Content      ..     20      21      22      23     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 22

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

D Method of determining

Acceleration/deceleration is performed with the largest tangent

the tangent acceleration

acceleration/deceleration that does not exceed the 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).

The acceleration in N3 is 1414 mm/sec² . At this point, the acceleration

on the X-axis is equal to the set value (1000 mm/sec² ).

Tangent feedrate

20ms

1000mm/sec²

1200mm/sec²

1414mm/sec²

gradient

gradient

gradient

20ms

20ms

20ms

D Acceleration

Acceleration is performed so that the feedrate programmed for a block is

attained at the beginning of the block.

Feedrate

Speed control by bell-shaped acceleration/

deceleration beforeinterpolation

Programmed speed

Time

N1

N2

N3

N4

N5

610

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

D Deceleration

Deceleration starts in advance so that the feedrate programmed for a block

is attained at the beginning of the block.

Deceleration can be performed over several blocks.

Feedrate

Speed control by

Deceleration

bell-shapedacceleration/

start point

deceleration before

interpolation

Programmed speed

Deceleration

start point

Time

D Deceleration based on a

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

distance

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.

D Single-block commands

If a single-block command is executed during look-ahead bell-shaped

during look-ahead

acceleration/deceleration control, the following control is applied.

bell-shaped

(1) If acceleration/deceleration is performed when the single-block

acceleration/deceleration

command is executed

before interpolation

(a) If A + B v Remaining amount of travel in the block executed

control

when the single-block command is executed

Deceleration is performed for a stop so that the feedrate falls to

zero at the point at which the block executed when the

single-block command was executed terminates.

Feedrate

Single-block command

##

""

### """

#A#

""

B

""

###

"""#

###

"""###

Time

A: Amount of travel to a point where the target feedrate is

attained and the current acceleration/deceleration ends

B: Amount of travel corresponding to deceleration from the

feedrate attained at the end of acceleration/deceleration to 0

611

22.

RISC PROCESSOR

PROGRAMMING

B-63534EN/02

(b) If A + B > Remaining amount of travel in the block being

executed when the single-block command is executed

A stop state may continue over several blocks.

The stop is made as described later.

Feedrate

Single-block command

%$$

Stop state continuing over multiple blocks

%%%$$

%%%$$

B$

%%A%

$

%%%$$""

Time

%%%$$"""

A: Amount of travel to a point where the target feedrate is

attained and the current acceleration/deceleration ends

B: Amount of travel corresponding to deceleration from the

feedrate attained at the end of acceleration/deceleration to 0

(2)

If acceleration/deceleration is not performed when the single-block

command is executed

(a) AvRemaining amount of travel in the block being executed

when the single-block command is executed

Movement is decelerated and stopped so that the feedrate falls to

zero at the end of the block which was being executed when the

single-block command was executed.

Feedrate

Single-block command

%%

%%%

%%%

A

%

%%%"

%%%"""

Time

A: Amount of travel corresponding to deceleration from the

current feedrate to 0

612

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

(b) If A > Remaining amount of travel in the block being executed

when the single-block command is executed

A stop state may continue over several blocks.

The stop is made as described later.

Feedrate

Single-block command

##

Stop state continuing over multiple blocks

###

####

##A##

###&&

Time

###&&&

A: Amount of travel corresponding to deceleration from the

current feedrate to 0

(3) Stopping a movement if the stop may continue over several blocks

Acceleration/deceleration is performed over several blocks to

decrease the feedrate to zero.

Feedrate

Single-block command

Time

In AI High Precision Countour Control mode, the feedrate is

22.1.2

automatically controlled by the reading-ahead of blocks.

Automatic Feedrate

The feedrate is determined using the following conditions. If the

Control Function

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

613

22.

RISC PROCESSOR

PROGRAMMING

B-63534EN/02

(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 assumed

difference in feedrate.

when Al High Precision

Contour Control is not

used

Tool path assumed

when Al High Precision

Contour Control is used

The machining error is decreased

because of the deceleration with

the acceleration.

