G68 Rotation (Group 16)

Next Generation Control Mill Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue
note: You must purchase the Rotation and Scaling option to use this G-code. A 200-hour option tryout is also available; refer to NGC - Option Tryout for instructions.
*G17, G18, G19 - Plane of rotation, default is current
*X/Y, X/Z, Y/Z - Center of rotation coordinates on the selected plane**
*R - Angle of rotation, in degrees. Three-place decimal, -360.000 to 360.000.

*indicates optional

**The axis designation you use for these address codes corresponds to the axes of the current plane. For example, in the G17 (XY plane), you would use X and Y to specify the center of rotation.

When you command a G68, the control rotates all X, Y, Z, I, J, and K values about a center of rotation to a specified angle (R),.

You can designate a plane with G17, G18, or G19 before G68 to establish the axis plane to rotate. For example:

G17 G68 Xnnn Ynnn Rnnn ;

If you do not designate a plane in the G68 block, the control uses the currently active plane.

The control always uses a center of rotation to determine the positional values after rotation. If you do not specify a center of rotation, the control uses the current location.

G68 affects all appropriate positional values in the blocks after the G68 command. Values in the line that contains the G68 command are not rotated. Only the values in the plane of rotation are rotated; therefore, if G17 is the current plane of rotation, the command affects only the X and Y values.

A positive number (angle) in the R address rotates the feature counterclockwise.

If you do not specify the angle of rotation (R), then the control uses the value in Setting 72.

In G91 mode (incremental) with Setting 73 ON, the rotation angle changes by the value in R. In other words, each G68 command changes the rotation angle by the value specified in R.

The rotational angle is set to zero at the beginning of the program, or you can set it to a specific angle with G68 in G90 mode.

These examples illustrate rotation with G68. The first program defines a Gothic window shape to cut. The rest of the programs use this program as a subprogram.

G68 Start Gothic Window, No rotation: [1] Work coordinate origin.

% O60681 (GOTHIC WINDOW SUBPROGRAM) ; F20 S500 (SET FEED AND SPINDLE SPEED) ; G00 X1. Y1. (RAPID TO LOWER-LEFT WINDOW CORNER) ; G01 X2. (BOTTOM OF WINDOW) ; Y2. (RIGHT SIDE OF WINDOW); G03 X1. R0.5 (TOP OF WINDOW) ; G01 Y1. (FINISH WINDOW) ; M99; &

The first example illustrates how the control uses the current work coordinate location as a rotation center (X0 Y0 Z0).

G68 Rotation Current Work Coordinate: [1] Work coordinate origin and center of rotation.

O60682 (ROTATE ABOUT WORK COORDINATE) ; G59 (OFFSET) ; G00 G90 X0 Y0 Z-0.1 (WORK COORDINATE ORIGIN) ; M98 P60681 (CALL SUBPROGRAM) ; G90 G00 X0 Y0 (LAST COMMANDED POSITION) ; G68 R60. (ROTATE 60 DEGREES) ; M98 P60681 (CALL SUBPROGRAM) ; G69 G90 X0 Y0 (CANCEL G68) ; M30 %

The next example specifies the center of the window as the rotation center.

G68 Rotation Center of Window: [1] Work coordinate origin, [2] Center of rotation.

% O60683 (ROTATE ABOUT CENTER OF WINDOW) ; G59 (OFFSET) ; G00 G90 X0 Y0 Z-0.1 (WORK COORDINATE ORIGIN) ; G68 X1.5 Y1.5 R60. ; (ROTATE SHAPE 60 DEGREES ABOUT CENTER) ; M98 P60681 (CALL SUBPROGRAM) ; G69 G90 G00 X0 Y0 ; (CANCEL G68, LAST COMMANDED POSITION) ; M30 ; %

This next example shows how the G91 mode can be used to rotate patterns about a center. This is often useful for making parts that are symmetric about a given point.

G68 Rotate Patterns About Center: [1] Work coordinate origin and center of rotation.

% O60684 (ROTATE PATTERN ABOUT CENTER) ; G59 (OFFSET) ; G00 G90 X0 Y0 Z-0.1 (WORK COORDINATE ORIGIN) ; M98 P1000 L6 (CALL SUBPROGRAM, LOOP 6 TIMES) ; M30 (END AFTER SUBPROGRAM LOOP) ; N1000 (BEGIN LOCAL SUBPROGRAM) ; G91 G68 R60. (ROTATE 60 DEGREES) ; G90 M98 P60681 (CALL WINDOW SUBPROGRAM) ; G90 G00 X0 Y0 (LAST COMMANDED POSITION) ; M99; %

Do not change the plane of rotation while G68 is in effect.

Rotation with Scaling:

If you use scaling and rotation at the same time, you should turn on scaling before rotation, and use separate blocks. Use this template:

% G51 ... (SCALING) ; ... ; G68 ... (ROTATION) ; ... program ; G69 ... (ROTATION OFF) ; ... ; G50 ... (SCALING OFF) ; %

Rotation with Cutter Compensation:

Turn on cutter compensation after the rotation command. Turn off cutter compensation before you turn off rotation.

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback