Content      ..     25      26      27      28     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 27

3. MANUAL OPERATION

OPERATION

B-63534EN/02

Restrictions

D Number of MPGs

Up to three manual pulse generators can be connected, one for each axis.

The three manual pulse generators can be simultaneously operated.

WARNING

Rotating the handle quickly with a large magnification such

as x100 moves the tool too fast. The feedrate is clamped

at the rapid traverse feedrate.

NOTE

Rotate the manual pulse generator at a rate of five rotations

per second or lower. If the manual pulse generator is

rotated at a rate higher than five rotations per second, the

tool may not stop immediately after the handle is no longer

rotated or the distance the tool moves may not match the

graduations on the manual pulse generator.

760

B-63534EN/02

OPERATION

3. MANUAL OPERATION

3.5

Whether the distance the tool is moved by manual operation is added to

the coordinates can be selected by turning the manual absolute switch on

MANUAL ABSOLUTE

or off on the machine operator’s panel. When the switch is turned on, the

ON AND OFF

distance the tool is moved by manual operation is added to the

coordinates. When the switch is turned off, the distance the tool is moved

by manual operation is not added to the coordinates.

Y axis

P2

Manual operation

P1

X axis

O

The coordinates values change by the amount of manual operation.

Fig. 3.5 (a) Coordinates with the switch ON

Y2

Y1

P2

O2

P1

X2

X1

O1

The coordinates do not change.

Fig. 3.5 (b) Coordinates with the switch OFF

761

3. MANUAL OPERATION

OPERATION

B-63534EN/02

Explanation

The following describes the relation between manual operation and

coordinates when the manual absolute switch is turned on or off, using a

program example.

G01G90

X100.0Y100.0F010

;

X200.0Y150.0

;

X300.0Y200.0

;

The subsequent figures use the following notation:

Movement of the tool when the switch is on

Movement of the tool when the switch is off

The coordinates after manual operation include the distance the tool is

moved by the manual operation. When the switch is off, therefore, subtract

the distance the tool is moved by the manual operation.

D Manual operation after

Coordinates when block

has been executed after manual operation

the end of block

(X-axis +20.0, Y-axis +100.0) at the end of movement of block.

Y

(220.0 , 250.0)

(120.0 , 200.0)

Manual

(200.0 , 150.0)

Switch ON

operation

Switch OFF

(100.0 , 100.0)

X

D Manual operation after a

Coordinates when the feed hold button is pressed while block

is being

feed hold

executed, manual operation (Y-axis + 75.0) is performed, and the cycle

start button is pressed and released.

Y

(300.0 , 275.0)

(200.0 , 225.0)

(150.0 , 200.0)

Manual

operation

(200.0 , 150.0)

(300.0 , 200.0)

(150.0 , 125.0)

X

Switch ON

Switch OFF

762

B-63534EN/02

OPERATION

3. MANUAL OPERATION

D When reset after a

Coordinates when the feed hold button is pressed while block

is being

manual operation

executed, manual operation (Y-axis +75.0) is performed, the control unit

following a feed hold

is reset with the RESET button, and block

is read again

Y

(300.0 , 275.0)

(200.0,225.0)

(150.0 , 200.0)

Manual

(300.0 , 200.0)

operation

(200.0,150.0)

(100.0 , 100.0)

(150.0 , 125.0)

Switch ON

X

Switch OFF

D When a movement

When there is only one axis in the following command, only the

command in the next

commanded axis returns.

block is only one axis

N1G01X100.0Y100.0F500;

Y

N2X200.0;

(200.0 , 150.0)

N3Y150.0;

Manual

operation

N3

Switch ON

N2

(200.0 , 100.0)

Switch OFF

N1

(100.0 , 100.0)

X

D When the next move

When the following commands are incremental commands, operation is

block is an incremental

the same as when the switch is OFF.

D Manual operation during

cutter compensation

When the switch is OFF

After manual operation is performed with the switch OFF during cutter

compensation, automatic operation is restarted then the tool moves

parallel to the movement that would have been performed if manual

movement had not been performed. The amount of separation equals to

the amount that was performed manually.

