I am cutting channels in 6061 T-6 aluminum, .31" deep with a 1/4" carbide EM. Its a two flute Niagra, solid micro-grain, 45 deg helix, .375" LOC, TiCN coated.

I'm spinning it at 5000 rpm (max for this machine), and feeding it at 30 ipm, with a DOC of .075"

The last EM I had was uncoated, and it got a builtup edge, clogged the flutes, and broke. No problem, switched to the coated Niagras, reduced the DOC, and tried it again. This time, I literally shelled it. Peeled the flutes right off the central spur, now I have a pointed engraving bit.

What gives here? I was pushing the uncoated mill at .004" per tooth, but I broke it. So I stepped the feed down to .003" per tooth.

I was cutting dry.

There was no alum stuck to this Niagra cutter.

I am at a loss here.

I've broken about $80 worth of mills on this job, and its really pinching my profit margin.

Somebody please help me here.

I'm doing everything they say to do with carbide and aluminum, and all I've got to show for it is a pile of junk cutters.

Arrrrrrghghghe!!!!!!!!! :mad:

Put some coolant on it, or run it up faster to try and generate some heat. Just a guess, but I'd try .05 DOC at 50ish IPM with a mister on it.

'Rekd

OK, I forgot some things.

I don't have a mister.

I've cut 16 of these parts (in a row) with one endmill (uncoated carbide no name). I was running it at 40 ipm with a .125" DOC.

Then all of the sudden, that mill broke. And the other one I had just like it lasted like 30 sec, and then another 30 deg helix EM lasted about 3 sec. So I ordered some coated Niagras with half the LOC so they would be stiffer. This one cut like a champ, and then just exploded. Not a sound, until it broke. Perfect surface finish, then boom.

I don't understand what is happening here.

I tried doing the same thing that worked for all those parts in a row, except now it only ends with exploded endmills.

What has changed?

Why won't that work now?

This is insane, I am contemlating giving up machine work, and buying a pottery wheel.


:rainfro: Somebody stop me!!!! :eek:

You prolly got lucky on that first EM. ;)

'Rekd

Is a channel in a larger part, or are you actually cutting a part that ends up looking like a channel ?

How is the work piece being held ?

Not to ask a stupid question, but after one endmill broke, are you cutting a fresh part or the same part?

What kind of tool holder are you using ? If a collet have you checked for runout ?

Coolhand, get a mist unit, it will likely cost the same as a pottery wheel, but you're already set up for machining, so what the heck :D

Lacking a mist unit, I would apply an air blast, and paint the surface with heavy cutting oil (so it won't blow off), in an attempt to get a little bit of lube on the cutter

OK, I started fresh with a new billet after the first two ate themselves.

My machine has a BT-40 taper spindle, and I am using a solid set screw EM holder less than .0002" TIR at the tip. Spindle bearings are solid and smooth.

I have a flood coolant system on this machine. The basin is currently filled with a water soluable lard oil mixed about 30:1

I can fortify that solution if it needs more lubricating power.

Here is what I am thinking of doing:

Reducing DOC to .050", increasing feed to 50 ipm (that's .005" ipt), and turning the hose on it (flood coolant).

At this point I don't even care if the EM wears out before it should, as that would indicate that I have kept one in a single piece long enought to wear it out.

Let me know if that is way out in left field.

Also, the reason I am resisting the mister is because my air compressor can barely supply enough air to keep the tool changer on my machine running, much less a constant bleed like a mister. I can buy a lot of $20 EMs for what a bigger/another air compressor will cost.

Thanks for your help guys.

Opps.

BTW, here is a pic of the parts I am cutting.

Click Here to view the Bane of all 1/4" EndMills (http://www.logicpaintball.com/)

Its the pic in the middle (or the only one on the page, depending on how you want to look at it.)

Thanks again guys. :D

Have you tried M3 instead of M4? :D

Seriously though, I would decrease the feed. What you are using is pretty heavy for that small of a cutter when it is completely engaged in the cut. The chip is likely a bit too heavy and wants to slip shear, which makes it pile up and seem thicker than it really is.

Cut deeper at a slower feedrate, maybe 10 to 15 ipm at .125" deep

Originally posted by HuFlungDung
Have you tried M3 instead of M4? . . . . . .

That's not funny. :p

I'm stupid . . . . but not that stupid.

Anyway, which way should I do this?

Thin DOC, fast feed

OR

Deep DOC, slow feed

I'm conflicted. :D

I would like to stay with the option that heats the workpiece the least. I also want to make the most efficiect use of the machine's time.

