FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Example

Program using tool offset

N12

N11

30R

N10

N13

30R

Y axis

N14

Origin

Tool diameter

20φ

Offset No.

Tool offset value

+10.0

Program

N1 G91 G46 G00 X80.0 Y50.0 D01 ;

N2 G47 G01 X50.0 F120.0 ;

N3 Y40.0 ;

N4 G48 X40.0 ;

N5 Y-40.0 ;

N6 G45 X30.0 ;

N7 G45 G03 X30.0 Y30.0 J30.0 ;

N8 G45 G01 Y20.0 ;

N9 G46 X0 ;

(Decreases toward the positive direction for movement amount "0". The tool moves

in the -X direction by the offset value.)

N10 G46 G02 X-30.0 Y30.0 J30.0 ;

N11 G45 G01 Y0 ; (Increase toward the positive direction for movement amount "0". The tool moves in

the +Y direction by the offset value.)

N12 G47 X-120.0 ;

N13 G47 Y-80.0 ;

N14 G46 G00 X-80.0 Y-50.0 ;

- 172 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

6.4

OVERVIEW OF CUTTER COMPENSATION (G40-G42)

When the tool is moved, the tool path can be shifted by the radius of the tool (Fig. 6.4 (a)).

To make an offset as large as the radius of the tool, CNC first creates an 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 the workpiece side and the head positions to the center of the tool.

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 point at the end of machining, cancel the cutter compensation mode.

Cutter

compensation

cancel

Start-up

Fig. 6.4 (a) Outline of cutter compensation

Format

Start up (cutter compensation start)

G00(or G01)G41(or G42) IP_D_;

G41 : Cutter compensation left (Group 07)

G42 : Cutter compensation right (Group 07)

IP_

: Command for axis movement

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

Cutter compensation cancel (offset mode cancel)

G40 IP_;

G40 : Cutter compensation cancel (Group 07)

(Offset mode cancel)

IP_

: Command for axis movement

- 173 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Selection of the offset plane

Offset plane

Command for plane selection

IP_

XpYp

G17 ;

Xp_Yp_

ZpXp

G18 ;

Xp_Zp_

YpZp

G19 ;

Yp_Zp_

Explanation

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.

Start-up

When a cutter compensation command (G41 or G42, D code other than 0) 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) or involute interpolation (G02.2, G03.2) is specified, alarm PS0034

occurs.

For the start-up and subsequent blocks, the CNC prereads as many blocks as the number of preread

blocks set in the parameter No. 19625.

Offset mode

In the offset mode, compensation is accomplished by positioning (G00), linear interpolation (G01), or

circular interpolation (G02, G03).

If three or more blocks that move the tool cannot be read in offset mode, the tool may make either an

excessive or insufficient cut.

If the offset plane is switched in the offset mode, alarm PS0037 occurs and the tool is stopped.

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.

G40 has been commanded.

0 has been commanded as the offset number for cutter compensation (D code).

When performing offset cancel, circular arc commands (G02 and G03) and involute commands (G02.2

and G03.2) are not available. If these commands are specified, an PS0034 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 mode cancel

(G40/D0)

Fig. 6.4 (b) Changing the offset mode

Change of the cutter compensation value

In general, the cutter compensation value shall be changed in the cancel mode, when changing tools. If

the cutter compensation value is changed in offset mode, the vector at the end point of the block is

calculated for the new cutter compensation value.

- 174 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Calculated from the cutter

compensation value in the block N6

compensation value in the block N7

Programmed path

Fig. 6.4 (c) Changing the cutter compensation value

Positive/negative cutter compensation value and tool center path

If the compensation value is negative (-), distribution is made for a figure in which G41's and G42's are

all replaced with each other on the program. Consequently, if the tool center is passing around the outside

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

Fig. 6.4 (d) shows one example.

Generally, the compensation value is programmed to be positive (+).

When a tool path is programmed as in <1>, if the compensation value is made negative (-), the tool center

moves as in <2>, and vice versa. Consequently, the same program permits cutting both male and female

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

Applicable if start-up and cancel is A type.

(See the descriptions about the start-up of cutter

compensation.)

<1>

<2>

Tool center path

Programmed path

Fig. 6.4 (d) Tool center paths when positive and negative cutter

compensation values are specified

Cutter compensation value setting

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

NOTE

The cutter compensation value for which the D code corresponds to 0 always

means 0.

It is not possible to set the cutter compensation value corresponding to D0.

