Content      ..     2      3      4      5     ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 4

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Small-hole peck drilling cycle (G83)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in

small-hole peck drilling cycle.

G83 X_ Y_ Z_ R_ Q_ F_I_ K_P_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

Q_

: Depth of cut for each cutting feed

F_

: Cutting feedrate

I_

: Forward or backward traveling speed (same format as F above)

(If this is omitted, the values in parameters Nos. 5172 and 5173 are assumed as

defaults.)

K_

: Number of repeats (When it is needed)

P_

: Dwell time at the bottom of a hole

(If this is omitted, P0 is assumed as the default.)

G83(G98)

G83(G99)

Initial level

Point R

Point R

Q

Q

Overload torque

Overload torque

Point Z

Point Z

Dwell

Dwell

Δ: Initial clearance when the tool is retracted to point R and the clearance from the bottom of the hole in the second or

subsequent drilling (parameter 5174)

q: Depth of each cut

Path along which the tool travels at the rapid traverse rate

Path along which the tool travels at the programmed cutting feedrate

Path along which the tool travels at the forward or backward rate during the cycle specified with parameters

(

)

In-position width for other than hole bottoms (regular)

In-position width for other than hole bottoms (for retraction in peck drilling cycle)

In-position width for hole bottoms

NOTE

When setting an effective area (for in-position check) enclosed in

, pay

attention to the clearance Δ (parameter No.5174). If the effective area is too

large for the retraction distance, it is likely that no retraction may be performed.

- 82 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Tapping cycle (G84)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in tapping

cycle.

G84 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G84(G98)

G84(G99)

Initial level

Spindle CW

Spindle CW

P

Point R

P

Point R

Point R level

P

Point Z

P

Point Z

Spindle CCW

Spindle CCW

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

CAUTION

When resuming the initial level, set an effective area (for in-position check)

enclosed in

, pay attention to the distance between point R and the

workpiece. If the effective area is too large for the distance between point R

and the workpiece, it is likely that the workpiece or tool may be damaged,

because a rapid traverse may occur before the tool retracts completely from the

workpiece.

NOTE

Enabling an in-position check at hole bottoms requires setting bit 6 of

parameter No. 5103 to 1.

- 83 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Boring cycle (G85)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in boring

cycle.

G85 X_ Y_ Z_ R_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G85(G98)

G85(G99)

Initial level

Point R

Point R

Point R level

Point Z

Point Z

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

CAUTION

When resuming the initial level, set an effective area (for in-position check)

enclosed in

, pay attention to the distance between point R and the

workpiece. If the effective area is too large for the distance between point R

and the workpiece,a rapid traverse may occur before the tool retracts completely

from the workpiece. Enabling an in-position check at hole bottoms requires using

the exact stop mode (G61).

- 84 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Boring cycle (G86)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in boring

cycle.

G86 X_ Y_ Z_ R_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G86(G98)

G86(G99)

Spindle CW

Initial level

Spindle CW

Point R

Point R

Point R level

Point Z

Point Z

Spindle stop

Spindle stop

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

- 85 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Back boring cycle (G87)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in back

boring cycle.

G87 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the

hole

R_

: The distance from the initial level to point R

level

Q_

: Shift amount at the bottom of a hole

P_

: Dwell time at the bottom of a hole

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G87(G98)

G87(G99)

Spindle orientation

Q Initial level

Tool

OSS

Spindle CW

Not used

OSS

Point Z

P

Spindle CW

Point

Shift amount q

In-position width for other than hole bottoms (for shift in boring cycles (G76 and G87)

In-position width for hole bottoms

CAUTION

When setting an effective area (for in-position check) enclosed in

, pay

attention to the distance between point R and the workpiece and the orientation

of the spindle. If too large an effective area is set, a shortcut is taken, resulting

in the tool interfering with the workpiece during rapid traverse.

A shortcut is taken, resulting in the

tool interfering with the workpiece.

- 86 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Boring cycle (G88)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in boring

cycle.

G88 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of a hole

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G88(G98)

G88(G99)

Spindle CW

Initial level

Spindle CW

Point R

Point R level

Point R

Point Z

Point Z

P

Spindle stop

P

Spindle stop

after dwell

after dwell

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

- 87 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Boring cycle (G89)

M

Shown below are the points where a dedicated effective area (for in-position check) is applied in boring

cycle.

