Helical High Feed Endmills for Aluminum

[Houdini]

Swiftcarb makes a 5/8 4.5loc 5 flute finisher for aluminum AF0625-5LG00L-S1

Have you tried them?
because I tried one of these, extremely rigid thick core, 5 flute (no bueno too much engagement)
and this thing sucked! and was mad expensive.
IMCO deep finisher

 

[crossthread82]

Have you tried them?
because I tried one of these, extremely rigid thick core, 5 flute (no bueno too much engagement)
and this thing sucked! and was mad expensive.
IMCO deep finisher

I haven't used one quite that long, but I have used a 3/4 3.5loc and it worked great. I wouldn't try to rough with one but swift claims it'll handle a 25% stepover. I typically just use it for full length ~0.010" finish passes.

You're saying the imco sucked?

 

[Machinerer]

Have you tried them?
because I tried one of these, extremely rigid thick core, 5 flute (no bueno too much engagement)
and this thing sucked! and was mad expensive.
IMCO deep finisher

Interesting that they claim that endmill is for.aluminum, yet the coating has aluminum in it.

 

[Houdini]

I haven't used one quite that long, but I have used a 3/4 3.5loc and it worked great. I wouldn't try to rough with one but swift claims it'll handle a 25% stepover. I typically just use it for full length ~0.010" finish passes.

You're saying the imco sucked?

Yeah I compared a standard YG-1 to the EMCO, and the EMCO chattered like crazy.
It is also definitely only a finisher, the chip load rating because of the thick core is small.

 

[Houdini]

Interesting that they claim that endmill is for.aluminum, yet the coating has aluminum in it.

Yeah its the old deal of just labeling something its not designed for, it also has 5 flutes. BS

 

[Garwood]

Wait, am I missing something a 1" 2 flute 1000sfm .01ipt is 3800rpm
I've never ran one of those tools below 8k, usually at max 10-12k though.

4.# hang out on one these in a 1" is kind of flimsy, yes.

I have a 1" 2 flute also, and mine is sticking out like this also, I had to relieve the shank myself.
yeah its not optimal for that length hangout.

I would buy a 1.5" personally, but you didn't mention the pocket size. So I don't know if it can ramp/helix in.

the 1.5" at that length is miles more rigid. actually its what I use for all my roughing, we have one of them for each machine and a couple extra ling ones towards the 4.# length.

Korloy 1.5" build your own kit. You can get one quick from here, cheaper than a Ingersoll, its only a .500 shank tool so make sure you can get a holder that works first.

Be aware folks that try to use these on machines with balls (like HMC's and VMC's with beef) tear the inserts right off the tool. The Korloy Ripper mills are for lighter duty, low power machines.

 

[Houdini]

Be aware folks that try to use these on machines with balls (like HMC's and VMC's with beef) tear the inserts right off the tool. The Korloy Ripper mills are for lighter duty, low power machines.

That's probably why they redesigned them. The ones they have had for years are being replaced Pro-X Mill replaced with Pro-V Mill.

 

[crossthread82]

Be aware folks that try to use these on machines with balls (like HMC's and VMC's with beef) tear the inserts right off the tool. The Korloy Ripper mills are for lighter duty, low power machines.

IMO for aluminum roughing with indexable cutters Mitsubishi is the only way to go. Two screws per insert with studs that fit into cbores in the back of the insert, its not gonna move.

 

[Machinerer]

IMO for aluminum roughing with indexable cutters Mitsubishi is the only way to go. Two screws per insert with studs that fit into cbores in the back of the insert, its not gonna move.

The old Ingersoll Rough-air tools had 2 screws as well, and an axial v-groove in the insert. They only offer a single screw version now. We run the 2" cutter in a lot of parts, and it's been a great tool for us.

The mitsu looks nice too.

 

[Mtndew]

I've NEVER been able to get a decent wall finish, stepping down a wall, so I usually avoid it whenever I can.

Add that to the long list of things I don't know!

Runout is crucial as is the end mill having zero taper. Combine those 2 and you'll get a damn near perfect wall with zero steps.
The best end mill I've used for this is a YG-1 AlumaPower 3 flute necked. That thing is insane.

 

[Mtndew]

IMO for aluminum roughing with indexable cutters Mitsubishi is the only way to go. Two screws per insert with studs that fit into cbores in the back of the insert, its not gonna move.

