tool change macro needed, EXCEL PMC-10T24 W/ Fanuc 21-M need 9001 please help!
I have seen a lot of Fanuc tool change macros but none specific to the 21-M, I do not know
if it necessarily has to be the exact control but i am sure the same machine type EXCEL PMC-10T24.
so I had to take the Boards out for a a repair and Fanuc Tech told me to back it up so i did but This being our only Fanuc and i have never had to work on or back it up i thought the usual machine and NC params would do! WRONG!
does anyone have #9001? I have seen alot of close ones but not the exact machine can anyone help me?
Hello rcd machinist,
When a Tool Change Program is absolutely necessary, it is common for a hard copy of the program to be included in one of the manuals that came with the machine (if they still exist). Have you searched for such a program copy in any manuals you may have, It will be in the Machine Tool Manuals, not in the Fanuc Manuals.
Tool Change can be carried out completely by the PMC, or a combination of the PMC and the Tool Change Macro. Accordingly, a Tool Change Program can range from very simple, just positioning the axes at a convenient location and possible not really necessary, to quite complex and necessary, with interaction between it and the PMC. I would first determine how necessary a Tool Change Macro is for your machine.
As the program number is O9001, check if the number 6 is registered in parameter 6071. If so, replace it with Zero. With a 6 registered in this parameter, executing M06 will result in the control attempting to execute program O9001, with an alarm being raised if the program doesn't exist. By removing the reference to 6 in the parameters, M06 will be treated like a normal M code and processed by the PMC when executed.
As your Tool Change Program was O9001, it will be called as a Subprogram and not a Macro Program. In this case no arguments are passed, so your original Macro will not be expecting any data, except perhaps the System Variable for the last T Code executed, which isn't passed as an argument.
To test if your machine really needs a Tool Change Macro and after setting parameter 6071 to Zero, register the following Main Program under whatever program number is available:
O0001
N1 G91 G28 Z0.0
G28 X0.0 Y0.0
T01 M06
M30
Either you will have the Tool Change execute correctly, meaning that a Tool Change Program is not absolutely necessary, or an alarm will be raised. If a Tool Change Program is determined to be necessary and no one come to your rescue with the correct program, it becomes tough. However, if you, or if you can get someone that can follow the PMC Ladder, you will be able to backward engineer the required Tool Change Program, but a bit of time will be involved.
Regards,
Bill