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

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Tapered thread

αx45° lead is LZ

αy45° lead is LX

Fig. 4.9 (e) LZ and LX of a Tapered Thread

In general, the lag of the servo system, etc. will produce somewhat

incorrect leads at the starting and ending points of a thread cut. To

compensate for this, a threading length somewhat longer than required

should be specified.

Table 4.9 lists the ranges for specifying the thread lead.

Table. 4.9 Ranges of lead sizes that can be specified

Least command increment

mm input

0.0001 to 500.0000mm

Inch input

0.000001 inch to 9.999999inch

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Explanations

1. Straight thread cutting

The following values are used in programming :

Thread lead :4mm

δ₁=3mm

δ₂=1.5mm

X axis

30mm

Depth of cut :1mm (cut twice)

(Metric input, Diameter programming)

δ₂

δ₁

G00

U-62.0 ;

G32

W-74.5 F4.0 ;

Z axis

G00

U62.0 ;

W74.5 ;

U-64.0 ;

(For the second cut, cut 1mm more)

G32 W-74.5 ;

G00

U64.0 ;

W74.5 ;

2. Tapered thread cutting

The following values are used in programming :

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

δ₁=2mm

δ₂=1mm

X axis

Cutting depth in the X axis direction is 1mm

(Cut twice)

φ50

δ₂

(Metric input, Diameter programming)

φ43

G00

X 12.0 Z72.0 ;

δ₁

G32

X 41.0 Z29.0 F3.5 ;

G00

X 50.0 ;

Z axis

Z 72.0 ;

φ14

X 10.0 ;

(Cut 1mm more for the second cut)

G32 X 39.0 Z29.0 ;

G00

X 50.0 ;

Z 72.0 ;

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

WARNING

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

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

suddenly increase the cutting depth. Thus, the feed hold function is ineffective while thread

cutting. If the feed hold button is pressed during thread cutting, the tool will stop after a block

not specifying thread cutting is executed as if the SINGLE BLOCK button were pushed.

However, the feed hold lamp (SPL lamp) lights when the FEED HOLD button on the machine

control panel is pushed. Then, when the tool stops, the lamp is turned off (Single Block stop

status).

When the FEED HOLD button is held down, or is pressed again in the first block that does not

specify thread cutting immediately after a thread cutting block, the tool stops at the block that

does not specify thread cutting.

When thread cutting is executed in the single block status, the tool stops after execution of the

first block not specifying thread cutting.

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

cutting, the tool stops at the first block not specifying thread cutting as when the feed hold button

is pushed as mentioned in Note 3.

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

stops after execution of the block not specifying thread cutting as for the single block mode in

Note 4.

When the previous block was a thread cutting block, cutting will start immediately without

waiting for detection of the 1-turn signal even if the present block is a thread cutting block.

G32Z _ F_ ;

Z _;

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

G32 ;

(Regarded as threading block.)

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

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

cutting and the spindle speed changes, the correct thread lead may not be cut. Therefore, do

not use the constant surface speed control during thread cutting. Instead, use G97.

A movement block preceding the thread cutting block must not specify chamfering or corner

A thread cutting block must not specifying chamfering or corner R.

10 The spindle speed override function is disabled during thread cutting. The spindle speed is

fixed at 100%.

11 Thread cycle retract function is ineffective to G32.

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

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

4.10

revolution enables variable-lead thread cutting to be performed.

VARIABLE-LEAD

THREAD CUTTING

(G34)

Fig. 4.10 Variable-lead screw

Format

G34 IP_F_K_;

IP : End point

F : Lead in longitudinal axis direction at the start point

K : Increment and decrement of lead per spindle revolution

Explanations

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

G32.

Table 4.10 lists a range of values that can be specified as K.

Table 4.10 Range of valid K values

Metric input

0.0001 to

500.0000 mm/rev

Inch input

0.000001 to

9.999999 inch/rev

P/S alarm (No. 14) is produced, for example, when K such that the value

in Table 4.10 is exceeded is directed, the maximum value of lead is

exceeded as a result of increase or decrease by K or the lead has a negative

value.

WARNING

The “Thread Cutting Cycle Retract” is not effective for G34.

Examples

Lead at the start point: 8.0 mm

Lead increment: 0.3 mm/rev

G34 Z-72.0 F8.0 K0.3 ;

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

This function for continuous thread cutting is such that fractional pulses

4.11

output to a joint between move blocks are overlapped with the next move

CONTINUOUS

for pulse processing and output (block overlap) .

