Content      ..     4      5      6      7     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 6

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

(a) Manual intervention performed when the manual absolute signal is off

(b) Move command executed in the machine lock state

(c) Movement by handle interrupt

(d) Operation using the mirror image function

(e) Setting the local coordinate system using G52, or shifting the

workpiece coordinate system using G92

In the case of (a) above, the workpiece coordinate system is shifted by the

amount of movement during manual intervention.

G54 workpiece coordinate

system before manual

Po

intervention

Amount of movement

during manual

intervention

Workpiece zero

WZo

point offset

value

Pn

Machine zero point

G54 workpiece coordinate

system after manual intervention

WZn

In the operation above, a workpiece coordinate system once shifted can

be preset using G code specification or MDI operation to a workpiece

coordinate system displaced by a workpiece zero point offset value from

the machine zero point. This is the same as when manual reference

position return operation is performed on a workpiece coordinate system

that has been shifted. In this example, such G code specification or MDI

operation has the effect of returning workpiece coordinate system zero

point WZn to the original zero point WZo, and the distance from WZo to

Pn is used to represent the current position in the workpiece coordinate

system.

Bit 3 (PPD) of parameter No. 3104 specifies whether to preset relative

coordinates (RELATIVE) as well as absolute coordinates.

When no workpiece coordinate system option (G54 to G59) is selected,

the workpiece coordinate system is preset to the coordinate system set by

automatic workpiece coordinate system setting. When automatic

workpiece coordinate system setting is not selected, the workpiece

coordinate system is preset with its zero point placed at the reference

position.

Limitations

D Cutter compensation,

When using the workpiece coordinate system preset function, cancel

tool length

compensation modes: cutter compensation, tool length compensation,

compensation, tool

and tool offset. If the function is executed without cancelling these

offset

modes, compensation vectors are temporarily cancelled.

D Program restart

The workpiece coordinate system preset function is not executed during

program restart.

D Prohibited modes

Do not use the workpiece coordinate system preset function when the

scaling, coordinate system rotation, programmable image, or drawing

copy mode is set.

130

B-63534EN/02

PROGRAMMING

7. COORDINATE SYSTEM

7.2.5

Besides the six workpiece coordinate systems (standard workpiece

coordinate systems) selectable with G54 to G59, 48 additional workpiece

Adding Workpiece

coordinate systems (additional workpiece coordinate systems) can be

Coordinate Systems

used. Alternatively, up to 300 additional workpiece coordinate systems

(G54.1 or G54)

can be used.

Format

D Selecting the additional

G54.1Pn ; or G54Pn ;

workpiece coordinate

Pn : Codes specifying the additional workpiece coordinate systems

systems

n

:

1 to 48 or 1 to 300

D Setting the workpiece

zero point offset value in

the additional workpiece

G10L20 Pn IIP_;

coordinate systems

Pn : Codes specifying the workpiece coordinate system for setting

the workpiece zero point offset value

n

:

1 to 48 or 1 to 300

IP_ : Axis addresses and a value set as the workpiece zero point

offset

Explanations

D Selecting the additional

When a P code is specified together with G54.1 (G54), the corresponding

workpiece coordinate

coordinate system is selected from the additional workpiece coordinate

systems

systems (1 to 48 or 1 to 300).

A workpiece coordinate system, once selected, is valid until another

workpiece coordinate system is selected. Standard workpiece coordinate

system 1 (selectable with G54) is selected at power-on.

G54.1 P1 . . . Additional workpiece coordinate system 1

G54.1 P2 . . . Additional workpiece coordinate system 2

G54.1 P48 . . Additional workpiece coordinate system 48

G54.1 P300 . Additional workpiece coordinate system 300

D Setting the workpiece

When an absolute workpiece zero point offset value is specified, the

zero point offset value in

specified value becomes a new offset value. When an incremental

the additional workpiece

workpiece zero point offset value is specified, the specified value is added

coordinate systems

to the current offset value to produce a new offset value.

As with the standard workpiece coordinate systems, the following

operations can be performed for a workpiece zero point offset in an

additional workpiece coordinate system:

(1) The OFFSET function key can be used to display and set a workpiece

zero point offset value.

(2) The G10 function enables a workpiece zero point offset value to be set

by programming (refer to II-7.2.3).

