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

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

Offset value +200.0 is set in offset No.11, +190.0 is set in offset No.15, and +150.0 is set in offset No.31

Program example

;

N001

G92X0Y0Z0;

Coordinate setting at reference position

N002

G90 G00 Z250.0 T11 M6;

Tool change

N003

G43 Z0 H11;

Initial level, tool length offset

N004

S30 M3

Spindle start

N005

G99 G81X400.0 R Y-350.0

Z-153,0R-97.0 F120;

Positioning, then #1 drilling

N006

Y-550.0;

Positioning, then #2 drilling and point R level return

N007

G98Y-750.0;

Positioning, then #3 drilling and initial level return

N008

G99X1200.0;

Positioning, then #4 drilling and point R level return

N009

Y-550.0;

Positioning, then #5 drilling and point R level return

N010

G98Y-350.0;

Positioning, then #6 drilling and initial level return

N011

G00X0Y0M5;

Reference position return, spindle stop

N012

G49Z250.0T15M6;

Tool length offset cancel, tool change

N013

G43Z0H15;

Initial level, tool length offset

N014

S20M3;

Spindle start

N015

G99G82X550.0Y-450.0

Positioning, then #7 drilling, point R level return

Z-130.0R-97.0P300F70;

N016

G98Y-650.0;

Positioning, then #8 drilling, initial level return

N017

G99X1050.0;

Positioning, then #9 drilling, point R level return

N018

G98Y-450.0;

Positioning, then #10 drilling, initial level return

N019

G00X0Y0M5;

Reference position return, spindle stop

N020

G49Z250.0T31M6;

Tool length offset cancel, tool change

N021

G43Z0H31;

Initial level, tool length offset

N022

S10M3;

Spindle start

N023

G85G99X800.0Y-350.0

Positioning, then #11 drilling, point R level return

Z-153.0R47.0F50;

N024

G91Y-200.0K2;

Positioning, then #12, 13 drilling. point R level return

N025

G28X0Y0M5;

Reference position return, spindle stop

N026

G49Z0;

Tool length offset cancel

N027

M0;

Program stop

220

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

The tapping cycle (G84) and left-handed tapping cycle (G74) may be

13.2

performed in standard mode or rigid tapping mode.

RIGID TAPPING

In standard mode, the spindle is rotated and stopped along with a

movement along the tapping axis using miscellaneous 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.

221

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.2.1

When the spindle motor is controlled in rigid mode as if it were a servo

motor, a tapping cycle can be sped up.

Rigid Tapping

(G84)

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 (Only for necessity of repeat)

G84.2 X_ Y_ Z_ R_ P_ F_ L_ ;

(FS15 format)

: Number of repeats (only for necessity of repeat)

G84(G98)

G84(G99)

Spindle stop

Initial level

Operation1

Operation6

Operation2

Spindle stop

Spindle CW

Spindle

Spindle CW

stop

Point R level

Point R

Operation3

Operation5

Point Z

Operation4

Spindle stop

Spindle CCW

Spindle stop

Spindle CCW

Explanations

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 reverse 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%.

However, the speed for extraction (operation 5) can be overridden by up

to 2000% depending on the setting at bit 4 (DOV) of parameter No.5200,

bit 3 (OVU) of parameter (No.5201), and parameter No.5211.

D 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).

222

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

D 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.

D Tool length

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

compensation

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

D FS15-format command

Rigid tapping can be performed using FS15-format commands. The

rigid tapping sequence (including data transfer to and from the PMC),

restrictions, and the like are the same as described for the 16i/18i.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled. If the drilling axis is changed in rigid mode, P/S alarm (No.

206) is issued.

D S command

D If a speed higher than the maximum speed for the gear being used is

specified, P/S alarm (No. 200) is issued.

D When the rigid tapping canned cycle is cancelled, the S command used

for rigid tapping is cleared to S0.

D Distribution amount for

For an analog spindle control circuit:

the spindle

Upon specifying a speed command requiring more than 4096 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

For a serial spindle:

Upon specifying a speed command requiring more than 32767 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

D F command

If a value exceeding the upper limit of cutting feedrate is specified, P/S

alarm (No. 011) is issued.

D 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

D M29

If an S command and axis movement are specified between M29 and G84,

P/S alarm (No. 203) is issued. If M29 is specified in a tapping cycle, P/S

alarm (No. 204) is issued.