THREAD CUTTING

Therefore, discontinuous machining sections caused by the interruption

of move during continuously block machining are eliminated, thus

making it possible to continuously direct the block for thread cutting

instructions.

Explanations

Since the system is controlled in such a manner that the synchronism

with the spindle does not deviate in the joint between blocks wherever

possible, it is possible to performed special thread cutting operation in

which the lead and shape change midway.

G32

Fig. 4.11 Continuous Thread Cutting

Even when the same section is repeated for thread cutting while changing

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

the threads.

NOTE

Block overlap is effective even for G01 command,

producing a more excellent finishing surface.

When extreme micro blocks continue, no block overlap may

function.

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Using the Q address to specify an angle between the one-spindle-rotation

4.12

signal and the start of threading shifts the threading start angle, making

MULTIPLE-THREAD

it possible to produce multiple-thread screws with ease.

CUTTING

Multiple-thread screws.

Format

(constant-lead threading)

G32 IP_ F_ Q_ ;

IP_ : End point

G32 IP_ Q_ ;

F_ : Lead in longitudinal direction

Q_ : Threading start angle

Explanations

D Available thread cutting

G32: Constant-lead thread cutting

commands

G34: Variable-lead thread cutting

G76: Multiple-thread cutting cycle

G92: Thread cutting cycle

Limitations

D Start angle

The start angle is not a continuous-state (modal) value. It must be

specified each time it is used. If a value is not specified, 0 is assumed.

D Start angle increment

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

can be specified.

Example:

For a shift angle of 180 degrees, specify Q180000.

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

D Specifiable start angle

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be

range

specified. If a value greater than 360000 (360 degrees) is specified, it is

rounded down to 360000 (360 degrees).

D Multiple-thread cutting

For the G76 multiple-thread cutting command, always use the FS15 tape

(G76)

format.

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Using the G35 and G36 commands, a circular thread, having the specified

4.13

lead in the direction of the major axis, can be machined.

CIRCULAR

THREADING

(G35, G36)

Circular thread

Format

G35

I _ K _

X (U) _ Z (W) _

F _ Q _ ;

G36

R _ _ _

G35

: Clockwise circular threading command

G36

: Counterclockwise circular threading command

X (U) : Specify the arc end point (in the same way as for G02,

G03).

Z (W)

I, K

: Specify the arc center relative to the start point, using

relative coordinates (in the same way as for G02, G03).

: Specify the arc radius.

: Specify the lead in the direction of the major axis.

: Specify the shift of the threading start angle (0 to 360°

in units of 0.001°)

Start point

End point (Z, X)

Arc center

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Explanations

D Specifying the arc radius

If R is specified with I and K, only R is effective.

D Selecting a plane other

If an additional axis other than the X- and Z-axes is provided, circular

than the ZX plane

threading can be specified for a plane other than the ZX plane. The

method of specification is the same as that for G02 and G03.

D Automatic tool

The G36 command is used to specify the following two functions:

compensation

Automatic tool compensation X and counterclockwise circular threading.

The function for which G36 is to be used depends on bit 3 (G36) of

parameter No. 3405.

D When parameter G36 is set to 0, the G36 command is used for

automatic tool compensation X.

D When parameter G36 is set to 1, the G36 command is used for

counterclockwise circular threading.

G37.1 can be used to specify automatic tool compensation X and G37.2

can be used to specify automatic tool compensation Z.

(Specification method)

G37.1 X_

G37.2 Z_

G code when bit 3 of parameter No. 3405 is set to 1

G code

G code group

Function

G35

Clockwise circular threading

G36

Counterclockwise circular threading

G37

Automatic tool compensation Z

G37.1

Automatic tool compensation X

G37.2

Automatic tool compensation Z

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Limitations

D Range of specifiable arc

An arc must be specified such that it falls within a range in which the

major axis of the arc is always the Z-axis or always the X-axis, as shown

in Fig. 4.13 (a) and (b). If the arc includes a point at which the major axis

changes from the X-axis to Z-axis, or vice versa, as shown in Fig. 4.13

(c), P/S alarm 5058 is issued.

Start point

End point

45°

Fig. 4.13 (a) Range in which the Z-axis is the major axis

Start point

45°

End point

Fig. 4.13 (b) Range in which the X-axis is the major axis

Start point

The major axis changes at this point.

