FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 104

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 788 -

Explanation
- When a coordinate system fixed on the table is used as the programming

coordinate system

The programming coordinate system is used for tool center point
control. When the G43.4 or G43.5 command is specified with bit 5
(WKP) of parameter No.19696 set to 0, the workpiece coordinate
system that is fixed on the table at that point of time becomes the
programming coordinate system. Thereafter, the programming
coordinate system rotates as the table turns around.
It does not rotate with the tool head.
X, Y, and Z mentioned hereinafter are assumed to be commanded on
the programming coordinate system.
When the G43.4 or G43.5 command is specified or when the rotary
axis of the table has moved in a block preceding G43.4 or G43.5, the
angle of the table's rotary axis represents the initial state of the
programming coordinate system.
In the case of type 2, the tool direction seen from the coordinate
system that is fixed on the table is specified by I, J, K.
In the descriptions that follow, the table-fixed coordinate system is
represented by X', Y', and Z'.

When G43.4 or G43.5 is
specified with C = 0
d

Tool center point control
in progress

Workpiece
coordinate
system

Programming
coordinate system

Tool center point control in
progress

C-axis reference position

Workpiece
coordinate
system

When G43.4 or G43.5 is
specified with C = 45 degrees

Programming
coordinate system

The C-axis reference position is the position where a movement is
made on the C-axis so that a command value for the C-axis is at the
scale position on the table.

Fig. 22.1 (f) Programming coordinate system fixed on the table

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 789 -

- When the workpiece coordinate system is used as the programming coordinate

system

When the G43.4 command is specified with bit 5 (WKP) of parameter
No.19696 set to 1, the workpiece coordinate system that is in use at
that point of time becomes the programming coordinate system.
In this case, the programming coordinate system does not rotate as the
table turns around but remains fixed on the workpiece coordinate
system.
Hereinafter, when X, Y, and Z are commanded, the tool moves along
a straight line toward the table (workpiece). For X, Y, Z, specify the
end point location after the rotation of the table, as seen from the
programming coordinate system.
Type 2 cannot be used. Specifying G43.5 when bit 5 (WKP) of
parameter No.19696 set to 1 causes alarm PS5459.
In the descriptions that follow, the coordinate values of the workpiece
coordinate system used as the programming coordinate system are
represented by X", Y", and Z".

When G43.4 is specified
with C = 0 degrees

Tool center point control
in progress

Workpiece
coordinate
system

Programming
coordinate
system

Tool center point control in

progress

C-axis reference position

Workpiece
coordinate
system

When G43.4 is specified with
C = 45 degrees

Programming
coordinate
system

The C-axis reference position is the position where a movement is made on the
C-axis so that a command value for the C-axis is at the scale position on the
table.

Fig. 22.1 (g) Programming coordinate system identical to the

workpiece coordinate system

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 790 -

- Notes on performing circular interpolation and helical interpolation when using

the workpiece coordinate system as the programming coordinate system

•

The start point, end point, and center of an arc change as the
table rotation axis rotates.

•

I, J, K commands the vector of the block start point to the center
of the arc from the start point in the rotary axis position.

•

Note the following:
<1> Only a table rotation axis normal to a selected plane can be

rotated during circular interpolation.

<2> During circular interpolation, those table rotation axes not

normal to a selected plane must continue to be at the same
position as when tool center point control is started.

If <1> or <2> is not satisfied, the alarm PS5421 is issued.
No restriction is imposed on rotation on a tool rotation axis.

- Program examples

•

In the case of a composite type machine

Descriptions are based on the following machine configuration.

C-axis

Center of C-axis rotation

Z-axis

Y-axis

X-axis

B-axis

Center of B-axis rotation

Tool center point

Workpiece

coordinate system

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 791 -

When the G17 (X-Y plane) command is executed

After the G43.4 command, the X-Y plane is selected using the G17
command and circular interpolation is performed by rotating the
C-axis (table rotation axis) (including those cases where the C-axis
moves before the G43.4 command).

→

This case corresponds to <1>

and allows circular interpolation.
Example)

:
(G01 C90. ;)
G43.4 H1 ;
G17 G02

B10. C20. ;

IP: Coordinates of the end point
IR: Arc radius

When the G18 (Z-X plane) or G19 (Y-Z plane) command is executed

After the G43.4 command, the Z-X plane is selected using the G18
command and circular interpolation is performed without rotating the
C-axis (including those cases where the C-axis moves before the
G43.4 command).

→

This case corresponds to <2> and allows

circular interpolation.
The same is also true when the G19 command is used.
Example)

:
(G01 C90. ;)
G43.4 H1 ;
G18 G02

;

After the G43.4 command, the Z-X plane is selected using the G18
command and the C-axis is rotated during circular interpolation .

→

Alarm (violation of <2>)
The same is also true when the G19 command is used.
Example)

:
G43.4 H1 ;
G18 G02

C20. ;

After the G43.4 command, the Z-X plane is selected using the G18
command and circular interpolation is performed after rotating the
C-axis.

→

Alarm (violation of <2>)

The same is also true when the G19 command is used.
Example)

:
G43.4 H1 ;
G01 C10.
G18 G02

;

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 792 -

•

In the case of a table rotation type machine

Descriptions are based on the following machine configuration.

A table rotation type machine can be considered equivalent to a
composite type machine if any of its two table rotation axes does
not move.

