[webgeek]

I know Halloween was a month ago but you'd think it was this afternoon in my garage. I've finally got around to hooking up my flood coolant and setting up vises, a tooling plate, etc. So I got all this set up and try to cut. It comes out so bad it's embarasing. Here are the specs...

12" x 24" .09" 6061-T6 aluminum sheet from Speedy Metals
Speedy Metals - .090" 6061-T6 Aluminum Sheet
0.25" 4-flute HSS endmill - brand new
.025" depth of cut
25 IPM
SynKool coolant

And here is a video showing the monstrosity:
[nomedia="http://www.youtube.com/watch?v=wiee3GQAEoQ"]YouTube - Beaver Nibbling Some 6061 Aluminum[/nomedia]

Any suggestions? I've never cut the plate before, always just small flat stock and I've never had anything gum up this bad. I tried this same metal with a BRAND NEW .25" 3-flute Maritool carbide bit, a lightly used 2-flute .25" end mill as well. I also tried from as slow as 20 IPM (MUCH WORSE) and up to ~35 IPM (no visible improvement).

Thanks in advance for the help!

-Mike

[dertsap]

heat
looks like a melt down problem caused by plunging a 4 flute
its clear when the tool rises in the z that there is aluminum stuck to the tool , best bet is to ramp in and use a 2 or 3 flute

[MrWild]

What Derstap said. 4 flute sucks for aluminum, but it also seems like that isn't 6061. Acting gumming like 50 series.

[webgeek]

Thanks for the quick replies!

looks like a melt down problem caused by plunging a 4 flute

The tool isn't plunging, it's actually ramping in along the cut path (a cool feature of Visual Cam). I've attached a screenshot of the cut level setup for that part. I might be misinterpreting the settings for this screen so please check it out. The "burning" of the bit occurred in a blink of an eye as it started ramping in even with coolant washing over it.

You guys mentioned this is a problem with 4-flute bits but I tried with both a dirt cheap Enco 2-flute bit and a nice carbide 3-flute endmill specifically designed for aluminum from Maritool and in all cases the behavior was the same. Ironically, the 2-flute junkie bit easily out-performed the expensive carbide bit. All of the results were terrible though.

Should i be using the carbide and running LOTS faster? I just can't seem to get this aluminum to cut. It's labeled 6061 right on the sheet but this cuts far worse than anything I've run into so I assumed it was me. Can there be something wrong with the metal?

-Mike

[foam27]

Quality carbide 2 fl, lower spindle speed, higher feed rate, go less on the depth of cut.

If all else fails, start at .005" DOC and increase DOC until quality degrades, then back off a bit.

my 2 cents.

[Geof]

It may be a low temper. 6061 is an alloy that is normally age hardened, it is done at a moderate temperature for a few hours. In the tempered form, normlly something like T655 it is very difficult to bend so sheet and plate stock is available un-tempered (T0) for applications that require bending.

T0 is horrible to machine beause it gums up the cutter. Definitely use a two flute cutter at a very high rpm. You could run a 1/4" cutter at 20,000rpm with plenty of coolant, a slowish feed such as 0.001" per tooth and it should machine okay.

[woffler]

I agree, i cut 6061 all day long i use a three flute end mill 3/16 coated i use a small depth of cut .05 ,9500rpm spindle speed 29 to 30 inch per min feed. and cut through 5/8 material with more corners and angles and several radius's there is something wrong with the material as suggested by Geof there is no way your cutting tru 6061 from what i saw in the clip.I have had a material mix up from suppliers before that has been mis marked at factory try a different supplier for a known source .

[woffler]

I ran your feeds and speeds threw the calculator i use that has a lot of variables figured into it and this is what i came up with, 6000 rpm ,depth of cut .025, width of cut .25, feed rate should be 28.8 inch per min. ,plunge rate 14.4 per minute ,tool deflection .0003 using a 2flute high speed steel end mill should give a good cut with no chatter.

[1%biker]

Hi there

I rout aluminum daily on a multi-cam 5000 series machine. I have found single flute Onsrud cutters the most superior cutters I have ever used. I would recomend using single flute cutters combined with Boelube coolant on modern routing machines. On soft alloys I use High spindle speed and a slow feed rate combined with mist coolant (Boelube liquid). My best results for 6061 use Spindle speed of 21000 rpm feed at 39.37 ipm. Soft alloys are always difficult to machine cleanly. What ever cutters you use I would suggest using the cutter manufacturers feeds and speeds reduced by 1/3. this generally works for me. Depending on machine, work holding, coolant and cutter you will only achieve good results by trial and error. Hope that is helpful.

Jim

[Don-in-Japan]

I only use SpeedyMetals 6061 flats on my little A2Z cnc machine.

25 IPM at around .020" 2800RPM dry cuts with plenty of plunges, and have no problems. (I only use the discount 9/64" 2 flute HSS end mills from Victor machinery).

My many failures at machining aluminum tell me it doesn't machine at all like 6061, and may be mislabeled. It screams too soft.

My 2 yens' worth.

[fizzissist]

I cut 6061 T6 all the time, and your video makes it look like the material isn't in a T6 condition or the cutter has flank wear. Surface scale??

