Content      ..     8      9      10      11     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. OPERATOR'S MANUAL - page 10

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

* Look-ahead bell-shaped acceleration/deceleration before interpolation is an optional function.

-

Setting an acceleration

T

A permissible acceleration for the linear acceleration/deceleration of each axis is set in parameter No.

1660. The acceleration/deceleration is performed with the maximum tangential acceleration not

exceeding the permissible acceleration of each axis specified in parameter No. 1660.

M

A permissible acceleration for the linear acceleration/deceleration of each axis is set in parameter No.

1660. For bell-shaped acceleration/deceleration, acceleration change time (B) (period of transition from

constant speed state (A) to constant acceleration/ deceleration state (C)) is set in parameter No. 1772. In

the constant acceleration/deceleration state (C), acceleration/deceleration is performed with the maximum

tangential acceleration not exceeding the permissible acceleration of each axis specified in parameter No.

1660.

The acceleration change time specified in parameter No.

1772 is held constant, regardless of the

tangential acceleration.

Tangential feedrate

An optimum gradient is

automatically calculated from the

setting made in parameter No.

1660.

(A)

(B)

(C)

(B)

(A)

(B)

(C)

(B)

(A)

Time set in parameter 1772

-

Method of determining the tangent acceleration

Acceleration/deceleration is performed with the largest tangent acceleration/deceleration that does not

exceed the permissible acceleration set for each axis.

(Example)

X-axis permissible acceleration:

1000 mm/sec²

Y-axis permissible acceleration:

1200 mm/sec²

Acceleration change time:

20 msec

Program:

N1 G01 G91 X20. F6000 ; (Move on the X-axis.)

G04 X0.01 ;

N2 Y20. ; (Move on the Y-axis.)

G04 X0.01 ;

N3 X20. Y20. ; (Move in the XY direction (at 45 degrees).)

- 246 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

Since N3 performs interpolation for the X and Y axes in the 45-degree direction, the acceleration of the Y

axis is controlled according to the X axis to become 1000 mm/s². Therefore, the combined acceleration

is 1414 mm/s².

Tangent feedrate

20ms

1000mm/sec²

1200mm/sec²

1414mm/sec²

gradient

gradient

gradient

20ms

20ms

20ms

-

Acceleration

Acceleration is performed so that the feedrate programmed for a block is attained at the beginning of the

block. When look-ahead acceleration/deceleration before interpolation is valid for multiple blocks,

acceleration can be performed across more than one block.

Feedrate

Speed control by look-ahead

acceleration/deceleration before interpolation

Programmed speed

Time

N1 N2

N3

N4

N5

- 247 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

-

Deceleration

Deceleration starts in advance so that the feedrate programmed for a block is attained at the beginning of

the block.

When look-ahead acceleration/deceleration before interpolation is valid for multiple blocks, deceleration

can be performed across more than one block.

Feedrate

Speed control by look-ahead

Deceleration

acceleration/deceleration before

start point

interpolation

Programmed speed

Deceleration

start point

Time

-

Deceleration based on a distance

If the total distance of the blocks read ahead becomes shorter than or equal to the deceleration distance

obtained from the current feedrate, deceleration starts.

If the total distance of the blocks read ahead during deceleration increases, acceleration is performed.

If the blocks of a small amount of travel are successively specified, deceleration and acceleration may be

performed alternately, making the feedrate inconsistent.

To avoid this, decrease the programmed feedrate.

M

-

Function for changing time constant of bell-shaped acceleration/deceleration

Bell-shaped acceleration/deceleration before interpolation is performed according to the acceleration and

acceleration change time set by the parameters, as shown in the figure below.

Feedrate

T1

Specified

feedrate

T1_low

Low specified

feedrate

Time

T2

T2

T1 : Time obtained from specified feedrate and specified acceleration

(specified feedrate/acceleration (parameter No. 1660))

T2 : Acceleration change time

(parameter No. 1772)

- 248 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

Here, the acceleration change time (T2) remains constant regardless of the specified feedrate, while the

acceleration time for the linear section

(T1), which is determined by acceleration, varies with the

specified feedrate. If T1 becomes shorter than T2 when the specified feedrate is low, linear

acceleration/deceleration not achieving the specified acceleration results, as shown in the figure below.

Linear acceleration/deceleration not achieving

specified acceleration/deceleration

Feedrate

Specified

feedrate

Time

T1low

T1low

T2

T1 : Time obtained from specified feedrate and specified acceleration (specified

feedrate/acceleration (parameter No. 1660))

T2 : Acceleration change time

(parameter No. 1772)

In such a case, set bit 3 (BCG) of parameter No. 7055 to 1. Then, the internal acceleration and vector

time constant of acceleration/ deceleration before interpolation are changed to make the

acceleration/deceleration pattern as close as possible to the optimum bell-shaped acceleration/deceleration

before interpolation based on a specified acceleration/deceleration reference speed, and so

acceleration/deceleration time is reduced.

