FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 110

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 836 - 

  - When the operation range of rotary axes is specified 

When tool center point control is used, the operation range of rotary 
axes can be set in parameter No. 19741 to No. 19744. 
If either of the rotary axes exceeds the set operation range during 
program execution when tool posture control is enabled, alarm 
DS0029 is issued. 
If tool posture control is disabled, rotary axis operation range 
specification based on parameter No. 19741 to No. 19744 is enabled 
only when the tool center point control type 2 command (G43.5) is 
specified.  If tool posture control is enabled, the check mentioned 
above can be made even when the tool center point control type 1 
command (G43.4) is specified. 
If the operation range of the first rotary axis is not specified, set 0 in 
both of parameter No. 19741 and No. 19742. 
If the operation range of the second rotary axis is not specified, set 0 
in both of parameter No. 19743 and No. 19744. 
 

  - When tool center point control type 1 is used 

Tool posture control can also be exercised by using the tool center 
point control type 1 command (G43.4), which specifies the tool 
posture at the end point of a block with the angular displacements of 
the two rotary axes.    However, when tool posture control is exercised 
using the tool posture at the end point of a block calculated from the 
rotary axis angular displacement specified by the program, alarm 
PS5421 is issued before execution of the block if the 
program-specified rotary axis angular displacement does not result. 
Example: 
 

Suppose that a tool rotation type machine where the master axis 
is the C-axis (about the Z-axis), the slave axis is the B-axis 
(about the Y-axis), the reference tool axis direction is the Z-axis 
direction, and the reference tool axis and rotary axes are not 
inclined is used.    If the rotary axis angular displacements at the 
end point of a block are specified as (B, C) = (-90

°

, -90

°

) (with 

the tool posture being in the positive Y-axis direction) when the 
rotary axis angular displacements at the start point of the block 
are (B, C) = (90

°

, 0

°

) (with the tool posture being in the positive 

X-axis direction), tool posture control needs to maintain the tool 
posture in parallel with the XY plane.  In this state, however, 
the specified end point (B, C) = (-90

°

, -90

°

) cannot be reached, 

so that alarm PS5421 is issued. 
If (B, C) = (90

°

, 90

°

) for representing the same tool posture in 

the positive Y-axis direction at the end point of a block is 
specified, tool posture control is possible. 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 837 - 

O0020 
… 
G43.4 H1 P1; 
… 
N10 X_ Y_ Z_ B90.0 C0.0; 
N20 X_ Y_ Z_ B-90.0 C-90.0;
… 
G49; 
M30; 

O0021 
… 
G43.4 H1 P1; 
… 
N10 X_ Y_ Z_ B90.0 C0.0; 
N20 X_ Y_ Z_ B90.0 C90.0;
… 
G49; 
M30; 

 

X

Y 

B=90.0, C=0.0

B=90.0, C=90.0 
or B=-90.0, C=-90.0

At the N20 end point of both of the programs 
O0020 and O0021, the tool posture is in the 
positive Y-axis direction.    However, the N20 
end point (B=-90.0, C=-90.0) of O0020 
cannot be reached from the N10 end point 
(B=90.0, C=0.0) by tool posture control.    So, 
alarm PS5421 is issued with O0020.   
However, the N20 end point (B=90.0, C-90.0) 
of O0021 can be reached by tool posture 
control. 

 

Fig. 22.2 (i)    Example where tool posture control is impossible when 

type 1 is specified 

 

  - When the tool posture directions at the start point and end point of a block match 

each other 

If the direction of the tool posture at the start point of a block matches 
the direction of the tool posture at the end point of the block (same 
direction or opposite direction), no plane can be determined by these 
tool postures.  So, tool posture control in that block is temporarily 
disabled.    However, whether to enable/disable tool posture control is 
kept as modal information.  So, tool posture control temporarily 
disabled for the cause mentioned above is enabled again in the 
subsequent blocks. 
 
For other notes, those described for tool center point control are 

applicable. 

 

Limitation 

This function is enabled for positioning (G00) and linear interpolation 
(G01). 
 
For other restrictions, those described for tool center point control are 
applicable. 
 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 838 - 

22.3 

TILTED WORKING PLANE COMMAND 

 

22.3.1 

Tilted Working Plane Command 

 

Overview 

Programming for creating holes, pockets, and other figures in a datum 
plane tilted with respect to the workpiece would be easy if commands 
can be specified in a coordinate system fixed to this plane (called a 
feature coordinate system).  This function enables commands to be 
specified in the feature coordinate system.  The feature coordinate 
system is defined in the workpiece coordinate system. 
For explanations about the relationship between the feature coordinate 
system and workpiece coordinate system, see Fig. 22.3 (a). 
 

Feature coordinate

system

(G68.2)

Machine coordinate system

Workpiece

coordinate system

(G54)

 

Fig. 22.3 (a)    Feature coordinate system 

 
The G68.2 command causes the programming coordinate system to 
switch to the feature coordinate system.  The commands in all 
subsequent blocks are assumed to be specified in the feature 
coordinate system until G69 appears. 
If G68.2 specifies the relationship between the feature coordinate 
system and the workpiece coordinate system, G53.1 automatically 
specifies the +Z direction of the feature coordinate system as the tool 
axis direction even if no angle is specified for the rotary axis.    (See 
Fig. 22.3 (c).) 
For explanations about the tool axis direction, see Fig. 22.3 (b). 
 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 839 - 

X

Y

Z

The tool axis direction is the
+Z-axis direction.