131

B-63534EN/02

PROGRAMMING

7. COORDINATE SYSTEM

When a program is created in a workpiece coordinate system, a child

7.3

workpiece coordinate system can be set for easier programming. Such a

LOCAL COORDINATE

child coordinate system is referred to as a local coordinate system.

SYSTEM

Format

G52 IP _; Setting the local coordinate system

G52 IIP0 ; Canceling of the local coordinate system

I

IP

Explanations

By specifying G52 IP _;, a local coordinate system can be set in all the

workpiece coordinate systems (G54 to G59). The origin of each local

coordinate system is set at the position specified by IP _ in the workpiece

coordinate system.

When a local coordinate system is set, the move commands in absolute

mode (G90), which is subsequently commanded, are the coordinate

values in the local coordinate system. The local coordinate system can

be changed by specifying the G52 command with the zero point of a new

local coordinate system in the workpiece coordinate system.

To cancel the local coordinate system and specify the coordinate value in

the workpiece coordinate system, match the zero point of the local

coordinate system with that of the workpiece coordinate system.

(Local coordinate system)

IP

(G54 : Workpiece coordinate system 1)

(Local coordinate system)

G55

G56

IP

G57

G58

(G59 : Workpiece coordinate system 6)

(Machine coordinate system)

Machine coordinate system origin

Reference point

Fig. 7.3 Setting the local coordinate system

133

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

WARNING

1

When an axis returns to the reference point by the manual reference point return function,the

zero point of the local coordinate system of the axis matches that of the work coordinate system.

The same is true when the following command is issued:

G52α0;

α:Axis which returns to the reference point

2

The local coordinate system setting does not change the workpiece and machine coordinate

systems.

3

Whether the local coordinate system is canceled at reset depends on the parameter setting.

The local coordinate system is canceled when either CLR, bit 6 of parameter No.3402 or RLC,

bit 3 of parameter No.1202 is set to 1.

4

If coordinate values are not specified for all axes when setting a workpiece coordinate system

with the G92 command, the local coordinate systems of axes for which coordinate values were

not specified are not cancelled, but remain unchanged.

5

G52 cancels the offset temporarily in cutter compensation.

6

Command a move command immediately after the G52 block in the absolute mode.

134

B-63534EN/02

PROGRAMMING

7. COORDINATE SYSTEM

Select the planes for circular interpolation, cutter compensation, and

7.4

drilling by G-code.

PLANE SELECTION

The following table lists G-codes and the planes selected by them.

Explanations

Table 7.4 Plane selected by G code

Selected

G code

Xp

Yp

Zp

plane

G17

Xp Yp plane

X-axis or an

Y-axis or an

Z-axis or an

G18

Zp Xp plane

axis parallel

axis parallel

axis parallel

to it

to it

to it

G19

Yp Zp plane

Xp, Yp, Zp are determined by the axis address appeared in the block in

which G17, G18 or G19 is commanded.

When an axis address is omitted in G17, G18 or G19 block, it is assumed

that the addresses of basic three axes are omitted.

Parameter No. 1022 is used to specify that an optional axis be parallel to

the each axis of the X, Y-, and Z-axes as the basic three axes.

The plane is unchanged in the block in which G17, G18 or G19 is not

commanded.

When the power is turned on or the CNC is reset, G17 (XY plane), G18

(ZX plane), or G19 (YZ plane) is selected by bits 1 (G18) and 2 (G19) of

parameter 3402.

The movement instruction is irrelevant to the plane selection.

Examples

Plane selection when the X-axis is parallel with the U-axis.

G17X_Y_ XY plane,

G17U_Y_ UY plane

G18X_Z_ ZX plane

X_Y_ Plane is unchanged (ZX plane)

G17

XY plane

G18

ZX plane

G17 U_

UY plane

G18Y_ ;

ZX plane, Y axis moves regardless without any

relation to the plane.

135

8. COORDINATE VALUE

B-63534EN/02

PROGRAMMING

AND DIMENSION

There are two ways to command travels of the tool; the absolute

8.1

command, and the incremental command. In the absolute command,

ABSOLUTE AND

coordinate value of the end position is programmed; in the incremental

INCREMENTAL

command, move distance of the position itself is programmed. G90 and

G91 are used to command absolute or incremental command,

PROGRAMMING

respectively.

