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

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64304EN-2/01

Table 2 G code list

G code

Group

Function

G54

Workpiece coordinate system 1 selection

G54.1

Additional workpiece coordinate system selection

G55

Workpiece coordinate system 2 selection

G56

Workpiece coordinate system 3 selection

G57

Workpiece coordinate system 4 selection

G58

Workpiece coordinate system 5 selection

G59

Workpiece coordinate system 6 selection

G60

Single direction positioning

G61

Exact stop mode

G62

Automatic corner override

G63

Tapping mode

G64

Cutting mode

G65

Macro call

G66

Macro modal call

G67

Macro modal call cancel

G68

Coordinate system rotation mode on

G69

Coordinate system rotation mode off

G73

Peck drilling cycle

G74

Left-handed tapping cycle

G75

Plunge grinding cycle (for grinding machine)

G76

Fine boring cycle

G77

Plunge direct sizing/grinding cycle (for grinding machine)

G78

Continuous-feed surface grinding cycle (for grinding machine)

G79

Intermittent-feed surface grinding cycle (for grinding machine)

Canned cycle cancel

G80

Electronic gear box : synchronization cancellation

G80.4

Electronic gear box : synchronization cancellation

G81.4

Electronic gear box : synchronization start

G81

Drilling cycle or spot boring cycle

Electronic gear box : synchronization start

G82

Drilling cycle or counter boring cycle

G83

Peck drilling cycle

G84

Tapping cycle

G84.2

Rigid tapping cycle (FS10/11 format)

G84.3

Left-handed rigid tapping cycle (FS10/11 format)

G85

Boring cycle

G86

Boring cycle

G87

Back boring cycle

G88

Boring cycle

G89

Boring cycle

G90

Absolute programming

G91

Incremental programming

G91.1

Checking the maximum incremental amount specified

G92

Setting for workpiece coordinate system or clamp at maximum spindle speed

G92.1

Workpiece coordinate system preset

G93

Inverse time feed

G94

Feed per minute

G95

Feed per revolution

G96

Constant surface speed control

G97

Constant surface speed control cancel

- 16 -

B-64304EN-2/01

PROGRAMMING

3.INTERPOLATION FUNCTION

3.1

SINGLE DIRECTION POSITIONING (G60)

For accurate positioning without play of the machine (backlash), final

positioning from one direction is available.

Overrun

Start point

Temporary stop

End point

Format

G60 IP_ ;

IP_ : For an absolute programming, the coordinates of an

end point, and for an incremental programming, the

distance the tool moves.

Explanation

An overrun and a positioning direction are set by the parameter No.

5440. Even when a commanded positioning direction coincides with

that set by the parameter, the tool stops once before the end point.

G60, which is a one-shot G-code, can be used as a modal G-code in

group 01 by setting 1 to the bit 0 (MDL) of parameter No. 5431.

This setting can eliminate specifying a G60 command for every block.

Other specifications are the same as those for a one-shot G60

command. When a one-shot G code is specified in the single direction

positioning mode, the one-shot G command is effective like G codes

in group 01.

(Example)

When one-shot G60 commands are used.

G90;

G60 X0Y0;

G60 X100;

Single direction positioning

G60 Y100;

G04 X10;

G00 X0Y0;

When modal G60 command is used.

G90G60;

Single direction positioning mode start

X0Y0;

X100;

Single direction positioning

Y100;

G04X10;

G00X0 Y0;

Single direction positioning mode cancel

- 19 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Overview of operation

•

In the case of positioning of non-linear interpolation type (bit

1 (LRP) of parameter No. 1401 = 0)

As shown below, single direction positioning is performed

independently along each axis.

Overrun distance in the Z-axis direction

Overrun distance in the

X-axis direction

Programmed end point

Programmed start point

•

In the case of positioning of linear interpolation type (bit 1

(LRP) of parameter No. 1401 = 1)

Positioning of interpolation type is performed until the tool once

stops before or after a specified end point. Then, the tool is

positioned independently along each axis until the end point is

reached.

