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

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

Compensation angle +Z Q sin(P)

360 (In inch input)

p T

Where,

Compensation angle : Absolute value with sign (degrees)

: Amount of travel along the Z axis after a

G81 command is issued (mm or inch)

: Twisted angle of the gear with sign (degrees)

: Ratio of the circumference of a circle to its

diameter

: Number of teeth

: Module (mm) or diametral pitch (1/inch)

Use P, T, and Q specified in the G81 block.

D Compensation direction

Parameter HDR (bit 2 of No. 7700)

in helical gear

compensation

When the HDR bit is set to 1

(a)

(b)

(c)

(d)

C : +, Z : +, P : +

C : +, Z : -, P : +

C : +, Z : -, P : -

Compensation direction : +

Compensation direction : -

Compensation direction : +

-Z

(e)

(f)

(g)

(h)

-C

–C

-C

C : -, Z : +, P : +

C : -, Z : +, P : -

C : -, Z : -, P : +

C : -, Z : -, P : -

Compensation direction : -

Compensation direction : + Compensation direction : +

Compensation direction : -

-Z

When the HDR bit is set to 0 ((a), (b), (c), and (d) are the same as when the HDR bit is set to 1)

(e)

(f)

(g)

(h)

-C

–C

-C

C : -, Z : +, P : +

C : -, Z : +, P : -

C : -, Z : -, P : -

Compensation direction : +

Compensation direction : + Compensation direction : -

Compensation direction : +

-Z

580

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

Examples

(1) When the master axis is the spindle, and the slave axis is the C-axis

1. G81.5 T10 C0 L1 ;

Synchronization between the master axis and C-axis is started at

the ratio of one rotation about the C-axis to ten rotations about the

master axis.

2. G81.5 T10 C0 L-1 ;

Synchronization between the master axis and C-axis is started at

the ratio of one rotation about the C-axis to ten rotations about the

master axis.

In this case, however, the direction of rotation is opposite to that of

1. above.

3. G81.5 T1 C3.26 ;

Synchronization between the master axis and C-axis is started at

the ratio of a 3.26-degree rotation about the C-axis per one rotation

about the master axis.

4. G81.5 P10000 C-0.214 ;

Synchronization between the master axis and C-axis is started at

the ratio of a -0.214 degree rotation about the C-axis to 10,000

feedback pulses from the pulse coder of the master axis.

(2) When the master axis is the spindle, the slave axis is the V-axis (linear

axis), and inch/metric conversion is performed

1. For a millimeter machine and metric input

G81.5 T1 V1.0 ;

Synchronization between the master axis and V-axis is started at

the ratio of a 1.00 mm movement along the V-axis per rotation

about the master axis.

2. For a millimeter machine and inch input

G81.5 T1 V1.0 ;

Synchronization between the master axis and V-axis is started at

the ratio of a 1.0 inch movement (25.4 mm) along the V-axis per

rotation about the master axis.

(3) When two groups of axes are synchronized simultaneously

Based on the controlled axis configuration described in Fig.20.8.5,

the sample program below synchronizes the spindle with the V-axis

while the spindle is synchronized with the C-axis.

581

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

O0100 ;

N01 Mxx ;

Performs spindle orientation.

N02 G00 G90 C... ;

Positions the C-axis.

Starts synchronization at the ratio of

N03 G81.5 T10 C0 L1 ;

one rotation about the C-axis to ten

spindle rotations.

N04 Myy S300

Rotates the spindle.

N05 G01 G91 X... Y... F... ;

Makes movements for grinding.

Grinding

N06 Mzz ;

Stops the spindle.

N10 G00 G90 V... ;

Positions the dressing axis.

N11 G81.5 P12000 V0.5 ;

Starts synchronization at the ratio of a

0.5 mm movement along the V-axis

Dressing

every 12,000 pulses on the spindle.

N12 Myy S300

N20 M98 P9500 ;

Rotates the spindle.

A subprogram for dressing is called.

N21 Mzz ;

Stops the spindle.

N30 G80.5 V0 ;

Cancels V-axis synchronization.

Grinding

N31 Myy S300 ;

Rotates the spindle

N32 G01 G91 X... Y... F... ;

Makes movements for grinding

N40 Mzz ;

Stops the spindle.

N41 G80.5 C0 ;

Cancels C-axis synchronization.

V-axis synchronization mode

C-axis synchronization mode

Thus, the synchronizations of two groups can be started and canceled

independently of each other.

(4)

Command specification for hobbing machines

Based on the controlled axis configuration described in Fig.20.8.5,

the sample program below sets the C-axis (in parameter 7710) for

starting synchronization with the spindle according to the command

specification method for hobbing machines.

582

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

O1234 ;

N01 G81 T20 L1 ; Starts synchronization with the spindle and

C-axis at the ratio of a 1/20 rotation about the

C-axis to one spindle rotation.

N02 Mxx S300 ; Rotates the spindle at 300 min^-1.

N03 X... F... ;

Makes a movement along the X-axis (for

cutting).

N04 Y... F... ;

Makes a movement along the Y-axis (for

grinding). Axes such as the C-axis, X-axis,

and Y-axis can be specified as required.

N05 X... F... ;

Makes a movement along the X-axis (for

retraction).

