13 Replies Latest reply on Jul 20, 2018 4:13 PM by Chase Evans

    Thread simulation

    Bence Rivasz

      Hi,

       

      how can i simulate this threaded connection to get the right stresses everywhere, without rotate the part in 3d.

      -If i fix the face of the bolt where it touches the "nut" (or use any advanced fixture) and take a load onto the nut the stress distribution there wont be accurate.

      -cooling down the bolt (or warm up the nut) to reach the preload  can make deviation: The space between the threads will be different as initial and it can show higher/lower stress.

      1.JPG

       

      3D model  uploaded

        • Re: Thread simulation
          Chase Evans

          Hey Bence - looks like you've moved onto another thread simulation! I'm really commenting because I'm interested to follow whether someone has an answer and to bump your post, I don't actually have a solid answer for you. As far as I can think a temperature differential and actually rotating the bolt/nut is the only things I can think of to get somewhere close to accurate stresses on each portion of the bolt/nut (shank, threads, underhead, etc..).

           

          Something to keep in mind if you are also concerned about the stresses in the bolt is that there will be additional shear and tensile stresses imparted into the bolt due to the combined torsional loading (torquing) and axial loading (bolt stretch) that may be difficult to replicate with other methods, including the temperature delta method.

            • Re: Thread simulation
              Bence Rivasz

              Hi,

               

              yea, during my work i should design many of threaded connections, and sometimes they have asymmetrical loads or/and should be so thin walled / compact as can be possible, so would be great to look behind the curtain of what is going there excatly.

              Thought that this topic with threads is  known more in SW and someone alredy has an off-the-shelf solution, but it looks not so general to simulate a 3D thread.

               

              i also didnt give up the previous bolt simulation with the strange pattern, slowly but it goes : ) I  give a feedback as soon i found something useful.

                • Re: Thread simulation
                  Chase Evans

                  Bence,

                   

                  Thats sounds fascinating. Unfortunately as I think you are finding out this does not seem to be a topic well explored at least in the general solidworks community. Additionally bolts and threaded connections are most often studied for their effects on the joints and surrounding components so certain liberties can be taken with approximation of the fasteners themselves. After analysis of the joint and verifying what kind of loading is imparted onto the fastener, hand calcs are typically sufficient to verify sizing and thread strength - there are plenty of empirical formulas readily available for that.

                   

                  If, as you are trying to do, actual stress distributions in the threads and fasteners themselves is desired to be analyzed as you have found that is much more difficult both I would imagine for the user and computationally difficult for the solver. Additionally any shortcuts as you are searching above (ie: how to analyze without rotating the bolt) will be almost guaranteed to result in some level of approximation in the final analysis - there is likely no way to get the results you seek without fully modeling the interaction. This is because any of these methods are simplified versions of the actual physical reality (ie: pulling the bolt instead of rotating it leaves out torsional forces) because as stated before the actual local stresses are typically not being analyzed but instead their effect on the larger component/assembly - in this case you are concerned with the actual threads themselves those physical realities probably have to be modeled as closely as possible. Because this is also largely uncharted territory at least in the public domain with solidworks it may also be best to verify your results with testing data.

                   

                  I would suggest maybe analyzing each part of the interaction separately (ie: threads vs. bolt face/head) however since you are modeling such a short bolt with threads in contact very near the head of the bolt there is probably quite of bit of interaction between the two which goes into the resulting stress distribution. This might be possible with a longer bolt with more unthreaded length.

                    • Re: Thread simulation
                      Shaun Bentley

                      I remember I was able to simulate your last thread example this with large alpha damping, intel sparse solver, and I think 100 ft.lbs of torque. I didn't bump into convergence difficulty until I added a nonlinear material. (ref: Thread simulation)  Do you need to include permanent deformation of material in your simulation as well?

                        • Re: Thread simulation
                          Bence Rivasz

                          Hi Shaun,

                           

                          i tried to repeat the simulation with the setting what you have described, without any success.

                          Can you please upload your model with the simulation settings?

                           

                          Thanks

                            • Re: Thread simulation
                              Shaun Bentley

                              Bence,

                               

                              I'll have to search on my home machine for it later on.  Will you please upload your attempt?  I would like to take a look at it to see if you might be missing something.  That should be pretty quick for me to do.

                               

                              Thanks,

                              Shaun

                                • Re: Thread simulation
                                  Bence Rivasz

                                  I attached the model which also contains the setup (see original post) It comes without friction and pretty raw mesh because as i realised they do not have any effect about the pattern.

                                   

                                  @James Riddell

                                  the problems with this simplification:

                                  -It supposes that the load distribution is equal on the face where the head of the bolt and the nut has contact. Its not true and influence the stress at the corner and if its close to the first thread like now (or more closer) also make false result with the load distribution/stresses  on the flank of the thread.

                                  -If we have additional loads (side ones or load at the top of the head) its also not works.

                                   

                                  @Chase Evans

                                  in this case, should not be than they go away after the rotation has stopped, with friction 0?

                                  Yes i also do not have a better idea, i calculate with peak stresses and has an additional safety.

                                    • Re: Thread simulation
                                      James Riddell

                                      Bence, I disagree with you about the load distribution (but only from a CAD/FEA POV).  Yes, there are imperfections in the manufacture resulting in the non-uniform boundary conditions but you can't practically model those w/o significant experimental input and fudge-factors.  Suffice to say, from an engineering viewpoint, this would be an easier problem in 2D analysis.  It's been done before and the top 3 threads will take the bulk of the stress - Saint-Venant to the rescue!

