Content .. 116 117 118 119 ..

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 118

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 900 -

22.5.1

Cutter Compensation in Tool Rotation Type Machine

Overview

In a 5-axis machine having two tool rotation axes as shown in Fig.
22.5.1 (a), this function can perform cutter compensation.
Shown below is a 5-axis machine that has tool rotation axis B on the
Y-axis and tool rotation axis C on the Z-axis.
This machine configuration is used as a sample configuration in the
following explanation unless otherwise noted.

Cutter compensation in tool rotation machines is classified into two
types according to the way of machining: tool side offset and
leading edge offset.

Workpiece coordinate system: A coordinate
system used for creating programs

Z Workpiece coordinate

system

Fig. 22.5.1 (a) Machine having two tool rotation axes

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 901 -

22.5.1.1

Tool side offset

Overview

This type of cutter compensation performs three-dimensional
compensation in a plane (compensation plane) perpendicular to the
tool vector.

Compensation
plane

Tool vector

Cutter compensation
amount

Tool center path
(path after
compensation)

Programmed path
(path before compensation)

Cutter compensation vector

Fig. 22.5.1.1 (a) Tool side offset

Format
- Tool side offset (type 1)

G41.2 (or G42.2)

_ D_ ;

_ ;

G41.2: Cutter compensation left (group 07)
G42.2: Cutter compensation right (group 07)

Value specified for axis movement (including rotary
axis)

D_:

Code specifying the cutter compensation amount (1
to 3 digits)

- Tool side offset (type 2)

G41.6 (or G42.6)

_ I_ J_ K_ D_ Q_ ;

_ I_ J_ K_ ;

G41.6: Cutter compensation left (group 07)
G42.6: Cutter compensation right (group 07)

Value specified for axis movement (without rotary
axis)

D_:

Code specifying the cutter compensation amount (1
to 3 digits)

Q_:

Tool’s angle of gradient (in degrees)

I_ J_ K_: Tool axis direction at the block end point as

viewed from the programming coordinate system

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 902 -

For type 2, do not specify a rotation axis but specify the direction at
the tool end point as viewed from the programming coordinate system
(workpiece coordinate system), with I, J, and K. Specifying a
rotation axis causes alarm PS5460 to be generated.

NOTE

When a movement perpendicular to the next
movement (bit 1 (SUV) of parameter No. 5003 is
set to 1) is specified as the operation performed
at the time of startup or cancellation, a move
command such as X_ Y_ Z_ must not be
specified in the G41.2 and G42.2 block.

The following are the notes on type 2.

NOTE

1 If one or two of I, J, and K are omitted, the omitted

ones of I, J, and K are assumed to be 0.

2 In a block in which all of I, J, and K are omitted,

the values of I, J, and K in the previous block are
used.

3 If there is only one rotation axis (a hypothetical

axis is used), type 2 cannot be used. In this
case, if an attempt is made to issue G41.6/G42.6,
alarm PS5460 is generated.

4 If using the rotation axis rollover function or rotary

axis control function, specify 360 degrees in
parameter No. 1260 (mount of travel per rotation
about the rotation axis).

5 Only tool side offset provides type 2 commands.

Leading edge offset, described later, does not
provide type 2 commands.

- Canceling the tool side offset

G40

_ ;

G40: Cancellation of cutter compensation (group 07)

_: Value specified for axis movement

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 903 -

Explanation
- Tool’s angle of gradient in type 2

For type 2 of 3-dimensional cutter compensation, the tool's angle of
gradient can be specified with address Q in a G41.6/G42.6 command
block. The tool's angle of gradient refers to the angle by which the
tool direction to be assumed when machining is actually performed is
inclined from the direction specified with (I, J, K) toward the traveling
direction on the plane formed by the tool direction specified with (I, J,
K) and the traveling direction in the programming coordinate system.
(See Fig. 22.5.1.1 (b).)
Because in general, the normal direction of the machining surface is
specified with (I, J, K), if it is desired to incline the tool direction to be
assumed when machining is actually performed from the normal
direction toward the traveling direction, correction may be performed
with a Q command.
If the direction specified with (I, J, K) matches the tool direction to be
assumed when machining is actually performed, no Q command is
necessary.

Tool direction to be assumed when
machining is actually performed

(Plane perpendicular to the "tool direction to be
assumed when machining is actually performed")

Tool direction
specified with (I, J, K)

Traveling
direction of
machining

Tool's angle of gradient (Q)

Compensation plane

Tool center path
(path after compensation)

Programmed path
(path before compensation)

Cutter
compensation
vector

Fig. 22.5.1.1 (b) Tool's angle of gradient in type 2

(Example)

To perform machining by inclining the tool's traveling direction
twice, issue a command such as the following:

G41.6 I_ J_ K_ H_ Q2.0

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 904 -

- Operation at startup and cancellation

<1> Type A

The tool is moved in the same way as for cutter compensation as
shown below.

