FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

Table. 19.10 (c) Example of setting parameters related to

acceleration pattern (2/2)

Parameter

Setting

Unit

Remarks

No.

Accelera-

19546,19552

18712

0.01%

At P1, 90(Nm) can be used for

tion at P1

19558,19564

the acceleration/deceleration,

so set the ratio 7717 (mm/sec²)

to 4124 (mm/sec²).

1.8712 = 7717/4124

Accelera-

19547-19549

0.01%

0 is set because P2 to P4 are

tion at P2

19553-19555

skipped.

to P4

19559-19561

19565-19567

Accelera-

19550,19556

14345

0.01%

At P5, 69(Nm) can be used for

tion at P5

19562,19568

the acceleration/deceleration,

so set the ratio 5916 (mm/sec²)

to 4124 (mm/sec²).

1.4345 = 5916/4124

With the above parameter settings, the acceleration pattern will be shown

as the following figure. The acceleration is 7716 (mm/sec²) in case speed

is up to 32000 (mm/min) and acceleration is calculated according to the

following figure in case speed is from 32000 (mm/min) up to 48000

(mm/min).

9000

8000

7000

6000

5000

4000

3000

2000

1000

16000

32000

48000

Speed mm/min

Fig.19.10 (f) Acceleration pattern with consideration of friction

NOTE

The values in the model a30/4000i speed-torque

characteristic diagram are just typical ones. The values will

change depending on the digital servo software,

parameters, input voltage, and other factors.

The optimum acceleration will, therefore, change due to the

characteristics of the machine.

520

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

D Examples of setting if

From the effect of gravity and friction, torque for acceleration/deceleration

the acceleration pattern

is different on each condition, such as acceleration, deceleration or plus move

differs depending on

(up), minus move (down).

whether acceleration or

The following example is for the vertical axis and gravity and friction torque

deceleration is in

are assumed as follows.

progress and whether

Torque of gravity : 20 (Nm)

the movement is in the

Torque of friction : 10 (Nm)

minus or plus direction

Because these value are different on each machine, it is necessary to observe

the output torque on the actual machine for deciding acceleration pattern

The conditions are the same as the previous example.

Motor speed at rapid traverse

3000 (min^-1)

Ball screw pitch

16 (mm)

Inertia

: The machine inertia is to be 2.0

times higher than that of the rotor.

Rotor inertia

0.0099 (Kgm²)

Maximum torque

100 (Nm) Speed: 0 to 2000 (min^-1)

Torque at rapid traverse

79 (Nm) Speed: 3000 (min^-1)

Minimum torque

58 (Nm) Speed: 4000 (min^-1)

(1) In case of plus move (up) and acceleration

Because torque of Gravity and friction work against the output torque of

motor, the torque for acceleration/deceleration is as follows.

Maximum torque

70(=100-20-10) (Nm)

Speed: 0 to 2000 (min^-1)

Torque at rapid traverse

49(=79-20-10) (Nm)

Speed: 3000 (min^-1)

Minimum torque

28(=58-20-10) (Nm)

Speed: 4000 (min^-1)

1000

2000

3000

4000

Speed(min^-1)

Fig.19.10(g) Torque for Acc/Dec in case of + move and acceleration

521

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

Parameter setting is as follows,

Parameter

Setting

Unit

Remarks

No.

Accel-

19545

14554

0.01

At P0, 70(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 6002 (mm/sec²) to

4124 (mm/sec²). 1.4554 =

6002/4124

Accel-

19546

14554

0.01

At P1, 70(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 6002 (mm/sec²) to

4124 (mm/sec²). 1.4554 =

6002/4124

Accel-

19547-19549

0.01

0 is set because P2 to P4 are

eration at

skipped.

P2 -P4

Accel-

19550

10187

0.01

At P5, 49(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 4201 (mm/sec²) to

4124 (mm/sec²). 1.0187 =

4201/4124

7000

6000

5000

4000

3000

2000

1000

16000

32000

48000

Speed (mm/min)

Fig.19.10(h) Acceleration pattern in case of + move and acceleration

(2) In case of plus move (up) and deceleration

Because torque of Gravity and friction work forward to the output torque

of motor, the torque for acceleration/deceleration is as follows.

Maximum torque

130(=100+20+10) (Nm)

Speed: 0 to 2000 (min^-1)

Torque at rapid traverse

109(=79+20+10) (Nm)

Speed: 3000 (min^-1)

Minimum torque

88(=58+20+10) (Nm)

Speed: 4000 (min^-1)

522

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

150

100

1000

2000

3000

4000

Speed(min^-1)

Fig.19.10(i) Torque for Acc/Dec in case of + move and deceleration

Parameter setting is as follows,

Parameter

Setting

Unit

Remarks

No.

Accel-

19557

27027

0.01

At P0, 130(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 11146 (mm/sec²) to

4124 (mm/sec²). 2.7027 =

11146/4124

Accel-

19558

27027

0.01

At P1, 130(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 11146 (mm/sec²) to

4124 (mm/sec²). 2.7027 =

11146/4124

Accel-

19559-19561

0.01

0 is set because P2 to P4 are

eration at

skipped.

P2 -P4

Accel-

19562

22662

0.01

At P5, 109(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 9346 (mm/sec²) to

4124 (mm/sec²). 2.2662 =

9346/4124

11500

11000

10500

10000

9500

9000

8500

8000

16000

32000

48000

Speed (mm/min)

Fig.19.10(j) Acceleration pattern in case of + move and deceleration

523

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

(3) In case of minus move (down) and acceleration

Because torque of Gravity works forward to the output torque of motor

and torque of friction works against the output torque of motor, torque for

acceleration/deceleration is as follows.

Maximum torque

110(=100+20-10) (Nm)

Speed: 0 to 2000 (min^-1)

Torque at rapid traverse

89(=79+20-10) (Nm)

Speed: 3000 (min^-1)

Minimum torque

68(=58+20-10) (Nm)

Speed: 4000 (min^-1)

150

100

1000

2000

3000

4000

Speed(min^-1)

Fig.19.10(k) Torque for Acc/Dec in case of - move and acceleration

Parameter setting is as follows,

Parameter

Setting

Unit

Remarks

No.

Accel-

19551

22869

0.01

At P0, 110(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 9431 (mm/sec²) to

4124 (mm/sec²). 2.2869 =

9431/4124

Accel-

19552

22869

0.01

At P1, 110(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 9431 (mm/sec²) to

4124 (mm/sec²). 2.2869 =

9431/4124

Accel-

19553-19555

0.01

0 is set because P2 to P4 are

eration at

skipped.

P2 -P4

Accel-

19556

18504

0.01

At P5, 89(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 7631 (mm/sec²) to

4124 (mm/sec²). 1.8504 =

7631/4124

10000

9000

8000

7000

6000

5000

4000

3000

2000

1000

16000

32000

48000

Speed (mm/min)

Fig.19.10(l) Acceleration pattern in case of - move and acceleration

524

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

(4) In case of minus move (down) and deceleration

Because torque of Gravity works against the output torque of motor and

torque of friction works forward to the output torque of motor, torque for

acceleration/deceleration is as follows.

Maximum torque

90(=100-20+10) (Nm)

Speed: 0 to 2000 (min^-1)

Torque at rapid traverse

69(=79-20+10) (Nm)

Speed: 3000 (min^-1)

Minimum torque

48(=58-20+10) (Nm)

Speed: 4000 (min^-1)

100

1000

2000

3000

4000

Speed(min^-1)

Fig.19.10(m) Torque for Acc/Dec in case of - move and deceleration

Parameter setting is as follows,

Parameter

Setting

Unit

Remarks

No.

Accel-

19563

18712

0.01

At P0, 90(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 7717 (mm/sec²) to

4124 (mm/sec²). 1.8712 =

7717/4124

Accel-

19564

18712

0.01

At P1, 90(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 7717 (mm/sec²) to

4124 (mm/sec²). 1.8712 =

7717/4124

Accel-

19565-19567

0.01

0 is set because P2 to P4 are

eration at

skipped.

P2 -P4

Accel-

19568

14345

0.01

At P5, 69(Nm) can be used for

eration at

the acceleration/deceleration, so

set the ratio 5916 (mm/sec²) to

4124 (mm/sec²). 1.4345 =

5916/4124

525

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

9000

8000

7000

6000

5000

4000

3000

2000

1000

16000

32000

48000

Speed (mm/min)

Fig.19.10(n) Acceleration pattern in case of - move and deceleration

Limitations

D Linear type positioning

When Optimum torque acceleration/deceleration is enabled, linear type

positioning for rapid traverse is selected automatically in AI high

precision contour control and AI nano high precision contour control

mode even if the parameter LRP, bit 1 of parameter No. 1401, is set to 0

(nonlinear type is selected).

D Modes and conditions

Optimum torque acceleration/deceleration is enabled when AI high

precision contour control or AI nano high precision contour control mode

is active and the conditions under which AI high precision contour control

and AI nano high precision contour control are satisfied.

D Target axes

Optimum torque acceleration/deceleration can be performed on axes

which are selected by parameter No.7510.

D Acceleration pattern

In the same direction move, it is necessary that the acceleration during

deceleration is set 1/3 of one during acceleration at least.