D P

Specify P in a block that performs drilling. If R is specified in a

non-drilling block, it is not stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G84 in a single block.

Otherwise, G84 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Program restart

A program cannot be restarted during rigid tapping.

223

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

Examples

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

224

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

13.2.2

When the spindle motor is controlled in rigid mode as if it were a servo

motor, tapping cycles can be speed up.

Left-Handed Rigid

Tapping Cycle

(G74)

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 (Only for necessity of repeat)

G84.3 X_ Y_ Z_ R_ P_ F_ L_ ; (FS15 format)

: Number of repeats (Only for necessity of repeat)

G74 (G98)

G74 (G99)

Spindle stop

Initial level

Operation1

Operation2

Operation6

Spindle

CCW

stop

CCW

Point R

Point R level

Point R

Point R level

Operation3

Operation5

Point Z

Spindle stop

Operation4 Spindle CW

Spindle stop

Spindle CW

Explanations

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%.

However, the speed for extraction (operation 5) can be overridden by up

to 2000% depending on the setting at bit 4 (DOV) of parameter 5200, bit

3 (OVU) of parameter (No.5201), and parameter 5211.

D 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 to1).

225

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

D 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.

D Tool length

If a tool length offset (G43, G44, or G49) is specified in the canned cycle,

compensation

the offset is applied at the time of positioning to point R.

D FS15-format command

Rigid tapping can be performed using FS15-format commands. The

rigid tapping sequence (including data transfer to and from the PMC),

restrictions, and the like are the same as described for the 16i/18i.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled. If the drilling axis is changed in rigid mode,P/S alarm (No.

206) is issued.

D S command

D Specifying a rotation speed exceeding the maximum speed for the gear

used causes P/S alarm (No. 200).

D When the rigid tapping canned cycle is cancelled, the S command used

for rigid tapping is cleared to S0.

D Distribution amount for

For an analog spindle control circuit:

the spindle

Upon specifying a speed command requiring more than 4096 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

For a serial spindle:

Upon specifying a speed command requiring more than 32767 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

D F command

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

P/S alarm (No. 011).

D 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

D M29

Specifying an S command or axis movement between M29 and G74

causes P/S alarm (No. 203).

Then, specifying M29 in the tapping cycle causes P/S alarm (No. 204).

D P

Specify P in a block that performs drilling. If R is specified in a

non-drilling block, it ss not stored as modal data.

D Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the

MDL bit (bit 0 of parameter 5431) is set to 1)) and G74 in a single block.

Otherwise, G74 will be canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

226

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Examples

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

G74 Z-100.0 R-20.0 F1.0 ;

Rigid tapping

227

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.2.3

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

Peck Rigid Tapping

rigid tapping cycle is useful.

Cycle (G84 or G74)

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, 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. The normal time

Point R level

constant is used.

Point R

Point R level

Point R

(2) Retraction can be overridden.

(1)

The retraction time constant is

used.

(2)

Point Z

⋅Peck tapping cycle

d=cutting start distance

(Parameter PCP(No.5200#5=1))

Initial level

(1) The tool operates at a normal

cutting feedrate. The normal time

constant is used.

Point R level

Point R

Point R level

Point R

(2) Retraction can be overridden.

(3)

The retraction time constant is

(1)

used.

(2)

(3) Retraction can be overridden.

The normal time constant is used.

During a rigid tapping cycle, in-position

check is performed at the end of each

operation of (1) and (2) in the peck tap-

ping cycle.

Point Z

228

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Explanations

D High-speed peck

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

tapping cycle

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.

D 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.

Limitations

D Axis switching

Before the drilling axis can be changed, the canned cycle must be

canceled. If the drilling axis is changed in rigid mode, P/S alarm (No.

206) is issued.

D S command

D Specifying a rotation speed exceeding the maximum speed for the gear

used causes P/S alarm (No. 200).

D When the rigid tapping canned cycle is cancelled, the S command used

for rigid tapping is cleared to S0.

D Distribution amount for

For an analog spindle control circuit:

the spindle

Upon specifying a speed command requiring more than 4096 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

For a serial spindle:

Upon specifying a speed command requiring more than 32767 pulses, in

detection units, within 8 ms, a P/S alarm (No.202) is issued because the

result of such an operation is unpredictable.

D F command

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

alarm (No. 011).

D Unit of F

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

D M29

Specifying an S command or axis movement between M29 and G84

causes P/S alarm (No. 203).

