FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 94

21.AXIS CONTROL FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 708 - 

NOTE 

1  During axis synchronous control, a movement based 

on the reference position return check (G27), automatic 
reference position return (G28), 2nd/3rd/4th reference 
position return (G30), or machine coordinate system 
selection (G53) command is made as described below 
according to the setting of bit 7 (SRF) of parameter No. 
8304. 
<1>  When SRF = 0, the same movement as made 

along the master axis is made along the slave 
axis. 

<2>  When SRF = 1, a movement is made along the 

slave axis to the specified position independently 
of a movement made along the master axis to the 
specified position. 

2  A command not involving a movement along an axis 

such as the workpiece coordinate system setting 
command (G92) and local coordinate system setting 
command (G52) is set with the master axis according 
to the master axis programming. 

3  During synchronous operation, the axis-by-axis signals 

such as for external deceleration, interlock, and 
machine lock are enabled for the master axis only.   
During synchronous operation, those signals for the 
slave axis are ignored. 

4  When switching the synchronization state in a program, 

be sure to specify M codes (parameter No. 8337 and 
No. 8338) for turning synchronization on and off.    By 
switching between the input signals SYNCx <G138> 
and SYNCJx <G140> from the PMC with the M codes, 
the synchronization state can be switched in the 
program. 

5  When controlled axis removal is performed, the 

synchronization state is cancelled.    When performing 
controlled axis removal, perform removal for the master 
axis and slave axis at the same time. 

6  If a programmed command is specified for the slave 

axis during synchronous operation, an alarm PS0213 is 
issued. 

 

A programmed command can be specified for the slave 
axis when switching between synchronous operation 
and normal operation is set to 0 (with bit 5 (SCA) of 
parameter No. 8304 set to 0) to select normal 
operation. 

7  Axis synchronous control and PMC axis control cannot 

be used at the same time. 

B-63944EN/03

 PROGRAMMING 

21.AXIS CONTROL FUNCTIONS

 

 

- 709 - 

21.2 

POLYGON TURNING (G50.2, G51.2) 

 
Polygon turning means machining a workpiece to a polygonal figure 
by rotating the workpiece and tool at a certain ratio. 
 

Workpiece

Workpiece

Tool

 

Fig. 21.2 (a)    Polygon turning 

 
By changing conditions which are rotation ratio of workpiece and tool 
and number of cutters, the workpiece can be machined to a square or 
hexagon.  The machining time can be reduced as compared with 
polygonal figure machining using the polar coordinate interpolation.  
The machined figure, however, is not exactly polygonal.    Generally, 
polygon turning is used for the heads of square and/or hexagon bolts 
or hexagon nuts. 
As the tool rotary axis, one of the following can be used: 

•

 

CNC controlled axis (servo axis) 

•

 

Second spindle (Two serial spindles are connected.) 

Polygonal machining performed using a servo axis as the tool rotary 
axis is referred to as polygon turning.  Polygonal machining 
performed using the second spindle as the tool rotary axis is referred 
to as polygon turning with two spindles. 
 

Function name

 

Workpiece axis

 

Tool rotary axis

 

Polygon turning 

Spindle 
(Either an analog spindle or 
serial spindle is usable.   
However, a detector 
equivalent to a position 
coder is required.) 

Servo axis 

Polygon turning with 
two spindles 

Spindle 
(Serial spindle) 

Spindle 
(Serial spindle) 

 

21.AXIS CONTROL FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 710 - 

Explanation 

A CNC controlled axis (servo axis) is assigned to the tool rotary axis.     
This rotary axis of tool is called Y-axis in the following description.   
As the workpiece axis (spindle), either a serial spindle or analog 
spindle can be used. 
The Y-axis is controlled by the G51.2 command, so that the ratio of 
the rotation speeds of the spindle (previously specified by 
S-command) and the tool becomes the specified ratio. 
When simultaneous start is specified by G51.2, the one-rotation signal 
sent from the position codes set on the spindle is detected.  After 
one-rotation signal detection, the Y-axis is controlled using the 
rotation ratio of the spindle and Y-axis specified by P and Q.    So, a 
position coder needs to be attached to the spindle.    This control will 
be maintained until the polygon turning cancel command is executed 
(G50.2).  Polygon turning is cancelled by any of the following in 
addition to the G50.2 command: 
(1) Power 

off 

(2) Emergency 

stop 

(3) Servo 

alarm 

(4)  Reset (external reset signal ERS, reset/rewind signal RRW, and 

RESET key on the MDI panel) 