Fig. 22.1.2 (a)

To enable this function, set the desired values for the following

parameters:

Parameter No. 8410:

Permissible feedrate difference used when the feedrate is to be

determined from the feedrate difference at a corner

Parameter No. 8470:

Permissible acceleration when the feedrate is to be determined

from the acceleration

For details, see the explanation of these parameters.

D Feedrate control

In automatic feedrate control mode, the feedrate is controlled as described

conditions

below:

(a) From the feedrate difference on each axis at a corner, the feedrate

in the corner is determined, and deceleration is performed to

achieve the feedrate at the corner.

(Example)

N1

Specified

Y

F

N2

X

N1

N2

N3

t

N3

(b) From the acceleration on each axis at the corners at the start and

end points of each block, the feedrate in the block is determined,

and deceleration is performed so that the feedrate in the block is

equal to or less than the determined feedrate.

(Example)

N2 N3

N1

N4

Y

Specified

feedrate

N5

X

N8

N6

N1

N2 N3 N6 N7

N8

t

N7

614

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

(c) During descent on the Z-axis, the cutting load increases, and

override is applied according to the Z-axis descent angle.

(Example)

N1

Z

N2

Specified

feedrate

X

N1

N2

N3

t

N3

Deceleration based on

With look-ahead acceleration/deceleration before interpolation, the

the feedrate difference at

tangent feedrate is changed smoothly. Thus, no path error occurs due to

a corner

acceleration/deceleration delay. With this acceleration/declaration,

however, acceleration/deceleration is not performed for any feedrate

change on any axis that may be made where the travel direction changes.

By using the function for deceleration based on the feedrate difference at

a corner, if a feedrate change occurs on an 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. 8410

does not occur, and deceleration is automatically performed.

615

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

(Example)

Program

N1 G01 G91 X100. F5000

N2 Y100.

N2

N1

Tangent feedrate

Tangent feedrate

The deceleration

based on the feedrate

difference is used.

X-axis feedrate

X-axis feedrate

The feedrate difference becomes

The tangent feedrate is

small, and the feedrate on each

smooth, but the feedrate

axis becomes smooth.

on each axis is not.

Y-axis feedrate

Y-axis feedrate

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. 8410 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.

616

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

(Example)

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

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

Deceleration to

Deceleration to

354 mm/min

500 mm/min

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 or acceleration may be up to 30% lower than that

determined if 0 is set.

(Example)

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

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

Deceleration to

Deceleration to

354 mm/min

354 mm/min

Example of determining

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

the feedrate with the

shown in the figure below, the feedrate differences on each axis at the

individual corners are not very large. Thus, deceleration with the feedrate

acceleration on each

differences is not effective. Consecutive small feedrate differences,

axis

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. 8470.

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.

D Example

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.

617

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

N8

N7

N9

N6

N5

Y

N1

N4

X

N3

N2

X-axis

feedrate

Y-axis

feedrate

Tangent

feedrate

N1

N5

N9

N1

N5

N9

Fig. 22.1.2 (b) Example of Determining the Feedrate with the Acceleration

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. 8470 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.

(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

618

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

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.

Example of determining

This function is enabled when parameter ZAG (bit 4 of No. 8451) is set

the feedrate with the

to 1.

cutting load

((((

((((((

((((((

’((((((’

’’’’’’’’

’’’’’’’’

Fig. 22.1.2 (c) During ascent on the Z-axis

q

(((((

((((((

’((((((’

’’’’’’’’

’’’’’’’’

Fig. 22.1.2 (d) During descent on the Z-axis

619

22.

RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Usually, the cutting resistance is higher when machining is performed

with the bottom of the cutter, as shown in Fig. 22.1.2 (c) an when

machining is performed with the side of the cutter, as shown in Fig. 22.1.2

(d). Deceleration is, therefore, required. In AI High Precision Countour

Control, the tool travel direction on the Z-axis is used as a condition for

calculating the machining feedrate.