N06 Mzz ;

Stops the spindle.

N07 G80 ;

Cancels the synchronization between the

spindle and C-axis.

D Synchronization Ratio

The programmed ratio (synchronization ratio) of a movement along the

Specification Range

slave axis to a movement along the master axis is converted to a detection

unit ratio inside the NC. If such converted data (detection unit ratio)

exceeds a certain allowable data range in the NC, synchronization cannot

be established correctly, and an alarm (P/S 181) is issued.

Even when a programmed master axis movement and a programmed

slave axis movement are within specifiable ranges, a detection unit ratio

obtained by conversion can exceed the allowable range, thus resulting in

an alarm.

Let K be a synchronization ratio. The internal data corresponding K is the

amount of slave axis movement (Kn) represented in the detection unit

divided by the amount of master axis movement (Kd) represented in the

detection unit; this fraction is represented as Kn/Kd (reduced to its lowest

terms) as indicated below.

mount of slave axis movement represented in the detection unit

K+

Kd⁺Amount of master axis movement represented in the detection unit

Kn and Kd must lie within the following ranges:

-2147483648

v Kn v 2147483647

v Kd v 65535

When Kn or Kd exceeds its allowable range above, an alarm is issued.

In conversion to the detection unit, when the CMR

(command

multiplication: parameter 1820) is a fraction or when inch/millimeter

conversion is used, the fraction is directly converted without modification

so that no error can occur in the conversion of specified amounts of

movement.

During conversion, the amount of movement is multiplied by 254/100 for

inch input on a millimeter machine, and 100/254 for metric input on an

inch machine. Thus, Kn and Kd can become large numbers. If a

synchronization ratio cannot be reduced to its lowest terms, an alarm

condition is likely to occur.

583

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

D Example 1)

Based on the controlled axis configuration described in Fig.20.8.5,

suppose that the spindle and V-axis are as follows:

Spindle pulse coder

72000pulse/rev (4 pulses for

one A/B phase cycle)

C-axis least command increment : 0.001 degree

C-axis CMR

V-axis least command increment : 0.001mm

V-axis CMR

Then, the C-axis detection unit is 0.0002 degree. The V-axis detection

unit is 0.0002 mm. In this case, the synchronization ratio (Kn, Kd) is

related with a command as indicated below. Here, let Pm and Ps be the

amounts of movements represented in the detection unit on the master

axis and slave axis specified in a synchronization start command,

respectively.

(1) When the master axis is the spindle, and the slave axis is the C-axis

(a)

Command : G81.5 T10 C0 L1 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of one rotation about the C-axis

to ten spindle rotations.

(Number of pulses per spindle rotation)

rotations → 72000

(Amount of movement per rotation about the

C-axis)

CMR

(one rotation) → 360000

60000

Kd+3

72000

Both Kn and Kd are within the allowable range. No alarm is output.

(b)

Command : G81.5 T10 C0 L-1 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of one rotation about the C-axis

to ten spindle rotations.

In this case, however, the direction of rotation is

opposite to that of (a) above.

(Number of pulses per spindle rotation)

revolutions → 72000

(Amount of movement per rotation about the

C-axis)

CMR

(one rotation) → -360000

360000

+*5

Kd^+*

72000

Both Kn and Kd are within the allowable range. No alarm is

output.

(c)

Command : G81.5 T1 C3.263 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of a 3.263-degree rotation about

the C-axis to one spindle rotation.

(Number of pulses per spindle rotation)

1 rotation

→ 72000

(Amount of C-axis movement) CMR → 3263

263

Kd+73

2000

14400

584

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

Both Kn and Kd are within the allowable range. No alarm is

output.

In this sample program, when T1 is specified for the master axis,

the synchronization ratio (fraction) of the CMR of the C-axis to

the denominator Kd can always be reduced to lowest terms, thus

Kd falls in the allowable range. So, the specifiable range of C is

as follows:

-99999999 v C v 99999999

(d)

Command : G81.5 T10 C3.263 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of a 3.263-degree rotation about

the C-axis to ten spindle rotations.

(Number of pulses per spindle rotation)

rotations → 72000

(Amount of the C-axis movement) CMR →

3263

263

Kd⁺72000

10+1

4400

In this case, an alarm is issued because Kd exceeds the specifiable

range.

(e)

Command : G81.5 P10000 C-0.214 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of a -0.214 degree rotation of the

C-axis to 10,000 feedback pulses from the pulse

coder of the spindle.

(Specified number of feedback pulses from the pulse

coder of the spindle) → 10000

(Amount of C-axis movement) CMR → -214

214

+*107

Kd^+*10000

1000

Both Kn and Kd are within the allowable range. No alarm is

output.

(2) When the master axis is the spindle, the slave axis is the V-axis (linear

axis), and inch/metric conversion is performed

(a) For a millimeter machine and metric input

Command : G81.5 T1 V1.0 ;

Operation

: Synchronization between the spindle and V-axis is

started at the ratio of a 1.00 mm movement along

the V-axis per spindle rotation.

(Number of pulses per spindle rotation)

rotation → 72000

(Amount of V-axis movement) CMR → 1000

000

Kd+1

72000

Both Kn and Kd are within the allowable range. No alarm is

output.

