Busting my butt trying to rough 3/16" slot in 6061-T651

snowshooze · Oct 28, 2020

Hi Guys, i could use some wisdom.
So, I am making these parts, a lot of 3/16" end-mill stuff in 6061.
I have tried Aluma-power 3 flute polished end mills, and swift tool 45 Degeree helix end mills, also the merlin 5 flute GXMD5 with chip load at .001" per flute. 40 IPM on the 5 flute, it made a dozen parts before it scattered.
I am dying of old age.
14" per minute at 8K RPM. .070" DOC.
Anybody know if I could do better, maybe with HSS?
I can afford to rough, and then clean the slot to .1895 with a finish, if that get's me away from 14" per minute, long run...
Thanks,
Mark

Milland · Oct 28, 2020

What are you using for coolant, if anything? Unless the Al is soft as poop, it should cut pretty well at those numbers, or even faster on the feed.

Phil in Montana · Oct 28, 2020

You need the right coolant and a lot of it to clear the chips...Phil

Finegrain · Oct 28, 2020

ZrN Coated 3/16 dia 3 Flute High Helix Carbide Rougher X .500 loc MariTool

precisionmetal · Oct 28, 2020

How about a spindle speeder? 25k would be more like it, I believe.

PM

Delw · Oct 28, 2020

snowshooze said:
Hi Guys, i could use some wisdom.
So, I am making these parts, a lot of 3/16" end-mill stuff in 6061.
I have tried Aluma-power 3 flute polished end mills, and swift tool 45 Degeree helix end mills, also the merlin 5 flute GXMD5 with chip load at .001" per flute. 40 IPM on the 5 flute, it made a dozen parts before it scattered.
I am dying of old age.
14" per minute at 8K RPM. .070" DOC.
Anybody know if I could do better, maybe with HSS?
I can afford to rough, and then clean the slot to .1895 with a finish, if that get's me away from 14" per minute, long run...
Thanks,
Mark

Are you ramping it down or plunging? need lots of coolant.
all so called alum endmills arent the same. I use Gar alumastar, S carb and niagra 345? 3 flute would be my choice.

D.D.Machine · Oct 28, 2020

I do a ton of 1/4" slots and have found a drill is your friend ,,, swap about .01 under slot width a only leave about .005 web between the holes and pound the hell out of the holes ,,, I run a 15/64 cobalt stub drill at 12K and feed is .02 or 240 IPM and go 3/4" deep with no peck, that is with no TSC. I have found out if I try drilling them with less feed I weld up the drills.

After drilling the holes I do a zig zag low angle ramp with a 3 flute and feed FAST ,,

FYI
uncoated cobalt parabolic drills well take a hell of a feed as long as you don`t peck them ,, I run YG1 mostly

Spruewell · Oct 29, 2020

I wouldn’t use a cutter with more than 3 flutes in that. Chip clearance in the flutes will be a problem. A 2 flute end mill may perform better as there will be more room for the chips to clear

Mtndew · Oct 29, 2020

How long is the slot?
How deep is the slot?

And like Spruewell said, do not use an end mill with more than 3 flutes for roughing in this scenario.

SIM · Oct 29, 2020

Its been mentioned, chips are not your friend, gotta get them out of your way. 4 flute is not enough space to clear chips, 5 is worse. A two flute would be great, but don't like being pushed and only 2 flutes cutting at a slow rpm can take awhile. 3 flute would be my starting point and spin as fast as possible with tons of coolant or pinpoint to blow chips out. A roughing mill that break chips could be helpful or as mentioned pre-drill.

In short, gotta get the chips out of the cut with aluminum or flutes packup'en pop.

No clue what your parts are...but can they be laid down to run past with a keycutter, slitting saw, wood drift.

It's an easy cut, but I assume your spindle is limited on rpm as your only spinning at 8k, makes for long cycle times. Keycutter at 1/2" diameter you could spin and push.

mmurray70 · Oct 29, 2020

snowshooze said:
Hi Guys, i could use some wisdom.
So, I am making these parts, a lot of 3/16" end-mill stuff in 6061.
I have tried Aluma-power 3 flute polished end mills, and swift tool 45 Degeree helix end mills, also the merlin 5 flute GXMD5 with chip load at .001" per flute. 40 IPM on the 5 flute, it made a dozen parts before it scattered.
I am dying of old age.
14" per minute at 8K RPM. .070" DOC.
Anybody know if I could do better, maybe with HSS?
I can afford to rough, and then clean the slot to .1895 with a finish, if that get's me away from 14" per minute, long run...
Thanks,
Mark

This one is too easy. Just get a 2FL, 45 degree, aluminum specific tool and get it done. I would run 8000 rpm, 40 IPM and then play with DOC, maybe start at 0.075 and go from there. Lots of coolant directly blasting on tool to clear chips.

I slot a lot of aluminum. I sometimes use the 3fl Alu-power and like them for certain things, but they clog up WAY faster then a good old 2 fl. The 3fl Alu-powers are NOT good tools for slotting aluminum, especially in smaller sizes. Forget about 5FL, 3 flutes is way to many all ready.

