Content      ..     8      9      10      11     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 10

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

- Operations

A taper cutting cycle performs the same four operations as a straight

cutting cycle.

However, operation 1 moves the tool from the start point (A) to the

position obtained by adding the taper amount to the specified

coordinate of the second axis on the plane (specified X-coordinate for

the ZX plane) in rapid traverse.

Operations 2, 3, and 4 after operation 1 are the same as for a straight

cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

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

The tool path is determined according to the relationship between the

sign of the taper amount (address I, J, or K) and the cutting end point

in the direction of the

length in the absolute or incremental

programming as follows.

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(F)

1(R)

X

U/2

3(F)

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(F)

U/2

3(F)

2(F)

1(R)

I

4(R)

W

X

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other

than G90, G92, or G94.

- 254 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.3.2

Threading Cycle (G92)

6.3.2.1

Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

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

the figure below) in the direction of the length

Q_

: Angle for shifting the threading start angle

(Increment: 0.001 degrees,

Valid setting range: 0 to 360 degrees)

F_

: Thread lead (L in the figure below)

X axis

Z

W

4(R)

3(R)

A

U/2

2(F)

1(R)

A’

X/2

Z axis

(R) ... Rapid traverse

(F)

Cutting feed

L

Approx.

(The chamfered angle in the left figure is 45

45°

degrees or less because of the delay in the

r

servo system.)

Detailed chamfered thread

Fig. 6.3.2 (c) Straight threading

Explanation

The ranges of thread leads and restrictions related to the spindle speed

are the same as for threading with G32.

- Operations

A straight threading cycle performs four operations:

(1) Operation

1 moves the tool from the start point

(A) to the

specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in

cutting feed. At this time, thread chamfering is performed.

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in rapid

traverse.

(Retraction after chamfering)

- 255 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

(4) Operation 4 moves the tool to the start coordinate of the first axis

on the plane

(start Z-coordinate for the ZX plane) in rapid

traverse.

(The tool returns to the start point (A).)

CAUTION

Notes on this threading are the same as in

threading in G32. However, a stop by feed hold is

as follows; Stop after completion of path 3 of

threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4

are performed by pressing cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other

than G90, G92, or G94.

- Acceleration/deceleration for threading after interpolation

Acceleration/deceleration for threading after interpolation 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.

- 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. A signal from the machine

tool, initiates thread chamfering. The chamfering distance r is

specified in a range from

0.1L to

12.7L in

0.1L increments by

parameter No. 5130.

(In the above expression, L is the thread lead.)

A thread chamfering angle between 1 to 89 degrees can be specified in

parameter No. 5131. When a value of 0 is specified in the parameter,

an angle of 45 degrees is assumed.

For thread chamfering, the same type of acceleration/deceleration after

interpolation, time constant for acceleration/deceleration after

interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and

angle of thread chamfering are used for this cycle

and threading cycle with G76.

- 256 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- 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

Description

No. 1466

(No. 1611#0)

0

Other than

Uses the type of acceleration/deceleration after

0

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.

- 257 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Feed hold in a threading cycle (threading cycle retract)

Feed hold may be applied during threading (operation 2). In this

case, the tool immediately retracts with chamfering and returns to the

start point on the second axis (X-axis), then the first axis (Z-axis) on

the plane.

Ordinary cycle

X axis

Motion at feed hold

Z axis

Start point

Rapid traverse

Cutting feed

Feed hold is effected here.

The chamfered angle is the same as that at the end point.

CAUTION

Another feed hold cannot be made during retreat.

- Inch threading

Inch threading specified with address E is allowed.

