Content      ..     15      16      17      18     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 17

16.

PATTERN DATA INPUT

FUNCTION

PROGRAMMING

B-63534EN/02

Table 16.3 (b) Numbers of subprograms employed in the pattern data input function

Subprogram No.

Function

O9500

Specifies character strings displayed on the pattern data menu.

O9501

Specifies a character string of the pattern data corresponding to pattern No.1

O9502

Specifies a character string of the pattern data corresponding to pattern No.2

O9503

Specifies a character string of the pattern data corresponding to pattern No.3

O9504

Specifies a character string of the pattern data corresponding to pattern No.4

O9505

Specifies a character string of the pattern data corresponding to pattern No.5

O9506

Specifies a character string of the pattern data corresponding to pattern No.6

O9507

Specifies a character string of the pattern data corresponding to pattern No.7

O9508

Specifies a character string of the pattern data corresponding to pattern No.8

O9509

Specifies a character string of the pattern data corresponding to pattern No.9

O9510

Specifies a character string of the pattern data corresponding to pattern No.10

Table. 16.3 (c) Macro instructions used in the pattern data input function

G code

H code

Function

G65

H90

Specifies the menu title.

G65

H91

Specifies the pattern name.

G65

H92

Specifies the pattern data title.

G65

G93

Specifies the variable name.

G65

H94

Specifies the comment.

Table. 16.3 (d) System variables employed in the pattern data input function

System variable

Function

#5900

Pattern No. selected by user.

460

17. PROGRAMMABLE PARAMETER

B-63534EN/02

PROGRAMMING

ENTRY (G10)

PROGRAMMABLE PARAMETER ENTRY (G10)

17

General

The values of parameters can be entered in a lprogram. This function is

used for setting pitch error compensation data when attachments are

changed or the maximum cutting feedrate or cutting time constants are

changed to meet changing machining conditions.

Format

Format

G10L50; Parameter entry mode setting

N_R_; For parameters other than the axis type

N_P_R_; For axis type parameters

G11; Parameter entry mode cancel

Meaning of command

N_: Parameter No. (4digids) or compensation position No. for pitch errors

compensation +10,000 (5digid)

R_: Parameter setting value (Leading zeros can be omitted.)

P_: Axis No. 1 to 8 (Used for entering axis type parameters)

Explanations

D Parameter setting

Do not use a decimal point in a value set in a parameter (R_).

value (R_)

a decimal point cannot be used in a custom macro variable for R_either.

D Axis No.(P_)

Specify an axis number (P_) from 1 to 8 (up to eight axes) for an axis type

parameter. The control axes are numbered in the order in which they are

displayed on theCNC display.

For example, specity P2 for the control axis which is displayed second.

WARNING

1

Do not fail to perform reference point return manually after

changing the pitch error compensation data or backlash

compensation data. Without this, the machine position can

deviate from the correct position.

2

The canned-cycle mode must be cancelled before entering

of parameters. When not cancelled, the drilling motion may

be activated.

NOTE

Other NC statements cannot be specified while in

parameter input mode.

461

17. PROGRAMMABLE PARAMETER

ENTRY (G10)

PROGRAMMING

B-63534EN/02

Examples

1. Set bit 2 (SBP) of bit type parameter No. 3404

G10L50 ;

Parameter entry mode

N3404 R 00000100 ;

SBP setting

G11 ;

cancel parameter entry mode

2. Change the values for the Z-axis (3rd axis) and A-axis (4th axis) in

axis type parameter No. 1322 (the coordinates of stored stroke limit

2 in the positive direction for each axis).

G10L50 ;

Parameter entry mode

N1322P3R4500 ;

Modify Z axis

N1322P4R12000 ;

Modify A axis

G11 ;

cancel parameter entry mode

462

18. MEMORY OPERATION USING

PROGRAMMING

FS15 TAPE FORMAT

B-63534EN/02

MEMORY OPERATION USING FS15 TAPE FORMAT

18

General

Memory operation of the program registered by FS15 tape format is

possible with setting of the setting parameter (No. 0001#1).

Explanations

Data formats for cutter compensation, subprogram calling, and canned

cycles are different between the Series 16/18 and Series 15. The Series

15 data formats can be processed for memory operation.Other data

formats must comply with the Series 16/18.When a value out of the

specified range for the Series 16/18 is registered, an alarm occurs.

