Content      ..     2      3      4      5     ..

FANUC Series 0i-MC. OPERATOR’S MANUAL - page 4

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.3

This function automatically controls the feedrate at a corner according to

the corner angle between the machining blocks or the feedrate difference

Automatic Corner

between the blocks along each axis.

Deceleration

This function is effective when ACD, bit 6 of parameter No. 1601, is set

to 1, the system is in G64 mode (machining mode), and a cutting-feed

block (block A) is followed by another cutting-feed block (block B).

The feedrate between machining blocks is controlled according to the

corner angle between the blocks or the feedrate difference between the

blocks along each axis. These two methods can be switched with CSD,

bit 4 of parameter No. 1602.

5.4.3.1

This function decelerates the feedrate when the angle between blocks A

and B on the selected plane is smaller than the angle specified in parameter

Corner Deceleration

No. 1740. The function executes block B when the feedrates along both

According to the Corner

the first and second axes are smaller than the feedrate specified in

Angle

parameter No. 1741. In this case, the function determines that the number

of accumulated pulses is zero.

Explanations

D Flowchart for feedrate

The flowchart for feedrate control is shown below.

control

START

Is the corner angle smaller than

No

the angle

specified in parameter

(No. 1740)?

Yes

Are the feedrates along the X-

No

and Y-axes smaller than that

specified in parameter

Further decelerates the

(No. 1741)?

feedrate in block A

Yes

The number of accumulated

pulses is

determined to be zero

and block B is executed

END

73

5. FEED FUNCTIONS

PROGRAMMING

B-64124EN/01

D Feedrate and time

When the corner angle is smaller than the angle specified in the

parameter, the relationship between the feedrate and time is as shown

below. Although accumulated pulses equivalent to the hatched area

remain at time t, the next block is executed because the feedrate of the

automatic acceleration/deceleration circuit is smaller than the

parameter-set value. This function is effective only for movement on

the selected plane.

Feedrate V

Block A

Block B

Í

Parameter-set feedrate

ÍÍÍÍ

t

Time t

D Angle between two

The angle between two blocks (blocks A and B) is assumed to be angle

blocks

θ, as shown below.

1. Between linear movements

2. Between linear and circular movements

3. Between circular movements

(angle between the linear movement

(angle between the tangents to

and tangent to the circular movement)

the circular movements)

θ

θ

θ

θ

D Selected plane

The machining angle is compared with the angle specified in parameter

(No. 1740) for movements on the selected plane only. Machining

feedrates are compared with that specified in parameter (No. 1741) for

movement along the first and second axes on the selected plane only. This

means, when movement occurs along three or more axes, only that

movement along the first and second axes on the selected plane is

considered.

D Corner roundness

Corner roundness is determined by the angle and feedrate specified in

parameter (Nos. 1740 and 1741). To always make a sharp corner, set

the angle to zero and the feedrate to 180000 (equivalent to 180

degrees).

D Exact stop

When G90 (exact stop) is specified, exact stop is performed irrespective

of the angle and feedrate specified in parameter (Nos. 1740 and 1741).

Limitations

This function cannot be enabled for a single block or during dry run.

74

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4.3.2

This function decelerates the feedrate when the difference between the

feedrates at the end point of block A and the start point of block B along

Corner Deceleration

each axis is larger than the value specified in parameter No. 1781. The

According to the

function executes block B when the feedrates along all axes are smaller

Feedrate Difference

than the feedrate specified in parameter No. 1741. In this case, the

between Blocks Along

function determines that the number of accumulated pulses is zero.

Each Axis

Explanations

D Flowchart for feedrate

The flowchart for feedrate control is shown below.

control

START

Is the feedrate difference between

No

blocks along each axis larger than

the value specified in parameter

(No. 1781)?

Yes

Are the feedrates along all axes

No

smaller than that specified in

parameter (No. 1741)?

Further decelerates the

feedrate in block A

Yes

The number of accumulated pulses

is determined

to be zero and block

B is executed.

