FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 28

6.REFERENCE POSITION

 PROGRAMMING 

B-63944EN/03

 

 

- 180 - 

  - Reference position return check (G27) 

G27 command positions the tool at rapid traverse rate.  If the tool 
reaches the reference position, the lamp for indicating the completion 
of reference position return lights up.   
When the tool returns to the reference position along only one axis, 
the lamp for the axis for indicating the completion of reference 
position return lights up. 
After positioning, if the tool has not reached the reference position 
along a specified axis, an alarm (PS0092) "ZERO RETURN CHECK 
(G27) ERROR" is issued. 
When no movement was made along the axis, whether the current 
position is the reference position is checked. 
 

B-63944EN/03

 PROGRAMMING 

6.REFERENCE POSITION

 

 

- 181 - 

  - Setting of the reference position return feedrate 

Before a coordinate system is established with the first reference 
position return after power-on, the manual and automatic reference 
position return feedrates and automatic rapid traverse rate conform to 
the setting of parameter No. 1428 for each axis.     
After a reference position is established upon the completion of 
reference position return, the manual reference position return feedrate 
conforms to the setting of the parameter No. 1428 for each axis. 
 

NOTE 

1  To this feedrate, a rapid traverse override (F0,25,50,100%) is applied, for which 

the setting is 100%. 

2  After a reference position has been established upon the completion of reference 

position return, the automatic reference position return feedrate will conform to the 

ordinary rapid traverse rate. 

3  When a value is set for parameter No. 1428, the feedrates conform to the 

parameter settings shown below. 

 

 

Before a coordinate system 

is established 

After a coordinate system is 

established 

 

Automatic reference position return (G28) 

No. 1428 

No.1420 

 

Automatic rapid traverse (G00) 

No.1428 

No.1420 

 

Manual reference position return (*1) 

No.1428 

No.1428 (*3) 

 

Manual rapid traverse rate 

No.1423 (*2) 

No.1424 

 

1420: Rapid traverse rate 

 

1423: Jog feedrate 

 

1424: Manual rapid traverse rate 

 

1428: Reference position return feedrate 

 

 

When parameter No. 1428 is set to 0, the feedrates conform to the parameter settings 
shown below.

 

 

 

Before a coordinate system 

is established 

After a coordinate system is 

established 

 

Automatic reference position return (G28) 

No. 1420 

No.1420 

 

Automatic rapid traverse (G00) 

No.1420 

No.1420 

 

Manual reference position return (*1) 

No.1424 

No.1424 (*3) 

 

Manual rapid traverse rate 

No.1423 (*2) 

No.1424 

 

*1  By using JZR (bit 2 of parameter No. 1401), the manual reference position 

return feedrate can always be set as a jog feedrate. 

 

*2  When RPD (bit 0 of parameter No. 1401) is 1, the setting of parameter No. 

1424 (manual rapid traverse rate) is used. 

 

 

When the setting of parameter No. 1424 (manual rapid traverse rate) is 0, 

parameter No. 1420 (rapid traverse rate) is used. 

 

*3  When reference position return without dogs is performed in rapid traverse 

mode, or when manual reference position return is performed in rapid 

traverse mode regardless of deceleration dogs after a reference position is 

established, the reference position return feedrate for each of these functions 

(setting of DLF (bit 1 of parameter No. 1404)) is used. 

6.REFERENCE POSITION

 PROGRAMMING 

B-63944EN/03

 

 

- 182 - 

Limitation 
  - Status the machine lock being turned on 

The lamp for indicating the completion of reference position return 
does not go on when the machine lock is turned on, even when the 
tool has automatically returned to the reference position.    In this case, 
it is not checked whether the tool has returned to the reference 
position even when a reference position return check command is 
specified. 
 

  - When automatic reference position return (G28) is executed if no reference 

position is established 

When automatic reference position return (G28) is executed if no 
reference position is established, movement from the intermediate 
position in a reference position direction is the same as that in manual 
reference position return. 
(This movement is referred to as a low-speed type of automatic 
reference position return (G28).) 
In this case, the tool moves in the direction for reference position 
return specified in parameter ZMIx (bit 5 of No. 1006).  Therefore 
the specified intermediate position must be a position to which 
reference position return is possible. 
 

NOTE 

 

When automatic reference position return (G28) is 
executed after a reference position is established, 
positioning is performed from the intermediate 
position to the reference position.    This movement 
is referred to as a high-speed type of automatic 
reference position return (G28). 

 

  - Reference position return check in an offset mode 

In an offset mode, the position to be reached by the reference position 
return check is the position obtained by adding the offset value.     
Therefore, if the position with the offset value added is not the 
reference position, the lamp for indicating the completion of reference 
position return does not light up, but an alarm is displayed instead.  
Usually, cancel offsets before G27 is commanded. 
 

  - Lighting the lamp when the programmed position does not coincide with the 

reference position 

When the machine tool system is an inch system with metric input, the 
lamp for indicating the completion of reference position return may 
also light up even if the programmed position is shifted from the 
reference position by the least setting increment.    This is because the 
least setting increment of the machine tool system is smaller than its 
least command increment. 
 

B-63944EN/03

 PROGRAMMING 

6.REFERENCE POSITION

 

 

- 183 - 

Example 

G28G90X1000.0Y500.0 ; 
 

(Programs movement  from A to B.  The tool moves to 
reference position R via intermediate position B.) 

T1111 ; 
 

(Changing the tool at the reference position) 

G29X1300.0Y200.0 ; 
 

(Programs movement from B to C.  The tool moves from 
reference position R to C specified with G29 via intermediate 
position B.) 