Then, specifying M29 in the tapping cycle causes P/S alarm (No. 204).

229

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

D 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.

D Cancel

Do not specify a group 01 G code (G00 to G03) and G73 in the same block.

If they are specified together, G73 is canceled.

D Tool offset

In the canned cycle mode, tool offsets are ignored.

D Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_

in an independent block.

13.2.4

The rigid tapping canned cycle is canceled. For how to cancel this cycle,

see II-13.1.14.

Canned Cycle Cancel

(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.

230

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

13.3

Canned grinding cycles make it easier for the programmer to create

programs that include grinding. With a canned grinding cycle, repetitive

Canned Grinding

operation peculiar to grinding can be specified in a single block with a G

Cycle

function; without canned grinding cycles, normally more than one block

(FOR GRINDING

is required. In addition, the use of canned grinding cycles shortens the

program to save memory. The following four canned grinding cycles are

MACHINE)

available:

⋅Plunge grinding cycle (G75)

⋅Direct constant-dimension plunge grinding cycle (G77)

⋅Continuous-feed surface grinding cycle (G78)

⋅Intermittent-feed surface grinding cycle (G79)

231

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.3.1

A plunge grinding cycle is performed.

Plunge Grinding Cycle

(G75)

Format

G75 I_ J_ K_ X(Z)_ R_ F_ P_ L_ ;

I_ : Depth-of-cut 1 (A sign in the command specifies the direction

of cutting.)

: Depth-of-cut 2 (A sign in the command specifies the direction

of cutting.)

K_ : Total depth of cut (A sign in the command specifies the direction

of cutting.)

X(Z)_ : Range of grinding (A sign in the command specifies the

direction of grinding.)

R_ : Feedrate for I and J

F_ : Feedrate for X (Z)

P_ : Dwell time

: Grinding-wheel wear compensation (Only for continuous dressing)

G75

X(Z)

(1) (R)

(3) (F)

(2) P

(4) (R)

(6) (F)

(5) P

X(Z)

Explanations

The plunge grinding cycle consists of six operation sequences.

Operations (1) to (6) are repeated until the depth reaches the total depth

of cut specified at address K. In the single block stop mode, operations

(1) to (6) are performed every cycle start.

D Grinding wheel cutting

(1) Cutting is performed along the Y-axis in cutting feed mode for the

amount specified by I (depth of cut 1). The feedrate is specified by R.

D Dwell

(2) Dwell is performed for the time specified by P.

D Grinding

(3) Cutting feed is performed for the amount specified by X (or Z). The

feedrate is specified by F.

D Grinding wheel cutting

(4) Cutting is performed along the Y-axis in cutting feed mode for the

amount specified by J (depth of cut 2). The feedrate is specified by R.

D Dwell

(5) Dwell is performed for the time specified by P.

D Grinding

(6) Feeding is performed in the reverse direction for the amount specified

(return direction)

by X (or Z) at a feedrate specified by F.

232

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Limitations

D X(Z), I, J, K

X, (Z), I, J, and K must all be specified in incremental mode.

D Clear

I, J, X, and Z in canned cycles are modal data common to G75, G77, G78,

and G79. They remain valid until new data is specified. They are cleared

when a group 00 G code other than G04 or a group 01 G code other than

G75, G77, G78, and G79 is specified.

D Operation performed

When the total depth of cut is reached during cutting using I or J, the

when the total depth of

subsequent operation sequences (up to

) are executed, then the cycle

cut is reached

terminates. In this case, no further cutting is performed after the total

depth of cut is reached.

D Chart of operation in which the total depth of cut is reached by cutting

specified by I and J:

D Chart of operation in which the total depth of cut is reached during

cutting specified by I and J:

233

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.3.2

A direct constant-dimension plunge grinding cycle is performed.

Direct

Constant-Dimension

Plunge Grinding Cycle

(G77)

Format

G77 I_ J_ K_ X(Z)_ R_ F_ P_ L_ ;

I_ : Depth-of-cut 1 (A sign in the command specifies the direction

of cutting.)

: Depth-of-cut 2 (A sign in the command specifies the direction

of cutting.)

K_ : Total depth of cut (A sign in the command specifies the direction

of cutting.)

X(Z)_ : Range of grinding (A sign in the command specifies the direction

of grinding.)

