Fluids

Fluids

Why EWF is not working properly?? Not getting residuals for EWF!

    • Anadi_Mondal
      Subscriber

      Hello ,

      Greetings! I am using EWF and DPM to model annular flow.

      For EWF , I got these information ANSYS user guide:

      1.The material properties for the secondary phase should be the same as the DPM particles.

      2.The name of the secondary phase material should be included in the name of the DPM particle’s material and should be appended with the string ‘-particle’ (for example, if the secondary phase material name is waterliquid- eulerian, then the DPM particle’s material name should be waterliquid-eulerian-particle).

      3.The wall film cannot be solved without first initializing the wall film model (using the Initialize button) to initialize the wall film variables and prepare the solver for the solution procedure.

      I am using vapor as primary phase and water as my secondary phase and droplets .

      Here is the short description of model:

      "The simulation includes a two-dimensional Eulerian liquid film model coupled to a three-dimensional core model (including vapor flow and droplets) based on the Eulerian – Lagrangian approach"

      Please see the attached image and would you give me any idea why I am not getting any residuals for liquid phase? Why the model is not showing data for wall film?(I know know it's not converging but that is not my concern now ,I can change other setting but I want to see the residuals for water)

      Thank You,

      Anadi

    • Surya Deb
      Ansys Employee
      Hello, Not really sure what is the issue here. I see all the proper residuals being displayed. I also see the volume fraction and velocity residuals of water.nThat is all the residuals that you need. You will be able to visualize EWF variables in Contours separately as well.nRegards,nSDn
    • Anadi_Mondal
      Subscriber
      Thank you sdeb!nHere you are seeing 6 residual curve (3 for vapor, one for continuity, one for k and final one for omega). I check the values for water in console ad it is zero. I have attached two images . I have tried to draw film thickness but not getting any single graph. Will you check the parameters ? I draw the pipe on XY plane and extrude in z direction. I have attached tube with zone for your convenience. I apply liquid mass flux at injection wall by EWF option. Mainly I need to draw wall film thickness of water and mass flow rate of water in annular section.nRegards,nAnadinn
    • DrAmine
      Ansys Employee
      Please plot first along a line and not the wall surface.nMoreover I am aware that some problems in the past related to EWF have been fixed during the last versions. Please update to the most recent version.nnWhat do you want to do?n
    • Anadi_Mondal
      Subscriber
      Hi DrAmine,nWhere should I plot a line? It'a 3D pipe. Actually I am trying to simulate annular flow in a tube. I divided the pipe in 3 section . 'Injection wall' to apply liquid mass flux, 'stabilization wall' to form the film and finally the film in 'annular' region. Mainly I need to draw wall film thickness of water and mass flow rate of water in annular section.nMore info about model,The simulation includes a two-dimensional Eulerian liquid film model coupled to a three-dimensional core model (including vapor flow and droplets) based on the Eulerian – Lagrangian approachnThe liquid film should be simulated as a two-dimensional Eulerian model while the vapor-droplets model should be simulated as a three-dimensional Eulerian – Lagrangian model, both models are simultaneously coupled.nnThank YounAnadi
    • DrAmine
      Ansys Employee
      I understand but why are you solving Eulerian Multiphase here if your core is (DPM) particle laden gas flow?.Doing XY Plot on surface is not pretty as you saw. Rather first check the contour plots of film thickness.n
    • Anadi_Mondal
      Subscriber
      Hello DrAmine,nDo you think I am doing mistake here? Without doing so, how can I get phases?nAnadinn
    • DrAmine
      Ansys Employee
      You have discrete droplets so you do require DPM model and not Eulerian model. Model the droplets with DPM.n
    • Anadi_Mondal
      Subscriber
      Hello DrAmine,nI am modeling the droplets with DPM. But if turn off multiphase then there is not option to select vapor or liquid at inlet. Actually I am flowing only vapor at the inlet . Please see the attached image. How to select 'vapor velocity' at inlet after turning off multiphase? or should I select water-vapor in cell zone conditions for both zones to confirm only water-vapor in tube initially? So water-vapor in the tube and we will apply water-liquid mass flux through EWF at the wall to form film in the tube. Am I correct?nn
    • YasserSelima
      Subscriber
      I see you have been in this issue for a while.nI suggest you increase the water void fraction at the inlet to a very small value .. let's say 1e-04 ... And then you can monitor the mass of liquid and see if condensation happens or not.n
    • DrAmine
      Ansys Employee
      Array that is wrong: he wants to use DPM Model.nArray: DPM is relying on Lagrangian Framework. You can add whatever you want as droplet as Injection. In the Injection you prescribe from where the particles should be injected, the flow rate, their initial velocity, diameter, etc...nnKeep default DPM Boundary at Inlet and Outlets.nAt the wall please change the DPM Boundary to Trap and enable EWF on that particular wall. For EWF Model activate DPM Coupling.
    • Rob
      Ansys Employee
