Content      ..     9      10      11      12     ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 11

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

Start-up

Offset cancel

Cycle start point

z

Offset cancel

Start-up

Fig. 7.1.1 (q)

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

A

Position between

A-A' in which start-up

Target figure program for

is performed

which tool nose radius

compensation is not applied

+X

A’

Tool nose center path when tool nose radius

+Z

compensation is applied with G42

Fig. 7.1.1 (r) Path when tool nose radius compensation is applied

A

B

A’

Position between

A-A' in which

+X

start-up

is

Target figure program for

f

d

Tool nose center path when tool

which tool nose radius

+Z

nose radius compensation is

compensation is not applied

applied with G42

Fig. 7.1.1 (s)

NOTE

To perform pocketing in the tool nose radius compensation mode, specify the

linear block A-A' outside the workpiece and specify the figure of an actual

pocket. This prevents a pocket from being dug.

- 292 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

-

Reducing the cycle time

In G71.7 and G72.7, the tool can be moved to the previous turning start point (operation 1) in rapid

traverse by setting bit 0 (ASU) of parameter No. 5107 to 1.

Bit 0 (ASU) of parameter No. 5107 is valid for both type I and II commands.

For the type I command

Operation 1

Previous

turning point

Operation 2

Current

turning point

+X

: Rapid traverse can be selected.

+Z

: The mode specified in the start block is followed.

Fig. 7.1.1 (t)

For the type I G71.7 and G72.7 commands, operations 1 and 2 to the current turning start point that are

usually performed in 2 cycles can be performed in 1 cycle by setting bit 1 (ASC) of parameter No. 5107

to 1. The feed mode specified in the start block in the program for a target figure (G00 or G01) is used.

Bit 1 (ASC) of parameter No. 5107 is valid only for the type I command.

For the type II command

Operation 1

Previous

turning point

Operation 2

Current

turning point

+X

+Z

Fig. 7.1.1 (u)

- 293 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

7.1.2

Stock Removal in Facing (G72.7)

This cycle is the same as G71.7 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

G72.7 P(ns) Q(nf) U(Δu) W(Δw) I(Δi) K(Δk) D(Δd) 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

G72.7 P(ns) Q(nf) V(Δw) W(Δu) J(Δk) K(Δi) D(Δd) F(f ) S(s ) T(t );

N (ns) ;

- - -

N (nf) ;

XpYp plane

G72.7 P(ns) Q(nf) U(Δw) V(Δu) I(Δk) J(Δi) D(Δd) F(f ) S(s ) T(t );

N (ns) ;

- - -

N (nf) ;

Δd

: Depth of cut

The cutting direction depends on the direction AA’.

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.

Δu

: Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane)

Δw : Distance of the finishing allowance in the direction of the first axis on the plane

(Z-axis for the ZX plane)

Δi

: Distance of the finishing allowance for rough cutting in the direction of the second

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

Δk

: Distance of the finishing allowance for rough cutting 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 G72.7 block is effective.

Decimal

Unit

Diameter/radius programming

Sign

point input

Depends on the increment

Not

Δd

Radius programming

Not allowed

system for the reference axis.

required

Depends on the increment

Depends on diameter/radius programming

Δu

Required

Allowed

system for the reference axis.

for the second axis on the plane.

Depends on the increment

Depends on diameter/radius programming

Δw

Required

Allowed

system for the reference axis.

for the first axis on the plane.

Depends on the increment

Not

Δi

Radius programming

Allowed

system for the reference axis.

required

Depends on the increment

Not

Δk

Radius programming

Allowed

system for the reference axis.

required

- 294 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

Δd

(F): Cutting feed

(R): Rapid traverse

C

A'

A

Tool path

(F)

e

(R)

(R)

45°

Target figure

(F)

+X

Δu/2

B

+Z

Δw

e: Escaping amount (Parameter No.5133)

Fig. 7.1.2 (a) Cutting path (type I) of the stock removal in facing

without the finishing allowance for rough cutting

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 Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left.

NOTE

1 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G72.7 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions.

2 When an option of constant surface speed control is selected, G96 or G97

command specified in the move command between points A and B are

ineffective, and that specified in G72.7 block or the previous block is effective.

-

Escaping amount (e)

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

No.

Unit

Diameter/radius programming

Sign

Depends on the increment system for the

5133

Radius programming

Not required

reference axis.

