Need Help!- Fanuc Ot DNC issue

[BrendanF]

Hi all. I've been trying to install dnc software to communicate with my very ancient CNC 350 Colchester with Fanuc ot controller.

Does anyone know a good...free package that actually works. And what are the parameters for the OT controller.

I have tried Nclite which appears to be an excellent program but I cannot get it to communicate with my machine.

Please help.

Thanks

BrendanF

[Dan Fritz]

Most DNC programs will work OK with the 0T, but if you have trouble, try a free 30-day demo of our PC-DNC Editor by clicking here:

http://www.sub-soft.com/download/Edi...itor_3.5.3.exe

Support in Australia is through Shera Bonnet & Associates at rb@shera.com.au

On the Fanuc 0T, go to the first parameter page and you will see a bit labeled "I/O". Set this bit to "0". Then, page up to parameter 002 and set the bit on the far left to "1" and the bit on the far right to "0" (the 6 bits in the middle are for something else, so don't change them). Then, page up to parameter 552 and set the number "10".

To match these settings on the DNC side, set the DNC software to use 4800 baud, 7 data bits, 1 stop-bit, and Even parity. Handshaking should be set to "Xon/Xoff"

The first test would be to try to send a program from the CNC to the PC. Get the DNC software ready to receive, then select EDIT on the Fanuc, Press the PRGRM key to display your program, then key in the letter "O" followed by a 4-digit number, then press Output/Start to begin transmission.

To send the other way, get the DNC software ready to send, put the CNC into EDIT mode, turn off the memory protect key switch, then press the INPUT key.

An alarm 086 usually indicates a cable problem. An alarm 087 usually indicates that the DNC software is not handshaking fast enough when the Fanuc tries to stop it with an Xoff character. If this happens, right-click on "My Computer", click "Manage" then "Device Manager". In the list of devices, click the (+) next to "Ports (COM and LPT)", right-click on the COM1 port, click "Properties", then "Port Settings", then "Advanced". Move the "Transmit buffer" slider all the way to the left,then click OK many times to exit all menus. Then, try your DNC software again.

Your cable should be a 9-25 "Null Modem", which you can buy anywhere. If you want to make your own, here's how it's done for the 0T:

25-pin male -------------- 9-pin female
pin 2 ------------------------- pin 2
pin 3 ------------------------- pin 3
pin 5 ------------------------- pin 7
pin 7 ------------------------- pin 5
pin 6 ----
pin 8 ---- <-- jumper these three pins together
pin 20 ---

Your PC may have a 25-pin female plug on the back, just like the Fanuc. DO NOT USE this plug. It's for a parallel printer, not RS232. Your PC should have a 9-pin MALE plug on the back, which matches the 9-pin female on this cable.

NOTE: A few 0T controls out there do not have the ability to send & receive ISO tape code. If you have no luck with these settings, try setting your DNC software to use EIA (RS244B) tape code instead.

[BrendanF]

Dan,

Thankyou so much for your help. I will let you know how I go.

Brendan

[BrendanF]

Hi Dan,

I have done everything you suggested but still no luck.

When you say parameter 002 do you mean 0002 or 0020? I tried both anyway. Also in the DNC settings the Handshaking section gives options of Software, Harware, Nothing or Both? There is no mention of Xon/Xoff here. The program is Nclite, I haven't tried the program you suggested yet.

I tend to agree that it could be a cable issue. I'm using a 25 to 9 pin cable but through a usb adaptor to a laptop. The laptop had no 9 pin ports. When Outputting the program I'm receiving no response at the pc, but no alarms on the CNC. I know the CNC does transmit because a technician downloaded the machine parameters off the machine when I bought it.

I went into the laptops device manager and was able to set the usb adaptor to match the settings you suggested for the DNC. 4800 buad, 7 bit, 1 stop bit, even parity and Xon/Xoff. So everything appears to be set correctly but no go.

I'm pulling out whats left of my hair. I think I may have to replace the laptop with a pc and a direct 9 pin port. Either that or I'll have to track down the technician from when I bought the machine.

Thanks for your help mate. Its greatly appreciated.

BrendanF

[Dan Fritz]

Xon/Xoff handshaking is sometimes called "Software" handshaking. Japanese companies use the term "DC codes", which are the same as Xon/Xoff

If you're getting no data in either direction, check your cable first. The USB adapter just gives your laptop a 9-pin male serial port. The cable from the USB adapter to the CNC needs to be a NUL MODEM cable, wired like the one I described earlier.

The parameters to set on the 0T are 002 and 552. Some later 0Ts will have a leading zero on these numbers (your's apparently does), so it will be parameters 0002 and 0552. The left-most bit of parameter 0002 should be a "1" and the right-most bit should be a "0". Parameter 0552 should be "10". That is a setting of 4800 baud, 1 stop-bit, 7 data bits, Even parity, and Xon/Xoff handshaking.

Try sending something from the CNC to the computer first. I don't know anything about your NCLite software, so I can't be of any help with it, sorry.

[BrendanF]

Dan,

Thanks Dan, you are the man. I followed your instructions precisely and my machine is now communicating with the laptop.

It appears there were two areas causing problems. 1. NClite is a piece of ****! It caused some serious Bios errors on the laptop so I had to delete it and do a complete windows install. 2. The cable was not wired as you had stated. I had my brother re-wire this correctly. I then download the dnc software you recommended and amazingly the setup worked correctly.

Thanks again Dan, I would have been lost witout your insight. If you ever head down to Aus drop a line and I'll shout you a beer or twenty!

BrendanF