Content      ..     1      2      3      4      ..

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 3

3. PREPARATORY FUNCTION

B-63524EN/01

PROGRAMMING

(G FUNCTION)

Table 3 G code list for T series (1/3)

G code

Group

Function

A

B

C

G00

G00

G00

Positioning (Rapid traverse)

G01

G01

G01

Linear interpolation (Cutting feed)

01

G02

G02

G02

Circular interpolation CW or helical interpolation CW

G03

G03

G03

Circular interpolation CCW or helical interpolation CCW

G04

G04

G04

Dwell

G05

G05

G05

High-speed cycle cutting

G07

G07

G07

Hypothetical axis interpolation

G07.1

G07.1

G07.1

Cylindrical interpolation

(G107)

(G107)

(G107)

00

G08

G08

G08

Look-ahead control

G10

G10

G10

Programmable data input

G10.6

G10.6

G10.6

Tool retract and return

G11

G11

G11

Programmable data input mode cancel

G12.1

G12.1

G12.1

Polar coordinate interpolation mode

(G112)

(G112)

(G112)

21

G13.1

G13.1

G13.1

Polar coordinate interpolation cancel mode

(G113)

(G113)

(G113)

G17

G17

G17

XpYp plane selection

G18

G18

G18

16

ZpXp plane selection

G19

G19

G19

YpZp plane selection

G20

G20

G70

Input in inch

06

G21

G21

G71

Input in mm

G22

G22

G22

Stored stroke check function on

09

G23

G23

G23

Stored stroke check function off

G25

G25

G25

Spindle speed fluctuation detection off

08

G26

G26

G26

Spindle speed fluctuation detection on

G27

G27

G27

Reference position return check

G28

G28

G28

Return to reference position

G30

G30

G30

00

2nd, 3rd and 4th reference position return

G30.1

G30.1

G30.1

Floating reference point return

G31

G31

G31

Skip function

G32

G33

G33

Thread cutting

G34

G34

G34

Variable-lead thread cutting

01

G35

G35

G35

Circular threading CW

Circular threading CCW (When the bit 3 (G36) of parameter

G36

G36

G36

No. 3405 is set to 1)

39

3.

PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-63524EN/01

Table 3 G code list for T series (2/3)

G code

Group

Function

A

B

C

Automatic tool compensation X (When the bit 3 (G36) of

G36

G36

G36

parameter No. 3405 is set to 0)

G37

G37

G37

Automatic tool compensation Z

00

G37.1

G37.1

G37.1

Automatic tool compensation X

G37.2

G37.2

G37.2

Automatic tool compensation Z

G39

G39

G39

Corner circular interpolation

G40

G40

G40

Tool nose radius compensation cancel

G41

G41

G41

07

Tool nose radius compensation left

G42

G42

G42

Tool nose radius compensation right

G50

G92

G92

Coordinate system setting or max. spindle speed setting

00

G50.3

G92.1

G92.1

Workpiece coordinate system preset

G50.2

G50.2

G50.2

Polygonal turning cancel

(G250)

(G250)

(G250)

20

G51.2

G51.2

G51.2

Polygonal turning

(G251)

(G251)

(G251)

G52

G52

G52

Local coordinate system setting

00

G53

G53

G53

Machine coordinate system setting

G54

G54

G54

Workpiece coordinate system 1 selection

G55

G55

G55

Workpiece coordinate system 2 selection

G56

G56

G56

Workpiece coordinate system 3 selection

14

G57

G57

G57

Workpiece coordinate system 4 selection

G58

G58

G58

Workpiece coordinate system 5 selection

G59

G59

G59

Workpiece coordinate system 6 selection

G60

G60

G60

Single direction positioning

00

G65

G65

G65

Macro calling

G66

G66

G66

Macro modal call

12

G67

G67

G67

Macro modal call cancel

G68

G68

G68

04

Mirror image for double turrets ON or balance cut mode

Coordinate system rotation start or three-dimensional coor-

G68.1

G68.1

G68.1

17

dinate system conversion mode on

Mirror image for double turrets OFF or balance cut mode

G69

G69

G69

04

cancel

Coordinate system rotation cancel or three-dimensional

G69.1

G69.1

G69.1

17

coordinate system conversion mode off

40

3. PREPARATORY FUNCTION

B-63524EN/01

PROGRAMMING

(G FUNCTION)