Also, the acceleration pattern data must be set so that the time required

for the deceleration from the rapid traverse rate to a speed of 0 does not

exceed 4000 (msec). This does not include the acceleration change time

of bell-shaped acceleration/deceleration.

If the deceleration acceleration ratio or the time required for the

deceleration to a speed of 0 exceeds the above range, P/S alarm (P/S5455)

will be issued at the time rapid traverse is executed.

A slight error will occur between the specified acceleration and the actual

acceleration.

D Tool center point control

Optimum torque acceleration/deceleration is disabled in tool center point

control mode (except startup and cancellation). If this occurs, the

acceleration/deceleration for rapid traverse follows the reference

acceleration.

526

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

It is possible to change the operating mode for two or more specified axes

20.1

to either synchronous operation or normal operation by an input signal

SIMPLE

from the machine.

SYNCHRONOUS

Synchronous control can be performed for up to four pairs of axes with

the Series

16i/160i/160is, or up to three pairs with the Series

CONTROL

18i/180i/180is, according to the parameter setting (parameter No. 8311).

The following operating modes are applicable to machines having two

tables driven independently by separate control axes. The following

example is of a machine with two tables driven independently by the Y

axis and V axis. If the axis names and axis sets that are actually being used

differ from those in the example, substitute the actual names for those

below.

Fig. 20 (a) Example of axis configuration of the machine operated

by simple synchronous control

Explanations

D Synchronous operation

This mode is used for, for example, machining large workpieces that

extend over two tables.

While operating one axis with a move command, it is possible to

synchronously move the other axis. In the synchronous mode, the axis

to which the move command applies is called the master axis, and the axis

that moves synchronously with the master axis is called the slave axis.

In this example, it is assumed that Y axis is the master axis and V axis is

the slave axis. Here, the Y axis and the V axis move synchronously in

accordance with program command Yyyyy issued to the Y axis (master

axis).

Synchronous operation is possible during automatic operation, jog feed,

manual handle feed using the manual pulse generator, and incremental

feed, but is not possible during manual reference position return.

528

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

D Normal operation

This operating mode is used for machining different workpieces on each

table. The operation is the same as in ordinary CNC control, where the

movement of the master axis and slave axis is controlled by the

independent axis address (Y and V). It is possible to issue the move

commands to both the master axis and slave axis in the same block.

(1) The Y axis moves normally according to program command Yyyyy

issued to the master axis.

(2) The V axis moves normally according to program command Vvvvv

issued to the slave axis.

(3) The Y axis and the V axis move simultaneously according to program

command YyyyyVvvvv.

Both automatic and manual operations are the same as in ordinary

CNC control.

D Switching between

For how to switch between the synchronous operation and normal

synchronous operation

operation modes, refer to the relevant manual published by the machine

and normal operation

tool builder.

D Automatic reference

When the automatic reference position return command (G28) and the

position return

2nd/3rd/4th reference position return command (G30) are issued during

synchronous operation, the V axis follows the same movement as the Y

axis returns to the reference position. After the return movement is

complete, the reference position return complete signal of the V axis goes

on when that of the Y axis goes on.

As a rule, commands G28 and G30 must be issued in the normal operating

mode.

D Automatic reference

When the automatic reference position return check command (G27) is

position return check

issued during synchronous operation, the V axis and Y axis move in

tandem. If both the Y axis and the V axis have reached their respective

reference positions after the movement is complete, the reference position

return complete signals go on. If either axis is not at the reference

position, an alarm is issued. As a rule, command G27 must be issued in

the normal operating mode.

D Specifying the slave axis

When a move command is issued to the slave axis during synchronous

operation, a P/S alarm (No. 213) is issued.

D Master axis and slave

The axis to be used as the master axis is set in parameter No. 8311.

axis

The slave axis is selected by an external signal.

D Displaying actual speed

Setting bit 7 (SMF) of parameter No. 3105 to 1 suppresses display of the

for master axis only

actual speed of the slave axes.

529

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

Limitations

D Setting a coordinate

In synchronous axis control, commands that require no axis motion, such

system

as the workpiece coordinate system setup command (G92) and the local

coordinate system setup command (G52), are set to the Y axis by program

command Yyyyy issued to the master axis.

D Externally-requested

For signals such as external deceleration, interlock, and machine lock,

deceleration, interlock,

only the signals issued to the master axis are valid in the synchronous

and machine lock

operating mode. Signals issued to other axes are ignored.

D Pitch error

Both the pitch error and backlash are compensated independently for the

compensation

master axis and the slave axis.

D Manual absolute

Turn on the manual absolute switch during synchronous operation. If it

is off, the slave axis may not move correctly.

D Synchronization error

The difference between the master axis and slave axis in servo positional

check using positional

deviation is always monitored. If the difference exceeds the parameter-

deviation

set limit, an P/S alarm (No. 213) is issued.

