What's new
What's new

DNC from memory card Parameters for MT2000 Fanuc 16/18

MetalmanTi

Plastic
Joined
Apr 16, 2009
Location
Uintah, Utah
I recently posted about looking for the Mapps II parameters to do this but was looking for the wrong parameters. I have been in contact with our local DMGMORI Applications guy and we worked through the process so I though I would deposit them here so they can be searched and looked up in the future.
I hope this helps someone. I will put a link to this thread in my other post.

Here is what I have:
Need to have memory card installed for this to work.

Parameters
Setting-50(F6 setting)- cap parameter write = 1, NC parameter write = 1

System-NCsystem-MDI-OPRT-enter parameter #- press no-search

20 = 4 (tried 15 but it went into a loop and wouldn’t do anything) IO channel
138.7 = 1 (DNC operation function by a memory card is enabled)
3404.2 = 1 (address P of the block including M198 in the subprogram call function 0=indicating file number, 1=program number)
6080 = 0 (m code that calls the custom macro of program number 9020)
6300.4 = 1 (external program number search enabled)
8700.3 = 1 (In DNC operation from the PMC, OPEN CNC, or C-EXE, pre-reading is performed)
8706.0 = 1 (high speed operation)
8706.1 = 1 ( when this parameter is set, the m198 can also be executed with FOCAS/HSSB)
CAPS Parameter #152=1 (with card DNC function)
Change both parameter write back to = 0
Shutdown machine and restart

For some reason I did not have to be in the Tape screen.
Main program is in cnc memory.
Run main program from cnc memory.
Sub-programs must not have any underscores in comments.
M198 callout examples:M198P44 for program O0044, M198P1001 for program O1001.
Sub-programs file name must not have an extension. (ie, .nc, .txt)
Sub-program file name must have a the letter O at the beginning.
I was able to pull up program numbers less than 1000 and above 1000.
insert an M99 at the end of the subprograms if you want to return to the program in the cnc memory.
 








 
Back
Top