Results 1 to 15 of 15
  1. #1
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Question Troublesome 3/4-14 npt program for Okuma

    U10 control:
    Single point ID thread wants to taper up in X, instead of down in X.

    Here's the meat of the program

    G0 X.88 Z.3
    G71 X1.003 Z-1.313 D.015 U.001 B60 A-1.7821 H.082 F.0714
    G0 Z.1

    As I stated, the taper wants to run the wrong way. This is an ID thread.

    Thanks for any help.

    Dean

  2. #2
    Tumbleweed Tim is offline Stainless
    Join Date
    Mar 2002
    Location
    Ramona, Ca. USA
    Posts
    1,377

    Default

    Try A1.7821 instead of A-1.7821.

  3. #3
    CordyCNC is offline Aluminum
    Join Date
    Oct 2007
    Location
    Port Orchard, WA
    Posts
    90

    Default

    Try use I instead of A. example I-.0005 which make .001 diameter smaller at end point than starting point.
    We have 3 Okuma LB lathes here. Their controller use I.

  4. #4
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Thanks, guys, but have tried both the A+ and I (- and +). When sign is changed, control alarms out because of the X start point (it's looking to make an OD thread with +).

    Got a query in with Gosiger in Dayton, but no answer yet.

  5. #5
    dabigguy is offline Aluminum
    Join Date
    Dec 2005
    Location
    Wisconsin east coast
    Posts
    130

    Default

    make the I-.0502, that is the length of the thread multiplied by 1.7833 tangent. I have never used the A in a thread line.

  6. #6
    CordyCNC is offline Aluminum
    Join Date
    Oct 2007
    Location
    Port Orchard, WA
    Posts
    90

    Default

    G0 X.88 Z.3
    G71 X1.003 Z-1.313 D.015 U.001 B60 A-1.7821 H.082 F.0714
    G0 Z.1

    try change to G0 X.80 Z.3

    reference point may need to be below than at end point of thread in first pass. or else it will alarm.

  7. #7
    metlmunchr is offline Diamond
    Join Date
    Jul 2004
    Location
    Asheville NC USA
    Posts
    8,341

    Default

    I think Cordy is probably right. The angle is going to move you in X- by .050 on the radius along the 1.613 total Z travel. I think that's going to put your X value at the end of travel smaller than the X value at the start of the cycle. I can't say specifically with reference to internal pipe threads, but anytime I've ever programmed any canned cycle on one of mine where the cutting motion goes outside the boundaries of the original start point, it'll throw an error.

    Actually, using the angle instead of an I value on tapered threads is a good practice IMO. If you use an I value, but decide for some reason to later change the Z start point, then the angle will be wrong unless the I is recalculated. By programming the angle directly, you can change the Z start and the angle will remain correct. Any part with a tapered cut extending to the end always involves starting at some point in space where the combined X and Z movements will (hopefully) put the tool at the right point when it gets to the part. When the angle is known, as it is on a pipe thread, programming that angle directly gets that one part of the equation nailed down so that you know its not going to be changed indirectly via some change in your other values.

    Friend of mine gets a rush job to chase some internal pipe threads in 316SS. It'll be an ongoing job, but they need about 50 parts fast. Not enough time to order in a plug gage, so they make their own and the comparator says its good. Makes the parts and sends them out, but gets a call in a few days saying they're rejected because the customer's gage goes too deep. By that time his proper plug gage has come in, so he runs a couple parts with the same setup and the depth looks to be right in the middle of where it's supposed to be. So he takes his gage and the extra parts and drives 50 miles to the customer's place. Turns out the customer's gage is some brass fitting whose threads look like they've been run into a hole and WAY overtightened. He shows them that the depth is good using his brand new ground and certified gage, and their only response was "how do you know that thread is right and ours is wrong?" Duhhh

  8. #8
    Tumbleweed Tim is offline Stainless
    Join Date
    Mar 2002
    Location
    Ramona, Ca. USA
    Posts
    1,377

    Default

    ""Actually, using the angle instead of an I value on tapered threads is a good practice IMO. If you use an I value, but decide for some reason to later change the Z start point, then the angle will be wrong unless the I is recalculated. By programming the angle directly, you can change the Z start and the angle will remain correct.""

    Good point Cliff.

  9. #9
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Smile Thanks for all the help, dudes!

    Four guys in the shop (all under 40) with about 35 years experience combined, and this is the first time anyone has tried to single point ID npt. First, tried dabigguy's I value and presto. Then, I realized that the programmer had the wrong H value, and changed that. We got threads before I saw any other posts, and Cordycnc was right about changing the X start point, but had to go to X.79 before it would work. After I messed with the X start point, I tried a positive A for sh!#s and giggles, like Tumbleweed Tim suggested and voila! Here's the best part, app guy at Gosiger in Dayton specifically said "...A-1.7821 for ID npt thread..." He seemed put off when he was told that I-.0502 worked (in relation to Z start point) and A1.7833 was correct..."...well, that's what I use..." Kinda fits with metlmunchr's thread gauge story...

  10. #10
    Tumbleweed Tim is offline Stainless
    Join Date
    Mar 2002
    Location
    Ramona, Ca. USA
    Posts
    1,377

    Default

    Okuma manuals are pretty good but one thing they lack is any examples for ID work. I have had the same kinds of problems with start points in LAP cycles and trial and error is how it usually gets resolved. Some day I will figure out the IGF and cheat a bit. Glad to hear you got it going.

  11. #11
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Tumbleweed,

    I agree with your take on the LAP cycles in ID work. I have been with the Okumas for 'bout a year after 8+ years with Fanuc controls. I think Okuma missed the goal with some of their LAP cycles and canned cycles. I'm not really interested in the IGF, because I like to have contol on varying DOC's with respect to material and workholding. I don't think you can change DOC in a rough turn in IGF to combat notch wear in the insert.

  12. #12
    Tumbleweed Tim is offline Stainless
    Join Date
    Mar 2002
    Location
    Ramona, Ca. USA
    Posts
    1,377

    Default

    You can change an IGF to a MIN file by re-naming it .min. Then you can do anything you want. Same code.

    "After I messed with the X start point, I tried a positive A for sh!#s and giggles, like Tumbleweed Tim suggested "
    I am far enough away that nothing is going to hit me. Ha-Ha (don't know about these new smile icons yet) I hope you ran the graphics and tried it in single block first.

  13. #13
    metlhed is offline Stainless
    Join Date
    Jan 2007
    Location
    Ohio
    Posts
    1,153

    Default

    Good to know 'bout the IGF file to .min. And yes, absoposivetoovley, machine lock, graphics and single block for playing around!!

  14. #14
    Tumbleweed Tim is offline Stainless
    Join Date
    Mar 2002
    Location
    Ramona, Ca. USA
    Posts
    1,377

    Default

    Yeh, as soon as you get complacent it will hurt itself.

  15. #15
    CordyCNC is offline Aluminum
    Join Date
    Oct 2007
    Location
    Port Orchard, WA
    Posts
    90

    Default

    Program create by IGF is pretty easy and faster than write in g-codes. If after you are done with IGF, but still need to tweaky g-codes to make it faster or better lap cycles etc, etc then do it. That is what I always do that.

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
  •