What's new
What's new

Roughing end mill help

SamS

Plastic
Joined
Feb 28, 2018
I haven't had much experience using a roughing end mill in a cnc machine previous to this part so I am a bit in the dark on how to run it. We have a lot of material to remove so it's important I get it right so we don't burn through tools! The material is 4140A, the set-up is not an issue, plenty to grab by in the vice. I am using a HSS 3/4 diameter x 1-5/8 length roughing endmill, machine has 20HP. I am side milling, the required depth is 1.5 inches. My initial numbers are 1.5 axial depth of cut, .116 radial depth of cut, speed 500 RPM and feed of 6.6 ipm. After the first piece the endmill seems to be cutting fine but already looks a bit worn, should I not be taking the full 1.5 inch depth at once?

Thanks for your help!
 
I would guess that you could bump up your feed considerably with that little radial engagement. Have you looked at the manufacture recommended speeds and feeds?
 
Are you cutting through mill scale? Your numbers aren't that far off maybe a bit more feed. Coolant?
 
I think you might be running a little too fast. Does your em have a coating? Sounds slow but I think 350 rpm and 5.0 in/min would be where I would start. That's .0039"/tooth and 64f/min.
 
One problem with not taking the full 1.5 depth is that you wear out the end of the flutes before the rest of the cutter is done. I'd go full depth.
Years ago, I had to use long 1.5" diameter roughing HSS mills on a weldment. I think the cut length was 6". Anything carbide we had was too short or ran too rough.
Just keep a good flood of coolant on your mill or it "could" weld to the part.
(Ask me how I know.....)
 
Wow guys thank you for all the quick responses!
We are using plenty of coolant. I think we could use a larger radial engagement but I am forced to feed into a corner so I was afraid it would be too much engagement in the corner. Not using carbide because I don't have much experience with this type of cutter and didn't wanna blow up an expensive tool! The chips look good (at least from what I can tell), small and silver, no crazy colors. The endmill does not have any coating on it, we just ordered something fairly cheap from MSC...so our cutter could be the problem.

We aren't cutting through any scale, it is a nice squared block. We have a lot of material to remove: 1.5 x 4 x 3.5 twice on 22 pieces (approximately, from memory)
 
Quality doesn't cost, it pays.

Are you leaving an island or facing? I'd almost say you should just plunge mill with the proper size cutter.

Let's be real with ourselves for a minute, a cheap uncoated hss endmill is not going to last long in 4140...let alone 22 pieces worth.
 
That is probably a max depth condition for a tool that diameter. I'd go for a 1" solid carbide rougher from Maritool. That is such a sweet cutting tool I wish I could use it more. Plus, it's carbide: you can get something done in an hour!! ;)

I had a bunch of 3/4" HSS roughers given to me, so I used them up on a job. Surprisingly, those would keep cutting when they looked like they were getting pretty dull. But with HSS, you are wasting time running too slow, that's got to add up to cost savings using carbide when the metal removal is serious.
 
Part starts as a rectangle and when its done it is an L with the large leg of the L against the back jaw. So it is sounding like our issue is the tool mostly. Would I run similar numbers with a carbide rougher or coated hss?
 
Part starts as a rectangle and when its done it is an L with the large leg of the L against the back jaw. So it is sounding like our issue is the tool mostly. Would I run similar numbers with a carbide rougher or coated hss?

If you go for the beefier carbide tool, you can increase the feed rate. This more than makes up for having to run the rpm lower than for a 3/4" endmill.

For me, a lot of what guides my choice of feed rate is how the machine setup reacts to the cut, If it is purring along, you feel comfortable increasing the feed. So don't limit yourself with a tool too small when the situation allows for the sturdier tool.
 
Looks like you are only removing 1.2 in^3 per minute. I should think you could do 10x that with your 20 HP, using carbide tools and HSM toolpaths. I would suggest commodity 1/2" 4- or 5-flute straight endmills instead of much more expensive 3/4" endmills. HSM parameters are readily found in this forum for the asking.

Regards.

Mike
 
If you go for the beefier carbide tool, you can increase the feed rate. This more than makes up for having to run the rpm lower than for a 3/4" endmill.