-

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 Δu and Δw are as follows:

- 295 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

B B

+X

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. 7.1.2 (b) Signs of the values specified at U and W in stock removal in facing

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,

“G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued.

When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation

is performed with cutting feed along A-A’.

In this start block, also select type I or II.

-

Check functions

During cycle operation, whether the target figure shows monotone increase or decrease is always

checked.

NOTE

When tool nose radius compensation is applied, the target figure to which

compensation is applied is checked.

The following checks can also be made.

Check

Related parameter

Checks that a block with the sequence number specified at address Q is

Enabled when bit 2 (QSR) of

contained in the program before cycle operation.

parameter No. 5102 is set to 1.

Checks the target figure before cycle operation.

Enabled when bit 2 (FCK) of

(Also checks that a block with the sequence number specified at address Q

parameter No. 5104 is set to 1.

is contained.)

-

Types I and II

Selection of type I or II

For G71.7 and G72.7, 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.

- 296 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

7.1.3

Pattern Repeating (G73.7)

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

G73.7 P(ns) Q(nf) U(Δu) W(Δw) I(Δi) K(Δk) D(d) 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

G73.7 P(ns) Q(nf) V(Δw) W(Δu) J(Δk) K(Δi) D(d) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

XpYp plane

G73.7 P(ns) Q(nf) U(Δw) V(Δu) I(Δk) J(Δi) D(d) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

Δi

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

plane)

Δk

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

plane)

d

: The number of division

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

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.

Δu

: Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane)

Δw : 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 G73.7 block are effective.

Decimal

Unit

Diameter/radius programming

Sign

point input

Depends on the increment

Δi

Radius programming

Required

Allowed

system for the reference axis.

Depends on the increment

ΔK

Radius programming

Required

Allowed

system for the reference axis.

Depends on the increment

Depends on diameter/radius programming

Δu

Required

Allowed

system for the reference axis.

for the second axis on the plane.

Depends on the increment

Depends on diameter/radius programming

Δw

Required

Allowed

system for the reference axis.

for the first axis on the plane.

- 298 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

Δk+Δw

D

Δw

Δi+Δu/2

Δu/2

C

A

(R)

B

(R)

(F)

Δu/2

A'

Δw

+X

(F): Cutting feed

Target figure

(R): Rapid traverse

+Z

Fig. 7.1.3 (a) 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 Δu/2 and Δw 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 G73.7 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 G71.7, there are four target figure patterns. Be careful about signs of Δu, Δw, Δi, and Δk

when programming this cycle.

-

Start block

In the start block in the program for a target figure (block with sequence number ns in which the path

between A and A’ is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065,

“G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued.

When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation

is performed with cutting feed along A-A’.

-

Check functions

The following check can be made.

Check

Related parameter

Checks that a block with the sequence number specified at address Q is

Enabled when bit 2 (QSR) of

contained in the program before cycle operation.

parameter No. 5102 is set to 1.

- 299 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

7.1.4

Finishing Cycle (G70.7)

After rough cutting by G71.7, G72.7 or G73.7, the following command permits finishing.

Format

G70.7 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 G71.7, G72.7, or G73.7 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

G70.7 cycle block is read.

-

Target figure

Check function

Following check can be made.

Check

Related parameter

Checks that a block with the sequence number specified at address Q is

Enabled when bit 2 (QSR) of

contained in the program before cycle operation.

parameter No. 5102 is set to 1.

-

Storing P and Q blocks

When rough cutting is executed by G71.7, G72.7, or G73.7, 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 G70.7

without searching memory from the beginning for them. After some G71.7, G72.7, and G73.7 rough

cutting cycles are executed, finishing cycles can be performed by G70.7 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

G71.7 P100 Q200 - - - ;

N100 - - - ;

- - - ;

- - - ;

N200 - - - ;

G71.7 P300 Q400 - - - ;

N300 - - - ;

- - - ;

- - - ;

N400 - - - ;

- - - ;

- - - ;

G70.7 P100 Q200 ;

(Executed without a search for the first to third cycles)

G70.7 P300 Q400 ;

(Executed after a search for the fourth and subsequent

cycles)

- 301 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

Example

Stock removal in facing (G72.7)

X axis

2

Start point

7

Z axis

60

10

10

10

20

20

2

190

(Diameter designation for X axis, metric input)

N011

G90 G92 X220.0 Z190.0 ;