(b) For a millimeter machine and inch input

Command : G81.5 T1 V1.0 ;

Operation

: Synchronization between the spindle and V-axis is

started at the ratio of a 1.0 inch movement (25.4

mm) along the V-axis per spindle rotation.

(Number of pulses per spindle rotation)

revolution → 72000

585

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

(Amount of V-axis movement) CMR

254 B

100 → 10000

254 B 100

0000

254

127

Kd+1

72000

100

Both Kn and Kd are within the allowable range. No alarm is

output.

Command : G81.5 T1 V0.0013 ;

Operation

: Synchronization between the spindle and V-axis is

started at the ratio of a 0.0013 inch (0.03302 mm)

movement along the V-axis per spindle rotation.

(Number of pulses per spindle rotation)

rotation → 72000

(Amount of V-axis movement) CMR

254 B

100 → 13

254 B 100

254

1651

Kd+1

72000

100

720000

In this case, an alarm is issued because Kd exceeds the specifiable

range.

D Example 2)

Based on the controlled axis configuration described in Fig.20.8.5,

suppose that the spindle and V-axis are as follows:

Spindle pulse coder

72000 pulse/rev (4 pulses for

one A/B phase cycle)

C-axis least command increment : 0.001 degree

C-axis CMR

1/2

V-axis least command increment : 0.001mm

V-axis CMR

1/2

Then, the C-axis detection unit is 0.002 degree. The V-axis detection

unit is 0.002 mm. In this case, the synchronization ratio (Kn, Kd) is

related with a command as indicated below. Here, let Pm and Ps be

the amounts of movements represented in the detection unit for the

master axis and slave axis specified in a synchronization start

command, respectively.

(1) When the master axis is the spindle, and the slave axis is the C-axis

(a) Command : G81.5 T1 C3.263 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of a 3.263-degree rotation about

the C-axis per spindle rotation.

(Number of pulses per spindle rotation)

rotation → 72000

(Amount of C-axis movement) CMR → 3263

1 B 2

263

Kd+73

2000

7200

In this case, an alarm is issued because Kd exceeds the specifiable

range.

(b) Command : G81.5 T1 C3.26 ;

Operation

: Synchronization between the spindle and C-axis is

started at the ratio of a 3.26-degree rotation about

the C-axis per spindle rotation.

(Number of pulses per spindle rotation)

1 revolution → 72000

586

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

(Amount of C-axis movement) CMR

→ 3260

1 B 2

260

Kd+73

2000

7200

(a) causes an alarm to be output because the values cannot be

abbreviated. (b) causes no alarm because the ratio of the travel

distances can be abbreviated to a simple ratio.

D Retraction function

When retract signal RTRCT is set to 1 (on the rising edge of the signal),

retraction is performed according to the retract value set in parameter No.

7741 and the feedrate set in parameter No. 7740.

The tool does not move along an axis for which the amount of retraction

is set to 0.

After retraction, retraction completion signal RTRCTF is output.

CAUTION

Retract operation is performed at the feedrate specified in

parameter No. 7740.

Feed hold cannot be applied to retraction.

In this case, the feedrate override capability is disabled.

NOTE

When the retract signal goes on during automatic operation,

retract operation is performed, and automatic operation is

stopped.

Automatic operation cannot be performed in retraction.

D Notes on parameter

Note the following points when specifying parameters for the electronic

settings

gear box.

1. Arrange the controlled axes such that a slave axis appears before a

dummy axis.

(Example)

Example of incorrect setting

Example of correct setting

Servo axis

Axis name

number

Axis name

number

(No.1023)

C (dummy axis)

C (slave axis)

C (dummy axis)

2. Do not use a name which is usually not allowed to be used as an axis

address, such as D.

3. Specify the same values for an EGB slave axis and an EGB dummy

axis in the following parameters.

587

20. AXIS CONTROL FUNCTIONS

PROGRAMMING

B-63534EN/02

1004#7

Ten times minimum input increment

1001#0

Inch/metric switching (rotation axis/linear axis)

1006#1

Shape of machine coordinate system (rotation axis/linear

axis)

1006#2

Shape of machine coordinate system for pitch error

compensation (rotation axis/linear axis)

1420

Rapid traverse rate

1421

Rapid-traverse override F0 speed

1820

Command multiplication

Specify the amount of travel per rotation about a rotation axis for a

slave axis in a parameter No. 1260.

Make the specification for a dummy axis in the following way.

1815#1

Whether to use separate detectors. Although an EGB

dummy axis uses the interface of a separate detector, set

these parameters to 0.

If the following parameters are not specified, an alarm (SV 417 servo

parameter invalid) may be generated. In such a case, make the

specification as described below.

20XX

Specify the same value for both a slave axis and a

dummy axis.

2084, 2085

Flexible feed gear.

Set parameters Nos. 2084 and 2085 to 1 for the

dummy axis.

Specify as large a feed-forward coefficient as possible to reduce the

synchronization error. For details of parameter setting, see Feed-forward

setting of Geometric error suppression function in FANUC AC SERVO

MOTOR αi series Parameter Manual (B-65270EN) or FANUC AC

SERVO MOTOR α series Parameter Manual (B-65150EN).

588

B-63534EN/02

PROGRAMMING

20. AXIS CONTROL FUNCTIONS

Alarms

Num-

Message

Contents

ber

P/S 181

FORMAT ERROR IN

Format error in the block in which EGB

G81 BLOCK

was specified

(1) The axis during synchronization by

EGB is specified by G81.5 again.

(2) U-axis is specified by G81.5/G80.5

with U-axis control.

(3) Format error in the block in which

G81.5/G80.5 was specified.

⋅ Data is specified to more than 2

slave axes in one block. Or noth-

ing is specified to the slave axis.

⋅ Data specified to the slave axis is

neither ‘b0 Lxx’ nor ‘bxx’.

⋅ Data is specified to more than 2

master axes in one block.

⋅ Data is specified to the axis which

is neither the master nor the slave

axis.

⋅ One of T, P or a codes is specified

redundantly.

⋅ Out of range data is specified by

one of T or L codes

⋅ An overflow occurred during cal-

culation of the synchronization co-

efficient.

P/S 184

ILLEGAL COMMAND

An illegal instruction was issued during

IN G81

synchronization by EGB.

(1) Slave axis was specified by G00,

G27, G28, G29, and G30 G codes.

(2) Inch/metric conversion was speci-

fied by G20 or G21 G codes.

P/S 186

PARAMETER SETTING

Erroneous EGB parameter setting

ERROR

The number of pulses (parameter Nos.

7782, 7783) per rotation is not set.

589

21. TWO-PATH CONTROL

B-63534EN/02

PROGRAMMING

FUNCTION

The two-path control function is designed for use on a machining center

21.1

where two systems are operated independently to simultaneously perform

GENERAL

cutting.

D Controlling two path

The operations of two path are programmed independently of each other,

independently at the

and each program is stored in program memory for each path. When

same time

automatic operation is to be performed, each path is activated after

selecting a program for machining with path 1 and a program for

machining with path 2 from the programs stored in program memory for

each path. Then the programs selected for the paths are executed

independently at the same time. When path 1 and path 2 need to wait for

each other during machining, the waiting function is available (Section

21.2)

Just one MDI is provided for the two paths. Before operation and display

on the MDI, the path selection signal is used to switch between the two

paths.

Transfer Line

Machining center (Left)

Transport device

Machining center (Right)

CNC

2-path control

WARNING

Simultaneous operation of the two paths or the operation of

only a single tool post can be selected by pressing a key on

the machine operator’s panel. For details, refer to the

manual supplied by the machine tool builder.

591

21. TWO-PATH CONTROL

FUNCTION

PROGRAMMING

B-63534EN/02

21.2

WAITING FOR PATHS

Explanations

Control based on M codes is used to cause one path to wait for the other

during machining. By specifying an M code in a machining program for

each path, the two paths can wait for each other at a specified block. When

an M code for waiting is specified in a block for one path during automatic

operation, the other path waits for the same M code to be specified before

staring the execution of the next block. This function is called the paths

waiting function.

A range of M codes used as M codes for waiting is to be set in the

parameters (Nos. 8110 and 8111) before hand.

Example

M100 to M103 are used as M codes for waiting.

Parameter setting:No. 8110=100

(Minimum M code for waiting: M100)

No. 8111=103

(Maximum M code for waiting: M103)

Path 1 program

Path 2 program

01357 ;

02468 ;

G50 X Z ;

G00 X Z T0101 ;

G00 X Z T0202 ;

S1000 M03 ;

S2000 M03 ;

M100 ;

Waiting

N1100 G01 X Z F

;

N2100 G01 X Z F

;

Simultaneous,

N2199

;

independent operation

M101 ;

of path 1 (N1100 to

N1199) and path 2

(N2100 to N2199)

N1199

;

M101 ;

M102 ;

Waiting

N2200 S3000 ;

G00 X Z T0202 ;

Operation of path 2

(N2200 to N2299)

only

N2299

;

M102 ;

Waiting

N1300

;

Simultaneous,

N2300

;

G00 X Z T0505 ;

G00 X Z T0707 ;

independent operation

of path 1 (N1300 to

N1399) and path 2

(N2300 to N2399)

N1399

;

N2399

;

M103 ;

Waiting

M30 ;

End of program

592

21. TWO-PATH CONTROL

B-63534EN/02

PROGRAMMING

FUNCTION

NOTE

An M code for waiting must always be specified in a single block.

If one path is waiting because of an M code for waiting specified, and a different M code for

waiting is specified with the other path, an P/S alarm (No. 160) is raised, In this case, both paths

stop operation.

PMC-CNC interface

Unlike other M codes, the M code for waiting is not output to the PMC.

4 Operation of a single path

If the operation of a single path is required, the M code for waiting need not be deleted. By using

the NOWT signal to specify that waiting be ignored (G0063, #1), the M code for waiting in a

machining program can be ignored. For details, refer to the manual supplied by the machine

tool builder.

593

21. TWO-PATH CONTROL

FUNCTION

PROGRAMMING

B-63534EN/02

A machine with two paths have different custom macro common

21.3

variables and tool compensation memory areas for path 1 and 2. Paths 1

MEMORY COMMON

and

2 can share the custom macro common variables and tool

TO PATH

compensation memory areas provided certain parameters are specified

accordingly.