The tool axis direction is the
+Y-axis direction.

The tool axis direction is the +X-axis direction.

 

Fig. 22.3 (b)    Tool axis direction 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 840 - 

This function regards the direction normal to the machining plane as 
the +Z-axis direction of the feature coordinate system.  After the 
G53.1 command, the tool is controlled so that it remains perpendicular 
to the machining plane. 
 

Coordinate system

origin shift

(xo,yo,zo)

Xc

Yc

Zc

Workpiece

coordinate system

X-Y-Z

Feature coordinate

system

Xc-Yc-Zc

X

Y

Z

•

    Only G68.2 is specified

•

    G53.1 is specified after G68.2

Xc

Yc

Zc

Control point shift (by

another command)

G53.1 automatically controls

the rotary axis.

X

Y

Z

B

C

Feature coordinate

system

Xc-Yc-Zc

Coordinate system

origin shift

(xo,yo,zo)

Workpiece

coordinate system

X-Y-Z

 

Fig. 22.3 (c)    G68.2 and G53.1 commands 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 841 - 

This function is applicable to the following machine configurations.  
(See Fig. 22.3 (d).) 
<1>  Tool rotation type machine controlled with two tool rotation 

axes 

<2>  Table rotation type machine controlled with two table rotation 

axes 

<3>  Composite type machine controlled with one tool rotation axis 

and one rotary axis 

 

The function can also be used for a machine configuration in which 
the rotary axis for controlling the tool does not intersect the rotary axis 
for controlling the table. 

 

<2>  Table rotation type 

machine

 

<3> Composite type 

machine

 

<1> Tool rotation 

type machine 

X

C

B

Z

Y

A

C

X

 

Z

Y

B

Y

X

 

Z

C

 

Fig. 22.3 (d)    Three types of 5-axis machine 

22.5-AXIS MACHINING FUNCTION

 PROGRAMMING 

B-63944EN/03

 

 

- 842 - 

Format 
  - Tilted working plane command (G68.2) 

M

 

G68.2 X x

0

 Y y

0

 Z z

0

 I

α

 J

β

 K

γ

 ; 

Tilted working plane command

 

G69 ; 

Cancels the tilted working plane command.

 

 

X, Y, Z : Feature coordinate system origin 
 

  The axes specified here are the three axes of the 

feature coordinate system.    Specify the three 
basic axes or parallel axes set by parameter No. 
1022.    When specification is omitted, the X, Y, 
and Z of the basic three axes are assumed to be 0.

I, J, K  : Euler's angle for determining the orientation of the 

feature coordinate system

 

 

T

 

G68.2 X x

0

 Y y

0

 Z z

0

 I

α

 J

β

 K

γ

 ; 

Tilted working plane command

 

G69.1 ; 

Cancels the tilted working plane command.

 

 

X, Y, Z : Feature coordinate system origin 
 

  The axes specified here are the three axes of the 

feature coordinate system.    Specify the three 
basic axes or parallel axes set by parameter No. 
1022.    When specification is omitted, the X, Y, 
and Z of the basic three axes are assumed to be 0.

I, J, K  : Euler's angle for determining the orientation of the 

feature coordinate system

 

 

  - Tool axis direction control (G53.1) 

G53.1 ; 

Controls the tool axis direction.

 

 

 CAUTION 

1  G53.1 must be specified in a block after the block 

that contains G68.2. 

 

An alarm occurs if G53.1 is specified without G68.2 
being specified in a preceding block. 

2  G53.1 must be specified in a block in which there is 

no other command. 

3  The rotary axis moves at the maximum rapid 

traverse federate in the case of rapid traverse and 
at the specified federate in the case of cutting feed. 

 

B-63944EN/03

 PROGRAMMING 

22.5-AXIS MACHINING FUNCTION

 

 

- 843 - 

Explanation 
  - Coordinate conversion using an Euler's angle 

Coordinate conversion by rotation is assumed to be performed around 
the workpiece coordinate system origin. 
Let the coordinate system obtained by rotating the workpiece 
coordinate system around the Z-axis by an angle of 

α

 degrees be 

coordinate system 1.  Similarly, let the coordinate system obtained 
by rotating coordinate system 1 around the X-axis by an angle of 

β

 be 

coordinate system 2.    The feature coordinate system is the coordinate 
system obtained by shifting the coordinate system that is obtained by 
rotating coordinate system 2 around the Z-axis through an angle of 

γ

 

degrees from the workpiece coordinate system origin by (Xo, Yo, Zo). 
Fig. 22.3 (e) shows the relationship between the workpiece coordinate 
system and the feature coordinate system. 
The figure also gives examples of displacement on the X-Y plane. 
 

γ

zc

yc

xc

x'

y''

γ

Conversion from workpiece
coordinate system X-Y-Z to
coordinate system 1 X'-Y'-Z

x

z

y

x'

y'

α

β

X'

z

y''

z''

y'

β

Conversion from coordinate
system 1 X'-Y'-Z to
coordinate system 2 X'-Y"-Z"

Conversion from coordinate system 2 X'-Y"-Z"
to feature coordinate system Xc-Yc-Zc

 

Fig. 22.3 (e)    Coordinate conversion using an Euler's angle 

 

  - I0 J0 K0 command 

When I0 J0 K0 is specified as an Euler's angle, the alarm (PS5457) 
(G68.2 format error) usually occurs.  When bit 1 (ATW) of 
parameter No. 13451 is set to 1, the feature coordinate system with a 
tilted angle of 0 degree is used.