Content      ..     4      5      6      7     ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 6

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Target figure

Patterns

As in the case of G71.7, there are four target figure patterns. Be careful about signs of Δu, Δw, Δi, and Δk

when programming this cycle.

-

Start block

In the start block in the program for a target figure (block with sequence number ns in which the path

between A and A’ is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065 is

issued.

When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation

is performed with cutting feed along A-A’.

-

Check functions

The following check can be made.

Check

Related parameter

Checks that a block with the sequence number specified at address Q is

Enabled when bit 2 (QSR) of

contained in the program before cycle operation.

parameter No. 5102 is set to 1.

-

Tool nose radius compensation

Like G71.7, this cycle operation is performed according to the figure determined by the tool nose radius

compensation path when the offset vector is 0 at start point A and start-up is performed in a block

between path A-A'.

- 142 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.8.4

Finishing Cycle (G70.7)

After rough cutting by G71.7, G72.7 or G73.7, the following command permits finishing.

Format

G70.7 P(ns) Q(nf) ;

ns : Sequence number of the first block for the program of finishing shape.

nf : Sequence number of the last block for the program of finishing shape.

Explanation

-

Operations

The blocks with sequence numbers ns to nf in the program for a target figure are executed for finishing.

The F, S, T, M, and second auxiliary functions specified in the G71.7, G72.7, or G73.7 block are ignored

and the F, S, T, M, and second auxiliary functions specified in the blocks with sequence numbers ns to nf

are effective.

When cycle operation terminates, the tool is returned to the start point in rapid traverse and the next

G70.7 cycle block is read.

-

Target figure

Check function

Following check can be made.

Check

Related parameter

Checks that a block with the sequence number specified at address Q is

Enabled when bit 2 (QSR) of

contained in the program before cycle operation.

parameter No. 5102 is set to 1.

-

Storing P and Q blocks

When rough cutting is executed by G71.7, G72.7, or G73.7, up to three memory addresses of P and Q

blocks are stored. By this, the blocks indicated by P and Q are immediately found at execution of G70.7

without searching memory from the beginning for them. After some G71.7, G72.7, and G73.7 rough

cutting cycles are executed, finishing cycles can be performed by G70.7 at a time. At this time, for the

fourth and subsequent rough cutting cycles, the cycle time is longer because memory is searched for P

and Q blocks.

Example

G71.7 P100 Q200 - - - ;

N100 - - - ;

- - - ;

- - - ;

N200 - - - ;

G71.7 P300 Q400 - - - ;

N300 - - - ;

- - - ;

- - - ;

N400 - - - ;

- - - ;

- - - ;

G70.7 P100 Q200 ; (Executed without a search for the first to third cycles)

G70.7 P300 Q400 ; (Executed after a search for the fourth and subsequent

cycles)

- 143 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.8.5

End Face Peck Drilling Cycle (G74.7)

This cycle enables chip breaking in outer diameter cutting. If the second axis on the plane (X-axis

(U-axis) for the ZX plane) and address P are omitted, operation is performed only along the first axis on

the plane (Z-axis for the ZX plane), that is, a peck drilling cycle is performed.

Format

G74.7R (e) ;

G74.7X_ Z_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e

: Return amount

This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command.

X_,Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and

Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

Δi

: Travel distance in the direction of the second axis on the plane (X-axis for the ZX

plane)

Δk

: Depth of cut in the direction of the first axis on the plane (Z-axis for the ZX plane)

Δd

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment system

e

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

Δi

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

Δk

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

Δd

Radius programming

Note

Allowed

for the reference axis.

NOTE

Normally, specify a positive value for Δd. When X and Δi are omitted, specify a

value with the sign indicating the direction in which the tool is to escape.

- 147 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Δk'

Δk

Δk

Δk

Δk

[0<Δk’≤Δk]

Δd

A

Δi

C

(R)

(R)

(F)

(F)

(F)

(F)

Δx/2

(R)

(R)

(R)

(R)

Δi

[0<Δi’≤Δi]

Δi’

X

Z

Δz

B

+X

(R) ... Rapid traverse

(F) ... Cutting feed

e

+Z

Fig. 5.8.5 (a) Cutting path in end face peek drilling cycle

Explanation

-

Operations

A cycle operation of cutting by Δk and return by e is repeated.

