Desperately need help cutting threads
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 24
  1. #1
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default Desperately need help cutting threads

    I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi Iím assuming that Iíll have to use the G32 code? Iíve never programmed a lathe before and am pretty lost. They are internal threads 1.125Ē deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.

  2. #2
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,040
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    267

    Default

    What controller?

    Just program it up in cam software if you donít know how to write gcode?

    Im confused how someone who doesnít know anything about a cnc lathe can end up programming one?

  3. Likes lumley32 liked this post
  4. #3
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Itís a hitaci seiki with a seicos j300L control. Iíve operated turning centers in the past and have edited programs but have only written one program. I donít have no cam software. No one in this shop knows anything about this machine I was just thrown to the wolves.

  5. #4
    Join Date
    Sep 2005
    Location
    Dunstable, UK
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    28

    Default

    Quote Originally Posted by Cec330 View Post
    Itís a hitaci seiki with a seicos j300L control. Iíve operated turning centers in the past and have edited programs but have only written one program. I donít have no cam software. No one in this shop knows anything about this machine I was just thrown to the wolves.
    Bloody hell this is ridiculous & downright dangerous!!!You need proper training & experience to run CNC & manual machines.Your so called managers need to get a grip & organise training etc.
    Tony

  6. #5
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    127
    Post Thanks / Like

    Default

    You don't have a programming manual for the machine?

  7. #6
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Tony Iíve been a machinist since 1993 itís all Iíve ever done, Iíve operated every machine tool you can think of Iíve just never programmed a turning center. Iím just asking for help figuring out how to cut these threads.

  8. #7
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Yes I have a programming manual but it says nothing about how to program threading.

  9. #8
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,360
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    657

    Default

    Quote Originally Posted by Cec330 View Post
    It’s a hitaci seiki with a seicos j300L control. I’ve operated turning centers in the past and have edited programs but have only written one program. I don’t have no cam software. No one in this shop knows anything about this machine I was just thrown to the wolves.
    What model/year?
    I may have some old progs as samples that I can dig out on a backup somewhere....

  10. #9
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    Year about 1993 and model hires-turn 20J

  11. #10
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    622
    Likes (Received)
    69

    Default

    Quote Originally Posted by Cec330 View Post
    I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi Iím assuming that Iíll have to use the G32 code? Iíve never programmed a lathe before and am pretty lost. They are internal threads 1.125Ē deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.
    Keeping it simple

    G97 S250 M3
    G0 X5.1 Z0.3 M8
    G92 X5.42 Z-1.125 F0.0833
    X5.43
    X5.44
    X5.45
    X5.46
    X5.470
    X5.477
    X5.483
    X5.488
    X5.493
    X5.497
    X5.5
    X5.502
    X5.504
    X5.505
    G0 Z0.5 M9
    G30 U0 W0
    M1

  12. #11
    Join Date
    Mar 2017
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    16
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2

    Default

    I stopped and talked to an old buddy of mine that programs and he told me about the G76. Iím trying to convert his fanuc program to my machines style of program.

  13. #12
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,360
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    657

    Default

    Quote Originally Posted by Cec330 View Post
    Year about 1993 and model hires-turn 20J
    Sorry - just checked and the only ones I have are backups for the milling section!

    I did a google and found this?
    Hitachi Seiki HT20!23!30J Programming J300L | PDF

  14. #13
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    435
    Post Thanks / Like
    Likes (Given)
    99
    Likes (Received)
    137

    Default

    The G76 format for the J300L is a single line and is as follows:

    G76 X Z K D F A

    X= diameter of final pass
    Z= ending Z position
    K= height of thread
    D= depth of 1st path
    F= thread lead
    A= angle of thread

    The Fanuc G76 cycle will probably be the 2-line format and will look something like this:

    G76 P010055 Q0015 R0.0015
    G76 X5.505 Z-1.125 P0475 Q0150 F0.083333

    The J300L version of that would look like this:

    G76 X5.505 Z-1.125 K0.0475 D0.0150 F0.083333 A55

    I hope this helps. I have a HT23J with J300L control. Let me know if you've got any other questions about the machine.

  15. Likes Houndogforever, pr0xify, kenton liked this post
  16. #14
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    3,251
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3212

    Default

    All I can say is WOW... I sure don't want to be anywhere near when the program first gets fired up and run.
    I'm with modelmakerblue on this ...bring spare underpants when you push the green button for the first time.

    Better yet, post your code here before you load it into the control.
    No guarantees, but if there's an obvious mistake in your code, hopefully someone will catch it and keep you from slamming the turret into the chuck or something else equally exciting.

    Whoever is OK with turning you loose on this has got big brass ones for sure.
    Will he still be OK when you crash the lathe?

    Good luck with it.

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

  17. #15
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    627
    Post Thanks / Like
    Likes (Given)
    23
    Likes (Received)
    306

    Default

    Are there no backup files anywhere? A pc somewhere in the shop with saved program files? It is highly unlikely that the previous operator cleaned out all the companies program files for this machine and the parts it ran (unless there was some serious bad blood). Most machines have a limited amount of memory available making it impractical (not to mention foolish) to leave all the programs on the control with no backup.

  18. #16
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    9,166
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    4450

    Default

    This wonderful machine can't run standard G33 threading passes ? Thats easy to figure out and also easy to single-block. It's pretty foolproof.

  19. #17
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,188
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1787

    Default

    Quote Originally Posted by Cec330 View Post
    I took a new job this week as an operator only to find out that the previous fella that ran this machine wiped all the programs out of the machine. I need help writing a program to cut 12 tpi I’m assuming that I’ll have to use the G32 code? I’ve never programmed a lathe before and am pretty lost. They are internal threads 1.125” deep inside of a 5.410 inside diameter. Just an example program would help a bunch. Thank you in advance for any help.
    Hello Cec330,
    Your control can use a Multi-repetitive Threading Cycle G76 in the following format:

    G76 X_ _ Z_ _ K_ _ D_ _ F_ _ A_ _ P_ _

    Where:
    X = X Coordinate of Minor Dia. when cutting and External Thread. Major Diameter when cutting an Internal Thread.
    Z = Z Finish Coordinate
    K = Thread Height (Radius Value)
    D = DOC for the first Threading Pass (Radius Value)
    F = Lead of Thread
    A = Included Angel of Thread Form (Included Angel of Threading Insert)
    P = Cutting Pattern (P1 to P4)

    The Cutting Pattern most commonly used is specified by P1 (Constant Cutting Amount - Single Cutting Edge). If the "P" address is omitted, P1 is assumed by the control.

    When cutting an Internal Thread, the Major Diameter is specified by the X address and the Thread Height by the K address. Given these two values, the control calculates the coordinate of the Minor Diameter, with the First Pass and all subsequent DOC being applied from that calculated diameter.

    In your example, you have specified the Minor Diameter and Thread Pitch (Lead). On the assumption that it a 60deg. Thread Form, the Major Diameter is 5.5".

    To cut an External Thread, you initially park the Threading Tool at a diameter larger than the Major Diameter, and for an Internal Thread, at a diameter smaller than Minor Diameter of the Thread. Provided the X and K values have been correctly specified, the control determines whether an Internal or External Thread is being cut by comparing the specified X value in the G76 Cycle and the current position of the Threading Tool in X.

    Constant RPM spindle speed should be specified and not Constant Surface Speed. If a not too difficult to cut steel is the material being used, a reasonable starting CSS would be circa 490SFM and at a Major Diameter of 5.5", that equates to 340RMP.

    Because the tool must accelerate from Zero to a Z axis Slide Velocity equaling the Thread Lead x Spindle RPM, each time a Threading Pass is Started, the tool should be parked at a Z coordinate far enough away form the start of the Thread, so that the correct Slide Velocity is reached before starting to cut. If not, then the lead of the first part of the Thread will be incorrect. The greater the Slide Velocity, the greater distance required for the correct Slide Velocity to be reached. There is a formula for calculating the minimum distance required, but with a Spindle Speed of 340 RPM and a Thread Lead of 0.0833" a 0.25" standoff in Z will be plenty.

    So, putting all the above together, a G76 Block something like the following will get you close:

    G76 X5.5 Z1.125 K0.0496 D0200 F0.08333 A60 P1

    Incorporated into the program, it may look something like the following for your control:

    N2 G28 U0.0
    G28 W0.0
    T0100 G97 S340 M03
    G00 Z0.25 T0101 M08
    G00 X5.3
    G76 X5.5 Z1.125 K0.0496 D0200 F0.08333 A60 P1 (P1 could be omitted)
    G28 U0.0 M09
    G28 W0.0
    M01

    Regards,

    Bill
    Last edited by angelw; 09-24-2021 at 04:55 PM.

  20. Likes Mtndew, barbter liked this post
  21. #18
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    6,145
    Post Thanks / Like
    Likes (Given)
    5754
    Likes (Received)
    3928

    Default

    Man, if it were me, I'd be looking for another place of employment. It says a lot about the company and how much they want to grow when nobody in the higher-ups know how to do a simple lathe program.
    I feel for ya, it doesn't sound like a great place to work.

  22. Likes Pathogen, barbter liked this post
  23. #19
    Join Date
    Aug 2010
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    129
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    27

    Default

    Quote Originally Posted by implmex View Post
    All I can say is WOW... I sure don't want to be anywhere near when the program first gets fired up and run.
    Doesn't anyone dry run, single block with feeds turned way down anymore? Or does everyone just simulate and send it now?


    Quote Originally Posted by Mtndew View Post
    Man, if it were me, I'd be looking for another place of employment. It says a lot about the company and how much they want to grow when nobody in the higher-ups know how to do a simple lathe program.
    I feel for ya, it doesn't sound like a great place to work.
    The guy that left and wiped the programs had the same idea. Isn't that straight up theft?

  24. Likes EnderDRM liked this post
  25. #20
    Join Date
    Oct 2007
    Country
    SPAIN
    Posts
    5,360
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    657

    Default

    Quote Originally Posted by Mtndew View Post
    Man, if it were me, I'd be looking for another place of employment. It says a lot about the company and how much they want to grow when nobody in the higher-ups know how to do a simple lathe program.
    I feel for ya, it doesn't sound like a great place to work.
    +1
    Not wanting to pile on the OP as he's obviously been dropped in the shit, but whenever I read threads like this, I wonder how places are and stay, in business.
    I'd be looking too....


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
  •