G89 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of a hole

F_

: Cutting feedrate

K_

: Number of repeats (When it is needed)

G89(G98)

G89(G99)

Initial level

Point R

Point R

Point R level

Point Z

Point Z

P

P

In-position width for other than hole bottoms (regular)

In-position width for hole bottoms

- 88 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.3

RIGID TAPPING

The tapping cycle (G84) and left-handed tapping cycle (G74) may be performed in standard mode or rigid

tapping mode.

In standard mode, the spindle is rotated and stopped along with a movement along the tapping axis using

auxiliary functions M03 (rotating the spindle clockwise), M04 (rotating the spindle counterclockwise),

and M05 (stopping the spindle) to perform tapping.

In rigid mode, tapping is performed by controlling the spindle motor as if it were a servo motor and by

interpolating between the tapping axis and spindle.

When tapping is performed in rigid mode, the spindle rotates one turn every time a certain feed (thread

lead) which takes place along the tapping axis. This operation does not vary even during acceleration or

deceleration.

Rigid mode eliminates the need to use a floating tap required in the standard tapping mode, thus allowing

faster and more precise tapping.

5.3.1

Rigid Tapping (G84)

When the spindle motor is controlled in rigid mode as if it were a servo motor, a tapping cycle can be

sped up.

Format

G84 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole and the position of the bottom of

the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of the hole and at point R when a return is made

F_

: Cutting feedrate

K_

: Number of repeats (if required)

G84.2 X_ Y_ Z_ R_ P_ F_ L_ ;

(Series 15 format)

L_

: Number of repeats (if required)

G84 (G98)

G84 (G99)

Spindle stop

Spindle stop

Initial level

Operation 1

Operation 6

Spindle stop

Operation 2

Spindle

Spindle CW

P

Spindle CW

P

stop

Point R

Point R level

Point R

Point R level

Operation 3

Operation 5

Point Z

Point Z

P

P

Spindle stop

Spindle CCW

Spindle stop

Spindle CCW

Operation 4

- 89 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Interlock

Interlock can also be applied in G84 (G74).

-

Feed hold and single block

When bit 6 (FHD) of parameter No. 5200 is set to 0, feed hold and single block are invalid in the G84

(G74) mode. When this bit is set to 1, they are valid.

-

Manual feed

For rigid tapping by manual handle feed, see the section "Rigid Tapping by Manual Handle."

With other manual operations, rigid tapping cannot be performed.

-

Backlash compensation

In the rigid tapping mode, backlash compensation is applied to compensate the lost motion when the

spindle rotates clockwise or counterclockwise. Set the amount of backlash in parameters Nos. 5321 to

5324.

Along the drilling axis, backlash compensation has been applied.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed

in rigid mode, alarm PS0206 is issued.

-

S command

• If a speed higher than the maximum speed for the gear being used is specified, alarm PS0200 is

issued.

• When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to

S0.

-

Distribution amount for the spindle

The maximum distribution amount is as follows (displayed on diagnosis data No. 451):

• For a serial spindle: 32,767 pulses per 8 ms

This amount is changed according to the gear ratio setting for the position coder or rigid tapping

command. If a setting is made to exceed the upper limit, alarm PS0202 is issued.

-

F command

If a value exceeding the upper limit of cutting feedrate is specified, alarm PS0011 is issued.

-

Unit of F command

Metric input

Inch input

Remarks

G94

1 mm/min

0.01 inch/min

Decimal point programming allowed

G95

0.01 mm/rev

0.0001 inch/rev

Decimal point programming allowed

-

M29

If an S command and axis movement are specified between M29 and G84, alarm PS0203 is issued. If

M29 is specified in a tapping cycle, alarm PS0204 is issued.

-

P

Specify P in a block that performs drilling. If P is specified in a non-drilling block, it is not stored as

modal data.

- 91 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.3.2

Left-Handed Rigid Tapping Cycle (G74)

When the spindle motor is controlled in rigid mode as if it were a servo motor, tapping cycles can be

speed up.

Format

G74 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole and the position of the bottom of

the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of the hole and at point R when return is made.

F_

: Cutting feedrate

K_

: Number of repeats (if required)

G84.3 X_ Y_ Z_ R_ P_ F_ L_ ;

(Series 15 format)

L_

: Number of repeats (if required)

G74 (G98)

G74 (G99)

Spindle stop

Spindle stop

Initial level

Operation 1

Operation 2

Operation 6

Spindle stop

Spindle CCW

Spindle CCW

Spindle

P

stop

P

Point R

Point R level

Point R

Point R level

Operation 3

Operation 5

Point Z

Point Z

P

P

Spindle stop

Spindle CW

Spindle stop

Spindle CW

Operation 4

Explanation

After positioning along the X- and Y-axes, rapid traverse is performed to point R.

Tapping is performed from point R to point Z. When tapping is completed, the spindle is stopped and a

dwell is performed. The spindle is then rotated in the normal direction, the tool is retracted to point R,

then the spindle is stopped. Rapid traverse to initial level is then performed.

While tapping is being performed, the feedrate override and spindle override are assumed to be 100%.

Feedrate override can be enabled by setting, however.

-

Rigid mode

Rigid mode can be specified using any of the following methods:

• Specify M29 S***** before a tapping command.

• Specify M29 S***** in a block which contains a tapping command.

• Specify G74 for rigid tapping. (bit 0 (G84) of parameter No. 5200 set to1).

-

Thread lead

In feed-per-minute mode, the thread lead is obtained from the expression, feedrate ÷ spindle speed. In

feed-per-revolution mode, the thread lead equals the feedrate.

- 93 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed

in rigid mode, alarm PS0206 is issued.

-

S command

• Specifying a rotation speed exceeding the maximum speed for the gear used causes alarm PS0200.

• When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to

S0.

-

Distribution amount for the spindle

The maximum distribution amount is as follows (displayed on diagnosis data No. 451):

• For a serial spindle: 32,767 pulses per 8 ms

This amount is changed according to the gear ratio setting for the position coder or rigid tapping

command. If a setting is made to exceed the upper limit, alarm PS0202 is issued.

-

F command

Specifying a value that exceeds the upper limit of cutting feedrate causes alarm PS0011.

-

Unit of F command

Metric input

Inch input

Remarks

G94

1 mm/min

0.01 inch/min

Decimal point programming allowed

G95

0.01 mm/rev

0.0001 inch/rev

Decimal point programming allowed

-

M29

Specifying an S command or axis movement between M29 and G84 causes alarm PS0203.

Then, specifying M29 in the tapping cycle causes alarm PS0204.

-

P

Specify P in a block that performs drilling. If P is specified in a non-drilling block, it is not stored as

modal data.

-

Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No.

5431 is set to 1)) and G74 in a single block. Otherwise, G74 will be canceled.

-

Tool offset

In the canned cycle mode, tool offsets are ignored.

-

Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

Example

Z-axis feedrate

1000 mm/min

Spindle speed

1000 min^-1

Thread lead

1.0 mm

<Programming for feed per minute>

G94 ;

Specify a feed-per-minute command.

G00 X120.0 Y100.0 ;

Positioning

M29 S1000 ;

Rigid mode specification

G74 Z-100.0 R-20.0 F1000 ; Rigid tapping

<Programming for feed per revolution>

G95 ;

Specify a feed-per-revolution command.

- 95 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.3.3

Peck Rigid Tapping Cycle (G84 or G74)

Tapping a deep hole in rigid tapping mode may be difficult due to chips sticking to the tool or increased

cutting resistance. In such cases, the peck rigid tapping cycle is useful.

In this cycle, cutting is performed several times until the bottom of the hole is reached. Two peck tapping

cycles are available: High-speed peck tapping cycle and standard peck tapping cycle. These cycles are

selected using the PCP bit (bit 5) of parameter 5200.

Format

G84 (or G74) X_ Y_ Z_ R_ P_ Q_ F_ K_ ;

X_ Y_ : Hole position data

Z_

: The distance from point R to the bottom of the hole

and the position of the bottom of the hole

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of the hole and at point R

when a return is made

Q_

: Depth of cut for each cutting feed

F_

: The cutting feedrate

K_

: Number of repeats (if required)

G84.2 (or G84.3) X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

(Series 15 format)

L_

: Number of repeats (if required)

G84, G74 (G98)

G84, G74 (G99)

• High-speed peck tapping cycle (Bit

d = retraction distance

5 (PCP) of parameter No. 5200=0)

<1> The tool operates at a normal

Initial level

cutting feedrate. The normal

time constant is used.

Point R

Point R level

Point R

Point R level

<2> Retraction can be overridden.

q

<1>

q

<1>

The retraction time

<2>

d

<2>

d

constant is used.

q

q

d

d

q

q

Point Z

Point Z

• Peck tapping cycle

d = cutting start distance

(Bit 5 (PCP) of parameter No.

