FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- 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 G84 for rigid tapping (parameter G84 No. 5200 #0 set to 1).

- 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 speed.

- Tool length compensation

If a tool length compensation (G43, G44, or G49) is specified in the

canned cycle, the offset is applied at the time of positioning to point

- Series 10/11 format command

Rigid tapping can be performed using Series 10/11 format commands.

The rigid tapping sequence (including data transfer to and from the

PMC), Limitation, and the like are the same as described in this

chapter.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

•

Extraction override

•

Override signal

See “Override during Rigid Tapping” below for details.

- Dry run

Dry run can be executed also in G84 (G74). When dry run is

executed at the feedrate for the drilling axis in G84 (G74), tapping is

performed according to the feedrate. Note that the spindle speed

becomes faster at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G74).

When G84 (G74) is executed in the machine lock state, the tool does

not move along the drilling axis. Therefore, the spindle does not also

rotate.

- 76 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Reset

When a reset is performed during rigid tapping, the rigid tapping

mode is canceled and the spindle motor enters the normal mode.

Note that the G84 (G74) mode is not canceled in this case when bit 6

(CLR) of parameter No. 3402 is set.

- 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.

- 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 display 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.

- 77 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- Unit of F command

Metric input

Inch input

Remarks

Decimal point programming

G94

1 mm/min

0.01 inch/min

allowed

Decimal point programming

G95

0.01 mm/rev

0.0001 inch/rev

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.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G74 in a

single block. Otherwise, G74 will be canceled.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

- Program restart

A program cannot be restarted during rigid tapping.

- 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

G94;

Specify a feed-per-minute command.

G00 X120.0 Y100.0 ;

Positioning

M29 S1000 ;

Rigid mode specification

G84 Z-100.0 R-20.0 F1000 ;

Rigid tapping

G95 ;

Specify a feed-per-revolution command.

G00 X120.0 Y100.0 ;

Positioning

M29 S1000 ;

Rigid mode specification

G84 Z-100.0 R-20.0 F1.0 ;

Rigid tapping

- 78 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.2.2

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

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

position of the bottom of the hole

: The distance from the initial level to point R level

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

made.

: Cutting feedrate

: Number of repeats (if required)

G84.3 X_ Y_ Z_ R_ P_ F_ L_ ;

(Series 10/11 format)

: Number of repeats (if required)

G74 (G98)

G74 (G99)

Spindle stop

Initial level

Operation 1

Operation 2

Operation 6

Spindle stop

Spindle CCW

Spindle

stop

Point R

Point R level

Point R

Point R level

Operation 3

Operation 5

Point Z

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.

- 79 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- 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. (parameter G84 (No. 5200#0) 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.

- Tool length compensation

If a tool length compensation (G43, G44, or G49) is specified in the

canned cycle, the offset is applied at the time of positioning to point

- Series 10/11 format command

Rigid tapping can be performed using Series 15 format commands.

The rigid tapping sequence (including data transfer to and from the

PMC), Limitation, and the like are the same as described in this

chapter.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

• Extraction override

• Override signal

See “Override during Rigid Tapping” below for details.

- Dry run

Dry run can be executed also in G84 (G74). When dry run is

executed at the feedrate for the drilling axis in G84 (G74), tapping is

performed according to the feedrate. Note that the spindle speed

becomes faster at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G74).

When G84 (G74) is executed in the machine lock state, the tool does

not move along the drilling axis. Therefore, the spindle does not also

rotate.

- 80 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Reset

When a reset is performed during rigid tapping, the rigid tapping

mode is canceled and the spindle motor enters the normal mode.

Note that the G84 (G74) mode is not canceled in this case when bit 6

(CLR) of parameter No. 3402 is set.

- 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.

- 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 display 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

- 81 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- 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) 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

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

G95 ;

Specify a feed-per-revolution command.

G00 X120.0 Y100.0 ;

Positioning

M29 S1000 ;

Rigid mode specification

G74 Z-100.0 R-20.0 F1.0 ;

Rigid tapping

- 82 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.2.3

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

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

the position of the bottom of the hole

: The distance from the initial level to point R level

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

a return is made

: Depth of cut for each cutting feed

: The cutting feedrate

: Number of repeats (if required)

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

(Series 1０・１１ format)

: Number of repeats (if required)

G84, G74 (G98)

G84, G74 (G99)

• High-speed peck tapping cycle

d = retraction distance

(Parameter

PCP(No.5200#5)=0)

Initial level

<1> The tool operates at a

normal cutting feedrate.

Point R

Point R level

Point R

Point R level

The normal time constant

<1>

is used.

<2>

<2> Retraction can be

overridden.

The retraction time

constant is used.