Cutter path after

manualoperation

Manual

operation

Cutter path

Programmed path

763

3. MANUAL OPERATION

OPERATION

B-63534EN/02

When the switch is ON during cutter compensation

Operation of the machine upon return to automatic operation after manual

intervention with the switch is ON during execution with an absolute

command program in the cutter compensation mode will be described.

The vector created from the remaining part of the current block and the

beginning of the next block is shifted in parallel. A new vector is created

based on the next block, the block following the next block and the

amount of manual movement. This also applies when manual operation

is performed during cornering.

Manual operation performed in other than cornering

Assume that the feed hold was applied at point P_H while moving from P_A

to P_B of programmed path P_A, P_B, and P_C and that the tool was manually

moved to P_H’. The block end point P_B moves to the point P_B’ by the

amount of manual movement, and vectors V_B1 and V_B2 at P_B also move

to V_B1’ and V_B2’. Vectors V_C1 and V_C2 between the next two blocks P_B

- P_C and P_C - P_D are discarded and new vectors V_C1’ and V_C2’ (V_C2’ =

V_C2 in this example) are produced from the relation between P_B’ - P_C and

P_C - P_D. However, since V_B2’ is not a newly calculated vector, correct

offset is not performed at block P_B’ - P_C. Offset is correctly performed

after P_C.

V_C1’

V_B2

V_C1

V_B1

P_B

P_C

V_C2

V_B2’

P_D

Programmed path

V_B1’

(absolute command)

PA

Cutter path after

P’

B

P

H

manual operation

Cutter path before

manual operation

Manual operation

P_H’

764

B-63534EN/02

OPERATION

3. MANUAL OPERATION

Manual operation during cornering

This is an example when manual operation is performed during cornering.

VA2’, VB1’, and VB2’ are vectors moved in parallel with VA2, VB1 and VB2

by the amount of manual movement. The new vectors are calculated

from V_C1 and V_C2. Then correct cutter compensation is performed for the

blocks following Pc.

V_C1’

V_B2

V_C1

V_B1

P_B

P_C

V_C2

V_B2’

V_B1’

Programmed path

(absolute command)

Cutter path after

PA

manual operation

Cutter path before

manual operation

VA2

VA1

P_H

PA’

Manual operation

VA2’

V

A1’

P_H’

Manual operation after single block stop

Manual operation was performed when execution of a block was

terminated by single block stop.

Vectors V_B1 and V_B2 are shifted by the amount of manual operation.

Sub-sequent processing is the same as case a described above. An MDI

operation can also be interveneted as well as manual operation. The

movement is the same as that by manual operation.

Cutter path after

V_C1’

manual operation

V_B2

V_C1

V_B1

P_B

P_C

V_C2

Manual

operation

V_B2’

Programmed path

V_B1’

P_B’

(absolute command)

P^A Cutter path before

manual operation

765

3. MANUAL OPERATION

OPERATION

B-63534EN/02

3.6

Tool axis direction handle feed moves the tool over a specified distance

by handle feed in the direction of the tool axis tilted by the rotation of the

TOOL AXIS

rotary axis.

DIRECTION HANDLE

FEED/TOOL AXIS

Tool axis direction handle feed B has the function of tool axis direction

handle feed, and also has the tool axis normal direction handle feed which

DIRECTION HANDLE

is handle feed at right angles to the tool axis.

FEED B

These functions are used, for example, with 5-axis engraving machines.

3.6.1

When the tool axis direction handle mode is selected and the manual pulse

generator is rotated, the tool is moved by the specified travel distance in

Tool Axis Direction

the direction of the tool axis tilted by the rotation of the rotary axis.

Handle Feed

A&C,

B&C

Tool Axis Normal Direction Handle Feed

Procedure

1

Select the HANDLE switch from the mode selection switches.

2

Select the tool axis direction handle feed switch.

MODE

EDIT

MEMORY

REMOTE

MDI

3

Select the tool axis direction handle feed mode axis as the handle feed

axis for the first manual pulse coder (parameter No. 7121).

