Results 1 to 12 of 12

Thread: Dynamic fixture offsets

  1. #1
    Registered
    Join Date
    Apr 2006
    Location
    USA
    Posts
    76
    Downloads
    0
    Uploads
    0

    Default Dynamic fixture offsets

    Does Okuma have dynamic fixture offsets? We just got a new horizontal and none of us have much 4 axis programming experience.

    I have read about G54.2 on Fanuc. Does Okuma have a similar feature?

    Similar Threads:


  2. #2
    Registered broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    674
    Downloads
    0
    Uploads
    0

    Default

    Yes they do!

    You program G15 Hx where 'x' is the coordinate system that you want to use.
    You need to have a look on the Zeroset page to see how many coordinate systems you have available to you, but could be between 50 and 200 depending on your options.
    Therefore G15 H1 will select coordinate system 1
    G15 H2 is coordinate system 2 ect...
    You can manually set the values for each system, or you can store the values in each program. That way, when you setup your fixture again, providing it is in the same position, the coordinate system is automatically loaded and used.
    To program a coordinate system use the following codes:
    VZOFX[x]=123.456
    VZOFY[x]=123.456
    VZOFX[x]=123.456
    VZOFB[x]=0

    Where the 'x' in the brackets is the coordinate system number that you want to set.
    Note that you are setting the coordinate for X Y & Z but on B axis you are setting an "Offset" value.
    This means that B axis is offset by whatever degrees you program.
    i.e. if you have a part on the pallet that is pointing towards B90 and you want this to be B0 you would program VZOFB[x]=90
    This will bring B0 to the B90 position.
    Hope that makes sense to you.
    The easiest way to find out the values to program is to "CAL" the required position on the ZEROSET page and then copy the values from there into your program.
    You do need to make sure you reset your "B" axis offset value at the end of your program, because if you forget it will be still effective for the next job, and that can ruin your whole day! Especially if you have clocked up a job, done it, forgot to reset and machine the next job only to realise that 0.5 degree offset you needed on the last job was still active and the current job is now a bucket of scrap metal. (trust me on that one! I know! )
    Hope this helps.
    Good luck with the new machine.
    Cheers
    Brian.



  3. #3
    Registered
    Join Date
    Apr 2006
    Location
    USA
    Posts
    76
    Downloads
    0
    Uploads
    0

    Default

    Thanks for your reply.

    You are just describing standard fixtures offsets. I'm good with those.

    A dynamic fixture offset lets you set one offset and use it at any B index you want.

    With the standard offsets, if you move VZOFX[1] by plus 2mm at B0, you need to also remember to move VZOFZ[1] 2mm plus at B90 and 2mm minus at B270.

    I was hoping for a utility to get around that short coming.



  4. #4
    Registered
    Join Date
    Jun 2008
    Location
    USA
    Posts
    313
    Downloads
    0
    Uploads
    0

    Default

    Yes, Okuma call it "Fixture Offset function" What control do you have?



  5. #5
    Registered
    Join Date
    Apr 2006
    Location
    USA
    Posts
    76
    Downloads
    0
    Uploads
    0

    Default

    This is a brand new MB-5000 machine with a Thinc control.



  6. #6
    Registered
    Join Date
    Jun 2008
    Location
    USA
    Posts
    313
    Downloads
    0
    Uploads
    0

    Default

    Check the spec sheet in the back of the machine to see if you have this option



  7. #7
    Registered broby's Avatar
    Join Date
    Apr 2006
    Location
    Australia
    Posts
    674
    Downloads
    0
    Uploads
    0

    Default

    We have written our own software to do this on the machine.
    I would think I would be hung if I gave you a copy! Sorry.
    A bit of a PITA to work out, but the maths is not that hard to work out.
    Hope you have the Okuma software, sounds interesting.
    Regards
    Brian.



