FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 107

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 812 - 

  - In the case of a composite type machine 

Explanations are given below assuming a composite type machine 
configuration that has one table rotation axis (which turns around the 
X-axis) and one tool rotation axis (which turns around the Y-axis).  
(See Fig. 22.1 (l).) 
 
If linear interpolation is specified for the X-, Y-, and Z-axes on the 
programming coordinate system and if the rotary axis that moves the 
rotation table and the tool rotation axis are specified (in the case of 
type 1) or the tool direction is specified (in the case of type 2), control 
is exerted in such a way that the tool center point moves along a 
specified straight line with respect to the table (workpiece) as the 
rotation table and tool rotate. 
Also, speed control is exerted so that the tool center point moves at the 
specified speed with respect to the table (workpiece). 
 
Example) 
When type 1 is selected and the coordinate system fixed on the table is 
used as the programming coordinate system 
(Bit 5 (WKP) of parameter No.19696 = 0): 

O300 (Sample Program3) ; 
N1 G00 G90 A0 B0 ; 
N2 G55 ; 

Prepares the programming coordinate 
system. 

N3 G43.4 H01 ; 

Starts tool center point control. 

 

  H01 is the tool compensation number. 

N4 G00 X200.0 Y150.0 Z20.0 ;  Moves to the start point. 
N5 G01 X5.0 Y5.0 Z5.0 A60.0 B45.0 F500; 
  

Linear 

interpolation 

N6 G49 ; 

Cancels tool center point control. 

N7 M30; 

 
When type 1 is selected and the workpiece coordinate system is used 
as the programming coordinate system 
(Bit 5 (WKP) of parameter No.19696 = 1): 

O300 (Sample Program3) ; 
N1 G00 G90 A0 B0 ; 
N2 G55 ; 

Prepares the programming coordinate 
system. 

N3 G43.4 H01 ; 

Starts tool center point control. 

 

 

H01 is the tool compensation number. 

N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point. 
N5 G01 X5.0 Y48.170 Z-79.772 A60.0 B45.0 F500; 
  

   

Linear 

interpolation 

N6 G49 ; 

Cancels tool center point control. 

N7 M30; 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 813 - 

For type 2 (when the coordinate system fixed on the table is used as 
the programming coordinate system (only when bit 5 (WKP) of 
parameter No.19696 is set to 0)): 

O300 (Sample Program3) ; 
N1 G00 G90 A0 B0 ; 
N2 G55 ; 

Prepares the programming coordinate 
system. 

N3 G43.5 H01 ; 

Starts tool center point control. 

 

 

H01 is the tool compensation number. 

N4 G00 X200.0 Y150.0 Z20.0 ; Moves to the start point. 
N5 G01 X5.0 Y5.0 Z5.0 I2.0 J1.732 K1.0 F500;   
  

Linear 

interpolation 

N6 G49 ; 

Cancels tool center point control. 

N7 M30; 

 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 814 - 

X'

Y'

Z'

B

A

X'

Y'

Z'

X'

Y'

Z'

X'

Z'

Y'

X'

Z'

Y'

X'

Z'

Y'

Control point path (of the

machine coordinate system)

Tool center point path seen from the table-fixed coordinate system

Tool center point path taken when
the programming coordinate
system does not move

Z"

Y

X

Z"

Y

X

Z"

Y

X

 

Fig. 22.1 (l)    Example for a composite type machine 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 815 - 

  - When linear interpolation is performed during tool center point control 

Examples are given below in which

 

each 100-mm-long side of an 

equilateral triangle is cut at B-axis angles of 0, 30 to 60, and 60 
degrees, respectively. 

 

Example) 
When type 1 is selected and the table-fixed coordinate system is used 
as the programming coordinate system: 

O400 (Sample Program4) ; 
N10 G55 ;   

 

Prepares the programming 
coordinate system. 

N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; 

Moves to the initial position. 

N30 G01 G43.4 H01 Z20.0 F500. ; 

Starts tool center point control. 

 

   

 

 

Moves to the approaching 
position. 

 

   

 

 

H01 is the tool compensation 
number. 

N40 X28.868 Y-50.0 Z10.0 B30.0 ; 

The Z-axis height on the 
machining plane is 10.0. 

N50 Y50.0 ; 
N60 B45.0 C120.0 ; 
N70 X-57.735 Y0 B60.0 C180.0 ; 

Moves X and Y while operating 
both B- and C-axes. 

N80 C240.0 ; 
N90 X28.868 Y-50.0 ; 
N100 X50.0 Y-70.0 Z20.0 B0 C360.0 ; 

X, Y, and Z are approaching 
positions. 