End point

45°

Fig. 4.13 (c) Example of arc specification which causes an alarm

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

Linear interpolation can be commanded by specifying axial move

4.14

following the G31 command, like G01. If an external skip signal is input

SKIP FUNCTION

during the execution of this command, execution of the command is

(G31)

interrupted and the next block is executed.

The skip function is used when the end of machining is not programmed

but specified with a signal from the machine, for example, in grinding. It

is used also for measuring the dimensions of a workpiece.

For details of how to use this function, refer to the manual supplied by the

machine tool builder.

Format

G31 IP_ ;

G31: One-shot G code (If is effective only in the block in which

it is specified)

Explanations

The coordinate values when the skip signal is turned on can be used in a

custom macro because they are stored in the custom macro system

variable #5061 to #5068, as follows:

#5061 X axis coordinate value

#5062 Z axis coordinate value

#5063 3rd axis coordinate value

#5068 8th axis coordinate value

WARNING

To increase the precision of the tool position when the skip

signal is input, feedrate override, dry run, and automatic

acceleration/deceleration is disabled for the skip function

when the feedrate is specified as a feed per minute value.

To enable these functions, set bit 7 (SKF) of parameter No.

6200 to 1. If the feedrate is specified as a feed per rotation

value, feedrate override, dry run, and automatic

acceleration/deceleration are enabled for the skip function,

regardless of the setting of the SKF bit.

NOTE

If G31 command is issued while tool nose radius

compensation is applied, an P/S alarm of No. 035 is

displayed. Cancel the cutter compensation with the G40

command before the G31 command is specified.

For the high-speed skip option, executing G31 during

feed-per- rotation mode causes P/S alarm (No. 211) to be

generated.

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

Examples

D The next block to G31 is an

incremental command

G31

W100.0 F100;

U50.0;

Skip signal is input here

50.0

100.0

Actual motion

Motion without skip signal

Fig.4.14 (a) The next block is an incremental command

D The next block to G31 is an

absolute command for 1

axis

G31

Z200.00 F100;

X100.0

X100.0;

Skip signal is input here

Z200.0

Actual motion

Motion without skip signal

Fig.4.14 (b) The next block is an absolute command for 1 axis

D The next block to G31 is an

absolute command for 2

axes

G31

G90X200.0 F100;

X300.0 Z100.0;

Skip signal is input here

100

(100,300)

Actual motion

Motion without skip signal

100

200

300

Fig 4.14 (c) The next block is an absolute command for 2 axes

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

In a block specifying P1 to P4 after G31, the multistage skip function

4.15

stores coordinates in a custom macro variable when a skip signal (4-point

MULTISTAGE SKIP

or 8-point ; 8-point when a high-speed skip signal is used) is turned on.

(G31)

Then, the function skips the entire amount of remaining movement. In

a block specifying Q1 to Q4 after G04, the function skips a dwell when

a skip signal (4-point or 8-point; 8-point when a high-speed skip signal

is used) is turned on.

A skip signal from equipment such as a fixed-dimension size measuring

instrument can be used to skip programs being executed.

In plunge grinding, for example, a series of operations from rough

machining to spark-out can be performed automatically by applying a

skip signal each time rough machining, semi-fine machining,

fine-machining, or spark-out operation is completed.

For details of how to use this function, refer to the manuals supplied by

the machine tool builder.

Format

Move command

G31 IP __ F __ P __ ;

IP_ : End point

F_ : Feedrate

P_ : P1-P4

Dwell

G04 X (U, P)__ (Q__) ;

X(U, P)_ : Dwell time

Q_ : Q1 - Q4

Explanations

Multistage skip is caused by specifying P1, P2, P3, or P4 in a G31 block.

For an explanation of selecting (P1, P2, P3, or P4), refer to the manual

supplied by the machine tool builder.

Specifying Q1, Q2, Q3, or Q4 in G04 (dwell command) enables dwell

skip in a similar way to specifying G31. A skip may occur even if Q is

not specified. For an explanation of selecting (Q1, Q2, Q3, or Q4), refer

to the manual supplied by the machine tool builder.

D Correspondence to skip

Parameter Nos. 6202 to 6205 can be used to specify whether the 4-point

signals

or 8-point skip signal is used (when a high-speed skip signal is used).

Specification is not limited to one-to-one correspondence. It is possible

to specify that one skip signal correspond to two or more Pn’s or Qn’s

(n=1, 2, 3, 4). Also, bits 0 (DS1) to 7 (DS8) of parameter No. 6206 can

be used to specify dwell.

