Content      ..     3      4      5      6     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. OPERATOR'S MANUAL - page 5

8.COORDINATE VALUE AND DIMENSION PROGRAMMING

B-64304EN/02

NOTE

1

A specified value less than the least increment is treated as shown below

(rounded off to the right side).

Example 1)

When a value is specified directly at an address (in the case of IS-B)

X-0.0004 ;

Treated as X0.000

X0.0004 ;

Treated as X0.000

X-0.0005 ;

Treated as X0.000

X0.0005 ;

Treated as X0.001

X-0.0006 ;

Treated as X-0.001

X0.0006 ;

Treated as X0.001

As shown in the table below, commands including positive and negative

fractions having the same absolute value with respect to zero are repeated.

In right side rounding, the results are periodical. In general rounding,

however, the results are not periodical due to rounding symmetry with respect

to zero.

To prevent this, right side rounding is used for calculation.

Right side rounding

General rounding

G90 G00 X0 ;

X 0.000

X 0.000

G91 X-0.0015 ;

X -0.001

X -0.002

G91 X0.0015 ;

X 0.000

X -0.001

G91 X-0.0015 ;

X -0.001

X -0.003

G91 X0.0015 ;

X 0.000

X -0.002

G91 X-0.0015 ;

X -0.001

X -0.004

G91 X0.0015 ;

X 0.000

X -0.003

Example 2)

When a value is assigned to a macro variable (in the case of IS-B)

Similarly, right side rounding is performed.

#100=1.2345 ;

X#100 ;

Treated as X1.235

#100=-1.2345 ;

X#100 ;

Treated as X-1.234

2

When more than nine 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:

X0.123456789 ;

Alarm PS0003 occurs because more than nine digits are specified.

X1234567.8 ;

If the least input increment is 0.001 mm, the value is converted to integer

1234567800. Because the integer has more than nine digits, an alarm

occurs.

- 96 -

B-64304EN/02

PROGRAMMING

8.COORDINATE VALUE AND DIMENSION

8.4

DIAMETER AND RADIUS PROGRAMMING

Since the workpiece cross section is usually circular in CNC lathe control programming, its dimensions

can be specified in two ways :

Diameter and Radius

A

B

R₂

R₁

D₁

D₂

X axis

D1, D2 : Diameter programming

R1, R2 : Radius programming

Z axis

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

called radius programming.

Explanation

-

Notes on diameter programming/radius programming for each command

Radius programming or diameter programming can be specified by bit 3 (DIA) of parameter No.1006.

When using diameter programming, note the conditions listed in the Table 8.4 (a).

Table 8.4 (a) Notes on specifying diameter value

Item

Notes

X axis command

Specified with a diameter value

Specified with a diameter value

Incremental command

In the above figure, specifies D2 minus D1 for tool path B to A.

Coordinate system setting

Specifies a coordinate value with a diameter value

Bit 1 of parameter No.5004 determines either diameter or

Component of tool offset value

radius value

Parameters in canned cycle (T series), such as

Specifies a radius value

cutting depth along X axis. (R)

Radius designation in circular interpolation (R,

Specifies a radius value

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

- 97 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

9 SPINDLE SPEED FUNCTION

(S FUNCTION)

The spindle speed can be controlled by specifying a value following address S.

Chapter 9, "SPINDLE SPEED FUNCTION (S FUNCTION)", consists of the following sections:

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE

98

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5-DIGIT COMMAND)

98

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97)

98

9.4 SPINDLE POSITIONING FUNCTION

102

9.5 SPINDLE SPEED FLUCTUATION DETECTION

107

9.6 SPINDLE CONTROL WITH SERVO MOTOR

110

9.1

SPECIFYING THE SPINDLE SPEED WITH A CODE

When a value is specified after address S, the code signal and strobe signal are sent to the machine to

control the spindle rotation speed.

A block can contain only one S code. Refer to the appropriate manual provided by the machine tool

builder for details such as the 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.

9.2

SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY

(S5-DIGIT COMMAND)

The spindle speed can be specified directly by address S followed by a max. five-digit value (min^-1). The

unit for specifying the spindle speed may vary depending on the machine tool builder. Refer to the

appropriate manual provided by the machine tool builder for details.

9.3

CONSTANT SURFACE SPEED CONTROL (G96, G97)

Specify the surface speed (relative speed between the tool and workpiece) following S. The spindle is

rotated so that the surface speed is constant regardless of the position of the tool.

Format

-

Constant surface speed control command

G96 Sxxxxx ;

↑ Surface speed (m/min or feet/min)

This surface speed unit may change according to machine tool builder's specification.

-

Constant surface speed control cancel command

G97 Sxxxxx ;

↑ Spindle speed (min^-1)

This surface speed unit may change according to machine tool builder's specification.

- 98 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

-

Constant surface speed controlled axis command

G96 Pα ;

P0 : Axis set in the parameter (No. 3770)

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

P5 : 5th axis

T

NOTE

If multi-spindle control (spindle selecting based on address P) is enabled, axis

specification based on address P is disabled. Use parameter No. 3770 for axis

specification.

-

Clamp of maximum spindle speed

G92 S_ ;

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

T

G50 S_ ;

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

NOTE

G50 can be used with G code system A.

Explanation

-

Constant surface speed control command (G96)

G96 (constant surface speed control command) is a modal G code. After 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 G92 S_ ; or G50 S_ ; (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.

- 99 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

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.

Relation between workpiece radius,

Radius (mm)

spindle speed and surface speed

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

-

Setting the workpiece coordinate system for constant surface speed control

To execute the constant surface speed control, it is necessary to set the workpiece coordinate system , and

so the coordinate value at the center of the rotary axis, for example, Z axis, (axis to which the constant

surface speed control applies) becomes zero.

X

Z

0

Fig. 9.3 (b) Example of the workpiece coordinate system for constant surface speed control

- 100 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

-

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

is stored, 0 is assumed.

Limitation

-

Constant surface speed control for threading

The constant surface speed control is also effective during 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.

-

Constant surface speed control for rapid traverse (G00)

In a rapid traverse block specified by G00, the constant surface speed control is not made by calculating

the surface speed to a transient change 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.

- 101 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

Example

T

Radius value

Programmed path

X

Tool path after offset

1

2

700

4

675

600

N11

N16

3

500

N15

N11

N14

400

N16

N15

375

300

N14

200

φ600

φ400

100

Z

300 400 500 600

700 800 900

1000

1100

1300 14001500

1200

1475

1050

N8 G00 X1000.0 Z1400.0 ;

N9 T33;

N11 X400.0 Z1050.0 ;

N12 G50 S3000 ; (Designation of max. spindle speed)

N13 G96 S200 ; (Surface speed 200 m/min)

N14 G01 Z700.0 F1000 ;

N15 X600.0 Z 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.