END

D Feedrate and time

When the feedrate difference between blocks along each axis is larger than

the value specified in parameter No. 1781, the relationship between the

feedrate and time is as shown below. Although accumulated pulses

equivalent to the hatched area remain at time t, the next block is executed

because the feedrate of the automatic acceleration/deceleration circuit is

smaller than the feedrate specified in parameter No. 1741.

Feedrate V

Block A

Block B

Parameter-set feedrate

ÍÍ

t

Time t

75

B-64124EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.5

DWELL (G04)

Format

Dwell G04 X_ ; or G04 P_ ;

X_ : Specify a time (decimal point permitted)

P_ : Specify a time (decimal point not permitted)

Explanations

By specifying a dwell, the execution of the next block is delayed by the

specified time. In addition, a dwell can be specified to make an exact

check in the cutting mode (G64 mode).

When neither P nor X is specified, exact stop is performed.

Bit 1 (DWL) of parameter No. 3405 can specify dwell for each rotation

in feed per rotation mode (G95).

Table 5.5 (a) Command value range of the dwell time

(Command by X)

Increment system

Command value range

Dwell time unit

IS-B

0.001 to 99999.999

s or rev

IS-C

0.0001 to 9999.9999

Table 5.5 (b) Command value range of the dwell time

(Command by P)

Increment system

Command value range

Dwell time unit

IS-B

1 to 99999999

0.001 s or rev

IS-C

1 to 99999999

0.0001 s or rev

77

B-64124EN/01

PROGRAMMING

6. REFERENCE POSITION

6.1

REFERENCE

POSITION RETURN

General

D Reference position

The reference position is a fixed position on a machine tool to which the

tool can easily be moved by the reference position return function.

For example, the reference position is used as a position at which tools

are automatically changed. Up to four reference positions can be

specified by setting coordinates in the machine coordinate system in

parameters (No. 1240 to 1243).

Y

2nd reference position

3rd reference position

Reference position

4th reference

position

X

Machine zero point

Fig. 6.1 (a) Machine zero point and reference positions

79

6. REFERENCE POSITION

PROGRAMMING

B-64124EN/01

D Reference position

Tools are automatically moved to the reference position via an

return and movement

intermediate position along a specified axis. Or, tools are automatically

from the reference

moved from the reference position to a specified position via an

position

intermediate position along a specified axis. When reference position

return is completed, the lamp for indicating the completion of return goes

on.

Reference position return A→B→R

Return from the reference positionR→B→C

R (Reference position)

B (Intermediate

position)

A (Start position for

C (Destination of return from the

reference position return)

reference position)

Fig. 6.1 (b) Reference position return and return form the reference

position

D Reference position

The reference position return check (G27) is the function which checks

return check

whether the tool has correctly returned to the reference position as

specified in the program. If the tool has correctly returned to the reference

position along a specified axis, the lamp for the axis goes on.

Format

D Reference position

return

G28IP_ ; Reference position return

(P2 can

G30 P2

IP_;

2nd reference position return

be omitted.)

G30 P3IP

_ ; 3rd reference position return

G30 P4

IP

_;

4th reference position return

IP_

: Command specifying the intermediate position

(Absolute/incremental command)

D Return from reference

position

G29

_;

IP

IP_

: Command specifying the destination of return from reference

position (Absolute/incremental command)

D Reference position

return check

G27

_;

IP

IP_

: Command specifying the reference position

(Absolute/incremental command)

80

6. REFERENCE POSITION

PROGRAMMING

B-64124EN/01

NOTE

1

To this feedrate, a rapid traverse override (F0,25,50,100%)

is applied, for which the setting is 100%.

2

After a machine coordinate system has been established

upon the completion of reference position return, the

automatic reference position return feedrate will conform to

the ordinary rapid traverse rate.

3

For the manual rapid traverse rate used before a machine

coordinate system is estavlished upon the completion of

reference position return a jog feedrate or manual rapid

traverse rate can be selected usting RPD (bit 0 of parameter

No. 1401).

