Machining a vial.....Carbide ball mill or HSS

[wrustle]

I have a job running right now that's giving me fits (to put it lightly).

.500" -.0002/-.0006" dia. x .960" lg. A2 material.

ID is like the inside of a test tube.....437" +/-.015" dia. x .835" dp. with a .2185"R (.437" dia.) at the bottom.

I drilled them all out (100pc order) with a .390" drill as deep as I could to allow for finishing the bottom with a carbide ball mill. Tried finishing them in the lathe 1300 RPM .005" IPR until full contact at bottom then .003" IPR.......NO WAY JOSE.....chatter like a SOB endmill crunched big time at the bottom......flutes probably chipped on the way down from vibration. $25.00 down the drain on the first piece. Tried a different holder shortened the amount sticking out to the least possible......reduced the speed.....same result.....another $25.00 down the drain. Basically said "F" this......made all the pieces minus the radius in the lathe.

Moving on to the VMC now, I bored a set of jaws to hold three parts per vise.

Went in with a .156" diameter drill to clean out the center to full depth.....went in with another .437" diameter carb. ball mill 1300 RPM 7 IPM until full contact then 1.5 IPM made it through 3 pieces...CRUNCH...again. Up to $75.00 down the drain now. Being a glutton for punishment I tried it again only cranked up the RPM to 1500......made it through 5 more pieces before.....you guessed it......$100.00 down the drain now!

I am seriously considering HSS ball mill now. I am making the caps (also A2 material) to these vials right now in the lathe and the bottom of the .500"+.0006" ID is flat and I have been using a .4375" HSS 2 flute em to make the bottom flat and rough the bore and it has held up for over 90 pieces so far.

Do not understand why these carb ball mills won't work.....then again......not 100% sure if I am going about this the right way......especially now!

Any opinions out there? Have you guys run anything like these parts before?

Best Regards,
Russ

 

[PaulT]

Russ, since the spec on the inside diameter is pretty loose, can't you use a 135 degree 7/16" drill to both cut the full inside in one pass and use the tip to remove a good part of the round cavity on the bottom (a 135 degree drill will take out more of the cavity)?

This way with less metal to remove in the end cavity the ball end mills will last longer, especially if you take the the drill point as close as you can to the end of the round cavity. Then the ball mill won't have much material to remove in the center, keep in mind that ball mills work really poorly when used in "drill mode" because of their poor center cutting performance, so try to cut as much as possible out with the drill tip.

Paul T.

 

[Perry Harrington]

Perhaps the problem is not the bottom, but the sides. Have you finished to depth with a square EM, then just spot the bottom with the carbide?

Also, as odd as it sounds, I've had good success with a carbide ball mill with one flute missing, basically acts like a boring bar. I surmised that the lack of a second flute allows the carbide to cut without flexing too much. With 2 cutting edges, if one digs in, it causes the other to turn off center and dig in worse, then the act repeats itself and causes the hole EM to orbit and break. Try grinding one of the flutes off and doing a stepover to final diameter.

 

[PhillipM]

I'd agree with that, you only want one flute cutting.

 

[wrustle]

Spoke with Carl out at LakeShore Carbide and he suggesting pecking as the only viable option due to nowhere for the chips to go when plunging.

So....I guess it's sit back and peck with an air blast to get the job done.....but just in case I did order 3 more carbide ball mills.

Later,
Russ

 

[HuFlungDung]

I think I'd try circular interpolation with a 5/16 or 3/8 ball mill. Not just one pass of course, but maybe 5 or so, to machine the surface in steps.

I suspect that the full diameter ball will probably create a scummy looking surface after its initial keen edge is lost. Interpolated will come out nice and shiny. Keep the feedrate really low because of the tiny circle being interpolated compared to the sweep of the tool.

 

[rklopp]

Neck down the ball end mill behind the tangent point for the ball part so it will only cut on the ball. You want to kill any tendency for the straight part of the flutes to cut, because when they do (and they will, due to springiness of the cutter, work, and spindle), you have a gigantic LOC and giant chatter problems. I get the same sort of problems if I try to drill too deep with an endmill. A drill's lands don't cut, but an endmill's does.

 

[cnctoolcat]

All good ideas you're gettin' Russ-key. Combining 2 ideas, you can grind away one of the ball's end flutes, and neck the ball end mill down on both sides. Basically make a half-ball-round-end boring-bar-thingy.

Even better, use a 3/8 ball end mill modified in this way, and sweep the bottom of the bore to create the 7/16 dia round id bottom.

Good luck.

Greg

 

[izzoe46]

Im confused, Did you give up on donig this job on the lathe after 2 tries? and where you using an endmill?

1" deep, .4something id lollypop, should be doable with a good boring bar.

maybe i dont understand.

machine alot of a2, d2, s7 and I dont go higher than 900 rpm .005-.01 ipr. doc about 20-30 thou. and thats cause its a lil toolroom haas.