G68 and G69 codes

[kot137]

can anyone help me out with these codes maybe asample program

[lgreeves]

On a Fanuc control G68 is coordinate rotation "On" and G69 Coordinate rotation "Cancel". On your line with G68 supply the X & Y value for the position of rotation and an "R" in degrees of rotation. A negative number will rotate CCW.

G68 X0 Y0 R90.

At the end of the run use the G69.

[ebragdon]

I found some more info but the string you gave me was helpful. On the mazatrol m plus its G17 G68 X0 Y0 R5 for example. But my machinist here has raised the issue of whether this code only has to be inserted at the beginning of the program or at each tool change. Can you shed some light on this for me?

Eric

[Andre' B]

Originally Posted by ebragdon I found some more info but the string you gave me was helpful. On the mazatrol m plus its G17 G68 X0 Y0 R5 for example. But my machinist here has raised the issue of whether this code only has to be inserted at the beginning of the program or at each tool change. Can you shed some light on this for me? Eric

Don't know much about mazatrol but on the controls I have programmed if you want to rotate the entire program you just put it at the start. If you want to rotate parts of the program you turn it on and off as needed.
Also if by chance you are also using local work offsets G52, in my experience mixing the two can sometimes be unpredictable.

[psychomill]

On most controls including Mazatrol, there are some commands that won't work in G68 mode and you probably wouldn't want it to anyway. So, things like tool change commands, G28/G30 commands, etc won't generally work. This means you need to turn G68 on/off for each tool in the program.

You also cannot randomly change work offsets in G68 mode so on some controls, using G53 as a retract may become a problem (Since this is viewed as an offset for some machines).

You can use it in G52 mode and it's not that it becomes "unpredictable" but you certainly need to visualize it enough to follow it.

A wise thing to do is after picking up your work offset, turn on G68. At the end of the tool (before tool change), turn off G68 (G69). Next tool do the same thing....

[sinha_nsit]

Syntax:
G17 G68 X_ Y_ R_;
as already described.
If you omit XY words, the current tool position becomes the center of rotation.