The Dataflute carbide endmills have given me awesome performance (I'm not a rep, just a happy customer), so I'd recommend their 2 flute stub ARF style in a C5...
ARF-ST-20250-32857
http://www.dataflute.com/catalogs/da...atalog2006.pdf

You should be able to run it at over 800SFM, .002 feed/tooth, all day long...12,000rpm, 48ipm

One BIG caveat....get that coolant focused and right on the cutting channel, so you get those chips outta there! Looks like you're hand-holding it. Make a clamp so it's consistent.

If the material is ringing, as thin stuff is prone to do, consider a heavy ring if you can that will sit outside the cutting zone that will weight down and dampen the sheet, and give you something extra to clamp onto.

......One other thing....Change that ramp angle down to 3 degrees! 10 is too steep.

When you're done, do another video!

[Cruiser]

The four flute is the root of your evil ! The 4flt doen not have enough room within the flute chanel to carry the chips from the heavy feed rate. they curl up and fill the channel then rub and melt. As the others are saying drop to a 2 or 3 flt designed for alum and you will see the bigger open area for the chips to flow in.

[mactec54]

webgeek

You have a lot of good replies, but there is only one that is most likely going to work for you

Don-in-Japan Has the best answer, when you have a problem like this, get the spindle RPM down 2800rpm is a good starting point with a .020 to .030 depth of cut feed start at 12 to 15ipm & It does not matter if you have 1 flute or 6 flute you will get it going just fine by doing this

[SORCHEROR]

a 2 flute non coated carbide endmill high helix data flute or similar,3000 rpms 25-30 imp
and will cut beautiful,trust me,have to climb cut also

[Jaxbubba]

Use a 2 flute High Speed Steel High Helix for Alum with Gold Coating, and you could probably cut this material dry. I would recommend that you use flood coolant if you have it or mist. The Gold Coating keeps the chips from sticking to the cutter. Start at 3500 Rpm with plunge at 20. and feed at 40. ipm, don't give the material time to get hot and try to stick. Just my opinion after
35 years of machining aluminum

[RalphWilson]

I watched and right off the bat I see two things wrong with this.
I had to laugh , been there did that.
Your melting the aluminum as you go. your making it happen.
Just stop and think about what your doing.

Your done before your starting, you plunged that cutter into the work piece and it was not a center cutting end mill;
After it got a glob of aluminum stuck in the center, and commenced on with out a care in the world as you boiled the coolant out and away from the the cutter that was not really doing anything but rub and rub it;s way down into the cut: thus melting instead of cutting.

I like to do that with a ban-saw cutting thin sheet 304 stainless, crank up the speed and just melt the stock out of the way.

Ok forget what I said below except one thing.

Chip load and speed.

4 x Cutting speed / cutter dia.

cutting speed for al is between 600 and 800 sfpm.
and a chip load of .01 and .015 per tooth for a face mill or inserted end mill.


Imagine a lathe not a mill , chips not strings.

speed or RPM's times chipload times teeth = IPM
7500X.01X2=150 IPM

Now if you max safe feed rate is 90 IPM then you got to adjust you speed to go with it right?
Well no it just means that you need to figure Your right combination of feed and speed.

if you say you got a 20k spindle then you got a wimpy feed rate.
it's just the facts.

Make a chip.........








Been cutting a lot of aluminum lately, the stuff it labeled incorrectly.
But some of the reply's you got were wrong, and some were right.

You got the famous "gig plate 6061 T515"
I been cutting it at 7500 rpms .200" deep ramp and 80ipm with a 3/4 3 flute twisted l flute end mill and straight side cuts at 1 1/2" deep taking .02" I also use the turn ramps off; it slows down in the corners.

Figure your max spindle speed and figure a .010" to .012" per tooth.
Tons of coolant, not on the cutter but the leading edge, also spend a little money on a old cutter, you can sometimes get them for nothing and have them resharpened, tell the guy to coat it with the good stuff and that you plan on using it only on aluminum and have the proper clearances ground so you can go the next step to max spindle and you need to do a little reading about setting your machine to monitor spindle load,

Or just get a inserted tool two inserts and holder will be around two hundred.
Max spindle just about max feed.

[UncleDonut]

Not to sound like a jerk or anything, but is it possible that the spindle was rotating in the wrong direction?

-Dave

[jhovel]

I'm with one of the other repondents: as soon as I saw the youtube clip, I said to my son: he's running a left hand cutter...
That looks distinctively like melting it's way through backwards......

[webgeek]

Ha ha, you guys are as amazing as always. Pardon me for a moment while I dig up a huge helping of humble pie. While enabling my coolant, I had to disable the spindle relay. I eyeballed things and everything appeared to be working properly making me think the relay was unwired to anything. Except it wasn't. The spindle was spinning CCW. Hell, I didn't even know my mill could spin CCW. Apparently this means the relay is necessary to kick things in the right direction. So that explains all the bad cutting. Thanks for the catch guys. I won't make this mistake every again

Sadly, this does mean there is still something wrong with my coolant relay as when it's enabled, the spindle doesn't work properly via M codes. I'll be calling em about that tomorrow.

Thanks much for all the help everyone!

-Mike

[Don-in-Japan]

CW rotation usually helps the cutting process

Forums are awesome tools for ideas (group)