CAUTION

Dwell is not skipped when Qn is not specified and

parameters DS1-DS8 (No. 6206#0-#7) are not set.

4. INTERPOLATION FUNCTIONS

PROGRAMMING

B-63524EN/01

With the motor torque limited (for example, by a torque limit command,

4.16

issued through the PMC window), a move command following G31 P99

TORQUE LIMIT SKIP

(or G31 P98) can cause the same type of cutting feed as with G01 (linear

(G31 P99)

interpolation).

With the issue of a signal indicating a torque limit has been reached

(because of pressure being applied or for some other reason), a skip

occurs.

For details of how to use this function, refer to the manuals supplied by

the machine tool builder.

Format

G31 P99 IP_ F_ ;

G31 P98 IP_ F_ ;

G31: One-shot G code (G code effective only in the block in which it

is issued)

Explanations

D G31 P99

If the motor torque limit is reached, or a SKIP signal is received during

execution of G31 P99, the current move command is aborted, and the next

block is executed.

D G31 P98

If the motor torque limit is reached during execution of G31 P98, the

current move command is aborted, and the next block is executed. The

SKIP signal <X0004#7/Tool post 2 X0013#7> does not affect G31 P98.

Entering a SKIP signal during the execution of G31 P98 does not cause

a skip.

D Torque limit command

If a torque limit is not specified before the execution of G31 P99/98, the

move command continues; no skip occurs even if a torque limit is

reached.

D Custom macro system

When G31 P99/98 is specified, the custom macro variables hold the

variable

coordinates at the end of a skip.

(See Section 4.9.)

If a SKIP signal causes a skip with G31 P99, the custom macro system

variables hold the coordinates based on the machine coordinate system

when it stops, rather than those when the SKIP signal is entered.

Limitations

D Axis command

Only one axis can be controlled in each block with G31 P98/99.

If two or more axes are specified to be controlled in such blocks, or no axis

command is issued, P/S alarm No. 015 is generated.

D Degree of servo error

When a signal indicating that a torque limit has been reached is input

during execution of G31 P99/98, and the degree of servo error exceeds

32767, P/S alarm No. 244 is generated.

D High-speed skip

With G31 P99, a SKIP signal can cause a skip, but not a high-speed skip.

B-63524EN/01

PROGRAMMING

4. INTERPOLATION FUNCTIONS

D Simplified

G31 P99/98 cannot be used for axes subject to simplified synchronization

synchronization and

or the X-axis or Z-axis when under slanted axis control.

slanted axis control

D Speed control

Bit 7 (SKF) of parameter No. 6200 must be set to disable dry run,

override, and auto acceleration or deceleration for G31 skip commands.

Do not use G31 P99/98 in consecutive blocks.

D Consecutive commands

WARNING

Always specify a torque limit before a G31 P99/98

command.

Otherwise, G31 P99/98 allows move

commands to be executed without causing a skip.

NOTE

If G31 is issued with tool nose radius compensation

specified, P/S alarm No. 035 is generated. Therefore,

before issuing G31, execute G40 to cancel tool nose radius

compensation.

Examples

O0001 ;

Mjj ;

The PMC specifies the torque limit

through the window.

G31 P99 X200. F100 ;

Torque limit skip command

Move command for which a torque

G01 X100. F500 ;

limit is applied

MDD ;

Torque limit canceled by the PMC

M30 ;

B-63524EN/01

PROGRAMMING

5. FEED FUNCTIONS

The feed functions control the feedrate of the tool. The following two feed

5.1

functions are available:

GENERAL

D Feed functions

1. Rapid traverse

When the positioning command (G00) is specified, the tool moves at!a

rapid traverse feedrate set in the CNC (parameter No. 1420).

2. Cutting feed

The tool moves at a programmed cutting feedrate.

D Override

Override can be applied to a rapid traverse rate or cutting feedrate using

the switch on the machine operator’s panel.

D Automatic acceleration/

To prevent a mechanical shock, acceleration/deceleration is automatically

deceleration

applied when the tool starts and ends its movement (Fig. 5.1 (a)).

