Content      ..     2      3      4      5     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 4

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

4.2.2

Stock Removal in Facing (G72)

This cycle is the same as G71 except that cutting is performed by an

operation parallel to the second axis on the plane (X-axis for the ZX

plane).

Format

ZpXp plane

G72 W(∆d) R(e) ;

G72 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;

N (ns) ;

The move commands for the target figure from A

to A’ to B are specified in the blocks with

N (nf) ;

sequence numbers ns to nf.

YpZp plane

G72 V(∆d) R(e) ;

G72 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ;

N (ns) ;

N (nf) ;

XpYp plane

G72 U(∆d) R(e) ;

G72 P(ns) Q(nf) U(∆w) W(∆u) F(f ) S(s ) T(t ) ;

N (ns) ;

N (nf) ;

∆d

: Depth of cut

The cutting direction depends on the direction AA'. This

designation is modal and is not changed until the other

value is designated. Also this value can be specified by

the parameter (No. 5132), and the parameter is changed

by the program command.

e

: Escaping amount

This designation is modal and is not changed until the

other value is designated. Also this value can be

specified by the parameter (No. 5133), and the

parameter is changed by the program command.

ns

: Sequence number of the first block for the program of

finishing shape.

nf

: Sequence number of the last block for the program of

finishing shape.

∆u

: Distance of the finishing allowance in the direction of the

second axis on the plane (X-axis for the ZX plane)

∆w : Distance of the finishing allowance in the direction of the

first axis on the plane (Z-axis for the ZX plane)

f,s,t : Any F , S, or T function contained in blocks ns to nf in

the cycle is ignored, and the F, S, or T function in this

G72 block is effective.

- 74 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the

∆d

increment system for

Radius programming

Not required

Allowed

the reference axis.

Depends on the

e

increment system for

Radius programming

Not required

Allowed

the reference axis.

Depends on

Depends on the

diameter/radius

∆u

increment system for

Required

Allowed

programming for the

the reference axis.

second axis on the plane.

Depends on

Depends on the

diameter/radius

∆w

increment system for

Required

Allowed

programming for the first

the reference axis.

axis on the plane.

∆d

(F): Cutting feed

(R): Rapid traverse

C

A'

A

Tool path

(F)

(R)

e

(R)

45°

Target figure

(F)

+X

∆u/2

B

+Z

∆w

Fig. 4.2.2 (q) Cutting path in stock removal in facing (type I)

- 75 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

Explanation

- Operations

When a target figure passing through A, A', and B in this order is

given by a program, the specified area is removed by ∆d (depth of cut),

with the finishing allowance specified by ∆u/2 and ∆w left.

NOTE

1 While both ∆d and ∆u are specified by the same

address, the meanings of them are determined by

the presence of addresses P and Q.

2 The cycle machining is performed by G72

command with P and Q specification.

3 F, S, and T functions which are specified in the

move command between points A and B are

ineffective and those specified in G72 block or the

previous block are effective. M and second

auxiliary functions are treated in the same way as

F, S, and T functions.

4 When the constant surface speed control function

is enabled (bit 0 (SSC) of parameter No. 8133 is

set to 1), the G96 or G97 command specified in the

move command between points A and B is

ignored. If you want to enable the G96 or G97

command, specify the command in the G71 or

previous block.

- Target figure

Patterns

The following four cutting patterns are considered. All of these cutting

cycles cut the workpiece with moving the tool in parallel to the second

axis on the plane (X-axis for the ZX plane). At this time, the signs of

the finishing allowances of ∆u and ∆w are as follows:

+X

B

B

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

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

+Z

A A

A'

A'

Both linear and circular

interpolation are possible

A'

A'

A

A

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

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

B B

Fig. 4.2.2 (r) Signs of the values specified at U and W in stock removal in

facing

- 76 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

Limitation

(1) For W(+), a figure for which a position higher than the cycle start

point is specified cannot be machined.

For W(-), a figure for which a position lower than the cycle start

point is specified cannot be machined.

