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

B-64604EN-1/01

PROGRAMMING

- 41 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Detailed chamfered thread

1(R)

Z axis

3(R)

4(R)

2(F)

U/2

X/2

X axis

Approx. 45

(The chamfered angle in the left figure

is 45 degrees or less because of the

delay in the servo system.)

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

A’

Fig. 4.1.2.2 (a) Taper threading cycle

Explanation

The ranges of thread leads and restrictions related to the spindle speed are the same as for threading with
G32.
The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the
length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.2.2 (a), a minus sign is
added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the
increment system for the reference axis. Specify a radius value at R.

- Operations

A taper threading cycle performs the same four operations as a straight threading cycle.
However, operation 1 moves the tool from the start point (A) to the position obtained by adding the taper
amount to the specified coordinate of the second axis on the plane (specified X-coordinate for the ZX
plane) in rapid traverse.
Operations 2, 3, and 4 after operation 1 are the same as for a straight threading cycle.

CAUTION

Notes on this threading are the same as in threading in G32. However, a stop by
feed hold is as follows; Stop after completion of path 3 of threading cycle.

PROGRAMMING

B-64604EN-1/01

- 42 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

NOTE

In the single block mode, operations 1, 2, 3, and 4 are performed by pressing
cycle start button once.

Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the sign of the taper amount (address R)
and the cutting end point in the direction of the length in the absolute or incremental programming as
Table 4.1.2.2 (a).

Table 4.1.2.2 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, R < 0

2. U > 0, W < 0, R > 0

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

3. U < 0, W < 0, R > 0

at |R|

≤

|U/2|

4. U > 0, W < 0, R < 0

at |R|

≤

|U/2|

U/2

3(F)

4(R)

1(R)

2(F)

U/2

3(F)

4(R)

1(R)

2(F)

Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

- Acceleration/deceleration after interpolation for threading
-

Time constant and FL feedrate for threading

- Thread chamfering
-

Retraction after chamfering

Shifting the start angle

Threading cycle retract

- Inch threading

See the pages on which a straight threading cycle is explained.

B-64604EN-1/01

PROGRAMMING

- 43 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.1.3

End Face Turning Cycle (G94)

4.1.3.1

Face cutting cycle

Format

G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the

direction of the end face

F_ :

Cutting

feedrate

X a x is

4 (R )

X /2

3 (F )

Z a x is

1 (R )

2 (F )

(R ) ... R a p id tra v e rs e
(F ).... C u ttin g fe e d

U /2

A’

Fig. 4.1.3.1 (a) Face cutting cycle

Explanation

- Operations

A face cutting cycle performs four operations:
(1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the first axis on the

plane (specified Z-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in cutting feed. (The tool is moved to the cutting end point (A') in
the direction of the end face.)

(3) Operation 3 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the
cycle start button once.

Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

PROGRAMMING

B-64604EN-1/01

- 44 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.1.3.2

Taper cutting cycle

Format

G94 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the

direction of the end face

: Taper amount (R in the Fig. 4.1.3.2 (a))

F_ :

Cutting

feedrate

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

4(R)

X/2

3(F)

Z axis

1(R)

2(F)

U/2

X axis

A’

Fig. 4.1.3.2 (a) Taper cutting cycle

Explanation

The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the
end face and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.3.2 (a), a minus sign is
added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the
increment system for the reference axis. Specify a radius value at R.

- Operations

A taper cutting cycle performs the same four operations as a face cutting cycle.
However, operation 1 moves the tool from the start point (A) to the position obtained by adding the taper
amount to the specified coordinate of the first axis on the plane (specified Z-coordinate for the ZX plane)
in rapid traverse.
Operations 2, 3, and 4 after operation 1 are the same as for a face cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the
cycle start button once.

B-64604EN-1/01

PROGRAMMING

- 45 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the sign of the taper amount (address R)
and the cutting end point in the direction of the end face in the absolute or incremental programming as
Table 4.1.3.2 (a).

Table 4.1.3.2 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, R < 0

2. U > 0, W < 0, R < 0

1(R)

U/2

3(F)

4(R)

2(F)

U/2

3(F)

4(R)

2(F)

1(R)

3. U < 0, W < 0, R > 0

at |R|

≤

|W|

4. U > 0, W < 0, R > 0

at |R|

≤

|W|

U/2

3(F)

4(R)

2(F)

1(R)

U/2

3(F)

4(R)

2(F)

1(R)

Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other than G90, G92, or G94.

