PROGRAMMING
B–63834EN/02
5. FEED FUNCTIONS
67
If the direction of movement changes between specified blocks during
cutting feed, a rounded–corner path may result (Fig. 5.1 (b)).
0
Programmed path
Actual tool path
X
Z
Fig. 5.1 (b) Example of tool path between two blocks
In circular interpolation, a radial error occurs (Fig. 5.1(c)).
0
r
∆r:Error
Programmed path
Actual tool path
X
Z
Fig. 5.1 (c) Example of radial error in circular interpolation
The rounded–corner path shown in Fig. 5.1(b) and the error shown in Fig.
5.1(c) depend on the feedrate. So, the feedrate needs to be controlled for
the tool to move as programmed.
G00 IP_ ;
G00 : G code (group 01) for positioning (rapid traverse)
IP_ ; Dimension word for the end point
The positioning command (G00) positions the tool by rapid traverse. In
rapid traverse, the next block is executed after the specified feedrate
becomes 0 and the servo motor reaches a certain range set by the machine
tool builder (in–position check).
A rapid traverse rate is set for each axis by parameter No. 1420, so no rapid
traverse feedrate need be programmed.
The following overrides can be applied to a rapid traverse rate with the
switch on the machine operator’s panel:F0, 25, 50, 100%
F0: Allows a fixed feedrate to be set for each axis by parameter No. 1421.
For detailed information, refer to the appropriate manual of the machine
tool builder.
D Tool path in a cutting
feed
5.2
RAPID TRAVERSE
Format
Explanations