(5)  Occurrence of alarms PS0217 to PS0221, PS0314, and PS05018 
 

NOTE 

1  Before polygon turning, reference position return 

operation on the Y-axis needs to be specified to 
determine the rotation start position of the tool.   
This reference position return operation is 
performed by detecting a deceleration limit as in the 
case of manual reference position return operation.   
(By setting bit 7 (PLZ) of parameter No. 7600, 
reference position return operation can be 
performed without detecting a deceleration limit.) 

2  The rotation direction on the Y-axis is determined 

by the sign of Q, and is not affected by the rotation 
direction of the position coder. 

3  Among Y-axis position indications, the indication of 

a machine coordinate (MACHINE) changes within 
the amount of movement for 0 to 1 revolution as a 
movement is made on the Y-axis.    The absolute 
coordinate and relative coordinate are not updated.   
So, when specifying an absolute-position command 
for the Y-axis after polygon turning mode 
cancellation, set a workpiece coordinate system 
after reference position return operation. 

B-63944EN/03

 PROGRAMMING 

21.AXIS CONTROL FUNCTIONS

 

 

- 711 - 

 

NOTE 

4  For the Y-axis engaged in polygon turning, jog feed 

and handle feed are disabled. 

5  For the Y-axis not engaged in polygon turning, a 

move command can be specified as in the case of 
other controlled axes. 

6  The Y-axis engaged in polygon turning is not 

counted in the number of simultaneously controlled 
axes. 

7  One workpiece must be machined using a fixed 

spindle speed until the workpiece is finished. 

8  Polygon turning with two spindles cannot be used at 

the same time. 

9  G50.2 is the G code for suppressing buffering. 

 

 CAUTION 

1  During polygon turning, threading cannot be 

performed. 

2  For the Y-axis engaged in synchronous operation, 

the signals below are valid or invalid: 
Signals valid for the Y-axis 

•

 Machine lock 

•

 Servo-off 

Signals invalid for the Y-axis 

•

 Feed hold 

•

 Interlock 

•

 Override 

•

 Dry run 

(At dry run time, however, the one-rotation 
signal is not awaited in a G51.2 block.) 

 

21.AXIS CONTROL FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 712 - 

Format 

G50.2 

Polygon turning cancel

 

 

G51.2  P_ Q_ ;

 

P,Q: Rotation ratio of spindle and Y-axis 
Specify range: 
P:    Integer from 1 to 999 
Q:    Integer from -999 to -1 or from 1 to 999 
 

When Q is a positive value, Y-axis makes positive 
rotation. 

 

When Q is a negative value, Y-axis makes 
negative rotation. 

 

NOTE 

 

Specify G50.2 and G51.2 in a single block. 

 

Example 

G00 X100. 0 Z20.0 S1000.0 M03 ; 
 

(Workpiece rotation speed 1000 (min

-1

))

 

G51.2 P1 Q2 ; 

(Tool rotation start (tool rotation speed 
2000 (min

-1

))

 

G01 X80.0 F10.0 ; 

(X-axis infeed)

 

G04 X2.0 ; 

(Waiting 2 seconds)

 

G00 X100.0 ; 

(X-axis escape)

 

G50.2 ; 

(Tool rotation stop)

 

M05 S0 ; 

(Spindle stop )

 

 

  - Principle of polygon turning   

The principle of polygon turning is explained below.  In the figure 
below the radius of tool and workpiece are A and B, and the angular 
speeds of tool and workpiece are 

α

 and 

β

.  The origin of XY 

Cartesian coordinates is assumed to be the center of the workpiece. 
Simplifying the explanation, consider that the tool center exists at the 
position 
P

o

 (A, 0) on the workpiece periphery, and the tool nose starts from 

position P

to

 (A-B, 0). 

