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

-------------------------------------------------------------------------------------------------------------------
OBAR2
N1 G50 S3000
G0 X22 Z22 M5
T010101
X.200 Z.02 T010101
M84
G4 F8 (pusher does full retract, so it doesn't whip in the sleeve. Slow to advance, hence the 8 second dwell)
M83
G4 F2
G0 Z1
IF [VDIN[24] EQ 1] N100 (what does this line mean?)
GOTO NRTS
N100 M77
M84
G0 X22 Z22
G4 F8
M436 (what the heck is this?)
M83
M76
G4 F2
G0 X.100 Z.02 T010101
M84
G4 F8
M83
G4 F2
G0 Z1
NRTS RTS

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

-------------------------------------------------------------------------------------------------------------------
OBAR2 (LABEL. Thats an uppercase 'O')
N1 G50 S3000 (SETS MAX RPM May default to zero and spindle won't start)
G0 X22 Z22 M5 (move away from end of job assuming X0Z0 at end. STOP spindle)
T010101 (Tool change)
X.200 Z.02 T010101 (Rapid move relative to tool 1 table settings IMHO)
M84 (unclamp?)
G4 F8 (pusher does full retract, so it doesn't whip in the sleeve. Slow to advance, hence the 8 second dwell)
M83 (Clamp?)
G4 F2 (Pause for clamping. Is this needed?)
G0 Z1 (1 unit inch/metric? from end of job)
IF [VDIN[24] EQ 1] N100 (what does this line mean?) (CLAMPED?)
GOTO NRTS (ABORT PROGRAM I think is check for correct clamping)
N100 M77 (??)
M84 (some canned machining cycle. Not much good if no material removed)
G0 X22 Z22 (RAPID Away from the job. The rest is a mystery)
G4 F8
M436 (what the heck is this?)
M83
M76
G4 F2
G0 X.100 Z.02 T010101
M84
G4 F8
M83
G4 F2
G0 Z1
NRTS RTS

I have had an different model Okuma and are making a few assumptions.

[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.

My M-Code Chart only goes to M362
M76 is Parts Catcher Retract
M77 is Parts Catcher Advance
Could VDIN[24] be the End of Bar signal? I don't have a maintenance manual.

I'm getting to understand some things now I think.
Yes, M77 and M76 are parts catcher adv and ret.
I do a search on the control for M436 and it's blank. Weird!

I think "VDIN[24]EQ 1]" is how many parts till end of bar, and when it sees EQ 1, (last part) it will then go to N100 and perform bar change.

OBAR2
N1 G50 S3000
G0 X22 Z22 M5
T010101
X.200 Z.02 T010101
M84
G4 F8 (pusher does full retract, so it doesn't whip in the sleeve. Slow to advance, hence the 8 second dwell)
M83
G4 F2
G0 Z1
IF [VDIN[24] EQ 1] N100
GOTO NRTS
N100 M77 (parts catcher adv)
M84 (chuck open)
G0 X22 Z22 (turret moves away from chuck)
G4 F8 (pusher pushes new bar 1/2" out of face of chuck pushing remnant from old bar into parts catcher, set by barfeeder settings)

M436 (still don't know)
M83 (chuck close)
M76 (parts catcher ret)
G4 F2 (dwell, prolly not needed, but was there when we got machine)
G0 X.100 Z.02 T010101 (rapids to position)
M84 (chuck opens)
G4 F8 (sigh! wait for pusher to come back and push bar to stop T0101)
M83 (chuck closes)
G4 F2 (dwell)
G0 Z1 (rapids 1" away from part)
NRTS RTS (returns to main proggy)

Thanks for the help guys, this site is awesome.
I still have to figure the barfeeder settings to match this OBAR2 sub program.
The barfeeder manual is converted Italian to english, so it doesn't make alot of sense. Gonna have to call IEMCA monday and talk to support.
Thanks again guys

Craven12

Have you tried entering M436 via MDI to see what happens?

Just had a look in my handbook, even tho it is quite old and is for OSP5000L-G controllers, it lists the inputs for 23~24 as being for External Inputs (EC), so my guess would be that the statement "IF [VDIN[24] EQ 1] N100" is def looking at the End of bar condition.