9.4

SPINDLE POSITIONING FUNCTION

Overview

T

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

mounted on the spindle. This spindle control status is referred to as spindle rotation mode.

The spindle positioning function turns the spindle connected to the spindle motor by a certain angle to

position the workpiece mounted on the spindle at a certain angle. This spindle control status is referred

to as spindle positioning mode.

The spindle positioning function involves the following three operations:

1.

Canceling the spindle rotation mode and entering the spindle positioning mode

- 102 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Place the spindle in the spindle positioning mode and establish a reference position by specifying a

given M code (set with a parameter).

(Spindle orientation)

2.

Positioning the spindle in the spindle positioning mode

The spindle is positioned in either of the two methods:

1)

Positioning with an arbitrary angle by an axis address

2)

Positioning with a semi-fixed angle by a given M code (set with a parameter)

3.

Canceling the spindle positioning mode, and entering the spindle rotation mode

Place the spindle in the spindle rotation mode by specifying a given M code (set with a parameter).

The least command increment, least input increment, and maximum value for the spindle positioning axis

are as follows:

• Least command increment

360

4096 ••0.088 deg (when the gear ratio of the spindle to the position coder

• Least input increment

0.001 deg (IS-B)

• Maximum value

±999999.999 deg

NOTE

1 Be sure to set 1 in bit 1 (AXC) of parameter No.8133 and 0 in bit 2 (SCS) of

parameter No.8133 to use the spindle positioning function.

2 Both serial spindle Cs contour control function and spindle positioning function

cannot be made effective at the same time.

If both are specified as AXC=1 and SCS=1, both functions become invalid.

Therefore, when a negative value is set in parameter No.1023 with above

specification, alarm (SV1026) is generated.

3 Be sure to set 0 in bit 1 (AXC) of parameter No.8133 and 1 in bit 2 (SCS) of

parameter No.8133 to use the serial spindle Cs contour control function.

9.4.1

Spindle Orientation

When spindle positioning is first performed after the spindle motor is used for normal spindle operation,

or when spindle positioning is interrupted, 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 serial spindle, it is set in bit 4 (RETSV) of parameter No. 4000. With the grid shift function, the

orientation position can be shifted in a range of 0 to 360 deg with parameter No. 4073 for a serial spindle.

-

Feedrate during spindle orientation

An orientation feedrate for a serial spindle is determined by a spindle parameter setting.

In orientation, the serial spindle stops at the orientation position after several rotations of the spindle

motor.

-

Omission of orientation

By using bit 2 (ISZ) of parameter No. 4950, orientation upon switching to spindle positioning mode can

be omitted if it is unnecessary

(for example, when no start position is specified and incremental

positioning from the current position is only required). More specifically, when an M code for

switching to spindle positioning mode is specified, the spindle control mode is simply switched to spindle

positioning mode and then the processing is completed without orientation.

- 103 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

-

Program reference position

The position at which orientation is completed is assumed to be a program reference position. However,

the program reference position can be changed through coordinate system setting (G92 or G50) or

automatic coordinate system setting (bit 0 (ZPR) of parameter No. 1201).

When a setting is made to omit orientation, a program reference position is not established, and operation

by an absolute command is unpredictable during spindle positioning with an axis address.

9.4.2

Spindle Positioning (T Series)

T

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

-

Positioning with a semi-fixed angle

Use an M code to specify a positioning angle. The specifiable M code value may be one of the six

values from Mα to M (α+5). Value α must be set in 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°

(Ex.) β = α + 5

Mα

β

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°

When the number of M codes to be used, value γ, is specified in parameter No. 4964, a specifiable M

code value may be in a range of values from Mα to M (α + (γ - 1)), up to 255 values from Mα to M (α +

(255 - 1)).

M code

Positioning angle

(Ex.) β = 30°

(Ex.) γ = 11

Mα

β

30°

M (α + 1)

2β

60°

M (α + 2)

3β

90°

M (α + 3)

4β

120°

M (α + 11 - 1)

11β

330°

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

-

Positioning with an arbitrary angle

Specify the position with an arbitrary angle using the axis address followed by a signed numeric value or

numeric values. The axis address must be specified in the G00 mode.

(The explanation below is given assuming that a C axis address is set.)

(Example)

C-45000

C180.000

A numeric with the decimal point can be entered. The value must be specified in degrees.

(Example)

C36.0=C36 degrees

-

Absolute commands and incremental commands

Incremental commands are always used for positioning with a semi-fixed angle (using M codes).

- 104 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

The direction of rotation can be specified with bit 1 (IDM) of parameter No. 4950.

Absolute and incremental commands can be used for positioning with an arbitrary angle.

With absolute commands for positioning with an arbitrary angle, when the rotation axis rollover function

is used (bit 0 (ROA) of parameter No. 1008 is 1), shortcut control is also enabled (bit 1 (RAB) of

parameter No. 1008 is 0).

Program reference position

90°

A

180°

B

G-code system A

G-code system B or C

Command format

Address

Command A-B in

Address used and G

Command A-B in

used

the above figure

code

the above figure

Specify the end point with a

Absolute command

distance from the program

C

C180. ;

G90,C

G90 C180. ;

reference position.

Specify a distance from

Incremental

the start point to the end

H

H90. ;

G91,C

G91 C90. ;

command

point.

-

Feedrate during positioning

The feedrate during positioning equals the rapid traverse speed specified in parameter No. 1420.

For the specified speed, an override of 100%, 50%, 25%, and F0 (parameter No. 1421) can be applied.

9.4.3

Canceling Spindle Positioning (T Series)

T

When modes are to be switched from spindle positioning to normal spindle rotation, the M code set in

parameter No. 4961 must be specified.

Also, the spindle positioning mode is canceled and the spindle rotation mode is set in the following cases:

<1> A reset operation (including an emergency stop) occurs when a servo alarm is issued.

<2> A reset operation (including an emergency stop) occurs when a spindle alarm is issued.

<3> An orientation operation in progress is stopped due to a reset or alarm, or for some other reason.

<4> A reset operation (including an emergency stop) occurs when bit (IOR) 0 of parameter No. 4950 is

1.

CAUTION

1 During execution of spindle positioning sequences (canceling the spindle rotation

mode and entering the spindle positioning mode, positioning the spindle in the

spindle positioning mode, and canceling the spindle positioning mode and

entering the spindle rotation mode), the automatic operation stop signal *SP is

invalid. This means that automatic operation does not stop until all the

sequences are completed, even when the *SP signal becomes 0.

- 105 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

9.5

SPINDLE SPEED FLUCTUATION DETECTION (T SERIES)

T

Overview

With this function, an overheat alarm (OH0704) is raised and the spindle speed fluctuation detection

alarm signal SPAL is issued when the spindle speed deviates from the specified speed due to machine

conditions.

