Conquest 42 threading cycles
Close
Login to Your Account
Results 1 to 15 of 15
  1. #1
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default Conquest 42 threading cycles

    Hello everyone

    I have a Hardinge Conquest 42 that is set to work in inches/minute, and the threading cycles are not working (G32, G76)
    I have tried G32 Z-0.15 F0.0313 for 10-32 thread but the machine does not move

    I have also tried S960 M3 and G32 G98 Z-0.15 F30 but it will not move

    What command do I need to have the threading cycles work?

    Thank you

  2. #2
    Join Date
    Oct 2010
    Location
    Dewees Texas
    Posts
    2,255
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    593

    Default

    I have a GT with the 18T control and on it the G76 threading cycle need to separate G76 lines on with parameters for the thread and another with the usual info. I do not single point that often and have to spend some time studying each time I do an new single point thread.
    Looked at your post again threading in inches per minute with a G98 in the line? Is that even possible? Why not inches per rev. No spindle encoder?

  3. Likes cameraman liked this post
  4. #3
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Quote Originally Posted by FredC View Post
    I have a GT with the 18T control and on it the G76 threading cycle need to separate G76 lines on with parameters for the thread and another with the usual info. I do not single point that often and have to spend some time studying each time I do an new single point thread.
    Looked at your post again threading in inches per minute with a G98 in the line? Is that even possible? Why not inches per rev. No spindle encoder?
    Coul you pleasr provide a sample of theading cycle for a 10-32
    Thanks

  5. #4
    Join Date
    Oct 2010
    Location
    Dewees Texas
    Posts
    2,255
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    593

    Default

    The only 10/32 or 5mm thread we have done on the GT was behind a shoulder with an thread mill.
    Here is a sample of what our machine looks for:
    (7/16 FINE THREAD))
    T26X.49834Z.25
    G76P010000Q00100R.0
    G76X.3749Z-.695P03067Q00970F.05
    G01
    The manual has a bunch of formulas for doing the Parameter line. We do so few that I have to spend some time working it out. I do not think this will help the OP, though.

  6. #5
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,870
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    7672

    Default

    If 2-line:

    G76 P010160 Q00100 R00100
    G76 X.147 Z-.15 P01970 Q00980 F.0312


    0 = If it is an "SP" model machine

    All depends on what year and what control that you have.
    I kan't hep with 1-line programming.


    --------------------

    Think Snow Eh!
    Ox

  7. #6
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Hello
    I just tried the codes then the machine moved the entry in X but then it stops in Z
    The machine doesn't move in Z with G32 or G76

  8. #7
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,870
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    7672

    Default

    Quote Originally Posted by Ox View Post

    All depends on what year and what control that you have.
    I kan't hep with 1-line programming.

    So again - what year and what control?

    0T or 18T are the likely choices - depending on the year.

    Maybe your machine takes a "1 line" threading code?
    Someone else would hafta hep you with that.


    --------------------------

    Think Snow Eh!
    Ox

  9. Likes cameraman liked this post
  10. #8
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Tha nachine has control O-T,
    Year: 2002

  11. #9
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    43

    Default

    will the machine feed in either IPR with the spindle running? Try the following in either MDI or AUTO modes this will determine if you have a spindle encoder feedback problem or not. I am guessing the spindle encoder is faulty as the G32 line you from your first post should have moved the Z axis
    M3S500G97
    G1G99W-.2F.01

    Tom

  12. Likes FaustoShuguli liked this post
  13. #10
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,870
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    7672

    Default

    It heps when you give us all the pertinent info.

    So then it is a Conquest T-42 with an 0i-T control maybe?

    If so - it should take the 2-line program.

    Does the Z axis work otherwise?

    Will it feed in G99?

    I'm guessin' that you somehow lost your spindle encoder.
    I don't know if that's the same as the one used for G99 or not?



    edit:

    That putz Tom snuck in ahead of me....


    ---------------------

    Think Snow Eh!
    Ox

  14. #11
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Quote Originally Posted by Tom View Post
    will the machine feed in either IPR with the spindle running? Try the following in either MDI or AUTO modes this will determine if you have a spindle encoder feedback problem or not. I am guessing the spindle encoder is faulty as the G32 line you from your first post should have moved the Z axis
    M3S500G97
    G1G99W-.2F.01

    Tom
    Hi,
    I have tried G1G99W-.2F.01, the machine does not move.
    Is this a spindle encoder problem??

  15. #12
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Hi,
    The machine is a conquest 42 with one spindle, control O-T, (one line programming)
    the machine has been configured in inch/min (ACT.F)

  16. #13
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,870
    Post Thanks / Like
    Likes (Given)
    5091
    Likes (Received)
    7672

    Default

    Then it's not a 2002.
    I don't even think that they were still building "T"-42's in 2002, but maybe...


    ----------------------

    Think Snow Eh!
    Ox

  17. #14
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    You right,
    There is a mistake in the machine year, the machine is 1990
    FS2000

  18. #15
    Join Date
    Mar 2003
    Location
    Upstate New York USA
    Posts
    281
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    43

    Default

    If the machine will not feed in G1G99 mode then you have a spindle encoder issue, could be the encoder, the wiring or possibly a belt - I believe that there is a timing belt from the spindle to the encoder on those. The same spindle encoder system is used for both IPR (G99) and all threading commands G32, G92, G76.
    On a side note unless someone changed the machine to the Fanuc System Type 10/11 then the G76 threading cycle is a 2 line callout (this was the standard setting on machines shipped), the type 10/11 format is a single line call out and was an option at the time

    Tom


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
  •