Functions not available in the Series 16/18 cannot be registered or used

for memory operation.

D Address for the cutter

Offset numbers are specified by address D in the Series 15. When an

compensation offset

offset number is specified by address D, the modal value specified by

number

address H is replaced with the offset number specified by address D.

D Subprogram call

If a subprogram number of more than four digits is specified, the four

low-order digits are regarded as the subprogram number. If no repeat

count is specified, 1 is assumed.

Table 18 (a) Subprogram call data format

CNC

Data format

Series 15

M98 Pfffff Lffff ;

P : Subprogram number

L : Repetition count (1 to 9999)

Series 16/18

M98 Pffff jjjj ;

Repetition count Subprogram number

(1 to 9999)

D Address for the canned

The Series 15 and Series 16/18 use different addresses for the repeat count

cycle repetition count

for canned cycles as listed in Table 18 (b).

Table 18 (b) Address for times of repetition of canned cycle

CNC

Address

Series 15

L

Series 16/18

K

463

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

19.1

HIGH-SPEED CYCLE

CUTTING

General

This function can convert the machining profile to a data group that can

be distributed as pulses at high-speed by the macro compiler and macro

executor. The function can also call and execute the data group as a

machining cycle using the CNC command (G05 command).

Format

G05 P10fff Lfff ;

P10fff is number of the machining cycle to be called first:

P10001 to P10999

Lfff is repetition count of the machining cycle

(L1 applies when this parameter is omitted.) :

L1 to L999

Call and execute the data for the high speed cutting cycle specified by the

macro compiler and macro executor using the above command.

Cycle data can be prepared for up to 999 cycles. Select the machining

cycle by address P. More than one cycle can be called and executed in

series using the cycle connection data in the header.

Specify the repetition count of the called machining cycle by address L.

The repetition count in the header can be specified for each cycle.

The connection of cycles and their repetition count are explained below

with an example.

Example) Assume the following:

Cycle 1 Cycle connection data 2 Repetition count 1

Cycle 2 Cycle connection data 3 Repetition count 3

Cycle 3 Cycle connection data 0 Repetition count 1

G05 P10001 L2 ;

The following cycles are executed in sequence:

Cycles 1, 2, 2, 2, 3, 1, 2, 2, 2, and3

NOTE

1

An alarm is issued if the function is executed in the G41/G42

mode.

2

Single block stop, dry run/feedrate override, automatic

acceleration/deceleration and handle interruption are

disabled during high-speed cycle machining.

465

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

Alarms

Alarm

Descriptions

number

115

The contents of the header are invalid. This alarm is issued in

the following cases.

1. The header corresponding to the number of the specified call

machining cycle was not found.

2. A cycle connection data value is not in the valid range (0 to

999).

3. The number of data items in the header is not in the valid

range (1 to 32767).

4. The first variable No. for storing data in the executable format

is not in the valid range (#20000 to #85535).

5. The last variable No. for storing data in the executable format

exceeds the limit (#85535).

6. The first variable No. for start data in the executable format

overlaps with a variable No. used in the header.

178

High-speed cycle machining was specified in the G41/G42

mode.

179

The number of control axes specified in parameter 7510 ex-

ceeds the maximum number.

466

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

When an arc is cut at a high speed in circular interpolation, a radial error

19.2

exists between the actual tool path and the programmed arc. An

FEEDRATE

approximation of this error can be obtained from the following

CLAMPING BY ARC

expression:

RADIUS

Y

∆r:Error

Programmed path

Actual path

r

0

X

1

v²

∆r=

(T₁

²+T₂₂)

2

r

∆r

:

Maximum radial error (mm)

v

:

Feedrate (mm/s)

r

:

Arc radius (mm)

T1 : Time constant (s) for exponential acceleration/deceleration of

cutting feed

T₂

:

Time constant of the servo motor (s)

When actual machining is performed, radius r of the arc to be machined

and permissible error Dr are given. Then, maximum allowable feedrate

v (mm/min) is determined from the above expression.

