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

1.GENERAL

PROGRAMMING

B-64304EN-1/01

1.1

OFFSET

Explanation

- Tool offset

Usually, several tools are used for machining one workpiece. The

tools have different tool length. It is very troublesome to change the

program in accordance with the tools.

Therefore, the length of each tool used should be measured in advance.

By setting the difference between the length of the standard tool and

the length of each tool in the CNC (see “Setting and Displaying Data”

in the User’s Manual (Common to Lathe System/Machining Center

System)), machining can be performed without altering the program

even when the tool is changed. This function is called tool offset.

Standard Rough

Finishing Grooving Threading

tool

cutting

tool

Workpiece

Fig. 1.1 (a) Tool offset

- 14 -

2.PREPARATORY FUNCTION

B-64304EN-1/01

PROGRAMMING

(G FUNCTION)

PREPARATORY FUNCTION

(G FUNCTION)

A number following address G determines the meaning of the

command for the concerned block.

G codes are divided into the following two types.

Type

Meaning

The G code is effective only in the block in which it

One-shot G code

is specified.

The G code is effective until another G code of the

Modal G code

same group is specified.

(Example)

G01 and G00 are modal G codes in group 01.

G01 X_ ;

Z_ ;

G01 is effective in this range.

X_ ;

G00 Z_ ; G00 is effective in this range.

X_ ;

G01 X_ ;

There are three G code systems in the lathe system : A,B, and C

(Table 2(a)). Select a G code system using bits 6 (GSB) and 7 (GSC)

parameter No. 3401. Generally, User’s Manual describes the use of G

code system A, except when the described item can use only G code

system B or C. In such cases, the use of G code system B or C is

described.

- 15 -

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64304EN-1/01

Explanation

When the clear state (parameter CLR (No. 3402#6)) is set at

power-up or reset, the modal G codes are placed in the states

described below.

(1) The modal G codes are placed in the states marked with

as indicated in Table 2.

(2) G20 and G21 remain unchanged when the clear state is set

at power-up or reset.

(3) Which status G22 or G23 at power on is set by parameter

G23

(No.

3402#7). However, G22 and G23 remain

unchanged when the clear state is set at reset.

(4) The user can select G00 or G01 by setting parameter G01

(No. 3402#0).

(5) The user can select G90 or G91 by setting parameter G91

(No. 3402#3).

When G code system B or C is used in the lathe system,

setting parameter G91 (No. 3402#3) determines which code,

either G90 or G91, is effective.

G codes in group 00 other than G10 and G11 are one-shot G

codes.

When a G code not listed in the G code list is specified, or a G

code that has no corresponding option is specified, alarm PS0010

occurs.

Multiple G codes can be specified in the same block if each G

code belongs to a different group. If multiple G codes that belong

to the same group are specified in the same block, only the last G

code specified is valid.

If a G code belonging to group 01 is specified in a for drilling,

the canned cycle for drilling is cancelled. This means that the

same state set by specifying G80 is set. Note that the G codes in

group 01 are not affected by a G code specifying a canned cycle.

When G code system A is used, absolute or incremental

programming is specified not by a G code (G90/G91) but by an

address word (X/U, Z/W, C/H, Y/V). Only the initial level is

provided at the return point of the canned cycle for drilling..

G codes are indicated by group.

- 16 -

2.PREPARATORY FUNCTION

B-64304EN-1/01

PROGRAMMING

(G FUNCTION)

Table 2 G code list

G code system

Group

Function

G00

Positioning (Rapid traverse)

G01

Linear interpolation (Cutting feed)

G02

Circular interpolation CW or helical interpolation CW

G03

Circular interpolation CCW or helical interpolation CCW

G04

Dwell

G05.4

HRV3 on/off

G07.1

Cylindrical interpolation

(G107)

G08

Advanced preview control

G09

Exact stop

G10

Programmable data input

G11

Programmable data input mode cancel

G12.1

Polar coordinate interpolation mode

(G112)

G13.1

Polar coordinate interpolation cancel mode

(G113)