Feedrate Acceleration/deceleration curve

Specified

feedrate

T1'

: Acceleration time during

T1'

optimum acceleration

T2'

: Time of optimum acceleration

T2'

T2'

change

There are three methods for specifying the acceleration/deceleration reference speed.

(1) Specifying the speed using an F in a G05.1 Q1 block

(2) Setting the speed on parameter No. 7066

(3) Setting the speed specified with the F command issued at the start of cutting as the reference speed

When F is specified in a G05.1Q1 block, the specified feedrate is assumed to be the

acceleration/deceleration reference speed. This command can be used only in the feed per minute mode.

If no F command is specified in a G05.1Q1 block, the feedrate specified in parameter No. 7066 is

assumed to be the acceleration/deceleration reference speed. If 0 is set in parameter No. 7066, the F

command specified in the cutting start block is assumed to be the acceleration/deceleration reference

speed.

- 249 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

-

Automatic feedrate control function

During the advanced preview control, AI advanced preview control, or AI contour control (II) mode, the

feedrate is automatically controlled by reading blocks in advance.

The feedrate is determined using the following conditions. If the specified feedrate exceeds the

determined feedrate, acceleration/ deceleration before interpolation is performed to achieve the

determined feedrate.

<1> Feedrate changes on each axis at a corner and the permissible feedrate change that has been set

<2> Expected acceleration on each axis and the permissible acceleration that has been set

<3> Cutting load that is expected from the travel direction on the Z-axis

Specified tool path

The machining error is decreased

because of the deceleration by

Tool path when advanced

difference in feedrate.

preview control, AI

advanced preview control,

or AI contour control mode

is not used

Tool path when advanced

preview control, AI advanced

preview control, or AI

contour control mode is used

The machining error is decreased

because of the deceleration with

the acceleration.

-

Speed control based on the feedrate difference on each axis at a corner

By using the speed control based on the feedrate difference on each axis at a corner, if a feedrate change

occurs on an axis on each axis at a corner, the feedrate is determined so that any feedrate difference

exceeding the permissible feedrate difference on that axis that has been set for parameter No. 1783 does

not occur, and deceleration is automatically performed.

- 250 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

(Example)

Program

N1 G01 G91 X100. F5000

N2 Y100.

N2

Y

N1

X

Tangent feedrate

Tangent feedrate

Time

The deceleration based

Parameter No.1783

on the feedrate difference

is used.

Time

X-axis feedrate

X-axis feedrate

The feedrate difference

becomes small, and the

The tangent feedrate is

feedrate on each axis

smooth, but the feedrate

becomes smooth.

on each axis is not.

Parameter No.1783

Time

Time

Y-axis feedrate

Y-axis feedrate

Parameter No.1783

Time

Time

When speed control based on the feedrate difference

When speed control based on the feedrate difference is

is invalid

valid

The method of deceleration based on the feedrate difference differs depending on the setting made for

parameter FNW (bit 6 of No. 19500).

If "0" is set, the largest feedrate that does not exceed the permissible feedrate difference set for parameter

No. 1783 is assumed to be the deceleration feedrate.

In this case, the deceleration feedrate differs if the travel direction differs, even if the shape is the same.

- 251 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

(Example)

If parameter FNW (bit 6 of No. 19500) = 0 and the

permissible feedrate difference = 500 mm/min (on all axes)

Decelerate the X/Y axis down to 250

mm/min

Decelerate the X axis

(The tangent direction feedrate is 354

down to 500 mm/min

mm/min.)

Y

X

In the left-side example in the figure above, the X axis is inverted at the corner from the position direction

to the negative direction, and deceleration is performed so that the feedrate difference becomes 500

mm/min. In other words, the feedrate is 250 mm/min both when the axis moves in the position direction

and when it moves in the negative direction. As a result, the tangent direction feedrate becomes 354

mm/min.

X-axis

feedrate

250mm/min

500mm/min

Time

Y-axis

feedrate

250mm/min

Time

If "1" is set, the feedrate is determined not only with the condition that

the permissible feedrate difference and permissible acceleration on each axis are not exceeded, but also

that the deceleration feedrate is constant regardless of the travel direction if the shape is the same.

If 1 is set for this parameter, the deceleration feedrate determined with the feedrate difference may be up

to 30% lower than that determined if 0 is set.

- 252 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

(Example)

If parameter FNW (bit 6 of No. 19500) = 1 and

permissible feedrate difference = 500 mm/min (on all axes)

Decelerate the X/Y axis down to

250 mm/min

(The tangent direction feedrate is

Decelerate the X axis

354 mm/min.)

down to 354 mm/min

Y

X

-

Speed control with acceleration in circular interpolation

When high-speed cutting is performed in circular interpolation or helical interpolation, the actual tool

path has an error with respect to the programmed path. In circular interpolation, this error can be

approximated from the equation given below.

