Content      ..     10      11      12      13     ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 12

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

Explanation

Override of gear ratio for flexible synchronization

This function enables to override the commanded gear ratio of flexible synchronous control.

Program example

Axis configuration: X,Y,Z,C, and U

Setting of flexible synchronous control：

Master axis : Z, slave axis : U,

M code for turning on the flexible synchronization control mode : M50

M code for turning off the flexible synchronization control mode : M51

G90 G00 X100.0 Y75.0 Z120.0 C0 U0 ;

Move to the start point.

M50 ;

Start Z-U synchronization.

G81.1 Z100.0 Q-25.0 R10.0 F3000. ;

Start chopping.

……………………

……………………

G80 ;

Cancel chopping.

M51 ;

Cancel Z-U synchronization.

Movement of chopping function by flexible synchronous control

Point R

(1)

Upper dead point

Movement process :

(2)

(1):Movement from point R to lower dead

Zm

point.

(2):Movement from lower dead point to

upper dead point.

(3)

(3):Movement from upper dead point to

Z

lower dead point.

After (1), repeat (2) and (3).

Lower dead point

Xs

X

When flexible synchronization is applied to Z axis (master) and X axis (slave), Amount

of travel Xs of X axis is as follows:

Xs = Zm × Gear ratio for flexible synchronization (parameter No.5680 to No.5693)

× override signal of gear ratio for flexible synchronization

Notes

1

The parameter setting and notes for flexible synchronous control and chopping are applied to this

function.

2

Flexible synchronous control is started and canceled by the flexible synchronous control mode select

signal. To start or cancel flexible synchronization during automatic operation, control the select

signal using the M code set in the relevant parameter.

3

Chopping can be specified using the following two ways: Specifying chopping in the program and

using the chopping start signal. Chopping started by specifying it in the program cannot be canceled

by inputting the signal.

4

Be sure to start or cancel chopping in flexible synchronous control for this function. (See “Program

example”.)

5

Before synchronization starts, the tool must be positioned along the slave axis.

6

When the servo delay compensation function during chopping operation is used with this function,

the compensation amount for the master axis is multiplied by the gear ratio of flexible

synchronization, and the result is output to the slave axis. If you want to adjust the compensation

- 322 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

amount for the slave axis, adjust the gear ratio using override signals of gear ratio for flexible

synchronization.

7

When this function is used for a rotation axis, the servo delay compensation function during

chopping operation cannot be used.

8.3

PARALLEL AXIS CONTROL

Overview

If a machine contains multiple heads and tables to machine multiple workpieces simultaneously, it is

possible to move multiple controlled axes assigned the same axis name, by using a move command for a

single program axis. This is called parallel operation.

Two or more axes that are moved simultaneously when a command for a single program axis, i.e., a

command with a single address, is issued are called parallel axes.

This function is effective to automatic operation, MDI operation, and manual numerical commands on

1-path machining centers. In manual operation, parallel operation is not possible, each controlled axis is

moved independently.

In parallel operation, the controlled axes belonging to a single program axis are moved in the same way in

principle. It is, however, possible to select specified ones from among multiple parallel axes and move

them (park the other axes), using appropriate external signals.

Y₂

Z₂

Y₁

Z₁

X

Fig. 8.3 (a)

In the Fig. 8.3 (a), Y₁ and Y₂ are parallel axes, and are operated in parallel with a command for a single

address Y.

Z₁ and Z₂ are also parallel axes, and are operated in parallel with a command for a single address Z.

There are two movements of each parallel axis, which are selected with appropriate external input signals.

• Normal (parking off)

The axis moves as commanded.

• Parking (parking on)

The axis ignores the command, and does not move.

- 323 -

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

NOTE

1

The parallel axis control function is effective to 1-path machining centers only.

2

The parallel axis control function does not support the functions below.

(1)

Smooth interpolation

(2)

Nano smoothing

(3)

3-dimensional coordinate system conversion

(4)

3-dimensional tool compensation

(5)

Tool length compensation in tool axis direction

(6)

Tool center point control

(7)

Tool posture control

(8)

3-dimensional cutter compensation

(9)

Tilted working plane command

(10) Nano smoothing 2

(11) Workpiece setting error compensation

(12) Tandem control

(13) Twin table control

(14) Synchronous/Composite control

(15) Superimposed Control

3

If coordinate system rotation (G68) is to be specified, the program coordinate

systems of the parallel axes must be identical. In the immediately preceding

block, therefore, it is necessary to execute a move command on all parallel axes,

using an absolute command (G90). (As long as the command is executed, there

may be any axes in parking.)