G17

XpYp plane selection

G18

ZpXp plane selection

G19

YpZp plane selection

G20

G70

Input in inch

G21

G71

Input in mm

G22

Stored stroke check function on

G23

Stored stroke check function off

G25

Spindle speed fluctuation detection off

G26

Spindle speed fluctuation detection on

G27

Reference position return check

G28

Return to reference position

G30

2nd, 3rd and 4th reference position return

G31

Skip function

G32

G33

Threading

G34

Variable lead threading

G36

Automatic tool offset (X axis)

G37

Automatic tool offset (Z axis)

G39

Tool nose radius compensation: corner rounding interpolation

G40

Tool nose radius compensation : cancel

G41

Tool nose radius compensation : left

G42

Tool nose radius compensation : right

G50

G92

Coordinate system setting or max spindle speed clamp

G50.3

G92.1

Workpiece coordinate system preset

G50.2

Polygon turning cancel

(G250)

G51.2

Polygon turning

(G251)

- 17 -

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64304EN-1/01

Table 2 G code list

G code system

Group

Function

G50.4

Cancel synchronous control

G50.5

Cancel composite control

G50.6

Cancel superimposed control

G51.4

Start synchronous control

G51.5

Start composite control

G51.6

Start superimposed control

G52

Local coordinate system setting

G53

Machine coordinate system setting

G54

Workpiece coordinate system 1 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

G61

Exact stop mode

G63

Tapping mode

G64

Cutting mode

G65

Macro call

G66

Macro modal call

G67

Macro modal call cancel

G68

Mirror image on for double turret or balance cutting mode

G69

Mirror image off for double turret or balance cutting mode cancel

G70

G72

Finishing cycle

G71

G73

Stock removal in turning

G72

G74

Stock removal in facing

G73

G75

Pattern repeating cycle

G74

G76

End face peck drilling cycle

G75

G77

Outer diameter/internal diameter drilling cycle

G76

G78

Multiple-thread cutting cycle

G71

G72

Traverse grinding cycle (for grinding machine)

G72

G73

Traverse direct sizing/grinding cycle (for grinding machine)

G73

G74

Oscillation grinding cycle (for grinding machine)

G74

G75

Oscillation direct sizing/grinding cycle (for grinding machine)

Canned cycle cancel for drilling

G80

Electronic gear box : synchronization cancellation

Spot drilling (FS10/11-T format)

G81

Electronic gear box : synchronization start

G82

Counter boring (FS10/11-T format)

G83

Cycle for face drilling

G83.1

High-speed peck drilling cycle (FS10/11-T format)

G84

Cycle for face tapping

G84.2

Rigid tapping cycle (FS10/11-T format)

G85

Cycle for face boring

G87

Cycle for side drilling

G88

Cycle for side tapping

G89

Cycle for side boring

G90

G77

G20

Outer diameter/internal diameter cutting cycle

G92

G78

G21

Threading cycle

G94

G79

G24

End face turning cycle

- 18 -

2.PREPARATORY FUNCTION

B-64304EN-1/01

PROGRAMMING

(G FUNCTION)

Table 2 G code list

G code system

Group

Function

G91.1

Maximum specified incremental amount check

G96

Constant surface speed control

G97

Constant surface speed control cancel

G96.1

Spindle indexing execution (waiting for completion)

G96.2

Spindle indexing execution (not waiting for completion)

G96.3

Spindle indexing completion check

G96.4

SV speed control mode ON

G98

G94

Feed per minute

G99

G95

Feed per revolution

G90

Absolute programming

G91

Incremental programming

G98

Canned cycle : return to initial level

G99

Canned cycle : return to R point level

- 19 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

3.1

POLAR COORDINATE INTERPOLATION (G12.1, G13.1)

Overview

Polar coordinate interpolation is a function that exercises contour

control in converting a command programmed in a Cartesian

coordinate system to the movement of a linear axis (movement of a

tool) and the movement of a rotary axis (rotation of a workpiece).

This function is useful in cutting a front surface and grinding a cam

shaft for turning.

Format

G12.1; Starts polar coordinate interpolation mode

(enables polar coordinate interpolation).

Specify linear or circular interpolation using

coordinates in a Cartesian coordinate system

consisting of a linear axis and rotary axis

(hypothetical axis).