ZERO

ÂÂ

HANDLE

JOG

TEACH

RETURN

ÂÂ

4

When the handle is turned, the tool moves in the tool axis direction by

the corresponding distance.

When both the tool axis direction handle feed mode and tool axis

right-angle direction handle feed mode are selected, neither mode is

set, but the ordinary handle mode is set.

The procedure above is only an example. Refer to the relevant manual

published by the machine tool builder for other possible operations.

766

B-63534EN/02

OPERATION

3. MANUAL OPERATION

Explanations

D Axis configuration

Assume that the rotary axes for basic axes X, Y, and Z are A, B, and C,

respectively. Assume also that the Z-axis represents the tool axis.

Depending on the axis configuration of the machine, four types of tool

axis directions are available. Specify the direction with parameter No.

7120.

(1) A-C axis type

(2) B-C axis type

Z (tool axis)

Z (tool axis)

C

C

B

A

Y

X

Y

X

(3) A-B axis (A-axis master) type

(4) A-B axis (B-axis master) type

Z (tool axis)

Z (tool axis)

B

B

A

A

X

Y

X

Y

D Pulse distribution to

The figure below shows handle pulse (Hp) distribution to the X-axis,

basic axes

Y-axis, and Z-axis for each of the four directions.

(1) A-C axis type

Xp = Hp

sin (a)

sin (c)

Yp = -Hp

sin (a)

cos (c)

Zp = Hp

cos (a)

Z

a

Zp

Hp

a

c

Xp

Yp

Y

X

Hpxy

767

3. MANUAL OPERATION

OPERATION

B-63534EN/02

(2) B-C axis type

Z

Xp = Hp sin (b) cos (c)

Yp = Hp sin (b) sin (c)

Zp = Hp cos (b)

b

Zp

Hp

X

b

C

Yp

Y

Xp

Hpxy

(3) A-B axis (A axis master) type

Z

Xp = Hp sin (b)

Yp = -Hp cos (b) sin (a)

Zp = Hp cos (b) cos (a)

a

Zp

b

Yp

Y

X

Xp

(4)A-B axis (B axis master) type

Xp = Hp cos (a) sin (b)

Yp = -Hp sin (a)

Z

Zp = Hp cos (a) cos (b)

b

a

Zp

Y

Yp

Xp

X

768

B-63534EN/02

OPERATION

3. MANUAL OPERATION

In the figures above, a, b, and c represent the positions (angles) of the

A-axis, B-axis, and C-axis from the machine zero point; those values

present when the tool axis direction handle feed mode is set or a reset

occurs are used. To change the feed direction, reenter the tool axis

direction handle feed mode, or press the reset key.

For tool axis direction determination, the coordinates (rotation angles) of

rotary axes can be set using bits 3 and 4 (3D1X and 3D2X) of parameter

No. 7104, and parameter Nos. 7144 and 7145.

D Setting basic axes and

Basic axes X, Y, and Z are determined by parameter No. 1022 (plane

rotary axes

selection). Rotary axes A, B, and C are determined by parameter No.

1020 (axis name).

D Tool axis direction

The direction of the tool X axis is determined by setting bit 0 (TLX) of

parameter No. 7104.

D Setting for 4-axis

This function is usually used with 5-axis machines. However, 4-axis

machines

machines (One axis is for rotation) can be used by setting bit 2 (CXC) of

parameter No. 7104 to 1.

Restrictions

D Axis configuration

If either of the two axes selected in type specification based on the axis

configuration is nonexistent as an axis, P/S alarm No. 5015 is issued.

3.6.2

When the tool axis normal direction handle mode is selected and the

manual pulse generator is rotated, the tool is moved by the specified travel

Tool Axis Normal

distance in the direction normal to the tool axis tilted by the rotation of

Direction Handle Feed

the rotary axis.

A- and C-axes

B- and C-axes

Center of rotation

Tool

Z

A&C , B&C

C

Transverse direction

of the tool (X-axis)

Longitudinal direction

of the tool

Y

B

Transverse direction

A

of the tool (Y-axis)

X

Workpiece

769

3. MANUAL OPERATION

OPERATION

B-63534EN/02

Tool Axis Direction Handle Feed

Procedure

1

Select the HANDLE switch from the mode selection switches.

