FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01)

B-64604EN-1/01

PROGRAMMING

- 249 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4

MULTIPLE REPETITIVE CANNED CYCLE

The multiple repetitive canned cycle is canned cycles to make CNC programming easy. For instance, the
data of the finish workpiece shape describes the tool path for rough machining. And also, a canned cycles
for the threading is available.

NOTE

1 When bit 3 (NMR) of parameter No.8137 is 0, "Multiple repetitive canned cycle"

can be used.
Though, a canned grinding cycle and multiple repetitive canned cycle cannot be
used simultaneously. When the canned grinding cycle (the option, "Grinding
function A" or "Grinding function B") is enabled, the multiple repetitive canned
cycle is disabled.

2 Explanatory figures in this section use the ZX plane as the selected plane,

diameter programming for the X-axis, and radius programming for the Z-axis.
When radius programming is used for the X-axis, change U/2 to U and X/2 to X.

3 A multiple repetitive canned cycle can be performed on any plane (including

parallel axes for plane definition). When G code system A is used, however, U,
V, and W cannot be set as a parallel axis.

PROGRAMMING

B-64604EN-1/01

- 250 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.1

Stock Removal in Turning (G71)

There are two types of stock removal in turning : Type I and II.

Format

ZpXp plane

G71 P(ns) Q(nf) U(

u) W(

w) I(

i) K(

k) D(

d) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

The move command between A and B is specified in the

blocks from sequence number ns to nf.

YpZp plane

G71 P(ns) Q(nf) V(

w) W(

u) J(

k) K(

i) D(

d) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

XpYp plane

G71 P(ns) Q(nf) U(

w) V(

u) I(

k) J(

i) D(

d) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

d : Depth of cut

The cutting direction depends on the direction AA'.

ns : Sequence number of the first block for the program of finishing shape.
nf : Sequence number of the last block for the program of finishing shape.

u : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane)

w : Distance of the finishing allowance in the direction of the first axis on the plane

(Z-axis for the ZX plane)

i : Distance of the finishing allowance of the roughing in the direction of the second

axis on the plane (X-axis for the ZX plane)

k : Distance of the finishing allowance of the roughing in the direction of the first axis

on the plane (Z-axis for the ZX plane)

f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the

F, S, or T function in this G71 block is effective.

NOTE

Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)
of parameter No. 3401 = 1), the unit of address D is least input increment. In
addition, when a decimal point is input in address D, the alarm PS0007 is issued.

Unit

Diameter/radius

programming

Sign

Decimal point

input

Depends on the increment
system for the reference axis.

Radius programming

Not

required

Not allowed

Depends on the increment
system for the reference axis.

Depends on diameter/radius programming for
the second axis on the plane.

Required Allowed

B-64604EN-1/01

PROGRAMMING

- 251 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Unit

Diameter/radius

programming

Sign

Decimal point

input

Depends on the increment
system for the reference axis.

Depends on diameter/radius programming for
the first axis on the plane.

Required Allowed

Depends on the increment
system for the reference axis.

Radius programming

Not

required

Allowed

Depends on the increment
system for the reference axis.

Radius programming

Not

required

Allowed

(R)

(F)

u/2

A’

Target figure

(F): Cutting feed
(R): Rapid traverse

e: Escaping amount (parameter No.5133)

Fig. 6.4.1 (a) Cutting path of an outer surface rough cutting cycle

without rough cutting finishing allowance (type I)

(R)

(F)

u/2

A’

Target figure

(F): Cutting feed

(R): Rapid

(R)

e: Escaping amount (parameter No.5133)

Fig. 6.4.1 (b) Cutting path of an outer surface rough cutting cycle

with rough cutting finishing allowance (type I)

Explanation

- Operations

If a target figure passing through A, A’, and B in this order is given by the program, a workpiece is cut
away by depth of cut

d at a time. The machining path varies as follows depending on whether the rough

machining finishing allowance is specified.

PROGRAMMING

B-64604EN-1/01

- 252 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

(1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut

d with finishing allowances

u/2 and

w left, and rough

cutting as finishing is performed according to the target figure program after the last machining.