Point Z

• Peck tapping cycle (Parameter

d = cutting start distance

PCP(No.5200#5)=1)

<1> The tool operates at a

Initial level

normal cutting feedrate.

The normal time constant is

Point R

Point R level

Point R

Point R level

<3>

used.

‡

<1>

<2> Retraction can be

<2>

overridden.

The retraction time constant

is used.

<3> Retraction can be

overridden.

The normal time constant is

Point Z

used.

- 83 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

Explanation

- High-speed peck tapping cycle

After positioning along the X- and Y-axes, rapid traverse is performed

to point R. From point R, cutting is performed with depth Q (depth

of cut for each cutting feed), then the tool is retracted by distance d.

The DOV bit (bit 4) of parameter 5200 specifies whether retraction

can be overridden or not. When point Z has been reached, the

spindle is stopped, then rotated in the reverse direction for retraction.

Set the retraction distance, d, in parameter 5213.

- Peck tapping cycle

After positioning along the X- and Y-axes, rapid traverse is performed

to point R level. From point R, cutting is performed with depth Q

(depth of cut for each cutting feed), then a return is performed to point

R. The DOV bit (bit 4) of parameter 5200 specifies whether the

retraction can be overridden or not. The moving of cutting feedrate

F is performed from point R to a position distance d from the end

point of the last cutting, which is where cutting is restarted. For this

moving of cutting feedrate F, the specification of the DOV bit (bit 4)

of parameter 5200 is also valid. When point Z has been reached, the

spindle is stopped, then rotated in the reverse direction for retraction.

Set d (distance to the point at which cutting is started) in parameter

5213.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following

override functions can be enabled by setting corresponding

parameters:

• Extraction override

• Override signal

See “Override during Rigid Tapping” below for details.

- Dry run

Dry run can be executed also in G84 (G74). When dry run is

executed at the feedrate for the drilling axis in G84 (G74), tapping is

performed according to the feedrate. Note that the spindle speed

becomes faster at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G74).

When G84 (G74) is executed in the machine lock state, the tool does

not move along the drilling axis. Therefore, the spindle does not also

rotate.

- 84 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Reset

When a reset is performed during rigid tapping, the rigid tapping

mode is canceled and the spindle motor enters the normal mode.

Note that the G84 (G74) mode is not canceled in this case when bit 6

(CLR) of parameter No. 3402 is set.

- 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.

- 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 display 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

- 85 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- 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) 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.

- d (parameter No.5213)

Perform operation in the peck tapping cycle within point R. That is,

set a value which does not exceed point R for d (parameter No. 5213).

5.2.4

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.

- 86 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.2.5

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

5.2.5.1 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

Override (% )

100

Spindle speed (specified at

)

Bit 6 (OVE) of parameter No. 5202 can be set to 1 to extend the

override value to 100% to 2000%. If the specified override value is

outside the range between 100% and 2000%, it is assumed to be

100%.

- 87 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

The override to be applied is determined according to the setting of

parameters and that in the command as shown in the table below.

When bit 6 (OVE) of parameter No. 5202 is set to 0

Parameter setting

DOV = 1

DOV = 0

Command

OV3 = 1

OV3 = 0

Within the range between

Command in the

Spindle speed at extraction

100% to 200%

program

Parameter

specified at address "J"

Outside the range between

100%

No. 5211

100% to 200%

No spindle speed at extraction specified at address "J"

Parameter No. 5211

When bit 6 (OVE) of parameter No. 5202 is set to 1

Parameter setting

DOV = 1

DOV = 0

Command

OV3 = 1

OV3 = 0

Within the range between

Command in the

Spindle speed at extraction

100% to 2000%

program

Parameter

specified at address "J"

Outside the range between

100%

No. 5211

100% to 2000%

No spindle speed at extraction specified at address "J"

Parameter No. 5211

NOTE

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.

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

If a minus sign is used, a value outside the range is assumed to be

specified.

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 5243). 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

)

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.

- 88 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.2.5.2

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

•

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%

•

At extraction

When the override cancel signal is set to 0

Value specified by the override signal

When the override cancel signal is set to 1 and extraction

override is disabled

100%

When the override cancel signal is set to 1 and extraction

override is enabled

Value specified for extraction override

NOTE

1 The maximum override is obtained using the following equation so

that the spindle speed to which override is applied do not exceed the

maximum used gear speed (specified in parameters Nos. 5241 to

5243). 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

)

2 Since override operation differs depending on the machine in use,

refer to the manual provided by the machine tool builder.

