Fanuc robodrill t10b - lost tool change program

Hello All,

I am in deep trouble.....one of my buddies was over helping me figure out my "new" Robodrill T10B and he deleted the tool change program that is used for tool changes. I now get error 078 when doing a tool change due to the program not being there anymore.

I don't know the program number but it was in the O9020-O9029 range from what I understand. I have manuals, but none of them actually have this program in there which I find utterly ridiculous.

Does anyone have a Robodrill T10B tool change program they can post for me? Maybe even a T10C or similar would be the same?? Not sure. I have a large run of tiny tapped parts due here shortly and this is my only rigid tapping machine, so I am dead in the water without it.

Any help would be greatly appreciated!
Thanks!
Nate

beginnermachinis said:

Hello All,

I am in deep trouble.....one of my buddies was over helping me figure out my "new" Robodrill T10B and he deleted the tool change program that is used for tool changes. I now get error 078 when doing a tool change due to the program not being there anymore.

I don't know the program number but it was in the O9020-O9029 range from what I understand. I have manuals, but none of them actually have this program in there which I find utterly ridiculous.

Does anyone have a Robodrill T10B tool change program they can post for me? Maybe even a T10C or similar would be the same?? Not sure. I have a large run of tiny tapped parts due here shortly and this is my only rigid tapping machine, so I am dead in the water without it.

Any help would be greatly appreciated!
Thanks!
Nate

Click to expand...

Hello Nate,

As there can be differences in Tool Change Macros for similar machines, as time goes by, your quickest option would be to contact the suppliers of the machine, or the Machine Tool Builder direct and ask for the supply of the Tool Change Macro for your particular machine. When calling, supply the Serial Number and Build Date of the machine.

Regards,

Bill

UPDATE:

I solved my problem(Methods Machine in Massachussets did, actually), but I wanted to post this on here to help any future poor Fanuc Robodrill souls out since it drives me nuts when people do not close these type of posts out with the solution.

Fanuc Robodrill T10B (I presume this if all Robodrills, but definitely the T10B) have an internal tool change program built into the SRAM or main program memory - this is NOT accessible by anyone from the machine panel - it is called on by the program through a parameter setting.

The only time you need an external 9000 series macro program for tool change is special cases (pallet changer, obstruction due to machining tall/large parts, etc). In those cases, you would program a separate 902X program as a custom macro INSTEAD of using the internal one. Basically you program a 6 into one of parameters 6080-6089 to access programs 9020-9029 when a M6 is called. This type of macro calling is in most Fanuc manuals (16M for my machine). If you were to put a 3 in, it would be when M3 was called, and so forth.

Basically,
parameter 6080 points to program 9020 (default factory setting is 0 for using internal program)
parameter 6081 points to program 9021 and so forth through the range.
Programs 9020 through 9029 that are able to be called with an M-Code callout. You put a 6 instead of a 0 in the parameter and that sets it to call a given program when that M code is called.

Example: In a given program, an M6 will call up program 9020 when 6080 has parameter as a 6 (when the parameters 6080 through 6089 set to 0, it will use the internal Fanuc tool change program).

My machine had a 6 programmed into parameter 6080 causing it to call program 9020 for tool changes whenever a M6 was used and when we accidentally deleted the program 9020, the machine errored out since it couldn't find the program. Removing the 6 from parameter 6080 and replacing with a 0 fixed it and allowed the machine to use the internal tool change program instead of looking for program 9020.
NOTE: If you have a pallet changer or other exception you probably can't use the internal tool change program due to potentially crashing the head into the machine.
If you get stuck, look me up at Samoco Industries and I will be happy to help you out if possible.

Nate

The 8 and 9 thousand programs should also be protected so they cannot be edited or deleted, I think it is in the 3400 parameters but would have to check.

Thanks, Wayne, you are right on. Should have been protected to begin with. But then again, I might be the one that changed that.