Fagor 8025 T CNC, Руководство по эксплуатации

Страница: 288 / 309

174 8025/8030 CNC PROGRAMMING MANUAL
P8: Finishing stock allowance along the Z axis. It must be greater or equal to zero or
error code 3 will be displayed.
P9: Feedrate of the finishing pass. If it is zero there will be no finishing pass. If it is
negative, error code 3 will be displayed.
NOTES:
1. The distance between the starting point 0 and final point (B) along the Z axis must
be equal or greater than P8. To avoid passes that are too thin or generating error 31
when operting with tool compensation the value of this distance (from 0 to B) should
be equal to P8+NP5, N being an entire number.
2. The distance from 0 to A along the X axis should be higher than P7.
3. The machining conditions (feedrate, spindle rotation, etc.) must be programmed
before calling the cycle. The parameters can be programmed in the calling block or
in previous blocks. The exit conditions of the cycle are G00 and G90.
4. If the position of the tool is not correct to execute the cycle, error code 4 will be
displayed. If it is correct a vertical facing will be carried out until it is reached and
then the cycle will be executed.
5. If there is a finishing pass, the cycle will be completed on the tool’s starting position
(0). If there is no finishing pass the cycle will end at point F.
6. If the last movement prior to calling the canned cycle (G82) has been executed in
G00, tool radius compensation (G41,G42) can be used. Otherwise error 35 will be
displayed.
The figure shows the elemental cycle. The movements 1-2 and 2-3 will be performed at
the programmed feedrate and the 0-1 and 3-0 in rapid.