Content      ..      1      2      3      ..

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 2

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Example

C (Imaginary axis)

Path after tool

compensation

Programmed path

N204

C-axis

N205

Tool

X-axis

N201

N202

N200

Z-axis

N203

Fig. 3.1 (e) Involute interpolation in the polar coordinate interpolation mode

O0001 ;

:

:

N010 T0101 ;

:

:

N100 G90 G00 X15.0 C0 Z0 ;

Positioning to the start point

N200 G12.1 ;

Polar coordinate interpolation started

N201 G41 G00 X-1.0 ;

N202 G01 Z-2.0 F

;

N203 G02.2 X1.0 C9.425 I1.0 J0 R1.0 ; Involute interpolation during polar coordinate interpolation

N204 G01 Z0 ;

N205 G40 G00 X15.0 C0 ;

N206 G13.1 ;

Polar coordinate interpolation cancelled

N300 Z

;

N400 X

C

;

:

:

M30 ;

Limitation

-

Number of involute curve turns

Both the start point and end point must be within 100 turns from the point where the involute curve starts.

An involute curve can be specified to make one or more turns in a single block.

If the specified start point or end point is beyond 100 turns from the point where the involute curve starts,

alarm PS0242 is issued.

-

Unspecifiable functions

In involute interpolation mode, optional chamfering and corner R cannot be specified.

- 22 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

-

Mode that does not allow involute interpolation specification

Involute interpolation cannot be used in the following mode:

G07.1: Cylindrical interpolation

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

Z

G33IP_ F_ ;

F : Long axis direction lead

Workpiece

X

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 increment

Command value range of the lead

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)

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

- 23 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

NOTE

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;

3.3

CONTINUOUS THREADING

Threading blocks can be programmed successively to eliminate a discontinuity due to a discontinuous

movement in machining by adjacent blocks.

Explanation

Since the system is controlled in such a manner that the synchronism with the spindle does not deviate in

the joint between blocks wherever possible, it is possible to performed special threading operation in

which the lead and shape change midway.

G33

G33

G33

Fig. 3.3 (a) Continuous threading

Even when the same section is repeated for thread cutting while changing the depth of cut, this system

allows a correct machining without impairing the threads.

3.4

MULTIPLE THREADING

Using the Q address to specify an angle between the one-spindle-rotation signal and the start of threading

shifts the threading start angle, making it possible to produce multiple-thread screws with ease.

L

L : Lead

Fig. 3.4 (a) Multiple thread screws

- 24 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

Format

(Constant lead threading)

G33 IP _ F_ Q_ ;

IP : End point

F_ : Lead in longitudinal direction

G33 IP _ Q_ ;

Q_ : Threading start angle

Explanation

-

Available threading commands

G33: Constant lead threading

G34: Variable lead threading

G76.7: Multiple threading cycle

Limitation

-

Start angle

The start angle is not a continuous state (modal) value. It must be specified each time it is used. If a

value is not specified, 0 is assumed.

-

Start angle increment

The start angle (Q) increment is 0.001 degrees. Note that no decimal point can be specified.

Example:

For a shift angle of 180 degrees, specify Q180000.

Q180.000 cannot be specified, because it contains a decimal point.

-

Specifiable start angle range

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be specified. If a value

greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).

-

Multiple threading cycle (G76.7)

For the G76 multiple threading cycle command, always use the FS15 tape format.

Example

Program for producing double-threaded screws (with start angles of 0 and

180 degrees)

G00 X40.0 ;

G33 W-38.0 F4.0 Q0 ;

G00 X72.0 ;

W38.0 ;

X40.0 ;

G33 W-38.0 F4.0 Q180000 ;

G00 X72.0 ;

W38.0 ;

- 25 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

3.5

CIRCULAR THREAD CUTTING B (G2.1,G3.1)

Overview

Circular thread cutting B can perform circular interpolation on two axes and, at the same time, can

perform linear interpolation between the major axis of the two axes subject to circular interpolation,

which has a longer traveling distance, and up to two other, arbitrary axes. This circular thread cutting

function does not move the tool in synchronization with the rotation of the spindle (workpiece) using the

spindle motor, but controls the rotation of the workpiece using a servo motor (rotation axis) to perform

threading at equal pitches along cylindrical material, grooving, tool grinding, and other machining.