 

200

300

500

200

1000

1300

Y

X

Automatic reference position return (G28)

A 

→

 B 

→

 R

Movement from the reference position (G29)

R 

→

 B 

→

 C

A (Start position for reference

position return)

B (Intermediate
position)

C (Destination of return from the

reference position)

R (Reference position)

 

Fig. 6.1 (c)    Reference position return and movement from the reference position 

 
 

6.REFERENCE POSITION

 PROGRAMMING 

B-63944EN/03

 

 

- 184 - 

6.2 

FLOATING REFERENCE POSITION RETURN (G30.1) 

 
Tools ca be returned to the floating reference position. 
A floating reference point is a position on a machine tool, and serves 
as a reference point for machine tool operation.   
A floating reference point need not always be fixed, but can be moved 
as required. 
 

Format 

G30.1 

IP

_; 

IP

_ :  Specify the intermediate position to the floating 

reference position in the absolute coordinate system. 
(absolute/incremental programming) 

 

Explanation 

Generally speaking, on a machining center or milling machine, cutting 
tools can be replaced only at specific positions. A position where tools 
can be replaced is defined as the second or third reference point. Using 
G30 can easily move the cutting tools back to these points.   
On some machine tools, the cutting tools can be replaced at any 
position unless they interfere with the workpiece.  With these 
machines, the cutting tools should be replaced at a position as close to 
the workpiece as possible so as to minimize the machine cycle time. 
For this purpose, the tool change position is to be changed, depending 
on the figure of the workpiece.  This operation can easily be 
performed using this function.   
That is, a tool change position suitable for the workpiece is 
memorized as a floating reference point. Then command G30.1 can 
easily cause return to the tool change position. 
A floating reference point becomes a machine coordinate position 
memorized by pressing the soft key [SETFRP] on the current 
positions display screen.  The coordinates of the floating reference 
position are stored with parameter No. 1244.     
The G30.1 block first positions the tool at the intermediate point along 
the specified axes at rapid traverse rate, then further moves the tool 
from the intermediate point to the floating reference point at rapid 
traverse rate.    Before using G30.1, cancel the compensation functions, 
such as tool radius compensation and tool length compensation. 
A floating reference point is not lost even if power is turned off. 
The function for movement from the reference position (G29) can be 
specified for moving the tool from the floating reference position. 
 

B-63944EN/03

 PROGRAMMING 

6.REFERENCE POSITION

 

 

- 185 - 

Example 

Y

X

Workpiece

Intermediate position (50,40)

Floating reference
position

G30.1 G90 X50.0 Y40.0 ;

 

 

7.COORDINATE SYSTEM

 PROGRAMMING 

B-63944EN/03

 

 

- 186 - 

7 

COORDINATE SYSTEM 

 
By teaching the CNC a desired tool position, the tool can be moved to 
the position. Such a tool position is represented by coordinates in a 
coordinate system. Coordinates are specified using program axes. 
When three program axes, the X-axis, Y-axis, and Z-axis, are used, 
coordinates are specified as follows: 
  X_Y_Z_  
This command is referred to as a dimension word. 

•

  For milling machining (Tool position specified by 

X40.0Y50.0Z25.0 ) 

Z

Y

X

40.0

50.0

25.0

 

•

 

For lathe cutting (Tool position specified by X50.0 Z40.0) 

X

Zero point

40.0

Z

50.0

 

 
Coordinates are specified in one of following three coordinate 
systems: 
(1)  Machine coordinate system 
(2)  Workpiece coordinate system 
(3)  Local coordinate system 
The number of the axes of a coordinate system varies from one 
machine to another. So, in this manual, a dimension word is 
represented as IP_. 

B-63944EN/03

 PROGRAMMING 

7.COORDINATE SYSTEM

 

 

- 187 - 

7.1 

MACHINE COORDINATE SYSTEM 

 
The point that is specific to a machine and serves as the reference of 
the machine is referred to as the machine zero point.    A machine tool 
builder sets a machine zero point for each machine. 
A coordinate system with a machine zero point set as its origin is 
referred to as a machine coordinate system. 
A machine coordinate system is set by performing manual reference 
position return after power-on (see III-3.1).  A machine coordinate 
system, once set, remains unchanged until the power is turned off. 
The reference position is not always the origin of the machine 
coordinate system. 
(See "Setting a machine coordinate system" described later.) 
 

Format 

 

M

 

(G90) G53 

IP

_ P1; 

IP

_:  Absolute dimension word 

P1:    Enables the high-speed G53 function. 

 

T

 

G53 

IP

_ P1; 

IP

_:  Absolute dimension word 

P1:    Enables the high-speed G53 function. 

 

Explanation 
  - Selecting a machine coordinate system (G53) 

When a command is specified the position on a machine coordinate 
system, the tool moves to the position by rapid traverse.    G53, which 
is used to select a machine coordinate system, is a one-shot G code; 
that is, it is valid only in the block in which it is specified on a 
machine coordinate system.    Specify an absolute command for G53.   
When an incremental command is specified, the G53 command is 
ignored. When the tool is to be moved to a machine-specific position 
such as a tool change position, program the movement in a machine 
coordinate system based on G53. 
 

  - High-speed G53 function 

This function enables the inter-rapid traverse block overlap function 
between machine coordinate selection command (G53) and 
positioning (rapid traverse) command (G00) blocks, thus making it 
possible to execute the next rapid traverse command (G00) without 
decelerating to a stop at the end of the machine coordinate selection 
command (G53).    Therefore, high-speed positioning is available even 
when the machine coordinate selection command (G53) is used. 
Specifying P1 in a G53 block enables the high-speed G53 function.