Content      ..     3      4      5      6     ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 5

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.7.1

Plunge Grinding Cycle (G75)

A plunge grinding cycle can be executed.

Format

G75 I_ J_ K_ α_ R_ F_ P_ L_ ;

I_

: First depth of cut (The cutting direction depends on the sign.)

J_

: Second depth of cut (The cutting direction depends on the sign.)

K_ : Total depth of cut (The cutting direction depends on the sign.)

α_

: Grinding range (The grinding direction depends on the sign.)

R_ : Feedrate for I and J

F_

: Feedrate for α

P_ : Dwell time

L_

: Grinding-wheel wear compensation number (during continuous dressing only)

G75

Y

α

I

<1> (R)

<3> (F)

<2> P

<4> (R)

J

<6> (F)

<5> P

α

NOTE

α is an arbitrary axis address on the grinding axis as determined with parameter

No. 5176.

Explanation

A plunge grinding cycle consists of a sequence of six operations.

Operations <1> to <6> are repeated until the depth of cut reaches the total depth of cut specified with

address K. For a single block, operations <1> to <6> are executed with a single cycle start.

-

Operation sequence in a cycle

<1> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount specified as the first depth of cut

I. The feedrate is the one specified with R.

<2> Dwell

Performs a dwell for the time specified with P.

<3> Grinding

Causes the machine to move with cutting feed by the amount specified with α. The grinding axis is

specified with parameter No. 5176. The feedrate is the one specified with F. If L is specified when

the continuous dressing function is enabled, dressing is performed with the cutting axis and the

dressing axis. The dressing axis is specified with parameter No. 5180.

- 112 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

<4> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount specified as the second depth of

cut J. The feedrate is the one specified with R.

<5> Dwell

Performs a dwell for the time specified with P.

<6> Grinding (return direction)

Feeds the machine at the feedrate specified with F in the opposite direction by the amount specified

with α. If L is specified when the continuous dressing function is enabled, dressing is performed

with the cutting axis and the dressing axis.

-

Continuous dressing

If the continuous dressing function is enabled, the grinding-wheel cut and the dresser cut are continuously

compensated for according to the dressing amount specified with L during the execution of grinding.

That is, continuous dressing is performed in each grinding operation in the sequence of operations in the

cycle, resulting in simultaneous 3-axis interpolation with compensation in the cutting axis direction and

compensation in the dressing axis direction simultaneous with movement along the grinding axis. At this

time, the travel distance (compensation) along the cutting axis is equal to the specified dressing amount,

and the travel distance along the dressing axis is equal to double the specified dressing amount (diameter).

For the dressing amount, specify an offset number (grinding-wheel wear compensation number) with

address L. Up to 400 offset numbers (L1 to L400) can be specified. Establish correspondence between

compensation amounts and offset numbers, and set it in offset memory in advance, using the MDI panel.

No compensation operation is performed in the following cases:

The continuous dressing function is disabled.

L is not specified.

L0 is specified.

Dresser

a: Amount of dressing

Dressing axis

Cutting axis

2a

Grinding wheel

a

Grinding axis

Workpiece

α

Limitations

-

Cutting axis

The cutting axis is the second controlled axis. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis

can be switched with a plane selection command (G17, G18, or G19).

-

Grinding axis

To specify a grinding axis, set its axis number, which must be other than that of the cutting axis, in

parameter No. 5176.

-

Dressing axis

To specify a dressing axis, set its axis number, which must be other than those of the cutting axis and the

grinding axis, in parameter No. 5180.

-

α,I,J,K

α, I, J, and K commands are all incremental ones.

- 113 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Spark-out (execution of movement in the grinding direction only) occurs in the following cases:

• I or J is not specified or I = J = 0

• K is not specified or K = 0

If I or J is not specified or if I = J = 0 is true, and K is not equal to 0, a grinding operation is performed

infinitely.

-

Clearing

The data items I, J, K, α, R, F, and P in a canned cycle are modal information common to G75, G77, G78,

and G79, so that once specified, they remain effective until specified anew. The data is cleared when a G

code of group 00 other than G04 or a G code of group 01 other than G75, G77, G78, and G79 is specified.

L is effective only in the block in which it is specified.

