FANUC MANUAL GUIDE i. OPERATOR’S MANUAL

2.LATHE

EXAMPLE OF PROGRAMMING

B-63874EN/05

In this programming example, round bar workpiece is used. So, enter

the blank figure as follows.

(ZX PLANE TURNING FIGURE - INSERT)

[LINE]

(LINE - INSERT)

[RIGHT]

(LINE DIRECTION)

0 INPUT

(END POINT Z)

→

[BLANK]

(ELEMENT TYPE)

[OK]

[LINE]

(LINE - INSERT)

[DOWN]

(LINE DIRECTION)

31 INPUT

(END POINT DX)

[OK]

Part figures are displayed in blue line, blank figures are displayed in

green line, and the currently selected figure is displayed in yellow

line.

Check the entered part figures and blank figures are correct by

comparing with the blue print, then register them as figure blocks into

CNC memory finally.

- 702 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

2.LATHE

Figure blocks can be registered into the current part program directly,

and also can be registered as another sub program.

Registered figure blocks can be used also for finishing, so in this

example, register them as a sub program.

(ZX PLANE TURNING FIGURE - INSERT)

[CREATE]

(METHOD OF FREE FIGURE CREATION)

↓

8100 INPUT

(SUBPRO NO.)

OUTER TURNING

(FIGURE NAME)

[OK]

NOTE

Registered sub program can be displayed in a figure

menu tab, “SUBPROGRAM”.

In this case, set the parameters No14720 to 14723

in advance.

For this example, set those parameters as follow.

No.14720=8000 (Minimum program number of sub

programs displayed in the turning

machining sub program menu)

No.14721=8499 (Maximum program number of sub

programs displayed in the turning

machining sub program menu)

No.14722=8500 (Minimum program number of sub

programs displayed in the milling

machining sub program menu)

No.14723=8999 (Maximum program number of sub

programs displayed in the milling

machining sub program menu)

- 703 -

2.LATHE

EXAMPLE OF PROGRAMMING

B-63874EN/05

2.5.5

Entering Tool Changing and Spindle Rotation Blocks for

Outer Finishing in ISO-code Form

Before starting the 2nd process of outer finishing, change tool to the

finishing tool (T0202), spindle rotation, and other necessary blocks in

ISO-code form with G-code and so on.

G28 U0 W0 ; INSERT

(Reference position return)

T0202 ; INSERT

(Tool change)

G99 G96 S300 ; INSERT

(Constant surface speed control, mm/rev mode)

M03 ; INSERT

(Spindle rotation)

G00 X120. Z20. ; INSERT

(Approaching)

Otherwise, you can enter them from the fixed form sentence menu.

(Soft-key group for Turning cycle menu)

[START]

<START>

↓

<<1.START PROCEDURE>>

[INSERT]

NOTE

There may be a case that undefined value is

entered by “?” in the fixed form sentence menu, so

in this case, you need to replace the “?” by proper

value can be used in actual machining.

- 704 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

2.LATHE

2.5.6

Entering Outer Finishing Cycle Machining Process

2.5.6.1 Entering figure for outer finishing cycle block

Enter the 2nd process : outer finishing by a general purpose finishing

tool (T0202).

Enter machining type, cutting condition and so on.

(Soft-key group for Turning cycle menu)

[CYCLE]

→

↓

<<7.TURNING(OUTER FINISH)>>

[SELECT]

(TURNING(OUTER FINISH) - INSERT)

[-Z]

(CUTTING DIRECTION)

.1 INPUT

(FEEDRATE)

[INSERT]

NOTE

1 In the cycle machining data menu window, all data

excepting cutting condition data are set

automatically. However, the data entered at

previously entered cycle of same kind are copied,

so you must enter the data if you have not entered

the same kind of cycle.

2 When you select the cycle machining type form

cycle machining menu, instead of selecting by the

cursor, you can use direct inputting of item number

and INPUT. (In this case, enter 7 INPUT)

- 705 -

2.LATHE

EXAMPLE OF PROGRAMMING

B-63874EN/05

2.5.6.2 Entering figure for outer finishing

By inserting the outer finishing cycle machining block, the window

for free form entering is displayed, so enter the final figure of

machining. But, the former registered figure blocks for roughing can

be used, so push [CANCEL] and go back to the turning figure menu

window, then select from the sub program menu.

(ZX PLANE TURNING FIGURE - INSERT)

(START POINT - INSERT)

[CANCEL]

(INSERT TURNING FIGURE)

→

↓

<<08100: OUTER TURNING>>

[SELECT]

2.5.6.3 Entering releasing motion blocks in ISO-code form

After outer finishing, return the tool to safety area before the next

C-axis drilling process.

Enter these motion blocks in form of ISO-code with such as G-code.

G00 X200. ; INSERT

(Releasing motion)

M05 ; INSERT

(Spindle stop)

G28 U0 W0 ; INSERT

(Reference position return)

- 706 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

2.LATHE

2.5.7

Entering Tool Changing and Spindle Rotating Blocks for

C-axis Drilling

2.5.7.1 Entering in ISO-code form directly

Enter blocks of tool changing, C-axis mode changing spindle rotation

approaching and releasing for C-axis drilling. You can enter these

blocks using ISO-code form.

M21. ; INSERT

(Change to C-axis mode)

T0303 ; INSERT

(Tool change)

G98 G97 ; INSERT

(mm/min mode)

M03 S800 ; INSERT

(Spindle rotation)

G00 X120. Z20. ; INSERT

(Approaching)

2.5.7.2 Entering by fixed form sentence menu

ISO-code form part program can be entered from the fixed form

sentence menu. But, in such a case, proper fixed form sentence must

be prepared in advance.

(Soft-key group for Milling cycle menu)

[START]

<START>

↓

<<2.C-AXIS MILLING START>>

[INSERT]

NOTE

There may be a case that undefined value is

entered by “?” in the fixed form sentence menu, so

in this case, you need to replace the “?” by proper

value can be used in actual machining.

- 707 -

2.LATHE

EXAMPLE OF PROGRAMMING

B-63874EN/05

2.5.8

Entering C-axis Drilling Process

2.5.8.1

Entering C-axis drilling cycle block

Enter the 3rd process : C-axis end face drilling by the drilling tool

(T0303).

Enter machining type, cutting condition and so on.

(Soft-key group for Milling cycle menu)

[CYCLE]

↓

<<2.DRILLING>>

[SELECT]

(DRILLING - INSERT)

5 INPUT

(PECKING CUT DEPTH)

INPUT

(REF.PT.MODE)

10 INPUT

(I POINT)

-20 INPUT

(CUT DEPTH)

2 INPUT

(GO PAST AMOUNT)

2 INPUT

(CLEARANCE)

100 INPUT

(FEEDRATE)

.5 INPUT

(DWELL TIME)

[INSERT]

NOTE

In the cycle machining data menu window, all data

excepting cutting condition data are set

automatically. However, the data entered at

previously entered cycle of same kind are copied,

so you must enter the data if you have not entered

the same kind of cycle.

- 708 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

2.LATHE

2.5.8.2 Entering hole position block

By inserting the drilling cycle block, the window of hole position

menu is displayed, so select the “Arc point” item.

(INSERT MILLING FIGURE)

↓

<<17.C-AXIS HOLE ON FACE (ARC POINTS)>>

[SELECT]

(XC-C AXIS HOLE (ARC POINTS) - INSERT)

<POS./SIZE>

0 INPUT

(BASE POSITION)

11 INPUT

(X AXIS POS.(RAD.))

0 INPUT

(START ANGLE)

→

90 INPUT

(PITCH ANGLE)

4 INPUT

(NUMBER OF HOLE)

[INSERT]

- 709 -

2.LATHE

EXAMPLE OF PROGRAMMING

B-63874EN/05

2.5.9

Operations in the “END” Menu

All necessary machining program have been entered, so enter end

procedure.

2.5.9.1

Entering in ISO-code form directly

Enter blocks for spindle stop, releasing and end M-code in ISO-code

form with G-code and son on.

M05. ; INSERT

(Spindle stop)

G00 X200. ; INSERT

(Releasing motion)

G28 U0 W0 ; INSERT

(Reference position return)

M02 ; INSERT

(End M-code)

2.5.9.2

Entering by fixed form sentence menu

ISO-code form part program can be entered from the fixed form

sentence menu. But, in such a case, proper fixed form sentence must

be prepared in advance.

(Soft-key group for Milling cycle menu)

[END]

<END>

↓

<<1.PROGRAM END>>

[INSERT]

NOTE

There may be a case that undefined value is

entered by “?” in the fixed form sentence menu, so

in this case, you need to replace the “?” by proper

value can be used in actual machining.

