Air or coolant?

[zedzero]

Ok so I'm old skool...been brought up on coolant for everything,just flood it, more the merrier type....

So some of the young fella's keep on asking how come I dont use more air to remove chips..

Anyway I've taken of the coolant pipe at the back of the progammable nozzle and connected a small compressor to the back and fixed up an extension in the pipe to bring it nearer the tool.

Bugger me it aint too bad,just feels kinda weird,wanna keep rushing to the keypad to press the coolant on button.

Just wondering...anyone use more air than coolant?

[Geof]

What are you machining?

I would never try air on aluminum alloys, but for most steel air can be better. Less thermal shock to the carbide can extend the tool life.

[wwendorf]

I use a fogbuster myself. Very little coolant, mostly air.

Wade

[PBMW]

Ijust finished a thousand parts in 4340 that I profiled with a half inch variable flute EM with a Altin coating. No coolant. 7700rpm, .3 DOC and 100ipm. I only took .075 radial doc cause I was only holding it by .05 in step jaws. Cuttier would run about a hundred parts.

[axis]

it all depends on the job that i am doing i have run just air in aluminum but its with a single flute cutter the thing is if you can use coolant it just makes life simpler than no using it. but not all jobs will allow flood coolant like ones with the door open or an open machine kind of suck with flood coolant. a mister could work for those but not all the time.

[pit202]

take a look here :

YouTube - Fraisa High Performance Milling 6061 Aluminum

YouTube - Fraisa High Performance Milling 6061 Aluminum

alu with no flood coolant.

[little bubba]

When you first start running dry, its a serious pucker, it just seems wrong, however when you realize how much longer your carbide lasts, and how much faster you can go, it makes sense.

What you need to keep telling yourself is that carbide can take heat, lots of heat, but it can't take thermal cycling, going hot to cold a couple thousand times a minute will eat up your tools pretty quick.

When I ran EVERYTHING wet, for good tool life 280sfm was tops in 1018 with carbide. Now, 500sfm to start up to 1100+ sfm depending on radial engagement, and better tool life, standard variflute TiAlN coating. Even uncoated will do better dry, though not as fast.

If you can get the coolant exactly where it needs to be constantly, then use it, however 99% of us don't have that capability.

On running aluminum dry, its something I don't do(I've puckered enough). Go over to the PM board, CNC forum, "murdering aluminum at 250ipm". Check the video, running aluminum dry on a Haas, 40+ cubes a minute. Explanation also.

[mc-motorsports]

Getting the chips out on aluminum and SS is by far the most important thing. High pressure coolant any day, second choice would be high pressure air with coolant mist, then just high pressure air, then drip feed coolant(low pressure). Just my 2 cents...

[Donkey Hotey]

Originally Posted by pit202 take a look here : alu with no flood coolant.

Okay guys, are any of the rest of you machining that fast (with or without coolant)? I watched that video and blurted out expletives not suitable for this forum.

I would have spent 10 minutes opening up that pocket in 6061: maybe 0.33D of XY engagement and 0.5D in Z at 40 IPM, 10K. That looked like 0.5D in XY and 2-3D in Z. I'm stunned.

[Geof]

Originally Posted by Donkey Hotey ......I would have spent 10 minutes opening up that pocket in 6061: maybe 0.33D of XY engagement and 0.5D in Z at 40 IPM, 10K. That looked like 0.5D in XY and 2-3D in Z. I'm stunned.

You are much too conservative. At 10000rpm with a 1/2" or 5/8: cutter I would take a depth of cut of maybe 0.4" and up to 100% engagement at 100 ipm on my VF2. I would expect this would give me around 80% spindle load.

Did you look at my thread about tearing into 6061?

http://www.cnczone.com/forums/showthread.php?t=52366

I noticed that the chips in that video were coming off in tiny fragments, much smaller than I see with the hig helx GAR cutters that I use. I suspect that might have been a variable helix cutter or a roughing cutter that has the helical grooving to fragment the chips.

[Donkey Hotey]

Originally Posted by Geof You are much too conservative. At 10000rpm with a 1/2" or 5/8: cutter I would take a depth of cut of maybe 0.4" and up to 100% engagement at 100 ipm on my VF2.

Yes, Geof, I saw that thread. But you wrote of vibration and noise. The video posted above was so quiet that you can still hear the hiss of the compressed air.

When I fully bury the leading edge of a tool, it howls and screams like crazy. I packed a few mills with chips doing the pocketing on those previously posted aluminum feet. I finally had to do them at 0.25" DOC to keep the 1/2" endmill from packing up solid.

0.005" per tooth? I'm about to start a job with lots of roughing in 6061. I'm getting a 1", 3-flute, cobalt bit for the job. I'll give it a whirl at 0.005-0.006 per tooth and get back to you.

[Matt@RFR]

Greg, my standard for roughing aluminum with a 1/2" variable flute 3 flute with a 1.25" LOC: 12000 RPM, 216 IPM, full DOC (up to the full 1.25" LOC) and .180" stepover... All while holding in an ER-32 collet. That only gives me about 50% spindle load and I've never loaded an endmill up. I think that's around .006" IPT (I'm not in the shop right now), and if I had a mill chuck I'd push the feed to .008" IPT. I've tried it in a collet but the endmill gets pulled out.

At the same feed and speed, I will go up to .480" stepover but at .250" DOC for some pockets. It'll slot just fine like that too. Be prepared for your doors to not open very easily after a few minutes of this though.

Do you have TSC? That's what I use in deep pockets or when I'm worried about starving the cutter when on the left side of a profile.