Looking for the perfect sized end mill for 5/8 aluminum

[AGauger]

I’m looking for advice on the best size end mill to cut out aluminum parts from. I’m almost always making parts from .625 inch thick 6061-T6. I began cutting these parts using a 1/4 inch end mill fluted for aluminum. This has worked fine but I recently purchased an 1/8 inch version of the same end mill for more detailed work. It cuts much faster and makes far less mess in chips. The 1/8 inch end mill only cuts to a depth of 3/8 though. I guess I could get a 1/8 end mill that cuts deeper but I need one that has some rigidity to it and will not be prone to breaking.
So it’s a compromise…
Smaller end mill = faster cut speed with less mess but is flimsy
Bigger = more rigidity but more mess and cuts more slowly.
Perhaps something between that works well for 5/8 aluminum would be the perfect solution? I know there are others out there that have far more experience then I, what size end mill would you use in this case?
Thanks,
~Aaron

[AGauger]

Should also mention that I'm cutting these parts on a Taig mill converted to CNC.

[HimyKabibble]

Originally Posted by AGauger I’m looking for advice on the best size end mill to cut out aluminum parts from. I’m almost always making parts from .625 inch thick 6061-T6. I began cutting these parts using a 1/4 inch end mill fluted for aluminum. This has worked fine but I recently purchased an 1/8 inch version of the same end mill for more detailed work. It cuts much faster and makes far less mess in chips. The 1/8 inch end mill only cuts to a depth of 3/8 though. I guess I could get a 1/8 end mill that cuts deeper but I need one that has some rigidity to it and will not be prone to breaking. So it’s a compromise… Smaller end mill = faster cut speed with less mess but is flimsy Bigger = more rigidity but more mess and cuts more slowly. Perhaps something between that works well for 5/8 aluminum would be the perfect solution? I know there are others out there that have far more experience then I, what size end mill would you use in this case? Thanks, ~Aaron

In terms of fast material removal, you want to go as large as you can. A larger diameter tool will allow you to plunge deeper on each pass, while maintaining the same feed rate, assuming spindle power and machine rigidity permit. I'd guess on the Taig, you're probably limited by both spindle power and rigidity. On my knee mill, I do most of the work with 1/2" 2-flute aluminum cutting HSS endmills, cutting at least 1/2" deep per pass, at 12 IPM (for slotting - deeper and faster for peripheral cuts). But I have a 3HP spindle. Most important thing is maintaining adequate chip load - 0.002" for a 1/2" endmill, at least 0.001" for a 1/4". Set RPM for 400 SFPM. If you can't maintain chipload, due to lack of power or rigidity, then reduce RPM to keep chipload up, or you'll wear out tools quickly through rubbing.

I'd guess in your case 1/4", or maybe 3/16" will work best. A long small-diameter tool is not going to work well on aggressive cuts. The tool and machine flexing will lead to breakage and bad surface finish, and the small diameter will lead to clogging on deep or aggressive cuts. A 1/4" tool will easily cut 1/4" deep in one pass, where a 3/16" or 1/8" will not generally cut one diameter depth for long without breaking.

Regards,
Ray L.

[mc-motorsports]

If your machine has the power to run a tool to it's max, the problem becomes removing the chips. A high pressure flood is best, your going to be limited to depth and feedrate with anything less. Aluminum chips like to weld, that is the biggest factor in milling aluminum. I would try 5/16" or 3/8" 2 flute carbide if you have enough power to cut efficiently and can keep the chips out. I use 1/2" carbide one pass myself, but I don't cut a whole lot of aluminum plate 5/8" thick though too. If I did, I would try a smaller cutter.

[sansbury]

You might want to try a roughing mill, the kind that has serrated edges. They require less torque, so you can take a heavier cut than otherwise. They do leave a serrated finish, though, so you might need to take one or two more passes with a finishing mill to get a smooth surface.

[project5k]

ok i have a feed rate question,

this last weekend i was cutting a part, and i was using a 1/4 inch HSS 2 flute endmill, spindle speed was 2000, and about the hardest i was willing to push was about 2IPM with a .125 DOC.

any faster, and it sounded like i was gonna break something.. and considering its the only peice of that stock i had, i couldnt risk messing it up.

