FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Tool movement around the outside corner at an obtuse angle (90°≤α<180°)

Linear→Linear

(Linear

connection type)

Workpiece

Programmed path

Intersection

Tool center path

Linear→Circular

(Linear

connection type)

Work-

piece

S L

Intersection

Tool center path Programmed path

Circular→Linear

(Linear connection type)

Workpiece

Programmed path

Intersection S

Tool center path

Circular→Circular

(Linear

connection type)

Programmed path

Work-

piece

Tool center

path

Intersection

- 166 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

Linear→Linear

(Circular

connection type)

Workpiece

Programmed path

Tool center path

Linear→Circular

(Circular

connection type)

Work-

piece

Tool center path

Programmed path

Circular→Linear

(Circular

connection type)

Workpiece

Programmed path

Tool center path

Circular→Circular

(Circular

connection type)

Programmed path

Work-

piece

Tool center path

- 167 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Tool movement around the outside corner at an acute angle (α<90°)

Linear→Linear

(Linear

connection type)

Workpiece

Programmed path

Tool center path

Linear→Circular

(Linear

connection type)

Work-

piece

Programmed path

Tool center path

Circular→Linear

(Linear

connection type)

Workpiece

Programmed path

Tool center path

Circular→Circular

(Linear

connection type)

Work-

piece

Tool center path

Programmed path

- 168 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

Linear→Linear

(Circular

connection type)

Workpiece

Programmed path

Tool center path

Linear→Circular

(Circular

connection type)

Work-

piece

Programmed path

Tool center path

Circular→Linear

(Circular

connection type)

Workpiece

Programmed path

Tool center path

Circular→Circular

(Circular

connection type)

Work-

piece

Tool center path

Programmed path

- 169 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- When it is exceptional

End point for the arc is not on the arc

If the end of a line leading to an arc is not on the arc as illustrated

below, the system assumes that the cutter compensation has been

executed with respect to an imaginary circle that has the same center

as the arc and passes the specified end point. Based on this

assumption, the system creates a vector and carries out compensation.

The same description applies to tool movement between two circular

paths.

End the arc

Work-

piece

Imaginary circle

Programmed path

Tool center path

Center of the arc

L S

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, PS0033 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 occurs and the tool stops

When the cutter compensation

value is large

When the cutter compensation

value is small

Center of the arc B

Center of the arc A

Programmed path

Arc A

Arc B

- 170 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- When the center of the arc is identical with the start point or the end point

If the center of the arc is identical with the start point or end point,

PS0041 is displayed, and the tool will stop at the start point of the

preceding block of the arc.

(G41)

N5 G91 G01 X50.0 ;

Tool center path

N6 X50.0 ;

N7 G02 X100.0 I0 J0 ;

Alarm is displayed and the

N8 G01 Y-100.0 ;

tool stops

Programmed path

- Change in the offset direction in the offset mode

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

compensation and the sign of the compensation value as follows.

Sign of compensation

G code

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.

- 171 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Tool center path with an intersection

Linear→Linear

Workpiece

G42

Intersection

Programmed path

G41

Workpiece

Tool center path

Linear→Circular

Workpiece

G41

G42

Programmed path

Workpiece

Intersection

Tool center path

Circular→Linear

Workpiece

G42

Programmed path

Tool center path

Intersection

G41

Workpiece

Circular→Circular

Workpiece

G42

Programmed path

G41

Tool center path

Workpiece

Intersection

- 172 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Tool center path without an intersection

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

and 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

W orkpiece

(G42)

Programmed path

G42

G41

W orkpiece

Tool center path

G42

Programmed path

G41

Tool center path

Linear→Circular

Intersection

Tool center path

(G41)

G42

(G41)

Programmed path

Circular→Circular

An arc whose end position

is not on the arc

G41

(G42)

Programmed path

(G42)

Center

Tool center path

- 173 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- The length of tool center path larger than the circumference of a circle

Normally there is almost no possibility of generating this situation.

However, when G41 and G42 are changed, or when a G40 was

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 item, "Interference Check" described later.

execute a circle with more than one circumference, the circle must be

specified in segments.