5200=1)

Initial level

<1> The tool operates at a normal

cutting feedrate. The normal

Point R

Point R level

Point R

Point R level

<3>

<3>

time constant is used.

‡

‡

<1>

<1>

q

q

<2> Retraction can be overridden.

<2>

d

<2>

d

The retraction time constant is

q

q

used.

d

d

<3> Retraction can be overridden.

q

q

The normal time constant is

used.

Point Z

Point Z

- 97 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

Manual feed

For rigid tapping by manual handle feed, see the section “Rigid Tapping by Manual Handle.”

With other manual operations, rigid tapping cannot be performed.

-

Backlash compensation

In the rigid tapping mode, backlash compensation is applied to compensate the lost motion when the

spindle rotates clockwise or counterclockwise. Set the amount of backlash in parameters Nos. 5321 to

5324.

Along the drilling axis, backlash compensation has been applied.

Limitation

-

Axis switching

Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed

in rigid mode, alarm PS0206 is issued.

-

S command

• Specifying a rotation speed exceeding the maximum speed for the gear used causes alarm PS0200.

• When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to

S0.

-

Distribution amount for the spindle

The maximum distribution amount is as follows (displayed on diagnosis data No. 451):

• For a serial spindle: 32,767 pulses per 8 ms

This amount is changed according to the gear ratio setting for the position coder or rigid tapping

command. If a setting is made to exceed the upper limit, alarm PS0202 is issued.

-

F command

Specifying a value that exceeds the upper limit of cutting feedrate causes alarm PS0011.

-

Unit of F command

Metric input

Inch input

Remarks

G94

1 mm/min

0.01 inch/min

Decimal point programming allowed

G95

0.01 mm/rev

0.0001 inch/rev

Decimal point programming allowed

-

M29

Specifying an S command or axis movement between M29 and G84 causes alarm PS0203.

Then, specifying M29 in the tapping cycle causes alarm PS0204.

-

P/Q

Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform

drilling, they are not stored as modal data.

When Q0 is specified, the peck rigid tapping cycle is not performed.

-

Cancel

Do not specify a group 01 G code (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No. 5431 is

set to 1)) and G84 in the same block. If they are specified together, G84 is canceled.

-

Tool offset

In the canned cycle mode, tool offsets are ignored.

-

Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

- 99 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

-

Amount of return and cutting start distance

Set the amount of return and the cutting start distance (No. 5213) so that point R is not exceeded.

5.3.4

Canned Cycle Cancel (G80)

The rigid tapping canned cycle is canceled. For how to cancel this cycle, see the Subsection 5.1.14,

"Canned Cycle Cancel for Drilling (G80)."

NOTE

When the rigid tapping canned cycle is cancelled, the S value used for rigid

tapping is also cleared (as if S0 is specified).

Accordingly, the S command specified for rigid tapping cannot be used in a

subsequent part of the program after the cancellation of the rigid tapping canned

cycle.

After canceling the rigid tapping canned cycle, specify a new S command as

required.

5.3.5

Override during Rigid Tapping

Various types of override functions are invalid. The following override functions can be enabled by

setting corresponding parameters:

• Extraction override

• Override signal

5.3.5.1 Extraction override

For extraction override, the fixed override set in the parameter or override specified in a program can be

enabled at extraction (including retraction during peck drilling/high-speed peck drilling).

Explanation

-

Specifying the override in the parameter

Set bit 4 (DOV) of parameter No. 5200 to 1 and set the override in parameter No. 5211.

An override from 0% to 200% in 1% steps can be set. Bit 3 (OVU) of parameter No. 5201 can be set to 1

to set an override from 0% to 2000% in 10% steps.

-

Specifying the override in a program

Set bit 4 (DOV) of parameter No. 5200 and bit 4 (OV3) of parameter No. 5201 to 1. The spindle speed at

extraction can be specified in the program.

Specify the spindle speed at extraction using address "J" in the block in which rigid tapping is specified.

Example) To specify 1000 min^-1 for S at cutting and 2000 min^-1 for S at extraction

M29 S1000 ;

G84 Z-100. F1000. J2000 ;

The difference in the spindle speed is converted to the actual override by the following calculation.

Therefore, the spindle speed at extraction may not be the same as that specified at address "J". If the

override does not fall in the range between 100% and 200%, it is assumed to be 100%.

