FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 125

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 956 -

Look-ahead acceleration/deceleration before interpolation

If the 3-dimensional cutter compensation mode is entered, look-ahead
acceleration/deceleration before interpolation is automatically enabled.
Set the look-ahead acceleration/deceleration parameter. If the
parameter is incorrectly set, an alarm is issued.

Deceleration at a corner

Under 3-dimensional cutter compensation,

the controlled point may

move along a curve even if a straight-line command is issued. Some
commands may cause a corner movement.

When AI contour control is not used, there is a possibility that the
machine is shocked at a corner.
Accordingly, it is recommended that AI contour control be used and
the permissible acceleration (parameter No. 1737) and permissible
speed difference at a corner (parameter No. 1783) be set.

Specifiable G codes

When the table coordinate system is used as the programming
coordinate system, the G codes that can be specified in the
3-dimensional cutter compensation mode are listed below.
Specifying a G code other than these codes results in alarm PS5460:

•

Positioning

(G00)

•

Linear interpolation (G01)

•

Dwell

(G04)

•

Exact stop (G09)

•

Programmable data input (G10)

•

Programmable data input mode cancel (G11)

•

Plane selection (G17/G18/G19)

•

Cutter compensation : cancel (G40)

•

Tool length compensation cancel (G49)

•

Programmable mirror image (G50.1/G51.1)

•

Macro call (G65)

•

Macro modal call A (G66)

•

Macro modal call B (G66.1)

•

Macro modal call A/B cancel (G67)

•

Absolute programming (G90)

•

Incremental programming (G91)

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 957 -

Modal G codes that allow specification of 3-dimensional cutter compensation

When the table coordinate system is used as the programming
coordinate system, 3-dimensional cutter compensation can be
specified in the modal G code states listed below.
In a modal state other than the following modal G codes, specifying
tool center point control results in alarm PS5421.

•

Modal G codes included in "Specifiable G codes" described

previously

•

Polar coordinate interpolation mode cancel (G13.1)

•

Polar coordinates command cancel (G15)

•

Input in inch (G20 (G70))

•

Input in mm (G21 (G71))

•

Tool center point control (G43.4/G43.5)

•

Polygon turning cancel (G50.2)

•

Workpiece coordinate system 1 selection (G54 to G59)

•

Canned cycle cancel (G80)

•

Constant surface speed control cancel (G97)

•

Canned cycle : return to initial level (G98)

•

Canned cycle : return to R point level (G99)

•

Coordinate system rotation start or 3-dimensional coordinate

conversion mode on (G69)

•

Feed per minute (G94)

•

Polar coordinate interpolation mode cancel (G113)

•

Mirror image for double turret off/balanced cutting mode cancel
(G69)

•

Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off (G69.1)

•

Feed per minute (G98 (G94))

Specification of axes not relating to 3-dimensional cutter compensation

Axes not relating to 3-dimensional cutter compensation cannot be
specified. If such an axis is specified, alarm PS5460 is issued.

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 958 -

22.5.6

Examples

O100 is a sample program.
This is an example in which each side of a square is cut at an angle of
30 degrees on the B-axis in a composite type machine.
Programs 1 to 3 all perform the same machining.

Program 1: Type 1 and the table coordinate system is selected as a

programming coordinate system

O100

（

Sample Program1

）；

N10 G55 ;

Preparations for the programming coordinate system

N20 G90 X0 Y0 Z300.0 B0 C0 ;

Movement to the initial position

N30 G01 G43.4 H01 Z40.0 F500. ;

Start of tool center point control

H01 is a tool length compensation number

N40 G41.2 D01;

Start of cutter compensation

D01 is a tool cutter compensation number

N50 X50.0 Y50.0 Z20.0 B30.0 C45.0 ; The Z-axis height on the machining plane is 20.0.
N60 X-50.0 C135.0 ;
N70 X-100.0 Y-100.0 C225.0 ;
N80 X100.0 C315.0 ;
N90 X50.0 Y50.0 C405.0 ;
N100 X0 Y0 Z40.0 B0 C360.0 ;
N110 G40 ;

Cutter compensation cancellation

N120 G49 Z300.0 ;

Tool center point control cancellation

Movement to the initial position on the Z-axis

N130 M30;

Program 2: Type 1 and the workpiece coordinate system is selected

as a programming coordinate system

(Note that the values specified in N50 to N90 differ from those in
program 1.)

