Program Call (Cycle 12, Din/Iso: G39); Cycle Function; Please Note While Programming; Cycle Parameters - HEIDENHAIN TNC 640 User Manual

11
11.3 PROGRAM CALL (Cycle 12, DIN/ISO:
G39)

Cycle function

Routines that you have programmed (such as special drilling cycles
or geometrical modules) can be written as main programs. These
can then be called like fixed cycles.

Please note while programming:

The program you are calling must be stored in the
internal memory 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 need only 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 a DIN/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.

Cycle parameters

Program name: Enter the name of the program
you want to call and, if necessary, the directory it
is located in or
Activate the file select dialog and select the
program to be called via the SELECT soft key.
Call the program with:
CYCL CALL (separate block) or
M99 (blockwise) or
M89 (executed after every positioning block)
318
Cycles: Special Functions | PROGRAM CALL (Cycle 12, DIN/ISO: G39)
HEIDENHAIN | User's manual for cycle programming | 10/2017
Designate program 50 as a cycle and
call it with M99
55 CYCL DEF 12.0 PGM CALL
56 CYCL DE 12.1 PGM TNC:
\KLAR35\FK1\50.H
57 L X+20 Y+50 FMAX M99