Need Help!- Cutting I.D. Grease Grooves

[darrellx]

I am need to cut a spiral (figure 8) grease groove on the I. D. of a bushing and cannot figure out how it is done. Any ideas as to how to do this would be appreciated.

Thanks

Darrellx

[LeftCoastCNC]

If you are working on a lathe, rapidly feed the Z-axis while taking a shallow cut with a boring bar or grooving tool. It would prabably be safer to feed away from the chuck.

[ZenOrbit]

Use light cut depths, and program your feed to whatever the pitch if your spiral has to be.

[mirage1000]

I also have the same problem.We used a cnc lathe with C axis and ball type carbide burr to cut the figure of eight oil groove and it worked for sampling purposes but I now have 500 parts to make from mild steel .My groove detail is different than yours in that the start and end points of the groove are 1/4" in from each end.There is a mechanical type machine available to do this I have heard that scrapes the material out based on a type of cam-auto type machine.I have not seen one working though.Can anyone help me???

[HuFlungDung]

Any chance you could cut the grooves on a mill instead of a lathe? I'm thinking the action is pretty fast for a cnc lathe, but rather leisurely for a milling op.

[Geof]

Isn't this what G32 is for?

[HuFlungDung]

I don't know Geof, I've never tried writing two G32's running in opposite directions, and sequentially, to see if the machine could accomplish it.

I would think that the closed end requirement of this groove would impose some constraints on what you could do, since any dwell of the tool would create an annular groove at each end of the groove. This might not be of any technical harm, but the customer would have to accept it.

Because the lead is high, and the cutting speed low, I would not anticipate good cutting action in steel with a stationary lathe tool, so that is why I was thinking a ball mill or a burr would do a better job. I'm pretty sure that a person could program the exact path on the mill without any unintended grooves occurring. A lollipop style ball mill would be required if a person were to do the job in a vertical stationary fixture.

[Geof]

Originally Posted by HuFlungDung I don't know Geof, I've never tried writing two G32's running in opposite directions, and sequentially, to see if the machine could accomplish it....

I bother I am going to have to read the bit about G32 again sometime; I got the impression G32 was bi-directional and that you could retract X while Z was moving.

EDIT: It would be almost trivial to program on a mill.

[mirage1000]

Yeah ,I have tried a mill before with a ball type carbide burr which worked ok.The problem with it is it means you need a large diameter cutter.The smallest I could get away with was 5/8" ball mounted on a 1/2" shank running at 3000rpm.A few years back we also used the c axis on a lathe to scrape the groove out as it allowed better control but it is only really succesful on brass/bronze materials.I think I have found one of these oil grooving lathes and will let you know how I get on.Cheers

[Bhua]

All,
You just add Q( for start angle ) into the same block with G32, then you will have as many start angles as you wish. Example program for figure 8 grease groove,

G97S250M3
G0X.400Z1.
G1Z-.125F.100M8
G32X.426Z-.955Q0(START AT 0 DEGREE)F....(PITCH DIM)
X...
X....
G32X.426Z-.955Q180.(START AT 180 DEG.)F...
X...
X...

but your machine need to have fast servo to achieve this thread G32. Other way you can achieve this task, that you need to do as broaching type cutting if you machine have C axis move(mill-turn machine type), here is example program:
YOU USE STAIONARY TOOL HOLDER, BUT SET ROTARY AS MILLING CW OR CCW.
G98.....(YOUR SAFETY BLOCK)
M45 (FANUC CONTROL, ACTIVATE MILLING MODE)
G0X.4Z1.C0Y0
G1Z-.125F100.M8
X.426F5.
H-180.Z-.955F1200.
X.4F50.
G0H180.Z-.125
X...(INCREASE DEEP OF CUT WITH YOUR CHOICE)
G1H-180.Z-.955F1200.
AND SO ON...

Wish you luck, and if you have other method to get this done, please share with me at huatrieubinh@yahoo.com.

Thanks,
Binh.