Content      ..     8      9      10      11     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 10

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

D Modes that must not be

The figure cannot be copied during chamfering, corner rounding, or tool

selected

offset.

D Unit system

The two axes of the plane for copying a figure must have an identical unit

system.

D Single block

Single-block stops are not performed in a block with G721.1 or G72.2.

D Specifying cutter

In a subprogram for copying a figure, the G code for cutter compensation

compensation and the

B or C or compensation amount (H or D code) cannot be changed. G92

workpiece coordinate

and G54 to G59 cannot be changed either. Those codes must be specified

system

before figure copying is started.

Examples

D Rotational copy

Y

P4

P3

Start point

P5

P2

P0

120

P6

P1

X

Main program

O1000 ;

N10 G92 X40.0 Y50.0 ;

N20 G00 G90 X_ Y_ ;

(P0)

N30 G01 G17 G41 X_ Y_ D01 F10 ;

(P1)

N40 G72.1 P2000 L3 X0 Y0 R120.0 ;

N50 G40 G01 X_ Y_ I_ J_ ;

(P0)

N60 G00 X40.0 Y50.0 ;

N70 M30 ;

Sub program

O2000 G03 X_ Y_ R30.0 ;

(P2)

N100 G01 X_ Y_ ;

(P3)

N200 G03 X_ Y_ R10.0 ;

(P4)

N300 G01 X_ Y_ ;

(P5)

N400 G03 X_ Y_ R30.0 ;

(P6)

N500 M99;

250

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

D Rotational copy

Y

(spot boring)

P1

P0

Start point

60°

X

Main program

O3000 ;

N10 G92 G17 X80.0 Y50.0 ;

(P0)

N20 G72.1 P4000 L6 X0 Y0 R60.0 ;

N30 G80 G00 X80.0 Y50.0 ;

(P0)

N40 M30 ;

Subprogram

O4000 N100 G90 G81 X_ Y_ R_ Z_ F_ ;

(P1)

N200 M99 ;

251

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

D Linear copy

Y

P4

P5

P2

P7

P

Start point

P1

P3

6

X

P0

70

70

70

P8

Main program

O1000 ;

N10 G92 X-20.0 Y0 ;

N20 G00 G90 X0 Y0 ;

N30 G01 G17 G41 X_ Y_ D01 F10 ;

(P0)

N40 Y_ ;

(P1)

N50 X_ ;

(P2)

N60 G72.2 P2000 L3 I70.0 J0 ;

N70 X_ Y_ ;

(P8)

N80 X0 ;

N90 G00 G40 X-20.0 Y0 ;

N100 M30 ;

Subprogram

O2000 G90 G01 X_ ;

(P3)

N100 Y_ ;

(P4)

N200 G02 X_ I_ ;

(P5)

N300 G01 Y_ ;

(P6)

N400 X_ ;

(P7)

N500 M99 ;

252

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

D Combination of rotational

Y

copying and linear

P0

copying (bolt hole circle)

Start point

P1

45°

X

Main program

O1000 ;

N10 G92 G17 X100.0 Y80.0 ;

(P0)

N20 G72.1 P2000 X0 Y0 L8 R45.0 ;

N30 G80 G00 X100.0 Y80.0 ;

(P0)

N40 M30 ;

Subprogram (rotational copy)

O2000 N100 G72.2 P3000 I0 J_ L3 ;

N200 M99 ;

Subprogram (linear copy)

O3000 N110 G90 G81 X_ Y_ R_ Z_ F_ ;

(P1)

N210 M99 ;

253

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

13.10

Coordinate conversion about an axis can be carried out if the center of

rotation, direction of the axis of rotation, and angular displacement are

THREE-

specified. This function is very useful in three-dimensional machining

DIMENSIONAL

by a die-sinking machine or similar machine. For example, if a program

COORDINATE

specifying machining on the XY plane is converted by the three-

dimensional coordinate conversion function, the identical machining can

CONVERSION

be executed on a desired plane in three-dimensional space.

