Face Mill Finishing Flute Count

So I am in the market to pick up a new face mill for finishing 6061. Looking at the ASX445.

My rep recommended a 4 flute over a 6 flute. Not that I question his expertise, but what would the reasoning be to choose a 4 flute over a 6 flute for finishing?

Prolly the dealer thinks you want more depth of cut over higher feedrate. The catalog classes these cutters as: coarse pitch = 4T, fine pitch = 6T, extra fine pitch = 8T.

Remember that face milling like at least 2 teeth in the work no matter whatever else you are doing so coarse pitch mills tend to really hammer with narrow workpieces.

Matt

Horsepower and rigidity are usually the driving factors for number of teeth. Is this Vise work on solid held pieces on a decent 40taper VMC, what size are you looking at here? Are you only going to use it for finishing.

If you are looking for a face mill for finishing 6061, you should be looking at an adjustable pocket PCD cutter. You dial in the heights of the cutters within a few microns, you can have as many inserts as you can order on the body, and you will likely only have to change them every few years.

If you want to run carbide and like to do a little roughing here and there, the Coromill Century are a solid adjustable cutter. Kennametal Fix Perfect is also a very solid choice. Run carbide cutters and two PCD wipers, with a fine pitch body. Carbide is really only there to protect the PCD, they will cut a little but will be a thou or so "behind" the pcd edges.

What have you been using?

Have to agree with Matt on wanting at least two inserts in the work at all times. I have some 1" 3 flute insert cutters that are real work horses but really hate the sound of those when the material thins out at the end of the cut. Now if I had a machine that weighed 5-10 tons with a spindle that weighed several hundred pounds it wouldn't be an issue but on my little gear driven machines it can sound like somethings going to break.
Dan

I go with fewer flutes for finishing aluminum. My experience with face mills with >4 flutes (in 2" & 3" diameter) is that they have more of a tendency to put chips back onto the surface. I don't know the correct term, but it is as if the chips or dust get welded onto the surface when you are trying to skim cut and leave a mirror like finish. It is like there is a minimum chip load per tooth and when I drop below that, I get that effect. Taking a heavier cut, or slower RPM, or more aggressive feed can fix that some of the time, but for ME, a four flute 2" cutter with 45 degree inserts, with a fairly positive rake gives the best result.

Secondly (as my wife will endorse), sometimes I'm and idiot and hit things with my face mill. Sometimes I get a little too close to my hardened steel stop. Sometimes I take a little bite out of a fixture screw. I've even hit a vise jaw before. The downside to high mix, low volume, going too fast while being an idiot Those little mess-ups cost $30 with my three flute, $40 with my 4 flute and $60 with my 6 flute. I can be an idiot twice as often with my 3 flute cutter

G00 Proto said:

I go with fewer flutes for finishing aluminum. My experience with face mills with >4 flutes (in 2" & 3" diameter) is that they have more of a tendency to put chips back onto the surface. I don't know the correct term, but it is as if the chips or dust get welded onto the surface when you are trying to skim cut and leave a mirror like finish. It is like there is a minimum chip load per tooth and when I drop below that, I get that effect. Taking a heavier cut, or slower RPM, or more aggressive feed can fix that some of the time, but for ME, a four flute 2" cutter with 45 degree inserts, with a fairly positive rake gives the best result.

Click to expand...

Mass of chip, space to evacuate and simple angular momentum all play a part in my book. Nothing fucks finish worse than re-cutting swarf, enough mass and momentum it flies clear, too little and it gets mashed back in!

Thanks all. This is on a "20hp" Haas VF2, with 10k and I am looking at their 3" cutter.

Currently using a Maritool 2.48" and while it is great for removing a lot of material, it only leaves OK finishes. So I was wanting to pick up something that can take a finish pass after roughing with the Maritool.

I have these parts set into the vise .150"

Will this ASX be a couple steps up in surface finish, or should I be looking at an adjustable pocket?

CGornet said:

Thanks all. This is on a "20hp" Haas VF2, with 10k and I am looking at their 3" cutter.

Currently using a Maritool 2.48" and while it is great for removing a lot of material, it only leaves OK finishes. So I was wanting to pick up something that can take a finish pass after roughing with the Maritool.

I have these parts set into the vise .150"

Will this ASX be a couple steps up in surface finish, or should I be looking at an adjustable pocket?

Click to expand...

If recutting chips aren't the reason for the poor finish, I'd just get an adjustable pocket face mill.
You'll just be chasing your tail with a normal body where you can't actually adjust anything.

CGornet said:

Thanks all. This is on a "20hp" Haas VF2, with 10k and I am looking at their 3" cutter.

Currently using a Maritool 2.48" and while it is great for removing a lot of material, it only leaves OK finishes. So I was wanting to pick up something that can take a finish pass after roughing with the Maritool.

I have these parts set into the vise .150"

Will this ASX be a couple steps up in surface finish, or should I be looking at an adjustable pocket?

Click to expand...

Or adjust feed and use only one insert and idealy a PCD one at that or for ungodly shiny and a £400 bank balance hole MCD

This is when I get thrown off this forum... sometimes when I just need a shiny ass surface finish, I use an old school flycutter with a hand ground HSS lathe tool. Something about those just gives the best damn surface finish in the world. I'll admit, I just drag it out when I need something shiny, but it sure works well.

Hey, flycutters work and have worked for years, they should be in every tooling crib.

BUT I use'm in a pinch when all else fails or tooling needed doesn't justify the cost.

HSS doesn't hold up and run out of balance to get real speed from them...but they do get the job done. If you like HSS finishes you should try some high positive polished Carbide inserts, they last and last, inexpensive compared to PVD, cut like a dream and leave super finishes. I fun in a Iscar Octomills and Allied ShearHogs