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

B-64604EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- 25 -

Tapered thread

α≤

lead is LZ

α≥

lead is LX

Fig. 3.2 (c) LZ and LX of a tapered thread

In general, the lag of the servo system, etc. will produce somewhat incorrect leads at the starting and
ending points of a thread cut. To compensate for this, a threading length somewhat longer than required
should be specified.
Table 3.2 (a) lists the ranges for specifying the thread lead.

Table 3.2 (a) Ranges of lead sizes that can be specified

Least command increment

Metric input

0.0001 to 500.0000 mm

Inch input

0.000001 to 9.999999 inch

- Continuous

threading

The "continuous threading" is effective for G32.

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64604EN-1/01

- 26 -

Example

Z axis

X axis

30mm

The following values are used in programming :
Thread lead :4mm

=3mm

=1.5mm

Depth of cut :1mm (cut twice)
(Metric input, diameter programming)

  G00 U-62.0 ;
  G32 W-74.5 F4.0 ;
  G00  U62.0  ;
    W74.5 ;
    U-64.0 ;
        (For the second cut, cut 1mm more)
  G32 W-74.5  ;
  G00  U64.0  ;

W74.5 ;

1. Straight threading

Z axis

X axis

The following values are used in programming :
Thread lead : 3.5mm in the direction of the Z axis

=2mm

=1mm

Cutting depth in the X axis direction is 1mm (cut twice)
(Metric input, diameter programming)
    G00 X 12.0 Z72.0 ;
    G32 X 41.0 Z29.0 F3.5 ;
    G00 X 50.0 ;
        Z 72.0 ;
   X 10.0 ;
        (Cut 1mm more for the second cut)
    G32 X 39.0 Z29.0    ;
    G00 X 50.0    ;
        Z 72.0    ;

2.Tapered threading

WARNING

1 Feedrate override is effective (fixed at 100%) during threading.
2 It is very dangerous to stop feeding the thread cutter without stopping the

spindle. This will suddenly increase the cutting depth. Thus, the feed hold
function is ineffective while threading. If the feed hold button is pressed during
threading, the tool will stop after a block not specifying threading is executed as
if the SINGLE BLOCK button were pushed. However, the feed hold lamp (SPL
lamp) lights when the FEED HOLD button on the machine control panel is
pushed. Then, when the tool stops, the lamp is turned off (Single Block stop
status).

3 When the FEED HOLD button is pressed again in the first block after threading

mode that does not specify threading (or the button has been held down), the
tool stops immediately at the block that does not specify threading.

4 When threading is executed in the single block status, the tool stops after

execution of the first block not specifying threading.

B-64604EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- 27 -

WARNING

5 When the mode was changed from automatic operation to manual operation

during threading, the tool stops at the first block not specifying threading as
when the feed hold button is pushed as mentioned in Warning 3.

However, when the mode is changed from one automatic operation mode to
another, the tool stops after execution of the block not specifying threading as for
the single block mode in Note 4.

6 When the previous block was a threading block, cutting will start immediately

without waiting for detection of the one-spindle-rotation signal even if the present
block is a threading block.

(Example)

G00 Z0.0 X50.0 ; One-rotation signal is
G32 Z10.0 F_ ; : Detected
Z20.0 ; : Not detected
G32 Z30.0 ; : Not detected

7 Because the constant surface speed control is effective during scroll thread or

tapered screw cutting and the spindle speed changes, the correct thread lead
may not be cut. Therefore, do not use the constant surface speed control during
threading. Instead, use G97.

8 A movement block preceding the threading block must not specify chamfering or

corner R.

9 A threading block must not specifying chamfering or corner R.
10 The spindle speed override function is disabled during threading. The spindle

speed is fixed at 100%.

11 Thread cycle retract function is ineffective to G32.
12 If tool offset (with the T code or G43.7) is specified in during of the threading

mode, or in a block for threading, alarm PS0509, “TOOL OFFSET COMMAND
IS NOT AVAILABLE”, is issued.