(G90, G91)

Format

Absolute command

G90

IP

_ ;

Incremental command G91

IP

_ ;

Examples

G90 X40.0 Y70.0 ;

Absolute command

G91 X-60.0 Y40.0 ; Incremental command

Y

End position

70.0

30.0

Start position

X

40.0

100.0

137

8. COORDINATE VALUE

PROGRAMMING

AND DIMENSION

B-63534EN/02

The end point coordinate value can be input in polar coordinates (radius

8.2

and angle).

POLAR COORDINATE

The plus direction of the angle is counterclockwise of the selected plane

COMMAND

first axis + direction, and the minus direction is clockwise.

Both radius and angle can be commanded in either absolute or

(G15, G16)

incremental command (G90, G91).

Format

Gjj Gff G16 ;

Starting the polar coordinate command (polar

coordinate mode)

Gff

IP _ ;

Polar coordinate command

G15 ;

Canceling the polar coordinate command (polar coordinate

mode)

G16

Polar coordinate command

G15

Polar coordinate command cancel

Gjj

Plane selection of the polar coordinate command

(G17, G18 or G19)

Gff G90 specifies the zero point of the work coordinate system as

the origin of the polar coordinate system, from which a radius

is measured.

G91 specifies the current position as the origin of the polar

coordinate system, from which a radius is measured.

IP

_

Specifying the addresses of axes constituting the plane se-

lected for the polar coordinate system, and their values

First axis : radius of polar coordinate

Second axis : angle of polar coordinate

D Setting the zero point of

Specify the radius (the distance between the zero point and the point) to

the workpiece

be programmed with an absolute command. The zero point of the work

coordinate system as the

coordinate system is set as the origin of the polar coordinate system.

origin of the polar

When a local coordinate system (G52) is used, the origin of the local

coordinate system

coordinate system becomes the center of the polar coordinates.

Command position

Command position

Radius

Radius

Actual position

Angle

Angle Actual position

When the angle is specified

When the angle is specified

with an absolute command

with an incremental command

138

8. COORDINATE VALUE

B-63534EN/02

PROGRAMMING

AND DIMENSION

D Setting the current

Specify the radius (the distance between the current position and the

position as the origin of

point) to be programmed with an incremental command. The current

the polar coordinate

position is set as the origin of the polar coordinate system.

system

Command position

Command position

Angle

Radius

Radius

Angle

Actual position

Actual position

When the angle is specified

When the angle is specified

with an absolute command

with an incremental command

Examples

Bolt hole circle

Y

- The zero point of the work coordinate

system is set as the origin of the polar

coordinate system.

- The XY plane is selected.

150°

30°

270°

X

100mm

D Specifying angles and a

N1 G17 G90 G16 ;

radius with absolute

Specifying the polar coordinate command and selecting the XY plane

commands

Setting the zero point of the work coordinate system as the origin of the

polar coordinate system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ;

Specifying a distance of 100 mm and an angle of 30 degrees

N3 Y150.0 ;

Specifying a distance of 100 mm and an angle of 150 degrees

N4 Y270.0 ;

Specifying a distance of 100 mm and an angle of 270 degrees

N5 G15 G80 ;

Canceling the polar coordinate command

D Specifying angles with

N1 G17 G90 G16;

incremental commands

Specifying the polar coordinate command and selecting the XY plane

and a radius with

Setting the zero point of the work coordinate system as the origin of the

absolute commands

polar coordinate system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ;

Specifying a distance of 100 mm and an angle of 30 degrees

N3 G91 Y120.0 ;

Specifying a distance of 100 mm and an angle of +120 degrees

N4 Y120.0 ;

Specifying a distance of 100 mm and an angle of +120 degrees

139

8. COORDINATE VALUE

B-63534EN/02

PROGRAMMING

AND DIMENSION

Either inch or metric input can be selected by G code.

8.3

INCH/METRIC

CONVERSION

(G20, G21)

Format

G20 ; Inch input

G21 ;_{mm input}

This G code must be specified in an independent block before setting the

coordinate system at the beginning of the program. After the G code for

inch/metric conversion is specified, the unit of input data is switched to

the least inch or metric input increment of increment system IS-B or IS-C

(II-2.3). The unit of data input for degrees remains unchanged.The unit

systems for the following values are changed after inch/metric

conversion:

- Feedrate commanded by F code

- Positional command

- Work zero point offset value

- Tool compensation value

- Unit of scale for manual pulse generator

- Movement distance in incremental feed

- Some parameters

When the power is turned on, the G code is the same as that held before

the power was turned off.

WARNING

1

G20 and G21 must not be switched during a program.

2

When switching inch input (G20) to metric input (G21) and vice versa, the tool compensation

value must be re-set according to the least input increment.

However, when bit 0 (OIM) of parameter 5006 is 1, tool compensation values are automatically

converted and need not be re-set.

CAUTION

For the first G28 command after switching inch input to metric input or vice versa, operation from

the intermediate point is the same as that for manual reference position return. The tool moves

from the intermediate point in the direction for reference position return, specified with bit 5

(ZMI) of parameter No. 1006.

NOTE

1

When the least input increment and the least command increment systems are different, the

maximum error is half of the least command increment. This error is not accumulated.

2

The inch and metric input can also be switched using settings (see III-11.4.3).

141

8. COORDINATE VALUE

PROGRAMMING

AND DIMENSION

B-63534EN/02

Numerical values can be entered with a decimal point. A decimal point

8.4

can be used when entering a distance, time, or speed. Decimal points can

DECIMAL POINT

be specified with the following addresses:

PROGRAMMING

X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, and F.

Explanations

There are two types of decimal point notation: calculator-type notation

and standard notation.

When calculator-type decimal notation is used, a value without decimal

point is considered to be specified in millimeters inch,or deg. When

standard decimal notation is used, such a value is considered to be

specified in least input increments.Select either calculator-type or

standard decimal notation by using the DPI bit (bit 0 of parameter

3401).Values can be specified both with and without decimal point in a

single program.

Examples

Pocket calculator

Standard type decimal

Program command

type decimal point

point programming

programming

X1000

1000mm

1mm

Command value without

Unit : mm

Unit : Least input increment

decimal point

(0.001 mm)

X1000.0

1000mm

1000mm

Command value with

Unit : mm

Unit : mm

decimal point

WARNING

In a single block, specify a G code before entering a value. The position of decimal point may

depend on the command.

Examples:

G20;

Input in inches

X1.0 G04;

X1.0 is considered to be a distance and processed as X10000. This command

is equivalent to G04 X10000. The tool dwells for 10 seconds.

G04 X1.0;

Equivalent to G04 X1000. The tool dwells for one second.

NOTE

1 Fractions less than the least input increment are truncated.

Examples:

X1.23456;

Truncated to X1.234 when the least input increment is 0.001 mm.

Processed as X1.2345 when the least input increment is 0.0001 inch.

2 When more than eight digits are specified, an alarm occurs. If a value is entered with a decimal

point, the number of digits is also checked after the value is converted to an integer according

to the least input increment.

Examples:

X1.23456789; P/S alarm 0.003 occurs because more than eight digits are specified.

X123456.7; If the least input increment is 0.001 mm, the value is converted to integer

123456700. Because the integer has more than eight digits, an alarm occurs.

142

9. SPINDLE SPEED FUNCTION

B-63534EN/02

PROGRAMMING

(S FUNCTION)

Specify the surface speed (relative speed between the tool and workpiece)

9.3

following S. The spindle is rotated so that the surface speed is constant

CONSTANT

regardless of the position of the tool.

SURFACE SPEED

CONTROL (G96, G97)

Format

D Constant surface speed

control command

G96 Sfffff ;

↑ Surface speed (m/min or feet/min)

Note : This surface speed unit may change according to machine tool

builder’s specification.

D Constant surface speed

control cancel command

G97 Sfffff ;

↑ Spindle speed (min^-1)

Note : This surface speed unit may change according to machine tool

builder’s specification.

D Constant surface speed

controlled axis

G96 Pα ;_{P0 : Axis set in the parameter (No. 3770)}

command

P1 : X axis, P2 : Y axis, P3 : Z axis, P4 : 4th axis

P5 : 5th axis, P6 : 6th axis, P7 : 7th axis, P8 : 8th axis

D Clamp of maximum

spindle speed

G92 S_ ;

The maximum spindle speed (min^-1) follows S.

