GSK 988T, User Manual

Page: 107 / 416

Chapter
Ⅱ
G Commands
93
Ⅰ
Programming
executes not to stop until the current block is executed completely; if the continuous thread
cutting is executed, the program run pauses after thread cutting blocks are executed completely;
Note 9: In Single block, the program stops run after the current block is executed. The program stops run
after all blocks for thread cutting are executed;
Note 10: The thread cutting decelerates to stop when the system resets, emergently stop or its driver
alarms;
Note 11: The system alarms when the thread run-out length is more than the thread machined length of the
long axis.
Note 12: In G32, the basic axis command cannot be in the same block with its parallel axis command,
otherwise, the system alarms.
Note 13: When machining the thread in the metric tool machine in the unit of tooth/inch, using the
expression calculated value programs F command. For example, when the thread with 10
teeth/inch is machined, using F[25.4/10] programs.
Note 14: The system automatically checks the spindle speed before machining the thread, the system
alarms when the spindle speed is not commanded. The spindle speed cannot be checked in the
course of the machining.
Example: Pitch: 2mm. δ 1 = 3mm, δ 2 = 2mm,total cutting depth 2mm with two times cut-in.
Fig. 2-57
Program:
O0009;
G00 X28 Z3; (First cut-in 1mm)
G32 X51 W-75 F2.0; (First taper cutting)
G00 X55; (Tool retraction)
W75; (Z returns to the starting point)
X27; (Second tool infeed 0.5mm)
G32 X50 W-75 F2.0; (Second taper thread cutting )
G00 X55; (Tool retraction)
W75 ; (Z returns to the starting point)
M30;
2.16.2 Thread cutting with variable lead G34
Command function: G34 can machine the metric, inch pitch. Machine metric or inch straight,
taper, end face thread with variable pitch.
Command format: G34 X(U) __ Z(W) __ F(I) __ J__ K__ R__ ;
Command specifications: G34 is modal;
IP_, J_, K_, Q_ Meaning and value range are the same those of G32