This function is useful, for example, for preventing the seizure of the guide bushing.

G26 enables spindle speed fluctuation detection.

G25 disables spindle speed fluctuation detection.

Format

-

Spindle fluctuation detection on

G26 Pp Qq Rr Ii；

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, a check is started at that

time.

Q: Tolerance (%) of a specified spindle speed

actual spindle speed

q

=1−

×

100

specified spndle speed

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

specified value. Then, the checking of an actual spindle speed is started.

R: Spindle speed fluctuation (%) at which the actual spindle speed is so fast that an

overheat can occur

speed that can cause overheat

r

=1−

×

100

speciofied spndle speed

If the fluctuation of the actual spindle speed to the specified spindle speed exceeds the

spindle speed fluctuation of R, the actual spindle speed is regarded as being so fast that

an overheat can occur.

I: Spindle speed fluctuation width at which the actual spindle speed (min^-1) is so fast that

an overheat can occur

If the fluctuation (width) between the specified and actual spindle speeds exceeds the

spindle speed fluctuation width of I, the actual spindle speed is regarded as being so fast

that an overheat can occur.

G26 enables the spindle speed fluctuation detection function. The values specified for P, Q, R, and I are

set in the following parameters: No. 4914, No. 4911, No. 4912, and No. 4913, respectively. Each

command address corresponds to a parameter number as listed below.

Command address

Parameter number

Q

No.4911

R

No.4912

I

No.4913

P

No.4914

If the P, Q, R, or I command address is omitted, the function detects the fluctuation of the actual spindle

speed according to the value set in the corresponding parameter (No. 4914, No. 4911, No. 4912, or No.

4913).

- 107 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

The parameters (No. 4914, No. 4911, No. 4912, and No. 4913) for the spindle on which the currently

selected position coder is mounted are used for the setting and spindle speed fluctuation detection check.

-

Spindle fluctuation detection off

G25;

G25 disables the spindle speed fluctuation detection function.

When G25 is specified, the parameters (No. 4914, No. 4911, No. 4912, and No. 4913) are unchanged.

When the power is turned on or after a reset (clear state (bit 6 (CLR) of parameter No. 3402 = 1)) is

executed, the spindle speed fluctuation detection function is disabled (G25). For the clear state, also

check the setting of bit 0 (C08) of parameter No. 3407.

Explanation

The function for detecting spindle speed fluctuation checks whether the actual speed varies for the

specified speed or not. Si or Sr, whichever is greater, is taken as the allowable fluctuation speed (Sm).

An alarm (OH0704) is activated when the actual spindle speed varies for the commanded speed (Sc)

under the condition that the variation width exceeds the allowable variation width (Sm).

|Sc - Sa| > Sm

Sc : Specified spindle speed

Sa : Actual spindle speed

Si : The allowable constant variation width which is independent of the specified spindle speed

(parameter (No.4913))

Sr : The allowable variation width which is obtained by multiplying Sc (commanded spindle speed)

by r (constant ratio). (r = parameter (No.4912))

Parameter FLR(No.4900#0)= 0

Parameter FLR(No.4900#0)= 1

r

r

Sr = Sc ×

Sr = Sc ×

100

1000

Sm: Si or Sr, whichever is greater

-

Conditions to start spindle speed fluctuation detection

If the specified spindle speed Sc changes, spindle speed fluctuation detection starts when one of the

conditions below is met:

<1> The actual spindle speed falls in a range of (Sc - Sq) to (Sc + Sq)

Sc : Specified spindle speed

Sq : Tolerance within which the spindle is assumed to attain the programmed speed

(parameter (No.4911))

Parameter FLR= 0

Parameter FLR= 1

q

q

Sq = Sc ×

Sq = Sc ×

100

1000

<2> When time p specified in parameter No. 4914 elapses after the specified speed Sc changes.

-

Examples of spindle speed fluctuation detection

(Example 1)

When an alarm (OH0704) is issued after a specified spindle speed is reached

- 108 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Spindle

speed

Sr

Sq

Si

Specified

Sq

Si

speed

Sr

P

Actual

CHECK

NO CHECK

CHECK

speed

G26 mode

Time

Specification of

Start of check

Alarm

another speed

(Example 2)

When an alarm OH0704 is issued before a specified spindle speed is reached

Spindle

speed

Sr

Sq

Si

Specified

speed

Sq

Si

Sr

P

CHECK NO CHECK CHECK

Actual

speed

G26 mode

Time

Specification of

Start of Alarm

another speed

check

Specified speed

:

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

Actual speed

: Speed detected with a position coder

p

: Period after a change occurs in the actual spindle speed until detection starts

Parameter No.4914, address P

Sq

:

(Specified spindle speed)× (Detection start tolerance (q))

Parameter No.4911, address Q

Parameter FLR = 0

Parameter FLR = 1

q

q

100

1000

Sr

:

(Specified spindle speed) × (Allowable variation (r))

Parameter No.4912, address R

Parameter FLR = 0

Parameter FLR = 1

r

r

100

1000

Si

: Allowable variation width

Parameter No.4913, address I

- 109 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

If the difference between the specified speed and actual speed exceeds both Sr and Si, an alarm OH0704

is raised.

-

Relationship between spindle speed control and each spindle

Spindle

Serial spindle

Function

1st spindle

2nd spindle

Spindle speed fluctuation detection

Possible

Possible^(*1)

NOTE

1 It is necessary to enable multi spindle control (bit 3 (MSP) of parameter No.

8133 is 1).

2 The spindle speed fluctuation detection function is effective for a single spindle.

The function cannot be executed for two or more spindles.

The spindle speed fluctuation detection function is effective for a spindle on

which the currently selected position coder is mounted. Just a single position

coder can be selected. Multiple position coders cannot be selected. For the

selection of a position coder, see the section of "Multi spindle."

* Position coder selection signals (PC2SLC<Gn028.7>)

3 The parameters that become valid are the parameters of the spindle speed

fluctuation detection function (No.4911, No.4912, No.4913, No.4914) for the

spindle on which the currently selected position coder is mounted.

-

Spindle for which to detect the spindle speed fluctuation

For the spindle for which to detect the spindle speed fluctuation, refer to the appropriate manual provided

by the machine tool builder.

9.6

SPINDLE CONTROL WITH SERVO MOTOR

Overview

The function for spindle control with servo motor allows a servo motor to be used for executing spindle

speed commands and spindle functions such as rigid tapping.

(1) Spindle control with servo motor

Velocity control can be performed by using a speed command (S command) with a servo motor set

as the tool rotation axis. No reference position return is necessary to switch between rotation and

positioning commands.

