G-Code, what is sub program... ++

[Vegabond]

Hello, i just started to job with cnc and run a fadal and a ledwell.

Can someone tell me something about sub programming? try to explain it easy.
Is it a "folder" there i put several codes or something?

Is it a easy way to learn the g/m-codes?


Greetings from Robert.

[angelw]

Hello, i just started to job with cnc and run a fadal and a ledwell.

Can someone tell me something about sub programming? try to explain it easy.
Is it a "folder" there i put several codes or something?

Is it a easy way to learn the g/m-codes?


Greetings from Robert.

Robert,
A sub program, whether its associated with CNC G code programs, or with software coding, is mostly used for reusable or repeatable code.

Lets say a pocket that uses 500 blocks to machine is repeated 10 times on a workpiece. You can either have a main program that has 5000 blocks plus a hand full of blocks to start and end the program, or you can have a main program that has the same hand full of blocks to start and end, plus 10 call blocks to the sub program and the sub program. Another example is if a large number of holes are being spot drilled, pilot drilled, drilled to a larger diameter, and then reamed. You could duplicate the X Y coordinated of the holes in the main program for each of the tools, or you could put the X Y coordinates in a Sub program and call it from the main program for each of the tools.

The structure of sub programs varies with the control, but the basic logic is the same. With a Fanuc controls, the sub programs are loaded as separate programs and called initially from the main program and then can call other sub programs or return to the main program. Hass controls have the subs loaded at the end of the main program, but are called from the main program and can call other subs.

Its neither easier nor harder to learn G and M codes using Sub programs, but it makes for more compact, structured programs, and usually more easy to follow, particularly if there is a lot of code involved. Sub programs also prove useful when proving a program. If for example the sub is to machine a number of identical pockets in the workpiece, once the detail has been proved correct for the first pocket, the detail will be correct for all subsequent pockets, only the position of each pocket will have to be checked on prove out.

Regards,

Bill

[Perfect Circle]

Go to page 368 it should help you with it some...
Good Luck~!
CNC programming handbook: a ... - Google Books

[Geof]

A subprogram or subroutine is just a group of commands you want to execute several times. Here is an example machining a slot:

The subroutine starts at line N1000 immediately below the M30 for the main program. Because this was written for a Haas both the main program and the subprogram are in the same file, on other machines they may be two separate files.

The main program positions the tool at X0. Y0. which is one end of the slot, just above the surface (Z0.005). Then line N8 does an incremental move the length of the slot going down Z-0.055. At the end of this move it executes the M97 P1000 command which tells the main program to look for line N1000 and continue execution from there. At line N1000 absolute movements are reinstated and the the machine goes back and forth along the slot returning on line N1004 to X0. Y0. then it reaches the M99 command which tells it to go back to the main program.

The slot has to be deeper than one pass which is why line N8 has the L3. As long as the remaining L value is greater than zero the M99 command tells the machine to go back to line N8. So it does and the same sequence happens until the subroutine has been used 3 times. When L has counted down to zero then the M99 command tells the machine to go back to line N9, retracts the tool and ends the program.

The only line number that is needed is N1000, I just put in the others for the description. This is an inefficient program because there is wasted motion in cutting the slot so nobody needs to tell me that.

O00015 (SLOTTING HOLES X AXIS)
N1 G00 G20 G40 G49 G80 G90 G98
G53 G00 Z0.
N2 G10 L12 G90 P1 R0.25
N3 T1 M06
N4 G43 H01
N5 M03 S2000
N6 G54 G00 X0. Y0. Z1.
N7 Z0.005 M08
N8 G91 G01 X-0.8 Z-0.055 F5. M97 P1000 L3
N29 G90 G00 Z1. M09
N30 G53 G00 Z0.
N32 G53 G00 Y-2.
N33 M30
N1000 G90 Y-0.005
N1001 X0. F10.
N1002 Y0.005
N1003 X-0.8 F20.
N1004 X0. Y0. F100.
N1005 M99

This example show a subroutine used at a single location to make something deeper. You can also use subroutines to do the same operation at different places and this just gets a little more complicated to set up with respect to work zeros and the absolute-incremental-absolute changes.

EDIT: The post above refers to a programming book which mentions M98 not M97. M98 uses a separate program as the subprogram. On Haas machines M97 calls a subroutine at the bottom of the main program and uses M98 to call a separate program just like other machines. Also the P in the M98 P(line number) may be M98 O(line number). Finally, Haas machines can use the L number to call a subroutine more than once, but I do not know if it is possible to use the L number with M98, I never use M98 but I use M97 in just about every program I write. Haas also allows for calling subroutines within subroutines within subroutines......which does get a bit complicated but is very useful.

[sinha_nsit]

L is allowed in M98 (on Fanucs). Up to 9999 repetitions are permitted (L9999). With seven-digit M98, only 999 repetitions are possible.