- 89 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

5.3

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

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

Inserted corner R

block

- 90 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

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 ;

N007 Y70.0 ,C5.0 ;

N008 X10.0 ,C5.0 ;

N009 Y10.0 ;

N010 G00 X0 Y0 ;

N011 M0;

N008

70.0

N007

60.0

N006

50.0

40.0

N009

N005

30.0

20.0

N004

10.0

N003

N010

N002

N011

N001

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.

- 91 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- 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 ;

The tool path without

chamfering is indicated

with a solid line.

Chamfering block to be inserted

Fig 5.3 (a) Exceeding the move range

- Plane selection

A chamfering or corner R block is inserted only for a command to

move the tool within the same plane.

Example:

When the U-axis is set as an axis parallel to the basic X-axis (by

setting parameter No.

1022 to

5), the following program

performs chamfering between cutting feed along the U-axis and

that along the Y-axis:

G17 U0 Y0

G00 U100.0 Y100.0

G01 U200.0 F100 ,C30.0

Y200.0

The following program causes alarm PS0055, however.

(Because chamfering is specified in the block to move the tool

along the X-axis, which is not on the selected plane)

G17 U0 Y0

G00 U100.0 Y100.0

G01 X200.0 F100 ,C30.0

Y200.0

The following program also causes alarm PS0055.

(Because

the block next to the chamfering command moves the tool along

the X-axis, which is not on the selected plane)

G17 U0 Y0

G00 U100.0 Y100.0

G01 Y200.0 F100 ,C30.0

X200.0

If a plane selection command (G17, G18, or G19) is specified in the

block next to the block in which chamfering or corner R is specified,

alarm PS0051 is issued.

- 92 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Travel distance 0

When two linear interpolation operations are performed, the

chamfering or corner R block is regarded as having a travel distance

of zero if the angle between the two straight lines is within ±1°.

When linear interpolation and circular interpolation operations are

performed, the corner R block is regarded as having a travel distance

of zero if the angle between the straight line and the tangent to the arc

at the intersection is within ±1°. When two circular interpolation

operations are performed, the corner R block is regarded as having a

travel distance of zero if the angle between the tangents to the arcs at

the intersection is within ±1°.

- Single block operation

When the block in which chamfering or corner R is specified is

executed in the single block mode, operation continues to the end

point of the inserted chamfering or corner R block and the machine

stops in the feed hold mode at the end point. When bit 0 (SBC) of

parameter No. 5105 is set to 1, the machine stops in the feed hold

mode also at the start point of the inserted chamfering or corner R

block.

- Unusable G codes

The following G codes are unusable in the same block as for

chamfering or corner R commands or with a block for chamfering or

corner R inputs that define continuous figures.

・G codes (except G04) in group 00

・G68 in group 16

- Threading

If ”,C” or “,R” is specified in a threading command block, the alarm

PS0050 is issued.

NOTE

When ",C" and ",R" are specified in the same

block, the address specified last is valid.

- 93 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

5.4

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 .

NOTE

To enable the index table indexing function, reset

bit 0 (ITI) of parameter No. 5501 to "0" and set bit 3

(IXC) of parameter No. 8132 to "1".

Explanation

- Indexing position

Specify an indexing position with address A, B, or C (set to bit 0 of

parameter ROTx No.1006).

The indexing position is specified by either of the following

(depending on bit 4 of parameter G90 No.5500):

Absolute value only (Bit 4 (G90) of parameter No.5500 =1)

Absolute or incremental value depending on the specified G

code: G90 or G91 (Bit 4 (G90) of parameter No.5500 =0)

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.

Value specified for rotation from A to B

(case 2 described above)

G90 B-45.0 ; or

G91 B-105.0;

+60°

0°

-45°

- 94 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- 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.

Using the auxiliary function specified in parameter No. 5511

(Address) (Indexing position) (Auxiliary 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

of parameter ABS 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.

Using no auxiliary functions

By setting to bits

3, and

4 of parameter ABS, INC,G90

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 of parameter ABS 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.

(2) Rotating in the specified direction

In the absolute programming, the value set in bit

2 of

parameter ABS 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

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.

- 95 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

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 display 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 5.4 (a) Index indexing function and other functions

Item

Explanation

Relative position display

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

Absolute position display

This value is rounded down when bit 2 of parameter ABS No.5500 specifies this option.

Movement in the machine

Impossible to move

coordinate system (G53)

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 stop

indexing axis

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.

Incremental commands for

The workpiece coordinate system and machine coordinate system must always agree

indexing the index table

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

index table

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 function is

Pole position detection function

used.

- 96 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.5

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

•

External

(2)

signal input

(3)

•

(1)

•

B(4)

X=0

Sensor placement

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 figure

above.

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 figure above.

- 97 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

NOTE

In-feed control function is optional function.

Format

G161 R_ ;

Profile program

G160 ;

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).

- 98 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

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.