                                       

                                      In answer to your loading issue - any additional loading or mis-loading of the head/nut is poor joint design, IMHO.  Any handbook that details bolted/riveted joints can point you in the correct direction to alleviate these issues.

                                       

                                      Of course if this is a purely academic or research exercise then I'd say SW is not the s/w you are looking for (to poorly paraphrase Obi-wan).

                                      • Re: Thread simulation
                                        Chase Evans

                                        Bence,

                                         

                                        I assume you're talking about the "wavelet" formation in the stress distributions and my initial assumption that stick-slip friction has something to do with it? I think you may be right - but also because I believe you said you ran the simulation without friction in the previous thread and the wavelets still appear. I think that one could be crossed off, or at least its effects are minimal.

                                         

                                        What I believe is that either:

                                         

                                        1) its an artifact of the FEA solver and how it solves no-penetration contact, as it seems to me this is a very complex contact problem for the software to handle

                                         

                                        2) its an effect of localized small scale buckling due to the difference in the way the loads are applied to the bolt shank/threads in torsion vs. in pure axial tension

                                         

                                        Or some combination of the two.

                                        • Re: Thread simulation
                                          Shaun Bentley

                                          Thank you for including your model and simulation setup.  I believe the study called "Torque" is the one I should be looking at, though this study does not show any of the characteristics I previously mentioned, i.e., large alpha damping, Intel sparse solver, half cosine load increment.  Let me restate some of this and give a few other recommendations as well.

                                           

                                          1) I do not see any Nonlinear-Dynamic studies in your model.  Therefore it does not appear you have applied any damping.  For this problem, I recommend starting with damping of alpha=100 and then scaling up and down (say 1000 or 10) after some scrutiny of the results.

                                           

                                          2) The study uses a fixed increment of 0.1.  Instead start with a smaller increment.  Change this to auto increment of 0.01 for initial and maximum.

                                           

                                          3) The load does not increase gradually to help convergence.  Use a quarter or half cosine like what I have shown here.  Do not use too many data points.  Maybe make the steps here about 5x larger than the time increment I described in (2) above.

                                           

                                           

                                          4) The study is using the FFEPlus solver.  Change to Intel Direct Sparse.

                                           

                                          5) Make the mesh very coarse initially to speed up trials substantially.

                                           

                                          If you are going to be using Nonlinear in SOLIDWORKS Simulation, you may want to take a quick look at a few troubleshooting tips I posted here:

                                          Nonlinear Analysis Troubleshooting 101 | DASI Solutions Blog

                            • Re: Thread simulation
                              James Riddell

                              Would you get the results you expect if you applied your clamp force under the head of the bolt (red) and grounded the base of the 'nut' (blue)?  Of course you'd have to define non-penetrating, non-bonded surfaces between the bolt & 'nut'.

                              • Re: Thread simulation
                                Chase Evans

                                Bence,

                                 

                                I think the only way you are going to get accurate results for ALL components and contact areas is by torsionally loading the connection (rotation in 3D) like you would in the real world. Additionally, I found the below youtube video which seems to show the "wavelet" creation that you were previously concerned about in your other simulation results. I think this is possibly a combination of several things, namely (1) stick/slip as the face of the thread is loaded axially due to elongation of the bolt as it is rotated (2) localized small scale buckling of the thread as the axial bolt tension attempts to pull it through the female thread (shaun's pulling a sheet of paper through a hole analogy - think of the thread as wrinkling like the paper would) and possibly (3) a result of what happens as the loading is distributed along the thread face. I don't think these are artifacts of the FEA program, I think these are directly a result of the geometry and type of contact - I wouldn't be worried about seeing such distributions, personally.

                                 

                                See 1:20 to 1:60 for the most pronounced visuals. This is from expertfea.com and there is a related tutorial, I might end up buying it and asking the creators some questions on it and see what they have to say.

                                 

                                ANSYS TUTORIAL 11: FINITE ELEMENT ANALYSIS of a Threaded bolt-washer-nut connection (final) - YouTube

                                • Re: Thread simulation
                                  Mohamed El Orche

                                  Hi Bence,

                                   

                                  I think the best way to simulate your threaded connections is to use a non-linear SOLIDWORKS simulation as the bolt preload causes a small plastic deformation. In addition, you need to create great non-penetration contacts and refine the mesh in the interface region.

                                   

                                  Regards

                                  M.

                                    • Re: Thread simulation
                                      Chase Evans

                                      Mohamed,

                                       

                                      I know almost for a fact that Bence has been using a nonlinear solver throughout his simulations. The only difference that Shaun is suggesting is to utilize nonlinear dynamic instead of static. Also i would think the biggest reason for utilizing a nonlinear solver is that from initial contact (ie: fastener is snugged up) to when full preload is achieved (ie: final torque value reached) the fastener can move through a pretty significant angular rotation - even well within the elastic region. I don't think a linear solver could handle such large displacements, at least not with any degree of accuracy. There may be some small local plastic deformations, but I think its impact on the overall model is probably pretty small. Obviously this changes if the bolt is being torque to or past yield - but I don't believe thats what Bence is trying to achieve here.