Before a coordinate

After a coordinate

system is established

system is established

Automatic reference posi-

No. 1428

No.1420

tion return (G28)

Automatic rapid traverse

No.1428

No.1420

(G00)

Manual reference position

No.1428

No.1428

return

Manual rapid traverse rate

No.1423 *1

No.1424

NOTE

When parameter No. 1428 is set to 0, the feedrates conform

to the parameter settings shown below.

Before a coordinate

After a coordinate

system is established

system is established

Automatic reference posi-

No. 1420

No.1420

tion return (G28)

Automatic rapid traverse

No.1420

No.1420

(G00)

Manual reference position

No.1424

No.1424

return

Manual rapid traverse rate

No.1423 *1

No.1424

1420 : Rapid traverse rate

1423 : Jog feedrate

1424 : Manual rapid traverse rate

*1 Setting of parameter No.1424 when RPD (bit 0 of parameter No.1401)

is set to 1.

82

B-64124EN/01

PROGRAMMING

6. REFERENCE POSITION

Restrictions

D Status the machine lock

The lamp for indicating the completion of return does not go on when the

being turned on

machine lock is turned on, even when the tool has automatically returned

to the reference position. In this case, it is not checked whether the tool

has returned to the reference position even when a G27 command is

specified.

D First return to the

When the G28 command is specified when manual return to the reference

reference position after

position has not been performed after the power has been turned on, the

the power has been

movement from the intermediate point is the same as in manual return to

turned on (without an

the reference position.

absolute position

In this case, the tool moves in the direction for reference position return

detector)

specified in parameter ZMIx (bit 5 of No. 1006). Therefore the specified

intermediate position must be a position to which reference position

return is possible.

D Reference position

In an offset mode, the position to be reached by the tool with the G27

return check in an offset

command is the position obtained by adding the offset value. Therefore,

mode

if the position with the offset value added is not the reference position, the

lamp does not light up, but an alarm is displayed instead. Usually, cancel

offsets before G27 is commanded.

D Lighting the lamp when

When the machine tool system is an inch system with metric input, the

the programmed position

reference position return lamp may also light up even if the programmed

does not coincide with

position is shifted from the reference position by the least setting

the reference position

increment. This is because the least setting increment of the machine tool

system is smaller than its least command increment.

Reference

D Manual reference

See III-3.1.

position return

Examples

G28G90X1000.0Y500.0 ; (Programs movement from A to B)

T1111 ; (Changing the tool at the reference position)

G29X1300.0Y200.0 ; (Programs movement from B to C)

Reference

Y

The tool is changed at the reference position

R position

500

B

300

A

200

C

200

1000

1300

X

Fig. 6.1 (c) Reference position return and return from the reference

position

83

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

COORDINATE SYSTEM

7

By teaching the CNC a desired tool position, the tool can be moved to the

position. Such a tool position is represented by coordinates in a

coordinate system. Coordinates are specified using program axes.

When three program axes, the X-axis, Y-axis, and Z-axis, are used,

coordinates are specified as follows:

X_Y_Z_

This command is referred to as a dimension word.

Z

25.0

Y

50.0

40.0

X

Fig. 7 Tool position specified by X40.0Y50.0Z25.0

Coordinates are specified in one of following three coordinate systems:

(1) Machine coordinate system

(2) Workpiece coordinate system

(3) Local coordinate system

The number of the axes of a coordinate system varies from one machine

to another. So, in this manual, a dimension word is represented as IP_.

84

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

The point that is specific to a machine and serves as the reference of the

7.1

machine is referred to as the machine zero point. A machine tool builder

MACHINE

sets a machine zero point for each machine.

COORDINATE

A coordinate system with a machine zero point set as its origin is referred

to as a machine coordinate system.

SYSTEM

A machine coordinate system is set by performing manual reference

position return after power-on (see III-3.1). A machine coordinate

system, once set, remains unchanged until the power is turned off.

