Content      ..     10      11      12      13     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 12

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5

CANNED CYCLE FOR DRILLING

Canned cycles for drilling make it easier for the programmer to create

programs. With a canned cycle, a frequently-used machining

operation can be specified in a single block with a G function; without

canned cycles, more than one block is required. In addition, the use

of canned cycles can shorten the program to save memory.

Table 6.5 (a) lists canned cycles for drilling.

Table 6.5 (a) Canned cycles for drilling

Drilling

Operation in

Retraction

G

operation

the bottom hole

operation

Applications

code

(-Z direction)

position

(-Z direction)

G80

------

------

------

Canceling

G81

Cutting feed

------

Rapid traverse

Drilling, Spot drilling

Drilling, Counter

G82

Cutting feed

Dwell

Rapid traverse

boring

Cutting

G83

------

Rapid traverse

Peck drilling cycle

feed/intermittent

Cutting feed/

High-speed peck

G83.1

------

Rapid traverse

intermittent

drilling cycle

Dwell →

G84

Cutting feed

Cutting feed

Tapping

Spindle CCW

Dwell →

G84.2

Cutting feed

Cutting feed

Rigid tapping

Spindle CCW

G85

Cutting feed

------

Cutting feed

Boring

G89

Cutting feed

Dwell

Cutting feed

Boring

Explanation

The canned cycle for drilling consists of the following six operation

sequences.

Operation 1

Positioning of X and Z axis (Another axis

may be targeted.)

Operation 2

Rapid traverse up to point R level

Operation 3

Hole machining

Operation 4

Operation at the bottom of a hole

Operation 5

Retraction to point R level

Operation 6

Rapid traverse up to the initial level

- 315 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

Operation 1

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Fig. 6.5 (a) Operation sequence of canned cycle for drilling

- Positioning plane

A positioning plane is determined by plane selection with G17, G18,

and G19.

The axes other than the drilling axis are used as positioning axes.

- Drilling axis

Although canned cycles include tapping and boring cycles as well as

drilling cycles, in this chapter, only the term drilling will be used to

refer to operations implemented with canned cycles.

The basic axis (X, Y, or Z) that does not exist on the positioning plane

or its parallel axis is used as the drilling axis.

The axis address of the drilling axis specified in the same block as the

G codes (G81 to G89) determines whether a basic axis or one of

parallel axes is used as the drilling axis.

If the axis address of the drilling axis is not specified, the basic axis is

used as the drilling axis.

Table 6.5 (b) Positioning plane and drilling axis

G code

Positioning plane

Drilling axis

G17

Xp-Yp-plane

Zp

G18

Zp-Xp-plane

Yp

G19

Yp-Zp-plane

Xp

Xp : X axis or its parallel axis

Yp : Y axis or its parallel axis

Zp : Z axis or its parallel axis

- 316 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- Example

Suppose parameter No. 1022 is set so that U, V, and W are the parallel

axes of X, Y, and Z, respectively.

G17 G81

Z _ _: Drilling axis is Z axis.

G17 G81

W _ _: Drilling axis is W axis.

G18 G81

Y _ _: Drilling axis is Y axis.

G18 G81

V _ _: Drilling axis is V axis.

G19 G81

X _ _: Drilling axis is X axis.

G19 G81

U _ _: Drilling axis is U axis.

G17, G18, and G19 may be specified in a block in which G73 to G89

are not present.

CAUTION

Before switching between drilling axes, cancel

canned cycles.

NOTE

The Z-axis can always be used as the drilling axis

by setting FXY (bit 0 of parameter No.5101). When

FXY is 0, the Z-axis is always used as the drilling

axis.

- Specification of point R

In the Series 0i command format, the distance from the initial level to

point R is specified using an incremental value during specification of

point R.

