GSK GSK988TA, Manual

Page: 132 / 531

GSK988TA/GSK988TA1/GSK988TB Turning Center CNC System User Manual 【 Programming & Operation 】
114
Ⅰ
Programming
Note 8: X=0: the theory speed is infinite but the actual speed corresponds to 10V voltage because the
maximum voltage of sent analog is 10V.
Example:
Fig.2-67
Program:
M3 G96 S300; (Spindle rotates clockwise, the constant surface speed control is valid
and the surface speed is 300m/min)
G0 X100 Z100; (Rapid traverse to A point with spindle speed 955 r/min)
G0 X50 Z0;
(Rapid traverse to B point with spindle speed 1910 r/min)
G1 W-30 F200; (Cut from B to C with spindle speed 1910 r/min)
X80 W-20 F150; (Cut from C to D with spindle speed 1910 r/min and surface speed
1194 r/min)
G0 X100 Z100; (Rapid retract to A point with spindle speed 955 r/min)
M30;
(End of program, spindle stop and cooling OFF)
2.22 Feedrate per Minute G98/G94, Feedrate per Rev G99/G95
G98 command function: G98 specifies the cutting feedrate is feedrate per minute, G98 is modal.
When the current is G98 modal, G98 cannot be input.
Command format: G98 Fxxxx;
G99 command function: G99 specifies the cutting feedrate is feedrate per rotation, G99is
modal. When the current is G99 modal, G99 cannot be input.
Command format: G99 Fxxxx;
Command explanation:
When G99 Fxxxx (B set of G code is G95) is executed, the actual cutting feedrate is
gotten by multiplying the F code value (mm/r) to the current spindle speed(r/min). If
the spindle speed varies, the actual feedrate changes too. If the spindle cutting feed
amount per rev is specified by G99 FXXXX (B set of G code is G95), the even cutting
texture on the surface of workpiece will be gotten. In G99 (B set of G code is G95)