Fanuc O-MB incremental input


Results 1 to 20 of 20

Thread: Fanuc O-MB incremental input

  1. #1
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default Fanuc O-MB incremental input

    Can anybody help me here. I'm used to using a HAAS machine, however we purchased a Mill with a Fanuc controller(O-MB) and I'm curious as to how to add incremental values when doing work offsets.
    Lets say you have set the X and Y but want to adjust it by an amount. Instead of calculating the new value, can you just type in an incremental amount and add it to the current value without overwriting what you already have.
    Or alternatively, can you move the bed to a certain point and somehow input that value by pushing a button as opposed to typing the value in.
    On the Z axis, we can Hold EOB and push the Z button, and it will automatically bring up the Z value. Then I push enter and it enters the value. I would like to be able to do something similar with the X and Y.

    Can anybody help me here.

    Thanks in Advance
    Greig
    Motorcycle Performance Engineering

    Similar Threads:


  2. #2
    Registered HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Hi Greig,

    I'm not sure how you are accustomed to working, but I always use an appropriate Gcode to define the tool's position relative to to the part datum. In particular I use a G92 command but this may not be what you would use. This does require actual editing of the code.

    It sounds like you want to make a movement outside of the work coordinate system. However, it seems to me that you could get yourself in a lot of trouble doing this because on the next work offset, you would still be carrying the error of your previous mdi movement. Sounds like a recipe for scrap I may not be understanding what you are saying though.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Community Moderator cadcam's Avatar
    Join Date
    Apr 2003
    Location
    United States
    Posts
    3543
    Downloads
    0
    Uploads
    0

    Default

    MPE Racing in the Fanuc O-M control you can not do as you except. the control wants a exact numer to be inputed in to the control.

    I agree with the Haas this is vary easy just add or subtract the amount you want to change and you are of and going.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .


  4. #4
    Registered hardmill's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    499
    Downloads
    0
    Uploads
    0

    Default Macro

    Do some research on using varables to shift the machine.
    See what the machine will and wont accept.
    If you show me exactly what you need i'll take a look when
    i get home i'm on my way out.
    Varibles are always a quick, short and easy solution when
    you understand the basics.

    And congrats on the fanuc. Their great controls.

    PEACE



  5. #5
    Member
    Join Date
    Mar 2003
    Location
    Saskatchewan, Canada
    Posts
    67
    Downloads
    6
    Uploads
    0

    Default

    Will G92 Set program part zero do anything for you?

    D. Paulson


  6. #6
    Community Moderator cadcam's Avatar
    Join Date
    Apr 2003
    Location
    United States
    Posts
    3543
    Downloads
    0
    Uploads
    0

    Default

    you use the G92 instead of useing a G54,G55 and you need to find the pickup location from Machine home and input this info to the front of the program.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .


  7. #7
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    Thanks guys. I'll have to keep doing it the way I have been already I guess.
    I like the idea of using variables Hardmill. My machine doesn't like G92 at the moment unfortunately, but I'l look at that. I'll be setting up some quick change set-ups on the machine, and when we have these I might set a bunch of home positions using variables to store them. This way if we have to work on the machine, and the positions change, it's only a matter of resetting 2 variables and we are away again. Cool idea, thanks.

    Here's another question. The tool diameter offset has to be input as a radius. Is there a parameter or something in the controller to convert this to a diameter. Another HAAS thing I'm used to. It saves having to think too much when adjusting offset diameters as well.

    Thanks in advance again

    Greig
    Motorcycle Performance Engineering



  8. #8
    Community Moderator cadcam's Avatar
    Join Date
    Apr 2003
    Location
    United States
    Posts
    3543
    Downloads
    0
    Uploads
    0

    Default

    You do know that the Haas will do either Radi or Dia it is a option in the Pramaters?

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .


  9. #9
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    Will the Fanuc allow it though? That's what I have

    Greig



  10. #10
    Registered hardmill's Avatar
    Join Date
    Mar 2003
    Location
    United States
    Posts
    499
    Downloads
    0
    Uploads
    0

    Default Re: Macro

    Originally posted by hardmill
    Do some research on using varables to shift the machine.
    See what the machine will and wont accept.

    PEACE
    Are you referring to variables?



  11. #11
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    Does the Fanuc have a parameter to change from radius to diameter.

    Greig



  12. #12
    Community Moderator cadcam's Avatar
    Join Date
    Apr 2003
    Location
    United States
    Posts
    3543
    Downloads
    0
    Uploads
    0

    Default

    MPe I think it does I will see if I can find the Pramaters if it does.
    This is the Fanuc O-M control correct?

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .


  13. #13
    Registered
    Join Date
    Apr 2003
    Location
    Yorkshire/u.k
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default

    Mpe the parameter for radius/diameter that you are referin to is parameter 0001 bit 4, if set to 1 offset becomes diameter designation. If set to 0 offset becomes radius designation. Beware, if you dont know the correct way to alter this setting you could easily loose all your parameters. For more info drop me a email.