2

Select the tool axis normal direction handle feed switch.

MODE

EDIT

MEMORY

REMOTE

MDI

3

Select the tool axis direction handle feed mode axis as the handle feed

axis for the first manual pulse coder (parameter No. 7141, No. 7142).

HANDLE

JOG

ZERO

TEACH

RETURN

4

When the handle is turned, the tool moves in normal direction to the

ÂÂ

tool axis direction by the corresponding distance.

When both the tool axis direction handle feed mode and tool axis

right-angle direction handle feed mode are selected, neither mode is

set, but the ordinary handle mode is set.

The procedure above is only an example. Refer to the relevant manual

published by the machine tool builder for other possible operations.

Explanations

D Axis configuration

Assume that the rotary axes for basic axes X, Y, and Z are A, B, and C,

respectively. Assume also that the Z-axis represents the tool axis.

Depending on the axis configuration of the machine, two types of tool axis

directions in which X-axis direction and Y-axis direction are available.

Specify the direction with parameter No. 7120.

(1) A-C axis type

(2) B-C axis type

Z (tool axis)

Z (tool axis)

C

C

B

A

Y

X

Y

X

770

B-63534EN/02

OPERATION

3. MANUAL OPERATION

D Pulse distribution to

The figure below shows handle pulse (Hp) distribution to the X-axis,

basic axes

Y-axis, and Z-axis for each of the four directions.

(1) A-C axis type (X-axis direction)

Xp = Hp COS (C)

Yp = Hp SIN (C)

Zp = 0

0

Y

C

The XY plane is drawn be-

cause A- and C-axes are spe-

C

0’

Yp

cified and because rotation

about the A-axis, which is on

the X-axis, does not cause the

tool to rotate about the X-axis

at the tool tip. Suppose that

C

Hp(X direction)

the Z-axis on this side of the

Xp

XY plane is positive.

X’

X

(2) A-C axis type (Y-axis direction)

Xp = -Hp COS (A) SIN (C)

Yp = Hp COS (A) COS (C)

Zp = Hp SIN (A)

Z

Hp (Y direction)

Hpxy

Zp

A

Yp

Xp

0

C

X

Y

771

3. MANUAL OPERATION

OPERATION

B-63534EN/02

(3) B-C axis type (X-axis direction)

Xp = Hp COS (B) COS (C)

Yp = Hp COS (B) SIN (C)

Zp = -Hp SIN (B)

Z

Xp

0’

Zp

Hp

X

(X direction)

B

C

X’

C

Yp

0

Hpxy

Y

(4)

B-C axis type (Y-axis direction)

Xp = -Hp SIN (C)

Yp = Hp COS (C)

Zp = 0

0

X

C

The XY plane is drawn be-

cause B- and C-axes are

specified and because rota-

Xp

tion about the B-axis, which is

on the Y-axis, does not cause

0’

the tool to rotate about the Y-

axis at the tool tip. Suppose

that the Z-axis on this side of

the XY plane is positive.

Yp

C Hp(Y direction)

Y’

Y

In the figures above, a, b, and c represent the positions (angles) of the

A-axis, B-axis, and C-axis from the machine zero point; those values

present when the tool axis direction handle feed mode is set or a reset

occurs are used. To change the feed direction, reenter the tool axis

direction handle feed mode, or press the reset key.

For tool axis direction determination, the coordinates (rotation angles) of

rotary axes can be set using bits 3 and 4 (3D1X and 3D2X) of parameter

No. 7104, and parameter Nos. 7144 and 7145.