4.1.4

How to Use Canned Cycles (G90, G92, G94)

An appropriate canned cycle is selected according to the shape of the material and the shape of the
product.

Straight cutting cycle (G90)

Shape of
product

Shape of material

PROGRAMMING

B-64604EN-1/01

- 46 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Taper cutting cycle (G90)

Shape of product

Shape of material

Face cutting cycle (G94)

Shape of product

Shape of material

Face taper cutting cycle (G94)

Shape of product

Shape of material

B-64604EN-1/01

PROGRAMMING

- 47 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.1.5

Canned Cycle and Tool Nose Radius Compensation

When tool nose radius compensation is applied, the tool nose center path and offset direction are as
shown below. At the start point of a cycle, the offset vector is canceled. Offset start-up is performed for
the movement from the start point of the cycle. The offset vector is temporarily canceled again at the
return to the cycle start point and offset is applied again according to the next move command. The offset
direction is determined depending of the cutting pattern regardless of the G41 or G42 mode.

Outer diameter/internal diameter cutting cycle (G90)

Tool nose radius center path

Offset direction

Total tool nose

Tool nose radius
center path

Programmed path

Total tool
nose

Total tool nose

End face cutting cycle (G94)

Total tool nose

Tool nose radius
center path

Programmed path

Total tool
nose

Total tool nose

Tool nose radius center path

Offset direction

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

PROGRAMMING

B-64604EN-1/01

- 48 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Differences between this CNC and the FANUC Series 0

-C

NOTE

This CNC is the same as the FANUC Series 0

-C in the offset direction, but

differs from the series in the tool nose radius center path.

- For this CNC
Cycle operations of a canned cycle are replaced with G00 or G01. In the first

block to move the tool from the start point, start-up is performed. In the last
block to return the tool to the start point, offset is canceled.

- For the FANUC Series 0

-C

This series differs from this CNC in operations in the block to move the tool

from the start point and the last block to return it to the start point. For details,
refer to "FANUC Series 0

-C Operator's Manual."

How compensation is applied for the FANUC Series 0

-C

G90 G94

4,8,3

5,0,7

1,6,2

4,5,1

8,0,6

3,7,2

Total tool
nose

Tool nose radius center path

Programmed path

4,5,1

8,0,6

3,7,2

Total tool
nose

4,8,3

5,0,7

1,6,2

Programmed path

Tool nose radius center path

4.1.6

Restrictions on Canned Cycles

Limitation

- Modal

Since data items X (U), Z (W), and R in a canned cycle are modal values common to G90, G92, and G94.
For this reason, if a new X (U), Z (W), or R value is not specified, the previously specified value is
effective.
Thus, when the travel distance along the Z-axis does not vary as shown in the program example below, a
canned cycle can be repeated only by specifying the travel distance along the X-axis.

B-64604EN-1/01

PROGRAMMING

- 49 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Example

Workpiece

X axis

The cycle in the above figure is executed by the following program:

N030 G90 U-8.0 W-66.0 F0.4;

N031 U-16.0;

N032 U-24.0;

N033 U-32.0;

The modal values common to canned cycles are cleared when a one-shot G code other than G04 is
specified.
Since the canned cycle mode is not canceled by specifying a one-shot G code, a canned cycle can be
performed again by specifying modal values. If no modal values are specified, no cycle operations are
performed.
When G04 is specified, G04 is executed and no canned cycle is performed.

Block in which no move command is specified

In a block in which no move command is specified in the canned cycle mode, a canned cycle is also
performed. For example, a block containing only EOB or a block in which none of the M, S, and T codes,
and move commands are specified is of this type of block. When an M, S, or T code is specified in the
canned cycle mode, the corresponding M, S, or T function is executed together with the canned cycle. If
this is inconvenient, specify a group 01 G code (G00 or G01) other than G90, G92, or G94 to cancel the
canned cycle mode, and specify an M, S, or T code, as in the program example below. After the
corresponding M, S, or T function has been executed, specify the canned cycle again.

Example

N003

T0101;

N010 G90 X20.0 Z10.0 F0.2;

N011 G00 T0202;

←

Cancels the canned cycle mode.

