grooving on Fanuc O-T

[Spiderman]

We are attempting to put a .5 wide groove (.25 radius) on a journal using a .312 wide groove insert (.156 radius). There seems to be in an issue with our program/controller. Our tool does not move in a coherent fashion.

Here is what we have:

Z-5.75(plunge cut)
X6.5M8
G1X5.8F0.01
G1X5.31F.006
G0X8.0
G1G42Z-5.808F.009
G1X5.8
G3X5.3Z-5.74R0.25F.004(2ND CUT)
G0X6.0
Z-5.622
G1X5.8F.009
G2X5.3Z-5.76R0.25F.004(3RD CUT)
G1G40X8.2F.015

We want to plunge on our first cut, move toward the shoulder of the part, cut again, then move away from the shoulder and make a third cut.

The Fanuc O-T controller is on an older Yang lathe (ML-55A).

Thanks for you help!

[Dwane]

Spiderman,
I have done this many times without using tool radius compensation. You didn't give much part information, but I am going to make these assumptions based on what you did write.

Your tool is .312 wide, with a full radius.
The tools Z zero to part Z zero, is its front edge.
The grooves greatest distance from part Z zero will be Z-5.808
The groove will be .5 wide, with a full radius.
The bottom of the groove will be 5.300 dia..
A safe diameter clearance above the part is is 6.0"

I usually program a inside radius by programming the desired part radius minus the tool radius (.250-.156=.094).
My simple program might look like this:

G0X6.0
Z-5.71 (CLOSE TO MIDDLE OF GROOVE, ABOVE PART)
G1X5.31 F?
GOX6.0
Z-5.808 (GROOVE FARTHEST FROM FACE)
G1X5.488
G2X5.3Z-5.714R.094
GOX6.
Z-5.62 (GROOVE CLOSEST TO FACE)
G1X5.488
G3X5.3Z-5.714R.094
GOX6.0

I left out feed rate. I don't think you really need the R.094, but I put it in anyway. I hope that I helped.
Dwane

[Spiderman]

Originally Posted by Dwane Spiderman, I have done this many times without using tool radius compensation. You didn't give much part information, but I am going to make these assumptions based on what you did write. Your tool is .312 wide, with a full radius. The tools Z zero to part Z zero, is its front edge. The grooves greatest distance from part Z zero will be Z-5.808 The groove will be .5 wide, with a full radius. The bottom of the groove will be 5.300 dia.. A safe diameter clearance above the part is is 6.0" I usually program a inside radius by programming the desired part radius minus the tool radius (.250-.156=.094). My simple program might look like this: G0X6.0 Z-5.71 (CLOSE TO MIDDLE OF GROOVE, ABOVE PART) G1X5.31 F? GOX6.0 Z-5.808 (GROOVE FARTHEST FROM FACE) G1X5.488 G2X5.3Z-5.714R.094 GOX6. Z-5.62 (GROOVE CLOSEST TO FACE) G1X5.488 G3X5.3Z-5.714R.094 GOX6.0 I left out feed rate. I don't think you really need the R.094, but I put it in anyway. I hope that I helped. Dwane

Dwane,

Sorry about the lack of information. Yes, I will be teaching the tool 'zero' from the end of the part and the edge of the tool.

Now, from the end of the part to the back of the groove is 6 inches. I believe I need to plunge prior to 6 inches because of the tool width (.312) with a full radius. Maybe my calculations were off, but I thought I would plunge -5.75 because of the .250 radius that is needed.

Maybe I can get a sketch and attach it to the next message.

[Dwane]

Spiderman,
I apologize, I have been working by memory, it has been a couple of years since I programmed a Fanuc lathe. I believe that I mixed up the G2 and G3.
G2 is clockwise, G3 is counterclockwise.
If the center of your groove is at Z-5.75, and you touched off your tool to the face of the part, then to get the center of the tool to the center of the groove, you must add half the width of the tool (.312/2 =.156) (.156 + 5.75 = 5.906).
I make it a practice to give the tool a little clearance doing the 1st radius sweep, so I would plunge in a little shy of Z-5.906.
I was figuring for the back of the groove to be Z-5.808 based on your other figures. If it is Z-6.0, the above program should work providing that you add .192 to all the Z- figures, and correct my mistaken G2 and G3.

It might look like this:

G0X6.0
Z-5.9 (CLOSE TO MIDDLE OF GROOVE, ABOVE PART)
G1X5.31 F?
GOX6.0
Z-6. (GROOVE FARTHEST FROM FACE)
G1X5.488
G3X5.3Z-5.906R.094
GOX6.
Z-5.812 (GROOVE CLOSEST TO FACE)
G1X5.488
G2X5.3Z-5.906R.094
GOX6.0

Again, I'm not sure that you need the R.094's in the program. It might work better without them since it has the necessary G2 and G3 information.

Dwane

[mhed]

the original prg doenst work cos, you move to the left with g42 and then moves to the right, still in g42 mode, wich should been changed to g41 or just turned off before that move.