FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 33

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 220 - 

NOTE 

1  When operating an input signal by using an M 

code, for example, during automatic operation, 
perform a switching operation according to the 
method below to reflect the state of diameter/radius 
specification switching in the execution block 
correctly. 
As an auxiliary function for switching, use an 
unbuffered M code (parameter No. 3411 and up).   
Use the following sequences for a specified M 
code: 

-  When switching is performed 

Ｍ

 code 

→

 Input signal ON 

→

 Confirmation of 

output signal ON 

→

 FIN 

-  When switching is cancelled   

Ｍ

 code 

→

 Input signal OFF 

→

 Confirmation of 

output signal OFF 

→

 FIN 

 

If a diameter/radius specification switch signal is 
operated during automatic operation without 
following the sequences above, alarm PS5320 is 
issued. 

2  If a diameter/radius specification switch signal is 

operated while a movement is made on an axis 
subject to switching, alarm PS5320 is issued. 

 

  - Switching method using a G code (programmable diameter/radius specification 

switching) 

The format of a G code for diameter/radius specification switching is 
as follows: 

    Format 

G10.9 

IP

_ ; 

IP

_ :  Address and command value of an specified axis 

subject to diameter/radius specification switching 
Specify 0 or 1 as the command value. 
0:  Radius specification  
1:  Diameter specification 

 

NOTE 

1  Specify G10.9 in a single block specifying no other 

codes. 

2  After an axis address, specify a command value 

without using the decimal point. 

 

B-63944EN/03

 PROGRAMMING 

8.COORDINATE VALUE AND DIMENSION

 

 

- 221 - 

 - Switching operation 

According to the switching methods above, diameter/radius 
specification is internally switched as described below. 
 
1)    Switching using a signal 

•

  When parameter DIAx = 0 (radius specification) 

→

 

Operation is performed with diameter specification. 

•

  When parameter DIAx = 1 (diameter specification) 

→

 

Operation is performed with radius specification. 

 
2)    Switching using a G code 

•

 

When the specified address value = 0 (radius specification) 

→

 Operation is performed with radius specification. 

•

  When the specified address value = 1 (diameter 

specification) 

→

 Operation is performed with diameter 

specification. 

 

NOTE 

1  When the diameter/radius specification switching 

state is to be cancelled using a reset or mode 
switching at the time of signal-based switching, the 
input signal needs to be operated. 

2  Switching using a G code is cancelled by a reset. 

 

 CAUTION 

 

When switching is performed from diameter 
specification to radius specification, the travel 
distance based on the same move command is 
doubled when compared with diameter 
specification.  So, when switching from diameter 
specification to radius specification, ensure safety 
in machine operation. 

 

  - Selecting the machine coordinate system 

When diameter and radius setting switching is taking place as directed 
with the diameter and radius setting switching function, the 
coordinates specified by a machine coordinate system select command 
(G53) vary depending on the value of bit 7 (PDM) of parameter No. 
11222.  If the parameter PDM is 0, diameter and radius switching 
occurs.    If the parameter PDM is 1, the coordinates vary according to 
the value of bit 3 (DIAx) of parameter No. 1006. 
 

Limitation 
 - Feedrate 

A radius-based feedrate is specified in both of diameter specification 
and radius specification at all times. 
 

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 222 - 

  - Data not switchable 

The following data follows the setting of parameter DIAx, so that 
diameter and radius switching is not performed: 

•

 Parameter 

•

 Offset 

•

 

Workpiece coordinate system 

•

 

Scale display on the graphic screen 

 

NOTE 

 

For offset data, the settings of bit 1 (ORC) of 
parameter No. 5004 and bit 2 (ODI) of parameter 
No. 5004 have priority. 

 

  - Switchable data and commands 

For the following data and commands, diameter and radius switching 
is performed according to the specified specification method: 

•

 

Programmed move command 

•

 

Current position display 

•

 

Workpiece coordinate system preset 

•

 

Movement based on the manual numeric command G00 or G01 

 

  - Use with other functions 

Diameter/radius specification switching cannot be performed for an 
axis on which a movement is being made with any of the functions 
indicated below. 
Moreover, none of the functions indicated below can be performed 
during diameter and radius switching. 

•

 Synchronous/composite 

control 

•

 Superimposed 

Control 

•

 

Axis synchronous control 

•

 

PMC axis control 

 

B-63944EN/03

 PROGRAMMING 

 

 

- 223 - 

9.SPINDLE SPEED FUNCTION

(S FUNCTION)

9 

SPINDLE SPEED FUNCTION   
(S FUNCTION) 

 
The spindle speed can be controlled by specifying a value following 
address S. 
Chapter 9, "SPINDLE SPEED FUNCTION (S FUNCTION)", 
consists of the following sections: 
 
9.1  SPECIFYING THE SPINDLE SPEED WITH A CODE .........224 
9.2  SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY 

(S5-DIGIT COMMAND) .........................................................224 

9.3  CONSTANT SURFACE SPEED CONTROL (G96, G97) ......225 
9.4  SPINDLE POSITIONING FUNCTION...................................230 
9.5  SPINDLE SPEED FLUCTUATION DETECTION.................236 
9.6  SPINDLE CONTROL WITH SERVO MOTOR......................241 
 

 PROGRAMMING 

B-63944EN/03

 

 

- 224 - 

9. SPINDLE SPEED FUNCTION 

(S FUNCTION) 

9.1 

SPECIFYING THE SPINDLE SPEED WITH A CODE 

 
When a value is specified after address S, the code signal and strobe 
signal are sent to the machine to control the spindle rotation speed. 
A block can contain only one S code. Refer to the appropriate manual 
provided by the machine tool builder for details such as the number of 
digits in an S code or the execution order when a move command and 
an S code command are in the same block. 
 