- 710 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.1

SETTING OF TOOL LENGTH OFFSET DATA

WARNING

1 Operation of tool offset setting varies from one

machine model to another. So operations described in

this section may differ from those ion actual machine.

As to the actual operation of tool offset setting on the

actual machine, refer to the applicable manual

supplied by the respective machine tool builders for

details.

If the set data does not match the characteristic of a

specific machine, the tool may bump against the

workpiece, and the machine may be forced to perform

unnatural machining, possibly causing damage to the

tool and/or machine, and even injuries.

2 As to the operations on a machine described in this

chapter, refer to the applicable manual supplied by the

respective machine tool builders for details.

If the operation does not match the characteristic of a

specific machine, the tool may bump against the

workpiece, and the machine may be forced to perform

unnatural machining, possibly causing damage to the

tool and/or machine, and even injuries.

Assume that the Z=0 position of the workpiece coordinate is the

surface of the workpiece, while the Z=0 position of the machine

coordinate is the machine origin.

By setting the distance between these 2 points to the tool length offset

data, workpiece coordinate of Z-axis can be defined.

Tool length is different between each tool for the actual machining, so

set the offset data respectively.

The tool length offset value is the relative coordinate value of Z-axis

at the point where the tool tip is touched to the surface of the

workpiece.

(1) Select the tool used for actual machining by switch on the

machine operator’s panel.

(2) Execute the machine reference position return of Z-axis.

(3) Press [ACTPOS] and make the relative coordinate data display.

(4) Press [PRESET], then push [ALL 0], and press [ALTER], then

the relative coordinate value of all axes are reset to 0. But, the

Z-axis coordinate only is used for measuring.

(5) Press [T-OFS] and make the tool offset widow open.

(6) Make the tool tip touch at the surface of the workpiece by JOG or

Manual handwheel. Then, the distance from the machine origin is

displayed as the Z-axis relative coordinate value.

(7) Select the tool length compensation column of the tool used for

measuring by moving the cursor by cursor key.

- 713 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

(8) Pressing [INP.C.] displays the window of INPUT RELATIVE

COORD. window, then move the cursor to the Z-axis.

(9) Pressing

[INPUT] makes the Z-axis relative coordinate value

enter as the tool offset length data.

Z=0 (Machine coordinate)

The tool used

for actual

machining

This distance is set as the tool

length offset value

Z=0 (Workpiece

coordinate)

Workpiece

NOTE

There is a case such as using a sensor called base

master instead of touching the tool to the workpiece

surface, so into details and actual operations, refer

to the manual made by machine tool builder.

- 714 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.2

SETTING OF WORKPIECE ORIGIN OFFSET VALUE

After setting the geometry offset data for necessary tools, set the

workpiece origin on the actual workpiece used for machining.

In order to carry out the actual machining by using the part program

made on the workpiece coordinate, set the distance between machine

coordinate and workpiece coordinate to the workpiece coordinate

system as the workpiece origin offset value.

In this section, operations, of which setting the center of the

workpiece (90x130) as the workpiece origin of X/Y/Z-axis by using

standard too with the radius 5mm, are described.

And, G54 is used as the workpiece coordinate system.

(1) Select the standard tool by using the switch on the machine

operator’s panel. There is a case of using special tool such as the

centering lever as the standard tool for easy operations and high

precision accuracy, so refer to the manual made by machine tool

builder for actual operations.

(2) After then, for safety, take measure to keep fully safety such as

closing the machine door.

(3) Select the manual handwheel mode on the machine operator’s

panel, and make the standard tool touch to the right side of the

workpiece

(A-position in the drawing) by referencing the

following drawing. At this time, make a spindle rotate by fully

safety speed if necessary, then you can avoid over-cutting by

stopping the tool moving at the position the tool begins cutting.

As to actual operations, refer to the manual made by the machine

tool builder.

Standard tool

Y-axis

direction

X-axis direction

90mm

130mm

(4) Pressing

[WK SET] displays the window of the workpiece

coordinate system.

(5) Select the G54 X-axis data by moving the cursor. When other tab

is displayed in the window, the cursor motion type might be the

tab transition type, so press

[CHCURS] for changing to item

transition type of cursor.