Y

Δr

: Error

Specified path Δr

: Maximum radius error (mm)

v

: Feedrate (mm/s)

r

: Arc radius (mm)

Actual path

a

: Acceleration (mm/s²)

T₁

: Time constant of

acceleration/deceleration after

interpolation at cutting (s)

r

T₂

: Time constant of servo motor (s)

0

X

2

1

2

2

v

1

2

2

Δr =

(T

+T

)

=

(T

+T

)⋅a

......................................................................................(Equation 1)

1

2

1

2

2

r

2

In actual machining, the permissible error Δr is given as the machining accuracy. Therefore, the

permissible acceleration a (mm/sec²) is determined by equation 1.

When a specified feedrate causes the radial error from an arc having a programmed radius to exceed the

permissible error, speed control with acceleration in circular interpolation automatically clamps the

arc-cutting feedrate by using parameter settings.

Let the permissible acceleration calculated from the permissible acceleration set for each axis be A.

Then, maximum permissible feedrate v with programmed radius r is expressed as follows:

v=

A⋅

r

...........................................................................................................................(Equation 2)

If a specified feedrate exceeds feedrate v obtained from equation 2, the feedrate is clamped at feedrate v

automatically.

The permissible acceleration is specified in parameter No. 1735. If there is a difference in permissible

acceleration between two axes for circular interpolation, the lower acceleration is regarded as the

permissible acceleration.

If the radius of an arc is small, too small value can be calculated as deceleration v. In such a case, the

lower feedrate limit can be set in parameter No. 1732 to prevent the feedrate from being decreased too

much.

- 253 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

M

-

Speed control with the acceleration on each axis

When consecutive small lines are used to form a curve, as in the example shown in the figure below, the

feedrate differences on each axis at the individual corners are not very large. Thus, deceleration with the

feedrate differences is not effective. Consecutive small feedrate differences, however, cause a large

acceleration on each axis, as a whole.

In such a case, deceleration can be performed to reduce the impact on the machine and the machining

error caused by too large an acceleration. The deceleration feedrate is determined to be the feedrate that

does not cause the acceleration on each axis to exceed the permissible acceleration set for parameter No.

1737.

The deceleration feedrate is determined for each corner. The actual feedrate is the smaller of the

deceleration feedrate determined at the start point of the block and that determined at the end point.

Depending on the specified figure, a very low deceleration feedrate may be calculated. In such a case,

the lower feedrate limit can be set in parameter No. 1738 to prevent the feedrate from being decreased too

much.

In the following example, the acceleration (gradient of the broken line in the feedrate graph) at too large

at corners N2 to N4 and N6 to N8 and, therefore, deceleration is performed.

N8

N7

N9

N6

N5

Y

N1

N4

X

N3

N2

X-axis

feedrate

Time

Time

Y-axis

feedrate

Time

Time

Tangent

feedrate

N1

N5

N9

N1

N5

N9

Time

Time

When speed control with the acceleration is invalid

When speed control with the acceleration is valid

The method of determining the feedrate with the acceleration differs depending on the setting of

parameter FNW (bit 6 of No. 19500).

If "0" is set, the highest feedrate that does not cause the permissible acceleration set for parameter No.

1737 to be exceeded is assumed to be the deceleration feedrate. In this case, the deceleration feedrate

differs depending on the travel direction even if the shape is the same, as shown in the figure below.

- 254 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

(Example) If a circular shape with a radius of 10 mm is specified with small

line blocks

Parameter FNW (bit 6 of No. 19500) = 0

Permissible acceleration = 1000 mm/s² (on all axes)

Tangent feedrate

F6000

The feedrate is

higher in these

directions.

Time

If "1" is set, the feedrate is determined with not only the condition that the permissible acceleration on

each axis is not exceeded but also the condition that the deceleration feedrate is constant regardless of the

travel direction if the shape is the same.

If

1 is set for this parameter, the deceleration feedrate determined with the feedrate difference or

acceleration may be up to 30% lower than that determined if 0 is set.

(Example) If a circular shape with a radius of 10 mm is specified with small

line blocks

Parameter FNW (bit 6 of No. 19500) = 1,

radius = 10 mm, permissible acceleration = 1000 mm/s² (on all axes)

Tangent feedrate

F6000

The tangent

feedrate is

constant.

Time

NOTE

In circular interpolation, the tangent feedrate is constant regardless of the setting

of the parameter.

M

-

Smooth speed control

In speed control with acceleration, the smooth speed control function recognizes the entire figure from

preceding and following blocks including blocks read ahead to make a smooth feedrate determination.

When a curve is specified with successive minute straight lines, programmed values are rounded to the

least input increment before issued, so the machining profile is approximated with a broken line.

When the feedrate is determined with acceleration in an ordinary manner, an optimum feedrate is

automatically calculated exactly for a programmed figure, so a large acceleration may result depending on

the command, which can lead to deceleration.