Tool center path Programmed path

(G42)

N5 G01 G91 X500.0 Y-700.0 ;

N6 G41 G02 J-500.0 ;

N7 G42 G01 X500.0 Y700.0 ;

- 174 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Cutter compensation G code in the offset mode

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

direction 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), see "Change in

the offset direction in the offset mode".

Linear→Linear

A block specified by G42

G42 mode

Tool center path

Intersection

Circular→Linear

A block specified by G42

G42 mode

Intersection

Programmed path

- 175 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Command canceling the offset vector temporarily

During offset mode, if G92 (workpiece coordinate system setting) or

G52 (local coordinate system setting) is 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

G92 block

(G41)

N5 G01 X700.0 Y300.0 ;

N6 X600.0 Y-300.0 ;

N7 G92 X200.0 Y100.0 ;

N8 G01 X800.0 Y400.0 ;

Before specifying G28 (reference position return), G29 (movement

from reference position), G30 (second, third, and fourth reference

position return), and G53

(machine coordinate system selection)

commands, cancel offset mode, using G40. If an attempt is made to

specify any of the commands in offset mode, the offset vector

temporarily disappears.

- 176 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If I, J, and K are specified in a G00/G01 mode block

At the start of cutter compensation or in that mode, by specifying I, J,

and K in a positioning mode (G00) or linear interpolation mode (G01)

block, it is possible to set the compensation vector at the end point of

that block in the direction vertical to that specified by I, J, and K.

This makes it possible to change the compensation direction

intentionally.

IJ type vector (XY plane)

The following explains the compensation vector (IJ type vector) to be

created on the XY compensation plane (G17 mode).

(The same

explanation applies to the KI type vector on the G18 plane and the JK

type vector on the G19 plane.) As shown in the figure below, it is

assumed that the compensation vector (IJ type vector) is the vector

with a size equal to the compensation value and vertical to the

direction specified by I and J, without performing intersection

calculation on the programmed path. I and J can be specified both at

the start of cutter compensation and in that mode. If they are

specified at the start of compensation, any start-up type set in the

appropriate parameter will be invalid, and an IJ type vector is

assumed.

Offset vector direction

In G41 mode, the direction specified by I, J, and K is assumed an

imaginary tool movement direction, and an offset vector is created

vertical to that direction and on the left side.

Compensation vector

I, J, K

In G42 mode, the direction specified by I, J, and K is assumed an

imaginary tool movement direction, and an offset vector is created

vertical to that direction and on the right side.

I, J, K

Compensation vector

- 177 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Example

If I and J are specified at the start of compensation (with

tool movement)

N50

N40

(G40)

N30

N60

N10 G91 G41 X100.0 Y100.0

N20

I1 D1 ;

N20 G04 X1000 ;

Tool center path

N30 G01 F1000 ;

N10

N40 S300 ;

N50 M50 ;

Programmed path

N60 X150. ;

Note) In N10, a vector is

specified with a size of D1

in the direction vertical to

the X axis, using I1.

If I and J are specified at the start of compensation

(without tool movement)

(G40)

N30

N10 G41 I1 D1 ;

N20 G91 X100. Y100. ;

Tool nose radius

N30 X150. ;

center path

N20

Note) In N10, a vector is

Programmed path

specified with a size

of D1 in the direction

N10

vertical to the X axis,

using I1.

If I and J are specified at the start of compensation (with

tool movement)

(G17 G41 G91 D1)

N10 G00 X150. J50. ;

N20 G02 I50. ;

(I,J)

N30 G00 X-150. ;

<2>

Note) In N10, a vector is specified

N10

N20

with a size of D1 in the

N30

direction vertical to the Y axis,

<1>

using J50.