When cutting reaches point C, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to

the direction of point B by Δi, and performs cutting again.

NOTE

1 For e and Δd, the same address must be specified. They are distinguished from

each other according to whether an axis, such as X, Y, and Z is specified. That

is, if an axis is specified, the address is regarded as being that for Δd.

2 A cycle operation is performed with a G74.7 command with an axis specified.

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 148 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.8.6

Outer Diameter / Internal Diameter Drilling Cycle (G75.7)

This cycle is equivalent to G74.7 except that the second axis on the plane (X-axis for the ZX plane)

changes places with the first axis on the plane (Z-axis for the ZX plane). This cycle enables chip breaking

in end facing. It also enables grooving during outer diameter cutting and cutting off (when the Z-axis and

Q are omitted for the first axis on the plane).

Format

G75.7R (e) ;

G75.7X_ Z_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e

: Return amount

This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command.

X_,Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and

Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

Δi

: Depth of cut in the direction of the second axis on the plane (X-axis for the ZX plane)

Δk

: Travel distance in the direction of the first axis on the plane (Z-axis for the ZX plane)

Δd

: Relief amount of the tool at the cutting bottom

f

: Feedrate

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment system

e

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

Δi

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

Δk

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

Δd

Radius programming

Note

Allowed

for the reference axis.

NOTE

Normally, specify a positive value for Δd. When Z and Δk are omitted, specify a

value with the sign indicating the direction in which the tool is to escape.

- 149 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

C

(R)

A

(R)

(F)

Δi

(R)

e

(F)

Δi

(R)

Δx/2

(F)

Δi

(R)

(F)

Δi

(R)

(F)

Δi’

B

Δd

Δk

X

Z

Δz

+X

(R)…Rapid traverse

(F)…Cutting feed

+Z

Fig. 5.8.6 (a) Outer diameter/internal diameter drilling cycle

Explanation

-

Operations

A cycle operation of cutting by Δi and return by e is repeated.

When cutting reaches point B, the tool escapes by Δd. Then, the tool returns in rapid traverse, moves to

the direction of point C by Δk, and performs cutting again.

Both G74.7 and G75.7 are used for grooving and drilling, and permit the tool to relief automatically. Four

symmetrical patterns are considered, respectively.

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 150 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.8.7

Multiple Threading Cycle (G76.7)

This threading cycle performs one edge cutting by the constant amount of cut.

Format

G76.7 P(m) (r) (a) Q(Δdmin) R(d ) ;

G76.7 X_ Z_ R(i ) P(k ) Q(Δd) F (L ) ;

m : Repetitive count in finishing (1 to 99)

This value can be specified by the parameter No. 5142, and the parameter is changed

by the program command.

r

: Chamfering amount (0 to 99)

When the thread lead is expressed by L, the value of L can be set from 0.0L to 9.9L in

0.1L increment (2-digit number). This value can be specified by the parameter No.

5130, and the parameter is changed by the program command.

a

: Angle of tool nose (thread angle)

One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected, and specified

by 2-digit number. This value can be specified by the parameter No. 5143, and the

parameter is changed by the program command.

m, r, and a are specified by address P at the same time.

(Example)When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).

P

02

12

60

a

r

m

Δdmin : Minimum cutting depth

When the cutting depth of one cycle operation becomes smaller than this limit, the

cutting depth is clamped at this value. This value can be specified by parameter

No. 5140, and the parameter is changed by the program command.

d

: Finishing allowance

This value can be specified by parameter No. 5141, and the parameter is changed

by the program command.

X_,Z_ : Coordinates of the cutting end point (point D in the Fig. 5.8.7 (a)) in the direction of

the length

For an absolute command, coordinates (X,Z)

For an incremental command, travel distance (Δx, Δz)

i

: Taper amount

If i = 0, ordinary straight threading can be made.

k

: Height of thread

Δd

: Depth of cut in 1st cut

L

: Lead of thread

- 151 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Diameter/radius

Decimal

Unit

Sign

programming

point input

Depends on the increment system

Δdmin

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

d

Radius programming

Not required

Allowed

for the reference axis.

Depends on the increment system

i

Radius programming

Required

Allowed

for the reference axis.