(2) For type I, the figure must show monotone increase or decrease

along the first and second axes on the plane.

(3) For type II, the figure must show monotone increase or decrease

along the second axis on the plane.

- Start block

In the start block in the program for a target figure

(block with

sequence number ns in which the path between A and A' is specified),

G00 or G01 must be specified. If it is not specified, alarm PS0065 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.

- 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

Enabled when bit 2 (QSR)

number specified at address Q is contained

of parameter No. 5102 is

in the program before cycle operation.

set to 1.

Checks the target figure before cycle

Enabled when bit 2 (FCK)

operation.

of parameter No. 5104 is

(Also checks that a block with the sequence

set to 1.

number specified at address Q is contained.)

- Types I and II

Selection of type I or II

For G72, there are types I and II.

When the target figure has pockets, be sure to use type II.

Escaping operation after rough cutting in the direction of the second

axis on the plane (X-axis for the ZX plane) differs between types I and

II. With type I, the tool escapes to the direction of 45 degrees. With

type II, the tool cuts the workpiece along the target figure. When the

target figure has no pockets, determine the desired escaping operation

and select type I or II.

- 77 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

4.2.3

Pattern Repeating (G73)

This function permits cutting a fixed pattern repeatedly, with a pattern

being displaced bit by bit. By this cutting cycle, it is possible to

efficiently cut work whose rough shape has already been made by a

rough machining, forging or casting method, etc.

Format

ZpXp plane

G73 W(∆k) U(∆i) R(d) ;

G73 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;

N (ns) ;

The move commands for the target figure from A to A’ to B are specified in

the blocks with sequence numbers ns to nf.

N (nf) ;

YpZp plane

G73 V(∆k) W(∆i) R(d) ;

G73 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ;

N (ns) ;

N (nf) ;

XpYp plane

G73 U(∆k) V(∆i) R(d) ;

G73 P(ns) Q(nf) U(∆w) V(∆u) F(f ) S(s ) T(t ) ;

N (ns) ;

N (nf) ;

∆i

: Distance of escape in the direction of the second axis on the plane (X-axis for the ZX

plane)

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

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

the program command.

∆k

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

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

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

the program command.

d

: The number of division

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

modal and is not changed until the other value is designated. Also, this value can be

specified by the parameter No. 5137, and the parameter is changed by the program

command.

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, and T function contained in the blocks between sequence number "ns" and

"nf" are ignored, and the F, S, and T functions in this G73 block are effective.

- 79 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment

∆i

system for the reference

Radius programming

Required

Allowed

axis.

Depends on the increment

∆k

system for the reference

Radius programming

Required

Allowed

axis.

Depends on

Depends on the increment

diameter/radius

∆u

system for the reference

Required

Allowed

programming for the

axis.

second axis on the plane.

Depends on

Depends on the increment

diameter/radius

∆w

system for the reference

Required

Allowed

programming for the first

axis.

axis on the plane.

NOTE

Decimal point input is allowed with d. However, a

value rounded off to an integer is used as the

number of division, regardless of the setting of bit 0

(DPI) of parameter No. 3401. When an integer is

input, the input integer is used as the number of

division.

∆k+∆w

D

∆w

∆i+∆u/2

∆u/2

C

A

(R)

(R)

B

(F)

∆u/2

A'

∆w

+X

(F): Cutting feed

Target figure

(R): Rapid traverse

+Z

Fig. 4.2.3 (s) Cutting path in pattern repeating

- 80 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

Explanation

- Operations

When a target figure passing through A, A', and B in this order is

given by a program, rough cutting is performed the specified number

of times, with the finishing allowance specified by ∆u/2 and ∆w left.

NOTE

1 While the values ∆i and ∆k, or ∆u and ∆w are

specified by the same address respectively, the

meanings of them are determined by the presence

of addresses P and Q.

2 The cycle machining is performed by G73

command with P and Q specification.

3 After cycle operation terminates, the tool returns to

point A.

