FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 15

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 76 - 

4.8 

POLAR COORDINATE INTERPOLATION (G12.1, G13.1) 

 

Overview 

Polar coordinate interpolation is a function that exercises contour 
control in converting a command programmed in a Cartesian 
coordinate system to the movement of a linear axis (movement of a 
tool) and the movement of a rotary axis (rotation of a workpiece).  
This function is useful for grinding a cam shaft. 
 

Format 

G12.1; 

Starts polar coordinate interpolation mode 
(enables polar coordinate interpolation). 

 

Specify linear or circular interpolation using 
coordinates in a Cartesian coordinate system 
consisting of a linear axis and rotary axis 
(hypothetical axis).

 

G13.1; 

Polar coordinate interpolation mode is 
cancelled (for not performing polar coordinate 
interpolation).

 

Specify G12.1 and G13.1 in Separate Blocks. 

 

Explanation 
  - Polar coordinate interpolation mode (G12.1) 

The axes of polar coordinate interpolation (linear axis and rotary axis) 
should be specified in advance, with corresponding parameters. 
Specifying G12.1 places the system in the polar coordinate 
interpolation mode, and selects a plane (called the polar coordinate 
interpolation plane) formed by one linear axis and a hypothetical axis 
intersecting the linear axis at right angles. The linear axis is called the 
first axis of the plane, and the hypothetical axis is called the second 
axis of the plane. Polar coordinate interpolation is performed in this 
plane. 
In the polar coordinate interpolation mode, both linear interpolation 
and circular interpolation can be specified by absolute or incremental 
programming. 
Tool radius compensation can also be performed. The polar coordinate 
interpolation is performed for a path obtained after tool radius 
compensation. 
The tangential velocity in the polar coordinate interpolation plane 
(Cartesian coordinate system) is specified as the feedrate, using F. 
 

  - Polar coordinate interpolation cancel mode (G13.1) 

Specifying G13.1 cancels the polar coordinate interpolation mode. 
 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 77 - 

  - Polar coordinate interpolation plane 

G12.1 starts the polar coordinate interpolation mode and selects a 
polar coordinate interpolation plane (Fig. 4.8 (a)). Polar coordinate 
interpolation is performed on this plane. 
 

Rotary axis (hypothetical axis) 

(unit: mm or inch) 

Linear axis 
(unit: mm or inch)

Origin of the local coordinate system (G52 command) 
(Or origin of the workpiece coordinate system) 

 

Fig. 4.8 (a)    Polar coordinate interpolation plane 

 
When the power is turned on or the system is reset, polar coordinate 
interpolation is canceled (G13.1). 
The linear and rotation axes for polar coordinate interpolation must be 
set in parameters Nos. 5460 and 5461 beforehand. 
 

 CAUTION 

 

The plane used before G12.1 is specified (plane 
selected by G17, G18, or G19) is canceled. It is 
restored when G13.1 (canceling polar coordinate 
interpolation) is specified. 

 

When the system is reset, polar coordinate 
interpolation is canceled and the plane specified by 
G17, G18, or G19 is used. 

 

  - Distance moved and feedrate for polar coordinate interpolation 

•

 

The unit for coordinates on the hypothetical axis is the same as 
the unit for the linear axis (mm/inch). 

 

In the polar coordinate interpolation mode, program commands 
are specified with Cartesian coordinates on the polar coordinate 
interpolation plane. The axis address for the rotary axis is used as 
the axis address for the second axis (hypothetical axis) in the 
plane. Whether a diameter or radius is specified for the first axis 
in the plane is the same as for the rotary axis regardless of the 
specification for the first axis in the plane. 

 

The hypothetical axis is at coordinate 0 immediately after G12.1 
is specified. Polar interpolation is started assuming the rotation 
angle of 0 for the position of the tool when G12.1 is specified. 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 78 - 

Example) 
 

When a value on the X-axis (linear axis) is input in 
millimeters 

 G12.1; 
 

G01 X10. F1000. ;.... A 10-mm movement is made on the 

Cartesian coordinate system. 

 

C20. ; ........................ A 20-mm movement is made on the 

Cartesian coordinate system. 

 G13.1; 
 
 

When a value on the X-axis (linear axis) is input in inches 

 G12.1; 
 

G01 X10. F1000. ;  .. A 10-inch movement is made on the 

Cartesian coordinate system. 

 

C20. ; ........................ A 20-inch movement is made on the 

Cartesian coordinate system. 

 G13.1; 
 

•

 

The unit for the feedrate is mm/min or inch/min. 

 

Specify the feedrate as a speed (relative speed between the 
workpiece and tool) tangential to the polar coordinate 
interpolation plane (Cartesian coordinate system) using F. 

