Setting G59 Offset through Macro Program

[Ashish B]

Hi

How to set Machine home position as offset (G59) in a program through Macro Programming.

Ash

[ggborgen]

If you mean machine home to be part zero this should work
#5321=X
#5322=Y
#5323=Z
These system variables are Fanuc.
Hope this helps

[Ashish B]

Hi

Actually these are the variables which stores the machine position (may be absolute, home, relative )

But how to transfer these values to G59 offset.

Ash

[christinandavid]

Search for posts/threads regarding the use of G10.

G10 is commonly used to load Work/Tool Offsets (or reset them).

eg G90 G10 L2 P6 X#5321 Y#5322 Z#5323

DP

[dcoupar]

I'm not quite sure if this is what you are trying to do, but...

On a 21iM-B:

#5021 is the current machine position in X
#5022 is the current machine position in Y

#5321 is the X value for G59
#5322 is the Y value for G59

G91 G28 X0 Y0 (MOVE X AND Y TO HOME)
#5321 = #5021 (SET G59 X TO CURR MACH POS)
#5322 = #5022 (SET G59 Y TO CURR MACH POS)

[Ashish B]

Hi

In the procedure mentioned, we need to go to call a home position return command first & than use
#5321=#5021


But is there any other way to directly set the Work offset as Home Position.


I think this may work -
#5321=0.0
#5322=0.0
G90 G59 X-15.0 Y-15.0

This will directly locate the spindle on a position offset by 15 mm from the machine home position.

Your comments/suggestion please.

Ash

[dcoupar]

Why not just use G53 instead of G59?

[Ashish B]

What G53 ?

[dcoupar]

Most Fanuc controls use G53 as a one-shot Machine Coordinate System.

G53 G90 X-15. Y-15. positions X and Y -15. from Machine Zero.

[Ashish B]

Ok...

If i say G53 G90 G0 X-10.0 Y-10.0

it will move directly to desired position (without going to home position)


AM I RIGHT ?

[dcoupar]

Yes

[Ashish B]

So, after G53 If i command G54 it will follow the G54 coordinate system...aM i Right ?


Is there any fuss to restore the Zero Position just like G92 which is a temporary shift command ?

Is G53 preset as machine zero by the controller or we need to define it.