- 715 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

(6) Pressing [MEASUR] displays the window of offset calculating.

(7) When the tool touches to the right side of the workpiece, the

X-axis position should be X=70.0mm, 65mm of the right side

position + 5mm of the tool radius, so enter 70.0 to the target

workpiece coordinate value. Then, the calculation result value is

displayed at the RESULT column, so confirm the result is correct.

(8) Pressing

[INPUT] sets the above calculated value to the

workpiece origin offset data.

(9) Release the tool from the workpiece once, and set the Y-axis

workpiece origin offset data by similar operations of (3) to (8). In

this case, touch the point B in the drawing and the entering target

value is Y=50.0mm.

- 716 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.3

PREPARING OF THE FIXED FORM SENTENCE MENU

As to the fixed form sentence, machine tool builder usually sets the

suitable menu for specified respective machine. But, you can enter his

own menu on the MANUAL GUIDE i screen by yourself.

3.3.1

Entering the Fixed Form Sentence for Milling

Enter the fixed form sentence menu which will be called by the

soft-key [FIXFRM] in the soft-key group for milling.

Enter programs for START and END.

[SETTING]

(SETTING)

<BASIC>

↓

<<1. REGISTER FIXED FORM SENTENCE FOR MILLING>>

[SELECT]

(REGISTER FIXED FORM SENTENCE FOR MILLING)

[NEW]

(CRATE NEW FIXED FORM SENTENCE)

MILLING START INPUT

G28 G91 Z0. ; G28 X0. Y0. ; T? M06 ; D? ; M03 S? ; G00 G90 G54 X0. Y0.; G43

Z100. H? ;

[ADD]

→

<FORM5>

[NEW]

(CREATE NEW FIXED FORM SENTENCE)

PROGRAM END INPUT

M05. ; G00 G90 Z100. ; G28 G91 Z0, ; M06 T0 ;M30 ;

[ADD]

[TO MNU]

- 717 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

3.4

SETTING OF THE TOOL DATA

Set the necessary tool data. These tool data are used for displaying

tool form of animation and calculation of cutting angle in the cycle

machining.

The tool length offset data were already set in section 3.1.

T01 : Flat end mill for roughing

T02 : Flat end mill for finishing

T03 : Drill

Display “TOOL OFFSET” window by [T-OFS]

TOOL OFFSET

NO.

TOOL LENGTH. COMP.

CUTTER COMPENSATOIN

GEOMETRY

WEAR

GEOMETRY

WEAR

001

Measured value

0.000

4.000

0.000

002

Measured value

0.000

3.000

0.000

003

Measured value

0.000

2.000

0.000

NOTE

1 The above offset data are just an example, and they

cannot be used for actual machining.

2 The above offset number 003 is used for drilling

tool, and if you use it for animation, you must set the

radius amount of the drill to radius offset data.

3 There is a case that the above offset screen might

not be displayed depending on the attached

optional function. Into details, refer to the manual

made by machine tool builder.

Display “TOOL DATA” tab by cursor key →

TOOL DATA

NO.

TOOL

SET

001

F END

002

F END

003

DRILL

140.0

- 718 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.5

CREATING OF PART PROGRAM

In the MANUAL GUIDE i , background editing can be used, but in

this section, part program creating operations are described by using

foreground editing on the EDIT mode.

3.5.1

Creating New Part Program

Create a new part program of O1234.

In case of creating a new part program directly

Select EDIT mode by using a mode-selecting switch on a machine-operating panel

[NEWPRG]

(CREATE NEW PROGRAM)

1234 [CREATE]

(NEW PROGRAM NO.)

In case of creating a new part program on the program list

window

Select EDIT mode by using a mode-selecting switch on a machine-operating panel

[O-LIST]

(OPEN PROGRAM)

[NEW]

(CREATE NEW PROGRAM)

1234 [CREATE]

(NEW PROGRAM NO.)

Select the newly entered program by ↓

[OPEN]

- 719 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

3.5.2

Operations of “START” Menu

By pushing [START] in the soft-key menu for milling, the window

“INSERT STARTING COMMAND FOR MILLING” with the

following tabs is displayed.

<START>

: Fixed form sentence menu used for the top of

part program or each machining process.

<COORD CONV> : Coordinate conversion menu, which is

necessary for the machine on the inclined

surface, this is not used in this section.