Format

(G90)G53 I

IP

IPP_; Absolute dimension word

Explanations

D Selecting a machine

When a command is specified the position on a machine coordinate

coordinate system (G53)

system, the tool moves to the position by rapid traverse. G53, which is

used to select a machine coordinate system, is a one-shot G code; that is,

it is valid only in the block in which it is specified on a machine coordinate

system. Specify an absolute command (G90) for G53. When an

incremental command (G91) is specified, the G53 command is ignored.

When the tool is to be moved to a machine-specific position such as a tool

change position, program the movement in a machine coordinate system

based on G53.

Restrictions

D Cancel of the

When the G53 command is specified, cancel the cutter compensation, tool

compensation function

length offset, and tool offset.

D G53 specification

Since the machine coordinate system must be set before the G53

immediately after

command is specified, at least one manual reference position return or

power-on

automatic reference position return by the G28 command must be

performed after the power is turned on. This is not necessary when an

absolute-position detector is attached.

Reference

When manual reference position return is performed after power-on, a

machine coordinate system is set so that the reference position is at the

coordinate values of (α, β) set using parameter No.1240.

Machine coordinate system

Machine zero

β

α

Reference position

85

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

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

7.2

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

WORKPIECE

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

COORDINATE

A machining program sets a workpiece coordinate system (selecting a

workpiece coordinate system).

SYSTEM

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

(changing a workpiece coordinate system).

7.2.1

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

Setting a Workpiece

(1) Method using G92

A workpiece coordinate system is set by specifying a value after G92

Coordinate System

in the program.

(2) Automatic setting

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

coordinate system is automatically set when manual reference

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

(3) Input using the CRT/MDI panel

Six workpiece coordinate systems can be set beforehand using the

MDI panel (see Part III-11.4.6.).

When using an absolute command, establish the workpiece

coordinate system in any of the above ways.

Format

D Setting a workpiece

(G90) G92 IP_

coordinate system by G92

Explanations

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

the tool tip, is at specified coordinates. If a coordinate system is set using

G92 during tool length offset, a coordinate system in which the position

before offset matches the position specified in G92 is set.

Cutter compensation is cancelled temporarily with G92.

Examples

Example 1

Example 2

Setting the coordinate system by the

Setting the coordinate system by the G92X600.0Z1200.0; command

G92X25.2Z23.0; command

(The base point on the tool holder is the start point for the program.)

(The tool tip is the start point for the program.)

Z

Base point

If an absolute command is is-

Z

1200.0

sued, the base point moves to

the commanded position. In

order to move the tool tip to the

commanded position, the dif-

23.0

ference from the tool tip to the

base point is compensated by

tool length offset.

0

25.2

X

X

0

600.0

86

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.2.2

The user can choose from set workpiece coordinate systems as described

below. (For information about the methods of setting, see II- 7.2.1.)

Selecting a Workpiece

(1) Once a workpiece coordinate system is selected by G92 or automatic

Coordinate System

workpiece coordinate system setting, absolute commands work with

the workpiece coordinate system.

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

CRT/MDI panel

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

coordinate systems 1 to 6 can be selected.

G54 Workpiece coordinate system 1

G55 Workpiece coordinate system 2

G56 Workpiece coordinate system 3

G57 Workpiece coordinate system 4

G58 Workpiece coordinate system 5

G59 Workpiece coordinate system 6

Workpiece coordinate system 1 to 6 are established after reference

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

on, G54 coordinate system is selected.

Examples

G90 G55 G00 X40.0 Y100.0 ;

Y

Workpiece coordinate system 2 (G55)

100.0

In this example, positioning is made to

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

coordinate system 2.

X

40.0

Fig. 7.2.2

87

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

7.2.3

The six workpiece coordinate systems specified with G54 to G59 can

be changed by changing an external workpiece zero point offset value

Changing Workpiece

or workpiece zero point offset value.

