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Pipe Thread in SolidWorks 2016

Question asked by David Roberts on Jan 22, 2016
Latest reply on Jan 26, 2016 by Rick McDonald

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I am trying to create a 3/4-14 NPT on a 1.050" boss in SolidWorks 2016. I have done this dozens of times in successfully in SolidWorks 2015. For some reason, the swept cut only follows the the Helix for a half turn. I have reopened pipe threads created in 2015 (they look fine by the way) to try to see if there is some default setting that is different in 2016 and cannot seem to find any difference. I considered using the new thread tool, but apparently it does not support pipe threads.

Result from SW 2015:

What I get in SW 2016:

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Rick McDonald Jan 25, 2016 9:48 AM
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Looks like it wants your boss diameter to be larger.
Since the thread is tapered it looks like the first thread is cutting but then the boss is not big enough to be cut.
I have only done a few pipe threads and only female threads with 1/8 and 1/4 NPT threads but found I had to change my hole diameter to adjust for the taper.
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- David Roberts @ Rick McDonald on Jan 25, 2016 10:56 AM
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  Rick,
  
  Thanks for your comment. Because of the limits of the model, I could not make the hub any bigger, so I tried making the helix starting diameter smaller. It did not seem to make a noticeable difference. A key point is that I have set up these types of threads dozens of times in SolidWorks 2015 and they work just fine. I think this may be a glitch in 2016. Either that or there is some default setting that is set differently somewhere that I am unaware of.
  
  Dave
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  - David Roberts @ David Roberts on Jan 25, 2016 10:59 AM
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    I have played with this a bit more. This time I tried reproducing the exact same model as I had done in 2015. I even copied the sketches from the 2015 model. No improvement. In the 2016 model the swept cut only follows the helix for a quarter turn, whereas in the 2015 model it follows the entire length of the helix. The only difference I see between the old and the new models is this: the user interface in my 2015 model gives you the option for profile twist "none", whereas in 2016 you do not have this option. The default in 2016 is "minimum twist."
    in 2016:
    
    In 2015:
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    - Jody Stiles @ David Roberts on Jan 25, 2016 11:59 AM
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      Hi guys,
      
      We made a number of significant architectural changes to Sweep in 2016. One of these might be causing the issue you are seeing. Can you get in touch with your SOLIDWORKS reseller and ask them to file a bug on your behalf? With the bug, please submit the models you have in 2015 and 2016 so that we can see what you were getting before and what you are getting now.
      
      A comment about the "None" option from pre-2016. That option is now called 'Natural'. The "None' option actually did have a little natural twist in it but it wasn't always prominent enough to be visible in the result. Depending on the tangent vectors of the helix, the profile could twist a little and so we had/have the 'Minimize Twist' option to remove as much of the natural twist the sweep has in it.
      
      You're correct about the Thread feature, it can only make straight helical threads at this time. We do have an enhancement request for it if you would like to vote for it.
      
      SPR 926901: Ability to create Cut thread on a non - cylindrical face or tapered face or body
      
      Jody
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      - Rick McDonald @ Jody Stiles on Jan 25, 2016 12:38 PM
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        Jody,
        Jody Stiles wrote:
        ....
        You're correct about the Thread feature, it can only make straight helical threads at this time. We do have an enhancement request for it if you would like to vote for it.
        
        SPR 926901: Ability to create Cut thread on a non - cylindrical face or tapered face or body
        
        Jody
        I am really surprised that this is even considered an "enhancement" since NPT threads have been part of the Hole Wizard for years. By definition, NPT threads are tapered not straight. Therefore, this has actually been a "Forever" BUG in SW and should have been addressed and treated as such years ago.
        Whoever is in charge of the hole wizard needs to do a bit more investigation of thread types and their definitions.
        I understand that most people will use straight threads, but NPT is heavily used also.
        
        To be able to do the NPT thread cuts I needed I had to find some features that someone had made as a library feature - and that is also a pain to scale because it doesn't define the thread start point for the taper.
        
        With the new 2016 Thread Feature, this should have been done as part of that and should definitely be look at as a bug in the Thread feature - not an enhancement.
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      - Rick McDonald @ Jody Stiles on Jan 25, 2016 12:40 PM
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        When I click on that link you attached I just get a blank screen.
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        Jody Stiles @ Rick McDonald on Jan 25, 2016 12:54 PM
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        Hi Rick,
        
        You should be getting a screen that looks like the one below (it's what I get when I click the link). I don't know why you aren't. Perhaps try another browser but that really shouldn't make a difference.
        
        Jody
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        David Roberts @ Jody Stiles on Jan 26, 2016 8:36 AM
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        I get a blank screen to in both IE and Google Chrome. Latest versions.
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      - David Roberts @ Jody Stiles on Jan 26, 2016 8:58 AM
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        I did end up contacting my SolidWorks reseller who was able to get this to work. Their comment was "Typically, when you do a 3D type sweep, you want to use the pierce relation instead of a standard coincident."
        
        Upon asking for further clarification, I was told: "I only converted your current thread profile to construction and made a new profile on the same plane to start on the end point of the helix. The pierce relation is easiest selected by selecting the point on the current sketch, then ‘somewhere’ on the curve you’re piercing; the closer to where you want it, the better."
        
        While this got the Swept Cut to work, it locked me into a specific major/minor diameter that could not be adjusted to get better thread appearance.
        In trying different options, what I found was that I simply needed to be on the side of the center line where the Helix end point contacted the front face of the extrusion. I did not need to be at the exact pierce point of the helix, it seems that as long as I was close to it, the swept cut worked. This was good as it allowed me modify the major/minor thread diameter as needed. Another way around this might be to simply adjust the circle diameter dimension of the sketch from which the helix was originally specified.
        
        For whatever reason I never ran into this issue in earlier versions of SolidWorks.
        
        Here are some screenshots of how it worked:
        
        Original Geometry (failed):
        
        Sketch with pierce point relation (worked):
        
        Sketch without pierce point relation, but with geometry close to this point and controlled with parametric dimensions (worked):
        Output using pierce point option (Helix & Sketches Hidden):
        
        Output with alternate sketch option - notice sharper thread appearance (Helix & Sketches Hidden):
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        Rick McDonald @ David Roberts on Jan 26, 2016 9:38 AM
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        Glad you got it working.
        I am not on 2016 but someday maybe and this will help me and others.
        I like your response, nicely detailed and clear.
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Pipe Thread in SolidWorks 2016

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