Need Help! Bar Feed Program for Haas Lathe


Results 1 to 18 of 18

Thread: Bar Feed Program for Haas Lathe

  1. #1
    Registered
    Join Date
    Sep 2007
    Location
    United States
    Posts
    49
    Downloads
    0
    Uploads
    0

    Default Bar Feed Program for Haas Lathe

    Does anyone know how to program for a lathe bar-feeder? Any sample programs out there!

    I know how to program a part but don't know how to program a bar feeder. How to check for the bar or any other variables that need to be considered.

    Please help!

    Thanks,
    wganders

    Similar Threads:


  2. #2
    Member
    Join Date
    May 2007
    Location
    USA
    Posts
    1003
    Downloads
    0
    Uploads
    0

    Default

    I don't think you have given enough information. Programming the barfeeder depends on which barfeed you have. They are not all programmed the same way. For example, on our Hardinge lathes using their barfeeders you simply position the barstop, open the collet, give it time to push the bar, close the collet and machine. (I actually stop ahead of where I want to be and push it in a bit after the bar feeds out, but...)

    On the LNS & SMW barfeeders it is a little different. It can even be different between certain models of a manufacturer.

    I know you are busy, but take the time to supply enough information for others to help you. Most of us enjoy passing our knowledge along. BUT...it is hard if the poster makes us guess. Many won't even bother to reply.

    Sorry. I know I am getting old and grouchy. Don't take offense. It is just that I see this scenario all too often.



  3. #3
    Registered
    Join Date
    Sep 2007
    Location
    United States
    Posts
    49
    Downloads
    0
    Uploads
    0

    Default Details

    OK!

    We're getting a Haas SL-20 with a Haas Servo 300 bar feeder. Could anyone post sample programs? I'm sure it's easy but I just started this new job and they think I know everything about machining/progamming.

    Thanks in advance.

    Wganders



  4. #4
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    In the upper right of this page there is a search window; not the browser one right at the top another one that just searchs CNCzone.

    Put 'Haas Servo 300 bar feeder' in this window and you will find dozens of posts that mention this bar feeder. You should be able to find what you need somewhere in these posts.

    EDIT: You have to scroll to the top of the page to see the search window I mean. It is not visible when you are reading this post.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  5. #5
    Member
    Join Date
    May 2007
    Location
    USA
    Posts
    1003
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Geof View Post
    In the upper right of this page there is a search window; not the browser one right at the top another one that just searchs CNCzone.

    Put 'Haas Servo 300 bar feeder' in this window and you will find dozens of posts that mention this bar feeder. You should be able to find what you need somewhere in these posts.

    EDIT: You have to scroll to the top of the page to see the search window I mean. It is not visible when you are reading this post.


    Once I saw "HAAS" I figured you could help him if anyone could.

    I cut-and-pasted your search criteria. I saw nothing that would help the OP with programming his barfeeder. Did I miss something?

    Like I said before, the Hardinge barfeeders are a breeze to figure out. (I believe their manual gives a barstop example.) The others I am familiar with require code that would be impossible to figure out without a sample from the barfeed manufacturer. They use different M-codes for loading a new bar. Also you need a block like

    /2 P8000

    How would a person figure this out without a manual telling how to set the barfeeder up? If the OP is getting a new machine, then all this information should be supplied with the machine/barfeed. If used, then maybe they left the barfeed subprogram in the control. Of course not everyone uses a subroutine, but programs the whole barfeed operation in the main program. We've bought used before, and usually there will be at least one program left in the control. Hopefully it would include a barstop operation.

    Here is my program for barfeeding the Hardinge lathes. All use Hardinge barfeeds except one. Think that is an LNS.

    N100G10P0Z-1.5 (BARSTOP)
    G200
    M1

    Here is the one I use for the Daewoos/Nakamura Tome (SMW/LNS barfeeders)

    N3200G10P0Z-8.63 (BARSTOP) (I don't set the workshift on the Nakamura)
    G65P9018X1.05F.01S900M4000T808
    M1

    The Hardinge subprogram barstops and goes back to the main program. The Daewoo/Nakamura barstops, dresses the new bar and then goes back to the main. My example is for 1 inch 52100 material. S900 = SFM, M4000 = 'S' in G50 block. Other 3 values are self explanatory. Actually there are a couple other variables depending on which model Daewoo the program is for.

