Cutter Question

[Namliek_J@TheeCircle™]

I am running a part in my HAAS VF-4. I am using a 3/4 ball end mill. Before I was using a 2 flute HSS endmill, but I have just changed to a TIN Coated Carbide 4 Flute Ball Endmill. With the 2 flute HSS I was running 1000 RPM and 6.0 IPM. When I run the same feedrate with my new 4 flute coated carbide, it chatters and squeals like a pig. My depth of cut is .2 inches. Any suggestions on how to stop the squealing? Am I trying to cut to much depth?? Any help?

[Psychomill]

First of all, what material are you cutting? and what type of cutting are you doing (pocketing, slotting, contour, 3D something?)?

 

About the tool, if you just plug it in and run the same rates, with the 4flute you cut the FPT in half. This can cause some chatter since your chip load is alot lighter now. Some other issue,... did the helix angles change? Chip clearance may be an issue now as well since the end gash ( from a 2fl to a 4fl) is alot tighter. This can be a problem (particularly in slotting or pocketing) in say Aluminum and such.

 

[Bill]

the chip load has been cut in half. I would double the feedrate and see what sounds that makes...

 

But that's just me. 6.0 IPM is purdy darn slow.

[Namliek_J@TheeCircle™]

I am cutting steel that has a little bit of lead in it 12L15 to be exact. I am doing a simple contour through the part to put a slot on the outside of a cylinder. I am doing this on a 4th axis. The helix angles have stayed the same I believe. I think the problem is that I have lightened the chip load and the cutter is not cutting right. I think I should slow my RPM down from 1000 to around 600. Does this sound right?

[robk]

+1 Psycho & Bill

You need to change your SFM & FPT. What are you cutting? If going too slow (like you are now) you will just burn the coating off.

For example this is where I would start if running in stainless; 200 SFM @ .004 FPT & that equals to 1019 RPM & 16 IPM. That is only a starting point and it is very conservative IMO.

[Namliek_J@TheeCircle™]

Like BillH said, if i double the feed rate, this would be the same thing as slowing the rpm

[robk]

Sorry, but I don't have experience with that steel.

The little bit of squealing could be the tool breaking in also (unless it's shot already).

[Tim Simmermon]

Don't slow your RPM down. You will burn up your cutter. Actually you need to increase your SFM (because it's carbide) and still increase your chipload. Chipload is only half of the equation. You need the correct SFM if you want any tool life. Rob's chipload is good, but start with a higher SFM (300 - 400). Then leave the RPM alone and play with the feed until you get ridd of the chatter. Faster feed usually gets rid of chatter.

[Namliek_J@TheeCircle™]

Thanks for all the info.

[ToolMan184]

You should be somewhere around 2500 rpm and about 30 ipm on feed. That steel cuts like butter with the lead in it. Open her up and let her cut.