Writing Work Offset/Tool Offsets (G10) - Siemens SINUMERIK 808D Programming And Operating Manual

Workpiece coordinate systems are setup after the reference point approach after Power On. The closed position of the
coordinate system is set in MD20154[13].
3.3.1.5

Writing work offset/tool offsets (G10)

The workpiece coordinate systems defined through G54 to G59 or G54 P{1 ... 93} can be changed with the following two
processes.
● Data inputting at HMI operator panel
● with the program commands G10 or G50 (setting actual value)
Format
Modified by G10:
G10 L2 Pp X (U)... Z(W)... ;
p=0: External workpiece work offset
p=1 to 6: The value of the workpiece work offset corresponds to the workpiece coordinate system G54 to G59 (1
= G54 to 6 = G59)
X, Z: Absolute setting data of the workpiece coordinate system offset.
U, W: Incremental setting data of the workpiece coordinate system offset.
Modified by G50:
G50 X... Z... ;
Explanations
Modified by G10:
G10 can be used to change each workpiece coordinate system individually. If the work offset with G10 is to be written only
when the G10 block is executed on the machine (main run block), then MD20734 $MC_EXTERN_FUNCTION_MASK, Bit 13
must be set. An internal STOPRE is executed in that case with G10. The machine data bits affect all G10 commands in the
ISO Dialect T and ISO Dialect M.
Modified by G50:
By specifying G50 X... Z..., a workpiece coordinate system that was selected earlier with a G command G54 to G59 or G54
P{1 ...93}, can be shifted and thus a new workpiece coordinate system can be set. If X and Z are programmed incrementally,
the workpiece coordinate system is defined in such a way that the current tool position matches the total of the specified
incremental value and the coordinates of the previous tool position (shift of coordinate system). Finally, the value of the
coordinate system shift is added to each individual value of the workpiece work offset. To put it another way: All workpiece
coordinate systems are shifted systematically by the same value.
Example
The tool in operation with G54 is positioned at (190, 150), and the workpiece coordinate system 1 (X' - Y') is created each
time in G50X90Y90 with a shift of Vector A.
Example of setting coordinates:
Programming and Operating Manual (ISO Turning/Milling)
01/2017
39