603,923 active members*
2,583 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Okuma > Okuma LS30-N tool index position distance?
Results 1 to 16 of 16
  1. #1
    Join Date
    Jul 2007
    Posts
    162

    Okuma LS30-N tool index position distance?

    For years I've wanted to set a safe distance for the LS30 lathe to perform its tool changes on both front and rear turrets. The LB15 we have is great in that the tool turret wont index unless its against a limit on either Z or X.

    Can I get the LS30-N to do this also? We have had one too many tool crashes and one edit mistake and the tool will index even when inside a job, ouch!

    If any one knows how to set this parameter please let me know.

    Thanks.

  2. #2
    Join Date
    Nov 2010
    Posts
    0
    Your LB-15 will do a tool change wherever you want it to,unless Okuma has changed their software since I last ran one. Are your programs in Z-,or Z+? Just curious. In my opinion,Z0.0 is always the face of the part.

  3. #3
    Join Date
    Jan 2008
    Posts
    575
    Quote Originally Posted by DSIF View Post
    Your LB-15 will do a tool change wherever you want it to,unless Okuma has changed their software since I last ran one. Are your programs in Z-,or Z+? Just curious. In my opinion,Z0.0 is always the face of the part.
    WHAT??? No it will not, if it is running it will NOT do a toolchange unless the turret is up against one of the stops. You can change the parameters to move the limits, but it will not index unless it is against the soft switches. Not from 2200 to P200.
    The beaten path, is exclusively for beaten men.

  4. #4
    Join Date
    Jul 2007
    Posts
    162
    The LB15 we have definatley will not change tools unless its against a soft limit in either X or Z. I'm not saying this cant be removed. But thats how our is. I personally like this feature and so this thread is actualy about me trying to find out how to get the LS30-N we have to do the same.

    At the moment our Okuma LS30-N with tool change any where which I dont like, especialy on a twin turret machine with long drills hanging out every where!

    Im hoping there is a parameter somwhere to set this?

  5. #5
    Join Date
    Nov 2010
    Posts
    0
    As a former service tech for Okuma in CA, I find this question strange because I thought the OSP5020 control setting pages allow you to set the turret tool change X-Z positions.

    Please check if this page exists and set the change position to suit the longest tool to prevent collisions.

  6. #6
    Join Date
    Feb 2009
    Posts
    6028
    5000L and newer must be at a soft limit on slant bed lathes, and small lathes (LC10, LB9 ETC) x or z or both.

    The flatbed lathes were different, because they were slower and usually way too long of beds.
    Limit was adjustable (user limit) to help shorten cycle time if you wanted. Variables can also be used for each tool to change the user limit if you really wanted to. The old 2000, 2200, and 3000 may not do that. It's been too long since i touched the older controls, so IDK.

  7. #7
    Join Date
    Nov 2010
    Posts
    0
    It's in the "user parameter" page. Z axis and X axis stroke limits. Move a safe distance away with your longest tool and put that value in. Enter that value or greater in your program-(it wont over travel),and do your tool change. The OSP 5000 and 5020 will both do it. In contrast,you can also set your turning tool to where it will not hit the chuck(a chuck barrier if you will).The Okuma controls have many "bells and whistles" like this.

  8. #8
    Join Date
    Jul 2007
    Posts
    162
    I know about stroke limits and chuck barriers etc, but this is not what I'm after. What I need to is set a Z and X value that will see neither turret index near the chuck. In not concerned about crashing tools but to hear the machine index 3mm from the chuck is gut wrenching!
    Just last week a worker missed a tool change edit and the he stuck a 2" drill into the chuck. It bent the H turret spindle and I’ve worked half the week to fix it.
    So thus I'm looking for a way to set a safe tool index position say X300 Z250 for both turrets.
    I don’t wont to set any tool barriers.

    Attached is the control its mono tone OSP 5000 year 1982-08
    Attached Thumbnails Attached Thumbnails Ls30-N full shot.jpg   OSP 5000 control 1982-8.jpg  

  9. #9
    Join Date
    Apr 2006
    Posts
    825
    Sorry Rotec, I am not sure which parameters to alter to get what you want...
    But...

    Have NONE of you used or heard of cycle time reduction coding?

    I can get the turret to index away from it's set home position very easily.
    Using M65 and M66
    With out the manual to hand, I may have the code explanations flipped but basically one is Turret Free Indexing (M65 I think) and Ignore Turret tool in-Position command (M66)

    Basically what you can do is tell the machine to index whilst on the move using these codes. Can be a bit interesting if you fail to take into account longer tools and the amount of time it takes the machine to index between stations!
    The way I use these codes is:

    Machining Program... with tool T010101
    N100 G0 Z800 (move at rapid to z Home position)
    N102 X(next diameter require) Z800 T020202 M65 M66 (Machine will now index the tool to Tool 2 while moving to the Next X axis position stated while keeping up against the Z axis home posn).
    N104 X(same value as on line N102) Z(reference position) T020202 (NOTE! REPEAT the tool number here!)
    Machining program for tool 2.
    ...