Overrun distance in the Z-axis direction

Overrun distance in the

X-axis direction

Programmed end point

Programmed start point

Limitation

• Single direction positioning is not performed along an axis for

which no overrun distance is set in parameter No. 5440.

• Single direction positioning is not performed along an axis for

which travel distance 0 is specified.

• The mirror image function is not applied in a parameter-set

direction. Even in the mirror image mode, the direction of single

direction positioning remains unchanged. If positioning of linear

interpolation type is used, and the state of mirror image when a

single direction positioning block is looked ahead differs from

the state of mirror image when the execution of the block is

started, an alarm is issued. When switching mirror image in the

middle of a program, disable looking ahead by specifying a

non-buffering M code. Then, switch mirror image when there is

no look-ahead block.

- 20 -

B-64304EN-2/01

PROGRAMMING

3.INTERPOLATION FUNCTION

• In the cylindrical interpolation mode (G07.1), single direction

positioning cannot be used.

• When specifying single direction positioning on a machine that

uses arbitrary angular axis control, first position the angular axis

then specify the positioning of the Cartesian axis. If the reverse

specification order is used, or the angular axis and Cartesian axis

are specified in the same block, an incorrect positioning direction

can result.

•

In positioning at a restart position by program restart function,

single direction positioning is not performed.

•

During canned cycle for drilling, no single direction positioning

is effected in drilling axis.

•

The single direction positioning does not apply to the shift

motion in the canned cycles of G76 and G87.

- 21 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-2/01

3.2

THREADING (G33)

Straight threads with a constant lead can be cut. The position coder

mounted on the spindle reads the spindle speed in real-time. The read

spindle speed is converted to the feedrate per minute to feed the tool.

Format

G33IP_ F_ ;

F : Long axis direction lead

Workpiece

Explanation

In general, threading is repeated along the same tool path in rough

cutting through finish cutting for a screw. Since threading starts

when the position coder mounted on the spindle outputs a 1-turn

signal, threading is started at a fixed point and the tool path on the

workpiece is unchanged for repeated threading. Note that the spindle

speed must remain constant from rough cutting through finish cutting.

If not, incorrect thread lead will occur.

In general, the lag of the servo system, etc. will produce somewhat

incorrect leads at the starting and ending points of a thread cut. To

compensate for this, a threading length somewhat longer than required

should be specified.

Table 3.2 (a) lists the ranges for specifying the thread lead.

Table 3.2 (a) Ranges of lead sizes that can be specified

Least

command

Command value range of the lead

increment

0.001 mm

F1 to F50000 (0.01 to 500.00mm)

Metric input

0.0001 mm

F1 to F50000 (0.01 to 500.00mm)

0.0001 inch

F1 to F99999 (0.0001 to 9.9999inch)

Inch input

0.00001 inch

F1 to F99999 (0.0001 to 9.9999inch)

- 22 -

B-64304EN-2/01

PROGRAMMING

3.INTERPOLATION FUNCTION

NOTE

1 The spindle speed is limited as follows :

1 ≤ spindle speed ≤ (Maximum feedrate) / (Thread

lead)

Spindle speed : min^-1

Thread lead : mm or inch

Maximum feedrate : mm/min or inch/min ; maximum

command-specified feedrate for feed-per-minute

mode or maximum feedrate that is determined

based on mechanical restrictions including those

related to motors, whichever is smaller

2 Cutting feedrate override is not applied to the

converted feedrate in all machining process from

rough cutting to finish cutting. The feedrate is fixed

at 100%

3 The converted feedrate is limited by the upper

feedrate specified.

4 Feed hold is disabled during threading. Pressing the

feed hold key during threading causes the machine

to stop at the end point of the next block after

threading (that is, after the G33 mode is terminated)

Example

Threading at a pitch of 1.5mm

G33 Z10. F1.5;

- 23 -

4.COORDINATE VALUE AND

B-64304EN-2/01

PROGRAMMING

DIMENSION

4.1

POLAR COORDINATE COMMAND (G15, G16)

The end point coordinate value can be input in polar coordinates

(radius and angle).