Coordinate System

Three methods are available to change an external workpiece zero

point offset value or workpiece zero point offset value.

(1) Inputting from the MDI panel (see III-11.4.6)

(2) Programming by G10 or G92

(3) Using the external data input function

An external workpiece zero point offset value can be changed by

input signal to CNC. Refer to machine tool builder’s manual for

details

Workpiece

Workpiece

Workpiece

Workpiece

coordinate

coordinate

coordinate

coordinate

system 1 (G54)

system 2 (G55)

system 3 (G56)

system 4 (G57)

ZOFS2

ZOFS3

ZOFS1

ZOFS4

Workpiece

coordinate

ZOFS5

system 5 (G58)

EXOFS

ZOFS6

Workpiece

Machine zero

coordinate

system 6 (G59)

EXOFS : External workpiece zero point offset value

ZOFS1 to ZOFS6 : Workpiece zero point offset value

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

Format

G10 L2 Pp IIP

_;

D Changing by G10

p=0

:

External workpiece zero point offset value

p=1 to 6 :

Workpiece zero point offset value correspond to workpiece

coordinate system 1 to 6

IP_ : For an absolute command (G90), workpiece zero point offset for

each axis.

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

workpiece zero point offset for each axis (the result of addition

becomes the new workpiece zero point offset).

D Changing by G92

G92 I

IP

88

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

Examples

Y

YȀ

G54 workpiece coordinate system

If G92X100Y100; is commanded when the tool

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

160

100

Tool position

piece coordinate system 1 (X’ - Y’) shifted by

vector A is created.

60

A

XȀ

New workpiece coordinate system

100

X

Original workpiece coordinate system

100

200

G54 Workpiece

Suppose that a G54 workpiece coordi-

coordinate system

nate system is specified. Then, a G55

Z’

workpiece coordinate system where

G55 Workpiece

the black circle on the tool (figure at the

coordinate system

1200.0

left) is at (600.0,1200.0) can be set with

ZȀ

the following command if the relative

relationship between the G54 work-

Z

piece coordinate system and G55

1200.0

workpiece coordinate system is set cor-

rectly:G92X600.0Z1200.0;Also, sup-

Z

pose that pallets are loaded at two dif-

X

ferent positions. If the relative relation-

600.0

ship of the coordinate systems of the

A

pallets at the two positions is correctly

set by handling the coordinate systems

X

XȀ

600.0

as the G54 workpiece coordinate sys-

B

A

tem and G55 workpiece coordinate

system, a coordinate system shift with

X

G92 in one pallet causes the same

C

coordinate system shift in the other pal-

let. This means that workpieces on two

pallets can be machined with the same

X’ - Z’ New workpiece coordinate system

program just by specifying G54 or G55.

X - Z Original workpiece coordinate system

A : Offset value created by G92

B : Workpiece zero point offset value in theG54

C : Workpiece zero point offset value in the G55

90

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.2.4

The workpiece coordinate system preset function presets a workpiece

coordinate system shifted by manual intervention to the pre-shift

Workpiece coordinate

workpiece coordinate system. The latter system is displaced from the

system preset (G92.1)

machine zero point by a workpiece zero point offset value.

There are two methods for using the workpiece coordinate system preset

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

uses MDI operations on the absolute position display screen, relative

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

Format

G92.1 IP 0 ;

IP 0 ; Specifies axis addresses subject to the workpiece

coordinate system preset operation. Axes that are

not specified are not subject to the preset operation.

Explanations

When manual reference position return operation is performed in the reset

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

point offset value from the machine coordinate system zero point.

Suppose that the manual reference position return operation is performed

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

a workpiece coordinate system is automatically set which has its zero

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

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

coordinate system to the reference position represents the current position

in the workpiece coordinate system.

G54 workpiece coordinate system

G54 workpiece zero

point offset value

Reference position

Reference position

Manual reference position return

If an absolute position detector is provided, the workpiece coordinate

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

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

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

position detector and the current position in the workpiece coordinate

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

from this machine position. The workpiece coordinate system set by

these operations is shifted from the machine coordinate system using the

commands and operations listed next page.