In the Series

10/11 command format, the specification method

depends on RAB (bit 6 of parameter No. 5102). When RAB = 0, an

incremental value is always used for specification. When RAB = 1 for

G code system A, an absolute value is used for specification. When

RAB = 1 for G code system B, C, an absolute value is used in G90

mode while an incremental value is used in G91 mode.

Series 0i

Series 10/11 command format

command

format

Parameter RAB (No.5102#6) = 1

RAB=0

G code

G code system B,C

system A

Incremental

Incremental

G90

G91

Absolute

Absolute

Incremental

- Diameter/radius programming

The diameter/radius specification of canned cycles for drilling R

command in the series 10/11 command format can be matched with

the diameter/radius specification of the drilling axis by setting RDI

(bit 7 of parameter No.5102) to 1.

- 317 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

- Return point level G98/G99

In G code system A, the tool returns to the initial level from the

bottom of a hole. In G code system B or C, specifying G98 returns

the tool to the initial level from the bottom of a hole and specifying

G99 returns the tool to the point-R level from the bottom of a hole.

The following illustrates how the tool moves when G98 or G99 is

specified. Generally, G99 is used for the first drilling operation and

G98 is used for the last drilling operation.

The initial level does not change even when drilling is performed in

the G99 mode.

G98 (Return to initial level)

G99 (Return to point R level)

Initial level

Point R level

Fig. 6.5 (b) Initial level and point R level

- Number of repeats

To repeat drilling for equally-spaced holes, specify the number of

repeats in L_.

L is effective only within the block where it is specified.

Specify the first hole position in incremental mode.

If it is specified in absolute mode, drilling is repeated at the same

position.

Number of repeats L

The maximum command value = 9999

When L0 is specified, drilling data is just stored without drilling being

performed.

NOTE

For L, specify an integer of 0 or 1 to 9999.

- C axis clamp

The M code for C axis clamp can be specified in the Series 0i

command format, but it cannot be specified in the Series

10/11

command format.

- 319 -

6. MEMORY OPERATION

USING Series 10/11 FORMAT

PROGRAMMING

B-64304EN-1/01

- Disabling the Series 10/11 format

The Series 10/11 command format can be disabled only during a

canned cycle for drilling by setting F0C (bit 3 of parameter No.5102)

to 1. However, the repetitive count must be specified by address L.

CAUTION

If F16 (bit 3 of parameter No.5102) is set to 1, the

settings of RAB (bit 6 of No.5102) and RDI (bit 7 of

No.5102) are disabled, and operation when RAB=0

and RDI=0 is performed.

- Cancel

To cancel a canned cycle, use G80 or a group 01 G code.

Group 01 G codes (Example)

G00 : Positioning (rapid traverse)

G01 : Linear interpolation

G02 : Circular interpolation (CW) or helical interpolation (CW)

G03 : Circular interpolation (CCW) or helical interpolation (CCW)

- Symbols in figures

Subsequent subsections explain the individual canned cycles.

Figures in these explanations use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

P

Dwell

- 320 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.1

Drilling Cycle, Spot Drilling Cycle (G81)

The normal drilling cycle is used. The tool is then retracted from the

bottom of the hole in rapid traverse.

Format

G81 X_ Y_ Z_ R_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G81 (G98 mode)

G81 (G99 mode)

Initial level

Point R level

Point R

Point R

Point Z

Point Z

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of

the X- and Y- axes.

Then, drilling is performed from point R level to point Z.

Escaping moves in rapid traverse.

- Spindle rotation

Before specifying G81, use an auxiliary function (M code) to rotate

the spindle.

- Auxiliary function

If the G81 command and an M code are specified in the same block,

the M code is executed at the first positioning. When repetitive count

L is specified, the operation above is performed for the first time and

the M code is not performed second and later times.

- 321 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.2

Drilling Cycle, Counter Boring (G82)

The normal drilling cycle is used. Cutting feed is performed to the

bottom of the hole, dwelling is performed at the bottom, and then

escaping from the bottom is performed in rapid traverse.