<2>

<1> IJ type vector

<2> Vector determined with

intersection calculation

Tool center path

Programmed path

Path determined with

intersection calculation

- 178 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

If I and J are specified in a block without tool movement in

compensation mode

N30

N40

Tool center

S S

path

Start-up/cancel type C

N20

N50

N10 G41 D1 G01 F1000 ;

(I, J)

N20 G91 X100. Y100. ;

Programmed path

N30 I10. ;

N40 X150. ;

N50 G40 ;

N10

Limitation

If an IJ type vector is specified, tool interference may occur due to that

vector alone, depending on the direction. If this occurs, no

interference alarm will occur, or no interference avoidance will be

performed. Overcutting may, therefore, result.

Overcutting

(I, J)

Start-up/cancel

Type C

N40

N30

Programmed

N10 G42 D1 F1000 ;

N20

path

N20 G91 X100. ;

N30 X100. Y-100. I10. ;

N10

N50

N40 X100. Y-100. ;

N50 G40 ;

Tool center path

- A block without tool movement

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

tool will not move even if cutter compensation is effected.

M05 ;

M code output

S21 ;

S code output

G04 X10.0 ;

Dwell

G22 X100000 ;

Machining area setting

G10 L11 P01 R10.0 ;

Cutter compensation value setting/changing

(G17) Z200.0 ;

Move command not included in the offset plane.

G90 ;, O10 ;, N20 ;

G, O, and N codes only

G91 X0 ;

Move distance is zero.

- 179 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- A block without tool movement specified in offset mode

Unless the number of blocks without movement consecutively

specified is more than N-2 blocks (where N is the number of blocks to

read in offset mode (parameter No. 19625)) in offset mode, the vector

and the tool center path will be as usual. This block is executed at

the single block stop point.

N6 G91 X100.0 Y100.0 ;

Programmed path

N7 G04 X10.0 ;

N8 X100.0 ;

Tool center path

Block N7 is executed here.

For an axis command for which the move distance is zero, however, a

vector with a size equal to the compensation value will be created

vertical to the movement direction in the previous block, even if the

number of block is 1. Note that specifying such a command may

result in overcutting.

N6 G91 X100.0 Y100.0 ;

N7 X0 ;

Programed path

N8 X100.0 ;

Tool center path

In offset mode, the number of blocks without movement consecutively

specified must not exceed N-2 (where N is the number of blocks to

read in offset mode

(parameter

(No. 19625)). 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

N7 S21 ;

Programmed path

N8 G04 X10.0 ;

N9 X100.0 ;

(No. of blocks to read in

offset mode = 3)

Tool center path

SSS

L Blocks N7 and N8 are executed here.

- 180 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If an M/G code that suppresses buffering is specified

If an M/G code that suppresses buffering is specified in offset mode, it

is no longer possible to read and analyze subsequent blocks regardless

of the number of blocks to read in offset mode, which is determined

by parameter

(No.

19625). Then, intersection calculation and a

interference check, described later, are no longer possible. If this

occurs, overcutting may occur because a vertical vector is output in

the immediately preceding block.

If an M code (M50) that suppresses buffering is not specified

(G42)

N5 G91 G01 X40.0 Y40.0 ;

Programmed path

N6 X40.0 ;

Tool center path

Intersection

If an M code (M50) that suppresses buffering is specified

(G42)

Programmed path

N5 G91 G01 X40.0 Y40.0 ;

N6 M50 ;

N7 X40.0 ;

Tool center path

Block N6 is executed here.

- 181 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Corner movement

When two or more offset 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 distance of corner

movement between the vectors is judged short due to the setting of

parameter (No. 5010)), corner movement is not performed. In this

case, the vector to the single block stop point takes precedence and

remains, while other vectors are ignored. This makes it possible to

ignore the very small movements arising from performing cutter

compensation, thereby preventing velocity changes due to interruption

of buffering.

This vector is ignored, if

∆V_X

∆V_X≤ ∆V_limitand

∆V_Y≤ ∆V_limit

∆V_Y

The vector to the single block

stop point remains even if

∆V_X ≤ ∆V_limit and ∆V_Y ≤ V_limit.

Tool center path

Programmed path

∆V_limit is determined with the setting of parameter (No. 5010).

