G & M Code List For Okuma OSP3000L

Does anybody have a link for the G&M code list for the Okuma OSP3000L?

Thanks in advance

You won't find that online. There are two manuals that cover programming for a 3000L. Basic programming is publication # 2021-E, and the optional functions are covered in 2028-E. You may find these on Ebay sometime, but its doubtful. Most okuma manuals showing up there are for 5000 controls. Unless you've already got it, there's another manual you'll also need. # 2022-E is operation and maintenance, and its the one that tells you how to operate the control as far as setting offsets, entering programs, etc. Last time I bought an okuma manual, they were $150 each. A simple list of the codes would be almost useless by itself. If there's some specific code you need to know, let me know and I'll answer if I can.

metlmunchr - thanks for the reply

I just started a new job and they have me on the Okuma with the OSP3000L.

I have the manual sitting next to me and I was typing out all the G&M codes for my reference notebook...

I never did take typing in High School because back then you only needed to type if you owned/used a typewritter

I was just looking for an easier way - copy & paste - to get it all down so I could print it out.

In 2021-E there is a complete list of codes beginning on Pg 21 and continuing thru Pg 31. Each one has a brief description of what it does. In mine, as few like G75 and G76 (corner radiusing and chamfering) are omitted, but most everything is there and in a language that's a whole lot closer to English than a lot of their manuals from that era

WOuld anyone be willing to post up thier list of G and M codes for the OSP3000?
I have one manual that has some of them, but its not a very long list, which makes me pretty sure that it is incomplete.
I just got an Okuma LC10 with the OSP3000 and am new to CNC/NC stuff.
Thanks
Wade

There is a little book called "the Okuma operators pocket ref book". I have a late model control, but I am under the impresion that not to much has changed in regards to the assinments of various G and M codes. These books are avalible from all Okuma dealers and service people that I have come in contact with. I wouldn't think they are very costly if they wern't giving them away, certanly not like a manual, but the info given is basic. Real handy at the machine.
Here is a web site that teaches Okuma lathe at BYU university. It has a list you may be able to use.
http://class.et.byu.edu/mfg230/CNC_code/okuma_code_index.htm
Good luck
Tim

Wade, the codes by themselves would be useless. The codes with explanations of what they do and how to use them is precisely what comprises the two programming manuals I mentioned above, and 300+ pages is a little long for a post here

Which manual do you have now? There should be a number on the front, along with a title.

Do you know what programming options it has, such as LAP or User Task? If it hasn't been misplaced, there should be a build sheet somewhere in the control cabinet that shows what programming options the machine has. Its a single sheet of paper with the model and serial number at the top.

Depending on what's there, you may or may not need the options manual. The operator's manual is an absolute necessity, because without it the likelihood of figuring out how to enter an offset, a parameter, or most anything else would be remote. I can tell you from experience it ain't intuitively obvious

If you don't find the build sheet, post that info and I can post a couple simple programs that will tell you whether or not LAP and UT are in the control or not. But, prior to that, its a necessity to familiarize yourself with how the control operates, and how to enter a program from the panel into memory.

Thanks so much for the info, and willingness to help... CNC wise, Im a complete self proclaimed and proven professional idiot. I have a book that is really thick, with the cover missing... - okay went and got what I have. I have a book with sections in it numbered 2023-E (Intro to your NC lathe) then the next section is 2020-E Programming manual for LC10 with OSP3000L then 2022-E Operations and Maintenance then 2028-E Instructional Manual for Optional functions. I also have a manual for the 5000L but havent gotten into it at all yet for fear of confusing myself with minute differences. I have been through there prety well, and have a list of what I could get from the book... and I have a pretty good understanding on whats going on, and setting some settings... zero offset, tool offset, softwired limit switches, using the manual (manual has an error in it on manual spindle control... found that the hard way) and tonight I dinked with the MDI... and I was very able to use the MDI to do things one chunk at a time... but there are some things about the DRO vs Actual that were messing with my mind... and still are.... Ill get into that later, as I dont want to hijack Longhair's post too badly. Anyway... I seem to have some of the basics understood, and can actually set some of the parameters without consulting the bible, but I have yet to figure out how to manually enter a program ans get it saved into memory to use on auto - memory. My main reason for interest in others lists of gcodes is the way my manuals are, there looks like there are gaps... and I want to fill the gaps so I can learn the right codes while Im learning. Most of my stuff will be done with plastic and aluminum, but it all has very weird curves, radii, tapers, stepped bores, and finish quality is a major concern. I compensated for the backlash on X tonight (Z was dead on with my .0001 indicator give or take .00005) - which was surprisingly easy considereing my mental status ie wet behind the ears with CNC).

