What's new
What's new

Deburring part off tool burr on thin rings?

Joined
Sep 27, 2020
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
 

Fadriver

Aluminum
Joined
Apr 24, 2011
Location
los angels ca.
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
 

FredC

Titanium
Joined
Oct 29, 2010
Location
Dewees Texas
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

Diamond
Joined
Aug 2, 2005
Location
CT
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

Hot Rolled
Joined
Mar 22, 2007
Location
Milwaukee
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.
 

Rob L

Aluminum
Joined
Nov 5, 2019
Location
Staffordshire, UK
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

Diamond
Joined
Aug 27, 2002
Location
West Unity, Ohio
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

Hot Rolled
Joined
Dec 14, 2017
Location
MO, USA
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

Stainless
Joined
Apr 10, 2007
Location
Morgantown, WV
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.
 








 
Top