How deep with a .375 Carbide cutter.

[Ken_Shea]

Need some advice on the following.

Particulars:
.375 carbide 2 flute
4140 annealed steel
Profile cutting
Final cut at -1.375
.050 DOC each pass

I have never used a .375 carbide to profile this deep and they are expensive enough I do not want to break one learning by experience.

Is 1.365 asking to much for a .375 carbide?
I could use a .5 and make a finish pass with .375 to finish the actual profile.

Thanks
Ken

[WayneHill]

I would recommend using a .500 rougher before the .375 finisher.

1.365 depth with a .375 endmilll? How tight are the gibbs on your machine?

[Ken_Shea]

Thanks Wayne,
I have been thinking on this further and agree, no need to use a .375 when I can use a .5 , the .5 will not fit into one of the areas but will remove most of the material in that area and then just clean up with the 3/8", could plunge these but they are odd ball sizes of which I do not have a end mill.


The machine is more then up to the task, just not using the cutter I would prefer.


Ken

[Rekd]

Go with a 3/8 or 1/2" verimill.

I'm running one now at 35ipm in 303 .125 deep cuts per pass, dry, roughing and finishing with the same tool. This same tool has been running (dry) for over 47 hours straight, and so far it has barely worn down a little bit of the coating. Still sharp on all edges/corners. Did I mention it's running dry?

BTW, I'm taking it easy on the cutter, I have 4 6" vises holding single bars that get seperated into 4 parts per vise, so I don't want to toss any of the parts as they get seperated.

Not bad for a $25.00 tool, eh?

'Rekd

[Ken_Shea]

Very impressive performance, where are the verimill available ?

2,3,4, flute?

Why the running dry?
Not questioning your methods Rekd since you can ascertain by my post that I have little machining experience, just wondering why.


Thanks
Ken

[Rekd]

Hanita makes the varimill. I'm still (ab)using that .375 4 flute on a different steel job.. Even after it loaded up on this job, not once, but twice and thrice.. and again! The 'once' and 'twice' times were with molten alum mixed with the sst during the setup. It wasn't me though, it was teh boss. We chissled it out and kept on cutting. Didn't even wear the coating down.

I had to (today) lower it 1/4" to get around some chipping that started to appear. On this last job it's doing a +-.0025 dia hole at 36 ipm. Prolly about 80 or more hours on this single tool so far, which cost less than $30.00.

I burned up a couple of them, (demo's ) a 3/8 and a 3/4" 5 flute by running 'em with coolant. Once I turned off the coolant and layed into the feeds it ran like a bat outta hell. I think it has something to do with thermal expansion, kind of like ceramics, but that's just a guess.

They make (I think) 2, thru 5 flute standard and long.

I'm real happy with this one I've been (ab)using.

[Joshman]

Hanita Varimill's are the best no doubt. I use them all the time also. I machine mostly free machining steel and run them at 800sfm and .002 per tooth. comes out to 6100 rpm and 70ipm. pretty awesome to see.

[DAB_Design]

We just started a couple of large titanium (6-4 and 6-6) jobs, and decided to try the verimills out on those. With the right conditions, they run great! Just try to use the shortest LOC you can, and keep the length as short as you can also.

We are using some extended shank verimills also on the same jobs, and have to say that their performance is just 'ok'. But with 5+ inches of stickout, 5/8 - 1.25 LOC (depending on diameter), I guess you can't ask for much. This is taking small finish steps. 'Small' being .05 or so side cutting with maybe .375 stepdown, and also around .05 deep cuts on floors.

What's with the chamfered corners on some of those? There are some of the .500 diameter verimills that come with a .02 chamfer rather than a radius. Seems to me that a chamfer would break down faster than a radius, as there are 2 corners. In my experience, corners (0 radius) always breakdown faster than any radius.

[metlmunchr]

Re the dry cutting.....A guy with Dapra told me they had run high speed videos of their carbide mills and found the cutter acts like a fan if it's running fast, and that its literally impossible to keep coolant on the cutter in sufficient quantity. Even with several nozzles converging on the cutter, only enough coolant hits the cutter to cause thermal shock and not consistent cooling. At the time, I was running a 1" ballnose insert cutter on D2 at Rc60+ doing a die rework. They recommended 5000 rpm and dry cutting, with an air jet sufficient to keep the chips clear. Worked great with good insert life. Being the brain surgeon type that I am, I had to try it with coolant anyway. Insert life dry was about 1 1/2 hours. With coolant......10 minutes and it looked like the edge had been beat with a hammer and chisel. Another of my theories shot to hell

[Mouldmaker]

We used coolant on our carbide cutters in the past but they used to wear too quickly. Since we are running them dry now (on tool steels), we dont have this problem anymore. The sales rep told us that by continously heating and cooling the carbide cutter one would anneal the cutter leading to wear in the edge.