Application example

For example, the grooving shown in Fig. 3.5 (a) can be performed by executing circular interpolation on

the ZpXp plane in synchronization with linear interpolation on the Z-axis and the C-axis.

X axis

Z axis

C axis

Fig. 3.5 (a) Example of grooving

- 26 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

Format

Xp-Yp plane

G02.1

I

J

G17

X Y α β

F

;

G03.1

R

Zp-Xp plane

G02.1

Z X α β

K I

G18

F

;

G03.1

R

Yp-Zp plane

G02.1

Y Z α β

J K

G19

F

;

G03.1

R

G02.1: Clockwise circular thread cutting B command

G03.1: Counterclockwise circular thread cutting B command

X,Y,Z: Coordinates of the end point for circular interpolation

α,β:

Coordinates of the end point for linear interpolation

I,J,K:

Signed distance from the start point to the center of an arc

R:

Arc radius

F:

Feedrate in the major axis direction

α and β are arbitrary axes other than the circular interpolation axis. Up to two such axes

can be specified.

X, Y, Z, I, J, K, and R are the same as those for G02 and G03.

In the case of the ZpXp plane, the major axis being the Z-axis, the minor axis

being the X-axis, the arbitrary axis being the C-axis, and clockwise direction

G91 G18 G02.1 Z_ C_

I_ K_

F_

R_

X axis

Start point

End point (X,Z)

C axis

Z axis

R

I

K

Arc center

Fig. 3.5 (b)

Explanation

Circular thread cutting B can perform circular interpolation on two axes and, at the same time, can

perform linear interpolation between the major axis of the two axes subject to circular interpolation,

which has a longer traveling distance, and up to two other, arbitrary axes. This circular thread cutting

function does not move the tool in synchronization with the rotation of the spindle (workpiece) using the

spindle motor, but controls the rotation of the workpiece using a servo motor (rotation axis) to perform

threading at equal pitches along cylindrical material, grooving, tool grinding, and other machining.

- 27 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

-

Relationship between major axis and minor axis

The relationship between the major axis and minor axis is as shown in Fig. 3.5 (c).

ΔX

Start

End

point

If |ΔX| > |ΔY|,

point

ΔY

the major axis is the X-axis, and the

minor axis is the Y-axis.

Y

If |ΔX| < |ΔY|,

45°

45°

the major axis is the Y-axis, and the

Center

minor axis is the X-axis.

X

Fig. 3.5 (c)

When diameter programming is used, the relationship between the major axis and minor axis is judged

with the radius value.

-

Permissible arc range

If the arc goes beyond the range shown in Fig. 3.5 (d) or Fig. 3.5 (e), alarm PS2070 is issued.

90°

Minor

Range in which

45° to 135°

axis

interpolation is

225° to 315°

enabled

45°

45°

0°

Major

45°

45°

Rotation

axis

axis

Fig. 3.5 (d)

90°

Major

axis

45°

45°

0°

Minor

Rotation

45°

45°

axis

axis

315° to 45°

Range in which

135° to 225°

interpolation is enabled

Fig. 3.5 (e)

-

Feedrate

If the specified feedrate for the major axis is F, the feedrate for the minor axis Fs and feedrate for the α

axis Fα are expressed as follows.

Length of α axis

Fα = F ×

(The maximum value is the maximum cutting feedrate for each axis.)