772

3. MANUAL OPERATION

OPERATION

B-63534EN/02

3.7

In manual handle feed or jog feed, the following types of feed operations

are enabled in addition to the conventional feed operation along a

MANUAL

specified single axis (X-axis, Y-axis, Z-axis, and so forth) based on

LINEAR/CIRCULAR

simultaneous 1-axis control:

INTERPOLATION

D Feed along a tilted straight line in the XY plane (linear feed) based on

simultaneous 2-axis control

D Feed along a circle in the XY plane (circular feed) based on

simultaneous 2-axis control

Y

Y

Workpiece

Workpiece

Tool

Tool

X

X

<<Linear feed>>

<<Circular feed>>

NOTE

The X-axis and Y-axis must be the first controlled axis and second controlled axis,

respectively.

Procedure for Manual Linear/Circular Interpolation

Procedure

1

To perform manual handle feed, select manual handle feed mode. To

perform jog feed, select jog feed mode.

2

To perform manual handle feed, select a feed axis (for simultaneous

1-axis feed along the X-axis, Y-axis, or Z-axis, or for simultaneous

linear or circular 2-axis feed along a specified straight line or circle in

the XY plane) subject to manual handle feed operation. Use the

handle feed axis select switch for this selection.

To perform jog feed, select a feed axis and direction with the feed axis

direction select switch. While a feed axis and its direction are

specified, the tool moves in the specified axis direction or along a

straight line or circle at the jog feedrate specified in parameter No.

1423.

3

For manual handle feed

The tool is moved along a specified axis by turning the respective

manual handle. The feedrate depends on the speed at which the

manual handle is turned. A distance to be traveled by the tool when

the manual handle is turned by one pulse can be selected using the

manual handle feed travel distance magnification switch.

774

B-63534EN/02

OPERATION

3. MANUAL OPERATION

For jog feed

The feedrate can be overridden using the manual feedrate override

dial.

The procedure above is just an example. For actual operations, refer

to the relevant manual provided by the machine tool builder.

Explanations

D Definition of a straight

For feed along an axis, no straight line/circle definition is required. For

line/circle

linear feed or circular feed, a straight line or circle must be defined

beforehand. (For circular feed, for example, data such as a radius and the

center of a circle must be set.) For details, refer to the relevant manual

provided by the machine tool builder.

D Manual handle feed

In manual handle feed, the tool can be moved along a specified axis

(X-axis, Y-axis, Z-axis, ..., or the 8th axis), or can be moved along a

tilted straight line (linear feed) or a circle (circular feed).

(1) Feed along a specified axis (simultaneous 1-axis control)

By turning a manual handle, the tool can be moved along the desired

axis (such as X-axis, Y-axis, and Z-axis) on a simultaneous 1-axis

control basis. (This mode of feed is the conventional type of manual

handle feed.)

Y

Path of travel using the Y-axis handle

Path of travel using the X-axis handle

X

Feed along a specified axis

775

3. MANUAL OPERATION

OPERATION

B-63534EN/02

(2) Linear feed (simultaneous 2-axis control)

By turning a manual handle, the tool can be moved along the straight

line parallel to a specified straight line on a simultaneous 2-axis

control basis. This manual handle is referred to as the guidance handle.

Moreover, by turning another manual handle, the tool can be moved

at right angles to a specified straight line on a simultaneous 2-axis

control basis. This manual handle is referred to as the approach

handle. When the guidance handle or approach handle is turned

clockwise or counterclockwise, the tool travels forward or backward

along the respective path.

Y

Path of travel using

the approach handle

Tool

Specified straight line

Path of travel using the

guidance handle

X

Linear feed

(3) Circular feed (simultaneous 2-axis control)

By turning a manual handle, the tool can be moved from the current

position along the concentric circle that has the same center as a

specified circle on a simultaneous 2-axis control basis. This manual

handle is referred to as the guidance handle. Moreover, by turning

another manual handle, the tool can be moved along the normal to a

specified circle on a simultaneous 2-axis control basis. This manual

handle is referred to as the approach handle. When the guidance

handle or approach handle is turned clockwise or counterclockwise,

the tool travels forward or backward along the respective path.

Y

Path of travel using the

approach handle

Specified circle

Path of travel using the

guidance handle

X

Circular feed

Feedrate

776

B-63534EN/02

OPERATION

3. MANUAL OPERATION

3.8

For execution of rigid tapping, set rigid mode, then switch to handle mode

and move the tapping axis with a manual handle. For more information

MANUAL RIGID

about rigid tapping, see Section II-13.2 and refer to the relevant manual

TAPPING

provided by the machine tool builder.