Depends on the increment system

k

Radius programming

Not required

Not allowed

for the reference axis.

Depends on the increment system

Δd

Radius programming

Not required

Not allowed

for the reference axis.

E

(R)

A

(R)

(R)

Δx/2

B

(F)

Δd

D

i

k

X

r

C

Z

Δz

+X

+Z

Fig. 5.8.7 (a) Cutting path in multiple threading cycle

Tool nose

B

a

Δd

Δd√n

1st

2nd

k

3rd

nth

d

Fig. 5.8.7 (b) Detail of cutting

- 152 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Repetitive count in finishing

The last finishing cycle (cycle in which the finishing allowance is removed by cutting) is repeated.

+X

k

+Z

Last finishing cycle

d (finishing allowance)

Fig. 5.8.7 (c)

Explanation

-

Operations

This cycle performs threading so that the length of the lead only between C and D is made as specified in

the F code. In other sections, the tool moves in rapid traverse.

NOTE

1 The meanings of the data specified by address P, Q, and R determined by the

presence of X (U) and Z (W).

2 The cycle machining is performed by G76.7 command with X and Z

specification.

3 The values specified at addresses P, Q, and R are modal and are not changed

until another value is specified.

4 Specify a value smaller than the height of thread as the finishing allowance. (d <

k)

CAUTION

Notes on threading are the same as those on G33 threading. For feed hold in a

threading cycle, however, see "Feed hold in a threading cycle" described below.

-

Relationship between the sign of the taper amount and tool path

The signs of incremental dimensions for the cycle shown in Fig. 5.8.7 (a) are as follows:

Cutting end point in the direction of the length for X and Z:

Minus (determined according to the directions of paths A-C and C-D)

Taper amount (i)

: Minus (determined according to the direction of path A-C)

Height of thread (k)

: Plus (always specified with a plus sign)

Depth of cut in the first cut (Δd)

: Plus (always specified with a plus sign)

The four patterns shown in the Table 5.8.7 (a) are considered corresponding to the sign of each address. A

female thread can also be machined.

- 153 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Table 5.8.7 (a)

Outer diameter machining

Internal diameter machining

1.

Δx < 0, Δz < 0, i < 0

2.

Δx > 0, Δz < 0, i > 0

X

X

Z

Z

Δz

4

(R)

2

(F)

i

Δx/2

3

(R)

1

(R)

X/2

Δx/2

3

(R)

1

(R)

i

X/2

2

(F)

Δz

4

(R)

3.

Δx < 0, Δz < 0, i > 0

4.

Δx > 0, Δz < 0, i <0

at |i |≦ |Δ x / 2|

at |i |≦ |Δ x / 2|

X

X

Z

Δz

Z

4

(R)

1

(R)

i

2

(F)

X/2

Δx/2

3

(R)

Δx/2

3

(R)

2

(F)

1

(R)

i

4

(R)

Δz

X/2

-

Acceleration/deceleration after interpolation for threading

Acceleration/deceleration after interpolation for threading is acceleration/deceleration of exponential

interpolation type. By setting bit 5 (THLx) of parameter No. 1610, the same acceleration/deceleration as

for cutting feed can be selected. (The settings of bits 1 (CTBx) and 0 (CTLx) of parameter No. 1610 are

followed.) However, as a time constant and FL feedrate, the settings of parameter No. 1626 and No. 1627

for the threading cycle are used.

-

Time constant and FL feedrate for threading

The time constant for acceleration/deceleration after interpolation for threading specified in parameter No.

1626 and the FL feedrate specified in parameter No. 1627 are used.

-

Thread chamfering

Thread chamfering can be performed in this threading cycle. A signal from the machine tool initiates

thread chamfering.

The maximum amount of thread chamfering (r) that can be specified in the command is 99 (9.9L). The

amount can be specified in a range from 0.1L to 12.7L in 0.1L increments in parameter No. 5130.

A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a

value of 0 is specified in the parameter, an angle of 45 degrees is assumed.

For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for

acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

-

Retraction after chamfering

The Table 5.8.7 (b) lists the feedrate, type of acceleration/deceleration after interpolation, and time

constant of retraction after chamfering.

Table 5.8.7 (b)

Bit 0 (CFR) of

Parameter No.

parameter No.