You're in a catch 22, Ryan. The tailn coatings require heat to work. Heat is not a bad thing so long as you can remove it quickly, either via coolant or taking it out with the chips. (The latter method is harder to achieve in certain situations)

'Rekd teh Trial and Error is too a science!! ;)

I would try a lighter feedrate, whatever depth is up to you experiment with. When guys are milling at high feedrates with a small cutter, it is usually not fully engaged in the cut.

I don't know if lard oil is good for aluminum or not. WD40 works good but it is stinky to be around.

I've been banging around Niagara's website, and this is what I came up with:

DOC is not to exceed 150% of diameter.

500 - 600 sfm (but I'm only gonna get about 375)

Recomended/Max feed = .002 ipt (Comes out to 20 ipm)

Must be run with some kind of Flood Coolant.


With that in mind, I think I'm going to go with this:

.075" DOC, 20 ipm feed, 5000 rpm, flood coolant

Obviously, I'm not trying this until tomorrow, so you guys have until then to talk me out of it.

Whadda ya think? :cool:

BTW, thanks for all your help guys.

Sounds more like what I would expect to work. :)

I have been using these cutters for aluminum with pretty good success when taking full width cuts in aluminum.

http://www.sgstool.com/productlines/sgs_catalogs/ShearCarb_Letter.pdf

SGS suggests 1300 SFM (which you wont get on your spindle)
max Axial DOC = 1D
Chip Load = .0024 IPT

I tried those feeds and speeds today, and everything worked like a champ.

Now, just think about how much money I could have saved if I had just went to Niagara's website BEFORE I started cutting. :eek:

I marvel at my stupidity sometimes. :rolleyes:

Anyway, I'm back in business.

No pottery wheel for me.

And I will never EVER use this smiley again. :rainfro:

Later, and thanks for your help guys.

I DO DAILY MILLING OF SLOTS AT 390 DEEP, SPEED OF 5000 ,FEED OF F10. IN ONE CUT USING A 281 2 FLUTE BALL NOSE END MILL WITH FLOODING COOLENT

[QUOTE=eightball3;375251]I DO DAILY MILLING OF SLOTS AT 390 DEEP, SPEED OF 5000 ,FEED OF F10. IN ONE CUT USING A 281 2 FLUTE BALL NOSE END MILL WITH FLOODING COOLENT[ BEENING A FORMAN SOME OF MY EMLOYEES DO NOT UNDER STAND THAT SOMETIME TOOLING DOES GET DULL AND NEEDS TO BE REPLACED LIKE MY BOSSES SON IS MOER INTERSTED IN MAKING MONEY THEN CHAGING A DULL TOOL HE WILL RUN IT TILL IT BREAKS AND WRECK A PART/QUOTE]

I DO DAILY MILLING OF SLOTS AT 390 DEEP, SPEED OF 5000 ,FEED OF F10. IN ONE CUT USING A 281 2 FLUTE BALL NOSE END MILL WITH FLOODING COOLENT[ BEENING A FORMAN SOME OF MY EMLOYEES DO NOT UNDER STAND THAT SOMETIME TOOLING DOES GET DULL AND NEEDS TO BE REPLACED LIKE MY BOSSES SON IS MOER INTERSTED IN MAKING MONEY THEN CHAGING A DULL TOOL HE WILL RUN IT TILL IT BREAKS AND WRECK A PART

That was 4 years ago. I think he might have given up on that job by now. ;)

That was 4 years ago. I think he might have given up on that job by now. ;)

Not gave up, so much as, long done and out the door.

In the years following this debacle (which shall henceforth be called "The week of the small brain"), I have since discovered the nirvana that is the high performance variable three flute endmill. Those things cut like lasers. Pew! Pew! Pew!:D

Glad to see you guys are still kicking over here.

Did you find more RPMs under your Christmas tree that year?

Did you find more RPMs under your Christmas tree that year?

I wish. I had thought about doing an 8,000 rpm retrofit, but when I got to pricing the parts, the cost would have been more than I have in the entire machine AND all the tooling that supports it.

Mostly, I've just gotten smarter over the last few years and learned how to push things to get the most out of what I have.

Mostly, the new tool geometries are allowing me to really up the chip loads from where I used to be, and the deep gullet three flute HP type cutters are letting me up my feed rates without plugging up. All in all, it's not so bad having a slow spindle anymore, I've got a lot more tools to work around it with now.

I did just rebuild the head and spindle on this machine, but I haven't gotten to put much time on it since. I'm looking forward to seeing how my surface finish improves.

Lard oil? I have never heard of anyone using lard oil.
Try actuall coolant, 1/4 em, depth of cut, .125, 50 to 100 ipm should be no problem.
I'm affraid to ask what kind of machine.