If the program coordinate systems of the parallel axes are not identical, alarm

PS0508, “G CODE TO NEED G90(PAC)” is issued.

Axis configuration in parallel axis control

The following limitations are imposed on the axis configuration in parallel axis control:

(1) All parallel axes must have the same axis name.

If different axis names are set, the axes cannot be recognized as parallel axes.

(2) To distinguish parallel axes from one another, specify the subscript for each of the axes.

(3) Parallel axes are regarded as controlled axes, and their respective speeds are added to the actual

cutting feedrate display. It is possible not to add the speed of a slave axis to the actual cutting

feedrate display (by setting bit 3 (NDFx) of parameter No. 3115 to 1).

(4) To perform circular interpolation or cutter compensation, it is necessary to specify to which basic

coordinate system each axis belongs, using parameter No. 1022. At this time, make the same settings

for parallel axes.

(5) If parallel axis control is used together with feed axis synchronization control, make sure that the

axes subject to feed axis synchronization control have different axis names.

The following shows an example in which parallel axis control is performed on a machine with five axes

X, Y1, Y2, Z1, and Z2.

Number of controlled axes = 5

Axis

Displayed

Axis name

Subscript

Basic coordinate axis setting

Servo axis number

number

axis name

(No. 1020)

(No. 3131)

(No. 1022)

(No. 1023)

1

X

88

0

1

1

2

Y1

89

1

2

2

3

Y2

89

2

2

3

4

Z1

90

1

3

4

5

Z2

90

2

3

5

- 324 -

B-64484EN-2/02

PROGRAMMING

8.AXIS CONTROL FUNCTIONS

Selecting coordinate systems on parallel axes

It is possible to set individual workpiece coordinate system offset values for the controlled axes belonging

to the same program axis. This makes it possible to create a program by considering independent

coordinate systems for the individual controlled axes.

For example, if there are two heads, each of which

have two controlled axes (X and Y), the tool

movement is as shown below.

Mid-point of head 2

Y

Y₁

Reference position

Mid-point of head 1

of head 1

Y

2

(f)

(e)

Current position of

(f)

tool of head 2

(a)

(d)

(a)

(c)

(d)

(c)

(b)

Current position of

(b)

tool of head 1

(e)

Reference position of

Workpiece coordinate system of

X₁

head 2

head 1

Workpiece coordinate system

X₂

Workpiece origin offset of

of head 2

head 1

Workpiece origin offset

of head 2

Origin of machine coordinate system

X

(a)

Movement with an incremental command

(Example) G91 X_ Y_;

(b)

Movement with an absolute command

(Example) G90 X0 Y0;

(c)

Move command with the machine coordinate system

Each axis moves to a single point on the machine coordinate system.

(Example) G90 G53 X_ Y_;

(d)

Automatic reference position return (G28, G30)

Each axis returns to the reference position of its controlled axis individually set with a parameter.

(Example) G91 G28 X0 Y0;

(e)

Reference position return check (G27)

A check is performed to see if each axis has returned to its reference position.

(Example) G91 G27 X0 Y0;

(f)

Automatic return to the reference position (G29)

Each axis is positioned to the position specified via its mid-point.

(Example) G91 G29 X30. Y50.;

Tool length compensation and tool offset on parallel axes

It is possible to set the difference between an H code number and the offset data number selected in

accordance with this number, i.e., bias value, in a parameter for each axis, and perform tool length

compensation on a different tool for each axis. It is also possible to apply an offset in the case of the tool

offset function.

Set the bias value of tool length compensation in parameter No. 10361.

Set the bias amount of tool offset in parameter No. 10360.

- 325 -

8.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64484EN-2/02

Tool of head 1

Tool of head 2

ε₁

ε₂

Programmed

position

Head

Offset number

Bias value

Offset data number

Offset value

Head 1

07

10

17

ε₁

Head 2

07

20

27

ε₂

If parallel operation is to be performed with the third and fourth axes as the Z1- and Z2-axes, let us

assume, for example, that 10 is set in parameter No. 10361 as the bias value for the Z1-axis, and 20 for

the Z2-axis. If a tool length compensation command G43 H07 ; is specified, tool length compensation is

performed by using the offset data number 17 (= 07 + 10) as the offset value for the tool of head 1 and the

offset data number 27 (= 07 + 20) as the offset value for the tool of head 2.

NOTE

The offset value for the offset number 00, i.e., H00, is always 0 regardless of the

bias value.

Travel distances on parallel axes

The travel distances on parallel axes differ as described below depending on whether the command is an

incremental or absolute one.

(1) For an incremental command

•

Rapid traverse and linear interpolation

The travel distances on all parallel axes are the same.