Description

1466

1611

Uses the type of acceleration/deceleration after interpolation for threading,

0

Other than 0

time constant for threading (parameter No. 1626), FL feedrate (parameter

No. 1627), and retraction feedrate specified in parameter No. 1466.

- 154 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Bit 0 (CFR) of

Parameter No.

parameter No.

Description

1466

1611

Uses the type of acceleration/deceleration after interpolation for threading,

0

0

time constant for threading (parameter No. 1626), FL feedrate (parameter

No. 1627), and rapid traverse rate specified in parameter No. 1420.

Before retraction a check is made to see that the specified feedrate has

become 0 (delay in acceleration/deceleration is 0), and the type of

1

acceleration/deceleration after interpolation for rapid traverse is used

together with the rapid traverse time constant and the rapid traverse rate

(parameter No. 1420).

By setting bit 4 (ROC) of parameter No. 1403 to 1, rapid traverse override can be disabled for the feedrate

of retraction after chamfering.

NOTE

During retraction, the machine does not stop with an override of 0% for the

cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

-

Shifting the start angle

The threading start angle cannot be shifted.

-

Feed hold in a threading cycle

When the threading cycle retract function is not used, the machine stops at the end point of retraction

after chamfering (point E on the cutting path for a multiple threading cycle) by feed hold applied during

threading.

-

Feed hold when the threading cycle retract function is used

When the "threading cycle retract" optional function is used, feed hold may be applied during threading

in a multiple threading cycle (G76.7). In this case, the tool quickly retracts in the same way as for the last

chamfering in a threading cycle and returns to the start point in the current cycle.

When cycle start is triggered, the multiple threading cycle resumes.

X-axis

Ordinary cycle

Motion at feed hold

Z-axis

Start point

in the current cycle

Rapid traverse

Cutting feed

Feed hold is applied at this point

The angle of chamfering during retraction is the same as that of chamfering at the end point.

CAUTION

Another feed hold cannot be performed during retraction.

-

Inch threading

Inch threading specified with address E is not allowed.

- 155 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Tool nose radius compensation

Tool nose radius compensation cannot be applied.

Example

X axis

Z axis

0

6

25

105

G80 X80.0 Z130.0;

G76.7 P011060 Q100 R200 ;

G76.7 X60.64 Z25.0 P3680 Q1800 F6.0 ;

5.8.8

Restrictions on Multiple Repetitive Cycle (G70.7, G71.7, G72.7,

G73.7, G74.7, G75.7, and G76.7)

Programmed commands

-

Program memory

Programs using G70.7, G71.7, G72.7, or G73.7 must be stored in the program memory. The use of the

mode in which programs stored in the program memory are called for operation enables these programs to

be executed in other than the MEM mode. Programs using G74.7, G75.7, or G76.7 need not be stored in

the program memory.

-

Blocks in which data related to a multiple repetitive cycle is specified

The addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

In a block in which G70.7, G71.7, G72.7, or G73.7 is specified, the following functions cannot be

specified:

• Custom macro calls (simple call, modal call, and subprogram call)

-

Blocks in which data related to a target figure is specified

In the block which is specified by address P of a G71.7, G72.7 or G73.7, G00 or G01 code in group 01

should be commanded. If it is not commanded, alarm PS0065 is generated.

- 156 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Format

-

Tool length compensation A

G43 Z_H_;

Shifts the coordinate system along the Z axis by the compensation value, to the + side.

G44 Z_H_;

Shifts the coordinate system along the Z axis by the compensation value, to the - side.

G43 (or G44) : + (or -) side offset at which to start tool length compensation

H_

: Address specifying the tool length compensation value

-

Tool length compensation B

G17 G43 Z_H_;

Shifts the coordinate system along the Z axis by the compensation value, to the + side.

G17 G44 Z_H_;

Shifts the coordinate system along the Z axis by the compensation value, to the - side.

G18 G43 Y_H_;

Shifts the coordinate system along the X axis by the compensation value, to the + side.

G18 G44 Y_H_;

Shifts the coordinate system along the X axis by the compensation value, to the - side.

G19 G43 X_H_;

Shifts the coordinate system along the Y axis by the compensation value, to the + side.