(G68, G69)

Z

Y

X

Three-dimensional coordinate conversion

Z

Y

X

Format

G68 Xp x₁ Yp y₁ Zp z₁ I_i1 J j₁ K k₁ R_α ; Starting three-dimensional

coordinate conversion

@

@

Three-dimensional coordi-

@

@

nate conversion mode

G69 ;

Canceling three-dimensional

coordinate conversion

Xp, Yp, Zp : Center of rotation (absolute coordinates) on the X, Y, and Z

axis or parallel axes

I, J, K :

Direction of the axis of rotation

R

:

Angular displacement

Explanations

D Command for

N1 G68 Xp x₁ Yp y₁ Zp z₁ I i₁ J j₁ K k₁ R α ;

three-dimensional

N2 G68 Xp x₂ Yp y₂ Zp z₂ I i₂ J j₂ K k₂ R β ;

coordinate conversion

Three-dimensional coordinate conversion can be executed twice.

(program coordinate

In the N1 block, specify the center, direction of the axis of rotation, and

system)

angular displacement of the first rotation. When this block is executed,

the center of the original coordinate system is shifted to (x₁, y₁, z₁), then

rotated around the vector (i₁, j₁, k₁) by angular displacement _α. The new

coordinate system is called X’Y’Z’. In the N2 block, specify the center,

direction of the axis of rotation, and angular displacement of the second

rotation. In the N2 block, specify coordinates and the angle with the

coordinate system formed after the N1 block in Xp, Yp, Zp, I, J, K, and

R. When the N2 block is executed, the X’Y’Z’ coordinate system is

shifted to (x₂, y₂, z₂), then rotated around the vector (i₂, j₂, k₂) by angular

displacement _β . The newest coordinate system is called X’’Y’’Z’’. In the

254

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

subsequent N3 block, coordinates in the X’’Y’’Z’’ coordinate system are

specified with Xp, Yp, and Zp. The X’’Y’’Z’’ coordinate system is called

the program coordinate system.

If (Xp, Yp, Zp) is not specified in the N2 block, (Xp, Yp, Zp) in the N1

block is assumed to be the center of the second rotation (the N1 and N2

blocks have a common center of rotation). If the coordinate system is to

be rotated only once, the N2 block need not be specified.

Example) G68 Xx₀ Yy₀ Zz₀ I0 J0 K1 Rα ;

G68 I1 J0 K0 Rβ ;

Z

Z’

Z"

Y"

β

Y’

β

P (x, y, z)

z

α

x

Y

y

O (x₀, y₀, z₀)

α

X

X, Y, Z

:

Workpiece coordinate system

X’, Y’, Z’ :

Coordinate system formed after the first conversion

X”, Y”, Z”

:

Coordinate system formed after the second conversion

α:

Angular displacement of the first rotation

β :

Angular displacement of the second rotation

O (x₀, y₀, z₀):

Center of rotation

P (x, y, z)

: Coordinates in the X’’Y’’Z’’ coordinate system (program

coordinate system)

D Format error

If one of the following format errors is detected, P/S alarm No. 5044

occurs:

1. When I, J, or K is not specified in a block with G68

(a parameter of coordinate system rotation is not specified)

2. When I, J, and K are all set to 0 in a block with G68

3. When R is not specified in a block with G68

D Center of rotation

Specify absolute coordinates with Xp, Yp, and Zp in the G68 block.

255

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

D Equation for

The following equation shows the general relationship between (x, y, z)

three-dimensional

in the program coordinate system and (X, Y, Z) in the original coordinate

coordinate conversion

system (workpiece coordinate system).