Table 3 G code list for T series (3/3)

G code

Group

Function

A

B

C

G70

G70

G72

Finishing cycle

G71

G71

G73

Stock removal in turning

G72

G72

G74

Stock removal in facing

G73

G73

G75

00

Pattern repeating

G74

G74

G76

End face peck drilling

G75

G75

G77

Outer diameter/internal diameter drilling

G76

G76

G78

Multiple threading cycle

G71

G71

G72

Traverse grinding cycle (for grinding machine)

Traverse direct constant-dimension grinding cycle

G72

G72

G73

01

(for grinding machine)

G73

G73

G74

Oscilation grinding cycle (for grinding machine)

Oscilation direct constant-dimension grinding cycle

G74

G74

G75

(for grinding machine)

G80

G80

G80

Canned cycle for drilling cancel

G83

G83

G83

Cycle for face drilling

G84

G84

G84

Cycle for face tapping

G86

G86

G86

10

Cycle for face boring

G87

G87

G87

Cycle for side drilling

G88

G88

G88

Cycle for side tapping

G89

G89

G89

Cycle for side boring

G90

G77

G20

Outer diameter/internal diameter cutting cycle

G92

G78

G21

01

Thread cutting cycle

G94

G79

G24

Endface turning cycle

G96

G96

G96

Constant surface speed control

02

G97

G97

G97

Constant surface speed control cancel

G98

G94

G94

Per minute feed

05

G99

G95

G95

Per rotation feed

G90

G90

Absolute programming

03

G91

G91

Incremental programming

G98

G98

Return to initial level (See Explanation 6.)

11

G99

G99

Return to R point level (See Explanation 6.)

G100

G100

G100

B axis control-Program registration completion

G101

G101

G101

B axis control-First program registration start

G102

G102

G102

00

B axis control-Second program registration start

G103

G103

G103

B axis control-Third program registration start

G110

G110

G110

B axis control-One motion operation programming

41

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

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

4.1

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

POSITIONING

rate.

(G00)

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

programmed.

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

Format

G00IP_;

IP_:

For an absolute command, the coordinates of an end

position, and for an incremental command, the distance

the tool moves.

Explanations

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

of parameter 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 the G00 command is set to the parameter

No. 1420 for each axis independently by the machine tool builder. In the

positioning 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.

43

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Examples

X

30.5

56.0

ÎÎÎ

30.0

ÎÎÎ

Î

Z

φ40.0

< Radius programming >

G00X40.0Z56.0 ; (Absolute command)

or

G00U-60.0W-30.5;(Incremental command)

Restrictions

The rapid traverse rate cannot be specified in the address F.

Even if linear interpolation positioning is specified, nonlinear

interpolation positioning is used in the following cases. Therefore, be

careful to ensure that the tool does not foul the workpiece.

D G28 specifying positioning between the reference and intermediate

positions.

D G53

44

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

4.2

Single Direction

Positioning (G60)

General

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

positioning from one direction is available.

Overrun

distance

Start

position

Start

position

Temporary

stop

End

+

position

Fig. 4.2 (a) When the positioning direction is minus

Format

G60IP_;

IP_:

For an absolute command, the coordinates of an end

position, and for an incremental command, 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 specified in the single direction positioning mode,

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

45

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

(example)

When one-shot G60 command are used

When modal G60 command is used

:

:

G90 ;

G90 G60 ;

S.D.P. mode start

G60 X0 Z0 ;

Single

X0 Z0 ;

Single

G60 X100 ;

direction

X100 ;

direction

G60 Z100 ;

positioning

Z100 ;

positioning

G04 X10 ;

G04 X10 ;

G00 X0 Z0 ;

G00 X0 Z0 ;

S.D.P. mode cancel

:

:

Summary of motion

D When the non-linear

The axes are positioned independently from start point by single direction

positioning is used

positioning as follows.

(parameter No.1401#1

LRP=0)

X

Overrun(Z-axis)

Overrun(X-axis)

End position

Z

Start position

D When the linear

The axes are positioned linear from start position to temporary stop

positioning is used

position or overrun position, and are positioned independently from

(parameter No.1401#1

temporary stop position or overrun position to end position.

LRP=1)

46

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

X

Overrun(Z-axis)

Overrun(X-axis)

End position

Z

Start position

NOTE

1

Single direction positioning is not performed in an axis for

which an overrun has not been set by the parameter

(No.5440).