G19 G44 X_H_;

Shifts the coordinate system along the Y axis by the compensation value, to the - side.

G17 (or G18, G19)

: Plane selection

G43 (or G44)

:

+ (or -) side offset at which to start tool length compensation

H_

: Address specifying the tool length compensation value

-

Tool length compensation C

G43 α_H_;

Shifts the coordinate system along a specified axis by the compensation value, to the + side.

G44 α_H_;

Shifts the coordinate system along a specified axis by the compensation value, to the - side.

G43 (or G44) : + (or -) side offset at which to start tool length compensation

α_

: Address of any one axis

H_

: Address specifying the tool length compensation value

-

Tool length compensation cancel

G49; or H0; Tool length compensation cancel

G49 (or H0)

: Tool length compensation cancel

Explanation

-

Offset direction

If the tool length compensation value specified with an H code (and stored in offset memory) is G43, the

coordinate system is shifted to the + side; if G44, to the - side. If the sign of the tool length compensation

value is -, the coordinate system is shifted to the - side if G43 and to the + side if G44. G43 and G44 are

modal G codes; they remain valid until another G code in the same group is used.

-

Specifying a tool length compensation value

The tool length compensation value corresponding to the number (offset number) specified with an H

code (and stored in offset memory) is used. The tool length compensation corresponding to the offset

number 0 always means 0. It is not possible to set a tool length compensation value corresponding to H0.

- 159 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

Example in which overcutting occurs in cutter compensation)

Overcutting may occur if tool length compensation is started or canceled in cutter compensation mode.

:

G40 G49 G00 G90 X0 Y0 Z100. ;

N1 G42 G01 X10. Y10. F500 D1 ;

Start of cutter compensation

N2 G43 Z0. H2 ;

Start of tool length compensation

N3 X100. ;

N4 Y100. ;

N5 X10. ;

N6 Y10. ;

N7 G49 Z100. ;

Cancellation of tool length compensation

N8 #100=#5023 ;

Custom macro command

N9 G40 X0 Y0 ;

Cancellation of cutter compensation

:

N2 contains G43 (start of tool length compensation) in cutter compensation (G42) mode and, therefore,

look-ahead of N3 and subsequent blocks is not performed.

As a result,

• Deceleration to a stop is performed between N2 and N3.

• The cutter compensation vector at the end point of N1 is vertical to block N1.

(Overcutting may occur.)

If it is assumed that look-ahead is performed, the vector is vertical to the start point of N2, and no

overcutting occurs.

Cutter compensation vector if look-ahead is not

Tool center path if look-ahead

performed

is not performed

Path specified by the

program

Tool

Tool center path if look-ahead is

Cutter compensation vector if

performed

look-ahead is performed

N7 contains G49 (cancellation of tool length compensation) in G42 mode and, therefore, look-ahead of

N8 and subsequent blocks is not performed.

As a result,

• Deceleration to a stop is performed at the end point of N7.

• The custom macro command in N8 is executed after the end of N7. This means that in this example,

variable #100 will be the machine coordinate on the Z-axis at the end point position of N7. (Variable

#5023: Machine coordinate on the third axis)

If it is assumed that look-ahead is performed, N8 is executed at the point the look-ahead of N8 is

performed, that is, before the end of N7, so that variable #100 will be a position before the end point

of N7.

• The cutter compensation vector at the end point of N6 is vertical to block N6.

(Overcutting or undercutting may occur.)

- 161 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

CAUTION

12 When a tool length compensation shift type is used, if the start or cancellation of

a tool length compensation or other command is specified tool radius ⋅ tool nose

radius compensation mode, look-ahead is not performed. As a result, overcutting

or undercutting may occur before or after the block in which the start or

cancellation is specified. Thus, specify the start and cancellation of tool length

compensation before the entry to tool radius ⋅ tool nose radius compensation

mode or at a location where machining is not affected.

6.2

AUTOMATIC TOOL LENGTH MEASUREMENT (G37)

By issuing G37 the tool starts moving to the measurement position and keeps on moving till the approach

end signal from the measurement device is output. Movement of the tool is stopped when the tool nose

reaches the measurement position.

Difference between coordinate value when tool reaches the measurement position and coordinate value

commanded by G37 is added to the tool length compensation amount currently used.

