12 Replies Latest reply on Dec 19, 2008 2:52 PM by Bill McEachern

    Turbulence and boundary layers

    Bob Fratantonio
      Hey guys,
      I am a new user of Floworks and I am trying to model the turbulence of a fairing on the hull of a ferry. The ferry runs at about 10 m/s (~20 knots) and generates a thick turbulent boundary layer on the face of the fairing. In my analysis so far I have not seen the presence of turbulent eddies that I expect, nor do I see a boundary layer on the fairing or the hull.

      For the initial conditions I specify a constant -10 m/s flow. The initial mesh is very fine (I suspect a boundary layer thickness of about 1 inch assuming Re ~10^7). For turbulence parameters I choose turbulent only but I understand that the turbulent energy and dissipation differ in every problem, so I don't really have numbers to insert there.

      My latest attempt includes specifying a boundary condition on the hull and using the flow inlet parameter to specify a 1 inch boundary layer thickness and 0 flow at the boundary. Viewing the results afterwards still shows a constant velocity profile of -10m/s and no turbulent eddies. I worry that I am setting the problem up wrong.

      Can anyone please help?

      Thanks much,
      Bob Fratantonio
        • Turbulence and boundary layers
          Bill McEachern
          the floworks turbulence model is starts to diverge from reality in the R'number range of about 6 million.

          To see the boundary layer you need to turn it on in a cut plot. Open up the options in the lower section of the in the dialog. I doubt you will see any eddies but you will see the growth of the b'layer down the hull.
            • Turbulence and boundary layers
              Bob Fratantonio
              I noticed that I had a warning "Unresolved Boundary condition" when I specify a boundary layer thickness. If I don't specify a value there, will Floworks automatically generate a growing boundary layer?

              I guess my question is this, how should I set up my problem to get a more turbulent flow regime? Is it just simply cranking up the values of k and epsilon? Does Floworks calculate turbulent energy and dissipation or do they leave it constant with the values I provide. From what I understand it is a very bad assumption to say those values are constant.

              Thanks,
              Bob
                • Turbulence and boundary layers
                  Bill McEachern
                  In the real world flows in the free ocean tend to have a high free stream turbulence than what is used in air. That said though i would just run it at the defaults and take a look at what you have as far as b'layers go. Obviously the free surface has an impact onthsi class of problem. You should be using an external flow type of problem and moving a computational domain boundary to an appropriate location to bound the domain. Alternatively you could just run a totally immersed problem. You can set the initial condition in the inital conditions panel and you can set the inital turbulence parameters (intesity and length) there. I would run it witht he defaults first and then run alternate studies and vary it to your hearts content.

                  It would be helpful to know exactly what you are trying to find out?

                  BTW this "My latest attempt includes specifying a boundary condition on the hull and using the flow inlet parameter to specify a 1 inch boundary layer thickness and 0 flow at the boundary. Viewing the results afterwards still shows a constant velocity profile of -10m/s and no turbulent eddies. I worry that I am setting the problem up wrong. " does not make any sense to me. I was pretty busy earlier so I didn't do it justice im my prior post.

                  Don't specify anything on the hull unless you want to assign it a wall condition with say a roughness. This isn't like a panel code with a transpiring wall method for aproximating b'layer effects. The wall model (on all the time) will handle that. Floworks uses the modified wall functions approach as a wall model. You can get the details from the technical reference - dig deep in the install directory. I have to run.
                    • Turbulence and boundary layers
                      Bob Fratantonio
                      Inside the fairing there is a Acoustic Doppler Current Profiler to measure currrent below the hull. The data is garbage because of the presence of air bubbles from the turbulent boundary layer. I want to recreate (as best as I can) this scenario and try to redesign the fairing or perhaps a rail system to create a divergent flow around the fairing.

                      I have been using setting the roughness value to 1 mm. My fairing is orientated so that positive z is downward toward the seafloor, x is along the length of the hull (the direction of the flow), and y is the width of the hull. I set an initial condition of -10 m/s in the x direction. To look at the boundary layer, I am creating a cut plot the the Z-Y plane and hoping to see no flow at the hull-water interface. The check box for Display Boundary Layer disappears as I move in the x direction and reach the fairing. But I don't see a boundary layer before or after anyways. I think it might be because my computational domain boundary in the Z coordinate is Z=0 which is in fact that fluid-solid boundary.