D Synchronization error

The difference between the master axis and slave axis in machine

check using machine

coordinates is always monitored. If the difference exceeds the parameter-

coordinates

set limit, an servo alarm (No. 407) is issued.

D Synchronization

When the power is turned on, compensation pulses are output for the slave

axis to match the machine position of the master axis with the machine

position of the slave axis.

(This is enabled only when the absolute

position detection function is used.)

D Compensation for

Compensation for out-of-synchronism (where the difference between

out-of-synchronism

the master and slave axes in servo positional deviation is always

monitored and the servo motor for the slave axis is compensated to reduce

the difference) is not performed.

D Manual reference

When the machine is manually returned to the reference position during

position return

synchronous operation, both the master axis and the slave axis move

synchronously until the acceleration movement is complete. However,

grid detection thereafter is carried out independently.

530

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

20.2

ROTARY AXIS

ROLL-OVER

The roll-over function prevents coordinates for the rotation axis from

20.2.1

overflowing. The roll-over function is enabled by setting bit 0 of

Rotary Axis Roll-over

parameter ROAx 1008 to 1.

Explanations

For an incremental command, the tool moves the angle specified in the

command. For an absolute command, the coordinates after the tool has

moved are values set in parameter No. 1260, and rounded by the angle

corresponding to one rotation. The tool moves in the direction in which

the final coordinates are closest when bit 1 of parameter RABx No. 1008

is set to 0. Displayed values for relative coordinates are also rounded by

the angle corresponding to one rotation when bit 2 of parameter RRLx No.

1008 is set to 1.

Examples

Assume that axis A is the rotating axis and that the amount of movement

per rotation is 360.000 (parameter No. 1260 = 360000). When the

following program is executed using the roll-over function of the rotating

axis, the axis moves as shown below.

Actual

Absolute coordinate

Sequence

G90 A0 ;

movement

value after movement

number

value

end

N1 G90 A-150.0 ;

-150

210

N2 G90 A540.0 ;

-30

180

N3 G90 A-620.0 ;

-80

100

N4 G91 A380.0 ;

+380

120

N5 G91 A-840.0 ;

-840

Relative

-360°

-0°

360°

coordinate value-720°

Absolute

-0°

coordinate value

210°(Absolute)

180°

100°

120°

NOTE

This function cannot be used together with the indexing

function of the index table.

531

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

20.2.2

This function controls a rotary axis as specified by an absolute command.

With this function, the sign of the value specified in the command is

Rotary Axis Control

interpreted as the direction of rotation, and the absolute value of the

specified value is interpreted as the coordinates of the target end position.

Explanations

This function is valid when rotary axis roll-over is enabled (ROAx bit (bit

0 of parameter 1008) is set to 1).

If the RAAx bit (bit 3 of parameter 1008) is set to 1, an absolute command

specified for the roll-over rotary axis is interpreted as follows: The sign

and absolute value of the value specified in the command represent the

direction of rotation and the end position of movement respectively.

If the RAAx bit (bit 3 of parameter 1008) is set to 0, the setting by the

RABx bit (bit 1 of parameter 1008) becomes significant.

Notes

NOTE

This function can be used only when the corresponding

option is provided.

This function is valid for a roll-over rotary axis.

If the RAAx bit (bit 3 of parameter 1008) is set to 1, the RABx

bit (bit 1 of parameter 1008) is ignored. To select a rotary

motion of a shorter travel distance, set both RAAx and RABx

to 0.

This function is not supported when the machine coordinate

system of the PMC axis control function is selected.

532

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

To replace the tool damaged during machining or to check the status of

20.3

machining, the tool can be withdrawn from a workpiece. The tool can

TOOL WITHDRAWAL

then be advanced again to restart machining efficiently.

AND RETURN (G10.6)

The tool withdrawal and return operation consists of the following four

steps:

⋅ Retract

The tool is retracted to a predefined position using the TOOL WITHDRAW

switch.

⋅ Withdrawal

The tool is moved to the tool-change position manually.

⋅ Return

The tool returns to the retract position.

⋅ Repositioning

The tool returns to the interrupted position.

For the tool withdrawal and return operations, see III-4.10.

: Position where the TOOL WITHDRAW switch was turned on

: Programmed position

: Position to which the tool is retracted by manual operation

: Retraction path

: Manual operation (withdraw path)

: Return path

: Repositioning

Format

Specify a retraction axis and distance in the following format:

Specify the amount of retraction, using G10.6.

G10.6

_ ;

_ : In incremental mode, retraction distance from the position

where the retract signal is turned on

In the absolute mode, retraction distance to an absolute position

The specified amount of retraction is effective until G10.6 is next

executed. To cancel the retraction, specify the following:

G10.6 ; (as a single block containing no other commands)

533

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

Explanations

D Retraction

When the TOOL WITHDRAW switch on the machine operator’s panel

is turned on during automatic operation or in the automatic operation stop

or hold state, the tool is retracted the length of the programmed retraction

distance. This operation is called retraction. The position at which

retraction is completed is called the retraction position. Upon completion

of retraction, the RETRACT POSITION LED on the machine operator’s

panel goes on.

When the TOOL WITHDRAW switch is turned on during execution of

a block in automatic operation, execution of the block is interrupted

immediately and the tool is retracted. After retraction is completed, the

system enters the automatic operation hold state.

If the retraction distance and direction are not programmed, retraction is

not performed. In this state, the tool can be withdrawn and returned.

When the TOOL WITHDRAW switch is turned on in the automatic

operation stop or hold state, the tool is retracted, then the automatic

operation stop or hold state is entered again.

When the TOOL WITHDRAW switch is turned on, the tool withdraw

mode is set. When the tool withdraw mode is set, the TOOL BEING

WITHDRAWN LED on the machine operator’s panel goes on.

D Withdrawal

When the manual mode is set, the tool can be moved manually (Manual

continuous feed or manual handle feed) to replace the tool or measure a

machined workpiece. This operation is called a withdrawal. The tool

withdrawal path is automatically memorized by the CNC.

D Return

When the mode is returned to automatic operation mode and the TOOL

RETURN switch on the machine operator’s panel is turned off, the CNC

automatically moves the tool to the retraction position by tracing the

manually-moved tool path backwards. This operation is called a return.

Upon completion of a return to the retraction position, the

RETRACTIONS POSITION LED comes on.

D Repositioning

When the cycle start button is pressed while the tool is in the retraction

position, the tool moves to the position where the TOOL WITHDRAW

switch was turned on. This operation is called repositioning. Upon

completion of repositioning, the TOOL BEING WITHDRAWN LED is

turned off, indicating that the tool withdrawal mode has terminated.

Operation after completion of repositioning depends on the automatic

operation state when the tool withdrawal mode is set.

(1) When the tool withdrawal mode is set during automatic operation,

operation is resumed after completion of repositioning.

(2) When the tool withdrawal mode is set when automatic operation is

held or stopped, the original automatic operation hold or stop state is

set after completion of repositioning. When the cycle start button is

pressed again, automatic operation is resumed.

534

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

Limitations

D offset

If the origin, presetting, or workpiece origin offset value (or External

workpiece origin offset value) is changed after retraction is specified with

G10.6 in absolute mode, the change is not reflected in the retraction

position. After such changes are made, the retraction position must be

respecified with G10.6.

When the tool is damaged, automatic operation can be interrupted with

a tool withdrawal and return operation in order to replace the tool. Note

that if the tool offset value is changed after tool replacement, the change

is ignored when automatic operation is resumed from the start point or

other point in the interrupted block.

D Machine lock, mirror

When withdrawing the tool manually in the tool withdrawal mode, never

image, and scaling

use the machine lock, mirror-image, or scaling function.

D Thread cutting

Tool withdrawal and return operation cannot be performed during thread

cutting.

D Drilling canned cycle

Tool withdrawal and return operation cannot be performed during a

drilling canned cycle.

D Reset

Upon reset, the retraction data specified in G10.6 is cleared. Retraction

data needs to be specified again.

D Retraction command

The tool withdrawal and return function is enabled even when the

retraction command is not specified. In this case, retraction and

repositioning are not performed.

WARNING

The retraction axis and retraction distance specified in

G10.6 need to be changed in an appropriate block

according to the figure being machined. Be very careful

when specifying the retraction distance; an incorrect

retraction distance may damage the workpiece, machine, or

tool.

535

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

When enough torque for driving a large table cannot be produced by only

20.4

one motor, two motors can be used for movement along a single axis.

TANDEM CONTROL

Positioning is performed by the main motor only. The submotor is used

only to produce torque. With this tandem control function, the torque

produced can be doubled.

Main motor

Table

Ball screw

Submotor

Fig. 20.4 (a) Example of operation

In general, the NC regards tandem control as being performed for one

axis. However, for servo parameter management and servo alarm

monitoring, tandem control is regarded as being performed for two axes.

For details, refer to the relevant manual published by the machine tool

builder.

536

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

When the angular axis makes an angle other than

90° with the

20.5

perpendicular axis, the angular axis control function controls the distance

ANGULAR AXIS

traveled along each axis according to the inclination angle. For the

CONTROL/

ordinary angular axis control function, the angular axis is always the

Y-axis and the perpendicular axis is always the Z-axis. For angular axis

ARBITRARY

control B, however, arbitrary axes can be specified as the angular and

ANGULAR AXIS

perpendicular axes, using parameters. A program, when created, assumes

that the angular axis and perpendicular axis intersect at right angles.

