GSK GSK988TA, Manual

Page: 142 / 531

GSK988TA/GSK988TA1/GSK988TB Turning Center CNC System User Manual 【 Programming & Operation 】
124
Ⅰ
Programming
be specified in G84/G88 blocks in the mode.
G84 X_ C_ Z_ R _ P_ F_ K_ M29 S_;
X_ C_;
G80;
G84/G88 is used for rigid tapping(Bit0 of No.5200 is set to 1); in the mode, G84/G88 is used for
only the rigid tapping mode instead of the common tapping mode.
G84 X_ C_ Z_ R _ P_ F_ K_ M _;
X_ C_;
G80;
M29 (the parameter sets other M code to specify it) is for rigid tapping, the system alarms when S
is specified between M29 and G84/G88 blocks or the axis movement code is specified; the system
alarms when M29 is specified repetitively in tapping cycle (M29 cannot be specified repetitively).
M29 Sxxxx codes rigid tapping mode. The corresponding switch is done after PLC receives M29
and the spindle stops rotation. The spindle output is equivalent to S0 output in M29.
2.24.2 End Rigid Tapping Cycle (G84) / Side Rigid Tapping Cycle (G88)
Command function: When the spindle is controlled in rigid mode (it is taken as the servo motor),
the rigid tapping cycle is executed.
Command format: G84 X (U)_ C (H)_ Z (W)_ R_ Q_ P_ F_ K_ M_ ; or
G88 Z (W)_ C (H)_ X (U)_ R_ Q_ P_ F_ K_ M_ ;
X_ C_ or Z_ C_ It is the hole position data and is valid only in the specified block; the
hole position data can specify other valid axes except for X, Z, C.
Z(W)_ or X(U)_ It specifies the coordinate value of hole bottom by using absolute
coordinate, or specifies the distance from point R plane to the hole
bottom by using incremental value, and it is valid in the specified
block.
R_ It is the distance from the initial plane to point R and is specified by
radius value with direction. Its unit and range is shown below.
P_ Hole bottom pause time. Unit of ISB system is 1ms and ISC is 0.1ms.
Q_ Cutting amount every time is specified by radius value. Its unit and
range are shown below.
When Q value is specified, G84/G88 selects the high speed deep hole
rigid tapping cycle or deep hole rigid tapping cycle by PCP (No.
5200#5). Q value is not specified or Q value is 0, the standard rigid
tapping cycle is selected.
F_ Cutting feedrate.
K_ Execution times of program
（
if neccessary
）
.
M_ M code for clamping C axis
（
if neccessary
）
.
The tapping feed axis specifies X or Z by G84/G88. The tapping axis specified by G84 is Z an the
one specified by G88 is X. the relevant G signal confirms to select a spindle (it is relevant with the
PLC).