                      Bob
                        • Turbulence and boundary layers
                          Bill McEachern
                          Hi Bob,

                          Is the air entrained or due to cavitation? If it is entrained floworks is probably not going to be much help. If due to caviation then you can use floworks to figure out where to put the sensor. Obviously you can probably solve all your problems by moving the sensor off the hull and into a protruding fairing so it is out of the B'layer altoghther but I suspect that just isn't practical.

                          I suggest you try to do and follow the flow over a cylinder problem in the tutorial manual (external flow) and at least get a look at a B'layer and how to properly execute an analysis. Then go back to the problem at hand. If you run a transient analysis for the cylinder problem and pick a sensible R'number you can see eddies shedding off the cylinder. I have compared these to hand clac's using Strohal number and they are right on as far as frequency goes. The analysis in the tutorial is 2D but the rest of the set up is the same as for a full 3D analysis.
                          • Turbulence and boundary layers
                            Bill McEachern
                            Hi Bob,

                            Attached is a picture from a Floworks analysis I did quite a while ago which has a NACA0012-64 airfoil at alpha of 2 deg (I think). It shows the wake and if you zoom in you can see the B'layer. The B'layer view is the view of the model (modified wall functions approach) and not of what you might see in a DNS simulation - there is no detail.

                            I would post a close up of the B'layer but it so time consuming to do that in this facility I can't justify it. Thought this might be interesting for you though.

                            The analsysis was 2D and it pretty much nailed the L/D ratio - put in as a goal.
                              • Turbulence and boundary layers
                                Bob Fratantonio
                                Bill,
                                I want to thank you for all of your help. I attached a picture of one of my simulations. I am wondering why there are velocity vectors coming out of the computational domain. How does Floworks treat these boundaries? Isn't there a no flow condition there?

                                Thanks,
                                Bob
                                  • Turbulence and boundary layers
                                    Bill McEachern
                                    Hi Bob,

                                    Good question - I had an idea of what it was but I asked the key guy at SWX to be sure and he wote me this:

                                    "They are actually called far-field boundaries but the developers have told me in the past they are treated like the environmental pressure boundary condition where the boundary pressure is treated as a total pressure if it is entering the domain and a static pressure if it is leaving the domain."

                                    Hope that helps.

                                      • Turbulence and boundary layers
                                        Bob Fratantonio
                                        Once again Bill, thank you for your contributions. I have another question. I am trying to get an idea of the drag forces on my rail structure. I was going to calculate this by integrating pressure and shear stresses along the boundary and projecting it onto the flow direction. Can I get Floworks to do this calculation for me or can Floworks output pressure and shear stress on the boundary for external post-processing?

                                        Thanks much,
                                        Bob Fratantonio
                                          • Turbulence and boundary layers
                                            Bill McEachern
                                            Hi Bob,

                                            You can add a goal to the study and track the quantity of interest as the inerations proceed or after hte solution is done you can use surface parameters to sum up the surfaces of interest. -Just pick the surfaces you want and then hit RMB on the surface parameters command in the tree. Should be pretty obvious. Also in the view settngs command you can view the parameter list and add parameters ifthey are not in the drop drop down on the view settings - there are lots of parameters that might not be turned on. Theya re all calculated but it allows you to keep the pull down to a managable length.
                                              • Turbulence and boundary layers
                                                Bob Fratantonio
                                                Bill,
                                                Is it possible to introduce an initial velocity profile to match that of an estimated turbulent boundary layer? I ask this because my fairing actually sits about 30 meters down the hull, whereas my computational domain is much smaller. Or am I better off extending my computational domain (with a broad mesh) to account for this?

                                                Thanks,
                                                Bob
                                                  • Turbulence and boundary layers
                                                    Bill McEachern
                                                    Hi Bob,

                                                    You can specify velocity profuiles for inlet conditions though I have never tried it for somehtig so compact as getting a B'layer profile upstream. You could give it a whirl but I think I would just extend the domain up stream to some point forward of the front of the hull and use a 1/2 symmetry model if you are not already.

                                                    Keep in mind that the floworks turbulence model start to heads south approaching R'number values of 6 million. See the tehcnical reference for how that goes - information is providedin the validation expamples - flow over a clyinder in particular.