11 replies to this topic

[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.