145

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-63534EN/02

Explanations

D Constant surface speed

G96 (constant surface speed control command) is a modal G code. After

control command (G96)

a G96 command is specified, the program enters the constant surface

speed control mode (G96 mode) and specified S values are assumed as a

surface speed. A G96 command must specify the axis along which

constant surface speed control is applied. A G97 command cancels the

G96 mode.When constant surface speed control is applied, a spindle

speed higher than the value specified in G92S_; (maximum spindle

speed) is clamped at the maximum spindle speed. When the power is

turned on, the maximum spindle speed is not yet set and the speed is not

clamped.S (surface speed) commands in the G96 mode are assumed as S

= 0 (the surface speed is 0) until M03 (rotating the spindle in the positive

direction) or M04 (rotating the spindle in the negative direction) appears

in the program.

Spindle speed (min^-1)

The spindle speed (min^-1) almost

coincides with the surface speed

(m/min) at approx. 160 mm (radius).

Surface speed

S is 600 m/min.

radius (mm)

Fig. 9.3 (a) Relation between workpiece radius, spindle speed

and surface speed

D Setting the workpiece

To execute the constant surface speed control, it is necessary to set the

coordinate system for

work coordinate system , and so the coordinate value at the center of the

constant surface speed

rotary axis, for example, Z axis, (axis to which the constant surface speed

control

control applies) becomes zero.

X

Z

0

Fig. 9.3 (b) Example of the workpiece coordinate system for

constant surface speed control

146

9. SPINDLE SPEED FUNCTION

B-63534EN/02

PROGRAMMING

(S FUNCTION)

D Surface speed specified

in the G96 mode

G96 mode

G97 mode

Specify the surface speed in m/min

(or feet/min)

G97 command

Store the surface speed in m/min

(or feet/min)

Specified

Command for

The specified

the spindle

spindle speed

speed

(rpm) is used

Not specified

The surface speed (m/min or

feet/min) is converted to the

spindle speed (rpm)

Commands other than G96

G96 command

Specified

The specified

surface

Command

speed is used

for the surface

speed

Not specified

The stored surface speed (m/min or

feet/min) is used. If no surface speed

is stored, 0 is assumed.

Restrictions

D Constant surface speed

The constant surface speed control is also effective during threading.

control for threading

Accordingly, it is recommended that the constant surface speed control

be invalidated with G97 command before starting the scroll threading and

taper threading, because the response problem in the servo system may

not be considered when the spindle speed changes.

D Constant surface speed

In a rapid traverse block specified by G00, the constant surface speed

control for rapid traverse

control is not made by calculating the surface speed to a transient change

(G00)

of the tool position, but is made by calculating the surface speed based on

the position at the end point of the rapid traverse block, on the condition

that cutting is not executed at rapid traverse.

147

9. SPINDLE SPEED FUNCTION

B-63534EN/02

PROGRAMMING

(S FUNCTION)

Explanations

The fluctuation of the spindle speed is detected as follows:

1. When an alarm is issued after a specified spindle speed is reached

Spindle speed

r

d

q

Specified

speed

q

d

r

Actual speed

Check

Check

No check

Time

Specification of

Start of check

Alarm

another speed

2. When an alarm is issued before a specified spindle speed is reached

Spindle speed

r

q

d

Specified

speed

q

d

r

p

Actual speed

Check

No check

Check

Time

Specification of

Start of check

Alarm

another speed

Specified speed :

(Speed specified by address S and five-digit value)×(spindle override)

Actual speed : Speed detected with a position coder

p : Time elapses since the specified speed changes until a check starts.

q : (Percentage tolerance for a check to start)×(specified speed)

r : (Percentage fluctuation detected as an alarm condition)×(specified speed)

d : Fluctuation detected as an alarm (specified in parameter (No.4913))

An alarm is issued when the difference between the specified speed and the actual

speed exceeds both r and d.

149

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-63534EN/02

NOTE

1

When an alarm is issued in automatic operation, a single

block stop occurs. The spindle overheat alarm is indicated

on the screen, and the alarm signal “SPAL” is output (set to

1 for the presence of an alarm). This signal is cleared by

resetting.

2

Even when reset operation is performed after an alarm

occurs, the alarm is issued again unless the cause of the

alarm is corrected.

3

No check is made during spindle stop state (*SSTP = 0).

4

By setting the parameter (No. 4913), an allowable range of

speed fluctuations can be set which suppresses the

occurrence of an alarm. However, an alarm is issued one

second later if the actual speed is found to be 0 rpm.

150

10. TOOL FUNCTION

B-63534EN/02

PROGRAMMING

(T FUNCTION)

10.2

Tools are classified into various groups, with the tool life (time or

frequency of use) for each group being specified. The function of

TOOL LIFE

accumulating the tool life of each group in use and selecting and using

MANAGEMENT

the next tool previously sequenced in the same group, is called the tool

FUNCTION

life management function.

Tool group number m

Code specifying

Tool

1

Tool life

The first tool life

tool compensa-

number

tion value

management data

n

The nth tool life

management data

Fig. 10.2 (a) Tool life management data (number of n tools)

By choosing a tool from a tool group specified by a machining program,

the tool life can be managed.

Tool life management data

Machining program

Machine and CNC operations

Tool group number 1

Machine

CNC

Places a se-

Automatically selects, from

Tool

lected tool in

tool group m, a tool whose

selection

Command for selecting

the wait state

life has not expired.

Tool group number m

tool group m

Attaches the

Starts counting the life of

tool in the wait

Tool change command

the tool attached to the

state to

(M06)

spindle.l

the spindle

Tool group number p

(tool change).

Fig. 10.2 (b) Tool Selection by Machining Program

For two-path control, tool life management is applied independently for

each path. Tool life management data is also set for each path.

153

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-63534EN/02

10.2.1

Tool life management data consists of tool group numbers, tool numbers,

codes specifying tool compensation values, and tool life value.

Tool Life Management

Data

Explanations

D Tool group number

The Max. number of groups and the number of tools per group that can

be registered are set by parameter (GS1,GS2 No. 6800#0, #1) (Table

10.2.1 (a)).

Table 10.2.1 (a) The Max. number of groups and tools that can be registered

The Max. number of groups and

The Max. number of groups

tools without optional function

and tools with optional function

GS1

GS2

of 512 tool pairs

of 512 tool pairs

(No. 6800#0)

(No. 6800#1)

Number of group

Number of tool

Number of group

Number of tool

0

0

16

16

64

32

0

1

32

8

128

16

1

0

64

4

256

8

1

1

128

2

512

4

WARNING

When bits 0 or 1 of parameter GS1,GS2 No.6800 is

changed, re-register tool life management data with the

G10L3 command (for registering and deleting data for all

groups). Otherwise, new data pairs cannot be set.

D Tool number

Specify a four-digit number after T.

D Code specifying tool

Codes specifying tool offset values are classified into H codes (for tool

compensation value

length offset) and D codes (cutter compensation). The maximum number

of the tool compensation value specification code which can be registered

is 255 when there are 400 tool compensation values (even if the option

for 512 tool life management sets is supported). The maximum number

is 32, 64, 99, 200, 499, or 999 when there are 32, 64, 99, 200, 499, or 999

tool compensation values.

NOTE

When codes specifying tool offset values are not used,

registration can be omitted.

D Tool life value

Refer to II- 10.2.2 and II-10.2.4.

154

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-63534EN/02

Format

D Register with deleting

Format

Meaning of command

all groups

G10L3 ;

G10L3 :Register with deleting all groups

P_L_ ;

P_

:Group number

T_H_D_ ;

L_

:Life value

T_H_D_ ;

T_

:Tool number

H_

:Code specifying tool offset value

(H code)

D_

:Code specifying tool offset value

P_L_ ;

(D code)

T_H_D_ ;

G11

:End of registration

T_H_D_ ;

G11 ;

M02 (M30) ;

D Addition and change of

Format

Meaning of command

tool life management

data

G10L3P1 ;

G10L3P1 :Addition and change of group

P_L_ ;

P_

:Group number

T_H_D_ ;

L_

:Life value

T_H_D_ ;

T_

:Tool number

H_

:Code specifying tool offset value

(H code)

