FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

A coordinate system used for machining a workpiece is referred to as a

7.2

workpiece coordinate system. A workpiece coordinate system is to be set

WORKPIECE

with the NC beforehand (setting a workpiece coordinate system).

COORDINATE

A machining program sets a workpiece coordinate system (selecting a

SYSTEM

workpiece coordinate system).

A set workpiece coordinate system can be changed by shifting its origin

(changing a workpiece coordinate system).

7.2.1

A workpiece coordinate system can be set using one of three methods:

Setting a Workpiece

(1) Method using G50

A workpiece coordinate system is set by specifying a value after G50

Coordinate System

in the program.

(2) Automatic setting

If bit

0 of parameter No. 1201 is set beforehand, a workpiece

coordinate system is automatically set when manual reference

position return is performed (see III-3.1.).

This function is, however, disabled when the workpiece coordinate

system option is being used.

(3) Input using the MDI panel

Six workpiece coordinate systems can be set beforehand using the

MDI panel.

Program commands G54 to G59 can be used to select the work axis

to be used. (see III-11.4.10.)

When an absolute command is used, a workpiece coordinate system

must be established in any of the ways described above.

Format

D Setting a workpiece

G50 IP_

coordinate system by G50

Explanations

A workpiece coordinate system is set so that a point on the tool, such as

the tool tip, is at specified coordinates. If IP is an incremental command

value, the work coordinate system is defined so that the current tool

position coincides with the result of adding the specified incremental

value to the coordinates of the previous tool position. If a coordinate

system is set using G50 during offset, a coordinate system in which the

position before offset matches the position specified in G50 is set.

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.2.2

The user can choose from set workpiece coordinate systems as described

below.

(For information about the methods of setting, see Subsec.

Selecting a Workpiece

II-7.2.1.)

Coordinate System

(1) G50 or automatic workpiece coordinate system setting

Once a workpiece coordinate system is selected, absolute commands

work with the workpiece coordinate system.

(2) Choosing from six workpiece coordinate systems set using the

MDI

By specifying a G code from G54 to G59, one of the workpiece

coordinate systems 1 to 6 can be selected.

G54 Workpiece coordinate system 1

G55 Workpiece coordinate system 2

G56 Workpiece coordinate system 3

G57 Workpiece coordinate system 4

G58 Workpiece coordinate system 5

G59 Workpiece coordinate system 6

Workpiece coordinate system 1 to 6 are established after reference

position return after the power is turned on. When the power is turned

on, G54 coordinate system is selected.

When bit 2 (G50) of parameter No. 1202 is set to 1, executing the G50

command results in the issue of P/S alarm No. 10. This is designed

to prevent the user from confusing coordinate systems.

Examples

G55 G00 X100.0 Z40.0 ;

Workpiece coordinate system 2 (G55)

100.0

In this example, positioning is made to

positions (X=100.0, Z=40.0) in workpiece

coordinate system 2.

40.0

Fig. 7.2.2

101

7. COORDINATE SYSTEM

PROGRAMMING

B-63524EN/01

7.2.3

The six workpiece coordinate systems specified with G54 to G59 can be

changed by changing an external workpiece zero point offset value or

Changing Workpiece

workpiece zero point offset value.

Coordinate System

Three methods are available to change an external workpiece zero point

offset value or workpiece zero point offset value.

(1) Inputting from the MDI panel (see III-11.4.10)

(2) Programming by G10 or G50

(3) Using the external data input function

An external workpiece origin offset can be changed by using a signal

input to the CNC. For details, refer to the relevant manual supplied

by the machine tool builder.

