584,805 active members*
5,223 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Okuma > LR-10 OSP5020L Program Running Problems
Results 1 to 20 of 20
  1. #1
    Join Date
    Aug 2011
    Posts
    0

    Question LR-10 OSP5020L Program Running Problems

    Hi All,

    I'm new to Okuma machines (Only programmed Fannuc and Fadal) and I have some questions on what I am doing wrong. I've managed to load programs into the machine and I can edit them just fine, but when I load the program to the Auto side the only thing that shows up on the program screen is:
    O2222
    M2
    This displays on both the A turret and B turret sides. I had an old program (already in the machine) that would show up on the A turret side, but when I re-loaded it the display now only shows the Program# End Program code. Here is a sample of my code:

    $UHMW1.MIN%

    O1111

    (UHMW1)
    (TOOL-1 OFFSET-1)
    (OD ROUGH RIGHT)

    (FACE)
    NB100 G0 X-6. Z10.
    M14
    T040404
    G97 S1457 M03 M42
    G42 G0 X3.9314 Z6.3
    G50 S3600
    G96 S1500
    Z6.2582
    G95 G1 X3.79 Z6.1875 F.01
    X-.0625
    G0 Z6.2875
    G1 G40 Z6.3875
    ...
    (FINISH NPTS 1-11.5 THREAD)
    NB500 G0 X-6. Z10.
    M14
    T0303
    G97 S200 M03 M40
    G0 X1.5455 Z6.4058
    G71 X1.1441 Z5.1875 I.0311 B29 D.0719 H.1391 M32 M75 F.087
    G0 X-6. Z10.
    M02
    %

    Any help would be greatly appreciated,

    Zack

    PS It's just me and my dad at our shop. I asked him and he doesn't know either :-)

  2. #2
    Join Date
    Feb 2009
    Posts
    6028
    M14? Think it's supposed to be G13 a turret, g14 b turret.

  3. #3
    Join Date
    Aug 2011
    Posts
    0
    G13 / G14 is what it is on the machine, I made a typo. Even when I leave that off it should default to G13, but I still get the same problem: 0nly Program# and last line display. Hitting cycle start just rewinds.

  4. #4
    Join Date
    Feb 2009
    Posts
    6028
    You did do a program select in auto right? Easiest way, program select(soft key) then * write. It will list the entire directory, cursor to the one you want then press write. Okumas use background edit every time, so if you don't re select in auto, changes won't be there.

  5. #5
    Join Date
    Aug 2011
    Posts
    0
    Yes the program select works. Each program is labeled with a unique program number so I could verify this. So, after front loading, the program display shows:
    O1111
    M2
    Or
    O2222
    M2
    Etc...
    So the front side loading gives me the first and last lines but nothing in between.

  6. #6
    Join Date
    Aug 2011
    Posts
    0
    Problem Solved! The program sample I displayed was M14 in the machine. The other two programs had G13/G14 either missing or in the wrong location.

  7. #7
    Join Date
    Aug 2011
    Posts
    0
    Well, that got the program to display correctly, but now it just alarms every time I hit go. The alarm is 743-2 ALM B Work Coordinate Mode Command Nothing. I thought this was related to the G140 telling it to work the main spindle, but it is either in a bad location or is completely un-related. Any help would be appreciated.

  8. #8
    Join Date
    Feb 2009
    Posts
    6028
    Think you need the G110/G111 since you are calling out CSS with the G96.

  9. #9
    Join Date
    Mar 2009
    Posts
    1982
    add G90 (absolute coordinate system) somewhere in the start of part program.
    show new version of part program here

  10. #10
    Join Date
    Apr 2006
    Posts
    822
    Can you post the entire program, indicating which line the cursor is flashing on when you hit cycle start?

  11. #11
    Join Date
    Aug 2011
    Posts
    2517
    That error is related to the G140/G141. You have it in the wrong place.

    This is the correct order for G13/G14/G140/G141

    Code:
    $TEST.MIN%
    (TURRET A PROGRAM)
    (LEFT CHUCK & TURRET A)
    G13
    G140
    (DO SOME MACHINING HERE)
    
    (RIGHT CHUCK & TURRET A)
    G141
    (DO SOME MACHINING HERE)
    
    (TURRET B PROGRAM)
    (LEFT CHUCK & TURRET B)
    G14
    G140
    (DO SOME MACHINING HERE)
    
    (RIGHT CHUCK & TURRET B)
    G141
    (DO SOME MACHINING HERE)
    
    M02
    all of this goes in one program and the machine will split it into 2 programs for turret A and turret B. turret B program starts at G14

  12. #12
    Join Date
    Aug 2011
    Posts
    0
    This was the problem. The machine does like certain things in certain places. To add to fordav11's solution: the machine also seems to require a G50 S#### before any actual operations otherwise it gives an alarm. I think i'm starting to get the hang of this machine finally. Thanks to everyone who replied.


    Quote Originally Posted by fordav11 View Post
    That error is related to the G140/G141. You have it in the wrong place.