CONTROL

However, the actual distance traveled is controlled according to an

inclination angle.

Program coordinate system

+Y Coordinate system actually used

(Angular axis)

+Z (Perpendicular axis)

θ : Inclination angle

Explanations

When the angular axis is the Y-axis and the perpendicular axis is the

Z-axis, the amount of travel along each axis is controlled according to the

formulas shown below.

The distance traveled along the Y-axis is determined by the following

formula:

Ya=Yp/cosθ

The distance traveled along the Z-axis is corrected by the inclination of

the Y-axis, and is determined by the following formula:

Za=Zp-Yp*tanθ

The speed component along the Y-axis is determined by the following

formula:

Fa=Fp/cosθ

Ya, Za, Fa : Actual distance and speed

Yp, Zp, Fp : Programmed distance and speed

D Method of use

The angular and perpendicular axes for which angular axis control is to

be applied must be specified beforehand, using parameters (No. 8211 and

8212).

Parameter AAC (No. 8200#0) enables or disables the inclined axis

control function. If the function is enabled, the distance traveled along

each axis is controlled according to an inclination angle parameter (No.

8210).

Parameter AZR (No. 8200#2) enables angular axis manual reference

point return only with a distance along the angular axis.

By setting the normal axis/angular axis control invalid signal NOZAGC

D Invalidity of normal axis

to 1, slanted axis control only for the angular axis can be available.

In this time the angular axis are converted to those along the slanted

coordinate system without affecting commands to normal axis.

537

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D Absolute and relative

An absolute and a relative position are indicated in the programmed

position display

Cartesian coordinate system.

D Machine position display

A machine position indication is provided in the machine coordinate

system where an actual movement is taking place according to an

inclination angle. However, when inch/metric conversion is performed,

a position is indicated which incorporates inch/metric conversion applied

to the results of inclination angle operation.

WARNING

After angular axis control parameter setting, be sure to

perform manual reference position return operation.

If once manual reference position return has been

performed along the angular axis, also perform manual

reference position return along the perpendicular axis.

P/S alarm No.090 is issued when an attempt is made to

manually return to the reference position along the

perpendicular axis although the angular axis is not on the

reference point.

Once the tool has been moved along the angular axis when

perpendicular/angular axis control disable signal NOZAGC

has been set to 1, manual reference position return must be

performed.

Before attempting to manually move the tool along the

angular and perpendicular axes simultaneously, set

perpendicular/angular axis control disable signal NOZAGC

to 1.

NOTE

For arbitrary angular axis control B, if the same axis number

has been specified in both parameters No.8211 and 8212,

or if a value outside the valid data range has been specified

for either parameter, the angular and perpendicular axes

become the following:

Angular axis: Second axis

Perpendicular axis: Third axis

If an inclination angle close to 0° or ±90° is set, an error can

occur. (A range from ±20° to ±60° should be used.)

Before a perpendicular axis reference position return check

(G27) can be made, angular axis reference position return

operation must be completed.

538

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

20.6

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

CHOPPING

the grinding axis (the axis with the grinding wheel) is being moved

FUNCTION

vertically, a contour program can be executed to instigate movement

(G80, G81.1)

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. For details of the

chopping function activated by signal input, refer to the manual provided

by the machine tool builder.

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

Explanations

D Chopping activated by

Before chopping can be started, the chopping axis, reference position,

signal input

upper dead point, lower dead point, and chopping feedrate must be set

using the parameter screen (or the chopping screen).

For details, refer to the manual provided by the machine tool builder.

D Chopping feedrate

From the start of chopping to point R, the tool moves at the rapid traverse

(feedrate of movement to

rate (specified by parameter No. 1420).

point R)

The override function can be used for either the normal rapid traverserate

or chopping feedrate, one of which can be selected by setting CPRPD (bit

0 of parameter No. 8360).

When the chopping feedrate is overridden, settings between 110% and

150% are clamped to 100%.

D Chopping feedrate

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

(feedrate of movement

the chopping is canceled, the tool moves at the chopping feedrate

from point R)

(specified by parameter No. 8374).

539

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

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.

D Setting chopping data

Set the following chopping data:

D Chopping axis:

Parameter No. 8370

D Reference point (point R):

Parameter No. 8371

D Upper dead point:

Parameter No. 8372

D Lower dead point:

parameter No. 8373

D Chopping feedrate:

Parameter No. 8374

D 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.

For details of how to set chopping data on the chopping screen, refer to

III 11.4.13 Displaying and Setting Chopping Data.

