Need Help!- G52 w/ COUNTER on Fanuc O-M

[bikebasher]

I am trying to machine 7 small, but complex, parts w/ a single push of the go button.

They can be offset uniformily by 2.30 inches on x axis.

I used ProMfg to generate the toolpaths and then Posthaste to get the code. Mill is SuperMax Rebel w/ Fanuc 0-M controller.

Here is the Boolean logic I tried to use:

G17 G20 G28 G40 G49 G80 G90
N1
COUNTER=0
N2
G52 X+(COUNTER*2.300)
*MY CODE STARTING W/ FIRST TOOL CHANGE*
N3
IF COUNTER=6 GOTO END
COUNTER=COUNTER+1
GOTO 2
END

When I loaded it, it was split into 2 programs. I don't think it knew "counter".

Is there a simple way to do this w/ my already generated code?

[dcoupar]

I'm sure your Fanuc is interpreting the "O" in COUNTER as a new program number.

Have you looked in your Fanuc Operator's Manual at the Custom Macro section? It would look more like this, I imagine (this may not be 100% accurate, but I think it's close).

N1
#101=0
N2
G52 X[#101*2.300]
N3
IF[#101EQ6]GOTO99
#101=[#101+1]
GOTO2
N99
M30

Custom Macro is a Fanuc option, and a lot of machines didn't come equipped with it. If yours doesn't have it, you probably could also accomplish this using M98 subprogram calls, and G10 (which is also an option) for adding 2.3 to the G54 work offset.

O1001 (MAIN PROGRAM)
G90 G10 L2 P1 X-22.5414 (SET G54 TO STARTING X)
M98 P011002 (CALL SUB 6 TIMES)
M30

O1002 (MACHINING SUB)
G0 G91 G28 Z0
T01 M06
...
...
G91 G10 L2 P1 X2.3 (ADD 2.3 TO G54 X)
G90 M99

[stevo1]

If it is not the fact that the control sees the "Counter" and thinks its another program then it could be splitting up into 2 programs because your program is to long. I have only seen this one time and not on a OM control. You say that they are complex parts so I assume that there is much more to the program then what is seen. Like I said I have not seen this on a OM but its possible.

You can try removing the Counter word or put parenthesis around the block before sending it.

However Dcoupar is correct in the format issue. The only time that I have seen the format as you have put it is in Pascal language. You should format it as Dcoupar had wrote. If you have the work coordinate options and G10 data settings I would go that way instead of G52.

Stevo

[bikebasher]

I didn't have any of the Fanuc manuals to consult, but I figured it was some numerical code specific to the controller.

I checked and I think the custom macro is loaded. I entered #101=1 and I didn't get an error message or alarm.

I have some manuals and programming refrence books on the way.

[stevo1]

I am not sure if it will alarm out or not. It might. Just make sure that #101 got set equal to 1. You can check parameter 913.7 for your macros. Let me know if you need any books.

Stevo