D_

:Code specifying tool offset value

P_L_ ;

(D code)

T_H_D_ ;

G11

:End of addition and change of

T_H_D_ ;

group

G11 ;

M02 (M30) ;

D Deletion of tool life

Format

Meaning of command

management data

G10L3P2 ;

G10L3P2 :Deletion of group

P_ ;

P_

:Group number

P_ ;

G11

:End of deletion of group

P_ ;

P_ ;

G11 ;

M02 (M30) ;

156

10. TOOL FUNCTION

B-63534EN/02

PROGRAMMING

(T FUNCTION)

D Setting a tool life cout

Format

Meaning of command

type for groups

G10L3

Q_ : Life count type (1:Frequency, 2:Time)

or

G10L3P1);

P_L_Q_ ;

T_H_D_ ;

T_H_D_ ;

P_L_Q_ ;

T_H_D_ ;

T_H_D_ ;

G11 ;

M02 (M30) ;

CAUTION

1

When the Q command is omitted, the value set in bit 7 (LTM)

of parameter No.6800 is used as the life count type.

2

G10L3P1 and G10L3P2 can be specified only when the

extended tool life management function is enabled.

(Parameter EXT (No.6801#6) = 1)

157

10. TOOL FUNCTION

(T FUNCTION)

PROGRAMMING

B-63534EN/02

10.2.3

Tool Life Management

Command in a

Machining Program

Explanations

D Command

The following command is used for tool life management:

Toooo; Specifies a tool group number.

The tool life management function selects, from a specified group, a

tool whose life has not expired, and outputs its T code. In oooo,

specify a number calculated by adding the tool life management cancel

number specified in parameter6810 to a group number. For example,

to set tool group 1 when the tool life management cancel number is

100, specify T101;.

NOTE

When oooo is less than a tool life management cancel

number, the T code is treated as an ordinary T code.

M06;

Terminates life management for the previously used tools,

and begins counting the life of the new tools selected with

the T code.

WARNING

When an option for speciofying multiple M codes is

selected, specify this code by itself or as the first M code.

H99;

Selects the H code of tool life management data for the tool

currently being used.

H00;

Cancels tool length offset

D99;

Selects the D code of tool life management data for the tool

currently being used.

D00;

Cancels cutter compensation

WARNING

H99 or D99 must be specified after the M06 command.

When a code other than H99 or D99 is specified after the

M06 command, the H code and D code of tool life

management data are not selected.

158

10. TOOL FUNCTION

B-63534EN/02

PROGRAMMING

(T FUNCTION)

D Types

For tool life management, the four tool change types indicated below are

available. The type used varies from one machine to another. For details,

refer to the appropriate manual of each machinde tool builder.

Table 10.2.3 Tool Change Type

Tool change

A

B

C

D

type

Tool group

Previously

Tools to be used next

number spe-

used tools

cified in the

same block

as the tool

change com-

mand (M06)

Tool life count

Life counting is performed for a tool in the

Life counting

timing

specified tool group when M06 is specified

is performed

next.

when a tool

in the tool

group speci-

fied in the

same block

as M06 is

specified.

Remarks

Normally, when a tool group

When only

number is specified by itself,

M06 is speci-

type B is used. However, no

fied, P/S

alarm is raised even if the

alarm No.

tool group number is speci-

153 is

fied by itself as type C.

issued.

Parameter

No. 6800#7

No. 6800#7 (M6T)=1

No.6801#7

(M6T)=0

No. 6801#7 (M6E)=0

(M6E)=1

No.6801#7

(M6E)=0

NOTE

When a tool group number is specified and a new tool is

selected, the new tool selection signal is output.

Examples

D Tool change type A

Suppose that the tool life management cancel number is 100.

T101; A tool whose life has not expired is selected from group 1.

(Suppose that tool number 010 is selected.)

M06; Tool life counting is performed for the tool in group 1.

(The life of tool number 010 is counted.)

T102; A tool whose life has not expired is selected from group 2.

(Suppose that tool number 100 is selected.)

M06T101; Tool life counting is performed for the tool in group 2.

(The life of tool number 100 is counted.)

The number of the tool currently used (in group 1) is

output with a T code signal. (Tool number 010 is

output.)

159

Content      ..     4      5      6      7     ..