- 258 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.3.2.2

Taper threading cycle

Format

ZpXp-plane

G92 X(U)_ Z(W)_ I_ F_ Q_ ;

YpZp-plane

G92 Y(V)_ Z(W)_ K_ F_ Q_ ;

XpYp-plane

G92 X(U)_ Y(V)_ J_ F_ Q_ ;

X_,Y_,Z_

: Coordinates of the cutting end point (point A' in

the figure below) in the direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A'

in the figure below) in the direction of the length

Q_

: Angle for shifting the threading start angle

(Increment: 0.001 degrees,

Valid setting range:

0 to 360 degrees)

I_,J_,K

: Taper amount (I in the figure below)

F_

: Thread lead (L in the figure below)

X axis

Z

W

A

4(R)

U/2

(R)

Rapid traverse

3(R)

1(R)

A’

(F)

Cutting feed

2(F)

I

X/2

Z axis

L

(The chamfered angle in the left figure

is 45 degrees or less because of the

Approx. 45°

delay in the servo system.)

r

Detailed chamfered thread

Fig. 6.3.2 (d) Taper threading cycle

- 259 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Explanation

The ranges of thread leads and restrictions related to the spindle speed

are the same as for threading with G32.

The figure of a taper is determined by the coordinates of the cutting

end point (A') in the direction of the length and the sign of the taper

amount (address I, J, or K). For the cycle in the figure above, a

minus sign is added to the taper amount.

NOTE

The increment system of address I, J, or K for

specifying a taper depends on the increment

system for the reference axis. Specify a radius

value at I, J, or K.

- Operations

A taper threading cycle performs the same four operations as a straight

threading cycle.

However, operation 1 moves the tool from the start point (A) to the

position obtained by adding the taper amount to the specified

coordinate of the second axis on the plane (specified X-coordinate for

the ZX plane) in rapid traverse.

Operations 2, 3, and 4 after operation 1 are the same as for a straight

threading cycle.

CAUTION

Notes on this threading are the same as in

threading in G32. However, a stop by feed hold is

as follows; Stop after completion of path 3 of

threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4

are performed by pressing cycle start button once.

- 260 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

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

The tool path is determined according to the relationship between the

sign of the taper amount (address I, J, or K) and the cutting end point

in the direction of the

length in the absolute or incremental

programming as follows.

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(F)

1(R)

X

U/2

3(F)

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(F)

U/2

3(F)

2(F)

1(R)

I

4(R)

W

X

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other

than G90, G92, or G94.

- Acceleration/deceleration for threading after interpolation

- Time constant and FL feedrate for threading

- Thread chamfering

- Retraction after chamfering

- Shifting the start angle

- Threading cycle retract

- Inch threading

See the pages on which a straight threading cycle is explained.

- 261 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

6.3.3

End Face Turning Cycle (G94)

6.3.3.1

Face cutting cycle

Format

G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the end face

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

the figure below) in the direction of the end face

F_

: Cutting feedrate

X axis

1

(R)

(R)

Rapid traverse

A

(F)

Cutting feed

2

(F)

4

(R)

U/2

A’

3

(F)

X/2

W

Z axis

Z

Fig. 6.3.3 (e) Face cutting cycle

Explanation

- Operations

A face cutting cycle performs four operations:

(1) Operation

1 moves the tool from the start point

(A) to the

specified coordinate of the first axis on the plane

(specified

Z-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the

second axis on the plane (specified X-coordinate for the ZX

plane) in cutting feed.

(The tool is moved to the cutting end

point (A') in the direction of the end face.)

(3) Operation 3 moves the tool to the start coordinate of the first axis

on the plane (start Z-coordinate for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in rapid

traverse.

(The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

- 262 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

6.3.3.2

Taper cutting cycle

Format

ZpXp-plane

G94 X(U)_ Z(W)_ K _ F_ ;

YpZp-plane

G94 Y(V)_ Z(W)_ J _ F_ ;

XpYp-plane

G94 X(U)_ Y(V)_ I _ F_ ;

X_,Y_,Z_

: Coordinates of the cutting end point (point A' in

the figure below) in the direction of the end face

U_,V_,W_ : Travel distance to the cutting end point (point A'

in the figure below) in the direction of the end

face

I_,J_,K_

: Taper amount (K in the figure below)

F_

: Cutting feedrate

X axis

1(R)

A

(R)

Rapid traverse

2(F)

4(R)

(F)

Cutting feed

U/2

A’

3(F)

X/2

K

W

Z axis

Z

Fig. 6.3.3 (f) Taper cutting cycle

Explanation

The figure of a taper is determined by the coordinates of the cutting

end point (A') in the direction of the end face and the sign of the taper

amount (address I, J, or K). For the cycle in the figure above, a

minus sign is added to the taper amount.

