Deburring part off tool burr on thin rings?

[Bradley.linsmeye]

Hi guys, I have 1000 rings to make on a lathe. .940 O.D x .677 I.D and .06 thick. Making the part is easy. But deburring is slowing the process down. Currently we're using a pencil grinder because they're so thin its hard to use whirly knives or debur with a countersink. And it's so thin with a flatness tolerance of .001 I don't want to clamp it in a vice to hit it with a counter sink and risk bending it. Any ideas? Thank you

 

[Orange Vise]

ID chamfer/groove before partoff?

 

[Fadriver]

Hi guys, I have 1000 rings to make on a lathe. .940 O.D x .677 I.D and .06 thick. Making the part is easy. But deburring is slowing the process down. Currently we're using a pencil grinder because they're so thin its hard to use whirly knives or debur with a countersink. And it's so thin with a flatness tolerance of .001 I don't want to clamp it in a vice to hit it with a counter sink and risk bending it. Any ideas? Thank you

Not an expert but i would try small groove before cut-off
then sand paper, i have done tooling not production never knows
cnc lathe

 

[Booze Daily]

I’d probably make something to hold it lightly and hit it with a cordless drill with a chamfer tool.

 

[FredC]

What Orange Vice said. Sharp cut off tool, probably not an insert tool. I have run the cut of blade in almost parting off then pulled out and moved .001 in Z and do it again completing it this time. If you have live tooling a rotary cut off saw give the least part off pressure and smallest bur.

 

[SeymourDumore]

One of my returning parts is a .925 x .645 x .030 washer, batches of 300-400 twice or thrice a year....

As such, I believe to be qualified to say that nothing but a proper 2nd op will produce a good part.
Part-off to .003-.005 longer in op1.
Then bore a 5C collet to just a tad deeper than half the width and finis face in the opposite direction of the cutoff.
I do it on a Hardinge by hand, having a sixpack, listening to 80-s Eurotrash ... maybe 3 hours tops?
Yours is even easier as you've got .060 thickness to work with.

 

[MCritchley]

ID chamfer/groove before partoff?

I’ve done the same. It’s also a crucial step it the ring has an ID thread that runs the length of the part.

.001” is easy- rough the OD cut off groove then cut the part off with the Id grooving bar. There will be a tiny burr on the face that you can stone off easily.

 

[Nerdlinger]

Tumbler with small cutting media stones?

 

[EnderDRM]

ID chamfer/groove before partoff?

yes but i use a radius.
It's easier to blend.
And I use a .003 r cutoff tool.
If you get the blend right you don't have to deburr them at all

 

[Rob L]

One of my returning parts is a .925 x .645 x .030 washer, batches of 300-400 twice or thrice a year....

As such, I believe to be qualified to say that nothing but a proper 2nd op will produce a good part.
Part-off to .003-.005 longer in op1.
Then bore a 5C collet to just a tad deeper than half the width and finis face in the opposite direction of the cutoff.
I do it on a Hardinge by hand, having a sixpack, listening to 80-s Eurotrash ... maybe 3 hours tops?
Yours is even easier as you've got .060 thickness to work with.

I hate to say it but this is what I have found too, I have a repeat job of POM washers and I've found the best way to get a burr free back is a second op, in my case I hit the ID with a boring bar with a chamfer insert. I've tried all sorts of other things, adding a chamfer before part off, using very sharp inserts with an angle on but all of them have ended up being more time consuming to faff around with than just doing the second op.

 

[Ox]

I too would chamfer from the bore as well.
Use a threading tool and set your tip to match the back edge of the part.

Then toss in the vibe when done.


--------------------

Think Snow Eh!
Ox

 

[guythatbrews]

You can get close with ID break before part off but if you really need no burr just form a chamfer in speed lathe. If you have trouble with secondary burr form a radius. Sometimes it pays to add a 2nd op and not fight it.

 

[Pete Deal]

What's acceptable depends on the part.

I agree that the only way to get a real nice back end is with a 2nd operation. I'm doing that now on some parts. Facing the back on my Southbend.

I have some parts that the the burr on the back side is ok with the customer. It's got a bore so as has been suggested I'm putting an inside groove using an old single tooth thread mill, then parting off. The inside groove, which winds up as a chamfer on the back side moves the burr out from the bore some so it doesn't interfere with the bore.

I use a PH Horn parting tool and when trying for a minimal part-off burr I use an insert that has a little angle to it. They sell them with right or left angle. This makes the burr very minimal.

 

[guythatbrews]

With something this small, an automated deburring system could deburr it in about 5 seconds.

Can you describe your system please?

 

[michiganbuck]

Might a 3/4" Norton point-mounted center lap wheel be used?
Hand-hold the ring to the wheel.
Glendo Accufinish

Center Laps | Grier Abrasive Co. Inc.

GRIER’s Center Lap Mounted Points have a 60 degree included angle. Center Lapping is used when you need to finish center holes in parts that require turning or grinding between centers. Center Lap Mounted Points are wax treated to minimize loading.

grierabrasive.com