Content      ..     12      13      14      15     ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 14

17. PROGRAMMABLE PARAMETER

B-64124EN/01

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.

373

17. PROGRAMMABLE PARAMETER

ENTRY (G10)

PROGRAMMING

B-64124EN/01

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

374

18. MEMORY OPERATION USING

B-64124EN/01

PROGRAMMING

FS10/11 TAPE FORMAT

MEMORY OPERATION USING FS10/11 TAPE FORMAT

18

General

Memory operation of the program registered by FS10/11 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 this Series and Series 10/11. The Series 10/11

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

must comply with this Series. When a value out of the specified range for

this Series is registered, an alarm occurs. Functions not available in this

Series cannot be registered or used for memory operation.

D Address for the cutter

Offset numbers are specified by address D in the Series 10/11. 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 10/11

M98 Pfffff Lffff ;

P : Subprogram number

L : Repetition count

Series 0i

M98 Pffff jjjj ;

Repetition count Subprogram number

D Address for the canned

The Series 10/11 and Series 16/18/21 use different addresses for the repeat

cycle repetition count

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

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

CNC

Address

Series 10/11

L

Series 0i

K

375

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

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

19.1

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 ∆r 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.

377

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

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

19.2

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

ADVANCED PREVIEW

servo system which increase as the feedrate becomes higher can be

CONTROL (G08)

suppressed.

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

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 Connection Manual (Function)

(B-64113EN-1). 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 functions listed below can be

specified

specified.

NOTE

To use a function other than the following functions, turn the

advanced preview control mode off, specify the desired

function, then turn the mode on again.

⋅ Inverse time feed

⋅ Axis control by the PMC

(Bits 4 (G8R) and 3 (G8C) of parameter No. 8004 can be set to also use

this function in the advanced preview control mode.)

⋅ Single direction positioning

⋅ Polar coordinate command

⋅ Helical interpolation

⋅ Rigid tapping

(Bit 5 (G8S) of parameter No. 1602 can be set to also use this function

in the look-ahead control mode. The serial spindle parameters must

also be set.)

378

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

D Functions valid in the AI

The functions listed below are valid in the AI advanced preview

advanced preview

control/AI contour control mode:

control/AI contour

⋅ Look-ahead linear acceleration/deceleration before interpolation

control mode

⋅ 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

⋅ Advanced preview feed forward

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 20 blocks (in the AI advanced

preview control mode) or 40 blocks (in the AI 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.

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.

381

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

(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

382

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

D Look-ahead bell-shaped

Linear acceleration/deceleration before interpolation for cutting feed in

acceleration/deceleration

the AI advanced preview control/AI contour control mode can be changed

before interpolation

to 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

383

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

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:

384

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

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

385

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

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

386

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

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:

Ǹ

v+

(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.

387

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

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

The value of ta is not constant and

depends on the rapid traverse rate

and the time constant of the rapid

traverse rate for the specified axis.

Time

tb

tb

tb

tb

The value of tb depends on the axis.

ta

ta

tc

tc

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

389

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

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.

NOTE

Rapid traverse block overlap is disabled.

D Corresponding

In the following tables, AI control means the AI advanced preview

parameter numbers in

control/AI contour control mode.

the normal mode,

(1) Parameters related to linear acceleration/deceleration before

advanced preview

interpolation

control mode, and AI

Parameter number

advanced preview

control/AI contour

Ad-

Parameter

control mode

vanced

AI

Normal

preview

contour

control

Acceleration/deceleration type (A or B)

FWB/1602#0

None

Parameter 1 for setting the acceleration

1630

1770

Parameter 2 for setting the acceleration

1631

1771

Feedrate at which an overtravel alarm occurs

1784

(2) Parameters related to automatic corner deceleration

Parameter number

Ad-

Parameter

vanced

AI

Normal

preview

contour

control

Method for determining whether to perform

CSD/1602#4

None

automatic corner deceleration (angle/fee-

drate difference)

Lower feedrate limit (control according to the

1778

1777

None

angle)

Angle at which automatic corner deceleration

1740

1779

None

is performed (control according to the angle)

Allowable feedrate difference for all axes

1780

None

(control according to the feedrate difference)

Allowable feedrate difference for each axis

1783

(control according to the feedrate difference)

Acceleration/deceleration type

FWB/1602#0

None

(Type A/Type B)

(3) Parameter related to feedrate clamping by acceleration

Parameter number

Ad-

Parameter

vanced

AI

Normal

preview

contour

control

Parameter for determining the allowable ac-

None

1785

celeration

390

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

(4) Parameters related to feedrate clamping by arc radius

Parameter number

Ad-

Parameter

vanced

AI

Normal

preview

contour

control

Arc radius corresponding to the upper fee-

1731

drate limit

Upper feedrate limit at arc radius R

1730

Lower clamped feedrate limit

1732

(5) Other parameters

Parameter number

Ad-

Parameter

vanced

AI

Normal

preview

contour

control

Precision of radius errors in circular interpola-

PCIR1/3403#0

None

tion

Maximum cutting feedrate (common to all

1422

1431

1422

axes)

Maximum cutting feedrate (for each axis)

1430

1432

Rapid traverse movement type*

LRP/1401#1

AIR/

7054#1

LRP/

1401#1

Time constant for bell-shaped acceleration/

1621

RBL/

deceleration for rapid traverse

1603#6

1621

Arc radius corresponding to the upper fee-

1731

drate limit

391

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

Alarms

Num-

Message

Description

ber

5110

IMPROPER G CODE

An unspecifiable G code was specified in

the AI advanced preview control/AI con-

(G05.1 Q1 MODE)

tour control mode.

5111

IMPROPER MODAL

An unavailable modal G code was found

G CODE

when the AI advanced preview control/AI

contour control mode was specified.

(G05.1 Q1)

5112

G08 CAN NOT BE

The look-ahead control command (G08)

COMMANDED

was specified in the AI advanced preview

control/AI contour control mode.

(G05.1 Q1)

5114

CAN NOT ERROR IN

Intervention by manual operation was per-

MDI MODE

formed during execution of the G28, G30,

or G53 command (linear interpolation

(G05.1 Q1)

type) in the AI advanced preview control/

AI contour control mode. After that, auto-

matic operation was restarted at a position

other than the stop position.

5156

ILLEGAL AXIS

In the AI advanced preview control/AI con-

OPERATION

tour control mode, the controlled axis

selection signal (PMC axis control)

(AICC)

changed.

In the AI advanced preview control/AI con-

tour control mode, the simple synchronous

axis selection signal changed.

5157

PARAMETER 0

The setting of the parameter for specifying

the maximum cutting feedrate (No. 1422,

(AICC)

1432, or 1420) is 0.

The setting of the parameter for specifying

acceleration/deceleration before interpola-

tion (No. 1770 or 1771) is 0.

Notes

1) The advanced preview control function (G08P1) can also be specified.

2) When the total distance of blocks read in advance reaches the distance

for decelerating from the current feedrate, deceleration is started.

When look-ahead operation proceeds and the total distance of blocks

increases by termination of deceleration, acceleration is started again.

If a series of blocks with a small amount of travel are specified, the

deceleration and acceleration may be alternated, which prevents the

feedrate from being constant. In this case, specify a lower feedrate.

3) When the dry run signal is inverted from ”0” to ”1” or from ”1” to ”0”

during movement along an axis, acceleration/deceleration is

performed to the specified feedrate without deceleration to feedrate 0.

4) If a non-movement block or one-shot G code command such as G04

is found in the AI advanced preview control/AI contour control mode,

the movement is decelerated and temporarily stopped in the preceding

block.

5) For acceleration/deceleration after interpolation, use linear or

bell-shaped acceleration/deceleration. Exponential acceleration/

deceleration cannot be used.

392

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

D Specifications

Axis control

f : Can be specified.

: Cannot be specified.

Name

Function

Number of controlled axes

3 to 4

Number of simultaneously con-

Up to 4

trolled axes

Axis name

The basic three axes are fixed to X, Y, and Z.

Other axes are any of U, V, W, A, B, and C.

Least input increment

0.001 mm, 0.001 deg, 0.0001 inch

One-tenth input increment

0.0001 mm, 0.0001 deg, 0.00001 inch

One-tenth input increment for each axis cannot be

used.

Simple synchronous control

f

However, switching between synchronous and

normal operation cannot be performed during

automatic operation (when the automatic op-

eration signal (OP) is set to 1) regardless of

whether the AI advanced preview control/AI

contour control mode is set. In this case,

switching causes a PS213 alarm.

Angular axis control

Tandem control

f

However, full preloading is not allowed.

Inch/metric conversion

f

(*1)

(G20, G21)

Interlock

f

Interlock for each axis

f

Movement along all axes stops.

To stop movement only along the interlock axis

in non-linear interpolation type positioning, set

bit 5 (AIL) of parameter No. 7054 to 1 and bit 4

(XIK) of parameter No. 1002 to 0.

Machine lock

f

When the machine lock signal for each axis

(MLK1 to MLK8) is turned on or off, accelera-

tion/deceleration is not applied to the axis for

which machine lock is performed.

Stroke limit check before move

Mirror image

f

Stored pitch error compensation

f

Position switch

f

Set bit 3 (PSF) of parameter No. 6901 to 1.

When this parameter is set to 1, the signal out-

put timing changes.

Abnormal load detection

f

Manual handle interruption

f

Manual handle interruption is disabled during

switching to the AI advanced preview control/AI

contour control mode.

External pulse synchronization

Interpolation functions

f : Can be specified.

: Cannot be specified.

Name

Function

Positioning (G00)

f

Single direction positioning (G60)

f To perform single direction positioning in the AI

advanced preview control/AI contour control

mode, set bit 4 (ADP) of parameter No. 7055 to

1.

Exact stop (G09)

f

Exact stop mode (G61)

f

Tapping mode (G63)

f

Linear interpolation (G01)

f

Circular interpolation (G02, G03)

f (Circular interpolation for multiple quadrants is

enabled.)

393

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

Name

Function

Dwell (G04)

f

(Dwell with the time in seconds or speed speci-

fied) For dwell with the speed specified, anoth-

er option is required.

Cylindrical interpolation (G07.1)

Helical interpolation (G02, G03)

f

(Circular interpolation + linear interpolation for

up to two axes)

Specify the feedrate including the helical axis in

the feedrate command.

Threading and synchronous feed

(G33)

Skip function (G31)

f

(*2)

High-speed skip function (G31)

f

(*2)

Multistage skip function (G31 Px)

f

(*2)

Reference position return (G28)

f

(*2)

To execute G28 in the status in which the refer-

ence position is not established, set bit 2 (ALZ)

of parameter No. 7055 to 1.

Reference position return check

f

(*2)

(G27)

2nd, 3rd, and 4th reference posi-

f

(*2)

tion return (G30)

Normal direction control

f

Set bit 2 (ANM) of parameter No. 5484 to 1.

(G41.1, G42.1)

Continuous dressing

In-feed control (G161)

Index table indexing

f

(*2)

To set follow-up of the index table indexing

axis (fourth axis), set bit 7 (NAH4) of parameter

No. 1819 and bit 0 (NMI4) of parameter No.

7052 to 1.

Feed functions

f : Can be specified.

: Cannot be specified.

Name

Function

Rapid traverse rate

Up to 240 m/min (0.001 mm)

Up to 100 m/min (0.0001 mm)

Rapid traverse rate override

F0, 25, 50, 100 %

Rapid traverse rate override in in-

0 to 100 %

crements of 1%

Feed per minute (G94)

f

Feed per revolution (G95)

Cutting feedrate clamp

f

Bell-shapedacceleration/decel-

f

eration for rapid traverse

Linearacceleration/deceleration

f

after cutting feed interpolation

Bell-typeacceleration/decelera-

f

tion after cutting feed interpolation

Linearacceleration/deceleration

f (Up to 20 blocks are read in advance in the AI

before cutting feed interpolation

advanced preview control mode.)

(Up to 40 blocks are read in advance in the AI

contour control mode.)

Feedrate override

0 to 254 %

Single-digit F code feed

f To enable feedrate change using a manual

handle, set bit 1 (AF1) of parameter No. 7055

to 1.

Inverse time feed (G93)

f

Override cancel

f

394

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

Name

Function

External deceleration

f

Look-ahead bell-shaped accel-

f

eration/deceleration beforeinter-

polation

Program input

f : Can be specified.

: Cannot be specified.

Name

Function

Control in/control out command ()

f

Optional block skip command

f

(/n: n is a number.)

Absolute command (G90)/

f

incremental command (G91)

Decimal point programming/pock-

f

et calculator type decimal point

programming

10-fold input unit

f

Plane selection (G17, G18, G19)

f

Rotation axis specification

f

Rotation axis roll over

f

Polar coordinate command (G16)

Local coordinate system (G52)

f

(*2)

Machine coordinate system (G53)

f

(*2)

Workpiece coordinate system

f

(G54 to G59)

(G54.1Pxx)

Workpiece coordinate system

f

(*2)

(G92)

Workpiece coordinate system pre-

f

(*2)

set (G92.1)

Arbitrary angle chamfering/corner

rounding

Programmable data input (G10)

f

(*2)

Only the tool offset value, workpiece origin off-

set, and parameter can be changed.

Custom macro B

f

See the description of ”Notes on using custom

macros.”

Addition of custom macro com-

f

mon variables

Pattern data input

Interruption type custom macro

Canned cycle (G73 to G89)

f

(*2)

Initial level return (G98)/

f

(*2)

point R level return (G99)

Small hole peck drilling cycle

(G83)

Arc radius R programming

f

Automatic corner override (G62)

f

Set bit 0 (ACO) of parameter No. 7055 to 1.

Automatic corner deceleration

f

Feedrate clamping by arc radius

f

Scaling (G51)

f

Coordinate system rotation (G68)

f

Programmable mirror image

f

(G51.1)

F10/11 tape format

f

395

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

Auxiliary functions/spindle-speed functions

f : Can be specified.

: Cannot be specified.

Name

Function

Miscellaneous function (Mxxxx)

f The function code and function strobe signals

are output only.

Second auxiliary function (Bxxxx)

f The function code and function strobe signals

are output only.

High-speed M/S/T/B interface

f

Multiple miscellaneous function

f

specification

Spindle-speed function (Sxxxx)

f

Spindle synchronous control

f

Rigid tapping

f

(*2)

Set bit 5 (G8S) of parameter No. 1602 or bit 3

(ACR) of parameter No. 7051 to 1.

Tool compensation functions

f : Can be specified.

: Cannot be specified.

Name

Function

Tool function (Txxxx)

f The function code and function strobe signals

are output only.

Tool length compensation

f

(G43, G44, G49)

Tool offset (G45 to G48)

Cutter compensation C

f

(G40, G41, G42)

Tool life management

Automatic tool length measure-

ment

Other functions

f : Can be specified.

: Cannot be specified.

Name

Function

Cycle start/feed hold

f

Dry run

f

Single block

f

Sequence number comparison

f

and stop

Program restart

f For the time constant for acceleration/decelera-

tion during movement to the restart position,

the following parameters are used:

When exponential acceleration/deceleration is

used: Parameter Nos. 1624 and 1625

Whenlinear/bell-shapedacceleration/decel-

eration is used: Parameter No. 1622

To set the acceleration/deceleration type, use

bits 0 and 1 of parameter No. 1610.

Rigid tapping return

Macro executor

(execution macro)

MDI operation

f

Manualintervention

f

NOTE

The above tables include a function that another option is

required for specifying.

1

Multiple blocks are not read in advance.

396

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

D Conditions for setting the

When G05.1 Q1 is specified, the modal G codes must be set as listed

AI advanced preview

below. If one of these conditions is satisfied, a PS5111 alarm occurs.

control/AI contour

G code(s)

Description

control mode

G00

Positioning

G01

Linear interpolation

G02

Circular interpolation (CW)

G03

Circular interpolation (CCW)

G15

Polar coordinate command cancel

G40

Cutter compensation cancel

G40.1

Normal direction control cancel mode

G49

Tool length compensation cancel

G50

Scaling cancel

G50.1

Programmable mirror image cancel

G64

Cutting mode

G67

Macro modal call cancel

G69

Coordinate system rotation cancel

G80

Canned cycle cancel

G94

Feed per minute

G97

Constant surface speed control cancel

G160

In-feed control function cancel

397

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

19.4

LOOK-AHEAD

BELL-SHAPED

ACCELERATION/DEC

ELERATION BEFORE

INTERPOLATION

TIME CONSTANT

CHANGE FUNCTION

General

In Look-ahead bell-shaped acceleration/deceleration before

interpolation, the speed during acceleration/deceleration is as shown in

the figure below.

