Programming manual
CNC 8055
CNC 8055i
REFERENCE SYSTEMS
4.
·M· & ·EN· MODELS
SOFT: V02.2X
·63·
Coordinate preset and zero offsets
The incremental zero offset is not canceled after applying a new absolute zero offset (G54-G57
or G159Nx).
As described earlier, only one incremental zero offset may be active; therefore, instructions G58
and G59 are incompatible with G158. This way, the last incremental zero offset programmed
cancels the incremental zero offset that is currently active.
Programming the G158 function alone in the block or G158 with a 0 value in the axes cancels the
incremental zero offset G158 activated earlier. Those instructions also cancel the incremental zero
offsets G58/G59 that are currently active.
Considerations:
An incremental zero offset, by itself, does not cause any axis movement.
When homing an axis in JOG mode, the incremental zero offset for that axis is canceled.
Function properties:
G158 is modal and incompatible with G53.
On power-up, the CNC assumes the incremental zero offset that was active when the CNC was
turned off. On the other hand, the incremental zero offset is neither affected by functions M02 and
M30 nor by RESETTING the CNC.
Display in the zero offset table:
In ISO mode and conversational mode, the zero offset table is one line over the the G54 position
where it identifies the G158 with its values X, Y, Z, etc.
This line cannot be modified from the table, it can only be modified by programming G158.
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.
To Next Page
Loading...
