Program Call (Cycle) - HEIDENHAIN ITNC 530 User Manual

PROGRAM CALL (Cycle 12)
Routines that you have programmed (such as special drilling cycles or
geometrical modules) can be written as main programs and then
called like fixed cycles.
Before programming, note the following:
The program you are calling must be stored on the hard
disk of your TNC.
If the program you are defining to be a cycle is located in
the same directory as the program you are calling it from,
you only need to enter the program name.
If the program you are defining to be a cycle is not located
in the same directory as the program you are calling it
from, you must enter the complete path (for example
TNC:\KLAR35\FK1\50.H.
If you want to define an ISO program to be a cycle, enter
the file type .I behind the program name.
As a rule, Q parameters are globally effective when called
with Cycle 12. So please note that changes to
Q parameters in the called program can also influence the
calling program.
Program name: Enter the name of the program you
want to call and, if necessary, the directory it is
located in.
Call the program with
CYCL CALL (separate block) or
M99 (blockwise) or
M89 (executed after every positioning block)
Example: Program call
A callable program 50 is to be called into a program via a cycle call.
HEIDENHAIN iTNC 530
7 CYCL DEF 12.0
PGM CALL
8 CYCL DEF 12.1
LOT31
9 ... M99
Example: NC blocks
55 CYCL DEF 12.0 PGM CALL
56 CYCL DEF 12.1 PGM TNC:\KLAR35\FK1\50.H
57 L X+20 Y+50 FMAX M99
0 BEGIN PGM
LOT31 MM
END PGM LOT31
477