Need Help!- Ball end cutter?

[79TigerPilot]

New to ball end cutters and need some advice.

I need to cut a series of 1" long round bottom slots with a 1/4" or 3/16" dia ball end mill. The slot depth slopes from .15" deep at one end to .01" deep at the other end. The slot width is the cutter width and not at all critical these are just drainage channels like on a meat cutting board. The material is 6061 Al and will be done on my CNC BP with a max RPM of 6700.

Can I cut this in one pass plunging the full depth of .15" at the start end then retracting the Z while moving to the far end? Or would it be better to start at the shallow end then move to the deeper end? Or do I need more than one pass.


Never used a ball type EM before so could use some wisdom.

Thanks,
Craig

[78nova]

What type ball end mill are you using?

2 flute?

4 flute?

High Speed?

Carbide?

Flute length?

Effective Set Length?

Dry, Coolant or Air?

[79TigerPilot]

Told you this was my first venture into ball cutters -- I gots to learn the lingo.

I guess its most likley going to be 2 FL carbide. That seems to be what I can get around here.

Will be standard lenghts -- what ever I can get -- doesn't need to be long but would not buy stub lenght.

For cutting fluid: WD40, I also have CoolMist, but I find the the WD40 to work out better on AL.

Will need to do some research of feed rate and speeds, my mill will do 6700 RPM.

Was just looking for some rules of thumb similar to what I use for normal end mills. I usually limit my DOC to < 1/2 the cutter diameter.

Criag

[78nova]

With the diameter you stated at .250, I would suggest getting a 4 flute if you can and definitely use carbide, with the shortest flute length you can get. A 4 flute will cut better than a 2 flute. A 2 flute will work if that is what you end up with but you cannot be as aggressive. Which ever one you end up with, get it chucked up as short as possible. If you have some test material to try out with go for the full depth of cut from the get go. I would think with this small of a tool that you are not going to be able to spin a lot of rpm so start conservative and work your way up if needed. Just remember, the longer the cutter flute length & cutter set effective length, the slower you will need to go. With that in mind, start at 1500 rpm @ 10 ipm with a 4 flute tool. With a 2 flute cut this in half. Adjust up or down from there. Too much rpm, with too long of a tool will chatter like all get out. Rigidity is a key varible here. Your part & holding device must be rigid. If your results are poor, make a rough & finish pass & reduce the feed & speed on the finish pass.

If this was on my machine, a 5 axis cnc horizontal mill, I would set the tool in a shrinker holder or in a solid extension at the shortest possible effective length I could using a tool with no more than 1.0" flute length. I would start out at 2500 rpm & 20 ipm, " IF " my part was nice & rigid. If it is flimsy, I would go down to 900 rpm & 5 ipm to start.

I hope this small amount of brain fodder helps you out some.

Good luck

Kenny

[ParkerMillguy]

I would start at the shallow end and ramp to the deep end leaving .005 for a finish pass. If you have room, use a .002 step over on finish pass to clean up tool deflection from rough pass (climb cut down the ramp, move over .004, climb cut the opposite wall coming up the ramp).

Aluminum is forgiving, but you should follow manufacturers specs for speeds and feeds.
For example, GARR Tool suggests 300-500 SFM for RPM calculation and .002-.005 CPT for your Feedrate calculation.
RPM=3.82 X SFM / D (3.82*400/.250=6112 RPM)
IPM=CPT X # of flutes X RPM (.004*2*6112=49 IPM)

Now keep in mind when you start out only .01 deep your cutting diameter is .098
3.82 * 400/.098=15,591 RPM
When you get to .150 dp you are using the full .250 cutting diamter so you probably want to average the 2 RPMs and run at 11,000 RPMs
.004*2*11,000=88 IPM
So att 11,000 RPM's you will be running at a feedrate of 88 IPM.

If surface finish is not a factor and speed is, then just do one pass. Personally I like to make parts look nice too. At 1" long slots and 88 IPM I don't think you'll be adding much!