-

Operation to be performed if the total depth of cut is reached

If, during cutting with I or J, the total depth of cut is reached, the cycle is ended after the subsequent

operations in the sequence (up to <6>) are executed.

If this occurs, the depth of cut is equal to or less than the total depth of cut.

• If the total depth of cut is reached due to a cutting operation with I or J

<1>

I

K

<3>

<2>

<4>

J

<6>

<5>

K

I

<1>

<2>

<3>

<5>

<6>

• If the total depth of cut is reached during a cutting operation with I or J

<1>

I

K

<3>

<2>

<4>

J

<5>

<6>

K

<1>

<3>

I

<2>

<5>

<6>

NOTE

1 If I, J, and K have different signs, alarm PS0455 is issued.

2 If G75 is specified, but a grinding axis is not specified, alarm PS0455 is issued.

3 If any two of the cutting axis number, the grinding axis number, and the dressing

axis number are the same, alarm PS0456 is issued.

4 While this cycle is effective, even if G90 (absolute command) is executed, the α,

I, J, and K commands are incremental ones.

- 114 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.7.2

Direct Constant-Dimension Plunge Grinding Cycle (G77)

A direct constant-dimension plunge grinding cycle can be performed.

Format

G77 I_ J_ K_ α_ R_ F_ P_ L_ ;

I_ : First depth of cut (The cutting direction depends on the sign.)

J_ : Second depth of cut (The cutting direction depends on the sign.)

K_ : Total depth of cut (The cutting direction depends on the sign.)

α_ : Grinding range (The grinding direction depends on the sign.)

R_: Feedrate for I and J

F_ : Feedrate for α

P_ : Dwell time

L_ : Grinding-wheel wear compensation number (during continuous dressing only)

G77

Y

α

I

<1> (R)

<3> (F)

<2> P

<4> (R)

J

<6> (F)

<5> P

α

NOTE

α is an arbitrary axis address on the grinding axis as determined with parameter

No. 5177.

Explanation

A direct constant-dimension plunge grinding cycle consists of a sequence of six operations.

Operations <1> to <6> are repeated until the depth of cut reaches the total depth of cut specified with

address K. For a single block, operations <1> to <6> are executed with a single cycle start.

-

Operation sequence in a cycle

<1> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount specified as the first depth of cut

I. The feedrate is the one specified with R.

<2> Dwell

Performs a dwell for the time specified with P.

<3> Grinding

Causes the machine to move with cutting feed by the amount specified with α. The grinding axis is

specified with parameter No. 5177. The feedrate is the one specified with F. If L is specified when

the continuous dressing function is enabled, dressing is performed with the cutting axis and the

dressing axis. The dressing axis is specified with parameter No. 5181.

<4> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount specified as the second depth of

cut J. The feedrate is the one specified with R.

- 115 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

<5> Dwell

Performs a dwell for the time specified with P.

<6> Grinding (return direction)

Feeds the machine at the feedrate specified with F in the opposite direction by the amount specified

with α. If L is specified when the continuous dressing function is enabled, dressing is performed

with the cutting axis and the dressing axis.

-

Continuous dressing

If the continuous dressing function is enabled, the grinding-wheel cut and the dresser cut are continuously

compensated for according to the dressing amount specified with L during the execution of grinding. For

details, see Explanation of G75.

-

Operation to be performed when a skip signal is input

With G77, by inputting a skip signal in a cycle, it is possible to end the cycle after interrupting the current

operation sequence (or after ending the current operation sequence).

The following shows the operation to be performed when a skip signal is input in each operation

sequence.

• If operation <1> or <4> in the sequence (movement with I or J) is in progress, the machine

immediately stops cutting and returns to the α coordinate, assumed at the start of the cycle.

Skip signal

Skip signal

(End)

(End)

• If operation <2> or <5> in the sequence (dwell) is in progress, the machine immediately cancels the

dwell and returns to the α coordinates, assumed at the start of the cycle.

• If operation <3> or <6> in the sequence (grinding movement) is in progress, the machine returns to

the α coordinate, assumed at the start of the cycle after the end of the α movement.

Skip signal

(End)

Skip signal

(End)

Limitations

-

Cutting axis

The cutting axis is the second controlled axis. By setting bit 0 (FXY) of parameter No. 5101 to 1, the axis

can be switched with a plane selection command (G17, G18, or G19).

