CNC 8035 - Programming manual - Fagor Automation

Programming manual
4.
REFERENCE SYSTEMS
Coordinate preset and zero offsets
CNC 8035
·T· MODEL
(SOFT V16.3X)
·64·
4.4.2 Zero offsets (G54..G59 and G159)
The CNC has a table of zero offsets, in which several zero offsets can be selected. The aim is to
generate certain part zeros independently of the part zero active at the time. The table values are
given in radius.
Access to the table can be obtained from the front panel of the CNC (as explained in the Operating
Manual), or via the program using high-level language commands.
There are two kinds of zero offsets :
Absolute zero offsets (G54 ... G57, G159N1 ... G159N20), which must be referred to machine
zero.
Incremental zero offsets (G58,G59).
Functions G54, G55, G56, G57, G58 & G59 must be programmed alone in the block, and work in
the following way:
When one of the G54, G55, G56, G57 functions is executed, the CNC applies the zero offset
programmed with respect to machine zero, canceling the possible active zero offsets.
If one of the incremental offsets G58 or G59 is executed, the CNC adds its values to the absolute
zero offset active at the time. Previously canceling the additive offset which might be active.
You can see (in the following example) the zero offsets which are applied when the program is
executed.
G54 Applies zero offsets G54 ==> G54
G58 Applies zero offsets G58 ==> G54+G58
G59 Cancels G58 and adds G59 ==> G54+G59
G55 Cancels whatever and applies G55 ==> G55
Once a Zero Offset has been selected, it will remain active until another one is selected or until a
home search is carried out (G74) in JOG mode. This zero offset will remain active even after
powering the CNC off and back on.
This kind of zero offsets established by program is very useful for repeated machining operations
at different machine positions.
Example: The zero offset table is initialized with the following values:
G54: X0 Z330
G55: X0 Z240
G56: X0 Z150
G58: X0 Z-900
G59: X0 Z-180