Operator`s manual

Advanced Haas Mill Programming Techniques Training Manual Page 40
G68 can be used in the G17, G18 or G19 planes. G17, G18 or G19 must be called up in the program before
the G68 command or the default G17 will be used.
The format for G68: G17 G68 Annn Bnnn Rnnn
A and B describe the corresponding axis or center of rotation coordinates for the selected plane. For G17
Xnnn and Ynnn would be used, G18 Xnnn and Znnn, G19 Ynnn Znnn. If no coordinates are called out on the
G68 command line the axis of rotation will be at the current location of the machine.
R is the angle of rotation specified in degrees. Up to 3 decimals may be used. A positive R value indicates a
counterclockwise rotation. Clockwise rotation is directed by a negative R value. If no R is given the
machine defaults to the value given in setting #72.
Below shows the tool paths of the part on the previous page. The left figure shows the part run normally.
On the right the code G68 X-2. Y-.5 R10. has been inserted at the beginning of the program. The part zero is
the center of the part. The coordinates for the lower left hand corner are X-2. Y-.5. The tool path has been
altered so that it is rotated 10° counter clockwise. The axis of rotation is the lower left hand corner of the
part. Note the X and Y values in the G68 are not rotated.
When using cutter compensation the G41 or G42 commands should be turned on after the G68 rotation is
called up and turned off with G40 before the G68 is cancelled with a G69.