3.3

VARIABLE LEAD THREADING (G34)

Specifying an increment or a decrement value for a lead per screw revolution enables variable lead
threading to be performed.

Fig. 3.3 (a) Variable lead screw

NOTE

When bit 1 (NVL) of parameter No.8137 is 0, this function can be used.

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64604EN-1/01

- 28 -

Format

G34

_ F_ K_ Q_ ;

_ : End point

F_  : Lead in longitudinal axis direction at the start point
K_  : Increment and decrement of lead per spindle revolution
Q_  : Shift amount of starting angle of thread cutting

Explanation

Address other than K are the same as in straight/taper thread cutting with G32.
The K value depends on the increment system of the reference axis, as indicated in Table 3.3 (a).
If the specified K value exceeds the range indicated in Table 3.3 (a), if the maximum lead is exceeded
after a change due to the K value, or if the lead value is negative, an alarm PS0313, "ILLEGAL LEAD
COMMAND", will be issued.

Table 3.3 (a) Range of valid K values

Increment system

of reference axis

Metric input (mm/rev)

Inch input (inch/rev)

IS-A

0.001 to

500.000

0.00001 to

50.00000

IS-B

0.0001 to

500.0000

0.000001 to

50.000000

IS-C

0.00001 to

50.00000

0.0000001 to

5.0000000

Table3.3 (b) Range of valid lead values

Metric input (mm)

Inch input (inch)

0.0001

to 500.0000

0.000001 to 50.000000

- Continuous

threading

The "continuous threading" is effective for G34.

CAUTION

The "thread cutting cycle retract" is not effective for G34.

Example

Lead at the start point: 8.0 mm
Lead increment: 0.3 mm/rev

G34 Z-72.0 F8.0 K0.3 ;

3.4

CIRCULAR THREADING (G35, G36)

Using the G35 and G36 commands, a circular thread, having the specified lead in the direction of the
major axis, can be machined.

L: Lead

Fig. 3.4 (a) Circular threading

B-64604EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- 29 -

NOTE

This function is an optional function.

Format

A sample format for the G18 plane (Z-X plane) is indicated below. When using the format for the G17
plane (X-Y plane), change the addresses Z, X, K, and I to X, Y, I, and J respectively. When using the
format for the G19 plane (Y-Z plane), change the addresses Z, X, K, and I to Y, Z, J, and K respectively.

G35 I_

G36

X(U)_ Z(W)_

F_ Q_ ;

G35  : Clockwise circular threading command
G36  : Counterclockwise circular threading command

X(U), Z(W) : Specify the arc end point (in the same way as for G02, G03).

I, K  : Specify the arc center relative to the start point, using relative coordinates (in the

same way as for G02, G03).

: Specify the arc radius.

: Specify the lead in the direction of the major axis.

: Specify the shift of the threading start angle

(0° to 360°, with least input increment of 0.001)

(The value cannot be programmed with a decimal point.)

End point (Z, X)

Arc center

Start point

Explanation

- Specifying the arc radius

If R is specified with I and K, only R is effective.

- Shift angle

If an angle greater than 360

is programmed, it is set to 360

- Continuous

threading

The "continuous threading" is effective for G35, G36.

- Thread cutting cycle retract

The "thread cutting cycle retract" is not effective for G35, G36.

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64604EN-1/01

- 30 -

Automatic tool compensation

The G36 command is used to specify the following two functions: Automatic tool compensation X and
counterclockwise circular threading. The function for which G36 is to be used depends on bit 3 (G36) of
parameter No. 3405.

•

When parameter G36 is set to 0, the G36 command is used for automatic tool compensation X.

•

When parameter G36 is set to 1, the G36 command is used for counterclockwise circular threading.