2

When the move distance 0 is commanded, the single

direction positioning is not performed.

3

The mirror image does not influence direction set by the

parameter.

The direction does not change during mirror image.

4

The G-code for single direction positioning is always G60,

if G-code system is A or B or C in all case.

5

The single direction positioning can not be commanded

during the cylindrical interpolation mode (G07.1).

6

The single direction positioning can not be commanded

during the polar coordinate interpolation mode (G12.1).

7

The single direction positioning can not be commanded

during the multiple repetitive cycle (G70-G76).

8

The single direction positioning can not be commanded

during the canned grinding cycle (G71-G74).

9

No single direction positioning is effected in the drilling or

patting axis, during canned cycle for drilling (G83-G89)

and the rigid tapping (G84, G88). But the single direction

positioning is effected in the drilling or patting axis.

10

The single direction positioning can not be commanded

during the canned cycle (G90, G92, G94).

11

During the single direction positioning mode (G60), the

following G-code can not be commanded.

G07.1, G12.1, G70-G76, G90-G94.

47

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

D Notice in case of using

In the angular axis control, the distance traveled along the perpendicular

with the angular axis

axis (X) is corrected by the inclination of the angular axis (Y), and is

control.

determined by the following formula.

Xa = - Yp × tanθ

The direction of ”Xa” is determined by the inclination angle (θ) and the

direction of the motion command to the angular axis (Y). In case the value

of tanθ is plus, the motion command of the angular axis (Y) and the

corrected command of the perpendicular (X) is opposite direction. For

example, if the inclination angle is 30 degree and the motion command

is plus to the angular axis (Y), the corrected command to the perpendicular

axis (X) is minus.

+X(perpendicular axis)

move to plus direction

correct to minus direction : Xa

motion command to plus : Yp

+Y (anglar axis)

coordinate system actually used

θ (inclination angle)

program coordinate system

Therefore positioning direction may be disagree with the actual correct

direction and the positioning direction of the parameter No.5440 in the

perpendicular axis (X) in the single direction positioning with angular

axis control.

For avoiding this disagreement, please set the parameter as follows.

48

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D In case the tan value of

Please set the opposite direction between the angular axis (Y) and the

the inclination angle is

perpendicular axis

(X) into the direction of the single direction

plus. (parameter

positioning. If the positioning direction of the perpendicular axis (X) is

No.8201=1° to 89° or 181°

minus, and the positioning direction of the angular axis (Y) is plus, the

to 269°)

motion of the each axes is as follows.

+X (perpendicular axis)

Y-axis:move to plus direction

temporary stop

X-axis:correct to minus direction

motion command to plus direction

+Y (angular axis)

coordinate system actually used

θ (inclination angle)

program coordinate system

Motion command to plus direction

+X (perpendicular axis)

X-axis:correct to plus direction

motion command to minus direction

Y-axis:move to minus direction

+Y (angular axis)

coordinate system actually used

θ (inclination angle)

program coordinate system

Motion command to minus direction

49

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

D In case the tan value of

Please set the same direction between the angular axis (Y) and the

the inclination angle is

perpendicular axis

(X) into the direction of the single direction

minus. (parameter

positioning. If the positioning direction of the perpendicular axis (X) is

No.8201=91° to 179° or

plus, and the positioning direction of the angular axis (Y) is plus, the

271° to 359°

motion of the each axes is as follows.

program coordinate system

+X (perpendicular axis)

motion command to plus direction

X-axis:correct to plus direction

temporary stop

Y-axis:mov to plus direction

θ (inclination angle)

+Y (angular axis)

coordinate system actually used

Motion command to plus direction

program coordinate system

+X (perpendicular axis)

Y-axis:move to minus

direction

X-axis:correct to minus direction

motion command to minus direction

θ (inclination angle)

+Y (angluar axis)

coordinate system actually used

Motion command to minus direction

50

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Tools can move along a line.

4.3

LINEAR

INTERPOLATION

(G01)

Format

G01 IP_F_;

IP_:

For an absolute command, the coordinates of an end

point , and for an incremental command, 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.

