Yaskawa YASNAC PC NC Programming Manual - Manual (Page 81)

3 - 31
YASNAC PCNC Programming Manual Chapter 3: Movement Control Commands
(2) Supplements to the Tool Length Offset Function
• If the offset amount is changed by MDI operation, the new offset amount becomes
valid from the block in which an H code is specified.
• It is possible to call up the tool position offset or tool radius offset C function in the
tool length offset mode.
• It is not allowed to specify G43, G44, or G49 in a canned cycle mode.
• If G92 is specified with a Z command while in the tool length offset mode, the tool
length offset mode is canceled. However, G92 should be specified in the state that the
tool length offset mode has been canceled.
• During automatic operation, it is possible to display the tool offset number (H code
number) that is presently valid.
• G43, G44, and G49 can be specified only in the G00 or G01 mode. Designation of
these G codes in the G02 or G03 mode is not allowed.
• For the execution of the reference point return command, including two axes, in the
tool length offset mode, whether the H code and the tool length offset amount should
be saved or canceled can be specified by the setting for a parameter.
• For the reset operation in the tool length offset mode, whether the H code and the tool
length offset amount should be saved or canceled can be specified by the setting for a
parameter. It is also possible to specify whether a G code (G49) in 08-group should be
saved or canceled.
pm4010 D = 0 Both the H code and the tool length offset amount are canceled.
pm4010 D = 1 Both the H code and the tool length offset amount are saved.
pm4010 D = 0 Both the H code and the tool length offset amount are canceled.
pm4010 D = 1 Both the H code and the tool length offset amount are saved.