8 Replies Latest reply on Mar 4, 2015 8:50 AM by Txon Aguirre

    3D external flow around a submersible hul

    Txon Aguirre

      We have performed a number of simulations for the case in the question. The goal is the drag Force(X) in our settings.

      The fact is that this is a fairly simple external simulation case. Fluid is water, the hull is stream lined, no appendages have been included .......

       

      Conditions are the same and only the initial mesh is changed. Initial mesh level changes from 4 to 8, and a new simulation is started for each case.

      We get no consistent data. I mean each case study gives a different result that shows no relationship or sign of convergence.

       

      May I have any clue about what could be happening and how to solve it ?

       

      I include a results table.

       

      Thanks in advance.DataS.jpg

        • Re: 3D external flow around a submersible hul
          Amit Katz

          I would recommend that you check how many cells your model actually has, rather than just relying on the automatic meshing level. After that, maybe trying using manual meshing techniques to refine your model even further and see how that affects your results.

          • Re: 3D external flow around a submersible hul
            Jared Conway

            the lvl of the mesh is important but what did the mesh actually look like? where was it improved? how many cells were generated? if you looked at the technical reference there is a good description of how meshing is done and that sometimes just increasing the level of mesh won't necessarily increase the number of cells because of the conservation rules in place.

             

            I also noticed that you only looked at one parameter, what did the other parameters look like? velocity...etc. this could just be a challenging value to converge upon. and in the end, what are you comparing it to and what are your expectations? I would recommend taking a look at some of the 2d simulation work that has been done recently and how many cells and the size of the comp domain that are needed in 2d to get good accurate results.

              • Re: 3D external flow around a submersible hul
                Txon Aguirre

                Hi all:

                Thanks for your answers.

                Jared: I spect a dragg of about 2-3 Newtons. Thats why all solutions I've got are inside the expected values and I cant discard any of them.

                I've only attached my goal results, but of course I've checked Velocites, pressures, pressure coefficient(Cp) and turbulence intensity for all the cases. The distributions agree with experience and manual calculations(traditional calculation).

                I'll follow your advice and check how each mesh is built (I didn't do it) I agree that there may be the key.

                 

                Thanks a lot.

                  • Re: 3D external flow around a submersible hul
                    Mark Keown

                    How much mesh is enough?  The short answer is when you add more you get the same results.  Once you think you have a valid solution it is good practice to spend some time 'proving' the simulation is stable.  For example make a small change to (one of) velocity, density, mesh... and see if the results are still reasonable.  If making a small change in the simulation gives unexpected results... one can not say the original simulation is valid.

                     

                    There some good ideas on the discussions on air foils that you could use.  Some problems resolved by making the domain larger 20x the length of the object and using local mesh.

                    • Re: 3D external flow around a submersible hul
                      Jared Conway

                      if everything else is right, then I would guess your method of outputting the force might have an issue.

                        • Re: 3D external flow around a submersible hul
                          Txon Aguirre

                          Hi all:

                          I've checked all posts related to my question, all answers and a lot of documentation regarding FloEFD. The problem has been rebuilt taking into account all advices and instructions and is running at this time.

                          The new Domain size is:(LOA=Lenght Over All)

                          10 LOA astern of the hull

                          5 LOA ahead of the hull

                          2.5 LOA each side, over and below  the hull

                          A local mesh has been included

                          Fluid=Sea Water, Winter North Atlantic standard.

                           

                          Kind regards and thanks a lot.

                            • Re: 3D external flow around a submersible hul
                              Jared Conway

                              similar to other posts about aerodynamic forces, i highly recommend starting with some very simple models to get a feel for mesh and comp domain size that is required.

                               

                              a plate, block and sphere are great examples to get tuned up with

                               

                              and also I think you may have missed that I recommended making sure that the way you output the forces is checked. if you do not choose all faces in contact with fluid in a closed loop, your results may be incorrect. check the help and solidworks KB for more about this.

                                • Re: 3D external flow around a submersible hul
                                  Txon Aguirre

                                  Dear Jared:

                                  I've followed all the advices and recomendations, and now my results converge quite well.

                                   

                                  Togheder with a new Domain, I've used a local mesh around the body and faces have been selected clockwise in a closed loop.

                                  Now, inside the same Fluid regime (Similar Re numbers), the relation F/F'= V²/V'² fits inside the expected margins. Where F and F' are drags.

                                   

                                  Thanks and regards for you all