G37.1 can be used to specify automatic tool compensation X and G37.2 can be used to specify automatic
tool compensation Z.
(Specification

method)

G37.1

G37.2

•

G code when bit 3 (G36) of parameter No. 3405 is set to 1

G code

G code group

Function

G35

Clockwise circular threading

G36

Counterclockwise circular threading

G37

Automatic tool compensation Z

G37.1

Automatic tool compensation X

G37.2

Automatic tool compensation Z

Limitation

- Range of specifiable arc

An arc must be specified such that it falls within a range in which the major axis of the arc is always the
Z-axis or always the X-axis, as shown in Fig. 3.4 (b) and Fig. 3.4 (c). If the arc includes a point at which
the major axis changes from the X-axis to Z-axis, or vice versa, as shown in Fig. 3.4 (d), an alarm PS5058,
"G35/G36 FORMAT ERROR", is issued.

Start point

End point

Fig. 3.4 (b) Range in which the Z-axis is the major axis

Start point

End point

Fig. 3.4 (c) Range in which the X-axis is the major axis

B-64604EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- 31 -

Start point

End point

The major axis changes at this point.

Fig. 3.4 (d) Example of arc specification which causes an alarm

- End point not on an arc

If the end point is not on an arc, a movement on an axis is made to a position of which coordinate matches
the corresponding coordinate of the end point. Then, a movement is made on another axis to reach the end
point.

Start point

Center

End point

Center

End point

Start point

Fig. 3.4 (e) Movement when the end point is not on an arc

3.5

CONTINUOUS THREADING

Threading blocks can be programmed successively to eliminate a discontinuity due to a discontinuous
movement in machining by adjacent blocks.

Explanation

Since the system is controlled in such a manner that the synchronism with the spindle does not deviate in
the joint between blocks wherever possible, it is possible to performed special threading operation in
which the lead and shape change midway.

G32

Fig. 3.5 (a) Continuous threading (Example of G32 in G code system A)

Even when the same section is repeated for threading while changing the depth of cut, this system allows
a correct machining without impairing the threads.

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64604EN-1/01

- 32 -

Available threading commands

G32: Constant lead threading (G code system A)
G33: Constant lead threading (G code system B/C)
G34: Variable lead threading
G35, G36: Circular threading

- Start

angle

The address Q (Angle for shifting the threading start angle) is only effective the first threading command
block of continuous threading.
In the continuous threading, the addresses Q of the threading in the blocks after the first are ignored.

3.6

MULTIPLE THREADING

Using the Q address to specify an angle between the one-spindle-rotation signal and the start of threading
shifts the threading start angle, making it possible to produce multiple-thread screws with ease.

L : Lead

Fig. 3.6 (a) Multiple thread screws.

Format

(Constant lead threading)
G32

_ F_ Q_ ;

: End point

F_ : Lead in longitudinal direction

G32

_ Q_ ;

Q_ : Angle for shifting the threading start angle

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

Explanation

- Available threading commands

G32: Constant lead threading
G34: Variable lead threading
G35, G36: Circular threading
G76/G78: Multiple threading cycle (Only when the FS10/11 tape format is used.)
G92: Threading cycle

Limitation

- Start angle

The start angle is not a continuous state (modal) value. It must be specified each time it is used. If a value
is not specified, 0 is assumed.

- Start angle increment

The start angle (Q) increment is 0.001 degrees. Note that no decimal point can be specified.
Example:

B-64604EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- 33 -

For a shift angle of 180 degrees, specify Q180000.

Q180.000 cannot be specified, because it contains a decimal point.

Note: Q1 is the command of 0.001 degree for the angle for shifting the threading start angle, regardless of

the setting of the followings.

Increment system IS-A/B/C(Parameter No.1013#1,#0)

Pocket calculator type decimal point programming (Bit 0(DPI) of parameter No.3401)

The least input increment is 10 times greater than the least command increment (Bit 7(IPR) of
parameter No.1004)

- Specifiable start angle range

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be specified. If a value greater than
360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).
If a minus value is specified, it works as a plus value.
Example:

If Q-90000 (-90 degrees) is specified, it works as Q90000 (90 degrees).