X

x

x₁

Y

= M₁

y₁

y

+

Z

z

z₁

When conversion is carried out twice, the relationship is expressed as follows:

X

x

x₂

x₁

Y

= M₁

M₂

M₁

y₂

y₁

y

+

+

Z

z

z₂

z₁

X, Y, Z

: Coordinates in the original coordinate system

(workpiece coordinate system)

x, y, z : Programmed value

(coordinates in the program coordinate system)

x₁, y₁, z₁

: Center of rotation of the first conversion

x₂, y₂, z₂

: Center of rotation of the second conversion

(coordinates in the coordinate system formed after the

first conversion)

M₁

: First conversion matrix

M₂

: Second conversion matrix

M1 and M2 are conversion matrices determined by an angular displacement and

rotation axis. Generally, the matrices are expressed as shown below:

n₁₂+(1-n₁₂) cosθ

n₁n₂ (1-cosθ)-n₃sinθ n₁n₃ (1-cosθ)+n₂sinθ

n₁ n₂ (1-cosθ)+n₃ sinθ

n₂₂+(1-n₂₂) cosθ

n₂ n₃ (1-cosθ)-n₁ sinθ

n₁ n₃ (1-cosθ)-n₂ sinθ n₂ n₃ (1-cosθ)+n₁ sinθ n₃₂+(1-n₃₂) cosθ

i

n₁

: Cosine of the angle made by the rotation axis and X-axis

p

j

n₂

: Cosine of the angle made by the rotation axis and Y-axis

p

k

n₃

: Cosine of the angle made by the rotation axis and Z-axis

p

θ: Angular displacement

Value p is obtained by the following:

p = i²+j²+k²

Conversion matrices for rotation on two-dimensional planes are shown below:

(1) Coordinate conversion on the XY plane

cosθ

-sinθ

0

M= sinθ cosθ

0

0

ă0

1

(2) Coordinate conversion on the YZ plane

1

0

0

M=

0

cosθ

-sinθ

0

sinθ

cosθ

(3) Coordinate conversion on the ZX plane

cosθ

0

sinθ

M=

0

1

0

–sinθ

0

cosθ

256

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

Examples

N1 G90 X0 Y0 Z0 ;

Carries out positioning to zero point H.

N2 G68 X10. Y0 Z0 I0 J1 K0 R30. ;

Forms new coordinate system X’Y’Z’.

N3 G68 X0 Y-10. Z0 I0 J0 K1 R-90. ; Forms other coordinate system X’’Y’’Z’’.

The origin agrees with

(0,

-10,

0) in

coordinate system X’Y’Z.

N4 G90 X0 Y0 Z0 ;

Carries out positioning to zero point H’’ on

coordinate system X’’Y’’Z’’.

N5 X10. Y10. Z0 ;

Carries out positioning to (10, 10, 0) on

coordinate system X’’Y’’Z’’.

Y

Y’

X’

10

30°

H

H’

X

N4

Y”

-10

H”

N5

Z

Z’

(10, 10, 0)

30°

Z”

X”

260

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

By specifying indexing positions (angles) for the indexing axis (one

13.11

rotation axis, A, B, or C), the index table of the machining center can be

INDEX TABLE

indexed.

INDEXING FUNCTION

Before and after indexing, the index table is automatically unclamped or

clamped .

Explanations

D Indexing position

Specify an indexing position with address A, B, or C (set to bit 0 of

parameter ROT_x No.1006).

The indexing position is specified by either of the following (depending

on bit 4 of parameter G90 No.5500):

1. Absolute value only

2. Absolute or incremental value depending on the specified G code:

G90 or G91

A positive value indicates an indexing position in the counterclockwise

direction. A negative value indicates an indexing position in the

clockwise direction.

The minimum indexing angle of the index table is the value set to

parameter 5512. Only multiples of the least input increment can be

specified as the indexing angle. If any value that is not a multiple is

specified, an P/S alarm (No. 135) occurs. Decimal fractions can also be

entered. When a decimal fraction is entered, the 1’s digit corresponds to

degree units.

A

Value specified for rotation from A to B

(case 2 described above)

G90 B-45.0 ; or

G91 B-105.0;

+60°

0°

-45°

B

D Direction and value of

The direction of rotation and angular displacement are determined by

rotation

either of the following two methods. Refer to the manual written by the

machine tool builder to find out which method is applied.

1. Using the miscellaneous function specified in parameter No. 5511

(Address) (Indexing position) (Miscellaneous function);

Rotation in the negative direction

(Address) (Indexing position);

Rotation in the positive direction (No miscellaneous functions are

specified.)

An angular displacement greater than 360°is rounded down to the

corresponding angular displacement within

360°when bit

2 of

parameter ABS No. 5500 specifies this option.

For example, when G90 B400.0 (miscellaneous function); is specified

at a position of 0 , the table is rotated by 40°in the negative direction.

261

13.

FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63534EN/02

2.

Using no miscellaneous functions

By setting to bits 2, 3, and 4 of parameter ABS, INC,G90 No.5500,

operation can be selected from the following two options.

Select the operation by referring to the manual written by the machine

tool builder.

(1) Rotating in the direction in which an angular displacement

becomes shortest

This is valid only in absolute mode. A specified angular

dis-placement greater than

360° is rounded down to the

correspond-ing angular displacement within 360° when bit 2 of

parameter ABS No.5500 specifies this option.

For example, when G90 B400.0; is specified at a position of 0, the

table is rotated by 40°in the positive direction.

(2) Rotating in the specified direction

In the absolute mode, the value set in bit 2 of parameter ABS

No.5500 determines whether an angular displacement greater than

360° is rounded down to the corresponding angular displacement

within 360°.

In the incremental mode, the angular displacement is not rounded

down.

For example, when G90 B720.0; is specified at a position of 0, the

table is rotated twice in the positive direction, when the angular

displacement is not rounded down.

D Feedrate

The table is always rotated around the indexing axis in the rapid traverse

mode.

Dry runs cannot be executed for the indexing axis.

WARNING

If a reset is made during indexing of the index table, a

reference position return must be made before each time

the index table is indexed subsequently.

NOTE

1

Specify the indexing command in a single block. If the

command is specified in a block in which another controlled

axis is specified, P/S alarm (No.136) occurs.

2

The waiting state which waits for completion of clamping or

unclamping of the index table is indicated on diagnostic

screen 12.

3

The miscellaneous function specifying a negative direction

is processed in the CNC.

The relevant M code signal and completion signal are sent

between the CNC and the machine.

4

If a reset is made while waiting for completion of clamping

or unclamping, the clamp or unclamp signal is cleared and

the CNC exits the completion wait state.

262

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

PROGRAMMING

D Indexing function and

other functions

Table 13.11 (a) Index indexing function and other functions

Item

Explanation

This value is rounded down when bit 1 of parameter REL No. 5500

Relative position display

specifies this option.

This value is rounded down when bit 2 of parameterABS No. 5500

Absolute position display

specifies this option.

Automatic return from the reference position (G29)

2nd reference position return (G30)

Impossible to return

Movement in the machine coordinate system

Impossible to move

Single direction positioning

Impossible to specify

2nd auxiliary function (B code)

Possible with any address other than B that of the indexing axis.

Unless otherwise processed by the machine, feed hold, interlock

Operations while moving the indexing axis

and emerrgency stop can be executed. Machine lock can be

executed after indexing is completed.

Disabled

SERVO OFF signal

The indexing axis is usually in the servo-off state.

The workpiece coordinate system and machine coordinate system

Incremental commands for indexing the index

must always agree with each other on the indexing axis (the work-

table

piece zero point offset value is zero.).

Manual operation is disabled in the JOG, INC, or HANDLE mode.

A manual reference position return can be made. If the axis selec-

Operations for indexing the index table

tion signal is set to zero during manual reference position return,

movement is stopped and the clamp command is not executed.

263

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

This function can be used by setting the difference between the tool length

14.1

assumed during programming and the actual tool length of the tool used

TOOL LENGTH

into the offset memory. It is possible to compensate the difference without

OFFSET

changing the program.

Specify the direction of offset with G43 or G44. Select a tool length offset

(G43, G44, G49)

value from the offset memory by entering the corresponding address and

number (H code).

Tool assumed dur-

Actual tool

ing programming

ÇÇ

ÇÇ

ÇÇ

ÇÇ

Specify this distance

ÇÇ

ÇÇ

as the value of tool

ÇÇ

length offset.

Fig. 14.1 Tool length offset

14.1.1

The following three methods of tool length offset can be used, depending

on the axis along which tool length offset can be made.

General

⋅Tool length offset A

Compensates for the difference in tool length along the Z-axis.

⋅Tool length offset B

Compensates for the difference in tool length along the X-,Y-,or

Z-axis.

⋅Tool length offset C

Compensates for the difference in tool length along a specified axis.

Format

Tool length offset A

G43 Z_ H_ ;

Explanation of each address

G44 Z_ H_ ;

G43

: Positive offset

G44

: Negative offset

Tool length offset B

G17 G43 Z_ H_ ;

G17

: XY plane selection

G17 G44 Z_ H_ ;

G18

: ZX plane selection

G18 G43 Y_ H_ ;

G19

: YZ plane selection

G18 G44 Y_ H_ ;

α : Address of a specified

G19 G43 X_ H_ ;

axis

G19 G44 X_ H_ ;

H : Address for specifying

the tool length offset

Tool length offset C

G43 α_ H_ ;

value

G44 α_ H_ ;

Tool length offset

G49 ; or H0 ;

cancel

265

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Explanations

D Selection of tool length

Select tool length offset A, B, or C, by setting bits 0 and 1 of parameter

offset

TLC,TLB No. 5001.

D Direction of the offset

When G43 is specified, the tool length offset value (stored in offset

memory) specified with the H code is added to the coordinates of the end

position specified by a command in the program. When G44 is specified,

the same value is subtracted from the coordinates of the end position. The

resulting coordinates indicate the end position after compensation,

regardless of whether the absolute or incremental mode is selected.

If movement along an axis is not specified, the system assumes that a

move command that causes no movement is specified. When a positive

value is specified for tool length offset with G43, the tool is moved

accordingly in the positive direction. When a positive value is specified

with G44, the tool is moved accordingly in the negative direction. When

a negative value is specified, the tool is moved in the opposite direction.

G43 and G44 are modal G codes. They are valid until another G code

belonging to the same group is used.

D Specification of the tool

The tool length offset value assigned to the number (offset number)

length offset value

specified in the H code is selected from offset memory and added to or

subtracted from the moving command in the program.

(1) Tool length offset A/B

When the offset numbers for tool length offset A/B are specified or

modified, the offset number validation order varies, depending on the

condition, as described below.

D When OFH (bit 2 of

parameter No. 5001) = 0

O××××;

H01 ;

:

G43Z_ ;

(1)

:

G44Z_H02 ;

(2)

:

(1) Offset number H01 is valid.

H03 ;

(3)

(2) Offset number H02 is valid.

:

(3) Offset number H03 is valid.

D When OFH (bit 2 of

parameter No. 5001) = 1

O××××;

H01 ;

:

G43Z_ ;

(1)

:

G44Z_H02 ;

(2)

:

(1) Offset number H00 is valid.

H03 ;

(3)

(2) Offset number H02 is valid.

:

(3) Offset number H02 is valid.

266

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

(2) Cutter compensation C

When the offset numbers for cutter compensation C are specified or

modified, the offset number validation order varies, depending on the

condition, as described below.

D When OFH (bit 2 of

parameter No. 5001) = 0

O××××;

H01 ;

:

G43P_ ;

(1)

(1)Offset number H01 is valid.

:

(2)Offset number H02 is valid.

G44P_H02 ;

(2)

(3)Offset number H03 is valid only for

:

the axis to which compensation

H03 ;

(3)

was applied most recently.

:

D When OFH (bit 2 of

parameter No. 5001) = 1

O××××;

H01 ;

:

G43P_ ;

(1)

:

G44P_H02 ;

(2)

(1) Offset number H00 is valid.

:

(2) Offset number H02 is valid.

H03 ;

(3)

(3) Offset number H02 is valid.

:

(However, the H number displayed

is changed to 03.)