I would love to talk with you some more in depth on some things, if you would be willing to take the time. I can start a new thread, or if you want to move to email or phone... Im good with that as well. I also realize there is something to be said for fighting through something on your own... So Im not giving up, just looking for a little nudge in the right direction. Ive probably read the answer to my problems twice and just didnt understand enough to realize it... yet.

My biggest problem is I live 200 miles from anything "civilized" so getting someone out here to help/train me is a killer on the ole pocket book. So any help you may be willing to offer would be greatly appreciated. I could go on and on with questions, but I doubt you all want to have to read through me fighting my way through learning how to use this machine and then figuring out how to make the damn Easytalk Plus 6.53 work with the DTE on this thing... If I can just get a program in memory, Ill have a good start....

Thanks again! and sorry for the ramble/thread hijacking.

Wade C
wade at webfoot custom calls dot com

[ 10-01-2005, 12:11 PM: Message edited by: Wade C ]

Wade, I'll try to help you with this tomorrow. Getting ready to hit the bed, and at 2am my mind is fuzzy enough that most anything I might tell you right now would be most likely wrong. For now, one thing for sure though is to forget about the 5000 manual. There are way too many differences for that manual to be anything but a source of confusion to you.

Another thing....the DRO will only be accurate on tool position 1 if you start out in manual mode. For it to be correct in any other tool position, you have to do the toolchange via MDI and not the index button on the panel. What happens is when a toolchange is called in MDI, or in a program, you've driven the turret to the soft limit and indexed it. Then, on the next x or z move, rapid or feed, the first thing that happens is the offset for that tool position is enabled. None of this happens when you're in manual mode. However, you can MDI the toolchange and spindle on, then push the manual button, and you can now make manual moves with the wheel or buttons and your readout will show the correct tool position, since it maintains the current offsets until the control is reset. However, once you're in manual, pushing the MDI button again will effectively reset the control, so using multiple tools manually and enabling the offsets for them as you go would be a pain in the butt. Its best to avoid manual or MDI mode except during setups if at all possible. One mis-move in either, especially if you're close to the chuck, is a recipe for a crash. We won't discuss how I know this, but I promise you its true

I knew it was too late to be thinking. Even tool 1 has to be called via MDI unless you use the zero offsets feature to make tool #1 offsets equal to zero. I normally keep a turning tool in #1, and set the zero offsets as above. That way the readout does correspond to actual position of tool 1 when you bring the control up in manual mode.

Thanks for the reply, and dont hurry or worry on my account. I realize this stuff takes time. Yes Im anzious to know everything there is to know, but I am realistic enough to know its not going to happen that fast.

Ill have to check and see if maybe I set the offset on T01 and then changed to T02... I dont remembmer, and since 1 and 2 are the same tools, i could have easily messed that up. Ill check that tomorrow when I get back home from opening day of duck season. Its only 12:30 here and I need to go load the pickup, so Im gonna get that done and then get up early and chase some quackers.

Thanks again. I also posted a new thread with three of my "dumb questions" incase people want to reply, instead of hounding any particular individuals uuntil they get so sick of me they cant see straight.

