Face Groove Chatter

[RACINGCONVERTERS]

Can anyone give me a better idea on cutting a face groove? I can not cut this groove with out chatter on any of my parts. It is .275 wide and .05 deep. I use a valenite tool with a .236 wide insert 150 sfm at .004 per rev. I have tried leaving more material for finish, less material for finish, slowing the feed down and slowing the sfm down all wothout any luck.

 

Any input I would be greatful for. Thank you in advance.

[chris m]

What material? How rigid is the part? How rigid is the setup? What radius on the insert?

 

Many things to try:

 

1) Narrower insert gives less tool pressure, try .118 or .157W

 

2) Heavier tool [bigger shank]

 

3) use 2 profiling tools instead of a grooving tool since you are so shallow

 

4) More feed [.004 is pretty light for 6mm wide insert]

 

the list goes on

[T_MALENA]

Can you switch to a narrower groover to finish with? Or try cutting a .05 wide x .05 deep relief into the face of the insert. As though you have 2 small inserts. This has worked for me in the past.

 

Matl?

[RACINGCONVERTERS]

The material is 1018 crs, If you know much about cars this is the fly wheel side of a torque converter. I bolt the three lugs (that bolt to the fly wheel) to a fixture plate on the chuck. the groove I.D. is 10.030.

 

The lathe is a Okuma captain l370, Chuck is Kitagawa 10" hydralic chuck, tool hoolder is 1" shank, insert has .03 radius.

 

I have also tried a smaller iscar tool without any luck also.

 

I do not have enough turret space to run two tools.

 

It only seems to chatter on the finish. It takes two rough plunges leaving .01 at the inside and outside of the groove. Than profiles the groove from inside to outside for the finish

 

What would be a good feed and sfm for this be.

[chris m]

On the speed / feed side I would definitely be running 350 - 400SFM in that material with an inserted tool but low rigidity can have a serious affect on surface speed. For finishing you probably want to feed about 1/2 of the TNR and run a smaller radius than you are; I'd probably be looking for an .008R [max] for a groove that shallow. With your DOC much smaller than the radius you are really setting yourself up badly from the get-go.

 

I have that machine and chuck combination and there is no issue there. You might consider taking up any space between the part and your fixture with some standoffs, hell, even tape or rags to suck up some vibration. Depending on how its laid out in the machine you could also try to hold a plastic [aluminum, whatever] cap on the part with the tailstock to try to soak that up.

[Tim Simmermon]

On your finish pass make sure that you are taking a pass from the outside to the middle of the groove and then from the inside to the middle of the groove. You don't want to take just a single pass on the finish and cut with the whole side of the tool. That will chatter no matter what.

[Kevangel]

another thing that has helped me in the past "on chatter" is really, really slow down the RPM(try one absurdly slow and see if this points you in a right direction)

[RACINGCONVERTERS]

Thanks guys,

 

I raised my sfm to 400 and feed at .008. Finished from both sides like Tim suggested and reduced the chatter so that with the right light you can see it but you can not feel it in the part anymore.

 

Thanks again for the quick response I am making parts again.

 

Matt