GOTO statement issue

Tim Johnson · 2007-08-01 21:26:22

I'm getting the error "Cannot locate sequence number 108 for GOTO. Subroutine: 532 (line #: 2-437), Subsystem: 1 "

Here's my Fanuc 18im code;

IF[#913EQ3]GOTO105
#524=1
IF[#526EQ1]GOTO108 (<<<<<<< trouble block)
.
.
.
/M30
M99P101 (<<<<<<<<<<<<<< line 437)
N108 M30 (END PROGRAM) (<<<<<<<<<< block 108)
N99001#3000=1(TOOL LENGTH IS TOO LONG FOR INDEXING)

The problem appears that the M99 in line 437 is shutting down Vericut's search. N99001 is the actual last block in this main program with 25/30 subs following. Is there a way to shut down the search at the next program number or % rather than the m99?
My GOTO Word/Address;

GOTO*
**
GotoJumpForwardBackwardStart

I've tried the other two GotoJump macros without success

SergeV · 2007-08-02 16:56:30

make sure the M99 is calling the macro ReturnFromSub instead of EndSub.

This macro is identical to EndSub, except it does not mark the current location as the end of the subroutine. This allows for multiple "returns" from a given subroutine.

Tim Johnson · 2007-08-02 19:14:32

Here's my M99 code:

M99
      (G 65 66 66.1)
              MacroVar

     (P*)
              ReturnFromSubCall
                        Scan
                        After

              GotoJumpForwardBackwardStart
                        Value = #100016
                        After

     **
              ReturnFromSub
                       Scan
                       After

I've just called up the current fan18im.ctl from the library and it looks the same(M99 anyway).

SergeV · 2007-08-02 20:03:34

make sure that "Scan NC Program Files" is checked in:

Project > Processing Options > G-Codes; Settings tab

To see a breack down on how VERICUT read your subroutines during the scan pass, do Info > G-Code Report...
Scroll down to the Subroutine section. It should tell you what are the lines recognized.

example: program O9001

SUBROUTINES
-------------
NC PROGRAM FILENAME: C:\my_files\test.mcd
SUBROUTINE: test.mcd
Lines: 0 - 0
Called = No
SUBROUTINE: 9001
Lines: 1 - 90
Called = Yes

Compare with the lines in your program to confirm where the program is ending.

I am wondering if it is not stopping at /M30 before the M99P...

Tim Johnson · 2007-08-02 21:59:45

"Scan NC Program Files" is checked.

SUBROUTINES
-------------
	NC PROGRAM FILENAME: E:\NCSYS\ENSHU JE60S\PART PROGRAMS J1.NC TO J500.NC\J428.NC
		SUBROUTINE: J428.NC (J428)
			Lines: 0 - 260 <<<<<<< correct
			Sequences: 108 - 99001 (lines: 259, 260)
			Called = No
		SUBROUTINE: 428  
			Lines: 2 - 258
			Sequences: 101 - 11 (lines: 8, 234)<<1st & last sequence between lines 
			Called = No
		SUBROUTINE: 5501 
			Lines: 262 - 0 <<262 correct, line 295 is the last 
			Sequences: 4 - 3 (lines: 291, 294)<< 1st & last sequence between lines
			Called = Yes

G91 G28 B0
 
/M30(<<<<<<<<<<<<<<<<line 257)
M99P101
N108 M30 (END PROGRAM)
N99001#3000=1(TOOL LENGTH IS TOO LONG FOR INDEXING)
 
O5501 (PROGRAM PREP)
WHILE[#908EQ1]DO1

I also was thinking the /M30 might be causing the problem but removing that block didn't help.

SergeV · 2007-08-02 22:21:04

something bugs me :?

you have the mesage error "Cannot locate sequence number 108 for GOTO. Subroutine: 532 (line #: 2-437), but from the G-code report, the GOTO is obviously located in subroutine 428.

Do you have a subroutine without a M99 in your program?

Might be a good idea to wrap up the files and send it to Tech Support, with all your files, they will be able to debug it.

Tim Johnson · 2007-08-03 10:25:36

Sorry, that's was my error. This error comes up in almost all my JE60S programs. I can work around this error using variables and usually run 2 to 4 programs a day. I mistakenly went back to a different program than I started with in this thread. I'll send off a file to tech Support.

Thanks for your help.

Tim Johnson · 2007-08-23 21:05:36

FYI

This is a problem with the search stopping at the M30. A request for a "problem"? fix was submitted.

SergeV · 2007-08-23 21:14:06

Make sure the M30 calls the macro EndProgramRewindSpecial.

This macro allow you to branck beyond the end of the program.

Tim Johnson · 2007-08-29 11:42:37

I replaced EndProgramRewind with EndProgramRewindSpecial but am getting the same error.

When I comment out the /M30 I lose the error. Turning the block skip on or off makes no difference.

VERICUT Users' Forum

#1 2007-08-01 21:26:22

GOTO statement issue

#2 2007-08-02 16:56:30

Re: GOTO statement issue

#3 2007-08-02 19:14:32

Re: GOTO statement issue

#4 2007-08-02 20:03:34

Re: GOTO statement issue

#5 2007-08-02 21:59:45

Re: GOTO statement issue

#6 2007-08-02 22:21:04

Re: GOTO statement issue

#7 2007-08-03 10:25:36

Re: GOTO statement issue

#8 2007-08-23 21:05:36

Re: GOTO statement issue

#9 2007-08-23 21:14:06

Re: GOTO statement issue

#10 2007-08-29 11:42:37

Re: GOTO statement issue

Board footer