CNC 8035 - Programming manual - Fagor Automation

Programming manual
3.
AXES AND COORDINATE SYSTEMS
Coordinate programming
CNC 8035
·T· MODEL
(SOFT V16.3X)
·52·
Programming example assuming that the Polar Origin is located at the Coordinate Origin.
Absolute coordinates:
G90 R430 Q0 ; Point P0
G03 Q33.7 ; Point P1, in an arc (G03)
G01 R340 Q45 ; Point P2, in a straight line (G01)
G01 R290 Q33.7 ; Point P3, in a straight line (G01)
G01 R230 Q45 ; Point P4, in a straight line (G01)
G01 R360 Q63.4 ; Point P5, in a straight line (G01)
G03 Q90 ; Point P6, in arc (G03)
Incremental coordinates:
G90 R430 Q0 ; Point 0
G91 G03 Q33.7 ; Point P1, in an arc (G03)
G01 R-90 Q11.3 ; Point P2, in a straight line (G01)
G01 R-50 Q-11.3 ; Point P3, in a straight line (G01)
G01 R-60 Q11.3 ; Point P4, in a straight line (G01)
G01 R130 Q18.4 ; Point P5, in a straight line (G01)
G03 Q26.6 ; Point P6, in arc (G03)
The polar origin, apart from being able to be preset using function G93 (described later) can be
modified in the following cases :
On power-up, after executing M02, M30 EMERGENCY or RESET, the CNC will assume, as the
polar origin, the coordinate origin of the work plane defined by the general machine
parameter"IPLANE".
Every time the work plane is changed (G16,G17,G18 or G19), the CNC assumes the coordinate
origin of the new work plane selected as the polar origin.
When executing a circular interpolation (G02 or G03), and if the general machine parameter
"PORGMOVE" has a value of 1, the center of the arc will become the new polar origin.