Lard oil? I have never heard of anyone using lard oil.
Try actuall coolant, 1/4 em, depth of cut, .125, 50 to 100 ipm should be no problem.
I'm affraid to ask what kind of machine.

You do realize this thread is like four years old, right?

If you've never heard of using lard oil and water coolant solution, you've not been around this stuff very long. At the time, I was using a lard oil based coolant because it was what I had, and it didn't cut too bad really. Its penchant for going rancid was its worst attribute. Now I use a soluble oil from Rustlick (which is a semi-synthetic IIRC). It lubes better and actually prevents rust on the machine. Plus it smells a lot better, and doesn't go sour in the sump.

Like I said, I've learned a lot in the last four years. That doesn't mean that lard oil is useless by any means though, you just won't catch me filling the sump on my CNC with it anymore. ;)

BTW, that 50-100 ipm is about 2-5 times what it actually took to make that EM live at 5,000 rpm. Might want to give a spindle speed the next time you suggest feed rates, eh? ('cause that's 0.010" ipt, and 1/8" doc, on a 1/4" carbide EM = BOOM or maybe CRUNCH, Grind, etc).

The machine is a Moog A-22 VMC. It's old and orange and still makes chips just fine, thank you.

Might want to read the thread, look at the dates, and not be so damned smug next time, 'cause your advice wasn't so great this go 'round. (nuts)

Sorry I have machines (Haas, Mori, ect...)that probably have more coolant pressure than a moog, whats a moog?

Cool Hand you are funny

:cheers:
:cheers:
;)
;)

Sorry I have machines (Haas, Mori, ect...)that probably have more coolant pressure than a moog, whats a moog?

I can just about guarantee that they do. The best my old girl can muster is about 2 psi, on a good day. Maybe more with a tail wind. ;) And that's not thru spindle, that's a weak little nozzle off to one side. That's as good as it got, until I "upgraded" the system myself. Now it'll blow the door open on the enclosure, and empty the basin in about two mins. lol Funny what a lawn sprinkler booster pump will do for your line pressure. :D

There is no reason for you to have ever heard of Moog, they've been out of business for a long time now.

Moog was a US distributor for MHP Machine Tools, and sold these (and several other) CNC's in the late 80's and early 90's. The base castings were manufactured in Spain, and the controls were assembled and attached in England before being imported into the US. For their time, they were pretty advanced, but by today's standards, they're a little "rustic".

My machine is a 1992 vintage, which was the last year they built VMC's. The company promptly went out of business and the rest is history. Happily, you can still find parts for them, as everything (or nearly so) is an off the shelf affair.

When you can't borrow $60k to start your business, those 15 yr old VMC's start to look pretty cherry, trust me. I've got in this machine less than a quarter of what a bargain basement HAAS costs, and that's with all the tooling, AND after a control retrofit, a head rebuild, and a spindle rebuild. It's paid for itself at least two or three times over by now. So, it's paid off, AND it's still in excellent shape (as opposed to wearing the machine out to make it's payments, resulting in it having to be replaced the instant it's paid off).

I dunno, at the time I had no other choice, but looking back, I'm pretty sure I'd do the same thing even if I'd have had the cash.

Ryan, I cut 6061 on my Mini Mill on a daily basis with .250 endmills. I'd not waste the money on the carbide, use a coated HSS, they're tougher and less prone to breaking in the manner you're describing. I'd go 5K speed, 2 X .150 roughing passes and about 20 ipm. If it's not howling pretty good, speed it up.

Ryan, I cut 6061 on my Mini Mill on a daily basis with .250 endmills. I'd not waste the money on the carbide, use a coated HSS, they're tougher and less prone to breaking in the manner you're describing. I'd go 5K speed, 2 X .150 roughing passes and about 20 ipm. If it's not howling pretty good, speed it up.

I guess I should quit bumping this thread.

The original post is over four years old. I've long ago figured this out (with the help of Niagara's website and the fine folks here, of course).

Currently I'm running these little ZrN coated HP 3 flt mills made by Accupro. They're holding up amazingly well, and they're taking a real beating while they're doing it. 5k RPM, 0.125" DOC, 0.1875" WOC, 30 IPM feed (that's 0.002 IPT), and they like it just fine. That's just about what I ended up at with the 2 flt Niagaras, but the DOC I settled at was less because my final depth was shallower (so I took two even cuts instead of one huge one and one tiny one) and the WOC was wider (100% in that case).

Perhaps Rekd ought to lock this one so folks don't keep wasting their time on it. No sense in re-solving a problem that's been out the door for four years. ;)

Thanks for the assist though. :D