GSK GSK988TA, Руководство пользователя

Страница: 149 / 531

Chapter 2 G Commands
131
Ⅰ
Programming
Command function: the spindle rotating one rotation makes Z move one pitch, which keeps
consistent with the screw tap’s pitch, forming a spiral grooving in the workpiece’s
inner hole to complete its thread machining one time.
Note: it is different from the
spindle tapping
.
Command format
：
G84 X (U)_ C (H)_ Z (W)_ R_ P_ F_ K_ M_ ;
G88 Z (W)_ C (H)_ X (U)_ R_ P_ F_ K_ M_ ;
Command explanation:
X_ C_ or Z_ C_ It is the hole position data and is valid in the specified blocks; specify
other axes which are not X, Z,C axis are valid at the hole position
data.
Z(W)_ or X(U)_ Using an absolute value specifies the hole bottom’s coordinate value
or using an incremental value specifies the distance from point R
plane to the hole bottom, and is valid in the specified blocks.
R_ Distance from the initial plane to point R, is presented with radius
value with direction.
P_
Hole bottom pause time, ISB system time is 1ms
，
ISC system time is
0.1ms.
F_
Cutting feedrate
，
K_
Program execution times （ if necessary ） .
M_
M code for C clamping
（
if necessary
）
.
The tapping feed axis specifies X or Z according to G84/G88. The tapping axis specified by G84
is Z and the tapping axis specified by G88 is X. The relevant G signal selects one spindle (relevant
with the PLC).
The cutting feedrate F (i.e. the tapping axis’ feedrate) and spindle speed S confirm the thread’s
lead.
In feed per minute mode, thread lead formular=cutting feedrate F /spindle speed S
；
In feed per rotation mode, thread lead formular=cutting feedrate F.
Note: Before the spindle speed S specifies the common tapping, the CNC memorizes the spindle speed S’s
modal value. The CNC counts the thread lead according to S’s modal value and F value specified in the
code. When a common tapping is executed, the spindle override is influenced by N0.3708#6.
When G84/G88 is the rigid tapping cycle, Q code and the parameter PCP determine three kind of
rigid tapping mode: standard rigid tapping cycle, high-speed deep-hole rigid tapping cycle and deep
hole rigid tapping cycle. When G84/G88 is the common tapping cycle, there is only one mode below.
Before G84/G88, the spindle rotation (the operator confirms the spindle rotation CW or CCW
according to the used screw tap) can be specified firstly, and the CNC can confirm the M code for the
spindl’s reverse rotation according to G84/G88’s previous spindle rotation direction; when it is not
specified, the spindle defaults the spindle rotation CW M03 when the system executes G84/G88
common tapping cycle.
Incremental
system
Metric input
（
mm
）
Inch input (inch)
ISB system
-99999.999 ～ 99999.999mm -9999.9999 ～ 9999.9999 inch
R
ISC system
-9999.9999
～
9999.9999 mm -999.99999
～
999.99999 inch