Milling some 6061, want to move lots of metal, what feeds and speeds?

Hey all, I'm going to be machining some 6061-T6 in a couple of days. I'll be using a VF-1. It's 12"x4"x1" stock. I need to cut a 2.5" slot in the middle.

I was thinking of using a 1" end mill (faily cheap tin coated HSS 2 flute) and do a full .5" deep cut right down the middle. (Down the 12" length)

For the first cut I was thinking 2000 rpm @ ~15 IPM feed. Next cut I was thinking of stepping it over 1/2" then going at ~30 IPM.

I'll be using flood coolant. Those seem like ok cuts, or am I way off the rocker?

Thanks!

How are you holding this material? And is that a CAT40 Spindle Taper? Feeds and Speeds have a lot to do with Part, Set-up, and Machine Rigidity. They require a bit of feel.

2000 rpm at 15 ipm seems pretty safe. Just watch your 1/2 D.O.C.. That 1/2 seems deep for a cheap cutter. You may wind up cranking it up a lot more after the first cut. Give it a try and see how it goes. As for your next pass on the sides try 20 ipm and go from there. If you take the ipm/rpm you will get your cpr. Divide that # by 2 flutes and you get cpt (chip per flute). I usually start at .005 cpt and work my way up. Shops around here use cheap tools, I hate cheap tools. :rolleyes:

Always start low and work your way up the latter.

BTW: What does a rocker have to do with it? ;)

:cheers:

Why use HSS? Carbide that diameter is expensive so go to carbide 3/4" dia. 45 degree helix two flute. On a VF0 with flood coolant we run these cutters at 7500 rpm, 0.4" to 0.6" depth of cut for slotting with a feed of around 40 to 50 ipm. When widening a slot or running a cut down the side of the stock we will run 0.6" DOC with 0.6" stepover and take the feed up to something 70 or 80 ipm. The thing you should be looking at is spindle load; just set your rpm at 7500 which is probably max for your machine and play with the feed rate overrides to keep your spindle load beteween 100-120%.

I agree with Geof completly. I use CGS 55 deg two flute endmills for aluminum and just the other day I was running a 1/2" cutter through 5/8" plate in one pass at 6000 rpm and 26 ipm. I probably could have gone a little faster on feed too. When only taking .1" doc I go at 10000 rpm and 50 to 60 ipm with a almost mirror finish. If you get a 3/4" endmill like Geof says you can easily go faster as the tool is stronger, I would run at your max rpms too.

Just make sure you have good coolant concentration and good flow hitting the tool. I had low concentration the other day and a lolipoped an endmill. Fixed the colant and everything ran like a charm.

JP

I'll put in my 2 cents. First, yes you do need chip clearance when hogging aluminum, but a 1" 2flute is ridiulous. A 4 flute would do you fine at that chip load and depth.

As others have suggested, I would go with carbide, I'm no Haas fan, but that machine is well capable of ripping out a whole lot more material than you're planning. 1/2" two flute carbide, still dirt cheap. 12,000 rpms, 150ipm, or 3 flute 5/8" carbide rougher, about $75-$100, 10,000 rpms 100-200 ipm.

Running 15ipm in aluminum is like buying those tiny little 6 ounce cans of beer. Whats the point, you might as well go home. Somebody spent good money on a decent machine, why waste that trying to save a few buck on a HSS cutter. Penny wise and dollar foolish.

I save the HSS/Cobalt for bigger roughers that need to go deep(on limited runs), other than that run carbide, it lasts longer is more accurate and will in the long run save you money, 1/2" and under the price difference is negligable, and a 1/2" carbide will put you a mile ahead compared to a 1" HSS, especially at 1/2" of depth.

In that case try DuraMill .5 Dia 1.0 Flute Length 3 Flute 60 degree helix 7,500 rpm 180 ipm Full 3/4 d.o.c. Solid Carbide TiN coated. :cool:
www.duramill.com $40.00 each :banana:

Starting to look like the battle of the End Mills here. :rolleyes:

Quote:

---

Originally Posted by JPMach

.......I had low concentration the other day and a lolipoped an endmill. Fixed the colant and everything ran like a charm. JP

---

I omitted mentioning this; good coolant flow is very important. And the reason I say 3/4" dia. is exactly as JP points out the cutter is strong enough that you can run the machine to its limit. With a 1/2" cutter you have to take more cuts but you cannot run the ipm up too high otherwise even with coolant you can finish up with just a stub in the spindle and a chunk of carbide buried partway down your slot.

Another approach is to go to the tool list in Current Commands and set the spindle load limit at 120%. Then go into into the Settings and change #84 Tool Overload Action to Autofeed. Then just program very high feedrates and let the machine back the feed down itself. This is the sloppy, lazy way of doing it but it works.

minicut has good highspeed roughers that can haul , speeds feeds ? as fast as you want to go , it s aluminum

Thanks for all the replies!

Wow, I didn't think I'd be able to run near that quick with carbide tools. That'll make some chips fly!

I'll pick one up, I only have a few slots like these to make, but it should be fun to make a lot of racket :)

if you only have a few 1/2 3 flute naigata 45 deg helix .5 deep 60 imp 6000rpms