Fluids

Fluids

Porous media for VOF

    • mozeer
      Subscriber

      Hi all,


       


      I am doing an analysis for a storm water trap which has a basket for trapping pollutants. I need to simulate the basket as a porous media. But I am always having errors or the continuity is diverging. 


      I wanted to know if we can simulate porous media on VOF, or what model is best? I am currently using VOF and K-epsilon for the model. 


       


      Thanks

    • Keyur Kanade
      Ansys Employee

      Please make sure that you have refined the mesh. Please reduce your time step size and check. 


      Regards,


      Keyur

    • mozeer
      Subscriber

      Thanks for your reply, 


      Yes the mesh is good and i tried reduce the time step as well. 


      I wanted to be sure if porous media can be used for VOF model?



       

    • DrAmine
      Ansys Employee

      Yes porous media can be used with the VOF model

    • Karthik R
      Administrator

      Hello,


      If you are still having convergence, please elaborate more on your set-up. You might want to add more about the geometry, show the mesh and boundary conditions, and describe your initialization. I'd also recommend that you provide some more information on the porous media treatment in your model. This way, we will be in better shape to help you.


      Thank you.


      Best Regards,


      Karthik

    • mozeer
      Subscriber

      this is my geometry, its a storm water trap with an internal and external  chamber. the bottom part of the internal chamber has a basket (the brown and green part, the brown part is solid since i want to simulate the basket as half full. the green part is my porous media volume)


      thats my meshing.


       


      in fluent I am putting the following parameters:


      Type: Pressure-based


      Velocity Formulation: Absolute


      Time: Transient


       gravity -9.81


      VOF multiphase model


      N of Eulerian Phase: 2


      Formulation: Explicit


      Interface Modelling: Sharp


       


      k-epsilon realizable turbulence model


       


      Phase 1: air


      Phase 2: water


      Surface tension: 0.072 constant


       


      cell zone conditions



      i have got the values for porous media from experimental work, plotting pressure against velocity as per Workbench guide. 


      Boundary Conditions:


       


      Water Inlet (velocity-inlet type)


      V: 0.45 m/s


      Initial Pressure: 0


      TKE: 1


      Epsilon: 1


      Phase 2 fraction: 1


       


      Outlet (pressure outlet)


       


      top (pressure outlet)


       


       


       


      Solution Methods:


      Pressure-Velocity Coupled (i have tried PISO as well)


      Pressure: PRESTO!


      Momentum: Second Order Upwind


      Volume Fraction: Compressive


      TKE: First Order Upwind


      Turbulent Dissipation Rate: First Order Upwind


      Transient Formulation: First Order Implicit


       


      Solution Control:


      Flow Courant: 200


      Eexplicit RF


      Momentum: 0.3 (i have tried the default as well)


      Pressure: 0.3


      Under RF


      Density: 1


      Body Forces: 0.5


      TKE: 0.6


      TDR: 0.6


      Turbulent Viscosity: 0.5


      Discrete Phase: 0.9


       


      std Initialization from inlet


      Time step size: 0.001(I have tried 0.01 as well)


      N of time step: 1000000


       


      would be great if you could help.


      Thanks


      Ikhlass

    • Keyur Kanade
      Ansys Employee

      What is mesh quality? Please use Quality option in Fluent to check quality. Also check the mesh in Fluent before proceedings. 


      Did you patch the vof after initialization? Please do it before you start iterations. 


      Please use PISO.


      Please increase urfs. 


      For time step, you can calculate ((Vcell_min)1/3)/vel


      Please set time step less than this value. 


      You can always get min cell volume when you check the mesh in Fluent. 


      If divergence occurs, please decrease time step by factor of 10. 


      Regards,


      Keyur


       

    • mozeer
      Subscriber

      Thanks for your reply.


      Yes i did patch it half full. i have checked the quality and do repair as well on fluent. 



      the minimum volume is very low..


      Whats urfs?


      In fact i am using implicit formulation for  VOF.


      Are the other parameters good? 


      Kind Regards

    • mozeer
      Subscriber


      I dont understand how i can improve the orthogonal quality, can you help please?


       


      Thanks

    • Keyur Kanade
      Ansys Employee

      The quality is really bad. You can improve it using Fluent Meshing as follows. 


      Please open Fluent in Meshing Mode. 


      Go to Mesh --> Tools --> Auto Node Move


      Set Quality Measure as Inverse Ortho


      Select all boundary zones. 


      Use 5 iterations


      Click apply. 


      Save .msh file and read in Fluent. 


      As you are using Workbench meshing, you need to find out where these low quality elements are. Please select orthogonal quality and plot histogram. Then you can click in histogram to see bad elements in the graphics. Then you may need to modify the geometry in SpaceClaim or use virtual topology in Meshing or may be use local sizing to refine the mesh further. Once done, generate mesh and check the quality before proceed. 


      Check following video which may help. 



       


      Hope this helps. 


      Regards,


      Keyur

    • Rob
      Ansys Employee

      I suspect the poor cells are where the pipes go through the casing. You may also be better off using a thin wall and using a porous jump rather than porous media. Hard to tell from the images, and we're limited in how much detailed help we can give in an open forum. 


      Is the brown volume to assist in the initialisation, or when you say the basket is full do you mean the unit has part filled with debris? 


       

    • mozeer
      Subscriber

      I cant find out where is the auto node move. is that in the previous version? 