Z

A (Start point)

Rapid

Measurement position is commanded

traverse

with G37

B (Deceleration position)

Measurement

feedrate

C (Measurement position)

The tool stops when the approach end

signal goes on.

X

0

Compensation value = (Current compensation value) + [(Coordinates of the

point at which the tool is stopped) - (Coordinates of the programmed measure

ment position)]

Fig. 6.2 (a) Automatic tool length measurement

Format

G92 IP_ ;

Sets the workpiece coordinate system.

(It can be set with G54 to G59. See Chapter "Coordinate System" in

OPERATOR’S MANUAL (Common to T/M series.))

Hxx ;

Specifies an offset number for tool length compensation.

G90 G37 IP_ ; Absolute programming

G37 is valid only in the block in which it is specified.

IP_ indicates the X-, Y-, Z-, or fourth axis.

Explanation

-

Setting the workpiece coordinate system

Set the workpiece coordinate system so that a measurement can be made after moving the tool to the

measurement position. The coordinate system must be the same as the workpiece coordinate system for

programming.

-

Specifying G37

Specify the absolute coordinates of the correct measurement position.

- 165 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Execution of this command moves the tool at the rapid traverse rate toward the measurement position,

reduces the federate halfway, then continuous to move it until the approach end signal from the measuring

instrument is issued. When the tool nose reaches the measurement position, the measuring instrument

sends an approach end signal to the CNC which stops the tool.

-

Changing the offset value

The difference between the coordinates of the position at which the tool reaches for measurement and the

coordinates specified by G37 is added to the current tool length compensation value. (If bit 6 (MDC) of

parameter No. 6210 is 1, it is subtracted.)

Offset value =

(Current compensation value)

+ [(Coordinates of the position at which the tool reaches for

measurement) - (Coordinates specified by G37)]

These offset values can be manually changed from MDI.

-

Alarm

When automatic tool length measurement is executed, the tool moves as shown in Fig. 6.2 (b). If the

approach end signal turns 1 while the tool is traveling from point B to point C, an alarm occurs. Unless

the approach end signal turns 1 before the tool reaches point F, the same alarm occurs. The alarm number

is PS0080.

Deceleration

feedrate

Rapid

(measurement

Approach end signal ON

traverse

feedrate)

A

B

Start

C

D

E F

point

Position commanded

by G37

Permitted range of approach end signal

Fig. 6.2 (b) Tool movement to the measurement position

WARNING

When a manual movement is inserted into a movement at a measurement

federate, return the tool to the position before the inserted manual movement for

restart.

NOTE

1 When an H code is specified in the same block as G37, an alarm is generated.

Specify H code before the block of G37.

2 The measurement speed (FP), γ, and ε are set as parameters (FP: No. 6241, γ:

No. 6251, ε: No. 6254) by the machine tool builder. Make settings so that e are

always positive and γ are always greater than ε.

3 When tool offset memory A is used, the offset value is changed. When tool offset

memory B is used, the tool wear compensation value is changed. When tool

offset memory C is used, the tool wear compensation value for the H code is

changed.

- 166 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

NOTE

4 A delay or variation in detection of the measurement position arrival signal is 0 to

2 msec on the CNC side excluding the PMC side (0.1 msec or less for

high-speed measurement position arrival signal input (optional)). Therefore, the

measurement error is the sum of 2 msec and a delay or variation (including a

delay or variation on the receiver side) in propagation of the skip signal on the

PMC side, multiplied by the feedrate set in parameter No. 6241.

5 A delay or variation in time after detection of the measurement position arrival

signal until a feed stops is 0 to 8 msec. To calculate the amount of overrun,

further consider a delay in acceleration/deceleration, servo delay, and delay on

the PMC side.

Example

G92 Z760.0 X1100.0 ; Sets a workpiece coordinate system with respect to the programmed absolute

zero point.

G00 G90 X850.0 ;

Moves the tool to X850.0.

That is the tool is moved to a position that is a specified distance from the

measurement position along the Z-axis.

H01 ;

Specifies offset number 1.

G37 Z200.0 ;

Moves the tool to the measurement position.

G00 Z204.0 ;

Retracts the tool a small distance along the Z-axis.