(2) Spindle indexing

With the spindle indexing function, a stop position can be programmed to stop a rotating axis at the

specified position. There are two types of spindle indexing. The first type allows the next-block

command to be executed before spindle indexing is finished. The second type allows the next

block to be executed only after spindle indexing is completed.

With the first type, it is possible to issue commands to axes other than the axis for which a spindle

indexing command has been issued, before the next command is issued to the axis. Before the next

command is issued to the axis for which a spindle indexing command has been issued, whether

spindle indexing is completed or not can be checked by programming or by using a signal. Using

this function can reduce the wait time. In addition, an axis can be stopped at a specified point by

issuing a spindle indexing command to the axis when the spindle is rotating.

(3) Axis movement

When bit 0 (PCE) of parameter No. 11006 is 1, if axis movement (G00/G01) is specified for a servo

motor spindle in the same way as in a normal controlled axis, position control can be performed.

(4) Rigid tapping with servo motor

Rigid tapping can be carried out by regarding a servo motor spindle as a rotation axis.

(5) Threading, feed per rotation feed, and constant surface speed control

- 110 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Threading, feed per rotation feed, and constant surface speed control can be performed using a servo

motor spindle as a spindle.

(6) Spindle output control with PMC

The rotation speed and polarity can be controlled by PMC.

-

Spindle motors and supported functions

Spindle functions

Conventional spindle control

Spindle control with servo motor

Feed per revolution

○

○

Threading

○

○

Polygon machining

○

×^*1

Spindle speed fluctuation detection

○

×

Spindle synchronous control

○

×

Simple spindle synchronous control

○

×

Polygon machining with two spindles

○

×

Spindle orientation

Multi-point orientation

○

×

Spindle output switching

Inter-path spindle control

○

○

Constant surface speed control

○

○

Multi-spindle control

○

○

Rigid tapping

○

○

Spindle output control with PMC

○

○

Actual spindle speed output

○

○

Spindle indexing

×

○

*1 Servo motor can be used as tool rotation axis.

It is not possible to use as a spindle which rotates workpiece.

Notes

(1) This function is optional.

(2) The available functions and spindle axis composition are predetermined according to the machine

used. Refer to the manual supplied by the machine tool builder.

(3) If necessary, refer to "SPINDLE CONTROL WITH SERVO MOTOR" in "CONNECTION

MANUAL (FUNCTION)" (B-64303EN-1).

9.6.1

Spindle Control with Servo Motor

Specification

-

Command with a program

This function can be used to specify the S spindle rotation command for a servo motor spindle in the SV

speed control mode. For rotation control of a servo motor, specify G96.4 to start the SV speed control

mode. Once the SV speed control mode is specified, the S command is valid for the servo motor until

the SV speed control mode is released. Do not specify a positioning command in the SV speed control

mode. Otherwise, alarm PS0445 is issued.

Before positioning operation, release the SV speed control mode. To release the SV speed control mode,

specify the spindle indexing command G96.1/G96.2. For details on spindle indexing, see "Spindle

Indexing Function". When bit 0 (PCE) of parameter No. 11006 is 1, a positioning command can be

specified. When bit 0 (PCE) of parameter No. 11006 is 0, a positioning command cannot be specified

for a servo motor spindle. If specified, alarm PS0601 is issued.

In a mode other than the SV speed control mode, the S command is invalid. However, since information

of the S command is recorded, if the SV speed control mode is entered, rotation starts at the specified

rotation speed.

- 111 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Explanation

-

Command

(1) Spindle speed command output

Set up the spindle speed command in the same way as for the ordinary speed command (S

command). Before specifying a speed command (S command), start the SV speed control mode.

When performing positioning, cancel the SV speed control mode, and select the position control

mode.

The sequence by the following input signals is unnecessary.

*ESPA, MRDYA, and SFRA

(2) Condition for stopping spindle speed output

Commands once output to a spindle become 0 if *SSTP becomes “0” or if a command (such as S0)

that makes the spindle speed command output 0 is issued. Also, issuing a spindle indexing

command (G96.1/G96.2) makes the spindle speed command output 0. In addition, an emergency

stop condition and servo alarm bring the spindle to a stop.

With M05, the CNC does not make the command output to the spindle 0.

(3) Stopping rotation by spindle indexing

Issuing a command that specifies a position enables the rotating axis to stop at the specified position.

For details, see Subsection, "Spindle Indexing Function."

(4) Maximum speed

The maximum speed that can be specified is usually 2777 min^-1.

However, setting bit 3 (IRC) of parameter No. 1408 to "1" may be able to increase the limit to about

27770 min^-1 depending on the performance of the related motor and detector.

-

Multi-spindle control and commands from another path

When a servo motor spindle and another spindle are present together in the same path, the multi-spindle

control function is required to specify a rotation command. The path spindle control function can handle

commands from another path. The address P-based spindle select function for multi-spindle control can

be used to select spindles in another path.

Example program commands follow.

Example 1:

(Spindle selection with address P)

Bit 3 (MPP) of parameter No. 3703 = "1": A spindle is selected with address P.

Spindle configuration (S1 = first spindle and S2 = second spindle)

Path 1

Path 2

S1 (spindle axis)

S3 (spindle axis)

S2 (servo motor spindle)

-

Setting address P for spindle selection in multi-spindle control

Parameter

Path 1

Path 2

11 (S1)

21 (S3)

3781

12 (S2)

-

Program example

Command issuing

Program

Operation

path

1

M03 S1000 P12 ;

S2 rotates in normal direction at 1000 min^-1.

1

M03 S1500 P21 ;

S3 rotates in normal direction at 1500 min^-1.

2

M04 S1500 P11 ;

S1 rotates in reverse direction at 1500 min^-1.

-

Manual operation of a servo motor spindle

Before performing the manual operation and manual reference position return of a servo motor spindle,

release the SV speed control mode. Manual operation and manual reference position return in the SV

speed control mode are invalid.

- 113 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

When using an absolute position detector, manual reference position return is not required. If reference

position return (G28) is performed in a program when position control is disabled (bit 0 (PCE) of

parameter No. 11006 is 0), alarm PS0601 is issued.

NOTE

If a movement command is specified for a servo motor spindle when position

control is disabled (bit 0 (PCE) of parameter No. 11006 is 0), alarm PS0601 is

issued.

-

Acceleration/deceleration (time constant)

It is possible to change the spindle acceleration/deceleration specified in a rotation command according to

the speed of the spindle.

Acceleration/deceleration can be switched at two points of speed, using parameters S0 and S1 (switching

speed). In addition, parameters Aa, Ab, and Ac are available to set up three acceleration/deceleration

spans.

Rotation

speed (min^-1)

Ac

S

S1

Ab

S0

Aa

Time (s)

S₀

: Setting of parameter No. 11020 (acceleration/deceleration is switched at rotation speed S₀ (min^-1)).