Workpiece

coordinate

system 1 (G54)

system 2 (G55)

system 3 (G56)

system 4 (G57)

ZOFS2

ZOFS3

ZOFS1

ZOFS4

Workpiece

coordinate

ZOFS5

system 5 (G58)

EXOFS

ZOFS6

Workpiece

Machine zero

coordinate

system 6 (G59)

EXOFS : External workpiece zero point offset value

ZOFS1 to ZOFS6 : Workpiece zero point offset value

Fig. 7.2.3 Changing an external workpiece zero point offset value or workpiece zero point offset value

Format

G10 L2 Pp IP _;

D Changing by G10

p=0 : External workpiece zero point offset value

p=1 to 6 : Workpiece zero point offset value correspond to

workpiece coordinate system 1 to 6

IP : For an absolute command (G90), workpiece zero point off-

set for each axis.

For an incremental command (G91), value to be added to

the set workpiece zero point offset for each axis (the sum

is set as the new offset).

D Changing by G50

G50 IP _;

102

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

Explanations

D Changing by G10

With the G10 command, each workpiece coordinate system can be

changed separately.

D Changing by G50

By specifying G50IP_;, a workpiece coordinate system (selected with a

code from G54 to G59) is shifted to set a new workpiece coordinate

system so that the current tool position matches the specified coordinates

(IP_).

If IP is an incremental command value, the work coordinate system is

defined so that the current tool position coincides with the result of adding

the specified incremental value to the coordinates of the previous tool

position.

(Coordinate system shift)

Then, the amount of coordinate system shift is added to all the workpiece

zero point offset values. This means that all the workpiece coordinate

systems are shifted by the same amount.

Examples

XȀ

G54 workpiece coordinate system

If G50X100Z100; is commanded when the tool

is positioned at (200, 160) in G54 mode, work-

160

100

Tool position

piece coordinate system 1 (X′ - Z′) shifted by

vector A is created.

Z′

New workpiece coordinate system

100

Original workpiece coordinate system

100

200

Suppose that a G54 workpiece coordi-

nate system is specified. Then, a G55

X′

workpiece coordinate system where

the black circle on the tool (figure at

the left) is at (600.0,12000.0) can be

set with the following command if the

X′

600.0

relative relationship between the G54

workpiece coordinate system and

ÎÎ

G55 workpiece coordinate system is

Z′

set correctly:G50X600.0Z1200.0;Also,

600.0

1200.0

suppose that pallets are loaded at two

ÎA

ÎÎ

different positions. If the relative rela-

ÎÎ

tionship of the coordinate systems of

Z′

the pallets at the two positions is cor-

1200.0

rectly set by handling the coordinate

A Î

systems as the G54 workpiece coordi-

nate system and G55 workpiece coor-

dinate system, a coordinate system

shift with G50 in one pallet causes the

same coordinate system shift in the

X′ - Z′ New workpiece coordinate system

other pallet. This means that work-

pieces on two pallets can be ma-

X - Z Original workpiece coordinate system

chined with the same program just by

A : Offset value created by G50

B : Workpiece zero point offset value in G54

specifying G54 or G55.

C : Workpiece zero point offset value in G55

103

7. COORDINATE SYSTEM

PROGRAMMING

B-63524EN/01

7.2.4

The workpiece coordinate system preset function presets a workpiece

coordinate system shifted by manual intervention to the pre-shift

Workpiece Coordinate

workpiece coordinate system. The latter system is displaced from the

System Preset (G92.1)

machine zero point by a workpiece zero point offset value.

There are two methods for using the workpiece coordinate system preset

function. One method uses a programmed command (G92.1). The other

uses MDI operations on the absolute position display screen, relative

position display screen, and overall position display screen (III - 11.1.4).

Format

G92.1 IP 0 ;

(G50.3 P0 ; for G code system A)

IP 0 ; Specifies axis addresses subject to the workpiece

coordinate system preset operation. Axes that are

not specified are not subject to the preset operation.

Explanations

When manual reference position return operation is performed in the reset

state, a workpiece coordinate system is shifted by the workpiece zero

point offset value from the machine coordinate system zero point.

Suppose that the manual reference position return operation is performed

when a workpiece coordinate system is selected with G54. In this case,

a workpiece coordinate system is automatically set which has its zero

point displaced from the machine zero point by the G54 workpiece zero

point offset value; the distance from the zero point of the workpiece

coordinate system to the reference position represents the current position

in the workpiece coordinate system.

