[giorgis]

Hello,
is there anyway to define,if there is any problem in the port(25pin) of my machine;I ask this,because i have tried several times to connect my pc with my machine and i cant't do anything.The parameters of the machine have been changed and the dnc software that i use is the NCnetlite of cadem.My machine is from Bulgary MC-063 and the controller of it is Fanuc 6m-b.I would be very grateful of any help
Thank you,giorgis

[Dan Fritz]

Here are some settings that we know will work with the 6M-B. If you have a bad serial port on the CNC or on the PC, there's almost no way to know that without using a testing device or an oscilloscope.

Setting page on CNC:

TVON = 0
PUNCH CODE = 1 (ISO)
INPUT DEVICE 1 = 0
INPUT DEVICE 2 = 1

Parameters:

311: 1 0 0 0 1 0 0 1
340: 2
341: 2

Cable to 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 Fanuc side
pin 20 ----

Set DNC software to:

4800 baud
7 data bits
1 stop bit
ASCII Even parity (or ISO)
Xon/Xoff handshaking
EOB code at the end of each block should be "LF" or Line-Feed (hex 0A or ASCII 10)

Program format should look something like this:

%
O1234
N1
N2 (your data)
N3
N4 M30
%

To send from PC to Fanuc:

Prepare DNC software to send file
Select EDIT mode
Turn off memory protect key switch (if one exists)
PROGRAM key to display programs
READ (data is read in, then appears on screen)


To send from CNC to PC:

Prepare DNC software to receive data
Select EDIT mode
Key in letter "O", then 4-digit number of program you want to send
PUNCH key

If you get any alarms on CNC, let us know what they are.

[giorgis]

Hello Mr.Fritz,and tank you for your answer.I will try exactly whatever you said,and i will notify for more details.
I tried to send to machine a program with different parameters,(2400baud,2stopbits,Even parity,Hardware handshake).I chose the EDIT mode before sending the program.Then I send the program from PC and when appears on PC's panel that the transmission have finished, I pressed the READ button.The result was an 086 ALARM RS-232c Interface Error.
I will try all that you suggest.
Thank you for your help

[dcoupar]

I think your NCnetLite needs to be configured to wait for the XON from the CNC. Or, if you can't do that, start the READ on the Fanuc first, then send from the PC.

[giorgis]

I will try what mention.I tried it out vice versa,by this I mean,that I first sent the commands from the PC and then I started the READ on the Fanuc.Thanks for the advice and I will let you know of any progress.dcoupar.Thank you again

[dcoupar]

The fact that the PC appears to have sent the program before you pressed the READ on the CNC means that the DNC wasn't waiting for the XON. Either that, or the DNC isn't configured for XON/XOFF (software) handshaking.

[giorgis]

Hello guys.I want to say a big thank you for your unvaluable help that you gave me.Mr. Fritz I tried exactly what you said and the results were very good.I will try to communicate with rym for the BTR.
Thank you again
giorgis