Yaskawa YASNAC PC NC Programming Manual - Manual (Page 60)

3 - 10
YASNAC PCNC Programming Manual Chapter 3: Movement Control Commands
• If an incorrect value is specified for “m” or “n”, alarm “0202” occurs.
(5) Supplements to Commands Used for Setting the Workpiece Coordinate System
• When the power is turned ON, the position where the tool is presently positioned is set
as (0, 0, 0). For the system not equipped with absolute position encoders, the present
tool position is temporarily set as the origin of the coordinate system until an appropri-
ate coordinate system is set.
• In the state where G92 (base coordinate system setting) is not specified, a workpiece
coordinate system is established in reference to the origin of the machine coordinate
system.
• In the state where G92 (base coordinate system setting) has been specified, a work-
piece coordinate system is established in reference to the origin of the base coordinate
system.
• If G92 is specified in the state where a workpiece coordinate system has been set, the
base coordinate system is set so that the present tool position takes the coordinate val-
ues specified in the G92 block. At the same time, the workpiece coordinate system is
defined in reference to the origin of the newly set base coordinate system.
• If G54 to G59 is executed in the tool length offset or tool position offset mode, present
offset is not canceled. Tool length offset or tool position offset should be canceled
before specifying G54 to G59.
Example of Programming
G43 Z0 H01; ? Position in workpiece coordinate system Z 100.
G54;
G90 Z1000. ? Position in workpiece coordinate system Z1100.
Actual Z-axis movement distance is 1400.
G54 shift distance Z = 300.
Offset H01 = 100.
• If G92 is specified while a program is executed in a workpiece coordinate system set
by G54 to G59, all workpiece coordinate systems (G54 to G59) and the base coordi-
nate system are shifted so that the coordinate values of the present position will be the
coordinate values specified in the G92 block. Therefore, G92 must not be specified in
the G54 to G59 mode.
• To change a workpiece coordinate system by G54 to G59, select the G90 mode before
calling the new coordinate system and select the G90 mode again before returning to
the base coordinate system.
• G54 to G59 must be specified in the G00 or G01 mode. If these G codes are specified
in another mode, alarm “0322” occurs.