FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 12

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 52 - 

Limitation 

The rapid traverse rate cannot be specified in the address F. 
Even if linear interpolation type positioning is specified, nonlinear 
type interpolation positioning is used in the following cases. Therefore, 
be careful to ensure that the tool does not foul the workpiece. 

•

  G28 specifying positioning between the reference and 

intermediate positions. 

•

 G53 

 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 53 - 

4.2 

SINGLE DIRECTION POSITIONING (G60) 

 
For accurate positioning without play of the machine (backlash), final 
positioning from one direction is available. 

Start point

Temporary stop

End point

Overrun

Start point

 

 

Format 

G60 

IP_ ;

 

IP_ : 

For an absolute programming, the coordinates of an 
end point, and for an incremental programming, the 
distance the tool moves. 

 

Explanation 

An overrun and a positioning direction are set by the parameter No. 
5440. Even when a commanded positioning direction coincides with 
that set by the parameter, the tool stops once before the end point. 
G60, which is a one-shot G-code, can be used as a modal G-code in 
group 01 by setting 1 to the bit 0 (MDL) of parameter No. 5431. 
This setting can eliminate specifying a G60 command for every block. 
Other specifications are the same as those for a one-shot G60 
command. When a one-shot G code is specified in the single direction 
positioning mode, the one-shot G command is effective like G codes 
in group 01. 
 
(Example) 

When one-shot G60 commands are used. 

G90; 
G60 X0Y0; 
G60 X100; 
G60 Y100; 
G04 X10; 
G00 X0Y0; 

 
 
Single direction positioning 
 

When modal G60 command is used. 

G90G60; 
X0Y0; 
X100; 
Y100; 
G04X10; 
G00X0 Y0; 

Single direction positioning mode start 
 
Single direction positioning 
 
 
Single direction positioning mode cancel 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 54 - 

  - Overview of operation 

•

 

In the case of positioning of non-linear interpolation type (bit 
1 (LRP) of parameter No. 1401 = 0) 

 

As shown below, single direction positioning is performed 
independently along each axis. 

 

Programmed end point

Programmed start point

Overrun distance in the 
X-axis direction 

Overrun distance in the Z-axis direction

Z

X 

 

 

•

 

In the case of positioning of linear interpolation type (bit 1 
(LRP) of parameter No. 1401 = 1) 

 

Positioning of interpolation type is performed until the tool once 
stops before or after a specified end point. Then, the tool is 
positioned independently along each axis until the end point is 
reached. 

 

Programmed end point

Programmed start point

Overrun distance in the 
X-axis direction 

Overrun distance in the Z-axis direction

Z

X

 

 

Limitation 

 

•

  Single direction positioning is not performed along an axis for 

which no overrun distance is set in parameter No. 5440. 

 

•

  Single direction positioning is not performed along an axis for 

which travel distance 0 is specified. 

 

•

  The mirror image function is not applied in a parameter-set 

direction. Even in the mirror image mode, the direction of single 
direction positioning remains unchanged. If positioning of linear 
interpolation type is used, and the state of mirror image when a 
single direction positioning block is looked ahead differs from 
the state of mirror image when the execution of the block is 
started, an alarm is issued. When switching mirror image in the 
middle of a program, disable looking ahead by specifying a 
non-buffering M code. Then, switch mirror image when there is 
no look-ahead block.   

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 55 - 

 

•

  In the cylindrical interpolation mode (G07.1), single direction 

positioning cannot be used.   

 

•

  In the polar coordinate interpolation mode (G12.1), single 

direction positioning cannot be used. 

 

•

  When specifying single direction positioning on a machine that 

uses arbitrary angular axis control, first position the angular axis 
then specify the positioning of the Cartesian axis. If the reverse 
specification order is used, or the angular axis and Cartesian axis 
are specified in the same block, an incorrect positioning direction 
can result. 

 

•

  In positioning at a restart position by program restart function, 

single direction positioning is not performed. 

 
 

M

 

•

 

During canned cycle for drilling, no single direction positioning 
is effected in drilling axis. 

•

  The single direction positioning does not apply to the shift 

motion in the canned cycles of G76 and G87. 

 

T

 

•

 

The G-code for single direction positioning is always G60, if 
G-code system is A or B or C in all case. 

•

 

The single direction positioning can not be commanded during 
the multiple repetitive cycle (G70-G76). 

•

  No single direction positioning is effected in the drilling or 

patting axis, during canned cycle for drilling (G83-G89) and the 
rigid tapping (G84, G88). However, it can be commanded for 
positioning. 

•

 

The single direction positioning can not be commanded during 
the canned cycle (G90, G92, G94). 

•

  During the single direction positioning mode (G60), the 

following G-code can not be commanded. 

 

G07.1, G12.1, G70-G76, G90-G94. 

