Content      ..     3      4      5      6     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 5

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

G93 is a modal G code and belongs to group 05 (includes G95 (feed per

revolution) and G94 (feed per minute)).

When an F value is specified in G93 mode and the feedrate exceeds the

maximum cutting feedrate, the feedrate is clamped to the maximum

cutting feedrate.

In the case of circular interpolation, the feedrate is calculated not from the

actual amount of movement in the block but from the arc radius. This

means that actual machining time is longer when the arc radius is longer

than the arc distance and shorter when the arc radius is shorter than the arc

distance. Inverse time feed can also be used for cutting feed in a canned

cycle.Notes

NOTE

1

In the G93 mode, an F code is not handled as a modal code and

therefore needs to be specified in each block. If an F code is not

specified, P/S alarm (No. 11 (indicating that cutting feedrate

specification is missing)) is issued.

2

When F0 is specified in G93 mode, P/S alarm (No. 11 (indicating

that cutting feedrate specification is missing)) is issued.

3

Inverse time feed cannot be used when PMC axis control is in

effect.

4

If the calculated cutting feedrate is smaller than the allowable

range, P/S alarm

(No.

11

(indicating that cutting feedrate

specification is missing)) is issued.

100

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

Cutting feedrate can be controlled, as indicated in Table 5.4 (a).

5.4

CUTTING FEEDRATE

CONTROL

Table 5.4 (a) Cutting Feedrate Control

Function name

G code

Validity of G code

Description

The tool is decelerated at the end point

This function is valid for specified

Exact stop

G09

of a block, then an in-position check is

blocks only.

made. Then the next block is executed.

Once specified, this function is

The tool is decelerated at the end point

Exact stop mode

G61

valid until G62, G63, or G64 is

of a block, then an in-position check is

specified.

made. Then the next block is executed.

Once specified, this function is

The tool is not decelerated at the end

Cutting mode

G64

valid until G61, G62, or G63 is

point of a block, but the next block is

specified.

executed.

The tool is not decelerated at the end

Once specified, this function is

point of a block, but the next block is

Tapping mode

G63

valid until G61, G62, or G64 is

executed.

specified.

When G63 is specified, feedrate override

and feed hold are invalid.

When the tool moves along an inner

corner during cutter compensation, over-

Once specified, this function is

Automatic override for

ride is applied to the cutting feedrate to

G62

valid until G61, G63, or G64 is

inner corners

suppress the amount of cutting per unit

specified.

Auto-

of time so that a good surface finish can

matic

be produced.

This function is valid in the cutter

Internal circular cutting

The internal circular cutting feedrate is

_

compensation mode, regardless of

feedrate change

changed.

the G code.

NOTE

1

The purpose of in-position check is to check that the servo

motor has reached within a specified range (specified with

a parameter by the machine tool builder).

In-position check is not performed when bit 5 (NCI) of

parameter No. 1601 is set to 1.

2

Inner corner angle θ: 2°< θ x α x 178°

(α is a set value)

Workpiece

θ

Tool

102

B-63534EN/02

PROGRAMMING

5. FEED FUNCTIONS

Format

Exact stop

G09 IP_ ;

Exact stop mode

G61 ;

Cutting mode

G64 ;

Tapping mode

G63 ;

Automatic corner override G62 ;

5.4.1

Exact Stop (G09, G61)

Cutting Mode (G64)

Tapping Mode (G63)

Explanations

The inter-block paths followed by the tool in the exact stop mode, cutting

mode, and tapping mode are different (Fig. 5.4.1 (a)).

Y

Position check

(2)

Tool path in the exact stop mode

(1)

Tool path in the cutting mode or

tapping mode

0

X

Fig. 5.4.1 (a) Example of Tool Paths from Block (1) to Block (2)

CAUTION

The cutting mode (G64 mode) is set at power-on or system

clear.

103

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

5.4.2

When cutter compensation is performed, the movement of the tool is

automatically decelerated at an inner corner and internal circular area.