In such a case, the use of smooth speed control enables speed control by recognizing the entire figure,

which provides smooth speed control while suppressing local deceleration, therefore increasing the

feedrate.

- 255 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

Large acceleration

: Programmed path

: Recognized figure

Also for a part of a programmed figure in which a large acceleration would be required, the acceleration

is obtained based on the figure recognized from multiple blocks, and the feedrate is determined so that the

acceleration is within the permissible acceleration set in parameter No. 1737.

Deceleration with acceleration

Tangential feedrate

in ordinary manner

Smooth speed control

Command with large acceleration

Time

Smooth speed control obtains the acceleration by using the figure recognized from the preceding and

following blocks including blocks read ahead, so smooth speed control is enabled even in parts in which

the acceleration increases.

Smooth speed control is enabled under the following conditions:

<1> Speed control with acceleration is enabled in the AI contour control II mode.

<2> Successive linear interpolation commands are specified.

<3> Bit 0 (HPF) of parameter No. 19503 is set to 1.

CAUTION

When smooth speed control is used, the feedrate in a certain figure such as a

corner may become larger than the feedrate obtained by ordinary speed control

with acceleration. For corners, set parameter No. 1783, which is the permissible

feedrate difference parameter for speed control with the feedrate difference at

corners, to perform appropriate deceleration by speed control with the corner

feedrate difference.

M

-

Speed control with the cutting load

Usually, the cutting resistance produced when machining is performed with the bottom of the cutter as the

tool lowers along the Z-axis is greater than the cutting resistance produced when machining is performed

with the side of the cutter as the tool rises along the Z-axis. Therefore, deceleration is required.

- 256 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

CAUTION

1 The speed control with the cutting feed is effective only when the tool is parallel

with the Z-axis. Thus, it may not be possible to apply this function, depending on

the structure of the machine used.

2 In the speed control with the cutting feed, the travel direction on the Z-axis is

determined with the appropriate NC command. If, therefore, manual intervention

is performed on the Z-axis with manual absolute on, or if a mirror image is

applied on the Z-axis, the direction on the Z-axis cannot be determined. When

using the speed control with the cutting load, do not use these functions.

3 When performing 3-dimensional coordinate conversion, determine the descent

angle on the Z-axis using the converted coordinate system.

4 Speed control with the cutting load is enabled for all interpolations in the AI

contour control II mode. This function, however, can be made valid only for linear

interpolations by setting bit 4 (ZOL) of parameter No. 19503 to 1.

M

-

Ignoring feedrate commands

In a block in which AI contour control II is enabled, all feedrate commands (F commands) can be ignored

by setting bit 7 (NOF) of parameter No. 8451.

The term feedrate commands, as used here, refer to the following commands:

<1> Modal F commands before the block in which AI contour control II is enabled

<2> F commands and modal F commands in the block in which AI contour control II is enabled

When the feedrate commands are ignored, it is assumed that the upper feedrate limit specified for

parameter No. 8465 is specified.

Note, however, that any issued F commands and modal F commands are stored within the CNC.

Thus, in a block in which AI contour control II changes from the enabled state to the disabled state, the

modal values of the F commands described in <1> and <2> described above are used as modal F

commands, instead of the modal values of the F commands calculated by AI contour control II.

-

Another example of determining the feedrate

If a specified feedrate exceeds the upper feedrate limit of advanced preview control/AI advanced preview

control/AI contour control (II) (in parameter No. 8465), the feedrate is clamped at the upper feedrate.

The upper feedrate limit is clamped at the maximum cutting feedrate (parameter No. 1432).

Limitations

- Conditions for temporarily canceling the advanced preview control, AI advanced

preview control, or AI contour control (II) mode

If any of the commands listed below is executed during advanced preview control, AI advanced preview

control, or AI contour control (II) mode is temporarily canceled. Note that the advanced preview control,

AI advanced preview control, or AI contour control (II) mode resumes as soon as it becomes available.

T

Function name

G code

Positioning (rapid traverse^{) (NOTE 1)}

G00

Spindle positioning

G00

Rigid tapping

G84,G88

Threading ^{(NOTE 2)}

G32

- 258 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

Function name

G code

Variable-lead threading ^{(NOTE 2)}

G34

Single threading cycle ^{(NOTE 2)}

G92

Multiple repetitive threading cycle ^{(NOTE 2)}

G76

When no move command is specified

－

G09

One-shot G code other than those shown at right ^{(NOTE 1)}

G38,G39

M

Function name

G code

Positioning (rapid traverse^{) (NOTE 1)}

G00

Single direction positioning

G60

Rigid tapping

G74,G84

Threading ^{(NOTE 2)}

G33

Electronic gear box (EGB)

G81

When no move command is specified

－

G09

One-shot G code other than those shown at right ^{(NOTE 1)}

G38,G39

G45,G46,G47,G48

NOTE

1 If the first three conditions (1) to (3) below are all met, the mode is not canceled

even when the rapid traverse command is specified. If all the conditions (1) to

(5) are met, the mode is not canceled even when the G28, G30, or G53

command is specified.