G13.1; Polar coordinate interpolation mode is

cancelled (for not performing polar coordinate

interpolation).

Specify G12.1 and G13.1 in Separate Blocks.

G112 and G113 can be used in place of G12.1 and G13.1,

respectively.

Explanation

- Polar coordinate interpolation mode (G12.1)

The axes of polar coordinate interpolation (linear axis and rotary axis)

should be specified in advance, with corresponding parameters.

Specifying G12.1 places the system in the polar coordinate

interpolation mode, and selects a plane (called the polar coordinate

interpolation plane) formed by one linear axis and a hypothetical axis

intersecting the linear axis at right angles. The linear axis is called the

first axis of the plane, and the hypothetical axis is called the second

axis of the plane. Polar coordinate interpolation is performed in this

plane.

In the polar coordinate interpolation mode, both linear interpolation

and circular interpolation can be specified by absolute or incremental

programming.

Tool nose radius compensation can also be performed. The polar

coordinate interpolation is performed for a path obtained after tool

nose radius compensation.

The tangential velocity in the polar coordinate interpolation plane

(Cartesian coordinate system) is specified as the feedrate, using F.

- Polar coordinate interpolation cancel mode (G13.1)

Specifying G13.1 cancels the polar coordinate interpolation mode.

- 21 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- Polar coordinate interpolation plane

G12.1 starts the polar coordinate interpolation mode and selects a

polar coordinate interpolation plane (Fig. 3.1 (a)). Polar coordinate

interpolation is performed on this plane.

Rotary axis (hypothetical axis)

(unit: mm or inch)

Linear axis

(unit: mm or inch)

Origin of the local coordinate system (G52 command)

(Or origin of the workpiece coordinate system)

Fig. 3.1 (a) Polar coordinate interpolation plane

When the power is turned on or the system is reset, polar coordinate

interpolation is canceled (G13.1).

The linear and rotation axes for polar coordinate interpolation must be

set in parameters Nos. 5460 and 5461 beforehand.

CAUTION

The plane used before G12.1 is specified (plane

selected by G17, G18, or G19) is canceled. It is

restored when G13.1 (canceling polar coordinate

interpolation) is specified.

When the system is reset, polar coordinate

interpolation is canceled and the plane specified by

G17, G18, or G19 is used.

- Distance moved and feedrate for polar coordinate interpolation

•

The unit for coordinates on the hypothetical axis is the same as

the unit for the linear axis (mm/inch).

In the polar coordinate interpolation mode, program commands

are specified with Cartesian coordinates on the polar coordinate

interpolation plane. The axis address for the rotary axis is used as

the axis address for the second axis (hypothetical axis) in the

plane. Whether a diameter or radius is specified for the first axis

in the plane is the same as for the rotary axis regardless of the

specification for the first axis in the plane.

The hypothetical axis is at coordinate 0 immediately after G12.1

is specified. Polar interpolation is started assuming the rotation

angle of 0 for the position of the tool when G12.1 is specified.

- 22 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

Example)

When a value on the X-axis

(linear axis) is input in

millimeters

G12.1;

G01 X10. F1000. ; ..A 10-mm movement is made on the

Cartesian coordinate system.

C20. ;

A 20-mm movement is made on the

Cartesian coordinate system.

G13.1;

When a value on the X-axis (linear axis) is input in inches

G12.1;

G01 X10. F1000. ;

A 10-inch movement is made on the

Cartesian coordinate system.

C20. ;

A 20-inch movement is made on the

Cartesian coordinate system.

G13.1;

•

The unit for the feedrate is mm/min or inch/min.

Specify the feedrate as a speed

(relative speed between the

workpiece and tool) tangential to the polar coordinate

interpolation plane (Cartesian coordinate system) using F.

- G codes which can be specified in the polar coordinate interpolation mode

G01

Linear interpolation

G02, G03

Circular interpolation

G04

Dwell

G40, G41, G42

Tool nose radius compensation

(Polar coordinate interpolation is applied to the

path after tool nose radius compensation.)

