HEIDENHAIN TNC 620 User Manual page 257

Circular path around circle center
Before programming a circular arc, you must first enter the circle
center I, J. The last programmed tool position will be the starting
point of the arc.
Direction of rotation
In clockwise direction: G02
In counterclockwise direction: G03
Without programmed direction: G05. The TNC traverses the
circular arc with the last programmed direction of rotation
Move the tool to the circle starting point
Enter the coordinates of the circle center
Enter the coordinates of the arc end point, and if
necessary:
Feed F
Miscellaneous function M
The TNC normally makes circular movements in the
active working plane. If you program circular arcs that
do not lie in the active working plane, e.g. G2 Z...
X... with a tool axis Z, and at the same time rotate
this movement, then the TNC moves the tool in a
spatial arc, which means a circular arc in 3 axes.
Example NC blocks
N50 I+25 J+25*
N60 G01 G42 X+45 Y+25 F200 M3*
N70 G03 X+45 Y+25*
Full circle
For the end point, enter the same point that you used for the
starting point.
The starting and end points of the arc must lie on the
circle.
The maximum value for input tolerance is 0.016 mm.
Set the input tolerance in the machine parameter
circleDeviation (no. 200901).
Smallest possible circle that the TNC can traverse:
0.0016 µm.
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Path contours  Cartesian coordinates
6
6.4
257