R_ : Feedrate for I and J

F_ : Feedrate for X (Z)

P_ : Dwell time

: Grinding-wheel wear compensation (Only for continuous

dressing)

G77

X(Z)

(R)

(F)

(R)

(F)

X(Z)

Explanations

The constant-dimension plunge grinding cycle consists of six operation

sequences. Operations

are repeated until the depth reaches the

total depth of cut specified at address K.

D Grinding wheel cutting

Cutting is performed along the Y-axis in cutting feed mode for the

amount specified by I (depth of cut 1). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Cutting feed is performed for the amount specified by X (or Z). The

feedrate is specified by F.

D Grinding wheel cutting

Cutting is performed along the Y-axis in cutting feed mode for the

amount specified by J (depth of cut 2). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Feeding is performed in the reverse direction for the amount specified

(return direction)

by X (or Z) at a feedrate specified by F.

234

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

D Skip signal

When the cycle is performed using G77, a skip signal can be input to

terminate the cycle. When a skip signal is input, the current operation

sequence is interrupted or completed, then the cycle is terminated.

The following shows how the system operates when the skip signal is

input during each operation sequence.

D When the skip signal is input during operation sequence 1 or 4 (cutting

feed specified by I or J), cutting is stopped immediately and the tool

returns to the X (Z) coordinate at which the cycle started.

Skip Signal

(End)

Skip Signal

(End)

D When the skip signal is input during operation sequence 2 or 5 (dwell),

dwell is stopped immediately and the tool returns to the X (Z)

coordinate at which the cycle started.

D When the skip signal is input during operation sequence 3 or 6

(movement), the tool returns to the X (Z) coordinate at which the cycle

started after the movement specified by X (Z) is completed.

Skip Signal

(End)

Skip Signal

(End)

Limitations

D X(Z), I, J, K

X, (Z), I, J, and K must all be specified in incremental mode.

D Clear

I, J, X, and Z in canned cycles are modal data common to G75, G77, G78,

and G79. They remain valid until new data is specified. They are cleared

when a group 00 G code other than G04 or a group 01 G code other than

G75, G77, G78, and G79 is specified.

235

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.3.3

A continuous-feed surface grinding cycle is performed.

Continuous-Feed

Surface Grinding Cycle

(G78)

Format

G78 I_ (J_) K_ X_ F_ P_ L_ ;

I_ : Depth-of-cut 1 (A sign in the command specifies the direction

of cutting.)

: Depth-of-cut 2 (A sign in the command specifies the direction

of cutting.)

K_ : Total depth of cut (A sign in the command specifies the direction

of cutting.)

X_ : Range of grinding (A sign in the command specifies the

direction of grinding.)

F_ : Feed rate

P_ : Dwell time

: Grinding-wheel wear compensation (Only for continuous

dressing)

G78

P(Dwell)

(F)

I(J)

(F)

P(Dwell)

Explanations

The continuous-feed surface grinding cycle consists of four operation

sequences. Operations

are repeated until the depth reaches

the total depth of cut specified in address K. In the single block stop mode,

operations

are performed every cycle start.

Dwell

Grinding

Dwell

Grinding (in reverse direction)

236

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Restrictions

D J

When J is omitted, it is assumed to be 1. J is valid only in the block where

it is specified.

D I, J, K, X

X, I, J, and K must all be specified in incremental mode.

D Clear

I, J, X, and Z in canned cycles are modal data common to G75, G77, G78,

and G79. They remain valid until new data is specified. They are cleared

when a group 00 G code other than G04 or a group 01 G code other than

G75, G77, G78, and G79 is specified.

D Operation performed

When the total depth of cut is reached during cutting using I or J, the

when the total depth of

subsequent operation sequences (up to

) are executed, then the cycle

cut is reached

terminates. In this case, no further cutting is performed after the total

depth of cut is reached.

D Chart of operation in which the total depth of cut is reached by cutting

specified by I and J:

D Chart of operation in which the total depth of cut is reached during

cutting specified by I and J:

237

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

13.3.4

An intermittent-feed surface grinding cycle is performed.

Intermittent-Feed

Surface Grinding Cycle

(G79)

Format

G79 I_ J_ K_ X_ R_ F_ P_ L_ ;

I_ : Depth-of-cut 1 (A sign in the command specifies the direction

of cutting.)

: Depth-of-cut 2 (A sign in the command specifies the direction

of cutting.)

K_ : Total depth of cut (A sign in the command specifies the direction

of cutting.)