•

Circular interpolation and helical interpolation

The travel distances on all parallel axes are the same.

This means that the same arc is interpolated simultaneously for a multiple number of times.

(2) For an absolute command

•

Rapid traverse and linear interpolation

The end points of all parallel axes are the same.

This means that if the start positions differ, the travel distances on the parallel axes differ.

•

Circular interpolation and helical interpolation

Interpolation is performed using the data for the first un-parked one in the list of controlled

axes, and for the other parallel axes, the same data as that used for interpolation is output.

This means that even if the command is an absolute one, if the start position of a parallel axis differs

from that of the axis the data for which is used for interpolation, the end point differs from the

specified one.

Feedrate calculation

For linear interpolation, the feedrate during parallel operation is calculated by selecting the one of the

parallel axes that has the longest travel distance. The data for the other parallel axes is not reflected in the

calculation of the feedrate.

- 326 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

9 GAS CUTTING MACHINE

Chapter 9, "GAS CUTTING MACHINE", consists of the following sections:

9.1 TOOL OFFSET B

328

9.2 CONER CONTROL BY FEED RATE

331

9.3 AUTOMATIC EXACT STOP CHECK

333

9.4 AXIS SWITCHING

336

9.5 GENTLE CURVE CUTTING

339

9.6 GENTLE NORMAL DIRECTION CONTROL

341

9.1

TOOL OFFSET B

Overview

With the G43H_ or G44H_ command, tool offset not affected by mirror image can be applied.

With the G49 command, tool offset can be canceled without being affected by mirror image.

The offset axes are the first axis and second axis for plane selection.

Format

G43 H_ ; Shifts the coordinate system by an offset value in the + direction.

G44 H_ ; Shifts the coordinate system by an offset value in the - direction.

G49 ; or G43 (or G44) H0 ; Tool offset B cancel

G43 (or G44) : Tool offset in the + (or -) direction

G49 (or H0)

: Tool offset cancel

H＿

:

Tool offset number

(G43,G44,G49: Modal G code)

Explanation

By setting bit 0 (GOB) of parameter No. 5033 to 1 and specifying G43H_; or G44H_;, tool offset not

affected by mirror image can be applied. The difference between the programmed tool position and the

tool position actually used for machining can be corrected using this function without modifying the

program, by setting the difference in the offset memory.

By using the H code, specify the offset memory number where a tool offset value is set.

As shown in Fig. 9.1 (a), eight offset directions are present for each of G43 and G44. Select a direction

with parameter No. 5032.

When G43 is specified

When G44 is specified

2

6

3

1

7

5

Y

4

0

0

4

X

5

７

1

3

6

2

Fig. 9.1 (a)

- 328 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

Offset direction

Value set in parameter No. 5032

G43

G44

0

X+a

X-a

1

X+a Y+a

X-a Y-a

2

Y+a

Y-a

3

X-a Y+a

X+a Y-a

4

X-a

X+a

5

X-a Y-a

X+a Y+a

6

Y-a

Y+a

7

X+a Y-a

X-a Y+a

a:

Offset value set in the offset memory number specified with the H code

By specifying

G49 ;

tool offset can be canceled without being affected by mirror image.

For example, this function can correct the difference between the position of the nozzle of the gas cutting

machine actually used for machining and the position of the marking pen for drawing used to check the

program, without modifying the program.

As in the sample program indicated below, the program need not be modified if the difference between

the position of the nozzle of the gas cutting machine and the position of the marking pen is set as an offset

value in offset number 02, and the optional block skip signal BDTn is set to 1 to perform gas cutting or is

set to 0 to perform marking.

O0001;

:

/G43 H02;

:

/G49;

:

%

NOTE

In a G43, G44, or G49 block, no move command must be specified.

Otherwise, an alarm is issued.

Parameter

#7

#6

#5

#4

#3

#2

#1

#0

5033

GOB

[Input type] Parameter input

[Data type] Bit path

NOTE

When this parameter is set, the power must be turned off before

operation is continued.

#0 GOB The tool offset B function (for a gas cutting machine) is:

0: Disabled.

1: Enabled.

- 329 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

5032

Direction of tool offset B

[Input type] Parameter input

[Data type] Byte path

[Valid data range]

0 to 7

Specify the offset direction of tool offset B (G43, G44).

