[pzzamakr1980]

Being a beginning machinist getting into this to make some fun stuff and maybe a little extra money I seem to have an endless well of questions. Heres this one. I was talking with a friend who is a machinist about why 2 flute endmill's are preferred over 4 flute or other. He had a variety of reasons, but none of them seemed particularly convincing. He also said that 3 flute endmills are much better and they leave a much better surface finish than 2 flute. So I bought a bunch of 3 flute endmills, the cheap ebay kind, and have now been having some problems, which Im concerned are due to my choice in number of flutes. The problem is the endmills will clog with aluminum and then of course, it all goes downhill from there. I am using a Sieg X3, at the max rpm, with a 1/4 3 flute endmill, with a koolmist system. The feedrate varies between 18-24 ipm. The feedrate was suggested by my friend as well and is much faster than what MasterCAM is suggesting. To be honest, I havent worked the feedrates for myself yet, but seeing how fast people like Hoss is running his it doesnt seem like it should be a problem. So... whats better and why, 3 flute or 2 flute, to work in aluminum

[Caprirs]

What is your max rpm and how deep are you cutting? Are you slotting? Or just side milling?

The 2 flutes allow more room for chip evacuation. Since it is possible to achieve high chip-per-tooth rates with aluminum, a lot of folks prefer the 2 flute endmill so there is a reduced likelihood of the chips packing up in the tool. However, the 2 flute has the least cross section and is the least rigid tool. The 2 flute also has only 2 cutting edges per revolution so the surface finish is not as nice as a tool with more flutes.

[snafu350]

Although still a rookie by some standards, I've been programming cnc machines and milling aluminum for over 5 years. 4 flute endmills are my last choice. As a beginner I figured 4 must be better than 3, which must be better than 2 right?? No way!! 3 flutes are the best balance. You are talking carbide right. 3 flute carbide endmill...what rpm are you running? At the feeds you mentioned you should be up around 4000 rpm anyway...good luck

[pzzamakr1980]

The deepest cuts I am making are less than 1/8. So if chip evacuation is what I'm after, increasing the rpm would increase the chip evacuation. Correct? Nope, hss with a paint coating. I say paint coating because the chinese endmills which these are have a very thin coating, very very thin. I am running about 2250 rpm. I say about because I've heard the sieg x3 is a bit off and can run a bit above or below its stated maximum.

[Ken_Shea]

Here are a couple of things to consider.
1) 18-24IPM is too fast for a .125doc, .250 HSS end mill at 2250rpm.
2) Try about 10IPM at .050 and work up from there.
3) Flood is best for chip evacuation or you can assist this using air blast.
4) When you can, purchase carbide in 3 flute for aluminum. Here is a good link for these. http://www.lakeshorecarbide.com/index.asp
5) Some aluminum is gummy and susceptible to flute clogging.


Ken

[pzzamakr1980]

I actually started at 6 ipm and progressed up to the 18 ipm point. My initial depth of cut was also .025. Which made cutting anything an hour and a half long process. The reason why I looked at what I was doing as slow was the fact that Mr Kemp, aka Hoss Machine.com was running his x2 with a huge freaking extended head at a feedrate far exceeding what I was doing with no coolant whatsoever. And while it sounded like his tooling was dying a fast and very very painful death, and im sure his finish wasnt great, his chips were clearing and he was cutting without clogging his cutter. He was cutting aluminum as far as I know. Like I said I do currently have a fog system which works pretty darn good but makes a big damn mess so I plan to switch to flood in the next few days. I have made a fixture plate that is a bit larger than the work envelope with a drain design so I didnt have to make a whole enclosure. In testing with a garden hose its worked great so far.

[Caprirs]

At 2250rpm and 18ipm, you're taking .004" per flute and .008" per rev. That's pretty aggressive for a small cheap endmill.

As suggested, I'd get a carbide 3 flute endmill if you want to feed that fast. I'd also try to find a way to speed up that spindle.

[pzzamakr1980]

Awesome, both of those can be done. I almost done with my belt drive conversion which will let the x3 do about 5000 rpm and exactly 5000 rpm after the tach is installed, and the carbide endmills can be bought easily. Cheap mill, what are you talking about. I paid 800 dollars for it. LOL. For that kind of money I should expect it to do double the feedrates and depth of what I'm doing and to smell like a rose too.
So the reason that a 3 flute is preferable is its stiffer and hence less tool deflection, and it can take more material with each revolution which will allow for higher feedrates and when finishing a better finish. Its drawback is less area for chip evacuation and hence more possibility of chip packing. This drawback can be offset by increasing the spindle rpm. If any of these statements are in error or not logical let me know. I just like to know the why of something, thats why I'm stating that.
If 3 flute seems preferable to many machinists for aluminum cutting, why are they never available or used to teach with. My teacher never once mentioned a 3 flute cutter as being ideal for aluminum cutting. I didnt even know they existed until I bought some from the ebay seller 800watt.

[Ken_Shea]

Couple more thoughts to factor in

1) Just because you can crank that baby to 5000rpm does not mean that those bearings will handle it. For a while, perhaps, how long is always a guess, but not long would be mine.

2) IPM cost money, when you purchase these affordable mills you have to learn to get patient. This is not a whack at the mill or looking down my nose at them, people do enough of that with my humble Haas TM-1 .
But you have to get realistic with any mill as they all have their limits.

The carbide 3 flute for aluminum and flood is a really good start in increasing
cutting efficiency, for not a lot of money, also, keep the tool overhang as short as possible.

