[RC-CNC]

I am busy trying to install a DNC server connection to my Fanuc 18iT controller. I have the cabling and parameters all set, however, when I go to output a program from the CNC to the PC, I keep getting the error 79 and 86. Looking in the manual these relate to incorrect file name or program names specified. I have the correct file name or program name, but it still won't punch out to the DNC. Any suggestions?

[dcoupar]

In my 18iT manual, 79 is Program Verify Error, and 86 is DR Signal Off.

How is your cable wired? In most cases, jumpering 6-8-20 on the PC end will eliminate 086 alarms.

What keys are you pressing to send from the CNC to the PC?

[RC-CNC]

In my 18iT manual, 79 is Program Verify Error, and 86 is DR Signal Off.

How is your cable wired? In most cases, jumpering 6-8-20 on the PC end will eliminate 086 alarms.

What keys are you pressing to send from the CNC to the PC?

Well I am going 25 pin from CNC to DB9 on the PC which is Serial to USB adapter.

To send from the CNC I am pressing Program > OPRT > O#### > (|>) > (PUNCH) > (EXEC)

[dcoupar]

What are the connections from the 25 pin to the 9 pin? The most common for XON/XOFF handshake is:

DB25 <---------------- > DB9
1 <---- shield --------- (no connection)
2 <----------------------> 2
3 <----------------------> 3
7 <----------------------> 5
4,5 jumpered (CNC end only)
6,8,20 jumpered (CNC end only)

[RC-CNC]

We are doing an RTS/CTS handshake as we are utilizing a Serial to USB adpater hub.

[Dan Fritz]

Don't jumper 6-8-20. Instead, connect pins 6 and 8 on the Fanuc side to pin 4 on the PC side.

The 6-8-20 jumper works on most Fanuc controls, but the newest, fastest ones will still throw an alarm 086 if you use the jumper.

[dcoupar]

Is this the only machine you have connected to this USB hub? I've never had much luck with USB -> Serial adapters and handshaking.

From what I can tell, (mostly from reading Dan's posts and then re-reading the Fanuc RS-232 "info"), Fanuc only uses RTS / CTS when PUNCHing. When READing, it sends a DC3 when the buffer is full and if the PC doesn't stop within 10 characters, you'll get a PS087 buffer overflow alarm.

I've never seen alarm PS079 when PUNCHing. It's supposedly only issued when you "collate" or verify when READing a program with the memory protect switch on and the NC detects an error.

[RC-CNC]

I was able to clear the 79 Code because I realized I didn't have the controller in EDIT mode. I had to rotate the selector switch on the operator panel to the correct EDIT setting. I still, however, get the 86 code.


I am going to try jumpering the three pins together first and see if I can talk with the PC, then I will try jumpering 8 and 6 on the CNC to 4 on the PC. Is this the pin config taking into account a DB25 on the PC or a DB9?

[dcoupar]

DB9, I believe.

[RC-CNC]

Hey guys, I just got some time on the machine. Jumpering the three pins 6 (DSR), 20 (DTR), and 8 (DCD) worked. I used an RS232 break out box for this. There was no 86 alarm and I was able to successfully input and output programs!

However, (isn't there always a however?) when inputting programs I received a PARITY ERROR and the program in the CNC was split into two programs. For instance, if the program number sent to the machine was O2222, the NC would split the program into O2222 and O2223, with O2223 starting at about line N900. I believe the problem is that the controller cannot handle such a large file. Is this the case? If so how can I remedy the situation so it reads it all as one file? Thanks a lot.

[dcoupar]

Look for an "O" or ":" outside parentheses in your program somewhere around N900. Program size shouldn't be a problem, unless you try to load a program that overfills the memory. Then you'll get a PS070 alarm.

[RC-CNC]

Look for an "O" or ":" outside parentheses in your program somewhere around N900. Program size shouldn't be a problem, unless you try to load a program that overfills the memory. Then you'll get a PS070 alarm.

I'll double check, but this has done the same thing on 2 different programs so far.

[RC-CNC]

Alright, so I noticed the program is cutting short at an M30 command (Program End and Reset). It seems this is used for a nested program for our operation of Cut off. After this M30 command the controller seems to take it upon itself to create a separate program for the following code and does not keep it all in one file. Does this provide any additional insight?

[dcoupar]

Why not post the portion of the code where it's hanging up. Then maybe we can see.

[RC-CNC]

Why not post the portion of the code where it's hanging up. Then maybe we can see.

sure thing. Here is the portion of the original program:

M79
G0W.02B-5.5M63M9
G53X0.Z-12.M64S800M3
T1088
M01

/M90
/M99P1000
M30
N900
M01
M98P8000(O8000 BAR CHANGE)
M99P1000(RETURN TO TOP OF PROGRAM)


N7777
#3000=3(CHECK TOOL LIFE)

And here is the end of the program and beginning of the second program it splits it into:

O2222

M79
G0W.02B-5.5M63M9
G53X0.Z-12.M64S800M3
T1088
M01

/M90
/M99P1000
M30
%

O2223

%
O2223N900
M01
M98P8000(O8000 BAR CHANGE)
M99P1000(RETURN TO TOP OF PROGRAM)


N7777
#3000=3(CHECK TOOL LIFE)

When the program O2222 is input into the controller, it stops the input at M30 and creates a separate program O2223 and inserts everything from N900 left into that other program. The operator tells me he used to have to do this anyway, that is, merge the programs back together after reading them in.

My assumption is that some parameter in the controller is telling it that when it reads a program end (M30) to reset and then as data is still entering the controller it creates another program with the leftover data. Thanks for any help you can provide.

[dcoupar]

Try a single blank line after the M30.

/M99P1000
M30

N900
M01
M98P8000(O8000 BAR CHANGE)

[RC-CNC]

Try a single blank line after the M30.

/M99P1000
M30

N900
M01
M98P8000(O8000 BAR CHANGE)

So the single blank line seemed to work. I still however get the DNC telling me there was a Parity Bit Error present on send. But when I check the filesize of the input and output programs they are the same so the integrity of the file was intact.


Any explanation as to why the space works after the M30? Also, any idea why I am getting a parity error? Thanks again for all your help. This has opened up a whole world to me and given me a wealth of knowledge. Thanks.

[dcoupar]

I *think* I remember reading about the blank line somewhere, but I can't remember where.

As for the parity error: What DNC software are you using? What are the configuration settings for sending?

[RC-CNC]

I *think* I remember reading about the blank line somewhere, but I can't remember where.

As for the parity error: What DNC software are you using? What are the configuration settings for sending?

I am using iLogic DNC Server 3.0 http://www.i-logic.com/dncserver.htm

My config settings for sending are:

Stop Bits: 2
Data Bits: 7
Even Parity
4200 Baud Rate
RTS/CTS Handshake

[Lancelot001]

Today I have a "079 program verify error". After a half of hour trying to transfer some programs, whithout succes, I see the "Protect program" key in wrong position. I switch the key and everithing is fine now.