S₁

: Setting of parameter No. 11021 (acceleration/deceleration is switched at rotation speed S₁ (min^-1)).

S

: Specified rotation speed (min^-1).

Aa

: Setting of parameter No. 11030 (acceleration/deceleration (min-1/s) used between rotation speeds 0

and S₀).

Ab : Setting of parameter No. 11031 (acceleration/deceleration (min-1/s) used between rotation speeds

S₀ and S₁).

Ac

: Setting of parameter No. 11032 (acceleration/deceleration (min-1/s) used between S1 and the

specified speed S).

Determine the setting of each parameter according to the torque characteristic of the motor.

-

Acceleration/deceleration after interpolation

Acceleration/deceleration after interpolation is available in the SV speed control mode. Bit 1 (TCR) of

parameter No.11001 can be used to select a time constant type, that is, parameter No. 1622

(Time constant of acceleration/deceleration in cutting feed for each axis) or parameter No. 11016 (Time

constant of acceleration/ deceleration in SV speed control mode for each axis).

-

Direction of rotation

The voltage polarity at the time of spindle speed output can be changed using bit 6 (CWM) and bit 7

(TCM) of parameter No. 3706.

It is also possible to reverse the direction of spindle rotation, using the SV reverse signal <Gn523>.

These functions are usable in the rotation mode and during rigid tapping. Changing the signal to

ON/OFF during rotation causes the spindle to decelerate, reverse, and then accelerate.

- 114 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Rotation

SV reverse signal ON

speed (min^-1)

S

Ac

S₁

Ab

S₀

Aa

0

Aa

-S₀

Ab

-S₁

-S

Ac

Time (sec)

-

Display

Bit 3 (NDF) of parameter No. 3115 can be used to specify whether to display the actual speed. This,

however, is not considered in the SV speed control mode regardless of the setting of the NDF parameter

bit. In addition, bits 0 (NDP) and 1 (NDA) of parameter No. 3115 can be used to specify whether to

display, respectively, the current position and the remaining amount of movement.

Restrictions

(1) When multi-spindle control is enabled, in settings other than multi-spindle P type, specifying G96.*

P is regarded as invalid.

(2) When starting or canceling the SV speed control mode during automatic operation, be sure to

specify the path of the target axis of the SV speed control mode. When it is specified from the other

path, alarm PS0602 is issued.

(3) Be sure to set M code which starts or cancels the SV speed control mode to M code preventing

buffering (parameter No.3411 to 3420, No.3421 to 3432).

(4) When the SV speed control mode is started or cancelled except for automatic operation, be sure to

perform manual reference position return before starting the automatic operation so that the target

axis lose its reference position.

The axis may not move correctly to the commanded position in SV speed control cancel mode

(position control mode) when the automatic operation is started without performing manual

reference position return.

Notes

(1) This function is optional.

(2) The available functions and spindle axis composition are predetermined according to the machine

used. Refer to the manual supplied by the machine tool builder.

(3) If necessary, refer to "Spindle Control with Servo Motor" in "CONNECTION MANUAL

(FUNCTION)" (B-64303EN-1).

(4) Unlike spindle motors, a servo motor spindle stops rotating when a servo alarm, an emergency stop,

or a machine lock occurs.

(5) The maximum motor speed is obtained by applying the feed gear to the maximum motor speed set in

parameter No. 11015.

(6) If bit 3 (IRC) of parameter No. 1408 is set to 0, the error prevention function may work when the

speed has reached around 2778 min^-1. When a speed of 2778 min^-1 or more is required, set the IRC

parameter bit to 1. If IRC is set to 1, it becomes possible to specify a speed of up to approximately

27770 min^-1.

- 115 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

9.6.2

Spindle Indexing Function

Format

G96.1 P_ R_ ; After spindle indexing is completed, the operation of the next block is

started.

G96.2 P_ R_ ; Before spindle indexing is completed, the operation of the next block

is started.

G96.3 P_ ;

After it is confirmed that spindle indexing is completed, the operation

of the next block is started.

P: Spindle selection with multi-spindle control

R: Stoppage angle [deg] (0 to (parameter No. 1260))

When multi-spindle control is enabled, select a spindle according to the specification of multi-spindle

control along with the G96.1/G96.2/ G96.3 command. When a spindle is selected with address P, to

specify address P, use parameter No. 3781 (P code for selecting a spindle). In any case, when a servo

motor spindle has not been selected, alarm PS0602 is issued.

When multi-spindle control is disabled, it is possible to command G96.4 independently. When there is no

servo motor spindle in the system, alarm PS0602 is issued.

In 2-path system, when it is specified from paths other than the path that a servo motor spindle belongs,

alarm PS0602 is issued.

To turn the position control mode ON without performing spindle indexing, do so after canceling the SV

speed control mode by issuing G96.1 command with no R specified when the motor is at a halt.

When the motor is rotating, issuing a G96.1 (or G96.2) command with no R specified results in the motor

coming to a halt by behaving in the same manner as for R0.

NOTE

1 When having specified G96.2, check the completion of the movement by

specifying G96.3 before specifying the next move command for the spindle. If

the next move command is specified without confirming the completion of the

movement, alarm PS0601 is issued. Similarly, if rigid tapping is specified

without confirming the completion of the movement, alarm PS0445 is issued.

2 A block specifying G96.1, G96.2, or G96.3 must not contain any other command.

If an axis command is specified in the same block, alarm PS0446 is issued.

-

Reference position return

Before executing the first command of spindle indexing to the tool rotation axis with a servo motor, be

sure to perform a manual reference position return. When the absolute-position detector is used,

however, a manual reference position return is not necessary. When the reference position return

command (G28) is executed in a program, alarm PS0601 is issued.

Spindle indexing command

-

Move command

(1) Command waiting for spindle indexing to be completed

If G96.1 is issued, the next block is executed after spindle indexing is completed.

(2) Command not waiting for spindle indexing to be completed

If G96.2 is issued, the next block can be executed before spindle indexing is completed.

-

Movement completion check command

G96.3 is used to check to see if spindle indexing is completed. If it has not been completed, the next

block waits for spindle indexing to be completed. If it is completed, the next block is executed.

- 116 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

-

SV speed control mode cancellation

If G96.1 is used to perform spindle indexing, the SV speed control mode is canceled when spindle

indexing is completed.

If G96.2 is used to perform spindle indexing, G96.3 can be used to check to see if spindle indexing is

completed and, if completed, cancel the SV speed control mode. Issuing G96.2 not followed by G96.3

cannot cancel the SV speed control mode even if spindle indexing is completed.

If SV speed control mode cancel, it is necessary to be commanded in the path to which the live tool axis

belongs.

