Fluids

Fluids

Wave generation in deep water (wave is getting damped)

    • surajgarad
      Subscriber

      I need to do wave generation for deep water condition in 2d or 3d. I think 2D is sufficient.

       I have tried with fines mesh like 100 cells per wavelength and 20 cells per waveheight.

       The basic requirements are, deep water conditions, wave shouldn’t get damped, first order airy theory and K-w SST model for turbulence.

       For wave generation I have used open channel wave BC, Implicit body force and Sharp from interface modelling. Interfacial Anti-diffusion is also ticked.

       In order to avoid reflection from opposite wall, numerical beach is provided over two wavelengths from opposite wall.

       For Pressure- Velocity coupling SIMPLE scheme is used, Pressure – PRESTO, momentum - second order upwind, Volume fraction – Modified HRIC, Turbulent K.E- second order upwind, Sp. Dissipation rate – second order upwind, transient formulation – second order implicit.

       For very low values of k and w (1e-06), the wave is not getting damped and I am getting expected results but when I am initializing simulation with calculated values of k and w, it gets damped.

       For reference, I have followed

      1)     Numerical simulation of an oscillating water column device using a code based on Navier - Stokes equations.

      2)     CFD modelling of a small–scale fixed multi–chamber OWC device

       3)     Fluent user manual

      4)     Fluent user guide

      5)     Scaling and air compressibility effects on a three-dimensional offshore stationary OWC wave energy converter

      6)     Tutorial: Heave and Pitch Simulation of Ship hull moving through head sea waves.

       

    • Rob
      Ansys Employee
      When you say initialised with values for k & w how long are you running the model to determine if the waves are being dissipated?
    • surajgarad
      Subscriber
      Thanks for the reply I am running simulations for nearly 20 wave cycles or crests. From the first wavelength itself, it starts damping.
    • Rob
      Ansys Employee
      How deep is the domain, and how much space is there above the water level? Is the model converging, and how are you defining k & w on the boundaries?
    • surajgarad
      Subscriber
      I have taken a domain length of 20 m ( to have a sufficient number of peaks in a domain )and a water depth of 2 m considering deep water conditions. I have given waveheight of 0.15 m with the time period of 1.0769 sec, the mean level is at zero. First I have defined very less values (1e-06) for k and w, in that case, I got an undamped wave with a converged solution but when I am using calculated values (used an online calculator) for k and w values, the solution is getting converged but wave got damped.
    • Rob
      Ansys Employee
      Where are you using the calculated values of k & w?
    • surajgarad
      Subscriber
      At the inlet (left side) where I am using open channel BC for generating a wave
      for the right side where pressure outlet is defined and top side with pressure outlet boundary condition.
    • surajgarad
      Subscriber
      I am using calculated k and w values at inlet, top and outlet.
    • Rob
      Ansys Employee
      What values are you using? If you plot the k & w values in the earlier model and compare with this case how does it look?
    • surajgarad
      Subscriber
      For undamped wave case, the values of k and w were very less i.e. 1e-06
      For damped case, k = 0.0106 and w = 0.05 (it is calculated from cfd online calculator https://www.cfd-online.com/Tools/turbulence.php )
      I have attached plots of k for reference.
    • Rob
      Ansys Employee
      Staff are not permitted to open or download attachments, please add in line with the text.
    • surajgarad
      Subscriber
      For undamped wave case, the values of k and w were very less i.e. 1e-06
      For damped case, k = 0.0106 and w = 0.05 (it is calculated from cfd online calculatorhttps://www.cfd-online.com/Tools/turbulence.php)
      I have attached plots of k for reference.

    • surajgarad
      Subscriber

    • Rob
      Ansys Employee
      Where's the free surface?
    • surajgarad
      Subscriber
      At 0 in y direction
    • Rob
      Ansys Employee
      Pictures? At the moment you have a domain that's 20cm high and 20m long with no waves and a turbulence field that's very quickly damped out. Please add enough data so we can actually see what's going on.
    • surajgarad
      Subscriber
      Yes, domain height is 20 cm while length of 20m. I have attached respective free surface elevations of the above mentioned k and w values. w.r.t. to these values of k and w, plots for turbulent kinetic energy are given earlier in this thread.

    • Rob
      Ansys Employee
      You may have over constrained the model, make the domain significantly higher in the y dimension so the boundary values don't unduly influence the flow and see what that does.
    • surajgarad
      Subscriber
      Ok, I will try with a higher domain in the y-direction. But is I need to increase cell count or can I keep the same?
    • surajgarad
      Subscriber
      The results which I have shown here are zoomed in. Please check the results for all domain. First result is of damped wave i.e. from calculated values of k and w while second figure is of undamped wave (expected result) for which very less value of k and w is used i.e. 1e-06.