N012

G00 X176.0 Z132.0 ;

N013

G72.7 P014 Q019 U4.0 W2.0 D7000 F0.3 S550 ;

N014

G00 Z56.0 S700 ;

N015

G90 G01 X120.0 Z70.0 F0.15 ;

N016

Z80.0 ;

N017

X80.0 Z90.0 ;

N018

Z110.0 ;

N019

X36.0 Z132.0 ;

N020

G70.7 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)

- 303 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

Pattern repeating (G73.7)

16

B

X axis

Z axis

0

2

14

20

40

10

40

10

20

40

220

(Diameter designation, metric input)

N011

G90 G92 X260.0 Z220.0 ;

N012

G00 X220.0 Z160.0 ;

N013

G73.7 P014 Q019 U4.0 W2.0 I14.0 K14.0 D3 F0.3 S0180 ;

N014

G00 X80.0 Z120.0 ;

N015

G01 Z100.0 F0.15 S0600 ;

N016

X120.0 Z90.0;

N017

Z70.0 S0400 ;

N018

G02 X160.0 Z50.0 R20.0 ;

N019

G01 X180.0 Z40.0 S0280 ;

N020

G70.7 P014 Q019 ;

- 304 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

7.1.5

End Face Peck Drilling Cycle (G74.7)

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

G74.7X_ Z_ I(Δi) K(Δk) D(Δd) 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

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

Δi

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

plane)

Δk

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

Δd

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Unit

Diameter/radius programming

Sign

Decimal point input

Depends on the increment

Not

Δi

Radius programming

Allowed

system for the reference axis.

required

Depends on the increment

Not

Δk

Radius programming

Allowed

system for the reference axis.

required

Depends on the increment

Δd

Radius programming

Note

Not allowed

system for the reference axis.

NOTE

Normally, specify a positive value for Δd. When X and Δi are omitted, specify a

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

Δk'

Δk

Δk

Δk

Δk

[0<Δk’≤Δk]

Δd

A

Δi

C

(R)

(R)

(F)

(F)

(F)

(F)

(F)

Δx/2

(R)

(R)

(R)

(R)

Δi

[0<Δi’≤Δi]

Δi’

X

Z

B

Δz

+X

(R) ... Rapid traverse

e

(F) ... Cutting feed

+Z ｅ: Return amount (parameterNo.5139)

Fig. 7.1.5 (a) Cutting path in end face peck drilling cycle

- 305 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

Explanation

-

Operations

A cycle operation of cutting by Δk and return by e is repeated.

When cutting reaches point C, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to

the direction of point B by Δi, and performs cutting again.

-

Return amount (e)

Set a return amount in parameter No. 5139.

No.

Unit

Diameter/radius programming

Sign

Depends on the increment system for

5139

Radius programming

Not required

the reference axis.

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

7.1.6

Outer Diameter / Internal Diameter Drilling Cycle (G75.7)

This cycle is equivalent to G74.7 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 and

Q are omitted for the first axis on the plane).

Format

G75.7 X_ Z_ I(Δi) K(Δk) D(Δd) 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

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

Δi

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

plane)

Δk

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

plane)

Δd

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment system

Δi

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

Δk

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

Δd

Radius programming

Note

Not allowed

for the reference axis.

NOTE

Normally, specify a positive value for Δd. When Z and Δk are omitted, specify a

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

- 306 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

C

(R)

A

(R)

(F)

Δi

e

(R)

(F)

Δi

(R)

Δx/2

(F)

Δi

(R)

(F)

Δi

(R)

(F)

Δi’

B

Δd

Δk

X

Z

Δz

+X

(R) ... Rapid traverse

(F) ... Cutting feed

e: Return amount (parameter No.5139)

+Z

Fig. 7.1.6 (a) Outer diameter/internal diameter drilling cycle

Explanation

-

Operations

A cycle operation of cutting by Δi and return by e is repeated.

When cutting reaches point B, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to

the direction of point C by Δk, and performs cutting again.

Both G74.7 and G75.7 are used for grooving and drilling, and permit the tool to relief automatically. Four

symmetrical patterns are considered, respectively.

-

Return amount (e)

Set a return amount (e) in parameter No. 5139.

No.

Unit

Diameter/radius programming

Sign

Depends on the increment system for the

5139

Radius programming

Not required

reference axis.

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 307 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

7.1.7

Multiple Threading Cycle (G76.7)

This threading cycle allows selection of four cut methods.

