1 modul cnc lathe v1.2

49

EXAMPLE 2
Make CANNED CYCLE programs G71 and G70 for the tool paths shown in Figure 2.

Figure 2.
50

PROGRAM DESCRIPTION

:1234; Program number ( ; = end of block sign)

N10 G28 U0. W0.; Tool Return to home position

N20 G92 S3500; G92 = maximum spindle speed. (N = block number)

N30 T101; Automatic tool change, change tool to no 3,

Roughing/finishing tool

N40 G96 S150 M03; CONSTANT SURFACE SPEED CONTROL (CSS) 150M/min,
spindle turn clockwise (refer: page 26 table)

N50 M08; Coolant on

N60 G00 X66. Z5.; (PSTART); Tool move from Home position to Pstart

N70 G71 U1. R0.5; Canned Cycle, Stock removal in turning first block

N80 G71 P90 Q200 U0.5 W0.1 F0.2; Canned Cycle, Stock removal in turning second block

N90 G42 G00 X16. Z5.; P1, G42 - tool nose radius compensation: right

N100 G01 X16. Z0.; P2

N110 G01 X20. Z-2.; P3

N120 G01 X20. Z-13.; P4

N130 G02 X24. Z-15. R2.; P5 ( R = arc radius )

N140 G01 X30. Z-15.; P6

N150 G01 X40. Z-45.; P7

N160 G01 X46. Z-45.; P8

N170 G01 X50. Z-47.; P9

N180 G01 X50. Z-60.; P10

N190 G01 X60. Z-60.; P11

N200 G40 G01 X66. Z-60.; Pend, G40 - tool nose radius compensation: Cancel

N210 G70 P90 Q200 F0.15; Canned Cycle, Finishing cycle

N220 G28 U0. W0.; Tool Return to home position

N230 M09; Coolant off

N240 M05; Spindle Stop

N250 M02; End of Program

51

G74 – END FACE PECK DRILLING CYCLE

G74 R__;
G74 Z__ Q__ F__;

R: peck lift off (retract volume)
Q: Cut volume in Z axis (Q5000=5mm)
Z: final depth in depth
F: Cutting feedrate

Example:
G74 R1;
G74 Z-65 Q10000 F0.15;

52

PROGRAMMING EXAMPLE: G74 – END FACE PECK DRILLING CYCLE

:1234; (DRILL ); N140 G40 G01 X81. Z-50.;
N10 G28 U0. W0.; N150 G70 P90 Q140 F0.15;
N20 G92 S3500; N160 G28 U0. W0.;
N30 T101; (Roughing/finishing tool) N170 T303;(Drill ø12mm)
N40 G96 S180 M03; N180 G97 S1000 M03;
N50 M08; N190 G00 X0. Z5.;
N60 G00 X81. Z5.; (PSTART); N200 G74 R5.;
N70 G71 U1. R0.5; N210 G74 Z-40. Q5000 F0.15;
N80 G71 P90 Q140 U0.5 W0.1 F0.2; N220 G00 X0. Z5.;
N90 G42 G00 X44. Z5.; N230 G28 U0. W0.;
N100 G01 X44. Z0.; N240 M09;
N110 G01 X50. Z-3.; N250 M05;
N120 G01 X50. Z-50.; N260 M02;
N130 G01 X80. Z-50.;

53

G75 – GROOVING CYCLE

G75 R__:
G75 X__ Z__ P__ Q__ F__:

R: peck lift off in X axis
X: final depth in X axis
Z: final depth in Z axis
Q: tool feed increment in Z axis (P1000= 1mm)
P: Cut volume or X axis (Designate the radius)(Q5000=5mm)
F: Cutting feedrate

Example:
G75 R1;
G75 X96 Z-70 P1000 Q6000 F0.15;

