Cycle 8 MIRRORING
ISO programming
G28
Application
The control can machine the mirror image of a contour in the working plane.
Mirroring takes effect as soon as it has been defined in the NC program. It is also in effect in the Manual operating mode in the MDI application. The active mirrored axes are shown in the additional status display.
- If you mirror only one axis, the machining direction of the tool is reversed; this does not apply to SL cycles
- If you mirror two axes, the machining direction remains the same.
The result of the mirroring depends on the location of the datum:
- If the datum lies on the contour to be mirrored, the element simply flips over.
- If the datum lies outside the contour to be mirrored, the element also “jumps” to another location.
Reset
Program Cycle 8 MIRRORING again with NO ENT.
Related topics
- Mirroring with TRANS MIRROR
Notes
- This cycle can only be executed in the FUNCTION MODE MILL machining mode.
For working in a tilted system with Cycle 8, the following procedure is recommended:
- First program the tilting movement and then call Cycle 8 MIRRORING!
Cycle parameters
Help graphic | Parameter |
---|---|
Mirror image axis? Enter the axes to be mirrored. You can mirror all axes—including rotary axes—with the exception of the spindle axis and its associated secondary axis. You can enter up to three NC axes. Input: X, Y, Z, U, V, W, A, B, C |
11 CYCL DEF 8.0 MIRRORING |
12 CYCL DEF 8.1 X Y Z |