[SCzEngrgGroup]

Today I tried to mill some 3/8" 6061-T651 cast plate. It was a disaster. Despite cutting MUCH shallower, and feeding MUCH slower than I'm used to in extruded 6061, it machined horribly, and destroyed two endmills in relatively short order. What is the trick to milling this cr@p?

Regards,
Ray L.

[tobyaxis]

What machine and what does your set-up consist of??
What exactly do you need to do to this material to complete your task?
Milling, Drilling, Tapping etc.
Need a little more info.

[SCzEngrgGroup]

What machine and what does your set-up consist of??
What exactly do you need to do to this material to complete your task?
Milling, Drilling, Tapping etc.
Need a little more info.

The machine is a BP clone. 8200 RPM, 3HP spindle. Drilling and tapping are no problem. Milling is another matter entirely....

Regards,
Ray L.

[tobyaxis]

The machine is a BP clone. 8200 RPM, 3HP spindle. Drilling and tapping are no problem. Milling is another matter entirely....

Regards,
Ray L.

What size end mill?
How many flutes?
Carbide, HSS?
What kind of milling operation?
Facing, Contouring, Pocketing, etc.

Work Holding Fixture, Vise, Clamped to the Table?

[SCzEngrgGroup]

What size end mill?
How many flutes?
Carbide, HSS?
What kind of milling operation?
Facing, Contouring, Pocketing, etc.

Work Holding Fixture, Vise, Clamped to the Table?

1/2", 2-flute HSS and 3-flute carbide. Slotting. The carbide loaded up and broke almost instantly at only 0.325" DOC. So, I switched to the HSS, 3200 RPM, 0.175" DOC, 10 IPM with very heavy mist coolant. If I kept to that slow, shallow cut, I got no welding, but the finish quality was horrendous, and after cutting only about 24", the endmill was destroyed - badly chipped on all the cutting edges. I've used these exact same endmills at 0.5" DOC on other 6061, running the same endmill for months at a time, with excellent results. This stuff cuts like crap, and chews the tool into junk in minutes. I've never seen anything like it.

Regards,
Ray L.

[Jadaan27]

If your workholding and your machine can handle it, I think you need to push that endmill much harder. I'd say your low chipload is creating a chip much too small to absorb all the heat created with the cut. Your tool loads up with heated aluminum and that's when bad things happen.
A coating on the endmill may also help decrease build-up as long as it's not AlTin-coated.
Flood coolant would help a LOT.
Sharp endmill, preferably one with higher than 30 deg. helix.
Try slowing your RPM down to around 2200 with a chipload of .004 -.006.
If mist coolant is your only option, you might need to reduce your RPM even more. But try to maintain the chipload. You also might need to use an air gun and blow the chips away from the tool while in-cut.
Cast Aluminum plate should be very easy to machine. Although I agree 6061-T6 does cut nicer.
Good luck

[tobyaxis]

1/2", 2-flute HSS and 3-flute carbide. Slotting. The carbide loaded up and broke almost instantly at only 0.325" DOC. So, I switched to the HSS, 3200 RPM, 0.175" DOC, 10 IPM with very heavy mist coolant. If I kept to that slow, shallow cut, I got no welding, but the finish quality was horrendous, and after cutting only about 24", the endmill was destroyed - badly chipped on all the cutting edges. I've used these exact same endmills at 0.5" DOC on other 6061, running the same endmill for months at a time, with excellent results. This stuff cuts like crap, and chews the tool into junk in minutes. I've never seen anything like it.

Regards,
Ray L.

6061 Cast is Gummy. Increase the RPM, Reduce Feed, with Shallower Depths Of Cut.

How are you holding this and what are the dimensions of the material your cutting??

[SCzEngrgGroup]

6061 Cast is Gummy. Increase the RPM, Reduce Feed, with Shallower Depths Of Cut.

How are you holding this and what are the dimensions of the material your cutting??

The workpiece is 3/8" plate, securely clamped to a large fixture plate - it's not going anywhere.

Regards,
Ray L.

[BobWarfield]

I cut a lot of MIC6 cast plate, which is similar. For you conditions, HSS 1/2" 3 flute full slot @ 0.175" DOC, I would use 3100 rpm and 45 IPM.

The cast really likes to chip weld. I usually get by with a strong air blast, but you have to keep the chips really cleared. I would not spare the chipload as I think the big chips will clear better, especially if they're getting coolant soaked. You might try without so much mist.

It sounds like something more is going on though. It just shouldn't be that bad to deal with.

Best,

BW

[SCzEngrgGroup]

I cut a lot of MIC6 cast plate, which is similar. For you conditions, HSS 1/2" 3 flute full slot @ 0.175" DOC, I would use 3100 rpm and 45 IPM.

