Data server/ sub program error?

[#Rekd™]

Hi,

 

I have this program for using our flash card as a data server but I am getting this error, any ideas?

 

O0010 (program #)

G20 G40 G80 G17 G49;

M198 P8;

M30;

 

Error 003 Too many digits

 

Thank you

 

John Ford

[Ocean Lacky™]

Fanuc? Look for an abnormally high feedrate. F10000 maybe? Sometimes I see this with block numbers also, but you don't seem to be using them.

[#Rekd™]

Fanuc Oi-MB.

 

It hangs up on the G20 G40 G80 G17 G49; line

 

when the alarm goes off.

 

John

[Tim Johnson]

Are you sure you're hanging on that line? Insert an empty eob after the G20 line and single block it to the lone eob. I'm thinking the error's probably in the sub.

[Hardmill]

You sure your I/O channel is set properly??

 

 

PEACE

[#Rekd™]

Hi,

 

When it alarms out the G20 line is highlighted?

 

I will check the I/O channels when the part is finished.

 

John

[#Rekd™]

Hi Tim,

 

I think you are correct. You have mail.

 

What could be the problem in the Subprogram?

 

John

[Rick46]

sounds like you have a line of code in your toolpath that resembles the g code at the start of your subprogram.

 

ex.. you say "It hangs up on the G20 G40 G80 G17 G49; line"

 

if that code is in your toolpath as well as the subprogram it will cause errors.. take the line that is similar or exact to the line of your subprogram out of the toolpath and try it.. this should fix it.. HTH...

[cheeves]

Is "M198" a valid code? Never saw that before.

[Guest]

quote:

---

Is "M198" a valid code? Never saw that before.

---

For that call to the data server, yes it is.

 

John,

 

Being away from the machines for a bit I don't "quite" remember all of the specifics but have you searched out the Data Server thread that James started and posted a lot of good information in, there "might" be a formatting issue with your code that you are forgetting or missing.

 

No % at the start or end, no entension on the file name and something esle I don't remember

[#Rekd™]

Hi,

 

It ended up being the subprogram number (O35565) had to many digits 5 instead of 4. I am not to sure why the Cimco editor did this, any ideas?

 

A big thank you to Tim for pointing this out.

 

John

[Guest CNC Apps Guy 1]

Also, your program number on your Dataserver/Flash Card needs to have "O" AND 4 digits with no file extension. Sometimes it will work without the leading zero(s) and with a file extension, but it will ALWAYS work if you follow "O" and 4 digits and NO file extenstion.

 

HTH

[Steve Hattori]

+1 to what CNC Apps guy said, and also check for Ocean Lacky's F10000- I have a couple of toolpaths that have that as a default feedrate in X2 and sometimes miss it before it posts.. Also , if you use a pause in any of the drill autocycles the Fanuc want to see a whole number, no decimal point, or you get that too many digits error. So a pause of .2 sec would be "P200", not "P.2".