Rapid traverse rate

F_R :Rapid traverse

F_R

rate

: Acceleration/

T_R

deceleration

time constant for

rapid traverse

rate

Time

T_R

Feed rate

F_C

: Feedrate

F_C

T_C : Acceleration/

deceleration time

constant for a cut-

ting feedrate

Time

T_C

Fig. 5.1 (a) Automatic acceleration/deceleration (example)

5. FEED FUNCTIONS

PROGRAMMING

B-63524EN/01

D Tool path in a cutting

If the direction of movement changes between specified blocks during

feed

cutting feed, a rounded-corner path may result (Fig. 5.1 (b)).

Programmed path

Actual tool path

Fig. 5.1 (b) Example of Tool Path between Two Blocks

In circular interpolation, a radial error occurs (Fig. 5.1 (c)).

∆r:Error

Programmed path

Actual tool path

Fig. 5.1 (c) Example of Radial Error in Circular Interpolation

The rounded-corner path shown in Fig. 5.1 (b) and the error shown in Fig.

5.1 (c) depend on the feedrate. So, the feedrate needs to be controlled for

the tool to move as programmed.

B-63524EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.2

RAPID TRAVERSE

Format

G00 IP_ ;

G00 : G code (group 01) for positioning (rapid traverse)

IP_ ; Dimension word for the end point

Explanations

The positioning command (G00) positions the tool by rapid traverse. In

rapid traverse, the next block is executed after the specified feedrate

becomes 0 and the servo motor reaches a certain range set by the machine

tool builder (in-position check).

A rapid traverse rate is set for each axis by parameter No. 1420, so no rapid

traverse feedrate need be programmed.

The following overrides can be applied to a rapid traverse rate with the

switch on the machine operator’s panel:F0, 25, 50, 100%

F0: Allows a fixed feedrate to be set for each axis by parameter No. 1421.

For detailed information, refer to the appropriate manual of the machine

tool builder.

5. FEED FUNCTIONS

PROGRAMMING

B-63524EN/01

Feedrate of linear interpolation (G01), circular interpolation (G02, G03),

5.3

etc. are commanded with numbers after the F code.

CUTTING FEED

In cutting feed, the next block is executed so that the feedrate change from

the previous block is minimized.

Two modes of specification are available:

1. Feed per minute (G98)

After F, specify the amount of feed of the tool per minute.

2. Feed per revolution (G99)

After F, specify the amount of feed of the tool per spindle revolution.

Format

Feed per minute

G98 ; G code (group 05) for feed per minute

F_ ;

Feedrate command (mm/min or inch/min)

Feed per revolution

G99 ; G code (group 05) for feed per revolution

F_ ;

Feedrate command (mm/rev or inch/rev)

Explanations

D Tangential speed

Cutting feed is controlled so that the tangential feedrate is always set at

constant control

a specified feedrate.

Starting

End point

point

Start

Center

End point

point

Linear interpolation

Circular interpolation

Fig. 5.3 (a) Tangential feedrate (F)

After specifying G98 (in the feed per minute mode), the amount of feed

D Feed per minute (G98)

of the tool per minute is to be directly specified by setting a number after

F. G98 is a modal code. Once a G98 is specified, it is valid until G99 (feed

per revolution) is specified. At power-on, the feed per revolution mode

is set.

An override from 0% to 254% (in 1% steps) can be applied to feed per

minute with the switch on the machine operator’s panel. For detailed

information, see the appropriate manual of the machine tool builder.

B-63524EN/01

PROGRAMMING

5. FEED FUNCTIONS

Feed amount per minute

(mm/min or inch/min)

Fig. 5.3 (b) Feed per minute

WARNING

No override can be used for some commands such as for

threading.

D Feed per revolution

After specifying G99 (in the feed per revolution mode), the amount of

(G99)

feed of the tool per spindle revolution is to be directly specified by setting

a number after F. G99 is a modal code. Once a G99 is specified, it is valid

until G98 (feed per minute) is specified.

An override from 0% to 254% (in 1% steps) can be applied to feed per

revolution with the switch on the machine operator’s panel. For detailed

information, see the appropriate manual of the machine tool builder.

If bit 0 (NPC) of parameter No. 1402 has been set to 1, feed-per-rotation

commands can be specified even when a position coder is not being used.

(The CNC converts feed-per-rotation commands to feed-per-minute

commands.)

Feed amount per spindle revolution

(mm/rev or inch/rev)

Fig. 5.3 (c) Feed per revolution

CAUTION

When the speed of the spindle is low, feedrate fluctuation

may occur. The slower the spindle rotates, the more

frequently feedrate fluctuation occurs.