The descent angle during descent on the Z-axis (angle formed by the XY

plane and the tool center path) is as shown in Fig. 22.1.2 (d). The descent

angle is divided into four areas, and the override values for the individual

areas are set for the following parameters:

Parameter No. 8456 for area 2

Parameter No. 8457 for area 3

Parameter No. 8458 for area 4

For area 1, however, no parameter is available, and an override of 100%

is used at all times. The feedrate obtained according to other feedrate

control is multiplied by the override value of the area to which descent

angle belongs.

Area1

0°v q <30°

Area2

30°v q <45°

Area3

45°v q <60°

Area4

60°v q v90°

Z

XY plane

30°

Area1

90°

60°

Area4

45°

Area2

Area3

620

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

CAUTION

1

The function for determining the feedrate 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 function for determining the feedrate 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 function for determining the feedrate with the cutting

load, do not use these functions.

3

When performing three-dimensional coordinate conversion,

determine the descent angle on the Z-axis using the

converted coordinate system.

Ignoring F code

In a block in which automatic feedrate control is enabled, all feed

commands

commands (F commands) can be ignored by setting parameter NOF (bit

7 of No. 8451). The term feed commands, as used here, refer to the

following commands:

(1) Modal F commands before the block in which automatic feedrate

control is enabled

(2) F commands and modal F commands in the block in which automatic

feedrate control is enabled

When the F 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 automatic feedrate control 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 automatic

feedrate control.

Override to a determined

The following gives the specifications of override to a feedrate

feedrate

determined by functions such as deceleration based on feedrate difference

in look-ahead acceleration/deceleration before interpolation and

deceleration based on acceleration rate in AI High Precision Countour

Control.

- When bit 3 (OVR) of parameter No. 8459 = 0

The conventional specifications apply.

Override is invalid for deceleration functions such as deceleration

based on feedrate difference and deceleration based on acceleration

rate.

- When bit 3 (OVR) of parameter No. 8459 = 1

Override is valid for deceleration functions such as deceleration based

on feedrate difference and deceleration based on acceleration rate.

621

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

D Restriction -5

When the following function is used, a AI High Precision Contour

Control and the AI Nano High Precision Contour Control cannot be used.

S Angular axis control

S Arbitary angular axis control

D Restriction -6

The limitation may be attached about the combination of the NC

instructions occasionaly.

Refer the description of the each functions.

NOTE

1

If the permissible acceleration set for one axis is two or more times

greater than that set for another, the feedrate may decrease

temporarily at those corners where the travel direction changes

abruptly.

2

If the machine lock signal is turned on during travel in look-ahead

acceleration/deceleration before interpolation mode, the machine

enters the machine lock state after the end of deceleration.

3

If there is a block with no travel or a one-shot G code command

such as G04 in look-ahead acceleration/deceleration before

interpolation mode, deceleration is performed for a stop in the

preceding block.

4

If the dry run signal changes from “0” to “1” or from “1” to “0” during

travel on an axis, acceleration/deceleration is performed to achieve

the prescribed feedrate without deceleration to feedrate 0.

The function for deceleration with the feedrate difference at a

corner is effective even during dry run.

22.1.4

The Function List

which Can be Used

Item

Specifications

Note

Axis control

Controlled axes

3 axes

Controlled paths

1-path

Simultaneously controlled axes

2 axes

Controlled axis expansion

Up to 8 axes

Simultaneously controlled axis expan-

Up to 6 axes

sion

625

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Axis control

Axis control by PMC

The axis which is used in the AI High

Precision Contour Control mode or in

the AI nano High Precision Contour

Control mode can not be used as the

control axis of the PMC Axis Control in

the AI High Precision Contour Control

mode or in the AI nano High Precision

Contour Control mode

Cs contour control

The nano interpolation and the Ad-

vanced preview feed-forward function

are canceled once when the command

for Cs axis in AI high precision contour

control mode or AI nano high precision

contour control mode

Axis name

3 basic axes: X,Y,Z; Additional axes:

U,V,W,A,B, or C

Twin table control

Synchronized operation/individual op-

eration/a normal drive cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode

Please include all the twin table control

axes to the maximum control axis

number (parameter No.7510) of RISC.

