Content .. 107 108 109 110 ..

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 109

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 828 -

22.2

TOOL POSTURE CONTROL

Overview

Under tool center point control, the tool tip moves along a specified
path even when the tool direction relative to the workpiece changes.
Usually, however, the two rotary axes are controlled independently of
each other, and the posture of the tool is not controlled.
Under tool posture control, the tool posture is controlled every
moment for operation on the plane formed by the tool postures (tool
length compensation vectors) at the start point and end point of a
block.
This control method is suitable for machining a plane with the side of
a tool by using tool center point control.

Tool posture control

Plane formed by Vs and Ve

Tool length compensation

vector Vs at block start point

Tool length compensation

vector Ve at block end point

Programmed path

Fig. 22.2 (a) Tool posture control

This function is optional. The tool center point control option is also
needed.

Format

G43.4

_ H_ P_ ; Tool center point control (type 1)

G43.5

_ H_ Q_ P_ ;

Tool center point control (type 2)

Description of symbols

: For an absolute command, the coordinates of travel end point of the tool

center point

For an incremental command, the travel distance of the tool center point

: For an absolute command, the coordinates of the end point of the rotation axis

For an incremental command, the travel distance of the rotation axis

H  : Tool offset number
Q  : Tool tilted angle (degree)
P  : Tool posture control disabled (P0) or tool posture control enabled (P1)

However, bit 0 (TPC) of setting parameter No. 19604 can be used to select
the behavior taken when the address P command is not present.

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 829 -

Tool posture control is enabled when P1 is specified or disabled when
P0 is specified in the G43.4 and G43.5 blocks. The behavior taken
when the address P command is not present can be selected by bit 0
(TPC) of parameter No. 19604. The setting of tool posture control
selected in the G43.4 and G43.5 blocks is kept until the tool center
point control cancellation command (G49) is specified.

Example:

O0010
…
N10 G90 G00 X30.0 Y-30.0 Z0.0;
N20 G43.5 H1 P1;
N30 G42.6 D2;
N40 G01 X20.0 Y-20.0 I-1 J1 K2 F_;
N50 Y20.0 I-1 J-1 K2;
N60 X-20.0 I1 J-1 K2;
N70 Y-20.0 I1 J1 K2;
N80 X20.0 I-1 J1 K2;
…
G40;
G49;
M30;

In N20 to N80 in program O0010 to the
left, the sides of a quadrangular pyramid
trapezoid as shown below can be
machined by the side of the tool using
tool posture control. The following figure
illustrates tool movement by N50. The
command in N30 is the three-dimensional
cutter compensation command.

Fig. 22.2 (b) Example of tool posture control

Explanation

In tool posture control, the two rotation axes are controlled so that the
momentary tool posture (tool length compensation vector) satisfies the
following conditions (Fig. 22.2 (c)).
The momentary tool posture (tool length compensation vector) is

present on the plane configured by the tool length compensation
vector at the block start point and that at the block end point.

The angle which the tool length compensation vector at the block start

point makes with the momentary tool length compensation vector
is the angle obtained by proportionally dividing the angle which
the tool length compensation vector at the block start point makes
with the tool length compensation vector at the block end point.

Tool posture control is enabled when P1 is specified or disabled when
P0 is specified in the tool center point control start command
(G43.4/G43.5) blocks. Bit 0 (TPC) of setting parameter No. 19604
can be used to select whether tool posture control is enabled or
disabled when the address P command is not present. The setting of
tool posture control selected in the G43.4 and G43.5 blocks is kept
until the tool center point control cancellation command (G49) is
specified.

This function can be used for positioning (G00) and linear
interpolation (G01) during tool center point control.

Other notes and restrictions are the same as those for tool center point
control.

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 830 -

Program specification path

Control
point

Tool center
point

Block start point

Block end point

Plane configured by tool length compensation vectors Vs and Ve
Momentary tool length compensation vector V is controlled so as to
be present on the plane.

Control is made so that angle

which Vs makes with V

satisfies this expression.

Fig. 22.2 (c) Tool posture control

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 831 -

Singular point
- "Tool-side rotary axis" and "workpiece-side rotary axis"

When tool center point control type 2 is specified, programming needs
to be performed considering a singular point and singular point
posture. The "tool-side rotary axis" and "workpiece-side rotary axis"
used in the descriptions of a singular point and singular point posture
later are explained below.
On a 5-axis machine that has two rotary axes, one rotary axis has a
function for tilting the tool toward a workpiece. This rotary axis is
referred to as a "tool-side rotary axis".
The other rotary axis is referred to as a "workpiece-side rotary axis".
The table below indicates the axes that represent these rotary axes for
each mechanical unit type.

Table 22.2 (a) "Tool-side rotary axis" and "workpiece-side rotary axis"

Mechanical unit type

(parameter No. 19680)

Tool-side rotary axis

Workpiece-side rotary

axis

Tool rotation type (2)

Slave axis

Master axis

Table rotation type (12)

Master axis

Slave axis

Composite type (21)

Tool rotary axis

Table rotary axis

Tool rotation type

Table rotation type

Composite type

Tool-side rotary axis

Workpiece-side rotary axis

Fig. 22.2 (d) "Tool-side rotary axis" and "workpiece-side rotary axis"

- Singular point, singular point posture

A tool posture is uniquely determined when the angular displacements
of the two rotary axes are determined. However, a combination of
the angular displacements of the two rotary axes for determining a
particular tool posture is not uniquely determined usually.
In particular, a tool posture with the angular displacement of the
workpiece-side rotary axis being arbitrary is referred to as a "singular
point posture", and the angular displacement of the tool-side rotary
axis that causes the tool posture to assume a singular point posture is
referred to as the "singular point (or singular point angular
displacement)". When the angular displacement of the tool-side
rotary axis is at a singular point, the center of the workpiece-side

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 832 -

rotary axis and the tool posture (tool orientation) are parallel with each
other.
Example)

Suppose that a tool rotation type machine is used, the master axis
is the C-axis (about the Z-axis), the slave axis is the B-axis
(about the Y-axis), and the reference tool axis direction is the
Z-axis direction. In this case, singular point B = ..., 0

, 180

, ...,

and a singular point posture (the same direction as the Z-axis
direction or the direction opposite to the Z-axis direction) results
at an arbitrary C-axis angular displacement.