       


       

    • mozeer
      Subscriber

      Hi Thanks for your reply. I will look into the porous jump ans see if i can use that. 


       


      Is there any way of me getting more detailed help, I am kind of stuck with these divergence. 


       


      the brown volume is solid in the geometry itself, not fluid, and this is representing the debris. 


      I have used another model as well using the whole basket volume as the porous media, and not the thin wall. I am still getting divergence. 

    • Karthik R
      Administrator

      Hello,


      Auto node move is part of Fluent Meshing. You will find this option when you right click on the 'Mesh objects' to find the Auto Node Move feature in Fluent meshing.



      If you are looking for more video to learn Fluent meshing, we can show you some online resources. If you are more familiar with WorkBench meshing, please use this tool to improve your mesh quality. Please follow the video shared by Keyur to obtain necessary mesh statistics during meshing.


      However, Keyur's point was that you will certainly have to improve your mesh to avoid divergence of your solution. It is always important to remember that a few bad cells can prevent your solution from converging. You might also want to include some line / surface / point monitors to understand your divergence better. 


      If you have not already watched these, I'd highly recommend going through them first. They will help you understand how you can improve the orthogonal quality of your mesh. This is a 4-part video series on Hex meshing.



      I hope this helps.


      Best Regards,


      Karthik

    • mozeer
      Subscriber

      Thanks for that, I am improving my mesh quality now, I hope that it will not converge anymore.

    • mozeer
      Subscriber


      I have changed the mesh and now it is now running at all. Is that still because of the meshing?


       

    • Keyur Kanade
      Ansys Employee

      Hello,


      What is new quality of mesh?


      Once you improved mesh, did you define all bcs and settings again? Did you patch again?


      Regards,


      Keyur

    • mozeer
      Subscriber

      yes I have started everything all over again. I hope the mesh is good tho. 


      Thanks


      ikhlass

    • Rob
      Ansys Employee

      Use Skewness, Aspect Ratio and Orthogonal skew(?) to check. Element Quality is for the Mech solver and is meaningless for Fluent. 

    • Keyur Kanade
      Ansys Employee

      Please check orthogonal quality. 


      Regards,


      Keyur

    • mozeer
      Subscriber


      Do you think this is good enough?


       

    • Keyur Kanade
      Ansys Employee

      Yes, quality looks ok now. 


      Once get into Fluent, please 'Check' the mesh and 'Quality'. 


      Please cross check if all settings are correct as discussed in previous posts. Initialize, patch. 


      Please run the case with the options already discussed and let us know the oputput. 


      Regards,


      Keyur

    • mozeer
      Subscriber

      alright i will run it now. Is time step size of 0.01 good? 


      also, for the patching, I am marking the cells then patch to start the simulation at half filled with water, is that what you meant? 


      Thanks


      Ikhlass

    • Keyur Kanade
      Ansys Employee

      For time step, you can calculate ((Vcell_min)1/3)/vel


      Please set time step less than this value. 


      You can always get min cell volume when you check the mesh in Fluent. 


      And yes, the you are using correction option for patching. 


      Once patched, please cross check volume fraction contours and then only proceed with iterations. 


      Regards,


      Keyur

    • mozeer
      Subscriber


      so if velocity is 0.786m/s


       ((Vcell_min)1/3)/vel = 0.006


      so time step of 0.005 should be fine isnt it?  just want to be sure because the iterations will take a long time. 


      yes checking contours as well. 


      Thanks so much


      ikhlass

    • Keyur Kanade
      Ansys Employee

      Yes, 0.005 is ok. 


      I would say go with 0.002 for first few time steps and then increase it to 0.005.


      Regards,


      Keyur

    • mozeer
      Subscriber

      Alright thank you!


       


      Regards


      Ikhlass

    • Keyur Kanade
      Ansys Employee

      Welcome!


      Let us know how it goes. 


      Regards,


      Keyur

    • mozeer
      Subscriber

      Yes so Its finally converging, but there is something wrong somewhere since the results are really bad. Its actually not simulating what it should. 


      Regards,


      Ikhlass

    • Karthik R
      Administrator

      Hello,


      Could you explain a little bit more so we understand what's wrong with your results? Please provide the necessary plots.


      Thank you.


      Best Regards,


      Karthik

    • mozeer
      Subscriber


      so basically the water level in the internal chamber should be less and in the external chamber it should be more. And the inlet and outlet flowrate as well really bad. 


      it should ideally be similar to the below one: 


    • Rob
      Ansys Employee

      OK. Flow is pushed into the inner chamber from the inlet. It passes through the porous media and then (ideally) flows to the outlet.  If the device is flooding then then the flow rate may be too high for the system. 

    • mozeer
      Subscriber

      yes, but I am using the same flow rate with which I did the testing in the lab. And all dimensions of geometry are same to the real model.

    • Rob
      Ansys Employee

      Have you got plots of the inflow & outflow mass with time? I ask as it's quite possible flow will not be constant on the outlet so the balance may be better.  For the lab model was the chamber half full of solid block and have you checked the porous resistance?

    • Keyur Kanade
      Ansys Employee

      Hi,


      How many time steps you ran? Did it converge in every time step? If not, please increase no. of iterations per time step to 30 or 40. 


      Can you please give more details about results. Insert more images of contours.


      Regards,


      Keyur


       

Viewing 34 reply threads
  • You must be logged in to reply to this topic.