Have you tried entering M436 via MDI to see what happens?

Yes sir I did, and it didn't seem to do anything. Still puzzled. Gonna call the rep on Monday and see what he has to say.

Craven12

Yes sir I did, and it didn't seem to do anything. Still puzzled. Gonna call the rep on Monday and see what he has to say.

Craven12

Bummer!
Was really hoping that you would see something happen!
But oh well, like you say... time to call for help from Okuma!
Cheers
Brian. (no "Sir" please!)

Bummer!
Was really hoping that you would see something happen!
But oh well, like you say... time to call for help from Okuma!
Cheers
Brian. (no "Sir" please!)


LOL! ok, thanks Brian.

Bummer!
Was really hoping that you would see something happen!
But oh well, like you say... time to call for help from Okuma!
Cheers
Brian. (no "Sir" please!)

Got it!

From Okuma: M436 automatic M Code to do a complete bar change and have the part sticking out to the top cut position. (sometimes M336)

Machine has to be in system link mode for this to work.

Finally! lol

Hi Craven12,
Well OK then, now we know a bit more about the various codes, your program is basically doing this:

Set Maximum Spindle Speed.
Start from Home posn, Spindle off
Select tool 1
Move to posn 0.02 from machined face
Open the Chuck
Wait for bar feeder to advance
Close the chuck
Wait another 2 seconds
Rapid to Z1
Check to see if Bar Feeder is empty, Jump to reload routine if it is
Jump to end of Sub Program if not empty.
N100 Advance the Part Catcher
Open the Chuck
Move at Rapid to Home Posn
Wait 8 Seconds
Change the Bar
Close the Chuck
Retract the Parts Catcher
Wait 2 seconds
Rapid to end of bar posn?
Open the Chuck
Wait 8 Seconds
Close the Chuck
Wait 2 seconds
Move to Z1
Return from Subprog.


I do have some questions however...
Where is Z0 on the job? Is it at the back face?
What is the length of Bar Feed each run?
Does the part move out of the chuck as the tool moves away, or does the tool move and then the chuck opens allowing the material to move out?
There appears to be no ability in your program to allow for varying the barfeed amount.
Hope you can answer these questions as I am curious to know how it is going.
Regards
Brian.

Hi Craven12,
Well OK then, now we know a bit more about the various codes, your program is basically doing this:

Set Maximum Spindle Speed.
Start from Home posn, Spindle off
Select tool 1
Move to posn 0.02 from machined face
Open the Chuck
Wait for bar feeder to advance
Close the chuck
Wait another 2 seconds
Rapid to Z1
Check to see if Bar Feeder is empty, Jump to reload routine if it is
Jump to end of Sub Program if not empty.
N100 Advance the Part Catcher
Open the Chuck
Move at Rapid to Home Posn
Wait 8 Seconds
Change the Bar
Close the Chuck
Retract the Parts Catcher
Wait 2 seconds
Rapid to end of bar posn?
Open the Chuck
Wait 8 Seconds
Close the Chuck
Wait 2 seconds
Move to Z1
Return from Subprog.


I do have some questions however...
Where is Z0 on the job? Is it at the back face?
What is the length of Bar Feed each run?
Does the part move out of the chuck as the tool moves away, or does the tool move and then the chuck opens allowing the material to move out?
There appears to be no ability in your program to allow for varying the barfeed amount.
Hope you can answer these questions as I am curious to know how it is going.
Regards
Brian.

Z0 is the front face of the part. The bar is fed 1.58" per push to the stop T0101.

The pusher keeps pushing till it hits the stop. (bar feeder settings) Then stop moves away after chuck closes.

During a bar change, the bar feeder is set up to push a new bar to .5" out of face of chuck. (top cut position) This also pushes the remnant out into the catcher. If the stop was there it would interfere with the remnant ejection.
The cycle then starts over.

It's early in the am barely awake yet, so I hope I made sense LOL.
I`m hoping it all goes good today.

