GSK GSK988TA, Manual

Page: 151 / 531

Chapter 2 G Commands
133
Ⅰ
Programming
mode) . The program can be modified according to the actual position of the spindle stop at the
hole bottom in G84/G88 machining away from G84/G88 start point’s coordinate value. So, remain
enough hole depth before G84/G88 machining to execute G84/G88 machining.
Note 2 ： Before tapping cycle, the operator can specify the spindle rotation direction (i.e., code the
spindle rotation CW/CCW in advance) in advance according to the screw tap. When the tool
reaches point R to start tapping, at the moment, the CNC does not output the spindle rotation M
code. After the tool reaches the hole bottom, the CNC automatically judges the corresponding M
code when the spindle rotates CCW. After the tapping ends, the spindle stops rotation. When
G84/G88 is still used in the next block, and the tool reaches point R, the CNC outputs again the M
code for the spindle rotation to make the spindle rotation, at the moment, the spindle rotation
direction is consistent with the specified in advance before tapping cycle.
When the spindle rotation is not specified before tapping, the CNC defaults the spindle rotation
CW M03 during tapping. After the fixed cycle is cancelled, the spindle stops rotation. The spindle
is started again when the machining should be continuously executed.
Note 3: During the tapping, the tapping axis’ move speed is determined by the spindle speed and pitch
instead of the cutting feedrate override; the spindle override is influenced by N0.3708#6 during
cutting.
Note 4: When the single block or feed hold is executed, the system displays “Pause”, and the tapping
cycle does not stop till the tapping is completed and the tool returns to the start point.
Note 5: When a reset, emergency stop or drive alarm occurs, the tapping cutting decelerates to stop. In
the course, the spindle needs to decelerate to stop but Z exactly stops feed, so, the workpiece
and screw tap maybe be damaged. So, G84/G88 should be not forcibly interrupted as possible
during machining.
Note 6: N0.5209#0=0, i.e., “in rigid tapping, the drilling axis executes the selection by the plane”. The
drilling axis is separate X, Z, Y for the separately specified G17, G18, G19 in G84; the drilling axis
is separate Y, X, Z for the separately specified G17, G18, G19 in G88.
Note 7: When R plane exceeds the initial plane and the hole bottom plane in the tapping blocks, an alarm
occurs.
Program example: in the following figure, thread M10×2
Fig. 2-78
G98 ；
Feed per minute mode
G0 X0 Z200
；
X and Z position to the start point
M3 S800 ；
The spindle rotates CW and the spindle speed is 800 rev/min.
After the block is execute, the spindle starts rotation
G84 Z160 P1000
F1600
；
The start point is X0 Z200
，
the hole position and the start point are
the same, the dwell time is 1sec and the thread’s lead is 2
according to F value and S value. When the rigid tapping mode
is not specified in advance, G84 is the common tapping cycle.
After the block is executed, the spindle stops rotation
N G80
；
The fixed cycle is cancelled