[quote=craven12;403215]2003 Okuma Captain L370M OSPE100L, IEMCA VIP 80 Barfeeder.
Hi folks, new to this site. For the last 10 years I have run Fanuc controls. We now have a used Okuma, which I have no
experience with. This is a SSB file that was with the machine when we got it. I am trying to understand it. It's for
the barfeeder. Can someone explain what some of the commands mean? G and M codes (except for the M436, I can't seem to find what that is) I do know, but VDIN, NRTS, RTS, I don't know.
Any help would be appreciated.
Craven12
-------------------------------------------------------------------------------------------------------------------
(Making the assumption this program is Imperial)
OBAR2 (sub program name, ie what is called from the main program)
N1 G50 S3000 (max spindle speed)
G0 X22 Z22 M5 (Rapid to Home posn and stop the spindle)
T010101 (select tool 1, Tool Nose Rad comp for 1 and Offset 1)
X.200 Z.02 T010101 (move to posn making sure tool 1 is selected first)
M84 (open the chuck)
G4 F8 (pusher does full retract, so it doesn't whip in the sleeve. Slow to advance, hence the 8 second dwell) (well you know the answer here already)
M83 (Close the chuck)
G4 F2 (wait another 2 seconds)
G0 Z1 (rapid to Z posn)
IF [VDIN[24] EQ 1] N100 (this is checking an input to see if it is on or not)
(to find out which one you need to have the maintenance manual)
(if the input is ON then it will jump to line N100)
GOTO NRTS (unconditional jump to line NRTS)
N100 M77 (what does M77 do when input via MDI?)
M84 (open the chuck?)
G0 X22 Z22 (rapid to home position, but if M84 is Chuck open then lookout!)
G4 F8 (wait 8 seconds)
M436 (what the heck is this? Have you tried via MDI to see what happens? With hand near E-Stop!)
M83 (close chuck)
M76 (Try via MDI to work out this M Code)
G4 F2 (wait 2 seconds)
G0 X.100 Z.02 T010101 (rapid to XZ position with tool 1)
M84 (chuck open)
G4 F8 (wait 8 seconds)
M83 (chuck Close)
G4 F2 (Wait 1 second)
G0 Z1 (rapid to Z1)
NRTS RTS (RTS means ReTurn from Sub, Equivalent of Fanuc's M99)
I would suggest that you try in MDI mode some of the M codes to see what they do, then the process of decoding the program will be much easier!
If this program is to be used for barfeeding it seems to contain some rather strange coding and movement values.
The SSB file I created for barfeeding is much easier to follow...
Program is written for a maetric system!
The call to the program contained several variables allowing the user to select the barfeed tool number, length to feed out, Diameter at which the tool is to be positioned at and the position at which the "cut" face is located at.
the G94 allows the machine to move in feed mode without the spindle rotating! (feed per minute rate rather than G95 feed per rev)
$B-FEED.SSB%
SUBPROGRAM OBARF USED FOR BAR FEEDING IN LCS15 ONLY
LAST UPDATED 29/08/97 BJR
TO USE, COPY FOLLOWING LINE INTO MAIN PROGRAM
CALL OBARF LEN=84.5 CUTP=-2.5 TOOL=505 DIAM=05
OBARF
N1 G0 X600 Z600
NBARF T=TOOL
N3 X=DIAM Z=LEN+5
N4 Z=CUTP
N5 M84
N6 G1 G94 Z=LEN+0.5 F3000
N7 G4 F1
N8 M83
N9 G0 G95 X600 Z600
N10 RTS
Hope some of this makes sense!
If not... oh well, one but can try eh!?!
Cheers
Brian.  |