    • Rob
      Ansys Employee
      Can you plot the phases so we can see the waves, the velocity field and also phases with node values off.
    • surajgarad
      Subscriber
      First 5 figures are for damped simulation case while remained figures are for undamped simulations.
    • DrAmine
      Ansys Employee
      Domain extents epscially above the free surface is very important: Please use there at least 1.5 or two wave length to put the top boundary.
    • DrAmine
      Ansys Employee
      Also use good initial values based on the Phase: this is possible with 21R1 and later.
    • DrAmine
      Ansys Employee
      Probably turbulence damping is required at the interface too.
    • surajgarad
      Subscriber
      Here we have license for Ansys 20, can you explain how to provide turbulence damping at interface. I will check with 1.5 m distance between top and free surface.

    • Rob
      Ansys Employee
      I assume you mean 2020Rx? It's an option in the Turbulence (Viscous) panel.
    • surajgarad
      Subscriber
      Ohh. Is it fine to go with default value for turbulence damping, under relaxation factor and k w values?
    • DrAmine
      Ansys Employee
      Yes: that is fine. If you do not measurements or power to do a sensitivity analysis stick to defaults.
      However as mentioned I recommend that you test with phase sensible turbulence field initialization first + extending the top boundary away from free-surface
    • surajgarad
      Subscriber
      I have checked simulation with extended top boundary and with default values of turbulence damping, URF and k -w values. Still wave get damped.
    • DrAmine
      Ansys Employee
      Turbulence Field initialization used?
    • surajgarad
      Subscriber
      Yeah, I have one small doubt, normally I am giving k-w values at the inlet boundary, pressure outlet, and at the top side. Is it ok to define k w values at three boundaries or have to provide only at the inlet boundary conditions?
    • Rob
      Ansys Employee
      You define k & w for any and all flow boundaries.
    • surajgarad
      Subscriber
      I have defined k and w at all boundary conditions. Distance between top boundary and free surface is also increased. Still wave get damped. From the console the recommended theories are nonlinear or stokes theories but I need to use linear/airy theory. Is that arising issue? or is there any problem with solution methods?
    • DrAmine
      Ansys Employee
      At wall boundaries? How have you done that?
      I recommend using Stokes Theory and check the results you are obtained.
    • surajgarad
      Subscriber
      I have checked with both linear and stokes theories, the wave height got damped. How the values of k and w affect the simulations, means to what level? I think k and w values only making trouble.
    • surajgarad
      Subscriber
      Hi I am still struggling to get results. Can you confirm is I am using correct boundary conditions and methods?
    • DrAmine
      Ansys Employee
      You wrote you are assigning values for k and omega at walls? How did you do that ( I am asking as this will require rewriting the wall functions).
      Again: Are you using localized turbulence initialization? Are you tracking the max velocity in the domain? Which are now the domain extents? Which is now your time resolution? Are you using numerical beach: if yes disable it if no is there a difference if you enable it
      Which version are you using?
      Which are the scenarios where the waves are not dampened?
      Goal is that you summarize the issue in single post.

    • surajgarad
      Subscriber
      1) Yeah, I have tried with default value and with calculated values at velocity inlet and pressure outlet, not at a wall boundary.
      2) Localized turbulence initialization means I am defining only on surfaces (as now performing 2D simulations so line) Domain extents are taken to have atleast 7-8 peaks (-10 to 10m). Here I have considered adaptive time stepping 1e-05 to 1e-03. Yes I have tried both with numerical beach and without beach also. In both cases it gets damped. From starting itself, means at a distance of one wavelength, wave starts getting damped so couldn't say much about effect of numerical beach.
      3) Fluent 18.1 and Fluent 2020
      4) K- w values of 0.02 and 2, Stoke 5 theory,
      I have tried with fines mesh like 100 cells per wavelength and 20 cells per waveheight.
      For wave generation I have used open channel wave BC, Implicit body force and Sharp from interface modelling. Interfacial Anti-diffusion is also ticked.
      In order to avoid reflection from opposite wall, numerical beach is provided over two wavelengths from opposite side.
      For Pressure- Velocity coupling SIMPLE scheme is used, Pressure ÔÇô PRESTO, momentum - second order upwind, Volume fraction ÔÇô Modified HRIC, Turbulent K.E- second order upwind, Sp. Dissipation rate ÔÇô second order upwind, transient formulation ÔÇô second order implicit.
      5) Basic requirements are: deep water conditions, first order airy theory, k w sst model
    • DrAmine
      Ansys Employee
      Can you use Compressive Scheme instead of HRIC.
      Can you try with 21R1 or 21R2?
      With localized Turbulence is something different I meant: To start with turbulence fields relative to phase volume fraction field. This is directly possible with 21R1

      If you are still seeing damping issues without beaching with Compressive Scheme on your 2D runs: please report and provide an academic contact address.
    • surajgarad
      Subscriber
      Ok, I will try with compressive scheme and let you know the results.
      We have license for Ansys 2020 version.
    • wangkai1
      Subscriber
      Hi´╝îHave you solved the problem? I also met the same problem. How did you solve it´╝îplease´╝ƒthank you´╝ü
    • Nazmul Islam Nishat
      Subscriber

      How to generate wave properly for owc ....?i need full tutorials.if any one give me suggestion or give me video how to do it. thnx

Viewing 42 reply threads
  • You must be logged in to reply to this topic.