Length of major axis

Fs = F × TAN θ

θ: Angle of a tangent to the major axis

- 28 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

End

Fs

θ

point

Minor

F

axis

Start point

Major

axis

Center

Fig. 3.5 (f)

-

Tool radius compensation

Tool radius compensation applies only to two axes of the plane on which circular interpolation is

performed.

Limitation

-

Tool offset and tool length compensation

In a block in which circular thread cutting B is specified, tool offset or tool length compensation cannot

be specified.

-

I,J,K and the R command

Either I,J,K or the R command cannot be omitted.

-

Unavailable functions

Circular thread cutting B cannot be used together with the following functions:

•

3-dimensional cutter compensation

•

Tool center point control

- 29 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

3.6

GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION

(G12.4, G13.4)

Overview

Groove cutting with a width greater than the tool diameter can be performed by causing the tool to make

continuous circle motion independently of axis movement by the groove cutting path program and

superposing the continuous circle motion on the axis movement by the groove cutting path program.

Continuous

circle motion

Groove cutting path

specification route

Fig. 3.6 (a)

Format

G12.4

P1Ii Kk Qq Ff;

(Mode on)

G13.4

:

:

(Groove cutting path program)

:

G12.4

P0;

(Mode cancel)

G13.4

G12.4 : Clockwise continuous circle motion

G13.4 : Counterclockwise continuous circle motion

i

: Groove width

k

: Tool diameter

q

: Travel distance in the groove cutting direction per continuous circle motion (pitch)

f

: Feedrate (speed of the center of a tool that performs continuous circle motion)

- 30 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

Groove cutting path program

i

(Groove width)

k (Tool diameter)

q (pitch)

Fig. 3.6 (b)

NOTE

1 In the G12.4/G13.4 blocks, addresses other than the commands mentioned

above cannot be used.

2 If bit 4 (GCC) of parameter No. 3452 is 0, continuous circle motion stops due to

the stoppage of axis movement by the groove cutting path program, but because

axis movement by the groove cutting path program is independent of continuous

circle motion, the stoppage will not exactly be at the position of continuous circle

motion converted from the groove cutting path program and the pitch.

Explanation

-

Mode on

The continuous circle motion-based groove cutting mode sets continuous circle motion-based groove

cutting mode to the on state. The continuous circle motion-based groove cutting enable signal must be

"1".

If the mode on command is specified with the continuous circle motion-based groove cutting enable

signal being "0", alarm PS0010 is issued.

No axis movement is performed with the continuous circle motion-based groove cutting mode on

command.

-

Mode cancel

The continuous circle motion-based groove cutting mode cancel command causes the tool to move with

cutting feed (continuous circle motion speed) from the present position on the continuous circle to the

end-specified position (groove center) of the groove cutting path program. After the end of movement, the

command sets continuous circle motion-based groove cutting mode to the cancel state.

-

Startup

In the first move command block of the groove cutting path program, the tool moves to a point on the

continuous circle with cutting feed (continuous circle motion speed). After the end of the movement to a

point on the continuous circle, continuous circle motion is started in synchronization with the move

command of the groove cutting path program.

Depending on the first move command block of the groove cutting path program, the direction of startup

varies.

- 31 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

• In the case of an axis command perpendicular to a plane or if there is no movement along an axis

used to form the currently selected plane

Assuming that R = (I-K)/2, the following holds true: (X,Y) = (-R,0)

Startup

R

Groove cutting

path command

Ｚ

Y

X

Fig. 3.6 (c)

• If there is movement along an axis used to form the selected plane

Direction opposite to the direction of movement projected onto the currently selected plane

Groove cutting path command

End

Startup

point

Y

R

X

Start point

Fig. 3.6 (d)

-

Increments systems for horizontal width, tool diameter, and pitch

The increment systems for I (horizontal width), K (tool diameter), and Q (pitch) follow the incremental

system of the reference axis (parameter No. 1031).

-

Feedrate

For the feedrate F, specify the central speed of the tool that performs continuous circle motion.

The speed on the groove cutting path is:

Speed on the groove cutting path

= F × Q / π (I-K)

-

Pitch

If the pitch is large, there may be portions left uncut. The tool diameter must be greater than the pitch.

-

Groove cutting path program

The groove cutting path program specifies the path of the center of continuous circle motion.

(1) Effective commands

The groove cutting path program can execute only the G01, G02, G03, G04, G90, G91, and

auxiliary functions. The G00 command causes alarm PS5256. By setting bit 0 (GG0) of parameter

No. 3452, however, the G00 command can be moved as G01 movement. The modal code changes

from G00 to G01.

(2) Specifying a controlled axis

The groove cutting path program can specify the control axes below.

•

Commands for the axes forming a plane

•

Commands for axes perpendicular to a plane (independent command for the Z-axis)

•

Commands for linear axes other than the axes forming a plane

•

Commands for rotation axes

- 32 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

(3) Specification of a pitch in a move command block

In addition to the specification of a pitch with the continuous circle motion-based groove cutting

mode on command, a pitch can be specified in each move command block.

The pitch specification is modal; the pitch last specified is effective from the time the mode is

entered with G12.4P1/G13.4P1 until the mode is exited.

(4) Command example

(Example 1) Example of a command for an axis perpendicular to a plane

(independent command for the Z-axis)

:

G12.4 P1 Ii Kk Ff ;

G01 Z--- Q--- ;

Specify the pitch for the Z-axis (pitch of this block).

X--- Y--- Q--- ;

Specify the pitch for the X- and Y-axes (pitch of the

subsequent blocks)

:

For a command for the Z-axis only, the pitch is regarded as the travel distance in

the Z-axis direction.

(Example 2) If a move command for other than a plane is included

:

G12.4P1 Ii Kk Ff ;

G01 X--- Y--- Z--- Q---

;

This is a pitch on a slanted path.

:

The pitch is the travel distance in the synthetic direction of the X-, Y-, and Z-axes.

(Example 3) Pitch switching

:

G12.4P1 Ii Kk Ff ;

G01 X--- Y--- Q--- ;

X--- Y--- Q--- ;

Specify Q in the block in which the pitch is to be changed.

:

The pitch is the travel distance in the synthetic direction of the specified axes.

(Example 4) Command containing a rotation axis

:

G12.4P1 Ii Kk Ff ;

G01 Ａ--- Q--- ;

X--- Y--- ;

Specify Q in the block in which the pitch is to be changed.

:

The increment system for Q follows that of the reference axis. Thus, if the

increment system for the reference axis is IS-B, the pitch Q100 will be 0.1°.

So that a cut along the Z-axis will start after the stabilization of the radius of continuous circle motion, the

continuous circle motion-based groove cutting mode on command must be specified in the air, apart from

the cut position by at least the pitch per rotation. Cutting with a constant groove width is possible by

letting the tool escape in the Z-axis direction at the end of cutting while keeping continuous circle motion

and then after the tool comes out into the air, executing the continuous circle motion-based groove cutting

mode cancel command to stop continuous circle motion.

- 33 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

NOTE

The radius of continuous circle motion is smaller than that specified at the start

of continuous circle motion, and is larger when continuous circle motion comes

to a deceleration stop. In the steady state, the radius is smaller than that

specified. This is an error that occurs due to acceleration/deceleration after

information and the delay of the servo system.

Error that occurs due to

acceleration/deceleration after

interpolation and the delay of the servo

system

Specified

Actual path

-

Mode in progress signal

This signal notifies the PMC that continuous circle motion-based groove cutting mode is in progress.

The signal is set to "1" if continuous circle motion-based groove cutting mode is turned on.

The signal is set to "0" if continuous circle motion-based groove cutting mode is canceled.

-

Clamping the feedrate with the acceleration of continuous circle motion

Using the I and K commands in G12.4/13.4 and the acceleration clamp value for continuous circle motion

(parameter No. 3490), the feedrate command F for continuous circle motion can be clamped.