Automatic Corner

This reduces the load on the cutter and produces a smoothly machined

Override

surface.

5.4.2.1

Automatic Override for

Inner Corners (G62)

Explanations

D Override condition

When G62 is specified, and the tool path with cutter compensation

applied forms an inner corner, the feedrate is automatically overridden

at both ends of the corner.

There are four types of inner corners (Fig. 5.4.2.1 (a)).

2,xθxθpx178, in Fig. 5.4.2.1 (a)

θp is a value set with parameter No. 1711. When θ is approximately

equal to θp, the inner corner is determined with an error of 0.001,or

less.

1. Straight line-straight line

:Tool

2. Straight line-arc

:Programmed path

:Cutter center path

θ

θ

3. Arc-straight line

4. Arc-arc

θ

θ

Fig. 5.4.2.1 (a) Inner corner

104

B-63534EN/02

PROGRAMMING

5. FEED FUNCTIONS

Override range

When a corner is determined to be an inner corner, the feedrate is

overridden before and after the inner corner. The distances Ls and Le,

where the feedrate is overridden, are distances from points on the cutter

center path to the corner (Fig. 5.4.2.1 (b), Fig. 5.4.2.1 (c), Fig. 5.4.2.1 (d)).

Ls and Le are set with parameter Nos. 1713 and 1714.

Programmed path

Le

Ls

b

a

Cutter center path

The feedrate is overridden from point a to point b.

FIg. 5.4.2.1 (b) Override Range (Straight Line to Straight Line)

When a programmed path consists of two arcs, the feedrate is overridden

if the start and end points are in the same quadrant or in adjacent quadrants

(Fig. 5.4.2.1 (c)).

Le

Programmed path

Ls

a

b

Cutter center path

The feedrate is overridden from point a to b.

Fig. 5.4.2.1 (c) Override Range (Arc to Arc)

Regarding program (2) of an arc, the feedrate is overridden from point a

to point b and from point c to point d (Fig. 5.4.2.1 (d)).

Programmed path

d

a

Le

Ls

Le

Ls

c

b

(2)

Cutter center path

Tool

Fig. 5.4.2.1 (d) Override Range (Straight Line to Arc, Arc to Straight Line)

105

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

Override value

An override value is set with parameter No. 1712. An override value is

valid even for dry run and F1-digit specification.

In the feed per minute mode, the actual feedrate is as follows:

F × (automatic override for inner corners) × (feedrate override)

Limitations

D Acceleration/deceleratio

Override for inner corners is disabled during acceleration/deceleration

n before interpolation

before interpolation.

D Start-up/G41, G42

Override for inner corners is disabled if the corner is preceded by a

start-up block or followed by a block including G41 or G42.

D Offset

Override for inner corners is not performed if the offset is zero.

5.4.2.2

For internally offset circular cutting, the feedrate on a programmed path

is set to a specified feedrate (F) by specifying the circular cutting feedrate

Internal Circular Cutting

with respect to F, as indicated below (Fig. 5.4.2.2). This function is valid

Feedrate Change

in the cutter compensation mode, regardless of the G62 code.

Rc

F

Rp

Rc : Cutter center path radius

Rp : Programmed radius

It is also valid for the dry run and the one-digit F command.

Programmed path

Rc Cutter center

path

Rp

Fig. 5.4.2.2 Internal circular cutting feedrate change

If Rc is much smaller than Rp, Rc/Rp80; the tool stops. A minimum

deceleration ratio (MDR) is to be specified with parameter No. 1710.

When Rc/RpxMDR, the feedrate of the tool is (F×MDR).