The tool length offset value may be set in the offset memory through the

CRT/MDI panel.

The range of values that can be set as the tool length offset value is as

follows.

Metric input

Inch input

Tool length offset value

0 to ±999.999mm

0 to ±99.9999inch

WARNING

When the tool length offset value is changed due to a

change of the offset number, the offset value changes to the

new tool length offset value, the new tool length offset value

is not added to the old tool length offset value.

H1 : tool length offset value 20.0

H2 : tool length offset value 30.0

G90 G43 Z100.0 H1 ; Z will move to 120.0

G90 G43 Z100.0 H2 ; Z will move to 130.0

CAUTION

When the tool length offset is used and set a parameter

OFH (No. 5001#2) to 0, specify the tool length offset with H

code and the cutter compensation with D code.

267

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

NOTE

The tool length offset value corresponding to offset No. 0,

that is, H0 always means 0. It is impossible to set any other

tool length offset value to H0.

D Performing tool length

Tool length offset B can be executed along two or more axes when the axes

offset along two or more

are specified in two or more blocks.

axes

Offset in X and Y axes.

G19 G43 H _ ; Offset in X axis

G18 G43 H _ ; Offset in Y axis

(Offsets in X and Y axes are performed)

If the TAL bit (bit 3 of parameter No. 5001) is set to 1, an alarm will not

occur even when tool length offset C is executed along two or more axes

at the same time.

D Tool length offset cancel

To cancel tool length offset, specify G49 or H0. After G49 or H0 is

specified, the system immediately cancels the offset mode.

NOTE

S After tool length offset B is executed along two or more

axes, offset along all the axes is canceled by specifying

G49. If H0 is specified, only offset along an axis

perpendicular to the specified plane is canceled.

S In the case of the offset in three axes or more, if the offset

is canceled by G49 code, the P/S alarm 015 is generated.

Cancel the offset by using G49 and H0.

268

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

Examples

Tool length offset (in boring holes No.1, 2, and 3)

t1

t3

20

(6)

30

+Y

(9)

(13)

(1)

t2

30

+X

120

30

50

+Z

Actual position

(2)

3

Programmed

35

(12)

position

(3)

(5)

(10)

18

22

offset

(7)

(8)

30

value

(4)

(11)

ε=4mm

8

⋅Program

H1=-4.0 (Tool length offset value)

N1 G91 G00 X120.0 Y80.0 ;

(1)

N2 G43 Z-32.0 H1 ;

(2)

N3 G01 Z-21.0 F1000 ;

(3)

N4 G04 P2000 ;

(4)

N5 G00 Z21.0 ;

(5)

N6 X30.0 Y-50.0 ;

(6)

N7 G01 Z-41.0 ;

(7)

N8 G00 Z41.0 ;

(8)

N9 X50.0 Y30.0 ;

(9)

N10 G01 Z-25.0 ;

(10)

N11 G04 P2000 ;

(11)

N12 G00 Z57.0 H0 ;

(12)

N13 X-200.0 Y-60.0 ;

(13)

N14 M2 ;

269

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

14.1.2

This section describes the tool length offset cancellation and restoration

performed when G53, G28, G30, or G31 is specified in tool length offset

G53, G28, G30, and

mode. Also described is the timing of tool length offset.

G30.1 Commands in

Tool Length Offset

(1) Tool length offset vector cancellation and restoration, performed when

Mode

G53, G28, G30, or G30.1 is specified in tool length offset mode

(2) Specification of the G43/G44 command for tool length offset A/B/C,

and independent specification of the H command

Explanations

D Tool length offset vector

When G53, G28, G30, or G30.1 is specified in tool length offset mode,

cancellation

tool length offset vectors are canceled as described below. However, the

previously specified modal G code remains displayed; modal code

display is not switched to G49.

(1) When G53 is specified

Command

Specified axis

Common to type A/B/C

G53P_;

Tool length offset

Canceled upon movement being

axis

performed according to a speci-

fied value

Other than tool

Not canceled

length offset axis

NOTE

When tool length offset is applied to multiple axes, all

specified axes are subject to cancellation.