Format

G76.7 X_ Z_ I(i) K(k) D(Δd) 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

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

a

: Angle of tool nose (thread angle) in degree units, the range being 0 to 120.

(If omitted, the angle is assumed 0 degrees.)

i

: Taper amount

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

k

: Height of thread

Δd

: Depth of cut in 1st cut

L

: Lead of thread

p

: Cut method (if omitted and if P0 is specified, the method is single-edged cutting with

a constant cutting amount.)

P1: Single-edged cutting with a constant cutting amount

P2: Both-edge zigzag thread cutting with a constant cutting amount

P3: Single-edged cutting with a constant depth of cut

P4: Both-edge zigzag thread cutting with a constant depth of cut

q

: Threading start angle shift

(0.001-degree units, range being 0 to 360 degrees)

NOTE

1 Address A is invalid even if a decimal point is added. That is, if 120 degrees is to

be specified, A120. is regarded as equivalent to A120.

2 Using cut methods P2 to P4 requires the multiple repetitive canned cycle II

option.

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment system

i

Radius programming

Required

Allowed

for the reference axis.

Depends on the increment system

ｋ

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

Δd

Radius programming

Not required

Not allowed

for the reference axis.

- 308 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

-

Relationship between the sign of the taper amount and tool path

The signs of incremental dimensions for the cycle shown in Fig. 7.1.7 (a) are as follows:

Cutting end point in the direction of the length for X and Z:

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 (Δd)

: Plus (always specified with a plus sign)

The four patterns shown in the Table 7.1.7 (a) are considered corresponding to the sign of each address. A

female thread can also be machined.

Table 7.1.7 (a)

Outer diameter machining

Internal diam eter m achining

1.

Δx < 0, Δz < 0, i < 0

2.

Δx > 0, Δz < 0, i > 0

X

X

Z

Z

Δz

4

(R)

2

(F)

i

Δx/2

3

(R)

1

(R)

X/2

Δx/2

3

(R)

1

(R)

i

X/2

2

(F)

4

(R)

Δz

3.

Δx < 0, Δz < 0, i > 0

4.

Δx > 0, Δz < 0, i < 0

at |i| ≤ |Δx / 2|

at |i| ≤ |Δx / 2|

X

X

Z

Z

Δz

4

(R)

i

1

(R)

2

(F)

X/2

Δx/2

3

(R)

Δx/2

3

(R)

2

(F)

1

(R)

i

4

(R)

Δz

X/2

-

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 parameters Nos. 1626 and 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.

-

Thread chamfering

Thread chamfering can be performed in this threading cycle. A signal from the machine tool initiates

thread chamfering.

Assuming that the lead is set to L with parameter No. 5130, the thread chamfering value may be set to

any value in the range of 0.1L to 12.7L, in 0.1L steps.

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.

- 311 -

7. MEMORY OPERATION

USING Series 15 FORMAT

PROGRAMMING

B-64484EN-2/02

-

Retraction after chamfering

The Table 7.1.7 (b) lists the feedrate, type of acceleration/deceleration after interpolation, and time

constant of retraction after chamfering.

Table 7.1.7 (b)

Bit 0 (CFR) of

Parameter No.

parameter No.

Description

1466

1611

0

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.

1

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

When the threading cycle retract function is not used, the machine stops at the end point of retraction

after chamfering (point E on the cutting path for a multiple threading cycle) by feed hold applied during

threading.

-

Feed hold when the threading cycle retract function is used

When the "threading cycle retract" option function is used, feed hold may be applied during threading in a

multiple 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.

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

X-axis

Ordinary cycle

Motion at feed hold

Z-axis

Start point

in the current cycle

Rapid traverse

Cutting feed

Feed hold is applied at this point

- 312 -

7.MEMORY OPERATION

B-64484EN-2/02

PROGRAMMING

USING Series 15 FORMAT

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 allowed.

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

Example

X axis

Z axis

0

6

25

105

G00 X80.0 Z130.0;

G76.7 X60.64 Z25.0 K3680 D1800 A60 P1 F6.0 ;

Parameter No.5130 = 10(1.0L)

7.1.8

Restrictions on Multiple Repetitive Cycle

Programmed commands

-

Program memory

Programs using G70.7, G71.7, G72.7, or G73.7 must be stored in the program memory. The use of the

mode in which programs stored in the program memory are called for operation enables these programs to

be executed in other than the MEM mode. Programs using G74.7, G75.7, or G76.7 need not be stored in

the program memory.

