Content      ..     1      2      3      4      ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 3

3.

PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-63534EN/02

G code list for M series (4/4)

G code

Group

Function

G80

09

Canned cycle cancel/external operation function cancel

G80.5

24

Synchronization start of electronic gear box (EGB) (for two axes program-

ming)

G81

09

Drilling cycle, spot boring cycle or external operation function

G81.1

00

Chopping function

G81.5

24

Synchronization start of electronic gear box (EGB) (for two axes program-

ming)

G82

Drilling cycle or counter boring cycle

G83

Peck drilling cycle

G84

Tapping cycle

G85

Boring cycle

09

G86

Boring cycle

G87

Back boring cycle

G88

Boring cycle

G89

Boring cycle

G90

Absolute command

03

G91

Increment command

G92

Setting for work coordinate system or clamp at maximum spindle speed

00

G92.1

Workpiece coordinate system preset

G94

Feed per minute

05

G95

Feed per rotation

G96

Constant surface speed control

13

G97

Constant surface speed control cancel

G98

Return to initial point in canned cycle

10

G99

Return to R point in canned cycle

G160

In-feed control function cancel(for grinding machine)

20

G161

In-feed control function(for grinding machine)

40

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

4.1

The G00 command moves a tool to the position in the workpiece system

POSITIONING (G00)

specified with an absolute or an incremental command at a rapid traverse

rate.

In the absolute command, coordinate value of the end point is

programmed.

In the incremental command the distance the tool moves is programmed.

Format

G00

IP

_;

IP: For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance

the tool moves.

Explanations

Either of the following tool paths can be selected according to bit 1 of

parameter LRP No. 1401.

D Nonlinear interpolation positioning

The tool is positioned with the rapid traverse rate for each axis

separately. The tool path is normally straight.

D Linear interpolation positioning

The tool path is the same as in linear interpolation (G01). The tool

is positioned within the shortest possible time at a speed that is not

more than the rapid traverse rate for each axis.

Start position

Linear interpolation positioning

End position

Non linear interpolation positioning

The rapid traverse rate in G00 command is set to the parameter No. 1420

for each axis independently by the machine tool builder. In the

posiitoning mode actuated by G00, the tool is accelerated to a

predetermined speed at the start of a block and is decelerated at the end

of a block. Execution proceeds to the next block after confirming the

in-position.

“In-position ” means that the feed motor is within the specified range.

This range is determined by the machine tool builder by setting to

parameter (No. 1826).

In-position check for each block can be disabled by setting bit 5 (NCI)

of parameter No.1601 accordingly.

42

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

4.2

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

positioning from one direction is available.

SINGLE DIRECTION

POSITIONING (G60)

Overrun

Start position

Start position

Temporary stop

End position

Format

G60

_;

IP

IP : For an absolute command, the coordinates of an end

position, and for an incremental commnad, the distance

the tool moves.

Explanations

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 an one-shot G-code, can be used as a modal G-code in

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

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

Other specifications are the same as those for an one-shot G60 command.

When an one-shot G code is sepcified in the single direction positioning

mode, the one-shot G command is effective like G codes in group 01.

Examples

When one-shot

When modal

G60 commands are used.

G60 command is used.

G90;

G90G60;

Single direction

positioning mode start

G60

X0Y0;

X0Y0;

Single direction

Single direction

G60

X100;

X100;

positioning

positioning

G60

Y100;

Y100;

G04

X10;

G04X10;

G00

X0Y0;

G00X0Y0; Single direction

positioning

mode cancel

44

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

Tools can move along a line

4.3

LINEAR

INTERPOLATION

(G01)

Format

G01

IP_F_;

_:For an absolute command, the coordinates of an end point ,

IP

and for an incremental commnad, the distance the tool moves.

F_:Speed of tool feed (Feedrate)

Explanations

A tools move along a line to the specified position at the feedrate

specified in F.

The feedrate specified in F is effective until a new value is specified. It

need not be specified for each block.

The feedrate commanded by the F code is measured along the tool path.

If the F code is not commanded, the feedrate is regarded as zero.

The feedrate of each axis direction is as follows.