G65, G66, G67

Custom macro command

G90, G91

Absolute programming, incremental programming

(For G code system B or C)

G98, G99

Feed per minute, feed per revolution

- Circular interpolation in the polar coordinate plane

The addresses for specifying the radius of an arc for circular

interpolation (G02 or G03) in the polar coordinate interpolation plane

depend on the first axis in the plane (linear axis).

•

I and J in the Xp-Yp plane when the linear axis is the X-axis or

an axis parallel to the X-axis.

•

J and K in the Yp-Zp plane when the linear axis is the Y-axis or

an axis parallel to the Y-axis.

•

K and I in the Zp-Xp plane when the linear axis is the Z-axis or

an axis parallel to the Z-axis.

The radius of an arc can be specified also with an R command.

NOTE

The parallel axes U, V, and W can be used in the G

code system B or C.

- 23 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- Movement along axes not in the polar coordinate interpolation plane in the polar

coordinate interpolation mode

The tool moves along such axes normally, independent of polar

coordinate interpolation.

- Current position display in the polar coordinate interpolation mode

Actual coordinates are displayed. However, the remaining distance to

move in a block is displayed based on the coordinates in the polar

coordinate interpolation plane (Cartesian coordinates).

- Coordinate system for the polar coordinate interpolation

Basically, before G12.1 is specified, a local coordinate system (or

workpiece coordinate system) where the center of the rotary axis is the

origin of the coordinate system must be set.

In the G12.1 mode, the coordinate system must not be changed (G50,

G52, G53, relative coordinate reset, G54 through G59, etc.).

- Compensation in the direction of the hypothetical axis in polar coordinate

interpolation

If the first axis of the plane has an error from the center of the rotary

axis in the hypothetical axis direction, in other words, if the rotary

axis center is not on the X-axis, the hypothetical axis direction

compensation function in the polar coordinate interpolation mode is

used. With the function, the error is considered in polar coordinate

interpolation. The amount of error is specified in parameter No. 5464.

Hypothetical axis (C-axis)

Rotary axis

(X, C)

X-axis

Error in the direction of

hypothetical axis (P)

Center of rotary axis

(X, C)

Point in the X-C plane (The center of the rotary axis is

considered to be the origin of the X-C plane.)

X coordinate in the X-C plane

Hypothetical axis coordinate in the X-C plane

Error in the direction of the hypothetical axis

(specified in parameter No. 5464)

- 24 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- Shifting the coordinate system in polar coordinate interpolation

In the polar coordinate interpolation mode, the workpiece coordinate

system can be shifted. The current position display function shows the

position viewed from the workpiece coordinate system before the shift.

The function to shift the coordinate system is enabled when bit 2

(PLS) of parameter No. 5450 is specified accordingly.

The shift can be specified in the polar coordinate interpolation mode,

by specifying the position of the center of the rotary axis C (A, B) in

the X-C (Y-A, Z-B) interpolation plane with reference to the origin of

the workpiece coordinate system, in the following format.

G12.1 X_ C_ ;

(Polar coordinate interpolation for the X-axis and C-axis)

G12.1 Y_ A_ ;

(Polar coordinate interpolation for the Y-axis and A-axis)

G12.1 Z_ B_ ;

(Polar coordinate interpolation for the Z-axis and B-axis)

G12.1 Xx Cc ;

Center of C-axis

Origin of workpiece

coordinate system

Limitation

- Changing the coordinate system during polar coordinate interpolation

In the G12.1 mode, the coordinate system must not be changed (G92,

G52, G53, relative coordinate reset, G54 through G59, etc.).

- Tool nose radius compensation

The polar coordinate interpolation mode (G12.1 or G13.1) cannot be

started or terminated in the tool nose radius compensation mode (G41

or G42). G12.1 or G13.1 must be specified in the tool nose radius

compensation canceled mode (G40).

- Tool offset command

A tool offset must be specified before the G12.1 mode is set. No offset

can be changed in the G12.1 mode.

- Program restart

For a block in the G12.1 mode, the program cannot be restarted.

