What's new
What's new

Carbide or cobalt end mills? Which is better for my daily machining?

David Boyer

Plastic
Joined
Mar 16, 2007
Location
Hastings MN
Hi, My shop uses carbide end mills almost exclusively and I think most machinists here have just got it in their heads that carbide is always going to be the fastest and most efficient way to remove material.

We do a lot of prototype work and I primarily run a 2 axis CNC mill that is a retrofit Sharp mill. With the 2 axis, I am the go to guy for quick turnaround modifications and onesy twosy parts where, by the time a 3 axis guy has his tools loaded and the programming done, I have already completed the part.

Anyway, my machine is limited to about 3500 RPM and is not the most rigid machine in the shop. It get's the job done, though. It is more rigid than most would think. So here's the deal: I almost always use carbide end mills but am almost NEVER running them under ideal conditions. Most of the time the RPM is too low, and there is never going to be perfect rigidity. Because of this I have a tool box full of dull, chipped carbide end mills. Even though I try to keep sharp finish end mills just for finish passes, I still end up with a bunch of chipped end mills over time. Eventually I send them out for regrind, but nobody seems to like to use regrinds.

So the other day I noticed that my boss had a few 1/2" cobalt 4 flute, fine tooth, coated (TiLN I think?), roughing end mills on his desk. I took one to try out.

I cleared a 5" diameter hole in 1018, 5/8" thick. I started with a 17/32" start hole and went all the way through the part in one shot. I used .040 width of cut and ramped up to 42 IPM. I ran about 2000 RPM I think. It cleared the hole in about 10 minutes. The end mill was not in the least bit warm afterwards. It cut effortlessly and I think I could have used a much heavier cut.

The end mill showed no signs of wear at all. I have used it several times since and it still looks and cuts like new.

So have I been wrong to use carbide all these years? Is cobalt better when conditions aren't perfect? Also, most of our CNC machines are not the best machines in the world. We go through A LOT of carbide end mills. I've seen videos of super rigid machines machining parts with carbide at just incredible speed and I think "we could never dream of doing that!"

I have requested that my boss get a variety of cobalt end mills for me to try out and he is all for it. So am I on the right track?? Is cobalt often better than carbide??

Thanks for any opinions!
 
You may think about getting speeder heads for your mills and use carbide in the 10,000 RPM + range. you may be able to run things 4X faster.

The rule is if you burn up tooling its too fast, if you chip tooling its too slow.
 
Regardless of cobalt vs carbide argument, the best endmills I have found for a low hp, low rigidity setup are the variable flute, variable helix endmills. You can take full width, full depth cut and machine will purr along like its nothing.

I do not know if variable flute/helix endmills are made in Cobalt, but the coated carbide 4 fluters (177 series) from M.A Ford are my favorite endmills of this type. Bridgeport is much happier with them than almost anything else.
 
What material do you mainly cut?
Using expensive carbide and cobalt end mills seem like a waist of over head $ to me when good quality HSS end mills will produce a LOT of chips on a Bridgeport type mill.

A HSS roughing end mill in certain materials can actually out perform the carbide with the RPM you are limited too.

If you use TiN coated HSS for cutting mild steel,some stainless grades or any thing below 30 Rockwell hardness you could save an ass load of cash in a years time.
 
Hi, My shop uses carbide end mills almost exclusively and I think most machinists here have just got it in their heads that carbide is always going to be the fastest and most efficient way to remove material.

We do a lot of prototype work and I primarily run a 2 axis CNC mill that is a retrofit Sharp mill. With the 2 axis, I am the go to guy for quick turnaround modifications and onesy twosy parts where, by the time a 3 axis guy has his tools loaded and the programming done, I have already completed the part.

Anyway, my machine is limited to about 3500 RPM and is not the most rigid machine in the shop. It get's the job done, though. It is more rigid than most would think. So here's the deal: I almost always use carbide end mills but am almost NEVER running them under ideal conditions. Most of the time the RPM is too low, and there is never going to be perfect rigidity. Because of this I have a tool box full of dull, chipped carbide end mills. Even though I try to keep sharp finish end mills just for finish passes, I still end up with a bunch of chipped end mills over time. Eventually I send them out for regrind, but nobody seems to like to use regrinds.

So the other day I noticed that my boss had a few 1/2" cobalt 4 flute, fine tooth, coated (TiLN I think?), roughing end mills on his desk. I took one to try out.

