
B–63284EN/03
3. TOOLING COUNT
EXPANSION FUNCTION
ADDITIONAL FUNCTIONS OF SERIES
BH1E/BH2E/BH3E AND BH1F/BH2F/BH3F
664
Bit 1 (WOF) of parameter No. 27004 is provided to allow the tool–nose
radius, tool radius, and imaginary tool nose direction of the tool used in
each process to be written in the NC offset data area at the beginning of
the execution of the process. This enables tooling with the same T code
and different tool ID numbers in machining with the tool mounting angle
changed using the ATC function, B–axis, and so forth.
#7
27004
#6 #5 #4 #3 #2 #1
WOF
#0
WOF At the beginning of each process during program execution,
conversational tool data (tool–nose radius, tool radius, and imaginary tool
nose direction) is:
1 : Written as offset data on the NC side.
0 : Not written as offset data on the NC side.
<Related parameters: Bit 5 (SPO) of No. 9760, bit 3 (PTF) of No. 9763,
bit 0 (TPO) of No. 9764, bit 2 (OSV) of No. 9766,
and bit 0 (TLC) of No. 9774>
NOTE
1 Set this parameter for each tool post.
2 In machining simulation when the offset data save and
restore function is used, the offset data before simulation is
maintained regardless of this function.
3 Even if tools having the same T code and different tool ID
numbers are found when execution is selected, warning
message “0703 SAME T CODE FOUND IN TOOLING
DATA” does not appear. The offset data is replaced by the
tool data of the last process.
4 When automatic residual machining is performed in the bar
machining process, the T code for the tool used for forward
cutting must be different from the T code for the tool used
for residual machining. Otherwise, the tool data for residual
machining is written to the NC offset data area.
5 When this function is used, the tool moves to the tool
change position at the end of each process regardless of
the settings of bit 0 (TPO) of parameter No. 9764 and bit 5
(SPO) of parameter No. 9760 even if the same tool is used
in consecutive processes.
6 If bit 0 (TLC) of parameter No. 9774 is set to 0, this function
is unavailable.
7 When the tool data protection function in tooling is used
(when bit 3 (PTF) of parameter No. 9763 is set to 1), this
function is unavailable.
8 After program execution (except machining simulation
when the offset data save and restore function is used), the
offset data on the NC side has been replaced by the most
recently executed status.
3.2.3
Writing Conversational
Tool Data into NC
Offset Data