.250 ball nose in aluminum

[dan m]

i am roughing with a .250 carbide ballnose endmill in aluminum. we are not that experianced with aluminum mostly just tool steels around here. I have to stick it out 3 inchs. i don't know the manufacturer it's just some cutters the boss dug up from some where. any suggestions will be appreciated.

[crazy^millman]

Well is it a 2,3, or 4 flute? 2 flute will be ok, but a 3 flute would be better. The 4 flute will work but you need to watch your depth of cut will have a tendency to load up. I would keep my chip load to .003 to .004 per tooth and problay 5000 to 6000 rpms. I might look at using a short tool you can really push, then come back with the long tool. The length of the tool is going to be the bear. To get around this you can do like a .025 depth of cut with a high feed rate and high rpms and in the long run come out furhter ahead.

 

HTH

[dan m]

it's 2 flute hihelix and we have been sticking it out a little more at a time (about .400 increments) we started out breaking them so where down 2 1000 rpm 10. ipm and .01 doc which seems very slow thats why i'm asking

[Justin Beebe at Folsom Tool]

That does seem slow especially for carbide. How are you holding the tool? In a collet or solid tool holder?

[Michael Sullivan]

Definately speed that baby up . Millman has the right Idea, 5000 to 6000 rpm. How long are the flutes? Better to have shorter flutes and a long shank. If it rubs a little on the shank it shouldn't matter for roughing. You'll find the rigitity will make a big difference. But If all you have is a long flute cuttter, try to take shallower cuts and crank up the feed as suggested.

[dan m]

we do have shallow flutes with a long length. i'm going to try millmans recomendations

[Hardmill]

@ 6000 rpm your still only @ 400sfm, crank that thing up and

do some smaller depth cuts.

 

JM2C and ima stickin to it

 

PEACE

[tpreb6]

Run your RPM as fast as you can!!! We run our .500 balls and bulls at 16,000 -20,000 RPM, feed at 300-600 ipm and take a full width of cut at .200 deep with the cutter extended out 1.75. This is an OSG Blizard cutter (uncoated) and we have only been through two in the past year. These parameters are off of our Makino S56. On our Fadals we run the spindle at max, 10,000rpm and feed at 200-300 ipm using the High Feed filter in Mastercam. When you are cutting this fast you need to keep your chipload heavy, anywhere from .012-.020. Also, use the High Speed toolpaths. They work great for this type of work.

 

As you extend the cutter out to 3" you can maintain your feeds and speeds. The only thing that you will have to change is the depth of cut.

 

One other thing, the cutters that we use only have about .5-.75 of flute and the rest is solid carbide. If you have a full fluted cutter you will not be able to push as hard as I have mentioned.

[tpreb6]

Ooops, Sorry!

 

I reread the post and noticed .25 and not .500.

 

I dido Millman, Michael.su and Hardmill

 

The biggest factor is the cutter design. Our .25 cutters only have about .250-.375 of flute and the rest is solid carbide. If your cutter is close to this you are going to be in good shape, however, if your cutter is a standard flute you are going to have to use more consevative feeds and speeds. The main thing to be concerned with is maintaining a good chip load. If you are to light it will chatter and to heavy it will pull.

 

I still suggest using the HS toolpaths which work better at maintaining a good consitant chipload, cutter engagement and smooth entry into the work piece as with the core roughing toolpath.

 

Try to use only Z level cutting stratagies to prevent the tool from being forced down into the work piece.

 

Is it possible to use a bull nose cutter for roughing and then finish with a ball in needed? With a ball you can run into some heavy cutter engagement like down in a pocket next to a wall where all of the flutes along the ball are cutting and this creates alot of extra pressure on the cutter.

 

And, use air or air/oil mist not a flood coolant. Especially if you are in a pocket. The air will blow the chips out where the flood coolant just makes a soupy mess and kills the cutter.

[dan m]

I just wanted to update everyone. The part should be done by morning. without the help from everyone it would have been another week at the way i was going about it. thanks for all the help

[Keith @ Solid Code Solutions]

Crank it up!

[terry5357]

I used to build vacuum forming molds. nothing but aluminum. I know this is not correct proceedure but always, always ran 10k+ on 1/4, 7500 on .500 and always 2 or 3 flute. Stand back and let that baby eat!

[Randy Morton @ Clem Industrial]

As with everybody else. That small of an BN EM, crank it up, super high! Max the spindle, and give'r small cuts at what might seem like a stupid feedrate. High speed machining at it's finest. =] 300+ IPM (depending on depth), no problem!

 

JM2C