Spindle speed at extraction (specified at

J)

Override (% )

=

×100

Spindle speed (specified at

S

)

- 100 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

The override to be applied is determined according to the setting of parameters and that in the command

as shown in the Table 5.3.5.1 (a).

Table 5.3.5.1 (a)

Parameter setting

DOV = 1

DOV = 0

Command

OV3 = 1

OV3 = 0

Within the range between 100%

Command in the program

Spindle speed at extraction

to 200%

Parameter

specified at address "J"

Outside the range between

100%

100%

No. 5211

100% to 200%

No spindle speed at extraction specified at address "J"

Parameter No. 5211

NOTE

1

Do not use a decimal point in the value specified at address "J".

If a decimal point is used, the value is assumed as follows:

Example)

When the increment system for the reference axis is IS-B

• When pocket calculator type decimal point programming is not used

The specified value is converted to the value for which the least input

increment is considered.

"J200." is assumed to be 200000 min^-1.

• When pocket calculator type decimal point programming is used

The specified value is converted to the value obtained by rounding down

to an integer.

"J200." is assumed to be 200 min^-1.

2

Do not use a minus sign in the value specified at address "J".

If a minus sign is used, a value outside the range between 100% to 200% is

assumed.

3

The maximum override is obtained using the following equation so that the

spindle speed to which override at extraction is applied do not exceed the

maximum used gear speed (specified in parameters Nos. 5241 to 5244). For this

reason, the obtained value is not the same as the maximum spindle speed

depending on the override.

Maximum spindle speed (specified in

parameters

)

Maximum override (%)

=

×

100

Spindle speed (specified at

S

)

4

When a value is specified at address "J" for specifying the spindle speed at

extraction in the rigid tapping mode, it is valid until the canned cycle is canceled.

5.3.5.2 Override signal

By setting bit 4 (OVS) of parameter No. 5203 to 1, override can be applied to cutting/extraction operation

during rigid tapping as follows:

• Applying override using the feedrate override signal

(When the second feedrate override signal turns 1, the second feedrate override is applied to the

feedrate to which feedrate override is applied.)

• Canceling override using the override cancel signal

There are the following relationships between this function and override to each operation:

• At cutting

-

When the override cancel signal is set to 0: value specified by the override signal

-

When the override cancel signal is set to 1: 100%

- 101 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

5.4

OPTIONAL CHAMFERING AND CORNER R

Overview

Chamfering and corner R blocks can be inserted automatically between the following:

• Between linear interpolation and linear interpolation blocks

• Between linear interpolation and circular interpolation blocks

• Between circular interpolation and linear interpolation blocks

• Between circular interpolation and circular interpolation blocks

Format

, C_ Chamfering

, R_ Corner R

Explanation

When the above specification is added to the end of a block that specifies linear interpolation (G01) or

circular interpolation (G02 or G03), a chamfering or corner R block is inserted.

Blocks specifying chamfering and corner R can be specified consecutively.

-

Chamfering

After C, specify the distance from the hypothetical corner intersection to the start and end points. The

hypothetical corner point is the corner point that would exist if chamfering were not performed.

<1> G91 G01 X100.0 ,C10.0 ;

<2> X100.0 Y100.0 ;

Inserted chamfering block

C

C

Hypothetical corner intersection

-

Corner R

After R, specify the radius for corner R.

<1> G91 G01 X100.0 ,R10.0 ;

<2> X100.0 Y100.0 ;

Center of a circle with radius R

R

Inserted corner R

block

Example

N001 G92 G90 X0 Y0 ;

N002 G00 X10.0 Y10.0 ;

N003 G01 X50.0 F10.0 ,C5.0 ;

N004 Y25.0 ,R8.0 ;

N005 G03 X80.0 Y50.0 R30.0 ,R8.0 ;

N006 G01 X50.0 ,R8.0 ;

- 103 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

N007 Y70.0 ,C5.0 ;

N008 X10.0 ,C5.0 ;

N009 Y10.0 ;

N010 G00 X0 Y0 ;

N011 M0;

Y

N008

70.0

N007

60.0

N006

50.0

40.0

N009

N005

30.0

20.0

N004

10.0

N003

N010

N002

N011

0

N001

X

10.0

20.0

30.0

40.0

50.0

60.0

70.0

80.0

Limitation

-

Invalid specification

Chamfering (,C) or corner R (,R) specified in a block other than a linear interpolation (G01) or circular

interpolation (G02 or G03) block is ignored.