For feed-per-minute mode under 2-axis simultaneous control, the

feedrate for a movement along each axis as follows :

G01ααββ Ff ;

Feed rate of α axis direction : Fa +a

f

L

b

Feed rate of β axis direction :

F_b +

f

L

L + a2 ) b²Ǹ

Examples

D Linear interpolation

< Diameter programming >

G01X40.0Z20.1F20 ; (Absolute command)

or

G01U20.0W-25.9F20 ; (Incremental command)

X

46.0

20.1

ÎÎ

ÎÎ

ÎÎ

End point

φ20.0

Z

φ40.0

Start point

51

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

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

4.4

CIRCULAR

INTERPOLATION

(G02, G03)

Format

Arc in the XpYp plane

G17

G02

I_J_

Xp_Yp_

F_

G03

R_

Arc in the ZpXp plane

G02

I_K_

G18

Xp_Zp_

F_

G03

R_

Arc in the YpZp plane

G02

Yp_Zp_

J_K_ F_

G19

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, radius value

J_

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

sign, radius value

k_

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

sign, radius value

R_

Arc radius with no sign (always with radius value)

F_

Feedrate along the arc

52

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

NOTE

The U-, V-, and W-axes (parallel with the basic axis) can

be used with G-codes B and C.

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

Start

j

Start

i

k

point

point

point

j

i

k

Center

Center

Center

I0, J0, and K0 can be omitted.

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

point exceeds the value in a parameter (No. 3410), an P/S alarm (No. 020)

occurs.

When X_p, Y_p , and Zp are omitted (the end point is the same as the start

D Full-circle programming

point) and the center is specified with I, J, and K, a 360° arc (circle) is

specified.

53

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

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. An arc with a sector angle of 180° or wider cannot be

specified. 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°)

G02 W60.0 U10.0 R50.0 F300.0 ;

For arc (2) (greater than 180°)

An arc with a sector angle of 180°

or wider cannot be specified

within a single block.

(2)

r=50mm

End point

(1)

Start point

r=50mm

X

Z

D Arc radius R with nine

When the option for specifying arc radius R with nine digits is selected,

digits (option)

the valid radius range for circular interpolation is expanded as follows:

Input increments

Metric input

Inch input

Incre-

IS-B

0.001 to 999999.999 mm

0.0001 to 99999.9999 inch

ment

system

IS-C

0.0001 to 99999.9999 mm

0.00001 to 9999.99999 inch

54

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

NOTE

When using the nine-digit arc radius R function, note the

following points.

1

Specifying an arc center with addresses I, K, and J

When the distance from the arc start point to the arc center

is specified with addresses I, K, and J, a P/S alarm (No.

5059) is issued if:

Ǹ

Maximum value which can be specified t I² ) K²

Example: When IS-B and metric input are selected,

issuing the following command

(radius

specification) will result in a P/S alarm

(No.

5059):

G50 X0 Z0;

G18G02X11.250 Z10. I-800000.000 K900000.000 F5.0;

MǸ

I² ) K²

+ (* 800000.000)² ) 900000.000²Ǹ

+ 1204159.458

u 999999.999

2

Tool nose radius compensation

In tool nose radius compensation mode, a P/S alarm (No.

5059) is issued if the distance from the tool nose radius

center to the arc center exceeds the maximum value which

can be specified.

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

tool nose radius compensation is applied.

Restrictions

D Simultaneously

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

specifying R with I, J,

by address R takes precedence and the other are ignored.

and K

D Specifying an axis that is

If an axis not contained in the specified plane is commanded, an alarm

not contained in the

is displayed.

specified plane

For example, when a ZX plane is specified in G-code B or C, specifying

the X-axis or U-axis (parallel to the X-axis) causes P/S alarm No. 028

to be generated.

D Difference in the radius

If the difference in the radius between the start and end points of the arc

between the start and

exceeds the value specified in parameter No. 3410, P/S alarm No. 020 is

end points

generated.

If the end point is not on the arc, the tool moves in a straight line along

one of the axes after reaching the end point.