    This is the correct order for G13/G14/G140/G141

    Code:
    $TEST.MIN%
    (TURRET A PROGRAM)
    (LEFT CHUCK & TURRET A)
    G13
    G140
    (DO SOME MACHINING HERE)
    
    (RIGHT CHUCK & TURRET A)
    G141
    (DO SOME MACHINING HERE)
    
    (TURRET B PROGRAM)
    (LEFT CHUCK & TURRET B)
    G14
    G140
    (DO SOME MACHINING HERE)
    
    (RIGHT CHUCK & TURRET B)
    G141
    (DO SOME MACHINING HERE)
    
    M02
    all of this goes in one program and the machine will split it into 2 programs for turret A and turret B. turret B program starts at G14

  13. #13
    Join Date
    Aug 2011
    Posts
    0
    This is interesting; I had not looked at this. According to the manual:

    To activate constant speed cutting mode on turret B, specify G111 with G96. To restore such mode on turret A again, specify G110.

    I am guessing this means the machine can only sync with one turret at a time. Is this correct? Can anyone think of a scenario where this could be a problem? Not a big deal, but still interesting.

    Quote Originally Posted by underthetire View Post
    Think you need the G110/G111 since you are calling out CSS with the G96.

  14. #14
    Join Date
    Mar 2009
    Posts
    1982
    the machine can only sync with one turret at a time
    Yep. exactly
    Can anyone think of a scenario where this could be a problem?
    1. asynchronous sub spindle revolution and both spindles G96 (CCS)
    2. main spindle axis C (live tool machining), subspindle - conventional turning

  15. #15
    Join Date
    Aug 2011
    Posts
    0
    Quote Originally Posted by Algirdas View Post
    Yep. exactly1. asynchronous sub spindle revolution and both spindles G96 (CCS)
    2. main spindle axis C (live tool machining), subspindle - conventional turning
    So if I understand correctly: when I use the sub-spindle to pick off a part I won't then be able to use both turrets in CSS. That could require too much thinking while programming. Making sure to alternate rough and finish passes. Hmmm. Good information. Thanks!

  16. #16
    Join Date
    Mar 2009
    Posts
    1982
    You can. You can synchronize both spindles, as they keep the same workpiece

  17. #17
    Join Date
    Aug 2011
    Posts
    0
    Quote Originally Posted by Algirdas View Post
    You can. You can synchronize both spindles, as they keep the same workpiece
    Sorry, I meant pull off a part and use turret A to finish the part on the sub spindle while roughing with B on the main spindle.

  18. #18
    Join Date
    Aug 2011
    Posts
    2517
    yes you can do that too (work with both spindles independently) but it's a real pain is the ass.
    you can read more here....
    http://www.cnczone.com/forums/okuma/...taneously.html

    you've only just realized about using G50 to set the top speed which has been standard on all CNC machines since the early 70's. I think you should read the manual in it's entirety and master the basics first. You must learn to walk before you can run like the wind.

  19. #19
    Join Date
    Aug 2011
    Posts
    0
    Quote Originally Posted by fordav11 View Post
    you've only just realized about using G50 to set the top speed which has been standard on all CNC machines since the early 70's. I think you should read the manual in it's entirety and master the basics first. You must learn to walk before you can run like the wind.
    No. I was referring to the placement of the G50. The machine requires three things before it will do anything:
    G14
    G140
    G50 S####
    My Fanuc controlled Lathes and Screw Machines are a little more forgiving with the G50. I only need to specify it before running the spindle. This particular Okuma won't let me do anything before a G50.

    As far as manuals, I have 12 of them. I have read each one cover to cover. As many people here know, information and application are two different things. Just because a G-Code is on a list or in a book, that does not mean it is ever applied anywhere in a manual. These manuals aren't even written for one machine, they apply to more than eight different models! It's un-realistic to assume that reading the manual would teach you the machine. That is why there are these wonderful forums where people that have already figured out all the little kinks of a machine can share them with people that haven't.

    Sorry for the rant. Thanks for all the helpful comments.

  20. #20
    Join Date
    Oct 2019
    Posts
    1
    Quote Originally Posted by ZandS View Post
    This was the problem. The machine does like certain things in certain places. To add to fordav11's solution: the machine also seems to require a G50 S#### before any actual operations otherwise it gives an alarm. I think i'm starting to get the hang of this machine finally. Thanks to everyone who replied.
    Hello all! I'm new to the Okuma here also..
    On LT15-M osp5020l
    Same alarm 743-2 ALARM B
    I'm in 'individual' mode (bottom turret /left spindle

    I've tried over & over everything..

    Can anyone help?

Similar Threads

  1. Setting program zero cadet LNC-8 OSP5020L
    By brandonzp in forum Okuma
    Replies: 9
    Last Post: 11-05-2012, 11:49 PM
  2. Need help running program from card
    By BOATDUDEGUY in forum Fanuc
    Replies: 5
    Last Post: 03-28-2012, 10:30 PM
  3. Running program with G0, G1, and/per F
    By Martcnc in forum CamSoft Products
    Replies: 3
    Last Post: 01-19-2011, 07:46 AM
  4. Replies: 4
    Last Post: 06-15-2010, 03:38 PM
  5. Problems getting X4 up and running
    By rickturner646 in forum Syil Products
    Replies: 18
    Last Post: 05-27-2008, 02:39 AM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •