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

CAUTION

8 If reference position return (G28 or G30) has been

specified, tool length compensation is canceled for

the axis specified at the time of positioning on the

reference point; however, tool length compensation

is not canceled for an un-specified axis. If

reference position return has been specified in the

same block as that containing tool length

compensation cancel (G49), tool length

compensation is canceled for both the specified and

un-specified axes at the time of positioning on the

mid-point.

9 With a machine coordinate system command

(G53), tool length compensation is canceled for the

axis specified at the time of positioning on the

specified point.

10 The tool length compensation vector canceled by

specifying G53, G28, or G30 during tool length

compensation is restored as described below:

• For tool length compensation types A and B, if

parameter EVO (No. 5001#6) is 1, the vector is

restored in the block buffered next; for all of tool

length compensation types A, B, and C, it is

restored in a block containing an H, G43, or G44

command if parameter is 0.

11 When a tool length compensation shift type is used,

if the start or cancellation of a tool length

compensation or other command is specified cutter

compensation mode, look-ahead is not performed.

As a result, overcutting or undercutting may occur

before or after the block in which the start or

cancellation is specified. Thus, specify the start and

cancellation of tool length compensation before the

entry to cutter compensation mode or at a location

where machining is not affected.

- 136 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

6.3

AUTOMATIC TOOL LENGTH MEASUREMENT (G37)

By issuing G37 the tool starts moving to the measurement position

and keeps on moving till the approach end signal from the

measurement device is output. Movement of the tool is stopped when

the tool nose reaches the measurement position.

Difference between coordinate value when tool reaches the

measurement position and coordinate value commanded by G37 is

added to the tool length compensation amount currently used.

A (Start point)

Rapid

Measurement position is commanded

traverse

with G37

B (Deceleration position)

Measurement

feedrate

C (Measurement position)

The tool stops when the approach end

signal goes on.

Compensation value = (Current compensation value) + [(Coordinates of the

point at which the tool is stopped) - (Coordinates of the programmed measure

ment position)]

Fig. 6.3 (a) Automatic tool length measurement

Format

G92 IP_ ;

Sets the workpiece coordinate system.

(It can be set with G54 to G59. See

Chapter "Coordinate System" in User’s

Manual (Common to T/M series.))

Hxx ;

Specifies an offset number for tool

length compensation.

G90 G37 IP_ ; Absolute programming

G37 is valid only in the block in which it is specified.

IP_ indicates the X-, Y-, Z-, or fourth axis.

Explanation

- Setting the workpiece coordinate system

Set the workpiece coordinate system so that a measurement can be

made after moving the tool to the measurement position. The

coordinate system must be the same as the workpiece coordinate

system for programming.

- 137 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Specifying G37

Specify the absolute coordinates of the correct measurement position.

Execution of this command moves the tool at the rapid traverse rate

toward the measurement position, reduces the federate halfway, then

continuous to move it until the approach end signal from the

measuring instrument is issued. When the tool nose reaches the

measurement position, the measuring instrument sends an approach

end signal to the CNC which stops the tool.

- Changing the offset value

The difference between the coordinates of the position at which the

tool reaches for measurement and the coordinates specified by G37 is

added to the current tool length compensation value. (If parameter

MDC (No. 6210#6) is 1, it is subtracted.)

Offset value =

(Current compensation value) + [(Coordinates of the position at which

the tool reaches for measurement) - (Coordinates specified by G37)]

These offset values can be manually changed from MDI.

- Alarm

When automatic tool length measurement is executed, the tool moves

as shown in Fig. 6.2 (b). If the approach end signal goes on while the

tool is traveling from point B to point C, an alarm occurs. Unless the

approach end signal goes on before the tool reaches point F, the same

alarm occurs. The alarm number is PS0080.

Deceleration

feedrate

Rapid

(measurement

traverse

feedrate)

Approach end signal ON

E F

Start

point

Position commanded

by G37

Permitted range of approach end signal

Fig. 6.3 (b) Tool movement to the measurement position

CAUTION

When a manual movement is inserted into a

movement at a measurement federate, return the

tool to the position before the inserted manual

movement for restart.

- 138 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

NOTE

When an H code is specified in the same block as

G37, an alarm is generated. Specify H code before

the block of G37.

The measurement speed (FP), γ, and ε are set as

parameters (FP: No. 6241, γ: No. 6251, ε: No.

6254) by the machine tool builder. Make settings

so that e are always positive and γ are always

greater than ε.

When tool offset memory A is used, the offset

value is changed. When tool offset memory C is

used, the tool wear compensation value for the H

code is changed.

A delay or variation in detection of the

measurement position arrival signal is 0 to 2 msec

on the CNC side excluding the PMC side.

Therefore, the measurement error is the sum of 2

msec and a delay or variation (including a delay or

variation on the receiver side) in propagation of the

skip signal on the PMC side, multiplied by the

feedrate set in parameter No. 6241.

A delay or variation in time after detection of the

measurement position arrival signal until a feed

stops is 0 to 8 msec. To calculate the amount of

overrun, further consider a delay in

acceleration/deceleration, servo delay, and delay

on the PMC side.

- 139 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Example

G92 Z760.0 X1100.0 ; Sets a workpiece coordinate system with

respect to the programmed absolute zero

point.

G00 G90 X850.0 ;

Moves the tool to X850.0.

That is the tool is moved to a position that is a

specified distance from the measurement

position along the Z-axis.

H01 ;

Specifies offset number 1.

G37 Z200.0 ;

Moves the tool to the measurement position.

G00 Z204.0 ;

Retracts the tool a small distance along the

Z-axis.

For example, if the tool reaches the measurement position with

Z198.0;, the compensation value must be corrected. Because the

correct measurement position is at a distance of

200 mm, the

compensation value is lessened by 2.0 mm (198.0 - 200.0 = -2.0).

760

200

Measurement

position along Z axis

850

1100

- 140 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

6.4

TOOL OFFSET (G45 - G48)

The programmed travel distance of the tool can be increased or

decreased by a specified tool offset value or by twice the offset value.

The tool offset function can also be applied to an additional axis.

Workpiece

Tool center path

Programmed path

Tool

Format

G45 IP_ D_ ; Increase the travel distance by the tool

offset value

G46 IP_ D_ ; Decrease the travel distance by the tool

offset value

G47 IP_ D_ ; Increase the travel distance by twice the

tool offset value

G48 IP_ D_ ; Decrease the travel distance by twice the

tool offset value

G45 to 48

: One-shot G code for increasing or decreasing

the travel distance

IP_

: Command for moving the tool

Code for specifying the tool offset value

* If bit 2 (OFH) of parameter No. 5001 ="0", setting bit 5

(TPH) of parameter No. 5001 to "1" enables address H to

be used as a code for specifying a tool position offset

value.

- 141 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Explanation

- Increase and decrease

As shown in Table 6.4 (a), the travel distance of the tool is increased

or decreased by the specified tool offset value.

In the absolute mode, the travel distance is increased or decreased as

the tool is moved from the end point of the previous block to the

position specified by the block containing G45 to G48.

Table 6.4 (a) Increase and decrease of the tool travel distance

When a positive tool offset

When a negative tool offset

G code

value is specified

Start point

End point

Start point

End point

G45

Start point

End point

Start point

End point

G46

Start point

End point

Start point

End point

G47

Start point

End point

Start point

End point

G48

Programmed movement distance

Tool offset value

Actual movement position

If a move command with a travel distance of zero is specified in the

incremental programming (G91) mode, the tool is moved by the

distance corresponding to the specified tool offset value.

If a move command with a travel distance of zero is specified in the

absolute programming (G90) mode, the tool is not moved.

- Tool offset value

Once selected by D code, the tool offset value remains unchanged

until another tool offset value is selected.

Tool offset values can be set within the following range:

D0 always indicates a tool offset value of zero.

* If bit 2 (OFH) of parameter No. 5001 ="0", setting bit 5 (TPH) of

parameter No. 5001 to "1" enables address H to be used as a code

for specifying a tool position offset value.

- 142 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

CAUTION

1 When G45 to G48 is specified to n axes (n=1-4)

simultaneously in a motion block, offset is applied to

all n axes.

When the cutter is offset only for cutter radius or

diameter in taper cutting, overcutting or undercutting

occurs.

Therefore, use cutter compensation (G40 - G42)

shown in II-6.4 or 6.6.

Shape actually cut

Desired

shape

Y axis

Overcutting

X axis

G01 X_ F_ ;

G47 X_ Y_ D_ ;

Y_ ;

Desired shape

Shape actually cut

Y axis

Undercutting

X axis

G01 G45 X_ F_ D_;

X_ Y_ ;

G45 Y_ ;

2 G45 to G48 (tool offset) must not be used in the

G41 or G42 (cutter compensation) mode.

- 143 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

NOTE

1 When the specified direction is reversed by

decrease as shown in the figure below, the tool

moves in the opposite direction.

Movement of the

Program command

Start

End

position

Tool offset value

Example

G46 X2.50 ;

Tool offset value

Equivalent command

+3.70

X-1.20 ;

Tool offset can be applied to circular interpolation

(G02, G03) with the G45 to G48 commands only for

1/4 and 3/4 circles using addresses I, J and K by the

parameter setting, providing that the coordinate

system rotation be not specified at the same time.

This function is provided for compatibility with the

conventional CNC program without any cutter

compensation. The function should not be used

when a new CNC program is prepared.

Tool offset for circular interpolation

Programmed tool path

Program

Actual tool path

N1 G46 G00 X_ Y_ D_ ;

N2 G45 G01 Y_ F_ ;

N3 G45 G03 X_ Y_ I_ ;

N4 G01 X_ ;

D code should be used in tool offset mode.

G45 to G48 are ignored in canned cycle mode.

Perform tool offset by specifying G45 to G48 before

entering canned cycle mode and cancel the offset

after releasing the canned cycle mode.

- 144 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

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 ;

- 145 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.5

OVERVIEW OF CUTTER COMPENSATION (G40-G42)

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

the tool (Fig. 6.5 (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. 6.5 (a) Outline of cutter compensation

- 146 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

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)

* Setting bit 2 (OFH) of parameter No. 5001 to "1" enables

address H to be used as a code for specifying a cutter

compensation amount. When bit 2 (OFH) of parameter

No. 5001 = "1", if tool length compensation and cutter

compensation are specified in the same block, the latter

command takes precedence.

- Cutter compensation cancel (offset mode cancel)

G40 IP_;

G40

: Cutter compensation cancel (Group 07)

(Offset mode cancel)

IP_

: Command for axis movement

- 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, nonzero

dimension word in the offset plane and command 0 in a non-D0 D

code) 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, 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).

- 147 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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 command (G02 or G03) is

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. 6.5 (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.

Calculated from the cutter

compensation value in the block N6

compensation value in the block N7

Programmed path

Fig. 6.5 (c) Changing the cutter compensation value

- 148 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- 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. 6.5 (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. 6.5 (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.

- 149 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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 1 (OFC) and 0 (OFA)

parameter No. 5042.

Valid compensation range (metric input)

OFC

OFA

Range

±9999.99mm

±9999.999mm

±9999.9999mm

Valid compensation range (inch input)

OFC

OFA

Range

±999.999inch

±999.9999inch

±999.99999inch

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.

- 150 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

G92 X0 Y0 Z0 ;

Specifies absolute coordinates.

The tool is positioned at the start point (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

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).

Notes

- Bit 2 (OFH) of parameter No.5001

If bit 2 (OFH) of parameter No. 5001 is set, cutter compensation takes

precedence over tool length compensation. Concrete explanations

follow:

If OFH = "0":

Processing is carried out properly according to a selected modal

state (G43, G44, or G49).

If OFH = "1":

In a block where G40, G41, or G42 is specified, tool length

compensation is disabled.

In the G40 mode, processing is carried out properly according to

a selected modal state (G43, G44, or G49).

In the G41 and G42 modes, tool length compensation is enabled

only in a block in which G43, G44, or G49 is specified. No

compensation amount is updated only with the H code.

G49 is enabled if G49 is specified in the same block as for G40,

however.

- 152 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

6.6

DETAILS OF CUTTER COMPENSATION

6.6.1

Overview

- 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°≤α

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 parameter

CCC (No. 19607#2).

<1> Linear connection type

<2> Circular connection type

[Bit 2 (CCC) of parameter

[Bit 2 (CCC) of

No.19607 = 0]

parameter No.19607 = 0]

Vectors are connected with linear

Vectors are connected with circular

interpolation.

- 153 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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

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.

As a start-up operation, one of the three types A, B, and C can be

selected by setting parameter SUP (No. 5003#0) and parameter SUV

(No. 5003#1) appropriately. The operation to be performed if the

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

- 154 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

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

Type C

When the start-up block and the cancel block are

blocks without tool movement, the tool moves by

the cutter 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.

- 155 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

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 parameter SUP (No. 5003#0) and

parameter SUV (No. 5003#1). The operation to be performed if the

tool turns around the inside is of a single type.

- 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.

- 156 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

6.6.2

Tool Movement in Start-up

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

moves as illustrated below (start-up):

Explanation

- Tool movement around an inner side of a corner (180°≤ α)

Linear→Linear

Workpiece

Programmed path

G42

Tool center path

Start point

Linear→Circular

Work-

G42

piece

Start point

Tool center path Programmed path

- 157 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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

parameter SUP (No.5003#0).

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

ork-

ece

Intersection

Programmed path

- 158 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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

parameter SUP (No.5003#0).

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

- 160 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

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

- 161 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- 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

For type C

The tool shifts by the compensation value in the direction vertical

to the block with tool movement subsequent to the start-up block.

Without tool

movement

Programmed path

Tool center path

Intersection

- 162 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

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 item,

“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.

- 163 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Tool movement around the inside of a corner (180°≤ α)

Linear→Linear

Workpiece

Programmed path

Tool center path

Intersection

Linear→Circular

Work-

piece

Intersection

Tool center path

Programmed path

Circular→Linear

Workpiece

Programmed path

Tool center path

C Intersection

Circular→Circular

Work-

Intersection

piece

Tool center

Programmed path

path

- 164 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 6