G01ααββγγζζ Ff ;

Feed rate of α axis direction : Fa +a

f

L

b

Feed rate of β axis direction :

F_b +

f

L

g

Feed rate of γ axis direction :

Fg +

f

L

z

Feed rate of ζ axis direction : F_z +

f

L

L + a2 ) b2 ) g2 ) z²Ǹ

The feed rate of the rotary axis is commanded in the unit of deg/min (the

unit is decimal point position).

When the straight line axis α(such as X, Y, or Z) and the rotating axisβ

(such as A, B, or C) are linearly interpolated, the feed rate is that in which

the tangential feed rate in the α and β cartesian coordinate system is

commanded by F(mm/min).

β-axis feedrate is obtained ; at first, the time required for distribution is

calculated by using the above fromula, then the β -axis feedrate unit is

changed to deg/min.

46

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

A calculation example is as follows.

G91 G01 X20.0B40.0 F300.0 ;

This changes the unit of the C axis from 40.0 deg to 40mm with metric

input. The time required for distribution is calculated as follows:

^Ǹ20² ) 40²

8 0.14907

(min)

300

The feed rate for the C axis is

40

8

268.3 degńmin

0.14907

In simultaneous 3 axes control, the feed rate is calculated the same way

as in 2 axes control.

Examples

D Linear interpolation

(G91) G01X200.0Y100.0F200.0 ;

Y axis

(End position)

100.0

X axis

0

(Start position)

200.0

D Feedrate for the

rotation axis

G91G01C-90.0 G300.0 ;Feed rate of 300deg/min

(Start point)

90°

(End point)

Feedrate is 300 deg/min

47

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

The command below will move a tool along a circular arc.

4.4

CIRCULAR

INTERPOLATION

(G02, G03)

Format

Arc in the XpYp plane

G02

I_ J_

G17

Xp_Yp_

F_ ;

G03

R_

Arc in the ZpXp plane

G02

I_ K_

G18

Xp_ p_

F_

G03

R_

Arc in the YpZp plane

G02

J_ K_

F_

G19

Yp_ Zp_

G03

R_

Table. 4.4 Description of the Command Format

Command

Description

G17

Specification of arc on XpYp plane

G18

Specification of arc on ZpXp plane

G19

Specification of arc on YpZp plane

G02

Circular Interpolation Clockwise direction (CW)

G03

Circular Interpolation Counterclockwise direction (CCW)

X_{p_}

Command values of X axis or its parallel axis

(set by parameter No. 1022)

Yp_

Command values of Y axis or its parallel axis

(set by parameter No. 1022)

Z_{p_}

Command values of Z axis or its parallel axis

(set by parameter No. 1022)

I_

X_p axis distance from the start point to the center of an arc

with sign

J_

Yp axis distance from the start point to the center of an arc

with sign

k_

Z_p axis distance from the start point to the center of an arc

with sign

R_

Arc radius (with sign)

F_

Feedrate along the arc

48

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Explanations

D Direction of the circular

“Clockwise”(G02) and “counterclockwise”(G03) on the X_pY_p plane

interpolation

(Z_pX_p plane or Y_pZ_p plane) are defined when the X_pY_p plane is viewed

in the positive-to-negative direction of the Z_p axis (Y_p axis or X_p axis,

respectively) in the Cartesian coordinate system. See the figure below.

Yp

Xp

Zp

G03

G03

G03

G02

G02

G02

Xp

Zp

Yp

G17

G18

G19

D Distance moved on an

The end point of an arc is specified by address Xp, Yp or Zp, and is

arc

expressed as an absolute or incremental value according to G90 or G91.

For the incremental value, the distance of the end point which is viewed

from the start point of the arc is specified.

D Distance from the start

The arc center is specified by addresses I, J, and K for the Xp, Yp, and Zp

point to the center of arc

axes, respectively. The numerical value following I, J, or K, however, is

a vector component in which the arc center is seen from the start point,

and is always specified as an incremental value irrespective of G90 and

G91, as shown below.

I, J, and K must be signed according to the direction.

End point (x,y)

End point (z,x)

End point (y,z)

y

x

z

x

Start

z

y

i

Start

j

Start

k

point

point

point

j

i

k

Center

Center

Center

I0,J0, and K0 can be omitted. When X_p, Y_p , and Zp are omitted (the end

point is the same as the start point) and the center is specified with I, J,

and K, a 360° arc (circle) is specified.