- 25 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- Cutting feedrate for the rotary axis

Polar coordinate interpolation converts the tool movement for a figure

programmed in a Cartesian coordinate system to the tool movement in

the rotary axis (C-axis) and the linear axis (X-axis). When the tool

comes close to the center of the workpiece, the C-axis velocity

component increases. If the maximum cutting feedrate for the C-axis

(parameter No. 1430) is exceeded, the automatic feedrate override

function and automatic speed clamp function are enabled.

If the maximum cutting feedrate for the X-axis is exceeded, the

automatic feedrate override function and automatic speed clamp

function are enabled.

WARNING

Consider lines L1, L2, and L3. ∆X is the distance the tool moves per time unit at the

feedrate specified with address F in the Cartesian coordinate system. As the tool

moves from L1 to L2 to L3, the angle at which the tool moves per time unit

corresponding to ∆X in the Cartesian coordinate system increases from θ1 to θ2 to

θ3. In other words, the C-axis component of the feedrate becomes larger as the

tool moves closer to the center of the workpiece. The C component of the feedrate

may exceed the maximum cutting feedrate for the C-axis because the tool

movement in the Cartesian coordinate system has been converted to the tool

movement for the C-axis and the X-axis.

∆X

θ1

θ2

θ3

L: Distance (in mm) between the tool center and workpiece center when the tool

center is the nearest to the workpiece center

R: Maximum cutting feedrate (deg/min) of the C axis

Then, a speed specifiable with address F in polar coordinate interpolation can be

given by the formula below. If the maximum cutting feedrate for the C-axis is

exceeded, the automatic speed control function for polar coordinate interpolation

automatically controls the feedrate.

F < L × R × ^π

(mm/min)

180

- Automatic speed control for polar coordinate interpolation

If the velocity component of the rotary axis exceeds the maximum

cutting feedrate in the polar coordinate interpolation mode, the speed

is automatically controlled.

- 26 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

- Automatic override

If the velocity component of the rotary axis exceeds the permissible

velocity

(maximum cutting feedrate multiplied by the permission

factor specified in parameter No. 5463), the feedrate is automatically

overridden as indicated below.

Override = (Permissible velocity) ÷ (Velocity component of rotary

axis) × 100(%)

- Automatic speed clamp

If the velocity component of the rotary axis after automatic override

still exceeds the maximum cutting feedrate, the speed of the rotary

axis is automatically clamped. As a result, the velocity component of

the rotary axis will not exceed the maximum cutting feedrate.

The automatic speed clamp function works only when the center of

the tool is very close to the center of the rotary axis.

C-axis

[Example]

G90 G00 X10.0 C0. ;

D C

B A

G12.1 ;

G01 C0.1 F1000 ;

X-axis

-10.

+10.

X-10.0 :

G13.1 ;

Automatic speed control for polar coordinate interpolation

Suppose that the maximum cutting feedrate of the rotary axis is 360

(3600 deg/min) and that the permission factor of automatic override

for polar coordinate interpolation (parameter No. 5463) is 0 (90%).

If the program indicated above is executed, the automatic override

function starts working when the X coordinate becomes 2.273 (point

A). The automatic speed clamp function starts working when the X

coordinate becomes 0.524 (point B).

The minimum value of automatic override for this example is 3%.

The automatic speed clamp function continues working until the X

coordinate becomes -0.524 (point C). Then, the automatic override

function works until the X coordinate becomes -2.273 (point D).

(The coordinates indicated above are the values in the Cartesian

coordinate system.)

NOTE

1 While the automatic speed clamp function is

working, the machine lock or interlock function may

not be enabled immediately.

2 If a feed hold stop is made while the automatic

speed clamp function is working, the automatic

operation halt signal is output. However, the

operation may not stop immediately.

3 The clamped speed may exceed the clamp value

by a few percent.

- 27 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

Example

Sample program for polar coordinate interpolation in a Cartesian

coordinate system consisting of the X-axis

(a linear axis) and a

hypothetical axis

Hypothetical axis

C axis

Path after tool nose radius compensation

Path before tool nose radius compensation

N204

N203

N205

N202

N201

N200

X axis

Tool

N208

N206

N207

Z axis

The X-axis is by diameter programming; the C-axis is by radius

programming.

