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

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.

;)

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

Quote:

---

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.

Quote:

---

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

Quote:

---

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.

Quote:

---

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

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. :D

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

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!

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.

Geof,

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

Eagle

Quote:

---

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?

Quote:

---

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.. :D :D

Quote:

---

Originally Posted by wms

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

---

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.

Quote:

---

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.

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.

---

Quote:

---

Originally Posted by Geof

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.

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.

Quote:

---

Originally Posted by WallyL7

.....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.

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.

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

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.

Quote:

---

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.

---

If you are referring to the video I made and posted:

The finish on the floor was about a 63 ..and remember this was a Roughing operation to remove the bulk of the material.... ;)

Can't speak for the other one..

Quote
I needed eight 1.640" diameter holes through some 3/4" hot rolled steel
Unquote

So we are talking about .75 depth cut which is 1.5x0.5 and opening the hole up to 1.640" diameter using the side of the end mill which I will assume has a 1" LOC. It works well with one pass for Z. I program these with Truemill and about a 72% engagement. make great cuts even on a light machine.

eagle

So Eagle, it sounds like you want to plunge all the way through before starting the helical rather than ramping down?

Best,

BW

I did a helical ramp all the way through, came back to the top moved to a larger radius did the helical ramp again then back to the top for the final one.

Yes an alternate method is to go through and spiral out and this spreads the wear on the cutter, but there is a problem. I am absolutely wonderful at hand coding :D but hand coding a spiral path could be something of a challenge. I have approximated a spiral by doing offset semicircles and increasing the radius on each one but even that involves a lot of coding when the radius increase is 0.025". Even coding sequential circles separated by radial moves out is a lot of work and the problem with this is that the radial move puts a big load on the cutter.

And I am d****d if I am going to learn writing macros or CAM just for one fixture.:)

I guess it gets down to how you create your programs. I never program on the machine and do all my coding with SurfCam Velocity. To do what I am talking about would be very diffcult to hand program.

Truemill does a helical plunge all the way through the material. I usually use a TiALN coated Carbide End Mill 0.5 Dia and with a 1" LOC for these cuts. Truemill then starts the side cut in such a manner as to never corner the endmill using what ever engagement that you think will correct, it defaults to about 72 degrees. If I am cutting pockets and not holes I like to use an end mill with a small radius on the tips.

The cutting patterns are weird and I would have never programmed in this manner but you always cut on the sweet side of the endmill so the removal is very fast and smooth. All done in the climb mode.

In long pockets it cuts a wide "D" shape cut and rapids across the open end, coming back to cut the edge patterns in sweeping cuts.

I never go over 35% on my load meter and my tooling lasts a long time. This is not for every cut but it is a great tool to have.

I know of shops that have cut their large hole cutting time by 80% by getting away from spade drills and reamers and just using endmills. I get tighter tolerances hole to hole than I have ever gotten before.

With faster machines and new tech tooling, I am convinced that this is the way we will all be doing things very soon.

If you have older slower machines like I do, I benefit from not working the machines as hard and being able to cut more metal faster and more accurately than I have ever been able to.

Eagle

I've been meaning to get a video camera and take some videos of some of the cutting demo's I've done...I think you can go a bit faster :)

Quote:

---

Originally Posted by MikeOD

I've been meaning to get a video camera and take some videos of some of the cutting demo's I've done...I think you can go a bit faster :)

---

Some day I am going to take videos set up a site to have them on.

I don't think I could have gone much faster productively on my setup. The first helical ramp into solid was pushing it because the cutter tips are entirely buried in metal and have no chance to cool. On the subsequent passes the engagement was less and cooling could take place.

I was thinking about the absolute fastest way to do holes like this and concluded it would likely be to use a coolant-through insert drill first, that would be a blink-of-the-eye operation. Then open the hole up to size by spiralling out with air blast and have the cutter extending below the part so the very tip is not doing anything at this step. Finally do a helical interpolation to take a tiny skim off and get the finished size using the so-far untouched tip of the tool. If I was doing several hundred holes a day I could get motivated but the job is done and I don't know when, if ever, I will want something similar.

SwiftCarb does a demo where they helical through .75" of A36 in Three spirals and then cut a 3" dia hole total time 90 seconds with a 0.5" 4 flute special endmil with small radiused cutting tips.. It is pretty slick. I don't have the power to drive things that hard but sure wish that I did.

