PROGRAMMING12. COMPENSATION FUNCTION
If the programmable mirror image function is specified when the
command for producing a mirror image is also selected by a CNC external
switch or CNC setting (see III–4.7), the programmable mirror image
function is executed first.
Applying a mirror image to one of the axes on a specified plane changes
the following commands as follows :
Circular command G02 and G03 are interchanged.
Cutter compensation G41 and G42 are interchanged.
Coordinate rotation CW and CCW (directions of rotation) are interchanged.
Processing proceeds from program mirror image to scaling and
coordinate rotation in the stated order. The commands should be specified
in this order, and, for cancellation, in the reverse order. Do not specify
G50.1 or G51.1 during scaling or coordinate rotation mode.
In programmable mirror image mode, G codes related to reference
position return (G27, G28, G29, G30, etc.) and those for changing the
coordinate system (G52 to G59, G92, etc.) must not be specified. If any
of these G codes is necessary, specify it only after canceling the
programmable mirror image mode.
D Mirror image by setting
D Mirror image on a single
axis in a specified plane
D Commands related to
reference position return
and coordinate system