Cheers, and have a good night!
Wade

Okay, I have the MDI to memory figured out... Not so obvious in the book... but now that I know, the book makes it seem a bit more obvious than it did to start with. DOnt quite have the handle on multiple programs in the mahcine and choosing from them... but I think I can get that figured out.... just take alittle more time. SO scratch that from the question list..

To add another program, go to the last line in the last currently entered program, move the cursor to just ahead of the *, enter another *, which will then move to the next line. Add a % in front of that * and proceed as usual. To scroll thru programs, you can just go into edit and hit % and <word search> repeatedly. Each time you search for % will take you to the beginning of the next program. If you want to describe the program, you can enter text in parentheses after the % and before the * in the first line like %(WOOD DUCK)* This is something I've never seen in the 3000 docs, but it works fine because the control ignores whats in the parentheses when its running. If you prefer program numbers, its easier to enter them as a letter and number combination on the line before the % line at the start of the program. Then you can search for P1234 for example, scroll forward to the first program line, leave edit mode, and you're ready to go on Program #1234. Caution though, because the program number is before the line containing the %, if you just search for P1234 and then exit edit without scrolling forward to the first program line, you'll make the previous program current instead of the one you planned to use. This can make for some real surprises The same text in parentheses thing can be used anywhere in the program, for tool descriptions for future reference or whatever. As long as you put it in parentheses, the control acts as if its not there.

Okumas read strictly in diameter. Offsets in X are entered as diametral offsets, and the control halves them internally to make the required change in radius position.

I tried cutting a .625" cylinder with MDI and came up at .650" So I manually moved the X - thinking it was reading Dia, to .620 and cut it with S1000 M3 G1 F30 Z0.0000... then mic'd it and came up with .643"

Click to expand...

The first cut indicates your offset was off by .025" You then moved the tool .005 on diameter, so you should have expected the next cut to be at .645" You got .643", or .002 less than expected. If the first cut was substantially heavier than the second, the .002 difference could come from deflection that occurred in the first cut, but not in the light second pass. If you took a couple more .005 cuts and got .638 and .633, then you'd be pretty sure the .002 difference was deflection. Not sure how you're setting x offsets, but the best way to set them accurately would be to take a manual light cut, and then, WITHOUT MOVING THE X AXIS, go into the tool offset page, and on the keyboard you'd enter X.643 <CAL>. When you do this, you're doing no calculations to arrive at the offset. You simply make a cut, measure the resulting diameter, and enter that amount. The cal function tells the control that the X position of the turret with this tool active produces this diameter. The control internally takes that info and calculates the proper offset for the tool based on that info, and enters it into the offset page.

A word about your feeds.....the control comes up in inches per revolution at startup. Your F30 looks sorta suspicious, as that would give you a feed of thirty inches per revolution. I'm gonna assume your feed wasnt quite that heavy

Also, if you were in MDI and entered M3S1000G1Z0F30 all on one line, and then hit cycle start, you should modify that. Start the spindle as one command, and then put your motion command in once the spindle is started. As written above, the motion and the spindle would start simultaneously. Generally it won't be a problem, but its always a better practice to program such that you're sure the spindle is at speed before any motion commences. This would apply regardless of whether you were entering commands in MDI or running a program from memory.

When keying a program in, or entering one via a BTR or your DTE device, you can eliminate the non-significant zeros. Z0 is the same as Z0.0000, Z.5 is same as Z.5000, Z1 is same as Z1.0000, and so forth. Saves time, and also saves memory, which is scarce on these older controls. I dont have any manuals here at home, but there's a key near the editing keys that will strip out all spaces and unnecessary other stuff in a program to minimize memory usage. I never put spaces in a line of code anyway, but thats just me. If the spaces make it more readable for you while getting things set up and proving a program, then you can put them in and strip them out later once the program is proven if you plan to hold a lot of programs in memory and need max space. In programs without branches, line numbers serve no purpose in these controls either. Unless they're of some benefit to you, they can be left out.

