Fagor 8025 T CNC, Руководство по эксплуатации

Страница: 298 / 309

184 8025/8030 CNC PROGRAMMING MANUAL
P5: Initial pass. It defines the depth of the first cutting pass. The subsequent passes will
depend on the sign given to the parameter:
- If the sign is positive, the depth of the second pass will be P5 2 and the
depth of the 11th will be P5 n , until the finishing depth is reached.
- If the sign is negative, the deepening increment will be constant and of a value
equal to the absolute value of the parameter.
- If the value is equal to zero, error 3 is generated.
P6: Safety distance. It indicates the distance from point B to point B'.
- If the value is positive, this movement will be done in G05 (rounded corner).
The 0 value is considered positive.
- If the value is negative, this movement will be done in G07 (square corner).
P8: Finishing pass:
- If it is 0, the previous pass is repeated.
- If the value is positive, the finishing pass will be carried out maintaining a P12/
2 angle with the Z axis.
- If the value is negative, the finishing pass will be done with radial entry.
P10: Thread pitch along X axis in radius.
Note: For threads per inch (or mm) use 1/threads per inch (or mm). Ex.:6 threads
per inch = P10 =K1 F4 K6.
P11: Thread exit (in radius). It defines the distance from the end of the thread to the point
where the exit starts. If it is negative, error code 3 will be displayed. If it is different
from zero, the section CB’ is a tapered thread whose pitch along X axis is P10. If
it is zero, the section CB’ is executed in G00 (X only while Z decelerates).
P12: Angle of the tool’s nose. It makes the starting points of the successive passes to be
at a P12/2 angle with the Z axis. Do not forget to adjust the tool angle by 1/2° if you
want each pass to shave the thread wall.
The machining conditions (feedrate, spindle rotation, etc.) must be programmed before the
cycle is called. The parameters can be programmed in the call block or in previous blocks.
The cycle does not alter the calling parameters and thus, they can be used for future cycles.
The parameters P80 to P99 are altered. The exit conditions are G00, G07, G40, G90 and
G97. The cycle starts with a G00 approach to point A’ and ends at A’ as well. When
executing the block, the F feedrate speed can’t be altered by turning the FEEDRATE knob
whose value will be frozen at 100%.