Making some ali chips, how hard can I push this?

I've posted before with my ali problems. The problem being that I don't do a lot of it, and I what I usually do is small or thin wall castings. I seldom have to make time on it.

This one has to go Monday. Big old giant C-clamp. 2 of them nested into a plate(standard old 6061, Kaiser plate), the plate is 2 x 19.1 x 35.75, actually 2.030 thick. Heavy bastards, I know since the forklift would not start this morning.

Running the Imco Streakers, 3 fluters, uncoated, mostly 1/2". Standard old 4020 Fadal, 10k spindle, 15hp, 22.5 peak. I can feed 250ipm in a straight line without messing with the override. The machine is tight, tool retention is about as good as you can get. Coolant is the re-plumbed 240V TSC pump. It showers the shop pretty well.


In process.

Running 8000rpm, and about 100-115 ipm in the pockets and slots, .2ish DOC. Running 8000rpm and 200ipm when there isn't full engagement. That's 10 cubic inches a minute, that's crappy. I'll run 4140 at 14 cubes a minute and 1018 at 18 cubes a minute, not slotting, but.... aluminum is not my thing, I have a habit of melting things.



My fear is gumming up the works, especially in a slot or pocket, and all I'm doing is slots and pockets.

How hard can I push it, I'm at 3 hours now for this OP. My weekend would be so much better if I could get it to 2 hours. 25 parts total, so 13 plates, maybe 14 if something goes really wrong, if not I have a really big chunk of material left (priced into the job).

I try to not run too long over 8000rpm since supposedly its really an 8k spindle that can do 10k. Its my spindle, so I'm a bit conservative there.

Any suggestions? I'll be up all night.

If anybody is wondering how you get 19.1" in a Kurt D688, I'll post up some pics when I pull this plate off. Its less than ideal, but it works, the plate is sitting flat within .007", with a .004 deviation in the thickness of the plate.

Quick .02 worth. From the looks of your "used" end mill I would guess your using a plunging entry?. If so try a ramp with say 3 or 4 degrees along the pocket perimeter to depth. Three fluters only really have one effective flute up to the centerline I've had trouble with 3flts and plunging.

Regards,

Tom Lipton

That giant spiral of death was from years and years ago. It didn't happen on this job. I keep it because it looks cool, but I've melted aluminum into more than one endmill, nothing as spectacular as that, but "melt down" is what I am most scared of.

No plunging on this job. I leaned that lesson a long time ago.

Sorry if that giant cluster-muck looked like it was from this job.

I could make this part quicker if it was annealed 4140 and even quicker if it was A36 or 1018. I might eat a few more tools, but I'd be more comfortable and get it done quicker than out of 6061. I know that is wrong. Its fricken aluminum.

I guess my first question is why you are using 1/2" endmills on a piece this size? I remove a ton of aluminum on a daily basis, although the parts are usually small enough to fit in the palm of your hand. What I have found works best for roughing are 3/4" carbide corncob endmills. I run them at 7500RPM and 60-75IPM. While this may seem slow at first, understand that I run at 100% axial DOC and 60-75% radial DOC. I've never understood running such shallow (.100-.200") axial DOCs, especially in aluminum. The cubic inches really start to fly when you bury the endmill. Of course, you need a rigid setup and a rigid machine, and don't forget full flood cooling.

Oh, and I always drill a pilot hole for the endmills. Ramping and helical entries work too, but I always have a drill that I'm using for another feature on the part, so I just use that. I hate clogged endmills.

Good luck

It might help to use an aluminum-specific coated EM for roughing at least if you have one laying around--they seem to keep aluminum from sticking quite as bad. I like the Garr Alumastars, but all the big names have an aluminum-specific coating now, and they all seem to work pretty well from what I can tell.

I'd say you can increase axial DOC a fair bit if you have plenty of coolant pressure and keep the coolant concentration up. If you ramp or helix into it, I'd think you could run at least .400"-.500" DOC on a rigid setup and machine like you've got here--I'm able to run more aggressive than your posted info even on wimpy Haas Mini Mills.

Take this with a grain of salt--you've probably forgotten more about this game than I've learned so far!

Nice setup, BTW! If it works like I think it does based on the picture, that's a great idea I've never seen before.

You pocketing out the pockets or profile cutting them? I'm not even sure of my terminology here to be honest. Asking if you are lifting out a solid chunk, or just making chips of it all. Chipping it would take more time, risk of hangups would be much reduced, no?

