Carbide end mill speed

[deverett]

I have recently come by a 40mm (1-1/2") diameter carbide insert shell end mill. It takes 6 AXGT inserts and I am running it on an X3 sized mill, but not too successfully. The cutter is held in an ER32 collet. The mill is in tram. One of the problems that is not possible to overcome is the fact that the tip cutting edges are about 3" below the spindle nose so there is probably some flexing going on.

Is the mill sturdy enough to run this type of cutter? If it is, what speed should I be running it at? I am cutting mild steel and iron castings with it.

Up to now I have tried speeds between 1000 - 1600 rpm with 25 thou depth of cut, but get a lot of chatter. Drive motor is 2 hp and I could turn faster if required. I have also tried varying the feed rate, but that doesn't seem to make much difference.

Dave
The Emerald Isle

 

[TarheelTom]

I'm not an expert on X3 sized mills, but I'm guessing that it's not sturdy enough.

My experience with cutting cast iron is that you need to cut it dry, and the slowest possible rpms. I don't cut enough steel to give any hints.

Tom

 

[xpylonracer]

Hi Dave

Have you tried a much lower spindle speed with more depth of cut but slower feed rate ? 1000 rpm with a 3" cutter in steel or cast iron seems a bit fast to me.

Rgds, Emgee

 

[Jasonb]

Dave, I've got a 40mm MT3 one that I use in my X3 and would not run it anywhere near that fast, can't say exactly what I run but its the high ratio and maybe quater turn of the dial so around 500rpm and just adjust it to what the machine sounds happy with

I don't use it that much but it is handy for castings when you don't know if there are any hard spots lurking, on steel, alloy and brass I find a fly cutter with HSS bit works better.

J

 

[rake60]

I'd say you are running it a bit too fast.

For steel I run carbide at 300 SFPM

There's a simple formula to calculate the RPM required to get any given SFPM.

RPM = (SFPM X 3.82) / Part Diameter OR Tool Diameter
In this case:
(300 X 3.82) / 1.5 = 764 RPM

If the material is steel I'd start at 750 RPM.
For brass or aluminum I'd multiply that speed by 1.25
Cast iron can be very abrasive to carbide. I'd rough it around 200 SFPM
and light finish cuts at 300 SFPM.

It's just a starting point.
The machine and material will tell you which way to go from there.

Rick

 

[deverett]

Thanks for all the replies. I always thought that carbide had to be spun fast, hence my thinking of the high revs. I'll try much lower rpms and increase the feed rate and see what that does.

Thanks for the formula, Rick. I remember seeing something like that in the dim distant past. Should have made a note of it at the time!

I have been using a flycutter up to now, but thought the shell mill would remove stock faster.

Dave
The Emerald Isle

 

[kvom]

I plugged the numbers into the G-wizard F&S calculator for a full width facing cut .02" deep. A moderate conservative result is 681 RPM @ 18 in/min feed. This is a .38HP cut. A .01 DOC has the same RPM and uses .19HP. 267 SFM.

 

[deverett]

Interesting result, kvom.

Next question. How does the number of tips affect the speed. So, for example a 1-1/2" flycutter with one tip and my 6 insert 1-1/2" shell mill.
We have now established that I should be running my 6 insert mill at about 700 rpm. What speed would a flycutter be run with a carbide tip? And by interpolation a 3 tip cutter should run at a speed halfway between the first two, I guess.

Dave
The Emerald Isle

 

[kvom]

Inserts are like flutes, so more means faster feed possible. With 4 flutes and everything else the same feed is 12 ipm. So feed is directly proportional to # of inserts. Not surprising as this means chipload per insert remains the same.

 

[deverett]

Thanks for that kvom.
As you explain, it makes sense to up the feed rate, so does the rotational speed remain the same for both type of cutter?

Dave
The Emerald Isle

 

[kvom]

RPM and thus SFM is the same for the same diameter cutter.

 

[deverett]

OK got it now, thanks kvom. Had a mental block, which is becoming more frequent these days!

Dave
The Emerald Isle