Okuma mill

[DODGERFAN]

Does anybody have a sample of a okuma mill sub program using the 4th axis? Any help would be appriciated.....

now back to

[chris m]

I would use MODIN for something like that.

 

Your main program would say something like this:

 

N206

( T06 )

( 1/2 2FL CARBIDE STUB EM )

( ROUGH POCKETS )

G00 G17 G40 G53 G80 G90 G95

G30 P1

IF[VATOL EQ 06]NS206

T6 M06

NS206

G15 H20

X0. Y1.11 A0.

S1736 M03

G56 H6 Z.25 M08

MODIN OPCKT

G00 X0. Y1.11

G00 A90.

G00 A180.

G00 A270.

MODOUT

G00 Z.25

G53 M09

G30 P01

M01

 

Your subprogram (after the M30 but before the %):

 

M30

OPCKT

 

( your code here )

 

RTS

%

 

Hopefully this is what you were looking for

 

C

[Goldorak]

simple

 

 

G15H1 (work offset #)

T1M6

S5000M3

G56G00X0Y0Z3M12

A0 (Angle value of A axis)

CALL OPKT (Call the sub program)

G00Z3 (retract to clear the part)

A90

CALL OPKT

G00Z3

A180

CALL OPKT

G00Z3

...

M9

M30

OPKT (sub progran name)

***INSERT POCKET CODE HERE***

RTS (return to main prog)

%

[DODGERFAN]

Thanks guys, it helped alot

[chris m]

Martin, what drives your decision to go the "CALL" route over MODIN? Is there something that works better that way, or is it just personal preference?

 

C

[Goldorak]

i never use the MODIN, i always used CALL for subroutines on our OKUMA

 

i can't really tell the difference

[DODGERFAN]

here are the parts i'm programming. The green hinges are the parts.

[T_MALENA]

Goldorak & Chris M. I always thought the CALL OMILL was to run the program for that instance only & no need to cancel. The MODIN OMILL will run the OMILL program at each program line following the MODIN until it reads a MODOUT - kind of like a G81 cycle is modal until reading G80.

 

Call OPKT needs to be entered at each A-axis move

 

G56G00X0Y0Z3M12

A0 (Angle value of A axis)

CALL OPKT (Call the sub program)

G00Z3 (retract to clear the part)

A90

CALL OPKT

G00Z3

A180

CALL OPKT

G00Z3

 

 

 

MODIN OPKT will cut at each line after reading MODIN.

 

MODIN OPCKT

G00 X0. Y1.11 1st

G00 A90. 2nd

G00 A180. 3rd

G00 A270. 4th

MODOUT

G00 Z.25

 

 

Boy I thought I was correct all this time. Is this how you guys use it?

[chris m]

You are exactly right. We typically use MODIN, but I can see using CALL if you weren't simply running back-to-back-to-back features:

 

CALL OPCKT

Do some other milling and move to a different location

CALL OPCKT

Do something different and move to another location

CALL OPCKT

 

This would not work with MODIN. However, if you were going to mill the same feature [50] times in a row, MODIN is really the way to go because it works (like you said) similarly to a canned cycle.

 

C

[Goldorak]

I learned something today

[Bob_Looney]

You can also use Q to repeat the sub call. Example below uses VC1 to hold work offset, starting at H1. Safe lines are in the sub.

/////////////

 

(NOTES:)

G15 H1 VC1=1

IF [VATOL EQ 8] NATA

T8 M06 (2.500 DIA. FACE MILL)

(SANDVICK)

NATA G00 G90

M01

T1

X7.125 Y0.0

CALL OSUBA Q2

G15 H1 VC1=1

IF [VATOL EQ 1] NATB

..............

OSUBA (TOOL 8; 2.500 DIA. FACE MILL)

(SANDVICK)

NSA

G15 H=VC1

IF [VC1 LE 0] NDA

IF [VC1 GT 2] NDA

G00 X7.125 Y0.0 S764

M12

G56 H8 D8

Z0.5 M03

Z0.1

G01 Z0.0 F22.9

X-7.125

G00 Z0.5

M09

VC1=VC1+1

NDA

RTS

OSUBB (TOOL 1; 1.000 DIA. END MILL)

[Bob_Looney]

On another note, I would get rid of the M6 tool change call and replace it with the Okuma tool change macro and use a G code macro for tool changes. Gets rid of the IF[VATOL] statements. The code shown above is older.