O0001 ;

N010 T0101 ;

N0100 G90 G00 X120.0 C0 Z

Positioning to start point

N0200 G12.1 ;

Start of polar coordinate interpolation

N0201 G42 G01 X40.0 F

;

N0202 C10.0 ;

N0203 G03 X20.0 C20.0 R10.0 ;

Geometry program

N0204 G01 X-40.0 ;

(program based on Cartesian

N0205 C-10.0 ;

coordinates on the plane of the

N0206 G03 X-20.0 C-20.0 I10.0 J0 ;

X-axis and virtual axis)

N0207 G01 X40.0 ;

N0208 C0 ;

N0209 G40 X120.0 ;

N0210 G13.1 ;

Cancellation of polar coordinate

N0300 Z

;

interpolation

N0400 X C

;

N0900 M30 ;

- 28 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

3.2

CONSTANT LEAD THREADING (G32)

Tapered screws and scroll threads in addition to equal lead straight

threads can be cut by using a G32 command.

The spindle speed is read from the position coder on the spindle in

real time and converted to a cutting feedrate for feed-per minute mode,

which is used to move the tool.

Straight thread

Tapered screw

Scroll thread

Fig. 3.2 (a) Thread types

Format

G32IP_F_;

X axis

End point_

IP_: End point

F _: Lead of the long axis

(always radius programming)

δ₂

Start point

δ₁

Z axis

Fig. 3.2 (b) Example of threading

- 29 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

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

one-spindle-rotation 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.

Tapered thread

α≤45° lead is LZ

α≥45° lead is LX

Fig. 3.2 (c) LZ and LX of a tapered thread

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

Metric input

0.0001 to 500.0000 mm

Inch input

0.000001 to 9.999999 inch

- 30 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

Example

1. Straight threading

The following values are used in programming :

Thread lead :4mm

X axis

30mm

δ₁=3mm

δ₂=1.5mm

Depth of cut :1mm (cut twice)

(Metric input, diameter programming)

δ₂

δ₁

G00 U-62.0 ;

Z axis

G32 W-74.5 F4.0 ;

G00 U62.0

;

W74.5

;

U-64.0 ;

(For the second cut, cut 1mm more)

G32 W-74.5

;

G00 U64.0

;

W74.5

;

2.Tapered threading

The following values are used in programming :

Thread lead : 3.5mm in the direction of the Z axis

δ₁=2mm

X axis

δ₂=1mm

Cutting depth in the X axis direction is 1mm (cut twice)

φ50

δ₂

(Metric input, diameter programming)

G00 X 12.0 Z72.0 ;

φ43

G32 X 41.0 Z29.0 F3.5 ;

δ₁

G00 X 50.0 ;

Z 72.0 ;

Z axis

X 10.0 ;

φ14

(Cut 1mm more for the second cut)

G32 X 39.0 Z29.0

;

G00 X 50.0

;

Z 72.0

;

- 31 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

WARNING

Feedrate override is effective (fixed at 100%) during threading.

It is very dangerous to stop feeding the thread cutter without stopping the spindle.

This will suddenly increase the cutting depth. Thus, the feed hold function is

ineffective while threading. If the feed hold button is pressed during threading, the

tool will stop after a block not specifying threading is executed as if the SINGLE

BLOCK button were pushed. However, the feed hold lamp (SPL lamp) lights when

the FEED HOLD button on the machine control panel is pushed. Then, when the

tool stops, the lamp is turned off (Single Block stop status).

When the FEED HOLD button is pressed again in the first block after threading

mode that does not specify threading (or the button has been held down), the tool

stops immediately at the block that does not specify threading.

When threading is executed in the single block status, the tool stops after execution

of the first block not specifying threading.

When the mode was changed from automatic operation to manual operation during

threading, the tool stops at the first block not specifying threading as when the feed

hold button is pushed as mentioned in Warning 3.

However, when the mode is changed from one automatic operation mode to

another, the tool stops after execution of the block not specifying threading as for

the single block mode in Note 4.

When the previous block was a threading block, cutting will start immediately

without waiting for detection of the one-spindle-rotation signal even if the present

block is a threading block.

G32Z _ F_ ;

Z _;

(A 1-turn signal is not detected before this block.)

