What's new
What's new

Helical High Feed Endmills for Aluminum

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.
I ended up going with the 4 flute version. The guy at SwiftCarb said the 5 flute would be too many points of contact for a thinwalled part. So I'll adjust the feed accordingly.
 
I ended up going with the 4 flute version. The guy at SwiftCarb said the 5 flute would be too many points of contact for a thinwalled part. So I'll adjust the feed accordingly.
With the length, be sweet for a custom single flute. low helix.
 
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?
I typically leave a few thousandths on the wall for a finish pass. I almost never spring pass unless I need to tickle it into tolerance.
 
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.
I would like to reiterate to the op: you will want to program the largest corner radius you can. Don't make a 8mm (.315") corner rad with that .312 radius tool. Do everything you can to make it larger so you can walk through it. Don't forget to slow way down when doing the tiny radius movement in the corner.

Maybe it's just my experience with spineless machines, but something tells me he's gonna end up running at 1000rpm or less with that noodle of a tool having such a long engagement.
 
Maybe it's just my experience with spineless machines, but something tells me he's gonna end up running at 1000rpm or less with that noodle of a tool having such a long engagement.
Sometimes its backwards, you need the rpm to reduce tool loading, especially on flimsy machines, but yeah.
 
Maybe it's just my experience with spineless machines, but something tells me he's gonna end up running at 1000rpm or less with that noodle of a tool having such a long engagement.
Preferably he'd use a necked stub length tool something like a Destiny Viper V3401232S 5/8 4.0lbs 3flt. And helically ramp the wall contour ~0.075" at a time. But he said he wants a full depth finish pass so...
 
Preferably he'd use a necked stub length tool something like a Destiny Viper V3401232S 5/8 4.0lbs 3flt. And helically ramp the wall contour ~0.075" at a time. But he said he wants a full depth finish pass so...
Not necessarily that I PREFER a full depth finish pass. But, I've just never been able to get any other method to work, and look acceptable. Definitely a lack of experience, on my part. I do plan to try to get a necked tool to work as well.
 
great way to dull the cutting edge from what i was told, right? doing spring passes that is.
Yeah but this is aluminum. He should be fine.
And sometimes you gotta bite the bullet and spring pass if you need to hold a couple of tenths or some stupid true position callout that we all hate :D
 
great way to dull the cutting edge from what i was told, right? doing spring passes that is.
Depending on what you got going on, the whole spring pass thing is a mess, especially when you have a long tool that deflects at the end.

If you get high rpm, and a decent feed you get parts done, if you slow it down for chatter parts done slower.

Either can deflect that tip because of length, you cant really take a spring pass if you have high rpm, and no material to hold the cutter, your gonna get chatter, its one and done.

If you go slow rpm, slow feed, you dont get parts done, but you can take a spring pass without as much risk to chatter.(usually, not always)

My preference to get shit done quick, and minimize deflection, drastically minimize how much cleanup you leave, I want just enough to keep the tool loaded so it doesn't chatter, then I run the higher rpm, and higher feed.
One and done, cosmetic+ .

On injection molds opposite, I need to hit tolerance, so cant have deflection at the bottom, long reach stub flute reduced shank, and a million passes. Polish the walls later, no spring pass still, but its wiping off .001"

But you know all this already, but for anyone else. :cheers:
 
Depending on what you got going on, the whole spring pass thing is a mess, especially when you have a long tool that deflects at the end.

If you get high rpm, and a decent feed you get parts done, if you slow it down for chatter parts done slower.

Either can deflect that tip because of length, you cant really take a spring pass if you have high rpm, and no material to hold the cutter, your gonna get chatter, its one and done.

If you go slow rpm, slow feed, you dont get parts done, but you can take a spring pass without as much risk to chatter.(usually, not always)

My preference to get shit done quick, and minimize deflection, drastically minimize how much cleanup you leave, I want just enough to keep the tool loaded so it doesn't chatter, then I run the higher rpm, and higher feed.
One and done, cosmetic+ .

On injection molds opposite, I need to hit tolerance, so cant have deflection at the bottom, long reach stub flute reduced shank, and a million passes. Polish the walls later, no spring pass still, but its wiping off .001"

But you know all this already, but for anyone else. :cheers:
Since you run a similar tool to the one I'm trying to use, what do you find is a sufficient amount of stock to hold the tool, and not chatter? I was thinking .010"?
 
Since you run a similar tool to the one I'm trying to use, what do you find is a sufficient amount of stock to hold the tool, and not chatter? I was thinking .010"?
.005-.01"
I think I may be at .008"
trial and error.

Also I don't have a tight ass corner like you, I usually would use the next smaller end mill size, but you are extremely limited with that length.
you need to calculate the feed rate for the corners correctly or its going to rip through them.

Hopefully your software has some way to modify corner speed changes.
Or make sure if your posting cutter comp, that it is modifying the rates automatically. :cheers:
 
Yes, I use Mastercam, which can slow down in the corners. I was also intending to "rest machine" the corners first, with a smaller tool, so it isn't engaging too heavily when it hits the corners. Not sure if that will help or not, but it has helped me with tight corners in the past.
 
Yes, I use Mastercam, which can slow down in the corners. I was also intending to "rest machine" the corners first, with a smaller tool, so it isn't engaging too heavily when it hits the corners. Not sure if that will help or not, but it has helped me with tight corners in the past.
I would too.
For stuff like this I have some 1/2" extended reach, stub flute, reduced neck, just to relieve.
If not that little .010" clean up with almost full rad engagement is a lot of engagement depending on arc length.
 
I would too.
For stuff like this I have some 1/2" extended reach, stub flute, reduced neck, just to relieve.
If not that little .010" clean up with almost full rad engagement is a lot of engagement depending on arc length.
Exactly what I was planning to use. Thanks for all the tips. Ill check back in after the part is cut to update.
 
Just an update, per the suggestions I got here, I ran that noodley facemill at 9069rpm and 95.3ipm (.005"ipt) and it sounded great.

That's an MRR difference of 5.73ci vs 2.29ci. Thanks again!!
What step over did you end up at?
 
Oops, meant to include that. .600rdoc, .100adoc

I could probably push it more. But I'll do that after I have good parts going out the door. Harmonics are such a strange thing. 9300 rpm was noisy as hell. 9069 sounded great.
I run mine at 9500 rpm, but that's the peak torque for my Haas MiniMills also, and same.
.5-.6DOC .1WOC 100-120IPM and -30db ear protection! :D
 








 
Back
Top