(1) Bit 1 (LRP) of parameter No. 1401 is set to 1.

(Interpolation type positioning

is valid.)

(2) Parameter No. 1671 (maximum acceleration during rapid traverse) is set.

(3) Bit 5 (FRP) of parameter No. 19501 is set to 1 (acceleration/deceleration

before interpolation is valid for rapid traverse).

(4) Bit 4 (ZRL) of parameter No. 1015 is set to 1 (the G28, G30, and G53

commands are of the interpolation type).

(5) Bit 1 (AMP) of parameter No. 11240 is set to 1 (acceleration/deceleration

before interpolation is valid for the G28, G30, and G53 commands in the

high-speed, high-precision mode).

2 Acceleration/deceleration before interpolation is invalid for a threading

command. Therefore, if acceleration/deceleration before interpolation is

enabled by a command that precedes or follows a threading command, the tool

is decelerated and stopped temporarily when the block changes.

Since the state of acceleration/deceleration before interpolation does not change

during continuous threading, deceleration does not occur when the block

changes.

-

Parameter list

Positioning

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Positioning type (non-linear (0)/interpolation (1))

1401#1 LRP

- 259 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Acceleration/deceleration type (acceleration constant

1603#4 PRT

(0)/time constant (1))

Acceleration/deceleration type (after interpolation (0)/before

19501#5 FRP

interpolation (1))

Time constant of acceleration/deceleration after interpolation

1620

in rapid traverse

Time constant of bell-shaped acceleration/deceleration after

1621

interpolation in rapid traverse

Maximum permissible acceleration of

1671

acceleration/deceleration after interpolation in rapid traverse

Acceleration change time of bell-shaped

acceleration/deceleration before interpolation in rapid

1672

traverse

Acceleration/deceleration before interpolation

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Maximum permissible acceleration of

1660

acceleration/deceleration before interpolation

Acceleration change time of bell-shaped

None

1772

acceleration/deceleration before interpolation

Valid/invalid state of the function for changing time constant

7055#3

None

of bell-shaped acceleration/deceleration before interpolation

BCG

Reference acceleration/deceleration speed for the function

for changing time constant of bell-shaped

None

7066

acceleration/deceleration before interpolation

Acceleration/deceleration after interpolation

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Acceleration/deceleration type of acceleration/deceleration

1602#3 BS2, 1602#6 LS2

after interpolation in cutting feed

FL rate of acceleration/deceleration after interpolation in

1763

cutting feed

Time constant of acceleration/deceleration after interpolation

1769

in cutting feed

Speed control based on the feedrate difference on each axis

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Permissible feedrate difference when determining the

1783

feedrate based on the feedrate difference at a corner

Method of determining the feedrate based on the feedrate

19500#6 FNW

difference or based on the acceleration

- 260 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

Speed control with acceleration in circular interpolation

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Lower-limit feedrate for the deceleration function with the

1732

acceleration in circular interpolation

Permissible acceleration for the deceleration function with

1735

the acceleration in circular interpolation

M

Speed control with the acceleration on each axis

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Permissible acceleration for the deceleration function with

None

1737

the acceleration

Lower-limit feedrate for the deceleration function with the

None

1738

acceleration

Method of determining the feedrate based on the feedrate

None

19500#6 FNW

difference or based on the acceleration

Others

Parameter No.

Parameter

Advanced

AI advanced

AI contour

preview control

preview control

control (II)

Maximum cutting feedrate during the mode of

1432

acceleration/deceleration before interpolation

Upper-limit feedrate for advanced preview control, AI

8465

advanced preview control, or AI contour control (II)

Upper-limit feedrate for advanced preview control, AI

advanced preview control, or AI contour control (II) (when

8466

only the rotation axis is specified)

16.2 MACHINING CONDITION SELECTING FUNCTION

Overview

By setting a speed- or precision-focused parameter set in an advanced preview control (T series) / AI

advanced preview control (M series) / AI contour control (II) (M series) function and specifying a

precision level in accordance with the machining conditions during machining, parameters suitable to the

conditions can be automatically calculated so that machining can be performed.

This function is an optional one.

Format

-

Changing the precision level using a program

In addition to being switched on the precision level selection screen, the precision level can be changed

using a program in the format below.

- 261 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

T

For advanced preview control

G08 P1 Rx ;

x

Level (1 to 10)

CAUTION

Once specified, a level remains effective even if the advanced preview control

mode is canceled.

M

For AI advanced preview control/AI contour control (II)

G05.1 Q1 Rx ;

x

Level (1 to 10)

CAUTION

Once specified, a level remains effective even if the AI advanced preview control

/ AI contour control (II) mode is canceled.