D Chopping after the upper

When the upper dead point or lower dead point is changed while chopping

dead point or lower dead

is being performed, the tool moves to the position specified by the old

point has been changed

data. Then, chopping is continued using the new data.

While chopping is being performed, data can be changed only on the

chopping screen. Changing the data on the parameter screen has no effect

on the current chopping operation.

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.

540

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

(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.

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.

541

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D Servo delay

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

compensation function

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 the effective area setting

(parameter No. 1826), the control unit no longer applies compensation,

allowing the tool to continue moving at its current feedrate.

A coefficient for the compensation amount for the displacement

generated by the servo delay incurred by chopping and the delay incurred

during acceleration/deceleration can be specified in parameter No. 8376.

Point R

Upper dead point

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 | < effective area setting (parameter No. 1826)

542

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

D Mode switching during

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

chopping

manual mode, the chopping axis cannot be moved manually. It can,

however, be moved manually by means of the manual interrupt.

D 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, mode is

canceled, and the tool stops immediately.

D Stopping chopping

The following table 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:

Operation after

Operation/command

Stop position

chopping stops

G80

Point R

Canceled

CHPST: “0”

The tool moves to the lower

Canceled

dead point, then to point R.

*CHLD: “0”

Point R

Restart after *CHLD

goes “1”

Reset

Point R

Canceled

Emergency stop

The tool stops immediately.

Canceled

Servo alarm

The tool stops immediately.

Canceled

P/S alarm

The tool moves to the lower

Canceled

dead point, then to point R.

OT alarm

The tool moves from the up-

Canceled

per or lower point to point R.

D Background editing

When an alarm or battery alarm is issued during background editing, the

tool does not stop at point R.

D Single block signal

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

continues.

Limitations

D Workpiece coordinate

While chopping is being performed, do not change the workpiece

system

coordinate system for the chopping axis.

D PMC axis

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

started.

D Mirror image

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

image function about the chopping axis.

D Move command during

If a move command is specified for the chopping axis while chopping is

chopping

being performed, a P/S 5050 alarm is issued.

D Advanced preview

This function does not support the advanced preview control function.

control

543

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D 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 a

P/S 5050 alarm 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.

Examples

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

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

D 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 ;

D The tool stops at point R.

544

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

20.7

Gears can be cut by turning the workpiece (C-axis) in sync with the

rotation of the spindle (hob axis) connected to a hob.

HOBBING MACHINE

Also, a helical gear can be cut by turning the workpiece (C-axis) in sync

FUNCTION (G80, G81)

with the motion of the Z-axis (axial feed axis).

Helical gear

Spindle

Hob

C-axis

Gear material

Format

G81 T_ L_ Q_ P_ ;

T : Number of teeth (Specifiable range: 1 to 5000)

L : Number of hob threads (Specifiable range: 1 to 20 with a sign)

⋅ The sign of L specifies the direction of rotation of the C-axis.

⋅ If L is positive, the C-axis rotates in the positive direction (+).

⋅ If L is negative, the C-axis rotates in the negative direction (-).

Q: Module or diametral pitch

For metric input, specify a module.

(Unit:

0.00001 mm, Specifiable range: 0.01 to 25.0 mm)

For inch input, specify a diametral pitch.

(Unit:

0.00001 inch^-1, Specifiable range: 0.01 to 250.0 inch^-1)

P : Gear helix angle

(Unit:

0.0001 deg, Specifiable range: -90.0 to +90.0 deg)

P and Q must be specified when a helical gear is to be cut.

G80; Cancels synchronization between the hob axis and C-axis.

Explanations

D Setting the C-axis

The C-axis (workpiece) is usually the fourth axis. However, any axis can

be set as the C-axis by setting the corresponding parameter appropriately

(parameter No. 7710).

D Maintaining the

The synchronization status is maintained provided:

synchronization status

⋅

The interlock signal for the C-axis is turned on.

⋅

The feed hold state exists.

545

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D Releasing the

Synchronization between the hob axis and C-axis can also be canceled

synchronization status

when:

⋅

The power is turned off.

⋅

An emergency stop or servo alarm occurs.

⋅

A reset (external reset signal, reset & rewind signal, or reset key on the

MDI panel) is issued.

By setting bit 0 (HBR) of parameter No. 7700, the release of the

synchronization status by a reset can be suppressed.

D Helical gear

When a helical gear is to be cut, compensation for the C-axis is needed

compensation

according to the amount of travel along the Z-axis (third axis) (axial feed)

and gear helix angle.