-

Next block

A block specifying chamfering or corner R must be followed by a block that specifies a move command

using linear interpolation (G01) or circular interpolation (G02 or G03). If the next block does not contain

these specifications, alarm PS0051 is issued.

Between these blocks, however, only one block specifying G04 (dwell) can be inserted. The dwell is

executed after execution of the inserted chamfering or corner R block.

-

Exceeding the move range

If the inserted chamfering or corner R block causes the tool to go beyond the original interpolation move

range, alarm PS0055 is issued.

G91 G01 X30.0 ;

G03 X7.5 Y16.0 R37.0 ,C28.0 ;

G03 X67.0 Y-27.0 R55.0 ;

C

C

The tool path without

chamfering is indicated

with a solid line.

Chamfering block to be inserted

Fig 5.4 (a) Exceeding the move range

- 104 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.5

INDEX TABLE INDEXING FUNCTION

By specifying indexing positions (angles) for the indexing axis (one rotation axis, A, B, or C), the index

table of the machining center can be indexed.

Before and after indexing, the index table is automatically unclamped or clamped .

Explanation

-

Indexing position

Specify an indexing position with address A, B, or C (set to bit 0 (ROTx) of parameter No. 1006).

The indexing position is specified by either of the following (depending on bit 4 of parameter G90

No.5500):

1.

Absolute value only

2.

Absolute or incremental value depending on the specified G code: G90 or G91

A positive value indicates an indexing position in the counterclockwise direction. A negative value

indicates an indexing position in the clockwise direction.

The minimum indexing angle of the index table is the value set to parameter 5512. Only multiples of the

least input increment can be specified as the indexing angle. If any value that is not a multiple is specified,

an alarm PS1561 occurs. Decimal fractions can also be entered. When a decimal fraction is entered, the

1's digit corresponds to degree units.

A

Value specified for rotation from A to B

(case 2 described above)

G90 B-45.0 ; or

G91 B-105.0;

+60°

0°

-45°

B

-

Direction and value of rotation

The direction of rotation and angular displacement are determined by either of the following two methods.

Refer to the manual written by the machine tool builder to find out which method is applied.

1.

Using the auxiliary function specified in parameter No.

5511 (Address)

(Indexing position)

(Miscellaneous function); Rotation in the negative direction (Address) (Indexing position); Rotation

in the positive direction (No auxiliary functions are specified.)

An angular displacement greater than

360° is rounded down to the corresponding angular

displacement within 360° when bit 2 (ABS) of parameter No. 5500 specifies this option.

For example, when G90 B400.0 (auxiliary function); is specified at a position of 0 , the table is

rotated by 40° in the negative direction.

2.

Using no auxiliary functions

By setting to bits 2 (ABS), 3 (INC), and 4 (G90) of parameter No. 5500, operation can be selected

from the following two options.

Select the operation by referring to the manual written by the machine tool builder.

(1) Rotating in the direction in which an angular displacement becomes shortest

This is valid only in absolute programming. A specified angular displacement greater than 360°

is rounded down to the corresponding angular displacement within 360° when bit 2 (ABS) of

parameter No. 5500 specifies this option.

For example, when G90 B400.0; is specified at a position of 0, the table is rotated by 40° in the

positive direction.

- 106 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

(2) Rotating in the specified direction

In the absolute programming, the value set in bit 2 (ABS) of parameter No. 5500 determines

whether an angular displacement greater than 360° is rounded down to the corresponding

angular displacement within 360°.

In the incremental programming, the angular displacement is not rounded down. For example,

when G90 B720.0; is specified at a position of 0, the table is rotated twice in the positive

direction, when the angular displacement is not rounded down.

-

Feedrate

The table is always rotated around the indexing axis in the rapid traverse mode.

Dry runs cannot be executed for the indexing axis.

WARNING

1 If a reset is made during indexing of the index table, a reference position return

must be made before each time the index table is indexed subsequently.

2 For a path on which the index table indexing function is not to be used, disable

the index table indexing function (set bit 0 (ITI) of parameter No. 5501 to 0).

NOTE

1 If an index table indexing axis and another controlled axis are specified in the

same block either alarm PS1564 is issued or the command is executed,

depending on bit 6 (SIM) of parameter No. 5500 and bit 0 (IXS) of parameter No.

5502.

2 The waiting state which waits for completion of clamping or unclamping of the

index table is indicated on diagnosis data No.12.

3 The auxiliary function specifying a negative direction is processed in the CNC.

The relevant M code signal and completion signal are sent between the CNC

and the machine.