For me, a lot of what guides my choice of feed rate is how the machine setup reacts to the cut, If it is purring along, you feel comfortable increasing the feed. So don't limit yourself with a tool too small when the situation allows for the sturdier tool.



I agree. If you were using 3/4" carbide endmill, your feed could easily increase 2 to 3 times. Most machines will run out of HP before maxing out a 1" carbide so you're still limited. But for tool longevity and rigidity in cutting steel, you can't beat it. For 22 parts it's worth spending the $100 up front. 1" carbide? I can't imagine my 15 HP spindle being able to make full use of it.
 
I'm going to be a dick..

That's 1.15 cubic inches a minute.. About a 1hp cut.. On a 20hp machine.

You might as well sell the damn machine and buy a hammer and chisel.

A half inch varifult, Maritool, Titan, Imco etc... Will cost under $50 each,
and tear up a shit load of material. Even trying to baby it, you should be
able to pull 4 cubic inches a minute.. Letting it rip, 10+ easily.. Turn that
whole block to chips in 2 minutes..

This is 4340 annealed, essentially the same as your 4140.. One single
sub $50 endmill created 3 of those piles (I know, it was the last pile,
and all the barrels in the shop were full, and the cleaning guy was
coming in the morning.) Pulling somewhere around 12 cubic inches a minute..

And it wasn't even on a real machine, it was a Fricken Fadal for cripes sake.

7587539652_7ac4e49779_c.jpg



I think its already been said, but you are playing the false economy game,
save a few dollars on a single endmill, and lose $100's to $1000's because
you didn't want to buy a quality tool for $5 more, that would last longer
and move material a hell of a lot quicker..

And did you buy just one?? You NEVER buy ONE.. If you buy one, it gets
lonely and commits suicide.. If you buy 3, the first one wants to go
party with the other 2 in the box, so it lasts forever.
 
I agree. If you were using 3/4" carbide endmill, your feed could easily increase 2 to 3 times. Most machines will run out of HP before maxing out a 1" carbide so you're still limited. But for tool longevity and rigidity in cutting steel, you can't beat it. For 22 parts it's worth spending the $100 up front. 1" carbide? I can't imagine my 15 HP spindle being able to make full use of it.

With a 1.5" depth of cut, you can always make use of the rigidity of the 1" diameter tool. The machine in use may dictate what is best: if your machine has no gearbox for low range, then perhaps you're better off running a smaller diameter tool at higher rpm to get the spindle into it's better part of the torque curve.

PS: and your feed rate (in IPM) should definitely increase 4 times or more, for the carbide tool over the HSS.
 
We bought 4, we learned that lesson before! You're helping me out a ton so I don't care if you're a little bit of dick. I should have mentioned we are using conversational programming for this part so HSM toolpaths are out of the equation. I totally see your point and I'll learn from this! My only worry with getting a 1/2 endmill is the rigidity to cut 1.5 inch depth.
 
My only worry with getting a 1/2 endmill is the rigidity to cut 1.5 inch depth.

Not a big deal with HSM toolpaths where deflection is pretty low, and is mostly inline with the cutting direction as opposed to traditional toolpaths where the deflection is more perpendicular to the cutting direction such that you start seeing the tool banging against the wall of the part.

Regards.
 
So I was able to run the program once I decreased by axial depth of cut. So it's cutting (albeit slowly) until the carbide cutter comes in from Maritool. We went with the 3/4 coated carbide from them. If you don't mind helping me again what would be some safe numbers to start off with side milling with carbide cutter? We are climb milling, still force to go into a .7 radius corner. Material is 4140A. Thanks again guys!
 
So I was able to run the program once I decreased by axial depth of cut. So it's cutting (albeit slowly) until the carbide cutter comes in from Maritool. We went with the 3/4 coated carbide from them. If you don't mind helping me again what would be some safe numbers to start off with side milling with carbide cutter? We are climb milling, still force to go into a .7 radius corner. Material is 4140A. Thanks again guys!

Which ONE did you get???
 
Part #: 1010-.750-1.5
4 Flute Carbide TIALN Coated Roughing End Mill 3/4 x 1.5 flute length
 








 
Back
Top