Diameter programming (G51/G52)

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.

Programing Example

Diameter programming (G51/G52) in G18

;General settings (optional):

;Display position values in the diameter P-CHAN-00256 (TRUE, 1)

;Settings of X axis:

;Face turning axis, translatory: P-AXIS-00015 (0x41)

;G51 with G90: P-AXIS-00058 (TRUE, 1)

;G51 with G91: P-AXIS-00059 (FALSE, 0)(optional)

;G92, G53–G59 in the diameter: P-CHAN-00091 (TRUE, 1) (optional)

;Settings of Z axis:

;Longitudinal turning axis, translatory: P-AXIS-00015 (0x81)

;

N05 G18

N10 G90 G01 F1000

N20 G51 X80        ;diameter 80 mm

N30 G92 X10        ;G92 by 10 mm in the diameter

N40 X0             ;position 0 + G92 => diameter 10 mm

N50 G91 X50        ;X relative +50mm, in the diameter

N80 G52            ;deselect diameter programming

;…

N90 M30