54

PROGRAMMING EXAMPLE: G75 – GROOVING CYCLE

:1234; (groove); N140 G70 P90 Q130 F0.15;
N10 G28 U0. W0.; N150 G28 U0. W0.;
N20 G92 S3500; N160 T202;(cut off/grooving tool)
N30 T101; (Roughing/finishing tool) N170 G96 S180 M03;
N40 G96 S180 M03; N180 G00 X101. Z5.;
N50 M08; N190 G00 X65. Z-23.;
N60 G00 X101. Z5.; (PSTART); N200 G75 R1.;
N70 G71 U1. R0.5; N210 G75 X40. Z-30. P5000 Q2000 F0.15;
N80 G71 P90 Q130 U0.5 W0.1 F0.2; N220 G00 X65.;
N90 G42 G00 X60. Z5.; N230 G28 U0. W0.;
N100 G01 X60. Z0.; N240 M09;
N110 G01 X60. Z-70.; N250 M05;
N120 G01 X100. Z-70.; N260 M02;
N130 G40 G01 X101. Z-70.;

55

G76 – COMPOUND TYPE THREAD CUTTING CYCLE

G76 P (m) (r) (a) Q (Ddmin)R (d);
G76 X(u) Z(w) R(i) P(k) Q(Dd) F(f);

P(m) : Repeating time before the final thread
(r) : Chamfering at the end part of thread
(a) : Angle between threads
Q(Ddmin) : Minimum cutting depth. (0.05mm is written 50 and 0.1 mm is written 100)
R(d) : Finishing allowance
X(u) : Core diameter of thread
[X = Outer diameter of thread – (height of thread x 2)]
Z(w) : Z coordinate at the end point of thread process
R(i) : Taper thread cut value
P(k) : Height of thread(P900=0.9mm) [Core diameter of thread, P (k) = 0.65 x Pitch]
Q(d) : depth cut in first pass (0.5mm is written 500) the radius value
F(f) : Cutting feedrate(Lead of the thread or pitch)

56

Example:
G76P021060 Q50 R0.025;
G76 X37.6 Z-40 R0 P1200 Q500 R0 F2;

57

PROGRAMMING EXAMPLE: G76 – COMPOUND TYPE THREAD CUTTING CYCLE

:1234; (THREAD ); N140 G40 G01 X51. Z-80.;
N10 G28 U0. W0.; N150 G70 P90 Q140 F0.15;
N20 G92 S3500; N160 G28 U0. W0.;
N30 T101; (Roughing/finishing tool) N170 T404; (external thread tool)
N40 G96 S180 M03; N180 G97 S1000 M03;
N50 M08; N190 G00 X30. Z5.;
N60 G00 X51. Z5.; (PSTART); N200 G76 P21060 Q50 R0.025;
N70 G71 U1. R0.5; N210 G76 X26.75 Z-30. R0. P1625 Q500 F2.5;
N80 G71 P90 Q140 U0.5 W0.1 F0.2; N220 G00 X30. Z5.;
N90 G42 G00 X24. Z5.; N230 G28 U0. W0.;
N100 G01 X24. Z0.; N240 M09;
N110 G01 X30. Z-3.; N250 M05;
N120 G01 X30. Z-80.; N260 M02;
N130 G01 X50. Z-80.;

58

Practical task 1

Process Facing process, outside diameter process

Dimension Ø46 x 60L

Material S45C

G90 X Z R G90 X Z R

Pstart P7

P1 P8

P2 P9

P3 P10

P4 P11

P5 Pend

P6

59

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

60

Practical task 2

Process Facing process, outside diameter taper process

Dimension Ø100 x 80L

Material SUS304L

G90 X Z R G90 X Z R
61

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

62

Practical task 3

Process Facing process, outside diameter process (R process)

Dimension Ø80 x 100L

Material Aluminium 6061

G90 X Z R G90 X Z R
63

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

64

Practical task 4

Process Facing process, outside diameter taper process (R process)

Dimension Ø120 x 80L

Material SKD 11

G90 X Z R G90 X Z R
65

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

66

Practical task 5

Process Facing process, outside diameter taper process, drilling process

Dimension Ø50 x 60L

Material AISI 1020 Low Carbon Steel

G90 X Z R G90 X Z R
67

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

68

Practical task 6

Process Facing process, outside diameter process (groove process, R process)

