part zero

[positiverake1]

How do you set the part "Z" zero after setting the tools on the Q setter on a puma 8s lathe with a mits, meldas 500 control? I just got the Q setter working,someone had the wire's pulled off? had to figure out the refrence numbers from home to the Q setter, the only way I could set the "Z" zero is after setting the tools, bring a tool back to the the number from the tool set(tool data) zero the pos. screen, go to my part zero and put that number in my G54 Z work shift, is this right? if it is, its kind of lame, Im use to a mori sieki with the button on the control panel, maybe a macro is in need?

[Hogger]

You should have figured it out by now but on our Puma 200 with Mits control you have to position the chosen tool at Z0, take the Machine Position and either add or subtract the Z Geo. position that gets put in by the tool setter. On our machine I believe you add a Geo. -# as a positive to the machine position to get part 0. Then enter that # in the G54 Z offset box, I have yet to find a way to let the machine do it for me like a Fanuc control will do.

[positiverake1]

I ended up writing a macro,it works good,almost like the button on the mori,the thing I was trying to get away from is having to punch in the numbers by hand and this macro sets it. no fat finger mastakes!

[Hogger]

I might be interested in how to write a macro for that, care to explain how it's done and what the program looks like?

[positiverake1]

Yes, I'll get it to you soon as I can, cant remember the machine numbers right now.

[positiverake1]

Here it is, this is for a puma 8s with a mits meldas 500 control, you can change what ever you want,I have it using tool #2,thats what I use for R.turning, I was going to write it to use any tool but it got to envolved for the time , anyway this works ok.

this is the program I call up after setting all my tools
O9(PART ZEOR PROGRAM)
G65P9003T2 (CALLS PROGRAM 9003 WITH TOOL 2)
M30

this is the macro

O9003(PART ZERO MACRO)
M0(SINGLE BLOCK/RAPID SLOW)
G28U0(GO HOME X)
G28W0(GO HOME Z)
#5222=0(SETS G54 TO 0)
G0T[#20*101] (PICKS UP OFF SET 2 FROM MAIN PROGRAM)
#100=[20*101] (SETS #100 TO 202)
IF[#100NE202]GOTO1 (CHECKS TO SEE IF T2 IS USED,ANYTHING BUT T2 FROM MAIN PROGRAM WILL ALARM)
G97S1000M3 (STARTS SPINDLE)
G0W0 (GOES TO TOOL SET ZERO) (AT THIS POINT GO TO MANUAL AND CRANK THE TOOL TO WHERE EVER YOU WANT YOUR Z ZERO TO BE)
#522=[5022-2102] (SUBTRACTS TOOL 2 DATA SET FROM MACHINE POSITION AND PUTS IT IN G54)
G28U0(GO HOME X) (PUT BACK IN AUTO)
G28W0(GO HOME Z)
T[#20*100] (DUMPS TOOL OFFSET)
M99(GO BACK TO MAIN PROGRAM)
N1#300=2(USE TOOL 2) (ALARMS IF WRONG TOOL IS USED)
M99

thats it, looks confusing but it works,this sets G54 only,and you need to be in single block so you can go into manual handle to find your z zero, if you want you can dump the tool 2 check stuff and just put t0202 or what ever tool you want in the macro,like I said I was going to have it use any tool ,maybe later when I got more time, hope you like it, add to it if you like, make it better!!