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

B-64604EN-1/01

PROGRAMMING

- 57 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

(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

plane

G71 U10.0 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).

. . .

Fig. 4.2.1 (f) 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 Fig. 4.2.1 (g) cannot be machined.

Monotone change is not
observed along the Z-
axis.

Fig. 4.2.1 (g) 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 “THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(FIRST AXES)” 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).

PROGRAMMING

B-64604EN-1/01

- 58 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

+ X

+ Z

Fig. 4.2.1 (h) 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. 4.2.1 (i) Cutting along the workpiece figure (type II)

The escaping amount after cutting (e) can be specified at address R or 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. 4.2.1 (j) 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.

B-64604EN-1/01

PROGRAMMING

- 59 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Depth of cut

{

Start point

{

Escaping operation after
rough cutting

Escaping operation after rough cutting
as finishing

Fig. 4.2.1 (k) 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. 4.2.1 (l) 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)

<3>

<2>

<1>

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

Fig. 4.2.1 (m) Rough cutting order in the case of monotone increase (type II)

The path in rough cutting is as shown Fig. 4.2.1 (n).

PROGRAMMING

B-64604EN-1/01

- 60 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Fig. 4.2.1 (n) Cutting path for multiple pockets (type II)

The following figure shows how the tool moves after rough cutting for a pocket in detail.

•

Rapid traverse

Escaping from
the bottom

Cutting feed

Fig. 4.2.1 (o) 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 FANUC 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.

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.

This CNC differs from the FANUC 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).
When bit 0 (R16) of parameter No. 5108 is set to 1, the cutting can be continued along the first axis on
the plane.
The cutting path that the target figure program of Fig. 4.2.1 (n) is executed by the setting of bit 0 (R16) of
parameter No. 5108, is shown in Fig. 4.2.1 (p).

B-64604EN-1/01

PROGRAMMING

- 61 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Fig. 4.2.1 (p) Cutting path (No.5108#0 is set to 1)

Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41,
G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel
command (G40) outside the programs (from the block specified with P to the block specified with Q)
specifying a target finishing figure.
If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm
PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued.

Program example
G42;..............................Specify this command before a multiple repetitive canned cycle command.
G71U1.0R0.5;
G71P10Q20;
N10G00X0;
:
N20X50.0;
G40;..............................Specify this command after the program specifying a target finishing figure.

When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled
during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled
again at the return to the cycle start point after termination of cycle operation. Start-up is performed again
according to the next move command. This operation is shown in the Fig. 4.2.1 (q).

Cycle start point

Start-up

Offset cancel

Start-up

Offset cancel

Fig. 4.2.1 (q)

PROGRAMMING

B-64604EN-1/01

- 62 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

This cycle operation is performed according to the figure determined by the tool nose radius
compensation path when the offset vector is 0 at start point A and start-up is performed in a block
between path A-A'.

Target figure program for
which tool nose radius
compensation is not applied

A’

Tool nose center path when tool nose radius
compensation is applied with G42

Position between A-
A' in which start-up is
performed

Fig. 4.2.1 (r) Path when tool nose radius compensation is applied

Target figure program for
which tool nose radius
compensation is not applied

Tool nose center path when tool
nose radius compensation is
applied with G42

A’

Position between
A-A' in which start-
up is performed

Fig. 4.2.1 (s)

NOTE

To perform pocketing in the tool nose radius compensation mode, specify the
linear block A-A' outside the workpiece and specify the figure of an actual
pocket. This prevents a pocket from being dug.

When the bit 2 (NT1) of parameter No. 5106 is set to 1, the tool nose radius compensation G40/G41/G42
commanded in the target figure program of the multiple repetitive cycle G71/G72/G73 is ignored and no
alarm is occurred.

When the bit 3 (NT2) of parameter No. 5106 is set to 1, the tool nose radius compensation commanded in
the target figure program of the multiple repetitive cycle G70 is valid. However there is following
limitations.
(1) The tool nose radius compensation cancel G40 is selected as the modal when the finishing cycle G70

is commanded.

If the tool nose radius compensation is commanded in the target figure program when G41/G42 is
selected as the modal at the finishing cycle G70 command, the alarm PS0325 “UNAVAILABLE
COMMAND IS IN SHAPE PROGRAM” is occurred.

B-64604EN-1/01

PROGRAMMING

- 63 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

(2) Do not command G41/G42 excluding the end block in the target figure program.