A common upper limit can be set on the cutting feedrate along each axis

D Cutting feedrate clamp

with parameter No. 1422. If an actual cutting feedrate (with an override

applied) exceeds a specified upper limit, it is clamped to the upper limit.

B-63524EN/01

PROGRAMMING

5. FEED FUNCTIONS

5.4

DWELL (G04)

Format

Dwell G04 X_ ; or G04 U_ ; or G04 P_ ;

X_ : Specify a time (decimal point permitted)

U_ : Specify a time (decimal point permitted)

P_ : Specify a time (decimal point not permitted)

Explanations

By specifying a dwell, the execution of the next block is delayed by the

specified time.

Bit 1 (DWL) of parameter No. 3405 can specify dwell for each rotation

in feed per rotation mode (G99).

Table 5.4 (a)

Command value range of the dwell time (Command by X or U)

Increment system

Command value range

Dwell time unit

IS-B

0.001 to 99999.999

s or rev

IS-C

0.0001 to 9999.9999

Table 5.4 (b)

Command value range of the dwell time (Command by P)

Increment system

Command value range

Dwell time unit

IS-B

1 to 99999999

0.001 s or rev

IS-C

1 to 99999999

0.0001 s or rev

B-63524EN/01

PROGRAMMING

6. REFERENCE POSITION

6.1

REFERENCE

POSITION RETURN

D Reference position

The reference position is a fixed position on a machine tool to which the

tool can easily be moved by the reference position return function.

For example, the reference position is used as a position at which tools

are automatically changed. Up to four reference positions can be

specified by setting coordinates in the machine coordinate system in

parameters (No. 1240 to 1243).

2nd reference position

3rd reference position

Reference position

4th reference

position

Machine zero point

Fig. 6.1 (a) Machine zero point and reference positions

6. REFERENCE POSITION

PROGRAMMING

B-63524EN/01

D Reference position

Tools are automatically moved to the reference position via an

return

intermediate position along a specified axis. When reference position

return is completed, the lamp for indicating the completion of return goes

on.

Intermediate position

Reference position

Fig. 6.2 (b) Reference position return

D Reference position

The reference position return check (G27) is the function which checks

return check

whether the tool has correctly returned to the reference position as

specified in the program. If the tool has correctly returned to the reference

position along a specified axis, the lamp for the axis goes on.

Format

D Reference position

return

G28IP

_ ;

Reference position return

G30 P2

_ ;2nd reference position return

(P2 can

be omitted.)

G30 P3

_ ;3rd reference position return

4th reference position return

G30 P4

_ ;

IP : Command specifying the intermediate position

(Absolute/incremental command)

D Reference position

return check

G27 IP _ ;

IP : Command specifying the reference position

(Absolute/incremental command)

B-63524EN/01

PROGRAMMING

6. REFERENCE POSITION

Explanations

D Reference position

Positioning to the intermediate or reference positions are performed at the

return (G28)

rapid traverse rate of each axis.

Therefore, for safety, the tool nose radius compensation, and tool offset

should be cancelled before executing this command.

D 2nd, 3rd, and 4th

In a system without an absolute-position detector, the first, third, and

reference position return

fourth reference position return functions can be used only after the

(G30)

reference position return (G28) or manual reference position return (see

III-3.1) is made. The G30 command is generally used when the automatic

tool changer (ATC) position differs from the reference position.

D Reference position

G27 command positions the tool at rapid traverse rate. If the tool reaches

return check (G27)

the reference position, the reference position return lamp lights up.

However, if the position reached by the tool is not the reference position,

an alarm (No. 092) is displayed.

Restrictions

D Status the machine lock

The lamp for indicating the completion of return does not go on when the

being turned on

machine lock is turned on, even when the tool has automatically returned

to the reference position. In this case, it is not checked whether the tool

has returned to the reference position even when a G27 command is

specified.

D First return to the

When the G28 command is specified when manual return to the reference

reference position after

position has not been performed after the power has been turned on, the

the power has been

movement from the intermediate point is the same as in manual return to

turned on (without an

the reference position.

absolute position

In this case, the tool moves in the direction for reference position return

detector)

specified in parameter ZMIx (bit 5 of No. 1006). Therefore the specified

intermediate position must be a position to which reference position

return is possible.

D Reference position

In an offset mode, the position to be reached by the tool with the G27

return check in an offset

command is the position obtained by adding the offset value. Therefore,

mode

if the position with the offset value added is not the reference position, the

lamp does not light up, but an alarm is displayed instead. Usually, cancel

offsets before G27 is commanded.

