HEIDENHAIN TNC 620 User Manual page 255

Rounded corners G25
The G25 function rounds off contour corners.
The tool moves on an arc that is tangentially connected to both the
preceding and subsequent contour elements.
The rounding arc must be machinable with the called tool.
Rounding radius: Enter the radius, and if
necessary:
Feed F (effective only in the G25 block)
Example NC blocks
N50 G01 X+10 Y+40 G41 F300 M3*
N60 G01 X+40 Y+25*
N70 G25 R5 F100*
N80 G01 X+10 Y+5*
In the preceding and subsequent contour elements,
both coordinates must lie in the plane of the
rounding arc. If you machine the contour without
tool-radius compensation, you must program both
coordinates in the plane.
The corner point is cut off by the rounding arc and is
not part of the contour.
A feed rate programmed in the G25 block is effective
only in that G25 block. After the G25 block, the
previous feed rate becomes effective again.
You can also use an G25 block for a tangential
contour approach.
HEIDENHAIN | TNC 620 | ISO Programming User's Manual | 9/2016
Path contours  Cartesian coordinates
6
6.4
255