      Is the aim to have the droplets form the film? Note, the Eulerian multiphase model and Eulerian Wall Film are not linked and are not the same model. n
    • Anadi_Mondal
      Subscriber
      ,Mainly the film will form on the tube surface due to applying water mass flux at a surface near inlet(injection_wall) by EWF model. But if liquid droplets from the core region(core region is consist of vapor and liquid droplets) touches the liquid film ,droplet will be trapped in the liquid film and added with the mass of liquid(liquid mass source)nThe overall scenario is:n1.In the core region of tube vapor and droplets will flow(core region is consist of vapor and liquid droplets)n2.Liquid film will form at the surface of tuben3.Liquid from the film can enter into the core as a droplets due to entrainment and if droplets touches the liquid film , it will be trapped ,and added with liquid mass (deposition)nI followed everything you mentioned in your last reply. nWould you tell me, Should I use Eulerian Multiphase model or not? If no, then I will turn off this model and run calculation again.nAccording to your reply, I am understanding this way,n1.Use DPM to simulate tube core. Here I can use injection to create droplets.n2.Use EWF to form liquid film on tube surface and coupled these two modelnAm I on right track?nI have added an image that I am trying to simulate.nThank you nAnadin
    • Anadi_Mondal
      Subscriber
      Hello All,nI try to run the simulation without Eulerian Multiphase but got this error:nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionnnError at Node 0: Floating point exceptionnError at Node 1: Floating point exceptionnError at Node 2: Floating point exceptionnError at Node 3: Floating point exceptionnError at Node 4: Floating point exceptionnError at Node 5: Floating point exceptionnError at Node 6: Floating point exceptionnError at Node 7: Floating point exceptionnnI have added the skewness report and I am using URF of DPM 0.1nWhat may be the problem?.Thank YounAnadin
    • DrAmine
      Ansys Employee
      listen to he summarized everything in 3 lines. It is only a matter of the film thickness. If it very thick or gets wavy then Thin film model is not deployable anymore.n
    • Anadi_Mondal
      Subscriber
      Array , I am experiencing the following error now. Do you have any idea to solve this?nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionn
    • DrAmine
      Ansys Employee
      Quite hard: Summarize now what you are using.nThe first thing if everything is well setup is to start with small time step size (assuming the mesh is of high quality).n
    • Anadi_Mondal
      Subscriber
      Here is the cross section of pipe I am using. It's structured hexahedral mesh. Actually I was using bigger time step to check if everything is working perfectly or not. Okay, I will use small step size. Any other suggestions?nnn
    • Rob
      Ansys Employee
      I'd look at a pave mesh, the O-grid or butterfly mesh method isn't used much now we've developed solvers that don't need block structured meshes. Ie it's not been needed for about 20 years! That also resolves the high aspect ratio near the walls that may not help the film. Ironically, you've resolved the flow in the middle where we don't care too much, and not near the wall where we do! n
    • Anadi_Mondal
      Subscriber
      Hello Array nI was getting this error,nDivergence detected in AMG solver: pressure couplednError at host: floating point exceptionnSo I am trying to find where is the error? This time I did not use UDF and DPM. I just use EWF and water-vapor in the core for test purpose. I check the contour and a think film is noticeable. But when I am trying to plot the film thickness, I am getting the following graph. Did I do any mistake to take the surfaces(X-axis)? How can I get a single graph of film thickness on the wall? or what is the way to plot film thickness? I plot the tube in XY plane and extrude in Z direction. If you need to know the mesh ,please see the 2nd top image of this post. If I can plot the film thickness, then I will turn on the DPM next.nThank You,nAnadin
    • Rob
      Ansys Employee
      You tend to plot thickness on the wall, and use local range. For an xy plot you need a line, the easiest way is to create a plane (or iso-surface of mesh) and select the wall when you do that. The result is the intersect of the two surfaces which tends to be a line. nDivergence will be because the time step is large relative to the amount of vapour moving to the film. Time scales tend to be VERY small, so just keep dropping the timestep by an order of magnitude until it works. Also look at sub-stepping in the film set up. It's an area we're actively working on, and I'm waiting on the build so I can start testing the new options. n
    • DrAmine
      Ansys Employee
      Plot on surfaces looks like that in 3D. Create a line. And: update to the most possible versions. n
    • Anadi_Mondal
      Subscriber
      and nI create a line at the wall of the tube and getting film thickness as below. I see at some location film thickness is zero. Do you think the high velocity of vapor (12m/s)in the core is responsible for that? Actually I am expecting a stable (almost parallel line) film thickness on the wall as I did not apply any heat flux to evaporate the film yet and allowed enough time to form stable film .nMoreover, I am using water-liquid as film materials and flowing water-vapor in the core from inlet.nI am using university vLabs .I see 19.2 is the most updated version there.nThank you,nAnadinn
Viewing 23 reply threads
  • You must be logged in to reply to this topic.