How to change the reference point on a fanuc 6MA

[alfaguilar]

I need some help, when I do G 28 X0 Y0 the machies goes all the way to the front right, I would like to have this point in the middle of the table, can can I do that, your help will be appreciated.

[fordav11]

on the 6M I worked the reference was set using G92 from where-ever the current position is.
If you are at zero return a command G92 X300.0 Y300.0 Z300.0 sets the home position to those numbers. You can set the zero anywhere you want. Simply move the machine to where you want zero then origin the position to 0 for X, Y and Z (on the position page press X then ORIGIN and repeat for Y and Z)
Then zero return the machine and check the current position and put those numbers in the G92 line at the top of the program. Thats a very rough way to set it. usually you would clock up a hole or something fixed on the job like the centre of the part and set X0 Y0 to there. Z0 is always zero return and the tool length will be a positive number and different for each tool so the machine knows where Z0 is. Some people set Z0 off a fixed block on the machine and the tool lengths come from there also. It depends on how the machine is configured.

This is pretty fundamental CNC setting stuff. If you don't understand the basics you should read up on it and/or check the machine manuals.

[alfaguilar]

Fordav11
Tha's what I do, I use G92 at the begining of the program but everytime I run the program it keeps moving the coordinates because of the G92, I need to use another comand that I can undo G92 at the end the program.
I am getting along with this, when I first start the machine the first thing I do I run a very short program that contains G92 and the coordinates that bring the table to the center then it takes the center as X0 Y0 then the real program has all the coordinates refered to the center then it works fine.
the problem I see, if I forget to run the short program with G92 my real program is off, if somebody else runs the program more than once the center will be moved, what happends with G92 on my machine is, it sets the new coordinates as zero, so running it again it will move the zero by the numbers on G92 everytime it runs.

If I could have a manual for the control, that would be very helpful like you said, but I cannot find one.

[fordav11]

a 6M manual wont help. what you need to do is fundamental and will be in every manual and the 6M is pretty simple from a programming point of view.
however the coordinates should not change by themselves no matter what. maybe you are in incremental mode when you set the G92 or an incremental command is throwing it out.
please post your program and we can take a look and see whats going on. I suspect you have some other command in there that should not be there.

[Dan Fritz]

See if you have "G30" (second reference point return). If you can enter a "G30" without getting an alarm #10 (illegal G-code), then you have a second reference point. You'll still have to zero return one time after you turn the control on with G28 or a manual zero-return, but after that you should be able to give it a "G91G30X0Y0Z0" to send it to a point that you can define.

The G30 point is set by parameters 159 (X) 160 (Y) and 161 (Z), and it is the distance from the G28 point. You will have to set this value in metric if the machine has metric ballscrews and in inch if it has inch ballscrews.

[yours_prabhat]

In Other way you can try to Grid shift Methos by parameter number 82,83,84,85 Regards
prabhatmishra@gmx.com

[Dan Fritz]

Grid shift lets you make small adjustments in the primary (G28) zero return position, but G30 lets you set any point on the machine as a "second" zero point. Grid shift is only good for +/- one full turn of the pulse coder.

[fordav11]

its also over-complicating a reasonably simple issue. now if we can just see the nc program we can solve it.....

[GPena]

When you send the machine to the first refernce position with G28 in absolute mode (G90) the machine moves first to the part zero (G54 or G92) and then to the machine zero position. When you send it in incremental mode it goes direct to the machine zero position. Try this:

G91 G28 X0 Y0 Z0;

This should work fine.

GP.