What's new
What's new

Okuma LC10/OSP3000L - Bar feeder options?

Wade C

Stainless
Joined
Jul 21, 2004
Location
Wiggins CO. USA
Any one have experience with these? My book shows it as an option... and Im just trying to do some homework on the idea.

Thanks
Wade
 
see my post a few rows down. Just getting into bar feeding too. Really works slick once you know what youre doing. Do you have a bar feeder or are you thinking of adding one?
RJT
 
Im trying to figure out how to add one... if my control will handle it and so forth. It dosnt like to do much with the chuck open... which adds complxity cause I cant use a bar puller...

I guess likely more day dreaming than reality... but sometimes in day dreaming... you find reality. :D
 
Wade you should be able to use a bar puller. You can't specify the feed in inches per rev and get the turret to move, because the spindle's not turning to generate the "rev" part. So, you have to use in/minute feedrate, which is G ninety-something, for the bar pulling cycle. Usually works better than using G0 for pulling. Just be sure to change back to in/rev on the first cutting line of your code.

If you were using a bar feed whose cycle was triggered by the closing of a switch and controlled from within the bar feed itself, then you might be able to either use a spare relay in the bank of relays that's located on one of the cabinet doors, or add a relay in a spare socket, and trigger it with an M code. But, you'd need to know what unused codes will operate which relays coils. If there was an option for the control itself to initiate and control a bar feed cycle, it would likely be a piece of code on an optional executive tape. You don't even want to price any exec tapes from Okuma. I'll see if I've got a wiring diagram for the LC10 that identifies the functions and codes for the various relays. Do you know if your lathe has programmable chuck opening and closing?

Something I checked on before, but forgot to email you back with an answer is the question about spindle speed. The tach on the panel does have 2 scales on it, but you only use the scale based on the pulley ratios of your specific lathe. There are not 2 speed ranges, so there's no need to put the M41, M42, etc in your code. You could use an optical tach to determine your max spindle speed by making sure you don't have a G50 spindle speed clamp in effect, and then doing something like an M3 S5000 to run it up to whatever max is available.
 
Ill have to do some looking into the programable chuck actuation.. but I dont remember anything about it in the manual back when I was digging though every page trying to learn the machine... cut it just seems it would have to be intertwined somehow, since it knows when its open or closed.

Ive been wondering about a in/min cycle for something else I was wanting to try, so if I can find that in the manual, that will Im sure will explain what I need to know about using it - and applying that to my other use, as well as using it with the bar pulling idea.

Maybe I missed something on the programable chuck actuation - if so, then that might simplify a few things... If not, and the additional relay spots in the relay bank would work with some various codes that appear to be undocumented in the manual I have... I could likely run something in there that will actuate the foot pedal for me. But that would be great if I could add a couple controlled relays to the system, as I have a couple other things Id like to do that would be much easier and much more fun if the control ran them... Like an air mist setup for running some gun drills.

Any info you run into would be greatly appreciated!

Thanks!
Wade
 
I know that G90something is in there... I remember finding one time and asking... but Im not finding it yet... so yif you run across that.... let me know.... I also found a few more codes in the book that are not in the "code list" from the book...

SO I know there are some codes that are there that I dont know about.

Wade
 
I think Mike is right on the G94/G95. I was deleting out an old program today that had a bar pull cycle in it and I'm pretty sure I saw a G94 flying by on its way to the trash can. But, the chuck open/close is definitely M83 and M84. I'll see what else I can find over the weekend.
 
AWESOME!!! ILL give them a try!!!

I know at one point in the book I saw an IPM deal... but for the life of me cant find it. Never have seen anything about the chuck other than the chuck barrier function.

Thanks!!!
Wade
 
Checked out the M83 and 84... Bingo on the chuck...

I see possibilities expanding with every second :D
Still gotta chase down some other codes in manual... Wish some one had the extensive list of codes for the OSP 3000L.. Ill get em chased down one way or another :D I hope
 
Okay... after some Quality Time spent with the manaul, I verified the G94 & G95

I think I can build/design my one bar puller to attach to the turret. Now Im left with one last issue to conjur up a solution for - if there is one.
Can you make the Okuma auto repeat?
I ran across the Q command in the manual, but it didnt make things very clear. (Im probably just too dense) Im wondering if at the end of the program (say program is N100 to N150), instead of the M2 on line N150, would a Q100 start the program over? Assuming that works... would placing the bar pull cycle at the begining of the program or the end of the program prior to the Q be smarter?

