[horst007]

how do i call a subprogram on this freak of a controller? All I want to do is turn my second postition program to a subprogram and call it up at the end of my first postion, but I constantly get errors. Ie. Subprogram doesnt exist and another one about M02 being in the wrong spot or not existing can't remember which. Please help.

[calgarykevvy]

Freak of a controller? They are all pretty easy once you learn the dialects.

Here's what I do on my E100L. Inside the MIN file:

...
CALL OBSET (B TURRET OFFSET CONFIG)
...
M02 (PROGRAM END)
(IN THE SAME FILE AFTER M02)
(--------<MACHINE OFFSETS: B TURRET>--------)
OBSET
G140
VZSHX=0
VZSHY=0
VZSHZ=0
VZSHC=0
G50 S3800
VZOFZ=V198+[V187+V186*V190]+[V185-V184]
G141
VZSHX=0
VZSHY=0
VZSHZ=0
VZSHC=0
G50 S5000
VZOFZ=V197-[V187+V186*V189]-[V183-V182]
G140
RTS (THIS SAYS END OF SUBROUTINE)

... next sub

Sub names must start with an "O". If the second characters is a number the remaining 3 or less characters must be numbers, no letters. If the second digit is alphabetic the remaining characters can be numbers or letters.

The sub's can also be contained in a .sub or .ssb or .lib but you have to look at how to format your program select when you do. More advanced subject than you need here I suspect.

You can also pass arguments as temporary variables (as opposed to using a machine register). I suggest you read the book on this as it is a very powerful programming tool. From what I can tell this is what really makes Okuma macro different than the others.

Kev

[Superman]

To add to Kev's post

Basic subs - placed at end of a running program
- The CALL statement must be followed by a space
- The sub being CALLed must start with letter O, with a maximun of 4 letters/numbers following the O ---OO cannot be used, this is system reserved
- The sub is placed after the M02/M30 line, & must be in a downward search pattern, ie - the sub being called cannot be defined above the CALL statement ( in the program )
- There is a mximum size allowed for each sub, it is possible to break up a sub into smaller subs & use CALL statements to join together
- Maximum of 32 sub definitions permitted
- The % ( if used for file transfer ) is placed at the end of the program

[horst007]

I have decided to attach a file to show you what I am getting. Superman - If I put the call after the M02 it doesn't read it. I could write a book after the M02 and the control could care less. The exact call commands I have tried are as follows:

CALL O222
CALL O222.SUB
CALL 0222
CALL 0222.SUB
CALL O222 Q1
CALL O222.SUB Q1

I am putting them right before the M02.

[Superman]

I have decided to attach a file to show you what I am getting. Superman - If I put the call after the M02 it doesn't read it. I could write a book after the M02 and the control could care less. The exact call commands I have tried are as follows:

CALL O222
CALL O222.SUB
CALL 0222
CALL 0222.SUB
CALL O222 Q1
CALL O222.SUB Q1

I am putting them right before the M02.

No, all subs are to go after the M2 or M30, then they are parse / checked into RAM

Your first CALL statement is correct, it is searching for the sub.
It is the definition of the sub it is erroring on
NOTE---subs do also have a maximum size, overcome by breaking into smaller subs

ie
N99 ...main body
N100 CALL O222 Q2
N101 ...
N102 ...
...
M2
() <--- I use these just to sepeate the subs
O222 ( SUB #222 ) <--- name of the sub, comments do work here (I put the T# to show what tool is using it )
your sub body
RTS <--- to end the sub, & return to continue with N101
()
%

[annoying]

I have OSP700 but would assume subprogram use to be the same. I'd first ask you if you use the program name in the actual sub file. Your "O222.SUB" is just the file name, not the program name. When you open the file to edit, you should have:

O222
......
......
......
......
RTS

To add to that, you can have several programs in 1 file. I use several G-code macros, and they are in one file. I use a library type file for this so it is always brought up at start.

The file name is "OGMAC.LIB"......this is only a file name, not a program name

Opening this file will show.........

OG111 <-- this is a program name
.....
.....
...
...
...
RTS
OG112 <-- this is a program name
...
...
...
...
...
RTS
OG113 <-- this is a program name
...
...
...
RTS

(and so on)

Secondly, if you are calling a sub from a seperate file, the sub needs to be registered in the library. If your sub is specific to 1 main program, there is no reason to make a seperate subprogram file.

Put the subprogram after the main program in the same file. File name can be up to 8 characters and does not need to start with O, but must start with a letter I think.

Program name... (YOURFILE)

inside........

OMAIN <-- main file name
....
...
......
CALL O222
....
..
....
CALL O222
....
..
....
M2

O222 <-- subprogram
....
..
....
..
RTS

For program specific subs, I put the subs in the same file as above. You can also have multiple main programs and subprograms all in the same.

such as....

OPRT1
...
CALL O222
...
M2
OPRT2
...
CALL O222
...
CALL O223
...
M2
O222
...
RTS
O223
...
RTS

On my control, when I pull up a file with multiple mains, I select the file, put comma and then main program name... MAINFILE.MIN,OPART

don't know if any of this will help you

[Algirdas]

very useful explanation.
Would be very nice to have description how to register macros and subprograms to library and how to load library on CNC start

[fordav11]

File name can be up to 8 characters and does not need to start with O, but must start with a letter I think.

Yeah this is quite annoying. We have around 50 CNC machines and do the same parts on whichever machine is free at that time. The program number is listed on the job sheet that comes with the job (we have close to 50000 programs but at least half of those are machine-specific and only available on certain machines). We keep all the programs for each machine in separate directories since most programs have some machine-specific code but we wanted to keep the program numbers the same across all machines for that same part & operation so our job sheets don't need to have 50 machines listed and which program number is used. It works quite well like this as Fanuc programs only use numbers (no letters allowed) but Okuma programs must start with a letter, it won't allow a number-only program name so we need to add a special entry for the Okuma on our job sheets so the operator knows which program to download from our automated PC file server.

I don't suppose anyone knows if this can be set somehow to accept number-only program names? A parameter maybe?

[Algirdas]

simple database (excel table) can help to handle that - program definition with program names listed for each mahine.
There is no way to start program name with number on Okuma. File name can be, suppose