Explanations

D Custom macro common

Paths 1 and 2 can share all or part of custom macro common variables

variables

#100 to #149 and #500 to #531, provided parameters 6036 and 6037 are

specified accordingly.

(The data for the shared variables can be written

or read from either path.) See Section 15.1 of Part II.

594

21. TWO-PATH CONTROL

B-63534EN/02

PROGRAMMING

FUNCTION

21.4

In a CNC supporting two-path control, specified machining programs

can be copied between the two paths by setting bit 0 (PCP) of parameter

COPYING A

No. 3206 to 1. A copy operation can be performed by specifying either

PROGRAM

a single program or a range. For information about operations, see

BETWEEN TWO

Section 9.10 in Part III.

PATHS

Explanations

D Single-program copy

Copy source number

0001

Copy destination number

: Not set

Copy source

Copy destination

O0001

Copy source number

0001

Copy destination

0010

Copy source

Copy destination

O0001

O0010

D Specified-range copy

Copy source number

0001 to 0100

Copy destination number

: Not set

Copy source

Copy destination

O0001

O0010

O0100

O1000

O2000

Copy source number

0001 to 0100

Copy destination

1000

Copy source

Copy destination

O0001

O1000

O0010

O1001

O0100

O1002

O1000

O2000

595

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

RISC PROCESSOR

General

The following functions are executed at high speed with RISC processor.

D AI high precision contour control

D AI NANO high precision contour control

D Cylindrical interpolation cutting point control

D Tool center point control

D Tool axis compensation in tool axis direction

D 3-dimensional cutter compensation

D 3-dimensional circular interpolation

Expansion of RISC

The parameter(No.19600#0-#5) setting expands the following functions

commnd

which is executed with RISC processor.

5-axis control mode

function

mode ON

mode OFF

G51

G50

Scaling

G51.1

G50.1

Programmable mirror image

G54.2 Pn

G54.2 P0

Rotary table dynamic fixture offset

(n=1-8)

G68

G69

Coordinate system rotation

G68 I_J_K_

G69

3-dimensional coordinate system

conversion

G41,G42

G40

Cutter compensation C

AI high precision contour control, AI NANO high precision contour

control, Tool center point control, Tool axis compensation in tool axis

direction,

3-dimensional cutter compensation and

3-dimensional

circular interpolation can be used in the mode of above mentioned

functions when the above mentioned function is set to be executed with

RISC processor.

Please refer to paragraph of restrictions for the restriction in this case.

AI high precision contour control, AI NANO high precision contour

control, Tool center point control, Tool axis compensation in tool axis

direction,

3-dimensional cutter compensation and

3-dimensional

circular interpolation can be used only when the state of the above

mentioned functions is canceling when the above mentioned function is

set to be executed with CNC.

The alarm(P/S5012) occurs if AI high precision contour control, AI

NANO high precision contour control, Tool center point control, Tool

axis compensation in tool axis direction,

3-dimensional cutter

compensation and 3-dimensional circular interpolation is used when the

state of the above mentioned function is not canceling.

596

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

5-axis control mode

The state to execute the each function of AI high precision contour

control, AI NANO high precision contour control, Tool center point

control, Tool axis compensation in tool axis direction, 3-dimensional

cutter compensation and

3-dimensional circular interpolation is

generically called five axis control mode.

The function set in the expansion of RISC command is included, too.

Restriction -1

The following commands can not be used in the AI High Precision

Contour Control mode or AI NANO High Precision Contour Control

mode. The alarm is issued if the function was used.

Custom macro

Exponential interpolation

-G02.3,G03.3

Dwell

-G04

High Speed Cutting Function relation

-G05

(G05P10000 and G05P0 are excluded)

AI contour control

-G05.1Q1,G5.1Q0

Hypothetical axis interpolation

-G07

Advanced preview control

-G08

(Please use AI High Precision Contour Control)

Polar coordinate interpolation

-G12.1,G13.1

Polar coordinate command

-G15,G16

Reference position return check

-G27

Reference point return

-G28

2nd. Reference point return

-G30

3rd/4th reference point return

-G30

Skip

-G31

Thread cutting

-G33

Automatic tool length measurement

-G37

Normal direction control

-G40.1,G41.1,G42.1

Cutter compensation B

-G41,G42,G39

(Cutter compensation C is available)

3-dimensional tool compensation

-G41

Wheel wear compensation

-G41

Tool offset

-G45,G46,G47,G48

Local coordinate system

-G52

Machine coordinate system

-G53

Single direction positioning

-G60

Automatic corner override

-G62

Tapping mode

-G63

Macro call

-G65,G66,G67

(SubProgram call is available)

Figure copying

-G72.1,G72.2

Simple electric gear box

-G80,G81

Functions for hobbing machine

-G80,G81

597

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

S External operation function

-G81

S Chopping function

-G81.1

S Setting a workpiece coordinate system

-G92

S Workpiece coordinate system preset

-G92.1

S Feed per revolution

-G95

S Constant surface speed control

-G96,G97

S Infeed control

-G160,G161

Restriction -2

The following functions can not be used in the AI High Precision Contour

Control mode, the AI NANO High Precision Contour Control mode or

the 5-axis control mode.

