FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 56

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 404 -

- Workpiece setting error compensation mode

By specifying G54.4 Pn (n: 1 to 7), the workpiece setting error
compensation mode is set.
With Pn, select a workpiece setting error from No. 01 to No. 07.
In the workpiece setting error compensation mode, the program is
executed in a "workpiece setting coordinate system" defined by
shifting the workpiece coordinate system.
G54.4 is a modal G code that belongs to group 33 with the M series or
group 26 with the T series.
By specifying G54.4 P0, the workpiece setting error compensation
mode is canceled.

In a block for starting workpiece setting error compensation, the
machine is not moved, but the absolute coordinates are changed by the
error. So, the next absolute command makes a movement to a
specified position in the workpiece setting coordinate system. This
means that an absolute command is needed after a block for starting
workpiece setting error compensation.

NOTE

1 Be sure to specify Pn in a block specifying G54.4.

If P is not specified, or a number (n) not within the
specifiable range is specified after P, alarm
PS0437 is issued.

2 Specify G54.4 singly. If another G code or axis

command is specified together, alarm PS0437 is
issued.

3 Workpiece setting error compensation is valid for

movement in automatic operation.

4 Any workpiece setting error between starting

blocks remains valid until the workpiece setting
error compensation mode is canceled.

5 Workpiece setting error compensation may not be

specified doubly. If G54.4 Pn (n 0) is specified in
the workpiece setting error compensation mode,
alarm PS0437 is issued.

6 No absolute coordinate is changed in a block for

starting workpiece setting error compensation
unless the two angles stated below exceed the
value specified in parameter No. 11204.

(1) Angle made by the current absolute coordinate

point and a singular point posture

(2) Angle made by a point sifted by a workpiece

setting error from the absolute coordinate point
and a singular point posture

7 If all the errors are 0, issuing the G54.4 command

cannot put the workpiece setting error
compensation mode in effect.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 405 -

- Tool direction compensation on a 5-axis machine

With a 5-axis machine, tool direction compensation must be
performed by setting bit 0 (RCM) of parameter No. 11200 to 1. This
means that rotation axis position compensation is performed to direct
the tool as programmed relative to the workpiece.
For tool direction compensation, the following parameters must be set:

Parameter No.

Description

19680

Type of mechanical section

19681

Controlled axis number of the first rotation axis

19682

Axis direction of the first rotation axis

19683

Inclination angle when the first rotation axis is inclined

19684

Rotation direction of the first rotation axis

19685

Rotation angle when the first rotation axis is a hypothetical axis

19686

Controlled axis number of the second rotation axis

19687

Axis direction of the second rotation axis

19688

Inclination angle when the second rotation axis is inclined

19689

Rotation direction of the second rotation axis

19690

Rotation angle when the second rotation axis is a hypothetical axis

19696#0

Whether the first rotation axis is an ordinary rotation axis/hypothetical
axis

19696#1

Whether the second rotation axis is an ordinary rotation
axis/hypothetical axis

19697

Tool axis direction

19698

Reference angle RA

19699

Reference angle RB

19700

Rotary table position (X-axis of the basic three axes)

19701

Rotary table position (Y-axis of the basic three axes)

19702

Rotary table position (Z-axis of the basic three axes)

19703

Intersection offset vector between the first and second rotation axes of
the table (X-axis of the basic three axes)

19704

Intersection offset vector between the first and second rotation axes of
the table (Y-axis of the basic three axes)

19705

Intersection offset vector between the first and second rotation axes of
the table (Z-axis of the basic three axes)

With a 5-axis machine, it is recommended that Workpiece setting
error compensation is commanded after AICC(AI contouring control)
is already active.(G05.1 Q1 is commanded or bit 0 (SHP) of
parameter No.1604 is 1.) And, the following parameters for
Acc/Deceleration are needed.

Parameter No.

Description

1432

Maximum cutting feedrate in the acceleration/deceleration before
interpolation mode

1660

Maximum allowable acceleration rate in acceleration/deceleration
before interpolation

1671

Maximum allowable acceleration rate for rapid traverse in
acceleration/deceleration before interpolation

1672

Acceleration/deceleration change time for rapid traverse in
bell-shaped acceleration/deceleration before interpolation

1737

Allowable acceleration rate for each axis when the deceleration
function based on acceleration/deceleration under AI contour control.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 406 -

Parameter No.

