FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 113

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 860 - 

The "output angle" is explained below using a tool rotation type 
machine as an example. 
This example illustrates a machine having a "BC type tool axis Z." 
 

•

    BC type tool axis Z

X

Y

Z

C-axis:

First rotation axis
(master)

B-axis: Second rotation axis

(slave)

 

Fig. 22.3 (o)    BC type tool axis Z 

 
The following two pairs of "computed basic angles" exist that direct 
the tool axis toward the +X-axis direction. 
(B 90 degrees; C 180 degrees) 
(B 270 degrees; C 0 degree) 
 
<1>  When the current rotary axis angles are (B -70 degrees; C 30 

degrees) 

 

The "output angles" are (B -90 degrees; C 0 degree). 
  0 degree is adopted because it is nearer to the current 

position (30 degrees) of the C-axis that is the master axis.  
For the B-axis, 270 degrees is adopted which is the same 
group.  However, this is changed to -90 degrees (270 
degrees - 360 degrees) which is the nearest to the current 
position of the B-axis (-70 degrees). 

<2>  When the current rotary axis angles are (B 80 degrees; C 500 

degrees) 

 

The "output angles" are (B 90 degrees; C 540 degrees). 
  540 degrees (180 degrees 

+

 360 degrees) is adopted because 

it is nearer to the current position (500 degrees) of the C-axis 
that is the master axis.  For the B-axis, 90 degrees is 
adopted which is the same group. 

<3>  When the current rotary axis angles are (B 60 degrees; C 90 

degrees) 

 

The "output angles" are (B 90 degrees; C 180 degrees). 
  Since the two candidates are equally near to the current 

position (90 degrees) of the C-axis that is the master axis, a 
judgment is made based on the current position of the B-axis.   
90 degrees is adopted because it is nearer to the current 
position (60 degrees) of the B-axis that is the slave axis.  
For the C-axis, 180 degrees is adopted which is the same 
group. 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 861 - 

<4>  When the current rotary axis angles are (B 180 degrees; C 90 

degrees)  

 

The "output angles" are (B 270 degrees; C 0 degree). 
  Since the two candidates are equally near to the current 

position (90 degrees) of the C-axis that is the master axis, a 
judgment is made based on the current position of the B-axis.   
In this case, however, the two candidates are also equally 
near to the current position of the B-axis (180 degrees).  
Therefore, the candidate is adopted in which the C-axis 
(master axis) is nearer to 0 degree. 

  That is, the pair is adopted whose C-axis angle is 0 degree 

and whose B-axis angle is 270 degrees. 

 
When the slave axis angle is 0 degree, the direction of the tool axis 
becomes fixed regardless of the master axis angle. 
In that case, the master axis does not move from the current angle. 
 
An explanation is shown below using a machine having a "BC type 
tool axis Z" as an example. 
 

•

    BC type tool axis Z

X

Y

Z

C

   

Fig. 22.3 (p)    BC type tool axis Z 

 
When the current rotary axis angles are (B 45 degrees; C 90 degrees), 
the "output angles" are (B 0 degree; C 90 degrees). 
 

  - Specification for rotary axes 

The tilted working plane command assumes that positioning of a 
rotary axis is performed by tool axis direction control (G53.1) and 
then machining is performed without the rotary axis being moved. 
When movement is made with the rotary axis specified directly, the 
movement of the rotary axis is not considered in the movement of the 
linear axis.    Do not specify the movement of the rotary axis during 
execution of the tilted working plane command to ensure correct 
machining. 
 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 862 - 

22.3.2 

Tilted Working Plane Command by Tool Axis Direction 

 

Overview 

By specifying G68.3, a coordinate system (feature coordinate system) 
where the tool axis direction is the +Z-axis direction can be 
automatically specified.    When a feature coordinate system is used, a 
program for cutting a hole or pocket in a plane tilted relative to the 
workpiece coordinate system can be made simpler. 
This function can automatically generate a feature coordinate system 
that is normal to the tool direction. 
 

 

Feature coordinate system (G68.3)

Machine coordinate system

Workpiece coordinate system (G54)

Yc

Zc 

Xc

 

Feature coordinate system 

 
When G68.3 is specified in a block, the coordinate system for 
programming is changed to a feature coordinate system.  All 
commands after the block are regarded as commands in the feature 
coordinate system until G69 is specified. 
 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 863 - 

Format 

 

Format

 

G68.3 X x

0

 Y y

0

 Z z

0   

R

α

 ;  Tilted working plane command 

 
G69 ; 

Cancel tilted working plane command (M series).

G69.1;  Cancel tilted working plane command (T series).

Explanation of symbols 

X,Y,Z  : Origin of a feature coordinate system (absolute) 
 

  By default, the current position is used as the origin of the 

feature coordinate system. 

R 

: Angular displacement about the Z-axis in the feature 

coordinate system. 

 

  The default is 0°. 

 

 

Coordinate system 
origin shift (xo,yo,zo) 

Workpiece 
coordinate 
system X-Y-Z

Feature coordinate 
system Xc-Yc-Zc 

α

 

X

Y

Z

Zc

Yc 

Xc

 

G68.3 command 

 

Explanation 
  - Feature coordinate system 

By specifying G68.3, a feature coordinate system with the tool axis 
direction being the +Z-axis direction can be created.  The tool axis 
direction means the tool axis direction based on the rotation axis 
position reached by automatic operation or manual operation. 
 

