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

B-64604EN-1/01

PROGRAMMING

- 265 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Unit

Diameter/radius

programming

Sign

Decimal point

input

Depends on the increment
system for the reference axis.

Radius programming

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

u/2

Target figure

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

(R)

(F)

Fig. 6.4.3 (c) 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 After cycle operation terminates, the tool returns to point A.
2 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.

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 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’.

B-64604EN-1/01

PROGRAMMING

- 267 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.4

Finishing Cycle (G70)

After rough cutting by G71, G72 or G73, the following command permits finishing.

Format

G70 P(ns) Q(nf) ;

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.

Explanation

- Operations

The blocks with sequence numbers ns to nf in the program for a target figure are executed for finishing.
The F, S, T, M, and second auxiliary functions specified in the G71, G72, or G73 block are ignored and
the F, S, T, M, and second auxiliary functions specified in the blocks with sequence numbers ns to nf are
effective.
When cycle operation terminates, the tool is returned to the start point in rapid traverse and the next G70
cycle block is read.

- Target figure
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.

Storing P and Q blocks

When rough cutting is executed by G71, G72, or G73, up to three memory addresses of P and Q blocks
are stored. By this, the blocks indicated by P and Q are immediately found at execution of G70 without
searching memory from the beginning for them. After some G71, G72, and G73 rough cutting cycles are
executed, finishing cycles can be performed by G70 at a time. At this time, for the fourth and subsequent
rough cutting cycles, the cycle time is longer because memory is searched for P and Q blocks.

Example

G71 P100 Q200 ...;

N100

...;

...;
...;
N200

...;

G71 P300 Q400 ...;

N300

...;

...;
...;
N400

...;

...;
...;

G70 P100 Q200 ; (Executed without a search for the first to third cycles)

G70 P300 Q400 ; (Executed after a search for the fourth and subsequent

cycles)

PROGRAMMING

B-64604EN-1/01

- 268 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

NOTE

The memory addresses of P and Q blocks stored during rough cutting cycles by
G71, G72, and G73 are erased after execution of G70.

All stored memory addresses of P and Q blocks are also erased by a reset.

Return to the cycle start point

In a finishing cycle, after the tool cuts the workpiece to the end point of the target figure, it returns to the
cycle start point in rapid traverse.

NOTE

The tool returns to the cycle start point always in the nonlinear positioning mode
regardless of the setting of bit 1 (LRP) of parameter No. 1401.

Before executing a finishing cycle for a target figure with a pocket cut by G71 or
G72, check that the tool does not interfere with the workpiece when returning
from the end point of the target figure to the cycle start point.

Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41 or
G42) before a multiple repetitive canned cycle command (G70) and specify the cancel command (G40)
after the multiple repetitive canned cycle command (G70).

Program example
G42;..............................Specify this command before a multiple repetitive canned cycle command.
G70P10Q20;
G40;..............................Specify this command after a multiple repetitive canned cycle command.

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'.

B-64604EN-1/01

PROGRAMMING

- 269 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

Example

Stock removal in facing (G72)

(Diameter designation for X axis, metric input)

N011

G50 X220.0 Z190.0 ;

N012

G00 X176.0 Z132.0 ;

N013

G72 P014 Q019 U4.0 W2.0 D7000 F0.3 S550 ;

N014

G00 Z56.0 S700 ;

N015 G01 X120.0 W14.0 F0.15 ;
N016 W10.0

;

N017 X80.0

W10.0

;

N018 W20.0

;

N019 X36.0

W22.0

;

N020

G70 P014 Q019 ;

Parameter No. 5133 = 1.0 (escaping amount)
Finishing allowance (4.0 in diameter in the X direction, 2.0 in the Z direction)

120

160

Start point

Z axis

X axis

190

PROGRAMMING

B-64604EN-1/01

- 270 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Pattern repeating (G73)

(Diameter designation, metric input)

180

Z axis

X axis

220

130

160

120

N011

G50 X260.0 Z220.0 ;

N012

G00 X220.0 Z160.0 ;

N013

G73 P014 Q019 U4.0 W2.0 I14.0 K14.0 D3 F0.3 S0180

N014

G00 X80.0 W-40.0 ;

