Fagor 8055 M - Page 61

Programming manual
CNC 8055
CNC 8055i
REFERENCE SYSTEMS
4.
·M· & ·EN· MODELS
SOFT: V02.2X
·61·
Coordinate preset and zero offsets
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 G158 (incremental zero offset)
The G158 instruction may be used to program and activate an incremental offset in a program. This
feature is used to define new part zeros in the same program without having to set them previously
in the offset table or use high level instructions.
When applying an incremental zero offset, the CNC adds it to the absolute zero offset active at a time.
Programming:
Incremental zero offset are defined by program using function G158 followed by the values of the
zero offset to be applied on each axis. To cancel the incremental zero offset, program function G158
without axes in the block. To cancel the incremental zero offset only on particular axes, program
a 0 (zero) incremental offset for each one of them.
X Y
G54 (G159N1) 20 20
G55 (G159N2) 120 20
N100 G54 (It applies the first zero offset)
··· (Machining of profile 1)
N200 G158 X20 Y45 (Apply incremental zero offset)
··· (Machining of profile 2)
N300 G55 (It applies the second zero offset. G158 stays active)
··· (Machining of profile 3)
N400 G158 (Cancel incremental zero offset. G55 stays active)
··· (Machining of profile 4)
Y
X
65
W
WW
W
50
20
20 40 60 120
1
2 3
4