A question for subprograms

[Hatebreeder]

Hello to all i am new with this and i have a problem with a subprogram calling.Is there a way when i call a subprogram to call in from a specific line number something like this

g54 x0 y0;
m98 p1000;
m98 p1000 ???N50;
m30;


o1000;
g91;
x50 y20;
m99;
n50 x55 y30;
m99;

I am using a Stama MC320 Fanuc 0M system.

Regards to all

[Geof]

Instead of using an external (M98) subprogram call use the internal (M97) call to a subroutine in the calling program?

[Hatebreeder]

m97 works with HAAS in fanuc is end of macro mode

[Geof]

Originally Posted by Hatebreeder m97 works with HAAS in fanuc is end of macro mode

Okay, what is the format to for an internal call in fanuc, use that.


I do wish the G and M codes had been correctly standardized years ago.

[Hatebreeder]

I don`t need internal call becouse in the subprogram are cycles that will be used by more than one program and i need to jump to specific line .. the other way is more subprograms....

[samu]

May be you can do it that way. Before macro call, define a variable with block number you want to beggin macro and start your macro with GOTO instruction.

g54 x0 y0;
#101=50
m98 p1000
m30;


o1000;
GOTO #101
g91;
x50 y20;
m99;
n50 x55 y30;
m99;

[Hatebreeder]

Originally Posted by samu May be you can do it that way. Before macro call, define a variable with block number you want to beggin macro and start your macro with GOTO instruction. g54 x0 y0; #101=50 m98 p1000 m30; o1000; GOTO #101 g91; x50 y20; m99; n50 x55 y30; m99;

I don`t think stama mc320 have goto function

[dcoupar]

GOTO is User Macro function.

[samu]

You said that you have a fanuc OM, It is wath i have and i can do that. Maybe you dont have macro b option turned on

[Hatebreeder]

Like i said i am new with this and i was never used macro i guess i will try to see what will happen

Thanks to all.


And i have another question do anyone have Fanuc 0M manual and parameters ... and can he send them to me my mail is castbreeder@inbox.com

[stevo1]

Samu is correct with the easist way to do it. If you have macroB programing option on your control.

G54X0Y0
#101=50-----------#101 will be set to the line number you want to jump to in this example its 50
M98P1000
M30

O1000
GOTO#101----------#101 is set to 50 or what ever you set it = to in your main program if #101=60 it would go to N60
G91X50Y20
M99
N50X55Y30
M99
N60X60Y40
M99

In every program you do right before your M98 call set #101 equal to what line number you want to jump to. You don't have to use #101.
#1-#33 are local variables and cleared when a program end code is seen or and with reset button
#100-#149 are common variables and cleared only at power down
#500-#999 are permanent common variables and are never cleared and changed only when you change them.

You said your new to this so I figured more detail might help.

Stevo

[Hatebreeder]

Originally Posted by stevo1 Samu is correct with the easist way to do it. If you have macroB programing option on your control. G54X0Y0 #101=50-----------#101 will be set to the line number you want to jump to in this example its 50 M98P1000 M30 O1000 GOTO#101----------#101 is set to 50 or what ever you set it = to in your main program if #101=60 it would go to N60 G91X50Y20 M99 N50X55Y30 M99 N60X60Y40 M99 In every program you do right before your M98 call set #101 equal to what line number you want to jump to. You don't have to use #101. #1-#33 are local variables and cleared when a program end code is seen or and with reset button #100-#149 are common variables and cleared only at power down #500-#999 are permanent common variables and are never cleared and changed only when you change them. You said your new to this so I figured more detail might help. Stevo

Thanks