I'm using a 1/2" 4 flt solid micrograin carbide square end mill to cut 0.75" deep slots in 6061 T-6 aluminum.

I'm spinning the tool at 5000 rpm, feeding it at 40 IPM at a DOC of 0.1"

That gives me .002 IPT, which I thought would be easy enough for the carbide to handle.

Wrong.

I have cut maybe 1800 linear inches with this tool, and already it is destroyed.

Not broken, but the ends are chipped, the flutes are chipped, and it is now leaving swirl marks all over. Basically, its done.

Whats wrong? I am using a water soluble lard oil cooland/lube, mostly to flush the chips out of the slots.

I've got to fix this somehow, as ruining a $40 endmill every time I cut this part is really cramping my profits.

I know something is wrong, but durned if I can figure out what.

Could it be poor quality tooling? I've been contemplating switching to indexable endmills, but I want to be sure that this won't happen with them too.

Any help would be most appreciated

Thanks for your time.

Try coated EMs, Tailn or Ticn. Also, bump up the chip load, double it or more. You're pre-maturely wearing down the cutter by 'rubbing' too much on the material. (Make each pass of the flute count, take as much as you can.. removes heat as well :cheers: )

Carbide will work nicely, but inserts will work better, IMNSHO.

Hardmill will prolly have a say on this as well... ;)

'Rekd

Originally posted by Rekd


Hardmill will prolly have a say on this as well... ;)

'Rekd

Up the SFM if you can and +1 rekd on the chip load.
But most important is ditch that 4 flute endmll (yuk!!)
Not nearly enough relief.

PEACE :D

I'm thinking of switching to a 1 flt .5" indexable, or a 2 flt .625" indexable.

I have to have a good surface finish when the part is done. Will the 1 flute still give me a decent finish?

5000 rpm is the top spindle speed on my machine, so SFM is as high as its gonna go. I can bump up the feed all the way to 280 IPM (max cutting feed) if needs be to get the FPT up where it should be.

BTW, what FPt would you guys suggest for the 4 flt? I've got one more setting here, so I might as well use it.

The indexables I was looking at suggest FPT in the neighborhood of .010" Would this be a good place to start for coated inserts with the right geometry?

Your previous suggestions are very helpful, any others would be equally well appreciated.

Thanks again for your time.

The problem with single flutes are the feed it needs to go to achieve the same chip load. (For finishing, this means much slower feeds to achieve a good finish as opposed to, say 4 or 6 flutes.) It might be worthwhile to rough and finish with 2 different tools, so you can finish faster.

'Rekd teh hardmill? We're tied again..

Either pass me or slow down, but get off my a%#:p

I really don't like that 4 flute, not nearly enough relief.
+1 on the fpt for the insert mills though, just make sure
they get you the proper inserts.( for alum)
Sorry to hear about the max spindle speed :(

PEACE:D

That idea had occured to me too.

I was thinking of using the 2flt 5/8" indexable to rough with, and a 1/2" 6 flt OSG rocket mill to finish with.

I'm also looking for a good indexable corner rounding endmill. Something with a 3/16" radius, and it would be nice if it were center cutting as well. Anybody know ofhand where I might find something like that? (Preferably for under $150)

BTW, Rekd, you are johnny on the spot with the replies tonight. Good job. Its almost as good as instant messages. :D

Thanks again.

I use 4 flutes almost exclusively for finishing microwave housings, (brass and alum) and other critical surfaces where I want to move quickly.

'Rekd teh 'Beep Beep'

Originally posted by CoolHand
That idea had occured to me too.

I was thinking of using the 2flt 5/8" indexable to rough with, and a 1/2" 6 flt OSG rocket mill to finish with.

I'm also looking for a good indexable corner rounding endmill. Something with a 3/16" radius, and it would be nice if it were center cutting as well. Anybody know ofhand where I might find something like that? (Preferably for under $150)

BTW, Rekd, you are johnny on the spot with the replies tonight. Good job. Its almost as good as instant messages. :D

Thanks again.

The rocket mill sounds good.

The center cutting CRE will prolly have to be custom made. I don't think I've seen them before.

I'm sitting here sipping a Rum & Coke, beating Hardmill to the new posts.. :D

'Rekd teh nuttin but love.. :rainfro:

I think he's on a dial-up, or types slow tonite.. :cheers:

Originally posted by Rekd
I think he's on a dial-up, or types slow tonite.. :cheers:
Hey pal I always tetete ype slow;)

PEACE:D

Originally posted by Rekd
The center cutting CRE will prolly have to be custom made. I don't think I've seen them before.

I was afeared of that.

Oh well, I'm off to bed.

Thanks for your help guys.

DON'T USE COATED ENDMILLS FOR ALUMINUM. THE COATING ACTUALY ATRACTS THE ALUMINUM CAUSING IT TO GALL UP, THUS CREATING FRICTION, THUS CREATING HEAT, AND SO ON AND SO ON. LOOK AT DATA FLUTE OR DURA MILL THEY ARE THE KINGS AS FAR AS CUTTING ALUMINUM. :idea: :idea: :idea:

Chad,

I use coated EM's for Alum ALL THE TIME. Your problem is that you're not generating enough heat to have the properties of the coating start working for you..

Those coatings need heat to work, which means you need to feed them harder. Try it, you'll be suprised at the results..

'Rekd

Chipping a carbide in 6061 aluminum? Sounds like a coolant problem. Unless you are feeding the coolant through the mill, I doubt that the cutter is even wet at 5000rpm, but for sure it is not being consistently cooled, which a problem for carbide.

I'd highly recommend something like a Trico air/oil coolant unit. It uses an incredibly small amount of lube, yet gets the job done. I have machined hundreds of feet of aluminum with one carbide cutter (3/4" 2 flute regular flute, uncoated) and I don't think it will ever wear out ;). I typically feed at .004 per flute.

Plus, you should use a high helix 2 flute for optimum chip flow. I don't think they had them readily available (in carbide) back when I bought this 3/4" cutter, but I would sure look high and low for high helix carbide, when this one is done.

Originally posted by HuFlungDung
I typically feed at .004 per flute.

Plus, you should use a high helix 2 flute for optimum chip flow. I don't think they had them readily available (in carbide) back when I bought this 3/4" cutter, but I would sure look high and low for high helix carbide, when this one is done.

+1
Thank you Mr.Dung:p

PEACE:D

Here's my two cents worth. The reason your end mill was breaking was that the material was building up on the edge, and as the cutter moved along the path, it was trying to cut with aluminium welded to it's cutting faces. My guess is that it chattered alot as well.

I would use a two flute standard carbide thirty degree helix 1/2" at up to 1000 sfm, 1/2" depth, and about 0.003" to 0.005" per tooth to rough. Then, if finish is a problem, use a multi-flute with high helix to go down each side, removing as little as you can get away with at full depth. Probably about 0.001" to 0.002" per tooth per rev. Or, if you really want to remove material quickly, use a carbide roughing end mill made for aluminium for your first step.

I've never had a heat problem in aluminium, either 6061 or 7075 as long as I'm removing enough material to send the heat out with the chip. The problem with using a four flute is that in order to achieve the proper chip load with a fully involved cut, you need to remove too much material for the flutes to spit out. It will usually tell you with chatter before it gives out.

Oh, and as far as coatings are concerned, you don't need them for aluminium. In fact, most coatings will tend to make the flute edges less sharp.

Good luck.

Adam