(2) When the rough cutting finishing allowance is specified

Cutting is performed by depth of cut

d with cutting allowances

u/2+

i and

k left, and the

tool returns to the start point (A) after the last cutting is performed. Then, rough machining as
finishing is performed along the target figure to remove cutting allowances

i and

Upon completion of rough machining as finishing, the block next to the sequence block specified by Q is
executed.

NOTE

1 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G71 block or the previous block
are effective. M and second auxiliary functions are treated in the same way as F,
S, and T functions.

2 When a constant surface speed control is enabled (bit 0 (SSC) of parameter No.

8133 is set to 1), G96 or G97 command specified in the move command
between points A and B are ineffective, and that specified in G71 block or the
previous block is effective.

Escaping amount (e)

The escaping amount (e) is set in parameter No. 5133.

No. Unit

Diameter/radius

programming

Sign

5133

Depends on the increment system for the
reference axis.

Radius programming

Not required

- Target figure
Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with
moving the tool in parallel to the first axis on the plane (Z-axis for the ZX plane). At this time, the signs
of the finishing allowances of

u and

w are as follows:

Both linear and
circular interpolation
are possible

U(+)…W (+)

U(+)…W (-)

U(-)…W (+)

U(-)…W (-)

Fig. 6.4.1 (c) Four target figure patterns

Limitation

(1) For U(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

B-64604EN-1/01

PROGRAMMING

- 253 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

For U(-), a figure for which a position lower than the cycle start point is specified cannot be
machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the first axis on the plane.

Start

block

In the start block in the program for a target figure (block with sequence number ns in which the path
between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065 is
issued.
When G00 is specified, positioning is performed along A-A'. When G01 is specified, linear interpolation
is performed with cutting feed along A-A'.
In this start block, also select type I or II.
If X-axis does not move at start block, alarm PS0325 “UNAVAILABLE COMMAND IS IN SHAPE
PROGRAM” is issued.

Check

functions

During cycle operation, whether the target figure shows monotone increase or decrease is always
checked.

NOTE

When tool nose radius compensation is applied, the target figure to which
compensation is applied is checked.

The following checks can also be made.

Check Related

parameter

Checks that a block with the sequence number specified at address
Q is contained in the program before cycle operation.

Enabled when bit 2 (QSR) of parameter No.
5102 is set to 1.

Checks the target figure before cycle operation.
(Also checks that a block with the sequence number specified at
address Q is contained.)

Enabled when bit 2 (FCK) of parameter No.
5104 is set to 1.

Types I and II

Selection of type I or II

For G71, there are types I and II.
When the target figure has pockets, be sure to use type II.
Escaping operation after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX
plane) differs between types I and II. With type I, the tool escapes to the direction of 45 degrees. With
type II, the tool cuts the workpiece along the target figure. When the target figure has no pockets,
determine the desired escaping operation and select type I or II.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II.
(1) When type I is selected

Specify the second axis on the plane (X-axis for the ZX plane). Do not specify the first axis on the
plane (Z-axis for the ZX plane).

(2) When type II is selected

Specify the second axis on the plane (X-axis for the ZX plane) and first axis on the plane (Z-axis for
the ZX plane).

When you want to use type II without moving the tool along the first axis on the plane (Z-axis for
the ZX plane), specify the incremental programming with travel distance 0 (W0 for the ZX plane).

PROGRAMMING

B-64604EN-1/01

- 254 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

- Type I

(1) In the block with sequence number ns, only the second axis on the plane (X-axis (U-axis) for the ZX

plane) must be specified.

Example

ZX plane
G71 V10.0 R5.0 ;
G71 P100 Q200....;

N100 X(U)_ ;

(Specifies only the second axis on the plane.)

: ;
: ;
N200…………;

(2) The figure along path A'-B must show monotone increase or decrease in the directions of both axes

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig.
6.4.1 (d).

No pockets are allowed.