Dimension Ø30 x 50L

Material AISI 1018 Low Carbon Steel

G90 X Z R G90 X Z R
69

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

70

Practical task 7

Process Facing process, outside diameter process (groove process, chamfering R process,
Dimesion thread process)
Ø120 x 140L

Material AISI 1020 Low Carbon Steel

G90 X Z R G90 X Z R
71

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

72

Practical task 8

Process Facing process, outside diameter process (groove process, chamfering R process,
Dimesion thread process, drill process)
Ø100 x 130L

Material AISI 1020 Low Carbon Steel

G90 X Z R G90 X Z R
73

N10 N260
N20 N270
N30 N280
N40 N290
N50 N300
N60 N310
N70 N320
N80 N330
N90 N340
N100 N350
N110 N360
N120 N370
N130 N380
N140 N390
N150 N400
N160 N410
N170 N420
N180 N430
N190 N440
N200 N450
N210 N460
N220 N470
N230 N480
N240 N490
N250 N500
N510

74

14. PROCEDURES: EXL-WIN 7 SIMULATION SOFTWARE

Complete example turning – manual program generation

In this part of the help are included the following sectors:

1. Create a new project for turning 2. Blank definition
technology
4. Defining the position of the coordinate
3. Selection of the tools system

5. Manual creation of the NC-program 6. Simulation

Problem

Picture 15-3: Drawing of the shaft
The shaft material is C 15. All indicated dimensions are dimensions with the medium
dimensional variation. The following profiles are to be machined:

 The outside profile,

75

Steps to prepare the project
It is recommended for beginner to develop a NC-sketch from the drawing. The
experimented users can use directly the drawing.
The the following three steps from a drawing to a sketch are:

 Defining the position of the coordinate system
 Marking all contour points and centres
 Develop a NC-sketch
1. Create a new project for turning technology
Select and double click > EXL-WIN Start With Management
Press pull down menu > Project > management and Project > New

Create New Project dialog box > key in Project name, example: Latihan1 > Apply and select
for control – Fanuc OTB

76

2. Blank definition

As blank, round bars cut to size with the dimensions ø 60 x 125 mm are to be used
Click pull down menu > Change To >Blank

125
60

A dialog window opens for entering the dimensions. After entering the length 125 mm, the
Diameter 60 mm, the material can be selected when pressing the pull-down button. The
inputs are confirmed and saved when pressing the button > OK.

3. Selection of the tools

The tool data must exactly be defined to get a practicable simulation.

Following tools shall be used for the work piece “Shaft”:

Outside profile: Roughing turning tool 80 0-indexable insert

You can call up the box for entering the tool management data with a click pull down menu,
Change To> Tool Memory > Empty Turret > Turret 12 > Load
Find required tools on complete tools window > click and drag the tool to tool changer
window.
(example: Roughing turning tool 80 0-indexable insert to T1) > Corrections > Measure >
Close > Close.

77

4. Definition of the programming zero point (click until zero point move to required

Click > Zero Point > Set default zero point icon
origin).

5. Manual creation of the NC-program
Click pull down menu, Window > User’s Defined View 3
Move to NC Editor Window > Key In Programming Code > File > Save As > Key in file name
- :1234
For a good assignment between the Program Number and the NC program, both should
have a same name.