O100

（

Sample Program2

）

;

N10 G55 ;

Preparations for the programming coordinate system

N20 G90 X0 Y0 Z300.0 B0 C0 ;

Movement to the initial position

N30 G01 G43.4 H01 Z40.0 F500. ;

Start of tool center point control

H01 is a tool length compensation number

N40 G41.2 D01;

Start of cutter compensation

D01 is a tool cutter compensation number

N50 X70.711 Y0 Z20.0 B30.0 C45.0 ; The Z-axis height on the machining plane is 20.0.
N60 C135.0 ;
N70 X141.421 C225.0 ;
N80 C315.0 ;
N90 X70.711 C405.0 ;
N100 X0 Y0 Z40.0 B0 C360.0 ;
N110 G40 ;

Cutter compensation cancellation

N120 G49 Z300.0 ;

Tool center point control cancellation

Movement to the initial position on the Z-axis

N130 M30;

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 959 -

Program 3: When the type 2 is used:

(The table coordinate system is selected as a
programming coordinate system)

O100

（

Sample Program3

）

;

N10 G55 ;

Preparations for the programming coordinate system

N20 G90 X0 Y0 Z300.0 B0 C0 ;

Movement to the initial position

N30 G01 G43.5 H01 Z40.0 F500. ;

Start of tool center point control

H01 is a tool length compensation number

N40 G41.6 D01;

Start of cutter compensation

D01 is a tool cutter compensation number

N50 X50.0 Y50.0 Z20.0 I35.355 J35.355 K86.603 ; The Z-axis height on the machining plane is 20.
N60 X-50.0 I-35.355 J35.355 K86.603 ;
N70 X-100.0 Y-100.0 I-35.355 J-35.355 K86.603 ;
N80 X100.0 I35.355 J-35.355 K86.603 ;
N90 X50.0 Y50.0 I35.355 J35.355 K86.603 ;
N100 X0 Y0 Z40.0 K1.0 ;
N110 G40 ;

Cutter compensation cancellation

N120 G49 Z300.0 ;

Tool center point control cancellation

Movement to the initial position on the Z-axis

N130 M30;

By using type 2 as in program 3, the same program can be used with
machines with different configurations, regardless of whether the
machine configuration is the tool rotation type, table rotation type, or
composite type.

Composite type (tool rotation axis: B-axis - table rotation axis:
C-axis - tool axis: Z direction

G55
Workpiece coordinate system

Rotation center of
B-axis

Rotation center of
C-axis

Fig. 22.5.6 (a) Machine configuration for example

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 960 -

Fig. 22.5.6 (b) shows the attitudes of the workpiece (object to be
machined) and the tool head (relative to the workpiece (object to be
machined)) as viewed in the positive Z direction of the programming
coordinate system fixed to the table (table coordinate system).

Operation as viewed from the table coordinate system

(X-100.0,Y-100.0)

(B 30.0)

(C 45.0)

(C 135.0)

(X-50.0,Y50.0)

(X50.0,Y50.0)

(B 30.0)

(C 225.0)

(C 315.0)

(X-100.0,Y-100.0)

Fig. 22.5.6 (b) Illustration of example

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 961 -

Exploded view of each block

Operation at control point
(machine coordinate values)

Block N70

(C 45.0)

(C 135.0)

Block N60

(C 225.0)

X'Y' : Table coordinate system
X"'Y" : Workpiece coordinate system

Fig. 22.5.6 (c) Exploded View of Each Block (1)

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 962 -

Block N90

Block N80

(C 225.0)

(C 315.0)

(C 405.0)

Fig. 22.5.6 (d) Exploded View of Each Block (2)

B-63944EN/03

PROGRAMMING

23.MUITI-PATH CONTROL FUNCTION

- 963 -

MUITI-PATH CONTROL FUNCTION

Chapter 23, "MUITI-PATH CONTROL FUNCTION", consists of the
following sections:

23.1 OVERVIEW...........................................................................964
23.2  WAITING FUNCTION FOR PATHS ...................................966
23.3  COMMON MEMORY BETWEEN EACH PATH................972
23.4  SPINDLE CONTROL BETWEEN EACH PATH.................974
23.5 SYNCHRONOUS/COMPOSITE/SUPERIMPOSED

CONTROL .............................................................................975

Content .. 123 124 125 126 ..