I cleared a 5" diameter hole in 1018, 5/8" thick. I started with a 17/32" start hole and went all the way through the part in one shot. I used .040 width of cut and ramped up to 42 IPM. I ran about 2000 RPM I think. It cleared the hole in about 10 minutes. The end mill was not in the least bit warm afterwards. It cut effortlessly and I think I could have used a much heavier cut.

The end mill showed no signs of wear at all. I have used it several times since and it still looks and cuts like new.

So have I been wrong to use carbide all these years? Is cobalt better when conditions aren't perfect? Also, most of our CNC machines are not the best machines in the world. We go through A LOT of carbide end mills. I've seen videos of super rigid machines machining parts with carbide at just incredible speed and I think "we could never dream of doing that!"

I have requested that my boss get a variety of cobalt end mills for me to try out and he is all for it. So am I on the right track?? Is cobalt often better than carbide??

Thanks for any opinions!

David.. You have already determined the best way. I mean it's not the machine, it's the operator. What you have done is pretty much optimized what your machine can do. Everyone else's machine in not yours. "You Run What You Brung." And then figure out it's limitations and work within those limitations. Your machine will look BIG to small parts. So don't do large parts. I'll bet it's pretty rigid using a .250" end mill. :)

Just go "shopping" for the work you can do.

Regards,

Stan-
 
You can get a decent 1/2 variflute carbide for $20 or $30....and that will outperform any hss/cobalt endmill in steel at 2500rpm....and last a hell of a lot longer. If not, perhaps there is an issue with the machine or the cutting methods being used.

I cleared a 5" diameter hole in 1018, 5/8" thick. I started with a 17/32" start hole and went all the way through the part in one shot. I used .040 width of cut and ramped up to 42 IPM. I ran about 2000 RPM I think. It cleared the hole in about 10 minutes. The end mill was not in the least bit warm afterwards. It cut effortlessly and I think I could have used a much heavier cut.

next time helically ramp the 5" diam leaving .02, knock out the slug, machine to size...should only take 2 min. and no need for a drilling op. that toolpath difference just payed for half the cutter.
 
Just my opinion, but I would stick with carbide. 3500 rpm is 458 sfm for a .500 endmill. This is in the working range of most carbide endmills. If chipping is an issue, a different geometry and carbide substrate will help. The process you used is great for material removal. While carbide can handle astronomical sfm in certain applications, it is not always a requirement. I would suggest a free cutting grind, minimum edge prep. While not as tough, it will not be subject to as much stress, and will not use up all of your machines horsepower as quickly. 1 cubic inch material removal per horsepower is an ideal goal for milling. My opinion is based on 33 years of machining in all types of shops. I also grind endmills as a part time business. Check out my milling videos on youtube, keyword search jamesu229
 
What material do you mainly cut?
Using expensive carbide and cobalt end mills seem like a waist of over head $ to me when good quality HSS end mills will produce a LOT of chips on a Bridgeport type mill.

A HSS roughing end mill in certain materials can actually out perform the carbide with the RPM you are limited too.

If you use TiN coated HSS for cutting mild steel,some stainless grades or any thing below 30 Rockwell hardness you could save an ass load of cash in a years time.


What material? It would be easier to answer what material I DON'T cut. I mean, you name it: Mild, 300 and 400 series stainless, 4140, aluminum, bronze, etc.

I guess I was thinking that cobalt might be a good compromise for a lot of what I am cutting, but I certainly could try a good coated HSS. I have burned up my share of HSS in the past, but that was generally uncoated. Also, would the rigidity of the tool be better with cobalt? I know it would with carbide but I'm not sure with cobalt.

My boss was saying that these cobalt end mills were about 1/2 the cost of carbide.
 
You can get a decent 1/2 variflute carbide for $20 or $30....and that will outperform any hss/cobalt endmill in steel at 2500rpm....and last a hell of a lot longer. If not, perhaps there is an issue with the machine or the cutting methods being used.



next time helically ramp the 5" diam leaving .02, knock out the slug, machine to size...should only take 2 min. and no need for a drilling op. that toolpath difference just payed for half the cutter.

Variable flute is something I don't think we ever get...I will definitely tell my boss about it. Thanks!