78

PROGRAM DESCRIPTION
:1234; Program number ( ; = end of block sign)
N10 G28 U0. W0.; Tool Return to home position
N20 G92 S3500; G92 = maximum spindle speed. (N = block number)
N30 T101; Automatic tool change, change tool to no 3,
N40 G96 S150 M03; CSS 150M/min, turn clockwise
N50 M08; Coolant on
N60 G00 X66. Z5.; (PSTART); Tool move from Home position to Pstart
N70 G71 U1. R0.5; Canned Cycle, Stock removal in turning first block
N80 G71 P90 Q200 U0.5 W0.1 F0.2; Canned Cycle, Stock removal in turning second block
N90 G42 G00 X16. Z5.; P1, G42 - tool nose radius compensation: right
N100 G01 X16. Z0.; P2
N110 G01 X20. Z-2.; P3
N120 G01 X20. Z-13.; P4
N130 G02 X24. Z-15. R2.; P5 ( R = arc radius )
N140 G01 X30. Z-15.; P6
N150 G01 X40. Z-45.; P7
N160 G01 X46. Z-45.; P8
N170 G01 X50. Z-47.; P9
N180 G01 X50. Z-60.; P10
N190 G01 X60. Z-60.; P11
N200 G40 G01 X66. Z-60.; Pend, G40 - tool nose radius compensation: Cancel
N210 G70 P90 Q200 F0.15; Canned Cycle, Finishing cycle
N220 G28 U0. W0.; Tool Return to home position
N230 M09; Coolant off
N240 M05; Spindle Stop
N250 M02; End of Program

6.Simulation
 Pull down menu, Simulation>Full Sequence ( F9 ) , The program is completely executed

Or;
Pull down menu, Simulation>Single block ( F8 ) , The program is executed step by step. The
next block will be executed only after pressing the icon or the key ( F8 ).

79

15. MACHINING PROCEDURES

a. Turn On CNC Machine
- Turn Counter Clockwise Main Power Isolator
- Turn Counter Clockwise Machine Power Isolator
- Press Green Control ON Pushbutton – Wait For 20 Second
- Press POS Button
- Release Emergency Stop Button
- Press Green Control ON Pushbutton

b. Handle Mode
- MANUAL MODE – Select X Or Z Axis – Select Handle Speed, X1, X10 OR X100 –
Turn clockwise or counter clockwise Manual Pulse Generator (MPG)

c. MDI Mode
- Command Tool– MDI MODE – PROG – Key In Tool No: T0101 – EOB – INSERT –
CYCLE START
- Command Spindle – MDI – PROG – Key In Spindle Speed: S1500 – MO3 – EOB –
INSERT – CYCLE START
- Spindle Stop – MDI – PROG – Key In: MO5 – EOB – INSERT – CYCLE START
- Move to Home Position – MDI – PROG – Key In: G28 U0 W0 – EOB – INSERT –
CYCLE START

d. Program Editing (Key In New Program)
- Press EDIT MODE – PROG – DIR
- Key In Program Number, Example O1234
- Press INSERT – EOB – INSERT
Or Transfer Data Using RS232 Cable
i. Machine Setting
- Press EDIT MODE – PROG – DIR
- Key In Program Number, Example O3323
- Press – + – READ – EXEC
- Lsk Bleeping

ii. Computer Setting
- Press EDIT – DATA TRANSFER – READ OUT – SELECT
- Select File Number, Example : O2236
- Press START

80

e. Checked Graphic
- Set Federate Override To 0%
- Press AUTO MODE – GRAPH (On Controller) – GRAPH (On Monitor) – OPRT –
EXEC

f. Geometry Offset Setting

i. Z Axis Setting
- Move Tool To Work Piece Z Axis Surface
- Press OFFSET SETTING – OFFSET – GEOM
- Move Cursor To The Tool No Required
- Key In The Work Piece Face Position, Example Z0.0 – Press MEASURE

ii. X Axis Setting
- Move Tool To Work Piece X Axis Surface
- Press OFFSET SETTING – OFFSET – GEOM
- Move Cursor To The Tool No Required
- Key In The Work Piece Diameter, Example X50.0 – Press MEASURE

iii. Offset setting confirmation
- Call required tool, example : T0101 – EOB – INSERT – CYCLE START
- MDI – PROG – Key In: G00 X60 Z0 – EOB – INSERT – CYCLE START
- TURN FEEDRATE OVERIDE TO 1%

g. Auto Cut
- Press EDIT MODE
- Select File Number, Example : O4223
- Press AUTO MODE – CYCLE START
- Set Federate Override To 100%

h. Turn Off Machine
- Push Emergency Stop Button
- Press Red Control OFF Pushbutton
- Turn Clockwise Machine Power Isolator and Turn Clockwise Main Power Isolator

81