When tool length offset cancellation is specified at the same time, tool

length offset vector cancellation is performed as indicated below.

Command

Specified axis

Common to type A/B/C

Tool length offset

Canceled upon movement being

G49G53P_;

axis

performed according to a speci-

fied value

Other than tool

Canceled upon movement being

length offset axis

performed according to a speci-

fied value

(2) When G28, G30, or G30.1 is specified

Command

Specified axis

Common to type A/B/C

G28P_;

Tool length offset

Canceled upon movement to a

axis

reference position being per-

formed

Other than tool

Not canceled

length offset axis

270

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

NOTE

When tool length offset is applied to multiple axes, all

specified axes involved in reference position return are

subject to cancellation.

When tool length offset cancellation is specified at the same time, tool

length offset vector cancellation is performed as indicated below.

Command

Specified axis

Common to type A/B/C

Tool length offset

Canceled upon movement to an

G49G28P_;

axis

intermediate position being per-

formed

Other than tool

Canceled upon movement to an

length offset axis

intermediate position being per-

formed

D Tool length offset vector

Tool length offset vectors, canceled by specifying G53, G28, G30, or

restoration

G30.1 in tool length offset mode, are restored as described below.

(1) When OFH (bit 2 of parameter No. 5001) = 0

Type

EVO (bit 6 of pa-

Restoration block

rameter No. 5001)

1

Block to be buffered next

A/B

0

Block containing an H command

or G43/44 command

Ignored

Block containing an H command

C

Block containing a

G43P_/G44P_ command

(2) When OFH (bit 2 of parameter No. 5001) = 1

In a mode other than tool length offset mode

Type

EVO (bit 6 of pa-

Restoration block

rameter No. 5001)

1

Block to be buffered next

A/B

0

Block containing an H command

or G43/44 command

Ignored

Block containing an H command

C

Block containing a

G43P_/G44P_ command

271

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

In tool length offset mode

Type

EVO (bit 6 of pa-

Restoration block

rameter No. 5001)

1

Block containing a G43/G44

block

A/B

0

Block containing an H command

and G43/44 command

Ignored

Block containing a

C

G43P_H_/G44P_H_ command

WARNING

When tool length offset is applied to multiple axes, all axes

for which G53, G28, G30, and G30.1 are specified are

subject to cancellation. However, restoration is performed

only for that axis to which tool length offset was applied last;

restoration is not performed for any other axes.

NOTE

In a block containing G40, G41, or G42, the tool length

offset vector is not restored.

272

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

By issuing G37 the tool starts moving to the measurement position and

14.2

keeps on moving till the approach end signal from the measurement

AUTOMATIC TOOL

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

LENGTH

reaches the measurement position.

Difference between coordinate value when tool reaches the measurement

MEASUREMENT

position and coordinate value commanded by G37 is added to the tool

(G37)

length offset amount currently used.

Z

Ç

Ç_{A (Start position)}

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.

X

0

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

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

ment position)]

Fig. 14.2 (a) Automatic tool length measurement

Format

G92

_ ; Sets the workpiece coordinate system. (It can be set

IP

with G54 to G59. See Chapter 7, “Coordinate System.”)

Hff; Specifies an offset number for tool length offset.

G90 G37IP_ ; Absolute command

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

IP

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

Explanations

D Setting the workpiece

Set the workpiece coordinate system so that a measurement can be made

coordinate system

after moving the tool to the measurement position. The coordinate system

must be the same as the workpiece coordinate system for programming.

D 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 tip reaches the measurement position,

the measuring instrument sends an approach end signal to the CNC which

stops the tool.

273

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

D Changing the offset

The difference between the coordinates of the position at which the tool

value

reaches for measurement and the coordinates specified by G37 is added

to the current tool length offset value.

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.

D Alarm

When automatic tool length measurement is executed, the tool moves as

shown in Fig. 14.2 (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 P/S alarm number is 080.