Clamp feedrate F = SQR (parameter No.3490 × (I-K) / 2)× 60

Example If parameter No. 3490 = 100

If G13.4 P1 I10.0 K5.0 Q1.0 F1000 ;, clamp feedrate = 948. Thus, execution with

an F value of 948

If G13.4 P1 I10.0 K8.0 Q1.0 F1000 ;, clamp feedrate = 600. Thus, execution with

an F value of 600

If G13.4 P1 I10.0 K9.0 Q1.0 F1000 ;, clamp feedrate = 424. Thus, execution with

an F value of 424

A continuous circle motion feedrate override is applied to the clamped feedrate.

-

Acceleration deceleration after interpolation

In continuous circle motion-based groove cutting mode, acceleration/deceleration after interpolation is

enabled.

-

Selecting stoppage conditions

(1) Stoppage of continuous circle motion due to a feed hold, single block, etc.

It can be selected whether to continue or stop continuous circle motion when a specified operation is

stopped due to one of the various stoppage conditions such as a feed hold and a single block, using a

parameter:

Bit 4 (GCC) of parameter No. 3452 = 0 : Stops continuous circle motion.

Bit 4 (GCC) of parameter No. 3452 = 1 : Continues continuous circle motion.

(2) Stoppage condition/mode switching

The conditions for groove cutting path operation, continuous circle motion stoppage/continuation,

and switching to operation mode in connection with stoppage conditions are as given in Table 3.6

(a).

- 34 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

Table 3.6 (a)

Continuous circle motion

Groove cutting

stoppage/continuation

Switching to operation

Stoppage condition

path operation

Stoppage

Continuation

mode

(GCC = 0)

(GCC = 1)

Feed hold

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

Single block

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

Switching to manual

Deceleration stop

Deceleration stop

Continuation

To be performed after the

mode

stoppage of path operation

Switching between

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

auto modes

of path operation

MDI operation

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

Pitch override of 0%

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

M/S/T code FIN

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

awaiting

of path operation

Programming error

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

Overheat alarm

Deceleration stop

Deceleration stop

Continuation

Possible after the stoppage

of path operation

BG edit alarm

Continuation

Continuation

Continuation

Automatic operation does

not stop.

Mode end

Deceleration stop

Withdrawal by the

Withdrawal by the

Follows other stoppage

radius/

radius/

conditions.

deceleration stop

deceleration stop

Reset

Deceleration stop

Deceleration stop

Deceleration stop

Possible after the end of all

operations

Machine lock

*1

Deceleration stop

Deceleration stop

Deceleration stop

―――

Servo off

*1

Deceleration stop

Deceleration stop

Deceleration stop

―――

Interlock

*2

Deceleration stop

Deceleration stop

Deceleration stop

―――

OT alarm

Deceleration stop

Deceleration stop

Deceleration stop

Possible after the end of all

operations

DS alarm

Deceleration stop

Deceleration stop

Deceleration stop

Possible after the end of all

operations

Emergency stop

Immediate stop

Immediate stop

Immediate stop

Possible after an

emergency stop is

canceled

PC-related alarm

Immediate stop

Immediate stop

Immediate stop

Possible after an alarm is

canceled

Servo alarm

Immediate stop

Immediate stop

Immediate stop

Possible after an alarm is

canceled

Spindle alarm

Immediate stop

Immediate stop

Immediate stop

Possible after an alarm is

canceled

System alarm

Immediate stop

Immediate stop

Immediate stop

The power must be turned

off and then back on.

*1: Stoppage occurs only on the axis on which the function is enabled.

*2: Stoppage occurs on all axes if the function is enabled on at least one axis.