  14. #14
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    Thanks Paxo, I just had a look at Parameter 0001 and my bit 4 is set to 0. I'll change that to diameter...Thanks again

    Greig
    Motorcycle Performance Engineering
    Brisbane



  15. #15
    Registered
    Join Date
    Mar 2003
    Location
    Utah
    Posts
    214
    Downloads
    0
    Uploads
    0

    Default

    Not Enough Fixture Offsets

    I also have found this to be one of the best ways.I have worked for one
    company that used to use G92 but found this to be a little more dangerous
    especially if it requires jumping in prog i.e. say when the tool/tips need
    replacing.Things don,t always go to plan as expected at first, it takes time
    for proving method,etc.

    We use the Zero Offsets in the program and it works just fine.
    > I use this way to do it.
    >
    > N5 (TESTING OF USING ZERO OFFZET IN PROGRAM)
    > N10 G10 L2 P1 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G54)
    > N15 G10 L2 P2 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G55)
    > N20 G10 L2 P3 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G56)
    > N25 G10 L2 P4 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G57)
    > N30 G10 L2 P5 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G58)
    > N35 G10 L2 P6 X999.999 Y-999.999 Z-999.999 ( ZERO OFFSETT G59)
    > N40 G90 M61 (CHANGE PALLETT TO NR 1)
    > N45 P2000 T2 M98 ( CHANGE TOOL TO TOOL NUMBER 2)
    > N50 G54 ( CALL OF ZERO OFFSET NUMER 1)
    > N55 G0 G43 X99.99 Y99.99 Z15.00
    > N60 ( CONTINUE OF THE PROGRAM....)
    N90 M30

    EXAMPLE OF A PROGRAM WITH OFFSETTS CHANGES, REMEMBER TO
    LOOK CLOSELY AND YOU HAVE TO PUT THE USE OF G10 AHEAD OF
    THE CALL OF YOUR ZERO OFFSETT. THATS VERY IMPORTANT, OTHERWISE
    YOU JUST WRITE THE VALUES TO THE OFFSETT PAGE AND DONT
    GET THE VALUES UNTILL NEXT PART,

    The "L" refers to the Type of offsets you are setting when used with G10
    (it does refer to repeats when used with sub calls). For example L2
    refers to Work offsets, L10 to Tool offsets (yes you can offset tools
    with G10) L11 - Tool Wear, L12 - Diameter offset, L13 Diameter Wear.
    These may vary on your control and I would consult the manuals to see
    which apply. You probably have figured out that "P" points to which
    address to set.

    Ken



  16. #16
    Registered
    Join Date
    May 2003
    Location
    India, Mumbai
    Posts
    41
    Downloads
    0
    Uploads
    0

    Default

    Dear MPE Racing,

    Press OFFSET / SETTING Key. Press Right Page-Up Key & 'OTHERS' Key, till you see a Softkey 'MEASURE'. Select any Free Work-Offset (G54, G55 etc.). Highlight the X or Y Value and press The 'MEASURE' Softkey, the Value in the 'Machine Co-ordinate system will be recorded in the respective G-Offset Table.

    Now simply call the G-Offset in the program.

    The Method Suggested by MORTEK is also good. However, you need Optional Work Offsets Beyond G59.

    SMA

    Last edited by smabhyan; 05-16-2003 at 10:06 AM.
    smabhyan


  17. #17
    Registered
    Join Date
    Mar 2003
    Location
    Utah
    Posts
    214
    Downloads
    0
    Uploads
    0

    Default

    The ability to load #'s into the offset registers solves the lack of more fixture offsets. I had a Chiron machine with the 180 degree rotating table (making two pallets so to say) I used all 6 offsets on each side of the table. I would load the new offsets in the program each time the table turned, enabling the use of more offsets.

    Ken



  18. #18
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    smabhyam, my controller must be a bit different to yours.
    The one I have is an O-MB. Even the G54 etc are just called, 01 02 03 04 etc......And you can't highlight the x or y line. You have to type it in to change it.

    Maybe there is a parameter for that too.....who knows...

    Greig



  19. #19
    Registered
    Join Date
    Apr 2003
    Location
    Yorkshire/u.k
    Posts
    7
    Downloads
    0
    Uploads
    0

    Default

    Mpe racing, here's something that maybe of interest. These are unlisted parameters but her goes anyway.. Parameter 910 bit 1, for g54-g59, Parameter 911 bit 3 give you a clock!. I havent had chance to try them on a OMB control but I have used them on a OMT and OMC. As usual dont mess about with the parameters unless you know what your up to.

    Next..........



  20. #20
    Registered
    Join Date
    May 2003
    Location
    Brisbane Australia
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default

    Thanks Paxo, I'll have a look at it

    Greig



Tags for this Thread

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 for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Fanuc O-MB incremental input

Fanuc O-MB incremental input

Fanuc O-MB incremental input