4 If a reset is made while waiting for completion of clamping or unclamping, the

clamp or unclamp signal is cleared and the CNC exits the completion wait state.

-

Indexing function and other functions

Table 5.5 (a) Index indexing function and other functions

Item

Explanation

This value is rounded down when bit 1 of parameter REL No.5500 specifies this

Relative position display

option.

This value is rounded down when bit 2 (ABS) of parameter No. 5500 specifies

Absolute position display

this option.

Single direction positioning

Impossible to specify

2nd auxiliary function (B code)

Possible with any address other than B that of the indexing axis.

Operations while moving the

Unless otherwise processed by the machine, feed hold, interlock and emergency

indexing axis

stop can be executed. Machine lock can be executed after indexing is completed.

Disabled

SERVO OFF signal

The indexing axis is usually in the servo-off state.

The workpiece coordinate system and machine coordinate system must always

Incremental commands for

agree with each other on the indexing axis (the workpiece zero point offset value

indexing the index table

is zero.).

Manual operation is disabled in the JOG, INC, or HANDLE mode.

Operations for indexing the

A manual reference position return can be made. If the axis selection signal is set

index table

to zero during manual reference position return, movement is stopped and the

clamp command is not executed.

This function cannot be used on an axis on which the pole position detection

Pole position detection function

function is used.

- 107 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5.6

IN-FEED CONTROL (FOR GRINDING MACHINE)

Overview

Each time the switch on the machine operator's panel is input when the machine is at a table swing end

point, the machine makes a cut by a constant amount along the programmed profile on the specified YZ

plane. This makes it possible to perform grinding and cutting in a timely manner and facilitating the

grinding of a workpiece with a profile.

X=a C

•

E

•

External

signal input

(2)

(3)

A α

•

•

•

(1)

B(4)

D

Y

X=0

X

Sensor placement

Z

Fig. 5.6 (a)

For example, it is possible to machine a workpiece with a profile programmed with linear interpolation,

circular interpolation, and linear interpolation on the YZ plane, such as that shown in the Fig. 5.6 (a).

A sensor is placed at a X = 0 position so that the switch on the machine operator's panel is input when the

sensor detects the grinding wheel. When the program is started at point A, the machine is first placed in

the state in which it waits for the input of the switch on the machine operator's panel.

Then, when the sensor detects the grinding wheel, the switch on the machine operator's panel is input, and

the machine makes a cut by the constant amount α along the programmed profile on the specified YZ

plane and moves to point B (operation (1)). The machine is then placed in the state in which it waits for

the input of the switch on the machine operator's panel again, and performs a grinding operation along the

X-axis. It grinds from point B to point C (operation (2)) and grinds back from point C to point B

(operation (3)). When the machine returns to point B, the sensor detects the grinding wheel again, and the

switch on the machine operator's panel is input, so that the machine makes a cut by the amount of α and

moves to point D (operation (4)). At point D, the machine performs a grinding operation along the X-axis.

Afterwards, each time the switch on the machine operator's panel is input, the machine makes a cut by the

amount of α along the profile program, so that the workpiece is machined to a profile such as that shown

in the Fig. 5.6 (a).

Format

G161 R_ ;

Profile program

G160 ;

- 108 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

Explanation

-

G161 R_

This specifies an operation mode and the start of a profile program.

A dept of cut can be specified with R.

-

Profile program

Program the profile of a workpiece on the YZ plane, using linear interpolation (G01) or circular

interpolation (G02, G03). Multiple-block commands are possible.

When a profile program is started, the machine is placed in the state in which it waits for the input of the

switch on the machine operator's panel. When the switch on the machine operator's panel is input in this

state, the machine makes a cut by the amount of cut specified with R. Later, until the end point of the

program, the machine makes a cut each time the switch on the machine operator's panel is input. If the

final depth of cut is less than R, the remaining travel distance is assumed the depth of cut.

The feedrate is the one specified in the program with an F code. As in normal linear interpolation (G01)

or circular interpolation (G02, G03), override can be applied.

-

G160

This specifies the cancellation of an operation mode (end of a profile program).

Limitation

-

G161 R_

If no value is specified with R or if the value specified with R is negative, alarm PS0230 is issued.

-

Profile program

In a profile program, do not issue move commands other than those for linear interpolation (G01) and

circular interpolation (G02, G03).