The plus direction of the angle is counterclockwise of the selected

plane first axis + direction, and the minus direction is clockwise.

Both radius and angle can be commanded in either absolute or

incremental programming (G90, G91).

Format

Gxx Gyy G16; Starting the polar coordinate

command (polar coordinate mode)

G00 IP_ ;

Polar coordinate command

G15;

Canceling the polar coordinate

command (polar coordinate mode)

G16

: Polar coordinate command

G15

: Polar coordinate command cancel

Gxx

: Plane selection of the polar coordinate command

(G17, G18 or G19)

Gyy

: Center selection of the polar coordinate command

(G90 or G91)

G90 specifies the origin of the workpiece coordinate

system as the origin of the polar coordinate system,

from which a radius is measured.

G91 specifies the current position as the origin of the

polar coordinate system, from which a radius is

measured.

IP_

: Specifying the addresses of axes constituting the

plane selected for the polar coordinate system, and

their values

First axis : radius of polar coordinate

Second axis : angle of polar coordinate

- 25 -

4. COORDINATE VALUE AND

DIMENSION

PROGRAMMING

B-64304EN-2/01

- Setting the origin of the workpiece coordinate system as the origin of the polar

coordinate system

Specify the radius (the distance between the origin and the point) to be

programmed with an absolute programming. The origin of the

workpiece coordinate system is set as the origin of the polar

coordinate system.

When a local coordinate system (G52) is used, the origin of the local

coordinate system becomes the center of the polar coordinates.

Command position

Radius

Angle

Actual position

Angle

Actual position

When the angle is specified with an

absolute command

incremental command

- Setting the current position as the origin of the polar coordinate system

Specify the radius (the distance between the current position and the

point) to be programmed with an incremental programming. The

current position is set as the origin of the polar coordinate system.

Command position

Angle

Radius Angle

Radius

Actual position

When the angle is specified with an

absolute command

incremental command

Example

Bolt hole circle

- The origin of the workpiece coordinate

system is set as the origin of the polar

coordinate system.

- The XY plane is selected.

150°

30°

270°

100mm

- 26 -

4.COORDINATE VALUE AND

B-64304EN-2/01

PROGRAMMING

DIMENSION

- Specifying angles and a radius with absolute programmings

N1 G17 G90 G16 ; Specifying the polar coordinate command and

selecting the XY plane

Setting the origin of the workpiece coordinate

system as the origin of the polar coordinate

system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ;

Specifying a distance of 100 mm and an angle

of 30 degrees

N3 Y150.0 ;

Specifying a distance of 100 mm and an angle

of 150 degrees

N4 Y270.0 ;

Specifying a distance of 100 mm and an angle

of 270 degrees

N5 G15 G80 ;

Canceling the polar coordinate command

- Specifying angles with incremental programmings and a radius with absolute

programmings

N1 G17 G90 G16; Specifying the polar coordinate command and

selecting the XY plane

Setting the origin of the workpiece coordinate

system as the origin of the polar coordinate

system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ;

Specifying a distance of 100 mm and an angle

of 30 degrees

N3 G91 Y120.0 ;

Specifying a distance of 100 mm and an angle

of +120 degrees

N4 Y120.0 ;

Specifying a distance of 100 mm and an angle

of +120 degrees

N5 G15 G80 ;

Canceling the polar coordinate command

Limitation

- Specifying a radius in the polar coordinate mode

In the polar coordinate mode, specify a radius for circular

interpolation or helical interpolation (G02, G03) with R.

- Axes that are not considered part of a polar coordinate command in the polar

coordinate mode

Axes specified for the following commands are not considered part of

the polar coordinate command:

• Dwell (G04)

• Programmable data input (G10)

• Local coordinate system setting (G52)

• Workpiece coordinate system setting (G92)

• Machine coordinate system setting (G53)

• Stored stroke check (G22)

• Coordinate system rotation (G68)

• Scaling (G51)

- Optional chamfering and corner R

Optional chamfering and corner R cannot be specified in polar

coordinate mode.

- 27 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.1

CANNED CYCLE FOR DRILLING

Overview

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, normally more than one block is required. In addition,

the use of canned cycles can shorten the program to save memory.

