Programmable Data Input; Changing The Tool Offset Value (G10) - Siemens SINUMERIK 808D Programming And Operating Manual

P2: Specification of the dwell time in USER DATA, _ZSFR[22]
Explanations
After the positioning at the bottom of a hole a traversing movement takes place to point R with rapid traverse. Thereafter,
drilling is done from point R to point Z, and a return is done to point R.
Example
M3 S2500
G00 X50.0 C0.0
G85 Z-40.0 R-5.0 P500 M31
C90.0 M31
C180.0 M31
C270.0 M31
G80 M05
Deselection of the fixed cycle for drilling (G80)
Fixed cycles can be deselected with G80.
Format
G80;
Explanations
The fixed cycle for drilling is deselected, and a transition is made to the normal operation again.
3.4.2

Programmable data input

3.4.2.1

Changing the tool offset value (G10)

With the command "G10 P ⋅⋅⋅ X(U) ⋅⋅⋅ Y(V) ⋅⋅⋅ Z(W) ⋅⋅⋅ R(C) ⋅⋅⋅ Q ;", the available tool offsets can be overwritten. However, it is
not possible to create new tool offsets.
For description of the addresses, see the table below:
Address Description
P Tool offset number (see explanation below)
X Tool offset for the X axis (absolute, incremental)
Y Tool offset for the X axis (absolute, incremental)
Z Tool offset for the Z axis (absolute, incremental)
78
;Rotate the drilling tool
;Positioning X and C axis
;Machining of hole 1
;Machining of hole 2
;Machining of hole 3
;Machining of hole 4
;Deselection of the cycle and
;Stopping of the drilling tool
Programming and Operating Manual (ISO Turning/Milling)
01/2017