Mike

I have an okuma l470m. osp-e100l
if you touch the "i" button (touchscreen) in the upper right hand corner of the screen, you can punch in whatever g or m code and it will tell you what it does. Also, if the machine throws an alarm, you can push the same button to tell you what the alarm code is for, why it happened, and how to fix it.

HTH

Hi Mike,
Thanks for the cycle description!
Program makes a hell of a lot more sense now.
So are you happy with the program or are you looking to "improve" it anyway, ie variable barfeed positions etc... or were you just hunting for clarification on your program only?
The "i" button as described by kazmir44 is a very handy button to use when learning! Pound it lots to look for any answers to a multitude of areas, basically it should contain your manuals online for you.
Mind you the alarm information is just the same as looking in the book, which sometimes is as good as reading tea leaves etc! i.e. Alarm A! Some thing is broken!
Gee Really? Had not figured that, seen as the whole system is stopped!
Mind you, do read the entire alarm message as quite often I am faced with an alarm on the machines here and the guys only read half of the information and wonder why they don't understand what the problem is! Got one apprentice that has blonde hair and totally "blonde" outlook on everything to go with it, if you know what I mean!
Had a fairly straight forward alarm the other day that the answer was straight forward, once he read the entire line! Took him 5 minutes with me telling him to read it again before he realised! Doh!!
Cheers
Brian.

I have an okuma l470m. osp-e100l
if you touch the "!" button (touchscreen) in the upper right hand corner of the screen, you can punch in whatever g or m code and it will tell you what it does. Also, if the machine throws an alarm, you can push the same button to tell you what the alarm code is for, why it happened, and how to fix it.

HTH

I tried that "i" button, and searched for m436, it did come up, but the description was blank.

That "i" button sure is handy though.

Mike

Hi Mike,
That was a tough break for you then!
I had thought that you would have searched for the M code defn this way, but it does seem strange that there is no defn for it on the "i" pages!
Bummer!
Cheers
Brian.

Hi Mike,
Thanks for the cycle description!
Program makes a hell of a lot more sense now.
So are you happy with the program or are you looking to "improve" it anyway, ie variable barfeed positions etc... or were you just hunting for clarification on your program only?
The "i" button as described by kazmir44 is a very handy button to use when learning! Pound it lots to look for any answers to a multitude of areas, basically it should contain your manuals online for you.
Mind you the alarm information is just the same as looking in the book, which sometimes is as good as reading tea leaves etc! i.e. Alarm A! Some thing is broken!
Gee Really? Had not figured that, seen as the whole system is stopped!
Mind you, do read the entire alarm message as quite often I am faced with an alarm on the machines here and the guys only read half of the information and wonder why they don't understand what the problem is! Got one apprentice that has blonde hair and totally "blonde" outlook on everything to go with it, if you know what I mean!
Had a fairly straight forward alarm the other day that the answer was straight forward, once he read the entire line! Took him 5 minutes with me telling him to read it again before he realised! Doh!!
Cheers
Brian.

Hey Brian, Like I said in my first post, I have zero experience with an Okuma. I am used to Fanuc. The other 2 Lathes we have are an old Wasino circa 1983..lol and a 2006 Nakamura Tome, both with Fanuc. This is all I know. So learning the OSP control has been fun. It will be alot nicer I can tell that. Should have seen me scratching my head how to send the turret home. Lo and behold, I did not have to with the Okuma.

So yeah, to answer your question, I was just looking for clarification on the sub program for the barfeeder. The main program was easy, I used Gibbs to create it. IGF is pretty cool, gonna take some time getting used to programming right at the machine. I've used Gibbs for so long I may keep doing just that, it's real quick.

Today I got everything working great. It mainly was an operator error (IE: ME!)
I had the barfeeder settings all messed up. Talked to the support guy and got it going soon after. Now I'm ripping off parts like I'm ripping off Farts!..lol

Anyways thanks again for the help guys. I may need you again.

Mike

Hi Mike,
Great to hear (and NOT smell) that you have got it all sorted! hehehe
Keep going with programming via Gibbs as programming at the machine gets pretty tired after awhile!
Not to mention Gibbs would be able to give you a hell of a lot more "what if" choices whtn doing the program.
Glad I could be of help to you.
Regards
Brian.