Cycle call
For cycles that remove material, you have to enter not only the cycle definition, but also the cycle call in the NC program. The call always refers to the machining cycle that was defined last in the NC program.
The control provides the following options for calling a cycle:
Syntax | Meaning |
---|---|
G79 corresponds to the CYCL CALL Klartext syntax | The control calls the most recently programmed machining cycle at the last programmed position. |
G79 PAT corresponds to the CYCL CALL PAT Klartext syntax | The control calls the most recently programmed machining cycle at all positions you have defined in a point table. |
G79|G01 corresponds to the CYCL CALL POS Klartext syntax | The control calls the most recently programmed machining cycle at the position you defined in the NC block with G79|G01. |
M89 and M99 | With M99, the control executes the most recently programmed machining cycle at the most recently programmed position. With M89, the control executes the most recently programmed machining cycle after each positioning block until it reads M99. |
N110 G79 M3 | ; Call cycle |
N110 G79 PAT F200 M3 | ; Call cycle at all positions in the point table |
N110 G79|G01 G90 X+0 X+25 | ; Call cycle at the defined position |
N110 G01 X+0 X+25 M89 | ; Call cycle at the defined position and for each new positioning block |
N120 G01 X+25 Y+25 | |
N130 G01 X+50 Y+25 M99 | ; Call cycle for the last time at the defined position |