Table 5.1 (a) lists canned cycles for drilling.

Table 5.1 (a) Canned cycles for drilling

Drilling

Operation at the

Retraction

G code

Application

(-Z direction)

bottom of a hole

(+Z direction)

High-speed

Intermittent

G73

Rapid traverse

peck drilling

feed

cycle

Dwell →

Left-hand

G74

Feed

Spindle CW

tapping cycle

Oriented spindle

Fine boring

G76

Feed

Rapid traverse

stop

cycle

G80

Cancel

Drilling cycle,

G81

Feed

Rapid traverse

spot drilling

cycle

Drilling cycle,

G82

Feed

Dwell

Rapid traverse

counter boring

cycle

Intermittent

Peck drilling

G83

Rapid traverse

feed

cycle

Dwell →

G84

Feed

Tapping cycle

Spindle CCW

G85

Feed

Boring cycle

G86

Feed

Spindle stop

Rapid traverse

Boring cycle

Back boring

G87

Feed

Spindle CW

Rapid traverse

cycle

Dwell →

G88

Feed

Manual

Boring cycle

Spindle stop

G89

Feed

Dwell

Feed

Boring cycle

Explanation

A canned cycle for drilling consists of a sequence of six operations.

Operation 1

Positioning of axes X and Y

(including also

another axis)

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 point

- 29 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

Operation 1

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Fig. 5.1 (a) Operation sequence of canned cycle for drilling

- Positioning plane

The positioning plane is determined by plane selection code G17, G18,

or G19.

The positioning axis is an axis other than the drilling axis.

- Drilling axis

Although canned cycles for drilling 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 drilling axis is a basic axis (X, Y, or Z) not used to define the

positioning plane, or any axis parallel to that basic axis.

The axis (basic axis or parallel axis) used as the drilling axis is

determined according to the axis address for the drilling axis specified

in the same block as G codes G73 to G89.

If no axis address is specified for the drilling axis, the basic axis is

assumed to be the drilling axis.

Table 5.1 (b) Positioning plane and drilling axis

G code

Positioning plane

Drilling axis

G17

Xp-Yp plane

G18

Zp-Xp plane

G19

Yp-Zp plane

Xp: X axis or an axis parallel to the X axis

Yp: Y axis or an axis parallel to the Y axis

Zp: Z axis or an axis parallel to the Z axis

- 30 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

Example

Assume that the U, V and W axes be parallel to the X, Y, and Z axes

respectively. This condition is specified by parameter No. 1022.

G17 G81 Z_ _

: The Z axis is used for drilling.

G17 G81 W_ _ : The W axis is used for drilling.

G18 G81 Y_ _ : The Y axis is used for drilling.

G18 G81 V_ _ : The V axis is used for drilling.

G19 G81 X_ _ : The X axis is used for drilling.

G19 G81 U_ _ : The U axis is used for drilling.

G17 to G19 may be specified in a block in which any of G73 to

G89 is not specified.

CAUTION

Switch the drilling axis after canceling a canned

cycle for drilling.

NOTE

A parameter FXY (No. 5101 #0) can be set to the Z

axis always used as the drilling axis. When

FXY=0, the Z axis is always the drilling axis.

- Travel distance along the drilling axis G90/G91

The travel distance along the drilling axis varies for G90 and G91 as

follows:

G90 (Absolute programming)

G91 (Incremental programming)

Point R

Z = 0

Point Z

Fig. 5.1 (b) Absolute programming and incremental programming

- Drilling mode

G73, G74, G76, and G81 to G89 are modal G codes and remain in

effect until canceled. When in effect, the current state is the drilling

mode.

Once drilling data is specified in the drilling mode, the data is retained

until modified or canceled.

Specify all necessary drilling data at the beginning of canned cycles;

when canned cycles are being performed, specify data modifications

only.

- 31 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- Return point level G98/G99

When the tool reaches the bottom of a hole, the tool may be returned

to point R or to the initial level. These operations are specified with

G98 and G99. 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. 5.1 (c) Initial level and point R level

- Repeat

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

repeats in K_.

