Ball End Mills - Dynamic SFPM/IPM

[M30]

I did a search but could not find the answer to my potentially noobish milling question:

I think I understand pretty well how to calculate rpm based on a target cutting speed and tool diameter. Calculating feed rate based on chip load, inserts and rpm is even easier. Now I am pondering how to deal with situations where a square end mill is not assumed.

It seems to me that the rpm or feed rate need to be adjusted dynamically when using a ball end mill due to a varying diameter. A ball end mill would require different speeds when cutting at the tip compared to cutting on the outside radius in order to keep a consistent SFPM. You could just assume the speeds for the outside radius for all points on the ball end mill, but this would be sub optimal during 3D surfacing.

I'm gearing up to do more complex surfacing with a ball end mills. Do CAM packages (I'm using MC X2) take this in to account? Should I expect varying changes in RPM and feed rate while contouring a surface?

Lastly, out of curiosity, does anyone do this when hand coding NC programs?

Thanks!

[RICHARD ZASTROW]

M30, Just to mess up your mind, google sturz milling. This is used a lot for airfoil and turbo wheels / blades.

This can cause hair fallout.

[mc_n_g]

You should considerer that after getting experience under your belt but that takes time. When you can do that type of calculation in your head let us know!
Yes there are packages out there that do that for you. $$$$ The idea is you keep the chip load constant throughout the cut so feed rate changes constantly. The cuts are more curve like and almost no straight lines. really cool to see in action. The cuts are in such a way that the load is constant to include the corners (no squealling). The step over rate varies tremendouly along with the feed rate. You end up with a bunch of little segment making arcs at different feedrates.
Take a look at:
http://www.surfware.com/default.asp?contentID=1
and http://www.surfware.com/default.asp?contentID=690
and http://www.surfware.com/default.asp?contentID=553
to get an idea.
Nice to have but most shops let alone people can afford it.

I am in no way affiliated with Surfware. I am just a hobbyist who likes to dream.

mc_n_g

[blowmebigtime]

You assume correct with having to recalculate your speeds and feeds with a ball. With a .25 ball taking finish pass of only .005 stock, your cutting dia is only .070" this MUST be taken into account if your going to do any sort of nice finishing work,, also for your tool life. One other very important factor is the feed rate, there is a term called chip thinning factor. This means if you program .001 chip load per tooth and you are only taking that same .005 stock off, you have no where near the correct feed. For a .25 dia ball endmill you would have to multiply your chip load by 3.6 to get your feed rate adjustment ( there are alot of charts for this, dapra makes a good one) For example when I do high speed machining to finish a mold made out of H-13 (50-52 RC.) I would leave about .005 for my finish pass, assuming I am finishing with a .25 dia ball, I would be using about 400 SFPM. Take 400 x 3.8=1520/ .07 (actual CUTTING dia.) = 21710 rpm's x .001 chip load x 2 (two flute ball) x feed rate adjustment (3.6) . = 157" feed rate.. PS. I always leave one percent of my cutter for the finish pass.. for example if I know I am finishing with a .250 dia ball, I will leave .0025 stock.. to take off on my finish pass.