The cast really likes to chip weld. I usually get by with a strong air blast, but you have to keep the chips really cleared. I would not spare the chipload as I think the big chips will clear better, especially if they're getting coolant soaked. You might try without so much mist.

It sounds like something more is going on though. It just shouldn't be that bad to deal with.

Best,

BW

Bob,

I'm curious how you come up with 45 IPM, especially for HSS. That's a chipload of 0.0048", which is way off the top end for any HSS tool I've ever seen a data sheet for. Have you actually cut at that rate? I've broken 1/2" endmills going far slower, so I can't reconcile those numbers with my experience.

Regards,
Ray L.

[The Engine Guy]

Today I tried to mill some 3/8" 6061-T651 cast plate. It was a disaster. Despite cutting MUCH shallower, and feeding MUCH slower than I'm used to in extruded 6061, it machined horribly, and destroyed two endmills in relatively short order. What is the trick to milling this cr@p?

Regards,
Ray L.

Hi Ray L

Been reading the posts and to be honest it sounds more like 5083 that 6061, to be fair I`ve never actually come across any 6061 in plate form, it is normally an extruded Alloy as far as I know!!

I`d be inclined to check with the supplier, I had a similar issue a few weeks ago, I ordered some 3 3/4" round bar 6082 T651 grade Alloy pre-cut to 2" billets, out of the 100 pieces 3 of them were a different material and I had exactly the same issues as you, luckily I was turning the pieces up on the Lathe first before milling and they just didn`t "chip" properly, I sent them back with the suppliers Rep for checking and it seems someone used some softer material to make up the numbers as it were, that did turn out to be 5083, really soft, I only turned one down to shape and had to change all my feeds and speeds to do it!!!

The other 97 pieces turned and milled fine so I think you need to go back to the supplier and check out the specification of the material!!

End of the day a spec is a spec, if it says 6061 T651 "on the tin" then the composition, hardness, heat treatment and stress relief should be the same regardless of the shape it comes in!!

Check the material specs here,

http://www.azom.com/Details.asp?ArticleID=3328

from these specs it should machine OK, if you use the same site to check the 5083 you will see it says very poor machining ability!!

Regards
Rob

[SCzEngrgGroup]

Hi Ray L

Been reading the posts and to be honest it sounds more like 5083 that 6061, to be fair I`ve never actually come across any 6061 in plate form, it is normally an extruded Alloy as far as I know!!

I`d be inclined to check with the supplier, I had a similar issue a few weeks ago, I ordered some 3 3/4" round bar 6082 T651 grade Alloy pre-cut to 2" billets, out of the 100 pieces 3 of them were a different material and I had exactly the same issues as you, luckily I was turning the pieces up on the Lathe first before milling and they just didn`t "chip" properly, I sent them back with the suppliers Rep for checking and it seems someone used some softer material to make up the numbers as it were, that did turn out to be 5083, really soft, I only turned one down to shape and had to change all my feeds and speeds to do it!!!

The other 97 pieces turned and milled fine so I think you need to go back to the supplier and check out the specification of the material!!

End of the day a spec is a spec, if it says 6061 T651 "on the tin" then the composition, hardness, heat treatment and stress relief should be the same regardless of the shape it comes in!!

Check the material specs here,

http://www.azom.com/Details.asp?ArticleID=3328

from these specs it should machine OK, if you use the same site to check the 5083 you will see it says very poor machining ability!!

Regards
Rob

Rob,

I would agree, except both pieces are clearly factory-marked "Alcoa 6061-T651" all over them. T651 is not extruded, but rolled, and stress-relieved by stretching. It also is apparently about 50% harder than 6061-T6, having a Brinell hardness of 95 vs about 65 for T6. It is odd that most of the references I can find indicate it should be no different from T6 in machinability, but that certainly is not what I'm seeing.

Regards,
Ray L.

[BobWarfield]

Bob,

I'm curious how you come up with 45 IPM, especially for HSS. That's a chipload of 0.0048", which is way off the top end for any HSS tool I've ever seen a data sheet for. Have you actually cut at that rate? I've broken 1/2" endmills going far slower, so I can't reconcile those numbers with my experience.

Regards,
Ray L.

Sure, I've cut at that rate, that's what I'm saying. Haven't broken any endmills doing it either. Heck I've done 30 IPM in mild steel with an HSS cutter too.

I've been through a bunch of such data sheets and factored them into G-Wizard. This is neither a crazy high nor a crazy low chipload for the application.

HSS will take quite a bit more chipload than carbide, so maybe you're thinking of carbide. The SFM more than makes up for it if you can spin the carbide fast enough.

Either way, what you're describing isn't a chipload problem, it's a chip welding problem so far as I can see.

Cheers,

BW

[SCzEngrgGroup]

Sure, I've cut at that rate, that's what I'm saying. Haven't broken any endmills doing it either. Heck I've done 30 IPM in mild steel with an HSS cutter too.

