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

B-64604EN-1/01

PROGRAMMING

- 233 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.3.1

Outer Diameter/Internal Diameter Cutting Cycle (G90)

This cycle performs straight or taper cutting in the direction of the length.

6.3.1.1

Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 6.3.1.1 (a)) in the

direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.1.1 (a)) in the

direction of the length

F_ :

Cutting

feedrate

X/2

X axis

Z axis

2(F)

3(F)

1(R)

4(R)

U/2

A’

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

Fig. 6.3.1.1 (a) Straight cutting cycle

Explanation

- Operations

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

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

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

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

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-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

- 234 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.3.1.2

Taper cutting cycle

Format

ZpXp-plane

G90 X(U)_ Z(W)_ I_ F_ ;

YpZp-plane

G90 Y(V)_ Z(W)_ K_ F_ ;

XpYp-plane

G90 X(U)_ Y(V)_ J_ F_ ;

X_,Y_,Z_

: Coordinates of the cutting end point (point A' in the Fig. 6.3.1.2 (a)) in the

direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.1.2 (a)) in the

direction of the length

I_,J_,K_

: Taper amount (I in the figure below)

F_ :

Cutting

feedrate

3 (F )

X /2

4 (R )

U /2

1 (R )

Z a xis

2 (F )

X a xis

A’

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

Fig. 6.3.1.2 (a) Taper cutting cycle

Explanation

Address I, J, or K for specifying a taper varies with the plane selected.
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 I, J, or K). For the cycle in the figure above, a minus sign
is added to the taper amount.

NOTE

The increment system of address I, J, or K for specifying a taper depends on the
increment system for the reference axis. Specify a radius value at I, J, or K.

- Operations

A taper cutting cycle performs the same four operations as a straight 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 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 cutting cycle.

B-64604EN-1/01

PROGRAMMING

- 235 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the
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 I,
J, or K) and the cutting end point in the direction of the length in the absolute or incremental
programming as Table 6.3.1.2 (a).

Table 6.3.1.2 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, I < 0

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

at |I|

≤

|U/2|

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

at |I|

≤

|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.

6.3.2

Threading Cycle (G92)

6.3.2.1

Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 6.3.2.1 (a)) in the

direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.2.1 (a)) in the

direction of the length

: Angle for shifting the threading start angle

(Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees)

: Thread lead (L in the Fig. 6.3.2.1 (a))

PROGRAMMING

B-64604EN-1/01

- 236 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

X/2

X axis

Z axis

1(R)

2(F)

3(R)

4(R)

Detailed chamfered thread

(The chamfered angle in the left figure is 45

degrees or less because of the delay in the

servo system.)

Approx.

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

A’

U/2

Fig. 6.3.2.1 (a) Straight threading cycle

Explanation

The ranges of thread leads and restrictions related to the spindle speed are the same as for threading with
G32.

- Operations

A straight threading cycle performs four operations:

(1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the second axis on

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

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

Z-coordinate for the ZX plane) in cutting feed. At this time, thread chamfering is performed.

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (Retraction after chamfering)

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

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

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.

NOTE

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

- Acceleration/deceleration for threading after interpolation

Acceleration/deceleration for threading after interpolation is acceleration/deceleration of exponential
interpolation type. By setting bit 5 (THLx) of parameter No. 1610, the same acceleration/deceleration as
for cutting feed can be selected. (The settings of bits 1 (CTBx) and 0 (CTLx) of parameter No. 1610 are
followed.) However, as a time constant and FL feedrate, the settings of parameter No. 1626 and No. 1627
for the threading cycle are used.

B-64604EN-1/01

PROGRAMMING

- 237 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Time constant and FL feedrate for threading

The time constant for acceleration/deceleration after interpolation for threading specified in parameter No.
1626 and the FL feedrate specified in parameter No. 1627 are used.
The FL feedrate is valid only for exponential acceleration/deceleration after interpolation.

- Thread chamfering

Thread chamfering can be performed. A signal from the machine tool, initiates thread chamfering. The
chamfering distance r is specified in a range from 0.1L to 12.7L in 0.1L increments by parameter No.
5130. (In the above expression, L is the thread lead.)
A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a
value of 0 is specified in the parameter, an angle of 45 degrees is assumed.
For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for
acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and angle of thread chamfering
are used for this cycle and threading cycle with G76.

Retraction after chamfering

The Table 6.3.2.1 (a) lists the feedrate, type of acceleration/deceleration after interpolation, and time
constant of retraction after chamfering.

Table 6.3.2.1 (a)

Bit 3 (CFR) of

parameter No. 1611

Parameter No.

1466

Description

Other than 0

Uses the type of acceleration/deceleration after interpolation for threading,
time constant for threading (parameter No. 1626), FL feedrate (parameter
No. 1627), and retraction feedrate specified in parameter No. 1466.

0 0

Uses the type of acceleration/deceleration after interpolation for threading,
time constant for threading (parameter No. 1626), FL feedrate (parameter
No. 1627), and rapid traverse rate specified in parameter No. 1420.

Before retraction a check is made to see that the specified feedrate has
become 0 (delay in acceleration/deceleration is 0), and the type of
acceleration/deceleration after interpolation for rapid traverse is used
together with the rapid traverse time constant and the rapid traverse rate
(parameter No. 1420).