- 116 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.7.3

Continuous-feed Surface Grinding Cycle (G78)

A continuous-feed surface grinding cycle can be performed.

Format

G78

Z

α

<1> P

<2> (F)

I

I(J)

<3> P

<4> (F)

α

NOTE

α is an arbitrary axis address on the grinding axis as determined with parameter

No. 5178.

Explanation

A continuous-feed surface grinding cycle consists of a sequence of four operations.

Operations <1> to <4> are repeated until the depth of cut reaches the total depth of cut specified with

address K. For a single block, operations <1> to <4> are executed with a single cycle start.

-

Operation sequence in a cycle

<1> Dwell

Performs a dwell for the time specified with P.

<2> Cutting with a grinding wheel＋Grinding

Performs cutting feed along the cutting axis (Z-axis) and the grinding axis at the same time. The

travel distance (depth of cut) along the cutting axis is equal to the amount specified as the first depth

of cut I, and the travel distance along the grinding axis is equal to the amount specified with α. The

grinding axis is specified with parameter No. 5178. The feedrate is the one specified with F. If L is

specified when the continuous dressing function is enabled, dressing is performed with the cutting

axis and the dressing axis. The dressing axis is specified with parameter No. 5182.

<3> Dwell

Performs a dwell for the time specified with P.

<4> Cutting with a grinding wheel＋Grinding (return direction)

Performs cutting feed along the cutting axis (Z-axis) and the grinding axis at the same time. The

travel distance (depth of cut) along the cutting axis is equal to the amount specified as the first depth

of cut I, and the travel distance along the grinding axis is equal to the amount specified with α, with

the direction being the opposite one.The feedrate is the one specified with F. If L is specified when

the continuous dressing function is enabled, dressing is performed with the cutting axis and the

dressing axis.

- 118 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

• If the total depth of cut is reached due to a cutting operation with I or J

K

<1>

<2>

I

<3>

J

<4>

K

<1>

<2>

I

<3>

J

<4>

• If the total depth of cut is reached during a cutting operation with I or J

K

<1>

<2>

I

<3>

J

<4>

K

<1>

<2>

I

<4>

<3>

NOTE

1 If I, J, and K have different signs, alarm PS0455 is issued.

2 If G78 is specified, but a grinding axis is not specified, alarm PS0455 is issued.

3 If any two of the cutting axis number, the grinding axis number, and the dressing

axis number are the same, alarm PS0456 is issued.

4 While this cycle is effective, even if G90 (absolute command) is executed, the α,

I, J, and K commands are incremental ones.

- 120 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.7.4

Intermittent-feed Surface Grinding Cycle (G79)

An intermittent-feed surface grinding cycle can be performed.

Format

G79 I_ J_ K_ α_ R_ F_ P_ L_ ;

I_

: First depth of cut (The cutting direction depends on the sign.)

J_

: Second depth of cut (The cutting direction depends on the sign.)

K_ : Total depth of cut (The cutting direction depends on the sign.)

α_

: Grinding range (The grinding direction depends on the sign.)

R_ : Feedrate for I and J

F_

: Feedrate for α

P_ : Dwell time

L_

: Grinding-wheel wear compensation number (during continuous dressing only)

G79

Z

α

I

<1> (R)

<3> (F)

<2> P

<4> (R)

J

<6> (F)

<5> P

α

NOTE

α is an arbitrary axis address on the grinding axis as determined with parameter

No. 5179.

Explanation

An intermittent-feed surface grinding cycle consists of a sequence of six operations.

Operations <1> to <6> are repeated until the depth of cut reaches the total depth of cut specified with

address K. For a single block, operations <1> to <6> are executed with a single cycle start.

-

Operation sequence in a cycle

<1> Cutting with a grinding wheel

Makes a cut in the Z-axis direction with cutting feed by the amount specified as the first depth of cut

I. The feedrate is the one specified with R.

<2> Dwell

Performs a dwell for the time specified with P.

<3> Grinding

Causes the machine to move with cutting feed by the amount specified with α. The grinding axis is

specified with parameter No. 5179. The feedrate is the one specified with F. If L is specified when

the continuous dressing function is enabled, dressing is performed with the cutting axis and the

dressing axis. The dressing axis is specified with parameter No. 5183.