A’

Fig. 6.4.1 (d) Figure which does not show monotone increase or decrease (type I)

CAUTION

If a figure does not show monotone change along the first or second axis on the
plane, alarm PS0064 or 0329 is issued. If the movement does not show
monotone change, but is very small, and it can be determined that the
movement is not dangerous, however, the permissible amount can be specified
in parameters Nos. 5145 and 5146 to specify that the alarm is not issued in this
case.

(3) The tool escapes to the direction of 45 degrees in cutting feed after rough cutting.

Escaping amount e (specified in the
command or parameter No. 5133)

Fig. 6.4.1 (e) Cutting in the direction of 45 degrees (type I)

(4) Immediately after the last cutting, rough cutting is performed as finishing along the target figure. Bit

1 (RF1) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.
When the rough cutting finishing allowance is specified, however, rough cutting as finishing is
performed.

B-64604EN-1/01

PROGRAMMING

- 255 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

- Type II

(F)

u/2

A’

Target figure

(F): Cutting feed
(R): Rapid traverse

(R)

(F)

(R)

Fig. 6.4.1 (f) Cutting path in stock removal in turning (type II)

When the figure program for instructing a target figure passing through A, A’, and B in this order is
specified, a workpiece is cut away by depth of cut

d at a time. In type II, cutting is performed along the

figure after rough cutting in the direction of the plane first axis (z-axis for the ZX plane).
The machining path varies as follows depending on whether the rough machining finishing allowance is
specified.
(1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut

d with finishing allowances

u/2 and

w left, and the tool

returns to the start point (A) after the last cutting is performed (one pocket is assumed because
Pn

→

Pm is parallel to the z-axis in the Fig. 6.4.1 (f), and the zone is cut). Then, rough machining as

finishing is performed according to the finishing figure program with finishing allowances

u/2 and

w left.

(2) When the rough cutting finishing allowance is specified

Cutting is performed by depth of cut

d with cutting allowances

u/2+

i and

k left, and the

tool returns to the start point (A) after the last cutting is performed. Then, rough machining as
finishing is performed along the target figure to remove cutting allowances

i and

Upon completion of rough machining as finishing, the block next to the sequence block specified by Q is
executed.

Type II differs from type I in the following points:
(1) In the block with sequence number ns, the two axes forming the plane (X-axis (U-axis) and Z-axis

(W-axis) for the ZX plane) must be specified. When you want to use type II without moving the tool
along the Z-axis on the ZX plane in the first block, specify W0.

Example

ZX plane
G71 V10.0 R5.0;
G71 P100 Q200.......;

N100 X(U)_ Z(W)_ ;

(Specifies the two axes forming the plane.)

: ;
: ;
N200…………;

(2) The figure need not show monotone increase or decrease in the direction of the second axis on the

plane (X-axis for the ZX plane) and it may have concaves (pockets).

PROGRAMMING

B-64604EN-1/01

- 256 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

. . .

Fig. 6.4.1 (g) Figure having pockets (type II)

The figure must show monotone change in the direction of the first axis on the plane (Z-axis for the
ZX plane), however. The following figure cannot be machined.

Monotone change is not
observed along the Z-axis.

Fig. 6.4.1 (h) Figure which cannot be machined (type II)

CAUTION

For a figure along which the tool moves backward along the first axis on the
plane during cutting operation (including a vertex in an arc command), the
cutting tool may contact the workpiece. For this reason, for a figure which does
not show monotone change, alarm PS0064 or PS0329 is issued. If the
movement does not show monotone change, but is very small, and it can be
determined that the movement is not dangerous, however, the permissible
amount can be specified in parameter No. 5145 to specify that the alarm is not
issued in this case.

The first cut portion need not be vertical. Any figure is permitted if monotone change is shown in
the direction of the first axis on the plane (Z-axis for the ZX plane).

+ X

+ Z

Fig. 6.4.1 (i) Figure which can be machined (type II)

(3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

Escaping amount e (specified in the command or parameter No. 5133)

Depth of cut

d (specified in

the command or parameter No. 5132)

Escaping after cutting

Fig. 6.4.1 (j) Cutting along the workpiece figure (type II)

B-64604EN-1/01

PROGRAMMING

- 257 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

The escaping amount e after cutting is set in parameter No. 5133.