When G43 is specified

When G44 is specified

2

6

3

1

7

5

Y

4

0

0

4

X

5

７

1

3

6

2

Fig. 9.1 (b)

Offset direction

Value set in parameter No. 5032

G43

G44

0

X+a

X-a

1

X+a Y+a

X-a Y-a

2

Y+a

Y-a

3

X-a Y+a

X+a Y-a

4

X-a

X+a

5

X-a Y-a

X+a Y+a

6

Y-a

Y+a

7

X+a Y-a

X-a Y+a

a:

Offset value set in the offset memory number specified with the H code

Note

• This function is optional. The tool offset B function needs to be specified.

• This function can be used only with the M series.

- 330 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

#3 EDT The function for corner control by feedrate (for a gas cutting machine) is:

0: Disabled.

1: Enabled.

When the feedrate has reduced to the feedrate set in parameter No. 1474, from which the

system regards the number of accumulated pulses as being 0, the next block is executed.

1474

Feedrate regarded as accumulated pulse 0. (corner control by feedrate (for gas cutting machine))

[Input type] Parameter input

[Data type] Real axis

[Unit of data] mm/min,inch/min,deg/min (machine unit)

[Valid data range] 0 to 32767

When a cutting feed block (block A) is followed by another cutting feed block (block B),

execution proceeds to block B if the feedrate in the automatic acceleration/deceleration

circuit for each axis is reduced to the setting of this parameter, and the number of

accumulated pulses in the automatic acceleration/deceleration circuit is assumed to be 0.

This setting is used for corner control by feedrate (for a gas cutting machine).

Note

1)

This function is optional. The function for corner control by feedrate needs to be specified.

2)

This function can be used only with the M series.

3)

If a block for cutting feed is followed by a block specifying a miscellaneous function only or a block

for rapid traverse, machining proceeds to the next block when the number of accumulated pulses has

actually decreased to 0.

4)

When enabling this function by setting bit 3 (EDT) of parameter No. 1403 to 1, set bit 5 (NCI) of

parameter No. 1601 to 1 and check only that the specified feedrate is 0 at deceleration time (delay in

acceleration/deceleration is 0).

5)

If a value other than 0 is specified in parameter No. 1474, the number of accumulated pulses in the

automatic acceleration/deceleration circuit of each axis is assumed to be 0 and machining proceeds

to the next block when the feedrate being decelerated on each axis with the automatic

acceleration/deceleration circuit has decreased to or below the feedrate set in parameter No. 1474. So,

the path at a corner may be round as shown below (Fig. 9.2 (b)).

Y

Programmed path

X

Actual tool center path

Fig. 9.2 (b)

So, when a sharp corner is needed particularly, insert a block such as for dwell (G04) between

successive blocks for cutting feed.

<Example>

G09 G01 X Y

;

G04 X0;

G09 G01 X Y

;

6)

When acceleration/deceleration before interpolation is performed, this function is disabled.

7)

If feed per revolution is specified in one of successive blocks, this function is disabled.

- 332 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

9.3

AUTOMATIC EXACT STOP CHECK

Overview

This function checks the corner inner angle between successive blocks specifying linear interpolation

(G01) or circular interpolation (G02, G03), and performs an exact stop automatically between the blocks

if the angle is equal to or less than the parameter-set critical angle.

Explanation

When successive blocks specify linear interpolation (G01) or circular interpolation (G02, G03) in the

cutting mode (G64), this function checks the corner inner angle between the blocks on the currently

selected plane and determine whether to automatically perform an exact stop. In the figure below, an

exact stop is automatically performed at the end of block A if the corner inner angle θ is equal to or less

than the critical angle set in parameter No. 1496. This operation is equivalent to operation performed

when an exact stop (G09) is specified in block A.

(1)

(2)

A (G01)

A (G01)

θ

B (G01)

θ

B (G03)

(3)

(4)

A (G02)

A (G02)

θ

θ

B (G01)

B (G02)

In the tool radius compensation mode as well, an automatic exact stop check is made for the corner inner

angles of the programmed path. At this time, an exact stop is performed at points A and B in the figure

below. (Point S represents a single-block stop point.)

(1)

A

A (S)

Offset vector

•

•^{B (S)}

•

Post-offset path

Programmed path

θ

θ

- 333 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

(2)

A

A

•

• ^{B (S)}

• S

θ

θ

(3)

A (S)

^A •

•B (S)

•

θ

θ

(4)

A

•

• ^{B (S)}

A (S)

•

θ

θ

(5)

θ

•

A (S)

θ

•

A (S)

If a small block specifies linear interpolation (G01) and also specifies the amounts of movement on the

two axes on the currently selected plane that are less than the value set in parameter No. 1497, the exact

stop check function can be disabled in the block.