G021; Command for a circle

If the difference between the radius at the start point and that at the

end point exceeds the permitted value in a parameter (No.3410), an P/S

alarm (No.020) occurs.

49

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

D Arc radius

The distance between an arc and the center of a circle that contains the arc

can be specified using the radius, R, of the circle instead of I, J, and K.

In this case, one arc is less than 180°, and the other is more than 180° are

considered. When an arc exceeding 180° is commanded, the radius must

be specified with a negative value. If Xp, Yp, and Zp are all omitted, if

the end point is located at the same position as the start point and when

R is used, an arc of 0° is programmed

G02R ; (The cutter does not move.)

For arc (1)(less than 180°)

G91 G02 X_P60.0 Y_P20.0 R50.0 F300.0 ;

For arc (2)(greater than 180°)

G91 G02 X_P60.0 Y_P20.0 R-50.0 F300.0 ;

2

r=50mm

End point

1

Start point

r=50mm

Y

X

D Feedrate

The feedrate in circular interpolation is equal to the feed rate specified by

the F code, and the feedrate along the arc (the tangential feedrate of the

arc) is controlled to be the specified feedrate.

The error between the specified feedrate and the actual tool feedrate is

±2% or less. However, this feed rate is measured along the arc after the

cutter compensation is applied

Restrictions

If I, J, K, and R addresses are specified simultaneously, the arc specified

by address R takes precedence and the other are ignored.

If an axis not comprising the specified plane is commanded, an alarm is

displayed.

For example, if axis U is specified as a parallel axis to X axis when plane

XY is specified, an P/S alarm (No.028)is displayed.

When an arc having a center angle approaching 180° is specified, the

calculated center coordinates may contain an error. In such a case, specify

the center of the arc with I, J, and K.

50

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Examples

Y axis

100

50R

60

60R

40

0

X axis

90

120 140

200

The above tool path can be programmed as follows ;

(1) In absolute programming

G92X200.0 Y40.0 Z0 ;

G90 G03 X140.0 Y100.0R60.0 F300.;

G02 X120.0 Y60.0R50.0 ;

or

G92X200.0 Y40.0Z0 ;

G90 G03 X140.0 Y100.0I-60.0 F300.;

G02 X120.0 Y60.0I-50.0 ;

(2) In incremental programming

G91 G03 X-60.0 Y60.0 R60.0 F300.;

G02 X-20.0 Y-40.0 R50.0 ;

or

G91 G03 X-60.0 Y60.0 I-60.0 F300. ;

G02 X-20.0 Y-40.0 I-50.0 ;

51

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

4.5

Helical interpolation which moved helically is enabled by specifying up

HELICAL

to two other axes which move synchronously with the circular

INTERPOLATION

interpolation by circular commands.

(G02, G03)

Format

Synchronously with arc of XpYp plane

G02

G17

I_J_

Xp_Yp_

α_(β_)F_;

G03

R_

Synchronously with arc of ZpXp plane

G02

G18

I_K_

Xp_Zp_

α_(β_)F_;

G03

R_

Synchronously with arc of YpZp plane

G02

J_K_

G19

Yp_Zp_

α_(β_)F_;

G03

R_

α,β: Any one axis where circular interpolation is not applied.

Up to two other axes can be specified.

Explanations

The command method is to simply or secondary add a move command

axis which is not circular interpolation axes. An F command specifies a

feed rate along a circular arc. Therefore, the feed rate of the linear axis

is as follows:

Length of linear axis

F×

Length of circular arc

Determine the feed rate so the linear axis feed rate does not exceed any

of the various limit values.Bit 0 (HFC) of parameter No. 1404 can be used

to prevent the linear axis feedrate from exceeding various limit values.

Z

Tool path

X

Y

The feedrate along the circumference of two cir-

cular interpolated axes is the specified feedrate.

Restrictions

⋅Cutter compensation is applied only for a circular arc.

⋅Tool offset and tool length compensation cannot be used in a block in

which a helical interpolation is commanded.

52

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.6

Helical interpolation B moves the tool in a helical manner. This

interpolation can be executed by specifying the circular interpolation

HELICAL

command together with up to four additional axes in simple

INTERPOLATION B

high-precision contour control mode (see II-19.7).

(G02, G03)

Format

With an arc in the XpYp plane

G02

G17

I_J_

Xp_Yp_

α_β_γ_δ_F_;

G03

R_

With an arc in the ZpXp plane

G02

G18

I_K_

Xp_Zp_

α_β_γ_δ_F_;

G03

R_

With an arc in the YpZp plane

G02

J_K_

G19

Yp_Zp_

α_β_γ_δ_F_;

G03

R_

α, β, γ, δ

: Any axis to which circular interpolation is not applied.

Up to four axes can be specified.

Explanations

Basically, the command can be specified by adding two movement axes

to a standard helical interpolation command (see II-4.5). Address F

should be followed by a tangential velocity, which has been determined

by also taking movement along the linear axes into consideration.

Z

Tool path

X

Y

The feedrate equals the tangential velocity determined by also

taking movement along the linear axes into consideration.

Limitations

⋅ The command of helical interpolation B can be specified only in AI

contour control mode.

⋅ Cutter compensation is applied only to an arc.

⋅ In a block containing the helical interpolation command, the tool offset

command or tool length compensation command cannot be specified.

53

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

4.7

Spiral interpolation is enabled by specifying the circular interpolation

command together with a desired number of revolutions or a desired

SPIRAL

increment (decrement) for the radius per revolution.

INTERPOLATION,

Conical interpolation is enabled by specifying the spiral interpolation

CONICAL

command together with one or two additional axes of movement, as well

as a desired increment (decrement) for the position along the additional

INTERPOLATION

axes per spiral revolution.

(G02, G03)

Format

D Spiral interpolation

XpYp plane

G02

G17

X_ Y_ I_ J_ Q_ L_ F_ ;

G03

ZpXp plane

G02

G18

Z_X_K_ I_ Q_ L_ F_ ;

G03

YpZp plane

G02

G19

Y_ Z_ J_ K_ Q_ L_ F_ ;

G03

X,Y,Z Coordinates of the end point

L

Number of revolutions (positive value without a decimal point)(*1)

Q Radius increment or decrement per spiral revolution(*1)

I,J,K Signed distance from the start point to the center

(same as the distance specified for circular interpolation)

F

Feedrate

(*1) Either the number of revolutions (L) or the radius increment or

decrement (Q) can be omitted. When L is omitted, the number of

revolutions is automatically calculated from the distance between

the current position and the center, the position of the end point,

and the radius increment or decrement. When Q is omitted, the

radius increment or decrement is automatically calculated from the

distance between the current position and the center, the position

of the end point, and the number of revolutions. If both L and Q are

specified but their values contradict, Q takes precedence. Gener-

ally, either L or Q should be specified. The L value must be a posi-

tive value without a decimal point. To specify four revolutions plus

90°, for example, round the number of revolutions up to five and

specify L5.

54

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Conical interpolation

XpYp plane

G02

G17

X_ Y_ Z_ I_ J_ K_ Q_ L_ F_ ;

G03

ZpXp plane

G02

G18

Z_ X_ Y_ K_ I_ J_ Q_ L_ F_ ;

G03

YpZp plane

G19

G02

Y_ Z_ X_ J_ K_ I_ Q_ L_ F_ ;

G03

X,Y,Z Coordinates of the end point

L

Number of revolutions (positive value without a decimal point)(*1)

Q

(Radius increment or decrement per spiral revolution(*1)

I,J,K

Two of the three values represent a signed vector from the start

point to the center. The remaining value is a height increment or

decrement per spiral revolution in conical interpolation(*1)(*2)

When the XpYp plane is selected:

The I and J values represent a signed vector from the start point

to the center.

The K value represents a height increment or decrement per

spiral revolution.

When the ZpXp plane is selected:

The K and I values represent a signed vector from the start point

to the center.

The J value represents a height increment or decrement per

spiral revolution.

When the YpZp plane is selected:

The J and K values represent a signed vector from the start point

to the center.

The I value represents a height increment or decrement per spiral

revolution.

