CNC 8035 - Programming manual - Fagor Automation

9.6.1 Basic operation
Drilling
1. Rapid move to the approach point located at a "D" distance from the first hole position.
2. First drilling operation. The drilling axis moves in G01 to the programmed incremental depth
"D+B".
3. Drilling loop. The following steps will be repeated until the programmed depth "I" is reached.
It first withdraws in rapid (G00) a distance “H” or to the approach point. Rapid approach (G00)
to a "C" distance from the next peck.
New drilling step. G1 move to the next incremental depth “B and R”.
4. Dwell “K” in hundredths of a second at the bottom of the hole, if programmed.
5. Withdrawal in rapid (G00) to the approach point.
Tapping
1. Rapid movement to the approach point located at a safety distance "D" from the tap point.
2. Tapping. The drilling axis moves in G01 to the programmed incremental depth "D+B".
3. Reverse the spindle turning direction.
If "K" has been programmed, the spindle stops and after the programmed dwell has elapsed,
the spindle starts turning in the other way.
4. Withdrawal in work feedrate to the approach point.
Rigid tapping
1. Tapping takes place at the center of the part (X0). Rapid movement to the approach point located
at a safety distance "D" from the tap point.
2. Tapping. Tapping to the incremental depth programmed in “D+B”.
It is carried out by interpolating the main spindle (that is turning) with the Z axis. Rigid tapping
cannot be interrupted, nor the machining conditions be changed. It is done at 100% of the
programmed "S" and "F".
3. Reverse the spindle turning direction.
If "K" has been programmed, the spindle stops and after the programmed dwell has elapsed,
the spindle starts turning in the other way.
4. Withdrawal in work feedrate to the approach point.
Rigid tapping is drawn with the color used for "uncompensated tool path". When the cycle is
completed, the spindle stops (M5).
Considerations
The machining conditions (feedrate, spindle speed, etc.) must be programmed before calling the
cycle.
When tapping (regular or rigid), the general logic output "TAPPING" (M5517) stays active during
the execution of the cycle.
Once the canned cycle has ended, the program will continue with the same feedrate F and G
functions active previous to calling the cycle. Only the tool radius compensation will be cancelled
(G40) if it was active.
Programming manual
CANNED CYCLES
G83. Axial drilling and tapping canned cycle 9.
CNC 8035
·T· MODEL
(SOFT V16.3X)
·185·