Content      ..     6      7      8      9     ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 8

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

PROGRAMMING

13.3.4

An intermittent-feed surface grinding cycle is performed.

Intermittent-Feed

Surface Grinding Cycle

(G79)

Format

G79 I_ J_ K_ X_ R_ F_ P_ L_ ;

I_ : Depth-of-cut 1 (A sign in the command specifies the direction

of cutting.)

J_

: Depth-of-cut 2 (A sign in the command specifies the direction

of cutting.)

K_ : Total depth of cut (A sign in the command specifies the direction

of cutting.)

X(Z)_ : Range of grinding (A sign in the command specifies the

direction of grinding.)

R_ : Feedrate for I and J

F_ : Feedrate for X (Z)

P_ : Dwell time

L_

: Grinding-wheel wear compensation (Only for continuous dressing)

G79

Z

X

I

(R)

(F)

J

P

(R)

(F)

P

X

Explanations

The intermittent-feed surface grinding cycle consists of six operation

sequences. Operations

to

are repeated until the depth reaches the

total depth of cut specified at address K. In the single block stop mode,

operations

to

are performed every cycle start.

D Grinding wheel cutting

Cutting is performed along the Z-axis in cutting feed mode for the

amount specified by I (depth of cut 1). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Cutting feed is performed for the amount specified by X (or Z). The

feedrate is specified by F.

D Grinding wheel cutting

Cutting is performed along the Z-axis in cutting feed mode for the

amount specified by J (depth of cut 2). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Feeding is performed in the reverse direction for the amount specified

(return direction)

by X at a feedrate specified by F.

193

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64124EN/01

Checking the Minimum

Compensation amounts set in offset memory can be modified by using the

Grinding Wheel Diameter

external tool compensation function or programming (by changing

(For Grinding Machine)

offsets using custom macro variables).

With these functions, the compensation amount for the diameter of the

dressed grinding wheel can be changed.

If the compensation amount associated with the offset number specified

in the H code is smaller than the minimum grinding wheel diameter

specified in parameter 5030 when programmed compensation (using G43

or G44) is performed, a signal is output to the PMC.

a : Amount of dressing

Dresser

2a

V

Y

Grinding

wheel

a

X

Workpiece

X

196

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

PROGRAMMING

Every time an external signal is input, cutting is performed by a fixed

13.5

amount according to the programmed profile in the specified Y-Z plane.

IN-FEED GRINDING

ALONG THE Y AND Z

AXES AT THE END

OF TABLE SWING

(FOR GRINDING

MACHINE)

Format

G161 R_ ;

profile program

G160 ;

Explanations

D G161 R_

Specify the start of an operation mode and profile program. Also specify

the depth of cut in R.

D Profile program

Program a workpiece figure in the Y-Z plane using linear interpolation

(G01) and/or circular interpolation (G02 or G03). One or more blocks can

be specified.

D G160

Cancel the operation mode (end of the profile program).

Restrictions

D Profile program

Do not specify codes other than G01, G02, and G03 within the profile

program.

Examples

O0001 ;

:

N0 G161 R10.0 ;

N1 G91 G01 Z-70.0 F100 ;

N2 G19 G02 Z-80.0 R67.0 ;

N3 G01 Z-70.0 ;

N4 G160 ;

:

70.0

80.0

70.0

α

N2

N3

N1

R=67.000

Y

Z

In the above program, every time the in-feed cutting start signal is input,

the tool is moved by 10.000 along the machining profile shown above.

α= Travel distance for each in-feed control cutting start signal input

The feedrate is programmed with an F code.

197

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64124EN/01

Chamfering and corner rounding blocks can be inserted automatically

13.6

between the following:

OPTIONAL ANGLE

⋅Between linear interpolation and linear interpolation blocks

CHAMFERING AND

⋅Between linear interpolation and circular interpolation blocks

⋅Between circular interpolation and linear interpolation blocks

CORNER ROUNDING

⋅Between circular interpolation and circular interpolationblocks

Format

, C_

Chamfering

, R_

Corner R

Explanations

When the above specification is added to the end of a block that specifies

linear interpolation (G01) or circular interpolation (G02 or G03), a

chamfering or corner rounding block is inserted.

Blocks specifying chamfering and corner rounding can be specified

consecutively.

D Chamfering

After C, specify the distance from the virtual corner point to the start and

end points. The virtual corner point is the corner point that would exist

if chamfering were not performed.

(1) G91 G01 X100.0 ,C10.0 ;

(2) X100.0 Y100.0 ;

Inserted chamfering block

C

C

Hypothetical corner intersection

D Corner R

After R, specify the radius for corner rounding.

(1) G91 G01 X100.0 ,R10.0 ;

(2) X100.0 Y100.0 ;

Center of a circle with radius R

R

198

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

PROGRAMMING

Examples

N001 G92 G90 X0 Y0 ;

N002 G00 X10.0 Y10.0 ;

N003 G01 X50.0 F10.0 ,C5.0 ;

N004 Y25.0 ,R8.0 ;

N005 G03 X80.0 Y50.0 R30.0 ,R8.0 ;

N006 G01 X50.0 ,R8.0 ;

N007 Y70.0 ,C5.0 ;

N008 X10.0 ,C5.0 ;

N009 Y10.0 ;

N010 G00 X0 Y0 ;

N011 M0 ;

Y

N008

70.0

N007

60.0

N006

50.0

40.0

N009

N005

30.0

20.0

N004

10.0

N003

N010

N002

N011

0

N001

X

10.0

20.0

30.0

40.0

50.0

60.0

70.0

80.0

199

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64124EN/01

Restrictions

D Plane selection

Chamfering and corner rounding can be performed only in the plane

specified by plane selection (G17, G18, or G19). These functions cannot

be performed for parallel axes.

D Next block

A block specifying chamfering or corner rounding must be followed by

a block that specifies a move command using linear interpolation (G01)

or circular interpolation (G02 or G03). If the next block does not contain

these specifications, P/S alarm No. 052 is issued.

D Plane switching

A chamfering or corner rounding block can be inserted only for move

commands which are performed in the same plane. In a block that comes

immediately after plane switching (G17, G18, or G19 is specified),

neither chamfering nor corner rounding can be specified.

D Exceeding the move

If the inserted chamfering or corner rounding block causes the tool to go

range

beyond the original interpolation move range, P/S alarm No.055 is issued.

G91 G01 X30.0 ;

G03 X7.5 Y16.0 R37.0 ,C28.0 ;

G03 X67.0 Y-27.0 R55.0 ;

The tool path without

C

C

chamfering is indicated

with a solid line.

Chamfering block to

be inserted

D Coordinate system

In a block that comes immediately after the coordinate system is changed

(G92, or G52 to G59) or a return to the reference position (G28 to G30)

is specified, neither chamfering nor corner rounding can be specified.

D Travel distance 0

When two linear interpolation operations are performed, the chamfering

or corner rounding block is regarded as having a travel distance of zero

if the angle between the two straight lines is within +1 . When linear

interpolation and circular interpolation operations are performed, the

corner rounding block is regarded as having a travel distance of zero if the

angle between the straight line and the tangent to the arc at the intersection

is within +1 . When two circular interpolation operations are performed,

the corner rounding block is regarded as having a travel distance of zero

if the angle between the tangents to the arcs at the intersection is within

+1 .

The following G codes cannot be used in a block that specifies chamfering

D Unavailable G codes

or corner rounding. They also cannot be used between chamfering and

corner rounding blocks that define a continuous figure.

⋅G codes of group 00 (except G04)

⋅G68 of group 16

D Threading

Corner rounding cannot be specified in a threading block.

D DNC operation

DNC operation cannot be applied to optional-angle chamfering or corner

rounding.

200

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64124EN/01

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

13.8

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.

202

13. FUNCTIONS TO SIMPLIFY

B-64124EN/01

PROGRAMMING

PROGRAMMING

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.

203

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64124EN/01

D Indexing function and

other functions

Table 13.8 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)

Impossible to return

2nd reference position return (G30)

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.

204

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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 (G43, G44,

changing the program.

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

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

206

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

(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.

208

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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 ;

210

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

14.1.2

This section describes the tool length offset cancellation and restoration

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

G53, G28, and G30

Also described is the timing of tool length offset.

Commands in Tool

Length Offset Mode

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

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

cancellation

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, or G30 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

211

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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, or G30 in

restoration

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

212

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

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, and G30 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.

213

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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.

A difference is determined between a coordinate value obtained when the

MEASUREMENT

tool reaches the measurement position and a coordinate value specified

(G37)

by G37. The difference is then added to the wear compensation value for

the H code of an offset number 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 II-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.

214

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

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

215

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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

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

4

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.)

216

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

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

217

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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 axis.

(G45-G48)

Workpiece

ÇÇÇ

Tool center path

Programmed path

ÇÇÇ

Tool

ÇÇ

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

218

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

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.

219

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

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.

220

B-64124EN/01

PROGRAMMING

14. COMPENSATION FUNCTION

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 tool

Program command

Start

Example

End

position

G46 X2.50 ;

position

Tool offset value

Equivalent command

+3.70

X-1.20 ;

Tool offset value

2

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 rotation be not specified at the same time. This function is provided for

compatibility with the conventional CNC tape without any cutter compensation. The function

should not be used when a new CNC program is prepared.

Tool offset for circular interpolation

Program

ÇÇ

N4

ÇÇ

N1 G46 G00 X_ Y_ D_ ;

N2 G45 G01 Y_ F_ ;

ÇÇN3ÇÇ

N3 G45 G03 X_ Y_ I_ ;

N4 G01 X_ ;

ÇÇÇ

Programmed tool path

ÇÇ

N2

Actual tool path

ÇÇ

N1

ÇÇÇ

ÇÇÇ

3

D code should be used in tool offset mode (G45 to G48). However, H code can be used by

setting the parameter TPH (No. 5001#5) because of compatibility with conventional CNC tape

format. The H code must be used under tool length offset cancel (G49).

4

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.

221

14. COMPENSATION FUNCTION

PROGRAMMING

B-64124EN/01

Examples

Program using tool offset

N12

N11

30R

N9

40

N10

N13

N8

N4

30R

40

N3

N5

N1

N7

N2

N6

50

ÇÇÇ

N14

ÇÇÇ

80

50

40

30

30

OriginÇÇ

Y axis

Tool diameter

:

20φ

Offset No.

:

01

Tool offset value

:

+10.0

X axis

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 theoffset 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 X80.0 Y-50.0 ;

222

Content      ..     6      7      8      9     ..