Example for specifying the start/cancellation of the SV speed control mode (when bit 3 (MPP) of parameter

No. 3703 = 1)

Spindle

Spindle selection P code

Servo motor spindle address

name

(parameter No. 3781)

S1

P1

C

Specification by programming (SV speed control mode in-progress signal <Fn521>)

Programmed

Start/cancellation of speed control mode

Operation

command

Start (SV speed control mode in-progress

G96.4 P1 ;

The SV speed control mode is started (C).

signal (C) = 1)

Servo motor spindle C turns in the forward

M03 S100 P1 ;

:

direction at 100 [min^-1].

:

:

:

Cancel (SV speed control mode in-progress

The servo motor spindle C stops when C = 0

G96.1 P1 R0 ;

signal (C) = 0)

(spindle indexing).

Mode switching by signal

Programmed

Start/cancellation of speed control mode

Operation

command

Start (SV speed control mode in-progress

The SV speed control mode is started by the M

M15 ;

signal (C) = 1)

code (C).

Servo motor spindle C turns in the forward

M03 S100 P1 ;

:

direction at 100 [min^-1].

:

:

:

Cancel (SV speed control mode in-progress

The servo motor spindle C stops when C = 0

G96.1 P1 R0 ;

signal (C) = 0)

(spindle indexing).

-

Spindle indexing command during spindle rotation

Issuing G96.1 or G96.2 with a position specified during spindle rotation causes the spindle to stop at the

specified position.

Example)

M03 S1000 ;

Rotation at S1000

G96.1 P1 R180. ;

Stoppage of rotation at the 180° position

-

Spindle indexing speed

Issuing G96.1 or G96.2 causes a move speed to be dedicated to spindle indexing. Specify the move

speed for spindle indexing, using parameter No. 11012.

- Spindle indexing acceleration/deceleration

Shown below is the acceleration/deceleration specified by G96.1/G96.2.

- 117 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

Rotation

speed (min^-1)

A

c

S

S₁

Ab

S₀

Aa

S_i

Aa

Time (s)

S₁

: Parameter No. 11020 setting

(acceleration/deceleration is switched at a rotation speed of S₁

(min^-1).)

S₀

: Parameter No. 11021 setting

(acceleration/deceleration is switched at a rotation speed of S₀

(min^-1).)

S

: Command-specified rotation speed (min^-1)

Si

: Spindle indexing speed (min-1) parameter No. 11012

Aa

: Parameter No. 11030 setting (acceleration/deceleration (min-1/s) used between rotation speeds 0

and S₀ (span 1))

Ab

: Parameter No. 11031 setting (acceleration/deceleration (min-1/s) used between rotation speeds S₀

and S₁ (span 2))

Ac

: Parameter No. 11032 setting (acceleration/deceleration (min-1/s) used between S1 and a specified

speed S (span 3)))

-

Example program commands

(1) A move command is issued to the spindle, using G96.2. The spindle starts moving, and the

execution of the next block begins.

The spindle keeps moving even when any other block is being executed.

(The spindle indexing signal SPP<Fn522> is "1" during spindle indexing.)

(2) When another command is issued to the spindle, G96.3 is used to heck in advance whether the

spindle has finished moving.

If the spindle is still moving (the spindle indexing signal is on), the CNC enters a wait state. If the

spindle has finished moving, the command is issued to cause the spindle to start moving.

Example: Command not waiting for spindle indexing to finish and command checking whether spindle

indexing has finished (parameter No. 3781 (S1) = "1")

Program command

Operation

Command not waiting for spindle indexing to finish.

G96.2 P1 R270.0

;

The first spindle S1 moves to 270.0.

G01 X10.0 Y20.0 F1000. ;

Starts cutting feed. No wait for spindle indexing to finish.

G02 X50.0 Y100.0 R50.0 ;

Starts circular interpolation. No wait for spindle indexing to finish.

G96.3 P1 ;

Checks whether spindle indexing has finished.

M29 S100 P1 ;

Starts rigid tapping if the spindle indexing signal is "0".

G84 X10.0 Y 20.0 R-5.0 Z-20.0 ;

Waits for rigid tapping command if the spindle indexing signal is "1".

Indexing by machine coordinates

In the function for spindle control with servo motor, the following operations can be selected:

(1) When the speed control mode is off, indexing to machine coordinate 0.000 is performed.

(2) When G code-based spindle indexing has been performed, an R command indicates a machine

coordinate value.

- 118 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Spindle indexing operation

Using bit 0 (SIC) of parameter No. 11005 can select which coordinate system, absolute or machine, is to

be used in spindle indexing.

Example:

If the difference between the machine and absolute coordinates (machine coordinate - absolute

coordinate) is 100.000:

•

Spindle indexing performed by turning the SV speed control mode signal <Gn521> OFF (1

t

0) or issuing a spindle indexing

G code (with no R specified)

1.

If bit 0 (SIC) of parameter No. 11005 = 0:

Spindle indexing is performed with a machine coordinate of 100.000 and an absolute

coordinate of 0.000.

2.

If bit 0 (SIC) of parameter No. 11005 = 1:

Spindle indexing is performed with a machine coordinate of 0.000 and an absolute

coordinate of 260.000.

•

G code-based spindle indexing (with R specified)

Assuming that spindle indexing is specified with R100.000:

1.

If bit 0 (SIC) of parameter No. 11005 = 0:

Spindle indexing is performed with a machine coordinate of 200.000 and an absolute

coordinate of 100.000.

2.

If bit 0 (SIC) of parameter No. 11005 = 1:

Spindle indexing is performed with a machine coordinate of 100.000 and an absolute

coordinate of 0.000.

Notes

(1) If G96.2 (not waiting for spindle indexing to finish) is issued, G96.3 must be issued to check

whether spindle indexing has finished. Be sure to issue G96.3 after G96.2. If a movement along

an axis is specified without checking (without issuing the G96.3 command), alarm PS0601 is issued.

Similarly, if rigid tapping is specified, alarm PS0445 is issued.

(2) If it has not been checked, for example, because of a reset, whether spindle indexing has finished

after G96.2 (not waiting for spindle indexing to finish) is issued, the SV speed control mode is not

canceled.

(3) If the spindle stops rotating because of spindle indexing, the spindle speed command output

becomes 0. To cause the spindle to restart rotating, place the spindle in the SV speed control mode,

and then, issue an S command.

(4) Spindle indexing is enabled only in the SV speed control mode.

(5) When the spindle indexing speed (parameter No. 11012) is 0, the acceleration/deceleration switching

speed

(1st step)

(parameter No.

11020) is the spindle indexing speed.

When the

acceleration/deceleration switching speed is also 0, the maximum speed (parameter No. 3741) of

each spindle that corresponds to gear 1 is the spindle indexing speed.