Simple synchronous control

Synchronized operation/individual op-

eration/a normal drive cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode

Please include all the simple synchro-

nous control axes to the maximum

control axis number (parameter

No.7510) of RISC.

Least input increment

0.001mm,0.001deg,0.0001inch

Incremental System 1/10

0.0001mm,0.0001deg,0.00001inch

Inch/metric conversion

Inch mode / metric mode cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode.

Interlock

All axes/each axis

Machine lock

All axes/each axis

Emergency stop

Stored stroke check 1

The stroke limit cannot be set by the

stroke limit external setting signal in

the AI high precision contour control

mode or in the AI nano high precision

contour control mode. Overrun on the

OT limit does not occur in the AI high

precision contour control mode or in

the AI nano high precision contour

control mode.

626

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Axis control

Stored stroke check 2

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if G22 or G23 is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode,

Mirror image

Do not change the state of the signal in

the AI High Precision Contour Control

mode or AI nano High Precision Con-

tour Control mode.

Backlash compensation for each rapid

traverse and cutting feed

Operation

Automatic operation

MDI operation

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if the MDI operation is used in

the AI high Precision Contour Control

mode or in the AI high Precision Con-

tour Control mode. At this time,

G05P10000 or G05P0 can not be used

by the MDI operation.

Cycle start/Feed hold

Program stop/Program end

Reset

Program restart

Program restart function can not be

used in NURBS interpolation, smooth

interpolation, and cylindrical interpola-

tion.

Dry run

Single block

Interpolation functions

Positioning

G00

The AI high precision contour control

function or AI nano high precision con-

tour control functions except the ad-

vanced preview feed-forward function,

multi buffer function , and the nano in-

terpolation become invalid.

Exact stop mode

G61

Exact stop

G09

Cutting mode

G64

627

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Interpolation functions

Linear interpolation

G01

Circular interpolation

G02,G03

Helical interpolation

(Circular interpolation) + (Linear inter-

polation for up to 2 axes)

Helical interpolation B

(Circular interpolation) + (Linear inter-

polation for up to 4 axes)

Involute interpolation

G02.2,G03.2

3-dimensional circular interpolation

G02.4,G03.4

The position is checked at the end

point of the block which cancel 3 di-

mensional circular interpolation or at

the end point of the previous block of

the 3 dimensional circular interpolation

if 3 dimensional circular interpolation is

used except in AI high precision con-

tour control mode or AI nano high pre-

cision contour control mode.

Smooth interpolation

G05.1

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

NURBS interpolation

G06.2

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

Cylindrical interpolation

G07.1

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

Cylindrical interpolation cutting point

G07.1

This function can be used in AI high

control

precision contour control mode or AI

nano high precision contour control

mode.

Conical / spiral interpolation

G02,G03

Feed functions

Feed per minute

G94

Cutting feedrate clamp

Linear acceleration/deceleration of cut-

ting feed after interpolation

Bell-type acceleration/deceleration of

cutting feed after interpolation

Feedrate override

0 to 254%

(1% step)

2nd. Feedrate override

0 to 254%

(1% step)

628

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Feed functions

F1 digit feed

Using the manual pulse generator can

not change Feedrate.

Inverse time feed

G93

External deceleration

External deceleration

Look ahead liner-type acceleration/

deceleration before interpolation.

Look ahead Bell-type acceleration/

Acceleration change time constant

deceleration before interpolation

type

Program input

Tape code

Automatic recognition of EIA/ISO

Program format

Word address format

Control in/out

Optional block skip

Absolute/incremental programming

G90/G91

Input unit 10 time multiply

Plane selection

G17,G18,G19

Rotary axis roll over

Workpiece coordinate system selec-

G54 to G59

The AI high precision contour control

tion

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Addition of workpiece coordinate sys-

48 sets / 300 sets

The AI high precision contour control

tem pair

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Manual absolute ON/OFF

Programmable parameter input

G10

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

629

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Program input

External memory and sub program

M198

calling function

Subprogram call

M98

Circular interpolation by R program-

ming

Scaling

G50,G51

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in scaling mode by set-

ting the parameter.

