Now I'm a believer; you can mill C1018 at 800 FPM

[Geof]

I needed eight 1.640" diameter holes through some 3/4" hot rolled steel so I figured I would be more daring than ever in the past.

Cutter 5 flute 1/2" diameter. (EDIT: some fancy coating but I forget what.)
Speed 6000 rpm which is about 800 feet per minute.
Feed 110 IPM which is close to 0.004" per tooth.
Depth of cut 0.025"
Engagement about 54% (0.27").

After four holes the first punch through created quite a fireworks display but the second two passes did not light up.

Immediately after the M30 I could grasp the cutter briefly in my fingers, the workpiece was barely warm and the chips had come off blue.

The cutter shows some wear but is still good for several more holes.

The last hole was the same size as the first as good as I can measure with a telescopic gauge and micrometer.

Probably the best approach would have been to bang a 1" diameter insert drill through first but I don't have one which is why I did helical interpolation from the start.

So now I will not be as sceptical of people who claim awesome speeds with coated carbides in steel.

EDIT: I forgot to mention air blast; very strong as close to the tool as possible.

[wms]

http://www.youtube.com/watch?v=BbY7VMBF7UI

http://www.youtube.com/watch?v=BbY7VMBF7UI

[Geof]

Originally Posted by wms http://www.youtube.com/watch?v=BbY7VMBF7UI

If you cannot do any better than pull up an advertising video to hijack a thread I suggest you go stifle yourself.

[mc-motorsports]

Originally Posted by Geof If you cannot do any better than pull up an advertising video to hijack a thread I suggest you go stifle yourself.

Have you met Geof? I was wondering where he went. He's back... LOL

Hey, what was your actual parameters on that?
Just a helical ramp at .025" pitch? 1/2" endmill on a 1.64" hole would have left a center to drop out... Assuming you did a helical plunge and did a 54% step over at .025" per level?

I'm a little confused. But you did peak my interest! I'm going to play with some TIalN tooling just for fun to see if I can save some time on a couple of production jobs. But the tool cost is 4x of what I pay for uncoated which would be fine concidering time is money, but mistakes will get expensive.

MC

[Geof]

Originally Posted by mc-motorsports ....Hey, what was your actual parameters on that?.....

He's back; more correctly coming from me I'm back, have been back for a few days. I went to the Galapagos Islands.

To answer your question (I hope);

I started with solid material no pilot hole or anything.

The first helical interpolation was at a tool centerline radius of about 0.25" at a plunge of .025" per circle running at 110ipm and 6000rpm. You can calculate the plunge angle.

Next pass was about 0.27" further out and the final pass was another 0.27".

I know these don't completely add up to the 0.82" radius needed for 1.64 diameter which is why I say 'about'.

I can pull the program out of the machine tomorrow.

[mc-motorsports]

Originally Posted by Geof He's back; more correctly coming from me I'm back, have been back for a few days. I went to the Galapagos Islands..

I meant the quick witted, crabby Geof Intenended with humor...


[/QUOTE]
I can pull the program out of the machine tomorrow.[/QUOTE]

No need, got it.

Where I come from, .25 radius initial helix, .025" per level, (probably) .025" pitch, 54% step over using 6000RPM and 110ipm feed.

I was just wondering. I'm going to play with coated endmills for production jobs, tripple the speed/feed sounds great, but mistakes will get expensive.

Thanks,
MC

[Geof]

Yes mistakes will happen. I was cutting a 1/2" notch in from the edge on the same part and there was an aluminum packing piece overlapping the location. No problem I thought I don't mind if the aluminum gets notched; WRONG the aluminum loaded up the flutes and things went downhill very fast. Didn't hurt the part beyond recovery but the cutter is unuseable with aluminum firmly welded into the end.

EDIT: Grouchy not crabby.

[lkenney]

This is what I have been posting about with SurfCam Velocity's True Mill and TiALN coated Carbide End Mills. No Coolant but air helps keep the hot chips out of the pocket.

Eagle

[miljnor]

ya aluminum Doesn't stand up to the same parameters when doing the awesome speed roughing, I found that out almost in the exact same way....cutting into an aluminum jaw as it was buzzing threw the steel piece.

Unfortunately for me, my steel piece wasn't savable.

Nice video even if it was advertisement though!

[Geof]

The opposite is okay; hitting a steel jaw with the cutter going like a bandit when cutting aluminum. I put a 5/8" wide slot 1/2" deep through the fixed jaw on a Kurt vise at 10,000 rpm and and 120 IPM. The embarassing part was that one of my guys was watching me. The interesting part was the cutter survived and could still cut aluminum with a good surface finish.

[lkenney]

Geof,

You should be able to cut your holes in a single Z cut and be fine. Saves time.

Eagle

[Geof]

Originally Posted by lkenney Geof, You should be able to cut your holes in a single Z cut and be fine. Saves time. Eagle

With a 0.500 diameter cutter and a 1.64" diameter hole on a Super MiniMill, how?