4 F, S, and T functions which are specified in the

move command between points A and B are

ineffective and those specified in G73 block or the

previous block are effective. M and second

auxiliary functions are treated in the same way as

F, S, and T functions.

- Target figure

Patterns

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

about signs of ∆u, ∆w, ∆i, and ∆k 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’.

- Check function

The following check can be made.

Check

Related parameter

Checks that a block with the sequence

Enabled when bit 2 (QSR)

number specified at address Q is contained

of parameter No. 5102 is

in the program before cycle operation.

set to 1.

- Tool nose radius compensation

Like G71, this cycle operation is performed according to the figure

determined by the tool nose radius compensation path when the offset

vector is

0 at start point A and start-up is performed in a block

between path A-A'.

- 81 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

4.2.4

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

Enabled when bit 2 (QSR)

number specified at address Q is contained

of parameter No. 5102 is

in the program before cycle operation.

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.

- 82 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

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)

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

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'.

- 83 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

Example

Stock removal in facing (G72)

X axis

2

Start point

7

Z axis

60

10

10

10

20

20

2

190

(Diameter designation for X axis, metric input)

N010 G50 X220.0 Z190.0 ;

N011 G00 X176.0 Z132.0 ;

N012 G72 W7.0 R1.0 ;

N013 G72 P014 Q019 U4.0 W2.0 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 ;

Escaping amount:

1.0

Finishing allowance (4.0 in diameter in the X direction, 2.0 in the Z direction)

- 84 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

Pattern repeating (G73)

16

B

X axis

Z axis

0

2

14

20

40

10

40

10

20

40

220

(Diameter designation, metric input)

N010

G50 X260.0 Z220.0 ;

N011

G00 X220.0 Z160.0 ;

N012

G73 U14.0 W14.0 R3 ;

N013

G73 P014 Q019 U4.0 W2.0 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 ;

- 85 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

4.2.5

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

G74R (e) ;

G74X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) F (f ) ;

e

: Return 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. 5139, and the

parameter is changed by the program command.

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.)

∆i

: Travel distance in the direction of the second axis on

the plane (X-axis for the ZX plane)

∆k

: Depth of cut in the direction of the first axis on the

plane (Z-axis for the ZX plane)

∆d

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment

e

Radius programming

Not required

Allowed

system for the reference axis.

Depends on the increment

∆i

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

∆k

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

∆d

Radius programming

NOTE

Allowed

system for the reference axis.

NOTE

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.

- 86 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

∆k'

∆k

∆k

∆k

∆k

[0 < ∆k’ ≤ ∆k]

∆d

A

∆i

C

(R)

(R)

(F)

(F)

(F)

(F)

(F)

U/2

(R)

(R)

(R)

(R)

∆i

[0 < ∆i’ ≤ ∆i]

∆i’

X

B

Z

W

+X

(R) ... Rapid traverse

(F) ... Cutting feed

e

+Z

Fig. 4.2.5 (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.

NOTE

1 While both e and ∆d are specified by the same

address, the meanings of them are determined by

specifying the X, Y, or Z axis. When the axis is

specified, ∆d is used.

2 The cycle machining is performed by G74

command with specifying the axis.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 87 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

4.2.6

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

G75R (e) ;

G75X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) F (f ) ;

e

: Return 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. 5139, and the

parameter is changed by the program command.

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.)

∆i

: Depth of cut in the direction of the second axis on

the plane (X-axis for the ZX plane)

∆k

: Travel distance in the direction of the first axis on

the plane (Z-axis for the ZX plane)

∆d

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment

e

Radius programming

Not required

Allowed

system for the reference axis.

Depends on the increment

∆i

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

∆k

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

∆d

Radius programming

NOTE

Allowed

system for the reference axis.

NOTE

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.

- 88 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

C

(R)

A

(R)

(F)

∆i

e

(R)

(F)

∆i

(R)

U/2

(F)

∆i

(R)

(F)

∆i

(R)

(F)

∆i’

B

∆d

∆k

X

Z

W

+X

(R) ... Rapid traverse

(F) ... Cutting feed

+Z

Fig. 4.2.6 (b) 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.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 89 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

4.2.7

Multiple Threading Cycle (G76)

This threading cycle performs one edge cutting by the constant

amount of cut.

