Need Help!- FANUC Handling of : characters within comments

[CAMFUN]

Hi guys,

I´ll take the opportunity to ask you something: We are implementing DNC-Max here and I know it has a ton of translators to do almost anything...
I´m transfering some headers to a Fanuc 0i-TB and I´m having problems to get the : character at the control side...

The port in my DNC software is set to operate in ASCII mode as well...

If I send this:

%
O7999 (PN:B112229-1 # REV. PN:A # FIX:1)
N20 (MAQUINA:ATOC II)
N30 (CONTROLE CNC:FANUC 0I-TB)
N40 (PROGRAMA:2079990)
N50 (ID ANTERIOR:WT3-2065.VTG)
N60 (CODIGO DE APLICACAO:0)
N70 (DESCRICAO:CORPO CONECTOR)
N80 (PART NUMBER:B112229-1)
N90 (REVISAO PART NUMBER:A)
N100 (PART INFO:B112229-1)
N110 (REVISAO PART INFO:B)
N120 (OPERACAO:USINAGEM F1)
N130 (FIXACAO:1)
N140 (PROGRAMADOR:dANIEL SANTOS)
N150 (*************************)
N160 G00 X1000.0 Z2000.0
N170 M30
%

I get this at the control side:

%
O7999 (PNOB112229-1 # REV. PNOA # FIXO1)
N20 (MAQUINAOATOC II)
N30 (CONTROLE CNCOFANUC 0I-TB)
N40 (PROGRAMAO2079990)
N50 (ID ANTERIOROWT3-2065.VTG)
N60 (CODIGO DE APLICACAOO0)
N70 (DESCRICAOOCORPO CONECTOR)
N80 (PART NUMBEROB112229-1)
N90 (REVISAO PART NUMBEROA)
N100 (PART INFOOB112229-1)
N110 (REVISAO PART INFOOB)
N120 (OPERACAOOUSINAGEM F1)
N130 (FIXACAOO1)
N140 (PROGRAMADORODANIEL SANTOS)
N150 (*************************)
N160 G00 X1000.0 Z2000.0
N170 M30
%

Settings at the control:

STOP BIT 2
NULL INPUT (EIA): NO
TV CHECK (NOTES): OFF
TV CHECK: OFF
PUNCH CODE: ISO
INPUT CODE: ASCII
FEED OUTPUT: NO FEED
EOB OUTPUT (ISO): LF

I want to get at the control side the ":" characters that there exists in the original file... is that possible in a FANUC control? Is there any hidden bit to do that?

Thanks in advance,

[sinha_nsit]

Colon is not available on Fanuc. Replace it by some other character. I normally use @ character for such applications. @ becomes available through C-EXT soft key.

edit:
set param 3205#0 (COL) to 1, to see a colon as a colon.

[CAMFUN]

sinha,

Thank you very much for your response. I searched everywhere for this answer...

That was really helpful!

Sincerely,

[sinha_nsit]

You are welcome. I am glad that I was of some help.

Sinha

[stevo1]

Hmmm. I have the colon sign in some of my programs on the 15, and 18 series Fanuc in the notes. I have not checked on the other controls. I could not find a parameter setting in the Om control that would not allow or disallow the colons.

IIRC I had a similar problem some time ago. It may be your DNC settings. There was a setting that would change the : (colon) to and O (letter O) before the program number. It maybe that this setting is replacing your : with O’s.

It’s worth a look.

Stevo

[sinha_nsit]

I could not find colon key on the MDI panel of 0i (or, I have not checked carefully).
How to type colon then?

[stevo1]

Sinha,
I apologize that I was not more specific. I do not have a key to type in a colon at the control. I can however use a colon when writing a program and download it to the control with no problems.

So I ass u me that if this is possible on the 15, and 18 series control that I checked it should certainly work on the newer then those Oi control.

I think that it is just too much of a coincidence that it is replacing the colon with the letter O considering the : and O are the 2 ways Fanuc identifies the program number. I would check the software to see if there is a setting for replacing : with O.

Stevo