Also, be very cautious of code generated via one of the converter type programs. Okumas have quite a few commands that don't follow the same format as Fanuc, and most converter programs I've seen tend to be more geared toward Fanuc controls, or controls with Fanuc emulation. Actually, if you learn to use the LAP features as much as possible, you'll soon find you can write programs by hand in just a few minutes. LAP is found in your 2028 section of the manual, and is all your auto roughing, grooving, drilling, and threading routines. Some of the stuff you can do isnt real obvious in the manual. For example, to use LAP for drilling, you specify a face grooving routine with the groove at X0. Add whatever peck increment you want to that grooving cycle and you have a peck drilling cycle. Take a look too at G75 and G75 in your 2028 manual. Those will do auto chamfers and corner radii by just adding either G75 or G76 to a G1 move, and specifying an L value for whatever chamfer or radius you want. Lots easier than creating a chamfer via an X-Z move or a radius via a G2 or G3, because the control does all the thinking when you use G75 or G76.

I had never heard of your DTE device, but it appears that its the equivalent of a BTR, but done via software in a PC. Always seemed to me that was something that someone would have done, as it ain't rocket science. I still need to add a BTR or something to one of my lathes for loading programs, so I'm curious if you happen to know what the DTE costs.

Thanks for the info!!!

ON the offsets, I was sure what ever the problem was, it came in the form of offsets and maybe a touch of deflection... but Since all the tools in the turret are not what Ill be using, I didnt go in and do all the offsets and my have had a different tool than the one I set in the tool offsets.

-One question about the offsets... with tools 1 through 8... can I take a pass with T01, mic it, and enter its atcual diamter <cal>, and then change to tool T02 and do that same thing... and the control knows which tool Im using, or do I have to set one tool, and then get into the tool offset parameters for each tool in the program? Its amazing to me how the book tells you how to do one thing, but doesnt mention (in many places) if you just do the same thing for others. THose of us that are more into directions and "for sure this is what I do" get a bit lost or worried about just assuming if you do it for tool one, you do it for tool 2-8. My thinking on this is, if you set the tool offset for the T01, then it could be one of two things... the machine knows where the carriage is to calculate other tool offset measurements, or the machine knows where the tip of T01 is, and just needs to know where T02 and up are. GUess Im maybe a bit too chicken...

On the feed rate... sorry, I wasw just cruising along typing... it was F00030 in the machine... I typed in F30 and it added the preceeding zeros. SO no, I wasnt cutting that fast. but dont think its cause Im super smart... I trieds putting in 10.000 when I first stared cause my Mach3 used that nubmber. I got an error saying the max was 6. SO I quickly leanrd that the okuma was in decimals.

Ill try and remember when I type out the code for this, to type it as it is... like you said...
%
G0 Z0 X0
M42
S1000
M3
G1 F.003 X1.5
etc...

Thanks for the tip on the zeros... I thought that was the case but was too chicken to try for sure just yet. Now I know for sure. Oh, lastnight about 1am I foudn in the book where it said it references in diameter only. Amazing what you find when you read it again and again. Thanks!!!

On the conversion stuff...
Thats exactly what started me up on here...looking for the Gcode list. From what Ive found so far, the book might not be missing any... I convert the DXFs to gcode in Mach3, then watch what it does in mach3, then I look at the g code, and compare the commands to the Okuma stuff... like G3 and so on. Then when that stuff matches and looks right, I plan on trying it block by block in mid air out fromt he chuck a ways. THen rezero and try it on plastic. If its right, then move on.. if not, I know exactly where my next lesson will start... the intracacies of Gcode.

THanks for the direction on the G75,76 and LAP stuff. I dont know if I have the LAP function, as I dont have the spec build sheet, (wish I did so I knew if I had the DNC=B option) so Im not sure, shy of trying to run something that is in the LAP function line and see if I get an error or if it runs. Any thoguhts there?