When linear interpolation (G01) is performed for A→B→C→D, an automatic exact stop check is made at

point B based on angle θ₁ formed by lines AB and BC and at point C based on angle θ₂ formed by lines

BC and CD. If the amount of movement on each of the two axes (X-axis and Y-axis in the figure below)

in the block for BC is less than the value set in parameter No. 1497, an automatic exact stop check is

made at point C based on angle θ₃ formed by lines AB and CD.

- 334 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

θ3

B

θ1

C

θ2

X

A

G17 plane

Y

D

NOTE

1 If successive small blocks specify a value less than the value set in parameter

No. 1497, the automatic exact stop check function is disabled in the first small

block and enabled in the next block, and this disable/enable cycle is repeated for

the rest.

2 In the cutter compensation mode, the automatic exact stop check function

cannot be disabled by parameter No. 1497.

- 335 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

9.4

AXIS SWITCHING

Overview

The machine axis to be actually used for movement by specifying X, Y, or Z in memory operation, DNC

operation, or MDI operation can be switched by using the setting data (No. 10371) or the switch on the

machine operator’s panel.

As shown in the example below, this function is useful when the coordinates where a workpiece is

actually set are changed from the programmed coordinates.

Switches X-axis command to Y-axis command.

Y

Y

Switches Y-axis command to X-axis command.

Switches Z-axis command to Z-axis command.

X

X

Programmed coordinates

Coordinates where workpiece is set

Explanation

・Axis switching No.

Six types of axis switching are possible as indicated below. The program addresses X, Y, and Z in each

type of axis switching correspond to the actually specified axes x, y, and z.

Programmed address

Axis switching No.

X

Y

Z

0

x

y

z

1

x

z

y

2

y

x

z

3

y

z

x

4

z

x

y

5

z

y

x

The axis switching number 0 means that axis switching is not performed.

・Axis switching specification method

(1) Specification based on the setting data

In the setting data (No. 10371), set an axis switching number (0 to 5).

(2) Specification based on programming

Specify programmable parameter input (G10L52) and set an axis switching number (0 to 5) in the

setting data (No. 10371).

(3) Specification using the switch on the machine operator's panel

For the method of specification, refer to the manual issued by the machine tool builder.

The table below indicates the relationship between specification (including programming) based on

setting data and specification using the switch on the machine operator's panel.

Setting of setting data

Setting of switch on machine

Valid setting

(No. 10371)

operator's panel

1

0

0

Axis switching is disabled.

2

1 to 5

0

Setting data

3

0

1 to 5

Switch on machine operator's panel

- 336 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

Setting of setting data

Setting of switch on machine

Valid setting

(No. 10371)

operator's panel

4

1 to 5

1 to 5

Switch on machine operator's panel

When axis switching is not performed, set both of the setting data and the switch on the machine

operator's panel to 0.

・Cases where axis switching is disabled

Axis switching is disabled when the commands below are specified.

(1) Manual operation

(2) Move command for moving to a particular machine position, command related to machine

coordinates, and command for coordinate system setting

(a) Automatic reference position return

G28, G30

(b) Floating reference position return

G30.1

(c) Return from reference position

G29

When bit 0 (RPC) of parameter No. 10370 is set to 1, axis switching is applied to the G29

command.

(d) Stored stroke check

G22, G23

(e) Coordinate system setting

G92, G68.2, G52

(f) Offset value setting

G10

(g) Dwell

G04

(h) Machine coordinate positioning

G53

(3) Real time custom macro

Example

When a command for axis switching is specified, the command is executed by performing program

interpretation in such a way that an address change is made according to the axis switching number.

Example) When axis switching No. = 4 is specified:

Specified command

:

G00 X100.0 Y200.0 Z300.0;

Axis switching command interpretation

:

G00 X200.0 Y300.0 Z100.0;

- 337 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

NOTE

1 When the same program is used by axis switching, for example, the amount and

direction of movement are changed by axis switching, depending on the start

position and whether incremental or absolute programming is used.

(Example)

When the same start position is used but the direction of movement in

incremental programming is changed by axis switching

Switches X-axis command to Y-axis command.

Switches Y-axis command to X-axis command.

Y

Y

Switches Z-axis command to Z-axis command.

Start position

Start position

Programmed coordinates

X

Coordinates after axis switching

X

2 The hole machining axis in a canned cycle and tool length compensation and the

axis to which tool length compensation is applied can be fixed at the Z-axis by

setting bits 1 (TLB) and 0 (TLC) of parameter No. 5001 and bit 0 (FXY) of

parameter No. 5101. Even in this case, however, if program address Z is

changed to the machine axis x or y by axis switching, the hole machining axis

and the axis to which tool length compensation is applied are also changed to x

or y.