-

Blocks in which data related to a multiple repetitive cycle is specified

The addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

- 313 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

8 AXIS CONTROL FUNCTIONS

Chapter 8, "AXIS CONTROL FUNCTIONS", consists of the following sections:

8.1 CHOPPING FUNCTION

315

8.2 CHOPPING FUNCTION BY FLEXIBLE SYNCHRONOUS CONTROL

321

8.3 PARALLEL AXIS CONTROL

323

8.1

CHOPPING FUNCTION

Overview

When contour grinding is performed, the chopping function can be used to grind the side face of a

workpiece. By means of this function, while the grinding axis (the axis with the grinding wheel) is being

moved vertically, a contour program can be executed to initiate movement along other axes.

In addition, a servo delay compensation function is supported for chopping operations. When the grinding

axis is moved vertically at high speed, a servo delay and acceleration/deceleration delay occur. These

delays prevent the tool from actually reaching the specified position. The servo delay compensation

function compensates for any displacement by increasing the feedrate. Thus, grinding can be performed

almost up to the specified position.

There are two types of chopping functions: that specified by programming, and that activated by signal

input.

Format

G81.1 Z_ Q_ R_ F_ ;

Z :Upper dead point

(For an axis other than the Z-axis, specify the axis address.)

Q :Distance between the upper dead point and lower dead point

(Specify the distance as an incremental value, relative to the upper dead point.)

R :Distance from the upper dead point to point R

(Specify the distance as an incremental value, relative to the upper dead point.)

F :Feedrate during chopping

G80 ; Cancels chopping

NOTE

For the chopping axis, specify a linear axis. It is not possible to perform a

chopping operation on a rotation axis.

Explanation

-

Chopping activated by signal input

Before chopping can be started, the chopping axis, reference position, upper dead point, lower dead point,

and chopping feedrate must be set using the parameter screen (or the chopping screen).

Chopping is started once chopping start signal CHPST has been set to 1. This signal is ignored, however,

during chopping axis movement.

When chopping hold signal *CHLD is set to 0 during chopping, the tool immediately moves to point R.

Again setting the chopping hold signal to 1 restarts chopping.

Chopping can also be stopped by setting chopping start signal CHPST to 0, but only when chopping was

started by using that signal.

- 315 -

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

Method of starting chopping

Method of stopping chopping

State

Signal CHPST = 0

Stopped

Signal CHPST = 1

G80

Stopped

Signal CHPST = 0

Not stopped

G81.1

G80

Stopped

NOTE

1 Switching to manual mode or suspending automatic operation, by means of feed

hold, does not stop chopping.

2 In chopping mode, a chopping axis move command or canned cycle command

cannot be specified.

3 If a G81.1 command is specified during chopping started by the signal, chopping

is not stopped. If point R, the upper dead point, lower dead point, or chopping

feedrate has been modified by using the G81.1 command, chopping is

continued, using the modified data.

4 The use of chopping start signal CHPST to start chopping is not enabled

immediately after power-on; it is not enabled until the completion of manual

reference position return.

5 For the chopping axis, specify a linear axis. It is not possible to perform a

chopping operation on a rotation axis.

-

Chopping feedrate (feedrate of movement to point R)

From the start of chopping to point R, the tool moves at the rapid traverse rate (specified by parameter No.

1420).

The override function can use either the normal rapid traverse override or chopping feedrate override, one

of which can be selected by setting ROV (bit 0 of parameter No. 8360).

When the chopping feedrate override is selected, settings between 110% and 150% are clamped to 100%.

-

Chopping feedrate (feedrate of movement from point R)

Between point R, reached after the start of chopping, and the point where the chopping is canceled, the

tool moves at the chopping feedrate (specified by parameter No. 8374).

The chopping feedrate is clamped to the maximum chopping feedrate (set with parameter No. 8375) if the

specified feedrate is greater than the maximum chopping feedrate.

The feedrate can be overridden by 0% to 150% by applying the chopping feedrate override signal.

-

Setting chopping data

Set the following chopping data:

• Chopping axis: Parameter No. 8370

• Reference point (point R): Parameter No. 8371

• Upper dead point: Parameter No. 8372

• Lower dead point: Parameter No. 8373

• Chopping feedrate: Parameter No. 8374

• Maximum chopping feedrate: Parameter No. 8375

All data items other than the chopping axis and maximum chopping feedrate can be set on the chopping

screen.