The accuracy of the hole depth is improved.

Format

G82 X_ Y_ Z_ R_ P_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of a hole

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G81 (G98 mode)

G81 (G99 mode)

Initial level

Point R level

Point R

Point R

Point Z

Point Z

P

P

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of

the X- and Y- axes.

Then, drilling is performed from point R level to point Z.

Dwelling is performed at the bottom of the hole and then escaping is

performed in rapid traverse.

- Spindle rotation

Before specifying G82, use an auxiliary function (M code) to rotate

the spindle.

- Auxiliary function

If the G82 command and an M code are specified in the same block,

the M code is executed at the first positioning. When repetitive count

L is specified, the operation above is performed for the first time and

the M code is not performed second and later times.

- 323 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.3

Peck Drilling Cycle (G83)

Peck drilling is performed.

Cutting feed is performed intermittently to the bottom of the hole

while chips are discharged.

Format

G83 X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time

Q_

: Depth of cut for each cutting feed

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G83 (G98 mode)

G83 (G99 mode)

Initial level

Point R level

Point R

Point R

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

P

P

Explanation

- Operations

Q indicates the depth of cut for each operation and is specified by an

incremental value.

In the second and later cutting operations, rapid traverse is changed to

cutting feed at the point distance "d" back from the previously drilled

position. "d" is set in parameter No. 5115.

A positive value must be specified for Q. A negative value is

ignored.

- Spindle rotation

Before specifying G83, use an auxiliary function (M code) to rotate

the spindle.

- Auxiliary function

If the G83 command and an M code are specified in the same block,

the M code is executed at the first positioning. When repetitive count

L is specified, the operation above is performed for the first time and

the M code is not performed second and later times.

- 325 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.4

High-speed Peck Drilling Cycle (G83.1)

This cycle performs high-speed peck drilling. It performs cutting feed

intermittently while discharging chips.

Format

G83.1 X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time

Q_

: Depth of cut for each cutting feed

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed)

G83.1 (G98 mode)

G83.1 (G99 mode)

Initial level

Point R

Point R

Point R level

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

P

P

Explanation

- Operations

Since intermittent feed in the Z-axis direction makes discharge of

chips easier and allows the fine setting of the escaping amount,

efficient machining can be performed.

Escape amount d is set in parameter No. 5114.

Escaping moves in rapid traverse.

- Spindle rotation

Before specifying G83.1, use an auxiliary function (M code) to rotate

the spindle.

- 327 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.5

Tapping Cycle (G84)

This cycle performs tapping.

In this tapping cycle, when the bottom of the hole has been reached,

the spindle is rotated in the reverse direction.

Format

G84 X_ Y_ Z_ R_ P_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G84 (G98 mode)

G84 (G99 mode)

Initial level

Spindle CW

Spindle CW

Point R

Point R

Point R level

Point Z

P

Point Z

P

Spindle CCW

Spindle CCW

Explanation

- Operations

Tapping is performed by rotating the spindle clockwise.

CAUTION

Feedrate override is ignored during tapping. In

addition, applying feed hold does not stop the

machine until return operation is completed.

- Spindle rotation

Before specifying G84, use an auxiliary function (M code) to rotate

the spindle.

When drilling in which the distance from the hole position and initial

level to the point R level is short is continuously performed, the

spindle may not reach the normal speed by the time cutting operation

for the hole is ready to be performed. In this case, reserve a time by

inserting dwelling by G04 before each drilling operation without

specifying repetitive count L.

Since this consideration may not be required depending on the

machine type, refer to the manual issued by the machine tool builder.

- 329 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.6

Tapping Cycle (G84.2)

Controlling the spindle motor in the same way as a servo motor

executes the high-speed tapping cycle.