G54 workpiece coordinate system

G54 workpiece zero

point offset value

Reference position

Manual reference position return

If an absolute position detector is provided, the workpiece coordinate

system automatically set at power-up has its zero point displaced from

the machine zero point by the G54 workpiece zero point offset value. The

machine position at the time of power-up is read from the absolute

position detector and the current position in the workpiece coordinate

system is set by subtracting the G54 workpiece zero point offset value

from this machine position. The workpiece coordinate system set by

these operations is shifted from the machine coordinate system using the

commands and operations listed next page.

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

(b) Move command executed in the machine lock state

(d) Operation using the mirror image function

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

workpiece coordinate system using G92

104

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

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

intervention

Amount of movement

during manual

Workpiece zero

WZo

intervention

point offset

value

G54 workpiece coordinate

Machine zero point

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.

Restrictions

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.

105

7. COORDINATE SYSTEM

PROGRAMMING

B-63524EN/01

7.2.5

When the coordinate system actually set by the G50 command or the

automatic system setting deviates from the programmed work system, the

Workpiece Coordinate

set coordinate system can be shifted (see III-3.1).

System Shift

Set the desired shift amount in the work coordinate system shift memory.

Explanations

X-Z: Coordinate system in programming

x-z : Current set coordinate system with shift amount 0

(coordinate system to be modified by shifting)

ÎÎÎ

ÎÎ

O′

Shift

Set the shift amount from O′ to O in the work coordinate system shift memory.

Fig. 7.2.5 Workpiece Coordinate System shift

See Section III-11.4.5 of Part III for how to specify the distance the work

coordinate system is shifted.

106

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

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

7.3

workpiece coordinate system may be set for easier programming. Such

LOCAL COORDINATE

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

SYSTEM

Format

G52 IP _; Setting the local coordinate system

G52 IP 0 ; Canceling of the local coordinate system

IP _ : Origin of the local coordinate system

Explanations

By specifying G52IP_;, 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.

Once a local coordinate system is established, the coordinates in the local

coordinate system are used in an axis shift command. 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.

IP_

(Local coordinate system)

(G54 : Workpiece coordinate

system 1)

G55

IP_

(Local coordinate system)

G56

G57

G58

(G59 : Workpiece coordinate system 6)

(Machine coordinate system)

Machine coordinate system origin

Reference point

Fig. 7.3 Setting the local coordinate system

107

7. COORDINATE SYSTEM

PROGRAMMING

B-63524EN/01

WARNING

The local coordinate system setting does not change the

workpiece and machine coordinate systems.

When G50 is used to define a work coordinate system, if

coordinates are not specified for all axes of a local

coordinate system, the local coordinate system remains

unchanged.

If coordinates are specified for any axis of a local coordinate

system, the local coordinate system is canceled.

G52 cancels the offset temporarily in tool nose radius

compensation.

Command a move command immediately after the G52

block in the absolute mode.

Whether the local coordinate system is canceled upon reset

depends on the specified parameters. The local coordinate

system is canceled upon reset when bit

6 (CLR) of

parameter No. 3402 or bit 3 (RLC) of parameter No. 1202

is set to 1.

108

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

Select the planes for circular interpolation, tool nose radius

7.4

compensation, coordinate system rotation, and 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

plane

G17

Xp Yp plane

X-axis or an

Y-axis or an

Z-axis or an

G18

Zp Xp plane

axis parallel

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 specifies whether each axis is a basic axis (X-axis,

Y-axis, or Z-axis) or an axis parallel to a basic axis.

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

commanded.

When the power is turned on, G18 (ZX plane) is selected .

The movement instruction is irrelevant to the plane selection.

NOTE

U-, V-, and W-axes (parallel to a basic axis) can be used

with G-codes B and C.

Direct drawing dimension programming, chamfering, corner

R, multiple repetitive canned cycle, and simple canned

cycle are enabled only for the ZX plane.

