Zero Shift/Max. Spindle Speed Set (G50) - Okuma OSP-P200L Programming Manual

2.

Zero Shift/Max. Spindle Speed Set (G50)

2-1. Zero Shift
[Function]
With the G50 code, zero offset value is automatically calculated and zero setting is carried out
according to the calculated value.
This feature is effective when cutting a workpiece on which the same contour is repeated.
[Programming format]
G50 X__ Z__ C__
X/Z/C : Specify the coordinate value to be taken as the actual position data after zero shift.
[Details]
For the present X- and Z-axis position, the coordinate value specified following G50 are assigned.
[Program]
N004 G00
N005 G50
N006 G00
With the program above, the axes are positioned to the coordinate point (X0, Z0) by the commands
in block N004 first. When the commands in N005 are executed, the coordinate system is re-
established so that (X0, Z0), where the axes have been positioned, now has the coordinate values
(X1, Z1) which are specified following G50.
This program shifts the origin of the coordinate system:
X = X0 - X1
Z = Z0 - Z1
Provided X0 = 100 mm and X1 = 200 mm, zero offset amount is calculated as;
100 - 200 = -100 mm
This amount can be checked on the screen.
Dimension words in sequences N006 and after that are all referenced to the origin newly
established by the commands in N005.
[Supplement]
1) Axes not specified in the block containing G50 are not subject to zero offset.
2) G50 is non-modal and active only in the programmed block. (Zero offset is calculated only in
the G50 block. All dimension words after that block are referenced to the shifted new origin.)
3) When the control is reset, all zero set data are cleared and the initial zero offset data become
effective.
4) No tool offset number entry is allowed in the block containing the G50 code.
X0 Z0
X1 Z1
X2 Z2
SECTION 4 PREPARATORY FUNCTIONS
5238-E P-41
LE33013R0300600030001