OT What do you think

[Joels]

There is alot of knowledge here. I uploaded a file in the MC9 folder called frame.mc9 Please check out the file and see if you agree with me. The question is tool #1. I use a cobalt roughing endmill 3/4 dia. We make this part from a solid piece of aluminum bar that is 2 inches thick. it takes about 12 minutes for tool one to complete. The question is would you do anything differently?

[Thad]

My first thought would be an insertable face mill and just tear a$$ into it. At a 12 minute run time, you probably won't gain much, if anything.

 

Thad

[Thad]

On second thought, running a .750 face mill at 200 IPM would cut you down to just over 2 minutes run time. I didn't got over all the settings with a fine toothed comb though.

 

Thad

[Joels]

i am running a cobalt roughing end mill at 6000 rpm and 35 ipm. I havent figured out the actual load per tooth but the machine runs good there and the tool doesnt break. My boos has come up with some ideas but nothing i thought would work. you said a face mill at 200 ipm can you tell me what kind of face mill would do this?

[T_MALENA]

what is the max rpm on your machine? How much of this part is in the vise?

[germ]

Sandvik makes a coromat style inserted endmill especially for alumunum. We run an 1 1/2" and a 2" at 8000rpm and 390ipm .300 d.o.c. and it eats aluminum for breakfast

[Joels]

I am using a Fadal 4020 with a max rpm of 10000. If i go above 6000 rpm the tool really starts to chatter.

 

Germ,

Thanks for the info i will look the tool up.

 

right now i am doing a .500 depth of cut

[Quickmike]

Put the file on the ftp so we can see how it sits in the vise.

[specv]

watermaker,

Try using a Benchmark 3 flute carbide em. we run a .625 dia 3 flute 294 ipm @ 14000 rpm. w/ .5 doc. these things love aluminum. @ 10000 rpm you could run your same path @ 210 ipm.

[Joels]

i did put the file in the mc9 folder. the vice is a Kurt and we use snap jaws to hold it. Since we machine the ends too. The main issue is that i make a thru hole in the center of a solid bar.

The bar weighs about 10 pounds when i start and i remove about 7-8 of it with a cobalt roughing end mill. i hold the part in the center and i am gripping about a inch of the material from the bottom up

[Joels]

one problem i have is the chips stay in the center pocket until the final pass breaks through. if i make the feedrate too high the cutter gets malled by the chips and breaks. I have coolant through the spindle which works great but it leaks on the spindle belts so we cant use it. Fadal has fixed this several times but it still leaks.

[T_MALENA]

Try running a Weldon Ski-carb mill 10,000rpm & 75 ipm(to start). I run these at 14000 & 100-300 ipm. Almost everybody has a "aluminum mill" that should work. I would think a aluminum mill would do better than a roughing mill. They cost more, but they are worth it in the end.

[Joels]

so if i understand everybody is basically i should us a indexable end mill instead of a cobalt roughing end mill right? can anybody give me some part numbers so i can look them up?

 

Thanks to everybody for their input!!!!

[T_MALENA]

Garr Tool(800-248-9003) Ø3/4 edp#85700, #86620

OSG (800-837-2223) Ø3/4 edp#440-7500, 445-7500

[mayday]

SGS Skicarb, 3/4" EDP#34525

1600-2000 sfm .008 per tooth feed

[T_MALENA]

sorry cant find th info on the Weldon ski-carb. All the mill I listed are solid carbide.

[T_MALENA]

Thanks Mayday. I was looking in my whalley book. I knew they were in Ohio, looking in wrong book.

[specv]

HILL INDUSTRIAL TOOLS (952)448-5874 3/4 DIA 3FL HH CARB ENDMILL W/1-1/2 L.O.C. ,4.0 OAL, 3/4 S.S. BRIGHT EDP:350-75024

[Thad]

It looks like you're in good hands.

 

Thad