What's new
What's new

Roughing, Climb only or both ways?

Not sure what's available as far as sizes, and I have nothing against the GWS endmills recommended by @crossthread82 but I've been using quite a bit of Garr's new A3 endmills. They don't offer them in coated, but they have a very high polished finish, and I haven't noticed any BUE. Check them out.
I haven't tried those but have been pretty impressed with the arc series from Garr.
 
Well I can't get any more coolant on it. 3 lines flushing away from the part and the it loaded up not during the pocket with walls around it and the chips needed to be flushed out, it loaded up with the 3 lines blasting on it and no floor below it and a side cut so the chip flushed away. They were piled up more than 3 feet away in the back left corner. Only way I can get more coolant might be if I use the wash down hose on a mag base mounted on the spindle. I'd like to stay away from coated for two reasons. Another shop had the job and used coated endmills and had chatter and the part warped .012" over 16". The part ends up .180" thick and aerofoil in shaped. I think they were inducing stress. I've never seen a coated end mill as sharp as the same brand uncoated. I do these with YG1 Alu-Power and got no chatter and flat with in .001". But not at 400 ipm, only 200 ipm with a 3 flute. But like the fine print says "your results may vary"
Have you tried air blast? I've read some applications need air to evacuate chips properly, coolant can't pull the chips out as well as air blast, but not sure if this works the same with aluminum.
 
What kind of tool life are you getting out of end mills running similar parameters as mine? I get about 10-12 hours with my conservative parameters, and the tools break near the holder face on the shank above the flutes. Called Helical about this and they said 10hours is considered good life for my parameters.
Good gawd, I get 100's of hours with Destiny Diamondback Stealth and Maritool corncob ZrN roughers. I actually don't know how long they would ultimately last, I just swap them out every 6 months or so. IME, the trouble areas for tool breakage are inside features like corners and slots. If I have a part with lots of that, I'll back off a little. But for outside, crank it up and watch it rip.

I use 35% axial for 1/2" x 1-1/4" LOC Maritool corncob and 1/2" x 2" Diamondback. 288 IPM for the 1-1/4" and 240 IPM for the 2".

Back to the original question ... I'd be wary of zigzagging with your 1/2" x 2". The sound of the conventional part of the cut just seems sketchy, compared to the climb cut, especially at the longer L/D's. But a 1/2" x 1-1/4", yeah, zigzag.

Regards.

Mike
 
Last edited:
What kind of tool life are you getting out of end mills running similar parameters as mine? I get about 10-12 hours with my conservative parameters, and the tools break near the holder face on the shank above the flutes. Called Helical about this and they said 10hours is considered good life for my parameters.
12 hours of cut time in aluminum? WTF! you should be getting MONTHS out of aluminum tools unless you break them.
 
I looked that one up. It does look promising. With HSM methods the chip thinning will allow 5 flute to do well for sure. Where do you buy the ASR-5? Directly from them? Can't find a seller or price anywhere.
Edit, I found them same place I get YG1, Suncoast but do not see the coated version
IF your machine can keep up with the feed rates! and a haas NEVER will. i would NEVER run anything over 3 flute in aluminum on a haas, you're wasting time by going light radial with 5flute cutters. a 3 flute with 40+% radial load will ALWAYS out perform 5 flute aluminum roughers on low end machines.
 
Question for y'all, in a roughing application does the corner radius increase tool life, performance, or both? I use the yg alupower with a sharp corner for all my roughing and finishing. I guess I am trying to determine if I were to implement a dedicated roughing tool would it be best to have a corner rad? ( I guess I would ask this about both aluminum and steel.) I have never gone out of my way to buy anything with a corner radius unless the part required a radius at the floor, maybe this is wrong?
a small corner rad will always give you better life. sharp corners are much easier to break.
 
Well I guess I need to work on it. Made it 20 minutes before loading up. I think its a problem with to much material for the 5 flute to evacuate. Maybe .05 step over or slower feed?
do yourself a favor, reach out to fraisa usa, ask for Doug Funfsinn, he'll send you a test tool for free, you'll never want to use anything else. there is ZERO reason to use 5 flute cutters in aluminum.
 
Have you tried air blast? I've read some applications need air to evacuate chips properly, coolant can't pull the chips out as well as air blast, but not sure if this works the same with aluminum.
horrible idea in aluminum, i've run our zimmerman for a few months without coolant (was waiting for our system to be built/delivered) and i snapped countless tools from aluminum welding, no matter what parameters i tried. using air blast, MQL etc. hell they would load up even if i sat in the machine and held the air gun right on the tool where its making a cut.
if you have coolant, run it.
 
Another thought ...
Depth cuts might save you some time. I've found that trying to tap-dance along with a 4xD cut ends up taking longer than if I just 2-step it with aggressive parameters. Run a 1/2" x 1-1/4" balls out, then get that final 1/2" with another high-rate cut. Extend a 1/2" x 1-1/4" a little farther out in the toolholder to give it just enough reach, and leave a few extra thousands on the 2nd depth pass, to avoid the EM shank rubbing on the 1st cut.

Yet another thought ...
Since you are running 4-figure quantities, I would invest in some custom tooling. Get the LOC exactly what you need, be it 1-3/4" or whatever. The difference between 2" LOC and 1-3/4" LOC can be significant.
 
Good gawd, I get 100's of hours with Destiny Diamondback Stealth
Same here, over 10,000 pockets I did in 2"x4"x4" 6061 aluminum, .06" wall,1.28" deep.
Running it as fast as my Brother would let me.
The ONLY thing I didn't like about that end mill was that it's fucking LOUD!
Part of it was the Brother isn't the quietest machine when cutting fast, but damn, that end mill is by far the loudest one I've ever used.
 








 
Back
Top