The function for clamping the feedrate by the arc radius automatically

clamps the feedrate of arc cutting to the value set in a parameter. This

function is effective when the specified feedrate may cause the radial

error for an arc with a programmed radius to exceed the permissible

degree of error.

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

builder.

467

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

A remote buffer can continuously supply a large amount of data to the

19.3

CNC at high speeds when connected to the host computer or input/output

HIGH-SPEED

equipment via a serial interface.

REMOTE BUFFER

RS-232-C / RS-422

Host

Remote

computer

CNC

buffer

Input/output

equipment

When the remote buffer is connected online to the host computer, fast and

reliable DNC operation is possible.

The remote buffer function includes high-speed remote buffer A and

high-speed remote buffer B for high-speed machining. High-speed

remote buffer A uses binary data. High-speed remote buffer B uses NC

language. For details on remote buffer specifications, refer to the

“Remote Buffer Supplement” (B-61802E-1).

19.3.1

Specify G05 only in a block using normal NC command format. Then

specify move data in the special format explained below. When zero is

High-Speed Remote

specified as the travel distance along all axes, normal NC command

Buffer A (G05)

format can be used again for subsequent command specification.

CNC

Remote buffer

RS-232-C / RS-422

Host computer

468

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

Format

VBinary input operation enabled : G05;

VBinary input operation disabled : The travel distance along

all axes are set to zero.

VData format for binary input operation

Byte

High byte

1st axis

Low byte

Data

sequence

High byte

2nd axis

Low byte

L

High byte

Nth axis

Low byte

Check byte

In the data format for binary input operation, the travel distance

along each axis (2 bytes) per unit time is specified. The travel dis-

tances along all axes are placed sequentially from the first axis,

then a check byte is added. (The data length for one block is [2 x N

+ 1] bytes).

All data must be specified in binary.

Explanations

D Selecting the unit time

The unit time (in ms) can be selected by setting bits 4, 5, and 6 of

parameter IT0,IT1,IT2 No. 7501.

D Travel distance data

The following unit is used for specifying the travel distance along each

axis.

(A negative travel distance is indicated in 2’s complement.)

Increment system

IS-B

IS-C

Unit

Millimeter machine

0.001

0.0001

mm

Inch machine

0.0001

0.00001

inch

The data format of the travel distance is as follows. The bits marked * are

used to specify a travel distance per unit time.

469

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

15

14

13

12

11

10

9

8

7

6

5

4

3

2

1

0

0

0

Example: When the travel distance is 700 µm per unit time

(millimeter machine with increment system IS-B)

15

14

13

12

11

10

9

8

7

6

5

4

3

2

1

0

0

0

0

0

1

0

1

0

0

1

1

1

1

0

0

0

D Check Byte

All bytes of the block except for the check byte ([2*N] bytes) are summed

up, and any bits above 8th bit are discarded.

D Transfer speed

The CNC reads (2 x N + 1)-byte data (where N is the number of axes) for

every unit time that is set in the parameter. To allow the CNC to continue

machining without interruption, the following minimum baud rate is

required for data transfer between the host and remote buffer:

11

(2×N+1) ×

× 1000 baud (T : Unit time)

T

D Cutter compensation

If G05 is specified in cutter compensation mode, the P/S 178 alarm is

issued.

D Feed hold and interlock

Feed hold and interlock are effective.

D Mirror image

The mirror image function (programmable mirror image and setting

mirror image) cannot be turned on or off in the G05 mode.

D Acceleration /

In binary input operation mode, when tool movement starts and stops in

deceleration type

cutting feed mode, exponential acceleration/deceleration is performed

(the acceleration/deceleration time constant set in parameter No. 1622 is

used).

Limitations

D Modal command

In binary input operation mode, only linear interpolation as specified in

the defined data format is executed (equivalent to the incremental

command for linear interpolation).

D Invalid functions

The single block, feedrate override, and maximum cutting feedrate clamp

functions have no effect. The program restart, block restart, and

high-speed machining functions cannot be used. In addition, miscella-

neous functions cannot be executed in binary operation.

D Memory registration

No data can be stored in memory.

470

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

19.3.2

High-speed remote buffer A uses binary data. On the other hand,

high-speed remote buffer B can directly use NC language coded with

High-Speed Remote

equipment such as an automatic programming unit to perform high-speed

Buffer B (G05)

machining.