In my head, again, assuming the Q command works, it seems, that it might be smart to write a initaial facing program at the begining of the whole program, that would clean up the end of a new rod of material. And to have that portion of the program preceeded with / (optional block delete) so that when I put in a new rod, I would start the program with the "Block Delete" OFF until it got past the optional delete section of the program. Then, have the bar pull cycle, then the actual program, followed up with the Q command instead of the M2. That in my head, would allow me to be less precise when inserting the new blank of material, and it would then run the program, and repeat (knowing that I turned the "Block Delete" back ON after the initial pass.) from there, I would just have to have a rough time of cycle for a full rod, and set my alarm to go off about the time it was done with that last piece or two, and once it finished, hit the "Reset" button when the turret was out of the way(not the Control Reset), load a new rod, and hit start again.

Am I crazy, or is it just wishful thinking that I might be able to do this, so it would cut an entire rod in to my parts theoretically unattended?

Thanks again for being a great source of info, things to ponder, new ideas, and as sounding boards for my own whacky ideas.

Wade
 
I think its M30 at the end if you want it to run forever.

You could make the facing routine the main program and run the part program as a subroutine. That way you can index the cycles and run a specific number of repetitions that use up your bar, and then stop. Be careful near the end of the bar when using a bar puller. If the puller pulls a stub out of the chuck and the cycle continues, that stub can cause a crash when the puller heads to the chuck on the next go-round.

Also, if you specify the number of repetitions as a variable then you can alter the value easily if you need less than a full bar of parts, or if you happen to have bar remnants that are less than full length.
 
Subroutine huh? Ill have to do some digging on that. Im not remembering seeing anything about sub routines... Unless thats what the Q stuff they were talking about was..

Hmmm.. Back to the book :D
 
Its the things where you do the branch and return with codes like G396, G397, etc. I think in the manuals they refer to them as owner's programs or user's programs, or some sort of wierd name like that.
 
boy... I was just starting to wonder about that (and afraid of that)
I skimmed through that when I was looking for verification on the G94-95 codes... and got totally lost. At least I know now where to go to study and try to "interpret" the english.
 
The programming manuals for the 3000 have to be the absolute worst and most confusing collection of words (yes words...most of whats there never makes a coherent sentence) that's ever been put on paper. To make the subroutine section even worse, they mixed in the use of variables which I've never seen mentioned anywhere else in the manual. For a long time I avoided the sub section like the plague and assumed one could only use variables in subroutines and not in the main program. Once you can figure out what the manual says, the actual programming isn't bad at all :D If their stuff wasn't so bulletproof we probably wouldn't still be contending with trying to translate. Most everything else that old is either dead or so obsolete you can't give it away.
 
Any suggestions for the "interpretation"... or any key points that might eliminate any major stumbling blocks in the comprehension?

I really dont have to be able to do this... but I konw me... and good enough is never good enough... but the M30 idea might be a solution to get me to something new and productive shortly, if it works right, and the optionaldelete will be a simple way out. Plus I have no intention to leave it unattended... Ill aways be some where close. Plus the idea I have for the bar puller, may be just less likely to cause a crash if it catches a stub. But I now have more to strive for. ;D

I havent even gotten to applying Constant cutting speed yet.

One question I dont remember if I asked before - and since I have the "Okuma Group's" ( :D ) attemtion, Ill ask now....

Say you were using an Iscar CutGrip, and it has an insert that has .125" wide cut, and .0635" corner radii, and the base portion of the insert is .090" wide (looks kind of like this - I cant remember the letters and numbers of the actual insert)

( )
||

Yeah you have to use your imagination a bit...

When using Rad Tool Comp (G40)... when you specify the I and K, will it work with this type of insert if you used I.0635 and K0.000?
 
Wade,
What you've described is a full radius insert since I'm assuming you mean .0625 for the corners. For a full radius tool I=K=.0625 To get nose radius comp to work correctly, the control needs to know the offset distance from the edge of the cutter to the centerpoint of the corner radius. Lets say you were using a CNMG432 for normal turning. The nose radius is 2/64 or 1/32" You'd set I.0313 and K.0313. The control runs a path as if you're cutting with a radius insert that's 1/16" diameter. Same thing applies to your cutgrip full radius insert.
 








 
Back
Top