Anyone else have a HAAS TL1 Next Gen Controller (threading issue) - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 58
  1. #21
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,612
    Post Thanks / Like
    Likes (Given)
    1512
    Likes (Received)
    1711

    Default

    Quote Originally Posted by LMNTS View Post
    Everybody:

    Yes, we used proper tools for measuring the thread minor OD. We have several people do it. It's off by 0.035" (not deep enough).

    Yes, we are using the proper measurement tools, the proper settings for the tooling, AND the proper G Code for the expected thread.

    We have tried this upside down, backwards, and in 8 different languages. We have had the experts of experts in here.

    It's either a machine problem, software problem, or Haas problem.

    My main goal of this post was to find someone with the same model and generation machine to confirm if what Haas is telling me is true.... that they do this on purpose.
    I still don't understand why you are checking the minor dia on an OD thread?. What does the PD check? Is it also off by .035" ??

    Just a thought, take your threading tool and program a little turn, maybe .25" long so you can accurately check, and let us know if that is the correct diameter. That might at least point to the threading cycle or a tool/offset problem...

  2. Likes doug925 liked this post
  3. #22
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,612
    Post Thanks / Like
    Likes (Given)
    1512
    Likes (Received)
    1711

    Default

    https://www.natool.com/wp-content/up...atp101-102.pdf

    https://www.fastenal.com/content/fed...s%20Design.pdf

    I'm sure there is a ton more info, my point is minor diameter is a poor choice for checking threads....

  4. #23
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Minor Dia, Major Diameter - it doesn't matter. The machine is not going deep enough by roughly 0.035".
    Simply put, the machine is deciding on it's own to not go to 0.416 like it says it will.

    Turning on this machine is only off by 0.001" or 0.002", which in my mind is great!

  5. #24
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Quote Originally Posted by Mike1974 View Post
    https://www.natool.com/wp-content/up...atp101-102.pdf

    https://www.fastenal.com/content/fed...s%20Design.pdf

    I'm sure there is a ton more info, my point is minor diameter is a poor choice for checking threads....
    It doesn't matter what we measure. It's all off by 0.035" for a 1/2-13 thread. Turning anything on this machine is dead on. It's only threading.

  6. #25
    Join Date
    Sep 2006
    Location
    SW Wisconsin
    Posts
    491
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    115

    Default

    (THREAD MAJOR DIAMETER = 0.5)
    (THREAD MINOR DIAMETER = 0.416923)
    (THREAD HEIGHT PER SIDE = 0.048077)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< PER SIDE!!!!!!
    (OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
    (SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
    T505
    G54
    G97 S550 M03
    G00 Z0.01
    G00 X0.52
    M08
    (**WATCH FOR LIVE CENTER INTERFERENCE**)
    (RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
    G00 X0.52 Z0.01 M24<<<<<<<<<<<<<<<<,should Z be larger???
    G76 X0.4169 Z-3. K0.0481 D0.012 F0.0769 A60<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< DIAMETER!!!!!!!!!!!!!!!
    G00 Z0.01
    M09



    After fixing that get away from the idea of measuring minor diameter, it WILL fake you out! Get a thread mike or at least thread wires if you want to do the best job.

    Ed.

  7. #26
    Join Date
    Dec 2003
    Location
    poulsbo, wa, usa
    Posts
    722
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    298

    Default

    This might sound nuts but give this a try .

    Set up your threading tool and just run it as a normal turning tool and spin a shaft down to lets say 1.000 dia with just a simple G1 feed move and then verify the dia it cut. without screwing with any of the cutter comp setting then run a G76 with a X dia of .950 and a low feed per rev of like .005 and see what the cut dia is ?

    ** ONLY SET X AND Y offsets for the threading tool ,,, leave all other lines blank for that tool offsets.

    That well tell you if the infeed for the G76 cycle is reading right or not ...