F

Feedrate (determined by taking movement along the linear axes

into consideration)

(*1)

One of the height increment/decrement (I, J, K), radius increment/

decrement (Q), and the number of revolutions (L) must be speci-

fied. The other two items can be omitted.

⋅ Sample command for the XpYp plane

K_

G02

G17

X_ Y_ I_ J_ Z_ ;

Q_

F_ ;

G03

L_

If both L and Q are specified, but their values contradict, Q takes

precedence. If both L and a height increment or decrement are

specified, but their values contradict, the height increment or

decrement takes precedence. If both Q and a height increment or

decrement are specified, but their values contradict, Q takes pre-

cedence. The L value must be a positive value without a decimal

point. To specify four revolutions plus 90°, for example, round the

number of revolutions up to five and specify L5.

(*2)

When two axes (of height) other than plane axes are specified, the

height increment or decrement (I, J, K) cannot be specified. Spec-

ify either a desired radius increment or decrement (Q) or a desired

number of revolutions (L).

55

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Limitations

D Radius

In spiral or conical interpolation, R for specifying an arc radius cannot be

specified.

D Corner deceleration

Corner deceleration between the spiral/conical interpolation block and

other blocks can be performed only in simple high-precision contour

control mode.

D Feed functions

The functions of feed per rotation, inverse time feed, F command with one

digit, and automatic corner override cannot be used.

D Program restart

A program including spiral or conical interpolation cannot be restarted.

D Retrace

A program including spiral or conical interpolation cannot be retraced.

D Normal direction control

Spiral interpolation and conical interpolation cannot be specified in

normal direction control mode.

Examples

D Spiral interpolation

20.

20.

120

Y axis

100

80

60

40

20

0

-120-100 -80 -60 -40

-20

0

20

40

60

80

100 120

–20

X axis

-40

-60

-80

-100

-120

The path indicated above is programmed with absolute and incremental

values, as shown below:

This sample path has the following values:

⋅ Start point

:

(0, 100.0)

⋅ End point (X, Y)

:

(0, -30.0)

⋅ Distance to the center (I, J)

:

(0, -100.0)

⋅ Radius increment or decrement (Q) :

-20.0

⋅ Number of revolutions (L)

:

4.

57

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

(1) With absolute values, the path is programmed as follows:

Q-20.0

G90 G02 X0 Y-30.0 I0 J-100.0

F300;

L4

(2) With incremental values, the path is programmed as follows:

Q-20.0

G91 G02 X0 Y-130.0 I0 J-100.0

F300;

L4

(Either the Q or L setting can be omitted.)

D Conical interpolation

+Z

25.0

25.0

(0,-37.5,62.5)

25.0

25.0

+Y

100.0

-100.0

+X

The sample path shown above is programmed with absolute and

incremental values as follows:

This sample path has the following values:

⋅ Start point

:

(0, 100.0, 0)

⋅ End point (X, Y, Z)

:

(0, -37.5, 62.5)

⋅ Distance to the center (I, J)

:

(0, -100.0)

⋅ Radius increment or decrement (Q) :

-25.0

⋅ Height increment or decrement (K)

:

25.0

⋅ Number of revolutions (L)

:

3

(1) With absolute values, the path is programmed as follows:

K25.0

G90 G02 X0 Y-37.5 Z62.5 I0 J-100.0 Q-25.0

F300;

L3

(2) With incremental values, the path is programmed as follows:

K25.0

G91 G02 X0 Y-137.5 Z62.5 I0 J-100.0 Q-25.0

F300;

L3

58

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Polar coordinate interpolation is a function that exercises contour control

4.8

in converting a command programmed in a Cartesian coordinate system

POLAR COORDINATE

to the movement of a linear axis (movement of a tool) and the movement

INTERPOLATION

of a rotary axis (rotation of a workpiece). This function is useful for

grinding a cam shaft.

(G12.1, G13.1)

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 (virtual axis).

G13.1 ;

Polar coordinate interpolation mode is cancelled (for not

performing polar coordinate interpolation)

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

Explanations

D Polar coordinate

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

interpolation plane

coordinate interpolation plane (Fig. 4.8 (a)). Polar coordinate

interpolation is performed on this plane.