    I would have to be at work in order to post what is in the subprogram calls. Sorry but I don't have that memorized. This information isn't going to help anyone without knowing what is in the suprograms. I doubt what is in the subprograms would be of much help unless you were using the same machine and barfeeder.

    I imagine that the barstop operation for your 'shop made' barfeeders (nice BTW ) would be similar to the Hardinge one, although it would be a simple matter to also dress the new bar. Doubt you use the /2 P8000 in your barstop routine.



  6. #6
    Registered
    Join Date
    Apr 2004
    Location
    Serbia and Montenegro
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default

    Here'a a barstop subroutine I've been using on HAAS SL-30...unfortunately, I can't remember the name of feeder vendor (it was not original HAAS):

    %
    O01022 (BARSTOP FEEDER SUBROUTINE)
    G21 G54
    T1212 (BARSTOP TOOL)
    M05
    G04 P1.
    G00 X200. Z200.
    G00 Z5. X0.
    G98 G01 Z1.5 F1000.
    M11
    M51
    G04 P5.
    M96 Q26 P100
    M61
    G04 P4.
    G01 Z150. F5000.
    M121
    G01 Z1.5 F2000.
    M10
    G00 Z200. X200.
    G99
    M99
    N100
    M61
    M10
    G04 P1.
    G01 Z5. F1000.
    G00 X200. Z200.
    G99
    M99
    %



  7. #7
    Registered
    Join Date
    Sep 2007
    Location
    United States
    Posts
    49
    Downloads
    0
    Uploads
    0

    Default Thanks

    Thanks Tex,

    That's exactly the kind of sample I'm looking for. It looks like you position a stop for the bar feeder to push against. Is that correct? Do you have any idea what all the special codes do? Like all the special M codes, etc... I hate to seem dumb but I like to get as much detail as I can.

    Thanks again,
    Bill



  8. #8
    Registered
    Join Date
    Sep 2007
    Location
    United States
    Posts
    49
    Downloads
    0
    Uploads
    0

    Default Thanks

    Sorry I missed it but thanks to G-Codeguy for his information! It is much appreciated.

    Bill



  9. #9
    Member
    Join Date
    Jul 2005
    Location
    Canada
    Posts
    12177
    Downloads
    0
    Uploads
    0

    Default

    This link takes you to a page on the Haas website:

    http://www.haascnc.com/custserv_updates.asp#manualupd

    Scroll down about halfway and you will see a column with this at the top:

    Turning Centers Manual Addendums

    The first entry in this column is:

    Bar 300
    96-0013AJ

    This is a pdf file that has all the information about setting up and operating the Servo 300 barfeed; you can download it.

    An open mind is a virtue...so long as all the common sense has not leaked out.


  10. #10
    Registered
    Join Date
    Apr 2004
    Location
    Serbia and Montenegro
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by wganders View Post
    Thanks Tex,

    That's exactly the kind of sample I'm looking for. It looks like you position a stop for the bar feeder to push against. Is that correct? Do you have any idea what all the special codes do? Like all the special M codes, etc... I hate to seem dumb but I like to get as much detail as I can.

    Thanks again,
    Bill
    You're very welcome.

    Yes, I've been using a specially made, but simple, tool as a bar stop. It was mounted like all the other tools, similar to the one on the attached picture.

    I know what "G" and "M" functions do. There is a simple file that lists all the HAAS G and M codes, I could mail it to you. You will find all these functions listed in the manual, which should be downloadable from HAAS site.