X_ : Range of grinding (A sign in the command specifies the

direction of grinding.)

R_ : Feedrate for I and J

F_ : Feedrate for X

P_ : Dwell time

: Grinding-wheel wear compensation (Only for continuous dressing)

G79

(R)

(F)

(R)

(F)

Explanations

The intermittent-feed surface grinding cycle consists of six operation

sequences. Operations

are repeated until the depth reaches the

total depth of cut specified at address K. In the single block stop mode,

operations

are performed every cycle start.

D Grinding wheel cutting

Cutting is performed along the Z-axis in cutting feed mode for the

amount specified by I (depth of cut 1). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Cutting feed is performed for the amount specified by X. The feedrate

is specified by F.

D Grinding wheel cutting

Cutting is performed along the Z-axis in cutting feed mode for the

amount specified by J (depth of cut 2). The feedrate is specified by R.

D Dwell

Dwell is performed for the time specified by P.

D Grinding

Feeding is performed in the reverse direction for the amount specified

(return direction)

by X at a feedrate specified by F.

238

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

This function enables continuous dressing.

13.4

When G75, G77, G78, or G79 is specified, grinding wheel cutting and

GRINDING-WHEEL

dresser cutting are compensated continuously according to the amount of

WEAR

continuous dressing during grinding.

COMPENSATION BY

CONTINUOUS

DRESSING

(FOR GRINDING

MACHINE)

Explanations

D Specification

Specify an offset number (grinding-wheel wear compensation number)

at address L in the block containing G75. The compensation amount set

in the offset memory area corresponding to the specified number is used

as the amount of dressing.

Up to 400 offset numbers (L1 to L400) can be specified. Compensation

amounts must be set beforehand in offset memory corresponding to offset

numbers from the MDI panel.

When L is omitted or L0 is specified in a surface grinding canned cycle

block, compensation is not performed.

D Compensation

Compensation is performed for every grinding operation

(every

movement along the X-axis) in the operation sequences of a canned

grinding cycle. While the tool moves along the X-axis, compensation is

performed along the Y-axis (grinding wheel cutting) and the V-axis

(dresser cutting) for simultaneous three-axis interpolation.

The travel distance (compensation amount) along the Y-axis is the same

as specified dressing amount, and the travel distance along the V-axis is

twice as long (diameter).

240

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

13.5

AUTOMATIC

GRINDING WHEEL

DIAMETER

COMPENSATION

AFTER DRESSING

13.5.1

Compensation amounts set in offset memory can be modified by using the

external tool compensation function or programming (by changing

Checking the Minimum

offsets using custom macro variables).

Grinding Wheel

With these functions, the compensation amount for the diameter of the

Diameter

dressed grinding wheel can be changed.

(For Grinding Machine)

If the compensation amount associated with the offset number specified

in the H code is smaller than the minimum grinding wheel diameter

specified in parameter 5030 when programmed compensation (using G43

or G44) is performed, a signal is output to the PMC.

a : Amount of dressing

Dresser

Grinding

wheel

Workpiece

241

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

Every time an external signal is input, cutting is performed by a fixed

13.6

amount according to the programmed profile in the specified Y-Z plane.

IN-FEED GRINDING

ALONG THE Y AND Z

AXES AT THE END

OF TABLE SWING

(FOR GRINDING

MACHINE)

Format

G161 R_ ;

profile program

G160 ;

Explanations

D G161 R_

Specify the start of an operation mode and profile program. Also specify

the depth of cut in R.

D Profile program

Program a workpiece figure in the Y-Z plane using linear interpolation

(G01) and/or circular interpolation (G02 or G03). One or more blocks can

be specified.

D G160

Cancel the operation mode (end of the profile program).

Restrictions

D Profile program

Do not specify codes other than G01, G02, and G03 within the profile

program.

Examples

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

In the above program, every time the in-feed cutting start signal is input,

the tool is moved by 10.000 along the machining profile shown above.

α= Travel distance for each in-feed control cutting start signal input

The feedrate is programmed with an F code.

242

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Chamfering and corner rounding blocks can be inserted automatically

13.7

between the following:

OPTIONAL ANGLE

⋅Between linear interpolation and linear interpolation blocks

CHAMFERING AND

⋅Between linear interpolation and circular interpolation blocks

⋅Between circular interpolation and linear interpolation blocks

CORNER ROUNDING

⋅Between circular interpolation and circular interpolationblocks

Format

, C_

Chamfering

, R_

Corner R

Explanations

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 rounding block is inserted.

