1/8 ball mill longest cut?

[1ctoolfool]

What's the practical limit of length for cutting aluminum with a 1/8" ball mill.
Right now I need 2.125" and I am very skeptical as to whether this will work.
Any recommendations or experience?
thanks

[Donkey Hotey]

Can you be any more specific? You're talking about side milling? Are you doing deep pockets or something? Can you rough with another tool to remove most of the material? Are you using a CAM program?

I'm awaiting opinions from the more experienced guys but my belief is that you can do it if you take many, many shallow cuts. In Mastercam, it would be 'Depth cuts'. I'd do a finish pass 'on every level' and I'd set the max depth to be 0.040" or something in that ballpark.

It's going to generate hundreds of rough and finish passes but that's the price you pay with a long mill like that. That's why I'd start by roughing most of the material with something bigger.

[PBMW]

I once had to make a pocket in 316 stainless. The pocket was about 3" deep. It needed to have .06 rads in the corners. I drilled them and roughed the pocket with a 3/4" spade drill. then went after it with a 3/4 carbide endmill. Then a half inch EM that had a reduced shank. Then I went to a 1/4th an dpecked out the corners finishing with a reduced shank 1/8 endmill. Took a long time but came out well
The longer it is, you have to take small depth cuts, small radial cuts, and slow it WAY down.
I used about three different lengths of .125 endmill to gain a little cycle time and finish. All I had to do was just the remachine from the previous cutter so it wasn't much.
The thing that will kill you is the length of flute in the cut. You have to keepthe length of flute to about two diameters. You only need to reduce the shank by about .005
Should work fine if you do your part.

[AMCTony]

If this is something that can be sent out for Wire EDM then I would do that due to the amount of time it will take. If it a blind pocket the you could rough it with a large cutter and have it finished with a sinker EDM. If the customer has deep pockets or you have lots of spare time with nothing else to do then I would take PBMW's route. None of these methods are the wrong way and it really depends on your work load, part cost, and time avaliable.

[Donkey Hotey]

My uneducated, gut-feeling is that if you mill this, you'll also need to conventional-cut rather than climb-cut. With shallow depth of cut and a flexy endmill, I'd imagine that it would tend to climb itself away from the material.

With a conventional cut, it would pull itself back into the work and with a long engagement, the cutter would not remove much on the previously cut depths.

But what the heck do I know?

[ltmquik]

Originally Posted by Donkey Hotey My uneducated, gut-feeling is that if you mill this, you'll also need to conventional-cut rather than climb-cut. With shallow depth of cut and a flexy endmill, I'd imagine that it would tend to climb itself away from the material. With a conventional cut, it would pull itself back into the work and with a long engagement, the cutter would not remove much on the previously cut depths. But what the heck do I know?

That depends on what your end tolerances are. If you conv. mill the cutter will suck into the side walls and create an undercut feature. I would tend to climb and deal with having to take spring passes to remove the taper that is material safe. Also, if this is for tooling, undercuts would be really undesireable. My $0.02....

Again, more info is needed. What is the feature. Can you use a larger diameter cutter with a bull nose?

The answer I would ultimately give is yes it can be done. You may have to take small cuts to achieve the goal.

[mc-motorsports]

Any longer than 6 times the cutters diameter is going to give you issues, just ask the mold guys. I wouldn't even attempt that with a 1/8" ballmill, unless your cutting plastic. What about EDMing it?