The alarm (P/S5012) occurs if the

mode of AI high precision contour con-

trol or of AI nano high precision con-

tour control is changed in scaling mode

(G51) when the parameter is not set.

The scaling mirror image by a negative

magnification can not be done.

Coordinate system rotation

G68,G69

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in coordinate system

rotation mode by setting the parameter.

The alarm (P/S5012) occurs if the

mode of AI high precision contour con-

trol or of AI nano high precision con-

tour control is changed in coordinate

system rotation mode (G51) when the

parameter is not set.

3-dimensional coordinate system con-

G68,G69

The mode of AI high precision contour

version

control or of AI nano high precision

contour control is permitted to change

ON and OFF in 3-dimensional coordi-

nate system conversion mode by set-

ting the parameter. The alarm

(P/S5012) occurs if the mode of AI

high precision contour control or of AI

nano high precision contour control is

changed in 3-dimensional coordinate

system conversion when the parame-

ter is not set.

Miscellaneous/spindle functions

Miscellaneous function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

630

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Miscellaneous/spindle functions

2nd. Auxiliary function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

1 block plural M commands

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

It is possible to command up to 3.

Spindle speed function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Tool functions

Tool function (T8-digit)

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Tool retract & recover

G10.6

Issue the G10.6 command prior to the

G05 P10000 command that causes

the system to enter AI high precision

contour control or AI nano contour con-

trol mode. The alarm (P/S 5000) oc-

curs if it is issued in this mode.

Tool length compensation

G43

Cutter compensation C

G38,G39,G40,G41,G42

The buffering is inhibited when the

command which automatically cancel

AI high precision contour control mode

or AI nano high precision contour con-

trol mode is used.

So the tool offset vector is held.

631

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Tool functions

3-dimensional tool compensation

G41.2,G42.2

The command which automatically

G41.3

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Tool axis direction tool length com-

G43.1

The command which automatically

pensation

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Tool center point control

G43.4,G43.5

The command which automatically

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Rotary table dynamic fixture offset

G54.2

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in rotary table dynamic

fixture offset mode by setting the pa-

rameter. The alarm (P/S5012) occurs if

the mode of AI high precision contour

control or of AI nano high precision

contour control is changed in rotary

table dynamic fixture offset mode when

the parameter is not set.

632

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

22.2

CYLINDRICAL

INTERPOLATION

CUTTING POINT

CONTROL (G07.1)

General

The conventional cylindrical interpolation function controls the tool

center so that the tool axis always moves along a specified path on the

cylindrical surface, towards the rotation axis (cylindrical axis) of the

workpiece. On the other hand, this function controls the tool so that the

tangents to the tool and a contour figure cutting surface always pass

through the rotation center of a workpiece

As shown in Fig.22.2 (a), control is exercised along the offset axis

(Y-axis) direction that is perpendicular to the tool, tool center axis, and

workpiece rotation center axis. Therefore, contour figure on the cutting

side can be assumed to be the same anytime without depending on the

amount of the cutter compensation.

This function can be used in AI high precision contour control mode or

in AI NANO high precision contour control mode.

Conventional cylindrical

Cylindrical interpolation based

interpolation

on this function

Rotation

Workpiece

Rotation

Cutting side

Cutting

side

Command Position

Y-axis

Command

Tool

Position

Tool

center

In the case of the amount of the

cutter compensation is large;

Workpiece

Rotation

Rotation

Cutting

Cutting

side

side

Y-axis

Command

Command

Position

Position

Shape on the cutting side changes de-

Shape on the cutting side does not de-

pending on the amount of cutter com-

pend on the amount of cutter com-

pensation because the tool path is

pensation by moving the Y axis.

compensated by moving the rotation

The cutting side is always vertical to

axis.

the cylinder.

Fig. 22.2 (a) Comparison with Conventional Interpolation

633

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Format

G05 P10000 ; Sets AI High precision contour control mode.