Deceleration

feedrate

Rapid

(measurement

Approach end signal ON

traverse

feedrate)

A

B

C

D

E F

Start

position

Position commanded

by G37

Permitted range of approach end signal

Fig. 14.2 (b) Tool movement to the measurement position

274

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

WARNING

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.

NOTE

1

When an H code is specified in the same block as G37, an

alarm is generated. Specify H code before the block!of

G37.

2

The measurement speed

(parameter No.

6241),

deceleration position (parameter No. 6251), and permitted

range of the approach end signal (parameter No. 6254) are

specified by the machine tool builder.

3

When offset memory A is used, the offset value is changed.

When offset memory B is used, the tool wear compensation

value is changed.

When offset memory C is used, the tool wear compensation

value for the H code is changed.

4

The approach end signal is monitored usually every 2 ms.

The following measuring error is generated:

ERR_max. : Fm×1/60×T_S/1000 where

T_S

: Sampling period, for usual 2 (ms)

ERR_max. : maximum measuring error (mm)

F_m

: measurement federate (mm/min.)

For example, when F_m = 1000 mm/min., ERR_max. = 0.003m

5

The tool stops a maximum of 16 ms after the approach end

signal is detected. But the value of the position!at which the

approach end signal was detected (note the value when the

tool stopped) is used to determine the

offset amount. The overrun for 16 ms is:

Q_max. = F_m × 1/60 ×16/1000

Q_max.: maximum overrun (mm)

F_m

:

measurement federate (mm/min.)

275

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Examples

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).

Z

Ç

ÇÇ

ÇÇÇÇ

760

Ç

200

Measurement

position along Z axis

0

850

1100

X

276

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

14.3

The programmed travel distance of the tool can be increased or decreased

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

TOOL OFFSET

The tool offset function can also be applied to an additional

(G45-G48)

axis.

Workpiece

ÇÇ

ÇÇÇ

Tool center path

Programmed path

ool

ÇÇT

Format

G45

IP

_D_ ; Increase the travel distance by the tool offset value

G46IP

_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 G48 : One-shot G code for increasing or decreasing the travel

distance

: Command for moving the tool

IP

D : Code for specifying the tool offset value

277

14. COMPENSATION FUNCTION

PROGRAMMING

B-63534EN/02

Explanations

D Increase and decrease

As shown in Table 14.3(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 position of the previous block to the position

specified by the block containing G45 to G48.

Table 14.3 (a) Increase and decrease of the tool travel distance

When a positive tool offset val-

When a negative tool offset

G code

ue is specified

value is specified

G45

Start position

End position

Start position

End position

G46

Start position

End position

Start position

End position

G47

Start position

End position

Start position

End position

G48

Start position

End position

Start position

End position

Programmed movement distance

Tool offset value

Actual movement position

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

incremental command (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 command (G90) mode, the tool is not moved.

D 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:

Table 14.3 (b) Range of tool offset values

Metric input

inch input

Tool offset value

0 to ±999.999mm

0 to ±99.9999inch

0 to ±999.999deg

0 to ±999.999deg

D0 always indicates a tool offset value of zero.

278

PROGRAMMING

14. COMPENSATION FUNCTION

B-63534EN/02

WARNING

1

When G45 to G48 is specified to n axes (n=1-6) 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 or G42) shown in II-14.4 or 14.5.

Shape actually cut

Desired shape

Ç

ÇÇÇ

ÇÇ

ÇÇÇ

ÇÇ

Desired

Shape actually cut

shape

Y axis

Y axis

ÇÇ

ÇÇÇ

ÇÇÇ

ÇÇÇ

ÇÇÇ

Overcutting

Undercutting

X axis

X axis

G01 X_ F_ ;

G01 G45 X_ F_ D_;

G47 X_ Y_ D_ ;

X_ Y_ ;

Y_ ;

G45 Y_ ;

2

G45 to G48 (tool offset) must not be used in the G41 or G42 (cutter compensation) mode.

279

Content      ..     8      9      10      11     ..