16.3 MACHINING QUALITY LEVEL ADJUSTMENT (M Series)

M

Overview

In nano smoothing, if the “level 1” and “level 10” parameters of a precision level and smoothing level are

set in order to specify a precision level and smoothing level according to the machining condition during

machining, the parameter values corresponding to the condition can be automatically calculated for

machining.

On the machining quality level adjustment screen, the machining quality/precision/speed level in nano

smoothing can easily be adjusted.

This function is an optional function.

Format

-

Changing the smoothing level by a program

The smoothing level can be switched on the machining level selection screen or machining quality level

adjustment screen; it can also be changed by a program with the following format.

G05.1 Q3 Rx ;

x

Level (1 to 10)

CAUTION

Once a level is specified, it remains valid even after the nano smoothing mode is

canceled.

-

Changing the precision level by a program

For information on the changing the precision level by a program, see Section 16.2, "MACHINING

CONDITION SELECTION FUNCTION".

- 262 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

16.4 JERK CONTROL (M Series)

M

16.4.1 Speed Control with Change of Acceleration on Each Axis

Overview

In portions in which acceleration changes largely, such as a portion where a programmed figure changes

from a straight line to curve, vibration or shock on the machine may occur. Speed control with change of

acceleration on each axis is a function to suppress machining errors due to vibration and machine shock

generated by change of acceleration. This function obtains a feedrate so that change of acceleration is

within the parameter-set permissible acceleration change amount for each axis, and performs deceleration

by using acceleration/deceleration before interpolation.

CAUTION

Before speed control with change of acceleration on each axis can be used, the

options for jerk control and AI contour control II are required.

Explanation

In the following example, the Y-axis acceleration changes largely at the contact point between a linear

interpolation and circular interpolation, so deceleration is performed.

From linear interpolation (N1) to circular interpolation (N2)

Y

N1

N1

N2

N2

X

Vibration due to change

of acceleration

Feedrate

Feedrate

Tangential

feedrate

Time

Time

Time

Time

Y-axis

acceleration

Acceleration

Acceleration

-

Setting the permissible acceleration change amount

The permissible acceleration change amount for each axis is set in parameter No. 1788. When 0 is set in

this parameter for a certain axis, speed control with change of acceleration is not performed for that axis.

• Parameter setting example

Suppose a figure shown below in which a straight line is followed by an arc. Let the specified feedrate

and the arc radius be 6000 mm/min and 10 mm, respectively. Then, the Y-axis acceleration change

amount at the contact point of the linear and arc portions is obtained as follows:

- 263 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

2

v

2

=1000mm

/

s

r

From straight line to arc

Y

Specified feedrate:

6000 mm/min

X

Arc radius:

10 mm

Time

Y-axis

Acceleration

acceleration

change amount:

1000 mm/s²

Acceleration

To suppress the change of acceleration to 300 mm/s², set 300 mm/s² for the Y-axis in parameter No. 1788.

Note that the change of acceleration is determined from the interpolation data of the CNC, so it may differ

from the theoretical value.

The actual machine is affected by acceleration/deceleration and other factors, so the value to be set in the

parameter should be determined after adjustments are made.

-

For successive linear interpolations

When there are successive linear interpolations, speed control with change of acceleration obtains the

deceleration feedrate from the change in acceleration between the start point and end point of a specified

block.

When a curve is specified using successive minute straight lines, programmed values are rounded to the

least input increment before issued, so the machining profile is approximated with a broken line. The

error due to rounding may increase change of acceleration, and especially when the line segments

specified by blocks are short, deceleration is performed frequently. As a result, the machining speed

cannot increase enough. In such a case, a relatively large value should be set in parameter No. 1789 as the

permissible acceleration change amount for each axis in successive linear interpolations to improve the

machining speed.

When a value other than 0 is set in parameter No. 1789 for an axis for which deceleration with change of

acceleration is enabled, this setting is regarded as the permissible acceleration change amount at corners

in which linear interpolations meet. (For portions where a linear interpolation and circular interpolation

meet and where circular interpolations meet, the setting in parameter No. 1788 is used.)

When 0 is set in parameter No. 1789 for an axis, the setting in parameter No. 1788 specifying the

ordinary permissible acceleration change amount is used even at a corner in which linear interpolations

meet.

When smooth speed control is used in speed control with permissible acceleration in AI contour control II,

the deceleration feedrate is obtained from the change of acceleration calculated by smooth speed control.

Therefore, the deceleration feedrate may be higher than the ordinary deceleration feedrate.

- 264 -

16.HIGH-SPEED CUTTING

B-64304EN/02

PROGRAMMING

FUNCTIONS

When linear interpolation is followed

by circular interpolation, speed

control is performed using the

permissible acceleration change

amount set in parameter No. 1788.

Linear

Circular

interpolation

interpolation

For successive linear interpolations,

speed control is performed using the

permissible acceleration change

amount set in parameter No. 1789.