 

B-63944EN/03

 PROGRAMMING 

21.AXIS CONTROL FUNCTIONS

 

 

- 713 - 

Y 

X

A

(0,0)

P

to

P

o

 

B 

Angular speed 

α

A : Workpiece radius 

B : Rool radius 

Angular 

speed 

β

 

Workpiece 

Tool

α

 : Workpiece angular speed

β

 : Tool angular speed 

Po  (A, 0)

Pto (A-B, 0)

 

Fig. 21.2 (b)    Principle of polygon turning 

 

(0, 0)

α

t

β

t

A

P

Start point

B

Pt (Xt, Yt)

 

Fig. 21.2 (c)    Tool nose position   

 
In this case, the tool nose position Pt (Xt, Yt) after time t is expressed 
by equations 1 and 2: 
 

Xt

=

A

cos

α

t

-

B

cos(

β

-

α

)

t

 (Equation 

1) 

 

Yt

=

A

sin

α

t

+

B

sin(

β

-

α

)

t

 (Equation 

2) 

Assuming that the rotation ration of workpiece to tool is 1:2, namely, 

β

=2

α

, equations 1 and 2 are modified as follows: 

 

Xt

=

A

cos

α

t

-Bcos

α

t

=(

A-B

)cos

α

t

 (Equation 

1)' 

 

Xt

=

A

sin

α

t

+Bsin

α

t

=(

A+B

)sin

α

t

 (Equation 

2)' 

These equations indicate that the tool nose path draws an ellipse with 
longer diameter A+B and shorter diameter A-B. 
Then consider the case when one tool is set at 180

°

 symmetrical 

positions, for a total of two.    A square can be machined with these 
tools as shown below. 
 

21.AXIS CONTROL FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 714 - 

 

 
If three tools are set at every 120

°

, the machining figure will be a 

hexagon as shown below. 
 

 

 

 WARNING 

 

For the maximum rotation speed of the tool, see 
the instruction manual supplied with the machine.   
Do not specify a spindle speed higher than the 
maximum tool speed or a ratio to the spindle speed 
that results in a speed higher than the maximum 
tool speed. 

 

B-63944EN/03

 PROGRAMMING 

21.AXIS CONTROL FUNCTIONS

 

 

- 715 - 

21.3 

SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED 
CONTROL BY PROGRAM COMMAND (G50.4, G51.4, 
G50.5, G51.5, G50.6, AND G51.6) 

 
Synchronous control, composite control, and superimposed control 
can be started or canceled using a program command instead of a DI 
signal. Synchronous control, composite control, and superimposed 
control based on a DI signal is also possible. 
 
For the basic operations of synchronous control, composite control, 
and superimposed control, see Section 8.5, "SYNCHRONOUS 
CONTROL AND COMPOSITE CONTROL", and Section 8.6, 
"SUPERIMPOSED CONTROL" in the CONNECTION MANUAL 
(FUNCTION) (B-63943EN-1). 
 

Format 

G51.4    P_ Q_    (L_) ;  Synchronous control start (L is omissible.)
G50.4    Q_ ; 

Synchronous control cancel 

 

P:  Synchronous master axis ID number 
Q:  Synchronous slave axis ID number 
 
L: Parking 

command 

 

1: Master parking (slave parking cancel) 

 

2: Slave parking (master parking cancel) 

 

0: No parking (parking cancel) 

 

(When L is omitted, the specification of L0 is assumed.) 

 

G51.5    P_ Q_ ; 

Composite control start 

G50.5    P_ Q_ ; 

Composite control cancel 

 

P:  Composite axis 1 ID number 
Q:  Composite axis 2 ID number 

 

G51.6    P_ Q_ ; 

Superimposed control start 

G50.6    Q_ ; 

Superimposed control cancel 

 

P:  Superimposed master axis ID number 
Q:  Superimposed slave axis ID number 
 
As an ID number, set a unique value for identifying each axis in parameter 
No. 12600 for both of P and Q. 

 
G51.4/G50.4, G51.5/G50.5, and G51.6/G50.6 are one-shot G codes of 
group 00.