- 121 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.8

MULTIPLE REPETITIVE CYCLE (G70.7, G71.7, G72.7,

G73.7, G74.7, G75.7,G76.7)

The multiple repetitive cycle is canned cycles to make CNC programming easy. For instance, the data of

the finish work shape describes the tool path for rough machining. And also, a canned cycles for the

threading is available.

NOTE

1 Explanatory figures in this section use the ZX plane as the selected plane,

diameter programming for the X-axis, and radius programming for the Z-axis.

When radius programming is used for the X-axis, change U/2 to U and X/2 to X.

2 A multiple repetitive cycle can be performed on any plane.

- 124 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.8.1

Stock Removal in Turning (G71.7)

There are two types of stock removal in turning : Type I and II.

To use type II, the "multiple repetitive canned cycle 2" optional function is required.

Format

ZpXp plane

G71.7 U(Δd) R(e) ;

G71.7 P(ns) Q(nf) U(Δu) W(Δw) 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

G71.7 W(Δd) R(e) ;

G71.7 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

XpYp plane

G71.7 V(Δd) R(e) ;

G71.7 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

Δd

: 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.

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, or T function contained in blocks ns to nf in the cycle is ignored, and the F,

S, or T function in this G71.7 block is effective.

Decimal

Unit

Diameter/radius programming

Sign

point input

Depends on the increment

Not

Δd

Radius programming

Allowed

system for the reference axis.

required

- 125 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Decimal

Unit

Diameter/radius programming

Sign

point input

Depends on the increment

Not

e

Radius programming

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.

(R)

C

B

A

Δd

(R)

(F)

45°

e

(F)

Target figure

Δu/2

+X

A’

(F): Cutting feed

ΔW

+Z

(R): Rapid traverse

e: Escaping amount

Fig. 5.8.1 (a) Cutting path in stock removal in turning (type I)

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. After the last

cutting is performed in the direction of the second axis on the plane (X-axis for the ZX plane), rough

cutting is performed as finishing along the target figure. After rough cutting as finishing, the block next to

the sequence block specified at Q is executed.

NOTE

1 While both Δd and Δu 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 G71.7 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 G71.7 block or the previous block

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

S, and T functions.

4 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 G71.7 block or the previous block is effective.

- 126 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Target figure

Patterns

The four cutting patterns in the Fig. 5.8.1 (b) are considered. All of these cutting cycles cut the workpiece

with moving the tool in parallel to the first axis on the plane (Z-axis for the ZX plane). At this time, the

signs of the finishing allowances of Δu and Δw are as follows:

B

A

A

B

U(+)…W(+)

U(+)…W(-)

A' A'

Both linear and

circular interpolation

A'

A'

are possible

U(-)…W(+)

U(-)…W(-)

B

A

A

B

+X

+Z

Fig. 5.8.1 (b) Four target figure patterns

Limitation

(1) For U(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For U(-), 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 first 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 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 is

parameter No. 5104 is set to 1.

contained.)

- 127 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Types I and II

Selection of type I or II

For G71.7, 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 first axis on the plane (Z-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.

NOTE

To use type II, the multiple repetitive canned cycle II option is required.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II.

(1) When type I is selected

Specify the second axis on the plane (X-axis for the ZX plane). Do not specify the first axis on the

plane (Z-axis for the ZX plane).

(2) When type II is selected

Specify the second axis on the plane (X-axis for the ZX plane) and first axis on the plane (Z-axis for

the ZX plane).

When you want to use type II because of no movement of the tool along the first axis on the plane

(Z-axis for the ZX plane), specify the function with a travel distance of 0.

-

Type I

(1) In the block with sequence number ns, only the second axis on the plane

(X-axis for the ZX plane) must be specified.

Example

ZX plane

G71.7 U10.0 R5.0 ;

G71.7 P100 Q200

;

N100 X_ ; (Specifies only the second axis on the plane.)

： ;

： ;

N200

;

(2) The figure along path A’-B must show monotone increase or decrease in the directions of both axes

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig.

5.8.1 (c).

B

A

A’

X

Z

No pockets are allowed.