Great idea on the helical ramp, but I did mention that I am running a 2 axis machine. No Z axis except me. If this were multiple parts, no doubt they would have been done on a 3 axis with a helical ramp, but this was one part. That's what I do; take ONE part, grab it and go. Spend about a minute programming, pop a tool in a collet and start cutting. Sure, many of the other guys run machines that can remove stock faster, but I make up for it with the speed of my set-ups and programming.

You know how they say some jobs are just better off on a manual machine? I completely disagree with that. There is nothing that can be done on a manual as fast as I can do it on the 2 axis CNC.
 
Regardless of cobalt vs carbide argument, the best endmills I have found for a low hp, low rigidity setup are the variable flute, variable helix endmills. You can take full width, full depth cut and machine will purr along like its nothing.

I do not know if variable flute/helix endmills are made in Cobalt, but the coated carbide 4 fluters (177 series) from M.A Ford are my favorite endmills of this type. Bridgeport is much happier with them than almost anything else.

Thank you! My boss is always willing to give things a try. I'm sure he would not have a problem trying these. In fact he was just mentioning how much he now loves these high helix coated carbide roughers he just started using. I don't know how similar that is to the variable flute.

Variable flute makes a lot of sense to me now that you mention it. I imagine it's like a variable tooth band saw blade; the harmonic is broken up by the variable pitch. I could see that working with a variable flute end mill in a lower rigidity environment.
 
horsepower

a roughing end mill is usually much faster with less vibration than a regular end mill as long a finish is ok with you.
.
a Series 1 Bridgeport mill even with a 3 hp motor has problems with any cutter using much more than 1 hp. it is a question of how rigid the machine is.
.
Carbide in any heavy vibration or chatter whether cause by it being too long a end mill, part too thin and not supported well, or machine itself vibrating will destroy carbide at 10 - 1000 fast rate than someone who only has experience with heavier machines doing large parts.
.
with Stainless i use carbide, with aluminum i would use HSS, with steel i often use roughing end mills of HSS or Cobalt. avoid using any end mill longer than it needs to be. many cases using a stub length end mill i can easily remove 2 - 10 times more metal per minute than regular or long length end mills.
 
On my manual mill I often use carbide for the soft stuff and steel, and HSS for the Stainless and hastelloy. Being much tougher, in a less rigid set up it lasts way longer, carbide gets chipped before it gets to cut in that material unless everything is really tight.
 
Thank you! My boss is always willing to give things a try. I'm sure he would not have a problem trying these. In fact he was just mentioning how much he now loves these high helix coated carbide roughers he just started using. I don't know how similar that is to the variable flute.

Variable flute makes a lot of sense to me now that you mention it. I imagine it's like a variable tooth band saw blade; the harmonic is broken up by the variable pitch. I could see that working with a variable flute end mill in a lower rigidity environment.
The M.A.Ford 177 endmills use a combination of a variable helix and variable pitch in the same tool. They are nothing short of amazing.

The 177s do not get chipped or broken unless you drop them on the floor or run them way too slow. They are absolutely the best thing for a bridgeport. The corner radius also helps to increase tool life. You would not run a dead sharp 0.000R insert on a lathe for roughing, same deal with the endmills.

I quit using corn cob roughers in HSS and carbide because of these endmills. We usually run the piss out of em in the CNCs and swap them out when they start rolling up a burr on the parts. Afterward, they go in the bridgeport tooling and we beat them senseless. ;) I run them on hard steel, soft steel, hastelloy, inconel, and even aluminum with a shot of WD40 to keep chips from sticking. Every once in a while, I will pull a new one out of the tube if I need a mirror finish on something.

It feels like cheating the first time you use one because it cuts almost anything with ease without chatter or noise. The corn cob roughers damp vibration because they are cutting in a different spot with each flute. The variable helix/pitch endmills are similar, but last a whole lot longer and can finish with same tool.
 
Buy the second cheapest shit you can until you know what your doing.

Tell the guys in my shop that I don't know what I'm doing. I'm sure they'll have a good laugh at that. Just because I'm not using the optimal end mills doesn't mean I'm not doing about the best I can with what I am provided. The fact that I am here asking shows that I DO know what I am doing. I am asking those who may know more than me what THEY would recommend. And the word is "you're" not "your".
 
So where do you order the M. A. ford 177's? Right from them or some other supplier?
We usually get them out of the crib. ;)

Sorry, I do not know where they buy them. I do know our resharp endmills have taken a nosedive after running these endmills. They last a long time, so stuff does not get resharpened nearly as often.
 








 
Back
Top