(6) The G96.* P command is invalid for settings other than multi-spindle control type P.

(7) The SV speed control mode during automatic operation must be switched by a command from the

path to which it belongs. When it is specified from the other path, alarm PS0602 is issued.

9.6.3

Rigid Tapping with Servo Motor

Format

The command format for this type of rigid tapping is the same as for the conventional type of rigid

tapping.

For details, refer to the chapter of "RIGID TAPPING" in the OPERATOR’S MANUAL (Lathe System)

(B-64304EN-1) or OPERATOR’S MANUAL (Machining Center System) (B-64304EN-2).

- 119 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

NOTE

Before rigid tapping can be specified, the SV speed control mode for the servo

motor spindle must be canceled. If rotation is in progress, use G96.1/G96.2 to

cancel the SV speed control mode. The mode of the servo motor spindle can

be checked by checking the SV speed control mode in-progress signal

(SVREV<Fn521>).

If rigid tapping is specified in the SV speed control mode, alarm PS0445 is

issued.

Rigid tapping specification

- Feedrate

For rigid tapping, the feedrate of a drilling axis is one specified in an F command, and that of the spindle

is S × the amount of movement per live tool axis (servo motor spindle) rotation [deg/min] (parameter No.

11011).

Feed per minute and feed per revolution are detailed later.

During rigid tapping, the spindle speed is limited by a parameter for specifying the maximum cutting

feedrate for the axis used as a live tool axis, that is, parameter No. 1430 (or No. 1432 if acceleration/

deceleration before interpolation is enabled).

Normally, the parameter of the maximum cutting feedrate (parameter No. 1430) (parameter No. 1432

when acceleration/deceleration before interpolation is enabled) can be set to up to 999999.999 [deg/min]

(equivalent to S2778 [min^-1]). However, for an axis set as the live tool axis (bit 3 (IRC) of parameter No.

1408 = 1) that is used for rigid tapping, the maximum feedrate is limited to ten times as large as the

setting of the maximum cutting feedrate parameter.

Example:

Maximum cutting feedrate parameter No. 1430 = 360000

Limit to the maximum spindle speed 360000×10 = 3600000 [deg/min] (S10000 [min^-1])

CAUTION

Make the tapper thread pitch equal to one specified by the program (F, S).

Otherwise, the tool or workpiece may be damaged.

Acceleration/deceleration control

-

Acceleration/deceleration after interpolation

Unlike conventional rigid tapping (with a spindle motor), rigid tapping with a servo motor allows the

application of linear acceleration/deceleration with constant acceleration/deceleration time or bell-shaped

acceleration/deceleration.

Resetting bit 0 (SRBx) of parameter No. 11001 to "0" makes it possible to apply linear

acceleration/deceleration after interpolation of constant acceleration time type. Setting the bit to "1"

makes it possible to apply bell-shape acceleration/deceleration after interpolation of constant acceleration

time type.

The time constant for each gear is specified in parameter Nos. 11060 to 11063. If bit 2 (TDR) of

parameter No. 5201 = "1", the tool extraction time constant for each gear is specified in parameter

Nos. 11065 to 11068. Specify each of these parameters for the live tool axis (servo motor spindle) used

in rigid tapping.

The acceleration/deceleration types and time constants used for drilling axes are set to the same values as

for live tool axes (servo motor spindles).

NOTE

This type of rigid tapping and conventional rigid tapping (with a spindle motor)

differ in time constant setting.

- 120 -

9.SPINDLE SPEED FUNCTION

B-64304EN/02

PROGRAMMING

(S FUNCTION)

Example: Parameter settings are: Time constant (TC) = 800 msec and speed (S) = 4000 min^-1

min^-1

4000

800

800

msec

-

Acceleration/deceleration before interpolation

In this type of rigid tapping, when advanced preview control can be used, rigid tapping can be specified

in the mode for acceleration/deceleration before look ahead interpolation to allow

acceleration/deceleration

before

look

ahead

interpolation

during

rigid

tapping.

Acceleration/deceleration before look ahead interpolation is enabled when the advanced preview control

mode is set to on. For the advanced preview control function, see "High-Speed High-Precision Function

(Advanced Preview Control)".

Parameter No. 11050 is used to specify the maximum allowable acceleration value for

acceleration/deceleration interpolation used in rigid tapping. Parameter No. 11051 is used to specify the

acceleration change time for bell-shape acceleration/deceleration before interpolation. As for

acceleration/deceleration before interpolation used in rigid tapping, the maximum allowable acceleration

value is 100000 [deg/s²].

It is possible to change a speed of up to S1000 [min^-1] (equivalent to 360000 [deg/min] in 60 [ms].

The time constant (parameter No. 11052) for cutting feed acceleration/deceleration after interpolation

usable in the "acceleration/deceleration before look-ahead interpolation" mode is a constant-time type.

NOTE

Specify the same time constant for both drilling and live tool axes (servo motor

spindle). Otherwise, it is likely that the machine may malfunction.

Spindle indexing

This function does not allow the spindle orientation function to be performed at the start of rigid tapping.

Before specifying rigid tapping, perform spindle indexing to the position at which tapping is to be

performed. For details, see "Spindle Indexing Function" described previously.

Notes

If the pitch is very small or the amount of travel along the drilling axis is large, the amount of travel along

the rotation axis becomes large, possibly resulting in alarm PS0003.

9.6.4

Feed per Revolution

Overview

The function for spindle control with servo motor allows a feed per revolution to be specified.

- 121 -

9. SPINDLE SPEED FUNCTION

(S FUNCTION)

PROGRAMMING

B-64304EN/02

From the separate detector connected to the spindle, the rate of feed per revolution is obtained. When

the detector built into the servo motor is to be used, the feedrate is obtained based on the servo motor

speed and gear ratio.

Which detector to use is specified by bit 1 (OPTx) of parameter No. 1815.

NOTE

If the machine is equipped with a live tool axis and spindle with servo motor,

using rotation commands requires the multi-spindle control function.

As for gear change, use T type gear change.

See Section, “MULTI-SPINDLE CONTROL,” in Connection Manual (Function)

(B-64303EN-1) for explanations about multi-spindle control.

Format

The command format for feed per revolution explained above is the same as for the ordinary types of feed

per revolution.

-

Examples

When the second spindle (C-axis) is used for rotation control and position control with the second spindle

assumed to be a servo motor spindle

(The G code system A in lathe system is selected.)

Program command

Operation

M*** ;

The C axis rotation control mode is turned ON.

M03 S100 P2 ;

The servo motor spindle (C axis) rotates at 100 min^-1.

G99 G01 Z-100. F10. ;

The Z axis moves at a feed-per-revolution speed of 1000 mm/min.

:

:

The C axis position control mode is set to ON (rotation control mode OFF).

