FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 29

 

  Index      Manuals     FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual (B-63944EN/03)

 

Search            copyright infringement  

 

 

 

 

 

 

 

 

  

 

 

Content      ..     27      28      29      30     ..

 

 

 

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 29

 

 

7.COORDINATE SYSTEM

 PROGRAMMING 

B-63944EN/03

 

 

- 188 - 

Limitation 
  - Cancel of the compensation function 

When the G53 command is specified, cancel the compensation 
functions such as the cutter compensation, tool length compensation, 
tool nose radius compensation, and tool offset. 
 

  - G53 specification immediately after power-on 

Since the machine coordinate system must be set before the G53 
command is specified, at least one manual reference position return or 
automatic reference position return by the G28 command must be 
performed after the power is turned on.    This is not necessary when 
an absolute-position detector is attached. 
 

  - Blocks in which the high-speed G53 function is usable 

The high-speed G53 function is usable in the following combinations 
of commands: 

•

 G53 

→

 G00 

•

 G53 

→

 G53 

The high-speed G53 function is unusable in the following 
combination of commands: 

•

 G00 

→

 G53 

 

  - Specification in the same block 

 

M

 

Commands G50/G51, G50.1/G51.1, and G68/G69 cannot be specified 
in the same block where the G53 command is specified. 
 

T

 

Commands G50/G51 (except for G code system A), G50.1/G51.1, and 
G68.1/G69.1 cannot be specified in the same block where the G53 
command is specified. 
 

Note 

NOTE 

 

G53 is a G code for disabling buffering. 

 

Reference 
  - Setting a machine coordinate system 

When manual reference position return is performed after power-on, a 
machine coordinate system is set so that the reference position is at the 
coordinate values of (

α

, 

β

) set using parameter No.1240. 

 

B-63944EN/03

 PROGRAMMING 

7.COORDINATE SYSTEM

 

 

- 189 - 

β

Reference position

Machine coordinate system

Machine zero point

α

 

 

7.COORDINATE SYSTEM

 PROGRAMMING 

B-63944EN/03

 

 

- 190 - 

7.2 

WORKPIECE COORDINATE SYSTEM 

 

Overview 

A coordinate system used for machining a workpiece is referred to as 
a workpiece coordinate system.    A workpiece coordinate system is to 
be set with the CNC beforehand (setting a workpiece coordinate 
system). 
A machining program sets a workpiece coordinate system (selecting a 
workpiece coordinate system). 
A set workpiece coordinate system can be changed by shifting its 
origin (changing a workpiece coordinate system).   
 

7.2.1 

Setting a Workpiece Coordinate System 

 
A workpiece coordinate system can be set using one of three methods: 
 
(1)  Method using a workpiece coordinate system setting G code 
 

A workpiece coordinate system is set by specifying a value in the 
program after a workpiece coordinate system setting G code. 

(2) Automatic 

setting 

 

If bit 0 of parameter ZPR No. 1201 is set to 1, a workpiece 
coordinate system is automatically set when manual reference 
position return is performed (see III-3.1.). 

 

This function is, however, disabled when the workpiece 
coordinate system option is being used. 

(3)  Method using a workpiece coordinate system selection G code 
 

Six workpiece coordinate systems can be set beforehand using 
the MDI panel.    Program commands G54 to G59 can be used to 
select the workpiece axis to be used.    (see III-12.3.4.) 

 
When using an absolute command, establish the workpiece coordinate 
system in any of the above ways. 
 

Format 
  - Setting a workpiece coordinate system 

 

M

 

(G90) G92 

IP

_ 

 

T

 

G50 

IP

_ 

 

B-63944EN/03

 PROGRAMMING 

7.COORDINATE SYSTEM

 

 

- 191 - 

Explanation 

A workpiece coordinate system is set so that a point on the tool, such 
as the tool tip, is at specified coordinates. 
 