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

Specify the first hole position in incremental programming (G91).

If it is specified in absolute programming (G90), drilling is repeated at

the same position.

Number of repeats K

The maximum command value = 9999

If K0 is specified, drilling data is stored, but drilling is not performed.

NOTE

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

- Single block

If a drilling cycle is performed in a single block, the control unit stops

at each of the end points of operations 1, 2, and 6 in Figure 5.1 (a).

This means that three starts are made to make a single hole. At the end

points of operations 1 and 2, the feed hold lamp turns on and the

control unit stops. If the repetitive count is not exhausted at the end

point of operation 6, the control unit stops in the feed hold mode, and

otherwise, stops in the single block stop mode. Note that G87 does not

cause a stop at point R in G87. G88 causes a stop at point Z after a

dwell.

- 32 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Cancel

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

Group 01 G codes

G00 : Positioning (rapid traverse)

G01 : Linear interpolation

G02 : Circular interpolation or helical interpolation (CW)

G03 : Circular interpolation or helical interpolation (CCW)

G60 : Single directional positioning (if bit 0 (MDL) of parameter No.

5431 is "1")

- Symbols in figures+

Subsequent sections explain the individual canned cycles. Figures in

these Explanation use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Manual feed

Oriented spindle stop

OSS

(The spindle stops at a fixed rotation position)

Shift (rapid traverse G00)

Dwell

- 33 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

5.1.1

High-Speed Peck Drilling Cycle (G73)

This cycle performs high-speed peck drilling.

It performs

intermittent cutting feed to the bottom of a hole while removing chips

from the hole.

Format

G73 X_ Y_ Z_ R_ Q_ F_ K_ ;

X_ Y_ : Hole position data

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

: The distance from the initial level to point R level

: Depth of cut for each cutting feed

: Cutting feedrate

: Number of repeats (if required)

G73 (G98)

G73 (G99)

Initial level

Point R

Point R level

Point Z

Explanation

- Operations

The high-speed peck drilling cycle performs intermittent feeding

along the Z-axis. When this cycle is used, chips can be removed

from the hole easily, and a smaller value can be set for retraction.

This allows, drilling to be performed efficiently. Set the clearance, d,

in parameter 5114.

The tool is retracted in rapid traverse.

- Spindle rotation

Before specifying G73, rotate the spindle using an auxiliary function

(M code).

- 34 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Auxiliary function

When the G73 code and an M code are specified in the same block,

the M code is executed at the time of the first positioning operation.

When K is used to specify the number of repeats, the M code is

executed for the first hole only; for the second and subsequent holes,

the M code is not executed.

- Tool length compensation

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

the canned cycle for drilling, the offset is applied after the time of

positioning to point R.

Limitation

- Axis switching

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

must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling

is not performed.

- Q

Specify Q in blocks that perform drilling. If they are specified in a

block that does not perform drilling, they cannot be stored as modal

data.

- Cancel

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

single block. Otherwise, G73 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ;

Cause the spindle to start rotating.

G90 G99 G73 X300. Y-250. Z-150. R-100. Q15. F120. ;

Position, drill hole 1, then return to point R.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial level.

G80 G28 G91 X0 Y0 Z0 ; Return to the reference position

M5 ;

Cause the spindle to stop rotating.

- 35 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

5.1.2

Left-Handed Tapping Cycle (G74)

This cycle performs left-handed tapping. In the left-handed tapping

cycle, when the bottom of the hole has been reached, the spindle

rotates clockwise.

Format

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

: The distance from the initial level to point R level

: Dwell time

: Depth of cut for each cutting feed (bit 6 (PCT) of

parameter No. 5104 = "1")

: Cutting feedrate

: Number of repeats (if required)

G74 (G98)

G74 (G99)

Initial level

Spindle

CCW

Point R

Point R level

Point Z

Spindle CW

Explanation

- Operations

Tapping is performed by turning the spindle counterclockwise.

When the bottom of the hole has been reached, the spindle is rotated

clockwise for retraction. This creates a reverse thread.

