[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]

[ame="http://www.youtube.com/watch?v=BbY7VMBF7UI"]http://www.youtube.com/watch?v=BbY7VMBF7UI[/ame]

[Geof]

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]

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]

....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]

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]

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?

[wms]

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

Well Geof sorry you feel that was..It wasn't an advertisement on my behalf..Just a video I grabbed off the web to add to the discussion..

I have made a few videos myself in my shop to test High Speed stuff..Remember I run a shop just like you..I make a living Cutting chips..

Here's One done On My Haas Standard MiniMill...

High_Speed_Video_wms

Off to Stifle Myself..What ever that is..

[Geof]

....Off to Stifle Myself..What ever that is..

It is an Englishism and it means stop talking, or in the context I used it stop posting.

You triggered a sore spot by taking something from somewhere and posting it rather than posting something arising from your own effort.

I know I am an irascible old coot but that's what comes with advanced age. Thank you for responding in such a gracious manner.

I think I had seen your video, or one very similar, and it shows what I suspect is a crucial thing for this kind of cutting; the tool is only in contact with the workpiece about 50% of the time and is being cooled by the airblast half the time. This kind of tool path is simple in CAM but hand coding it completely impractical. My competence does not extend to CAM which is part of the reason I have never played around with these high rates before.

[mc-motorsports]

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.

It is an Englishism and it means stop talking, or in the context I used it stop posting.

You triggered a sore spot by taking something from somewhere and posting it rather than posting something arising from your own effort.

I know I am an irascible old coot but that's what comes with advanced age. Thank you for responding in such a gracious manner.

I think I had seen your video, or one very similar, and it shows what I suspect is a crucial thing for this kind of cutting; the tool is only in contact with the workpiece about 50% of the time and is being cooled by the airblast half the time. This kind of tool path is simple in CAM but hand coding it completely impractical. My competence does not extend to CAM which is part of the reason I have never played around with these high rates before.

That program was written with MasterCam or something with HIGH SPEED MILLING opps. Cheaper CAM systems don't offer tool paths such as that. When it's cutting the half moon profiling the slot, it's should also be lifting the endmill a few thou to further cool the tool and brings it back to Z depth to prep the next cut engagement. And yes, damn near impossible or atleast absolutly not feasable to program by hand.

[WallyL7]

Sorry to continue with the video talk, Geof. (nice job on those holes, BTW)

But the floor of that pocket looked very bad. I couldn't let that part leave my shop looking like that (unless the print was calling out for scallops)!!!

Sorry I hate sounding like a pompous ass here, but I had to mention it.

[Geof]

.....But the floor of that pocket looked very bad. I couldn't let that part leave my shop looking like that (unless the print was calling out for scallops)!!!

Sorry I hate sounding like a pompous ass here, but I had to mention it.

What floor? What pocket? It was a through hole.

Don't feel bad about sounding like a pompous ass, you are nowhere near my level. I take pride in it.

Later on I will post what I am making; the part was actually two lengths of hot rolled clamped either side of a piece of 1/2 cold rolled. These will form the jaw sections of a fixture for holding a bunch of round parts.

[WallyL7]

Sorry Geof - I hinted at bringing back the video discussion (regretfully) which is what I was referring to regarding the floor of the pocket. Not your through holes.

It was right around 3:30 of the video - could have just been the light, but it did seem the floor was iffy... If it was just the light, then mybad - nice vid.

On a similar note - Geof, I cut a big chunk of T1 yesterday for a tractor...Seemed pretty fast at 11 ipm and 1100 rev's with a 5/8 Z-carb. No coolant and plenty of sparks on breakthrough!

Fun stuff - thanks for the post, Geof.

[lkenney]

Geof,

By taking your z cut all the way through the stock with your helical plunge before starting to open the hole. You are only using the side of the end mill with no drag on the end cutters that way. I cut routinely 1.5 x dia of my endmills in 1018 and 4140.

Eagle

[WallyL7]

Look at his hole diameter - he needs 1.64" with a 1/2" tool. 1.5 times the diameter is, well, not 1.64"

I think he is doing what you are saying, starting smaller, then opening them up.