Format

G76 P(m) (r) (a) Q(∆dmin) R(d ) ;

G76 X(U)_ Z(W)_ R(i ) P(k ) Q(∆d) F (L ) ;

m : Repetitive count in finishing (1 to 99)

This value can be specified by the parameter No. 5142,

and the parameter is changed by the program command.

r

: Chamfering amount (0 to 99)

When the thread lead is expressed by L, the value of L

can be set from 0.0L to 9.9L in 0.1L increment (2-digit

number). This value can be specified by the parameter

No. 5130, and the parameter is changed by the program

command.

a

: Angle of tool nose

One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°,

can be selected, and specified by 2-digit number. This

value can be specified by the parameter No. 5143, and

the parameter is changed by the program command.

m, r, and a are specified by address P at the same time.

(Example) When m=2, r=1.2L, a=60°, specify as shown

below (L is lead of thread).

P

02

12

60

a

r

m

∆dmin

: Minimum cutting depth

When the cutting depth of one cycle operation

becomes smaller than this limit, the cutting depth is

clamped at this value. This value can be specified

by parameter No. 5140, and the parameter is

changed by the program command.

d

: Finishing allowance

This value can be specified by parameter No. 5141,

and the parameter is changed by the program

command.

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

(When G code system A is used. In other cases,

X_,Z_ is used for specification.)

i

: Taper amount

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

k

: Height of thread

∆d

: Depth of cut in 1st cut

L

: Lead of thread

- 90 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment

∆dmin

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

d

Radius programming

Not required

Allowed

system for the reference axis.

Depends on the increment

i

Radius programming

Required

Allowed

system for the reference axis.

Depends on the increment

k

Radius programming

Not required

Not allowed

system for the reference axis.

Depends on the increment

∆d

Radius programming

Not required

Not allowed

system for the reference axis.

E

(R)

A

(R)

(R)

U/2

B

(F)

∆d

D

i

k

X

r

C

Z

W

+X

+Z

Fig. 4.2.7 (c) Cutting path in multiple threading cycle

Tool nose

B

a

∆d

∆d√n

1st

k

2nd

3rd

nth

d

Fig. 4.2.7 (d) Detail of cutting

- 91 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

- Repetitive count in finishing

The last finishing cycle (cycle in which the finishing allowance is

removed by cutting) is repeated.

+X

k

+Z

Last finishing cycle

d (finishing allowance)

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 G92 (canned

cycle).

NOTE

1 The meanings of the data specified by address P,

Q, and R determined by the presence of X (U) and

Z (W).

2 The cycle machining is performed by G76

command with X (U) and Z (W) specification.

3 The values specified at addresses P, Q, and R are

modal and are not changed until another value is

specified.

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.

- 92 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

- Relationship between the sign of the taper amount and tool path

The signs of incremental dimensions for the cycle shown in Fig. 4.2.7

(c) 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 below are considered

corresponding to the sign of each address. A female thread can also be

machined.

Outer diameter machining

Internal diameter machining

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

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

X

X

W

Z

Z

4(R)

2(F)

i

U/2

3(R)

1(R)

X

U/2

3(R)

1(R)

i

X

2(F)

4(R)

W

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

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

at |i|≤|U/2|

at |i|≤|U/2|

X

X

Z

W

Z

4(R)

1(R)

i

2(F)

X

U/2

3(R)

U/2

3(R)

2(F)

1(R)

i

4(R)

W

X

- 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 bit

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.

- 93 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

- 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.

- 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) that can be specified

in the command is 99 (9.9L). The amount can be specified in a range

from 0.1L to 12.7L in 0.1L increments in parameter No. 5130.

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 following table lists the feedrate, type of acceleration/deceleration

after interpolation, and time constant of retraction after chamfering.

Parameter

Parameter

CFR (No.