CAUTION

Feedrate overrides are ignored during left-handed

tapping. A feed hold does not stop the machine

until the return operation is completed.

- 36 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

- Spindle rotation

Before specifying G74, use an auxiliary function (M code) to rotate

the spindle counterclockwise.

If drilling is continuously performed with a small value specified for

the distance between the hole position and point R level or between

the initial level and point R level, the normal spindle speed may not be

reached at the start of hole cutting operation. In this case, insert a

dwell before each drilling operation with G04 to delay the operation,

without specifying the number of repeats for K. For some machines,

the above note may not be considered. Refer to the manual provided

by the machine tool builder.

- Q command

After setting bit 6 (PCT) of parameter No. 5104 to 1, add address Q to

the ordinary tapping cycle command format and specify the depth of

cut for each tapping.

In the peck tapping cycle, the tool is retracted to point R for each

tapping. In the high-speed peck tapping cycle, the tool is retracted

by the retraction distance specified for parameter No. 5213 in advance.

Which operation is to be performed can be selected by setting bit 5

(PCP) of parameter No. 5200.

Operation

First, ordinary tapping cycle operation is explained as basic operation.

Before specifying a tapping cycle, rotate the spindle using an auxiliary

function.

When a command to position the tool to a hole position,

positioning is performed.

When point R is specified, positioning to point R is performed.

Tapping is performed to the bottom of the hole in cutting feed.

When a dwell time (P) is specified, the tool dwells.

Auxiliary function M05 (spindle stop) is output and the machine

enters the FIN wait state.

When FIN is returned, auxiliary function M04 (reverse spindle

rotation) is output and the machine enters the FIN wait state.

When FIN is returned, the tap is removed until point R is reached

in cutting feed.

When a dwell time (P) is specified, the tool dwells.

Auxiliary function M05 (spindle stop) is output and the machine

enters the FIN wait state.

10. When FIN is returned, auxiliary function M03 (forward spindle

rotation) is output, and the machine enters the FIN wait state.

11. When FIN is returned, the tool returns to the initial point in rapid

traverse when return to the initial level is specified.

When the repetitive count is specified, operation is repeated from step

- 37 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

Tapping

<1> Positioning to a hole

<1> Positioning to the next hole

<11> Positioning to the initial point

<2> Positioning to point R

Point R level

<8> Dwell

<3> Tapping to the bottom of the hole

<9> Output of auxiliary function M05

<10> Output of auxiliary function M03

<7> Return to point R

<4> Dwell

Hole bottom level

<5> Output of auxiliary function M05

Workpiece

<6> Output of auxiliary function M04

Peck tapping cycle

When bit 6 (PCT) of parameter No. 5104 is set to 1 and bit 5 (PCP) of

parameter No. 5200 is set to 1, the peck tapping cycle is used.

Step 3 of the tapping cycle operation described above changes as

follows:

3-1. The tool cuts the workpiece by the depth of cut q specified by

address Q.

3-2. Auxiliary function M05 (spindle stop) is output, and the machine

enters the FIN wait state.

3-3. When FIN is returned, auxiliary function M04 (reverse spindle

rotation) is output, and the machine enters the FIN wait state.

3-4. When FIN is returned, the tool is retracted to point R in cutting

feed.

3-5. Auxiliary function M05 (spindle stop) is output, and the machine

enters the FIN wait state.

3-6. When FIN is returned, auxiliary function M03 (forward spindle

rotation) is output, and the machine enters the FIN wait state.

3-7. When FIN is returned, the tool moves to the position the

clearance d (parameter No. 5213) apart from the previous cutting

point in cutting feed (approach).

3-1. The tool cuts the workpiece by the clearance d (parameter No.

5213) + depth of cut q (specified by address Q).

Tapping is performed to the bottom of the hole by repeating the above

steps.

When a dwell time (P) is specified, the tool dwells only when it

reaches at the bottom of the hole and reaches point R last.