NOTE

The increment system of address I, J, or K for

specifying a taper depends on the increment

system for the reference axis. Specify a radius

value at I, J, or K.

- 264 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- Operations

A taper cutting cycle performs the same four operations as a face

cutting cycle.

However, operation 1 moves the tool from the start point (A) to the

position obtained by adding the taper amount to the specified

coordinate of the first axis on the plane (specified Z-coordinate for the

ZX plane) in rapid traverse.

Operations 2, 3, and 4 after operation 1 are the same as for a face

cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

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

The tool path is determined according to the relationship between the

sign of the taper amount (address I, J, or K) and the cutting end point

in the direction of the

end face in the absolute or incremental

programming as follows.

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, K < 0

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

X

Z

X

1(R)

Z

K

W

Z

3(F)

U/2

2(F)

4(R)

U/2

2(F)

4(R)

3(F)

1(R)

K

W

Z

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

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

at |K|≤|W|

at |K|≤|W|

X

W

X

K

Z

Z

3(F)

1(R)

2(F)

4(R)

U/2

U/2

2(F)

4(R)

1(R)

3(F)

Z

K

Z

W

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other

than G90, G92, or G94.

- 265 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

6.3.4

How to Use Canned Cycles

An appropriate canned cycle is selected according to the shape of the

material and the shape of the product.

- Straight cutting cycle (G90)

Shape of material

Shape of

product

- Taper cutting cycle (G90)

Shape of material

Shape of product

- 266 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- Face cutting cycle (G94)

Shape of material

Shape of product

- Face taper cutting cycle (G94)

Shape of material

Shape of product

- 267 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

6.3.5

Canned Cycle and Tool Nose Radius Compensation

When tool nose radius compensation is applied, the tool nose center

path and offset direction are as shown below. At the start point of a

cycle, the offset vector is canceled. Offset start-up is performed for

the movement from the start point of the cycle. The offset vector is

temporarily canceled again at the return to the cycle start point and

offset is applied again according to the next move command. The

offset direction is determined depending of the

cutting

pattern

regardless of the G41 or G42 mode.

Outer diameter/internal diameter cutting cycle (G90)

Tool nose radius center path

Offset direction

0

Tool nose radius center path

8

3

Whole tool nose

4

5

7

1

2

6

Whole tool nose

Whole

tool nose

Programmed path

End face cutting cycle (G94)

Tool nose radius center path

Offset direction

0

Tool nose radius center path

8

Whole tool nose

4

3

5

7

1

2

6

Whole

Whole tool nose

tool nose

Programmed path

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

- 268 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

Differences between this CNC and the Series 0i-C

NOTE

This CNC is the same as the Series 0i-C in the

offset direction, but differs from the series in the

tool nose radius center path.

• For this CNC

Cycle operations of a canned cycle are replaced

with G00 or G01. In the first block to move the

tool from the start point, start-up is performed.

In the last block to return the tool to the start

point, offset is canceled.

• For the Series 0i-C

This series differs from this CNC in operations in

the block to move the tool from the start point

and the last block to return it to the start point.

For details, refer to "Series 0i-C Operator's

Manual."

How compensation is applied for the Series 0i-C

G90

G94

Tool nose radius center path

Tool nose radius center path

4,8,3

0

4,8,3

0

8

8

3

5,0,7

3

5,0,7

4

4

5

7

5

7

2

2

1,6,2

1

1,6,2

1

6

6

Whole

Whole

4,5,1

8,0,6

tool nose4,5,1

8,0,6

tool nose

3,7,2

3,7,2

Programmed path

Programmed path

- 269 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

6.3.6

Restrictions on Canned Cycles

Limitation

- Modal

Since data items X (U), Z (W), and R in a canned cycle are modal

values common to G90, G92, and G94. For this reason, if a new X

(U), Z (W), or R value is not specified, the previously specified value

is effective.