NOTE

Chopping data can be changed using the program command, the parameter

screen, and the chopping screen. If, during a chopping operation, the upper

dead point, lower dead point, or feedrate for chopping is specified or set, servo

delay compensation temporarily stops even if the same value is used. Also, the

upper dead point or lower dead point may be exceeded.

- 316 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

-

Chopping after the upper dead point or lower dead point has been changed

When the upper dead point or lower dead point is changed while chopping is being performed, the tool

moves to the position specified by the old data. Then, chopping is continued using the new data.

When movement according to the new data starts, the servo delay compensation function stops the servo

delay compensation for the old data, and starts the servo delay compensation for the new data.

The following describes the operations performed after the data has been changed.

(1) When the upper dead point is changed during movement from the upper dead point to the lower

dead point

New upper dead point

Previous upper dead point

Previous lower dead point

The tool first moves to the lower dead point, then to the new upper dead point.

Once movement to the lower dead point has been completed, the previous servo delay compensation

is set to 0, and servo delay compensation is performed based on the new data.

(2) When the lower dead point is changed during movement from the upper dead point to the lower

dead point

Previous upper dead point

New lower dead point

Previous lower dead point

The tool first moves to the previous lower dead point, then to the upper dead point, and finally to the

new lower dead point.

Once movement to the upper dead point has been completed, the previous servo delay compensation

is set to 0, and servo delay compensation is performed based on the new data.

(3) When the upper dead point is changed during movement from the lower dead point to the upper

dead point

New upper dead point

Previous upper dead point

Previous lower dead point

The tool first moves to the previous upper dead point, then to the lower dead point, and finally to the

new upper dead point.

- 317 -

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

Once movement to the lower dead point has been completed, the previous servo delay compensation

is set to 0, and servo delay compensation is performed based on the new data.

(4) When the lower dead point is changed during movement from the lower dead point to the upper

dead point

Previous upper dead point

Previous lower dead point

New lower dead point

The tool first moves to the upper dead point, then to the new lower dead point.

Once movement to the upper dead point has been completed, the previous servo delay compensation

is set to 0, and servo delay compensation is performed based on the new data.

-

Servo delay compensation function

When high-speed chopping is performed with the grinding axis, a servo delay and

acceleration/deceleration delay occur. These delays prevent the tool from actually reaching the specified

position. The control unit measures the difference between the specified position and the actual tool

position, and automatically compensates for the displacement of the tool.

To compensate for this displacement, an amount of travel equal to the distance between the upper and

lower dead points, plus an appropriate compensation amount, is specified. When a chopping command is

specified, the feedrate is determined so that the chopping count per unit time equals the specified count.

When the difference between the displacement of the tool from the upper dead point and the displacement

of the tool from the lower dead point becomes smaller than the setting of parameter No. 8377, after the

start of chopping, the control unit performs compensation.

When compensation is applied, the chopping axis moves beyond the specified upper dead point and lower

dead point, and the chopping feedrate increases gradually.

When the difference between the actual machine position and the specified position becomes smaller than

in-position width (parameter No. 1826), the control unit stops further compensation, and the tool continue

moving at its current feedrate.

A coefficient for the compensation amount for the displacement which has generated by the servo delay

and the acceleration /deceleration delay during chopping can be specified in parameter No. 8376.

-

If servo delay compensation can cause the chopping speed to exceed the

maximum allowable chopping feedrate:

Servo delay compensation during a chopping operation can gradually increase the chopping speed. If the

chopping speed is about to exceed the maximum allowable chopping feedrate, it is clamped to the

maximum allowable chopping feedrate. In servo delay compensation, the distance specified in a

movement command is increased by a compensation amount that matches the distance yet to go before

the top and bottom dead points are reached, and the chopping speed is also increased, so that the distance

yet to go can be compensated for.

If the chopping speed is clamped to the maximum allowable chopping feedrate, the increase in the

distance specified in the movement command stops as soon as the speed is clamped.