CAUTION

If a move command other than those for linear interpolation (G01) and circular

interpolation (G02, G03) is issued in a profile program, an unexpected

movement may result.

-

Grinding operation

In this operation mode, a grinding operation that causes the machine to move to and from the grinding

wheel cannot be specified in an NC program. Perform such an operation in another way.

-

Block overlap

In this operation mode, block overlap is disabled.

-

Switch on the machine operator's panel

The switch on the machine operator's panel is disabled when it is input before a profile program is started.

Input the switch on the machine operator's panel after the start of a profile program. Also, even if the

switch on the machine operator's panel is input during a cut, this is not accepted in the next cut. It is

necessary to input the switch again after the end of the cut, when the machine is in the state in which it

waits for the input of the switch on the machine operator's panel.

- 109 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

Example

O0001 ;

:

N0 G161 R10.0 ;

N1 G91 G01 Z-70.0 F100 ;

N2 G19 G02 Z-80.0 R67.0 ;

N3 G01 Z-70.0 ;

70.0

80.0

70.0

N4 G160 ;

:

α

N2

N1

N3

Y

R=67.000

Z

Fig. 5.6 (b)

The program above causes the machine to move by 10.000 along the machining profile in the Fig. 5.6 (b)

each time the switch on the machine operator's panel is input.

α = Travel distance at each input of the switch on the machine operator's panel.

The feedrate is the one specified in the program with an F code.

Note

NOTE

If manual intervention is performed during in-feed control, the tool path after the

manual intervention can be switched by setting the manual absolute switch to on

or off as in normal linear/circular interpolation. When the manual absolute switch

is on, the machine returns to the programmed path for an absolute command or

for an incremental command with bit 1 (ABS) of parameter No. 7001 being 1.

5.7

CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

With the canned grinding cycle, repetitive machining operations that are specific to grinding and are

usually specified using several blocks can be specified using one block including a G function. So, a

program can be created simply. At the same time, the size of a program can be reduced, and the memory

can be used more efficiently. Four types of canned grinding cycles are available:

• Plunge grinding cycle (G75)

• Direct constant-dimension plunge grinding cycle (G77)

• Continuous-feed surface grinding cycle (G78)

• Intermittent-feed surface grinding cycle (G79)

In the descriptions below, an axis used for cutting with a grinding wheel and an axis used for grinding

with a grinding wheel are referred to as follows:

Axis used for cutting with a grinding wheel: Cutting axis

Axis used for grinding with a grinding wheel: Grinding axis

Axis on which to make a dresser cut:

Dressing axis

- 110 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

During execution of a canned grinding cycle, the following functions cannot be used:

•

Programmable mirror image

•

Scaling

•

Coordinate system rotation

•

3-dimensional coordinate conversion

•

One-digit F code feed

•

Tool length compensation

For a depth of cut on a cutting axis and a distance of grinding on a grinding axis, the incremental system

(parameter No. 1013) for the reference axis (parameter No. 1031) is used. If 0 is set in parameter No.

1031 (reference axis), the incremental system for the first axis is used.

WARNING

The G codes for canned grinding cycles G75, G77, G78, and G79 are G codes

of group 01. A G code for cancellation such as G80 used for a canned cycle for

drilling is unavailable. By specifying a G code of group 00 other than G04, modal

information such as a depth of cut is cleared but no canned grinding cycle can

be canceled. To cancel a canned grinding cycle, a G code of group 01 other

than G75, G77, G78, and G79 needs to be specified. So, when switching to

another axis move command from canned grinding cycles, for example, be sure

to specify a G code of group 01 such as G00 or G01 to cancel the canned

grinding cycle. If another axis move command is specified without canceling the

canned grinding cycle, an unpredictable operation can result because of

continued cycle operation.

NOTE

1 If the G code for a canned grinding cycle (G75, G77, G78, or G79) is specified,

the canned grinding cycle is executed according to the values of I, J, K, α, R, F,

and P preserved as modal data while the cycle is valid, even if a block specified

later specifies none of G75, G77, G78, and G79.

Example:

G75 I_ J_ K_ α_ R_ F_ P_ ;

;

← The canned grinding cycle is executed even if an empty block is specified.

%

2 When switching from a canned cycle for drilling to a canned grinding cycle,

specify G80 to cancel the canned cycle for drilling.

3 When switching from a canned grinding cycle to another axis move command,

cancel the canned cycle according to the warning above.

- 111 -

Content      ..     2      3      4      5     ..