Procedure for Manual Rigid Tapping

Procedure

1

Stop the spindle and servo axes, then set MDI mode by pressing the

MDI switch among the mode selection switches.

2

Enter and execute the following program:

M29 S1000 ;

G91 G84 Z0 F1000 ;

The program above is required to determine a screw lead and set rigid

tapping mode. In this program, a tapping axis must always be

specified. Specify a value that does not operate the tapping axis.

WARNING

In this MDI programming, never specify commands to

position the tool at a drilling position and at point R.

Otherwise, the tool moves along an axis.

3

When the entered program is executed, rigid tapping mode is set.

4

After rigid mode is set upon completion of MDI program execution,

switch to the handle mode by pressing the handle switch among the

mode selection switches.

CAUTION

At this time, never press the reset key. Otherwise, rigid

mode is canceled.

5

To perform rigid tapping, select a tapping axis with the handle feed

axis select switch, and move the tapping axis with the manual handle.

779

B-63534EN/02

OPERATION

3. MANUAL OPERATION

3.9

The manual numeric command function allows data programmed

through the MDI to be executed in jog mode. Whenever the system is

MANUAL NUMERIC

ready for jog feed, a manual numeric command can be executed. The

COMMAND

following eight functions are supported:

(1) Positioning (G00)

(2) Linear interpolation (G01)

(3) Automatic reference position return (G28)

(4)2nd/3rd/4th reference position return (G30)

(5) M codes (miscellaneous functions)

(6) S codes (spindle functions)

(7) T codes (tool functions)

(8) B codes (second auxiliary functions)

By setting the following parameters, the commands for axial motion and

the M, S, T, and B functions can be disabled:

(1) Positioning (G00):

(2) Linear interpolation (G01):

Bit 0 (JAXx) of

(3) Automatic reference position return (G28): . .

parameter No. 7010

(4)2nd/3rd/4th reference position return (G30): .

(5) M codes (miscellaneous functions):

. . . . . . . . . . . . . . . . . . . . . . . . . . . Bit 0 (JMF) of parameter No. 7002

(6) S codes (spindle functions):

Bit 1 (JSF) of parameter No. 7002

(7) T codes (tool functions):

Bit 2 (JSF) of parameter No. 7002

(8) B codes (second auxiliary functions):

. . . . . . . . . . . . . . . . . . . . . . . . . . . Bit 3 (JBF) of parameter No. 7002

Procedure

Manual numeric command

Procedure

1

Press the jog switch (one of the mode selection switches).

2

Press function key

PROG

MODE

3

Press soft key [JOG] on the screen. The following manual numeric

EDIT

MEMORY

REMOTE

MDI

command screen is displayed.

HANDLE

TEACH

Example 1: When the maximum number of controlled axes is six

JOG

ZERO

RETURN

PROGRAM (JOG)

O0010 N00020

G00 P

(ABSOLUTE)

(DISTANCE TO GO)

X

X

0.000

X

0.000

Y

Y

0.000

Y

0.000

Z

Z

0.000

Z

0.000

U

U

0.000

U

0.000

V

V

0.000

V

0.000

W

W

0.000

W

0.000

M

S

T

B

>_

JOG

* * * *

* * *

* * *

00 : 00 : 00

PRGRM

JOG

CURRNT

NEXT

(OPRT)

781

3. MANUAL OPERATION

OPERATION

B-63534EN/02

Example 2: When the maximum number of controlled axes is 7 or 8

PROGRAM (JOG)

O0010 N00020

G00 P

(ABSOLUTE)

(DISTANCE TO GO)

X

X

0.000

X

0.000

Y

Y

0.000

Y

0.000

Z

Z

0.000

Z

0.000

U

U

0.000

U

0.000

V

V

0.000

V

0.000

W

W

0.000

W

0.000

A

A

0.000

A

0.000

C

C

0.000

C

0.000

M T

S

B

>_

JOG

* * * *

* * *

* * *

00 : 00 : 00

PRGRM

JOG

CURRNT

NEXT

(OPRT)

4

Enter the required commands by using address keys and numeric keys

on the MDI panel, then press soft key [INPUT] or the

INPUT

key to set

the entered data.

