1 1/4 - 11 1/2 internal thread
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default 1 1/4 - 11 1/2 internal thread

    I need some help.

    Each pass is getting smaller not bigger like it needs to do.

    I put this together myself.

    G76 P000060 Q0025 R.0005
    G76 X1.562 Z-1.250 P0695 Q0005 R-.0387 F.0869

    The second line the R value is negative which makes the taper go the right way but nothing I have done so far will make each pass go deeper.

    Its bored out to 1.5

    What am I doing wrong?

  2. #2
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,779
    Post Thanks / Like
    Likes (Given)
    1172
    Likes (Received)
    1901

    Default

    What X are you at before you call the threading cycle?

  3. #3
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    396
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    115

    Default

    Starting X position being too large would be my first guess.

    But then that Q value in the 2nd line is way too small. I wonder if that could cause issues.

  4. #4
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1740

    Default

    Quote Originally Posted by blueboy View Post
    I need some help.

    Each pass is getting smaller not bigger like it needs to do.

    I put this together myself.

    G76 P000060 Q0025 R.0005
    G76 X1.562 Z-1.250 P0695 Q0005 R-.0387 F.0869

    The second line the R value is negative which makes the taper go the right way but nothing I have done so far will make each pass go deeper.

    Its bored out to 1.5

    What am I doing wrong?
    Hello blueboy,
    As alluded to by wmpy and Booze Daily, the control determines the direction to apply the DOC by comparing the current X position of the Threading Tool and the X coordinate specified in the second G76 Block. If the Tool is at an X position less than the X coordinate specified in the G76 Block, the DOC will be applied in a plus direction.

    In your first G76 Block, you have the minimum DOC increment set at 0.0025", but in the second G76 Block, the first DOC pass is set at 0.0005", which is less than the minimum DOC set in the first G76 Block. The G76 Cycle sets each successive DOC using the following algorithm:

    DOC = d x SQR(N)

    Where:
    d = first pass DOC set in the second G76 Block
    N = the Nth number of the Threading Pass (1st, 2nd, 3rd etc.)

    The control continues applying the DOC based on the above algorithm until the DOC calculated for the next pass, minus the DOC for the previous DOC is less than the minimum DOC set in the first G76 Block.

    Accordingly, you should make the first pass DOC at least as large as the minimum DOC set in the first G76 Block. Rule of Thumb, is that the First Pass DOC should be whatever the work-piece set up and the Threading Tool can handle. Of course, you would start off with an initial DOC that is conservative and then increase it to achieve the best cycle time and tool life. Having the whole thread cut with a DOC that doesn't exceed 0.0025" is just wasting time.

    Notwithstanding that you say that the taper amount (radius value) has been set as a negative value and you're getting the taper applied in the correct way, this is not the way in which it should be applied, if its a Fanuc control and Negative is towards the centre line of the machine.

    For an External Thread, the Minor Diameter of the Large Diameter of the Taper is specified with the X coordinate of the second G76 Block and the Taper specified as the difference in the Thread Radius in a Negative direction.

    For an Internal Thread, the Major Diameter of the Small Diameter of the Taper is specified with the X coordinate of the second G76 Block and the Taper specified as the difference in the Thread Radius in a Positive direction.

    Regards,

    Bill

  5. #5
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    Before the cycle X is 1.640

    Wow Bill that is going to take some analyzing.

    Thanks guys! Hopefully I'll get it working tomorrow. I'll let you know how it goes.

  6. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    8,333
    Post Thanks / Like
    Likes (Given)
    451
    Likes (Received)
    2217

    Default

    G00 X1.4 Z.1
    G76 P000060 Q0025 R.0005
    G76 X1.562 Z-1.250 P0695 Q005 R.0387 F.0869

    That should work as you've intended it to,

  7. #7
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    396
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    115

    Default

    For the taper to have a negative value but appear to be moving in the correct direction, it makes me wonder if the internal threading bar hasn't been mounted "upside down". Make sure the cutting edge of the threading tool is pointed in the positive X direction.

  8. #8
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    Quote Originally Posted by SeymourDumore View Post
    G00 X1.4 Z.1
    G76 P000060 Q0025 R.0005
    G76 X1.562 Z-1.250 P0695 Q005 R.0387 F.0869
    This makes each pass go deeper but the taper is going in the wrong direction.
    If I put the R-.0387 back in the angle is right but the each pass gets smaller.

    The BB is up side down and the spindle is CCW G97M04S500


  9. #9
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    396
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    115

    Default

    Can you mount your tool right side up? If the tool is upside down, you have to change your program to use negative X values.

    And why are you using M04? Is your tool left hand cutting? Won't that make left hand threads? I've never heard of a left hand NPT thread.

  10. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1740

    Default

    Quote Originally Posted by blueboy View Post
    This makes each pass go deeper but the taper is going in the wrong direction.
    If I put the R-.0387 back in the angle is right but the each pass gets smaller.

    The BB is up side down and the spindle is CCW G97M04S500

    Describe your interpretation of upside down Boring Bar and on what side of the machines centre line are the cutting tools mounted?

    Is the X plus direction toward the back of the machine, or are the cutting tools between the operator and the machine centre line? If the Internal Threading Tool is cutting the bore closest to the back of the machine, that is, with the machine centre line between the operator and the tool, then the Internal Threading Tool should be upside down and the spindle running CCW (looking at the face of the chuck), which would be M03. In this case, a RH Thread would result.