For example, if the tool reaches the measurement position with Z198.0;, the compensation value must be

corrected. Because the correct measurement position is at a distance of 200 mm, the compensation value

is lessened by 2.0 mm (198.0 - 200.0 = -2.0).

Z

760

200

Measurement

position along Z axis

0

850

1100

X

- 167 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

6.3

TOOL OFFSET (G45 TO G48)

The programmed travel distance of the tool can be increased or decreased by a specified tool offset value

or by twice the offset value.

The tool offset function can also be applied to an additional axis.

Workpiece

Tool center path

Programmed path

Tool

Format

G45 IP_ D_ ; Increase the travel distance by the tool offset value

G46 IP_ D_ ; Decrease the travel distance by the tool offset value

G47 IP_ D_ ; Increase the travel distance by twice the tool offset value

G48 IP_ D_ ; Decrease the travel distance by twice the tool offset value

G45 to 48 : One-shot G code for increasing or decreasing the travel distance

IP_

: Command for moving the tool

D_

Code for specifying the tool offset value

Explanation

-

Increase and decrease

As shown in Table 6.3 (a), the travel distance of the tool is increased or decreased by the specified tool

offset value.

In the absolute mode, the travel distance is increased or decreased as the tool is moved from the end point

of the previous block to the position specified by the block containing G45 to G48.

Table 6.3 (a) Increase and decrease of the tool travel distance

G code

When a positive tool offset value is specified

When a negative tool offset value is specified

Start point

End point

Start point

End point

G45

Start point

End point

Start point

End point

G46

- 168 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

G code

When a positive tool offset value is specified

When a negative tool offset value is specified

Start point

End point

Start point

End point

G47

Start point

End point

Start point

End point

G48

Programmed movement distance

Tool offset value

Actual movement position

If a move command with a travel distance of zero is specified in the incremental programming (G91)

mode, the tool is moved by the distance corresponding to the specified tool offset value.

If a move command with a travel distance of zero is specified in the absolute programming (G90) mode,

the tool is not moved.

-

Tool offset value

Once selected by D code, the tool offset value remains unchanged until another tool offset value is

selected.

Tool offset values can be set within the following range:

D0 always indicates a tool offset value of zero.

- 169 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64484EN-2/02

CAUTION

1 When G45 to G48 is specified to n axes (n=1-6) simultaneously in a motion

block, offset is applied to all n axes.

When the cutter is offset only for cutter radius or diameter in taper cutting,

overcutting or undercutting occurs.

Therefore, use cutter compensation (G40 or G42) shown in II-6.4 or 6.6.

Shape actually cut

Desired

shape

Y axis

Overcutting

X axis

G01 X_ F_ ;

G47 X_ Y_ D_ ;

Y_ ;

Desired shape

Shape actually cut

Y axis

Undercutting

X axis

G01 G45 X_ F_ D_;

X_ Y_ ;

G45 Y_ ;

2 G45 to G48 (tool offset) must not be used in the G41 or G42 (cutter

compensation) mode.

- 170 -

B-64484EN-2/02

PROGRAMMING

6.COMPENSATION FUNCTION

NOTE

1 When the specified direction is reversed by decrease, the tool moves in the

opposite direction.

Movement of the

Program command

Start

End

position

position

Tool offset value

Example

G46 X2.50 ;

Tool offset value

Equivalent command

+3.70

X-1.20 ;

2

Tool offset can be applied to circular interpolation (G02, G03) with the G45 to

G48 commands only for 1/4 and 3/4 circles using addresses I, J and K by the

parameter setting, providing that the coordinate system rotation be not specified

at the same time. This function is provided for compatibility with the conventional

CNC program without any cutter compensation. The function should not be used

when a new CNC program is prepared.

Tool offset for circular interpolation

N4

N3

Programmed tool path

N2

Program

Actual tool path

N1 G46 G00 X_ Y_ D_ ;

N2 G45 G01 Y_ F_ ;

N1

N3 G45 G03 X_ Y_ I_ ;

N4 G01 X_ ;

3

D code should be used in tool offset mode.

4

G45 to G48 are ignored in canned cycle mode. Perform tool offset by specifying

G45 to G48 before entering canned cycle mode and cancel the offset after

releasing the canned cycle mode.

- 171 -

Content      ..     4      5      6      7     ..