    M05 - SPINDLE STOP
    M10 - CHUCK CLAMP
    M11 - CHUCK UNCLAMP
    M51 - OPTIONAL USER M CODE SET
    M61 - OPTIONAL USER M CODE CLEAR
    M96 - JUMP IF NO SIGNAL (P,Q)
    M99 - SUB-PROGRAM/ROUTINE RETURN OR LOOP (P)
    M121- OPTIONAL USER M CODE INTERFACE WITH M-FIN SIGNAL

    You don't seem dumb at all. A few years ago, when I had a lot of trouble programming SL-30 to do a thread deburring routine, guys from this forum helped me and their help was priceless!

    Attached Thumbnails Attached Thumbnails Bar Feed Program for Haas Lathe-barstop-jpg  


  11. #11
    Registered
    Join Date
    Apr 2004
    Location
    Serbia and Montenegro
    Posts
    60
    Downloads
    0
    Uploads
    0

    Default

    I’ve forgotten to mention that units in the barstop subroutine I'd posted above are millimeters.



  12. #12
    Registered
    Join Date
    Mar 2009
    Location
    usa
    Posts
    23
    Downloads
    0
    Uploads
    0

    Default

    Look inside the door on the controls, both of ours have the G & M codes posted there for a reference. As well as pressing "Help" on the control panel and getting them listed for you on the monitor. If you have a Haas rep that frequents your shop, ask if they still have the little red or green books with lots of tips and notes. Usually give 2 or 3 out when you get a new machine.
    Frequent their website, has a lot of helpful info.

    regards
    P.G.



  13. #13
    Member
    Join Date
    May 2007
    Location
    USA
    Posts
    1003
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by Geof View Post
    This link takes you to a page on the Haas website:

    http://www.haascnc.com/custserv_updates.asp#manualupd

    Scroll down about halfway and you will see a column with this at the top:

    Turning Centers Manual Addendums

    The first entry in this column is:

    Bar 300
    96-0013AJ

    This is a pdf file that has all the information about setting up and operating the Servo 300 barfeed; you can download it.
    Thanks Geof. Not sure if I saw that page, but am saving the link 'just in case.' Never know when it might come in handy.



  14. #14
    Member
    Join Date
    May 2007
    Location
    USA
    Posts
    1003
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by wganders View Post
    Sorry I missed it but thanks to G-Codeguy for his information! It is much appreciated.

    Bill
    Bill. Sorry that I couldn't be of any help. Have never run a Haas.



  15. #15
    Registered
    Join Date
    Oct 2008
    Location
    USA
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default

    I know this thread is old, but we run a Haas TL-25 with a Servo Bar Feeder. The g code we use is G105 with I,J, and K variables. I is Initial Push Out, J is Part length + cutoff tool width, and K is Minimum clamping length. You have to set the "reference point" of the bar feeder to the face of the chuck or collet, then it will push out the exact "I" length from there.



  16. #16
    Registered
    Join Date
    Feb 2010
    Location
    Lebanon
    Posts
    3
    Downloads
    0
    Uploads
    0

    Default

    hello dears
    i have Gsk cnc Lathe,i have manual barfeeder,somebody can write for me any program how i can use my machine with this barfeede,any small example please



  17. #17
    Registered
    Join Date
    Jan 2010
    Location
    USA
    Posts
    6
    Downloads
    0
    Uploads
    0

    Default

    I can't remember for sure, but I think we had the same setup when I was in school. on the sl20, go to the current commands screen and page down. you will find a page to input initial push length, push length, how many parts/bars, etc. The command to feed the bar is g105. Once all is set up, you can just use g105 in your program. while you are setting it up, lift the cover on the bar feeder and you will see a list of q values. you use these with the g105 (g105 q8) i can't remember what each q does, but it'll say under the cover.



  18. #18
    Member pedrog1's Avatar
    Join Date
    Apr 2020
    Posts
    1
    Downloads
    0
    Uploads
    0

    Arrow hola soy nuevo necesito ayuda para programar un cargador de barras fedek dh65l s2

    hi i am new i need help to program a fedek dh65l s2 bar loader on a fanuc oi-tf lathe. thank you in advance



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

Bar Feed Program for Haas Lathe

Bar Feed Program for Haas Lathe