I've run some corncob 3/4 HSS roughers to clear away inside and outside some of the larger parts, using an offset from my part, then done full depth passes to clean up the perimeter with an end mill after, on some stuff I made of 7075-t7, 2.125". Can't give you numbers at all, but I was sure impressed at how much faster it went than trying to clear all the material with an EM.
I have an old Milltronics Knee mill with about 3500rpm/5hp on tap, I know next to no Gcode, but am slightly better than FNG status with Gibbscam...I tend to make changes on the fly and try the next idea, programming while the tried and true is running. Dunno if you have that option.

Looks like a pretty interesting part. Be interested to see what comes up here.

Cheers
Trev

First one is done, its taken a while, I've been screwing around with it, was on the phone for a bit, ate some dinner, and I've been messing around on here.

Pumped some feeds up, pumped some depths up. Where I am running into problems is that if the chips get too big or too heavy, they won't move out of my slots. My backplot is telling me that I'm getting closer to 2 hours. Those drilled holes are an attempt to get the chips out, it added 3 minutes, I can live with 3 minutes, though I may eliminate it, we'll see how she goes.



I could not get a decent pic of this damn thing, and yes its hanging from a Kant-Twist. I've had much heavier things hanging from a Kant-Twist.

There are 7 places approximately 3/4x3/8 that I need to blast through with a sawzall, the rest of it is only .015 thick and will come apart with some aviation snips.

The crappy set up, and a tutorial on how NOT to expand the capacity of a Kurt D688.





There is a 1/2" spacer on the back jaw also, if you can call a 1-2-3 block a spacer. I consider a 1-2-3 block a consumable. Total mish mash of hard and soft jaws, and an angle plate for a stop. A bit unorthodox, but functional for a small qty of parts.

Aww crap, I managed to take a good pic of where I had machined into my vise. It wasn't this job, but its still mildly embarrassing, and it was an accident.

1/2" endmills, because that's what I've got. Running 3/4" when I'm getting past 1.5" deep, but not ali specific.

Pockets are all chips.

Just noticed this plate is "Kaiser Select". What the hell does that mean? The last plate we got was just "Kaiser" in blueish ink, not pretty red and it had all kinds of crap smashed/rolled into the surface. It was pretty rotten considering it was also labeled "tooling plate". I guess you could make tools if you melted down the plate, and all the other unidentifiable objects smashed into the surface.

Does it get the "select" label when somebody noticed it didn't have a coke can or a small engine block on the ingot/billet? before it went in the rolling machine?

If you have a product that is "select", isn't that just another way of saying "all our other products suck", especially when they are all to the same spec.

Maybe "select" means "pretty red ink". Then again, it could be red for 'caution', as in "Caution, we 'selected' this material because you may encounter a cast iron intake manifold, or a hardened bearing race".

Depending on how fast your tool change is, you might be better off chucking a couple different endmills up, for each doc. If i'm figuring right, I think you can get 100ish ipm at .75 doc, if you are only sticking out .8something. The trick would be sneaking some serious flood coolant in there. Anyway, if you can keep the chips away, you might try it. That would get you closer to 40 cubes MRR. Then switch to a inch and a half for about 50 ipm, @ 1.5 depth, then your third cut etc.

Though, if you're using a .75 eventually anyway, you might be able to move more with it than those .5's, even if it's not a high helix. Is your .75 a two flute, at least? A carbide 2 flute will run about 60ipm at 1" doc. with your 8k... that's quite a few chips. Like bucktruck said, see how deep you can get it, then creep up on the feed, while staying short short on the endmill...

-Parker

4:06am. Mountain time. I think I got her well under 2 hours. Lost an endmill, didn't actually lose it since it was embedded in the part. 3/8" 3 flute, .092 radius. 9000rpms, 150ipm.... 900ish sfm, .0166 per rev, .0055 per tooth, .600 deep, full width, not a good combo. I've had that damn endmill for 4 years, I had to break out the backup.

Just lost the backup..........

Had to grind one, 3 fluters suck to grind. I should have grabbed a 2 fluter.

On the 1/2's, running 9k and 150-225 ipm. .300 deep on a full slot.

I just don't see how I can go much further than that. Thats 33+ cubic inches a minute. Over .008 per tooth. Its sounding like a pretty nice little hail storm in there, I like that.

If I'm under 2 hours I'm good and I might get to go home at some point. Though I'm sure the old lady is loving having the bed to herself. No Me and no Dogs.

Parker, running a multitude of 1/2"s.

The 3/4 I'm running, well, its not ideal, TiAlN coated 4 fluter. Just ripping out the very bottom.