55

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

D Specifying a semicircle

If an arc having a central angle approaching 180° is specified with R, the

with R

calculation of the center coordinates may produce an error. In such a case,

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

Examples

D Command of circular

interpolation X, Z

G02X_Z_I_K_F_;

G03X_Z_I_K_F_;

G02X_Z_R_F_;

Center of arc

End point

End point

End point

Center of arc

X-axis

X-axis

X-axis

(Diameter

R

(Diameter

(Diameter

programming)

programming)

programming)

Start point

Start point

X

X

X

Start point

Z

K

Z

Z-axis

Z

Z-axis

Z-axis

K

(Absolute programming)

(Absolute programming)

(Absolute programming)

X

R25.0

(Diameter programming)

15.0

G02X50.0Z30.0I25.0F0.3; or

ÎÎ

G02U20.0W-020.0I25.0F0.3; or

G02X50.0Z30.0R25.0F0.3 or

ÎÎ

10.0

G02U20.0W-20.0R25.F0.3;

φ50.0

Z

30.0

50.0

56

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Helical interpolation which moved helically is enabled by specifying up

4.5

to two other axes which move synchronously with the circular

HELICAL

interpolation by circular commands.

INTERPOLATION

(G02, G03)

Format

Synchronously with arc of XpYp plane

G02

G17

I_J_

Xp_Yp_

a_(b_)F_;

G03

R_

Synchronously with arc of ZpXp plane

G02

G18

I_K_

Xp_Zp_

a_(b_)F_;

G03

R_

Synchronously with arc of YpZp plane

G02

J_K_

G19

Yp_Zp_

a_(b_)F_;

G03

R_

a, b : 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.

Limitations

D Tool nose radius compensation is applied only for a circular arc.

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

which a helical interpolation is commanded.

57

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Polar coordinate interpolation is a function that exercises contour control

4.6

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 method is useful in cutting

(G12.1, G13.1)

a front surface and grinding a cam shaft on a lathe.

Format

G12.1 ;

Starts polar coordinate interpolation mode (enables

D Specify G12.1 and G13.1

polar coordinate interpolation)

in Separate Blocks.

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)

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

respectively.

Explanations

D Polar coordinate

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

interpolation plane

coordinate interpolation plane

(Fig.

4.6

(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 workpiece coordinate system

Fig. 4.6 (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.

58

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Restrictions

D Coordinate system for the

Before G12.1 is specified, a workpiece coordinate system) where the

polar coordinate

center of the rotary axis is the origin of the coordinate system must be set.

interpolation

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

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

D Tool nose radius

The polar coordinate interpolation mode cannot be started or terminated

compensation command

(G12.1 or G13.1) 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).

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

tool nose radius compensation is applied) does not move close to the

center of the workpiece.

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

∆

X

Cartesian coordinate system. As the tool moves from L1 to L2 to

θ1

L1

L3, the angle at which the tool moves per time unit corresponding

θ2

L2

to ∆X in the Cartesian coordinate system increases fromθ1 toθ 2

θ3

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

D Diameter and radius

Even when diameter programming is used for the linear axis (X-axis),

programming

radius programming is applied to the rotary axis (C-axis).

60

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

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 tool nose radius compensation

Program path

N204

N203

N205

N202

N201

N200

X axis

Tool

N208

N206

N207

Z axis

X axis is by diameter programming, C axis is by radius programming.

O0001 ;

N010 T0101

N0100 G00 X120.0 C0 Z _ ;

Positioning to start position

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 ;

N0204 G01 X-40.0 ;

Geometry program

N0205 C-10.0 ;

(program based on cartesian coordinates on

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

X-C′ plane)

N0207 G01 X40.0 ;

N0208 C0 ;

N0209 G40 X120.0 ;

N0210 G13.1 ;

Cancellation of polar coordinate interpolation

N0300 Z __ ;

N0400 X __C __ ;

N0900M30 ;

61

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

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

4.7

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

(G07.1)

amount of travel of the rotary axis.

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

G07.1 IP r ; Starts the cylindrical interpolation mode

:

(enables cylindrical interpolation).

:

:

G07.1 IP 0 ; The cylindrical interpolation mode is cancelled.

IP : An address for the rotation axis

r : Radius value of the cylinder

Specify G07.1 IP r ; and G07.1 IP 0; in separate blocks.

G107 can be used instead of G07.1.

Explanations

D Plane selection

Use parameter No. 1002 to specify whether the rotation axis is the X-, Y-,

(G17, G18, G19)

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.

NOTE

The U-, V-, and W-axes (parallel with the basic axis) can

be used with G-codes B and C.

D Feedrate

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

developed cylindrical surface.