NOTE

When internal circular cutting must be performed together with override for inner corners, the

feedrate of the tool is as follows:

Rc

F

(override for the inner corners)×(feedrate override)

Rp

106

B-63534EN/02

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

107

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

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

ÍÍ

Parameter-set feedrate

t

Time t

D Acceleration/

When acceleration/deceleration before interpolation is effective, the

deceleration before

relationship between the feedrate and time is as shown below. When the

interpolation

angle between blocks A and B on the selected plane is smaller than the

angle specified in parameter (No. 1740), and the feedrates specified in

blocks A and B are larger than that specified in parameter (No. 1777), the

feedrate is decelerated to the parameter-set value in block A, and

accelerated to the feedrate specified in block B. The acceleration depends

on the parameter for acceleration/deceleration before interpolation.

Feedrate

Block A

Block B

Parameter-set feedrate

(parameter No. 1777)

Time

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

108

B-63534EN/02

PROGRAMMING

5. FEED FUNCTIONS

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).

D Look-ahead control

Those parameters related to automatic corner deceleration in look-ahead

control mode are shown below.

Look-ahead

Normal

Parameter description

control

mode

mode

Switching the methods for automatic corner de-

No.1602#4

←

celeration

Lower limit of feedrate in automatic corner decel-

No.1777

No.1778

eration based on the angle

Limit angle in corner deceleration based on the

No.1740

No.1779

angle

Limitations

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

109

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

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

110

B-63534EN/02

PROGRAMMING

5. FEED FUNCTIONS

D Acceleration /

When acceleration/deceleration before interpolation is effective, the

deceleration before

relationship between the feedrate and time is as described below.

interpolation

When the feedrate difference between blocks A and B along each axis is

larger than the value specified in parameter No. 1780, the feedrate is

decelerated to the corner feedrate calculated from the feedrate difference

along each axis.

Let the feedrate be F. Compare the feedrate difference along each axis

(Vc[X], Vc[Y], ...) with the value specified in parameter No. 1780, Vmax.

When the difference exceeds Vmax, calculate R as shown below.

Vc

R=

Vmax

Find the maximum value for R among the calculated values for the axes.

Let it be Rmax. Then, the corner feedrate can be obtained as follows:

1

Fc=F

Rmax

(Example)

N2

N1 G01 G91 X80. Y20. F3000 ;

N2 X20. Y80. ;

N1

When this movement is specified, the feedrate along each axis is as

shown in the next figure.

Vc [X(Y)]

Rmax=

Vmax

1

F

Rmax

From the figure, it can be seen that the feedrate differences along the X-

and Y-axes (Vc[X] and Vc[Y]) exceed Vmax. Calculate Rmax to get

Fc. When the feedrate is decelerated to Fc at the corner, the feedrate

difference along each axis do not exceed Vmax.

111

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

Without corner deceleration

With corner deceleration

Feedrate along

Vc [X]

Vmax

the X-axis

Vmax

Feedrate along

the Y-axis

Vc [Y]

Vmax

Feedrate along

the tangent

at the corner

1

F

Rmax

N1

N2

t

D Setting the allowable

The allowable feedrate difference can be specified for each axis in

feedrate difference along

parameter No. 1783.

each axis

D Checking the feedrate

The feedrate difference is also checked during dry-run operation or

difference

during deceleration caused by an external signal, using feedrate

commands specified in a program.

D Exact stop

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

of the parameter settings.

D Override

If an override is changed during operation, the feedrate difference will

not be checked correctly.

112

B-63534EN/02

PROGRAMMING

5. FEED FUNCTIONS

D Look-ahead control

Parameters related to automatic corner deceleration in look-ahead

control mode are shown below.

Normal

Look-ahead

Parameter description

mode

control mode

Switching the methods for automatic corner

No.1602#4

No.1602#4

deceleration

Allowable feedrate difference (for all axis) in

automatic corner deceleration based on the

No.1780

No.1780

feedrate difference

Allowable feedrate difference

(for each

axis) in automatic corner deceleration

No.1783

No.1783

based on the feedrate difference

Limitations

This function is not effective for feed-per-rotation commands,

address-F-with-one-digit commands, rigid tapping, and a single block.