Linear

interpolation

- 265 -

16. HIGH-SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64304EN/02

16.4.2 Look-Ahead Smooth Bell-Shaped Acceleration/Deceleration

before Interpolation

Overview

In look-ahead bell-shaped acceleration/deceleration before interpolation performs smooth

acceleration/deceleration by changing the acceleration at a constant rate in specified acceleration change

time.

In look-ahead smooth bell-shaped acceleration/deceleration before interpolation, the jerk change time is

specified in parameter No. 1790 by using the percentage to the acceleration change time for look-ahead

bell-shaped acceleration/deceleration before interpolation, and change of acceleration is also controlled so

that the change is bell-shaped. This enables smoother acceleration/deceleration, therefore reducing

machine vibration and shock due to acceleration/ deceleration.

(Look-ahead bell-shaped

(Look-ahead smooth bell-shaped

acceleration/deceleration before interpolation)

acceleration/deceleration before interpolation)

Tangential feedrate

Tangential feedrate

Time

Time

Acceleration

Acceleration

Acceleration change time

Time set in parameter No.

1772

Time

Time

Jerk

Jerk change time

Jerk

acceleration

Time set in parameter No.

acceleration

1790 by using the

percentage to the

acceleration change time

Time

Time

CAUTION

Before look-ahead smooth bell-shaped acceleration/deceleration before

interpolation can be used, the option for jerk control and AI contour control II is

required.

- 266 -

17.AXIS CONTROL FUNCTIONS PROGRAMMING

B-64304EN/02

17 AXIS CONTROL FUNCTIONS

Chapter 21, "AXIS CONTROL FUNCTIONS", consists of the following sections:

17.1 AXIS SYNCHRONOUS CONTROL

268

17.2 ROTARY AXIS ROLL-OVER

277

17.3 ARBITRARY ANGULAR AXIS CONTROL

278

17.4 TANDEM CONTROL

287

17.1 AXIS SYNCHRONOUS CONTROL

Overview

When a movement is made along one axis by using two servo motors as in the case of a large gantry

machine, a command for one axis can drive the two motors by synchronizing one motor with the other.

When a synchronous error exceeding a set value occurs, a synchronous error check can be made to issue

an alarm and stop a movement along the axis.

An axis used as the reference for axis synchronous control is referred to as a master axis (M-axis), and an

axis along which a movement is made in synchronism with the master axis is referred to as a slave axis

(S-axis).

Y

Z

A

(Slave axis)

X

(Master axis)

Fig. 17.1 (a) Example of machine with X and A being synchronous axes

The synchronous establishment function can be used for automatic compensation to eliminate a machine

coordinate error in cases such as emergency stop cancellation.

An external signal can be used to turn synchronization on and off.

17.1.1 Axis Configuration for Axis Synchronous Control

Explanation

-

Master axis and slave axis for axis synchronous control

An axis used as the reference for axis synchronous control is referred to as a master axis (M-axis), and an

axis along which a movement is made in synchronism with the master axis is referred to as a slave axis

(S-axis).

By setting the axis number of a master axis in the parameter No. 8311 of the slave axis, the axis

configuration for axis synchronous control is determined.

- 268 -

17.AXIS CONTROL FUNCTIONS PROGRAMMING

B-64304EN/02

Controlled

Axis name

Subscript

Axis name

Master axis number

axis

Parameter

Parameter

Operation

indication

Parameter (No.8311)

number

(No. 1020)

(No.3131)

XM

1

88

77

0

Y

2

89

0

0

A movement is made in

X1

3

88

49

1

synchronism with the XM-axis.

A movement is made in

X2

4

88

50

1

synchronism with the XM-axis.

When one master axis has multiple slave axes, synchronous establishment, and synchronous error check

are performed for each slave axis independently.

-

Combination with tandem control

Tandem control can be used with each of the master and slave axes. The same restriction on axis

arrangement as imposed in the case of normal tandem control is imposed. No particular restriction is

imposed on axis synchronous control.

-

Axis selection on the screen display

On a screen such as the current position display screen, a slave axis is also displayed. The display of a

slave axis can be disabled by setting bit 0 (NDP) of parameter No. 3115 to 1 and setting bit 1 (NDA) of

parameter No. 3115 to 1.

-

Axis selection in actual cutting feedrate display

By setting bit 2 (SAF) of parameter No. 8303 to 1 for a slave axis, the slave axis can be included in an

actual cutting feedrate display calculation during synchronous operation.

-

Axis synchronous control with an absolute-position detector

When bit 7 (SMA) of parameter No. 8302 is set to 1 to attach an absolute-position detector, and bit 4

(APZ) of parameter No. 1815 for an axis placed in synchronous operation is turned off, APZ for the axis

(axes) placed together in synchronous operation is also turned off.

-

Slave axis mirror image

By setting parameter No. 8312, a mirror image can be applied to a slave axis placed in synchronous

operation. When the mirror image function is enabled, the direction in which the absolute and relative

coordinates change is the same as for the machine coordinates.

At this time, synchronization establishment, synchronization error check, and correction mode cannot be

used.

