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

[lkenney]

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

[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

[Geof]

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.

[lkenney]

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

[Geof]

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.

[Donkey Hotey]

I'm not going to embed any videos and get stomped () 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.

[lkenney]

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

[Matt@RFR]

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.)

[Geof]

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.

[Donkey Hotey]

Greenleaf ceramic inserts

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

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

[tobyaxis]

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

[Geof]

But these also are insert cutters.