simple to keep the machine running as much as possible. For a 2", 5 flute face mill in any tool steel I run at 900 RPM, 50 IPM, and .060 DOC regardless of stepover. I only worry about optimizing the toolpaths if it's a multi piece order (20+ parts), a common part that comes thru often, or it needs a lot of stock removed.
As far as the chatter, a smaller diameter has less engagement in the material and works better in a non-rigid situation. Like facing a thin part. Multi stepovers with a smaller dia mill works a ton better than one with a big mill.