 

 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 56 - 

4.3 

LINEAR INTERPOLATION (G01) 

 
Tools can move along a line. 
 

Format 

G01 

IP_ 

F_ ; 

IP_ : 

For an absolute programming, the coordinates of an 
end point, and for an incremental programming, the 
distance the tool moves. 

F_ :  Speed of tool feed (Feedrate) 

 

Explanation 

A tools move along a line to the specified position at the feedrate 
specified in F. 
The feedrate specified in F is effective until a new value is specified. 
It need not be specified for each block. 
The feedrate commanded by the F code is measured along the tool 
path. If the F code is not commanded, the feedrate is regarded as zero. 
The feedrate of each axis direction is as follows. 

G01 

α

α

 

β

β

 

γ

γ

 

ζ

ζ

 Ff ; 

Feed rate of 

α

 axis direction : 

f

L

F

×

=

α

α

 

Feed rate of 

β

 axis direction : 

f

L

F

×

=

β

β

 

Feed rate of 

γ

 axis direction :

 

f

L

F

×

=

γ

γ

 

Feed rate of 

ζ

 axis direction :

 

f

L

F

×

=

ζ

ζ

 

2

2

2

2

ζ

γ

β

α

+

+

+

=

L

 

 
The feedrate of the rotary axis is commanded in the unit of deg/min 
(the unit is decimal point position). 
When the straight line axis 

α

 (such as X, Y, or Z) and the rotating axis 

β

 (such as A, B, or C) are linearly interpolated, the feedrate is that in 

which the tangential feedrate in the 

α

 and 

β

 cartesian coordinate 

system is commanded by F (mm/min).   

β

-axis feedrate is obtained ; at first, the time required for distribution 

is calculated by using the above formula, then the 

β

-axis feedrate unit 

is changed to deg/min. 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 57 - 

A calculation example is as follows. 
G91 G01 X20.0B40.0 F300.0 ; 
This changes the unit of the C axis from 40.0 deg to 40mm 
with metric input. The time required for distribution is 
calculated as follows: 

 

300

40

20

2

2

+

)

(

14907

.

0

mm

 

The feedrate for the C axis is 

 

14907

.

0

40

min

deg/

3

.

268

 

 
In simultaneous 3 axes control, the feedrate is calculated the same way 
as in 2 axes control. 
 

Example 
 - Linear interpolation 

•

 

For milling machining 

 

(G91) G01X200.0Y100.0F200.0;

Y axis

100.0 

200.0 

0 (Start point) 

(End point) 

X axis 

 

 

•

 

For lathe cutting 

(Diameter programming) 
   G01X40.0Z20.1F20; (Absolute programming) 
      or 
   G01U20.0W-25.9F20; (Incremental programming) 

Z

20.1

46.0

φ

20.0 

X

φ

40.0 

Start 
point

End 
point

 

 

4.INTERPOLATION FUNCTIONS

 PROGRAMMING 

B-63944EN/03

 

 

- 58 - 

  - Feedrate for the rotary axis 

90

°

(Start point) 

(End point) 

Feedrate is 300 deg/min 

G91G01C-90.0 F300.0 ;Feed rate of 300deg/min 

 

 

B-63944EN/03

 PROGRAMMING 

4.INTERPOLATION FUNCTIONS

 

 

- 59 - 

4.4 

CIRCULAR INTERPOLATION (G02, G03) 

 
The command below will move a tool along a circular arc. 
 

Format 

Arc in the XpYp plane 

G02 I_ 

J_ 

G17 

G03 

Xp_ Yp_ 

R_ 

F_ ; 

Arc in the ZpXp plane 

G02 I_ 

K_

G18 

G03 

Zp_ Xp_ 

R_ 

F_ ; 

Arc in the YpZp plane 

G02 J_ 

K_

G19 

G03 

Yp_ Zp_ 

R_ 

F_ ; 

 

Command Description 

G17 Specification 

of arc on XpYp plane 

G18 Specification 

of arc on ZpXp plane 

G19 

Specification of arc on YpZp plane 

G02 

Circular Interpolation : Clockwise direction (CW) 

G03 

Circular Interpolation : Counterclockwise direction (CCW) 

Xp

_

 

Command values of X axis or its parallel axis   
(set by parameter No. 1022) 

Yp

_ 

Command values of Y axis or its parallel axis   
(set by parameter No. 1022) 

Zp

_ 

Command values of Z axis or its parallel axis   
(set by parameter No. 1022) 

I_ 

Xp axis distance from the start point to the center of an arc 
with sign 

J_ 

Yp axis distance from the start point to the center of an arc 
with sign 

K_ 

Zp axis distance from the start point to the center of an arc 
with sign 

R_ 

Arc radius (with sign, radius value for lathe cutting) 

F_ 

Feedrate along the arc 

 

T

 

NOTE 

 

The U-, V-, and W-axes can be used with G-codes 
B and C.