Format

G05P01 ; Start high-speed machining

G05P00 ; End high-speed machining

Example :

O1234 ;

L

G05P01 ; ← Start high-speed machining

X_ Y_ Z_ ;

L

G05P00 ; ← End high-speed machining

L

M02 ;

Explanations

D Specified data

The following data can be specified during high-speed machining:

Address

Data

X

Travel distance along the X-axis

Y

Travel distance along the Y-axis

Z

Travel distance along the Z-axis

F

Cutting feedrate

Data other than the above cannot be specified.

D Number of controlled

Be sure to set 3 in parameter No. 7510 as the number of controlled axes.

axes

Limitations

D Incremental command

Move commands can be specified only in incremental mode.

D Functions that cannot be

Cutter compensation B and C cannot be specified. The feedrate cannot

specified

be overridden.

D Feedrate clamp

The maximum cutting feedrate clamp function is disabled.

D Binary data format

The format of high-speed remote buffer A can also be used for

high-speed remote buffer B. This format, however, cannot be used

together with NC language within the same program.

471

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

During high-speed machining, the distribution processing status is

19.4

monitored. When distribution processing terminates, P/S alarm No. 000

DISTRIBUTION

and P/S alarm No. 179 are issued upon completion of the high-speed

PROCESSING

machining command (according to the setting of ITPDL (bit 7 of

parameter No. 7501)).

TERMINATION

MONITORING

These P/S alarms can be canceled only by turning off the CNC power.

FUNCTION FOR THE

HIGH-SPEED

MACHINING

COMMAND (G05)

Explanations

D High-speed machining

High-speed machining using the high-speed remote buffer A function,

command

high-speed remote buffer B function, and high-speed cycle function

based on the G05 command

D Distribution processing

Failure to perform normal distribution processing because distribution

termination

processing required for high-speed machining exceeded the CNC

processing capacity, or because distribution data sent from the host was

delayed for some reason while the high-speed remote buffer A or G

function was being used

Alarm

Alarm No.

Message

Contents

000

PLEASE

During high-speed machining, distribution pro-

TURN OFF

cessing was terminated.

POWER

Related parameters:

Remote buffer transfer baud rate (parameter

179

PARAM.

No. 133)

(PRM No.

Number of controlled axes in high-speed ma-

7510)

chining (parameter No. 7150)

SETTING

High-speed axis selection during high-speed

ERROR

machining (bit 0 of parameter No. 7510)

472

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

19.5

The high-speed linear interpolation function processes a move command

related to a controlled axis not by ordinary linear interpolation but by

HIGH-SPEED

high-speed linear interpolation. The function enables the high-speed

LINEAR

execution of an NC program including a series of minute amounts of

INTERPOLATION

travel.

(G05)

Format

G05 P2

;

Start high-speed linear interpolation

G05 P0

;

End high-speed linear interpolation

A block for specifying G05 must not contain any other command.

Explanations

D High-speed linear

The high-speed linear interpolation start command G05 P2; places the

interpolation mode

system in high-speed linear interpolation mode, in which high-speed

linear interpolation is executed. The high-speed linear interpolation end

command G05 P0; places the system in the standard NC program

operation mode.

At power-up or in the NC reset state, the system enters the standard NC

program operation mode.

D Commands in

The commands that can be programmed in high-speed linear

high-speed linear

interpolation mode are:

interpolation mode

X/Y/Z/C-axis incremental travel distance command, cutting feedrate

command, and high-speed linear interpolation end command.

In high-speed linear interpolation mode, an address other than those

listed in the following table is ignored.

Address

Description

X---.---

X-axis incremental travel distance

Y---.---

Y-axis incremental travel distance

Z---.---

Z-axis incremental travel distance

C---.---

C-axis incremental travel distance

G05 P0 ;

High-speed linear interpolation end command

D X/Y/Z/C-axis incremental

A travel distance specified in high-speed linear interpolation mode is

traveling distance

regarded as being an incremental travel distance, regardless of the

G90/G91 mode setting.

D Cutting feedrate

Specify a cutting feedrate in high-speed linear interpolation mode. If no

cutting feedrate is specified, the modal F value is assumed.