Rotary axis (virtual 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. 4.8 (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 (No. 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.

59

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Tool offset command

The polar coordinate interpolation mode cannot be started or terminated

(G12.1 or G13.1) in the tool offset mode (G41 or G42). G12.1 or G13.1

must be specified in the tool offset canceled mode (G40).

D Tool length offset

Tool length offset must be specified in the polar coordinate interpolation

command

cancel mode before G12.1 is specified. It cannot be

specified in the polar coordinate interpolation mode. Furthermore, no

offset values can be changed in the polar coordinate interpolation mode.

D 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.

D Program restart

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

D Cutting feedrate for the

Polar coordinate interpolation converts the tool movement for a figure

rotation axis

programmed in a Cartesian coordinate system to the tool movement in the

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

closer to the center of the workpiece, the C-axis component of the

feedrate becomes larger and may exceed the maximum cutting feedrate

for the C-axis (set in parameter (No. 1422)), causing an alarm (see the

figure below). To prevent the C-axis component from exceeding the

maximum cutting feedrate for the C-axis, reduce the feedrate specified

with address F or create a program so that the tool (center of the tool when

cutter compensation is applied) does not move close to the center of the

workpiece.

WARNING

∆ X

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

θ1

at the feedrate specified with address F in the Cartesian coordinate system.

L1

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

θ2

L2

time unit corresponding to ∆X in the Cartesian coordinate system increases

θ3

fromθ1 toθ 2 to θ3.

L3

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.

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.

Specify a speed allowed by the formula. The formula provides a theoretical value; in practice, a value slightly

smaller than a theoretical value may need to be used due to a calculation error.

π

F < L × R ×

(mm/min)

180

61

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

Examples

Example of Polar Coordinate Interpolation Program

Based on X Axis(Linear Axis) and C Axis

(Rotary Axis)

C’(hypothetical axis)

C axis

Path after cutter compensation

Program path

N204

N203

N205

N200

N202

N201

X axis

Tool

N208

N206

N207

Z axis

O0001 ;

N010 T0101

N0100 G90 G00 X60.0 C0 Z_ ; Positioning to start position

N0200 G12.1 ;

Start of polar coordinate interpolation

N0201 G42 G01 X20.0 F_ ;

N0202 C10.0 ;

N0203 G03 X10.0 C20.0 R10.0 ;

N0204 G01 X-20.0 ;

Geometry program

N0205 C-10.0 ;

(program based on cartesian coordinates on

N0206 G03 X-10.0 C-20.0 I10.0 J0 ;

X-C’ plane)

N0207 G01 X20.0 ;

N0208 C0 ;

N0209 G40 X60.0 ;

N0210 G13.1 ;

Cancellation of polar coordinate interpolation

N0300 Z_ ;

N0400 X_ C_ ;

N0900M30 ;

62

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

The amount of travel of a rotary axis specified by an angle is once

4.9

internally converted to a distance of a linear axis along the outer surface

CYLINDRICAL

so that linear interpolation or circular interpolation can be performed with

INTERPOLATION

another axis. After interpolation, such a distance is converted back to the

amount of travel of the rotary axis.

(G07.1)

The cylindrical interpolation function allows the side of a cylinder to be

developed for programming. So programs such as a program for

cylindrical cam grooving can be created very easily.

Format

G07.1IPr ; Starts the cylindrical interpolation mode

(e

:

:

:

G07.1

IP

0 ; The cylindrical interpolation mode is cancelled.

IP

: An address for the rotation axis

r : The radius of the cylinder

Specify G07.1 IPr ; and G07.1

IP

0; in separate blocks.

G107 can be used instead of G07.1.

Explanations

D Plane selection

Use parameter (No. 1022) to specify whether the rotation axis is the X-,

(G17, G18, G19)

Y-, or Z-axis, or an axis parallel to one of these axes. Specify the G code

to select a plane for which the rotation axis is the specified linear axis.

For example, when the rotation axis is an axis parallel to the X-axis, G17

must specify an Xp-Yp plane, which is a plane defined by the rotation axis

and the Y-axis or an axis parallel to the Y-axis.

Only one rotation axis can be set for cylindrical interpolation.

