main progam to run sub programs

[Rick46]

I have a main program that I used on a fanuc model 18i series control few years back for cutting electrodes at different wcs and it worked great but Im trying to use the same main on a newer 18i-mb series fanuc and its not working properly..

 

I have my paths stripped of all the safe start header and wcs output as well as a M99 at the end of the paths I run. the problem im having is it fails to cancel the tool length offset in the control and errors out when it goes back to running in AI NANO mode. here is an example of the main im running..

 

 

%
O0003(MULTIPLE WCS 3X)
G00G40G49G80
G91G28Z0.
(PROGRAM TO CALL SUBPROGRAM)
G00G90G55
M198P1000
G00G90G56
M198P1000
G00G90G57
M198P1000
M05
G91G28Z0.
G91G28Y0.
M30
%

 

 

the machine isn't going back to the top to run the safe start header before running the next subprogram and there for does not cancel out the tool length offset and causes me the AI NANO error..

 

any help on modifying this is greatly appreciated. also the machine is a toyoda FV1680

 

thanks in advance..

[BenK]

When returning to the main program it doesn't go to the top it continues from the point it left off. You need to have it cancel the offsets in the sub program.

[Brando]

like ben said, id cancel that in the subs too, heres what the end of my subs look like, used on a fanuc 16i , 18i and 32i doosan horizontals,

 

G00 Z3.712

G05.1 Q0

M09

G91 G28 Z0.

G49 G90

M01

M99

 

hth

[Mr.ZX]

My question is why would you want to cancel the tool length offsets?

[Mr.ZX]

You should never have to cancel a tool length offset when switching between WCO systems. Fanuc is still very down ward comparable, An old program should work fine.

Some thing like this

 

N1G28G91Z0M5

GOG40G49G80G90G98

T1M6

G54X1.Y1.M3S6500

G43Z3.H1M8

M98P1000

G55X1.Y1.

M98P1000

G56X1.Y1.

M98P1000

M9

G29G91Z0M5

G28G91Y0

M30

 

Your WCO system should adjust for the Z values.Are you using positive or negative offsets?

[Rick46]

cause I get an error stating a modal code has not been reset before running G5.1 Q1 on my next path due to the tool length offet not being canceled out. its error 5111 in my fanuc manual and also a fanuc rep told me the same but could not tell me which one. After watching it I found the g43 was not returning back to g49 before starting new path. thanks all I will try your suggestions today..

 

@Mr Zx yes im using positive offsets in my programs. and my lengths offsets page as well.. thanks.

[Matthew Hajicek - Singularity]

If your sub is only using one tool you can put the tool pickup and G5.1 in the main, and the G49 at the end of the main. Otherwise you can put the G49 just before every toolchange like I do. "G49 T1 M6"

[Rick46]

like ben said, id cancel that in the subs too, heres what the end of my subs look like, used on a fanuc 16i , 18i and 32i doosan horizontals,

 

G00 Z3.712

G05.1 Q0

M09

G91 G28 Z0.

G49 G90

M01

M99

 

hth

 

I modified my post to output the end of my subprograms as recommended by Brandon Renwick and has been working great all day. thanks for everyone else's suggestions on the matter as well.