Maximum

Interpolation period:

Interpolation period:

feedrate

8 msec

4 msec

(IS-B, metric input)

122,848

mm/min

245,696

mm/min

(IS-B, inch input)

12,284.8

inch/min

24,569.6

inch/nim

(IS-C, metric input)

12,284

mm/min

24,569

mm/min

(IS-C, inch input)

1,228.48

inch/min

2,456.96

inch/min

473

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

(Maximum feedrate) =

8

122,848

(IS-B, metric input)

(interpolation period)

Minimum

Interpolation period:

Interpolation period:

feedrate

8 msec

4 msec

(IS-B, metric input)

4

mm/min

8

mm/min

(IS-B, inch input)

0.38

inch/min

0.76

inch/mim

(IS-C, metric input)

4

mm/min

8

mm/min

(IS-C, inch input)

0.38

inch/min

0.76

inch/min

8

(Minimum feedrate) = 4

(IS-B, metric input)

(interpolation period)

D Interpolation period

In high-speed linear interpolation mode, the NC interpolation period can

be changed. As the interpolation period decreases, the machining speed

and precision increase.

IT2, IT1, and IT0 bits (bits 6, 5, and 4 of parameter 7501)

IT2

IT1

IT0

Interpolation period

0

0

0

8 msec in high-speed linear interpolation mode

0

1

0

4 msec in high-speed linear interpolation mode

0

0

1

2 msec in high-speed linear interpolation mode

0

1

1

1 msec in high-speed linear interpolation mode

1

1

1

0.5 msec in high-speed linear interpolation mode

Limitations

D Controlled axes

Up to four axes can be controlled. The names of the controlled axes are

X, Y, Z, and C. Any other axis name is ignored. Set X, Y, Z, then C in

axis name setting parameter 1020.

D Enabled interpolation

Only the linear interpolation function can be executed. Circular

interpolation and other interpolation functions cannot be executed.

D Absolute command

Movement cannot be specified by absolute values. A specified travel

distance is always considered as an incremental travel distance, regardless

of the G90/G91 mode setting.

D Feed per rotation

The feed per rotation command cannot be specified. Feed per minute is

always assumed, regardless of the G94/G95 mode setting.

D Cutter compensation

High-speed linear interpolation commands cannot be specified in cutter

compensation mode (G41/G42). If the high-speed linear interpolation

start command is specified in cutter compensation mode, P/S alarm No.

178 is issued.

D Modes related to the

The high-speed interpolation commands cannot be specified in polar

coordinate system

coordinate interpolation mode

(G12.1), scaling mode

(G51), or

coordinate system rotation mode.

474

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

This function is designed for high-speed precise machining. With this

19.6

function, the delay due to acceleration/deceleration and the delay in the

ADVANCED

servo system which increase as the feedrate becomes higher can be

PREVIEW CONTROL suppressed.

The tool can then follow specified values accurately and errors in the

(G08)

machining profile can be reduced.

This function becomes effective when advanced preview control mode is

entered.

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

builder.

Format

G08 P_

P1 : Turn on advanced preview control mode.

P0 : Turn off advanced preview control mode.

Explanations

D Available functions

In advanced preview control mode, the following functions are available:

(1) Linear acceleration/deceleration before interpolation

(2) Automatic corner deceleration function

For details on the above functions, see the descriptions of the functions.

Each function, specific parameters are provided.

D Reset

Advanced preview control mode is canceled by reset.

Limitations

D G08 command

Specify G08 code only in a block.

D Functions that can be

In the advanced preview control mode, the optional functions listed below

specified

can be specified.

NOTE

To use a function other than the following optional functions,

turn the advanced preview control mode off, specify the

desired function, then turn the mode on again.

476

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

19.7

AI CONTOUR

CONTROL

FUNCTION/AI NANO

CONTOUR CONTROL

FUNCTION

Overview

The AI contour control/AI nano contour control function is provided for

high-speed, high-precision machining.

This function enables

suppression of acceleration/deceleration delays and servo delays that

become larger with increases in the feedrate and reduction of machining

profile errors.

Look-ahead acceleration/deceleration before interpolation is enabled for

up to 40 blocks in AI contour control or for up to 180 blocks in AI nano

contour control. This enables execution of smooth acceleration/

deceleration extending over multiple blocks and higher machining.

