Siemens SINUMERIK 808D ADVANCED Programming And Operating Manual page 57

This results in the current workpiece coordinate system. The rewritten dimensions use this as a reference.
The offset is possible in all axes.
Note
In the X-axis, the workpiece zero should be in the turning center due to the functions of diameter programming (DIAMON)
and constant cutting speed (G96). For this reason, use no offset or only a small offset (e.g. as allowance) in the X axis.
See the following effect of the programmable offset:
Programming
TRANS Z... ; programmable offset, deletes old instructions for offsetting, rotation, scaling factor, mirroring
ATRANS Z... ; programmable offset, additive to existing instructions
TRANS ; without values: clears old instructions for offset, rotation, scaling factor, mirroring
The instructions that contain TRANS or ATRANS each require a separate block.
Programming example 1
N10 G54
N20 TRANS Z5
N30 L10
N40 ATRANS X10
N50 TRANS
N60 M30
Subroutine call: see Section "Subroutine technique (Page 113)".
Programming example 2
G90 G18 G500
T3D1
M4S1500
G0X50 Z10
CYCLE95( "CON1:CON1_E", 0.50000, 0.20000, 0.20000, ,0.20000, 0.20000, 0.15000, 9, , ,2.00000)
M4S1200
G0X100Z-10
R0=46
LAB1:
TRANS X=R0 Z-25
AROT RPL=-10
R1=-45
R2=14
Programming and Operating Manual (Turning)
6FC5398-5DP10-0BA2, 06/2015
; programmable offset, 5 mm in Z-axis
; Subroutine call; contains the geometry to be offset
; programmable offset, 10 mm in x-axis
; offset cleared
57