Content .. 52 53 54 55 ..

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 54

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 388 -

Example

Sample program of a scaling in each axis

O1;

G51 X20.0 Y10.0 I750 J250; (

0.75 in the X direction,

0.25 in

the Y direction)

G00 G90 X60.0 Y50.0;

G01 X120.0 F100;

G01

Y90;

G01

X60;

G01

Y50;

G50;
M30;

Y axis

X axis

100

Programmed figure

Scaled figure

Scaling center

120

(60,50)

Fig. 15.2 (g) Program example of scaling in each axis

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 389 -

15.3

PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1)

A mirror image of a programmed command can be produced with
respect to a programmed axis of symmetry (Fig. 15.3 (a)).

100

(1)

(2)

(3)

(4)

(1) Original image of a programmed command
(2) Image symmetrical about a line parallel to the Y-axis and crossing the

X-axis at 50

(3) Image symmetrical about point (50, 50)
(4) Image symmetrical about a line parallel to the X-axis and crossing the

Y-axis at 50

Axis of symmetry (X=50)

Axis of symmetry
(Y=50)

Fig. 15.3 (a) Programmable mirror image

Format

G51.1

_ ;

Setting a programmable image

A mirror image of a command specified in

these blocks is produced with respect to

the axis of symmetry specified by G51.1

_;.

G50.1

_ ;

Canceling a programmable mirror image

_ : Point (position) and axis of symmetry for producing a

mirror image when specified with G51.1.

Axis of symmetry for producing a mirror image when
specified with G50.1. Point of symmetry is not
specified.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 390 -

Explanation
- Mirror image by setting

If the programmable mirror image function is specified when the
command for producing a mirror image is also selected by a CNC
external switch or CNC setting (see III-4.5), the programmable mirror
image function is executed first.

- Mirror image on a single axis in a specified plane

Applying a mirror image to one of the axes on a specified plane
changes the following commands as follows :

Command Explanation

Circular command

G02 and G03 are interchanged.

Tool radius

⋅

tool nose radius

compensation

G41 and G42 are interchanged.

Coordinate system rotation

CW and CCW (directions of rotation)

are interchanged.

Limitation
- Scaling and coordinate system rotation

Processing proceeds from program mirror image to scaling and
coordinate system rotation in the stated order. The commands should
be specified in this order, and, for cancellation, in the reverse order.
Do not specify G50.1 or G51.1 during scaling or coordinate system
rotation mode.

- Commands related to reference position return and coordinate system

In programmable mirror image mode, G codes related to reference
position return (G27, G28, G29, G30, etc.) and those for changing the
coordinate system (G52 to G59, G92, etc.) must not be specified. If
any of these G codes is necessary, specify it only after canceling the
programmable mirror image mode.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 391 -

15.4

NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1)

Overview

When a tool with a rotation axis (C-axis) is moved in the XY plane
during cutting, the normal direction control function can control the
tool so that the C-axis is always perpendicular to the tool path (Fig.
15.4 (a)).

Tool

Programmed tool path

Normal direction (in
which the tool moves)

C-axis

Fig. 15.4 (a) Sample Movement of the tool

Format

G41.1 ;   Normal direction control, left
G42.1 ;  Normal direction control, right
G40.1 ;  Cancel normal direction control

The normal direction control, left (G41.1) command is
used when the workpiece is on the right side of the tool as
viewed while you are looking into the tool’s way.
Once either G41.1 or G42.1 is issued, normal direction
control is enabled (normal direction control mode).
Issuing G40.1 cancels the normal direction control mode.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 392 -

Center of the arc

Programmed tool path

Tool center path

Programmed tool path

Fig. 15.4 (b) Normal direction control, left (G41.1) Fig. 15.4 (c) Normal direction control, right (G42.1)

Explanation
- Angle of the C axis

When viewed from the center of rotation around the C-axis, the
angular displacement about the C-axis is determined as shown in Fig.
15.4 (d). The positive side of the X-axis is assumed to be 0, the
positive side of the Y-axis is 90

