okuma OSP100 User Manual

Program construction

Program:

The most controller are using as a job control language the symbols from the DIN66025. After this the partprogram are contains a sequence of lines. A line contains several words. A word contains a letter and a number.

Part program:

N10 G50 S2500 N20 G0 X500 Z500 N30 G0 X50 Z2 T0101 G97 S2500 M3 M8

24

OKUMA

Line:

N20 G0 X500 Z500

Word:

X 500

Address Number

The separate line contains:

• Program technical information.

• Geometrical information.

• Technical information.

24

OKUMA

Program technical information:

For the execution of the program are necessary.

For example : + Plus

— Minus

. decimal point

Geometrical information.

Means motion of some axis in the machine, the

word for the motion is from that address G

( Engl. Word for Go ) and some numbers behind.

The most important G commands are:

G00 positioning

G01 linear interpolation

24

OKUMA

Technical information. F = Feedrate T = Tool S = Spindlespeed M = additional function

For example: F – command = F0.25 ( mm/rpm ) T – command = T0101 ( Tool no. 1 ) S – command = S1000 ( 1000 rpm ) M – command = M03 ( spindle direction CW )

25

OKUMA

Main Address Characters

•N Block Number

• G Preparatory Function (See List)

• X Diameter Value

• Z Length Value

• F Feedrate (mm/min or mm/rev)

• (or Dwell time in seconds)

• S Spindle Speed (m/min or rev/min)

• T Turret Station/Offset Number

• M Miscellaneous Function (See List)

M––

M

M – function are help function, just to switch on some additional function, e.g. coolant on or off, C –axis on or off.

Function

25

OKUMA

Lesson with G01

Program construction for 2 axis lathe machine

G50 S4500

G00 X500 Z500 G00 X0 Z2 T0101 G96 S250 M03 M08

G01 Z0 F0.15 G01 X40

G01 Z-20 G01 X60

G01 Z-50 G01 X100 Z-80

G01 X140 G01 Z-110

G01 X160 G01 Z-130

G00 X500 Z500 M09 M02

Tool command

G Code for constant cutting speed

M- code coolant on

M-code for spindle direction

Cutting speed in m/min

Note

The G00 command means that the machine will move with rapid feedrate , the rapid feedrate

is dependent on the machine. The unit for rapid feedrate is m/min. The G01 command means that the machine will move with feedrate, therefore it is necessary

to program in the first line with G01 a feedrate command. The address for feedrate is ”F ” for example F0.25 = 0.25mm by one rotation of the spindle

OKUMA

Lesson with G85 Lap cycle

Program construction for G85 Lap cycle

G50 S4500

G00 X500 Z500 G00 X160 Z2 T0101 G96 S250 M03 M08

G85 NAP1 D5 U0.5 W0.1 F0.35

F = Feedrate

W = Stock removal in Z U = Stock removal in X

D = Cuttingdepth in diameter

NAP1 G81 G81 = Cutting direction in Z - axis G01 X0 Z0

X40 Z-20

X60 Z-50

X100 Z-80 X140

Z-110 X160

G80 G00 X500 Z500 M09

M02

27

OKUMA

Exercise G85 /G81

28 ( 29 )

OKUMA

Lesson G85 Lap Cycle in X --

Lesson G85 Lap Cycle in X

Blank material D= 162

Direction

Program construction for G85 Lap cycle in X -Direction

G50 S4500 G00 X500 Z500 G00 X162 Z2 T0101 G96 S250 M03 M08 G85 NAP1 D4 U0.5 W0.1 F0.35 NAP1 G82 G0 Z-110 G1 X140 G1 Z-80 G1 X100 G1 X60 Z-50 G1 Z-20 G1 X40 G1 Z0 G80 G00 X500 Z500 M02

Note

Please consider, the G82 contour description start from the spindle and will go in direction of the tailstock.

30

OKUMA

Exercise G85 / G82

31 ( 32 )

OKUMA

Lesson G85 Lap Cycle in Z ––

Lesson G85 Lap Cycle in Z

contour definition

Blank material D= 162

direction with blank

G50 S4500

G00 X500 Z500

G00 X165 Z2 T0101 G96 S250 M03 M08

G85 NAP1 D4 U0.5 W0.1 F0.35

NAP1 G83 G – Code for blank material

G0 X0 Z5

G1 X45

G1 Z-15

G1 X65 Z-45

G1 X105 Z-75 Blank material definition

G1 X145

G1 Z-105

G1 X170

G81 G – Code for longitudinal shape designation

G0 X0 Z2

G1 Z0

G1 X40

G1 Z-20

G1 X60 Z-50 Finish shape

G1 X100 Z-80

G1 X140

G1 Z-110

G1 X160

G1 Z-130 G1 X162

G80

G00 X500 Z500 M02 33

OKUMA

Exercise G85 / G83

)

Exercise G85 / G83

34 ( 35

OKUMA

Lesson G85 Lap Cycle with G84 changing cutting

condition

Blank material D= 162

Program construction for G85 Lap cycle with changing cutting

condition

G50 S4500 G00 X500 Z500

G00 X165 Z2 T0101 G96 S250 M03 M08 G85 NAP1 D4 U0.5 W0.1 F0.35

$ G84 NAP1 G81

G00 X0 Z2 G01 Z0 F0.1

G01 X40 G01 Z-20

G01 X60 G01 Z-50

G01 X100 Z-80 G01 X140

XA=100 ZA=2 DA=1 FA=0.1

Feedrate

Cutting depth Start point in Z for reduction of the cutting condition Start point in X for reduction of the cutting condition

G01 Z-110 G01 X160

G80 G00 X500 Z500

M02

OKUMA