What's new
What's new

Need help with machining 6063-T52 angle extrusion.

gundog

Hot Rolled
Joined
May 31, 2004
Location
Southwest Washington USA
Is 6063-T52 machinable? I have been machining some parts from 6061 T6 and everything is going good I am using a Niagara 1/4" 2 flute carbide cutter same cutter with same feeds and speed 4" and the cutter is gummed up? Niagara gives a .002" chip load so that is what I have been doing 4000 RPM & 16 IPM feed. That has been working great until I started on this angle extrusion I dropped the depth of cut to .125" and it still gummed up. Any help would be appreciated I have destroyed 2 brand new cutters in short order. I am using a bed mill so no flood coolant just mist.
 
That shit is bubble gum. I hate it. It's also super easy to bend when you clamp it up, and it doesn't spring back at all.

Do you absolutely have to have the sharp inside corner?

I would much rather run 6061 angle. Ask the customer for an alternate material spec if you have that option.
 
I used to machine a lot of 6063 T6 but never any T52. I found lots of good flood coolant was necessary while being very careful not to get too aggressive with heavier cuts, it likes to gum up. You are in real trouble with the mister. I would try Destiny Tool Viper or Diamonback mills with their stealth coating, probably 3 flute so you can drop the spindle speeds a little, a rich mist coolant, and then play with how hard, or not, you can run the tool. Keep the chip load around .002" per tooth and play with slowing the spindle down. You just need to learn it's peculiarities and how to get around them. I have only tried one Niagara aluminum specific end mill, a 3/16" one, and thought it left a lot to be desired. It was not a free cutting mill, something you want with gummy aluminum, and a good coating. Probably Tib2 would work real well too.
 
I've done quite a bit of 6063 T52. I don't recall ever having a melt down or a problem..

Though that doesn't mean you aren't having one...

I HAVE had problems in 6061, where you get a shitty bar or a soft spot in some giant plate..

Drop the speed (your speed is already pretty damn low) and UP the feed.

Make sure your cutter isn't all beat to hell, and dull and causing the problem..

.002 a tooth.. That works if the material is at the proper hardness, and if you are gumming up, its
probably not.. FEED it.

You are running about 250sfm, you shouldn't even be moving fast enough to have a melt down.. IF
your cutter geometry is proper..


Isn't Niagra a MSC brand.. Which would mean its the cheapest POS they could find to overcharge you for?
 
My suggestion would be Harvey tool or an Imco streaker using a high concentrate of Oemeta coolant you
may have to use a paint brush to keep significant amount of coolant in the cut.

I just finished a 101 copper job with .030 slots it worked amazingly well....GL

I would start with a .01 per flute and .08 doc...If you get something working reply back..THX
 
Don't think I ever machined that temper in that grade. Yes Niagara is carried by msc, yes they are one of the more over priced pieces of crap around. Sounds like your running to fast for that feed, just a guess somewhat for that material, but for that rpm, DOC, at full WOC your feed should be around 30ipm.
 
Gummy ass material. If you do get it to cut, it will raise a giant burr. Tons of flood coolant (or better yet cutting oil) and a corncob rougher. Then finish with your Niagara finish endmill. If you leave ~.050" it will get rid of some of the burr. You are not going to have much fun with this job.
 
Why are you using this over 6061 t6? From what I read it's weaker then 6061 t6 and it's one benefit is bending it, but you say this is extruded angle, are you bending it? Are your cuts thru or blind?
 
6063 is architectural, it has a nicer surface finish and sharp corners on both sides. 6061 is structural, it has a radius on the inside corners and a mill finish that is not so clean.

Sometimes you want those sharp corners and the better finish for cosmetics.

But it is soft, gooey shit. Even fresh brand new cutters, especially drilling- I always get big burrs. It looks pretty, but 6061 is a lot easier to machine, at least in my experience. Maybe I just haven't figured out the secret.
 
I chose this material for the sharp corners the products are for my business but they are a new line of products one of the parts could be made from the other type material with the taper but one of them needs the flat inside edge. My ignorance on the material being that soft. I may try to cut it on my router I have a better mist system on it I regularly cut 5052 on the router. I bought the Niagara cutter from my local tool supplier. I use Onsrud aluminum specific carbide 1 flute bits on the router for profile cuts.