- 338 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

9.5

GENTLE CURVE CUTTING

Overview

If the V-axis is added as an axis parallel with the Y-axis, the V-axis is treated as an axis parallel with the

Y-axis in the gentle curve cutting cancel mode (G13), and a command for the Y-axis alone is assumed to

be specified for the V-axis as well and enables movement also on the V-axis.

In the gentle curve cutting mode (G12), a command for the Y-axis is valid for the Y-axis alone, and a

command for the V-axis is valid for the V-axis alone.

x2

y2

y1

x1

v1

x2

v2

x1

G12 ;

G01 Xx1 Yy1 Vv1 F

;

Xx2 Yy2 Vv2 ;

NOTE

Be sure to specify G12 or G13 in a block specifying no other commands.

Explanation

If the V-axis is added as an axis parallel with the Y-axis, the V-axis is treated as an axis parallel with the

Y-axis in the gentle curve cutting cancel mode (G13), and a command for the Y-axis alone is assumed to

be specified for the V-axis as well and enables movement also on the V-axis. This means that the setting

of an axis parallel with the Y-axis is equivalent to the specification of the same axis name as the Y-axis.

However, the V-axis is treated as a slave of the Y-axis, so that no command may be specified for the

V-axis. If a command is specified for the V-axis, the alarm PS009, “IMPROPER NC-ADDRESS” is

issued. For details of a parallel axis, see the item of parallel axis control.

In the gentle curve cutting mode (G12), a command for the Y-axis is valid for the Y-axis alone, and a

command for the V-axis is valid for the V-axis alone.

G13;

Gentle curve cutting mode cancel

G12;

Gentle curve cutting mode

<Sample program>

Y move amount V move amount

G13;

G91 Y1000.0;

1000

1000

Y500.0;

500

500

G12;

Y35.0V50.0;

35

50

Y40.0V120.0;

40

120

- 339 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

NOTE

1 Be sure to specify G13 or G12 in a block specifying no other commands.

2 Ensure that the axis number of the basic axis is smaller than the axis number of

a parallel axis. Otherwise, no operation is enabled on the V-axis in the G13

mode.

3 If a command is specified for the V-axis in the G13 mode, the alarm PS0009,

“IMPROPER NC-ADDRESS” is issued.

4 In the G12 mode, do not specify circular interpolation (G02/G03).

5 In the G12 mode, be sure to set the G40 (cutter compensation cancel) mode.

Parameter

1022

Setting of each axis in the basic coordinate system

[Input type] Parameter input

[Data type] Byte axis

[Valid data range] 0 to 7

To determine a plane for circular interpolation, cutter compensation, and so forth (G17:

Xp-Yp plane, G18: Zp-Xp plane, G19: Yp-Zp plane) and a

3-dimensional tool

compensation space (XpYpZp), specify which of the basic three axes (X, Y, and Z) is

used for each control axis, or a parallel axis of which basic axis is used for each control

axis.

A basic axis (X, Y, or Z) can be specified only for one control axis.

Two or more control axes can be set as parallel axes for the same basic axis.

Setting

Meaning

0

Rotation axis (Neither the basic three axes nor a parallel axis)

1

X axis of the basic three axes

2

Y axis of the basic three axes

3

Z axis of the basic three axes

5

Axis parallel to the X axis

6

Axis parallel to the Y axis

7

Axis parallel to the Z axis

- 340 -

B-64484EN-2/02

PROGRAMMING

9.GAS CUTTING MACHINE

9.6

GENTLE NORMAL DIRECTION CONTROL

Overview

Gentle normal direction control enables movement on a rotary axis (C-axis) under normal direction

control simultaneously with movement on a linear axis (X/Y-axis). This makes the function applicable to

a gas cutting machine.

Explanation

Gentle normal direction control executes C-axis rotation and X/Y-axis movement at the same time when

the C-axis rotation angle generated by normal direction control is less than the value of parameter No.

5485.

Y

T1

T2

N2

N1

N3

α: Angle set in parameter No. 5485

X

T1: Rotation angle from N1 to N2 (T1＜α)

T2: Rotation angle from N2 to N3 (T2≧α)

Fig. 9.6 (a)

As shown in the Fig. 9.6 (a), when movement in the order of N1, N2, and N3 is specified:

1)

From N1 to N2, because T1 is less than α, the C-axis rotates angle T1 together with the movement of

the X- and Y-axes indicated by N2.

In this case, the movement distance of the C-axis is not included in calculation and the speed on the

XY plane is specified by F. (normal direction control)

2)

From N2 to N3, because T2 is equal to or greater than α, the C-axis rotates angle T2 before

movement of the X- and Y-axes in N3.(gentle normal direction control)

When the angle formed by a line and an arc or the angle formed between arcs is less than the angle set in

parameter No. 5485, the C-axis rotates with the movement of the X- and Y-axes as in the angle formed

between lines.