S Flexible synchronous control

S Sequence number comparison and stop

It is not possible to stop by the sequence number in the AI High

Precision Contour Control mode , in the AI Nano High Precision

Contour Control mode or in the 5-axis control mode.

S Index table indexing

S Retrace function

Do not use retrace function in the program which uses the AI

High Precision Contour Control mode or the AI Nano High

Precision Contour Control or 5-axis control mode.

S Rotary axis control

S Gentle curve normal direction control

S Tool life management

Tool life value is counted in the AI High Precision Contour

Control mode or in the AI Nano AI High Precision Contour

Control mode. However , do not use the command related to the

tool life management function.

S Macro executor (Execution macro)

S Manual handle interruption

S Feedrate change of F1 digit feed by manual pulse generator

S External deceleration (External deceleration is not aviailable )

Restriction -3

The following commands can not be used in the 5-axis control mode. The

alarm is issued if the function was used.

- M,S,T and B function with motion command

- NURBS interpolation

-G06.2

– Workpiece coordinate system

-G54-G59, G54.1

– Canned cycle

-G73 to G79,

G80 to G89,G98,G99

- Manual interruption operaton

- Tool retract and recover

Restriction -4

In the 5-axis control mode, the following functions cannot be used, The

warning message is displayed on the screen when the following functions

are used. :

598

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

– MDI intervention

Restriction -5

When the following function is used, the function which executed with

RISC processor cannot be used.

S Angular axis control

S Arbitary angular axis control

Restriction -6

The following modal G code are placed in the cleared state when the reset

is executed in AI high precision contour control mode , AI NANO high

precision contour control mode or 5-axis control mode,

[Modal status]

[Clear status]

–

3-dimensional circular

-G02.4/G03.4

-G00 or G01

interpolation

NURBS interpolation

-G06.2

-G00 or G01

–

Cutter compensation C

-G41/G42

-G40

–

3-dimensional cutter

-G41.2,G42.2,G41.3 -G40

compensation

Tool axis compensation

in tool axis direction

-G43.1

-G49

–

Tool center point control

-G43.4

-G49

–

Scaling

-G51

-G50

–

Programmable mirror

-G51.1

-G50.1

image

Rotary table dynamic

-G54.2Pn

-G54.2P0

fixture offset

Coordinate system

-G68

-G69

rotation

3-dimensional coordinate -G68

-G69

conversion

(The alarm(P/S5453) occur when the program is restart after reset is

executed if the parameter D3R(No.5400#2) =1 in 3-dimensional

coordinate system conversion mode.

This alarm can be canceled by both <RESET> key and <CAN> key

operations pushed at the same time.)

Restriction -7

The alarm (P/S5000) occurs if, in any of the following modes, an attempt

is made to issue a command that will cause the system to enter 5-axis

control mode (tool center point control, tool axis compensation in tool

axis direction,

3-dimensional cutter compensation,

3-dimensional

circular interpolation, or a function expanded with bits 0 to 5 of parameter

No. 19600 to be executed on a RISC processor).

S Advanced preview control

S AI contour control

S AI namo contour control

Restriction -8

The limitation may be attached about the combination of the NC

instructions occasionaly. Refer the description of the each functions.

599

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

The Function list which

can be used

Item

Specifications

Note

Axis control

Controlled axes

3 axes

Controlled paths

1-path

Simultaneously controlled axes

2 axes

Controlled axis expansion

Up to 8 axes

Simultaneously controlled axis expan-

Up to 6 axes

sion

Axis control by PMC

The axis which is used in the AI High

Precision Contour Control mode or in

the AI nano High Precision Contour

Control mode can not be used as the

control axis of the PMC Axis Control in

the AI High Precision Contour Control

mode or in the AI nano High Precision

Contour Control mode

Cs contour control

The nano interpolation and the Ad-

vanced preview feed-forward function

are canceled once when the command

for Cs axis in AI high precision contour

control mode or AI nano high precision

contour control mode

Axis name

3 basic axes: X,Y,Z; Additional axes:

U,V,W,A,B, or C

Twin table control

Synchronized operation/individual op-

eration/a normal drive cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode

Please include all the twin table control

axes to the maximum control axis

number (parameter No.7510) of RISC.

Simple synchronous control

Synchronized operation/individual op-

eration/a normal drive cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode

Please include all the simple synchro-

nous control axes to the maximum

control axis number (parameter

No.7510) of RISC.

Least input increment

0.001mm,0.001deg,0.0001inch

Incremental System 1/10

0.0001mm,0.0001deg,0.00001inch

Inch/metric conversion

Inch mode / metric mode cannot be

changed in the AI high precision con-

tour control mode or in the AI nano

high precision contour control mode.

600

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Axis control

Interlock

All axes/each axis

Machine lock

All axes/each axis

Emergency stop

Stored stroke check 1

The stroke limit cannot be set by the

stroke limit external setting signal in the

AI high precision contour control mode

or in the AI nano high precision contour

control mode. Overrun on the OT limit

does not occur in the AI high precision

contour control mode or in the AI nano

high precision contour control mode.

Stored stroke check 2

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if G22 or G23 is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode,

Mirror image

Do not change the state of the signal in

the AI High Precision Contour Control

mode or AI nano High Precision Con-

tour Control mode.