Specifying these functions for other planes causes P/S

alarm No. 212 to be generated.

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.

109

8. COORDINATE VALUE

B-63524EN/01

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

PROGRAMMING

G91 are used to command absolute or incremental command,

respectively.

(G90, G91)

Absolute programming or incremental programming is used depending

on the command used. See following tables.

G code system

B or C

Command method

Address word

G90, G91

Format

D G code system A

Absolute command

Incremental command

X axis move command

Z axis move command

Y axis move command

C axis move command

D G code system B or C

Absolute command

G90 IP_ ;

Incremental command G91 IP_ ;

Examples

D Tool movement from point

G code system A

G code system B or C

P to point Q (diameter

Absolute command

X400.0 Z50.0 ;

G90 X400.0 Z50.0 ;

programming is used for

the X-axis)

Incremental command

U200.0 W-400.0 ;

G91 X200.0 Z-400.0 ;

(400, 50)

(200, 450)

φ400

φ200

450

NOTE

Absolute and incremental commands can be used together

in a block.

In the above example, the following command can be

specified :

X400.0 W-400.0 ;

When both X and U or W and Z are used together in a block,

the one specified later is effective.

Incremental commands cannot be used when names of the

axes are A and B during G code system A is selected.

111

8. COORDINATE VALUE

AND DIMENSION

PROGRAMMING

B-63524EN/01

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

8.2

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

(Section 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

G20 and G21 must not be switched during a program.

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

Movement from the intermediate point is the same as that

for manual reference position return. The direction in which

the tool moves from the intermediate point is the same as

the reference position return direction, as specified with bit

5 (ZMI) of parameter No. 1006.

NOTE

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.

The inch and metric input can also be switched using setting

of data setting (III-11.4.7).

112

8. COORDINATE VALUE

B-63524EN/01

PROGRAMMING

AND DIMENSION

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

8.3

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, 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. 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 with-

Unit : mm

Unit : Least input increment

out decimal point

(0.001 mm)

X1000.0

1000mm

Command value with

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

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.

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 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 P/S alarm 003

occurs.

113

8. COORDINATE VALUE

AND DIMENSION

PROGRAMMING

B-63524EN/01

Since the work cross section is usually circular in CNC lathe control

8.4

programming, its dimensions can be specified in two ways :

DIAMETER AND

Diameter and Radius

RADIUS

When the diameter is specified, it is called diameter programming and

PROGRAMMING

when the radius is specified, it is called radius programming.

R₂

R₁

D₁

D₂

X axis

D₁, D₂ : Diameter programming

R₁, R₂

: Radius programming

Z axis

Explanations

D Notes on diameter

Radius programming or diameter programming can be specified by

programming/radius

parameter DIA (No.1006#3). When using diameter programming, note

programming for each

the conditions listed in the table 8.4.

command

Table 8.4 Notes on specifying diameter value

Item

Notes

X axis command

Specified with a diameter value

Incremental command

Specified with a diameter value

In the above figure, specifies D2 minus

D1 for tool path B to A.

Coordinate system setting (G50)

Specifies a coordinate value with a diam-

eter value

Component of tool offset value

Parameter (No.5004#1) determines either

diameter or radius value

Parameters in canned cycle,

Specifies a radius value

such as cutting depth along X

axis. (R)

Radius designation in circular in-

Specifies a radius value

terpolation (R, I, K, and etc.)

Feedrate along axis

Specifies change of radius/rev. or change

of radius/min.

Display of axis position

Displayed as diameter value

114

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED FUNCTION

SPINDLE SPEED FUNCTION

The spindle speed can be controlled by specifying a value following

address S.

In addition, the spindle can be rotated by a specified angle.

This chapter contains the following topics.