D Lighting the lamp when

When the machine tool is an inch system with metric input, the reference

the programmed position

position return lamp may also light up even if the programmed position

does not coincide with

is shifted from the reference position by least input increment. This is

the reference position

because the least input increment of the machine is smaller than its least

command increment.

Reference

D Manual reference

See III-3.1.

position return

6. REFERENCE POSITION

PROGRAMMING

B-63524EN/01

Tools ca be returned to the floating reference position.

6.2

A floating reference point is a position on a machine tool, and serves as

FLOATING

a reference point for machine tool operation.

REFERENCE

A floating reference point need not always be fixed, but can be moved as

POSITION RETURN

required.

(G30.1)

Format

G30.1

;

IP _ : Command of the intermediate position of the floating reference

position

(Absolute command/incremental command)

Explanations

On some machine tools, the cutting tools can be replaced at any position

unless they interfere with the workpiece or tail stock.

With these machines, the cutting tools should be replaced at a position as

close to the workpiece as possible so as to minimize the machine cycle

time. For this purpose, the tool change position is to be changed,

depending on the figure of the workpiece. This operation can easily be

performed using this function. That is, a tool change position suitable for

the workpiece is memorized as a floating reference point. Then command

G30. 1 can easily cause return to the tool change position.

D Floating reference

The G30.1 block first positions the tool at the intermediate point along the

position

specified axes at rapid traverse rate, then further moves the tool from the

intermediate point to the floating reference point at rapid traverse rate.

Before using G30.1, cancel cutter compensation and tool offset.

D Setting of floating

A floating reference point becomes a machine coordinate position

reference position

memorized by pressing the soft key [SET FRP] on the current positions

display screen.

A floating reference point is not lost even if power is turned off.

Examples

G30.1 X40.0 Z50.0 ;

Intermediate position (40, 50)

Floating

reference

Workpiece

position

B-63524EN/01

PROGRAMMING

7. COORDINATE SYSTEM

COORDINATE SYSTEM

By teaching the CNC a desired tool position, the tool can be moved to the

position. Such a tool position is represented by coordinates in a

coordinate system. Coordinates are specified using program axes.

When two program axes, the X-axis and Z-axis, are used, coordinates

are specified as follows:

X_Z_

This command is referred to as a dimension word.

ÎÎÎ

ÎÎ

Zero point

Fig. 7 Tool Position Specified by XαZβ

Coordinates are specified in one of following three coordinate systems:

(1) Machine coordinate system

(2) Workpiece coordinate system

(3) Local coordinate system

The number of the axes of a coordinate system varies from one machine

to another. So, in this manual, a dimension word is represented as IP_.

7. COORDINATE SYSTEM

PROGRAMMING

B-63524EN/01

The point that is specific to a machine and serves as the reference of the

7.1

machine is referred to as the machine zero point. A machine tool builder

MACHINE

sets a machine zero point for each machine.

COORDINATE

A coordinate system with a machine zero point set as its origin is referred

SYSTEM

to as a machine coordinate system.

A machine coordinate system is set by performing manual reference

position return after power-on (see III-3.1). A machine coordinate

system, once set, remains unchanged until the power is turned off.

Format

G53 IP _ ;

IP _; Absolute dimension word

Explanations

D Selecting a machine

When a position has been specified as a set of machine coordinates, the

coordinate system (G53)

tool moves to that position by means of rapid traverse. G53, used for

selecting the machine coordinate system, is a one-shot G code. Any

commands based on the selected machine coordinate system are thus

effective only in the block containing G53. The G53 command must be

specified using absolute values. If incremental values are specified, the

G53 command is ignored. When the tool is to be moved to a

machine-specific position such as a tool change position, program the

movement in a machine coordinate system based on G53.

Restrictions

D Cancel of the

When the G53 command is specified, cancel the tool nose radius

compensation function

compensation and tool offset.

D G53 specification

Since the machine coordinate system must be set before the G53

immediately after

command is specified, at least one manual reference position return or

power-on

automatic reference position return by the G28 command must be

performed after the power is turned on. This is not necessary when an

absolute-position detector is attached.

Reference

When manual reference position return is performed after power-on, a

machine coordinate system is set so that the reference position is at the

coordinate values of (α, β) set using parameter No.1240.

Machine coordinate system

Machine zero

Reference position

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 4