Backlash compensation for each rapid

traverse and cutting feed

Operation

Automatic operation

MDI operation

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if the MDI operation is used in

the AI high Precision Contour Control

mode or in the AI high Precision Con-

tour Control mode. At this time,

G05P10000 or G05P0 can not be used

by the MDI operation.

Cycle start/Feed hold

Program stop/Program end

Reset

Program restart

Program restart function is performed

with folowing functions:

NURBS interpolation, and Cylindrical

intyerpolation

Dry run

Single block

601

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Interpolation functions

Positioning

G00

The AI high precision contour control

function or AI nano high precision con-

tour control functions except the ad-

vanced preview feed-forward function

, multi buffer function , and the nano

interpolation become invalid.

Cutting mode

G64

Linear interpolation

G01

Circular interpolation

G02,G03

Helical interpolation

(Circular interpolation) + (Linear inter-

polation for up to 2 axes)

Helical interpolation B

(Circular interpolation) + (Linear inter-

polation for up to 4 axes)

Involute interpolation

G02.2,G03.2

3-dimensional circular interpolation

G02.4,G03.4

The position is checked at the end

point of the block which cancel 3 di-

mensional circular interpolation or at

the end point of the previous block of

the 3 dimensional circular interpolation

if 3 dimensional circular interpolation is

used except in AI high precision con-

tour control mode or AI nano high pre-

cision contour control mode.

Smooth interpolation

G05.1

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

NURBS interpolation

G06.2

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

Cylindrical interpolation

G07.1

This function can be used in AI high

precision contour control mode or AI

nano high precision contour control

mode.

Cylindrical interpolation cutting point

G07.1

This function can be used in AI high

control

precision contour control mode or AI

nano high precision contour control

mode.

Conical / spiral interpolation

G02,G03

Feed functions

Feed per minute

G94

Cutting feedrate clamp

Linear acceleration/deceleration of cut-

ting feed after interpolation

602

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Feed functions

Bell-type acceleration/deceleration of

cutting feed after interpolation

Feedrate override

0 to 254%

(1% step)

2nd. Feedrate override

0 to 254%

(1% step)

F1 digit feed

Using the manual pulse generator can

not change Feedrate.

Inverse time feed

G93

Look-ahead liner-type acceleration/

deceleration before interpolation.

Look-ahead bell-type acceleration/

Acceleration change time constant

deceleration before interpolation

type

AI high-precision contour control

AI nano high-precision contour contreol

Program input

Tape code

Automatic recognition of EIA/ISO

Program format

Word address format

Control in/out

Optional block skip

Absolute/incremental programming

G90/G91

Input unit 10 time multiply

Plane selection

G17,G18,G19

Rotary axis roll over

Workpiece coordinate system selec-

G54 to G59

The AI high precision contour control

tion

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Addition of workpiece coordinate sys-

48 sets / 300 sets

The AI high precision contour control

tem pair

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Manual absolute ON/OFF

603

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Program input

Programmable parameter input

G10

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

External memory and sub program

M198

calling function

Subprogram call

M98

Circular interpolation by R program-

ming

Scaling

G50,G51

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in scaling mode by set-

ting the parameter.

The alarm (P/S5012) occurs if the

mode of AI high precision contour con-

trol or of AI nano high precision con-

tour control is changed in scaling mode

(G51) when the parameter is not set.

The scaling mirror image by a negative

magnification can not be done.

Coordinate system rotation

G68,G69

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in coordinate system

rotation mode by setting the parameter.

The alarm (P/S5012) occurs if the

mode of AI high precision contour con-

trol or of AI nano high precision con-

tour control is changed in coordinate

system rotation mode (G51) when the

parameter is not set.

3-dimensional coordinate system con-

G68,G69

The mode of AI high precision contour

version

control or of AI nano high precision

contour control is permitted to change

ON and OFF in 3-dimensional coordi-

nate system conversion mode by set-

ting the parameter. The alarm

(P/S5012) occurs if the mode of AI

high precision contour control or of AI

nano high precision contour control is

changed in 3-dimensional coordinate

system conversion when the parame-

ter is not set.

604

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Item

Specifications

Note

Miscellaneous/spindle functions

Miscellaneous function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

2nd. Auxiliary function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

1 block plural M commands

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

It is possible to command up to 3.

Spindle speed function

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Tool functions

Tool function (T8-digit)

The AI high precision contour control

mode or the AI nano high precision

contour control mode is automatically

canceled once and the buffering is in-

hibited if this function is used in the AI

high Precision Contour Control mode

or in the AI high Precision Contour

Control mode.

Tool length compensation

G43

Cutter compensation

G38,G39,G40,G41,G42

The buffering is inhibited when the

command which automatically cancel

AI high precision contour control mode

or AI nano high precision contour con-

trol mode is used.

So the tool offset vector is held.

605

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Item

Specifications

Note

Tool functions

3-dimensional tool compensation

G41.2,G42.2

The command which automatically

G41.3

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Tool axis direction tool length com-

G43.1

The command which automatically

pensation

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Tool center point control

G43.4,G43.5

The command which automatically

cancel AI high precision contour con-

trol mode or AI nano high precision

contour control mode can not be used.

