[gtdinc]

Hello,
I am new to this forum. I hope someone can help.
We have a Seiki mill with a Fanuc 11 controller that we feed from a computer via RS232 from the Esprit programming package, using DNC. Everthing works great with smaller programs. My problem is with programs that are too large to fit in memory. Can I set this up to drip feed?
I have been told that I can connect the RS232 feed to the tape input and do it that way. The tape unit is plugged into connector CD5 (50 pin) and the RS232 is plugged into connector CD4 (25 pin) on the system board, so that doesn't appear to be a direct swap. Does anyone know how to hook this up?
Some documentation shows the tape unit plugged into CA11 (25 pin) on the system board. I have no idea what needs to be done.

Thanks.

[gtdinc]

I found out that all I need to do is set the mode switch to tape and send my program. It works! Now we'll see if data starvation is an issue.

[Dan Fritz]

The INPUT DEVICE setting on the SETTING screen is the key here. If it's set to "0", then the paper tape reader will start if you press Cycle Start in TAPE mode. If it's set to one of the three possible serial devices (1, 2, or 3) it will read a program through the serial port.

The Fanuc 11M has two "speed limits" when drip-feeding. One limit is the number of bytes per second that you can send through the serial port (baudrate). The other limit is the number of blocks per second that the CNC can process. The baudrate can go up to 9600 on the 11M, so that limit is 960 characters/second. If your program has 30 characters per block, and the point-to-point moves per block are .005 inch, then your maximum feedrate is (960/30) x .005 x 60 inches per minute, or 9.6 in/min. If you need to feed faster than that, you can do one of two things: Increase the distance per block, or reduce the number of characters per block. Eliminating N-numbers, spaces, and redundant dimensions will help. To get radical with file compression, format your numbers to trailing zero (no decimals) and go to G91 (incremental). That will greatly reduce the number of characters by at least 50%

To test for your CNCs "blocks per second" limit, feed it a 1000 block long program that has just N-numbers and run it with a stopwatch. If it runs 1000 blocks in 20 seconds, that's 50 blocks per second. That limit can't be exceeded in drip-feed mode, even if you could run at a higher baudrate.

[gtdinc]

Thanks Dan for the excellent information. We have been using 4800 as our baud rate for several years. I tried to change it to 9600, but it did not work. Am I missing something? All I changed was the baud rate, no other parameters, and yes, I changed it at both the CNC and the computer used to DNC the program.

[Dan Fritz]

The 11M should work at 9600 baud. Try making these settings:

On Fanuc SETTING screen:

5110: 3
5111: 1
5112: 11

5120: 3
5121: 1
5122: 11

5130: 3
5131: 1
5132: 11

On your DNC software, set 9600 baud, Even parity, 7 data bits, 1 stop bit, and Xon/Xoff handshaking. This combination should work fine. The only problem you might encounter would be a "BUFFER OVERFLOW" alarm on the CNC when trying to read in a program or run DNC. In that case, do this:

Right-click on your MY COMPUTER icon (assuming Windows XP)
Click "Manage", then "Device Manager"
Click on the (+) next to "Ports (COM and LPT)"
Right-click on the COM port you are using for DNC (usually COM1)
Click "Properties", then "Port Settings", then "Advanced"
Move the "Transmit buffer" slider control all the way to the LEFT (lowest setting)
Click OK many times to exit all menus.

Try your DNC operation again. If you get an alarm, let us know what the alarm says.

Good luck!

[starweldengg]

Hey! Can anyone help me with a parameter manual for Fanuc 11M.