Blocks specifying chamfering and corner rounding can be specified

consecutively.

D Chamfering

After C, specify the distance from the virtual corner point to the start and

end points. The virtual 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

D Corner R

After R, specify the radius for corner rounding.

(1) G91 G01 X100.0 ,R10.0 ;

(2) X100.0 Y100.0 ;

Center of a circle with radius R

243

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Restrictions

D Plane selection

Chamfering and corner rounding can be performed only in the plane

specified by plane selection (G17, G18, or G19). These functions cannot

be performed for parallel axes.

D Next block

A block specifying chamfering or corner rounding 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, P/S alarm No. 052 is issued.

D Plane switching

A chamfering or corner rounding block can be inserted only for move

commands which are performed in the same plane. In a block that comes

immediately after plane switching (G17, G18, or G19 is specified),

neither chamfering nor corner rounding can be specified.

D Exceeding the move

If the inserted chamfering or corner rounding block causes the tool to go

range

beyond the original interpolation move range, P/S alarm No.055 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

D Coordinate system

In a block that comes immediately after the coordinate system is changed

(G92, or G52 to G59) or a return to the reference position (G28 to G30)

is specified, neither chamfering nor corner rounding can be specified.

D Travel distance 0

When two linear interpolation operations are performed, the chamfering or

corner rounding 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

rounding 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

rounding 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_ .

The following G codes cannot be used in a block that specifies chamfering

D Unavailable G codes

or corner rounding. They also cannot be used between chamfering and

corner rounding blocks that define a continuous figure.

⋅G codes of group 00 (except G04)

⋅G68 of group 16

D Threading

Corner rounding cannot be specified in a threading block.

D DNC operation

Arbitrary angle chamfering and corner rounding cannot be enabled for

DNC operation.

245

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

Upon completion of positioning in each block in the program, an external

13.8

operation function signal can be output to allow the machine to perform

EXTERNAL MOTION

specific operation.

FUNCTION

Concerning this operation, refer to the manual supplied by the machine

tool builder.

(G81)

Format

G81 IP_ ; ( IP_ Axis move command )

Explanations

Every time positioning for the IP_ move command is completed, the CNC

sends a external operation function signal to the machine. An external

operation signal is output for each positioning operation until canceled by

G80 or a group 01 G code.

Restrictions

D A block without X or Y

No external operation signals are output during execution of a block that

axis

contains neither X nor Y.

D Relationship with canned

G81 can also be used for a drilling canned cycle (II-13.1.4). Whether G81

cycle G81

is to be used for an external motion function or for a drilling canned cycle

is psecified with EXC, bit 1 of parameter No.5101.

246

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

Machining can be repeated after moving or rotating the figure using a

13.9

subprogram.

FIGURE COPY

(G72.1, G72.2)

Format

D Rotational copy

Xp-Yp plane (specified by G17) : G72.1 P_ L_ Xp_ Yp_ R_ ;

Zp-Xp plane (specified by G18) : G72.1 P_ L_ Zp_ Xp_ R_ ;

Yp-Zp plane (specified by G19) : G72.1 P_ L_ Yp_ Zp_ R ;_

P :Subprogram number

L :Number of times the operation is repeated

Xp :Center of rotation on the Xp axis

(Xp : X-axis or an axis parallel to the X-axis)

Yp :Center of rotation on the Yp axis

(Yp: Y-axis or an axis parallel to the Y-axis)

Zp :Center of rotation on the Zp axis

(Zp: Z-axis or an axis parallel to the Z-axis)

R :Angular displacement

(A positive value indicates a counterclockwise angular displacement.

Specify an incremental value.)

Specify a plane selection command (G17, G18, or G19) to select the plane on

which the rotational copy is made.

Xp-Yp plane (specified by G17) : G72.2 P_ L_ I_ J_ ;

D Linear copy

Zp-Xp plane (specified by G18) : G72.2 P_ L_ K_ I_ ;

Yp-Zp plane (specified by G19) : G72.2 P_ L_ J_ K_;

P :Subprogram number

L :Number of times the operation is repeated

:Shift along the Xp axis

J :Shift along the Yp axis

K :Shift along the Zp axis

Specify a plane selection command (G17, G18, or G19) to select the plane on

which the linear copy is made.