NOTE

1 When C-axis rotation included in an X/Y-axis move block is performed at the

same time, actual cutting feedrate display in linear interpolation (cutting) mode

shows the feedrate obtained from the following equation:

F’ = F×√(X²+Y²+C²)/√(X²+Y²)

2 The C-axis moves in response to X/Y-axis movement. If the C-axis feedrate

exceeds the maximum cutting speed or rapid traverse rate, however, the C-axis

feedrate is clamped at the maximum cutting speed or rapid traverse rate. The

X/Y-axis feedrate may therefore be different from the specified feedrate.

- 341 -

9.GAS CUTTING MACHINE

PROGRAMMING

B-64484EN-2/02

Limitation

(1) The normal direction control function is required for this function to be used.

(2) If the number of controlled axes including the C-axis exceeds the maximum number of

simultaneously controlled axes, the option for "simultaneously controlled axes expansion" is

required.

(3) F1 digit code cannot be specified.

(4) Restrictions on normal direction control applies to this function as well.

9.6.1

Linear Distance Setting

Explanation

By setting parameter No. 5486 to a travel distance for a block to move until the rotation of a normal

direction axis is completed, the normal direction axis is controlled to start rotation simultaneously with

the command block and terminates it upon completion of movement over the parameter-specified

distance.

This function is valid when the conditions for executing gentle normal direction control for rotating the

normal direction axis simultaneously with the command block are satisfied.

Assuming parameter No. 5486 specifying "a", the normal direction axis rotates an angle of T1 when the

N2 block having started execution reaches distance "a".

When the travel distance of the N2 block is less than or equal to the setting of parameter No. 5486, the

normal direction axis moves that travel distance.

Y

T1

a

T2

N2

N1

N3

X

Fig. 9.6.1 (a)

・Conditions

All of the following conditions must be satisfied for execution of gentle normal direction control:

(1) Gentle normal direction control is valid. (Bit 0 of parameter No. 5484 is set to 1.)

(2) The travel distance of the command block is equal to or more than the setting of parameter No. 5483

maintaining the normal direction angle of the previous block.

(3) The rotation angle calculated under normal direction control is more than the setting of parameter

No. 5482 for rotation of the normal direction control axis.

(4) The rotation angle calculated under normal direction control is less than the setting of parameter No.

5485 for rotation under gentle normal direction control.

This function rotates the normal direction axis according to the travel distance specified by parameter No.

5486 when the travel distance of the command block is more than the setting of parameter No. 5486 while

the conditions for execution of gentle normal direction control are satisfied.

- 342 -

B-64484EN-2/02

OPERATION

1.SETTING AND DISPLAYING DATA

1 SETTING AND DISPLAYING DATA

Chapter 1, "SETTING AND DISPLAYING DATA", consists of the following sections:

1.1 SCREENS DISPLAYED BY FUNCTION KEY

..................................................................347

1.1.1 Setting and Displaying the Tool Compensation Value

347

1.1.2 Tool Length Measurement

352

1.1.3 Tool Length/Workpiece Origin Measurement

355

1.1.4 Setting and Displaying the Rotary Table Dynamic Fixture Offset

374

1.1.5 Input of Tool Offset Value Measured B

377

1.1.6 Spindle Unit Compensation, Nutating Rotary Head Tool Length Compensation

377

SCREENS DISPLAYED BY FUNCTION KEY

1.1

Press function key

to display or set tool compensation values and other data.

This section describes how to display or set the following data:

1.

Tool compensation value

2.

Tool length measurement

3.

Tool length/workpiece origin measurement

4.

Rotary table dynamic fixture offset

5.

Tool offset value

6.

Spindle unit compensation, nutating rotary head tool length compensation

1.1.1

Setting and Displaying the Tool Compensation Value

Tool offset values, tool length compensation values, and cutter compensation values are specified by D

codes or H codes in a program. Compensation values corresponding to D codes or H codes are displayed

or set on the screen.

Procedure for setting and displaying the tool compensation value (for 8.4/10.4-inch

display unit)

Procedure

1

Press function key

For the two-path control, select the path for which tool compensation values are to be displayed with

the tool post selection switch.

2

Press chapter selection soft key [OFFSET] or press function key

several times until the tool

compensation screen is displayed.

The screen varies according to the type of tool compensation memory.

