Yaskawa YASNAC PC NC Programming Manual - Manual (Page 201)

4 - 64
YASNAC PCNC Programming Manual Chapter 4: Enhanced Level Commands
(5) Supplements to the Mirror Image ON/OFF Function
• Before specifying G28 or G29 to execute tool change or to end machining, make sure
to turn OFF the mirror image function by specifying M94. If G28 or G29 is specified
without canceling the mirror image function, alarm “0127” occurs.
• The mirror image function is invalid for offset distance used by the tool length offset
function. In the mirror image mode, the present position data (POS) display the actual
tool movements.
• Using the mirror image function with the workpiece coordinate rotation, scaling, and/
or coordinate rotation function
The functions must be specified in a predetermined order. If they are specified by dis-
regarding the predetermined order, alarm “0285” occurs.
Workpiece coordinate rotation (G54) > Mirror image (M94) >
Scaling (G51) > Coordinate rotation (G68)
• If the scaling function is called up in the mirror image mode, it is applied to the center
point of scaling.
If the coordinate rotation function is called up in the mirror image mode, it is applied
to the center of rotation and also in the direction of rotation.
• If the axes for which mirror image is applied are specified using the M code, buffering
of the M codes which set and reset the axes must be disabled by the setting for appro-
priate parameters (pm4400 to pm4409).
4.1.7 Programmable Data Input (G10) *
By using the G10 command, it is possible to write the tool offset amount and the work coordinate
system.
(1) Setting the Tool Offset Amount
The tool offset amount can be set by using the specially provided screen. By using a program,
the tool offset amount is set in either of the following two types (H and D used in common,
and H and D used independently, and tool wear offset function provided/not provided).
(a) When H and D are used in common
By specifying “G10 L10P • • • R 00 • • •; (P: tool offset number, R: tool offset amount, L10:
omissible)”, the tool offset data of the specified tool offset number can be changed to the
required amount.
• If G10 is executed in the G90 mode, the value set for R is saved as the tool offset
amount.
• If G10 is executed in the G91 mode, the value set for R is added to the existing offset
amount.
• Tool wear offset function provided.