CNC 8035 - Programming manual - Fagor Automation

Using absolute zero offsets:
G54 ; Applies G54 offset
Profile execution ; Executes profile A1
G55 ; Applies G55 offset
Profile execution ; Executes profile A2
G56 ; Applies G56 offset
Profile execution ; Executes profile A3
Using incremental zero offsets:
G54 ; Applies G54 offset
Profile execution ; Executes profile A1
G58 ; Applies offsets G54+G58
Profile execution ; Executes profile A2
G59 ; Applies offsets G54+G59
Profile execution ; Executes profile A3
Function G159
To apply any zero offset defined in the table.
The first six zero offsets are the same as programming G54 through G59, except that the values
of G58 and G59 are absolute. This is because function G159 cancels functions G54 through G57
and, consequently, there is no active zero offset to add the G58 or G59 to.
Function G159 is programmed as follows:
G159 Nn where n is a number from 1 to 20 that indicates the number of the zero offset being
applied.
Function G159 is modal, it is programmed alone in the block and is incompatible with functions G53,
G54, G55, G56, G57, G58, G59 and G92.
On power-up, the CNC assumes the zero offset that was active when the CNC was turned off. On
the other hand, the zero offset is neither affected by functions M02 and M30 nor by RESET.
This function is displayed in the history like G159Nn where the n is the active zero offset.
Examples:
G159 N1 It applies the first zero offset. It is the same as programming G54.
G159 N6 It applies the sixth zero offset. It is the same as programming G59, but it is applied
in absolute.
G159 N20 It applies the 20th zero offset.
Programming manual
REFERENCE SYSTEMS
Coordinate preset and zero offsets 4.
CNC 8035
·T· MODEL
(SOFT V16.3X)
·65·