M

 

If a coordinate system is set using G92 during tool length offset, a 
coordinate system in which the position before offset matches the 
position specified in G92 is set.  Cutter compensation is cancelled 
temporarily with G92. 
 

T

 

If IP_ is an incremental command value, the workpiece coordinate 
system is defined so that the current tool position coincides with the 
result of adding the specified incremental value to the coordinates of 
the previous tool position.  If a coordinate system is set using G50 
during offset, a coordinate system in which the position before offset 
matches the position specified in G50 is set. 
 

Example 

 

M

 

 

25.2

X

Z

23.0

0

X

Z

600.0

IIf an absolute command is issued, the
base point moves to the commanded
position. In order to move the tool tip to
the commanded position, the    difference
from the tool tip to the base point is
compensated by tool length offset (see II-
14.1).

(Example 2)
Setting the coordinate system by the G92X600.0Z1200.0; command (The
base point on the tool holder is the start point for the program.)

0

Base point

1200.0

(Example 1)
Setting the coordinate system by the
G92X25.2Z23.0; command (The tool tip is the start
point for the program.)

 

 

7.COORDINATE SYSTEM

 PROGRAMMING 

B-63944EN/03

 

 

- 192 - 

T

 

 

(Example 1)
Setting the coordinate system by the G50X128.7Z375.1;
command (Diameter designation) (The tool nose is the

start point for the program.)

(Example 2)
Setting the coordinate system by the G50X1200.0Z700.0;
command (Diameter designation) (The base point on the turret is

the start point for the program.)

Z

X

Origin

375.1

Start point

φ

12

8.

7

Z

X

700.0

Start point

(base point)

φ

1200.0

 

 

 CAUTION 

 

The set workpiece coordinate system depends on 
diameter programming or radius programming. 

 

Notes 
  - Command for setting a workpiece coordinate system in the tool length 

compensation mode 

Executing a workpiece coordinate system setting G code command 
(G92 or, for G code system A in the lathe system, G50) presets a 
coordinate system in such a way that the specified position will be a 
pre-compensation position. 
However, this G code cannot be used together with a block where tool 
length compensation vectors vary.  For example, it cannot be used 
together with the following blocks. 
 

EXAMPLE 

1  Block in which G43/G44 is issued 
2  Block which is in the G43 or G44 mode and in 

which an H code is issued 

3  Block which is in the G43 or G44 mode and in 

which G49 is issued 

4  Block in which, in the G43 or G44 mode, 

compensation vectors are canceled using a G code 
such as G28 or G53 and then resumed again 

 
When presetting a workpiece coordinate system, using the workpiece 
coordinate system setting G code, do not stop in the previous block to 
change a tool length compensation offset selected, for example, with 
the MDI. 
 

B-63944EN/03

 PROGRAMMING 

7.COORDINATE SYSTEM

 

 

- 193 - 

7.2.2 

Selecting a Workpiece Coordinate System 

 
The user can choose from set workpiece coordinate systems as 
described below.    (For information about the methods of setting, see 
II-7.2.1.) 
 
(1)  Once a workpiece coordinate system is set by a workpiece 

coordinate system setting G code or by automatic workpiece 
coordinate system setting, absolute commands indicate positions 
in the workpiece coordinate system. 

(2)  Choosing from six workpiece coordinate systems set using the 

MDI panel 

 

By specifying a G code from G54 to G59, one of the workpiece 
coordinate systems 1 to 6 can be selected. 
G54 :  Workpiece coordinate system 1 
G55 :  Workpiece coordinate system 2 
G56 :  Workpiece coordinate system 3 
G57 :  Workpiece coordinate system 4 
G58 :  Workpiece coordinate system 5 
G59 :  Workpiece coordinate system 6 

 

Workpiece coordinate system 1 to 6 are established after 
reference position return after the power is turned on. When the 
power is turned on, G54 coordinate system is selected. 

 
When bit 2 (G92) of parameter No. 1202 is set to 1, executing the 
workpiece coordinate system setting G92 code command results in the 
issue of an alarm PS0010.    This is designed to prevent the user from 
confusing coordinate systems. 
 