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY

(S5-DIGIT COMMAND)

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97)

9.4 SPINDLE SPEED FLUCTUATION DETECTION FUNCTION

(G25, G26)

9.5 SPINDLE POSITIONING FUNCTION

115

9. SPINDLE SPEED FUNCTION

PROGRAMMING

B-63524EN/01

Specifying a value following address S sends code and strobe signals to

9.1

the machine. On the machine, the signals are used to control the spindle

SPECIFYING THE

speed. A block can contain only one S code. Refer to the appropriate

SPINDLE SPEED

manual provided by the machine tool builder for details such as the

WITH A CODE

number of digits in an S code or the execution order when a move

command and an S code command are in the same block.

The spindle speed can be specified directly by address S followed by a

9.2

five-digit value (min^-1). The unit for specifying the spindle speed may

SPECIFYING THE

vary depending on the machine tool builder. Refer to the appropriate

SPINDLE SPEED

manual provided by the machine tool builder for details.

VALUE DIRECTLY

(S5-DIGIT

COMMAND)

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 Clamp of maximum

spindle speed

G50 S_ ;

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

116

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED FUNCTION

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 G50S_; (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.

The spindle speed (min^-1) almost

(min^-1)

coincides with the surface speed

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

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 , Z axis, (axis to which the constant surface speed

constant surface speed

control applies) becomes zero.

control

Fig. 9.3 (b) Example of the Workpiece Coordinate

System for Constant Surface Speed Control

117

9. SPINDLE SPEED FUNCTION

PROGRAMMING

B-63524EN/01

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

(min^-1) is used

Not specified

The surface speed (m/min or

feet/min) is converted to the

spindle speed (min^-1)

Commands other than G96

G96 command

Specified

The specified

Command

surface

for the surface

speed is used

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.

118

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED FUNCTION

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.

Radius value

Programmed path

Tool path after offset

700

675

600

N11

N16

N15

500

N11

N14

400

N16

N15

375

N14

300

200

100

φ600

300

400

500

600

700

800

900

1000

1100 1200

1300 1400

1500

1475

1050

Example

N8 G00 X1000.0Z1400.0 ;

N9 T33;

N11 X400.0Z1050.0;

N12 G50S3000 ; (Designation of max. spindle speed)

N13 G96S200 ; (Surface speed 200 m/min)

N14 G01 Z 700.0F1000 ;

N15 X600.0Z 400.0;

N16 Z … ;

The CNC calculates the spindle speed which is proportional to the

specified surface speed at the position of the programmed coordinate

value on the X axis. This is not the value calculated according to the X

axis coordinate after offset when offset is valid. At the end point N15 in

the example above, the speed at 600 dia. (Which is not the turret center

but the tool nose) is 200 m/min. If X axis coordinate value is negative,

the CNC uses the absolute value.

119

9. SPINDLE SPEED FUNCTION

PROGRAMMING

B-63524EN/01

With this function, an overheat alarm (No. 704) is raised when the spindle

9.4

speed deviates from the specified speed due to machine conditions.

SPINDLE SPEED

This function is useful, for example, for preventing the seizure of the

FLUCTUATION

guide bushing.

DETECTION

FUNCTION

(G25, G26)

Format

G26 enables spindle speed fluctuation detection.

G25 disables spindle speed fluctuation detection.

G26 Pp Qq Rr ;

Spindle fluctuation detection on

G25 ;

Spindle fluctuation detection off

p : Time (in ms) from the issue of a new spindle rotation command (S

command) to the start of checking whether the actual spindle speed is

so fast that an overheat can occur.

When a specified speed is reached within the time period of P, spindle

speed is checked at that time.

q : Tolerance (%) of a specified spindle speed

1-actual spindle speed

100

specified spindle speed

If a specified spindle speed lies within this range, it is regarded as

having reached the specified value. Then, an actual spindle speed is

checked.

r : Spindle speed fluctuation (%) at which the actual spindle speed is so

fast that an overheat can occur

1-speed that can cause overheat

100

specified spindle speed

G26 enables the spindle speed fluctuation detection function, and G25

disables the spindle speed fluctuation detection.

Even if G25 is specified, p, q, and r are not cleared.

120

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED 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

Specified

speed

Actual speed

Check

check

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

Specified

speed

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 4913)

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

the actual speed exceeds both r and d.