 

  - G codes which can be specified in the polar coordinate interpolation mode 

G01 .......................Linear interpolation 
G02, G03...............Circular interpolation 
G02.2, G03.2.........Involute interpolation 
G04 .......................Dwell, Exact stop 
G40, G41, G42......Tool radius compensation 

(Polar coordinate interpolation is applied to the 
path after tool radius compensation.) 

G65, G66, G67......Custom macro command 
G90, G91...............Absolute programming, incremental programming 
G94, G95...............Feed per minute, feed per revolution 
 

  - Circular interpolation in the polar coordinate plane 

The addresses for specifying the radius of an arc for circular 
interpolation (G02 or G03) in the polar coordinate interpolation plane 
depend on the first axis in the plane (linear axis). 

•

 

I and J in the Xp-Yp plane when the linear axis is the X-axis or 
an axis parallel to the X-axis. 

•

 

J and K in the Yp-Zp plane when the linear axis is the Y-axis or 
an axis parallel to the Y-axis. 

•

 

K and I in the Zp-Xp plane when the linear axis is the Z-axis or 
an axis parallel to the Z-axis. 

The radius of an arc can be specified also with an R command. 
 

NOTE 

 

In a lathe system, the parallel axes U, V, and W 
can be used in the G code system B or C. 

 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 79 - 

  - Movement along axes not in the polar coordinate interpolation plane in the polar 

coordinate interpolation mode 

The tool moves along such axes normally, independent of polar 
coordinate interpolation. 
 

  - Current position display in the polar coordinate interpolation mode 

Actual coordinates are displayed. However, the remaining distance to 
move in a block is displayed based on the coordinates in the polar 
coordinate interpolation plane (Cartesian coordinates). 
 

  - Coordinate system for the polar coordinate interpolation 

Basically, before G12.1 is specified, a local coordinate system (or 
workpiece coordinate system) where the center of the rotary axis is the 
origin of the coordinate system must be set. 
 

  - Compensation in the direction of the hypothetical axis in polar coordinate 

interpolation 

If the first axis of the plane has an error from the center of the rotary 
axis in the hypothetical axis direction, in other words, if the rotary 
axis center is not on the X-axis, the hypothetical axis direction 
compensation function in the polar coordinate interpolation mode is 
used. With the function, the error is considered in polar coordinate 
interpolation. The amount of error is specified in parameter No. 5464. 
 

(X, C) 

Hypothetical axis (C-axis)

 

Error in the direction of 

hypothetical axis (P)

 

Center of rotary axis

X-axis

Rotary axis

 

(X, C) 

Point in the X-C plane (The center of the rotary axis is 
considered to be the origin of the X-C plane.)

 

X 

X coordinate in the X-C plane

 

C 

Hypothetical axis coordinate in the X-C plane

 

P 

Error in the direction of the hypothetical axis   
(specified in parameter No. 5464)

 

 

 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 80 - 

  - Shifting the coordinate system in polar coordinate interpolation 

In the polar coordinate interpolation mode, the workpiece coordinate 
system can be shifted. The current position display function shows the 
position viewed from the workpiece coordinate system before the shift. 
The function to shift the coordinate system is enabled when bit 2 
(PLS) of parameter No. 5450 is specified accordingly. 
The shift can be specified in the polar coordinate interpolation mode, 
by specifying the position of the center of the rotary axis C (A, B) in 
the X-C (Y-A, Z-B) interpolation plane with reference to the origin of 
the workpiece coordinate system, in the following format. 
 

G12.1 X_ C_ ;    (Polar coordinate interpolation for the X-axis and C-axis) 
G12.1 Y_ A_ ;  (Polar coordinate interpolation for the Y-axis and A-axis) 
G12.1 Z_ B_ ;  (Polar coordinate interpolation for the Z-axis and B-axis) 

 

X

C

x

c

Center of C-axis

G12.1 Xx Cc ;

Origin of workpiece

coordinate system

 

 

Limitation 
  - Changing the coordinate system during polar coordinate interpolation 

In the G12.1 mode, the coordinate system must not be changed (G92, 
G52, G53, relative coordinate reset, G54 through G59, etc.). 
 

  - Tool radius/tool nose radius compensation 

The polar coordinate interpolation mode (G12.1 or G13.1) cannot be 
started or terminated in the tool radius/tool nose radius compensation 
mode (G41 or G42). G12.1 or G13.1 must be specified in the tool 
radius/tool nose radius compensation canceled mode (G40). 
 

  - Tool length offset command 

Tool length offset must be specified in the polar coordinate 
interpolation cancel mode before G12.1 is specified. It cannot be 
specified in the polar coordinate interpolation mode. Furthermore, no 
offset values can be changed in the polar coordinate interpolation 
mode. 
 