 CAUTION 

 

The set workpiece origin offset value depends on 
diameter programming or radius programming. 

 

Example 

X

Y

100.0

40.

Workpiece coordinate system 2 (G55)

In this example, positioning is made to
positions (X=40.0, Y=100.0) in workpiece
coordinate system 2.

G90 G55 G00 X40.0 Y100.0 ;

 

Fig. 7.2.2 (a)   

 

7.COORDINATE SYSTEM

 PROGRAMMING 

B-63944EN/03

 

 

- 194 - 

7.2.3 

Changing Workpiece Coordinate System 

 
The six workpiece coordinate systems specified with G54 to G59 can 
be changed by changing an external workpiece origin offset value or 
workpiece origin offset value. 
Three methods are available to change an external workpiece origin 
offset value or workpiece origin offset value. 
(1)  Inputting from the MDI panel (see III-12.3.4) 
(2)  Programming (using a programmable data input G code or a 

workpiece coordinate system setting G code) 

(3)  Using the external data input function 
 

An external workpiece origin offset value can be changed by 
input signal to CNC. Refer to machine tool builder's manual for 
details. 

 

 

Workpiece 
coordinate system 1
(G54) 

Workpiece 
coordinate system 2 
(G55) 

Workpiece 
coordinate system 3 
(G56) 

Workpiece 
coordinate system 4 
(G57) 

Workpiece coordinate 
system 5    (G58) 

Workpiece coordinate 
system 6    (G59) 

ZOFS2 

ZOFS3 

ZOFS4 

ZOFS5 

ZOFS1 

ZOFS6 

Machine zero point 

EXOFS : External workpiece origin offset value 
ZOFS1 to ZOFS6 : Workpiece origin offset value 

EXOFS 

 

Fig. 7.2.3 (a)    Changing an external workpiece origin offset value or workpiece origin offset value 

 

Format 
  - Changing by inputting programmable data 

 

G10 L2 Pp 

IP

_; 

p=0 

: External workpiece origin offset value 

p=1 to 6  : Workpiece origin offset value correspond to 

workpiece coordinate system 1 to 6 

IP

_  : For an absolute command, workpiece origin offset for 

each axis. 

 

  For an incremental command, value to be added to 

the set workpiece origin offset for each axis (the result 
of addition becomes the new workpiece origin offset). 

 

B-63944EN/03

 PROGRAMMING 

7.COORDINATE SYSTEM

 

 

- 195 - 

  - Changing by setting a workpiece coordinate system 

 

M

 

G92 

IP

_ ; 

 

T

 

G50 

IP

_ ; 

 

Explanation 
  - Changing by inputting programmable data 

By specifying a programmable data input G code, the workpiece 
origin offset value can be changed for each workpiece coordinate 
system. 
 

  - Changing by setting a workpiece coordinate system 

By specifying a workpiece coordinate system setting G code, the 
workpiece coordinate system (selected with a code from G54 to G59) 
is shifted to set a new workpiece coordinate system so that the current 
tool position matches the specified coordinates (IP_). 
Then, the amount of coordinate system shift is added to all the 
workpiece origin offset values.  This means that all the workpiece 
coordinate systems are shifted by the same amount. 
 

 CAUTION 

 

When a coordinate system is set with workpiece 
coordinate system setting G92 code command 
after an external workpiece origin offset value is 
set, the coordinate system is not affected by the 
external workpiece origin offset value.    When 
G92X100.0Z80.0; is specified, for example, the 
coordinate system having its current tool reference 
position at X = 100.0 and Z = 80.0 is set. 

 

T

 

If IP is an incremental command value, the workpiece coordinate 
system is defined so that the current tool position coincides with the 
result of adding the specified incremental value to the coordinates of 
the previous tool position.    (Coordinate system shift) 
 

 

 

 

 

 

 

 

Content      ..     27      28      29      30     ..