On the DTE... (Direct Tape Emulation) so yeah, basiaclly a BTR. This one came with, so I have no idea what the cost was associated. But, I know that it was sold by the company that sells the Easytalk Plus Program (www.cnc1.com - Ive been talking with Dave or Jim - both really nice guys) THe software I bet is the expensive part, the card is probably just a basic breakout card with maybe some signal converting abilities. My biggest catch is the Easyatlk software doesnt like to run in windows, and I dont have a DOS machine, so Im trying to face it by runnign Win 98 in its DOS shell. Couple that unsure operating technique with not nowing how to make it work... and well... thats where I am right now. Ill prolly end up paying the tech service for the phone consultation to get it running... WHen I talk with them Illa sk about new parts and DTE. I know they said if I couldnt get it to work, I might have to buy a BTR which is around 1500 give or take (this was before I knew what I had) so Im guessing that its prolly in a similar range, but used might be a different story.

THanka again for all the info and thoughts. Im always open for "do this this way" or "dont do this ever" and even the the most basic stuff... I may already know it but the reminder is well worth the price of admission... like the scrolling through the program. Once you explained the secone program idea, then the scrolling made sense, and my computer logic side said, if youre before that %* then youre in the previous program. Im glad some of my addumptions like that are correct.

Thanks a ton! I dont know how I could ever repay you!

Wade

Okay... Im making good progress... got the tool offsets done, prorgam zero set, plugged in my program, section at a time and tested each (I have basically 5 separate programs that I combine to make one) and I have found, exactly what Metlmunchr said... isues with the G2 & G3 stuff... And I can tell this will be a stumbling block for me... because my part designs seldom have a straight line in them. All most all curves and radius'. I have the roughing out part all done, so all thats left is to fight these radius commads, or figure out if I have LAP and if I do, how in the heck to use it (havent read that part of the book yet). I really think Im going to need the help of a system/program to extrapolate those curves from the autocad drawings I make, because Im not sure im smart enough to get the "specifics" ouf of Autocad to make the Gcode myself let alone understand the I and K stuff just yet. I guess Im kind of saying HELP!!!
I can tell Im gaining on the learning curve, but there is much more to digest before I have a complete handle on this, but Im gaining.

Any tips on understanding the G2 & G3 would be greatly appreciated, as well as some tips on checking for the LAP funtionality and tips that will make the book a bit more understandable, are greatly appreciated. SOrry for so many nieve and basic questions, I just have a hard time learning from reading the books because there is always some sort of intelectual gap that I have to fight.

By the way, when I get this stuff all skewared away, Ill post up all the G and M codes I have incase someone doesnt have them.

THanks again
Wade

[ 10-03-2005, 09:46 AM: Message edited by: Wade C ]

I read some on LAP last night... look spretty interesting and the book even makes it sort of understandable. Im assuming to find out if I have the LAP option, I should just try something simple with it... and see if I get an error code?

Assuming it does work, I assume, that where the example shows simple coordinates, (Xa Za, XbZb, XcZc) one could use about any program string of G01,02,03,75,76. Just so long as its a single path, even if it has a few arcs or curves in the middle of a straigh line? Or is that too complicated for it to compute, when in bar turning or copy mode?

I saw reference to G72 in a different thread... does the Okuma support that as well? THe reason I ask is that the manual does not list the chamfering/radius G75/G76 in its chart, but as you read through the book, all of a sudden, there it is in the middle of the text... and Im just wondering if I missed seeing G72 as well.

Still fighting the curve issue, but am going to read more on the G75 and G76 ( I found it late last night after I got through LAP, and wanted to digest LAP first) and see if I can get the info I need from Autocad to make the G75 and 76 codes work instead of G02 and 03... ANy suggestions, hints, or tips?

These are the types of curves and part designs Im dealing with.


THanks a bunch.
Wade