Explanations

D First block of the

Always specify a move command in the first block of a subprogram that

subprogram

performs a rotational or linear copy. If the first block contains only the

program number such as O1234; and does not have a move command,

movement may stop at the start point of the figure made by the n-th (n

= 1, 2, 3, ...) copying.

Specify the first move command in the absolute mode.

(Example of an incorrect program)

O1234 ;

G00 G90 X100.0 Y200.0 ;

⋅⋅⋅⋅

;

⋅⋅⋅⋅

;

M99 ;

247

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-63534EN/02

(Example of a correct program)

O1000 G00 G90 X100.0 Y200.0 ;

⋅⋅⋅⋅

;

⋅⋅⋅⋅

;

M99 ;

D Combination of

The linear copy command can be specified in a subprogram for a

rotational and linear

rotational copy. Also, the rotational copy command can be specified in

copying

a subprogram for a linear copy.

D Subprogram calling

In a subprogram for rotational or linear copying, M98 for calling another

subprogram or G65 for calling a macro can be specified.

D Specifying the center of

The center of rotation specified with G72.1 is processed as an absolute

rotation

position even in the incremental mode.

D Specifying address

In a block with G72.1, addresses other than P, L, Xp, Yp, Zp, or R are

ignored. The subprogram number (P), coordinates of the center of

rotation (Xp, Yp, Zp), and angular displacement (R) must be specified.

In a block with G72.2, addresses other than P, L, I, J, or K are ignored.

The subprogram number (P) and shift (I, J, K) must be specified.

D Address P

If the subprogram number specified with P is not found, P/S alarm No.

078 occurs. If P is not specified, P/S alarm No. 076 occurs.

D Address L

If L is omitted, the repetition count is assumed to be 1 and the sub-

program is called only once.

D Increment in angular

In a block with G72.1, an increment in angular displacement is specified

displacement or shift

with address R. The angular displacement of the figure made by the n-th

rotation is calculated as follows : R x (n - 1).

In a block with G72.2, an increment in shift is specified with addresses

I, J, and K. The shift of the figure made by the n-th movement is

calculated as follows :

(Programmed shift) x (n - 1).

D Nesting level of a

If a subprogram is called by G72.1 or G72.2, the nesting level is increased

subprogram

by one in the same manner as when M98 is specified.

D Block end position

The coordinates of a figure moved rotationally or linearly (block end

position) can be read from #5001 and subsequent system variables of the

custom macro of rotational or linear copy.

D Disagreement between

If the end point of the figure made by the n-th copy does not agree with

end point and start point

the start point of the figure to be made by the next (n + 1) copy, the figure

is moved from the end point to the start point, then copying is started.

(Generally, this disagreement occurs if an incorrect angular displacement

or shift is specified.)

248

13. FUNCTIONS TO SIMPLIFY

B-63534EN/02

PROGRAMMING

End point of the first copy

D D

D D D

Start point of the second copy

Start point

Main program

O1000 ;

N10 G92 X-20.0 Y0 ;

N20 G00 G90 X0 Y0 ;

N30 G01 G17 G41 X20. Y0 D01 F10 ;

(P0)

N40 Y20. ;

(P1)

N50 X30. ;

(P2)

N60 G72.2 P2000 L3 I90. J0 ;

Although a shift of 70 mm was required, I90.0 was

specified instead of I70.0. Since an incorrect shift

was specified, the end point of the figure made by

the n-th copy disagrees with the start point of the

figure to be made by the next (n + 1) copy.

Subprogram

O2000 G90 G01 X40. ;

(P3)

N100 Y40. ;

(P4)

N200 G01 X80. ;

(P5)

N300 G01 Y20. ;

(P6)

N400 X100. ;

(P7)

N500 M99;

Limitations

D Specifying two or more

G72.1 cannot be specified more than once in a subprogram for making a

commands to copy a

rotational copy (If this is attempted, P/S alarm No.160 will occur). G72.2

figure

cannot be specified more than once in a subprogram for making a linear

copy (If this is attempted, P/S alarm No. 161 will occur).

D Commands that must not

Within a program that performs a rotational or linear copy, the following

be specified

must not be specified:

⋅Command for changing the selected plane (G17 to G19)

⋅Command for specifying polar coordinates

⋅Reference position return command

⋅Coordinate system rotation, scaling, programmable mirror image

The command for rotational or linear copying can be specified after a

command for coordinate system rotation, scaling, or programmable

mirror image is executed.

249

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 9