Content      ..     1      2      3      4      ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 3

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

The command below will move a tool along a circular arc.

4.4

CIRCULAR

INTERPOLATION

(G02,G03)

Format

Arc in the XpYp plane

G02

I_ J_

G17

Xp_Yp_

F_ ;

G03

R_

Arc in the ZpXp plane

G02

I_ K_

G18

Xp_ p_

F_

G03

R_

Arc in the YpZp plane

G02

J_ K_

F_

G19

Yp_ Zp_

G03

R_

Table 4.4 Description of the command format

Command

Description

G17

Specification of arc on XpYp plane

G18

Specification of arc on ZpXp plane

G19

Specification of arc on YpZp plane

G02

Circular Interpolation Clockwise direction (CW)

G03

Circular Interpolation Counterclockwise direction (CCW)

X_{p_}

Command values of X axis or its parallel axis

(set by parameter No. 1022)

Yp_

Command values of Y axis or its parallel axis

(set by parameter No. 1022)

Z_{p_}

Command values of Z axis or its parallel axis

(set by parameter No. 1022)

I_

X_p axis distance from the start point to the center of an arc

with sign

J_

Yp axis distance from the start point to the center of an arc

with sign

k_

Z_p axis distance from the start point to the center of an arc

with sign

R_

Arc radius (with sign)

F_

Feedrate along the arc

43

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

Explanations

D Direction of the circular

“Clockwise”(G02) and “counterclockwise”(G03) on the X_pY_p plane

interpolation

(Z_pX_p plane or Y_pZ_p plane) are defined when the X_pY_p plane is viewed

in the positive-to-negative direction of the Z_p axis (Y_p axis or X_p axis,

respectively) in the Cartesian coordinate system. See the figure below.

Yp

Xp

Zp

G03

G03

G03

G02

G02

G02

Xp

Zp

Yp

G17

G18

G19

D Distance moved on an

The end point of an arc is specified by address Xp, Yp or Zp, and is

arc

expressed as an absolute or incremental value according to G90 or G91.

For the incremental value, the distance of the end point which is viewed

from the start point of the arc is specified.

D Distance from the start

The arc center is specified by addresses I, J, and K for the Xp, Yp, and Zp

point to the center of arc

axes, respectively. The numerical value following I, J, or K, however, is

a vector component in which the arc center is seen from the start point,

and is always specified as an incremental value irrespective of G90 and

G91, as shown below.

I, J, and K must be signed according to the direction.

End point (x,y)

End point (z,x)

End point (y,z)

y

x

z

x

Start

z

y

i

Start

j

Start

k

point

point

point

j

i

k

Center

Center

Center

I0,J0, and K0 can be omitted. When X_p, Y_p , and Zp are omitted (the end

point is the same as the start point) and the center is specified with I, J,

and K, a 360° arc (circle) is specified.

G021; Command for a circle

If the difference between the radius at the start point and that at the

end point exceeds the permitted value in a parameter (No.3410), an P/S

alarm (No.020) occurs.

44

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Arc radius

The distance between an arc and the center of a circle that contains the arc

can be specified using the radius, R, of the circle instead of I, J, and K.

In this case, one arc is less than 180°, and the other is more than 180° are

considered. When an arc exceeding 180° is commanded, the radius must

be specified with a negative value. If Xp, Yp, and Zp are all omitted, if

the end point is located at the same position as the start point and when

R is used, an arc of 0° is programmed

G02R ; (The cutter does not move.)

For arc (1)(less than 180°)

G91 G02 X_P60.0 Y_P20.0 R50.0 F300.0 ;

For arc (2)(greater than 180°)

G91 G02 X_P60.0 Y_P20.0 R-50.0 F300.0 ;

2

r=50mm

End point

1

Start point

r=50mm

Y

X

D Feedrate

The feedrate in circular interpolation is equal to the feed rate specified by

the F code, and the feedrate along the arc (the tangential feedrate of the

arc) is controlled to be the specified feedrate.

The error between the specified feedrate and the actual tool feedrate is

±2% or less. However, this feed rate is measured along the arc after the

cutter compensation is applied

Restrictions

If I, J, K, and R addresses are specified simultaneously, the arc specified

by address R takes precedence and the other are ignored.

If an axis not comprising the specified plane is commanded, an alarm is

displayed.

For example, if axis U is specified as a parallel axis to X axis when plane

XY is specified, an P/S alarm (No.028)is displayed.

When an arc having a center angle approaching 180° is specified, the

calculated center coordinates may contain an error. In such a case, specify

the center of the arc with I, J, and K.

45

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

Examples

Y axis

100

50R

60

60R

40

0

X axis

90

120 140

200

The above tool path can be programmed as follows ;

(1) In absolute programming

G92X200.0 Y40.0 Z0 ;

G90 G03 X140.0 Y100.0R60.0 F300.;

G02 X120.0 Y60.0R50.0 ;

or

G92X200.0 Y40.0Z0 ;

G90 G03 X140.0 Y100.0I-60.0 F300.;

G02 X120.0 Y60.0I-50.0 ;

(2) In incremental programming

G91 G03 X-60.0 Y60.0 R60.0 F300.;

G02 X-20.0 Y-40.0 R50.0 ;

or

G91 G03 X-60.0 Y60.0 I-60.0 F300. ;

G02 X-20.0 Y-40.0 I-50.0 ;

46

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.5

Helical interpolation which moved helically is enabled by specifying up

HELICAL

to two other axes which move synchronously with the circular

INTERPOLATION

interpolation by circular commands.

(G02,G03)

Format

Synchronously with arc of XpYp plane

G02

G17

I_J_

Xp_Yp_

α_(β_)F_;

G03

R_

Synchronously with arc of ZpXp plane

G02

G18

I_K_

Xp_Zp_

α_(β_)F_;

G03

R_

Synchronously with arc of YpZp plane

G02

J_K_

G19

Yp_Zp_

α_(β_)F_;

G03

R_

α,β: Any one axis where circular interpolation is not applied.

Up to two other axes can be specified.

Explanations

The command method is to simply or secondary add a move command

axis which is not circular interpolation axes. An F command specifies a

feed rate along a circular arc. Therefore, the feed rate of the linear axis

is as follows:

Length of linear axis

F×

Length of circular arc

Determine the feed rate so the linear axis feed rate does not exceed any

of the various limit values.Bit 0 (HFC) of parameter No. 1404 can be used

to prevent the linear axis feedrate from exceeding various limit values.

Z

Tool path

X

Y

The feedrate along the circumference of two cir-

cular interpolated axes is the specified feedrate.

Restrictions

Cutter compensation is applied only for a circular arc.

Tool offset and tool length compensation cannot be used in a block in

which a helical interpolation is commanded.

47

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

The amount of travel of a rotary axis specified by an angle is once

4.6

internally converted to a distance of a linear axis along the outer surface

CYLINDRICAL

so that linear interpolation or circular interpolation can be performed with

INTERPOLATION

another axis. After interpolation, such a distance is converted back to the

amount of travel of the rotary axis.

(G07.1)

The cylindrical interpolation function allows the side of a cylinder to be

developed for programming. So programs such as a program for

cylindrical cam grooving can be created very easily.

Format

G07.1IPr ; Starts the cylindrical interpolation mode

(e

:

:

:

G07.1

IP

0 ; The cylindrical interpolation mode is cancelled.

IP

: An address for the rotation axis

r : The radius of the cylinder

Specify G07.1 IPr ; and G07.1

IP

0; in separate blocks.

G107 can be used instead of G07.1.

Explanations

D Plane selection

Use parameter (No. 1022) to specify whether the rotation axis is the X-,

(G17, G18, G19)

Y-, or Z-axis, or an axis parallel to one of these axes. Specify the G code

to select a plane for which the rotation axis is the specified linear axis.

For example, when the rotation axis is an axis parallel to the X-axis, G17

must specify an Xp-Yp plane, which is a plane defined by the rotation axis

and the Y-axis or an axis parallel to the Y-axis.

Only one rotation axis can be set for cylindrical interpolation.

D Feedrate

A feedrate specified in the cylindrical interpolation mode is a speed on the

developed cylindrical surface.

D Circular interpolation

In the cylindrical interpolation mode, circular interpolation is possible

(G02,G03)

with the rotation axis and another linear axis. Radius R is used in

commands in the same way as described in II-4.4.

The unit for a radius is not degrees but millimeters (for metric input) or

inches (for inch input).

< Example Circular interpolation between the Z axis and C axis >

For the C axis of parameter (No.1022), 5 (axis parallel with the X axis)

is to be set. In this case, the command for circular interpolation is

G18 Z__C__;

G02 (G03) Z__C__R__;

For the C axis of parameter (No.1022), 6 (axis parallel with the Y axis)

may be specified instead. In this case, however, the command for

circular interpolation is

G19 C__Z__;

G02 (G03) Z__C__R__;

48

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

Examples

Example of a Cylindrical Interpolation Program

C

O0001 (CYLINDRICAL INTERPOLATION );

N01 G00 G90 Z100.0 C0 ;

Z

R

N02 G01 G91 G18 Z0 C0 ;

N03 G07.1 C57299 ;

N04 G90 G01 G42 Z120.0 D01 F250 ;

N05 C30.0 ;

N06 G03 Z90.0 C60.0 R30.0 ;

N07 G01 Z70.0 ;

N08 G02 Z60.0 C70.0 R10.0 ;

N09 G01 C150.0 ;

N10 G02 Z70.0 C190.0 R75.0 ;

N11 G01 Z110.0 C230.0 ;

N12 G03 Z120.0 C270.0 R75.0 ;

N13 G01 C360.0 ;

N14 G40 Z100.0 ;

N15 G07.1 C0 ;

N16 M30 ;

Z

mm

N05

N13

N12

120

110

N06

N11

90

N07

70

N08

N09

N10

60

C

0

30

60

70

150

190

230

270

360

deg

50

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Straight threads with a constant lead can be cut. The position coder

4.7

mounted on the spindle reads the spindle speed in real-time. The read

THREAD CUTTING

spindle speed is converted to the feedrate per minute to feed the tool.

(G33)

Format

Z

G33

IP

_ F_ ;

F : Long axis direction lead

Workpiece

X

Explanations

In general, thread cutting is repeated along the same tool path in rough

cutting through finish cutting for a screw. Since thread cutting starts when

the position coder mounted on the spindle outputs a 1-turn signal,

threading is started at a fixed point and the tool path on the workpiece is

unchanged for repeated thread cutting. Note that the spindle speed must

remain constant from rough cutting through finish cutting. If not,

incorrect thread lead will occur.

In general, the lag of the servo system, etc. will produce somewhat

incorrect leads at the starting and ending points of a thread cut. To

compensate for this, a thread cutting length somewhat longer than

required should be specified.

Table 4.7 lists the ranges for specifying the thread lead.

Table. 4.7 Ranges of lead sizes that can be specified

Least command

Command value range of the lead

increment

0.001 mm

F1 to F50000 (0.01 to 500.00mm)

mm input

0.0001 mm

F1 to F50000 (0.01 to 500.00mm)

0.0001 inch

F1 to F99999

(0.0001 to 9.9999inch)

Inch input

0.00001 inch

F1 to F99999

(0.0001 to 9.9999inch)

51

B-64124EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Linear interpolation can be commanded by specifying axial move

4.8

following the G31 command, like G01. If an external skip signal is input

SKIP

during the execution of this command, execution of the command is

FUNCTION(G31)

interrupted and the next block is executed.

The skip function is used when the end of machining is not programmed

but specified with a signal from the machine, for example, in grinding. It

is used also for measuring the dimensions of a workpiece.

Format

G31

_ ;

IP

G31: One-shot G code (If is effective only in the block in which it

is specified)

Explanations

The coordinate values when the skip signal is turned on can be used in a

custom macro because they are stored in the custom macro system

variable #5061 to #5064, as follows:

#5061 1st axis coordinate value

#5062 2nd axis coordinate value

#5063 3rd axis coordinate value

#5064 4th axis coordinate value

WARNING

Disable feedrate override, dry run, and automatic

acceleration/deceleration

(however, these become

available by setting the parameter SKF No.6200#7 to 1.)

when the feedrate per minute is specified, allowing for an

error in the position of the tool when a skip signal is input.

These functions are enabled when the feedrate per rotation

is specified.

NOTE

If G31 command is issued while cutter compensation C is

applied, an P/S alarm of No.035 is displayed. Cancel the

cutter compensation with the G40 command before the G31

command is specified.

53

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

Examples

D The next block to G31 is

an incremental

command

G31

G91X100.0 F100;

Y50.0;

Skip signal is input here

50.0

Y

100.0

Actual motion

X

Motion without skip signal

Fig. 4.8 (a) The next block is an incremental command

D The next block to G31 is

an absolute command

for 1 axis

G31

G90X200.00 F100;

Y100.0

Y100.0;

Skip signal is input here

X200.0

Actual motion

Motion without skip signal

Fig. 4.8 (b) The next block is an absolute command for 1 axis

D The next block to G31 is

an absolute command

for 2 axes

G31

G90X200.0 F100;

X300.0 Y100.0;

Y

Skip signal is input here

100

(300,100)

Actual motion

Motion without skip signal

X

100

200

300

Fig. 4.8 (c) The next block is an absolute command for 2 axes

54

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-64124EN/01

D Simplified

G31 P99/98 cannot be used for axes subject to simplified synchronization

synchronization and

or the X-axis or Z-axis when under slanted axis control.

slanted axis control

D Speed control

Bit 7 (SKF) of parameter No. 6200 must be set to disable dry run,

override, and auto acceleration or deceleration for G31 skip commands.

Do not use G31 P99/98 in consecutive blocks.

D Consecutive commands

WARNING

Always specify a torque limit before a G31 P99/98

command.

Otherwise, G31 P99/98 allows move

commands to be executed without causing a skip.

Examples

O0001 ;

:

:

The PMC specifies the torque limit

Mjj ;

through the window.

:

:

G31 P99 X200. F100 ;

Torque limit skip command

:

Move command for which a torque

G01 X100. F500 ;

limit is applied

:

:

MDD ;

Torque limit canceled by the PMC

:

:

M30 ;

:

%

58

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

The feed functions control the feedrate of the tool. The following two feed

5.1

functions are available:

GENERAL

D Feed functions

1. Rapid traverse

When the positioning command (G00) is specified, the tool moves at

a rapid traverse feedrate set in the CNC (parameter No. 1420).

2. Cutting feed

The tool moves at a programmed cutting feedrate.

D Override

Override can be applied to a rapid traverse rate or cutting feedrate using

the switch on the machine operator’s panel.

D Automatic acceleration/

To prevent a mechanical shock, acceleration/deceleration is automatically

deceleration

applied when the tool starts and ends its movement (Fig. 5.1 (a)).

Rapid traverse rate

F_R : Rapid traverse

F_R

rate

T_R

: Acceleration/

deceleration time

constant for rap-

id traverse rate

0

Time

T_R

T_R

Feed rate

F_C

: Feedrate

F_C

T_C : Acceleration/

deceleration time

constant for a cut-

ting feedrate

0

Time

T_C

T_C

Fig. 5.1 (a) Automatic acceleration/deceleration (example)

60

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

D Tool path in a cutting

If the direction of movement changes between specified blocks during

feed

cutting feed, a rounded-corner path may result (Fig. 5.1 (b)).

Y

Programmed path

Actual tool path

0

X

Fig. 5.1 (b) Example of tool path between two blocks

In circular interpolation, a radial error occurs (Fig. 5.1 (c)).

Y

∆r:Error

Programmed path

Actual tool path

r

0

X

Fig. 5.1 (c) Example of radial error in circular interpolation

The rounded-corner path shown in Fig. 5.1 (b) and the error shown in

Fig. 5.1 (c) depend on the feedrate. So, the feedrate needs to be controlled

for the tool to move as programmed.

61

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

Feedrate of linear interpolation (G01), circular interpolation (G02, G03),

5.3

etc. are commanded with numbers after the F code.

CUTTING FEED

In cutting feed, the next block is executed so that the feedrate change from

the previous block is minimized.

Four modes of specification are available:

1.

Feed per minute (G94)

After F, specify the amount of feed of the tool per minute.

2.

Feed per revolution (G95)

After F, specify the amount of feed of the tool per spindle revolution.

3.

Inverse time feed (G93)

Specify the inverse time (FRN) after F.

4.

F1-digit feed

Specify a desired one-digit number after F. Then, the feedrate set with

the CNC for that number is set.

Format

Feed per minute

G94 ; G code (group 05) for feed per minute

F_ ; Feedrate command (mm/min or inch/min)

Feed per revolution

G95 ; G code (group 05) for feed per revolution

F_ ; Feedrate command (mm/rev or inch/rev)

Inverse time feed (G93)

G93 ; Inverse time feed command

G code (05 group)

F_ ; Feedrate command (1/min)

F1-digit feed

Fn ;

n : Number from 1 to 9

Explanations

D Tangential speed

Cutting feed is controlled so that the tangential feedrate is always set at

constant control

a specified feedrate.

Y

Y

Starting

End point

point

F

F

Start

point

Center

End point

X

X

Linear interpolation

Circular interpolation

Fig. 5.3 (a) Tangential feedrate (F)

63

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

D Feed per minute (G94)

After specifying G94 (in the feed per minute mode), the amount of feed

of the tool per minute is to be directly specified by setting a number after

F. G94 is a modal code. Once a G94 is specified, it is valid until G95 (feed

per revolution) is specified. At power-on, the feed per minute mode is

set.

An override from 0% to 254% (in 1% steps) can be applied to feed per

minute with the switch on the machine operator’s panel. For detailed

information, see the appropriate manual of the machine tool builder.

Feed amount per minute

(mm/min or inch/min)

Tool

Workpiece

Table

Fig. 5.3 (b) Feed per minute

WARNING

No override can be used for some commands such as for

threading.

D Feed per revolution

After specifying G95 (in the feed per revolution mode), the amount of

(G95)

feed of the tool per spindle revolution is to be directly specified by setting

a number after F. G95 is a modal code. Once a G95 is specified, it is valid

until G94 (feed per minute) is specified.

An override from 0% to 254% (in 1% steps) can be applied to feed per

revolution with the switch on the machine operator’s panel. For detailed

information, see the appropriate manual of the machine tool builder.

F

Feed amount per spindle revolution

(mm/rev or inch/rev)

Fig. 5.3 (c) Feed per revolution

CAUTION

When the speed of the spindle is low, feedrate fluctuation

may occur. The slower the spindle rotates, the more

frequently feedrate fluctuation occurs.

64

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

D Inverse time feed (G93)

When G93 is specified, the inverse time specification mode (G93 mode)

is set. Specify the inverse time (FRN) with an F code.

A value from 0.001 to 9999.999 can be specified as FRN, regardless of

whether the input mode is inches or metric, or the increment system is

IS-B or IS-C.

F code specification value

FRN

F1

0.001

F1 *1

1.000

F1.0

1.000

F9999999

9999.999

F9999 *1

9999.000

F9999.999

9999.999

NOTE

*1

Value specified in fixed-point format with bit 0 (DPI) of parameter

No. 3401 set to 1

Explanations

For linear interpolation (G01)

1

feedrate

Feedrate:mm/min

(for metric input)

FRN=

=

time (min)

distance

inch/min(for inch input)

Distance:mm

(for metric input)

inch(for inch input)

- To end a block in 1 (min)

1

1

FRN =

=

= 1

Specify F1.0.

time (min)

1 (min)

- To end a block in 10 (sec)

1

1

FRN =

=

= 6

Specify F6.0.

time (sec) / 60

10/60 (sec)

- To find the movement time required when F0.5 is specified

1

1

Time

(min) =

=

= 2

2 (min) is required.

FRN

0.5

- To find the movement time required when F10.0 is specified

1

60

60

Time (sec) =

=

= 6

6 (sec) is required.

FRN

10

For circular interpolation (G01)

1

feedrate Feedrate: mm/min (for metric input)

FRN=

=

time (min) arc radius inch/min(for inch input)

Arc radius: mm (for metric input)

inch(for inch input)

NOTE

In the case of circular interpolation, the feedrate

is

calculated notfrom the actual amount of movement in the

block but from the arcradius.

65

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

G93 is a modal G code and belongs to group 05 (includes G95 (feed per

revolution) and G94 (feed per minute)).

When an F value is specified in G93 mode and the feedrate exceeds the

maximum cutting feedrate, the feedrate is clamped to the maximum

cutting feedrate.

In the case of circular interpolation, the feedrate is calculated not from the

actual amount of movement in the block but from the arc radius. This

means that actual machining time is longer when the arc radius is longer

than the arc distance and shorter when the arc radius is shorter than the arc

distance. Inverse time feed can also be used for cutting feed in a canned

cycle.Notes

NOTE

1

In the G93 mode, an F code is not handled as a modal code and

therefore needs to be specified in each block. If an F code is not

specified, P/S alarm (No. 11 (indicating that cutting feedrate

specification is missing)) is issued.

2

When F0 is specified in G93 mode, P/S alarm (No. 11 (indicating

that cutting feedrate specification is missing)) is issued.

3

Inverse time feed cannot be used when PMC axis control is in

effect.

4

If the calculated cutting feedrate is smaller than the allowable

range, P/S alarm

(No.

11

(indicating that cutting feedrate

specification is missing)) is issued.

66

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

Cutting feedrate can be controlled, as indicated in Table 5.4.

5.4

CUTTING FEEDRATE

CONTROL

Table 5.4 Cutting Feedrate Control

Function name

G code

Validity of G code

Description

Exact stop

This function is valid for specified

The tool is decelerated at the end point

G09

blocks only.

of a block, then an in-position check is

made. Then the next block is executed.

Exact stop mode

Once specified, this function is

The tool is decelerated at the end point

G61

valid until G62, G63, or G64 is

of a block, then an in-position check is

specified.

made. Then the next block is executed.

Cutting mode

Once specified, this function is

The tool is not decelerated at the end

G64

valid until G61, G62, or G63 is

point of a block, but the next block is

specified.

executed.

Tapping mode

Once specified, this function is

The tool is not decelerated at the end

valid until G61, G62, or G64 is

point of a block, but the next block is

G63

specified.

executed.

When G63 is specified, feedrate override

and feed hold are invalid.

Auto- Automatic override for

Once specified, this function is

When the tool moves along an inner

matic

inner corners

valid until G61, G63, or G64 is

corner during cutter compensation, over-

specified.

ride is applied to the cutting feedrate to

G62

suppress the amount of cutting per unit

of time so that a good surface finish can

be produced.

Internal circular cutting

This function is valid in the cutter

The internal circular cutting feedrate is

feedrate change

_

compensation mode, regardless of

changed.

the G code.

NOTE

1

The purpose of in-position check is to check that the servo

motor has reached within a specified range (specified with

a parameter by the machine tool builder).

In-position check is not performed when bit 5 (NCI) of

parameter No. 1601 is set to 1.

2

Inner corner angle θ: 2°< θ x α x 178°

(α is a set value)

Workpiece

θ

Tool

68

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

Format

Exact stop

G09 IP_ ;

Exact stop mode

G61 ;

Cutting mode

G64 ;

Tapping mode

G63 ;

Automatic corner override G62 ;

5.4.1

Exact Stop (G09, G61)

Cutting Mode (G64)

Tapping Mode (G63)

Explanations

The inter-block paths followed by the tool in the exact stop mode, cutting

mode, and tapping mode are different (Fig. 5.4.1).