By setting bit 4 (ROC) of parameter No. 1403 to 1, rapid traverse override can be disabled for the feedrate
of retraction after chamfering.

NOTE

During retraction, the machine does not stop with an override of 0% for the
cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

Shifting the start angle

Address Q can be used to shift the threading start angle.
The start angle (Q) increment is 0.001 degrees and the valid setting range is between 0 and 360 degrees.
No decimal point can be specified.

Feed hold in a threading cycle (Threading cycle retract)

When feed hold is applied during threading(operation 2), the tool immediately retracts with chamfering
and returns to the start point on the second axis (X-axis), then the first axis (Z-axis) on the plane.

PROGRAMMING

B-64604EN-1/01

- 238 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

F e e d h o ld is effec te d h e re .

Sta rt p o in t

O rd in a ry c yc le

R a p id tra ve rs e

M o tio n a t fe e d h o ld

X a xis

Z a xis

C u ttin g fe e d

The chamfered angle is the same as that at the end point.

CAUTION

Another feed hold cannot be made during retraction.

- Inch threading

Inch threading specified with address E is allowed.

6.3.2.2

Taper threading cycle

Format

ZpXp-plane

G92 X(U)_ Z(W)_ I_ F_ Q_ ;

YpZp-plane

G92 Y(V)_ Z(W)_ K_ F_ Q_ ;

XpYp-plane

G92 X(U)_ Y(V)_ J_ F_ Q_ ;

X_,Y_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 6.3.2.2 (a)) in the

direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.2.2 (a)) in the

direction of the length

: Angle for shifting the threading start angle

(Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees)

I_,J_,K

: Taper amount (I in the figure below)

: Thread lead (L in the Fig. 6.3.2.2 (a))

B-64604EN-1/01

PROGRAMMING

- 239 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

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. 6.3.2.2 (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 I, J, or K). For the cycle in the figure above, a minus sign
is added to the taper amount.

NOTE

The increment system of address I, J, or K for specifying a taper depends on the
increment system for the reference axis. Specify a radius value at I, J, or K.

- 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

- 240 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

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

Table 6.3.2.2 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, I < 0

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

at |I|

≤

|U/2|

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

at |I|

≤

|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 for threading after interpolation
-

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

- 241 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.3.3

End Face Turning Cycle (G94)

6.3.3.1

Face cutting cycle

Format

G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 6.3.3.1 (a)) in the

direction of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.3.1 (a)) in the

direction of the end face

F_ :

Cutting

feedrate

X a xis

4 (R )

X /2

3 (F )

Z a xis

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. 6.3.3.1 (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

- 242 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.3.3.2

Taper cutting cycle

Format

ZpXp-plane

G94 X(U)_ Z(W)_ K _ F_ ;

YpZp-plane

G94 Y(V)_ Z(W)_ J _ F_ ;

XpYp-plane

G94 X(U)_ Y(V)_ I _ F_ ;

X_,Y_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 6.3.3.2 (a)) in the

direction of the end face

U_,V_,W_ : Travel distance to the cutting end point (point A' in the Fig. 6.3.3.2 (a)) in the

direction of the end face

I_,J_,K_ : Taper amount (K in the Fig. 6.3.3.2 (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. 6.3.3.2 (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 I, J, or K). For the cycle in the figure above, a minus
sign is added to the taper amount.

NOTE

The increment system of address I, J, or K for specifying a taper depends on the
increment system for the reference axis. Specify a radius value at I, J, or K.

- 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.

B-64604EN-1/01

PROGRAMMING

- 243 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the
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 I,
J, or K) and the cutting end point in the direction of the end face in the absolute or incremental
programming as Table 6.3.3.2 (a).

Table 6.3.3.2 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, K < 0

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

at |K|

≤

|W|

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

at |K|

≤

|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.

PROGRAMMING

B-64604EN-1/01

- 244 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

6.3.4

How to Use Canned Cycles

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

Taper cutting cycle (G90)

Shape of product

Shape of material

Face cutting cycle (G94)

Shape of product

Shape of material

B-64604EN-1/01

PROGRAMMING

- 245 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Face taper cutting cycle (G94)

Shape of product

Shape of material

6.3.5

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

Whole tool nose

Tool nose radius center path

Programmed path

Whole
tool nose

Whole tool nose

End face cutting cycle (G94)

Tool nose radius center path

Offset direction

Whole tool nose

Tool nose radius center path

Programmed path

Whole
tool nose

Whole tool nose

PROGRAMMING

B-64604EN-1/01

- 246 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

Differences between Series 0

-F and the Series 0

-C

NOTE

Series

-F is the same as the Ser

es 0

-C in the offset direction, but differs from

the series in the tool nose radius center path.
- For Series 0

-F

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 Ser

es 0

-C

This series differs from Series 0

-F in operations

n the block to move the tool

from the start po

nt and the last block to return it to the start point. For details,

refer to "Series 0

-C Operator's Manual."

How compensation is applied for the Series 0

-C

G90 G94

4,8,3

5,0,7

1,6,2

4,5,1

8,0,6

3,7,2

Whole
tool nose

Tool nose radius center path

Programmed path

4,5,1

8,0,6

3,7,2

Whole
tool nose

4,8,3

5,0,7

1,6,2

Programmed path

Tool nose radius center path

6.3.6

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

- 247 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Example

W orkpiece

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 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

- 248 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

- 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

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 16