<BLANK>

: Blank form menu, which is necessary for

animation.

3.5.2.1

Entering blank form data

By selecting a tab <BLANK> by cursor key, blank form menu is

displayed.

(INSERT STARTING COMMAND FOR MILLING)

<BLANK>

↓

<<1. RECTANGULAR BLANK FIGURE>>

[SELECT]

Enter blank form data as a round bar.

(RECTANGULAR BLANK FIGURE - INSERT)

130 INPUT

(WIDTH)

90 INPUT

(LENGTH)

30 INPUT

(HEIGHT)

65 INPUT

(WORK ORIGIN X)

45 INPUT

(WORK ORIGIN Y)

0 INPUT

(WORK PROGIN Z)

[INSERT]

- 720 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.5.3

Entering Tool Changing and Spindle Rotating Blocks for

Roughing Flat End Mill

3.5.3.1

Entering in ISO-code form directly

It is difficult to define the action of tool changing, spindle rotation,

approaching and releasing generally because there are many

difference depending on machine configuration. So, using ISO-code

form program can realize more flexible and safety part program.

G28 G91 Z0. ; INSERT

(Z-axis reference position return)

G28 G91 X0. Y0. ; INSERT

(X/Y-axis reference position return)

T01 M06 ; INSERT

(Tool change)

D1 ; INSERT

(Selecting tool data)

M03 S1000 ; INSERT

(Spindle rotation)

G00 G90 G54 X0. Y0. ; INSERT (X/Y-axis approaching)

G43 Z100. H1 ; INSERT

(Z-axis approaching)

3.5.3.2

Entering by fixed form sentence menu

ISO-code form part program can be entered from the fixed form

sentence menu. But, in such a case, proper fixed form sentence must

be prepared in advance.

(Soft-key group for milling cycle menu)

[START]

(INSERT STARTING COMMAND FOR MILLING)

<START>

↓

<<3.MILLING START>>

[INSERT]

NOTE

There may be a case that undefined value is

entered by “?” in the fixed form sentence menu, so

in this case, you need to replace the “?” by proper

value can be used in actual machining.

Place the cursor to the address with “?”, enter

numeric data, then push “ALTER”.

After altering the data, return the cursor to the EOB

at the end of the program.

- 721 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

3.5.4

Entering Outer Wall Contouring Process

3.5.4.1

Entering outer wall contouring (rough) cycle block

Enter the 1st process : outer wall contouring process by the roughing

flat endmill (T01).

Enter machining type, cutting condition and so on.

(Soft-key menu for milling cycle menu)

[CYCLE]

(INSERT MILLING CYCLE)

→

↓

<<1.OUTER WALL CONTOURING(ROUGH)>>

[SELECT]

(OUTER WALL CONTOURING(ROUGH) - INSERT)

20 INPUT

(BOTTOM THICKNESS)

5 INPUT

(SIDE THICKNESS)

3 INPUT

(CUT DEPTH OF RADIUS)

10 INPUT

(CUT DEPTH OF AXIS)

0 INPUT

(SIDE FINISH AMOUNT)

0 INPUT

(BOTTOM FINISH AMOUNT)

500 INPUT

(FEED RATE - SING.CUT)

300 INPUT

(FEED RATE - BOTH CUT)

200 INPUT

(FEED RATE - AXIS)

[INSERT]

- 722 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

NOTE

1 In the cycle machining data menu window, all data

excepting cutting condition data are set

automatically. However, the data entered at

previously entered cycle of same kind are copied,

so you must enter the data if you have not entered

the same kind of cycle.

2 In the cycle machining data menu window, 2 tabs,

<CUT COND.> and <DETAIL>, are displayed.

In the <CUT COND.>, all data must be set. In the

<DETAIL>, all data are automatically set, so check

those data and modify them if necessary only

3.5.4.2

Entering figure for outer wall contouring (rough)

By inserting the cycle machining block, the window of contouring

figure menu is displayed, so select the XY-SQUARE CONVEX

(INSERT MILLING FIGURE)

<CONT. FIG.>

<<1.XY-SQUARE CONVEX>>

[SELECT]

(XY-SQUARE - INSERT)

<POS./SIZE>

[CONVEX]

(FIGURE TYPE)

0 INPUT

(BASE POSITION)

-20 INPUT

(HEIGHT/DEPTH)

0 INPUT

(CENTER POINT (X))

0 INPUT

(CENTER POINT (Y))

120 INPUT

(LENGTH FOR X AXIS)

80 INPUT

(LENGTH FOR Y AXIS)

[INSERT]

- 723 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

3.5.5

Entering Pocket Roughing Process

3.5.5.1

Entering pocket roughing cycle block

Enter the 2nd process : pocket roughing by a roughing flat endmill

(T01).