• If bit 4 (GCC) of parameter No. 3452 is 0, continuous circle motion stops due to the stoppage of axis

movement by the groove cutting path program, but because axis movement by the groove cutting

path program is independent of continuous circle motion, the stoppage will not exactly be at the

position of continuous circle motion converted from the groove cutting path program and the pitch.

- 35 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

•

After the mode is switched to manual mode, the axes on which manual movement is possible do not

include the axes on which to perform continuous circle motion.

•

If continuous circle motion is to continue (bit 4 (GCC) of parameter No. 3452 = 1), there will be no

fluctuations in radius because continuous circle motion continues.

•

Movement to the continuous circle motion start position and movement to the groove cutting path

program end position after the end of continuous circle motion will stop under the stoppage

conditions below.

Reset

Deceleration stop

Machine lock

Deceleration stop

Servo off

Deceleration stop

Interlock

Deceleration stop

OT alarm

Deceleration stop

DS alarm

Deceleration stop

Emergency stop

Immediate stop

PC-related alarm

Immediate stop

Servo alarm

Immediate stop

Spindle alarm

Immediate stop

System alarm

Immediate stop

-

Feedrate specification and pitch override

(1)

Feedrate specification

For the feedrate during cutting, specify the feedrate for continuous circle motion.

This feedrate is displayed as a specified feedrate.

(2)

Continuous circle motion feedrate override

The feedrate override signals

(*FV0 to *FV7) are not effective to the specified feedrate for

continuous circle motion. Use the continuous circle motion feedrate override signals (*CGROV7 to

*CBROV0). If the continuous circle motion feedrate override is at 0%, continuous circle motion can

be stopped independently of the movement on the groove cutting path.

(3)

Feedrate override

The feedrate on the groove cutting path is determined with the pitch command. The feedrate

override signals (*FV0 to *FV7) are effective to the feedrate on the groove cutting path. This makes

it possible to change the feedrate for continuous circle motion independently of the feedrate on the

groove cutting path.

Also, the override cancel signal (OVC) and the second feedrate override signal (optional function)

are effective to the feedrate on the groove cutting path.

(4)

Dry run

The feedrate during a dry run is as given in Table 3.6 (b).

A dry run is not effective to the feedrate on the groove cutting path.

Table 3.6 (b)

Feedrate

Override

Feedrate on the groove

Feedrate F for continuous circle motion ×

Feedrate override

cutting path

pitch / 2πR

Manual rapid traverse selection signal (RT)

Feedrate for continuous

Dry run rate

0

1

circle motion

(Parameter No.1410)

JV

JVmax

JV :

Manual feedrate override

Jvmax :

Maximum manual feedrate override

- 36 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Example

If the following program is executed, the center of the tool moves as shown in

the figure below.

(This program is merely a sample. The Q and F commands must be determined

according to the cutting conditions.)

O0002 ;

N01 G90 G0 X0 Y0 Z0 ;

N02 G91 G00 X20.0 Y20.0 ;

N03 G01 Z-25.0 F5000 ;

N04 G13.4 P1 I20.0 K10.0 Q5.0 F3000 ;

N05 Y40.0 ;

N06 X40.0 Y20.0 ;

N07 G02 X40.0 Y-40.0 R40.0 ;

N08 X-20.0 Y-20.0 R20.0 ;

N09 G01 X-60. ;

N10 G13.4 P0 ;

N11 G00 Z25.0 ;

N12 X-20.0 Y-20.0 M02 ;

%

- 40 -

4.COORDINATE VALUE AND

B-64484EN-2/02

PROGRAMMING

DIMENSION

4 COORDINATE VALUE AND DIMENSION

Chapter 4, "COORDINATE VALUE AND DIMENSION", consists of the following sections:

4.1 POLAR COORDINATE COMMAND (G15, G16)

41

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

-

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

Command position

Radius

Radius

Angle

Actual position

Angle

Actual position

When the angle is specified with an

When the angle is specified with an

absolute command

incremental command

- 41 -

4. COORDINATE VALUE AND

DIMENSION

PROGRAMMING

B-64484EN-2/02

-

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

Command position

Angle

Radius Angle

Radius

Actual position

Actual position

When the angle is specified with an

When the angle is specified with an

absolute command

incremental command

Example

Bolt hole circle

Y

- The origin of the workpiece coordinate

system is set as the origin of the polar

coordinate system.