Fig. 5.8.1 (c) Figure which does not show monotone increase or decrease (type I)

- 128 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

CAUTION

If a figure does not show monotone change along the first or second axis on the

plane, alarm PS0064 or PS0329 is issued. If the movement does not show

monotone change, but is very small, and it can be determined that the

movement is not dangerous, however, the permissible amount can be specified

in parameters Nos. 5145 and 5146 to specify that the alarm is not issued in this

case.

(3) The tool escapes to the direction of 45 degrees in cutting feed after rough cutting.

Escaping amount e (specified in the

45°

command or parameter No. 5133)

Fig. 5.8.1 (d) Cutting in the direction of 45 degrees (type I)

(4) Immediately after the last cutting, rough cutting is performed as finishing along the target figure. Bit

1 (RF1) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

-

Type II

(R)

(F)

C

(R)

B

A

Δd

(R)

(F)

Δd

(F)

Target figure

Δu/2

A’

+X

(F): Cutting feed

ΔW

+Z

(R): Rapid traverse

Fig. 5.8.1 (e) Cutting path in stock removal in turning (type II)

When a target figure passing through A, A', and B in this order is given by the program for a target figure

as shown in the Fig. 5.8.1 (e), the specified area is removed by Δd (depth of cut), with the finishing

allowance specified by Δu/2 and Δw left.

Type II differs from type I in cutting the workpiece along the figure after rough cutting in the direction of

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

After the last cutting, the tool returns to the start point specified in G71.7 and rough cutting is performed

as finishing along the target figure, with the finishing allowance specified by Δu/2 and Δw left.

Type II differs from type I in the following points:

(1) In the block with sequence number ns, the two axes forming the plane (X-axis and Z-axis for the ZX

plane) must be specified. When you want to use type II because of no movement of the tool along

the Z-axis on the ZX plane in the first block, specify the function with a travel distance of 0.

- 129 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Example

ZX plane

G71.7 U10.0 R5.0;

G71.7 P100 Q200

;

N100 X_ Z_ ;

(Specifies the two axes forming the plane.)

: ;

: ;

N200

;

(2) The figure need not show monotone increase or decrease in the direction of the second axis on the

plane (X-axis for the ZX plane) and it may have concaves (pockets).

+X

+Z

10

・・・

3

2

1

Fig. 5.8.1 (f) Figure having pockets (type II)

The figure must show monotone change in the direction of the first axis on the plane (Z-axis for the

ZX plane), however. The Fig. 5.8.1 (g) cannot be machined.

Monotone change is not

observed along the Z-axis.

+X

+Z

Fig. 5.8.1 (g) Figure which cannot be machined (type II)

CAUTION

For a figure along which the tool moves backward along the first axis on the

plane during cutting operation (including a vertex in an arc command), the

cutting tool may contact the workpiece. For this reason, for a figure which does

not show monotone change, alarm PS0064 or PS0329 is issued. If the

movement does not show monotone change, but is very small, and it can be

determined that the movement is not dangerous, however, the permissible

amount can be specified in parameter No. 5145 to specify that the alarm is not

issued in this case.

The first cut portion need not be vertical. Any figure is permitted if monotone change is shown in

the direction of the first axis on the plane (Z-axis for the ZX plane).

+X

+Z

Fig. 5.8.1 (h) Figure which can be machined (type II)

- 130 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

(3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

Escaping amount e (specified in the command or parameter No. 5133)

Escaping after cutting

Depth of cut Δd

(specified in the

command or parameter No. 5132)

Fig. 5.8.1 (i) Cutting along the workpiece figure (type II)

The escaping amount after cutting (e) can be specified at address R or set in parameter No. 5133.

When moving from the bottom, however, the tool escapes to the direction of 45 degrees.

e (specified in the command or

45°

parameter No. 5133)

Bottom

Fig. 5.8.1 (j) Escaping from the bottom to the direction of 45 degrees

(4) When a position parallel to the first axis on the plane (Z-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket.

(5) After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool

temporarily returns to the cycle start point. At this time, when there is a position whose height equals

to that at the start point, the tool passes through the point in the position obtained by adding depth of

cut Δd to the position of the figure and returns to the start point.

Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes

through the point in the obtained position (to which depth of cut Δd is added) when returning to the

start point.

Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

Escaping operation after rough cutting as finishing

Escaping operation after rough cutting

Start point

{

{

Depth of cut Δd

Fig. 5.8.1 (k) Escaping operation when the tool returns to the start point (type II)

- 131 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

(6)

Order and path for rough cutting of pockets

Rough cutting is performed in the following order.

(a)

When the figure shows monotone decrease along the first axis on the plane (Z-axis for the ZX

plane)

Rough cutting is performed in the order <1>, <2>, and <3>

from the rightmost pocket.

<3>

<2>

<1>

+X

+Z

Fig. 5.8.1 (l) Rough cutting order in the case of monotone decrease (type II)

(b)

When the figure shows monotone increase along the first axis on the plane (Z-axis for the ZX

plane)

Rough cutting is performed in the order <1>, <2>, and <3>

from the leftmost pocket.

<1>

<2>

<3>

+X

+Z

Fig. 5.8.1 (m) Rough cutting order in the case of monotone increase (type II)

The path in rough cutting is as shown Fig. 5.8.1 (n).

35

4

3

1

5

34

24

9

10

25

2

23

29

22

21

11

6

28

30

8

26

15

27

7

33

31

12

14

20

16

32

13

19

18

17

Fig. 5.8.1 (n) Cutting path for multiple pockets (type II)

The Fig. 5.8.1 (o) shows how the tool moves after rough cutting for a pocket in detail.

g

Rapid traverse

21

22

•

D

20

Escaping from

the bottom

19

Cutting feed

Fig. 5.8.1 (o) Details of motion after cutting for a pocket (type II)

- 132 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Start-up

Offset cancel

Cycle start point

z

Offset cancel

Start-up

Fig. 5.8.1 (p)

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. 5.8.1 (q) Path when tool nose radius compensation is applied

A

B

A’

Position between

+X

A-A' in which start-up

is performed

Target figure program for

Tool nose center path when tool

which tool nose radius

+Z

nose radius compensation is

compensation is not applied

applied with G42

Fig. 5.8.1 (r)

- 134 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

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.

-

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. 5.8.1 (s)

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. 5.8.1 (t)

- 135 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.8.2

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 W(Δd) R(e) ;

G72.7 P(ns) Q(nf) U(Δu) W(Δw) 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 V(Δd) R(e) ;

G72.7 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

XpYp plane

G72.7 U(Δd) R(e) ;

G72.7 P(ns) Q(nf) U(Δw) W(Δu) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

Δd

: 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.

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, 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

Allowed

system for the reference axis.

required

Depends on the increment

Not

e

Radius programming

Allowed

system for the reference axis.

required

- 136 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Decimal

Unit

Diameter/radius programming

Sign

point input

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.

Δd

(F): Cutting feed

(R): Rapid traverse

C

A'

A

Tool path

(F)

(R)

e

(R)

45°

Target figure

(F)

+X

Δu/2

B

+Z

Δw

Fig. 5.8.2 (a) Cutting path in stock removal in facing (type I)

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 While both Δd and Δu 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 G72.7 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 G72.7 block or the previous block

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

S, and T functions.

4 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.

-

Target figure

Patterns

The four cutting patterns in the Fig. 5.8.2 (b) 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:

- 137 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

+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. 5.8.2 (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 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 is

parameter No. 5104 is set to 1.

contained.)

-

Types I and II

Selection of type I or II

For 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.

- 138 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.8.3

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 W(Δk) U(Δi) R(d) ;

G73.7 P(ns) Q(nf) U(Δu) W(Δw) 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 V(Δk) W(Δi) R(d) ;

G73.7 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ;

N (ns) ;

- - -

N (nf) ;

XpYp plane

G73.7 U(Δk) V(Δi) R(d) ;

G73.7 P(ns) Q(nf) U(Δw) V(Δu) 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)

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.

Δk

: 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.

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.

- 140 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

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.

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.

Δk+Δw

D

Δw

Δi+Δu/2

Δu/2

C

A

(R)

(R)

B

(F)

Δu/2

A'

+X

Δw

Target figure

(F): Cutting feed

(R): Rapid traverse

+Z

Fig. 5.8.3 (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 While the values Δi and Δk, or Δu and Δw 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 G73.7 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 G73.7 block or the previous block

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

S, and T functions.

- 141 -

Content      ..     3      4      5      6     ..