Agree 100%.
Mitsubishi has been the king of indexables for aluminum as long as I can remember.

 

[Houdini]

Runout is crucial as is the end mill having zero taper. Combine those 2 and you'll get a damn near perfect wall with zero steps.
The best end mill I've used for this is a YG-1 AlumaPower 3 flute necked. That thing is insane.

And actually I would say the opposite, a YG=1 Alu is a polished flute end mill, leaves an awesome mirror finish on the parts.

So if you do a finish pass in steps its far less likely to hide any lines.

I actually stopped using them because any little flaw in the end mill and it starts to leave lines, a non polished is all lines so nothing to worry about.

 

[Mtndew]

So if you do a finish pass in steps its far less likely to hide any lines.

Yes you could see the lines, but you couldn't feel any steps or see any with an indicator.
The machining lines were still visible, those are tough to hide unless you have an end mill with full length flute.

 

[kyleisraaddd]

https://harveyperformance.widen.net/content/aouiv6pj8e/pdf/SF_HFAL-2.pdf

I find it hard to believe that a .750 dia high feed mill at 4.5 stickout, "did not play nice" milling at .0375 depths of cut?? and that's towards the max of their tolerance. if .0375 depth cuts are too harsh they recommend as low as .0225" DOC.

Not saying it would be the most efficient way,... but if I were doing let's say a second op where I'm only holding on to a little bit of the finished op10, I'd go for the high feed mill to do a lot of roughing to ease up on the tool pressure, and lessen the likelihood of tossing the part out of the jaws.

Agree 100%.
Mitsubishi has been the king of indexables for aluminum as long as I can remember.

Soon I'll be tooling up a few machines for a more "permanent" tool library (90 + 330 tool ATCs)
Any recommendations for a mitsu indexable mill for aluminum? probably around .75-1" dia, sort of a "do-it-all" cutter?

 

[Houdini]

Soon I'll be tooling up a few machines for a more "permanent" tool library (90 + 330 tool ATCs)
Any recommendations for a mitsu indexable mill for aluminum? probably around .75-1" dia, sort of a "do-it-all" cutter?

AXD

 

[Mtndew]

AXD

Yep, the AXD.
We have the 2" AXD 4000. We cut a ton of 7075 with it last year and our only limitation was the spindle HP and torque. It wanted more.
It was on our Hyundai KF7600L, Cat40 12k spindle and about 28hp. If this was on our Genos M560V we could have pushed it harder because of torque but the parts were simply too large.

 

[kyleisraaddd]

Yep, the AXD.
We have the 2" AXD 4000. We cut a ton of 7075 with it last year and our only limitation was the spindle HP and torque. It wanted more.
It was on our Hyundai KF7600L, Cat40 12k spindle and about 28hp. If this was on our Genos M560V we could have pushed it harder because of torque but the parts were simply too large.

That's great to hear. I'll keep it in mind for the new matsuuras
thanks @Houdini16

 

[Machinerer]

I haven't used one quite that long, but I have used a 3/4 3.5loc and it worked great. I wouldn't try to rough with one but swift claims it'll handle a 25% stepover. I typically just use it for full length ~0.010" finish passes.

You're saying the imco sucked?

What kind of speeds and feeds do you run on that?

 

[Machinerer]

Runout is crucial as is the end mill having zero taper. Combine those 2 and you'll get a damn near perfect wall with zero steps.
The best end mill I've used for this is a YG-1 AlumaPower 3 flute necked. That thing is insane.

I'll have to play around with it, because it would give me lots more options in my "toolbox" if I could get this right. Do you usually spring pass something like this? Or leave a healthy amount of stock and 1 shot it?

 

[crossthread82]

What kind of speeds and feeds do you run on that?

In my case I was running 3.500 axial 0.010 radial 6500rpm and 35ipm, took one finish pass then a spring pass.

If you were going to run that 5/8 4.5loc I'd start at 3600rpm and 20ipm .010-.015 radial and see how it sounds. Definitely don't just ram it into the corner or it will bark really bad. You may be able to go faster given you are taking a full length cut and the endmill would have 10 flutes in the cut at one time.

Edit: Swiftcarb will put chipbreakers along the flute to help with chip control if you ask them, doesn't seem to effect the finish much. 4.2" deep is going to make some serious horse hair chip mats in the machine.