Fanuc output program + subprograms

[Mr_T]

Hi !
I want to send my program from the Fanuc cnc to PC.
The problem is that the subprograms dont "follow" the main prog.
(Yasnac has that function, it "packets" it and send it to PC.)
Does anyone now if Fanuc has a similar function?

//Otto

[Chris D]

I believe that if you want to output all programs, enter

O0-9999 then press the output (or punch key). The O0-9999 is just a range of numbers, in this case zero to 9,999.

chris

[Mr_T]

Thanks for your answer!
But i was looking for a way to get the fanuc controll to automaticly inclued the relevant SUB-programs with the main-program.

//Otto

[scubanick]

Not Gona Be Able To Get That

[MMTechi]

i have always disliked having to send multiple programs ( main and a sub) so i created my own structure of program and which included sub programs. this makes for a single program download and easy to edit because you don't have to jump around in different programs or from top to bottom thereby reducing the chance for error. i highly doubt that i have created anthing new. it is what i use all the time now because i sometimes run a particular cut routine using up to 12 different work piece coordinates and sometimes up to 60 or more locations depending on the feature. i would be glad to send you one of my programs or try and edit one down to show you the method. it utilizes the m97 and m99 a lot. here is one section of my program. let me know if anyone needs to see more.

bob flores
231-632-6669

ps i use discriminator for viewing and editing my nc programs and i program with surfcam.



N30
G40 G80 G90
T30 D30 M6 (T30 .500 DIA CARB EMILL/DR FOR .9475 DIA .0655 DP)
G1 G41 X0.750 Y0 F200. G43 Z0.3 H30 M8
S4000 F50.
M3

(CALL LOCAL SUB)
X0.75 Y0. G1 F200. (HOLE LOC)
M97 P301
X2.35 Y0. G1 G41 F200. (HOLE LOC)
M97 P301
X3.95 Y0. G1 G41 F200. (HOLE LOC)
M97 P301

G0 X10. Z6.M5

M1
M5
M99 P100 (NEXT TOOL NBLOCK)


N301
G80 G90
T30 D30 M6 (T30 .500 DIA CARB EMILL/DR FOR .9475 DIA .0655 DP)
G1 G43 Z0.3 F200. H30 M8
S4000 F50.
M3

G0 Z0.03
G1 Z.005 F15.
G1 Z-0.025 F10.
G1 Z-0.02
G1 Z-0.045
G1 Z-0.04

G1 Z-0.065
G91 (NOW CUTTING IN INCREMENTAL)
G3 X0.2167 I0.1083 J0 F10.
I-0.2168 J0 F18.
G3 X-0.04 I-0.0201 J0 Z-.0005 F9.

G3 X0.0469 I0.0235 J0 F20.
I-0.2237 J0
I-0.2237 J0 F14.
X-0.2236 I-0.1118 J0
G90
G0 Z.3

G91
G0 G40 X0.01
G90

M99


N100
G1 X10. Z10. M9 F200.
G90
M30
%

[Dan Fritz]

All Fanuc controls can output ALL the files from memory with the "O-9999" command, but only a few models can output just SOME of the files from a particular range of O-numbers.

The Fanuc 10, 11, 12, and 15 controls can output all the O-numbers within a certain range by using the soft-function keys. You press the PUNCH soft key, then the PROG# key, then the first O-number, then the PROG# key again, then the last O-number, then EXEC. Only the O-numbers between those two numbers are output.

This procedure does not work on other Fanuc models like the 0T and 0M. All you can do with these controls is output all of the O-numbers in memory, or one O-number at a time. When sending all the programs, you won't event be able to control the sequence that the programs are punched.

We can't help you with this shortcoming in the Fanuc control, but we do have used this solution, which may help you:

Our DNC software (and many others as well) have the ability to receive data until a certain "timeout" occurs. In our software, you can receive data until the data stops coming in for (x) seconds. If you set this value to about 10 seconds, you can send your main program, then send each sub-program one at a time until you've sent them all. As long as you don't pause for more than 10 seconds between files, the DNC software will save all your programs in a single file. If 10 seconds isn't enough time for you to push the buttons, you can always set it to a longer timeout.

Once your main program and all subs are saved in one file on your DNC system, you can send them all back to the CNC control in one shot by pressing "O-9999" then INPUT or READ. Also, you will have fewer files to organize on your hard drive because all the subs are attached to the main programs.

[psychomill]

Bob posted what looks like internal subs from a Haas machine. This won't work on a Fanuc ( unless you loop an M99 internally, but some controls don't like that either - Dan could probably elaborate).

And as a take off from Dan's post, if your subs are numbered "relative" to the main, you can output a range of programs by also typing in for ex: "O1500" "," "O1567" ....

The comma is the seperater and this will output all programs from number 1500 to 1567.

[Mr_T]

Thank´s for all your answers.
Our fanuc systems does not handle subs in the main-prog so it seems like i have to take the "long way" with my fanuc systems.
Yasnac´s solution to this was great, just send the main prog and it scanned for the subs and included them.

//Otto

[chuy]

what bob posted was for a hass those are local sub routines not sub programs...anyway what do is make sure the memory is clear of any unrelated programs and just "punch all" but if you have a newer control. and your subprograms in sequence IE..o1001,o1002 and so on you can hit punch
this "O1001,O1014" O1014 being the last program in the sequence and it will send all the those subs back to your pc.. hope that's clear...

[Per_N]

If you have the macro option and understand it well, it's possible the make a program that print out a series of program.