Linear

Speed

acceleration/deceleration

Non-linear

Non-linear

acceleration/deceleration

acceleration/deceleration

Specified

speed

Time

T1

T2

T2

T1: Time determined from the specified speed and the specified acceleration

Specified acceleration:

In case of AI contour control

Parameter No.1770/Parameter No.1771

T2: Acceleration change time

In case of AICC : Parameter No.1772

Fig.19.4 (a)

The time T1, shown above, varies with the specified speed. If the

specified speed is low, the speed will be as shown below, causing linear

acceleration/deceleration not reaching the specified acceleration.

398

19. HIGH SPEED CUTTING

B-64124EN/01

PROGRAMMING

FUNCTIONS

Linear acceleration/deceleration not reaching specified acceleration/deceleration

Speed

Specified

speed

Time

T1

T1

T2

Fig.19.4 (b)

If linear acceleration/deceleration not reaching the specified acceleration

occurs in AI contour control mode as shown above, this function shortens

the acceleration/deceleration time by changing the internal acceleration

for acceleration/deceleration before interpolation and the bell-shaped

time constant in order to generate an acceleration/deceleration pattern as

close as possible to that permits optimum bell-shaped

acceleration/deceleration before interpolation for the specified speed.

Optimum bell-shaped acceleration/deceleration before interpolation, as

mentioned here, refers to bell-shaped acceleration/deceleration before

interpolation in which

if T2 > T1, T1 and T2 are changed to T1’ and T2’ as shown in the figure

below so that linear acceleration/deceleration not reaching the specified

acceleration/deceleration does not occur.

This function becomes effective for the Acceleration /deceleration before

look-ahead interpolation in AI contour control mode.

Speed Non-linear acceleration/deceleration

Specified speed

Time

T1’

T2’

T2’

Fig.19.4 (c)

399

19. HIGH SPEED CUTTING

FUNCTIONS

PROGRAMMING

B-64124EN/01

Description

D Methods of specifying the

The acceleration/deceleration reference speed is the feedrate used as the

acceleration/deceleration

reference for calculating optimum acceleration. In Fig.19.4 (c), it is

reference speed

equivalent to the specified speed used to determine T1’ and T2’.

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

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

cutting as the reference speed

NOTE

This function is effective if BCG (No. 7055 bit 3) is 1.

(1) Specifying the speed

If an F command is used in a G05.1 Q1 block, the speed specified with

in a G05.1 Q1 block

the F command is assumed the acceleration/deceleration reference speed.

This acceleration/deceleration reference speed is cleared upon a reset.

After the acceleration/deceleration reference speed is cleared upon a reset

or after the power is turned off and then on again, the

acceleration/deceleration reference speed specified for parameter No.

7066 will be used. (Method (2), described later)

If the acceleration/deceleration reference speed specified for the

parameter is 0, the feedrate assumed at the start of cutting will be assumed

the acceleration/deceleration reference speed.

(Method (3), described

later)

(Program example)

G05.1 Q1 F5000 ; ··· Sets the reference speed to 5000 mm/min.

The F command used in a G05.1 block is used to

specify the acceleration/deceleration reference speed,

and is also used as a normal F command.

Even if the feedrate is changed during the execution of the machining

program, the acceleration/deceleration reference speed specified with the

above command remains in effect. If this occurs, the machining time may

become longer because machining is performed at the feedrate different

from the acceleration/deceleration reference speed.

For this reason, the acceleration/deceleration reference speed to be

specified with the above command should be as close as possible to the

actual machining speed.

NOTE

The G05.1Q1Fxxxx command must be issued in feed per

minute (G94) mode.

If this command is issued in another mode, the speed

specified with this command will be generated the alarm

(PS5111).

400

Content      ..     12      13      14      15     ..