fanuc 11m not enough memory

[Nikola]

Hello! I'm new here and I need some help! Execuse me for my bad english! It's like this.. I dont have enough memory on my machine because my programs consists from 20000lines and my machine (Kitamura) with fanuc 11m recieves about 3000. So is there any way that i can send program directly from my PC?
Thank you for your help!

[Dan Fritz]

Yes, you can run directly off a PC using one of the Fanuc's serial ports in TAPE mode. You'll need some DNC software, a properly made cable, and you'll have to match the settings between the DNC software and your Fanuc's parameters.

Here's a diagram of a serial cable (using a 9-pin serial port on your PC)

CNC side (25-pin male) ------ PC side (9-pin female)
pin 1 ----------------- cable shield ----
pin 2 -------------------------------------- pin 2
pin 3 -------------------------------------- pin 3
pin 5 -------------------------------------- pin 7
pin 7 -------------------------------------- pin 5
pin 6 -----
pin 8 ----- <--jumper these 3 together on CNC side only
pin 20 ----


Parameters in Fanuc:

5110: 3
5111: 1
5112: 11

Set your DNC software to 9600 baud, 7 data bits, Even parity, Xon/Xoff handshaking

Also on the Fanuc "Settings/Handy" page, set the INPUT DEVICE FG (Foreground) at "1"

To run the program, get the DNC software ready to send, then put the Fanuc into TAPE mode and press CYCLE START.

If you get a "BUFFER OVERFLOW" alarm when you try to run your part, do this (assuming that you're using Windows 2000 or XP):

Control panel
Double-click SYSTEM
Click HARDWARE
Click DEVICE MANAGER
Double-click "Ports (COM and LPT)"
Right-click on COM port you're using on the PC (usually COM1)
Click PROPERTIES
Click PORT SETTINGS
Click ADVANCED
set the "Transmit buffer" slider control all the way to the LEFT (low)
Click OK many times to exit all menus
Try again

Good luck!

[nessei]

U maybe can using DNC under "Tape" selection, but for shortcoming u can't call sub program on DNC mode.

[Dan Fritz]

When running in TAPE mode, you can call a sub-program with an M98Pxxxx command, but the sub-program must be in the Fanuc memory. If you want to call a FILE on your PC as a sub-program, you can do that too with our PC-DNC Editor and PC-DNC Plus software. The software sees a "CALL" statement as a command to merge a file into the main program, like this:


N1
N2
N3 CALL FILEX
N4
N5

The DNC software does not send N3 to the machine at all. Instead, it sends "FILEX". You can also CALL sub-files from within sub-files (up to 7 layers deep).

[Nikola]

Thats great! Thank you Dan! I'll try that in a few day's when i complete my model and program. And yust another question. If I fail, is there any program that i can cut nc prog in few pieces? I use mastercam for making programs and im new in al that so it's hard for me to do that manualy!

[Nikola]

I'm not in this
I sent quick reply but its not shown.
I ment to say that ill try doing that bu if I fail, is there any program that can cut nc code in a few pieces so that i can fit it in machine memory few times?
I'm new in that programming and not so good yet to do that manually!

[cncdiag]

You could buy a replacement for your bubble memory that has more memory.
Tulip Electronic have memory boards that go up to 2meg for the Fanuc 11 control.
Cheaper than Fanuc to.