Carbide tool life?

[ozzie34231]

I'm in the process of milling some quick change lathe tool holders.
My machine is a Shoptask.
I'm using a solid carbide 1/2" mill, not coated, running at 1300 RPM, 5 IPM, Depth of only .025", water soluable coolant. I just finished the main slot in #5 of 13 work pieces, and the mill needs to be changed. I figure I've milled about 1000 linear inches at the above specs.

Is that normal wear, or are my speeds and feeds off enough to cause excessive wear?

Jerry

Oh yes, the workpieces are A2 and A10

[HuFlungDung]

Being as it is uncoated, that does not work in your favour. Coatings make a big difference when milling steel.

Water soluble coolant needs to be applied in flood conditions when using carbide, and even then, if flow is interrupted to the tool, it can cause cracking and thus premature failure of the carbide.

Your feedrate is maybe a bit light, but then, so might be your machine. A heavier machine can use a heavier feedrate, and the result is less wear per inch of cut.

It sounds like you've done pretty good with what you've got.

The sharp corners of the tool may be gone, but if you have a green stone (or natural diamond), you might be able to continue to use that tool as a rougher, if you can chamfer the worn/chipped
corners properly so as to give proper clearance. This involves grinding a relief chamfer all the way from the cutting edge, around the periphery to the back of each flute. Might be a challenge, but if the tool is garbage anyway, what can it hurt, especially as a rougher.

/me runs away in case Camminc sees this reply

[ozzie34231]

Okay, cool, thanks. Coolant flow has always been good flood.
I never consider a mill or bit junk unless it breaks badly. one of these days I'll finish designing my CNC sharpening grinder, (already collected a few diamond wheels).

Jerry

[ozzie34231]

If one were to try increasing the feed or depth of cut by say 20%, would one be more advantageous?

[HuFlungDung]

Sure, whatever power and rigidity your machine has available, use it to the max, then back off a bit

Just to give you an idea, lots of guys would run that tool (well, a coated version) at .25" deep, and maybe 2400rpm at .010" or more feed per tooth. So you've got lots of leeway yet, but limited by your spindle horsepower and rigidity of your machine and setup.

However, since this tool is not quite the right one for the job, its better to not push it too hard in case it chips in mid cut. When the tool gets damaged, then it starts to put a lot more stress on everything until you notice there is a problem.

[ozzie34231]

So, would you say that by babying the job, I'm paying a price in tool wear?
In other words, by going faster and harder, it is possible that I'll remove more metal before the tool wears out?

[HuFlungDung]

Well, with a coated carbide of the proper grade, yes you should feed faster and at a greater depth of cut. Using an uncoated grade in steel though, it's impossible to give a safe recommendation because the tool is so much more prone to unexpected failure.

[ozzie34231]

Yes, but my question is;
assuming the machine and motor can handle the cut, and assuming the mill doesn't fail by breakage, can I remove more metal with a given bit before it WEARS OUT, by going faster and harder?
Let me put it this way. As a mill tooth passes through the metal, does a .005 cut wear the tooth five times as much as a .001 cut or not that much.

Also what is the effect of spindle speed on the mill, (assuming one can keep it cool). Does faster, wear the tooth more, or less?

Thanks for your help,
Jerry

[HuFlungDung]

Too light of a chip will wear the tool faster than a heavier chip, because the edge spends more time rubbing on the surface before it finally penetrates. Yes, a heavier feed will allow you to remove more material, before the tool is worn out.

Think of it in terms of rub cycles: the tool rubs every time it takes a chip. Within its strength limits, the tool could care less how heavy the chip is after it has begun to penetrate the material.

[ozzie34231]

Many thanks.
One last question about the subject. I presume that depth that is just a matter of rigidity and horsepower. Are there advantages to lighter or deeper cuts other than the obvious time saving of a deeper cut?
Jerry

[little bubba]

I would guess that you are going way too light on the chipload, if your running a 4 fluter, less than a thou per tooth, that would put you more in the pushing instead of cutting range. I would shoot for a bit more feed, at least a thou per tooth, minimum. On the depth of cut versus more feed, your using .025 of the endmill, that leaves a whole lot of sharp flute above that. I would say, unless your running on a mini mill, that you should have no problem taking a deeper cut. Another thing I've learned along the way, on some long run jobs, is that you will find there is a wall were your tool life just drops signifigantly, and if you back off from that about 20%, you'll get virtually unlimited tool life. On the other hand I had one job in A286 were the wall was at 140sfm, backed off to 100sfm and got about 100 minutes of tool life, bumped up to 130 and got 300 minutes of tool life(same chipload), wierd.

I guess I'm in disagreement here with some people on coatings, on that A286 job we had the opportunity to ruin many many many endmills and I kept track of tool life, feeds, speeds, etc, and very consistantly the TiAlN coated endmills gave 30% less tool life. I'm sure that had a lot to do with the material though, almost everything else I've worked on lately is too short of a run to get a good gauge on tool life.

Another thought, have you considered using roughers? A lot less cutting force. My general rule of thumb (I came up with this myself through expierience) is that a rougher will give you about 3X the metal removal of a finisher and that carbide will give you the same advantage over HSS or Cobalt. Therefore, a carbide rougher (I love these things) will give you about 9X the metal removal of a HSS finisher.

[DareBee]

In regards to cutters and coatings. I recently ran a 200 part run which had 1.5 holes at 1.5 deep. I neede some cutters. After looking at carbide coated with TiAN ($180), which is my normal cutter, I decided to try a Niagara TiCN coated HSS ($35) instead.
I was amazed at the life of this cutter!
IMO the TiCN coated HSS lasted longer than an uncoated carbide would have. I bought 3 cutters and did the job as well as the test and tune (had some significant squealing for a while) with just 1.
For the price point I still will only recomend coated carbide for .5 dia or less.