Description

No. 1466

1611#0)

Uses the type of acceleration/deceleration after

interpolation for threading, time constant for

Other than

0

threading (parameter No. 1626), FL feedrate

0

(parameter No. 1627), and retraction feedrate

specified in parameter No. 1466.

Uses the type of acceleration/deceleration after

interpolation for threading, time constant for

0

0

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

1

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.

- 94 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

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

The threading start angle cannot be shifted.

- Feed hold in a threading cycle（threading cycle retract）

Feed hold may be applied during threading in a combined threading

cycle (G76). In this case, 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 (position where the workpiece is cut by

∆dn).

When cycle start is triggered, the multiple threading cycle resumes.

X-axis

Ordinary cycle

Motion at feed hold

Z-axis

Start point

(position where the

workpiece is cut by ∆dn)

Rapid traverse

Feed hold is applied at this point.

The angle of chamfering during retraction is the same as that of

chamfering at the end point.

CAUTION

Another feed hold cannot be performed during

retraction.

- Inch threading

Inch threading specified with address E is not allowed.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 95 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

Example

X axis

Z axis

0

6

25

105

G80 X80.0 Z130.0;

G76 P011060 Q100 R200 ;

G76 X60.64 Z25.0 P3680 Q1800 F6.0 ;

- 96 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

4.3

CANNED CYCLE FOR DRILLING

Canned cycles for drilling make it easier for the programmer to create

programs. With a canned cycle, a frequently-used machining

operation can be specified in a single block with a G function; without

canned cycles, more than one block is required. In addition, the use of

canned cycles can shorten the program to save memory.

Table 4.3 (a) lists canned cycles for drilling.

Table 4.3 (a) Canned cycles for drilling

Operation in

Drilling

Hole machining

Retraction

G code

the bottom hole

Applications

axis

operation

operation

position

G80

-

-

-

-

Cancel

Cutting feed /

Front drilling

G83

Z axis

Dwell

Rapid traverse

intermittent

cycle

Dwell →

Front tapping

G84

Z axis

Cutting feed

Cutting feed

spindle CCW

cycle

Front boring

G85

Z axis

Cutting feed

Dwell

Cutting feed

cycle

Cutting feed /

Side drilling

G87

X axis

Dwell

Rapid traverse

intermittent

cycle

Dwell →

Side tapping

G88

X axis

Cutting feed

Cutting feed

Spindle CCW

cycle

Side boring

G89

X axis

Cutting feed

Dwell

Cutting feed

cycle

Explanation

The canned cycle for drilling consists of the following six operation

sequences.

Operation 1

Positioning of X (Z) and C axis

Operation 2

Rapid traverse up to point R level

Operation 3

Hole machining

Operation 4

Operation at the bottom of a hole

Operation 5

Retraction to point R level

Operation 6

Rapid traverse up to the initial level

- 99 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

Operation 1

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Fig. 4.3 (a) Operation sequence of canned cycle for drilling

- Positioning axis and drilling axis

The C-axis and X- or Z-axis are used as positioning axes. The X- or

Z-axis, which is not used as a positioning axis, is used as a drilling

axis. A drilling G code specifies positioning axes and a drilling axis as

shown below.

Although canned cycles include tapping and boring cycles as well as

drilling cycles, in this chapter, only the term drilling will be used to

refer to operations implemented with canned cycles.

Table 4.3 (b) Positioning axis and drilling axis

G code

Positioning axis

Drilling axis

G83, G84, G85

X axis, C axis

Z axis

G87, G88, G89

Z axis, C axis

X axis

G83 and G87, G84 and G88, and G85 and G89 have the same

function respectively except for axes specified as positioning axes and

a drilling axis.

- Drilling mode

G83 to G85/G87 to G89 are modal G codes and remain in effect until

canceled. When in effect, the current state is the drilling mode.

Once drilling data is specified in the drilling mode, the data is retained

until modified or canceled.

Specify all necessary drilling data at the beginning of canned cycles;

when canned cycles are being performed, specify data modifications

only.