Thus, when the travel distance along the Z-axis does not vary as

shown in the program example below, a canned cycle can be repeated

only by specifying the travel distance along the X-axis.

Example

X axis

66

4

8

12

16

Workpiece

0

The cycle in the above figure is executed by the following

program:

N030 G90 U-8.0 W-66.0 F0.4;

N031 U-16.0;

N032 U-24.0;

N033 U-32.0;

The modal values common to canned cycles are cleared when a

one-shot G code other than G04 is specified.

Since the canned cycle mode is not canceled by specifying a one-shot

G code, a canned cycle can be performed again by specifying modal

values. If no modal values are specified, no cycle operations are

performed.

When G04 is specified, G04 is executed and no canned cycle is

performed.

- 270 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.4.1

Stock Removal in Turning (G71)

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

Format

ZpXp plane

G71 P(ns) Q(nf) U(∆u) W(∆w) I(∆i) K(∆k) D(∆d) F(f ) S(s )

T(t );

The move command between A and B is specified in the

N (ns) ;

blocks from sequence number ns to nf.

N (nf) ;

YpZp plane

G71 P(ns) Q(nf) V(∆w) W(∆u) J(∆k) K(∆i) D(∆d) F(f ) S(s )

T(t );

N (ns) ;

N (nf) ;

XpYp plane

G71 P(ns) Q(nf) U(∆w) V(∆u) I(∆k) J(∆i) D(∆d) F(f ) S(s ) T(t );

N (ns) ;

N (nf) ;

∆d

: 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.

∆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)

∆i

: Distance of the finishing allowance of the roughing in the direction

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

∆k

: Distance of the finishing allowance of the roughing 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 block is effective.

NOTE

Even if pocket calculator type decimal point

programming is specified (DPI (bit 0 of parameter

No. 3401) = 1), the unit of address D is least input

increment. In addition, when a decimal point is

input in address D, the alarm (PS0007) is issued.

- 273 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the

∆d

increment system for the

Radius programming

Not required

Not allowed

reference axis.

Depends on

Depends on the

diameter/radius

∆u

increment system for the

Required

Allowed

programming for the

reference axis.

second axis on the plane.

Depends on

Depends on the

diameter/radius

∆w

increment system for the

Required

Allowed

programming for the first

reference axis.

axis on the plane.

Depends on the

∆i

increment system for the

Radius programming

Not required

Allowed

reference axis.

Depends on the

∆k

increment system for the

Radius programming

Not required

Allowed

reference axis.

(R)

C

B

A

(R)

∆d

(F)

45°

e

(F)

Target figure

∆u/2

A’

+X

(F): Cutting feed

∆W

+Z

(R): Rapid traverse

e: Escaping amount (parameter No.5133)

Fig. 6.4.1 (a) Cutting path of an outer surface rough cutting cycle

without rough cutting finishing allowance (type I)

- 274 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

C

B

(R)

A

(R)

∆d

(R)

(F)

45°

e

(F)

Target figure

∆i

∆u/2

+X

A’

(F): Cutting feed

∆K

+Z

(R): Rapid

∆W

e: Escaping amount (parameter No.5133)

Fig. 6.4.1 (b) Cutting path of an outer surface rough cutting cycle with

rough cutting finishing allowance (type I)

- 275 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Explanation

- Operations

If a target figure passing through A, A’, and B in this order is given by

the program, a workpiece is cut away by depth of cut ∆d at a time.

The machining path varies as follows depending on whether the rough

machining finishing allowance is specified.

(1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut

∆d with finishing

allowances ∆u/2 and ∆w left, and rough cutting as finishing is

performed according to the target figure program after the last

machining.

(2) When the rough cutting finishing allowance is specified

Cutting is performed by depth of cut ∆d with cutting allowances

∆u/2+∆i and ∆w+∆k left, and the tool returns to the start point

(A) after the last cutting is performed. Then, rough machining as

finishing is performed along the target figure to remove cutting

allowances ∆i and ∆k.

Upon completion of rough machining as finishing, the block next to

the sequence block specified by Q is executed.

