CNC 8035 - Programming manual - Fagor Automation

Programming manual
9.
CANNED CYCLES
G86. Longitudinal threading canned cycle
CNC 8035
·T· MODEL
(SOFT V16.3X)
·200·
9.9.1 Basic operation
1. Rapid move (G00) to the approach point located at a safety distance “D” from the initial point
(X, Z).
2. Threading loop. The following steps will be repeated until the finishing coordinate is reached;
programmed depth “I” minus the finishing stock “L”.
·1· Rapid move (G00) to the programmed depth indicated by “B”. This move will be made
according to the penetration angle of the selected tool (A).
·2· Performs the threading of the programmed section with the selected exit “J”. The feedrate
F cannot be varied with the feedrate override switch while threading; it will stay at 100%. At
the beginning of the machining operation on large lathes, when cutting long threads, the
spindle speed may be overridden in the first passes to prevent the part from bending.
·3· Withdrawal in rapid (G00) to the approach point.
3. Thread finishing. Rapid move (G00) to the programmed depth coordinate “I”.
This move will be radial or according to the tool penetration angle (A) which depends on the sign
assigned to parameter “L”.
4. Performs the threading of the programmed section with the selected exit “J”.
The feedrate F cannot be varied with the feedrate override switch while threading; it will stay at
100%. It will not be possible to vary the spindle speed override in the last threading pass, it will
be set to the value imposed in the previous pass.
5. Withdrawal in rapid (G00) to the approach point.
Thread repair
To do a thread repair, proceed as follows:
1. Home (reference) the spindle.
2. Measure the angle of the root of the thread, K W parameters.
3. Define the G87 cycle for thread repair.
4. Execute the canned cycle.
Considerations
The machining conditions (feedrate, spindle speed, etc.) must be programmed before calling 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.