Since same tool with the 1st process is used, tool changing blocks are

not necessary.

Enter machining type, cutting condition and so on.

(Soft-key group for Milling cycle menu)

[CYCLE]

(INSERT MILLING CYCLE)

→

↓

<<1.POCKETING(ROUGH)>>

[SELECT]

(POCKETING(ROUGH) - INSERT)

INPUT

(BOTTOM THICKNESS)

INPUT

(SIDE THICKNESS)

3 INPUT

(CUT DEPTH OF RADIUS)

10 INPUT

(CUT DEPTH OF AXIS)

0.5 INPUT

(SIDE FINISH AMOUNT)

0.5 INPUT

(BOTTOM FINISH AMOUNT)

500 INPUT

(FEED RATE - SING.CUT)

300 INPUT

(FED RATE - BOTH CUT)

200 INPUT

(FEED RATE - AXIS)

[INSERT]

- 724 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

NOTE

1 In the cycle machining data menu window, all data

excepting cutting condition data are set

automatically. However, the data entered at

previously entered cycle of same kind are copied,

so you must enter the data if you have not entered

the same kind of cycle.

2 In the cycle machining data menu window, 2 tabs,

<CUT COND.> and <DETAIL>, are displayed.

In the <CUT COND.>, all data must be set. In the

<DETAIL>, all data are automatically set, so check

those data and modify them if necessary only

- 725 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

3.5.5.2

Entering figure for pocket roughing

By inserting the cycle machining block, the window of

pocketing

figure menu, so select the XY-FREE CONCAVE FIGURE.

(INSERT MILLING FIGURE)

↓

<<4.XY-FREE CONCAVE FIGURE>>

[SELECT]

(XY PLANE FREE FIGURE - INSERT)

(START POINT - INSERT)

INPUT

(FIGURE TYPE)

-50 INPUT

(START POINT X)

0 INPUT

(START POINT Y)

0 INPUT

(BASE POSITION)

-10 INPUT

(HEIGHT/DEPTH)

[OK]

[ARC

]

(ARC (CW) - INSERT)

INPUT

(END POINT X)

INPUT

(END POINT Y)

INPUT

(RADIUS)

-35 INPUT

(CENTER POINT CX)

0 INPUT

(CENTER POINT CY)

INPUT

(LAST CONNECTION)

[TANGNT]

(NEXT CONNECTION)

[OK]

[LINE]

(LINE - INSERT)

[R-UP]

(LINE DIRECTION)

INPUT

(END POINT X)

INPUT

(END POINT Y)

INPUT

(ANGLE)

[TANGNT]

(NEXT CONNECTION)

[OK]

[ARC

]

(ARC (CW) - INSERT)

INPUT

(END POINT X)

INPUT

(END POINT Y)

30 INPUT

(RADIUS)

0 INPUT

(CENTER POINT CX)

0 INPUT

(CENTER POINT CY)

[TANGNT]

(NEXT CONNECTION)

[OK]

[LINE]

(LINE - INSERT)

[R-DOWN]

(KINE DIRECTION)

INPUT

(END POINT X)

INPUT

(END POINT Y)

INPUT

(ANGLE)

[TANGNT]

(NEXT CONNECTION)

[OK]

- 726 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

[ARC

]

(ARC (CW) - INSERT)

INPUT

(END POINT X)

INPUT

(END POINT Y)

15 INPUT

(RADIUS)

35 INPUT

(CENTER POINT CX)

0 INPUT

(CENTER POINT CY)

[TANGNT]

(NEXT CONNECTION)

[OK]

[LINE]

(LINE - INSERT)

[L-DOWN]

(LINE DIRECTION)

INPUT

(END POINT X)

INPUT

(END POINT Y)

INPUT

(ANGLE)

[TANGNT]

(NEXT CONNECTION)

[OK]

[ARC

]

(ARC (CW) - INSERT)

INPUT

(END POINT X)

INPUT

(END POINT Y)

