3" Male NPT Single Point with G76

Results 1 to 8 of 8

Thread: 3" Male NPT Single Point with G76

  1. #1
    Member
    Join Date
    Aug 2011
    Location
    United States
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default 3" Male NPT Single Point with G76

    I am having the hardest time with these G76 cycles. Im using the 2 line format for a 3" NPT. However the first single point cut is HEAVY. Like .030" But was told by a few people my program looks fine. Can anyone help me and figure out what I did wrong.

    Here is the Thread Cycle.

    N300(3IN NPT THREAD)
    G00 G97 X10. Z10. T0606 S350 M03
    X4. Z1.
    G01 X3.6 Z.2 F.05 M08
    G76 P020060 Q0030 R0005
    G76 X3.341 Z-1.2 P0373 Q0030 R-.0437 F.125
    G00 X2. M09
    G00 X10. Z10.
    T0600
    M30



  2. #2
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    1567
    Downloads
    5
    Uploads
    2

    Default Re: 3" Male NPT Single Point with G76

    ...the 2nd G76 block/statement Q is 1st pass depth right?
    CNC Fanuc G76 Threading Cycle - Helman CNC



  3. #3
    Member
    Join Date
    Aug 2011
    Location
    United States
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by machinehop5 View Post
    ...the 2nd G76 block/statement Q is 1st pass depth right?
    CNC Fanuc G76 Threading Cycle - Helman CNC
    Yeah I do believe thats correct. But if im not mistaken its set as .003 for first cut. And im getting .030" and the thread tool is plussed up about .04"



  4. #4
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    1567
    Downloads
    5
    Uploads
    2

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by 07BlackOps View Post
    Yeah I do believe thats correct. But if im not mistaken its set as .003 for first cut. And im getting .030" and the thread tool is plussed up about .04"
    snip:
    N5 G76 P010060 Q100 R0.05


    ...Q : Depth of normal cut ( these values are given in hundreds, so the depth of cut will be 0.1 ).



  5. #5
    Member
    Join Date
    Aug 2011
    Location
    United States
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by machinehop5 View Post
    snip:
    N5 G76 P010060 Q100 R0.05


    ...Q : Depth of normal cut ( these values are given in hundreds, so the depth of cut will be 0.1 ).
    I guess im just confused as it seems like my first cut would be .003" regardless. But q100 is going to be .1000 depth of cut?



  6. #6
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    1567
    Downloads
    5
    Uploads
    2

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by 07BlackOps View Post
    I guess im just confused as it seems like my first cut would be .003" regardless. But q100 is going to be .1000 depth of cut?
    ...that's the way it sounds like. Try Q0001 or just Q1 and see what happens dry running it watching the Display readouts
    . I assume decimal points are not allowed but, you might try it too.



  7. #7
    Member
    Join Date
    May 2007
    Location
    USA
    Posts
    1003
    Downloads
    0
    Uploads
    0

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by 07BlackOps View Post
    I am having the hardest time with these G76 cycles. Im using the 2 line format for a 3" NPT. However the first single point cut is HEAVY. Like .030" But was told by a few people my program looks fine. Can anyone help me and figure out what I did wrong.

    Here is the Thread Cycle.

    N300(3IN NPT THREAD)
    G00 G97 X10. Z10. T0606 S350 M03
    X4. Z1.
    G01 X3.6 Z.2 F.05 M08
    G76 P020060 Q0030 R0005
    G76 X3.341 Z-1.2 P0373 Q0030 R-.0437 F.125
    G00 X2. M09
    G00 X10. Z10.
    T0600
    M30
    I noticed 2 things right away. R0005 should be R.0005 P's & Q's have no decimal points. R's do. The 2nd thing was thread height. P0373 is way too small. I've never done a pipe thread that large so I had to look it up. Thread height should be P1000 and I would increase Q0030 (2nd block which is amount of 1st pass) to Q0120 minimum.

    BTW, leading zeros can be omitted. Control reads from right to left which is probably why R0005 works. I use to program lathes that didn't use decimal points at all.

    So it can be written as

    G76 P020060 Q30 R.0005
    G76 X3.341 Z-1.2 P1000 Q120 R-.0437 F.125

    Also Z.2 gives 1.6 revolutions for acceleration before cutting if the thread starts at Z0. You may want to back up a bit. You do realize that P020060 will keep the threading insert in the part at Z-1.2 for one revolution before withdrawing. P020160 will cause the insert to withdraw in the shortest possible distance (along Z-axis).

    Should you go to something like G76 X3.341 Z-1.2 P1000 Q200 R-.0437 F.125 in order to get the number of passes within reason, but have trouble with the insert chipping...lie. Increase P1000. It will make the first cutting depth lighter, but not give as many extra passes than decreasing Q200 to Q150 would.

    Also P020060 only cuts on one side of the insert. I only use it when chatter is giving me a problem even after slowing RPM. Consider using P020029 or P020055



  8. #8
    Member
    Join Date
    Aug 2011
    Location
    United States
    Posts
    14
    Downloads
    0
    Uploads
    0

    Default Re: 3" Male NPT Single Point with G76

    Quote Originally Posted by g-codeguy View Post
    I noticed 2 things right away. R0005 should be R.0005 P's & Q's have no decimal points. R's do. The 2nd thing was thread height. P0373 is way too small. I've never done a pipe thread that large so I had to look it up. Thread height should be P1000 and I would increase Q0030 (2nd block which is amount of 1st pass) to Q0120 minimum.

    BTW, leading zeros can be omitted. Control reads from right to left which is probably why R0005 works. I use to program lathes that didn't use decimal points at all.

    So it can be written as

    G76 P020060 Q30 R.0005
    G76 X3.341 Z-1.2 P1000 Q120 R-.0437 F.125

    Also Z.2 gives 1.6 revolutions for acceleration before cutting if the thread starts at Z0. You may want to back up a bit. You do realize that P020060 will keep the threading insert in the part at Z-1.2 for one revolution before withdrawing. P020160 will cause the insert to withdraw in the shortest possible distance (along Z-axis).

    Should you go to something like G76 X3.341 Z-1.2 P1000 Q200 R-.0437 F.125 in order to get the number of passes within reason, but have trouble with the insert chipping...lie. Increase P1000. It will make the first cutting depth lighter, but not give as many extra passes than decreasing Q200 to Q150 would.

    Also P020060 only cuts on one side of the insert. I only use it when chatter is giving me a problem even after slowing RPM. Consider using P020029 or P020055
    So unfortunately my control doesnt like decimal points at all when it comes to G76 and G83 cycles. We tried them and the machine just pops an error message for incorrect parameters. So I got it figured out. I realized what I was doing when my dumbass realized there is a whole other section of the machinist handbook that is a continued table for pipe threads. But yeah thank you for that information my man. My shop is very old school and usually uses a pipe threader to do NPT male threads. We just dont have a 3" die.



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

3" Male NPT Single Point with G76

3" Male NPT Single Point with G76