91

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

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

(b) Move command executed in the machine lock state

(c) Movement by handle interrupt

(d) Operation using the mirror image function

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

workpiece coordinate system using G92

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

amount of movement during manual intervention.

G54 workpiece coordinate

system before manual

Po

intervention

Amount of movement

during manual

intervention

Workpiece zero

WZo

point offset

value

Pn

Machine zero point

G54 workpiece coordinate

system after manual intervention

WZn

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

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

coordinate system displaced by a workpiece zero point offset value from

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

position return operation is performed on a workpiece coordinate system

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

operation has the effect of returning workpiece coordinate system zero

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

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

system.

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

coordinates (RELATIVE) as well as absolute coordinates.

Limitations

D Cutter compensation,

When using the workpiece coordinate system preset function, cancel

tool length

compensation modes: cutter compensation, tool length compensation,

compensation, tool

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

offset

modes, compensation vectors are temporarily cancelled.

D Program restart

The workpiece coordinate system preset function is not executed during

program restart.

D Prohibited modes

Do not use the workpiece coordinate system preset function when the

scaling, coordinate system rotation, programmable image, or drawing

copy mode is set.

92

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

7.2.5

Besides the six workpiece coordinate systems (standard workpiece

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

Adding Workpiece

coordinate systems (additional workpiece coordinate systems) can be

Coordinate Systems

used. Alternatively, up to 300 additional workpiece coordinate systems

(G54.1 or G54)

can be used.

Format

D Selecting the additional

G54.1Pn ; or G54Pn ;

workpiece coordinate

Pn : Codes specifying the additional workpiece coordinate systems

systems

n

:

1 to 48

D Setting the workpiece

zero point offset value

in the additional

G10L20 Pn IIP_;

workpiece coordinate

Pn : Codes specifying the workpiece coordinate system for setting

systems

the workpiece zero point offset value

n

:

1 to 48

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

offset

Explanations

D Selecting the additional

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

workpiece coordinate

coordinate system is selected from the additional workpiece coordinate

systems

systems (1 to 48).

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

workpiece coordinate system is selected. Standard workpiece coordinate

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

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

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

G54.1 P48 . . Additional workpiece coordinate system 48

As with the standard workpiece coordinate systems, the following

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

additional workpiece coordinate system:

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

zero point offset value.

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

by programming (refer to II-7.2.3).

(3) A custom macro allows a workpiece zero point offset value to be

handled as a system variable.

(4) Workpiece zero point offset data can be entered or output as external

data.

(5) The PMC window function enables workpiece zero point offset data

to be read as program command modal data.

93

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

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

7.3

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

LOCAL COORDINATE

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

SYSTEM

Format

G52 IP _; Setting the local coordinate system

G52 IIP0 ; Canceling of the local coordinate system

I

IP

Explanations

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

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

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

coordinate system.

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

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

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

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

local coordinate system in the workpiece coordinate system.

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

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

coordinate system with that of the workpiece coordinate system.

(Local coordinate system)

IP

(G54 : Workpiece coordinate system 1)

(Local coordinate system)

G55

G56

IP

G57

G58

(G59 : Workpiece coordinate system 6)

(Machine coordinate system)

Machine coordinate system origin

Reference point

Fig. 7.3 Setting the local coordinate system

95

7. COORDINATE SYSTEM

PROGRAMMING

B-64124EN/01

WARNING

1

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

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

The same is true when the following command is issued:

G52α0;

α:Axis which returns to the reference point

2

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

systems.

3

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

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

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

4

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

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

not specified are not cancelled, but remain unchanged.

5

G52 cancels the offset temporarily in cutter compensation.

6

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

96

B-64124EN/01

PROGRAMMING

7. COORDINATE SYSTEM

Select the planes for circular interpolation, cutter compensation, and

7.4

drilling by G-code.