Description

1769

Time constant for acceleration/deceleration after cutting feed
interpolation in the acceleration/deceleration before interpolation mode

1772

Acceleration/deceleration change time in bell-shaped
acceleration/deceleration before interpolation

1783

Allowable speed difference in speed determination based on a corner
speed difference

NOTE

1 If any of the parameters above is set incorrectly, alarm

PS0438 is issued.

2 Depending on the machine configuration, it may be

physically impossible to orient the tool in the compensation
direction. In such a case, alarm DS0030 is issued.

3 In a block for starting workpiece setting error compensation,

the absolute coordinate on a rotation axis is changed
considering the workpiece setting error. At this time,
depending on the machine configuration, a rotation axis for
orienting the tool in the tool direction as viewed from the
workpiece setting coordinate system may be absent. In
such a case, alarm PS0438 is issued.

4 In the workpiece setting error compensation mode,

look-ahead acceleration/deceleration before interpolation is
automatically valid. Moreover, be sure to set the following
parameters:
(1) Bit 1 (LRP) of parameter No. 1401=1:

Linear rapid traverse

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

Use acceleration/deceleration before interpolation for
rapid traverse.

(3) Parameter No. 1671:

Maximum allowable acceleration rate for rapid traverse
in acceleration/deceleration before interpolation

(4) Parameter No. 1660:

Maximum allowable acceleration rate in
acceleration/deceleration before interpolationIf the
parameters above are not set, alarm PS0438 is issued.

5 When TCP(Tool center point control) or G53.1 of TWP(Tilted

working plane command) is used during Workpiece setting
error compensation, Tool direction compensation is needed
(Bit 0 (RCM) of parameter No.11200 is 1. ) Otherwise, in
the case of TCP, the alarm PS5421, in the case of G53.1 of
TWP, the alarm PS5458 occurs.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 407 -

If linear interpolation or circular interpolation is specified on a
machine of table rotation type or composite type, linear interpolation
or circular interpolation is performed as viewed from the workpiece
on the table.

<Example>

The machine is a table rotation type with A axis(master axis)
around X axis and C axis (slave axis) around Z axis (when A=0).

Firstly, suppose that Workpiece setting error is 0 and the
following program is commanded.

O1
N10 G55 (G55 is X50.0 Y0.0 Z0.0.)
N20 X0 Y0 Z0 A0 C0
N30 G01 X

－

50.0 Y150.0 C

－

90.0 F100.0

Next, suppose that Workpiece setting error has

∆

c=5.0, which is

the error around Z axis, and N15,N16 are added to O2 as follows :

When Tool direction compensation is available (Bit 0 (RCM) of

parameter No.11200 is 1), the path will be as follows :

O2
N10 G55
N15 G05.1 Q1
N16 G54.4 P1
N20 X0 Y0 Z0 A0 C0
N30 G01 X

－

50.0 Y150.0 C

－

90.0 F100.0

The path looked from the workpiece in the middle of the block is
linear.

C -90

N20 end

N30 end

Path in the middle
of the block

Path looked from the
workpiece in the middle of
the block

C -90

N20 end

N30 and

Path in the middle
of the block

Path looked from the
workpiece in the middle of
the block

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 408 -

- "Rotation axis closer to the tool" and "rotation axis closer to the workpiece" on a

5-axis machine

When tool direction compensation is performed on a 5-axis machine, a
singular point and singular point posture need to be considered. Here,
a "rotation axis closer to the tool" and "rotation axis closer to the
workpiece", which are used in a description of a singular point and
singular point posture provided later, are explained.
On a 5-axis machine with two rotation axes, one rotation axis
functions to tilt the tool toward the workpiece. This rotation axis is
referred to as a "rotation axis closer to the tool".
The other rotation axis is referred to as a "rotation axis closer to the
workpiece".
Depending on the type of mechanical section, the rotation axis closer
to the tool and rotation axis closer to the workpiece are determined as
indicated in Table 1.

