FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
B–62764EN/01
9. COORDINATE VALUE
AND DIMENSION
129
Either inch or metric input can be selected by G code.
G20 ;
G21 ;
Inch input
mm input
This G code must be specified in an independent block before setting the
coordinate system at the beginning of the program. After the G code for
inch/metric conversion is specified, the unit of input data is switched to
the least inch or metric input increment of increment system IS–B or IS–C
(II– 2.3). The unit of data input for degrees remains unchanged.The unit
systems for the following values are changed after inch/metric
conversion:
– Feedrate commanded by F code
– Positional command
– Work zero point offset value
– Tool compensation value
– Unit of scale for manual pulse generator
– Movement distance in incremental feed
– Some parameters
When the power is turned on, the G code is the same as that held before
the power was turned off.
WARNING
1 G20 and G21 must not be switched during a program.
2 When switching inch input (G20) to metric input (G21) and vice versa, the tool compensation
value must be re–set according to the least input increment.
However, when bit 0 (OIM) of parameter 5006 is 1, tool compensation values are automatically
converted and need not be re–set.
CAUTION
For the first G28 command after switching inch input to metric input or vice versa, operation from
the intermediate point is the same as that for manual reference position return. The tool moves
from the intermediate point in the direction for reference position return, specified with bit 5
(ZMI) of parameter No. 1006.
NOTE
1 When the least input increment and the least command increment systems are different, the
maximum error is half of the least command increment. This error is not accumulated.
2 The inch and metric input can also be switched using settings.
9.3
INCH/METRIC
CONVERSION
(G20,G21)


Leave a Reply

Your email address will not be published. Required fields are marked *