PLANE

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

SELECTION

Explanations

Table 7.4 Plane selected by G code

Selected

G code

Xp

Yp

Zp

plane

G17

Xp Yp plane

X-axis or an

Y-axis or an

Z-axis or an

G18

Zp Xp plane

axis parallel

axis parallel

axis parallel

to it

to it

to it

G19

Yp Zp plane

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

which G17, G18 or G19 is commanded.

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

that the addresses of basic three axes are omitted.

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

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

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

commanded.

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

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

parameter 3402.

The movement instruction is irrelevant to the plane selection.

Examples

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

G17X_Y_ XY plane,

G17U_Y_ UY plane

G18X_Z_ ZX plane

X_Y_ Plane is unchanged (ZX plane)

G17

XY plane

G18

ZX plane

G17 U_ UY plane

G18Y_ ; ZX plane, Y axis moves regardless without any

relation to the plane.

97

8. COORDINATE VALUE

B-64124EN/01

PROGRAMMING

AND DIMENSION

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

8.1

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

ABSOLUTE AND

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

INCREMENTAL

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

G91 are used to command absolute or incremental command,

PROGRAMMING

respectively.

(G90, G91)

Format

Absolute command

G90

IP_ ;

Incremental command G91

IP_ ;

Examples

G90 X40.0 Y70.0 ;

Absolute command

G91 X-60.0 Y40.0 ; Incremental command

Y

End position

70.0

30.0

Start position

X

40.0

100.0

99

8. COORDINATE VALUE

AND DIMENSION

PROGRAMMING

B-64124EN/01

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

8.2

and angle).

POLAR COORDINATE

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

COMMAND

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

Both radius and angle can be commanded in either absolute or

(G15, G16)

incremental command (G90, G91).

Format

Gjj Gff G16 ;

Starting the polar coordinate command (polar

coordinate mode)

Gff

IP _ ;

Polar coordinate command

G15 ;

Canceling the polar coordinate command (polar coordinate

mode)

G16

Polar coordinate command

G15

Polar coordinate command cancel

Gjj

Plane selection of the polar coordinate command

(G17, G18 or G19)

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

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

is measured.

G91 specifies the current position as the origin of the polar

coordinate system, from which a radius is measured.

IP

_

Specifying the addresses of axes constituting the plane se-

lected for the polar coordinate system, and their values

First axis : radius of polar coordinate

Second axis : radius of polar coordinate

D Setting the zero point of

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

the workpiece

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

coordinate system as the

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

origin of the polar

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

coordinate system

coordinate system becomes the center of the polar coordinates.

Command position

Command position

Radius

Radius

Actual position

Angle

Angle Actual position

When the angle is specified

When the angle is specified

with an absolute command

with an incremental command

100

8. COORDINATE VALUE

B-64124EN/01

PROGRAMMING

AND DIMENSION

D Setting the current

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

position as the origin of

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

the polar coordinate

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

system

Command position

Command position

Angle

Radius

Radius

Angle

Actual position

Actual position

When the angle is specified

When the angle is specified

with an absolute command

with an incremental command

Examples

Bolt hole circle

Y

- The zero point of the work coordinate

system is set as the origin of the polar

coordinate system.

- The XY plane is selected.

150°

30°

270°

X

100mm

D Specifying angles and a

N1 G17 G90 G16 ;

radius with absolute

Specifying the polar coordinate command and selecting the XY plane

commands

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

polar coordinate system

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

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

N3 Y150.0 ;

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

N4 Y270.0 ;

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

N5 G15 G80 ;

Canceling the polar coordinate command

D Specifying angles with

N1 G17 G90 G16;

incremental commands

Specifying the polar coordinate command and selecting the XY plane

and a radius with

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

absolute commands

polar coordinate system

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

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

N3 G91 Y120.0 ;

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

N4 Y120.0 ;

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

101

Content      ..     2      3      4      5     ..