However M,S,T and B command can

be used without the command that

move some axes. In this case, the off-

set vector is held because the buffer-

ing is inhibited.

Rotary table dynamic fixture offset

G54.2

The mode of AI high precision contour

control or of AI nano high precision

contour control is permitted to change

ON and OFF in rotary table dynamic

fixture offset mode by setting the pa-

rameter. The alarm (P/S5012) occurs if

the mode of AI high precision contour

control or of AI nano high precision

contour control is changed in rotary

table dynamic fixture offset mode when

the parameter is not set.

606

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

22.1

AI HIGH PRECISION

CONTOUR CONTROL/

AI NANO HIGH

PRECISION CONTOUR

CONTROL

General

This function is designed to achieve high-speed, high-precision

machining with a program involving a sequence of very small straight

lines and NURBS curved lines, like those used for metal die machining.

This function can suppress the servo system delay and delay caused by

acceleration/deceleration that increase as a higher feedrate is used.

This function can be used to ensure that the tool strictly traces the

specified values, thus minimizing machining profile errors and achieving

high-speed, high-precision machining.

HPCC stands for high precision contour control. In AI High Precision

Countour Control mode, acceleration/deceleration is performed more

precisely than in the conventional HPCC mode, resulting in an increase

in the cutting speed.

AI Nano High Precision Countour Control can use the Nano interpolation

with all functions of AI High Precision Countour Control.

The output from the NC to the servo is usually in units of detection units.

This function allows output to the servo in units of thousandths of

detection units, thereby improving machining precision. This is

particularly effective for improving the surface roughness.

Note that the positioning precision depends on the machine conditions,

such as the resolution of the detector.

AI Nano High Precision Countour Control is the same as a AI High

Precision Countour Control excluding being able to use the Nano

interpolation.

In the following explanations, only AI High Precision Countour Control

is described.

Format

The following command turns AI high precision contour control mode on

and off.

In AI high precision contour control mode, ”AI HPCC” flashes at the

lower right corner of the screen.

In AI nano high precision contour control mode, ”NANO HP” flashes.

G05 P10000

: AI High Precision Countour Control mode on

G05 P0

: AI High Precision Countour Control mode off

Specify G05 alone in a block.

Functions enabled

In AI High Precision Countour Control mode, the following functions are

enabled:

Thus, this function can be used to ensure that the tool strictly traces the

specified values, thus minimizing machining profile errors for

higher-speed, higher-precision machining.

607

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

(1) Linear acceleration/deceleration before interpolation or bell-shaped

acceleration/deceleration before interpolation

(Acceleration change time constant type)

(2) Deceleration function based on feedrate differences at corners

(3) Advanced feed-forward function

(4) Feedrate determination based on acceleration on each axis

(5) Deceleration function based on Z-axis fall angle

(6)

200-block multi-buffer function

22.1.1

Look-ahead

Acceleration/Decelerati

on Before Interpolation

Acceleration/

There are two types of acceleration/deceleration, the linear

deceleration types

acceleration/deceleration type and the bell-shaped acceleration/

deceleration type. When bit 7(BDO) and bit 1(NBL) of parameter

No.8402 is set to 1 or bit 3(RSB) of parameter No.1603 is set to 1,

bell-shaped acceleration/deceleration is assumed.

Bell-shaped

acceleration / deceleration produces smoother acceleration / deceleration.

Look-ahead linear

acceleration/deceleration

before interpolation

D Example of deceleration

Deceleration starts in advance so that the feedrate specified for a block can

be attained when the block is executed.

Feedrate

Programmed speed

Feedrate obtained by

acceleration/

deceleration

beforeinterpolation

Time

To decrease the feedrate from F3 to F2, deceleration must be started from

P1.

To decrease the feedrate from F2 to F1, deceleration must be started from

P2.

Because multiple blocks are read in advance, deceleration can be

performed over all those blocks.

608

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

D Example of acceleration

Acceleration is performed so that the feedrate specified for a block is

attained when the block is executed.

Feedrate

Programmed speed

Feedrate obtained by

acceleration/

deceleration

beforeinterpolation

Time

Look-ahead bell-shaped If “1” is set to bit 7(BDO) and bit 1(NBL) of parameter No.8402 or bit

3(RSB) of parameter No.1603, bell-shaped acceleration/deceleration is

acceleration/deceleration

applied as the acceleration/deceleration before interpolation.

before interpolation

D Setting an acceleration

A permissible acceleration for the linear acceleration/deceleration of each

axis is set in parameter 19510. Acceleration change time (B) (period of

transition from constant speed state

(A) to constant acceleration/

deceleration state (C)) is set in parameter 8416 (common to all axes). In

the constant acceleration/deceleration state (C), acceleration/deceleration

is performed with the maximum tangential acceleration not exceeding the

permissible acceleration of each axis specified in parameter 19510.

The acceleration change time specified in parameter

8416 is held

constant, regardless of the tangential acceleration.

Tangential feedrate

An optimum gradient is automatically

calculated from the setting made in

parameter 19510.

(A)

(B)

(C)

(B)

(A)

(B)

(C)

(B)

(A)

Time set in parameter 8416

609

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 21