Helical gear compensation is performed by adding compensation pulses,

calculated using the formula below, to the C-axis which is synchronized

with the hob axis:

Z sin (P)

Compensation angle =

360 (For metric input)

π T Q

Z Q sin (P)

Compensation angle =

360 (For inch input)

π T

where

Compensation angle : Signed absolute value (deg)

: Amount of travel along the Z-axis after the

specification of G81 (mm or inches)

Total amount of travel along the Z-axis in both

automatic and manual modes

: Signed gear helix angle (deg)

: Number of teeth

Q : Module (mm) or diametral pitch (inch^-1)

The values of P, T, and Q must be programmed.

546

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

D Direction of helical gear

1 When bit 2 (HDR) of parameter No. 7700 = 1

compensation

(a)

(b)

(c)

(d)

- Z

C : +

Z : +

Z : -

P : +

P : -

P : +

P : -

Compensation

direction

(e)

(f)

(g)

(h)

- C

- Z

C : -

Z : +

Z : -

P : +

P : -

P : +

P : -

Compensation

direction

2 When bit 2 (HDR) of parameter No. 7700 = 0 (Items (a) to (d) are the

same as for 1.)

(e)

(f)

(g)

(h)

- C

- Z

C : -

Z : +

Z : -

P : +

P : -

P : +

P : -

Compensation

direction

547

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D Setting the helical gear

The Z-axis (axial feed axis) is usually the third axis. However, any axis

axial feed axis

can be set as the Z-axis by setting the corresponding parameter

appropriately (parameter No. 7709).

D C-axis servo delay

The servo delay is proportional to the speed of the hob axis. Therefore,

compensation (G82, G83,

in a cycle where rough machining and finish machining are performed at

G84)

different hob axis speeds, compensation for the servo delay is required.

The servo delay is calculated as follows:

E= {(

)

(

+C:M+L) +Sup} N

where

: C-axis servo delay compensation

(deg)

: C-axis speed when G83 is specified

(deg/min)

: Servo loop gain (LPGIN of parameter No. 1825)

(sec^-1)

: Delay incurred in the CNC

(sec)

: Delay compensation magnification 1 in the CNC

(SVCMP1 of parameter No. 7715)

: Delay incurred by smoothing, as specified by

parameter No. 7701

(sec)

Sup

: Remaining pulse error caused by acceleration/

deceleration

(deg)

: C-axis servo delay compensation magnification 2

(SVCMP2 of parameter No. 7714)

When the hob axis speed is changed, C-axis servo delay compensation

is performed using the following two methods:

S Compensation is specified both before and after the speed is

changed. Each time G83 is specified, compensation for the delay

at that time is applied.

S Before the speed is changed, the servo delay is recorded. After the

speed is changed, compensation for the difference between the

recorded delay and that observed when the command is specified

is performed.

The latter method, in which the compensation before speed change is

recorded, can be used by setting bit 5 (DLY) of parameter No. 7701 to 1.

This method, in comparison with that where the amount of compensation

is not recorded, offers the advantage of processing being possible at

higher speeds.

548

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

⋅

Method in which compensation for the delay when a command is

specified is performed (G82, G83)

G82: Cancels C-axis servo delay compensation.

G83: Executes C-axis servo delay compensation.

(Example)

G81 T__ L__

;

· · · Starts synchronization.

M03 S100

;

· · · Rotates the hob axis.

G04 P2000 ;

· · · Dwell to assure constant hob axis rotation.

G01 G83

F__

;

· · · Performs C-axis delay compensation.

G01 X__

F__

;

G82 ;

· · · Cancels C-axis servo delay.

S200 ;

· · · Changes the speed.

G04 P2000 ;

· · · Dwell to assure constant hob axis rotation.

G01 G83

F__

;

· · · Performs C-axis delay compensation.

⋅

Method in which the delay before change is recorded (G82, G83,

G84)

G82: Cancels C-axis servo delay compensation.

G83: Performs compensation for the difference between the C-axis

servo delay, observed when G83 is specified, and the delay

recorded by G84.

G84: Records the C-axis servo delay observed when G84 is specified.

(The recorded value remains as is until G81 is specified or

another G84 is specified.)

(Example)

G81 T__ L__

;

· · · Starts synchronization.

M03 S100 ;

· · · Rotates the hob axis.

G04 P2000 ;

· · · Dwell to assure constant hob axis rotation.

G84 ;

· · · Records the C-axis servo delay at the

current speed.

G01 X__ F__

;

S200

;

· · · Changes the speed.

G04 P2000 ;

· · · Dwell to assure constant hob axis rotation

G01 G83

F__;

· · · Performs C-axis servo delay compensation.

⋅

Notes

S Specify the G83 block in G01 mode. Also, specify a feedrate using

the F code.

S Once G83 has been specified, another G83 command cannot be

specified until compensation is canceled by specifying G82, or

C-axis synchronization is canceled.

S Specify G83 once a constant hob axis rotation speed has been

achieved.

549

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 19