When moving from the bottom, however, the tool escapes to the direction of 45 degrees.

e (specified in the command or

parameter No. 5133)

Bottom

Fig. 6.4.1 (k) Escaping from the bottom to the direction of 45 degrees

(4) When a position parallel to the first axis on the plane (Z-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket.

(5) After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool

temporarily returns to the cycle start point. At this time, when there is a position whose height equals
to that at the start point, the tool passes through the point in the position obtained by adding depth of
cut

d to the position of the figure and returns to the start point.

Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes
through the point in the obtained position (to which depth of cut

d is added) when returning to the

start point.

Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

Depth of cut

{

Start point

{

Escaping operation after
rough cutting

Escaping operation after rough cutting
as finishing

Fig. 6.4.1 (l) Escaping operation when the tool returns to the start point (type II)

(6) Order and path for rough cutting of pockets

Rough cutting is performed in the following order.
(a) When the figure shows monotone decrease along the first axis on the plane (Z-axis for the ZX

plane)

<1>

<2>

<3>

Rough cutting is performed in the order <1>, <2>, and <3>
from the rightmost pocket.

Fig. 6.4.1 (m) Rough cutting order in the case of monotone decrease (type II)

(b) When the figure shows monotone increase along the first axis on the plane (Z-axis for the ZX

plane)

PROGRAMMING

B-64604EN-1/01

- 258 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

<3>

<2>

<1>

Rough cutting is performed in the order <1>, <2>, and <3> from
the leftmost pocket.

Fig. 6.4.1 (n) Rough cutting order in the case of monotone increase (type II)

The path in rough cutting is as shown Fig. 6.4.1 (o).

Fig. 6.4.1 (o) Cutting path for multiple pockets (type II)

The Fig. 6.4.1 (p) shows how the tool moves after rough cutting for a pocket in detail.

•

Rapid traverse

Escaping from
the bottom

Cutting feed

Fig. 6.4.1 (p) Details of motion after cutting for a pocket (type II)

Cuts the workpiece at the cutting feedrate and escapes to the direction of 45 degrees. (Operation 19)
Then, moves to the height of point D in rapid traverse. (Operation 20)
Then, moves to the position the amount of g before point D. (Operation 21)
Finally, moves to point D in cutting feed.
The clearance g to the cutting feed start position is set in parameter No. 5134.
For the last pocket, after cutting the bottom, the tool escapes to the direction of 45 degrees and returns to
the start point in rapid traverse. (Operations 34 and 35)

CAUTION

1 This CNC differs from the Series 0

-C in cutting of a pocket.

The tool first cuts the nearest pocket to the start point. After cutting of the pocket
terminates, the tool moves to the nearest but one pocket and starts cutting.

B-64604EN-1/01

PROGRAMMING

- 259 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

CAUTION

2 When the figure has a pocket, generally specify a value of 0 for

w (finishing

allowance). Otherwise, the tool may dig into the wall on one side.

3 This CNC differs from the Series 0

-C in the path of cutting after turning

depending on the figure of the workpiece. When the tool becomes moving only
along the first axis on the plane (Z-axis for the ZX plane) according to the figure
of the workpiece during cutting, it starts retraction along the second axis on the
plane (X-axis for the ZX plane).

About bit 0 (R16) of parameter No. 5108, please refer to the explanations of Stock Removal in Turning
(G71) in [FUNCTIONS TO SIMPLIFY PROGRAMMING].

Tool nose radius compensation

Please refer to the explanations of Stock Removal in Turning (G71) in [FUNCTIONS TO SIMPLIFY
PROGRAMMING].

Reducing the cycle time

Please refer to the explanations of Stock Removal in Turning (G71) in [FUNCTIONS TO SIMPLIFY
PROGRAMMING].

PROGRAMMING

B-64604EN-1/01

- 260 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.2

Stock Removal in Facing (G72)

This cycle is the same as G71 except that cutting is performed by an operation parallel to the second axis
on the plane (X-axis for the ZX plane).

Format

ZpXp plane

G72 P(ns) Q(nf) U(Du) W(Dw) I(Di) K(Dk) D(Dd) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

The move command between A and B is specified in the blocks from sequence

number ns to nf.