If G41 or G42 is specified at the last block of the target figure program, the PS0325 alarm
(UNAVAILABLE COMMAND IS IN SHAPE PROGRAM) is issued.

(3) Command G40 at the last block of the target figure program (commanded by Q address)

If G40 is not commanded at the last block of the target figure program when G41 or G42 is
commanded at the first block, the PS0538 alarm “OFFSET IS NOT CANCELED” is occurred.

Program example of the tool nose radius compensation in the target figure of G70)
G40

;

G70 P10 Q20 ... ;

N10 G41 ... ;

N20 G40 ... ;

Reducing the cycle time

In the multiple repetitive cycle G71/G72 of type

Ⅰ

, if bit 1 (DTP) of parameter No. 5108 is set to 1, the

tool return to the cycle start point directly from the end point of the finishing program after rough cutting
of the finishing shape program is finished.

Cycle start point

Path of DTP = 1

Path of DTP = 0

End point of finishing
shape

Cycle start point

＋

Distance of the finishing
allowance

Fig. 4.2.1 (t) Return to cycle start point

In the multiple repetitive cycle G71/G72 of type II, when bit 3 (NSP) of parameter No. 5108 is set to 1,
the cutting is executed not to repeat the same cutting path. (When bit 3 (NSP) of parameter No. 5108 is
set to 1, the operation of bit 0 (R16) of parameter No. 5108 = 1 is always selected.)

Case of target figure without pocket.

In the conventional method, the path AB is cut twice as Fig. 4.2.1 (w).

When bit 3 (NSP) of parameter No. 5108 is set to 1, the overlap is avoided as Fig. 4.2.1(x).

Fig. 4.2.1 (u) Target figure without pocket (No.5108#3=0)

PROGRAMMING

B-64604EN-1/01

- 64 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Fig. 4.2.1 (v) Target figure without pocket (No.5108#3=1)

Case of target figure with pocket.

In the conventional method, the path AB and CD are cut twice as Fig. 4.2.1 (y).

The cutting path when bit 3 (NSP) of parameter No. 5108 is set to 1 is shown in Fig. 4.2.1(z). The
path AB is overlapped as same as Fig. 4.2.1 (y), however the path AB is executed by rapid traverse
at second times. The overlap path CD is avoided.

(1)

(2)

(3)

(4)

Fig. 4.2.1 (w) Target figure with pocket (No.5108#3=0)

(1)

(2)

(3)

(4)

Fig. 4.2.1 (x) Target figure with pocket (No.5108#3=1)

Case of consecutive pockets

In the conventional method, the tool moves to point I after finish the cutting of a pocket and
positioning to the start point of a next pocket as Fig. 4.2.1 (aa). In this way, the path is overlapped at
BI, DI, FI and HI.

The cutting path when bit 3 (NSP) of parameter No. 5108 is set to 1 is shown in Fig. 4.2.1(bb). The
movement to point I is executed just first time and then the pocket cutting is executed one after
another.

Fig. 4.2.1 (y) Consecutive pockets (No.5108#3=0)

PROGRAMMING

B-64604EN-1/01

- 66 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.2.2

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 W(

d) R(e) ;

G72 P(ns) Q(nf) U(

u) W(

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

N (ns) ;

...

N (nf) ;

The move commands for the target figure from A
to A’ to B are specified in the blocks with
sequence numbers ns to nf.

YpZp plane

G72 V(

d) R(e) ;

G72 P(ns) Q(nf) V(

w) W(

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

N (ns) ;

...

N (nf) ;

XpYp plane

G72 U(

d) R(e) ;

G72 P(ns) Q(nf) U(

w) V (

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

N (ns) ;

...

N (nf) ;

d : Depth of cut

The cutting direction depends on the direction AA'. This designation is modal and is not

changed until the other value is designated. Also this value can be specified by the
parameter No. 5132, and the parameter is changed by the program command.

e :

Escaping

amount

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5133, and the parameter is changed
by the program command.

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)

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.

Unit Diameter/radius

programming

Sign

Decimal point

input

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

B-64604EN-1/01

PROGRAMMING

- 67 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Unit Diameter/radius

programming

Sign

Decimal point

input

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

u/2

Tool path

(F)

(R)

(F)

Target figure

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

Fig. 4.2.2 (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 While

both

d and

u are specified by the same address, the meanings of them

are determined by the presence of addresses P and Q.

