What's new
What's new

What are the best end-mills???

snowshooze

Stainless
Joined
Sep 15, 2010
Location
Anchorage, Alaska, USA
Hi guys;
I have been having pretty good luck with Imco,Iscar and the Aluma-Power.
But, my software puts out speeds like 700 SFPM in 1018 steel...
I'm look at that and say to myself...
They haven't bought the end mills I have.
I usually rough at 250 and finish at 300.
Good end mill life.
Maybe it is just the idiots writing that crap, I dunno.
But, if I actually could run that hard in the Fadal 4020 or the Haas TM...
It would be a kick.
Thanks again!
Mark
 
TM with or without an enclosure? I can't speak to the rigidity. I only once used an open TM-2 and the mess was more the limit than RPM or feeds.

Yes, 1018 will (and needs to) cut at much higher speeds. Just looked at the Haas online catalog. Standard 1/2" 4-flute end mill, side cutting in steel, 390-520 SFPM, 0.003" per tooth.

A VF would run that all day. The TM might protest because of rigidity. That I don't know. Can't speak to the Fadal.
 
Is the software saying 700 SFM for a finish pass? I could believe that.

I tend to rough somewhere in the 250-300 range like you said (WARNING - PROTOTYPE SHOP. My speeds and feeds are likely not "competitive").

A 4020 has plenty of backbone for a machine its size...What sizes of cut are you taking? Any full slots?
 
Is the software saying 700 SFM for a finish pass? I could believe that.

I tend to rough somewhere in the 250-300 range like you said (WARNING - PROTOTYPE SHOP. My speeds and feeds are likely not "competitive").

A 4020 has plenty of backbone for a machine its size...What sizes of cut are you taking? Any full slots?
Everything. All the time.
Job shop. All materials.
Anything for a buck.
I haven't made a 700 SFPM cut in my life, unless it was an accident.
Oh, maybe in Aluminum...
Software recommends 600 SFM on a 1/2" 4 Fl, with a .002" chip per tooth.
That is 1/4" D.O.C. On the rough.
 
Last edited:
TM with or without an enclosure? I can't speak to the rigidity. I only once used an open TM-2 and the mess was more the limit than RPM or feeds.

Yes, 1018 will (and needs to) cut at much higher speeds. Just looked at the Haas online catalog. Standard 1/2" 4-flute end mill, side cutting in steel, 390-520 SFPM, 0.003" per tooth.

A VF would run that all day. The TM might protest because of rigidity. That I don't know. Can't speak to the Fadal.
What the catalog says is a sales pitch,
They are selling machines.
Machinists', they are not.
Open TM.
Don't give a damn about the mess.
That problem is for the helper.
 
I've never been able to get away with that SFM except for light finishing on something like 1018. I'm generally more like 250 for heavy roughing, 350-400 for finishing.
Exactly. Based on the real-world.
But, I always wondered where they came up with that insanity.
I am now fairly satisfied that I ain't missin' much.
 
Hi guys;
I have been having pretty good luck with Imco,Iscar and the Aluma-Power.
But, my software puts out speeds like 700 SFPM in 1018 steel...
I'm look at that and say to myself...
They haven't bought the end mills I have.
I usually rough at 250 and finish at 300.
Good end mill life.
Maybe it is just the idiots writing that crap, I dunno.
But, if I actually could run that hard in the Fadal 4020 or the Haas TM...
It would be a kick.
Thanks again!
Mark
My 2008 vf2 in 1018steel.
2006 Tm-1 I had to go a lot lighter, lost too much torque at high rpm.

 
Wow!
Dogly dog, kicking ass.
I'd like to see the code on that one.
But I fear sparks.
That is goddamn amazing.
That's been the state of the industry for a long time (2015 or earlier?). This is why all of us need to go to trade shows or at very least watch YouTube videos. What are you using for CAM?

 
Bobcad V-32 and am having to work at it to try to transition to Fusion 360...
Not sure how much you understand about those cutter paths but, this is the basics if that's new to you. It goes by a bunch of names but, what it's doing is trying to always keep the cutter engaged the same amount.

In normal offset tool paths, a cutter going into a pocket corner will go from say 20% of the cutter engaged to 80% when it hits the wall. It's that screech every time the cutter goes into another corner. We program all the straights so that the end mill doesn't overload and snap in the corners.

What all the zigzagging of a constant-engagement path does is picks how far it's going to cut radially. Lets say 15% of the cutter diameter. It then tries to break up all the moves so the cutter never exceeds that engagement limit. By taking pass after pass, over the same area, it's able to never overload the cutter. The sound of the cut is usually one, single tone, all the time. It peels off those layers until it gets to the final dimensions of the part, then runs one continual finish pass around the periphery and it's done.

It's great for less rigid machines, makes use of more of the side of the cutter and cuts cycle time in most cases. Fusion 360 does have those style cutter paths so you have what you need. Sorry, I'm not up on Fusion so I can't point directly to how to do it.

 
1018 I could believe that speed. I set all my endmills to rough out 4340 at 500SFM, but these are on dual contact 50 taper machines that you could put your little dinky TM machine in and turn it into chips.

From the tests I've done for the price, MA Ford and Niagara can't be beat for pushing an endmill hard.
 
A good endmill will last a while in 1018 at 700sfm at 10-15% stepover.
I ran a 3/8 Kennametal Harvi I dry in A2 at 800sfm for over an hour cutting time. Sounded terrible by the end, but still looked good.
A 3/4 Kennametal 5 fl spent 20min in 1018 at 900sfm, .080" WOC, 1.5" doc, .008"/tooth, ~21hp cut.
Chips came out straw coloured, and the endmill looks new.
 
I run steel in semi-convetional cutting mode at 180m/s, about 540sfm, and about 30% higher in HSM mode with 10% radial DOC. So it is 500-750 sfm range for non alloyed steel, like s355/1045
However ramping in is 2/3 of rpm and 1/2 of chipload of normal cut, saves on square endmill flute tips, no sparks
 
multiple factors to calculate that. 3.82 x recommended sfm / dia. of EM = RPM, but if carbide x2-ish.. plus the horsepower of your machine spindle and rigidity. so on a fadal i'd say use the formula above and minus about 30% and see how it does. i'd start at 200sfm in that formula and tweak the override knobs. as for feed rate depending on your flutes, you would take your first initial above formula RPM x number of flutes x .003(usually .003 is fine)
 








 
Back
Top