Full radius groove...

[Tancuda]

Hi all,
can someone help me on this (see pic attached).

I'm working on a lathe with an OSP P200LA,
I have some experience on OSP U100L, so I'm pretty comfortable with
the one touch IGF stuff. I want to program that full radius groove, but
with a round tool and in OD, not in grooving, so from right to left.

I'm having trouble with Z finishing stock, the tool will left finish in Z
but only on the left side. I have tried with tip 0-3-8, "multi fonction tool".

If I check the G code produced, there's always a G42 for the shape, and did not find a way to generate G40, to try with center cutter.

Any expert out there !

Thanks a lot.

[underthetire]

Did you set the correct p code in your offsets for that tool geometry?

I always used a grooving cycle when I did those, so idk on turning.

[Tancuda]

Did try P code 0, 3 and 8, always the same.

And with the turning method, the finish is in one pass.

[fordav11]

the G code for a radius groove set at the center line of the insert is pretty simple.
you don't say what size your grooving insert is or the radius of it.
assuming 0.200" radius (0.400" wide).....

G0 X4.1 Z-1.5
G1 X3.01 F.005
G0 X4.1
Z-1.2
G1 X3.6
G2 X3.0 Z-1.5 R0.3
G0 X4.1
Z-1.8
G1 X3.6
G3 X3.0 Z-1.5 R0.3
G0 X4.1

If the insert radius is smaller take a few straight plunge cuts then clean it up with the G2/G3 above.
Or if you give me the width and radius of your tool I'll write you the G-Code for it....

[Tancuda]

Thanks Fordav11, but I'm programming with the one touch IGF,
automatic decision (process).

My tool would be .375 wide (.1875 Radius).

The machine is new (LB4000EX M) and I have to develop it as much as I can
with the IGF.

Thanks

[txcncman]

Nice. Lie to the IGF until you get it to cut the profile wanted.

[OkumaWiz]

You've found the weak spot in IGF. In order for IGF to groove it has to have a flat in the bottom of the groove greater than or equal to the tool width. It is one of the checks it performs for tool clearance.

That being said, you can use a straight grooving process to rough out the center and an OD turning process to "turn" the left and right profiles of the groove using the correct tool nose comp for each process.

Best regards,

[Tancuda]

Thanks OkumaWiz, I'll give it a try,
now that I know it's a weak spot, I can go on.....

Thanks again.