- Multiple threading cycle (G76 (G code system A/B)) (G78 (G code system C))

The address Q of the G76/G78 multiple threading cycle command is used for the minimum cutting depth
or the depth of cut in 1st cut. For this reason, the angle for shifting the threading start angle can not be
commanded.
However, if the FS10/11 tape format is used, in G76/G78 multiple threading cycle, the address Q is
possible to specify the angle for shifting the threading start angle.

Example

Program for producing double-threaded screws (with start angles of 0 and 180
degrees)

X40.0 ;
W-38.0 F4.0 Q0 ;
X72.0 ;
W38.0 ;
X40.0 ;
W-38.0 F4.0Q180000 ;
X72.0 ;
W38.0 ;

PROGRAMMING

B-64604EN-1/01

- 34 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

FUNCTIONS TO SIMPLIFY PROGRAMMING

Chapter 4, "FUNCTIONS TO SIMPLIFY PROGRAMMING", consists of the following sections:

4.1 CANNED CYCLE (G90, G92, G94)..................................................................................................34
4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) ...............................................................52
4.3 CANNED

CYCLE

FOR DRILLING .................................................................................................91

4.4 RIGID

TAPPING..............................................................................................................................106

4.5  CANNED GRINDING CYCLE (FOR GRINDING MACHINE)....................................................119
4.6  CHAMFERING AND CORNER R ..................................................................................................129
4.7  MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) ...............................................................135
4.8  DIRECT DRAWING DIMENSION PROGRAMMING .................................................................136

4.1

CANNED CYCLE (G90, G92, G94)

There are three canned cycles : the outer diameter/internal diameter cutting canned cycle (G90), the
threading canned cycle (G92), and the end face turning canned cycle (G94).

NOTE

1 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.

2 A 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.

3 The direction of the length means the direction of the first axis on the plane as

follows:

ZX plane: Z-axis direction

YZ plane: Y-axis direction

XY plane: X-axis direction

4 The direction of the end face means the direction of the second axis on the

plane as follows:

ZX plane: X-axis direction

YZ plane: Z-axis direction

XY plane: Y-axis direction

B-64604EN-1/01

PROGRAMMING

- 35 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.1.1

Outer Diameter/Internal Diameter Cutting Cycle (G90)

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

4.1.1.1

Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.1 (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. 4.1.1.1 (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

- 36 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

4.1.1.2

Taper cutting cycle

Format

G90 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the

direction of the length

: Taper amount (R in the Fig. 4.1.1.2 (a))

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 ve rs e
(F ) ....C u ttin g fe e d

Fig. 4.1.1.2 (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
length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.1.2 (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 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.

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 R)
and the cutting end point in the direction of the length in the absolute or incremental programming as
Table 4.1.1.2 (a).

B-64604EN-1/01

PROGRAMMING

- 37 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

Table 4.1.1.2 (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.

4.1.2

Threading Cycle (G92)

4.1.2.1

Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.1 (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. 4.1.2.1 (a))

PROGRAMMING

B-64604EN-1/01

- 38 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

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. 4.1.2.1 (a) Straight threading

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 after interpolation for threading

Acceleration/deceleration after interpolation for threading 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

- 39 -

4.FUNCTIONS TO SIMPLIFY

PROGRAMMING

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

Table 4.1.2.1 (a)

Bit 0 (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.

PROGRAMMING

B-64604EN-1/01

- 40 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

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.

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 retreat.

- Inch threading

Inch threading specified with address E is not allowed.

4.1.2.2

Taper threading cycle

Format

G92 X(U)_Z(W)_R_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.2 (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)

: Taper amount (R in the Fig. 4.1.2.2 (a))

: Thread lead (L in the Fig. 4.1.2.2 (a))

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 3