  8. #8

    Default Caution use only where appropriate

    While this type of offset has some advantages, there is a downside. The function assumes the machine has perfect geometry. While I have a lot of respect for Okuma as one of the few builders that actually checks machine geometry and delivers a report (cutting tests also), there is always some error in the machine. If you are machining anything down to a few thousandths tolerance from one B position to another there is really no substitute for picking up individual offsets for each index position.
    Here is an example: I was setting up a gear housing on an Okuma MH400, and trammed the same locator pin at B0 and B90 for the Y offsets. There was a difference of .0015 in Y. The other programmer at the shop said "what are you doing" and when I explained his response was "that's bull, it should be perfect." Well that error would have put the part out of tolerance and he would have been chasing his tail to find the problem, whereas my first piece was good (at least on that feature ;-).
    BTW I worked for a major machine tool builder and quantifying machine geometrical error was a big part of my job. I used ANSI B5.54 tests extensively and without getting into a long thread on the different static and dynamic error you might find, please be aware that your machine is not perfect (niether is your CMM; next time they reject your parts ask to see the R&R report).

    Last edited by mfgbydesign; 06-27-2011 at 10:30 AM.


  9. #9
    Registered christinandavid's Avatar
    Join Date
    Aug 2009
    Location
    New Zealand
    Posts
    661
    Downloads
    0
    Uploads
    0

    Default

    You could get around machine error/variation to some extent if Okuma has the equivalent of the EXT Offset on the Fanuc.

    Alternatively, if you create your own macro to automatically calculate the new work offset position, you can designate a particular work offset as your EXT offset and incorporate it into your macro. The EXT offset has been essential to help get my bores in line...my machine sways and swells like a ship on the high seas...

    This is a macro b version of the offset calculating trig, should anyone need it: -

    (get offset values)

    #710=(original X offset)
    #711=(original Z offset)

    #712=1049.97 (pallet centreline in X)
    #713=-250.04 (pallet centreline in Z)

    #714=[#710]-[#712]
    #715=[#713]-[#711]
    #716=SQR[[ABS[#714]*ABS[#714]]+[ABS[#715]*ABS[#715]]]
    #717=[[ATN[[#715],[#714]]]-[#705]]

    #718=[#712]+[[COS[#717]]*[#716]] (new X offset)
    #719=[#713]-[[SIN[#717]]*[#716]] (new Z offset)

    (add EXT X offset value to new X offset if necessary)
    (add EXT Z offset value to new Z offset if necessary)

    (save new offset values in designated offset. don't overwrite the originals whatever you do)


    You would have to check the ATAN format on the Okuma to see if it comes up with the same results (ie 0-360 deg - not +/-180deg)

    DP



  10. #10

    Default Re: Dynamic fixture offsets

    Hi DP,
    I am interested in adapting your code below

    #710=(original X offset)
    #711=(original Z offset)

    #712=1049.97 (pallet centreline in X)
    #713=-250.04 (pallet centreline in Z)

    #714=[#710]-[#712]
    #715=[#713]-[#711]
    #716=SQR[[ABS[#714]*ABS[#714]]+[ABS[#715]*ABS[#715]]]
    #717=[[ATN[[#715],[#714]]]-[#705]]

    #718=[#712]+[[COS[#717]]*[#716]] (new X offset)
    #719=[#713]-[[SIN[#717]]*[#716]] (new Z offset)

    for a OSP200L VTM. Could you tell me what #705 does or is taken from?

    Many thanks



  11. #11
    Registered
    Join Date
    Apr 2009
    Location
    USA
    Posts
    546
    Downloads
    0
    Uploads
    0

    Default Re: Dynamic fixture offsets

    #701 would be an Okuma common variable such as VC101. You should have at least 200 of them on a P200 control that you can play with.

    Best regards,



  12. #12

    Default Re: Dynamic fixture offsets

    Thanks for you answer. I am ok using common variables on the OSP.

    I was really looking for a description for #705 as there isn't one in the supplied code. All other variables shown have a description.

    Suppose I will have to try to work it out.

    Thanks



Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed