FANUC Series 0i-MC. OPERATOR’S MANUAL

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

When the tool is moved, the tool path can be shifted by the radius of the

14.4

tool (Fig. 14.4 (a)).

OVERVIEW OF

To make an offset as large as the radius of the tool, CNC first creates an

CUTTER

offset vector with a length equal to the radius of the tool (start-up). The

offset vector is perpendicular to the tool path. The tail of the vector is on

COMPENSATION C

the workpiece side and the head positions to the center of the tool.

(G40-G42)

If a linear interpolation or circular interpolation command is specified

after start-up, the tool path can be shifted by the length of the offset vector

during machining.

To return the tool to the start position at the end of machining, cancel the

cutter compensation mode.

Cutter

compensation

cancel

Start-up

ÇÇÇ

Fig. 14.4 (a) Outline of cutter compensation C

223

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Format

D Start up

G00(or G01)G41(or G42)

IP_ D_ ;

(Tool compensation

G41

: Cutter compensation left (Group07)

start)

G42

: Cutter compensation right (Group07)

: Command for axis movement

: Code for specifying as the cutter compensation value(1-3digits)

(D code)

D Cutter compensation

;

G40

cancel

(offset mode cancel)

G40 : Cutter compensation cancel(Group 07)

(Offset mode cancel)

: Command for axis movement

D Selection of the offset

Offset plane

Command for plane selection

IP_

plane

XpYp

G17 ;

Xp_Yp_

ZpXp

G18 ;

Xp_Zp_

YpZp

G19 ;

Yp_Zp_

Explanations

D Offset cancel mode

At the beginning when power is applied the control is in the cancel mode.

In the cancel mode, the vector is always 0, and the tool center path

coincides with the programmed path.

D Start Up

When a cutter compensation command (G41 or G42, nonzero dimension

words in the offset plane, and D code other than D0) is specified in the

offset cancel mode, the CNC enters the offset mode.

Moving the tool with this command is called start-up.

Specify positioning (G00) or linear interpolation (G01) for start-up. If

circular interpolation (G02, G03) is specified, P/S alarm 34 occurs.

When processing the start-up block and subsequent blocks, the CNC

prereads two blocks.

D Offset mode

In the offset mode, compensation is accomplished by positioning (G00),

linear interpolation (G01), or circular interpolation (G02, G03). If two or

more blocks that do not move the tool (miscellaneous function, dwell,

etc.) are processed in the offset mode, the tool will make either an

excessive or insufficient cut. If the offset plane is switched in the offset

mode, P/S alarm 37 occurs and the tool is stopped.

224

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Offset mode cancel

In the offset mode, when a block which satisfies any one of the following

conditions is executed, the CNC enters the offset cancel mode, and the

action of this block is called the offset cancel.

1. G40 has been commanded.

2. 0 has been commanded as the offset number for cutter

compensation.

When performing offset cancel, circular arc commands (G02 and G03) are

not available. If a circular arc is commanded, an P/S alarm (No. 034) is

generated and the tool stops.

In the offset cancel, the control executes the instructions in that block and

the block in the cutter compensation buffer. In the meantime, in the case

of a single block mode, after reading one block, the control executes it and

stops. By pushing the cycle start button once more, one block is executed

without reading the next block.

Then the control is in the cancel mode, and normally, the block to be

executed next will be stored in the buffer register and the next block is not

read into the buffer for cutter compensation.

Start up

(G41/G42)

Offset cancel mode

Offset mode

Offset modecancel

(G40/D0)

Fig. 14.4 (b) Changing the offset mode

D Change of the

In general, the cutter compensation value shall be changed in the cancel

Cutter compensation

mode, when changing tools. If the cutter compensation value is changed

value

in offset mode, the vector at the end point of the block is calculated for

the new cutter compensation value.

Calculated from the cutter

compensation value in the block

compensation value in the block N7

Programmed path

Fig. 14.4 (c) Changing the cutter compensation value

225

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Positive/negative cutter

If the offset amount is negative (-), distribution is made for a figure in

compensation value and

which G41’s and G42’s are all replaced with each other on the program.

tool center path

Consequently, if the tool center is passing around the outside of the

workpiece, it will pass around the inside, and vice versa.

The figure below shows one example. Generally, the offset amount is

programmed to be positive (+).

When a tool path is programmed as in ((1)), if the offset amount is made

negative

(-), the tool center moves as in

((2)), and vice versa.

Consequently, the same tape permits cutting both male and female

shapes, and any gap between them can be adjusted by the selection of the

offset amount. Applicable if start-up and cancel is A type. (See II- 14.5.2

and 14.5.4)

(1)

(2)

ÇÇÇ

Tool center path

ÇÇÇ

ÇÇ

Programmed path

Fig. 14.4 (d) Tool center paths when positive and negative

cutter compensation values are specified

D Cutter compensation

Assign a cutter compensation values to the D codes on the MDI panel.

value setting

The table below shows the range in which cutter compensation values can

be specified.

mm input

inch input

Cutter compensation value

0 to ±999.999mm

0 to ±99.9999inch

NOTE

The cutter compensation value corresponding to offset No.

0, that is, D0 always means 0. It is impossible to set D0 to

any other offset amount.

Cutter compensation C can be specified by H code with

parameter OFH (No. 5001 #2) set to 1.

D Offset vector

The offset vector is the two dimensional vector that is equal to the cutter

compensation value assigned by D code. It is calculated inside the control

unit, and its direction is up-dated in accordance with the progress of the

tool in each block.

The offset vector is deleted by reset.

D Specifying a cutter

Specify a cutter compensation value with a number assigned to it. The

compensation value

number consists of 1 to 3 digits after address D (D code). The D code is

valid until another D code is specified. The D code is used to specify the

tool offset value as well as the cutter compensation value.

226

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Plane selection and

Offset calculation is carried out in the plane determined by G17, G18 and

vector

G19, (G codes for plane selection). This plane is called the offset plane.

Compensation is not executed for the coordinate of a position which is not

in the specified plane. The programmed values are used as they are.

In simultaneous 3 axes control, the tool path projected on the offset plane

is compensated.

The offset plane is changed during the offset cancel mode. If it is

performed during the offset mode, a P/S alarm (No. 37) is displayed and

the machine is stopped.

227

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Examples

250R

C1(700,1300)

C3 (-150,1150)

P4(500,1150) P5(900,1150)

C2 (1550,1550)

650R

P3(450,900)

P6(950,900)

(1150,900)

(250,900)

P9(700,650)

(250,550)

(1150,550)

N10

Y axis

N11

Unit : mm

ÇÇÇ

X axis

Start position

ÇÇÇ

ÇÇ

G92 X0 Y0 Z0 ;

Specifies absolute coordinates.

The tool is positioned at the start position (X0, Y0, Z0).

N1 G90 G17 G00 G41 D07 X250.0 Y550.0 ; Starts cutter compensation (start-up). The tool is shifted to the

left of the programmed path by the distance specified in D07.

In other words the tool path is shifted by the radius of the tool

(offset mode) because D07 is set to 15 beforehand (the radius of

the tool is 15 mm).

N2 G01 Y900.0 F150 ;

Specifies machining from P1 to P2.

N3 X450.0 ;

Specifies machining from P2 to P3.

N4 G03 X500.0 Y1150.0 R650.0 :

Specifies machining from P3 to P4.

N5 G02 X900.0 R-250.0 ;

Specifies machining from P4 to P5.

N6 G03 X950.0 Y900.0 R650.0 ;

Specifies machining from P5 to P6.

N7 G01 X1150.0 ;

Specifies machining from P6 to P7.

N8 Y550.0 ;

Specifies machining from P7 to P8.

N9 X700.0 Y650.0 ;

Specifies machining from P8 to P9.

N10 X250.0 Y550.0 ;

Specifies machining from P9 to P1.

N11 G00 G40 X0 Y0 ;

Cancels the offset mode.

The tool is returned to the start position (X0, Y0, Z0).

228

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

This section provides a detailed explanation of the movement of the tool

14.5

for cutter compensation C outlined in Section 14.4.

DETAILS OF CUTTER

This section consists of the following subsections:

COMPENSATION C

14.5.1

General

14.5.2 Tool Movement in Start-up

14.5.3 Tool Movement in Offset Mode

14.5.4 Tool Movement in Offset Mode Cancel

14.5.5 Interference Check

14.5.6 Overcutting by Cutter Compensation

14.5.7

Input Command from MDI

14.5.8

G53,G28,G30 and G29 Commands in Cutter

Compensation C Mode

14.5.9

Corner Circular Interpolation (G39)

14.5.1

General

D Inner side and outer side

When an angle of intersection created by tool paths specified with move

commands for two blocks is over 180°, it is referred to as “inner side.”

When the angle is between 0° and 180°, it is referred to as “outer side.”

Inner side

Outer side

Programmed path

Workpiece

Programmed path

180°xα

0°xα<180°

D Meaning of symbols

The following symbols are used in subsequent figures:

- S indicates a position at which a single block is executed once.

- SS indicates a position at which a single block is executed twice.

- SSS indicates a position at which a single block is executed three times.

- L indicates that the tool moves along a straight line.

- C indicates that the tool moves along an arc.

- r indicates the cutter compensation value.

- An intersection is a position at which the programmed paths of two

blocks intersect with each other after they are shifted by r.

- indicates the center of the tool.

229

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

14.5.2

When the offset cancel mode is changed to offset mode, the tool moves

as illustrated below (start-up):

Tool Movement in

Start-up

Explanations

D Tool movement around

an inner side of a corner

Linear→Linear

(180°xα)

Workpiece

Programmed path

G42

Tool center path

Start position

Linear→Circular

Work-

G42

piece

Start

position

Tool center path

230

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool movement around

Tool path in start-up has two types A and B, and they are selected by

the outside of a corner at

parameter SUP (No. 5003#0).

an obtuse angle

(90°xα<180°)

Linear→Linear

Start position

G42

Workpiece

Programmed path

Tool center path

Type

Linear→Circular

Start position

G42

Work-

piece

Tool center path

Programmed path

Linear→Linear

Start position

G42

Workpiece

Programmed path

Tool center path

Intersection

Type

Linear→Circular

Start position

G42

Work-

piece

Intersection

Tool center path

Programmed path

231

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Tool movement around

Tool path in start-up has two types A and B, and they are selected by

the outside of an acute

parameter SUP (No.5003#0).

angle (α<90°)

Linear→Linear

Start position

G42

Workpiece

α L

Programmed path

Tool center path

Type

Linear→Circular

Start position

G42

Work-

piece

Tool center path

Programmed path

Linear→Linear

Start position

G42

Workpiece

Programmed path

Tool center path

Type

Linear→Circular

Start position

G42

Work-

piece

Tool center path

Programmed path

D Tool movement around

the outside linear→linear

Tool center path

at an acute angle less

than 1 degree

(α<1°)

Programmed path

G41

Start position

Less than 1 deg

232

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

14.5.3

In the offset mode, the tool moves as illustrated below:

Tool Movement in

Offset Mode

Explanations

D Tool movement around

the inside of a corner

Linear→Linear

(180°xα)

Workpiece

Programmed path

Tool center path

Intersection

Linear→Circular

Work-

piece

Intersection

Programmed path

Tool center path

Circular→Linear

Workpiece

Programmed path

Tool center path

Intersection

Circular→Circular

Work-

Intersection

piece

Programmed path

Tool center path

234

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Tool movement around

the outside corner at an

Linear→Linear

obtuse angle

(90°xα<180°)

Workpiece

Programmed path

Intersection

Tool center path

Linear→Circular

Work-

piece

Intersection

Programmed path

Tool center path

Circular→Linear

Workpiece

Programmed path

IntersectionSL

Tool center path

Circular→Circular

Programmed path

Work-

piece

Tool center path

Intersection

236

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool movement around

the outside corner at an

acute angle

Linear→Linear

(α<90°)

Workpiece

Programmed path

Tool center path

Linear→Circular

Work-

piece

Programmed path

Tool center path

Circular→Linear

Workpiece

Programmed path

Tool center path

Circular→Circular

Work-

piece

Tool center path Programmed path

237

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D When it is exceptional

End position for the arc is not

If the end of a line leading to an arc is programmed as the end of the arc

on the arc

by mistake as illustrated below, the system assumes that cutter

compensation has been executed with respect to an imaginary circle that

has the same center as the arc and passes the specified end position. Based

on this assumption, the system creates a vector and carries out

compensation. The resulting tool center path is different from that created

by applying cutter compensation to the programmed path in which the

line leading to the arc is considered straight.

Leading of the arc End the arc

Work-

Imaginary circle

piece

Programmed path

Tool center path

Center of the arc

The same description applies to tool movement between two circular

paths.

There is no inner intersection

If the cutter compensation value is sufficiently small, the two circular tool

center paths made after compensation intersect at a position

(P).

Intersection P may not occur if an excessively large value is specified for

cutter compensation. When this is predicted, P/S alarm No.033 occurs

at the end of the previous block and the tool is stopped. In the example

shown below, tool center paths along arcs A and B intersect at P when a

sufficiently small value is specified for cutter compensation. If an

excessively large value is specified, this intersection does not occur.

Alarm(No.033)occurs and the tod stops

When the cutter compensation value

is large

When the cutter compensa-

tion value is small

Center of the arc B

Center of the arc A

Programmed path

Arc A

Arc B

238

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

The center of the arc is identiĆ

If the center of the arc is identical with the start position or end point, P/S

cal with the start position or

alarm (No. 038) is displayed, and the tool will stop at the end position of

the end position

the preceding block.

Alarm(No.038)is displayed and the tool

(G41)

stops

N5 G01 X100.0 ;

N6 G02 X100.0 I0 J0 ;

N7 G03 Y-100.0 J-100.0 ;

Tool center path

Programmed path

D Change in the offset

The offset direction is decided by G codes (G41 and G42) for cutter radius

direction in the offset

and the sign of cutter compensation value as follows.

mode

Sign of offset amount

Gcode

G41

Left side offset

Right side offset

G42

Right side offset

Left side offset

The offset direction can be changed in the offset mode. If the offset

direction is changed in a block, a vector is generated at the intersection

of the tool center path of that block and the tool center path of a preceding

block. However, the change is not available in the start-up block and the

block following it.

239

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Tool center path with an inter-

section

Linear→Linear

Workpiece

G42

Programmed path

G41

Tool center path

Workpiece

Linear→Circular

Workpiece

G41

G42

Programmed path

Workpiece

Tool center path

Circular→Linear

Workpiece

G42

Programmed path

Tool center path

G41

Workpiece

Circular→Circular

Workpiece

G42

Programmed path

G41

Tool center path

Workpiece

240

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

Tool center path without an in-

When changing the offset direction in block A to block B using G41 and

tersection

G42, if intersection with the offset path is not required, the vector normal

to block B is created at the start point of block B.

Linear→Linear

Workpiece

(G42)

G41

Programmed path

Workpiece

Tool center path

G42

Programmed path

G41

Tool center path

Linear→Circular

Tool center path

(G41)

G42

(G41)

Programmed path

Circular→Circular

An arc whose end position

is not on the arc

G41

Programmed path

(G42)

L SL

Tool center path

Center

241

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

The length of tool center path Normally there is almost no possibility of generating this situation.

larger than the circumference However, when G41 and G42 are changed, or when a G40 was

of a circle

commanded with address I, J, and K this situation can occur.

In this case of the figure, the cutter compensation is not performed with

more than one circle circumference: an arc is formed from P₁ to P₂ as

shown. Depending on the circumstances, an alarm may be displayed due

to the “Interference Check” described later. To execute a circle with more

than one circumference, the circle must be specified in segments.

Tool center path

Programmed path

P₁

P₂

(G42)

N5 G01 G91 X500.0 Y-700.0 ;

N6 G41 G02 J-500.0 ;

N7 G42 G01 X500.0 Y700.0 ;

242

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Temporary cutter

If the following command is specified in the offset mode, the offset mode

compensation cancel

is temporarily canceled then automatically restored. The offset mode can

be canceled and started as described in II-14.5.2 and 14.5.4.

Specifying G28 (automatic re-

If G28 is specified in the offset mode, the offset mode is canceled at an

turn to the reference position)

intermediate position. If the vector still remains after the tool is returned

in the offset mode

to the reference position, the components of the vector are reset to zero

with respect to each axis along which reference position return has been

made.

G28

Intermediate position

G00

(G42 G00)

Reference position

Specifying G29 (automatic re-

If G29 is commanded in the offset mode, the offset will be cancelled at

turn from the reference posi-

the intermediate point, and the offset mode will be restored automatically

tion) in the offset mode

from the subsequent block.

G29 specified immediately after G28

Intermediate position

Programmed path

G28

G29

G00

(G42 G00)

Tool center path Reference position

G29 specified not immediately after G28

Intermediate position

Programmed path

G29

G00

(G42 G00)

Tool center path

243

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Cutter compensation G

The offset vector can be set to form a right angle to the moving direction

code in the offset mode

in the previous block, irrespective of machining inner or outer side, by

commanding the cutter compensation G code (G41, G42) in the offset

mode, independently. If this code is specified in a circular command,

correct circular motion will not be obtained.

When the direction of offset is expected to be changed by the command

of cutter compensation G code (G41, G42), refer to “change in the offset

direction in the offset mode” in this Subsec.14.5.3.

Linear→Linear

G42 mode

A block specified by G42

Tool center path

Intersection

Circular→Linear

A block specified by G42

G42 mode

S Intersection

Programmed path

D Command cancelling the

During offset mode, if G92 (absolute zero point programming) is

offset vector temporarily

commanded,the offset vector is temporarily cancelled and thereafter

offset mode is automatically restored.

In this case, without movement of offset cancel, the tool moves directly

from the intersecting point to the commanded point where offset vector

is canceled. Also when restored to offset mode, the tool moves directly

to the intersecting point.

Tool center path

Programmed path

(G41)

G92 block

N5 G91 G01 X300.0 Y700.0 ;

N6 X-300.0 Y600.0 ;

N7 G92 X100.0 Y200.0 ;

N8 G90 G01 X400.0 Y800.0 ;

244

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D A block without tool

The following blocks have no tool movement. In these blocks, the tool

movement

will not move even if cutter compensation is effected.

M05 ; . M code output

S21 ; . S code output

G04 X10.0 ; Dwell

Commands (1)

G10 L11 P01 R10.0 ; Cutter compensation value setting

to (6) are of no

(G17) Z200.0 ; Move command not included in the

movement.

offset plane.

G90 ; . G code only

G91 X0 ; Move distance is zero.

When a single block without tool movement is commanded in the offset

A block without tool move-

ment specified in offset mode

mode, the vector and tool center path are the same as those when the block

is not commanded. This block is executed at the single block stop point.

N6 G91 X100.0 Y100.0 ;

N7 G04 X100.0 ;

Programmed path

N8 X100.0 ;

Tool center path

Block N7 is executed here.

However, when the move distance is zero, even if the block is commanded

singly, tool motion becomes the same as that when more than one block

of without tool movement are commanded, which will be described

subsequently.

N6 G91 X100.0 Y100.0 ;

Programmed path

N7 X0 ;

N8 X100.0 ;

Tool center path

Two blocks without tool movement should not be commanded

consecutively. If commanded, a vector whose length is equal to the offset

value is produced in a normal direction to tool motion in earlier block, so

overcutting may result.

N6 G91 X100.0 Y100.0 ;

N7 N8

Programmed path

N7 S21 ;

N8 G04 X10.0 ;

N9 X100.0 ;

SSS

Tool center path

Blocks N7 and N8 are executed

here.

245

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Corner movement

When two or more vectors are produced at the end of a block, the tool

moves linearly from one vector to another. This movement is called the

corner movement.