- 38 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

q: Depth of cut

<5> Output of auxiliary function M05

d: Clearance

<6> Output of auxiliary function M03

<7> Approach

Point R level

<4> Retraction

<1> Tapping

<4> Retraction

<7> Approach

<1> Tapping

<2> Output of auxiliary function M05

<3> Output of auxiliary function M04

Repeated until the bottom of the hole is reached.

Workpiece

Hole bottom level

High-speed peck tapping cycle

When bit 6 (PCT) of parameter No. 5104 is set to 1 and bit 5 (PCP) of

parameter No. 5200 is set to 0, the high-speed peck tapping cycle is

used.

Step 3 of the tapping cycle operation described above changes as

follows:

3-1. The tool cuts the workpiece by the depth of cut q specified by

address Q.

3-2. Auxiliary function M05 (spindle stop) is output, and the machine

enters the FIN wait state.

3-3. When FIN is returned, auxiliary function M04 (reverse spindle

rotation) is output, and the machine enters the FIN wait state.

3-4. When FIN is returned, the tool is retracted by the retraction

distance d specified by parameter No. 5213 in cutting feed.

3-5. Auxiliary function M05 (spindle stop) is output, and the machine

enters the FIN wait state.

3-6. When FIN is returned, auxiliary function M03 (forward spindle

rotation) is output, and the machine enters the FIN wait state.

3-1. When FIN is returned, the tool cuts the workpiece by the

retraction distance d

(parameter No. 5213) + depth of cut q

(specified by address Q).

Tapping is performed to the bottom of the hole by repeating the above

steps.

- 39 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

When a dwell time (P) is specified, the tool dwells only

when it

reaches at the bottom of the hole and reaches point R.

q: Depth of cut

d: Retraction distance

Point R level

<1> Tapping

<5> Output of auxiliary function M05

<6> Output of auxiliary function M03

<4> Retraction

<1> Tapping

<4> Retraction

<1> Tapping

<2> Output of auxiliary function M05

<3> Output of auxiliary function M04

Repeated until the bottom of the hole is reached.

Workpiece

Hole bottom level

Notes

The depth of cut specified by address Q is stored as a modal

value until the canned cycle mode is canceled.

In both examples 1 and 2 below, address Q is not specified in the

N20 block, but the peck tapping cycle is performed because the

value specified by address Q is valid as a modal value. If this

operation is not suitable, specify G80 to cancel the canned cycle

mode as shown in N15 in example 3 or specify Q0 in the tapping

block as shown in N20 in example 4.

Example 1

N10 G84 X100. Y150. Z-100. Q20. ;

N20 X150. Y200 ; ĸ The peck tapping cycle is also performed

in this block.

N30 G80 ;

Example 2

N10 G83 X100. Y150. Z-100. Q20. ;

N20 G84 Z-100. ; ĸ The peck tapping cycle is also performed in

this block.

N30 G80 ;

- 40 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

Example 3

N10 G83 X100. Y150. Z-100. Q20. ;

N15 G80 ; ĸ The canned cycle mode is canceled.

N20 G84 Z-100. ;

N30 G80 ;

Example 4

N10 G83 X100. Y150. Z-100. Q20. ;

N20 G84 Z-100. Q0 ; ĸQ0 is added.

N30 G80 ;

The unit for the reference axis that is set by parameter No. 1031,

not the unit for the drilling axis is used as the unit of Q. Any

sign is ignored.

- Auxiliary function

When the G74 command and an M code are specified in the same

block, the M code is executed at the time of the first positioning

operation. When K is used to specify the number of repeats, the M

code is executed for the first hole only; for the second and subsequent

holes, the M code is not executed.

- Tool length compensation

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

the canned cycle for drilling, the offset is applied after the time of

positioning to point R.

Limitation

- Axis switching

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

must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling

is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block

that does not perform drilling, it cannot be 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 for drilling, tool offsets are ignored.

- 41 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

Example

M4 S100 ;

Cause the spindle to start rotating.

G90 G99 G74 X300. Y-250. Z-150. R-120. F120. ;

Position, tapping hole 1, then return to point R.

Y-550. ;

Position, tapping hole 2, then return to point R.

Y-750. ;

Position, tapping hole 3, then return to point R.