If the vectors are not judged to almost coincide (therefore, are not

erased), movement to turn around the corner is performed. The

corner movement that precedes the single block stop point belongs to

the previous block, while the corner movement that succeeds the

single block stop point belongs to the latter block.

This move belongs to block N6, thus, the feedrate is equal

to that in block N6.

This move belongs to block N7, thus, the

feedrate is equal to that in block N7.

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

above function is not performed.

- 182 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

The reason for this is as follows:

P₂ P₃ P₄ P5

N4 G41 G91 G01 X150.0 Y200.0 ;

N5 X150.0 Y200.0 ;

N6 G02 J-600.0 ;

N7 G01 X150.0 Y-200.0 ;

P₁

P₆

N8 G40 X150.0 Y-200.0 ;

N₅ N7

N₄

N₈

N₆

Programmed path

Tool center path

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.

- Interruption of manual operation

For manual operation during the offset mode, see "Manual Absolute

ON and OFF."

- 183 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.4

Tool Movement in Offset Mode Cancel

Explanation

- If the cancel block is a block with tool movement, and the tool moves around the

inside (180° ≤ α)

Linear→Linear

Workpiece

Programmed path

G40

Tool center path

Circular→Linear

Work-

piece

G40

Programmed path

Tool center path

- 184 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If the cancel block is a block with tool movement, and the tool moves around the

outside at an obtuse angle (90° ≤ α < 180°)

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

SUP (No.5003#0).

Linear→Linear

G40

Workpiece

Programmed path

Tool center path L

Type

Circular→Linear

G40

Work-

piece

Programmed path

Tool center path

Linear→Linear

(Linear

connection type)

G40

Workpiece

Programmed path

Tool center path

Intersection

Type

Circular→Linear

(Linear

connection type)

G40

Work-

piece

Inter-

section

Programmed path

Tool center path

- 185 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If the cancel block is a block with tool movement, and the tool moves around the

outside at an acute angle (α<90°)

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

SUP (No.5003#0).

Linear→Linear

G40

W orkpiece

Programmed path

G42

Tool center path

Type

Circular→Linear

G40

W ork-

piece

G42

Tool center path

Programmed path

Linear→Linear

(Linear

connection type)

W orkpiece

G40

Programmed path

Tool center path

Type

Circular→Linear

(Linear

connection type)

W ork-

piece

Tool center path

Programmed path

- 187 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Linear→Linear

(Circular

connection type)

Workpiece

G40

Programmed path

Tool center path

Type

Circular→Linear

(Circular

connection type)

Work-

piece

Tool center path

Programmed path

- If the cancel block is a block with tool movement, and the tool moves around the

outside at an acute angle of 1 degree or less in a linear → linear manner (α≤1°)

Tool center path

Programmed path

(G42)

1° or less

G40

- 188 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- A block without tool movement specified together with offset cancel

For types A and B

In the block preceding the cancel block, a vector is created with a

size equal to the cutter compensation value in the vertical

direction. The tool does not operate in the cancel block. The

remaining vectors are canceled with the next move command.

N6 G91 X100.0 Y100.0 ;

N7 G40 ;

N8 X130.0 ;

Programmed path

Tool center path

For type C

The tool shifts by the compensation value in the direction vertical

to the block preceding the cancel block.

Programmed path

Tool center path

G40 (without

movement)

- 189 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Block containing G40 and I_J_K_

The previous block contains G41 or G42

If a G41 or G42 block precedes a block in which G40 and I_, J_, K_

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

path from the end point 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 nose radius center moves

towards P.

N2 G40 Xa Yb I_ J_ ;

In the N2 block, the tool nose radius moves towards E.

E(a, b)

(I, J)

G40

Tool center path

(G42) Programamed 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)

- 190 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Length of the tool center path larger than the circumference of a circle

In the Example shown below, the tool does not trace the circle more

than once. It moves along the arc from P₁ to P₂. The interference

check function described below may raise an alarm.

To make the tool trace a circle more than once, program two or more

arcs.