Valid compensation value range

The valid range of values that can be set as a compensation value is either of the following, depending on

the bits 3 (OFE), 2 (OFD), 1 (OFC), and 0 (OFA) of parameter No. 5042.

Valid compensation range (metric input)

OFE

OFD

OFC

OFA

Range

±9999.99 mm

±9999.999 mm

±9999.9999 mm

±9999.99999 mm

- 175 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

OFE

OFD

OFC

OFA

Range

±999.999999 mm

Valid compensation range (inch input)

OFE

OFD

OFC

OFA

Range

±999.999 inch

±999.9999 inch

±999.99999 inch

±999.999999 inch

±99.9999999 inch

The compensation value corresponding to offset No. 0 always means 0. It is not possible to set the

compensation value corresponding to offset No. 0.

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.

Specifying a cutter compensation value

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

Plane selection and vector

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

PS0037 is displayed and the machine is stopped.

- 176 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Example

250R

C1(700,1300)

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

(-150,1150)

C2 (1550,1150)

650R

P3(450,900)

P6(950,900)

(250,900)

(1150,900)

P9(700,650)

(250,550)

(1150,550)

N10

Y axis

N11

Unit : mm

X axis

Start point

G17 G92 X0 Y0 Z0 ;

Specifies absolute coordinates.

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

N1 G90 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 point (X0, Y0, Z0).

- 177 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.5

OVERVIEW OF TOOL NOSE RADIUS COMPENSATION

(G40-G42)

The tool nose radius compensation function automatically compensates for the errors due to the tool nose

roundness.

Workpiece

Tool path without compensation

Tool path with compensation

Insufficient

Tool nose

depth of

cutting

Shape processed without tool

nose radius compensation

Fig. 6.5 (a) Tool path of tool nose radius compensation

6.5.1

Imaginary Tool Nose

The tool nose at position A in Fig. 6.5.1 (a) does not actually exist.

The imaginary tool nose is required because it is usually more difficult to set the actual tool nose radius

center to the start point than the imaginary tool nose.

Also when imaginary tool nose is used, the tool nose radius need not be considered in programming.

The position relationship when the tool is set to the start point is shown in Fig. 6.5.1 (a).

Start position

When programmed using the tool

When programmed using the

nose center

imaginary tool nose

Fig. 6.5.1 (a) Tool nose radius center and imaginary tool nose

- 178 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

CAUTION

In a machine with reference positions, a standard position like the turret center

can be placed over the start point. The distance from this standard position to

the tool nose radius center or the imaginary tool nose is compensated by the tool

length compensation function.

Setting the distance from the standard position to the tool nose radius center as

the offset value is the same as placing the tool nose radius center over the start

point, while setting the distance from the standard position to the imaginary tool

nose is the same as placing the imaginary tool nose over the standard position.

To set the offset value, it is usually easier to measure the distance from the

standard position to the imaginary tool nose than from the standard position to

the tool nose radius center.

OFX

(Tool length

compensation in

X axis)

OFZ

(Tool length

compensation

in Z axis)

Compensates for the distance from the standard

position to the tool nose center by the tool length

position to the imaginary tool nose by the tool

compensation

length compensation

The start position is placed over the tool nose center

The start position is placed over the imaginary tool

nose

Fig. 6.5.1 (b) Tool length compensation when the turret center is placed over the start point

Unless tool nose radius compensation is

If tool nose radius compensation is used, accurate

performed, the tool nose center path is the

cutting will be performed.

same as the programmed path.

Start-

Tool nose center path

Programmed path

Fig. 6.5.1 (c) Tool path when programming using the tool nose center

Without tool nose radius compensation, the

With tool nose radius compensation, accurate

tool nose radius center path is the same as

cutting will be performed.

the programmed path.

Imaginary tool

nose path

Start-

Programmed path

Fig. 6.5.1 (d) Tool path when programming using the imaginary tool nose

- 179 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.5.2

Direction of Imaginary Tool Nose

The direction of the imaginary tool nose viewed from the tool nose center is determined by the direction

of the tool during cutting, so it must be set in advance as well as offset values.

The direction of the imaginary tool nose can be selected from the eight specifications shown in the Fig.

6.5.2 (a) below together with their corresponding codes. Fig. 6.5.2 (a) illustrates the relation between the

tool and the start point. The following apply when the tool geometry offset and tool wear offset option are

selected.

G18

G17

G19

Imaginary tool nose number 1

Imaginary tool nose number 2

Imaginary tool nose

number 3

number 4

Imaginary tool nose number 5

Imaginary tool nose number 6

Imaginary tool nose number 7

Imaginary tool nose number 8

Fig. 6.5.2 (a) Direction of imaginary tool nose

Imaginary tool nose numbers 0 and 9 are used when the tool nose center coincides with the start point. Set

imaginary tool nose number to address OFT for each offset number.

Imaginary tool nose number 0 or 9

- 180 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

6.5.3

Offset Number and Offset Value

Explanation

Offset number and offset value

Tool nose radius compensation value

(Tool nose radius value)

Table 6.5.3 (a) Offset number and offset value (example)

Offset number Up to 999

(Tool compensation value)

(Direction of imaginary tool nose)

sets

001

0.200

002

0.250

003

0.120

004

005

Command of offset value

An offset number is specified with the D code.

Setting range of offset value

The range of values that can be set as a compensation value is either of the following, depending on the

bits 3 (OFE), 2 (OFD), 1 (OFC), and 0 (OFA) of parameter No. 5042.

Table 6.5.3 (b) Valid compensation range (metric input)

OFE

OFD

OFC

OFA

Range

±9999.99 mm

±9999.999 mm

±9999.9999 mm

±9999.99999 mm

±999.999999 mm

Table 6.5.3 (c) Valid compensation range (inch input)

OFE

OFD

OFC

OFA

Range

±999.999 inch

±999.9999 inch

±999.99999 inch

±999.999999 inch

±99.9999999 inch

The offset value corresponding to the offset number 0 is always 0.

No offset value can be set to offset number 0.

6.5.4

Workpiece Position and Move Command

In tool nose radius compensation, the position of the workpiece with respect to the tool must be specified.

G code

Workpiece position

Tool path

G40

(Cancel)

Moving along the programmed path

- 181 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

G code

Workpiece position

Tool path

G41

Right side

Moving on the left side the programmed path

G42

Left side

Moving on the right side the programmed path

The tool is offset to the opposite side of the workpiece.

X axis

G42

Z axis

Workpiece

G41

The imaginary tool nose is on the

programmed path.

G40

Imaginary tool nose

number 1 to 8

number 0

Fig. 6.5.4 (a) Workpiece position

The workpiece position can be changed by setting the coordinate system as shown below.

Z axis

G41 (the workpiece is on

the left side)

X axis

Workpiece

G42 (the workpiece is on

NOTE

the right side)

If the tool nose radius

compensation value is negative,

the workpiece position is changed.

Fig. 6.5.4 (b) When the workpiece position is changed

G40, G41, and, G42 are modal.

- 182 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Don't specify G41 while in the G41 mode. If you do, compensation will not work properly.

Don't specify G42 while in the G42 mode for the same reason.

G41 or G42 mode blocks in which G41 or G42 are not specified are expressed by (G41) or (G42)

respectively.

CAUTION

If the sign of the compensation value is changed from plus to minus and vice

versa, the offset vector of tool nose radius compensation is reversed, but the

direction of the imaginary tool nose does not change. For a use in which the

imaginary tool nose is adjusted to the starting point, therefore, do not change the

sign of the compensation value for the assumed program.

Explanation

Tool movement when the workpiece position does not change

When the tool is moving, the tool nose maintains contact with the workpiece.

(G42)

Enlarged

diagram

Fig. 6.5.4 (c) Tool movement when the workpiece position does not change

Tool movement when the workpiece position changes

The workpiece position against the tool changes at the corner of the programmed path as shown in the

following figure.

Workpiece

G41

position

G42

Workpiece

position

G41

G42

Fig. 6.5.4 (d) Tool movement when the workpiece position changes

Although the workpiece does not exist on the right side of the programmed path in the above case, the

existence of the workpiece is assumed in the movement from A to B. The workpiece position must not be

changed in the block next to the start-up block. In the example in the Fig. 6.5.4 (b), if the block specifying

motion from A to B were the start-up block, the tool path would not be the same as the one shown.

- 183 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Start-up

The block in which the mode changes to G41 or G42 from G40 is called the start-up block.

G40 _ ;

G41 _ ; (Start-up block)

Transient tool movements for offset are performed in the start-up block. In the block after the start-up

block, the tool nose center is positioned vertically to the programmed path of that block at the start point.

G40

(G42)

G42 (Start-up)

Fig. 6.5.4 (e) Start-up

Offset cancel

The block in which the mode changes to G40 from G41 or G42 is called the offset cancel block.

G41 _ ;

G40 _ ; (Offset cancel block)

The tool nose center moves to a position vertical to the programmed path in the block before the cancel

block.

The tool is positioned at the end point in the offset cancel block (G40) as shown below.

End position

G40

(G42)

Fig. 6.5.4 (f) Offset cancel

Changing the compensation value

In general, the compensation value is to be changed when the tool is changed in offset cancel mode. If the

compensation value is changed in offset mode, however, the vector at the end point of the block is

calculated using the compensation value specified in that same block.

The same applies if the imaginary tool nose direction and the tool offset value are changed.

Calculated from the compensation

value specified in block N6.

value specified in block N7.

Programmed path

Fig. 6.5.4 (g) Changing the compensation value

- 184 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Specification of G41/G42 in G41/G42 mode

When a G41 or G42 code is specified again in G41/G42 mode, the tool nose center is positioned vertical

to the programmed path of the preceding block at the end point of the preceding block.

(G42)

G42

(G18) G42 G91 Z-500.0 X-500.0 ;

Fig. 6.5.4 (h) Specification of G41/G42 in G41/G42 mode

In the block that first changes from G40 to G41/G42, the above positioning of the tool nose center is not

performed.

Tool movement when the moving direction of the tool in a block which

includes a G40 (offset cancel) command is different from the direction of the

workpiece

When you wish to retract the tool in the direction specified by X and Z canceling the tool nose radius

compensation at the end of machining the first block in Fig. 6.5.4 (i), specify the following :

G40 X _ Z _ I _ K _ ;

where I and K are the direction of the workpiece in the next block, which is specified in incremental

mode.

I,K

X,Z

Actual move command

G40

(G42)

G40 X_ Z_ I_ K_ ;

Fig. 6.5.4 (i) If I and K are specified in the same block as G40

Thus, this prevents the tool from overcutting, as shown in Fig. 6.5.4 (j).

X, Z

Actual move command

G40

(G42)

G40 X_ Z_ ;

Fig. 6.5.4 (j) Case in which overcutting occurs in the same block as G40

The workpiece position specified by addresses I and K is the same as that in the preceding block.

Specify I_K_; in the same block as G40. If it is specified in the same block as G02 or G03, it is assumed

to be the center of the arc.

- 185 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

G40 X_ Z_ I_ K_ ;

Tool nose radius compensation

G02 X_ Z_ I_ K_ ;

Circular interpolation

If I and/or K is specified with G40 in the cancel mode, the I and/or K is ignored. The numeral is followed

I and K should always be specified as radius values.

G40 G01 X_ Z_ ;

G40 G01 X_ Z_ I_ K_ ; Offset cancel mode (I and K are ineffective.)

Example

<3>

φ300

<1>

<2>

200

φ60

120

150

(G40 mode)

<1> G42 G00 X60.0 ;

<2> G01 X120.0 Z-150.0 F10 ;

<3> G40 G00 X300.0 Z0 I40.0 K-30.0 ;

6.5.5

Notes on Tool Nose Radius Compensation

Explanation

Blocks without a move command that are specified in offset mode

<1> M05 ;

M code output

<2> S210 ;

S code output

<3> G04 X10.0 ;

Dwell

<4> G22 X100000 ;

Machining area setting

<5> G91 G01 X0 ;

Feed distance of zero

<6> G90 ;

G code only

<7> G10 L11 P01 R10.0 ;

Offset change

If the number of such blocks consecutively specified is more than N-2 blocks (where N is the number of

blocks to read in offset mode (parameter No. 19625)), the tool arrives at the position vertical to this block

at the end point of the previous block.

If the feed distance is 0 (<5>), this applies even if only one block is specified.

- 186 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Programmed path

(G42 mode)

N6 G91 Z100.0 ;

N7 S21 ;

N8 M04 ;

U9 X-100.0 Z100.0 ;

(Number of blocks to be read

Tool nose center path

in offset mode = 3)

Fig. 6.5.5 (a)

Overcutting may, therefore, occur in the Fig. 6.5.5 (a).

Tool nose radius compensation when chamfering is performed

Movement after compensation is shown Fig. 6.5.5 (b).

(G42 mode)

G91 G01 Z-20.0, C10.0;

X20.0;

(G42)

Programmed path

(G41)

Fig. 6.5.5 (b)

Tool nose radius compensation when a corner R is performed

Movement after compensation is shown Fig. 6.5.5 (c).

(G42 mode)

G91 G01 Z-20.0, R10.0;

X20.0;

(G42)

Programmed path

(G41)

Fig. 6.5.5 (c)

- 187 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.6

DETAILS OF CUTTER OR TOOL NOSE RADIUS

COMPENSATION

6.6.1

Overview

The following explanation focuses on the cutter compensation, but applies to the tool nose radius

compensation as well.

Inner side and outer side

When an angle of intersection of the tool paths specified with move commands for two blocks on the

workpiece side 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°≤a

0°≤α<180°

Outer corner connection method

If the tool moves around an outer corner in cutter compensation mode, it is possible to specify whether to

connect compensation vectors with linear interpolation or with circular interpolation, using bit 2 (CCC) of

parameter No. 19607.

<1> Linear connection type [Bit

<2> Circular connection type

2 (CCC) of parameter No.

[Bit 2 (CCC) of

19607 = 0]

parameter No. 19607 = 1]

Vectors are connected with linear

Vectors are connected with circular

interpolation.

Cancel mode

The cutter compensation enters the cancel mode under the following conditions. (The system may not

enter the cancel mode depending on the machine tool.)

<1> Immediately after the power is turned on

<2> When the

key on the MDI panel is pushed

<3> After a program is forced to end by executing M02 or M30

<4> After the cutter compensation cancel command (G40) is exercised

- 188 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

In the cancel mode, the compensation vector is set to zero, and the path of the center of tool coincides

with the programmed path. A program must end in cancel mode. If it ends in the cutter compensation

mode, the tool cannot be positioned at the end point, and the tool stops at a location the compensation

vector length away from the end point.

NOTE

The operation to be performed when a reset operation is performed during cutter

compensation differs depending on bit 6 (CLR) of parameter No. 3402.

- If CLR is 0

The system enters the reset state. G41/G42 are retained as the modal code

of group 07, but to perform cutter compensation, an offset number (D code)

must be specified again.

- If CLR is 1

The system enters the clear state. The modal code of group 07 is G40, and to

perform cutter compensation again, G41/G42 and an offset number (D code)

must be specified.

Start-up

When a block which satisfies all the following conditions is executed in cancel mode, the CNC enters the

cutter compensation mode. Control during this operation is called start-up.

<1> G41 or G42 is contained in the block, or has been specified to place the CNC in the cutter

compensation mode.

<2> 0 < compensation number of cutter compensation ≤ maximum compensation number

<3> Positioning (G00) or linear interpolation (G01) mode

<4> A compensation plane axis command with a travel distance of 0 (except start-up type C) is specified.

If start-up is specified in circular interpolation (G02, G03) mode, PS0034 will occur.

In a start-up block, workpiece coordinate system switching (G54 to G59) cannot be specified.

As a start-up operation, one of the three types A, B, and C can be selected by setting bit 0 (SUP) of

parameter No. 5003 and bit 1 (SUV) of parameter No. 5003 appropriately. The operation to be performed

if the tool moves around an inner side is of single type only.

Table 6.6.1 (a) Start-up/cancel operation

SUV

SUP

Type

Operation

Type A

A compensation vector is output, which is vertical to the block

subsequent to the start-up block and the block preceding the cancel

block.

Tool center path

G41

Programmed path

Type B

A compensation vector is output, which is vertical to the start-up

block and the cancel block. An intersection vector is also output.

Intersection

Tool center path

Programmed path

G41

- 189 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

SUV

SUP

Type

Operation

Type C

When the start-up block and the cancel block are blocks without tool

movement, the tool moves by the tool radius ⋅ tool nose radius

compensation value in the direction vertical to the block subsequent

to the start-up block and the block preceding the cancel block.

Intersection

Tool center path

Programmed path

Programmed

path

G41

For a block with tool movement, the tool follows the SUP setting: If it

is 0, type A is assumed and if 1, type B is assumed.

Reading input commands in cutter compensation mode

In cutter compensation mode, input commands are read from usually three blocks and up to eight blocks

depending on the setting of parameter No. 19625 to perform intersection calculation or an interference

check, described later, regardless of whether the blocks are with or without tool movement, until a cancel

command is received.

To perform intersection calculation, it is necessary to read at least two blocks with tool movement. To

perform an interference check, it is necessary to read at least three blocks with tool movement.

As the setting of parameter No. 19625, that is, the number of blocks to read, increases, it is possible to

predict overcutting (interference) for up to more subsequent commands. Increases in blocks to read and

analyze, however, cause reading and analysis to take more time.