N015

G01 W-20.0 F0.15 S0600 ;

N016 X120.0

W-10.0;

N017

W-20.0 S0400 ;

N018

G02 X160.0 W-20.0 R20.0 ;

N019

G01 X180.0 W-10.0 S0280 ;

N020

G70 P014 Q019 ;

B-64604EN-1/01

PROGRAMMING

- 271 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.5

End Face Peck Drilling Cycle (G74)

This cycle enables chip breaking in outer diameter cutting. If the second axis on the plane (X-axis
(U-axis) for the ZX plane) and address P are omitted, operation is performed only along the first axis on
the plane (Z-axis for the ZX plane), that is, a peck drilling cycle is performed.

Format

ZpXp-plane

G74X(U)_ Z(W)_ I(

i) K(

k) D(

d) F(f ) ;

YpZp-plane

G74Y(V)_ Z(W)_ J(

k) K(

i) D(

d) F(f ) ;

XpYp-plane

G74X(U)_ Y(V)_ I(

k) J(

i) D(

d) F(f ) ;

X_,Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B

and

Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C

U_,W_ : Travel distance along the second axis on the plane (U for the ZX plane) from

point A to B

Travel distance along the first axis on the plane (W for the ZX plane) from point

A to C
(When G code system A is used. In other cases, X_, Z_ is used for
specification.)

: Travel distance in the direction of the second axis on the plane (X-axis for the

ZX plane)

: Depth of cut in the direction of the first axis on the plane (Z-axis for the ZX

plane)

: Relief amount of the tool at the cutting bottom

f :

Feedrate

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

Depends on the increment system for
the reference axis.

Radius programming

NOTE 1

Not allowed

NOTE

1 Normally, specify a positive value for

d. When X (U) and

i are omitted, specify

a value with the sign indicating the direction in which the tool is to escape.

2 Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)

of parameter No. 3401 = 1), the unit of address D is least input increment. In
addition, when a decimal point is input in address D, an alarm PS0007,
“ILLEGAL USE OF DECIMAL POINT” is issued.

PROGRAMMING

B-64604EN-1/01

- 272 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

U/2

i’

(R)

(F)

(R)

(F)

[0 <

k’

≤

(R)

[0 <

i’

≤

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

e : Return amount (parameter No.5139)

Fig. 6.4.5 (a) Cutting path in end face peek drilling cycle

Explanation

- Operations

A cycle operation of cutting by

k and return by e is repeated.

When cutting reaches point C, the tool escapes by

d. Then, the tool returns in rapid traverse, moves to

the direction of point B by

i, and performs cutting again.

Return amount (e)

The return amount (e) is set in parameter No. 5139.

No. Unit

Diameter/radius

programming

Sign

5139

Depends on the increment system for the
reference axis.

Radius programming

Not required

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

B-64604EN-1/01

PROGRAMMING

- 273 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.6

Outer Diameter / Internal Diameter Drilling Cycle (G75)

This cycle is equivalent to G74 except that the second axis on the plane (X-axis for the ZX plane)
changes places with the first axis on the plane (Z-axis for the ZX plane). This cycle enables chip breaking
in end facing. It also enables grooving during outer diameter cutting and cutting off (when the Z-axis
(W-axis) and Q are omitted for the first axis on the plane).

Format

ZpXp-plane

G75 X(U)_ Z(W)_ I(

i) K(

k) D(

d) F (f ) ;

YpZp-plane

G75 Y(V)_ Z(W)_ J(

k) K(

i) D(

d) F(f ) ;

XpYp-plane

G75 X(U)_ Y(V)_ I(

k) J(

i) D(

d) F(f ) ;

X_, Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B

and

Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C

U_, W_ : Travel distance along the second axis on the plane (U for the ZX plane) from

point A to B

Travel distance along the first axis on the plane (W for the ZX plane) from point

A to C

: Depth of cut in the direction of the second axis on the plane (X-axis for the ZX

plane)

: Travel distance in the direction of the first axis on the plane (Z-axis for the ZX

plane)

: Relief amount of the tool at the cutting bottom

f :

Feedrate

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

Depends on the increment system for
the reference axis.