113

5. FEED FUNCTIONS

PROGRAMMING

B-63534EN/02

5.5

DWELL (G04)

Format

Dwell G04 X_ ; or G04 P_ ;

X_ : Specify a time or spindle speed (decimal point permitted)

P_ : Specify a time or spindle speed (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

114

6. REFERENCE POSITION

PROGRAMMING

B-63534EN/02

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

116

PROGRAMMING

6. REFERENCE POSITION

B-63534EN/02

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

G28 IP_ ; 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

I

: Command specifying the intermediate position

(Absolute/incremental command)

D Return from reference

position

G29

_;

IP

I

: Command specifying the destination of return from reference

position (Absolute/incremental command)

D Reference position

return check

G27

_;

IP

I

: Command specifying the reference position

(Absolute/incremental command)

117

PROGRAMMING

6. REFERENCE POSITION

B-63534EN/02

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.

119

6. REFERENCE POSITION

PROGRAMMING

B-63534EN/02

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

Manual reference position

See III-3.1.

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

120

PROGRAMMING

6. REFERENCE POSITION

B-63534EN/02

6.2

Tools ca be returned to the floating reference position.

A floating reference point is a position on a machine tool, and serves as

FLOATING

a reference point for machine tool operation.

REFERENCE

A floating reference point need not always be fixed, but can be moved as

POSITION RETURN

required.

(G30.1)

Format

G30.1

IP_;

IP

_ :

Command of the intermediate position of the floating reference

position

(Absolute command/incremental command)

Explanations

Generally speaking, on a machining center or milling machine, cutting

tools can be replaced only at specific positions. A position where tools can

be replaced is defined as the second or third reference point. Using G30

can easily move the cutting tools back to these points. On some machine

tools, the cutting tools can be replaced at any position unless they interfere

with the workpiece.

With these machines, the cutting tools should be replaced at a position as

close to the workpiece as possible so as to minimize the machine cycle

time. For this purpose, the tool change position is to be changed,

depending on the figure of the workpiece. This operation can easily be

performed using this function. That is, a tool change position suitable for

the workpiece is memorized as a floating reference point. Then command

G30. 1 can easily cause return to the tool change position.

A floating reference point becomes a machine coordinate position

memorized by pressing the soft key [SET FRP] on the current positions

display screen (see III-11.1.7). The G30.1 block first positions the tool

at the intermediate point along the specified axes at rapid traverse rate,

then further moves the tool from the intermediate point to the floating

reference point at rapid traverse rate.

Before using G30.1, cancel cutter compensation and tool length

compensation.

A floating reference point is not lost even if power is turned off.

The function for returning from the reference position (G29) can be used

for moving the tool from the floating reference position (see II-6.1).

Examples

G30.1 G90 X50.0 Y40.0 ;

Y

Intermediate position (50,40)

Floating reference

position

Workpiece

X

121

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

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_.

122

B-63534EN/02

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

123

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

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) Method using G54 to G59

Six workpiece coordinate systems can be set beforehand using the

CRT/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

124

B-63534EN/02

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 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

125

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

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

II

P

: 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

126

B-63534EN/02

PROGRAMMING

7. COORDINATE SYSTEM

Explanations

D Changing by G10

With the G10 command, each workpiece coordinate system can be

changed separately.

D Changing by G92

By specifying G92IP_;, a workpiece coordinate system (selected with a

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

system so that the current tool position matches the specified coordinates

( IP _).

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

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

systems are shifted by the same amount.

WARNING

When a coordinate system is set with G92 after an external

workpiece zero point offset value is set, the coordinate

system is not affected by the external workpiece zero point

offset value. When G92X100.0Z80.0; is specified, for

example, the coordinate system having its current tool

reference position at X = 100.0 and Z = 80.0 is set.

127

7. COORDINATE SYSTEM

PROGRAMMING

B-63534EN/02

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

(600.0,12000.0) can be set

ZȀ

with the following command if the rela-

tive 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

128

B-63534EN/02

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.

129

Content      ..     3      4      5      6     ..