, the negative side of the X-axis is

180

, and the negative side of the Y-axis is 270

Center of rotation

180

270

Fig. 15.4 (d) Angle of the C axis

- Normal direction control of the C axis

When the cancel mode is switched to the normal direction control
mode, the C-axis becomes perpendicular to the tool path at the
beginning of the block containing G41.1 or G42.1.
In the interface between blocks in the normal direction control mode,
a command to move the tool is automatically inserted so that the
C-axis becomes perpendicular to the tool path at the beginning of each
block. The tool is first oriented so that the C-axis becomes
perpendicular to the tool path specified by the move command, then it
is moved along the X- and Y axes.
In the cutter compensation mode, the tool is oriented so that the C-axis
becomes perpendicular to the tool path created after compensation.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 393 -

In single-block operation, the tool is not stopped between a command
for rotation of the tool and a command for movement along the X- and
Y-axes. A single-block stop always occurs after the tool is moved
along the X- and Y-axes.

Programmed tool path

S : Single block stop point

Tool center path

Fig. 15.4 (e) Point at which a single-block stop occurs in the normal

direction control mode

Before circular interpolation is started, the C-axis is rotated so that the
C-axis becomes normal to the arc at the start point. During circular
interpolation, the tool is controlled so that the C-axis is always
perpendicular to the tool path determined by circular interpolation.

Center of the arc

Programmed tool path

Tool center path

The tool is controlled so that the C-axis
is always normal to the tool path
determined by circular interpolation.

A rotation command is inserted so
that the C-axis becomes normal to
the arc at the start point.

Fig. 15.4 (f) Normal direction control of the circular interpolation

NOTE

During normal direction control, the C axis always
rotates through an angle less than 180 deg. I.e., it
rotates in whichever direction provides the shorter
route.

15.COMPENSATION FUNCTION

PROGRAMMING

B-63944EN/03

- 394 -

- C axis feedrate

Movement of the tool inserted at the beginning of each block is
executed at the feedrate set in parameter 5481. If dry run mode is on at
that time, the dry run feedrate is applied. If the tool is to be moved
along the X-and Y-axes in rapid traverse (G00) mode, the rapid
traverse feedrate is applied.
The feedrate of the C axis during circular interpolation is defined by
the following formula.

Amount of movement of the C axis (deg)

Length of arc (mm or inch)

(deg/min)

F : Feedrate (mm/min or inch/min) specified by the corresponding

block of the arc

Amount of movement of the C axis :

The difference in angles at the beginning and the end of the
block.

NOTE

If the feedrate of the C axis exceeds the maximum
cutting speed of the C axis specified to parameter
No. 1430, the feedrate of each of the other axes is
clamped to keep the feedrate of the C axis below
the maximum cutting speed of the C axis.

- Normal direction control axis

A C-axis to which normal-direction control is applied can be assigned
to any axis with parameter No. 5480.

- Angle for which figure insertion is ignored

When the rotation angle to be inserted, calculated by normal-direction
control, is smaller than the value set with parameter No. 5482, the
corresponding rotation block is not inserted for the axis to which
normal-direction control is applied. This ignored rotation angle is
added to the next rotation angle to be inserted, the total angle being
subject to the same check at the next block.
If an angle of 360 degrees or more is specified, the corresponding
rotation block is not inserted.
If an angle of 180 degrees or more is specified in a block other than
that for circular interpolation with a C-axis rotation angle of 180
degrees or more, the corresponding rotation block is not inserted.

B-63944EN/03

PROGRAMMING

15.COMPENSATION FUNCTION

- 395 -

- Movement for which arc insertion is ignored

Specify the maximum distance for which machining is performed with
the same normal direction as that of the preceding block.

•

Linear

movement

When distance N2, shown below, is smaller than the set value,
machining for block N2 is performed using the same direction as
that for block N1.

Tool center path

Distance

Programmed tool path

•

Circular

movement

When the diameter of block N2, shown below, is smaller than the
set value, machining for block N2 is performed using the same
normal direction as that for block N1. And control as
compensation along the circular arc is not performed.

Tool center path

Programmed tool path

Diameter

NOTE

1 Do not specify any command to the C axis during

normal direction control. Any command specified at
this time is ignored.

2 Before processing starts, it is necessary to

correlate the workpiece coordinate of the C axis
with the actual position of the C axis on the
machine using the coordinate system setting (G92)
or the like.

3 The helical cutting option is required to use this

function. Helical cutting cannot be specified in the
normal direction control mode.

4 Normal direction control cannot be performed by

the G53 move command.

5 The C-axis must be a rotation axis.

Content .. 52 53 54 55 ..