- 318 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

Point R

Upper dead point

L2

L4

L6

L1

L3

L5

Lower dead point

Time

Displacement between the tool and the upper dead point: L2, L4, L6

Displacement between the tool and the lower dead point: L1, L3, L5

Compensation starts when:

| L3 - L2 | < (parameter No. 8377)

When the following condition is satisfied, compensation is no longer applied, and the tool

continues to move at its current feedrate:

| L6 | < in-position width (parameter No. 1826)

-

Acceleration

For the acceleration/declaration along the chopping axis, acceleration/deceleration after cutting feed

interpolation is effective.

-

Mode switching during chopping

If the mode is changed during chopping, chopping does not stop. In manual mode, the chopping axis

cannot be moved manually. It can, however, be moved manually by means of the handle interrupt.

-

Reset during chopping

When a reset is performed during chopping, the tool immediately moves to point R, after which chopping

mode is canceled.

If an emergency stop or servo alarm occurs during chopping, chopping is canceled, and the tool stops

immediately.

-

Stopping chopping

The Table 8.1 (a) lists the operations and commands that can be used to stop chopping, the positions at

which chopping stops, and the operation performed after chopping stops:

Table 8.1 (a)

Operation/

Stop position

Operation after chopping stops

command

G80

Point R

Canceled

CHPST : “0”

The tool moves to the lower dead point, then to point R

Canceled

*CHLD : “0”

Point R

Restart after *CHLD goes "1"

Reset

Point R

Canceled

Emergency stop

The tool stops immediately

Canceled

- 319 -

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

Operation/

Stop position

Operation after chopping stops

command

Servo alarm

The tool stops immediately

Canceled

PS alarm

The tool moves to the lower dead point, then to point R

Canceled

OT alarm

The tool moves from the upper or lower point to point R

Canceled

-

Background editing

When an alarm of background editing or battery alarm is issued, the tool does not stop at point R.

-

Single block signal

Even when single block signal SBK is input during chopping, chopping continues.

Limitation

- Workpiece coordinate system

While chopping is being performed, do not change the workpiece coordinate system for the chopping

axis.

- PMC axis

When the chopping axis is selected as the PMC axis, chopping is not started.

- Mirror image

While chopping is being performed, never attempt to apply the mirror image function about the chopping

axis.

- Move command during chopping

If a move command is specified for the chopping axis while chopping is being performed, an alarm

PS5050, “ILL-COMMAND IN G81.1 MODE” is issued.

- Program restart

When a program contains G codes for starting chopping (G81.1) and stopping chopping (G80), an

attempt to restart that program results in an alarm PS5050, “ILL-COMMAND IN G81.1 MODE” being

output.

When a program that does not include the chopping axis is restarted during chopping, the coordinates and

amount of travel set for the chopping axis are not affected after the restart of the program.

- Canned Cycle

While chopping is being performed, do not be specified canned cycle.

- Inch/Metric conversion commands

While chopping is being performed, do not be specified inch/metric conversion commands.

- General purpose retract

While chopping is being performed, do not be performed retraction. The chopping motion does not stop

by retraction.

- Stored stroke check

Stored stroke check 1-I (parameter Nos. 1320 and 1321) is only effective during chopping motion.

- Arbitrary angular axis control

Do not set angular axis and perpendicular axis of arbitrary angular axis control to chopping axis.

- 320 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

- Three-dimensional coordinate conversion / Tilted working plane command

While chopping is being performed, do not be specified three-dimensional coordinate conversion / tilted

working plane command.

- Cs contour control axis

Do not set Cs contour control axis to chopping axis.

- Composite control

Do not set composite control axis to chopping axis.

- Polygon turning

Do not set control axis for polygon turning to chopping axis.

Example

Example)

G90 G81.1 Z100. Q-25. R10. F3000 ;

•

Perform rapid traverse to position the tool to Z110. (point R).

•

Then, perform reciprocating movement along the Z-axis between Z100. (upper dead point) and

Z75. (lower dead point) at 3000 mm/min. Chopping override is enabled.

Point R

(Z110. )

Upper dead point

(Z100. )

Lower dead point

(Z75. )

Time

To cancel chopping, specify the following command:

G80 ;

•

The tool stops at point R.

8.2

CHOPPING FUNCTION BY FLEXIBLE SYNCHRONOUS

CONTROL

Overview

This function enables the chopping of simultaneous 2-axis control by using a flexible synchronous

control with the chopping.

It is possible to synchronize an axis with a chopping axis. This function is suitable for the taper hole

processing by a grinder etc.

- 321 -

Content      ..     9      10      11      12     ..