    an example program using values might look like the following (simplified lots):
    N100 G0 X400 Z800
    N102 G97 S500 M3 M8
    N104 X100 Z102 T010101
    N106 G1 Z100 F0.2
    N108 X0 (FACE PART)
    N110 G0 Z800
    N112 X102 Z800 T020202 M65 M66
    N114 X102 Z102 T020202
    N116 G85 N118 D5 F0.3 U0.5 W0.1
    N118 G81
    N120 G0 X20
    N122 G1 Z100
    N124 X100 Z50 (MACHINE A TAPER FOR EXAMPLE)
    N200 G80
    N202 G0 Z800
    N204 X20 Z800 T030303 M65 M66
    N206 X20 Z102 T030303
    N208 G87 N118
    N210 G0 X400 Z800 M5 M9
    N212 M2

    In the above example, the machine will index the turret to the next tool whilst moving along X axis and keeping the turret at Z home.
    The reason for putting the same Tool number on the next line is so that the machine will confirm the required tool is actually in position BEFORE moving to the nominated posn.
    If you do not do this and the turret is still indexing when the next X axis position is reached, the machine will then start moving towards the part... now THAT could be very exciting if a long tool was between tool positions programmed!

    Another 2cents worth
    Cheers
    Brian.

  10. #10
    Join Date
    Jan 2008
    Posts
    575
    Can I get the LS30-N to do this also? We have had one too many tool crashes and one edit mistake and the tool will index even when inside a job, ouch!

    If any one knows how to set this parameter please let me know.
    Sorry, has the question for this machine been answered? I cannot speak from experience. I can only be a smart ass when it is called for. Oh I guess sometimes when it isn't called for also.

    Robert
    The beaten path, is exclusively for beaten men.

  11. #11
    Join Date
    Feb 2009
    Posts
    6028
    Again, the flatbed lathes didn't have to be at limit. They were just too big and slow, so Okuma didn't put the limit in the software.

  12. #12
    Join Date
    Jul 2007
    Posts
    162

    Smile

    Tool changes while the turret is in transit is the exact oppersite of what I'm after! hahaha.
    Those codes in the hand of my dyslexic programers would lead to disaster

    Looks like the flat bed machines cant have this feature. ie where a tool changes only occure at a set distance from the chuck.

    I'm surprised that this cant be done.

    Oh well. Thanks for listening.

  13. #13
    Join Date
    Apr 2006
    Posts
    825
    Quote Originally Posted by rotec View Post
    Tool changes while the turret is in transit is the exact oppersite of what I'm after! hahaha.
    Those codes in the hand of my dyslexic programers would lead to disaster

    Looks like the flat bed machines cant have this feature. ie where a tool changes only occure at a set distance from the chuck.

    I'm surprised that this cant be done.

    Oh well. Thanks for listening.
    Yes well... I did realise that this was the case... But I was mainly trying to make a point that you can index a machine away from the limits using the appropriate codes!
    I also agree with you that these codes, used in the wrong way could be a disaster in the making.
    Good luck.
    Brian.

  14. #14
    Join Date
    Apr 2009
    Posts
    1273
    Does your machine have User Task 2? If it does, there may be another way to make it happen using System variables.

    You could check the VAPAZ to see IF it is > or = to Z123.4567 or whatever.
    If yes, index, if not, Alarm. Zero offset could be taken into account as well.

    Let us know.

    Best regards,

  15. #15
    Join Date
    Apr 2006
    Posts
    825
    Quote Originally Posted by OkumaWiz View Post
    Does your machine have User Task 2? If it does, there may be another way to make it happen using System variables.

    You could check the VAPAZ to see IF it is > or = to Z123.4567 or whatever.
    If yes, index, if not, Alarm. Zero offset could be taken into account as well.

    Let us know.

    Best regards,
    The problem with that would be that you need to call the macro before each and every tool change! Once again, operator error can creep in and really mess up your day!
    The only solution that would work would involve a change in software on the machine that would command the machine to only perform a tool change when on a limit.

  16. #16
    Join Date
    Apr 2009
    Posts
    1273
    Yes, you will need a tool change "SUB". Everyone know that your chances of getting Okuma to get you new software for that control are as likely as taking a deep breath with your helmet off on the moon...

    Even though it's not ideal, I think you could throw a parameter with the sub call to get the correct tool and always pull back away from the spindle by a fixed distance based on your Zero set and a distance of your choice.

    Still better than indexing 3mm from the chuck. Yikes!

    If you don't have User Task 2, A spec change from Okuma would be possible...

    Best regards and happy "safer" indexing,

Similar Threads

  1. Replies: 3
    Last Post: 12-10-2010, 12:51 AM
  2. using encoder index for homing and a axes position
    By rokag3 in forum CNC Machine Related Electronics
    Replies: 22
    Last Post: 10-16-2009, 12:57 PM
  3. Tool Change/index Problem
    By JMO09 in forum Okuma
    Replies: 7
    Last Post: 04-08-2009, 04:35 PM
  4. Need Help Re-Set Home Position on Okuma
    By PSSJEFF in forum RFQ Feedback
    Replies: 0
    Last Post: 02-09-2009, 04:35 PM
  5. Tool Turret Index Failure
    By hatchmar in forum DNC Problems and Solutions
    Replies: 6
    Last Post: 06-10-2005, 12:36 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
  •