Radius programming

NOTE 1

Not allowed

NOTE

1 Normally, specify a positive value for

d. When Z (W) and

k are omitted,

specify a value with the sign indicating the direction in which the tool is to
escape.

2 Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)

of parameter No. 3401 = 1), the unit of address D is least input increment. In
addition, when a decimal point is input in address D, an alarm PS0007,
“ILLEGAL USE OF DECIMAL POINT” is issued.

PROGRAMMING

B-64604EN-1/01

- 274 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

(R)

(F)

(R)

(F)

(R)

(F)

(R)

U/2

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

(R)

i’

e : Return amount (parameter No.5139)

Fig. 6.4.6 (a) Outer diameter/internal diameter drilling cycle

Explanation

- Operations

A cycle operation of cutting by

i and return by e is repeated.

When cutting reaches point B, the tool escapes by

d. Then, the tool returns in rapid traverse, moves to

the direction of point C by

k, and performs cutting again.

Both G74 and G75 are used for grooving and drilling, and permit the tool to relief automatically. Four
symmetrical patterns are considered, respectively.

Return amount (e)

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

No. Unit

Diameter/radius

programming

Sign

5139

Depends on the increment system for the
reference axis.

Radius programming

Not required

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

B-64604EN-1/01

PROGRAMMING

- 275 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.4.7

Multiple Threading Cycle (G76)

The multiple threading cycle can select four cutting methods.

Format

ZpXp-plane

G76 X(U)_ Z(W)_ I(i) K(k) D(

d) A(a) F(L) P(p) Q(q) ;

YpZp-plane

G76 Y(V)_ Z(W)_ J(k) K(i) D(

d) A(a) F(L) P(p) Q(q) ;

XpYp-plane

G76 X(U)_ Y(V)_ I(k) J(i) D(

d) A(a) F(L) P(p) Q(q) ;

X_, Z_ : Coordinates of the cutting end point (point D in the figure) in the direction of the

length

U_, W_ : Travel distance to the cutting end point (point D in the figure) in the direction of the

length

: Angle of tool nose

From 0 to 120 in steps of 1 degree (The default is 0.)

i :

Taper

amount

If i = 0, ordinary straight threading can be made.

: Height of thread

: Depth of cut in 1st cut

: Lead of thread

: Cutting method (one-edge threading with constant cutting amount by default or for

P0)
P1 :  One-edge threading with constant cutting amount
P2 :  Both-edge zigzag threading with constant cutting amount
P3 :  One-edge threading with constant depth of cut
P4 :  Both-edge zigzag threading with constant depth of cut

: Threading start angle shift (From 0 to 360 degrees in steps of 0.001 degrees)

NOTE

1 Even if pocket calculator type decimal point programming is specified (bit 0 (DPI)

of parameter No. 3401 = 1), the unit of address D is least input increment. In
addition, when a decimal point is input in address D, an alarm PS0007,
“ILLEGAL USE OF DECIMAL POINT” is issued.

2 A decimal point included in address A has no meaning. That is, ‘A120.’ is

equivalent to ‘A120’ in specifying 120 degrees.

3 Address Q does not allow decimal point input.

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

Not required

Allowed

Depends on the increment system for
the reference axis.

Radius programming

Not required

Not allowed

PROGRAMMING

B-64604EN-1/01

- 276 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

(F)

(R)

U/2

(R)

r: Amount of thread chamfering (parameter No.5130)

Fig. 6.4.7 (a) Cutting path in multiple threading cycle

Explanation

- Operations

This cycle performs threading so that the length of the lead only between C and D is made as specified in
the F code. In other sections, the tool moves in rapid traverse.
The time constant for acceleration/deceleration after interpolation and FL feedrate for thread chamfering
and the feedrate for retraction after chamfering are the same as for thread chamfering with canned cycle.

CAUTION

Notes on threading are the same as those on G32 threading. For feed hold in a
threading cycle, however, see "Feed hold in a threading cycle" described below.

- Cutting method

There are four cutting methods.

Tool tip

1st

3rd

2nd

nth

One-edge thread cutting with constant cutting amount(P1)

d (finishing allowance)

4th

√

Tool tip

Both-edge zigzag thread cutting with constant cutting amount(P2)

d (finishing allowance)

√

⋅Δ

d / 2

1st

2nd

3rd

5th

6th

Fig. 6.4.7 (b) One-edge threading with constant cutting amount,

both-edge zigzag threading with constant cutting amount (P1/2)

B-64604EN-1/01

PROGRAMMING

- 277 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

d (finishing allowance)

One-edge thread cutting with constant depth of cut (P3)

d (finishing allowance)

Both-edge zigzag thread cutting with constant depth of cut (P4)

Tool tip

Fig. 6.4.7 (c) One-edge threading with constant depth of cut,

both-edge zigzag threading with constant depth of cut (P3/4)

Repetitive count in finishing

The last finishing cycle (cycle in which the finishing allowance is removed by cutting) is repeated.
The repetitive count is set in parameter No. 5142.
If the setting is 0, the operation is performed once.

d (finishing allowance)

Last finishing cycle

Minimum depth of cut

When a cutting method with constant cutting amount is selected (P1 or P2), clamping can be performed
with the minimum depth of cut to prevent the depth of cut from becoming too small.
The minimum depth of cut is set in parameter No. 5140.

No. Unit

Diameter/radius

programming

Sign

5140

Depends on the increment system for the
reference axis.

Radius programming

Not required

- Finishing allowance

The finishing allowance is set in parameter No. 5141.

No. Unit

Diameter/radius

programming

Sign

5141

Depends on the increment system for the
reference axis.

Radius programming

Not required

NOTE

Set a value smaller than the height of thread as the finishing allowance. (No.
5141 < k)

PROGRAMMING

B-64604EN-1/01

- 278 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

Relationship between the sign of the taper amount and tool path

The signs of incremental dimensions for the cycle shown in Fig. 6.4.7 (a) are as follows:
Cutting end point in the direction of the length for U and W:

Minus (determined according to the directions of paths A-C and C-D)

Taper amount (i)

: Minus (determined according to the direction of path A-C)

Height of thread (k)

: Plus (always specified with a plus sign)

Depth of cut in the first cut (

d) : Plus (always specified with a plus sign)

The four patterns shown in the Table 6.4.7 (a) are considered corresponding to the sign of each address. A
female thread can also be machined.

Table 6.4.7 (a)

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, i < 0

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

U/2

3(R)

4(R)

1(R)

2(F)

U/2

3(R)

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(R)

4(R)

1(R)

2(F)

U/2

3(R)

4(R)

1(R)

2(F)

- 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.

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 in this threading cycle. A signal from the machine tool initiates
thread chamfering.
The maximum amount of thread chamfering (r) can be specified in a range from 0.1L to 12.7L in 0.1L
increments in parameter No. 5130.

B-64604EN-1/01

PROGRAMMING

- 279 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

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 G92 threading cycle.

Retraction after chamfering

The Table 6.4.7 (b) lists the feedrate, type of acceleration/deceleration after interpolation, and time
constant of retraction after chamfering.

Table 6.4.7 (b)

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.

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 start angle of threading.
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 when the threading cycle retract function is used

When feed hold is applied during threading in a multiple threading cycle (G76), the tool quickly retracts
in the same way as for the last chamfering in a threading cycle and returns to the start point in the current
cycle.
When cycle start is triggered, the multiple threading cycle resumes.

PROGRAMMING

B-64604EN-1/01

- 280 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

F e e d h o ld is a p plied a t th is po in t

Sta rt p o in t
in the c urre n t c yc le

O rd in a ry c yc le

R a p id tra ve rs e

M o tio n a t fe ed h old

X -a xis

Z -a xis

C u ttin g fe ed

The angle of chamfering during retraction is the same as that of chamfering at the end point.

CAUTION

Feed hold operation during retraction is disabled.

- Inch threading

Inch threading specified with address E is allowed.

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

Example

G00 X80.0 Z130.0;
G76 X60.64 Z25.0 K3680 D1800 A60 P1 F6.0 ;
Parameter No.5130 = 10(1.0L)

Z axis

105

60.

X axis

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 18