The AI nano contour control function calculates a position command to

be output to the digital servo in nanometers (nm) with nano-interpolation,

so the machine can be moved smoothly and the surface precision is

improved.

Explanation

This function is enabled by setting the AI contour control or AI nano

contour control mode.

D Format

G05.1 Q _ ;

Q1 : AI contour control/AI nano contour control mode on

Q0 : AI contour control/AI nano contour control mode off

NOTE

1

Always specify G05.1 in an independent block.

2

The AI contour control/AI nano contour control mode is also

canceled by a reset.

3

When the AI nano contour control option is installed, bit 0

(NAN) of parameter No. 7053 is set to 1 to set the AI contour

control mode.

478

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

D Functions valid in the AI

The functions listed below are valid in the AI contour control/AI nano

contour control/AI nano

contour control mode:

contour control mode

⋅ Nano-interpolation (only in the AI nano contour control mode)

⋅ Look-ahead linear acceleration/deceleration before interpolation

⋅ Look-ahead bell-shaped acceleration/deceleration before interpolation

(The option of look-ahead bell-shaped acceleration/deceleration

before interpolation is required.)

⋅ Automatic corner deceleration

⋅ Feedrate clamping by acceleration

⋅ Feedrate clamping by arc radius

⋅ Block overlap (up to five blocks)

⋅ Advanced preview feed forward

D Nano-interpolation (only

Nano-interpolation calculates a position command to be output to the

in the AI nano contour

digital servo in nanometers (nm) for a conventional program (IS-B or

control mode)

IS-C command). Using the calculation results, a smooth position

command is output to the servo, so the machine can be moved smoothly

and the surface precision is improved.

Nano-

NC program

High-precision

Servo motor

interpolation

servo control

Uses a conventional

Calculates the

program.

position precisely.

Combination with HRV

control improves the

follow-up ability.

NOTE

The positioning precision depends on the detection unit.

D Look-ahead linear

For a cutting feed command in the feed per minute mode, linear

acceleration/deceleration

acceleration/deceleration can be applied before interpolation, that is, for

before interpolation

the specified feedrate by reading up to 40 blocks (in the AI contour control

mode) or 180 blocks (in the AI nano contour control mode) in advance.

With acceleration/deceleration after interpolation, the interpolated data is

changed because acceleration/deceleration is applied to the data. With

acceleration/deceleration before interpolation, the interpolated data

cannot be changed by acceleration/deceleration because acceleration/

deceleration is applied to the feedrate data before interpolation. For this

reason, the interpolated data can always be applied to the specified

straight line or curve to eliminate machining profile errors caused by

acceleration/deceleration delays.

479

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

Linear accelera-

tion/deceleration

before

interpolation

Specified

Distribution

Acceleration/

feedrate

pulse

Feedrate

Interpolation

deceleration

Servo

calculation

calculation

after

control

interpolation

Linear interpolation,

circular interpolation, etc.

(Example of deceleration)

Deceleration is started in a prior block so that the feedrate specified for

the target block is reached at the execution.

Feedrate

Specified feedrate

Point1

Feedrate determined by

F3

acceleration/deceleration

beforeinterpolation

Point2

F2

F1

Time

N1

N2

To decelerate from feedrate F3 to F2, deceleration must start with point 1.

To decelerate from feedrate F2 to F1, deceleration must start with point 2.

Multiple blocks can be read in advance to perform deceleration extending

over several blocks.

(Example of acceleration)

Acceleration is performed so that the feedrate specified for the target

block is reached at the execution.

Feedrate

Specified feedrate

Feedrate determined by

F3

acceleration/deceleration

beforeinterpolation

F2

F1

Time

N1

N2

480

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

D Look-ahead bell-shaped

Linear acceleration/deceleration before interpolation for cutting feed in

acceleration/deceleration

the AI contour control/AI nano contour control mode can be changed to

before interpolation

bell-shaped acceleration/deceleration before interpolation.

With

bell-shaped acceleration/deceleration before interpolation, smooth

acceleration/deceleration can be applied to the cutting feedrate to reduce

the shock on the machine by fluctuations in acceleration that are involved

in changes in the cutting feedrate.