:

G07.1 IPr ;

Sets cylindrical interpolation mode.

:

..G41(G42)..

Sets cutter compensation mode.

:

..G40..

Clear cutter compensation mode.

:

G07.1 IP0 ;

Clears cylindrical interpolation mode.

G05 P0 ;

Clears AI high precison contour control mode.

IP

: One rotation axis address

r

: Cylinder radius of rotation axis

Specify each of G07.1 IPr; and G07.1 IP0; singly in a block.

Explanations

D Cutting point

compensation

(1) Cutting point compensation between blocks

As shown in Fig. 22.2 (b), cutting point compensation is achieved by

moving between blocks N1 and N2.

1) Let C1 and C2 be the heads of the vectors normal to N1 and N2

from S1, which is the intersection of the tool center paths of blocks

N1 and N2

2) After the tool moves to S1 according to the command of N1, the

tool moves through V on the C-axis as a result of cutting point

p

compensation, then through -V

r along the Y-axis.

180

Z-axis

V

: C-axis component of C1 - C2

C1 : Cutting surface of block N1

C2 : Cutting surface of block N2

S1

C2

Cutting surface

of block N2

C1

N1

Programmed path

N2

V

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (b) Cutting Point Compensation between Blocks

(2)

Cutting point compensation in a circular command block

As shown in

Fig. 22.2 (c), the movement required for cutting point compensation

is made simultaneously with circular interpolation in block N1.

634

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

1) Let C0 be the head of the vector normal to N1 from S0, which is

the tool center position at the start point of circular block N1. Let

C1 be the head of the similar vector at the end point.

2) As the tool moves from S0 to S1, a superimposed movement is

made by the C-axis component of (C1 - C2) (V in the figure) on

the C-axis, and a superimposed movement is made by

p

-V

r along the Y-axis. along the Y-axis. That is, the

180

following expressions are valid. As movement is made through

L as shown in

Fig. 22.2 (c), the superimposed movements are made on the C-axis

and Y-axis as follows:

DC + DV

p

DY + *

(DV)r

180

nV

: Cutting point compensation value (nV2 - nV1) for

movement of nL

nV1 : C-axis component of the vector normal to N1 from the

tool center of the start point of nL

nV2 : C-axis component of the vector normal to N1 from the

tool center of the end point of nL

R

: Arc radius

V

: C-axis component of C1 - C0

C0 : Cutting surface at the start

Z-axis

point of block N1

C1 : Cutting surface at the end point

of block N1

Tool center path

S1

C0

C1

nL

V

nV2

nV1

R

Programmed path

N1

C0

S0

O

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (c) Cutting Point Compensation in a Circular Command Block

(3) When cutting point compensation is not applied between blocks

When, as shown in Fig. 22.2 (d) and Fig. 22.2 (e), the cutting point

compensation value (V in the figures) is less than the value set in

parameter No. 6112, one of the operations below is performed. (The

operation that is performed depends on the setting of bit 6 (CYS) of

parameter No. 6004.

1) When bit 6 (CYS) of parameter No. 6004 is set to 1

Cutting point compensation is not applied between blocks N1 and

N2, but is applied when block N2 is executed.

635

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

V

: C-axis component of C2 - C1

Z-axis

C1 : Cutting surface of block N1

C2 : Cutting surface after the end of

block N1

Tool center path

S1

S2

C2

C1

N1

C2

N2

V

N3

Programmed path

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (d) When Bit 6 (CYS) of Parameter No. 6004 Is Set to 1

2) When bit 6 (CYS) of parameter No. 6004 is set to 0

Cutting point compensation is not performed between blocks N1

and N2. Whether to apply cutting point compensation between

block N2 and N3 is determined by taking the cutting point

compensation value between blocks N2 and N3 (V1 in the figure)

into consideration.