Ken

[dertsap]

edit

[pzzamakr1980]

The bearing are definitely a weak point, and this has actually been discussed a few times over, because a lot of us who use this mill feel that exact way. However, because this is not a production machine, or at least a production machine like a haas or fadal or etc, its not going to see that amount of time in constant use that those do. Hence, the bearing should still last awhile. When they need to be replaced, and it is definitely a when, it wouldnt be a huge expenditure. Even if I replaced them with stock stuff again rather than upgrading. As far as thumbing the nose, I just kinda laugh about it. This machine does everything I ask from it, and it really did cost 800 dollars. So for 92,200 or such left over from not purchasing a (insert expensive ass vmc or hmc) I can afford to have stuff fail and to replace it. As well as be a bit patient, because no matter how much I would like to think it is, my time is not worth THAT much. One other really nice thing about this machine is, it fits in my parents 3rd car garage with lots and lots and lots of room to spare and I just have to plug it in to an outlet. So I dont even have to pay for electricity.
Thank you very very much for the suggestions and information, I guess I can pat my friend on the back and say he was right, which will make him very happy. Now I can mosey on over to the which endmill is best thread and start reading there for endmill tips. Although ken, I already bought two of the ones you suggested, so Ill try those out. If I like em Ill keep using em. Thx again all.

[Ken_Shea]

dertsap,
I agree with what you are saying, however, I do not remember reading where anyone said that 3 flute were best.

I would say that they are a very good comproimise, especially for the hobbiest where the expense of high end cutters in many configurations cannot be justified.
Heavy engagement is not going to fly on a Sieg X3.

pzzamakr1980,
So for 92,200 or such left over from not purchasing
That was pretty much my same thinking considering my expected use, when I purchased my mill.

EDIT:
And what I could afford


Ken

[dertsap]

Ken
the thread title is : is three flute better
i read it as best
overall its personal preference as what to use for a given application , and i agree for the hobbiest it would be to narrow it down to best bang for the buck

[pzzamakr1980]

Your right ken, no one did say they were the best, but as you stated they were a good compromise for what I have and what is affordable, how bout instead of best, Best for my expected uses.
Yeah, I like that whole affordable thing. It had a whole lot to do with the mill purchase, I didnt want to spend as much on a mill as Im going to be soon spending on a house. LOL

[Oldmanandhistoy]

Nope, hss with a paint coating. I say paint coating because the chinese endmills which these are have a very thin coating, very very thin.

I think em coating is worthy of a mention here; it is a fact that some coatings Tin for instance will course you problems in aluminium.

John

[mrk]

A couple of quick thoughts from fellow newbie.

My CNC is a big old Acroloc fairly cheap on ebay. I am pushing the RPM up a bit and my brother in law and I recently built a system to inject a mix of air/oil into the spindle bearings while it runs. The idea was from an Acroloc service guy and others have done the same thing with good results. My machine now has much less heat on the spindle since the air oil mixture is cooling the roller bearings. The conversion was fairly simple with an air/oil regulator hooked up to the old auto oiler port on the spindle. It might be possible to rig up a similar system with your machine.

Now with respect to 2 flute vs. 3 flute. I am really liking my 3 flute end mills but it is more complex then just feed per tooth. You need to look at the cut angle of tool engagement, and other factors. For a profile cut that is light you can really feed very fast. For a slot or plunge you need to slow down a lot since the tool is surrounded by metal.

[big_mak]

Search for Gorilla mills, they make a line called Silverback bof aluminum, where you can go 1X the diameter in DOC, and the feed rates are reasonable. Not ultra fast, but consider that you are removing more material, and this is for slotting!!!!!

[chipsinpan]

I would like more feedback on 3 vs 4 flute end mills. Someone suggested that a 4 flute will actually "recut" a chip that gets caught on the side opposite the cut , causing the tool to deflect . I am using 4 fl Garr tialn that cost about $9.00 each . Running a 1/4 mill at 4500rpm /8 IPM in and a 20ipm springpass out to mill 1/4" keyways . I can do a 3" keyway in about 44 seconds , but am getting a bit sloppy on the width . I have been using 4 flutes for so long, that I forgot why I never tried 3 flutes . BTW these GARR mills are the best value per inch of keyway that we have ever tried . Increased my bottom line by going to a cheaper mill ! Was using HS Tin before I got smarter!

[big_mak]

If your tool deflects, then you run a spiring pass, of course your width is going to be over size. I'd use a 3/16 or 5mm endmill, and contour the profile, then you can use d-comp to control the size of your slot!!!

[Geof]

....Running a 1/4 mill at 4500rpm /8 IPM in and a 20ipm springpass out to mill 1/4" keyways . I can do a 3" keyway in about 44 seconds , but am getting a bit sloppy on the width....

For this specific application my suggestion is go to a five or six flute to get less feed per tooth and therefore less deflection.

Do the keyway in one pass do not take a springpass, that is where your slop is coming from because you are making the keyway wider by the amount of the tool deflection on the first cut. Omitting the springpass means you can maybe drop your feed to 6 ipm and still get the same overall time.

To avoid the recutting of chips on the opposite side use an airblast ahead of the cut to blow the chips back out of the keyway but inject coolant into the airblast to keep the cutter cool. It may be possible to get away with just using airblast but taking full keyway depth in one cut might mean the cutter overheats.

These suggestions are based on experience cutting lots of keyways on manual machines; some stuff does carry over to CNC.