YpZp plane

G72 P(ns) Q(nf) V(

w) W(

u) J(

k) K(

i) D(

d) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

XpYp plane

G72 P(ns) Q(nf) U(

w) V(

u) I(

k) J(

i) D(

d) F(f ) S(s ) T(t );

N (ns) ;

...

N (nf) ;

d : Depth of cut

The cutting direction depends on the direction AA'.

ns : Sequence number of the first block for the program of finishing shape.
nf : Sequence number of the last block for the program of finishing shape.

u : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane)

w : Distance of the finishing allowance in the direction of the first axis on the plane

(Z-axis for the ZX plane)

i : Distance of the finishing allowance of the roughing in the direction of the second

axis on the plane (X-axis for the ZX plane)

k : Distance of the finishing allowance of the roughing in the direction of the first axis

on the plane (Z-axis for the ZX plane)

f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the

F, S, or T function in this G72 block is effective.

NOTE

Even if pocket calculator type decimal point programming is specified bit 0 (DPI)
of parameter No. 3401 = 1, the unit of address D is least input increment. In
addition, when a decimal point is input in address D, the alarm PS0007,
“ILLEGAL USE OF DECIMAL POINT” is issued.

B-64604EN-1/01

PROGRAMMING

- 261 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Unit Diameter/radius

programming

Sign

Decimal point

input

Depends on the increment
system for the reference axis.

Radius programming

Not required

Not allowed

Depends on the increment
system for the reference axis.

Depends on diameter/radius programming
for the second axis on the plane.

Required Allowed

Depends on the increment
system for the reference axis.

Depends on diameter/radius programming
for the first axis on the plane.

Required Allowed

Depends on the increment
system for the reference axis.

Radius programming

Not required

Allowed

Depends on the increment
system for the reference axis.

Radius programming

Not required

Allowed

u/2

Tool path

(F)

(R)

(F)

Target figure

(F): Cutting feed
(R): Rapid traverse

e: Escaping amount (parameter No.5133)

Fig. 6.4.2 (a) Cutting path in stock removal in facing (type I)

Explanation

- Operations

When a target figure passing through A, A', and B in this order is given by a program, the specified area
is removed by

d (depth of cut), with the finishing allowance specified by

u/2 and

w left.

NOTE

1 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G72 block or the previous block
are effective. M and second auxiliary functions are treated in the same way as F,
S, and T functions.

2 When a constant surface speed control is enabled (bit 0 (SSC) of parameter No.

8133 is set to 1), G96 or G97 command specified in the move command
between points A and B are ineffective, and that specified in G72 block or the
previous block is effective.

PROGRAMMING

B-64604EN-1/01

- 262 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Escaping amount (e)

The escaping amount (e) is set in parameter No. 5133.

No. Unit

Diameter/radius

programming

Sign

5133

Depends on the increment system for the
reference axis.

Radius programming

Not required

- Target figure
Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with
moving the tool in parallel to the second axis on the plane (X-axis for the ZX plane). At this time, the
signs of the finishing allowances of

u and

w are as follows:

Both linear and circular

interpolation are possible

U(-)...W(+)...

U(-)...W(-)...

U(+)...W(+)...

U(+)...W(-)...

Fig. 6.4.2 (b) Signs of the values specified at U and W in stock removal in facing

Limitation

(1) For W(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For W(-), a figure for which a position lower than the cycle start point is specified cannot be
machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the second axis on the plane.

Start

block

In the start block in the program for a target figure (block with sequence number ns in which the path
between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065,
“G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued.
When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation
is performed with cutting feed along A-A’.
In this start block, also select type I or II.
If Z-axis does not move at start block, alarm PS0325 “UNAVAILABLE COMMAND IS IN SHAPE
PROGRAM” is issued.

Check

functions

During cycle operation, whether the target figure shows monotone increase or decrease is always
checked.

NOTE

When tool nose radius compensation is applied, the target figure to which
compensation is applied is checked.

The following checks can also be made.