Table 15.5 "Rotation axis closer to the tool" and "rotation axis closer to

the workpiece"

Type of mechanical

section (No. 19680)

Rotation axis closer

to the tool

Rotation axis closer

to the workpiece

Tool rotation type (2)

Slave axis

Master axis

Table rotation type (12)

Master axis

Slave axis

Composite type (21)

Tool rotation axis

Table rotation axis

Tool rotation type

Table rotation type

Composite type

Rotation axis closer to the tool

Rotation axis closer to the workpiece

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 409 -

- Singular point and singular point posture on a 5-axis machine

A tool posture is uniquely determined when the angles of the two
rotation axes are determined.  Usually, however, a combination of
the angles of the two rotation axes for achieving a certain tool posture
is not determined uniquely.
In particular, such a tool posture that the angle of the rotation axis
closer to the tool is arbitrary is referred to as a "singular point posture".
Moreover, such an angle of the rotation axis closer the tool that the
tool posture becomes a singular point posture is referred to as a
"singular point (or singular point angle)".  When the angle of the
rotation axis closer to the tool is a singular point, the center of the
rotation axis closer to the workpiece and the tool posture (tool
direction) are parallel with each other.
Example:

When the C-axis (about the Z-axis) is the master axis, the B-axis
is the slave axis (about the Y-axis), and the reference tool axis
direction is along the Z-axis on a 5-axis machine of tool rotation
type, the singular point is B = …, 0 deg, 180 deg, .... At this
time, an arbitrary C-axis angle represents a singular point posture
(in the same direction as the Z-axis or in the direction opposite to
the Z-axis).

If the angle of the B-axis is B = 0 (singular point) as shown in
Fig. 4, for example, an arbitrary C-axis angle represents the same
tool posture (singular point posture).

Fig. 15.5 (d) Singular point and singular point attitude

When the reference tool axis direction is inclined (parameter No.
19698, No. 19699), or the rotation axis is an angular axis (parameter
No. 19682, No. 19683, No. 19687, No. 19688), for example, no
singular point and singular point posture exist on some machines.

B=0

(Singular

point)

C=0

C=60

B=0

(Singular

point)

Singular point

posture

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 410 -

- Conditions to decide that Tool is in singular posture

When the angle between the tool and the singular posture is less than
the parameter No.11204, it is decided that the tool is in singular
posture.
In the descriptions below, the description ‘when the tool is in
singular…’ means that ‘when it is decided that the tool is in singular
posture….’.
In addition, whether the tool is in singular point posture is decided at
each end point of tool paths calculated in the NC.    If the parameter
No. 11204 value is very small and the feedrate and the override value
are large, it is likely that the tool may pass by a singular point without
deciding that the tool is in a singular point posture at each end point
even when the tool path crosses the singular point.    In this case, the
tool will not be able to go beyond the singular point.    To avoid this
problem, set parameter No. 11204 with a value slightly larger than the
quotient of the division of the highest rotation axis move speed (the
highest cutting feedrate (parameter No. 1432) among the rotation axes
or the rapid traverse rate (parameter No. 1420) whichever is higher)
by 15000.

- Movement in the case that Tool direction is compensated

In the case that the tool direction is compensated (bit 0 (RCM) of
parameter No.11200=1) on a 5 axis machine, the compensation is
performed in every interpolation, and the rotation axes may move to
positions which are different from the commanded positions.
In general, there are two pairs of rotation axes positions in the region
between 0 degree to 360 degree to turn the tool in a certain direction.
And in the case that the tool is in singular point posture, the position
of the rotation axis closer to the workpiece is not determined uniquely.
How the positions are determined is described as follows :
(1) In the case that the current machine position is singular and the

position after movement in real time is also singular.
(a) When the absolute position after movement in real time is

not singular, the rotation axis closer to the workpiece does
not move.

Example:

The rotation axis about the Z-axis is the master axis,
the rotation axis about the Y-axis is the slave axis, and
the reference tool axis direction is along the Z-axis on
a 5-axis machine of tool rotation type.

The tool posture before movement

The tool posture after movement
(Not singular)

The tool posture in the
absolute coordinate system

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 411 -

Assume that the workpiece setting error around the
Y-axis exists, and the tool posture after the
compensation of tool direction becomes like following
figure. (The tools before and after movement are in
singular point posture.)

In this case, the rotation axis about the Z-axis (the
rotation axis closer to the workpiece) does not move.
(Only the rotation axis closer to the tool moves.)

If the parameter No.11204 is set to the value except 0,
the tools both before and after movement may be in
singular point posture like the above example.

In this case, the rotation axis closer to the workpiece
does not move. The rotation axis closer to the tool
moves in the move direction in which the tool in the
machine system (machine coordinate system) is
decided to be in a singular point posture, but not move
in the opposite direction.

The tool posture in the
machine coordinate system

The calculated tool
posture after movement
(Singular)

The tool posture before movement
(Singular)

The actual tool posture after
movement

Content .. 54 55 56 57 ..