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 ;

N4 G160 ;

70.0

80.0

70.0

R=67.000

The program above causes the machine to move by 10.000 along the

machining profile in the figure above 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.

- 99 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.6

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

During execution of a canned grinding cycle, the following functions

cannot be used:

•

Programmable mirror image

•

Scaling

•

Coordinate system rotation

•

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.

- 101 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

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.

- 102 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.6.1

Plunge Grinding Cycle (G75)

A plunge grinding cycle can be executed.

Format

G75 I_ J_ K_ α_ R_ F_ P_ L_ ;

: First depth of cut (The cutting direction depends on the sign.)

: Second depth of cut (The cutting direction depends on the sign.)

K_ : Total depth of cut (The cutting direction depends on the sign.)

α_

: Grinding range (The grinding direction depends on the sign.)

R_ : Feedrate for I and J

: Feedrate for α

P_ : Dwell time

: Grinding-wheel wear compensation number (during continuous

dressing only)

G75

<1> (R)

<3> (F)

<2> P

<4> (R)

<6> (F)

<5> P

NOTE

α is an arbitrary axis address on the grinding axis

as determined with parameter No. 5176.

- 103 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

Explanation

A plunge grinding cycle consists of a sequence of six operations.

Operations <1> to <6> are repeated until the depth of cut reaches the

total depth of cut specified with address K. For a single block,

operations <1> to <6> are executed with a single cycle start.

- Operation sequence in a cycle

<1> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount

specified as the first depth of cut I. The feedrate is the one specified

with R.

<2> Dwell

Performs a dwell for the time specified with P.

<3> Grinding

Causes the machine to move with cutting feed by the amount specified

with α. The grinding axis is specified with parameter No. 5176. The

feedrate is the one specified with F. If L is specified when the

continuous dressing function is enabled, dressing is performed with

the cutting axis and the dressing axis. The dressing axis is specified

with parameter No. 5180.

<4> Cutting with a grinding wheel

Makes a cut in the Y-axis direction with cutting feed by the amount

specified as the second depth of cut J. The feedrate is the one specified

with R.

<5> Dwell

Performs a dwell for the time specified with P.

<6> Grinding (return direction)

Feeds the machine at the feedrate specified with F in the opposite

direction by the amount specified with α. If L is specified when the

continuous dressing function is enabled, dressing is performed with

the cutting axis and the dressing axis.

- Continuous dressing

If the continuous dressing function is enabled, the grinding-wheel cut

and the dresser cut are continuously compensated for according to the

dressing amount specified with L during the execution of grinding.

That is, continuous dressing is performed in each grinding operation

in the sequence of operations in the cycle, resulting in simultaneous

3-axis interpolation with compensation in the cutting axis direction

and compensation in the dressing axis direction simultaneous with

movement along the grinding axis. At this time, the travel distance

(compensation) along the cutting axis is equal to the specified dressing

amount, and the travel distance along the dressing axis is equal to

double the specified dressing amount (diameter).

For the dressing amount, specify an offset number (grinding-wheel

wear compensation number) with address L. Up to 400 offset numbers

(L1 to L400) can be specified. Establish correspondence between

compensation amounts and offset numbers, and set it in offset memory

in advance, using the MDI panel.

- 104 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

No compensation operation is performed in the following cases:

The continuous dressing function is disabled.

L is not specified.

L0 is specified.

Dresser

a: Amount of dressing

Dressing axis

Cutting axis

Grinding wheel

Grinding axis

Workpiece

NOTE

Continuous dressing function is optional function.

Limitations

- Cutting axis

The cutting axis is the second controlled axis. By setting bit 0 (FXY)

of parameter No. 5101 to 1, the axis can be switched with a plane

selection command (G17, G18, or G19).

- Grinding axis

To specify a grinding axis, set its axis number, which must be other

than that of the cutting axis, in parameter No. 5176.

- Dressing axis

To specify a dressing axis, set its axis number, which must be other

than those of the cutting axis and the grinding axis, in parameter No.

5180.

- α,I,J,K

α, I, J, and K commands are all incremental ones.

Spark-out (execution of movement in the grinding direction only)

occurs in the following cases:

•

I or J is not specified or I = J = 0

•

K is not specified or K = 0

If I or J is not specified or if I = J = 0 is true, and K is not equal to 0, a

grinding operation is performed infinitely.

- Clearing

The data items I, J, K, α, R, F, and P in a canned cycle are modal

information common to G75, G77, G78, and G79, so that once

specified, they remain effective until specified anew. The data is

cleared when a G code of group 00 other than G04 or a G code of

group 01 other than G75, G77, G78, and G79 is specified. L is

effective only in the block in which it is specified.

- 105 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 4