121

9. SPINDLE SPEED FUNCTION

PROGRAMMING

B-63524EN/01

NOTE

When an alarm is issued in automatic operation, a single

block stop occurs. The spindle overheat alarm is indicated

on the CRT screen, and the alarm signal “SPAL” is output

(set to 1 for the presence of an alarm). This signal is cleared

by resetting.

Even when reset operation is performed after an alarm

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

alarm is corrected.

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

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 min^-1.

122

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED FUNCTION

In turning, the spindle connected to the spindle motor is rotated at a certain

9.5

speed to rotate the workpiece mounted on the spindle. The spindle

SPINDLE

positioning function turns the spindle connected to the spindle motor by

POSITIONING

a certain angle to position the workpiece mounted on the spindle at a

FUNCTION

certain angle. The spindle is positioned about the C-axis.

The spindle positioning function involves the following three operations:

1. Canceling the spindle rotation mode and entering the spindle

positioning mode (spindle orientation)

2. Positioning the spindle in the spindle positioning mode

3. Canceling the spindle positioning mode, and entering the spindle

rotation mode

9.5.1

When spindle positioning is first performed after the spindle motor is used

for normal spindle operation, or when spindle positioning is interrupted,

Spindle Orientation

the spindle orientation is required.

Orientation permits the spindle to stop at a predetermined position.

Orientation is directed by the M code set in parameter No. 4960. The

direction of orientation can be set with a parameter. For the analog

spindle, the direction is set in ZMIx (bit 5 of parameter 1006).

For the serial spindle, it is set in RETRN (bit 5 of parameter 4005).

9.5.2

The spindle can be positioned with an arbitrary angle or semi-fixed angle.

Spindle Positioning

D Positioning with a

Address M is followed by a 2-digit numeric. The specifiable value may

semi-fixed angle

be one of the six values from Mα to M (α+5). Value α must be set in

specified by an M code

parameter No. 4962 beforehand. The positioning angles corresponding

to Mα to M (α+5) are listed below. Value β must be set in parameter No.

4963 beforehand.

M-code

Positioning angle

(Ex.)β=30°

Mα

30°

M(α+1)

2β

60°

M(α+2)

3β

90°

M(α+3)

4β

120°

M(α+4)

5β

150°

M(α+5)

6β

180°

Specify the command with incremental values. The direction of rotation

can be specified in parameter IDM (bit 1 of parameter 4950).

123

9. SPINDLE SPEED FUNCTION

PROGRAMMING

B-63524EN/01

D Positioning with a given

Specify the position using address C or H followed by a signed numeric

angle specified by

value or numeric values. Addresses C and H must be specified in the G00

address C or H

mode.

(Example) C-1000

H4500

The end point must be specified with a distance from the program

reference position (in absolute mode) using address C. Alternatively, the

end point must also be specified with a distance from the start point to the

end point (in incremental mode) using address H.

A numeric with the decimal point can be entered.

The value must be specified in degrees.

(Example) C35.0=C35 degrees

D Program reference

The position to which the spindle is oriented is assumed as the program

position

reference position. The program reference position can be changed by

setting of a coordinate system (G50) or automatic setting of a coordinate

system (#OZPR of parameter 1202).

D Feedrate for positioning

Program reference

position

90°

180°

G code A

G code B and C

Command

Addres

Command

Command format

Addres

A-B in the

s used

A-B in the

s used

above

and G

above

figure

code

figure

Specify the

end point

with a dis-

Absolute

tance from

C180.0 ;

G90,C

G90C180.;

command

the program

reference

position.

Specify a dis-

tance from

Incremental

the start

H90.0 ;

G91,C

G90C90. ;

command

point to the

end point.

124

B-63524EN/01

PROGRAMMING

9. SPINDLE SPEED FUNCTION

D Feedrate during

The feedrate during positioning equals the rapid traverse speed specified

positioning

in parameter No. 1420. Linear acceleration/deceleration is performed.

