GSK 988T, User Manual

Page: 111 / 416

Chapter
Ⅱ
G Commands
97
Ⅰ
Programming
cutting is completed with
Pause
on screen;
Note 8: After executing single block in thread cutting, the program run stops after the system returns to
starting point(one thread cutting cycle is completed);
Note 9: Thread cutting decelerates to stop when the system resets, emergently stops or its driver alarms;
Note 10: The system alarms when the thread run-out length of the long axis is more than the thread
machining length of the long axis;
Note 11: The system alarms when the thread run-out length of the short axis is more than the thread
machining length of the short axis;
Note 12: The system automatically checks the spindle speed, and an alarm occurs when the spindle speed
is not specified. The spindle speed cannot be checked during the machining.
Example:
Fig. 2-62
Program:
O0012;
M3 S300 G0 X150 Z50 T0101; (Thread tool)
G0 X65 Z5; (Rapid traverse)
G92 X58.7 Z-28 F3 J3 K1; (Machine thread with 4 times cutting, the first tool
infeed 1.3mm)
X57.7 ; (The second tool infeed 1mm)
X57; (The third tool infeed 0.7mm)
X56.9; (The fourth tool infeed 0.1mm)
M30;
2.16.4 Multiple thread cutting cycle G76
Command function: Machining thread with specified depth of thread (total cutting depth)is
completed by multiple roughing and finishing, if the defined angle of
thread is not 0°, thread run-in path of roughing is from its top to bottom,
and angle of neighboring thread teeth is the defined angle of thread.
G76 can be used for machining the straight and taper thread with
thread run-out path, which is contributed to thread cutting with single
tool edge to reduce the wear of tool and to improve the precision of
machining thread. But G76 cannot be used for machining the face
thread. machining path is as Fig.2-55.
Command format ： G76 P （ m ）（ r ） （ a ） Q （ dmin △ ） R （ d ）；
G76 X
（
U
）
Z
（
W
）
R
（
i
）
P
（
k
）
Q
（
d
△ ）
F J_ K_
；