PROGRAM (JOG)

O0010 N00020

G00 P

(ABSOLUTE)

(DISTANCE TO GO)

X

10.000

X

0.000

X

0.000

Y

Y

0.000

Y

0.000

Z

Z

0.000

Z

0.000

U

U

0.000

U

0.000

V

V

0.000

V

0.000

W

W

0.000

W

0.000

M

S

T

B

>Z120.5_

JOG

* * * *

* * *

* * *

00 : 00 : 00

CLEAR

INPUT

The following data can be set:

1. G00: Positioning

2. G01: Linear interpolation

3. G28: Automatic reference position return

4. G30: 2nd/3rd/4th reference position return

5. M codes: Miscellaneous functions

6. S codes: Spindle functions

7. T codes: Tool functions

8. B codes: Second auxiliary functions

The set data is maintained even when the screen or mode is changed.

782

B-63534EN/02

OPERATION

3. MANUAL OPERATION

NOTE

When an alarm state exists, data cannot be set.

5

Press the cycle start switch on the machine operator’s panel to start

command execution. The status is indicated as ”MSTR.” (When the

9” screen is being used, the actual feedrate ”ACT.F” and spindle

speed ”SACT” appear on the key input line.) The automatic operation

signal, STL, can be turned on by setting bit 2 (JST) of parameter No.

7001.

~

~

ACT.F

1000 SACT

0

JOG MSTR *** MTN

00 : 00 : 00

~

~

NOTE

If the cycle start switch is pressed while an alarm state

exists, a ”START IMPOSSIBLE” warning is generated, and

the entered data cannot be executed.

6

Upon the completion of execution, the ”MSTR” status indication is

cleared from the screen, and automatic operation signal STL is turned

off. The set data is cleared entirely. G codes are set to G00 or G01

according to the setting of bit 0 (G01) of parameter No. 3402.

Explanations

D Positioning

An amount of travel is given as a numeric value, preceded by an address

such as X, Y, or Z. This is always regarded as being an incremental

command, regardless of whether G90 or G91 is specified.

The tool moves along each axis independently at the rapid traverse rate.

Linear interpolation type positioning (where the tool path is linear) can

also be performed by setting bit 1 (LRP) of parameter No. 1401.

Manual rapid traverse selection switch

Off

On

Rapid traverse rate for each

Feedrate

Jog feedrate for each axis

axis

(parameter)

(No. 1423)

(No. 1420)

Automatic

Exponential acceleration/

Linear acceleration/

acceleration/

deceleration in jog feed for

deceleration in rapid traverse

deceleration

each axis

for each axis

(parameter)

(No. 1624)

(No. 1620)

Override

Manual feed override

Rapid traverse override

783

3. MANUAL OPERATION

OPERATION

B-63534EN/02

NOTE

When the manual rapid traverse selection switch is set to

the OFF position, the jog feedrate for each axis is clamped

such that a parameter-set feedrate, determined by bit 1

(LRP) of parameter No. 1401 as shown below, is not

exceeded.

LRP = 0: Manual rapid traverse rate for each axis

(parameter No. 1424)

LRP = 1: Rapid traverse rate for each axis

(parameter No. 1420)

D Linear interpolation

An amount of travel is given as a numeric value, preceded by an address

(G01)

such as X, Y, or Z. This is always regarded as being an incremental

command, regardless of whether G90 or G91 is specified. Axial

movements are always performed in incremental mode even during

scaling or polar coordinate interpolation. In addition, movement is

always performed in feed per minute mode regardless of the specification

of G94 or G95.