Eagle

I am still skeptical of some of these demos. To me the key is how many holes can you do at that speed with the same endmill? As I mentioned several posts earlier I crammed a 5/8" high helix two flute through a hardened vise jaw and it survived so probably I could interpolate a nice hole in A36 very fast with the same cutter, but the key point could be a hole not several holes. Taking 90 seconds of time at the cost of replacing a $40 or $50 tool every five or ten holes may not be good economics.

I'm not going to embed any videos and get stomped (:D) but Greenleaf had a pretty impressive demo running at Westec last year. They were facing off something like 1/2" layers from steel blocks in the same manner. IIRC, they hadn't changed the cutter all morning. It was eye-opening stuff. I think those were ceramic inserts.

The thing that surprised me was how much more tool life I got when i started using Truemil, TiALN coated Carbides and I quict using the coolant.

Swift and Iscar both told me and gave me endmills to prove it with, that TiALN doesn't handle the thermal shock of going in heated up and out of the cut to being chilled by coolant. The coating will blow off the edges and the endmill will fail. I think I read that the coating doesn't really get slick until you get to 1400 degrees F..

When I quit using the coolant, (steel only) and took my heat off in the chip then endmills are lasting 2-3 times longer than uncoated carbides. I had to do a lot of unlearning to make it work but but it sure does. Studies show that most of us throw away 1/2 of every end mill we use. I am an R&D shop and do very little production work so I don't see the benefits from tool life that i might if I was doing repetitive work.

Some shops, I understand, keep a grinder on staff to stub off the dull edges and resharpen. I would like to do that but can't so this is better. I am using at least 3/4 od the cutting edges and making better time with smoother finishes.

I believe that a great many machinists have laid the foundations for these new methods with their hard work and clever programming. These methods use software, highspeed machines, new designs and coating for cutters as a package to allow more people to take avantage of faster, better machining than we would have without the skills that have driven every shop up till now.


Eagle

Quote:

---

Originally Posted by Geof

but hand coding a spiral path could be something of a challenge.

---

Geof, look into G12/G13. You could do those holes with two lines of code. First line is a looped G2/G3 to depth, then the G12/G13 line to spiral out, including finish pass (I think...maybe three lines of code to include a finish pass. I'm one of those know-nothing CAM programmers.)

Quote:

---

Originally Posted by Matt@RFR

Geof, look into G12/G13. ....

---

But unless they have changed things you need to pre-drill at the center.

Donkey Hotey...you are in a different ball game with ceramics and I don't think ceramic end mills are available yet. :)

:) Greenleaf ceramic inserts

:o Greenleaf videos (listed down the left side of the screen)

(this is why I spend two days wandering aimlessly at Westec)

You might find these videos interesting Geof. These are from Ingersoll.

One is actually Milling Inconel X750 at around 250 IPM.

Enjoy my friend:)


http://www.ingersoll-imc.com/en/ingersolltv/index.htm

But these also are insert cutters.

Quote:

---

Originally Posted by Geof

But these also are insert cutters.

---

Are you saying that I am Off Topic Sir?:)

Yes they are. I will see if Hanita has a video of of the VariMill End Mill.

Did a quick search, no luck.:confused:

Quote:

---

Originally Posted by tobyaxis

Are you saying that I am Off Topic Sir?:)...

---

I'll let you get away with it because you called me 'Sir'.

Insert cutters behave very different to solid end mills and it is not difficult to drive them at very high speeds and feeds. They are generally bigger and can take bigger cuts which means the heat departs in the chip more effectively. Most of the videos I have seen of inserts cutters being driven show the cutter just ploughing straight through not doing the scalloping type cut that works with solid endmills.

Quote:

---

Originally Posted by Geof

I'll let you get away with it because you called me 'Sir'.

Insert cutters behave very different to solid end mills and it is not difficult to drive them at very high speeds and feeds. They are generally bigger and can take bigger cuts which means the heat departs in the chip more effectively. Most of the videos I have seen of inserts cutters being driven show the cutter just ploughing straight through not doing the scalloping type cut that works with solid endmills.

---

SIR (LOL:))

Watch the Ingersoll Vids. There are some very nice Profile and Helical Cuts. All different alloys and cutting shapes.

Ahh...OK...I didn't know we were excluding insert cutters. Nope, no solid ceramic endmills that I know of.