Format

G84.2 X_ Y_ Z_ R_ P_ F_ L_ S_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

S_

: Spindle speed

G84.2 (G98 mode)

G84.2 (G99 mode)

Spindle stop

Spindle stop

Initial level

Spindle CW

Spindle stop

Spindle CW

Spindle stop

Point R

Point R

Point R level

Point Z

P

Point Z

P

Spindle stop

Spindle CCW

Spindle stop

Spindle CCW

A G code cannot discriminate between the front face tapping cycle

and side face tapping cycle using Series 10/11 format commands.

The drilling axis is determined by plane selection (G17, G18, or G19).

Specify the plane selection that becomes equivalent to the front face

tapping cycle or side face tapping cycle as appropriate.

(When bit 0

(FXY) of parameter No. 5101 is set to 0, the Z-axis is used as the

drilling axis. When the bit is set to 1, place selection is as follows.)

Plane selection

Drilling axis

G17 Xp-Yp plane

Zp

G18 Zp-Xp plane

Yp

G19 Yp-Zp plane

Xp

Xp: X-axis or an axis parallel to it

Yp: Y-axis or an axis parallel to it

Zp: Z-axis or an axis parallel to it

- 331 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.7

Boring Cycle (G85)

This cycle is used to bore a hole.

Format

G85 X_ Y_ Z_ R_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G85 (G98 mode)

G85 (G99 mode)

Initial level

Point R level

Point R

Point R

Point Z

Point Z

Explanation

- Operations

Rapid traverse to the point R level is performed after positioning of

the X- and Y- axes.

Then, drilling is performed from point R level to point Z.

After reaching point Z, return to point R in cutting feed.

- Spindle rotation

Before specifying G85, use an auxiliary function (M code) to rotate

the spindle.

- Auxiliary function

If the G85 command and an M code are specified in the same block,

the M code is executed at the first positioning. When repetitive count

L is specified, the operation above is performed for the first time and

the M code is not performed second and later times.

- 333 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.8

Boring Cycle (G89)

This cycle is used to bore a hole.

Format

G89 X_ Y_ Z_ R_ P_ F_ L_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time at the bottom of a hole

F_

: Cutting feedrate

L_

: Number of repeats (When it is needed.)

G89 (G98 mode)

G89 (G99 mode)

Initial level

Point R level

Point R

Point R

Point Z

Point Z

P

P

Explanation

- Operations

This is the same as G85, but dwelling is performed at the bottom of

the hole.

- Spindle rotation

Before specifying G89, use an auxiliary function (M code) to rotate

the spindle.

- Auxiliary function

If the G89 command and an M code are specified in the same block,

the M code is executed at the first positioning. When repetitive count

L is specified, the operation above is performed for the first time and

the M code is not performed second and later times.

- 335 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.5.9

Canned Cycle for Drilling Cancel (G80)

G80 cancels canned cycle for drilling.

Format

G80 ;

Explanation

Canned cycle for drilling is canceled to perform normal operation.

Point R and point Z are cleared.

Other drilling data is also canceled (cleared).

6.5.10 Precautions to be Taken by Operator

- Reset and emergency stop

Even when the controller is stopped by resetting or emergency stop in

the course of drilling cycle, the drilling mode and drilling data are

saved ; with this mind, therefore, restart operation.

- Single block

When drilling cycle is performed with a single block, the operation

stops at the end points of operations 1, 2, 6 in Fig. 6.5 (a).

Consequently, it follows that operation is started up 3 times to drill

one hole. The operation stops at the end points of operations 1, 2

with the feed hold lamp ON. If there is a remaining repetitive count

at the end of operation 6, the operation is stopped by feed hold. If

there is no remaining repetitive count, the operation is stopped in the

single block stop state.

- Feed hold

When "Feed Hold" is applied between operations 3 and 5 by G84/G88,

the feed hold lamp lights up immediately if the feed hold is applied

again to operation 6.

- Override

During operation with G84 and G88, the feedrate override is 100%.

- 337 -

B-64304EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

7.1

POLYGON TURNING (G50.2, G51.2)

Polygon turning means machining a workpiece to a polygonal figure

by rotating the workpiece and tool at a certain ratio.

W orkpiece

W orkpiece

Tool

Fig. 7.1 (a) Polygon turning

By changing conditions which are rotation ratio of workpiece and tool

and number of cutters, the workpiece can be machined to a square or

hexagon. The machining time can be reduced as compared with

polygonal figure machining using the polar coordinate interpolation.

The machined figure, however, is not exactly polygonal. Generally,

polygon turning is used for the heads of square and/or hexagon bolts

or hexagon nuts.

As the tool rotary axis, one of the following can be used:

•

CNC controlled axis (servo axis)

•

Second spindle (Two serial spindles are connected.)

Polygonal machining performed using a servo axis as the tool rotary

axis is referred to as polygon turning.

Polygonal machining

performed using the second spindle as the tool rotary axis is referred

to as polygon turning with two spindles.

Function name

Workpiece axis

Tool rotary axis

Spindle

(Either an analog spindle or

serial spindle is usable.

Polygon turning

Servo axis

However, a detector

equivalent to a position

coder is required.)

Polygon turning with

Spindle

Spindle

two spindles

(Serial spindle)

(Serial spindle)

- 339 -

B-64304EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

NOTE

4

For the Y-axis engaged in polygon turning, jog feed

and handle feed are disabled.

5

For the Y-axis not engaged in polygon turning, a

move command can be specified as in the case of

other controlled axes.

6

The Y-axis engaged in polygon turning is not

counted in the number of simultaneously controlled

axes.

7

One workpiece must be machined using a fixed

spindle speed until the workpiece is finished.

8

Polygon turning with two spindles cannot be used at

the same time.

9

G50.2 is the G code for suppressing buffering.

CAUTION

1

During polygon turning, threading cannot be

performed.

2

For the Y-axis engaged in synchronous operation,

the signals below are valid or invalid:

Signals valid for the Y-axis

• Machine lock

• Servo-off

Signals invalid for the Y-axis

• Feed hold

• Interlock

• Override

• Dry run

(At dry run time, however, the one-rotation

signal is not awaited in a G51.2 block.)

- 341 -

B-64304EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

- Principle of polygon turning

In the figure below the radius of tool and workpiece are A and B, and

the angular speeds of tool and workpiece are α and β. The origin of

XY Cartesian coordinates is assumed to be the center of the

workpiece.

Simplifying the explanation, consider that the tool center exists at the

position

P_o (A, 0) on the workpiece periphery, and the tool nose starts from

position P_to (A-B, 0).

A : Workpiece radius

Y

B : Rool radius

α : Workpiece angular speed

β : Tool angular speed

X

Angular speed α

A

B

P_to

Tool

(0,0)

P_o

Angular

Workpiece

speed β

Po

(A, 0)

Pto (A-B, 0)

Fig. 7.1 (b) Principle of polygon turning

Pt (Xt, Yt)

B

P

βt

A

αt

Start point

(0, 0)

Fig. 7.1 (c) Tool nose position

In this case, the tool nose position Pt (Xt, Yt) after time t is expressed

by equations 1 and 2:

Xt=Acosαt-Bcos(β-α)t

(Equation 1)

Yt=Asinαt+Bsin(β-α)t

(Equation 2)

Assuming that the rotation ration of workpiece to tool is 1:2, namely,

β=2α, equations 1 and 2 are modified as follows:

Xt=Acosαt-Bcosαt=(A-B)cosαt

(Equation 1)'

Xt=Asinαt+Bsinαt=(A+B)sinαt

(Equation 2)'

These equations indicate that the tool nose path draws an ellipse with

longer diameter A+B and shorter diameter A-B.

Then consider the case when one tool is set at 180° symmetrical

positions, for a total of two. A square can be machined with these

tools as shown below.

- 343 -

Content      ..     10      11      12      13     ..