Lenze ETC Motion Control - Manual (Page 144)

CNC programming
G functions
G functions individual descriptions
3
3.2
3.2.2
l
144 EDSTCXN EN 2.0
3.2.2.56 G143 Parameters of grinding phases during noncircular grinding
With G143, the parameters must be programmed for every grinding phase,
e.g. roughing, smoothing, fine finishing and sparking out.
G143 X D C F L J I
X Overmeasure for this phase in mm.
D Positioning amount per revolution in mm.
C Motion range of the C axis in which the positioning should take place. If it
is not programmed, the positioning takes place via a complete revolution
of the C axis.
F Path speed during this phase in mm/min.
L Program number of the subprogram in which the finished profile is
described.
J Block number in the current program, from which the finished profile is
described.
I Number of additional revolutions without positioning.
G143 is needed to define the grinding phases during noncircular grinding. At
least one grinding phase is necessary.
For L, the number of the program is specified, in which the finished profile is
described. As an alternative to L, the block number, from which the finished
profile is described in the current program, can also be specified with J. In any
case, the description of the finished profile must be ended with G99.
The profile is described in a virtual X/Y plane, with the X position 0
°
and the
Y position 90
°
corresponding to the C axis. For this, both cartesian
coordinates (G1, G2, G3) and polar coordinates (G101, G102, G103) can be
used.
When using the spline interpolation, G5 must not be programmed in the
finished profile. Instead, it must already be switched on before the first G143
and switched off after the last G143.
The total number of workpiece revolutions of a grinding phase results from
the programmed overmeasure and the positioning amount per revolution
(X/D) plus the programmed number of revolutions without positioning.
See G140/G141/G142
Syntax
Meaning of the addresses
Explanation
Example