Circular Path C Around Circle Center Cc - HEIDENHAIN iTNC 530 User Manual

Circular path C around circle center CC

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
U
Move the tool to the circle starting point.
U Enter the coordinates of the circle center
U Coordinates of the arc end point, and if necessary:
3
U
Feed rate F
U 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, for example 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.
Input tolerance: up to 0.016 mm (selected with MP7431).
Smallest possible circle that the TNC can traverse:
0.0016 µm.
HEIDENHAIN iTNC 530 221