30 INPUT

(RADIUS)

0 INPUT

(CENTER POINT CX)

0 INPUT

(CENTER POINT CY)

[TANGNT]

(NEXT CONNECTION)

[OK]

[LINBE]

(LINE - INSERT)

[L-UP]

(LINE DIRECTION)

INPUT

(END POINT X)

INPUT

(END POINT Y)

INPUT

(ANGLE)

[TANGNT]

(NEXT CONNECTION)

[OK]

[ARC

]

(ARC (CW) - INSERT)

-50 INPUT

(END POINT X)

0 INPUT

(END POINT Y)

15 INPUT

(RADIUS)

-35 INPUT

(CENTER POINT CX)

0 INPUT

(CENTER POINT CY)

INPUT

(NEXT CONNECTION)

[OK]

- 727 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

There is an island in a pocket, so enter island figure continuously.

(START POINT - INSERT)

INPUT

(FIGURE TYPE)

-15 INPUT

(START POINT X)

-7.5 INPUT

(START POINT Y)

0 INPUT

(BASE POSITION)

-10 INPUT

(HEIGHT / DEPTH)

[OK]

[LINE]

(LINE - INSERT)

[UP]

(LINE DIRETION)

7.5 INPUT

(END POINT Y)

[OK]

[LINE]

(LINE - INSERT)

[RIGHT]

(LINE DIRECTION)

15 INPUT

(END POINT X)

[OK]

[LINE]

(LINE - INSERT)

[DOWN]

(LINE DIRECTION)

-7.5 INPUT

(END POINT Y)

[OK]

[LINE]

(LINE - INSERT)

[LEFT]

(LINE DIRECTION)

-15 INPUT

(END POINT X)

[OK]

Entered figure blocks were already defined to make as a subprogram,

so check the contents of them and create it as a subprogram by

pressing [OK]

(XY PLANE FREE FIGURE - INSERT)

[CREATE]

(METHOD OF FREE FIGURE CREATION)

[OK]

- 729 -

3.MACHINING CENTER

EXAMPLE OF PROGRAMMING

B-63874EN/05

NOTE

Registered sub program can be displayed in a figure

menu tab, “SUBPROGRAM”.

In this case, set the parameters No14720 to 14723 in

advance.

For this example, set those parameters as follow.

No.14720=8000 (Minimum program number of sub

programs displayed in the turning

machining sub program menu)

No.14721=8499 (Maximum program number of sub

programs displayed in the turning

machining sub program menu)

No.14722=8500 (Minimum program number of sub

programs displayed in the milling

machining sub program menu)

No.14723=8999 (Maximum program number of sub

programs displayed in the milling

machining sub program menu)

- 730 -

B-63874EN/05

EXAMPLE OF PROGRAMMING

3.MACHINING CENTER

3.5.6

Entering Tool Changing and Spindle Rotating Blocks for

Finishing Flat End Mill

3.5.6.1

Entering in ISO-code form directly

For pocket finishing, enter commands for operations including

changing tools, specifying the spindle, and approaching the machining

start point.

G28 G91 Z0. ; INSERT

(Z-axis reference position return)

G28 G91 X0. Y0. ; INSERT

(X/Y-axis reference position return)

T02 M06 ; INSERT

(Tool change)

D2 ; INSERT

(Selecting tool data)

M03 S1500 ; INSERT

(Spindle rotation)

G00 G90 G54 X0. Y0. ; INSERT (X/Y-axis approaching)

G43 Z100. H2 ; INSERT

(Z-axis approaching)

3.5.6.2

Entering by fixed form sentence menu

ISO-code form part program can be entered from the fixed form

sentence menu. The already prepared fixed form sentence as

3.MILLING START was made with entering undefined data as “?”,

so it can be used also for finishing.

(Soft-key group for milling cycle menu)

[START]

(INSERT STARTING COMMAND FOR MILLING)

<START>

↓

<<3.MILLING START>>

[INSERT]

NOTE

There may be a case that undefined value is

entered by “?” in the fixed form sentence menu, so

in this case, you need to replace the “?” by proper

value can be used in actual machining.

Place the cursor to the address with “?”, enter

numeric data, then push “ALTER”.

After altering the data, return the cursor to the EOB

at the end of the program.

- 731 -

FANUC MANUAL GUIDE i. OPERATOR’S MANUAL - page 25