M*** ;

The spindle stops with C = 0.000.

9.6.5

Spindle Output Control with PMC

Overview

The “spindle control with servo motor” function enables the PMC to be sued for spindle output control.

How to specify

After the start of the SV speed control mode, this function can be specified in the same way as in ordinary

spindle control (with a spindle motor).

Refer to Section,

“SPINDLE OUTPUT CONTROL BY THE PMC,” in this manual for detailed

descriptions.

NOTE

For the “spindle control with servo motor” function, the maximum motor speed is

one specified in parameter No.11015.

- 122 -

B-64304EN/02

PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)

10 TOOL FUNCTION (T FUNCTION)

Chapter 10, "TOOL FUNCTION (T FUNCTION)", consists of the following sections:

10.1 TOOL SELECTION FUNCTION

123

10.2 TOOL LIFE MANAGEMENT

124

10.1 TOOL SELECTION FUNCTION

By specifying an up to 8-digit numerical value following address T, a code signal and a strobe signal are

transmitted to the machine tool. This is 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 commendable 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:

(i)

Simultaneous execution of the move command and T function commands.

(ii) Executing T function commands upon completion of move command execution.

The selection of either (i) or (ii) depends on the machine tool builder's specifications. Refer to the

manual issued by the machine tool builder for details.

Explanations

T

The value after the T code indicates the desired tool. Part of the value is also used as a tool offset

number that specifies the amount of tool offset or the like. The tool can be selected as follows according

to the specification method and parameter settings.

Description of a T code (Note 1)

How to specify the offset number for each

LGN (No.5002#1) = 0

LGN (No.5002#1) = 1

parameter setting (Note 2)

T{{{{{{{

{

T{{{{{{{

{

The tool wear offset number is specified using

↑

↑

↑

↑

the low-order one digit of a T code.

Tool selection Tool geometry

Tool selection Tool wear

tool wear

tool geometry offset

When parameter (No.5028) is set to 1

offset

offset

T{{{{{{

{{

T{{{{{{

{{

The tool wear offset number is specified using

↑

↑

↑

↑

the low-order two digits of a T code.

Tool selection Tool geometry

Tool selection Tool wear

tool wear

tool geometry offset

When parameter (No.5028) is set to 2

offset

offset

T{{{{{

{{{

T{{{{{

{{{

The tool wear offset number is specified using

↑

↑

↑

↑

the low-order three digits of a T code.

Tool selection Tool geometry

Tool selection Tool wear

tool wear

tool geometry offset

When parameter (No.5028) is set to 3

offset

offset

- 123 -

10.TOOL FUNCTION (T FUNCTION) PROGRAMMING

B-64304EN/02

NOTE

1 The maximum number of digits of a T code can be specified by parameter

(No.3032) as 1 to 8.

2 When parameter (No.5028) is set to 0, the number of digits used to specify the

offset number in a T code depends on the number of tool offsets.

Example)

When the number of tool offsets is 1 to 9:

Low-order one digit

When the number of tool offsets is 10 to 99:

Low-order two digits

When the number of tool offsets is 100 to 200: Low-order three digits

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)

N1 G00 X1000 Z1400 ;

N2 T0313 ;

(Select tool No. 3 and tool offset value No. 13)

N3 X400 Z1050 ;

10.2 TOOL LIFE MANAGEMENT

Tools are classified into several groups, and a tool life (use count or use duration) is specified for each

group in advance. Each time a tool is used, its life is counted, and when the tool life expires, a new tool

that is sequenced next within the same group is selected automatically. With this function, the tool life

can be managed while machining is being performed continuously. Data for tool life management

consists of tool group numbers, tool life values, tool numbers, and codes for specifying a tool offset value.

These data items are registered in the CNC.

Tool group number m

Tool life value l

1

Tool number (T)

Code for specifying tool offset

1st-tool management data

value (H/D)

2

:

:

2nd-tool management data

:

:

:

:

:

:

:

:

n

:

:

nth-tool management data

Machining program

Machine and CNC operations

:

Machine

CNC

Tool life

:

Places a

Automatically

management data

selected tool

selects, from tool

Command for selecting

Tool group number 1

in the wait

group m, a tool

tool group m

state.

whose life has not

:

Select

:

expired.

:

Attaches the

Starts counting the

tool.

:

Tool group number m

tool in the

life of the tool

Tool change command

wait state to

attached to the

:

(M06)

the spindle

spindle.

:

(tool

:

change).

Tool group number p

:

Fig. 10.2 (a) Tool selection from machining program

M

A group is selected by a T code, and tool life counting is started by the M06 command. (ATC type)

- 124 -

B-64304EN/02

PROGRAMMING 10.TOOL FUNCTION (T FUNCTION)

T

A group is selected, tool compensation is specified, and tool life counting is started only by a T code.

(turret type)

-

Maximum number of tool life management groups and 2-path system

A maximum of 128 tool life management groups can be used for each path.

For each path, set a maximum number of groups to be used in parameter No. 6813.

The maximum number of groups must be a multiple of the minimum number of groups (eight groups).

A setting of 0 indicates 128 groups.

CAUTION

When parameter No. 6813 is changed and the power is turned on, all data in the

tool life management file is initialized. So, it is necessary to set life

management data for all paths that use tool life management.

10.2.1 Tool Life Management Data

Tool life management data consists of tool group numbers, tool numbers, codes for specifying a tool

offset value, and tool life values.

Explanation

- Tool group number

A maximum of 128 tool life management groups can be used for each path.

Set the maximum number of groups to be used in parameter No. 6813. Up to two tools can be registered

for each of a maximum number of groups. If bit 0 (GS1) of parameter No. 6800 and bit 1 (GS2) of

parameter No. 6800 is set, it is possible to change the combination of the number of registrable groups

and the maximum number of tools.

Table 10.2.1 Maximum numbers of registrable groups and tools

GS2

GS1

Number of groups

Number of tools

(No. 6800#1)

(No. 6800#0)

0

0

1 to Maximum number of groups (parameter No.6813) x 1/8

1 to 16

0

1

1 to Maximum number of groups (parameter No.6813) x 1/4

1 to 8

1

0

1 to Maximum number of groups (parameter No.6813) x 1/2

1 to 4

1

1

1 to Maximum number of groups (parameter No.6813)

1 to 2

CAUTION

After changing the setting of bit 0 (GS1) and bit 1 (GS2) of parameter No. 6800,

re-register tool life management data by issuing the G10L3 (registration after

deletion of data for all groups).

Otherwise, the newly set combination does not become valid.

- Tool number

A tool number is specified with a T code. A number consisting of up to eight digits (99999999) can be

specified.

NOTE

The maximum number of digits usable in the T code is specified in parameter

No. 3032.

- 125 -

Content      ..     3      4      5      6     ..