 

   

 

 

The rotary axes move to their 
original positions. 

N110 G49 Z300.0 ; 

Cancels tool center point 
control. 

 

   

 

 

Moves the Z-axis to its initial 
position. 

N120 M30; 

 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 816 - 

When type 1 is selected and the workpiece coordinate system is used 
as the programming coordinate system 
(Note that the values of N60 to N90 are different from those specified 
in the preceding example.): 

O400 (Sample Program4) ; 
N10 G55 ;   

 

Prepares the programming 
coordinate system. 

N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; 

Moves to the initial position. 

N30 G01 G43.4 H01 Z20.0 F500. ; 

Starts tool center point control. 

 

   

 

 

Moves to the approaching 
position. 

 

   

 

 

H01 is the tool compensation 
number. 

N40 X28.868 Y-50.0 Z10.0 B30.0 ; 

The Z-axis height on the 
machining plane is 10.0. 

N50 Y50.0 ; 
N60 Y-50.0 B45.0 C120.0 ; 
N70 X57.735 Y0 B60.0 C180.0 ; 

Moves X and Y while operating 
both B- and C-axes. 

N80 X28.868 Y-50.0 C240.0 ; 
N90 Y50.0 ; 
N100 X50.0 Y-70.0 Z20.0 B0 C360.0 ; 

X, Y, and Z are approaching 
positions. 

 

   

 

 

The rotary axes move to their 
original positions. 

N110 G49 Z300.0 ; 

Cancels tool center point 
control. 

 

   

 

 

Moves the Z-axis to its initial 
position. 

N120 M30; 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 817 - 

When type 2 is selected and the table-fixed coordinate system is used 
as the programming coordinate system: 

O400 (Sample Program4) ; 
N10 G55 ;   

 

Prepares the programming 
coordinate system. 

N20 G90 X50.0 Y-70.0 Z300.0 B0 C0 ; 

Moves to the initial position. 

N30 G01 G43.5 H01 Z20.0 F500. ; 

Starts tool center point control. 

 

   

 

 

Moves to the approaching 
position. 

 

   

 

 

H01 is the tool compensation 
number. 

N40 X28.868 Y-50.0 Z10.0 I1.0 K1.732 ;  The Z-axis height on the 

machining plane is 10.0. 

N50 Y50.0 ; 
N60 I-0.5 J0.866 K1.0 ; 
N70 X-57.735 Y0 I-1.732 K1.0 ; 

Moves X and Y while operating 
both B- and C-axes. 

N80 I-0.866 J1.5 K1.0 ; 
N90 X28.868 Y-50.0 ; 
N100 X50.0 Y-70.0 Z20.0 K1.0 ; 

X, Y, and Z are approaching 
positions. 

 

   

 

 

The rotary axes move to their 
original positions. 

N110 G49 Z300.0 ; 

Cancels tool center point 
control. 

 

   

 

 

Moves the Z-axis to its initial 
position. 

N120 M30; 

 

C

G55 workpiece coordinate system

Center of the B-axis 
rotation 

X

Z

Y

B

Center of the   
C-axis rotation 

 

•

  Composite type machine (tool rotation axis = B-axis; table rotation 

axis = C-axis; tool axis = Z direction) 

 

Machine configuration for the example 

 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 818 - 

The following figure illustrates the position of the workpiece, as well 
as the position of the tool head (relative to the workpiece), as seen 
from the table-fixed programming coordinate system in the +Z 
direction. 
 

•

    Behavior as seen from the table-fixed programming coordinate system

(X -57.735, Y 0)

(B 30.0)

(B 30.0)

(B 45.0)

(B 60.0)

(B 60.0)

(B 60.0)

(C 0)

(C 120.0)

(C 240.0)

(X 28.868, Y 50.0)

(X 28.868, Y -50.0)

X'

Y'

Illustration of the example (1) 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 819 - 

•

    Detailed diagram of each block

Y"

X"

(C 0)

(B 30.0)

(B 0)

Behavior of the tool
center point

Behavior of the control point
(machine coordinate value)

(B 30.0)

C-axis rotates, with C
being 120 degrees.

(B 45.0)

(C 0)

(C 120.0)

(B 30.0)

B-axis rotates, with
B being 45 degrees.

N60 block

N70 block

(C 120.0)

(B 45.0)

(B 60.0)

C-axis rotates, with C
being 180 degress.

(C 180.0)

Y"

X"

Y"

X"

X'

Y'

X'

Y'

X'

Y'

 

Detailed diagram of each block (1)