Minimizing "Tits" on Lathe

[Crashmaster]

Does anyone have any suggestions for how to minimize "tits" that form when cutting off stock on a lathe. Mine are around .055" in diameter. Is this just something that has to be dealt with?

[CountZero]

Sounds like you need to raise your tool up about 0.055"/2.

[Bowman]

Yep sounds like your pip tits are from the toolbit not being centered to the workpiece.

A trick is to take a small piece of shim stock and run the toolbit into the round workpiece with the shim inbetween. If the shim tilts up you need to lower your bit if it tilts down you need to raise the bit. when the shim stay vertical with little or no tilt you know your near dead center. This is just a quick way to tell where your at with the toolbit.


Bo

[Crashmaster]

Thanks guys, So in a perfect world you wont have a tit?

[cdlenterprises]

Where are you trying to remove the tit from, the part or the remaining bar? I have never found a way to remove all of the cutoff tit from the part. I had always thought that was due to the material getting so weak at such a small diameter that it can't withstand the cutting pressure and breaks off. Slowing the feed down and using an angled cutoff tool vs. a straight or flat one can help to minimize the 'tit" but I haven't found a way to eliminate it. Maybe some of you screw machine guys can help out...

[Bowman]

You may always get some sort of small tit due to the toolbit deflection pushing it slightly off centerline. And as Cdlenterprises noted the metal will get weak when you get down to the center especially depending on how big a piece is hanging off the end. We always cut through to nearly full depth then backed off and just broke the piece off by work hardening the little remaining connection spot with backand forth motion. Then just chuck up that end and face the part smooth.

[Geof]

cdlenterprises has it pretty well complete; as soon as the cutting force at the parting tool is greater than the strength of the remaining material the part breaks off leaving a tip on the parted off piece. Going very slow and having an angled parting tool will minimize it.

Depending on the depth of the part and the material it may be possible to have a large angle so the tip barely exists. Brass and Delrin are two materials that can be parted with a parting tool tip at around 45 degrees. Using any angle on aluminum and many other materials that generate stringy turnings rather than chips is almost impossible.

If you are doing this on a manual machine there may not be much you can do. I technique I have used with production work on a CNC lathe is part using a straight carbide tool down to a diameter large than the break-off size, then go in with a HSS parting tool that is thinner than the carbide and has a large angle to make the final cut and part off the piece with almost no tip. This does put an extra tool change in a cycle but the time taken here can be more than recovered by the time saved in deburring operations later on.

When parting off into a bore the tip is actually a ring that can have a really sharp edge and can be a real pain to deburr. A technique I have used is to use a threading tool to cut a vee groove inside the bore and then part down to meet the groove. When the parting tool edge is aligned nicely with the center of the groove the residual ring can be polished off with a quick swipe across a piece of fime emery on a flat surface.

[Crashmaster]

My problem is that I am running several thousand parts and they are only 5/16 in dia and .6 long, kind of a pain to grind all of those tits. I will try slowing the feed down and see if that minimizes it at all. I would be happier if the tit were on the stock, then it wouldn't matter.

[jackson]

Originally Posted by Crashmaster My problem is that I am running several thousand parts and they are only 5/16 in dia and .6 long, kind of a pain to grind all of those tits. I will try slowing the feed down and see if that minimizes it at all. I would be happier if the tit were on the stock, then it wouldn't matter.

try slowing the feed down and the speed right at the bottom, i do this and it helps alot

[Geof]

Originally Posted by Crashmaster My problem is that I am running several thousand parts and they are only 5/16 in dia and .6 long, kind of a pain to grind all of those tits. I will try slowing the feed down and see if that minimizes it at all. I would be happier if the tit were on the stock, then it wouldn't matter.

Don't spend time even doing this; put in two parting tools as I do.

[jackson]

Originally Posted by Geof Don't spend time even doing this; put in two parting tools as I do.

Why 2?????

[Geof]

Originally Posted by jackson Why 2?????

From Post #7 above:

"... technique I have used with production work on a CNC lathe is part using a straight carbide tool down to a diameter large than the break-off size, then go in with a HSS parting tool that is thinner than the carbide and has a large angle to make the final cut and part off the piece with almost no tip. This does put an extra tool change in a cycle but the time taken here can be more than recovered by the time saved in deburring operations later on..."

This is with material such as leaded steel and aluminum where doing the whole part using a large angle tool is not possible.