The feedrate specified at F is retained also after the drilling cycle is

canceled. When Q data is required, it must be specified in each block.

Once specified, the M code used for C-axis clamp/unclamp functions

as a modal code. It is canceled by specifying G80.

- 100 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

- Return point level (G98, G99)

In G code system A, the tool returns to the initial level from the

bottom of a hole. In G code system B or C, specifying G98 returns the

tool to the initial level from the bottom of a hole and specifying G99

returns the tool to the point R level from the bottom of a hole.

The following illustrates how the tool moves when G98 or G99 is

specified. Generally, G99 is used for the first drilling operation and

G98 is used for the last drilling operation.

The initial level does not change even when drilling is performed in

the G99 mode.

G98 (Return to initial level)

G99 (Return to point R level)

Initial level

Point R level

- Number of repeats

To repeat drilling for equally-spaced holes, specify the number of

repeats in K_.

K is effective only within the block where it is specified.

Specify the first hole position in incremental programming.

If it is specified in absolute programming, drilling is repeated at the

same position.

Number of repeats K

The maximum command value = 9999

When K0 is specified, drilling data is just stored without drilling being

performed.

NOTE

For K, specify an integer of 0 or 1 to 9999.

- 101 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64304EN-1/01

- M code used for C-axis clamp/unclamp

When an M code specified in parameter No.

5110 for C-axis

clamp/unclamp is coded in a program, the following operations occur.

•

The CNC issues the M code for C-axis clamp after the tool is

positioned and while the tool is being fed in rapid traverse to the

point-R level.

•

The CNC issues the M code for C-axis unclamp (the M code for

C-axis clamp +1) after the tool retracts to the point-R level.

•

After the CNC issues the M code for C-axis unclamp, the tool

dwells for the time specified in parameter No. 5111.

- Cancel

To cancel a canned cycle, use G80 or a group 01 G code.

Group 01 G codes (Example)

G00 : Positioning (rapid traverse)

G01 : Linear interpolation

G02 : Circular interpolation (CW)

G03 : Circular interpolation (CCW)

- Symbols in figures

Subsequent subsections explain the individual canned cycles. Figures

in these explanations use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

P1

Dwell specified in the program

P2

Dwell specified in parameter No.5111

Mα

Issuing the M code for C-axis clamp

(The value of α is specified with parameter No. 5110.)

M (α + 1)

Issuing the M code for C-axis unclamp

CAUTION

1 In each canned cycle, addresses R, Z, and X are

handled as follows:

R_

: Always handled as a radius.

Z_ or X_ : Depends on diameter/radius

programming.

2 For the B or C G-code system, G90 or G91 can be

used to select an incremental or absolute

programming for hole position data (X, C or Z, C),

the distance from point R to the bottom of the hole

(Z or X), and the distance from the initial level to

the point R level (R).

- 102 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

PROGRAMMING

4.3.1

Front Drilling Cycle (G83)/Side Drilling Cycle (G87)

The peck drilling cycle or high-speed peck drilling cycle is used

depending on the setting in RTR, bit 2 of parameter No. 5101. If depth

of cut for each drilling is not specified, the normal drilling cycle is

used.

- High-speed peck drilling cycle (G83, G87) (parameter RTR (No. 5101#2) =0)

This cycle performs high-speed peck drilling. The drill repeats the

cycle of drilling at the cutting feedrate and retracting the specified

retraction distance intermittently to the bottom of a hole. The drill

draws cutting chips out of the hole when it retracts.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

or

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data

Z_ or X_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of a hole

Q_

: Depth of cut for each cutting feed

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

M_

: M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Mα

Initial level

Mα

M (α + 1), P2

Point R

M (α + 1), P2

Point R

Point R level

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

P1

P1

Mα

: M code for C-axis clamp

M (α + 1) : M code for C-axis unclamp

P1

: Dwell specified in the program

P2

: Dwell specified in parameter No. 5111

d

: Retraction distance specified in parameter No. 5114

- 103 -

Content      ..     2      3      4      5     ..