  - Origin of a feature coordinate system 

The origin of a feature coordinate system must be specified using an 
absolute command. 
Even in the incremental command mode, the specified origin is 
regarded as an absolute position. 
When 1 address or 2 addresses are omitted in X, Y, Z, alarm PS5457 
is issued. 
When the origin of a feature coordinate system is not specified, the 
position when G68.3 is specified is used as the origin. 
 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 864 - 

  - Determination of a feature coordinate system 

When G68.3 is specified, the tool axis direction vector (

T

) represents 

the +Z direction (

Zc

) of the feature coordinate system. 

The vector normal to a plane formed by the +Z direction (

Zc

) of the 

feature coordinate system and the vertical axis direction vector (

P

) 

(parameter No. 12321) represents the +X direction (

Xc

) of the 

feature coordinate system. 
Expression:  

Zc

P

Xc

×

=

 

The vector normal to the +Z direction (

Zc

) of the feature coordinate 

system and the +X direction (

Xc

) of the feature coordinate system 

represents the +Y direction (

Yc

) of the feature coordinate system. 

Expression:  

Xc

Zc

Yc

×

=

 

When R is commanded, a coordinate system rotated by R around Zc 
from the above-mentioned coordinate system is the feature coordinate 
system. 
 

 
 
 
 

X-axis of feature coordinate 
system 

  Y-axis of feature 
 coordinate system 

Vertical axis direction:    P 

Z-axis of feature coordinate 
system (Tool axis direction: 
T) 

Xc 

Yc

Zc 

 

Determination of a feature coordinate system 

 
When the tool axis direction vector (

T

) is parallel with the vertical 

axis direction vector (

P

) (parameter No. 12321) (when the angle 

between the vector (

T

) and the vector (

P

) is equal to or less than the 

value of parameter No. 12322), the feature coordinate system 
Xc-Yc-Zc is as indicated below.    By specifying angular displacement 
R, a feature coordinate system rotated about the Z-axis of this 
coordinate system can be specified. 
 

Parameter 

No. 12321 

Z-axis of feature 

coordinate system

Zc 

X-axis of feature 

coordinate system 

Xc 

Y-axis of feature 

coordinate system 

Yc 

1 

+X direction 

+Y direction 

+Z direction 

2 

+Y direction 

+Z direction 

+X direction 

3 

+Z direction 

+X direction 

+Y direction 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 865 - 

 
When 0 is set in parameter No. 12321, the vertical axis direction is the 
reference tool axis direction (parameter No. 19697). 
If a value other than 0 through 3 is set in parameter No. 12321, the 
PS5459 alarm is issued. 
 

 CAUTION 

 

Tool axis direction is Z-axis direction of feature 
coordinate system regardless of the reference tool 
axis direction (parameter No. 19697). 

 

  - Angular displacement R 

Angular displacement R is positive when a rotation is made clockwise 
viewed in the Z-axis direction of the feature coordinate system.    The 
range of angular displacement R is:    0.0

°

 

≤

 R 

≤

 360.0

°

. 

 

  - Machine of table rotation type 

On a machine of table rotation type, the tool direction remains 
unchanged.    So, a feature coordinate system based on the reference 
tool axis direction (parameter No. 19697) is set.    However, the origin 
specification of the feature coordinate system and angular 
displacement R about the Z-axis are valid. 

 

Workpiece coordinate system X-Y-Z

Example:  When reference tool axis direction represents +Z-axis 

direction (with 3 set in parameter No. 19697) 

Feature coordinate system
Xc-Yc-Zc 

X 

Y 

Z 

Xc 

Yc 

Zc

 

 

  - Use in combination with tool length compensation 

The G68.3 command can be specified even during tool length 
compensation. 
 

NOTE 

 

Do not specify G68.3 during workpiece setting 
error compensation.    Otherwise, alarm PS0437 is 
issued. 

 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 866 - 

  - Example of operation 

An example of operation on a machine of tool rotation type is given 
below. 
The machine configuration is "BC type reference tool axis Z-axis". 

 

B:  2nd rotation axis (slave)

C:    1st rotation axis (master)

 

Control point 

Tool holder offset value 
  = Parameter No. 19666 

Tool length offset = H01

 

BC type tool axis Z-axis

 

(Axes are intersecting.) 

Tool center point

 

 

Sample program 1 

O0100 ; 
N1 G55 ; 
N2 G90 G01 X0Y0Z50.0 F1000 ; 
N3 G43 H01 X0 Y0 Z0 ; 
N4 B-45.0 ; 
N5 G68.3 ; 

: 

N6 G69 ; 

: 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 867 - 

 

 

 

 

 

 

 

 

 

 

 

Xc

Yc 

Zc

X 

Y

Z

X 

Y

Z

X 

Y

Z

Machine operation by sample program 1

N3 command

N6 command

N5 command

N4 command

Workpiece coorditate system
X-Y-Z 

Workpiece coordinate system
X-Y-Z 

Feature coordinate system Xc-Yc-Zc 

 

 

N3 block: Performs tool length compensation in the workpiece 

coordinate system. 

 

The tool center point moves to the origin of the workpiece 
coordinate system. 

N4 block:  Tilts the tool. 
N5 block: Sets a feature coordinate system where the tool axis 

direction is the Z-axis direction and the tool center point is 
placed at the origin. 

N6 block: Cancels the feature coordinate system to return to the 

workpiece coordinate system.