P₁

Tool center path

P₂

Programmed path

(I, J)

(G41)

N5 G01 G91 X100.0 ;

N6 G02 J-60.0 ;

N7 G40 G01 X50.0 Y50.0 I-10.0 J-10.0 ;

- 191 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.5

Prevention of Overcutting Due to Cutter Compensation

Explanation

- Machining a groove smaller than the diameter of the tool

Since the cutter compensation forces the tool center path to move in

the reverse of the programmed direction, overcutting will result. In

this case an alarm is displayed and the CNC stops at the start of the

block.

An alarm is displayed and

Tool center path

the operation stops

Programmed path

Workpiece

Overcutting if the operation would not stop

Fig. 6.6.5 (a) Machining a groove smaller than the diameter of the tool

- 192 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Machining a step smaller than the tool radius

For a figure in which a workpiece step is specified with an arc, the

tool center path will be as shown in Fig. 6.6.5 (b). If the step is

smaller than the tool radius, the tool center path usually compensated

as shown in Fig. 6.6.5 (c) may be in the direction opposite to the

programmed path. In this case, the first vector is ignored, and the

tool moves linearly to the second vector position. The single block

operation is stopped at this point. If the machining is not in the

single block mode, the cycle operation is continued.

If the step is of linear, no alarm will be generated and cut correctly.

However uncut part will remain.

Single block stop point

Tool center path

Programmed path

Arc center

Workpiece

Fig. 6.6.5 (b) Machining a step larger than the tool radius

Single block stop point

Linear movement

Tool center path

Path to be taken if

the

Programmed path

vector is not ignored

The first vector is ignored

Arc center

Arc

Workpiece

An overcutting will result if the first vector is not ignored.

However, tool moves linearly.

Fig. 6.6.5 (c) Machining a step smaller than the tool radius

- 193 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Starting compensation and cutting along the Z-axis

It is usually used such a method that the tool is moved along the Z

axis after the cutter compensation (normally XY plane) is effected at

some distance from the workpiece at the start of the machining. In

the case above, if it is desired to divide the motion along the Z axis

into rapid traverse and cutting feed, follow the procedure below.

Let us consider the following program, assuming the number of blocks

to read in cutter compensation mode (parameter (No. 19625)) to be 3.

N1 G91 G00 G41 X500.0 Y500.0 D1 ;

N3 G01 Z-300.0 F100 ;

N6 Y1000.0 F200 ;

After compensation

Workpiece

N3:Move command in Z axis (one block)

In the program example above, when executing block N1, blocks N3

and N6 are also entered into the buffer storage, and by the relationship

among them the correct compensation is performed as in the figure

above.

Then, suppose that the block N3 (move command in Z axis) is divided

into N3 and N5.

N1 G91 G00 G41 X500.0 Y500.0 D1 ;

N3 G01 Z-250.0 ;

N5 G01 Z-50.0 F100 ;

N6 Y1000.0 F200 ;

After compensation

Workpiece

N3, N5:Move command for the Z axis (two blocks)

At this time, because the number of blocks to read is 3, blocks up to

N5 can be read at the start of N1 compensation, but block N6 cannot

be read. As a result, compensation is performed only on the basis of

the information in block N1, and a vertical vector is created at the end

of the compensation start block. Usually, therefore, overcutting will

result as shown in the figure above.

- 194 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

In such a case, it is possible to prevent overcutting by specifying a

command with the exactly the same direction as the advance direction

immediately before movement along the Z axis beforehand, after the

tool is moved along the Z axis using the above rule.

N1 G91 G00 G41 X500.0 Y400.0 D1 ;

N2 Y100.0 ;

N3 Z-250.0 ;

N5 G01 Z-50.0 F100 ;

N6 Y1000.0 F200 ;

After compensation

W orkpiece

N3, N5 : Move command for the Z axis (2 blocks)

As the block with sequence N2 has the move command in the same

direction as that of the block with sequence N6, the correct

compensation is performed.

Alternatively, it is possible to prevent overcutting in the same way by

specifying an IJ type vector with the same direction as the advance

direction in the start-up block, as in N1 G91 G00 G41 X500. Y500. I0

J1 D1;, after the tool has moved along the Z axis.

- 195 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 7