Leadwell v-40 m6 subprogram accidentally deleted

Hello machinist fellas

I accidentally deleted programs numbered 9000-9004. I'm in trouble now because M6 won't change tools now. When i try to change tool with m6, alarm "078 NUMBER NOT FOUND" appears and nothing happens. I dont have any manuals and no idea, how to write that again. Machine is Leadwell V-40 with Fanuc Series 21-M panel. This question might sound stupid but I'am student. And yes, my teacher dont know neither.

Thanks already
Sirkuskissa

sirkuskissa said:

Hello machinist fellas

I accidentally deleted programs numbered 9000-9004. I'm in trouble now because M6 won't change tools now. When i try to change tool with m6, alarm "078 NUMBER NOT FOUND" appears and nothing happens. I dont have any manuals and no idea, how to write that again. Machine is Leadwell V-40 with Fanuc Series 21-M panel. This question might sound stupid but I'am student. And yes, my teacher dont know neither.

Thanks already
Sirkuskissa

Click to expand...

Hello Sirkuskissa,
First, look at bit 5 of parameter 6001. If set to 1, Program O9000 will be called by a "T" code. This program will normally only apply to a Umbrella type tool changer where each tool can only reside in respective individual pockets. This type of system doesn't actually require an M06 to carry out a tool change. If bit 5 is set to Zero, you can disregard program O9000 for the moment.

For programs O9001 through O9004, look in the corresponding parameters 6071 through 6074 for the registration of the numeral "6". Whichever parameter in that range of 6071 through 6074, has 6 registered, will call the respective program O9001 through O9004. Lets say that 6 is registered in parameter 6072, then program O9002 will be called when M06 is executed in a program. In this case, if you were to register a program in memory under the number O9002 as follows:

O9002
M99

then the issue of the "078 NUMBER NOT FOUND" alarm would be resolved, but no tool change would occur. You really need to know the content of the program that's was being called by M06.

The Tool Change of any Fanuc controlled machined can be totally carried out by the PLC (PMC in Fanuc Speak), or by a combination of program commands and the PMC. The Tool Change Macro being called by M06 may be no more than ensuring the Z axis is at Reference Return and the X/Y axes are in a safe location for a Tool Change to occur, or it could cater for a more complex interaction with the PMC.

If you don't have a copy of the 9000 series programs, I'd suggest that your best action would be to contact the local agent and or machine builder of the machine, stating the serial number of the machine.

Regards,

Bill

For the future I believe 3202.4 will prevent editing of 9000 series programs

Contact Leadwell or their local-ish distributor to get it. If an email doesn't work then try by phone, or phone first. They will want the serial # of the machine.

What year and serial is your leadwell?

This is from a 1999 machine, "series no L1SIH037"

The front is square/boxy rather than some models (cant remember which year) that are curved.

If your machine is older or newer, it may still work, but I can't guarantee the ladder and counters are the same.




:9001
M6T#4120
#1132=0
IF[#1012EQ1]GOTO60
M66
IF[#1008EQ1]GOTO60
G80
#130=#4003
#131=#4006
G91G28Z0
G49
IF[#1013EQ0]GOTO60
#1102=1
N10IF[#1009EQ0]GOTO10
G30Z0
N30IF[#1010EQ0]GOTO30
G28Z0
#1132=0
G#130
G#131
N50IF[#1011EQ0]GOTO50
N60M67
M99


Also, as a side note, you should really just tell the teacher. I'm sure the guy has program backups to the machine. or at least he should...

I found backup program and i changed the delete protect parameter for 9000 programs. Thanks for the help guys!

-Sirkuskissa

dandrummerman21 said:

What year and serial is your leadwell?

This is from a 1999 machine, "series no L1SIH037"

The front is square/boxy rather than some models (cant remember which year) that are curved.

If your machine is older or newer, it may still work, but I can't guarantee the ladder and counters are the same.




:9001
M6T#4120
#1132=0
IF[#1012EQ1]GOTO60
M66
IF[#1008EQ1]GOTO60
G80
#130=#4003
#131=#4006
G91G28Z0
G49
IF[#1013EQ0]GOTO60
#1102=1
N10IF[#1009EQ0]GOTO10
G30Z0
N30IF[#1010EQ0]GOTO30
G28Z0
#1132=0
G#130
G#131
N50IF[#1011EQ0]GOTO50
N60M67
M99


Also, as a side note, you should really just tell the teacher. I'm sure the guy has program backups to the machine. or at least he should...

Click to expand...

I already told the teacher but he couldn't help me so I asked from you guys. That program you sent is correct