Yaskawa YASNAC PC NC Programming Manual - Manual (Page 178)

4 - 41
YASNAC PCNC Programming Manual Chapter 4: Enhanced Level Commands
During tapping cycle in the solid tap mode, feed hold is invalid.
(f) Mode change
During tapping cycle in the solid tap mode, mode change is invalid.
(g) Program re-start
If the program is restarted from a block in the solid tap mode, G93 is not executed. There-
fore, to restart a program from a block in the solid tap mode, it is necessary to enter and
execute G93 in the MDI mode.
(h) Special options for canned cycles
Although an E command for reciprocal feed does not cause an alarm, it is disregarded.
The return feedrate is set for parameter pm 1252.
(5) Supplements to the Solid Tap Function
• In the G93 block, only S, F, and N codes can be specified. If other commands are
specified in the G93 block, alarm “0250” occurs.
• In the G93 mode, an S code is processed as the S command for solid tap operation.
• In the G93 mode, only G codes indicated below can be specified. If a G code not indi-
cated below is specified, alarm “0250” occurs. Concerning G01, although it can be
specified in the G93 mode, axis move commands cannot be specified.
G codes that can be specified in the G93 mode
G00, G01, G04, G70, G71, G72, G74, G80, G84, G90, G91, G98, G99
• Spindle indexing called in the G93 mode is the indexing to the fixed position in refer-
ence to the zero point pulse (C-axis) that is output from the spindle PG.
• If the G93 mode is established once, the spindle will fail to start even if the G93 mode
is canceled by G94 unless M03 or M04 is specified. Note that this feature is deter-
mined by the processing sequence of the machine. Although an S command remains,
gear selection signal is not output in the G93 mode. Accordingly, it is necessary to
specify an S command again when specifying M03 or M04.
• If there is more than one gear range, it is necessary to select the gear range to be used
for solid tap before specifying G93. Execute G93 only after the appropriate gear has
been selected.
• Concerning the R-point and Z-point level commands, G98/G99, G90/G91, L com-
mand, etc., all the precautions described for conventional tapping operation apply.
• The output voltage for spindle forward rotation/reverse rotation in G84/G74 cycle will
have a different sign according to the setting for the parameter. If “pm1001 D0 = 0”
“+” for the forward rotation, and if “pm 1001 D0 = 1”, “–” “for the forward rotation.
For reversing the spindle rotation direction, the NC automatically reverses the sign
without using SINV signal.
• To specify G94 after the completion of solid tap, make sure to cancel the canned cycle