Tool

G41.2

G40

: Tool center path
: Programmed path

Operation in linear interpolation

: Tool center path
: Programmed path

Tool

G42.2

G40

Operation in circular interpolation

Fig. 22.5.1.1 (c) Operation at startup and cancellation (type A)

When the G40 block contains no movement command, type C
cancellation is performed (see <3> Type C below).

<2> Type B

The tool is moved in the same way as for cutter compensation as
shown below.

Tool

G41.2

G40

: Tool center path
: Programmed path

Operation in linear interpolation

: Tool center path
: Programmed path

Tool

G42.2

G40

Operation in circular interpolation

Fig. 22.5.1.1 (d) Operation at startup and cancellation (type B)

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 905 -

When the G40 block contains no movement command, type C
cancellation is performed (see <3> Type C below).

<3> Type C

When G41.2, G42.2, or G40 is specified as shown below, a linear
block specifying movement by the amount of cutter
compensation in the direction orthogonal to the movement
direction of the block following startup or the block preceding
cancellation is inserted.

Tool

G41.2

G40

: Tool center path
: Programmed path

Operation in linear interpolation

: Tool center path
: Programmed path

Tool

G42.2

G40

Operation in circular interpolation

Fig. 22.5.1.1 (e) Operation at startup and cancellation (type C)

NOTE

For type C (bit 1 (SUV) of parameter No. 5003 is
1), the following conditions need to be satisfied
during startup and cancellation.

1 A block specifying G40, G41.2, or G42.2 must

be in the G00 or G01 mode.

2 A block specifying G40, G41.2, or G42.2 must

contain no move command.

3 The block next to a block specifying G41.2 or

G42.2 must contain move command G00, G01,
G02, or G03.

22.5-AXIS MACHINING FUNCTION

PROGRAMMING

B-63944EN/03

- 906 -

- Operation during compensation

Operations such as change of the offset direction and offset value,
retention of a vector, and interference checks are performed in the
same way as for cutter compensation. However, G39 (corner
rounding) cannot be specified. So, note the following:

<1> When the tool center path goes outside the programmed path at a

corner, a linear movement takes place at the corner without
inserting an arc. When the tool center path goes inside the
programmed path, nothing is inserted.

: Tool center path

: Programmed path

Example <1>-1
Going outside of corner at
acute angle

Example <1>-2
Going inside of corner

Linear block inserted

Tool

Workpiece

Tool compensation

amount

Nothing inserted

Fig. 22.5.1.1 (f) Operation during compensation <1>-1 and <1>-2

In the above examples, the terms "inside" and "outside" denote
how the tool center path is positioned with respect to the
programmed path. In the figure below, example <1>-3 shows
the same relationship between the tool center path and
programmed path as example <1>-1 and indicates that the tool
center path is outside the programmed path; example <1>-4
shows the same relationship as example <1>-2 and indicates that
the tool center path is inside the programmed path.

: Tool center path
: Programmed path

Example <1>-3

Example <1>-4

Actual
tool

Reference
tool

Actual
tool

Reference
tool

Workpiece

Workpiec

: Tool compensation

amount

Fig. 22.5.1.1 (g) Operation during compensation <1>-3 and <1>-4

B-63944EN/03

PROGRAMMING

22.5-AXIS MACHINING FUNCTION

- 907 -

<2> When the tool moves at a corner, the feedrate of the previous

block is used if the corner is positioned before a single-block
stop point; if the corner is after a single-block stop point, the
feedrate of the next block is used.

: Tool center path
: Programmed path

Example <2>-1

F100

Tool

Program <2>-1

N1 G90 G41.2 Xp Yp Zp Bp Cp D1 ;

N2 G01 Xq Yq Zq F100 ;

N3 Xr Yr Zr F200 ;

Q1'

Q2' (single-block stop point)

Fig. 22.5.1.1 (h) Operation during compensation <2>

In the above example, the single-block stop point of N2 is Q2', so
the feedrates along paths P'-Q1' and Q1'-Q2' are both F100.

<3> When a command that makes the tool retrace the path of the

previous block is specified, the tool path can match the locus of
the previous block by changing the G code to change the offset
direction. If the G code is left unchanged, the operation shown
in example <3>-2 results:

: Tool center path

: Programmed path

Example <3>-1
When changing G41.2 to G42.2
(G41.2 mode)

G91 G01 X100.0
G42.2 X-100.0

Example <3>-2
When leaving G code unchanged
(G41.2 mode)

G91 G01 X100.0
X-100.0

Fig. 22.5.1.1 (i) Operation during compensation <3>

Content .. 116 117 118 119 ..