For example, when the B-axis angular displacement is B = 0 (singular
point) as shown in Fig. 22.2 (e), the same tool posture (singular point
posture) is assumed at an arbitrary C-axis angular displacement.

C=0

C=60

B=0

(Singular point)

Singular point

posture

B=0

(Singular point)

Fig. 22.2 (e) Singular point and singular point posture

There is no singular point and singular point posture on some types of
machines as in the case where the reference tool axis direction is tilted
(parameter No. 19698 and No. 19699) or a rotary axis is an angular
axis (parameter No. 19682, No. 19683, No. 19687, and No. 19688).

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 833 -

- When the tool posture is close to a singular point posture

When tool posture control is exercised on a machine that has a
singular point, and the tool posture becomes close to a singular point
posture during execution of a block, the operation of the
workpiece-side rotary axis can become so large, resulting in unstable
machine operation.
In such a case, machine operation can be made stabler, the machining
time can be reduced, and the surface roughness can be improved by
changing the tool posture at the block end point so that the tool
posture passes through a singular point posture.

A large and abrupt movement is made on
the workpiece-side rotary axis when the tool
posture passes through a singular point

close posture.

A large and abrupt movement on the workpiece-side
rotary axis can be avoided by passing through a
singular point posture. By passing through a
singular point posture, the tool posture at the block

end is changed within the allowable range.

Fig. 22.2 (f) Changing the tool posture at a block end point

When tool posture control is used, and the angle between a tool
posture and singular point posture is equal to or less than the value of
(parameter No. 19738), the tool posture is determined to be close to a
singular point posture.    The tool posture at this time is referred to as a
"singular point close posture". When tool center point control is
specified (G43.5) based on type 2, which specifies the tool posture at
the block end point with tool axis direction (I, J, K), each block is
checked to see if a singular point close posture is assumed.  If a
singular point close posture is assumed in a block, the tool posture at
the end point of the block is changed (the rotary axis angular
displacement is changed) to pass through a singular point posture.    If
the end points before and after the workpiece-side rotary axis is
changed vary largely from each other as the result of changing the tool
posture at the block end point, the change in the tool posture at the
block end point can be suppressed.
However, if the value of parameter No. 19738 is 0, the tool posture at
the block end point is not changed.
If the tool posture at the start point or end point of a block is a singular
point posture or the tool posture becomes a singular point posture in
the middle of a block, the tool posture is not changed at the block end
point.

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 834 -

If this angle is equal to or
less than the value of
parameter No. 19738, a
singular point close
posture is assumed.

Tool posture

Singular
point posture

Fig. 22.2 (g) Singular point close posture

If a singular point close posture is assumed during execution of a
block, change the angular displacements of the rotary axes at the end
point of the block calculated from the tool posture specified by (I, J,
K) so that the tool posture passes through a singular point posture in
the block as indicated below.
Tool-side rotary axis:

Turned reversely relative to the singular point angular
displacement
Example:

When the end point angular displacement before a change is
60

, and the singular point angular displacement is 20

, the

end point angular displacement after a change is -20

Workpiece-side rotary axis:

Same as the angular displacement at the start point
Example:

When the end point angular displacement after a change is
30

, and the start point angular displacement is -150

, the

end point angular displacement after a change is -150

However, if both of the difference between the end point angular
displacement before a change and (end point angular displacement
after a change + 180

) and the difference between the end point

angular displacement before a change and (end point angular
displacement after a change - 180

) are equal to or greater than the

value of parameter No. 19739, the program is executed according to
the setting of bit 3 (NPC) of parameter No. 19696, suppressing the
change, or alarm PS5421 is issued.
This function is used to avoid unstable machine operation in a block
where a singular point close posture is assumed as shown in Fig. 22.2
(f).

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 835 -

Notes
- When the reference tool axis or a rotary axis is inclined

When tool center point control is used, the inclination of the reference
tool axis can be set in parameter No. 19698 and No. 19699, and the
inclination of a rotary axis can be set in parameter No. 19682, No.
19683, No. 19687 and No. 19688.
On a machine with the reference tool axis or a rotary axis being
inclined, all tool postures cannot be assumed. Some tool postures
can never be assumed by setting the angular displacements of the two
rotary axes in any way. If the tool posture passes through any of
those impossible tool postures during program execution when tool
posture control is enabled, alarm PS0432 is issued before execution of
the block.
Example:

On 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), and the reference tool axis direction is inclined relative
to the positive Z-axis direction (a non-zero value is set in
parameter No. 19698 and No. 19699), no tool posture can be
assumed in the positive or negative direction of the Z-axis. So,
if a block specifies such a tool posture during tool posture control,
alarm PS0432 is issued before execution of the block.

O0010
…
G43.5 H1 P1;
…
N10 X_ Y_ Z_ I1 J0 K2;
N20 X_ Y_ Z_ I-1 J0 K2;
…
G49;
M30;

I1 J0 K2;

Positive Z-axis direction

I-1 J0 K2;

If O0010 is executed on the machine in
the example above, the tool posture
assumes the positive Z-axis direction
during N20, so alarm PS0432 is issued
before execution of N20.

Fig. 22.2 (h) Example of impossible tool posture

Content .. 107 108 109 110 ..