Its amazing how many people have become dependent on HEM toolpaths and cant cut a slot in aluminum. Blows my mind.

Hardplates · Oct 29, 2020

Mtndew said:
How long is the slot?
How deep is the slot?

And like Spruewell said, do not use an end mill with more than 3 flutes for roughing in this scenario.

As Mtndew said, the depth of the slot is going to be an important factor here.

Without the specs on the slot everything is just a guess.

I rarely get to play with aluminum but when I have I've rarely ran into an issue that can't be fixed by either better coolant placement or more RPM. I run HEM toolpaths for almost everything I do but when it comes to aluminum I find I can usually just plow straight through it unless it's very deep.

Job Shopper TN · Oct 29, 2020

With a GWS ZrN coated end mill I could easily cut 1XD deep at a time. 8k RPM, 36 IPM to start. Coolant would be helpful. I don’t know the product line off the top of my head.

Guest · Oct 29, 2020

Are you using a good quality aluminum? Chinese 6061 can make your life hell. It is gummy and can easily weld itself to cutting tools.

Mike1974 · Oct 29, 2020

As stated, just some guess work without more details.

We pretty much baby everything as cycle time is not as much concern as stability, plus alot of the time we are only holding onto less than .10" in our first op. Programming a job now, 1/8" em, .25 loc, 69 ipm, 9100rpm, .030 doc, flood coolant, 60% stepover.

toolsteel · Oct 29, 2020

I agree with the 3 flute options and the guys who have said blast the chips out of the way with good coolant. Use through spindle if you have it.
I dont cut much AL but I ran into an issue once where i couldnt tap holes in it for shit. Found out my coolant was not reccomended for AL. It didnt have the lubricity required. I switched to a coolant reccomended for AL and all my problems went away.

Jashley73 · Oct 29, 2020

Can you get away with a corner-radius?

If so, you can always go shallow on the Z-depths and just run it back & fourth at 100ipm or so, at whatever depth the corner radius is. That'll give plenty of clearance for the chips to get out of there.

I'm also in the camp that 1/4" & under, an aluminum roughing tool taking any kind of higher width-of-cut, has no business having anymore than 2 flutes.

ChipSplitter · Oct 29, 2020

If all else fails, a bit of WD40 does wonders. If you haven't tried it, you should.

About the only thing it's good at, too.

implmex · Oct 29, 2020

Hi snowshooze:
I'm a big fan of plunge roughing for slots, especially deep narrow slots in aluminum.
I've never found a faster way and I've tried chain drilling, deep cuts at slow feeds, shallow cuts at high feeds, skinny cutters and trochoidal milling, ramping etc etc.

As some have pointed out, chip clearing is vital, and when you have a cutter taking up space in the slot, you will always have a problem getting the shit out and getting the coolant in.
As so many of us know, starve the cutter of lubricant for just an instant too long and you have a welded on mess and usually a broken cutter and a fucked up job.

Plunge roughing has been good to me in three ways:

1) I can really put the coals to it, and although the cutter is engaged only half the time, the rest of the time I can flush out the slot completely, keeping it fully wet and keeping the crap out of it so my cutter stays clean and cutting parent metal, not re-cutting chips and cold welding blobs onto itself.

2) The cutter is being loaded in it's strongest orientation...carbide is great in compression so I can push feedrates and chiploads in a way I never can if I load it sideways.

3) The cutter tends to deflect sideways less, so even with a deep skinny slot I have a better chance to clean it up and I can put down a bigger stiffer cutter, especially if I choose a necked down stubby like the ones Frank Mari sells, and keep the stickout just a tiny bit longer than the slot depth.

So yes, I'm a fan.

Cheers

Marcus
Implant Mechanix • Design & Innovation > HOME
Vancouver Wire EDM -- Wire EDM Machining

DavidScott · Oct 29, 2020

Finegrain said:
ZrN Coated 3/16 dia 3 Flute High Helix Carbide Rougher X .500 loc MariTool

When I bought those 3 years ago I found out they are defective, the 3/16" mill photo is NOT of a 3/16" mill. The scallops are too big/deep so the cores are tiny making them very fragile. Garr makes the best 3/16" corn cob roughers I have found. I was slotting 6061 .24" deep at 120 ipm and 6k spindle speed. I could have gone faster if I could flush the chips better.

I think a good 3 flute mill is best for this application, problem is slotting really shows who isn't good, Niagara. For my money it's Destiny tool or Harvey, Harvey's are tougher and more loc options but more $$ and I can't order direct.

Busting my butt trying to rough 3/16" slot in 6061-T651

Stainless

Diamond

Stainless

Diamond

Stainless

Stainless

Stainless

Hot Rolled

Diamond

Titanium

Stainless

Stainless

Cast Iron

Guest

Guest

Diamond

Titanium

Titanium

Titanium

Diamond

Diamond

Similar threads