- 347 -

1.SETTING AND DISPLAYING DATA OPERATION

B-64484EN-2/02

Fig. 1.1.1 (a) Tool compensation memory A (10.4-inch display unit)

Fig. 1.1.1 (b) Tool compensation memory B (10.4-inch display unit)

- 348 -

B-64484EN-2/02

OPERATION

1.SETTING AND DISPLAYING DATA

Fig. 1.1.1 (c) Tool compensation memory C (10.4-inch display unit)

If the cutting point command option is enabled, press the MDI key

several times on the tool

compensation memory C screen, the corner R offset setting screen is displayed.

Fig. 1.1.1 (d) Screen used for the cutting point command (10.4-inch display unit)

3

Move the cursor to the compensation value to be set or changed using page keys and cursor keys, or

enter the compensation number for the compensation value to be set or changed and press soft key

[NO.SRH].

4

To set a compensation value, enter a value and press soft key [INPUT].

To change the compensation value, enter a value to add to the current value (a negative value to

reduce the current value) and press soft key [+INPUT]. Or, enter a new value and press soft key

[INPUT].

- 349 -

1.SETTING AND DISPLAYING DATA OPERATION

B-64484EN-2/02

Procedure for setting and displaying the tool compensation value (for 15/19-inch

display unit)

Procedure

1

Press function key

For the two-path control, select the path for which tool compensation values are to be displayed with

the tool post selection switch.

2

Press the chapter selection key, in Fig.1.1.1 (e) Tool compensation memory A (15-inch display unit),

vertical soft key [OFFSET].

Or, press function key

several times until the tool compensation screen is displayed.

The screen varies according to the type of tool compensation memory.

Fig.1.1.1 (e) Tool compensation memory A (15-inch display unit)

Fig. 1.1.1 (f) Tool compensation memory B (15-inch display unit)

- 350 -

B-64484EN-2/02

OPERATION

1.SETTING AND DISPLAYING DATA

Fig. 1.1.1 (g) Tool compensation memory C (15-inch display unit)

Fig. 1.1.1 (h) Screen used for the cutting point command (15-inch display unit)

3

Move the cursor to the compensation value to be set or changed using page keys and cursor keys, or

enter the compensation number for the compensation value to be set or changed and press horizontal

soft key [NO.SRH].

4

To set a compensation value, enter a value and press horizontal soft key [INPUT].

To change the compensation value, enter a value to add to the current value (a negative value to

reduce the current value) and press horizontal soft key [+INPUT]. Or, enter a new value and press

horizontal soft key [INPUT].

Explanation

-

Decimal point input

A decimal point can be used when entering a compensation value.

- 351 -

B-64484EN-2/02

OPERATION

1.SETTING AND DISPLAYING DATA

Fig. 1.1.2 (a) Current position display screen (10.4-inch display unit)

3

Reset the relative coordinate for the Z-axis to 0.

4

Press function key

several times until the tool compensation screen is displayed.

5

Use manual operation to move the tool to be measured until it touches the same specified position.

The difference between the length of the reference tool and the tool to be measured is displayed in

the relative coordinates on the screen.

6

Move the cursor to the compensation number for the target tool (the cursor can be moved in the

same way as for setting tool compensation values).

7

Press the address key

. If either

or

key is depressed instead of

key, the X or

Y axis relative coordinate value is input as an tool length compensation value.

8

Press the soft key [INP.C.]. The Z axis relative coordinate value is input and displayed as an tool

length compensation value.

Reference

tool

The difference is set as a tool

length offset value

A prefixed position

Procedure for tool length measurement (for 15/19-inch display unit)

1

Use manual operation to move the reference tool until it touches the specified position on the

machine (or workpiece.)

2

Press function key

to display the overall position display screen.

- 353 -

1.SETTING AND DISPLAYING DATA OPERATION

B-64484EN-2/02

Fig. 1.1.2 (b) Current position display screen (15-inch display unit)

3

Reset the relative coordinate for the Z-axis to 0.

4

Press function key

several times until the tool compensation screen is displayed.

5

Use manual operation to move the tool to be measured until it touches the same specified position.

The difference between the length of the reference tool and the tool to be measured is displayed in

the relative coordinates on the screen.

6

Move the cursor to the compensation number for the target tool (the cursor can be moved in the

same way as for setting tool compensation values).

7

Press the address key

. If either

or

key is depressed instead of

key, the X or

Y axis relative coordinate value is input as an tool length compensation value.

8

Press the horizontal soft key [INP.C.]. The Z axis relative coordinate value is input and displayed as

an tool length compensation value.

Reference

tool

The difference is set as a tool

length offset value

A prefixed position

- 354 -

Content      ..     10      11      12      13     ..