Diameter programming (G51/G52)
Syntax: | ||
G51 | Select diameter value | modal |
G52 | Deselect diameter value | modal, initial state |
W | Workpiece zero point | P | Cutting point |
X | Face turning axis | Z | Longitudinal turning axis |
M | Machine zero point | A | Fixed stop point |
C | Control zero point | d | Programmed dimension for diameter programming |
When diameter programming is selected, the positional values for the face turning axis in a motion block are interpreted as diameter values relative to the turning centre point.
It should be noted that the programmed coordinates of the face turning axis only correspond to the workpiece diameter if the zero point of the face turning axis is located at the turning centre point (irrespective of whether offsets act as a diameter; see Programming example).
The axis parameters can parameterise axes in "face turning” mode:
- G51 with absolute programming (G90) (P-AXIS-00058)
- … and/or G51 with relative programming (G91) (P-AXIS-00059
- Reference point programming (G92) and zero point programming (G53 – G59) in the diameter (P-CHAN-00091)
G51 acts on the axis which is operated in "face turning” mode. When the face turning axis is selected, the face turning axis must exist in the machining plane (G17, G18, G19).
The coordinates of the circle centre point (I, J, K) and circle radius programming (R) are not programmed in the diameter.
Diameter programming is deselected with G52.
Programming Example
Diameter programming (G51/G52) in G18