G32 ;

(Regarded as threading block.)

Z_ F_ ; (One turn signal is also not detected.)

Because the constant surface speed control is effective during scroll thread or

tapered screw cutting and the spindle speed changes, the correct thread lead may

not be cut. Therefore, do not use the constant surface speed control during

threading. Instead, use G97.

A movement block preceding the threading block must not specify chamfering or

corner R.

A threading block must not specifying chamfering or corner R.

10 The spindle speed override function is disabled during threading. The spindle

speed is fixed at 100%.

11 Thread cycle retract function is ineffective to G32.

- 32 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

3.3

VARIABLE LEAD THREADING (G34)

Specifying an increment or a decrement value for a lead per screw

revolution enables variable lead threading to be performed.

Fig. 3.3 (a) Variable lead screw

Format

G34 IP_ F_ K_ ;

IP_ : End point

: Lead in longitudinal axis direction at the start point

K_ : Increment and decrement of lead per spindle revolution

Explanation

Address other than K are the same as in straight/taper thread cutting

with G32.

The K value depends on the increment system of the reference axis, as

indicated in Table 3.3 (a).

If the specified K value exceeds the range indicated in Table 3.3 (a), if

the maximum lead is exceeded after a change due to the K value, or if

the lead value is negative, an alarm PS0313 will be issued.

Table 3.3 (a) Range of valid K values

Increment system

Metric input (mm/rev)

Inch input (inch/rev)

of reference axis

IS-A

±0.001

±500.000

±0.00001

to ±50.00000

IS-B

±0.0001

±500.0000

±0.000001 to ±50.000000

IS-C

±0.00001

±50.00000

±0.0000001 to

±5.0000000

CAUTION

The "thread cutting cycle retract" is not effective for

G34.

Example

Lead at the start point: 8.0 mm

Lead increment: 0.3 mm/rev

G34 Z-72.0 F8.0 K0.3 ;

- 33 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

3.4

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.

G32

Fig. 3.4 (a) Continuous threading (Example of G32 in G code system A)

Even when the same section is repeated for threading while changing

the depth of cut, this system allows a correct machining without

impairing the threads.

- 34 -

B-64304EN-1/01

PROGRAMMING

3.INTERPOLATION FUNCTION

3.5

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 : Lead

Fig. 3.5 (a) Multiple thread screws.

Format

(Constant lead threading)

G32 IP _ F_ Q_ ;

IP : End point

F_ : Lead in longitudinal direction

G32 IP _ Q_ ;

Q_ : Threading start angle

Explanation

- Available threading commands

G32: Constant lead threading

G34: Variable lead threading

G76: Multiple threading cycle

G92: 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.

- 35 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- 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)

For the G76 multiple threading cycle command, always use the

FS10/11 command format.

Example

Program for producing double-threaded screws

(with start angles of 0 and 180 degrees)

G00 X40.0 ;

G32 W-38.0 F4.0 Q0 ;

G00 X72.0 ;

W38.0 ;

X40.0 ;

G32 W-38.0 F4.0Q180000 ;

G00 X72.0 ;

W38.0 ;

- 36 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

FUNCTIONS TO SIMPLIFY

PROGRAMMING

Chapter

4, "FUNCTIONS TO SIMPLIFY PROGRAMMING",

consists of the following sections:

4.1 CANNED CYCLE (G90, G92, G94)

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

4.3 CANNED CYCLE FOR DRILLING

4.4 RIGID TAPPING

115

4.5 CANNED GRINDING CYCLE

(FOR GRINDING MACHINE)

131

4.6 CHAMFERING AND CORNER R

145

4.7 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)

153

4.8 DIRECT DRAWING DIMENSION PROGRAMMING

155

- 37 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

4.1

CANNED CYCLE (G90, G92, G94)

There are three canned cycles : the outer diameter/internal diameter

cutting canned cycle (G90), the threading canned cycle (G92), and the

end face turning canned cycle (G94).

NOTE

1 Explanatory figures in this section use the ZX plane

as the selected plane, diameter programming for

the X-axis, and radius programming for the Z-axis.