- The XY plane is selected.

150°

30°

X

270°

100mm

-

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.

- 42 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

5 FUNCTIONS TO SIMPLIFY PROGRAMMING

Chapter 5, "FUNCTIONS TO SIMPLIFY PROGRAMMING", consists of the following sections:

5.1 CANNED CYCLE FOR DRILLING

44

5.2 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLES

75

5.3 RIGID TAPPING

89

5.4 OPTIONAL CHAMFERING AND CORNER R

103

5.5 INDEX TABLE INDEXING FUNCTION

106

5.6 IN-FEED CONTROL (FOR GRINDING MACHINE)

108

5.7 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

110

5.8 MULTIPLE REPETITIVE CYCLE (G70.7, G71.7, G72.7, G73.7, G74.7, G75.7,G76.7)

124

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)

G73

Intermittent feed

-

Rapid traverse

High-speed peck drilling cycle

G74

Feed

Dwell → Spindle CW

Feed

Left-hand tapping cycle

G76

Feed

Spindle orientation

Rapid traverse

Fine boring cycle

G80

-

-

-

Cancel

Drilling cycle, spot drilling

G81

Feed

-

Rapid traverse

cycle

Drilling cycle, counter boring

G82

Feed

Dwell

Rapid traverse

cycle

G83

Intermittent feed

-

Rapid traverse

Peck drilling cycle

G84

Feed

Dwell → Spindle CCW

Feed

Tapping cycle

G85

Feed

-

Feed

Boring cycle

G86

Feed

Spindle stop

Rapid traverse

Boring cycle

G87

Feed

Spindle CW

Rapid traverse

Back boring cycle

G88

Feed

Dwell → Spindle stop

Manual

Boring cycle

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

- 44 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

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

Zp

G18

Zp-Xp plane

Yp

G19

Yp-Zp plane

Xp

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

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.

- 45 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

CAUTION

Switch the drilling axis after canceling a canned cycle for drilling.

NOTE

A bit 0 (FXY) of parameter No. 5101 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 Fig. 5.1 (b):

G90 (Absolute programming)

G91 (Incremental programming)

R

R

Point R

Point R

Z = 0

Z

Point Z

Z

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.

-

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 operations performed when G98 and G99 are

specified are shown in Fig. 5.1 (c). 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

- 46 -

5.FUNCTIONS TO SIMPLIFY

B-64484EN-2/02

PROGRAMMING

PROGRAMMING

-

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 Fig. 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.

-

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)

-

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

OSS

Oriented spindle stop (The spindle stops at a fixed rotation position)

Shift (rapid traverse G00)

P

Dwell

- 47 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

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

Z_

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

R_

: The distance from the initial level to point R level

Q_

: Depth of cut for each cutting feed

F_

: Cutting feedrate

K_

: Number of repeats (if required)

G73 (G98)

G73 (G99)

Initial level

Point R

Point R

Point R level

q

q

d

d

q

q

d

d

q

q

Point Z

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).

-

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.

- 48 -

5. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-64484EN-2/02

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_ F_ K_ ;

X_ Y_ : Hole position data

Z_

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

R_

: The distance from the initial level to point R level

P_

: Dwell time

F_

: Cutting feedrate

K_

: Number of repeats (if required)

G74 (G98)

G74 (G99)

Initial level

Spindle

Spindle

CCW

CCW

P

Point R

P

Point R

Point R level

Point Z

Point Z

P

P

Spindle CW

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.

-

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.

-

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.

- 50 -

Content      ..      1      2      3      ..