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 G71 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 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.

- Escaping amount (e)

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

Diameter/radius

No.

Unit

Sign

programming

Depends on the increment

Not

5133

Radius programming

system for the reference axis.

required

- 276 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- 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

first axis on the plane (Z-axis for the ZX plane). At this time, the

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

B

A

A

B

U(+)…W(+)

U(+)…W(-)

A'

A'

Both linear and

A'

A'

circular interpolation

are possible

U(-)…W(+)

U(-)…W(-)

B

A

A

B

+X

+Z

Fig. 6.4.1 (c) 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.

- 277 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

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) of

number specified at address Q is contained

parameter No. 5102 is set to

in the program before cycle operation.

1.

Checks the target figure before cycle

Enabled when bit 2 (FCK) of

operation.

parameter No. 5104 is set to

(Also checks that a block with the sequence

1.

number specified at address Q is contained.)

- Types I and II

Selection of type I or II

For G71, 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.

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 without moving the tool along the

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

incremental programming with travel distance 0 (W0 for the ZX

plane).

- 278 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- Type I

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

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

Example

ZX plane

G71 V10.0 R5.0 ;

G71 P100 Q200

;

N100 X(U)_ ;

(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 figure below.

B

A

A’

X

Z

No pockets are allowed.

Fig. 6.4.1 (d) Figure which does not show monotone increase or

decrease (type I)

CAUTION

If a figure does not show monotone change along

the first or second axis on the plane, alarm PS0064

or 0329 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.

- 279 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

(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. 6.4.1 (e) 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. When the rough cutting finishing allowance is

specified, however, rough cutting as finishing is performed.

- Type II

(R)

(F)

C

(R)

B

A

∆d

(R)

(F)

∆d

(F)

Target figure

∆u/2

A’

+X

(F): Cutting feed

∆W

+Z

(R): Rapid traverse

Fig. 6.4.1 (f) Cutting path in stock removal in turning (type II)

When the figure program for instructing a target figure passing

through A, A’, and B in this order is specified, a workpiece is cut

away by depth of cut ∆d at a time. In type II, cutting is performed

along the figure after rough cutting in the direction of the plane first

axis (z-axis for the ZX plane).

The machining path varies as follows depending on whether the rough

machining finishing allowance is specified.

- 280 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

(1) When the rough cutting finishing allowance is not specified

Cutting is performed by depth of cut

∆d with finishing

allowances ∆u/2 and ∆w left, and the tool returns to the start

point

(A) after the last cutting is performed

(one pocket is

assumed because Pn→Pm is parallel to the z-axis in the above

figure, and the zone is cut). Then, rough machining as finishing

is performed according to the finishing figure program with

finishing allowances ∆u/2 and ∆w left.

(2) When the rough cutting finishing allowance is specified

Cutting is performed by depth of cut ∆d with cutting allowances

∆u/2+∆i and ∆w+∆k left, and the tool returns to the start point

(A) after the last cutting is performed. Then, rough machining as

finishing is performed along the target figure to remove cutting

allowances ∆i and ∆k.

Upon completion of rough machining as finishing, the block next to

the sequence block specified by Q is executed.

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 (U-axis) and Z-axis (W-axis) for the ZX plane)

must be specified. When you want to use type II without

moving the tool along the Z-axis on the ZX plane in the first

block, specify W0.

Example

ZX plane

G71 V10.0 R5.0;

G71 P100 Q200

;

N100 X(U)_ Z(W)_ ;

(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

10

3

2

1

+Z

Fig. 6.4.1 (g) 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

following figure cannot be machined.

- 281 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Monotone change is not

observed along the Z-

axis.

+X

+Z

Fig. 6.4.1 (h) 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. 6.4.1 (i) Figure which can be machined (type II)

- 282 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

(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

∆d

(specified in the

command or parameter No. 5132)

Fig. 6.4.1 (j) Cutting along the workpiece figure (type II)

The escaping amount e after cutting is 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. 6.4.1 (k) 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 ∆d 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 ∆d 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.

- 283 -

Content      ..     8      9      10      11     ..