V

: C-axis component of C2 - C1

C1 : Cutting surface of blocks N1

Z-axis

and N2

C2 : Cutting surface at the end of

block N3

Tool center path

V

S1

S2

C1

C2

C1

N1

N2

N3

Programmed path

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (e) When Bit 6 (CYS) of Parameter No. 6004 Is 0

636

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

3) When the amount of travel (L1) of block N2 is less than the value

set in parameter No. 6113, as shown in Fig. 22.2 (f), cutting point

compensation is not applied between blocks N1 and N2. Instead,

block N2 is executed with the cutting point compensation of the

previous block. When the amount of travel (L2) of block N3 is

greater than the value set in parameter No. 6113, cutting point

compensation is applied between blocks N2 and N3.

V

: C-axis component of C2 - C1

C1 : Cutting surface of blocks N1 and N2

Z-axis

C2 : Cutting surface at the end of block N3

L1

V

L2

C1

C2

C1

Tool center path

N2

N1

N3

Programmed path

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (f) When the Amount of Travel (L1) of Block N2 Is Less Than the

Parameter Value

4) When, as shown in Fig. 22.2 (g), the diameter of an arc (R in the

figure) is less than the value set in parameter No. 6113, cutting

point compensation is not applied simultaneously with circular

interpolation

637

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

V

: Cutting point compensation between

blocks N2 and N3

C1 : Cutting surface of blocks N1 and N2

Z-axis

C2 : Cutting surface of block N3

L1

V

R

S2

N2

S1

C1

C2

N3

C1

Tool center path

N1

Programmed path

C-axis on the

Y-axis

cylindrical surface

Fig. 22.2 (g) When the Diameter of an Arc Is Less Than the Parameter

Value

D Feedrate during cutting

point compensation

(1)

The tool moves at a specified feedrate while cutting point

compensation is being applied between blocks.

(2)

The actual speed indication and feedrate during circular interpolation

are as described below.

Actual speed indication

The speed component of each axis after cutting point compensation

at a point in time during circular interpolation is as follows:

Fz’=Fz

- - - Speed component of linear axis

Fc’=Fc+(Vce-Vcs)

- - - Speed component of rotation axis

p

r

Fy’=-(Vce-Vcs)

– - - Speed component of offset axis

180

Fz : Speed component of a cylindrical interpolation linear axis

before cutting point compensation

Fc : Speed component of cylindrical interpolation rotation axis

before cutting point compensation

Vcs: Rotation axis component of a tool contact point vector (Vs

in the figure) at the start point at a point in time

Vce: Rotation axis component of tool contact point vector (Ve in

the figure) at the end point at a point in time

r :

Radius of the cylinder of a rotation axis

Accordingly, the actual speed indication during circular

interpolation is greater than the specified value when |Fc’| >

|Fc|(inner offset of the arc). Conversely, the actual speed

indication during circular interpolation is less than the

specified value when |Fc’| < |Fc|(outer offset of the arc).

638

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Z-axis

Fc’

Programmed path

Tool center path

Ve

Tool

Vce

Fz = Fz’

Vs

Vcs

Fc

C-axis

Y-axis

Fig. 22.2 (h) Actual Speed Indication during Circular Interpolation

D Usable G codes

(1) In any of the following G code modes, cylindrical interpolation

cutting point compensation can be specified:

G17,G18,G19 : Plane selection

G22

: Stored stroke check function on

G64

: Cutting mode

G90,G91

: Absolute command programming, incremental

command programming

G94

: Feed per minute

(2) Any of the following G codes can be specified in cylindrical

interpolation cutting point compensation mode:

G01,G02 ,G03 : Linear interpolation, circular interpolation

G04

: Dwell

G40,G41,G42 : Cutter compensation

G40.1-G42.

: Normal direction control

G64

: Cutting mode

G65-G67

: Macro call

G90,G91

: Absolute command programming, incremental

command programming

D Parameter

Set to use this function as parameter CYA (No.19530#5)=1.

Limitation

D Overcutting during inner

Theoretically, when the inner area of a corner is cut using linear

corner cutting

interpolation as shown in Fig. 22.2 (i), this function slightly overcuts the

inner walls of the corner. This overcutting can be avoided by specifying

a value of R that is slightly greater than the radius of the tool at the corner.

639

Content      ..     20      21      22      23     ..