Feedrate

Dry run feedrate

(parameter)

(No. 1410)

Exponential acceleration/deceleration

Automatic acceleration/deceleration

in cutting feed for each axis

(parameter)

(No. 1622)

Override

Manual feed override

NOTE

Since the feedrate is always set to the dry run feedrate,

regardless of the setting of the dry run switch, the feedrate

cannot be specified using F. The feedrate is clamped such

that the maximum cutting feedrate, set in parameter No.

1422, is not exceeded.

D Automatic reference

The tool returns directly to the reference position without passing through

position return (G28)

any intermediate points, regardless of the specified amount of travel. For

axes for which no move command is specified, however, a return

operation is not performed.

Feedrate

Rapid traverse rate

(parameter)

(No. 1420)

Linear acceleration/deceleration in

Automatic acceleration/deceleration

rapid traverse for each axis

(parameter)

(No. 1620)

Override

Rapid traverse override

784

B-63534EN/02

OPERATION

3. MANUAL OPERATION

D 2nd, 3rd, or 4th reference

The tool returns directly to the 2nd, 3rd, or 4th reference position without

position return (G30)

passing through any intermediate points, regardless of the specified

amount of travel. To select a reference position, specify P2, P3, or P4 in

address P. If address P is omitted, a return to the second reference position

is performed.

Feedrate

Rapid traverse rate for each axis

(parameter)

(No. 1420)

Linear acceleration/deceleration in

Automatic acceleration/deceleration

rapid traverse for each axis

(parameter)

(No. 1620)

Override

Rapid traverse override

NOTE

The function for 3rd/4th reference position return is optional.

⋅ When the option is not selected

Return to the 2nd reference position is performed,

regardless of the specification of address P.

⋅ When the option is selected

If neither P2, P3, nor P4 is specified in address P, a

”START IMPOSSIBLE” warning is generated, and the

entered data cannot be executed.

D M codes (miscellaneous

After address M, specify a numeric value of no more than the number of

functions)

digits specified by parameter No. 3030. When M98 or M99 is specified,

it is executed but not output to the PMC.

NOTE

Neither subprogram calls nor custom macro calls can be

performed using M codes.

D S codes (spindle

After address S, specify a numeric value of no more than the number of

functions)

digits specified by parameter No. 3031.

NOTE

Subprogram calls cannot be performed using S codes.

D T codes (tool functions)

After address T, specify a numeric value of no more than the number of

digits specified by parameter No. 3032.

NOTE

Subprogram calls cannot be performed using T codes.

785

3. MANUAL OPERATION

OPERATION

B-63534EN/02

D B codes (second

After address B, specify a numeric value of no more than the number of

auxiliary functions)

digits specified by parameter No. 3033.

NOTE

1

B codes can be renamed ”U,” ”V,” ”W,” ”A,” or ”C” by setting

parameter No. 3460. If the new name is the same as an axis

name address, ”B” is used. When ”B” is used, and axis

name ”B” exists, ”B” is used as the axis address. In this

case, no second auxiliary function can be specified.

2

Subprogram calls cannot be performed using B codes.

D Data input

(1) When addresses and numeric values of a command are typed, then soft

key [INPUT] is pressed, the entered data is set. In this case, the input

unit is either the least input increment or calculator-type input format,

according to the setting of bit 0 (DPI) of parameter No. 3401.

The

INPUT

key on the MDI panel can be used instead of soft key

[INPUT].

(2) Commands can be typed successively.

(3) Key entry is disabled during execution.

If soft key [INPUT] or the

INPUT

key on the MDI panel is pressed during

execution, an ”EXECUTION/MODE SWITCHING IN PROGRESS”

warning is output.

(4) If input data contains an error, the following warnings may appear:

Warning

Description

⋅ A G code other than G00, G01, and G28 has been

entered.

FORMAT ERROR

⋅ An address other than those displayed on the manual

numeric command screen has been entered.

A value that exceeds the following limitations has been

entered.

⋅ Address G: 2 digits

TOO MANY DIGITS

⋅ Address P: 1 digit

⋅ Axis address: 8 digits

⋅ M, S, T, B: The parameter-set number of digits

NOTE

Even when the memory protection key is set, key input can

nevertheless be performed.

786

Content      ..     25      26      27      28     ..