I am still in the prototype phase on these parts if I can't make this material work I may have to reevaluate the product line this is a real important part of the system.
 
Is it a thru cut? How thick? Maybe you could punch it. We have a decent size danly die setup, machine our own bottom and top punch and forming dies. We use it for making mostly sheet metal parts up to like 4", maybe a little bigger. Setup on a big arbor press we can punch up to 3/16" thick 6061 t6 with a decent quality cut. Typically use it on thinner aluminium, brass, and copper around 1/16" thick and that gives good looking cut.
 
Gundog,

I think you may struggle a bit with only having spray mist. Probably some experimentation with different fluids might lead to something positive.

The other thing that may really help is finding the right coating and geometry for your carbide end mill. I've had excellent luck with Helical (brand) end mils with their "Z Plus" coating.

I've been around a fair bit of 6063 machining, but alway ran flood coolant with a pretty high concentration of Oemeta.

PM
 
I am still in the prototype phase on these parts if I can't make this material work I may have to reevaluate the product line this is a real important part of the system.
gundog, you are really close by. I have a box of Onsrud end mills and drills, I'll see if there's anything that small in there. You don't need carbide.

I've got a 2 flute YG1 HSS if you want to try one. That's the cutter I'd be running. At least if you melt one down you're only out about $15. And you got another end. :D

Don't re-evaluate the product line for want of a better spray mister. Setup a twin nozzle, blast the hell out of the cutter. Drop the rpm if you have to, bump up the chipload, and get some chips flying. :)
 
Anytime I'm dealing with an exotic or rarely used material, I usually call Onsrud and ask one of their engineers. They've never steered me wrong (even when they say they don't a cutter that can help me but XYZ company might)
 
6063 is hard to cut without it gumming everything up. I would try an aluminum specific, high helix HSS end mill. As much coolant as you can muster up.
 
Isn't Niagra a MSC brand.. Which would mean its the cheapest POS they could find to overcharge you for?


If memory serves me correctly, they're part of Seco. I've always had great luck with their end mills, but I've never machined anything out of the ordinary with them either.
 
I am not stuck with using a 1/4" EM it is a perimeter cut so cutter size can be what I want it to be. I will post a top picture of the part I am trying to cut from this material. The 3x2 angle PDF is shown as one piece you have to use your imagination for the angle this is the part I could use the other type angle with the thicker web as only the top surface needs to be flat. The other PDF is a detail of both surfaces of the angle I need to use the inside of one surface and the outside of the other surface so the non flat area would need to be milled flat to use the inside of the angle. I may actually change this part to be made from 2 flat pieces and form a "T" which would be better than the angle but I am worried about strength bolting the 2 pieces I really don't want to have the expense of sending the 2 pieces out to be welded.
 

Attachments

  • Angle 2x2.pdf
    10.2 KB · Views: 156
  • Angle 3 x 2.pdf
    9.1 KB · Views: 224
gundog, I looked in that box, I have 2 brand new 1/2" carbide, long flute Onsrud, low helix 2 flute. One 3/16" same thing, but it isn't new and isn't very sharp. And various drills, don't know what size holes you are making. Also some new 1/4" YG1's I mentioned earlier and a couple 1/4" Niagara 3 flute high helix carbides.

There are 2 spare Kool Mist hose assemblies with nozzles, and a tank with a dual hose setup sitting here too.

You are welcome to try any or all of it.

I'm in the Pearl District in PDX, about 25 miles south of you.
 
gundog, I looked in that box, I have 2 brand new 1/2" carbide, long flute Onsrud, low helix 2 flute. One 3/16" same thing, but it isn't new and isn't very sharp. And various drills, don't know what size holes you are making. Also some new 1/4" YG1's I mentioned earlier and a couple 1/4" Niagara 3 flute high helix carbides.

There are 2 spare Kool Mist hose assemblies with nozzles, and a tank with a dual hose setup sitting here too.

You are welcome to try any or all of it.

I'm in the Pearl District in PDX, about 25 miles south of you.

Now there's and offer for a guy in trouble :)

Well done jancolic
 








 
Back
Top