Fagor 8025 T CNC, Operating Manual

Page: 184 / 309

70 8025/8030 CNC PROGRAMMING MANUAL
6.21.1. G59 as additive zero offset
If P616(4) =1 When a G64-G59 function is executed the zero offset applied to each
axis will be the value indicated in the table (G54....G59) plus the value
indicated in position G59 on the table. It does not affect G53.
If P616(4)=0 In this case, the zero offset which is applied to each axis will be the value
indicated on the table.
6.22. G65. INDEPENDENT AXIS EXECUTION
With function G65 it is possible to move one axis independently while other axes are being
interpolated.
In the following program:
N0 G65 Y100 F1
N10 G01 X10 Z5 F1000
N20 G01 X20
When executing block "N0", the Y axis starts moving at a feedrate of F1. Then, block
"N10" starts executing the XZ interpolation at F1000 while the Y axis keeps moving at F1.
If "P621(4)=0", the CNC executes block "N20" once "N10" is completed regardless of
whether "N0" is completed or not (Y axis has reached position or not).
If "P621(4)=1", the CNC waits until blocks "N0" and "N10" are completed (all axes have
reached position) before executing block "N20".
6.23. G70/G71 UNITS OF MEASUREMENT
G70 : Programming in inches
G71 : Programming in millimeters
Depending on whether G70 or G71 is programmed, the CNC takes the subsequent
coordinates as being in inches or millimeters respectively.
Functions G70/G71 are modal and incompatible with one another.
The CNC assumes the units set by parameter P13 when being turned on, after M02,M30,
EMERGENCY or RESET.