Ending (canceling) cutter compensation

In cutter compensation mode, cutter compensation is canceled if a block that satisfies at least either one of

the following conditions is executed:

<1> G40 is specified.

<2> D00 is specified as the compensation number of cutter compensation.

If cutter compensation cancel is to be performed, it must not be by a circular command (G02, G03).

Otherwise, an alarm will occur.

For a cancel operation, one of three types, A, B, and C, can be selected by appropriately setting bit 0

(SUP) of parameter No. 5003 and bit 1 (SUV) of parameter No. 5003. The operation to be performed if

the tool turns around the inside is of a single type.

- 190 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Bit 0 (SBK) of parameter No. 5000

When bit 0 (SBK) of parameter No. 5000 is set to 1, a single block stop can be performed in a block

created internally for cutter compensation.

Use this parameter to check a program including cutter compensation.

Stop point in a block created internally

Single block stop point

Cutter center path

Programmed path

NOTE

When an auxiliary function (M code), spindle speed function (S code), tool

function (T code), or second auxiliary function (B code) is specified in the N1

block in the figure above, FIN is not accepted if the tool stops at the stop point in

a block created internally (excluding the single block stop point).

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 tool radius ⋅ tool nose radius 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.

- 191 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Cases in which the start-up block is a block with tool movement and the tool

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

Tool path in start-up has two types A and B, and they are selected by bit 0 (SUP) of parameter No. 5003.

Linear→Linear

Start point

G42

Workpiece

Programmed path

Tool center path

Type

Linear→Circular

Start point

G42

Work-

piece

Tool center path

Programmed path

Linear→Linear

(Linear connection type)

Start point

G42

Workpiece

Programmed path

Tool center path

Intersection

Type

Linear→Circular

Start point

(Linear connection type)

G42

Work-

piece

Intersection

Tool center path

Programmed path

- 193 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Cases in which the start-up block is a block with tool movement and the tool

moves around the outside at an acute angle (α<90°)

Tool path in start-up has two types A and B, and they are selected by bit 0 (SUP) of parameter No. 5003.

Linear→Linear

Start point

G42

Workpiece

α L

Programmed path

Tool center path

Type

Linear→Circular

Start point

G42

Work-

piece

Tool center path

Programmed path

Linear→Linear

Start point

(Linear connection type)

G42

Workpiece

Programmed path

Tool center path

Type

Linear→Circular

Start point

(Linear connection type)

G42

Work-

piece

Tool center path

Programmed path

- 195 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Linear→Linear

Start point

(Circular

connection type)

G42

Workpiece

Programmed path

Tool center path

Type

Linear→Circular

Start point

(Circular

connection type)

G42

Work-

piece

Tool center path

Programmed path

Tool movement around the outside linear → linear at an acute angle less than

1 degree (α<1°)

Tool center path

Programmed path

(G41)

G41

Start point

Less than 1 deg

A block without tool movement specified at start-up

For type A and B

If the command is specified at start-up, the offset vector is not created. The tool does not operate in a

start-up block.

Tool center path

G40 … ;

N6 X100.0 Y100.0 ;

N7 G41 X0 ;

N8 Y-100.0 ;

N9 Y-100.0 X100.0 ;

Programmed path

- 196 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.6.3

Tool Movement in Offset Mode

In offset mode, compensation is performed even for positioning commands, not to speak of linear and

circular interpolations. To perform intersection calculation, it is necessary to read at least two blocks with

tool movement. If, therefore, two or more blocks with tool movement cannot be read in offset mode

because blocks without tool movement, such as auxiliary function independent commands and dwell, are

specified in succession, excessive or insufficient cutting may occur because intersection calculation fails.

Assuming the number of blocks to read in offset mode, which is determined by parameter No. 19625, to

be N and the number of commands in those N blocks without tool movement that have been read to be M,

the condition under which intersection calculation is possible is (N - 2) ≥ M. For example, if the

maximum number of blocks to read in offset mode is 5, intersection calculation is possible even if up to

three blocks without tool movement are specified.

NOTE

The condition necessary for an interference check, described later, differs from

this condition. For details, see the explanation of the interference check.

If a G or M code in which buffering is suppressed is specified, no subsequent commands can be read

before that block is executed, regardless of the setting of parameter No. 19625. Excessive or insufficient

cutting may, therefore, occur because of an intersection calculation failure.

- 198 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

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

- 201 -

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 7