9.2 

SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY 
(S5-DIGIT COMMAND) 

 
The spindle speed can be specified directly by address S followed by a 
max. five-digit value (min

-1

). The unit for specifying the spindle speed 

may vary depending on the machine tool builder. Refer to the 
appropriate manual provided by the machine tool builder for details. 
 

B-63944EN/03

 PROGRAMMING 

 

 

- 225 - 

9.SPINDLE SPEED FUNCTION

(S FUNCTION)

9.3 

CONSTANT SURFACE SPEED CONTROL (G96, G97) 

 
Specify the surface speed (relative speed between the tool and 
workpiece) following S. The spindle is rotated so that the surface 
speed is constant regardless of the position of the tool. 
 

Format 
  - Constant surface speed control command 

G96Sxxxxx ; 

       

↑

 Surface speed (m/min or feet/min) 

This surface speed unit may change according to machine 
tool builder's specification. 

 

  - Constant surface speed control cancel command 

G97Sxxxxx ; 

       

↑

 Spindle speed (min

-1

) 

This surface speed unit may change according to machine 
tool builder's specification. 

 

  - Constant surface speed controlled axis command 

G96P

α

 ; 

P0 : Axis set in the parameter (No. 3770) 
P1 : X axis, P2 : Y axis, P3 : Z axis, P4 : 4th axis 
P5 : 5th axis, P6 : 6th axis, P7 : 7th axis, P8 : 8th axis 

 

NOTE 

 

If multi-spindle control (spindle selecting based on 
address P or spindle name expansion) is enabled, 
axis specification based on address P is disabled.   
Use parameter No. 3770 for axis specification. 

 

  - Clamp of maximum spindle speed 

G92 S_ ;

 

The maximum spindle speed (min

-1

) follows S. 

 

T

   

G50 S_ ;   

The maximum spindle speed (min

-1

) follows S. 

 

NOTE 

 

G50 can be used with G code system A. 

 

 PROGRAMMING 

B-63944EN/03

 

 

- 226 - 

9. SPINDLE SPEED FUNCTION 

(S FUNCTION) 

Explanation 
  - Constant surface speed control command (G96) 

G96 (constant surface speed control command) is a modal G code.  
After a G96 command is specified, the program enters the constant 
surface speed control mode (G96 mode) and specified S values are 
assumed as a surface speed. A G96 command must specify the axis 
along which constant surface speed control is applied. A G97 
command cancels the G96 mode.  When constant surface speed 
control is applied, a spindle speed higher than the value specified in 
G92S_; or G50S_; (maximum spindle speed) is clamped at the 
maximum spindle speed. When the power is turned on, the maximum 
spindle speed is not yet set and the speed is not clamped. S (surface 
speed) commands in the G96 mode are assumed as S = 0 (the surface 
speed is 0) until M03 (rotating the spindle in the positive direction) or 
M04 (rotating the spindle in the negative direction) appears in the 
program. 

The spindle speed (min

-1

) almost coincides

with the surface speed (m/min) at approx.
160 mm (radius).

Spindle speed (min

-1

)

Relation between workpiece radius,
spindle speed and surface speed

Radius (mm)

Surface speed S is 600 m/min.

 

Fig. 9.3 (a)    Relation between workpiece radius, spindle speed and 

surface speed 

 

B-63944EN/03

 PROGRAMMING 

 

 

- 227 - 

9.SPINDLE SPEED FUNCTION

(S FUNCTION)

  - Setting the workpiece coordinate system for constant surface speed control 

To execute the constant surface speed control, it is necessary to set the 
workpiece coordinate system , and so the coordinate value at the 
center of the rotary axis, for example, Z axis, (axis to which the 
constant surface speed control applies) becomes zero. 

X

Z

0

 

Fig. 9.3 (b)    Example of the workpiece coordinate system for constant 

surface speed control 

 

  - Surface speed specified in the G96 mode 

G96 mode

G97 mode

Specify the surface speed in m/min

(or feet/min)

G97 command

Store the surface speed in m/min

(or feet/min)

Command for

the spindle

speed

Specified

The specified

spindle speed

(min

-1

) is used

Not specified

The surface speed (m/min or
feet/min) is converted to the

spindle speed (min

-1

)

Commands other than G96

G96 command

The specified

surface

speed is used

Command

for the surface

speed

The stored surface speed (m/min or

feet/min) is used.    If no surface

is stored, 0 is assumed.

Specified

Not specified