D Feedrate

A feedrate specified in the cylindrical interpolation mode is a speed on the

developed cylindrical surface.

D Circular interpolation

In the cylindrical interpolation mode, circular interpolation is possible

(G02,G03)

with the rotation axis and another linear axis. Radius R is used in

commands in the same way as described in II-4.4.

The unit for a radius is not degrees but millimeters (for metric input) or

inches (for inch input).

< Example Circular interpolation between the Z axis and C axis >

For the C axis of parameter (No.1022), 5 (axis parallel with the X axis)

is to be set. In this case, the command for circular interpolation is

G18 Z__C__;

G02 (G03) Z__C__R__;

For the C axis of parameter (No.1022), 6 (axis parallel with the Y axis)

may be specified instead. In this case, however, the command for

circular interpolation is

G19 C__Z__;

G02 (G03) Z__C__R__;

63

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Examples

Example of a Cylindrical Interpolation Program

C

O0001 (CYLINDRICAL INTERPOLATION );

N01 G00 G90 Z100.0 C0 ;

Z

R

N02 G01 G91 G18 Z0 C0 ;

N03 G07.1 C57299 ; (*)

N04 G90 G01 G42 Z120.0 D01 F250 ;

N05 C30.0 ;

N06 G02 Z90.0 C60.0 R30.0 ;

N07 G01 Z70.0 ;

N08 G03 Z60.0 C70.0 R10.0 ;

N09 G01 C150.0 ;

N10 G03 Z70.0 C190.0 R75.0 ;

N11 G01 Z110.0 C230.0 ;

N12 G02 Z120.0 C270.0 R75.0 ;

N13 G01 C360.0 ;

N14 G40 Z100.0 ;

N15 G07.1 C0 ;

N16 M30 ;

* A command with a decimal point can also be used.

Z

mm

N05

N13

N12

120

110

N06

N11

90

N07

70

N08

N09

N10

60

C

0

30

60

70

150

190

230

270

360

deg

65

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

4.10

Involute curve machining can be performed by using involute

interpolation. Involute interpolation ensures continuous pulse distribution

INVOLUTE

even in high-speed operation in small blocks, thus enabling smooth and

INTERPOLATION

high-speed machining. Furthermore, machining tapes can be created

(G02.2, G03.2)

easily and efficiently, reducing the required length of tape.

Format

Involute interpolation on the X-Y plane

G17 G02.2 X__Y__I__J__R__F__ ;

G17 G03.2 X__Y__I__J__R__F__ ;

Involute interpolation on the Z-X plane

G18 G02.2 Z__X__K__I__R__F__ ;

G18 G03.2 Z__X__K__I__R__F__ ;

Involute interpolation on the Y-Z plane

G19 G02.2 Y__Z__J__K__R__F__ ;

G19 G03.2 Y__Z__J__K__R__F__ ;

Where,

G02.2 : Involute interpolation (clockwise)

G03.2 : Involute interpolation (counterclockwise)

G17/G18/G19 : X -Y / Z-X / Y-Z plane selection

X, Y, Z

: Involute curve end coordinate

I, J, K : Center of the base circle for an involute curve viewed

from the start point

R : Base circle radius

F : Cutting feedrate

Yp

Yp

Po

Ps

I

R

End point

J

0

Pe

Start point

I

Po

Ps

J

0

R

Base circle

Pe

End point

Xp

Xp

Clockwise involute interpolation (G02.2)

Yp

Yp

End point

Ro

Pe

R

Start point

0

Ps

I

Po

P

e

End point

J

J

0

R

I

Ps

Start point

Xp

Xp

Counterclockwise involute interpolation (G03.2)

66

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Explanations

D Involute curve

An involute curve on the X-Y plane is defined as follows ;

X (θ)=R [cos θ+ (θ-θ₀ ) sin θ] +X₀

Y (θ)=R [sin θ- (θ-θ₀ ) cos θ] +Y₀

where,

X₀ , Y₀

: Coordinates of the center of a base circle

R

: Base circle radius

θ₀: Angle of the start point of an involute curve

θ

: Angle of the point where a tangent from the current position

to the base circle contacts the base circle

X (θ), Y (θ): Current position on the X-axis and Y-axis

Y

Involute curve

Start point

(X,Y)

R

θ0

θ

(X0,Y0)

End point

Base circle

X

Fig. 4.10 (a) Involute Curve

Involute curves on the Z-X plane and Y-Z plane are defined in the same

way as an involute curve on the X-Y plane.

