HEIDENHAIN TNC 620 User Manual page 386

10
Description of function
Mirroring is a modal function that is effective as soon as it has been
defined in the NC program.
The control mirrors contours or positions about the active workpiece
datum. If the datum is outside the contour, the control will also
mirror the distance to the datum.
If you mirror only one axis, the machining direction of the tool is
reversed The rotational direction defined in a cycle will remain
unchanged, e.g. if defined within one of the OCM cycles (option 167).
Depending on the selected AXIS axis values, the control will mirror
the following working planes:
X: The control mirrors the YZ working plane
Y: The control mirrors the ZX working plane
Z: The control mirrors the XY working plane
Further information: "Designation of the axes on milling machines",
Page 87
You can select up to three axis values.
If mirroring is active, the control displays it on the TRANS tab of the
additional status display.
Further information: User's Manual for Setup, Testing and Running
NC Programs
Input
11 TRANS MIRROR AXIS X
The NC function includes the following syntax elements:
Syntax Meaning
element
Start of syntax for mirroring
TRANS
MIRROR
AXIS or Enter mirroring of axis values or reset mirroring
RESET
X, Y or Z Axis values to be mirrored
Only if AXIS has been selected
386
Special functions | NC functions for coordinate transformations
; Mirror the machining operations
about the X axis
HEIDENHAIN | TNC 620 | Klartext Programming User's Manual | 01/2022