Reference Point Approach (G74) - Siemens SINUMERIK 828D Programming Manual

14.4

Reference point approach (G74)

Function
When the machine has been powered up (where incremental position measuring systems
are used), all of the axis slides must approach their reference mark. Only then can traversing
movements be programmed.
The reference point can be approached in the NC program with G74.
Syntax
G74 X1=0 Y1=0 Z1=0 A1=0 ...
Significance
G74
X1=0 Y1=0 Z1=0 ...
A1=0 B1=0 C1=0 ...
Note
A transformation must not be programmed for an axis which is to approach the reference
point with G74.
The transformation is deactivated with command TRAFOOF.
Example
When the measurement system is changed, the reference point is approached and the
workpiece zero point is initialized.
Program code
N10 SPOS=0
N20 G74 X1=0 Y1=0 Z1=0 C1=0 ;
N30 G54
N40 L47
N50 M30
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
:
:
:
; Programmed in a separate NC block
Search for reference
Specified machine axis address X1, Y1, Z1... Search for
reference for linear axes
Specified machine axis address A1, B1, C1... Search for
reference for rotary axes.
Comment
; Spindle in position control
Reference point approach for linear axes and rotary
axes
; Zero offset
; Cutting program
; End of program
Supplementary commands
14.4 Reference point approach (G74)
411