X1000. ;

Position, tapping hole 4, then return to point R.

Y-550. ;

Position, tapping hole 5, then return to point R.

G98 Y-750. ;

Position, tapping hole 6, then return to the initial

level.

G80 G28 G91 X0 Y0 Z0

; Return to the reference position

M5 ;

Cause the spindle to stop rotating.

- 42 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.1.3

Fine Boring Cycle (G76)

The fine boring cycle bores a hole precisely. When the bottom of the

hole has been reached, the spindle stops, and the tool is moved away

from the machined surface of the workpiece and retracted.

Format

G76 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data

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

: The distance from the initial level to point R level

: Shift amount at the bottom of a hole

: Dwell time at the bottom of a hole

: Cutting feedrate

: Number of repeats (if required)

G76 (G98)

G76 (G99)

Spindle CW

Spindle orientation

Initial level

Tool

Spindle CW

Point R level

Point R

OSS

Point Z

Shift amount q

Explanation

- Operations

When the bottom of the hole has been reached, the spindle is stopped

at the fixed rotation position, and the tool is moved in the direction

opposite to the tool nose and retracted. This ensures that the

machined surface is not damaged and enables precise and efficient

boring to be performed.

- Spindle rotation

Before specifying G76, use a Auxiliary function (M code) to rotate the

spindle.

- Auxiliary function

When the G76 command and an M code are specified in the same

block, the M code is executed at the time of the first positioning

operation. When K is used to specify the number of repeats, the M

code is executed for the first hole only; for the second and subsequent

holes, the M code is not executed.

- 43 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-2/01

- Tool length compensation

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

the canned cycle for drilling, the offset is applied after the time of

positioning to point R.

Limitation

- Axis switching

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

must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any additional axes,

drilling is not performed.

- P/Q

Be sure to specify a positive value in Q. If Q is specified with a

negative value, the sign is ignored. Set the direction of shift in the

parameter (No.5148).

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.

CAUTION

Q (shift at the bottom of a hole) is a modal value

retained within canned cycles for drilling. It must

be specified carefully because it is also used as the

depth of cut for G73 and G83.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G76 in a

single block. Otherwise, G76 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S500 ;

Cause the spindle to start rotating.

G90 G99 G76 X300. Y-250.

Position, bore hole 1, then return to point R.

Z-150. R-120. Q5.

Orient at the bottom of the hole, then shift by 5

mm.

P1000 F120. ;

Stop at the bottom of the hole for 1 s.

Y-550. ;

Position, drill hole 2, then return to point R.

Y-750. ;

Position, drill hole 3, then return to point R.

X1000. ;

Position, drill hole 4, then return to point R.

Y-550. ;

Position, drill hole 5, then return to point R.

G98 Y-750. ;

Position, drill hole 6, then return to the initial level.

G80 G28 G91 X0 Y0 Z0 ;

Return to the reference position

M5 ;

Cause the spindle to stop rotating.

- 44 -

5.FUNCTIONS TO SIMPLIFY

B-64304EN-2/01

PROGRAMMING

5.1.4

Drilling Cycle, Spot Drilling (G81)

This cycle is used for normal drilling. Cutting feed is performed to

the bottom of the hole. The tool is then retracted from the bottom of

the hole in rapid traverse.

Format

G81 X_ Y_ Z_ R_ F_ K_ ;

X_ Y_ : Hole position data

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

: The distance from the initial level to point R level

: Cutting feedrate

: Number of repeats (if required)

G81 (G98)

G81 (G99)

Initial level

Point R

Point R level

Point Z

Explanation

- Operations

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

to point R.

Drilling is performed from point R to point Z.

The tool is then retracted in rapid traverse.

- Spindle rotation

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

the spindle.

- Auxiliary function

When the G81 command and an M code are specified in the same

block, the M code is executed at the time of the first positioning

operation. When K is used to specify the number of repeats, the M

code is performed for the first hole only; for the second and

subsequent holes, the M code is not executed.

- Tool length compensation

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

the canned cycle for drilling, the offset is applied after the time of

positioning to point R.

- 45 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 2