To use this function, the option of look-ahead bell-shaped acceleration/

deceleration before interpolation is required.

Feedrate

Linear acceleration/

deceleration

Bell-shaped acceleration/

deceleration

ta Depends on the linear acceleration.

tb Time constant for bell-shaped

acceleration/deceleration

tc Bell-shapedacceleration/

deceleration time

tc = ta + tb

ta is not constant and depends

on the specified feedrate.

Specified feedrate

Time

ta =

tb

tb

tb

tb

Linear acceleration

tb is constant.

ta

ta

tc

tc

Acceleration

tb

tb

Linear acceleration/

deceleration

Bell-shaped acceleration/

deceleration

ta Depends on the linear acceleration.

Time

tb Time constant for bell-shaped

acceleration/deceleration

tc Bell-shapedacceleration/

deceleration time

tb

tb

12.

tc = ta + tb

ta

ta

tc

tc

481

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

When the feedrate is changed, deceleration and acceleration are

performed as follows:

For deceleration: Bell-shaped deceleration is started in the preceding

block so that deceleration terminates by the beginning of the block in

which the feedrate is changed.

For acceleration: Bell-shaped acceleration is started after the

beginning of the block in which the feedrate is changed.

Deceleration

Fa

Fb

Time

N1

N2

Acceleration

Feedrate

Fb

Fa

Time

N1

N2

D Automatic corner

Between contiguous two blocks, the feedrate difference for an axis may

deceleration

exceed the setting (parameter No. 1783). In this case, the feedrate at the

corner is calculated as follows based on the axis for which the ratio of the

actual feedrate difference to the allowable feedrate difference is the

largest. Deceleration is performed so that the feedrate is reached at the

interface of the blocks.

The change in the feedrate for each axis (Vx, Vy, ...) during movement at

the specified feedrate F is compared with the setting of parameter No.

1783 (Vprm-x, Vprm-y, ...). If the change in the feedrate for any axis

exceeds the setting of the parameter, the following expression is used:

Vx

Vy

Rmax + maxƪ

,

,,,ƫ

Vprm * x

Vprm * y

The required feedrate (Fc) is obtained as follows and deceleration is

performed at the corner:

1

Fc + F

Rmax

For example, assume that the tool move direction changes by 90 degrees

from movement along the X-axis to that along the Y-axis. Also assume

that the specified feedrate is 1000 mm/min and the allowable feedrate

difference

(parameter No. 1783) is

500 mm/min. Deceleration is

performed as shown in the figure below:

482

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

N1 G01 G91 X100. F1000 ;

N2 Y100. ;

N2

Tool path when deceleration

is not performed at the corner

Tool path when deceleration is

performed at the corner

N1

Feedrate

When deceleration is not performed

F1000

at the corner

When deceleration is performed

at the corner

F500

N1

Time

Feedrate

F1000

F500

N2

Time

Feedrate

F1000

F500

N1

N2

Time

483

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

D Feedrate clamping by

When continuous minute straight lines form curves as shown in the

acceleration

example in the figure below, the feedrate difference for each axis at each

corner is not so large. For this reason, deceleration according to the

feedrate difference is not effective. Continuous small feedrate differences

make a large acceleration for each axis as a whole, however.

In this case, deceleration is performed to suppress the shock on the

machine and machining errors caused by too large acceleration. The

feedrate is decreased so that the acceleration for each axis that is obtained

using the expression below does not exceed the allowable acceleration

setting for all axes.

The allowable acceleration is set based on the maximum cutting feedrate

(parameter No. 1432) and time required to reach the feedrate (parameter

No. 1785).

Acceleration for each axis =

Feedrate difference for each axis at each corner

maxƪ^{Traveldistanceinprecedingblock}

,^{Traveldistanceinfollowingblock}ƫ

F

F

The decreased feedrate is obtained for each corner. The decreased feedrate

obtained at the start or end point of the block, whichever is lower, is used

as the actual feedrate.

(Example) In the example below, deceleration is performed because the

acceleration (gradient of each dotted line in the feedrate

graphs) from N2 to N4 and from N6 to N8 is too large.

