GSK GSK980TDc, Руководство пользователя

Страница: 158 / 470

GSK980TDc Turning CNC System User Manual
140
Ⅰ
Progra
mming
O0100; (#100 is the machined workpiece number, its
initial value=0)
G00 X100 Z100;
T0101;
IF[#100<100]GOTO10; (has continuously machined
100
？
)
G65 P9580 U-0.01 W-0.01; (call the macro program
compensation tool wear)
N10 G00 X50 Z50;
……;
……;
……;
Machine program;
……;
T0202;
IF[#100<100]GOTO20; (has continuously machined
100
？
)
G65 P9580 U-0.01 W-0.01; (call the macro program
compensation tool wear)
N20 ……;
……;
……;
#100=#100+1; (machined workpiece 1)
IF[#100==101]THEN #100=0;
M30;
O9580;
G65 H23 P#101 Q#4120 R100; (obtain the
tool offset No.)
#102=2000+#101; (X wear macro
variable)
#103=2100+#101; (Z wear macro
variable)
#9102=#9102+#21; (modify X wear)
#9103=#9103+#23; (modify Z wear)
T#4120; (call a new tool offset value)
M99;
3.25.2 Operation and jump command G65
Command format:
G65 Hm P# i Q# j R# k;
m: operation or jump command, range 01
～ 99.
# I: macro variables name for storing values.
# j: macro variables name 1 for operation, can be constant.
# k: macro variables name 2 for operation, can be constant.
Command significance: # i = #j O # k
Example: P#100 Q#101 R#102…..#100 = #101 O #102;
P#100 Q#101 R15….#100 = #101 O 15;
P#100 Q-100 R#102…..#100 = -100 O #102;
Note: Macro variable name has no “#” when it is presented directly with constant.
Macro command list
Command format Functions Definitions
G65 H01 P#i Q#j Assignment # i = # j assign value of j to i
G65 H02 P#i Q#j R#k; Decimal add operation # i = # j + # k
G65 H03 P#i Q#j R#k; Decimal subtract operation # i = # j - # k
Operation sign specified by Hm