Programming instructions

3-20
Motion Commands, Dimension Inputs NC Programming 17VRS
DOK-MTC200-NC**PRO*V17-ANW1-EN-P
position. With circles the circle center points and end points are to be
stated as a difference in diameter relative to the starting point.
•
The thread lead is interpreted as a radius dimension when machining
face threads on a lathe.
•
Functions like constant surface speed and feed per revolution in the X
direction are not affected by diameter programming.
•
If position data are read into a NC-variable for the diameter axis, this is
the diameter value.
•
The zero offsets for the X axis are programmed in radius.
•
The tool corrections in the X axis are interpreted as radius values.
•
The diameter symbol
∅
is used in the position display to indicate the
axis in which diameter programming is active.
3.8 Dimensional Units
Upon setup, machine tools are specified for a certain basic programming
unit (mm or inches). To produce workpieces which are dimensioned in a
different dimensioning unit on this machine, the dimensional units can be
changed for coordinate values, speed values, and programmable offsets
by using Preparatory G-functions.
Note:
The basic unit to be used in programming is specified by the
machine builder in the process parameters.
Inch Programming Input 'G70'
If millimeters is set in the process parameters as the basic programming
unit, the subsequent values are interpreted as inch data and are con-
verted to inches internally after G70 has been programmed.
•
Motion commands (coordinate values); for example X5.5 inches is
converted to X139.7 mm.
•
Interpolation parameters I, J and K and radius R;
•
Feed data F and G95 F; for example, F20 inch/min is internally conver-
ted to F508 mm/min;
•
Programmed offsets G50, G51 and G52;
•
Motion commands assigned by means of NC-variables (X=@050),
interpolation parameters (I=@051), feedrate information (F=@052)
and programmable offsets (G50 X=@053).
G70 remains in effect until the end of the program or until it is overwritten
by G71.