Y

Position check

(2)

Tool path in the exact stop mode

(1)

Tool path in the cutting mode or

tapping mode

0

X

Fig. 5.4.1 Example of tool paths from block (1) to block (2)

CAUTION

The cutting mode (G64 mode) is set at power-on or system

clear.

69

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

5.4.2

When cutter compensation is performed, the movement of the tool is

automatically decelerated at an inner corner and internal circular area.

Automatic Corner

This reduces the load on the cutter and produces a smoothly machined

Override

surface.

5.4.2.1

Automatic Override for

Inner Corners (G62)

Explanations

D Override condition

When G62 is specified, and the tool path with cutter compensation

applied forms an inner corner, the feedrate is automatically overridden

at both ends of the corner.

There are four types of inner corners (Fig. 5.4.2.1 (a)).

2,xθxθpx178, in Fig. 5.4.2.1 (a)

θp is a value set with parameter No. 1711. When θ is approximately

equal to θp, the inner corner is determined with an error of 0.001,or

less.

1. Straight line-straight line

:Tool

2. Straight line-arc

:Programmed path

:Cutter center path

θ

θ

3. Arc-straight line

4. Arc-arc

θ

θ

Fig. 5.4.2.1 (a) Inner corner

70

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

Override range

When a corner is determined to be an inner corner, the feedrate is

overridden before and after the inner corner. The distances Ls and Le,

where the feedrate is overridden, are distances from points on the cutter

center path to the corner (Fig. 5.4.2.1 (b), Fig. 5.4.2.1 (c), Fig. 5.4.2.1 (d)).

Ls and Le are set with parameter Nos. 1713 and 1714.

Programmed path

Le

Ls

b

a

Cutter center path

The feedrate is overridden from point a to point b.

FIg. 5.4.2.1 (b) Override Range (Straight Line to Straight Line)

When a programmed path consists of two arcs, the feedrate is overridden

if the start and end points are in the same quadrant or in adjacent quadrants

(Fig. 5.4.2.1 (c)).

Le

Programmed path

Ls

a

b

Cutter center path

The feedrate is overridden from point a to b.

Fig. 5.4.2.1 (c) Override Range (Arc to Arc)

Regarding program (2) of an arc, the feedrate is overridden from point a

to point b and from point c to point d (Fig. 5.4.2.1 (d)).

Programmed path

d

a

Le

Ls

Le

Ls

c

b

(2)

Cutter center path

Tool

Fig. 5.4.2.1 (d) Override Range (Straight Line to Arc, Arc to Straight Line)

71

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

Override value

An override value is set with parameter No. 1712. An override value is

valid even for dry run and F1-digit specification.

In the feed per minute mode, the actual feedrate is as follows:

F × (automatic override for inner corners) × (feedrate override)

Limitations

D Acceleration/deceleratio

Override for inner corners is disabled during acceleration/deceleration

n before interpolation

before interpolation.

D Start-up/G41, G42

Override for inner corners is disabled if the corner is preceded by a

start-up block or followed by a block including G41 or G42.

D Offset

Override for inner corners is not performed if the offset is zero.

5.4.2.2

For internally offset circular cutting, the feedrate on a programmed path

is set to a specified feedrate (F) by specifying the circular cutting feedrate

Internal Circular Cutting

with respect to F, as indicated below (Fig. 5.4.2.2). This function is valid

Feedrate Change

in the cutter compensation mode, regardless of the G62 code.

Rc

F

Rp

Rc : Cutter center path radius

Rp : Programmed radius

It is also valid for the dry run and the one-digit F command.

Programmed path

Rc Cutter center

path

Rp

Fig. 5.4.2.2 Internal circular cutting feedrate change

If Rc is much smaller than Rp, Rc/Rp80; the tool stops. A minimum

deceleration ratio (MDR) is to be specified with parameter No. 1710.

When Rc/RpxMDR, the feedrate of the tool is (F×MDR).

NOTE

When internal circular cutting must be performed together with override for inner corners, the

feedrate of the tool is as follows:

Rc

F

(override for the inner corners)×(feedrate override)

Rp

72

Content      ..     1      2      3      4      ..