Fanuc 0m. Confirmation when changing local coordinate system

[JuanCruz]

Hello everybody,

Our new machine acquisition has a small problem in regular operation. It's a ENSHU DT-CL with a FANUC 0M control.

During program execution, if we want to change the local coordinate system (for example from g55 to g57) we need to press the physical button of program start to continue with execution.

Is there any parameter to switch automatically between different coordinate systems?

Best regards and thanks in advance,

[drdos]

What happens when you program G59? Does the program just stop? Do you alarm out? Can you post a sample program?

[Heavy_Metal]

Hi JuanCruz,

Are you sure it isn't program related ?
Just like drdos asked, can you post a sample program or a part of one Tool.

Regards,
Heavy_Metal.

[JuanCruz]

Dear,

Thanks for your fast replies. We change the coordinate system in the main program before executing several small subprograms. In bold you can see below where the program stops.

DRDOS: Program stops with no alarm
HEAVY_METAL: I don't think so. I use this same control in other machine with no needed to confirm coordinates system changes.

O0800
(HERRAMIENTA Y POSICIÓN)


G17 G40 G49 G54 G80 G90 G94 (CANCELACIÓN DE COMPENSACIONES)
G54 (DEBE ESTAR DEFINIDA EN ORÍGENES MÁQUINA)


(DEFINICIÓN DE ORIGENES PIEZA, EL CONTROL YASNAC TOMA LOS ORÍGENES RESPECTO A LA REFERENCIA ABSOLUTA MÁQUINA)
G90 G10 L2 P1 X212.Y-97.5Z-50.(G54 PUNTO TALADRO PALLET M61)
G90 G10 L2 P2 X219.1Y-282.1Z-50.(G55 PUNTO TALADRO ROSCADO PALLET M61)
G90 G10 L2 P3 X212.Y-97.5Z-50.(G56 PUNTO TALADRO PALLET M62)
G90 G10 L2 P4 X219.1Y-282.1Z-50.(G57 PUNTO TALADRO ROSCADO PALLET M62)




M98 P0002 (ENTRADA PALLET M61)
G54 (PROGRAM STOPS)
M98 P0801
G55 (PROGRAM STOPS)
M98 P0802
G55 (PROGRAM STOPS)
M98 P0803


M98 P0003 (ENTRADA PALLET M62)
G56 (PROGRAM STOPS)
M98 P0801
G57 (PROGRAM STOPS)
M98 P0802
G57 (PROGRAM STOPS)
M98 P0803


M30 (FIN DE PROGRAMA)


Thanks in advance,

[JuanCruz]

Sorry, program stops when executing a subprogram.

Also, do you know how to execute automatically?

[Heavy_Metal]

Hi JuanCruz,

Can you post let's say the first and last 5 lines of your subprogram.
What's in between is not important.

Regards,
Heavy_Metal.

[JuanCruz]

Dear H_M,

Of course, find one of the subprogram below.

O0801 (SUBRUTINA TALADRADO COMPENSADOR 51x21)


M06T1 (TALADRADO DIÁMETRO 11,70 mm)
M3S3500
M8


G0 G90 X0. Y0.
.
.
.


G99M05
G90 Z100. (POSICIÓN DE SEGURIDAD)


M99 (FIN SUBRUTINA TALADRADO COMPENSADOR 51x21)

[Heavy_Metal]

Hi,

Maybe you have to change some lines.

M98 P0002 (ENTRADA PALLET M61)
G54 G17 G40 G49 G80 G90 G94 (PROGRAM STOPS)
M98 P0801
G55 G17 G40 G49 G80 G90 G94 (PROGRAM STOPS)
M98 P0802
G55 G17 G40 G49 G80 G90 G94 (PROGRAM STOPS)

Are you sure that your toolchange position is correct when you call a subprogram.
Maybe you have to add a G00 G28 G91 Z0 at the beginning or end of a subprogram.

Regards,
Heavy_Metal.

[Heavy_Metal]

Hi JuanCruz,

Are you sure the G90 G10 L2 P1 X212.Y-97.5Z-50. works on this control.
Check whether the value of G10 has been entered in the offset table.
Is the value in the WORK table for the G54 --- X212. Y-97.5 Z-50. ???
Otherwise enter the value manually and delete the G10 lines.

What happens when you try to run a subprogram without the main ?
Add these lines at top of subprogram and try to run the program.

G54 G17 G40 G49 G80 G90 G94
G00 G28 G91 Z0
M06 T01
S___ M03
G00 G90 X---.--- Y---.---
G43 Z---.--- H01
-
-

Regards,
Heavy_Metal.

[JuanCruz]

Dear Heavy_Metal,

Best solution ever!! Thank you very much, just adding the tool change height (G91 G28 Z0.), the program does not stop.

Best regards!

[Heavy_Metal]

Hi JuanCruz,

You're welcome, glad to hear it works.

Regards,
Heavy_Metal.