If these vectors almost coincide with each other, the corner movement

isn’t performed and the latter vector is ignored.

nVx

Tool center path

nV_Y

This vector is ignored, if

∆Vxx∆V Limit, and

∆V_Yx∆V Limit

Programmed path

If ∆Vxx∆Vlimit and ∆Vyx∆Vlimit, the latter vector is ignored. The

∆Vlimit is set in advance by parameter (No. 5010).

If these vectors do not coincide, a move is generated to turn around the

corner. This move belongs to the latter block.

This move belongs to block N7, thus, the feedrate

is equal to that in block N7.

If the block N7 is G00 mode, the tool is moved at

G00 mode, while if it is G01, G02, G03, the tool is

moved at G01 mode.

However, if the path of the next block is semicircular or more, the above

function is not performed.

The reason for this is as follows:

246

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

N4 G41 G91 G01 X150.0 Y200.‘0 ;

P₂ P3P4P5

N5 X150.0 Y200.0 ;

N6 G02 J-600.0 ;

N7 G01 X150.0 Y-200.0 ;

P₁

N8 G40 X150.0 Y-200.0 ;

P₆

N₇

N₅

N₄

N₈

Programmed path

Tool center path

N₆

If the vector is not ignored, the tool path is as follows:

P₁ → P₂ → P₃ → (Circle) → P₄ → P₅ → P₆

But if the distance between P2 and P3 is negligible, the point P3 is

ignored. Therefore, the tool path is as follows:

P₂ → P₄

Namely, circle cutting by the block N6 is ignored.

D Interruption of manual

For manual operation during the cutter compensation, refer to Section

operation

III-3.5, “ Manual Absolute ON and OFF.”

247

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool movement around

Tool path has two types, A and B; and they are selected by parameter SUP

an outside corner at an

(No. 5003#0).

obtuse angle

(90°xα<180°)

Linear→Linear

G40

Workpiece

Programmed path

Tool center path

Type

Circular→Linear

G40

Work-

piece

Programmed path

Tool center path

Linear→Linear

G40

Workpiece

Programmed path

Tool center path

Intersection

Type

Circular→Linear

G40

Work-

piece

LIntersection

Programmed path

Tool center path

249

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Tool movement around

Tool path has two types, A and B : and they are selected by parameter SUP

an outside corner at an

(No. 5003#0)

acute angle

(α<90°)

Linear→Linear

G40

Workpiece

L α

Programmed path

G42

Tool center path

Type

Circular→Linear

G40

G42

Work-

piece

Tool center path

Programmed path

Linear→Linear

G40

Workpiece

Programmed path

Tool center path

Type

Circular→Linear

Work-

piece

Tool center path

Programmed path

250

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

D Tool movement around

the outside linear→linear

Tool center path

at an acute angle less

than 1 degree (α<1°)

Programmed path

(G42)

1°or less

G40

Start position

D A block without tool

When a block without tool movement is commanded together with an

movement specified

offset cancel, a vector whose length is equal to the offset value is produced

together with offset

in a normal direction to tool motion in the earlier block, the vector is

cancel

cancelled in the next move command.

N6 G91 X100.0 Y100.0

;

N7 G40 ;

N8 X100.0 Z0 ;

Programmed path

Tool center path

251

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

D Block containing G40

and I_J_K_

The previous block contains If a G41 or G42 block precedes a block in which G40 and I_, J_, K_ are

G41 or G42

specified, the system assumes that the path is programmed as a path from

the end position determined by the former block to a vector determined

by (I,J), (I,K), or (J,K). The direction of compensation in the former block

is inherited.

N1 (G42 mode) ;

In the N1 block, the tool center moves towards X.

N2 G40 Xa Yb I_ J_ ;

In the N2 block, the tool moves towards E.

E(a, b)

(I, J)

G40

Tool center path

(G42) Programmed path

Workpiece

In this case, note that the CNC obtains an intersection of the tool path

irrespective of whether inner or outer side machining is specified

G40

Tool center path

Programmed path

(G42)

(I, J)

When an intersection is not obtainable, the tool comes to the normal

position to the previous block at the end of the previous block.

G40

Tool center path

(G42)

Programmed path

(I, J)

252

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 9