GSK 988T, User Manual

Page: 150 / 416

GSK988T Turning CNC System User Manual
136
Ⅰ
Programming
2.22.4 Macro program statement and NC statement
The following blocks are macro program statements:
Including arithmetic or logical operation (=);
Including control statement(such as GOTO, DO, END);
Including macro program call command (G65, G66, G67).
Any NC blocks except for macro program statement are NC statements.
In Single Block mode, when No.6000 Bit5 (SBM) is set to 0, the system directly skips the
macro program statement and the machine does not stop, but it is set to 1, the system stops run
and enters the stop state.
One block cannot have the macro program statement and NC statement simultaneously.
2.22.5 Macro program call
（
1
）
Non-modal call of macro program G65
Command format : G65 P L __
〈
argument list
〉；
Command function : The system calls macro program L times specified by P and transfers
the argument to the called macro program.
Command explanations: P: specify the macro program to be called;
L
：
times of calling the macro program, and its default is 1 and its
range is 1 ～ 9999;
Argument list: data transferred to macro programs.
Argument specification
：
Two types of argument specification are available. Argument specification I uses letters other than
G, L, O, N and P once each. Argument specification II uses A, B and C once each and also uses I,
J, and K up to ten times. The types of argument specification is determined automatically
according to the letters used.
Argument specification I
Address Variable No. Address Variable No. Address Variable No.
A #1 I #4 T #20
B #2 J #5 U #21
C #3 K #6 V #22
D #7 M #13
W #23
E #8 Q #17 X #24
F #9 R #18 Y #25
H #11 S #19 Z #26
Addresses G, L, N, O and P cannot be used in arguments;
Addresses that need not be specified can be omitted and local variables corresponding to an
omitted address are set to null;
Addresses do not need to be specified alphabetically. They conform to word address format.