Printable View
Hi All,
I have just had my first go at using variables in a Fanuc program.
The part required me to shift the Z offset for consecutive parts.
One of the Sys Variables I ended up using left me confused. I am using #5263 for Z axis, G56, Turret 2 (makes sense) and #5222 for Z axis, G54, Turret 1.
I originally was trying #5223 for the latter, but this did nothing to the offset.
Can someone please explain which variables do what in a multi turret lathe (MoriSeiki NZ)?
thanks.
Gidday zooloader, I am using a zt1500yb . The Sys Variables that i am using were set up in a master program by the agent who supplied the machine. I am not sure this will help but here goes. This is how they are used in my programs.
This is what is written into the program for head 1 and is equal to the values in the work offset screen
These are also written into the program for head 2 with the values coresponding to the values in work offset screen as well.
#5201=0 (COMMON)
#5202=0
#5203=0
#5204=0
#5221=0
#5222=0 (G54Z)
#5223=0
#5224=0
#5241=0
#5242=0 (G55Z)
#5243=0
#5244=0
A value set in the common variables above will shift the coordinate sys in the same direction disregarding wether it is sp1 or sp2 that is used.
G54 work coordinate sys is selected automaticly when the power is turned on.
Allen at Qmac would be your best bet for information if you are close to Brisbane.
Cheers have a good one.
(flame2)
if you need to make only 7 parts or less then just pre-set the workshift G54-G59 to some values then call up each workshift in the main program before running the part with a M98.
i.e.
O0001
G54
M98 P0002
G55
M98 P0002
G56
M98 P0002
G57
M98 P0002
G58
M98 P0002
G59
M98 P0002
G54
M30
%
it's a little bit dangerous to incrementally adjust workshifts using macro system variables without proper checks otherwise the machine can be in the wrong workshift or out of position by multiple incremental shifts if/when a re-start is needed.
another way is to write the machining program in incremental (generally using W instead of Z). position the tool then call the program (M98 Pxxxx) and it'll do it's work from that position. at the end before the M99 return the tool to the same start position then shift it again using W from the main program then call the incremental sub again.
you can keep going like this all day not just 7 times...or at least until you shift into the chuck ;)
Thanks Blue1. That's interesting because it still doesn't match what I'm using. #5263 for me, but you suggest #5262 . I had several phone calls with Alan Clinch prior to my original post, and he was going to look deeper into it for me.
I did a second similar job fine using this shift/loop to make 11 parts from the billet.
I just need to make a parts catcher now!