    Also check with Haas if the control might be using a infeed at a angle and not just in X direction. I some place remember reading about a control setting to change how the is done well doing a G76 on Haas

  8. Likes doug925 liked this post
  9. #27
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Quote Originally Posted by atex57 View Post
    (THREAD MAJOR DIAMETER = 0.5)
    (THREAD MINOR DIAMETER = 0.416923)
    (THREAD HEIGHT PER SIDE = 0.048077)<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< PER SIDE!!!!!!
    (OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
    (SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
    T505
    G54
    G97 S550 M03
    G00 Z0.01
    G00 X0.52
    M08
    (**WATCH FOR LIVE CENTER INTERFERENCE**)
    (RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
    G00 X0.52 Z0.01 M24<<<<<<<<<<<<<<<<,should Z be larger???
    G76 X0.4169 Z-3. K0.0481 D0.012 F0.0769 A60<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<< DIAMETER!!!!!!!!!!!!!!!
    G00 Z0.01
    M09



    After fixing that get away from the idea of measuring minor diameter, it WILL fake you out! Get a thread mike or at least thread wires if you want to do the best job.

    Ed.

    Hi Ed, after fixing what? Per Side! Diameter!!

    Not sure what you're talking about.

    Try running the program I posted on your machine and tell me what happens!

  10. #28
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    31
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default

    How many passes does the machine make to get to its final point? Curious if its stopping early or if its going to the wrong location.

    Going to throw something stupid into the ring: try checking your G76 minimum depth of cut setting (Setting 99). Remember the D is, unless stated otherwise, the INITIAL depth of cut. It reduces it from that point based on the A value to keep constant cross section. D.012 is a pretty small number, so your definitely hitting that setting. I don't know the behavior if the minimum cut is 0. It may just stop. We had our machine set to .003 I think. Could also try adding a P3/P4 to the Gcode line, it'll infeed the D value the constant amount. The conversational wont do that for you though.

  11. #29
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    21

    Default

    i replied to your other thread as well:

    so i just made a 1"-12 thread on the TL1 here at the Haas Factory, and I used VPS to program the thread

    both VPS and the internet say the minor diameter is nominally .909

    I had to budge the X wear offset by -.013 to get the go gauge to fit, which is typical.

    i don't think there's anything wrong with your machine.

  12. Likes Booze Daily liked this post
  13. #30
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    21

    Default

    here's the program i used

    %
    O02323 (THREAD)
    (OD THREAD CYCLE)
    ( SAFETY LINE BELOW )
    G00 G54 G18 G40 G80 G97 G99
    (TOOL = 2 / OFFSET = 2)
    (WORK OFFSET = 54)
    (SPINDLE RPM = 630)
    (THREADS PER INCH = 12.)
    (THREAD MAJOR DIAMETER = 1.)
    (THREAD MINOR DIAMETER = 0.91)
    (THREAD HEIGHT PER SIDE = 0.052083)
    (OPTIMIZED "A" VALUE FOR 60 DEGREE THREADS)
    (SEE SETTINGS 95, 96, 99 AND 289 ON THE CONTROL)
    T202
    G54
    G97 S630 M03
    G00 Z0.3
    G00 X1.4
    M08
    (**WATCH FOR LIVE CENTER INTERFERENCE**)
    (RECOMMENDED Z-AXIS START IS 3 THREADS FROM START POINT)
    G00 X1.4 Z0.3 M24
    G76 X0.91 Z-1. K0.0521 D0.013 F0.0833 A59
    G00 Z0.3
    M09
    G00 G53 X0.
    G00 G53 Z0.
    M05
    ( END OD THREAD CYCLE )
    M01
    %

  14. #31
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Thanks for the reply.

    Any chance you can do a 1/2-13? We don't do any 1" and we don't have inserts to try your program and verify.

    On the 1/2-13 it says it would go to 0.416, but it is off around 0.035" every time, regardless of insert, insert age, etc.

    If there is nothing wrong with the machine, I would expect that you would have to do something similar.

  15. #32
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Also, can you please tell me where you are setting your X wear offset of -.013"?

  16. #33
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    21

    Default

    if the machine is making good 1" threads, it will also make good 1/2" threads; i made a 1" since that was the gauge i had handy.

    you never said how much X wear offset you were making when dialing in your thread.

    if your go gage won't go, keep subtracting -.003 from the X wear offset until it goes nicely.

    I think that's what you're missing

  17. #34
    Join Date
    Oct 2012
    Location
    Orange county, CA
    Posts
    99
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    21

    Default

    on the tool offset page, scroll to the right until you can see the wear offset. you can't just type in -.013, you have to sneak up on whatever value incrementally, generally by less than the tolerance of your pitch diameters which should be listed on your gauges.

  18. #35
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,089
    Post Thanks / Like
    Likes (Given)
    656
    Likes (Received)
    1059

    Default

    Are you sure you have your X offset set correctly? If you program it to go to .416 but have to cheat it .035 , it doesn’t sound like it.

    How are you checking the minor?

    Ok, so now you have your thread insert cutting at .416. Now what?
    It’s still not gonna gage. You need to edit the X value until it does.
    Who cares what that number is if you get a good thread.


    Also, you don’t say what kind of threading tool you’re using. If it’s a Top Notch style your X offset between a groove insert and thread insert won’t be the same.

    Also, the major dia for a 1/2-13 isn’t .500 you need to turn it down

    Also, if you edit your target X make sure you adjust your K accordingly or you’ll take a hellacious first cut.

  19. #36
    Join Date
    Sep 2006
    Location
    SW Wisconsin
    Posts
    491
    Post Thanks / Like
    Likes (Given)
    15
    Likes (Received)
    115

    Default

    Hi Ed, after fixing what? Per Side! Diameter!!

    Not sure what you're talking about.

    Try running the program I posted on your machine and tell me what happens!



    The point I was looking at was a possible wrong parameter that uses diameter instead of radius on offsets.

    My nephew has a TL1 and said the program you list as correct, check your offsets.

    Get a thread mike or wires so you can get a true reading of size and/or keep cutting deeper until a nut fits.

    Do you know how pitch diameter works?

    Ed.

  20. #37
    Join Date
    Nov 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    18
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    1

    Default

    Quote Originally Posted by coyoinu View Post
    on the tool offset page, scroll to the right until you can see the wear offset. you can't just type in -.013, you have to sneak up on whatever value incrementally, generally by less than the tolerance of your pitch diameters which should be listed on your gauges.
    I will try this first thing Monday morning and feedback our results.

  21. #38
    Join Date
    Feb 2013
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    668
    Post Thanks / Like
    Likes (Given)
    139
    Likes (Received)
    717

    Default

    Quote Originally Posted by LMNTS View Post
    I will try this first thing Monday morning and feedback our results.
    Also, when it is running the final pass, look at the X position on the DRO... what does it read?

  22. #39
    Join Date
    Jun 2016
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    235
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    105

    Default

    How long have you ran cnc lathes? You are freaking out over this not working yet anyone that has run any amount of CNC lathes know you have to fudge things. Whether it was an old Dynapath or a Mori Seiki I have ALWAYS had to fudge. The thing being though, is normally once you figure out by how much on what lathe, you put that in your wear offset, so then you don't have to mess with the programs.

    Also the fact you will not explain how you are taking measurements is a little disturbing. You should be using a thread wire guage set if you to have a optical guage to check minor. Also, your Z was 3in long which could result in deflection easily if you are not using a tailstock(noticed your program warns user , but didn't know if you are)

    Good luck, but this is small peanuts compared to guys running 11 axis lathes. Adjust your wear for that thread tool and get on with making parts.

  23. Likes g-coder05 liked this post
  24. #40
    Join Date
    Mar 2013
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,763
    Post Thanks / Like
    Likes (Given)
    725
    Likes (Received)
    2073

    Default

    Quote Originally Posted by LMNTS View Post
    We have spent several hundred hours working on this.
    JFC dude... melodramatic much?

    If you've honestly spent "hundreds" of hours on a minor issue that can be fixed by bumping an offset, how the hell do you stay in business?


Tags for this Thread

Bookmarks

Posting Permissions

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