For the specified speed, an override of 100%, 50%, 25%, and F0

(parameter No. 1421) can be applied.

D Speed during orientation

The tool moves at the rapid traverse speed set in parameter No.1420 until

a sufficient speed for orientation is attained. After the speed for

orientation has been attained, orientation is performed at the speed set in

parameter No. 1425.

9.5.3

When modes are to be switched from spindle positioning to normal

spindle rotation, the M code set in parameter No. 4961 is specified.

Canceling Spindle

Positioning

WARNING

Feed hold, dry run, machine lock, and auxiliary function lock

cannot be performed during spindle positioning.

Parameter No.

4962 must always be set even when

positioning with a semi-fixed angle specified in an M-code

is not performed. If the parameter is not set, M-codes from

the M00 to M05 do not function properly.

NOTE

Specify spindle positioning alone in a block. A move

command for the X or Z axis cannot be specified within the

same block.

When emergency stop is applied during spindle positioning,

spindle positioning stops. To resume it, restart with the

orientation step.

The serial spindle Cs-axis contour control function and the

spindle positioning function cannot be used at a time. If both

options are specified, the spindle positioning function has

priority.

The spindle positioning axis is indicated in pulses in the

machine coordinate system.

125

B-63524EN/01

PROGRAMMING

10. TOOL FUNCTION (T FUNCTION)

By specifying a 2-digit/4-digit numerical value following address T, a

10.1

code signal and a strobe signal are transmitted to the machine tool. This

TOOL SELECTION

is mainly used to select tools on the machine.

One T code can be commanded in a block. Refer to the machine tool

builder’s manual for the number of digits commandable with address T

and the correspondence between the T codes and machine operations.

When a move command and a T code are specified in the same block, the

commands are executed in one of the following two ways:

1. Simultaneous execution of the move command and T function

commands.

2. Executing T function commands upon completion of move command

execution.

The selection of either sequence depends on the machine tool builder’s

specifications. Refer to the machine tool builder’s manual for details.

1. Last one digit of T-code designates the offset number.

T ff

Tool offset number

Tool selection

2. Last two digits of T-code designate the offset number.

T ff

Tool offset number

Tool selection

Explanations

The value after the T code indicates the desired tool. Part of the values

is also used as the offset number indicating the compensation amount for

tool offset.

Refer to the machine tool builder’s manual for correspondence between

the T-code and the tool and the number of digit to specify tool selection.

Example (T2+2)

N1G00X1000Z1400

N2T0313; (Select Tool No. 3 and Offset value No. 13)

N3X400Z1050;

Some machines use a 1-digit value to specify tool selection.

127

10. TOOL FUNCTION (T FUNCTION)

PROGRAMMING

B-63524EN/01

Tools are classified into some groups. For each group, a tool life (time

10.2

or frequency of use) is specified. Each time a tool is used, the time for

TOOL LIFE

which the tool is used is accumulated. When the tool life has been

MANAGEMENT

reached, the next tool previously determined in the same group is used.

This function is called the tool life management function.

With 2-path control, tool life management is performed for each tool post

separately. So tool life management data is also set for each tool post.

10.2.1

Program of Tool Life

Data

Format

Tools used sequentially in each group and their tool life are registered in

the CNC as following program format of table 10.2.1 (a).

Table 10.2.1 (a) Program format of life management

Tape format

Meaning

O_ _ _ _

;

Program number

G10L3;

Start of setting tool life data

P_ _ _ L_ _ _ _

;

P___ :Group number (1 to 128)

L___ :Tool life (1 to 9999)

T_ _ _ _

;

(1)

T:____ Tool number

T_ _ _ _

;

(2)

Tools are selected from

(n)

(1)to (2) to ... to (n).

P_ _ _ L_ _ _ _ ;

T_ _ _ _

;

Data for the next group

T_ _ _ _

;

G11;

End of setting tool life data

M02(M30);

End of program

For the method of registering tool life data in CNC, refer to Subsec.

III-11.4.14.

128

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 5