What's new
What's new

Helical High Feed Endmills for Aluminum

Machinerer

Cast Iron
Joined
Jun 12, 2009
Location
Clearwater, FL
Has anyone tried any of these??

https://www.helicaltool.com/products/tool-details-87299

I have a deep pocket in an aluminum part (4.2") and I'm currently roughing it with a 1", 2 flute Ingersoll Hi-Pos Alu. I use a shorter tool to reach what I can, then move to a longer tool. Unfortunately, I had to reduce the cutting parameters pretty drastically because of the length. I think that feed mill might be a better solution, IF it can do what they say it can.
 
because people fail to qualify questions missing info, I will here.

1st the helical tool may work but usually HF milling Aluminum is slower.

What specs are we talking about?
what machine? spindle rpm available? spindle tool holder CAT40,50 HSK...
pocket dimensions, and smallest pocket radii?
what tool holders available usable, heat shrink, hydraulic, ER..?

I personally rough Aluminum with larger indexables not smaller end mills.

Hope this helps. :cheers:

 
Are you trying to use a smaller diameter tool or just be able to run harder?
Smaller diameter is only because it's what they have. I'm trying to cut out cycle time
because people fail to qualify questions missing info, I will here.

1st the helical tool may work but usually HF milling Aluminum is slower.

What specs are we talking about?
what machine? spindle rpm available? spindle tool holder CAT40,50 HSK...
pocket dimensions, and smallest pocket radii?
what tool holders available usable, heat shrink, hydraulic, ER..?

I personally rough Aluminum with larger indexables not smaller end mills.

Hope this helps. :cheers:
OKK HM600, Cat50, 12k RPM I have pretty much any holder available, except for shrink.

Smallest pocket rad is 8mm, but I'm only roughing right now, and don't NEED to get into every corner. The pocket is just over 4" deep. The Ingersoll HiPos Alu is 4.75" out of the holder, and I'm running it at 1000SFM, and .01" ipt. .300" adoc, .100" rdoc. Putting the SFM much higher creates some pretty terrible sounds.

FWIW, the HiPos Alu looks to be pretty identical to the Korloy tool you referred to.
 
Last edited:
Smaller diameter is only because it's what they have. I'm trying to cut out cycle time

OKK HM600, Cat50, 12k RPM I have pretty much any holder available, except for shrink.

Smallest pocket rad is 8mm, but I'm only roughing right now, and don't NEED to get into every corner. The pocket is just over 4" deep. The Ingersoll HiPos Alu is 4.75" out of the holder, and I'm running it at 1000SFM, and .01" ipt. .300" adoc, .100" rdoc. Putting the SFM much higher creates some pretty terrible sounds.

FWIW, the HiPos Alu looks to be pretty identical to the Korloy tool you referred to.
Can you plunge rough it?
 
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.
 
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.
Originally I tried running it at 2500SFM, which is where I normally run it, it didn't sound good at all.

The pockets are roughly 2.750x 4.750. I was using the 1" because it seemed like the biggest tool I could get in there, and still be able to generate a toolpath without turning too tight of a toolpath radius. That's when the tool likes to bark.

I'm a little confused. You say it's a .500" shank? Surely a .500" shank on a 1.5" tool isn't going to help me any, unless it's just early on a Monday and I'm totally missing something.

*edit* - .5" arbor. Nevermind, lol
 
We use Mitsubishi's AXD4000 cutters with a 1.5" cutting diameter and 1.25" shank diameter @ 6.5" stickout in Maritool hydraulic holders with great results, in both CAT40 and CAT50 HMCs. Parameters are dialed back but only slightly.

If I needed to cut more aggressively, I would have gone with a 1.5" cutting diameter + 1.5" shank, and then cut my own relief on the lathe down to 1.437". I didn't because the MRR is high enough in this application to overwhelm our chip management, i.e. overflowing the 2 yard hopper unless someone moves the chips around with a pitchfork every 30 minutes.

The feedmill you linked with a 3/4" cutting diameter at 4.5" reach in solid carbide is probably more rigid than it needs to be, given the DOC limitations of a feedmill.
 
Last edited:
We use Mitsubishi's AXD4000 cutters with a 1.5" cutting diameter and 1.25" shank diameter @ 6.5" stickout in Maritool hydraulic holders with great results, in both CAT40 and CAT50 HMCs. Parameters are dialed back but only slightly.

If I needed to cut more aggressively, I would have gone with a 1.5" cutting diameter + 1.5" shank, and then cut my own relief on the lathe down to 1.437". I didn't because the MRR is high enough in this application to overwhelm our chip management, i.e. overflowing the 2 yard hopper unless someone moves the chips around with a pitchfork every 30 minutes.

In your case, at 4.5" stickout, a 1.5" cutter could be run at full published parameters, or slightly dialed back on a 1" cutter with a 1" shank + relief.

The feedmill you linked with a 3/4" cutting diameter at 4.5" reach in solid carbide is probably more rigid than it needs to be, given the DOC limitations of a feedmill.
Maybe it's my toolpath, or my approach, rather than my speeds and feeds. I seem to have the worst luck with long tools. Can never quite figure out what I'm doing wrong.
 
usually the bigger issue on this stuff is chip evacuation. wishing you had a horizontal.
If this thing is 4" deep that's a big issue. unless you have coolant pressure from the gods to keep it clear.
gotta love when there's no holes in the bottom of the pocket.
 
usually the bigger issue on this stuff is chip evacuation. wishing you had a horizontal.
If this thing is 4" deep that's a big issue. unless you have coolant pressure from the gods to keep it clear.
gotta love when there's no holes in the bottom of the pocket.
I am in fact, on an HMC, AND I have high pressure TSC. So I'm doing pretty well, in terms of chip evac.
 
Drill the corners so the current tool doesn't squeal/bark/chatter when approaching and changing directions?

Make swiss cheese for similar reasons? Then up your parameters with current tool? (forgive me if you've already tried this with no dice)

I can't see a high feed mill making cycle time shorter. Maybe more reliable, but not shorter.
 
Maybe it's my toolpath, or my approach, rather than my speeds and feeds. I seem to have the worst luck with long tools. Can never quite figure out what I'm doing wrong.
What's your axial DOC? That's the first thing I would reduce if you're seeing chatter, without touching feeds and speeds.

What kind of tool holder are you using?
 








 
Back
Top