    If the Internal Threading Tool is cutting the bore closest to the operator and the tool is upside down, then the spindle would have to run CW (looking at the face of the chuck) which would be M03. In this case, a LH Thread would result.

    Regards,

    Bill

  11. #11
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    5,106
    Post Thanks / Like
    Likes (Given)
    1335
    Likes (Received)
    2908

    Default

    Quote Originally Posted by blueboy View Post
    I need some help.

    Each pass is getting smaller not bigger like it needs to do.

    I put this together myself.

    G76 P000060 Q0025 R.0005
    G76 X1.562 Z-1.250 P0695 Q0005 R-.0387 F.0869

    The second line the R value is negative which makes the taper go the right way but nothing I have done so far will make each pass go deeper.

    Its bored out to 1.5

    What am I doing wrong?
    Quote Originally Posted by blueboy View Post
    Before the cycle X is 1.640

    Wow Bill that is going to take some analyzing.

    Thanks guys! Hopefully I'll get it working tomorrow. I'll let you know how it goes.
    Quote Originally Posted by blueboy View Post
    This makes each pass go deeper but the taper is going in the wrong direction.
    If I put the R-.0387 back in the angle is right but the each pass gets smaller.

    The BB is up side down and the spindle is CCW G97M04S500

    Notice, your starting position is greater than your finished Major Diameter. That's why your R value isn't acting accordingly. Use 1.4 as a start position, then it's smalker than you finished Major Diameter., and your Minor Diameter.

    I understand your logic, but the controls function needs to be ideal, for all the pieces to operate correctly. The start position should be smaller or equal to (I always go smaller for peace of mind) than the smallest Minor Diameter (the small end of the taper). Theoretically you shouldn't even need an R value, if you were the mathimatical genius that Bill is. I'm just some dummy, and guess at a lot of the values for Tspered Threads. That's how I get through them.

    R

  12. #12
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    4,117
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1740

    Default

    Quote Originally Posted by litlerob1 View Post
    Theoretically you shouldn't even need an R value, if you were the mathimatical genius that Bill is. I'm just some dummy, and guess at a lot of the values for Tspered Threads. That's how I get through them.

    R
    Hello Rob,
    An "R" value is mandatory if a Tapered Thread is to be cut with the G76 Cycle. If its omitted, R0.0 is assumed by the control and a parallel thread will be cut.

    Regards,

    Bill

  13. #13
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    Quote Originally Posted by angelw View Post
    Is the X plus direction toward the back of the machine, or are the cutting tools between the operator and the machine centre line? If the Internal Threading Tool is cutting the bore closest to the back of the machine, that is, with the machine centre line between the operator and the tool, then the Internal Threading Tool should be upside down and the spindle running CCW (looking at the face of the chuck), which would be M03. In this case, a RH Thread would result.
    Is the X plus direction toward the back of the machine YES or are the cutting tools between the operator and the machine centre line? If the Internal Threading Tool is cutting the bore closest to the back of the machine, that is, with the machine centre line between the operator and the tool, then the Internal Threading Tool should be upside down and the spindle running CCW it is(looking at the face of the chuck), which would be M03 Do you mean M04?. In this case, a RH Thread would result.

  14. #14
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,779
    Post Thanks / Like
    Likes (Given)
    1172
    Likes (Received)
    1901

    Default

    M03 is correct

  15. #15
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    396
    Post Thanks / Like
    Likes (Given)
    92
    Likes (Received)
    115

    Default

    It's rare, but I have seen some machine tool builders use M04 for right hand cutting spindle direction instead of the much more commonly used M03. It makes things confusing. What machine is this on?

  16. #16
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    Quote Originally Posted by wmpy View Post
    It's rare, but I have seen some machine tool builders use M04 for right hand cutting spindle direction instead of the much more commonly used M03. It makes things confusing. What machine is this on?
    Bridgeport PowerPath 15
    ROMI Bridgeport

  17. #17
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    img_8944.jpgimg_8942.jpg

    Top of chuck rotates towards you.

  18. #18
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    OK I am going insane! This POS lathe is stupid. Near as I can tell there has to be a way to change for threading the ID. In the manual I found ID threading in MDI or "do event mode". Never had this kind of trouble running a HASS lathe. So I'm still at it. I'll get this figured out, hopefully before I run out of aspirin.


    Actually in my post #8 each pass was not going deeper. Each pass was moving towards the center line. The only thing that would change is the angle depending on the + or - R value.
    Last edited by blueboy; 04-09-2021 at 11:49 AM.

  19. #19
    Join Date
    Dec 2015
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    63
    Post Thanks / Like
    Likes (Given)
    10
    Likes (Received)
    19

    Default

    Well I'm done. I wrote a new program using G78 threading cycle. You put in each pass that gives you total control of the direction and still use the R value for the taper.
    I want to thank everyone for your help!
    This forum is awesome!

    img_8948.jpg

  20. #20
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    216
    Post Thanks / Like
    Likes (Given)
    532
    Likes (Received)
    57

    Default

    G78 threading means your lathe was setup as a mill with the type B Fanuc G code. I'd like to know why that genius decided to do that.


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
  •