D Start point and end point

The end point of an involute curve is specified using address X, Y, or Z.

An absolute value or incremental value is used to specify an X, Y, or Z

value. When using an incremental value, specify the coordinates of the

end point viewed from the start point of the involute curve.

When no end point is specified, P/S alarm No. 241 is issued.

If the specified start point or end point lies within the base circle, P/S

alarm No. 242 is issued. The same alarm is issued if cutter compensation

C causes the offset vector to enter the base circle. Be particularly careful

when applying an offset to the inside of an involute curve.

D Base circle specification

The center of a base circle is specified with I, J, and K, corresponding to

X, Y, and Z. The value following I, J, or K is a vector component defined

when the center of the base circle is viewed from the start point of the

involute curve; this value must always be specified as an incremental

value, regardless of the G90/G91 setting. Assign a sign to I, J, and K

according to the direction.

If I, J, and K are all left unspecified, or I0J0K0 is specified, P/S alarm No.

241 or No. 242 is issued.

If R is not specified, or R <

0, P/S alarm No. 241 or No. 242 is issued.

67

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63534EN/02

D Choosing from two types

When only a start point and I, J, and K data are given, two types of involute

of involute curves

curves can be created. One type of involute curve extends towards the

base circle, and the other extends away from the base circle. When the

specified end point is closer to the center of the base circle than the start

point, the involute curve extends toward the base circle. In the opposite

case, the involute curve extends away from the base circle.

D Feedrate

The cutting feedrate specified in an F code is used as the feedrate for

involute interpolation. The feedrate along the involute curve (feedrate

along the tangent to the involute curve) is controlled to satisfy the

specified feedrate.

D Plane selection

As with circular interpolation, the plane to which to apply involute

interpolation can be selected using G17, G18, and G19.

D Cutter compensation C

Cutter compensation C can be applied to involute curve machining. As

with linear and circular interpolation, G40, G41, and G42 are used to

specify cutter compensation.

G40 : Cutter compensation cancel

G41 : Cutter compensation left

G42 : Cutter compensation right

Cutter compensation for an involute curve is implemented as described

below.

First, near the start point of an involute curve, an arc with a curvature close

to the curvature of the involute curve is found. Next, an offset intersection

between the arc and the linear line or arc in the previous block is found.

Similarly, an offset intersection is found near the end point. Then, the

involute curve passing through the two points is used as the tool center

path.

In involute interpolation mode, cutter compensation cannot be started or

cancelled.

Tool center path

Programmed

Start point

path

Arc with a curvature

closer to the curva-

R

ture of the involute

curve near the start

End point

point

Arc with a curvature closer to the

curvature of the involute curve near

the end point

68

B-63534EN/02

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Specifiable G codes

The following G codes can be specified in involute interpolation mode:

G04 : Dwell

G10 : Data setting

G17 : X-Y plane selection

G18 : Z-X plane selection

G19 : Y-Z plane selection

G65 : Macro call

G66 : Macro modal call

G67 : Macro modal call cancel

G90 : Absolute command

G91 : Incremental command

D Modes that allow

Involute interpolation can be specified in the following G code modes:

involute interpolation

G41 : Cutter compensation left

specification

G42 : Cutter compensation right

G51 : Scaling

G51.1

: Programmable mirror image

G68 : Coordinate rotation

D End point error

As shown below the end point may not be located on an involute curve

that passes through the start point.

When an involute curve that passes through the start point deviates from

the involute curve that passes through the end point by more than the value

set in parameter No. 5610, P/S alarm No. 243 is issued.

When there is an end point error, the feedrate is not guaranteed.

Y

End point

Deviation

Pe

Path after correction

Start

point

Ps

Correct involute curve

X

Fig. 4.10 (b) End Point Error in Counterclockwise Involute Interpolation

(G03.2)

69

Content      ..     1      2      3      4      ..