Need Help!- DNC Program Restart using Fanuc OTC

[tommcc]

Yang ML-28A lathe, Fanuc OTC control, PC running DNC4U communication program. How do I redirect program control under DNC operations back to the beginning of my program as I normally do when running a program from the Fanuc control by simply ending the program with M99Psequence number. I receive an alarm 078 when running the program DNC'd from the PC. The Fanuc and PC communicate receive and send just fine. Will I ever be able to restart programs under dnc mode with one click of a cycle start?

[MysticMonkey]

I think your DNC software has to support file queuing for instance XpertDNC I can queue a file and right click then select 'continuous' which will send this file 999 times

[angelw]

Originally Posted by tommcc Yang ML-28A lathe, Fanuc OTC control, PC running DNC4U communication program. How do I redirect program control under DNC operations back to the beginning of my program as I normally do when running a program from the Fanuc control by simply ending the program with M99Psequence number. I receive an alarm 078 when running the program DNC'd from the PC. The Fanuc and PC communicate receive and send just fine. Will I ever be able to restart programs under dnc mode with one click of a cycle start?

It depends on your software. My own software can be set so that that it returns to the beginning of the program indefinitely, the same as when running the program from memory, or it can be set to just run certain parts of the program.

You got the 078 alarm because you programmed an M99 command in the DNC program. If you are running a program that has sub programs (called with M98) the sub must be loaded into the control's memory. The M99 in a main program being used in a DNC session will cause an alarm because the control can't search the data on the PC and will be looking for a sequence number in the control that does not exist.

Regards,

Bill

[sinha_nsit]

I was under the impression that one cannot use M98 in DNC mode. But, as you said, and as I interpreted it, it can be used provided the sub is there in the control's memory. After the execution of sub is over, DNC execution would again start from the following blocks (after M98 block). Can you please once again confirm this. Thanks.

[dcoupar]

Originally Posted by tommcc Yang ML-28A lathe, Fanuc OTC control, PC running DNC4U communication program. How do I redirect program control under DNC operations back to the beginning of my program as I normally do when running a program from the Fanuc control by simply ending the program with M99Psequence number. I receive an alarm 078 when running the program DNC'd from the PC. The Fanuc and PC communicate receive and send just fine. Will I ever be able to restart programs under dnc mode with one click of a cycle start?

Have you tried using the DNC File Queue (see attached)?

[angelw]

Originally Posted by sinha_nsit I was under the impression that one cannot use M98 in DNC mode. But, as you said, and as I interpreted it, it can be used provided the sub is there in the control's memory. After the execution of sub is over, DNC execution would again start from the following blocks (after M98 block). Can you please once again confirm this. Thanks.

Thats absolutly correct Sinha, and was the same with old CNC controls that used paper tapes to run programs that were too large for memory. The Sub would be loaded into memory and called by M98 from the tape.

If the sub is in the memory of the control, when the M98 Pxxxx is read from the DNC stream, the sub is executed and the DNC is paused by an Xoff or RTS/CTS handshake until the sub has been completed.

Regards,

Bill

[sinha_nsit]

Thanks for info.