Milling 6061-T651 Cast Plate

[HimyKabibble]

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.

[HimyKabibble]

Originally Posted by 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.

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]

Originally Posted by HimyKabibble 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?

[HimyKabibble]

Originally Posted by tobyaxis 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]

Originally Posted by HimyKabibble 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??

[HimyKabibble]

Originally Posted by tobyaxis 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

[HimyKabibble]

Originally Posted by 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

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]

Originally Posted by HimyKabibble 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

[HimyKabibble]

Originally Posted by The Engine Guy 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.