[sansbury]

Way too deep and way too slow on the spindle and feed. With a small CNC mill the smartest game is to take lots of shallow cuts as fast as you can.

Just for giggles try .02" deep, spindle 4000rpm, and feed 10IPM. Try increasing each parameter from there.

EDIT: For some reason I thought you have a Taig. With an X3 I'd try maybe .05" DOC (depth of cut) to start, maximum spindle RPM. That's still conservative. With a 1/4" endmill your maximum feed will be limited by spindle speed first. You need the spindle going fast enough to not fill the flutes with chip--smaller endmills need faster speeds. That's where a 3/8" or 1/2" will give you better performance. This chart and calculator (see bottom of the chart) is a good place to start:

http://www.littlemachineshop.com/Ref...ds.php#Milling

[JimPAC]

Sounds like you have a sweet setup on that little mill! Are you willing to spend the bucks on Cutting tools?

Look at Weldons CresCut or try a tight spiral, main thing is keeping the chips and debris clear of the cutting area! it sounds like your probably already there in terms of max efficiency! Be good that machine jewelry and it will be good to you.

Next step is a bigger truck!

Keep the chips flying"

Jim

[japroach]

What exactly are you cutting here?

It sounds like you are doing 2D profiles, and are attempting to cut quite deep in one pass?

[HimyKabibble]

Originally Posted by project5k ok i have a feed rate question, this last weekend i was cutting a part, and i was using a 1/4 inch HSS 2 flute endmill, spindle speed was 2000, and about the hardest i was willing to push was about 2IPM with a .125 DOC. any faster, and it sounded like i was gonna break something.. and considering its the only peice of that stock i had, i couldnt risk messing it up.

Here's how you set speed and feed:

1) Calculate RPM, based on SFPM. Use 400 SFPM for HSS in aluminum. This gives you about 6100 RPM for a 1/4" endmill. If you can't achieve the calculated speed, get as close as you can.

2) Pick your chipload. For a 1/4" tool, 0.001-0.0015 is a reasonable maximum. Use this, and your actual RPM, to calcaulte feedrate.

3) Start taking test cuts, using the above calculated RPM and feedrate. Start with a light depth of cut, especially on a small machine. Steadily increase depth of cut, until finish quality starts deteriorating, or the spindle starts laboring.

Use coolant (mist works really well, even on large machines, and is mot messy) to keep things cool, especially with aluminum. This will improve surface finish, and increase tool life.

Regards,
Ray L.

[mc-motorsports]

You know what a lot of people here don't take into account, how ridgid is your machine, how ridgid is your spindle, how ridgid is your set-up and how much power do you have available at the spindle?

Don't expect a bench-top machine to cut at high end CNC speeds and or even feeds. HUGE limiting factor. JFI, I would cut this at full depth, 1/2" carbide endmill, uncoated and I don't like the high helix as they require more RPM that I don't have, 2400 RPM and 8imp, finish pass at 25 IPM if your not dropping a slug out of a plate, assuming your using a fixture, and that's on a retrofitted bridgeport. I would expect to get a little more feed and speed out of a high end machine.

I used to hog out 1/2" aluminum, 1 pass at 12imp with a 5/8" endmill on a Mori at my previous job.

One thing about aluminum, you can take a bigger chip, more speed and more feed with a larger endmill because a smaller endmill doesn't have the flute clearance to clear the chips... Steel is a slightly diffrent story, a larger diameter endmill is more ridgid and can take more heat. But you still have to have a ridgid machine and enough motor to spin the spindle to take advantage of this. If you TAIG would cut as fast and as nice as a Mori, then Mori would have been out of business years ago. Just sayin...

[HimyKabibble]

Originally Posted by mc-motorsports You know what a lot of people here don't take into account, how ridgid is your machine, how ridgid is your spindle, how ridgid is your set-up and how much power do you have available at the spindle?..

The procedure I outlined takes all that into account. You sneak up on the limits of the machine, and as you get close, if you're power-limited, you'll start bogging down the spindle motor, and if you're rigidity-limited, the surface finish will start deteriorating when you start pushing too hard.

Regards,
Ray L.