Need Help!- Special thin washers cutting on CNC lathe

[ARIK]

We are running thin washers job: OD=0.25" ID=0.1" and the thickness is 0.015" only. The washers are from AL 6061-T6
Any tips and tricks regarding how to minimize the burrs left after cutting and improving surface finish?

Thanks
Arik at Micron E.M.E Ltd.

[Shane123]

Originally Posted by ARIK We are running thin washers job: OD=0.25" ID=0.1" and the thickness is 0.015" only. The washers are from AL 6061-T6 Any tips and tricks regarding how to minimize the burrs left after cutting and improving surface finish? Thanks Arik at Micron E.M.E Ltd.

change your g97 to g96 for constant surface feed with your cutter. I like to run mine at g96 s450 with the max spindle at about 1200 for cutoff, and feed about .002 per rev, sometimes .001 depending on the finish... that will give you a better finish. as for burrs, i am assuming you are talking about the burr on the hole on the cutoff side? If you are, you can get cutoff inserts (or grind your cutoff) to be angled toward the part side. it helps but is not always the cure. you might need to to use some needle nose to pull the burr and then rub the cut off side on a sheet of emory paper.

[Sinistersam]

I don't really have any experience with something like that, but the first thought in my mind was the use of a vibratory tumbler. It should deburr and put a finish on them, in mass quantity.

[Monkey King]

If you do in mass, better by blanking die.

[ARIK]

Thanks shane and Monkey king.
I will try the G96 and update you, I can not make it using die since those are special washers with 3D face surface, they must be machined.
Arik

[mattstawicki]

Originally Posted by ARIK Thanks shane and Monkey king. I will try the G96 and update you, I can not make it using die since those are special washers with 3D face surface, they must be machined. Arik

If you want to cut them off clean, grind your cut-off tool 20 degrees across the front (point towards the part), w/ 18 degrees clearance (under). 3-4 degrees clearance (under) on each side, and tapered back 1-2 degrees on each side. I'd run it at least 6000 rpm's, with a .0005-.0007 feed. Also, keep the tool as narrow as possible to reduce cutting pressure and the size of the chip that will rub on the part. If I was using 1/4" barstock, I'd make the tool around .035 wide.