2 The cycle machining is performed by G72 command with P and Q specification.
3 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.

4 When the constant surface speed control function 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.

- 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:

PROGRAMMING

B-64604EN-1/01

- 68 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Both linear and circular

interpolation are possible

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

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

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

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

Fig. 4.2.2 (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.

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.

B-64604EN-1/01

PROGRAMMING

- 69 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

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

- 70 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.2.3

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 work whose rough shape has already been made by a rough
machining, forging or casting method, etc.

Format

ZpXp plane

G73 W(

k) U(

i) R(d) ;

G73 P(ns) Q(nf) U(

u) W(

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

N (ns) ;

...

N (nf) ;

The move commands for the target figure from A
to A’ to B are specified in the blocks with
sequence numbers ns to nf.

YpZp plane

G73 V(

k) W(

i) R(d) ;

G73 P(ns) Q(nf) V(

w) W(

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

N (ns) ;
...
N (nf) ;

XpYp plane

G73 U(

k) V(

i) R(d) ;

G73 P(ns) Q(nf) U(

w) V(

u) 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)

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5135, and the parameter is changed
by the program command.

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

plane)

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5136, and the parameter is changed
by the program command.

: The number of division

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

modal and is not changed until the other value is designated. Also, this value can be
specified by the parameter No. 5137, and the parameter is changed by the program
command.

: 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.

B-64604EN-1/01

PROGRAMMING

- 71 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Unit

Diameter/radius

programming

Sign

Decimal point

input

Depends on the increment
system for the reference axis.

Radius programming

Required

Allowed

Depends on the increment
system for the reference axis.

Radius programming

Required

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

NOTE

Decimal point input is allowed with d. However, a value rounded off to an integer
is used as the number of division, regardless of the setting of bit 0 (DPI) of
parameter No. 3401. When an integer is input, the input integer is used as the
number of division.

u/2

Target figure

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

(R)

(F)

Fig. 4.2.3 (a) Cutting path in pattern repeating

Explanation

- Operations

When a target figure passing through A, A', and B in this order is given by a program, rough cutting is
performed the specified number of times, with the finishing allowance specified by

u/2 and

w left.

NOTE

1 While the values

i and

k, or

u and

w are specified by the same address

respectively, the meanings of them are determined by the presence of
addresses P and Q.

2  The cycle machining is performed by G73 command with P and Q specification.
3  After cycle operation terminates, the tool returns to point A.
4  F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G73 block or the previous block
are effective. M and second auxiliary functions are treated in the same way as F,
S, and T functions.

PROGRAMMING

B-64604EN-1/01

- 72 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

- Target figure
Patterns

As in the case of G71, there are four target figure patterns. Be careful about signs of

i, and

when programming this cycle.

- Start block

In the start block in the program for the 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’.

- Check function

The following check can 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.

Tool nose radius compensation

Like G71, this cycle operation is performed according to the figure determined by the tool nose radius
compensation path when the offset vector is 0 at start point A and start-up is performed in a block
between path A-A'.

Single block operation

The single block stop position can be selected by setting of bit 2 (PRS) of parameter No. 5125.
When bit 2 (PRS) of parameter No. 5125 is set to 0, the stop position of single block operation are the end
point of each cycles and the end point of each blocks in the finishing shape.
When bit 2 (PRS) of parameter No. 5125 is set to 1, the stop position of single block operation are the end
point of each cycles and the end point of escape from the cycle start point. (FS16i compatible
specification)

It explains that the movement when the O0001 shown in Fig. 4.2.3 (b) is executed by the single block
operation.
The finishing shape specified by N10-N30 of the O0001 is shown in Fig. 4.2.3 (c).

O0001;
G00X100.0Z0.0;
G73U6.0W6.0R3.0;
G73P10Q30U6.0W3.0F1.0S500;
N10G00X60.0W0.0;
N15G01Z-10.0;
N20G02X80.0Z-20.0R10.0;
N30G01X100.0;
M30;

N10

N15

N20

N30

Fig. 4.2.3 (b) Sample program

Fig. 4.2.3 (c) Finishing shape of O0001

When bit 2 (PRS) of parameter No. 5125 is set to 0, in case the O0001 is executed by the single block
operation, the stop position of single block operation are the end point of each cycles and the end point of
each blocks in the finishing shape as shown in Fig. 4.2.3 (d). The single block stop does not executed at
the end point of escape from the cycle start point.

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 5