  - Tool offset command 

A tool offset must be specified before the G12.1 mode is set. No offset 
can be changed in the G12.1 mode. 
 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 81 - 

 - Program restart 

For a block in the G12.1 mode, the program and the block cannot be 
restarted. 
 

  - Cutting feedrate for the rotary axis 

Polar coordinate interpolation converts the tool movement for a figure 
programmed in a Cartesian coordinate system to the tool movement in 
the rotary axis (C-axis) and the linear axis (X-axis). When the tool 
comes close to the center of the workpiece, the C-axis velocity 
component increases. If the maximum cutting feedrate for the C-axis 
(parameter No. 1430) is exceeded, the automatic feedrate override 
function and automatic speed clamp function are enabled. 
If the maximum cutting feedrate for the X-axis is exceeded, the 
automatic feedrate override function and automatic speed clamp 
function are enabled. 
 

 WARNING 

1  Consider lines L1, L2, and L3. 

∆

X is the distance the tool moves per time unit at the 

feedrate specified with address F in the Cartesian coordinate system. As the tool 
moves from L1 to L2 to L3, the angle at which the tool moves per time unit 
corresponding to 

∆

X in the Cartesian coordinate system increases from 

θ

1 to 

θ

2 to 

θ

3. In other words, the C-axis component of the feedrate becomes larger as the 

tool moves closer to the center of the workpiece. The C component of the feedrate 
may exceed the maximum cutting feedrate for the C-axis because the tool 
movement in the Cartesian coordinate system has been converted to the tool 
movement for the C-axis and the X-axis. 

L1

L2

L3

 

θ

3

 

θ

2

 

θ

1

∆

X

 

L:  Distance (in mm) between the tool center and workpiece center when the tool 

center is the nearest to the workpiece center 

R:  Maximum cutting feedrate (deg/min) of the C axis 

 

Then, a speed specifiable with address F in polar coordinate interpolation can be 
given by the formula below. If the maximum cutting feedrate for the C-axis is 
exceeded, the automatic speed control function for polar coordinate interpolation 
automatically controls the feedrate. 

 

F < L 

×

 R 

×

 

180

π

 (mm/min) 

2  The following function cannot be used for the rotary axis of polar coordinate 

interpolation. 

 

•

    Index table indexing function 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 82 - 

  - Automatic speed control for polar coordinate interpolation 

If the velocity component of the rotary axis exceeds the maximum 
cutting feedrate in the polar coordinate interpolation mode, the speed 
is automatically controlled. 
 

 - Automatic override 

If the velocity component of the rotary axis exceeds the permissible 
velocity (maximum cutting feedrate multiplied by the permission 
factor specified in parameter No. 5463), the feedrate is automatically 
overridden as indicated below. 
Override = (Permissible velocity) 

÷

 (Velocity component of rotary 

axis) 

×

 100(%) 

 

  - Automatic speed clamp 

If the velocity component of the rotary axis after automatic override 
still exceeds the maximum cutting feedrate, the speed of the rotary 
axis is automatically clamped. As a result, the velocity component of 
the rotary axis will not exceed the maximum cutting feedrate. 
The automatic speed clamp function works only when the center of 
the tool is very close to the center of the rotary axis. 

C-axis 

A 

B 

C 

D

X-axis 

-10. 

+10. 

[Example] 

G90 G00 X10.0 C0. ; 
G12.1 ; 
G01 C0.1 F1000 ; 
X-10.0 : 
G13.1 ;

 

 

Automatic speed control for polar coordinate interpolation 

 
Suppose that the maximum cutting feedrate of the rotary axis is 360 
(3600 deg/min) and that the permission factor of automatic override 
for polar coordinate interpolation (parameter No. 5463) is 0 (90%).  
If the program indicated above is executed, the automatic override 
function starts working when the X coordinate becomes 2.273 (point 
A). The automatic speed clamp function starts working when the X 
coordinate becomes 0.524 (point B). 
The minimum value of automatic override for this example is 3%.  
The automatic speed clamp function continues working until the X 
coordinate becomes -0.524 (point C). Then, the automatic override 
function works until the X coordinate becomes -2.273 (point D). 
(The coordinates indicated above are the values in the Cartesian 
coordinate system.) 
 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 83 - 

NOTE 

1  While the automatic speed clamp function is 

working, the machine lock or interlock function may 
not be enabled immediately. 

2  If a feed hold stop is made while the automatic 

speed clamp function is working, the automatic 
operation halt signal is output. However, the 
operation may not stop immediately. 

3  The clamped speed may exceed the clamp value 

by a few percent.