HEIDENHAIN TNC 640 User Manual page 62

2
Cycle call with M99/M89
The M99 function, which is active only in the block in which it
is programmed, calls the last defined fixed cycle once. You can
program M99 at the end of a positioning block. The TNC moves to
this position and then calls the last defined fixed cycle.
If the TNC is to run the cycle automatically after every positioning
block, program the first cycle call with M89.
To cancel the effect of M89, program:
M99 in the positioning block in which you move to the last
starting point, or
Use CYCL DEF to define a new fixed cycle
Cycle call with SEL CYCLE
If the PGM CALL key is pressed, with SELECT CYCLE you can use
any NC program as a machining cycle. The syntax is displayed and
SELECT FILE enables you to select an NC program. Call this with
CYCLE CALL, CYCL CALL PAT, CYCL CALL POS or M99.
If you run a program selected with SEL CYCLE it is
executed in Program Run, Single Block without a stop
after each block. It is also only visible as one block in
Program Run, Full Sequence.
CYCL CALL PAT and CYCL CALL POS use positioning
logic before the cycle is performed. SEL CYCLE and
Cycle 12 PGM CALL are identical with regard to the
positioning logic: With a point pattern the clearance
height to be approached is calculated via the maximum
from the Z position at the start of the pattern and all
Z positions in the point pattern. With CYCL CALL POS
there is no pre-positioning in the tool axis direction.
You must program pre-positioning within the called file
yourself in that case.
62
Using Fixed Cycles | Working with fixed cycles
HEIDENHAIN | User's manual for cycle programming | 10/2017