Which end-mill to use ???

[patrickb]

Hi everyone, this is my first question on this forum.

I need a tough end-mill to cut 1018, 4140 steel,
no more than 30 rc.

It will be for slotting, I want to use either 1/2" to 3/4 dia. end-mill
with at least .300" DOC.

I'm presently using Niagara cardide rougher elite series end-mill (TIALN)
they cut very well, no noise,
but they don't last long enought for me, that is when following the
company feed and speed. 225 to 300 sfm, .0015-.002"/tooth.

The tool will be use on a rigid 3 and 5 axes milling.

Any advice would be appreciate.

Pat

[mrainey]

What kind of failure do you see, wear or chipping? How are you starting the slots, with a drilled hole, plunging, or ramping in?

Chip recutting can kill a carbide end mill pretty fast. A strong air blast or coolant flow will help prevent it.

[patrickb]

I start the slot outside the material,

I see chipping on the end-mill but I have a good high pressure
coolant on it, may be I can redirect the coolant to improve the
evacuation of the chip. I didn't bother too much about that, but
I will now and you have a good point about chip recutting.

May be I'm asking too much from the end-mill, may be I can't
do better.

Thanks mrainey

[HuFlungDung]

Pat,
That depth of cut and chipload sounds a bit 'old-school', such as one would use for HSS tooling. You did not specify how deep you were cutting, but if the tool eventually gets buried pretty deep, then the coolant simply cannot get to the flutes consistently, and then the danger of thermal shock to the carbide is greater. Air might be better for chip removal and easier on the carbide in that type of operation.

Probably, it might be recommended to try cutting only .1" DOC and at a chipload of .005"/tooth at 400 SFM when cutting full width of the tool. The job will be completed at least as quickly as before, and the likelihood of a catastrophic tool failure occurring should decrease. Thicker chip will carry the heat out, the tool will rub a lot less, and the shallower depth of cut will be easier to get the chips out on every pass.

[DareBee]

That is a great endmill and should last a long time.
Removing chips is very important.
If you are getting chipping your SFM is too low.
Increase your rpm a bit.
Although IMO your chipload is half what I figure it should be.

[patrickb]

Thanks guys, the chip looks like "steel wool" is that ok ?

Here's the company spec : http://www.niagaracutter.com/techinf...medcarbst.html

[DareBee]

[QUOTE=patrickb]Thanks guys, the chip looks like "steel wool" is that ok ? [QUOTE]

Yes.

Here is a link to Ultra Tool's problem solver.
Cutter chipping shouldn't happen if things are running correct, hope this helps.

http://www.speedsandfeeds.com/PDF%20...cationtips.pdf

[tobyaxis]

Correct my spelling, but a Hanieta Very Flute is an excellent tool. It's a 4 flute set at 80 degrees and 100 degrees. I use a 1/2 4 flute in just about every exotic material, and they cut great. Zcarb from OSG seems to be on the same level, but I haven't tried them on my mill yet.

Hope this helps

BTW: Cool site Darebee

tobyaxis

[nitrosnfr]

A good mill insert that I have found for good tool life and able to handle any steel is made by Iscar Multimaster.

One paticular I use to mill out a 3.5" radius in 4340 pre hard.Run it at 1500rpm and feed it at 20.0 IPM at .100 doc.this one awsome for what I am running.I also run it dry no coolant or air blast.Have done about 30 or so parts on one insert.

[DareBee]

Thanks Toby