Fanuc help

[Buddy J]

Howdy Again,

 

I've searched here and in the manual for info about How to repeat a toolpath(s) within a program with a fanuc oi control.

With Yasnac It was simply G25 Pxxxx Qxxxx.

What replaces this w/fanuc?

M98 could jump around a Yasnac control also but all I could find in the manual is jumping to subs or macros.

Control only has 250K memory and I'm machining 2+2 sides of a block (horn) and want to repeat 180 degs data from zero, 270 from 90 so I don't have to run off the flash card

Am I SOL??

Thanks

[Guest CNC Apps Guy 1]

According to the FANUC Manual, G25 is Spindle Speed Fluctuation Detection Off.

 

Subprogram repeat is usually M98 Pxxx Lxxx

 

HTH

[Buddy J]

According to the FANUC Manual, G25 is Spindle Speed Fluctuation Detection Off.

 

Subprogram repeat is usually M98 Pxxx Lxxx

 

HTH

 

Yeah, G25 was Yasnac

Anything within same program for fanuc?

[Scott Lundin Shopware Inc.]

Back in fanuc 6M I used to jump around within a single program using M99Pxxx. Yes I said M99. The P number was which N line number I wanted to jump to.

[Buddy J]

Trying the M99 approach never got off the ground, control quit upload @ the 1st M99 it read.

The M98 Pxxxx Lxxxx gave me the same error, file not found.

 

Guess I'm stuck running from the card

[Tim Johnson]

I have several files with 60+ M99's. The only thing that should stop an upload is the % sign.

 

Back in fanuc 6M I used to jump around within a single program using M99Pxxx. Yes I said M99. The P number was which N line number I wanted to jump to.

 

I still use that today;

 

%
O646(JE60S 625-710-524 OP1)
(MACHINE NAME - ENSHU JE60S)
(DATE: APR-26-11)

#152=0
#915=0

N101 M98P5501 (PROGRAM PREP)  <<<<<<<<<<<<<<<<<<<<<<<<<<<<
N102 G00 G17 G20 G40 G49 G80 G90 G94



G91 G28 B0
IF[#915EQ4]GOTO110
IF[#913NE3]GOTO108
GOTO104
G90 G53
N110
/GOTO108 (END PROGRAM)
M99 P101 <<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
N99001 #3000=1(TOOL LENGTH IS TOO LONG)
N99002 #3000=2(TOOL LENGTH IS TOO SHORT)
N99003 #3000=3(WRONG PALLET IS IN WORK AREA)
N108 M30 (END PROGRAM)

[Buddy J]

Welp, I figured out that I had to change a parameter to allow multiple M99's to load.

#3201 N99=1 (bit#5)

 

While great for jumping around within the program I still havn't figured

out how to copy one section then move on to another section, ie: get past the M99 that let me do the initial copy and resume beyond that point.

I can't belive fanuc dosen't have a means to do that.

 

Thanks for the responses

[Grievous]

Just an example of what you can do (I useit all the time):

 

In main prg use G65 to call subprg:

G65 Pxxxx A1.(LETTER A=#1)

G65 Pxxxx A2.

 

SUB:

 

Oxxxx

GOTO#1(jump)

 

N1

...CODES HERE

GOTO99

 

 

N2

...CODES HERE

GOTO99

 

 

N3

...CODES HERE

GOTO99

 

N99M99