need help communicating to Fanuc Omc controller

[maxvic]

I am trying to download g code from mastercam version 8 to a Fanuc Omc controller but I don't know the proper settings for parity bit -even, odd, or none? plus I am very new at this CNC stuff and I don't know whether to have the panel on the mill set to "edit" or "memory" for proper transmission. If someone could walk me through I would greatly appreciate it.

Thanks,
Jim

[Dan Fritz]

The proper settings on the Mastercam side would be 7 data bits and Even parity. The baudrate and stop-bits setting must match the parameters in the CNC control.

The 0MC parameters responsible for these settings are 0002, 0012, 552 and 553. If you tell me how those parameters are set, I can tell you the baudrate and stop-bits setting on the control.

When Mastercam is ready to send a file, put the Fanuc into EDIT mode, then select the Program page on the CRT, turn off the memory protect key switch, and press the INPUT button. Some of the 0MC controls have soft-function keys to read and punch programs, others do not. If you have the "soft" keys on the bottom of your CRT, you should be able to use either those soft keys or the INPUT and OUTPUT/START buttons on the panel to send and receive files.

[maxvic]

Thanks for the info Dan, I'll look up the parameters and let you know. How important is it to have the proper post processor settings on the mastercam side - MC has just about every known controller except the fancuc stuff, just wondering if I can send it to machine under some other generic post and then just change whatever small details that don't jive with the Omc by hand once it is in the machine. I've been trying to send it over under the post processor MPfan1 which seems to output pretty generic looking Gcode.

Thanks again,
Jim

[maxvic]

Hi Dan, parameters 0002, 0012, 0552, 0553 all read: 00000000. One of the settings on my settings page is set for ISO but I only have options for ASCII, EIA and BIN for output from mastercam, am I safe to assume ASCII and ISO are similar enough to work or should I change my setting page to EIA to jive with mastercam?

Thanks again for your help.

Jim

[Dan Fritz]

Are you sure that those parameters are all zero'ed out? Could you be looking at the Diagnostics page instead? Also, are you ABSOLUTELY sure that its a 0MC control ?

In any case, here are some recommeded settings:

On the Fanuc 0MC:

1st paramter page:
set PUNCH CODE = 0 (ISO)
set I/O bit = 0

Page up to parameter 0002 and enter:

1 x x x x x x 1 (all bits marked "x" are for something else -don't change them)

Page up to parameter 552 and enter:

10

At the Mastercam side, make these settings:

baudrate: 4800
stop-bits: 2
data bits: 7
Code: ASCII
Parity: Even
End-of-block code: LF (or) LF/CR
Handshake protocol: Xon/Xoff (sometimes called "DC codes")

Be sure that your files have a separate line with a "%" at the beginning and also at the end.

That should do it. Prepare Mastercam to send the file, put the CNC into EDIT mode, turn off the memory protect key switch, then press the INPUT button. If the file has an O-number in it, then the Fanuc will save under that O-number. If there is no O-number in the file, then you'll have to key in the letter "O" plus a 4-digit number before pressing INPUT.

Hope this helps.

[maxvic]

Hi Dan, I must have been looking at the diagnostic list, do I page up from my initial settings page to get to the other parameters? It is definitely an Omc. I'll enter the above info and give it a try, I kept getting an 085 alarm when I would try to download so I know something wasn't jiving.
Thanks again for all your help - I'll let you know how it goes
Jim

[maxvic]

Hi Dan, I got the things talking to each other today. Your settings worked. Thanks again.

Jim