62

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Examples

Example of a Cylindrical Interpolation Program

C

O0001 (CYLINDRICAL INTERPOLATION );

N01 G00 Z100.0 C0 ;

N02 G01 G18 W0 H0 ;

Z

R

N03 G07.1 H57299 ;

N04 G01 G42 Z120.0 D01 F250 ;

N05 C30.0 ;

N06 G03 Z90.0 C60.0 R30.0 ;

N07 G01 Z70.0 ;

N08 G02 Z60.0 C70.0 R10.0 ;

N09 G01 C150.0 ;

N10 G02 Z70.0 C190.0 R75.0 ;

N11 G01 Z110.0 C230.0 ;

N12 G03 Z120.0 C270.0 R75.0 ;

N13 G01 C360.0 ;

N14 G40 Z100.0 ;

N15 G07.1 C0 ;

N16 M30 ;

Z

mm

N0

N12

N13

120

5

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-63524EN/01

In helical interpolation, when pulses are distributed with one of the

4.8

circular interpolation axes set to a hypothetical axis, sine interpolation is

HYPOTHETICAL AXIS

enable.

INTERPOLATION

When one of the circular interpolation axes is set to a hypothetical axis,

(G07)

pulse distribution causes the speed of movement along the remaining axis

to change sinusoidally. If the major axis for threading (the axis along

which the machine travels the longest distance) is set to a hypothetical

axis, threading with a fractional lead is enabled. The axis to be set as the

hypothetical axis is specified with G07.

Format

G07 a 0; Hypothetical axis setting

G07 a 1; Hypothetical axis cancel

Where, a is any one of the addresses of the controlled axes.

Explanations

D Sine interpolation

The a axis is regarded as a hypothetical axis for the period of time from

the G07 a 0 command until the G07 a 1 command appears.

Suppose sine interpolation is performed for one cycle in the YZ plane.

The hypothetical axis is them the X axis.

X² + Y² = r² (r is the radius of an arc.)

2p

Y = r SIN (

Z )

1

1 is the distance traveled along the Z-axis in one cycle.)

Y

r

p

2p

Z

0

p

2

1

D Interlock, stroke limit,

Interlock, stroke limit, and external deceleration can also apply to the

and external

hypothetical axis.

deceleration

D Handle interrupt

An interrupt caused by the handle also applies to the hypothetical axis.

This means that movement for a handle interrupt is performed.

66

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Limitations

D Manual operation

The hypothetical axis can be used only in automatic operation. In manual

operation, it is not used, and movement takes place.

D Move command

Specify hypothetical axis interpolation only in the incremental mode.

D Coordinate rotation

Hypothetical axis interpolation does not support coordinate rotation.

Examples

D Sine interpolation

Y

10.0

Z

0

20.0

N001 G07 X0 ;

N002 G91 G17 G03 X-20.0 Y0.0 I-10.0 Z20.0 F100 ;

N003 G01 X10.0 ;

N004 G07 X1 ;

From the N002 to N003 blocks, the X-axis is set to a hypothetical axis.

The N002 block specifies helical cutting in which the Z-axis is the linear

axis. Since no movement takes place along the X axis, movement along

the Y-axis is performed while performing sine interpolation along the

Z-axis.

In the N003 block, there is no movement along the X-axis, and so the

machine dwells until interpolation terminates.

D Changing the feedrate to

(Sample program)

form a sine curve

G07Z0 ;

The Z-axis is set to a hypothetical axis.

G02X0Z0I10.0F4. ; The feedrate on the X-axis changes sinusoidally.

G07Z1 ;

The use of the Z-axis as a hypothetical axis is

canceled.

F

4.0

Xt

67

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Tapered screws and scroll threads in addition to equal lead straight threads

4.9

can be cut by using a G32 command.

CONSTANT LEAD

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

THREADING (G32)

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

is used to move the tool.

L

L

L

Fig. 4.8 (a) Straight Thread

Fig. 4.8 (b) Tapered Screw

Fig. 4.8 (c) Scroll Thread

Format

X axis

G32IP_F_;

End point

IP_: End point

F_: Lead of the long axis

(always radius programming)

δ₂

X

α

Start point

Z

δ₁

0

Z axis

L

Fig. 4.9 (d) Example of Thread Cutting

Explanations

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

cutting through finish cutting for a screw. Since thread cutting 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 thread cutting. Note that the spindle speed must

remain constant from rough cutting through finish cutting. If not,

incorrect thread lead will occur.

68

Content      ..     1      2      3      4      ..