Programming principles
1.3 Axis movements
Turning Part 2: Programming (Siemens instructions)
Programming and Operating Manual, 05/2012, 6FC5398-5DP10-0BA0
49
1.3.11 Fixed point approach: G75
Functionality
By using G75, a fixed point on the machine, e.g. tool change point, can be approached. The
position is stored permanently in the machine data for all axes. A maximum of four fixed
points can be defined for each axis.
No offset is effective. The velocity of each axis is its rapid traverse.
G75 requires a separate block and acts non-modal. The machine axis identifier must be
programmed!
In the part program block after G75, the previous G command of the "Interpolation type"
group (G0, G1,G2, ...) is active again.
Programming
G75 FP=<n> X1=0 Z1=0
Note
FPn is referencing with axis machine date MD30600 $MA_FIX_POINT_POS[n-1]. If no FP is
programmed, then the first fixed point is selected.
Table 1- 2 Explanation
Command Significance
G75 Fixed point approach
FP=<n> Fixed point that is to be approached. The fixed point number is specified: <n>
Value range of <n>: 1, 2, 3, 4
If no fixed point number is specified, fixed point 1 is approached automatically.
X1=0 Z1=0 Machine axes to be traversed to the fixed point.
Specify the axes with value "0" with which the fixed point is to be approached
simultaneously.
Each axis is traversed with the maximum axial velocity.
Programming example
N05 G75 FP=1 X1=0 ; Approach fixed point 1 in X
N10 G75 FP=2 Z1=0 ; Approach fixed point 2 in Z, e. g. for
tool change
N30 M30 ; End of program
Note
The programmed position values for X1, Z1 (any value, here = 0) are ignored, but must still
be written.
To Next Page
Loading...
Need help?
General