N012 G90 X20.5 Z10.0;

Plane selection command

Specify a plane selection command (G17, G18, or G19) before setting a canned cycle or specify it in the
block in which the first canned cycle is specified.
If a plane selection command is specified in the canned cycle mode, the command is executed, but the
modal values common to canned cycles are cleared.
If an axis which is not on the selected plane is specified, alarm PS0330, “ILLEGAL AXIS COMMAND
IS IN THE TURNING CANNED CYCLE” is issued.

- Parallel axis

When G code system A is used, U, V, and W cannot be specified as a parallel axis.

PROGRAMMING

B-64604EN-1/01

- 50 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

- Reset

If a reset operation is performed during execution of a canned cycle when any of the following states for
holding a modal G code of group 01 is set, the modal G code of group 01 is replaced with the G01 mode:

•

Reset state (bit 6 (CLR) of parameter No. 3402 = 0)

•

Cleared state (bit 6 (CLR) of parameter No. 3402 = 1) and state where the modal G code of group 01
is held at reset time (bit 1 (C01) of parameter No. 3406 = 1)

Example of operation)

If a reset is made during execution of a canned cycle (X0 block) and the X20.Z1. command is
executed, linear interpolation (G01) is performed instead of the canned cycle.

- Manual intervention

After manual intervention is performed with the manual absolute on command before the execution of a
canned cycle or after the stop of the execution, when a cycle operation starts, the manual intervention
amount is canceled even with an incremental cycle start command.

1(R)

3(F)

4(R)

2(F)

Manual intervention

Cancellation

Example of G94

B-64604EN-1/01

PROGRAMMING

- 51 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.2

MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

The multiple repetitive canned cycle is canned cycles to make CNC programming easy. For instance, the
data of the finish work 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

- 52 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.2.1

Stock Removal in Turning (G71)

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

Format

ZpXp plane

G71 U(

d) R(e) ;

G71 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

G71 W(

d) R(e) ;

G71 P(ns) Q(nf) V(

w) W(

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

N (ns) ;

...

N (nf) ;

XpYp plane

G71 V(

d) R(e) ;

G71 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 G71 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

- 53 -

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

(R)

(F)

u/2

A’

Target figure

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

e: Escaping amount

Fig. 4.2.1 (a) Cutting path in stock removal in turning (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. After the last

cutting is performed in the direction of the second axis on the plane (X-axis for the ZX plane), rough
cutting is performed as finishing along the target figure. After rough cutting as finishing, the block next to
the sequence block specified at Q is executed.

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 G71 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 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.

4 When the constant surface speed control function is enabled (bit 0 (SSC) of

parameter No. 8133 is set to 1), the 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.

- 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:

PROGRAMMING

B-64604EN-1/01

- 54 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

Both linear and
circular interpolation
are possible

U(+)…W (+)

U(+)…W (-)

U(-)…W (+)

U(-)…W (-)

Fig. 4.2.1 (b) 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.

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,
“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 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.

B-64604EN-1/01

PROGRAMMING

- 55 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

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.

NOTE

To use type II, the multiple repetitive canned cycle II option is required.

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).

- 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

plane

G71 U10.0 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.
4.2.1 (c).

No pockets are allowed.

A’

Fig. 4.2.1 (c) Figure which does not show monotone increase or decrease (type I)

PROGRAMMING

B-64604EN-1/01

- 56 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

CAUTION

If a figure does not show monotone change along the first or second axis on the
plane, alarm PS0064, “THE FINISHING SHAPE IS NOT A MONOTONOUS
CHANGE(FIRST AXES)” or PS0329, “THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(SECOND 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 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. 4.2.1 (d) 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.

- Type II

(F)

u/2

A’

Target figure

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

(R)

(F)

(R)

Fig. 4.2.1 (e) Cutting path in stock removal in turning (type II)

When a target figure passing through A, A', and B in this order is given by the program for a target figure
as shown in the Fig. 4.2.1 (e), the specified area is removed by

d (depth of cut), with the finishing

allowance specified by

u/2 and

w left. Type II differs from type I in cutting the workpiece along the

figure after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX plane).
After the last cutting, the tool returns to the start point specified in G71 and rough cutting is performed as
finishing along the target figure, with the finishing allowance specified by

u/2 and

w left.

Type II differs from type I in the following points:

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 4