B-64604EN-1/01

PROGRAMMING

- 263 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Check Related

parameter

Checks that a block with the sequence number specified at address Q is
contained in the program before cycle operation.

Enabled when bit 2 (QSR) of
parameter No. 5102 is set to 1.

Checks the target figure before cycle operation.
(Also checks that a block with the sequence number specified at address Q is
contained.)

Enabled when bit 2 (FCK) of
parameter No. 5104 is set to 1.

Types I and II

Selection of type I or II

For G72, there are types I and II.
When the target figure has pockets, be sure to use type II.
Escaping operation after rough cutting in the direction of the second axis on the plane (X-axis for the ZX
plane) differs between types I and II. With type I, the tool escapes to the direction of 45 degrees. With
type II, the tool cuts the workpiece along the target figure. When the target figure has no pockets,
determine the desired escaping operation and select type I or II.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II.
(1) When type I is selected

Specify the first axis on the plane (Z-axis for the ZX plane). Do not specify the second axis on the
plane (X-axis for the ZX plane).

(2) When type II is selected

Specify the second axis on the plane (X-axis for the ZX plane) and first axis on the plane (Z-axis for
the ZX plane).

When you want to use type II without moving the tool along the second axis on the plane (X-axis for
the ZX plane), specify the incremental programming with travel distance 0 (U0 for the ZX plane).

- Type I

G72 differs from G71 in the following points:
(1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane).

(2) In the start block in the program for a target figure (block with sequence number ns), only the first

axis on the plane (Z-axis (W-axis) for the ZX plane) must be specified.

- Type II

G72 differs from G71 in the following points:
(1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane).

(2) The figure need not show monotone increase or decrease in the direction of the first axis on the

plane (Z-axis for the ZX plane) and it may have concaves (pockets). The figure must show
monotone change in the direction of the second axis on the plane (X-axis for the ZX plane),
however.

(3) When a position parallel to the second axis on the plane (X-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket.

(4) After all rough cutting terminates along the second axis on the plane (X-axis for the ZX plane), the

tool temporarily returns to the start point. Then, rough cutting as finishing is performed.

Tool nose radius compensation

See the pages on which G71 is explained.

Reducing the cycle time

See the pages on which G71 is explained.

PROGRAMMING

B-64604EN-1/01

- 264 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.3

Pattern Repeating (G73)

This function permits cutting a fixed pattern repeatedly, with a pattern being displaced bit by bit. By this
cutting cycle, it is possible to efficiently cut workpiece whose rough shape has already been made by a
rough machining, forging or casting method, etc.

Format

ZpXp plane

G73 P(ns) Q(nf) U(Du) W(Dw) I(Di) K(Dk) D(d) F(f ) S(s ) T(t ) ;

N (ns) ;

...

N (nf) ;

The move command between A and B is specified in the blocks from sequence

number ns to nf.

YpZp plane

G73 P(ns) Q(nf) V(

w) W(

u) J(

k) K(

i) D(d) F(f ) S(s ) T(t ) ;

N (ns) ;

...

N (nf) ;

XpYp plane

G73 P(ns) Q(nf) U(

w) V(

u) I(

k) J(

i) D(d) F(f ) S(s ) T(t ) ;

N (ns) ;

...

N (nf) ;

: Distance of escape in the direction of the second axis on the plane (X-axis for the

ZX plane)

: Distance of escape in the direction of the first axis on the plane (Z-axis for the ZX

plane)

: The number of division

This value is the same as the repetitive count for rough cutting.

: Sequence number of the first block for the program of finishing shape.

: Sequence number of the last block for the program of finishing shape.

: Distance of the finishing allowance in the direction of the second axis on the

plane (X-axis for the ZX plane)

: Distance of the finishing allowance in the direction of the first axis on the plane

(Z-axis for the ZX plane)

f, s, t : Any F, S, and T function contained in the blocks between sequence number "ns"

and "nf" are ignored, and the F, S, and T functions in this G73 block are effective.

NOTE

Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)
of parameter No. 3401 = 1), the unit of address D is the least input increment. In
addition, when a decimal point is input in address D, alarm PS0007 is issued.

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 17