I've been through a bunch of such data sheets and factored them into G-Wizard. This is neither a crazy high nor a crazy low chipload for the application.

HSS will take quite a bit more chipload than carbide, so maybe you're thinking of carbide. The SFM more than makes up for it if you can spin the carbide fast enough.

Either way, what you're describing isn't a chipload problem, it's a chip welding problem so far as I can see.

Cheers,

BW

Bob,

Just when I think I understand..... The way it behaved, increasing chipload appeared to make things worse, as I was getting severe welding at higher chiploads. But I've decided to scrap the parts I made yesterday, so I'll use them for experimentations, and try what you've suggested, and let you know what happens.

Regards,
Ray L.

[BobWarfield]

I'm in the camp that says somebody slipped you a weird alloy. What you're describing sounds downright nasty.

Best,

BW

[SCzEngrgGroup]

I'm in the camp that says somebody slipped you a weird alloy. What you're describing sounds downright nasty.

Best,

BW

Bob,

OK, you've almost convinced me everything I know is wrong.... I just did a couple of test cuts - just air, no coolant, 3500 RPM, 40 IPM, and it worked reasonably well. The finish was very rough, but no clogging or welding. Now I just need to understand why....

I can accept that the heavier chipload does a better job of carrying heat away from the tool. But, as I said earlier, all the HSS data sheets I've seen recommend chiploads in the 0.002" range, which is why I was at the feedrate I was. I've always calculated RPM, based on tool diameter and SFPM, using 400 for aluminum. Then picked chipload based on specs, using 0.002" for a 1/2" HSS tool. Then tested to see how deep I could go, adding coolant as required to prevent welding. Certainly, going 40 IPM instead of 12 IPM will give me greatly increased productivity, even if the cuts are shallower, so I'm happy to go that way. But surely there's a trade-off in tool life?

I'm so confused.....

Regards,
Ray L.

[BobWarfield]

Ray, the old rule of thumb is too much SFM burns tools while too much Chipload breaks tools. What I take from that is that so long as you're not snapping the tools (and yes, I know you were from the welding), the higher chipload is not harming your tool life. Spinning the tool too fast is what's more likely to cut the life way down.

Now as to all they whys and wherefors, I am but a humble practitioner of an empirical sort. Mostly, I enter manufacturer's data in G-Wizard tables, make sure it uses the data properly, and then constantly check every example I can to make sure.

Best,

BW

[seniormachinist]

Was the material supplied as cast jig plate? If so it has finer grain structure, is more dimensionally stable,and machines like crap. Slower spindle speeds and feeds and oil based cutting fluids will help. If free machining is necessary, avoid jig plate.

[Jim G]

My .02 worth from experience.

They skimped on the heat-treat.

I used to buy extruded bar 6061-T6511 from Alcoa out of Arkansas.
I got a lot in 3000ft that was all over the map in hardness. Some pieces worked great, some were gummy as all get out and wouldn't turn in our lathe.
They were good about discounting it, but that didn't help the problem though.

I now buy Alcoa from Tube Service and haven't had the problem since.
They also package it up much better than the other place.

Really soft stuff, aluminum or copper isn't much fun to cut.

If you have a large enough piece, you might find some sections are harder than others.

Talk to your supplier.
Tell them it's as soft as playdough and cuts just as well too.
Maybe they'll work with you to replace it.

Good luck!
Jim

[The Engine Guy]

Was the material supplied as cast jig plate? If so it has finer grain structure, is more dimensionally stable,and machines like crap. Slower spindle speeds and feeds and oil based cutting fluids will help. If free machining is necessary, avoid jig plate.

Ahh, good thinking "seniormachinist", I had forgotten about that stuff, used some a few years ago, call it "tool plate" over here and it comes ready ground nice and flat, great for just drilling/tapping for clamps/fixtures/screws etc for cutting multiple parts which is what I used it for!!

And yes, you`re dead right, it is a nightmare to cut, drills and taps OK but as you say, nice and slowly does it for cutting and lots and lots of flood coolant with a couple of good powerful direct jets to wash the chips away!!

I was mainly using 8mm 20 grain Carbide 3 Flute with either 45 or 55 degree Helix, the 55 degree came out with quite a good finish using a 0.1mm finish pass!!

Ran at 3450rpm with a DOC of around 0.75mm and feed rate of 1200mm/min in a slot that had to go 12mm deep. Also had some pockets to do that were 6mm and 10mm deep.
So lots of shallow cuts which did work out slightly quicker than what I would normally have run, just means a lot more and faster machine movements!!!
Didn`t have any tool wear issues though, cutters lasted fine!!

Basically a case of throw all the charts/books away for that stuff, trial and error to suit your machine I think is the order of the day!!!

Regards
Rob

Stay :rainfro:
.