I wish I had some more Ali specific tooling, but I don't. I just don't do it enough, and the stuff I normally do is small. I've probably got 15 3/8" aluminum specific endmills, unused sitting in the drawer. Nothing over 1/2".

I didn't expect this material to show up until next Wednesday, but.... if we get it done by early next week we get paid next Friday, otherwise we have to wait 2 more weeks, and I could really use the money right now. That customer is on a short leash.

I was going to start programming her on Monday, and order up a few bigger tools, but that didn't happen. Under 2 hours, I'm OK with that. Actually 2 hours makes me happy. I was going to say it was kind of a gravy job, but that would screw me. I've got one threaded hole to set up, that I'm a bit worried about, after I get some sleep.

If you're restricted on cutters, one dodge is to grind a few nicks in a helical pattern on the flutes (corner of a SC wheel)

IME they don't have to be too ''fancy' and only about 2 - 3X chip thickness deep - think semi finishing cutter.

They do really help breaking up the chips as well as letting me push the cutter harder.

Agree with bucktruck on the roughers. Never have packed the flutes on one in AL regardless of DOC. Because of that, its pretty safe to keep on increasing the feed to load the motor.

Is there a reason you're facing the entire plate?

You said you were dropping the waist plate off with a sawzall, so you could also do the same thing with the pockets. Profile the pockets instead of turning the whole thing into chips and drill a starter hole or two for the sawzall.

7:04AM still up, still running. I've packed 3 endmills in a row, in the exact same spot in the exact same pocket, and the first pass in the pocket. So not that deep.


Woops, make that 4, this one snapped, I'm getting down to the skinny on these guys, same damn pocket.

I've got some Cobalt roughers, I think I might try one of those. More to come. This is pissing me off.

8:08 now, still up. Backed her off a bit, using an old coated Niagra 3 flute carbide, 1/2". 7200 rpm, 108ipm, down to .22" DOC. She's humming pretty nice, doesn't sound like she's doing much, but I'll take a bit of time for consistency. I'm wondering how much of the packing endmills is material related, same spot, not going nuts, 1200sfm, .005 per tooth, excellent coolant pressure.

The cleaning guy came in at 6am, he cut apart all the plates I had done, so now I have a big pile of semi finished giant C-clamps. He's more than a cleaning guy, he'll run parts when we need him to. Pick up material, deliver parts, keeps the weeds down. Pours cement, helps fix machines. Hardest worker I've ever met in New Mexico. And yes he's legal. He does 4 10's for the state Monday to Thursday. I wish I could give him a raise.

My left nipple hurts, my shirt pocket is full of chips, and I need a nap.

I'll have to remember those jaw "extenders" the next time I have some large plates to mill.

Don't know what to tell ya Bob. Seems to me to be a straight forward job. (But I guess I mill plenty Ali.) You may be better off with an mist lube air blast than flood coolant? Better pick up a few Ali EM's in various sizes for next time.

Matt@RFR said:

Is there a reason you're facing the entire plate?

You said you were dropping the waist plate off with a sawzall, so you could also do the same thing with the pockets. Profile the pockets instead of turning the whole thing into chips and drill a starter hole or two for the sawzall.

Click to expand...

Pockets from both sides, not through. Facing the whole thing just because I can, 2"±.030 and its 2.030 from the get go. I'm pulling .015 off of each side just so my chamfers are nice and pretty and consistant.

Facing is under 2 minutes for the entire plate which has 2 parts. I'm worried about hours, not minutes. Though minutes add up to hours.

All dimensions are landing within .002 with calipers. I'll take that since its ±.030 work and some of it is ±.060.

Ahh, I didn't catch that the pockets were not through from the pictures, sorry.

I'm with David N. Seems like you're about topped out for a 1/2" 3 flute. I know I couldn't run any faster on my Haas, though I do have through spindle coolant which would help a lot.

Do you have a 1" or so indexable endmill that you can get aluminum specific inserts for? I have one from Curtis that I run conservatively at .200 deep, full width, 12k RPM and 250 IPM.

We all done the melted AL endmill trick at some time or another * too much feed, not enough flute space for the chips to get out killed this one

The tool that most impressed me for doing jobs like that is a 25mm Walter 2 tip Al cutter (not got the part number to hand) ramp it in at a shallow angle in the pockets, then give it some beans at 12 000 rpm, about 200ipm feed
Then whap the corners out and finish profile with your 1/2" endmill

Boris

*And the legendary Mr Slammy in the background, resting after a hard day 'encouraging' the operaters to behave

I was wondering if that was Mr Slammy.