Programming instructions

ADT-CNC4620 Programming Manual
- 18 -
Fig. 2-4-1
The program follows:
O0010;
G00 X160 Z80; (move the machine tool to safe position first)
G98;
G0 X50 Z0; (move to point B quickly from point A through point M)
G1 W-30 F250; (B→C)
X100 W-20; (C→D)
X140; (D→E)
G2 W-40 R20; (EFG arc interpolation)
W-10; (G→H)
M30;
%
2.4.3. G98, G99
Instruction format: G98 Fxxxx; (F0001~F8000, the leadin 0 can be omitted, specify the feeding
speed every minute, mm/min)
Instruction function: specify the cutting feeding speed in the unit mm/min, G98 is mode G
instruction. If current mode is G98, it isn’t required to enter G98.
Instruction format: G99 Fxxxx
; (F0.0001~F500, the leadin 0 can be omitted)
Instruction function: specify the cutting feeding speed in the unit mm/r, G99 is mode G instruction.
If current mode is G99, it isn’t required to enter G99. When the system executes G99 Fxxxx
, the
product of of F instruction value (mm/r) and current principal axis rotation (r/m) is used as the
instruction feeding speed to control the actual cutting feeding speed. When the principal axis
rotation is changed, the actual cutting feeding speed also changes. Use G99 Fxxxx to specify the
cutting feeding every rotation of the principal axis, and form even cutting grain on the surface of the
workpiece. In G99 mode, the machine tool must be installed with principal axis encoder, and set
principal axis encoder wires.
G98 and G99 are in the same group of mode G instruction, and only one is valid at the same time.
G98 is initial G instruction, and G98 is valid by default when the system is electrified.