Workpiece coordinate
system

When the G17 (X-Y plane) command is executed

The master axis (A-axis) moves before the G43.4 command and, after
the G43.4 command, circular interpolation is performed without
rotating the A- or C-axis (including those cases where the C-axis
moves before the G43.4 command).

→

This case corresponds to

<2> and allows circular interpolation.
Example)

:
G01 A90. (C10.);
G43.4 H1 ;
G17 G02

;

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 793 -

The master axis (A-axis) moves before the G43.4 command and, after
the G43.4 command, circular interpolation is performed using the G17
(X-Y plane) command by rotating the C-axis, or the C-axis is rotated
during circular interpolation.

→

Alarm (violation of <2>)

Example)

:
G01 A90.;
G43.4 H1 ;
G01 C10. ;
G17 G02

;

:
:
G01 A90.;
G43.4 H1 ;
G17 G02

C10.;

After the G43.4 command, the A-axis is moved and circular
interpolation is performed using the G17 command (X-Y plane).

→

Alarm (violation of <2>)
Example)

:
G43.4 H1 ;
G01 A10. ;
G17 G02

C10.;

G19 (Y-Z plane) command is executed
The G43.4 command is executed after moving the A-axis and circular
interpolation is performed while rotating the A-axis using the G19
(Y-Z plane) command.

→

This case corresponds to <1> and

allows circular interpolation.
Example)

:
G01 A90. ;
G43.4 H1 ;
G19 G02

A10. ;

After the G43.4 command, the C-axis is rotated and circular
interpolation is performed using the G19 (Y-Z plane) command.

→

Alarm (violation of <2>)
Example)

:
G43.4 H1 ;
G01 C10. ;
G19 G02

;

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 794 -

When the G18 (Z-X plane) command is executed
The G43.4 command is executed after moving the A- and C-axes, and
circular interpolation is performed using the G18 (Z-X plane)
command without moving any rotary axis.

→

This case corresponds

to <2> and allows circular interpolation.
Example)

:
G01 A90. C10. ;
G43.4 H1 ;
G18 G02

;

After the G43.4 command, circular interpolation is performed using
the G18 command (Z-X plane) by moving any of the rotary axes.

→

Alarm (violation of <2>)
Example)

:
G43.4 H1 ;
G01 A10. (C10.)
G18 G02

;

- Tool center point control command

During tool center point control, the command specifies the location
of each block end point as seen from the programming coordinate
system.
The program specifies the tool center point.
As for the rotary axis, the command specifies the coordinate values of

each block end point in the case of type 1 or the tool direction at each
block end point in the case of type 2.

The feedrate is specified by the tangential speed relative to the
workpiece (the tool's relative speed as opposed to the workpiece),
which is represented by F.

- Commands that can be specified during tool center point control

The commands that can be specified during tool center point control

are linear interpolation (G01), positioning (G00), circular
interpolation (G02, G03), and helical interpolation (G02, G03).

When linear interpolation (G01) is specified during tool center point

control, speed control is exerted so that the tool center point moves at
the specified speed.

The circular interpolation command (G02, G03) controls the

tangential speed of the arc path along which the tool center point
moves.

The helical interpolation command (G02, G03) controls the tangential

speed of the arc path along which the tool center point moves or a
synthetic speed including that of the helical axis. (This is dependent
on the setting of bit 5 (HTG) of parameter No.1403.)

As the actual speed, the speed at the control point is shown.

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 795 -

NOTE

When the tool center point control mode is entered,
acceleration/deceleration before look ahead
interpolation is enabled automatically. Be sure to
specify the following parameters:

(1) Bit 1 (LRP) of parameter No.1401=1 :

Linear rapid traverse

(2) Bit 5 (FRP) of parameter No.19501=1 :

Acceleration/deceleration before interpolation
is used for rapid traverse.

(3) Parameter No.1671 :

Acceleration before interpolation for rapid
traverse.

(4) Parameter No.1672 :

Change time for bell-shaped acceleration
before interpolation for rapid traverse.

(5) Parameter No.1660 :

Maximum permissible acceleration for
acceleration/deceleration before interpolation

If they are not specified, alarm PS5420 is
generated.

- Rotary axis command

If a command is specified during tool center point control that
prohibits the tool center point from moving with respect to the
workpiece, the maximum cutting speed (parameter No.1430) is
assumed as the feedrate of the rotary axis when bit 6 (RFC) of
parameter No.19696 is 0, and the speed specified by F is assumed
when bit 6 (RFC) of parameter No.19696 is 1.
The rotary axis command cannot be specified during tool center point
control of type 2. Specifying the command with type 2 causes alarm
PS5421.

- The moving distance of the rotary axis is long compared to that of the linear axis

If the moving distance of the rotary axis is long compared to that of

the linear axis, the rotary axis moves faster so that the tool center
point moves at the specified speed, possibly resulting in the tool
center point traveling on an inadequate path.

In such a case, it is possible to exert control to slow down the speed

and ensure that the tool center point travels on the specified path, by
setting bit 6 (CRS) of parameter No.19746 to 1. When using this
control, specify in parameter No.19751 (for rapid traverse) and
parameter No.19752 (for cutting feed) the extent of deviation of the
path at which the speed is to be slowed down (maximum allowable
deviation of the path). When 0 is specified, the least input increment
is regarded as the maximum allowable deviation of the path.

Content .. 102 103 104 105 ..