When radius programming is used for the X-axis,

change U/2 to U and X/2 to X.

2 A canned cycle can be performed on any plane

(including parallel axes for plane definition). When

G-code system A is used, however, U, V, and W

cannot be set as a parallel axis.

3 The direction of the length means the direction of

the first axis on the plane as follows:

ZX plane: Z-axis direction

YZ plane: Y-axis direction

XY plane: X-axis direction

4 The direction of the end face means the direction of

the second axis on the plane as follows:

ZX plane: X-axis direction

YZ plane: Z-axis direction

XY plane: Y-axis direction

- 38 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.1.1

Outer Diameter/Internal Diameter Cutting Cycle (G90)

This cycle performs straight or taper cutting in the direction of the

length.

4.1.1.1

Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length

: Cutting feedrate

X axis

(R)

Rapid traverse

(F)

Cutting feed

4(R)

3(F)

2(F)

1(R)

U/2

A’

X/2

Z axis

Fig. 4.1.1 (a) Straight cutting cycle

Explanation

- Operations

A straight cutting cycle performs four operations:

(1) Operation

1 moves the tool from the start point

(A) to the

specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in

cutting feed. (The tool is moved to the cutting end point (A') in

the direction of the length.)

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in cutting

feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis

on the plane

(start Z-coordinate for the ZX plane) in rapid

traverse. (The tool returns to the start point (A).)

- 39 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.1.1.2

Taper cutting cycle

Format

G90 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length

: Taper amount (R in the figure below)

: Cutting feedrate

X axis

(R)

Rapid traverse

(R)

(F)

Cutting feed

(F)

U/2

(R)

A’

(F)

X/2

Z axis

Fig. 4.1.1 (b) Taper cutting cycle

Explanation

The figure of a taper is determined by the coordinates of the cutting

end point (A') in the direction of the length and the sign of the taper

amount (address R). For the cycle in the figure above, a minus sign is

added to the taper amount.

NOTE

The increment system of address R for specifying a

taper depends on the increment system for the

reference axis. Specify a radius value at R.

- Operations

A taper cutting cycle performs the same four operations as a straight

cutting cycle.

However, operation 1 moves the tool from the start point (A) to the

position obtained by adding the taper amount to the specified

coordinate of the second axis on the plane (specified X-coordinate for

the ZX plane) in rapid traverse.

Operations 2, 3, and 4 after operation 1 are the same as for a straight

cutting cycle.

- 41 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

B-64304EN-1/01

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the

sign of the taper amount (address R) and the cutting end point in the

direction of the length in the absolute or incremental programming as

follows.

Outer diameter machining

Internal diameter machining

1. U < 0, W < 0, R < 0

2. U > 0, W < 0, R > 0

4(R)

2(F)

U/2

3(F)

1(R)

U/2

3(F)

1(R)

2(F)

4(R)

3. U < 0, W < 0, R > 0

4. U > 0, W < 0, R < 0

at |R|≤|U/2|

4(R)

1(R)

2(F)

U/2

3(F)

U/2

3(F)

2(F)

1(R)

4(R)

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other

than G90, G92, or G94.

- 42 -

4.FUNCTIONS TO SIMPLIFY

B-64304EN-1/01

PROGRAMMING

4.1.2

Threading Cycle (G92)

4.1.2.1

Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length

: Angle for shifting the threading start angle

(Increment: 0.001 degrees,

Valid setting range: 0 to 360 degrees)

: Thread lead (L in the figure below)

X axis

4(R)

3(R)

1(R)

2(F)

U/2

A’

X/2

Z axis

(R) ... Rapid traverse

(F)

Cutting feed

Approx.

(The chamfered angle in the left figure is 45

45°

degrees or less because of the delay in the

servo system.)

Detailed chamfered thread

Fig. 4.1.2 (c) Straight threading

Explanation

The ranges of thread leads and restrictions related to the spindle speed

are the same as for threading with G32.

- Operations

A straight threading cycle performs four operations:

(1) Operation

1 moves the tool from the start point

(A) to the

specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in

cutting feed. At this time, thread chamfering is performed.

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in rapid

traverse. (Retraction after chamfering)

- 43 -

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