N8

N7

N9

N6

N5

N4

N1

N3

N2

484

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

N1

N5

N9

N1

N5

N9

D Feedrate clamping by

The maximum allowable feedrate v for an arc of radius r specified in a

arc radius

program is calculated using the arc radius R and maximum allowable

feedrate V (setting of a parameter) for the radius as follows so that the

acceleration in an arc block does not exceed the allowable value. If the

specified feedrate exceeds the feedrate v, the feedrate is automatically

clamped to the feedrate v.

Maximum allowable feedrate +^V2

R

R : Arc radius

V : Feedrate for arc radius R

then, the maximum allowable feedrate v for an arc of radius r can be

obtained using the following expression:

v + Ǹ (rńR) V

NOTE

As the specified arc radius becomes smaller, the maximum

allowable feedrate v becomes lower. If the maximum

allowable feedrate v is lower than the setting of parameter

No. 1732 (lower feedrate limit for feedrate clamping by arc

radius), it can be assumed to be the setting of the parameter

to prevent the maximum allowable feedrate from becoming

too low.

485

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

Feedrate

Linear acceleration/

deceleration

Bell-shaped acceleration/

deceleration

ta Depends on the linear acceleration.

tb Time constant for bell-shaped

acceleration/deceleration

tc Bell-shapedacceleration/

deceleration time

tc = ta + tb

ta

tb

Time

tb

tb

tb

tb

ta

ta

tc

tc

487

19. HIGH SPEED CUTTING FUNCTIONS

PROGRAMMING

B-63534EN/02

If the feedrate during movement is F, the acceleration for linear

acceleration/deceleration is A, the time constant for bell-shaped

acceleration/deceleration is T, the time required for acceleration/

deceleration can be obtained as follows:

Time required for acceleration/deceleration

= F/A

(linear acceleration/deceleration)

= F/A+T (bell-shaped acceleration/deceleration)

Feedrate

F

F/A : Time required for linear acceleration

T

: Time required for rounding the corner

Time

T/2

F/A

T/2

T

T

When the non-linear interpolation type is selected, movement is

performed at the feedrate set in parameter No.

1420 with

acceleration/deceleration set in parameter No. 1620. The corresponding

value can be set in parameter No.

1621 to select bell-shaped

acceleration/deceleration.

(To select bell-shaped acceleration/deceleration,

the option of bell-shaped acceleration/deceleration for rapid traverse is

required.)

NOTE

Rapid traverse block overlap is disabled.

To use bell-shaped acceleration/deceleration, the option of

bell-shaped acceleration/deceleration for rapid traverse is

required.

In the AI nano contour control mode, the non-linear

interpolation type cannot be selected.

488

B-63534EN/02

PROGRAMMING

19. HIGH SPEED CUTTING FUNCTIONS

D Involute interpolation

During involute interpolation, the following overrides are applied to the

(only in the AI contour

specified cutting feedrate. By this function, a good cutting surface with

control mode)

higher machining precision can be obtained.

(1) Override for inward offset in cutter compensation

(2) Override near the base circle

(1)

(Override for inward offset in cutter compensation

When cutter compensation C is applied to involute interpolation, control

is exercised in ordinary involute interpolation so that the tangential

feedrate on the tool-center path always keeps the specified feedrate.

Under the control, the actual cutting feedrate

(feedrate around the

perimeter of the tool (cutting point) on the path specified in the program)

changes because the curvature of the involute curve changes every

moment. If the tool is offset in the inward direction of the involute curve

in particular, the actual cutting feedrate becomes higher than the specified

feedrate as the tool gets nearer to the base circle.

For smooth machining, it is desirable to control the actual cutting feedrate

so that the feedrate keeps the specified feedrate. This function calculates

the override commensurate with the curvature of the involute curve which

changes every moment in involute interpolation, in particular, with

inward offset. The function also controls the actual cutting feedrate

(tangential feedrate at the cutting point) so that it always keeps the

specified feedrate.

Tool-center path

Rcp

Cutting point

Rofs

Base circle

Path specified in the program

The override is calculated as follows:

Rcp

OVRa +

100

Rcp ) Rofs

Rcp : Radius of curvature at the center of the tool of the involute

curve passing through the center of the tool

Rofs : Radius of the cutter

489

Content      ..     15      16      17      18     ..