The mirror image set by bit 0 (MIR) of parameter No. 0012 cannot be applied to the slave axis. Because

this mirror image differs from the mirror image set by parameter MIR, it does not affect input signal MIx

<G106> or output signal MMIx <F108>.

-

External machine coordinate system shift

Bit 7 (SYE) of parameter No. 8304 can be set to 1 for the slave axis to shift the slave axis by the same

amount as specified for the master axis when external machine coordinate system shift is specified by

external data input/output for the master axis in synchronous control.

-

Manual operation to slave axis

The move command cannot be performed to the slave axis in axis synchronous control with manual

operation (JOG feed, HANDLE feed, etc.).

- 270 -

17.AXIS CONTROL FUNCTIONS PROGRAMMING

B-64304EN/02

NOTE

When the grid position difference between the master axis and slave axis is

large, a reference position shift can occur, depending on the timing of the *DEC

signal set to 1. In the example below, the shift along the slave axis is so large

that the position shifted one grid point from the actual reference position is

regarded as the reference position.

(Example) When the reference position on the slave axis is shifted one grid point

*DEC

Master axis feedrate

Master axis grid

Actual reference position

Slave axis feedrate

Slave axis grid

Actual reference position

Stop at position shifted one

grid point

In such a case, match the grid position according to Subsection 17.1.3,

"Automatic Setting for Grid Position Matching."

-

Synchronous establishment based on absolute position detection

When an absolute-position detector is used as the position detector, the machine positions on the master

axis and slave axis are found at power-up time for automatic establish synchronization.

-

Synchronous establishment after emergency stop cancellation, etc.

Synchronous establishment is also performed when servo position control is turned on, for example, at

emergency stop cancellation, servo alarm cancellation, or servo-off cancellation time.

However, synchronous establishment is not performed at the time of axis removal cancellation. So,

synchronous establishment based on manual reference position return operation is required as in the case

of power-up time.

-

One-direction synchronous establishment

Synchronous establishment can be performed by setting bit 0 (SSO) of parameter No. 8305 to 1 to move

the machine in one direction along the master axis and slave axis. The move direction depends on the

reference position setting based on bit 0 (SSA) of parameter No. 8304. When SSA = 0, for example, the

machine coordinate on the master axis or slave axis, whichever larger, is used as the reference point. So,

the machine moves in the + direction along the axes.

When bit 1 (SSE) of parameter No. 8305 is set to 1, normal synchronous establishment is performed

instead of one-direction synchronous establishment after an emergency stop.

17.1.3 Automatic Setting for Grid Position Matching

Explanation

Before axis synchronous control can be performed, the reference position on the master axis must be

matched with the reference position on the slave axis. With this function, the CNC automatically

matches the reference positions (grid positions) on the master axis and slave axis under axis synchronous

control.

- 272 -

B-64304EN/02

PROGRAMMING

17.AXIS CONTROL FUNCTIONS

17.1.6 Axis Synchronous Control Torque Difference Alarm

Explanation

If a movement made along the master axis differs from a movement made along the slave axis during axis

synchronous control, the machine can be damaged. To prevent such damage, the torque command

difference between the two axes is observed. If the difference is abnormal, a servo alarm SV0420 can be

issued.

Position gain

Master axis

+

torque command

Feedrate

Kp

control

Master axis

-

position

command

Master axis

position feedback

Torque command

+

Compare absolute

difference

value with threshold

Alarm detection

Position gain

-

+

Feedrate

Kp

control

Slave axis torque

Slave axis

-

command

position

command

Slave axis

position feedback

Fig. 17.1.6 (a) System configuration

[Method of use]

Specify the threshold parameter No. 2031 according to the procedure below.

1.

Set 0 in parameter No. 2031, and disable the torque difference alarm detection function.

2.

To check the absolute value of the torque difference between the synchronous axes, set the

parameters below. Set the same value for the two axes placed under axis synchronous control.

Parameter No. 2115 = 0

Parameter No. 2151 is as described below.

• For the T series (2-path control system), set it to 434 if the setting of parameter No. 1023

is 1, 2, 5, 6, 9, 10… and to 6578 if it is 3, 4, 7, 8, 11, 12…

• For 1-path control system, set it to 434.

3.

Display the diagnostic screen by pressing the function key

then the [DGNOS] soft key.

Diagnose No. 0353 indicates the absolute value of the torque difference between the two axes.

4.

Read the absolute torque difference value presented when normal operation is being performed. In

the threshold parameter No. 2031, set a value obtained by adding some margin to the read absolute

value.

The absolute torque difference value can be observed with the Servo Guide.

-

Enabling/disabling of alarm detection

Alarm detection is enabled when the time set in parameter No. 8327 has elapsed after the servo ready

signal SA <F000.6> is set to 1. When the input signal NSYNCA <G059.7> is set to 1, alarm detection

is disabled.

- 275 -

Content      ..     8      9      10      11     ..