Fluids

Fluids

Pseudo-Transient in Flow Boiling Case

    • farizanluthfi
      Subscriber

      Dear ANSYS expert,


      I have one simulation in boiling case using pseudo-transient approach with RPI wall boiling in the helically-coiled tube. The simulation is currently still on progress and seems like fluctuating until 200k iterations. Not only that, when I try to check the outlet temperature to calculate the vapor quality, the temperature is also fluctuating.


      My questions is do you think I should stop the running and try to do some another options or do you have any better approach to solve my problems in boiling case using pseudo-transient?


      Thank you in advance,


      Luthfi

    • DrAmine
      Ansys Employee
      If not depicting a steady state behaviour you should run unsteady.
      Generally boiling cases are run steady because they are expensive. Sometimes the trick is to use larger time scale to smooth out transient effect. Stop using automatic time scale and use a bit larger one. That helped me in my last 5 years boiling projects
    • farizanluthfi
      Subscriber

      Thank you for your quick response regarding this matter.


      Our simulation should be in pseudo-transient is because of the steady-state give me the diverged solution. However, this problem exists only when I am trying to increase the mesh to conduct a mesh independent study for this case. Before that, when I'm using the lower mesh, the solution is fine and give me a good result.


      So I just wondering, do I need to run the simulation using pseudo-transient based on your recommendation in any mesh that we would like to put for the validation purpose or only in the simulation that gives me the diverged solution? Because I'm afraid the result will be different between the steady-state approach and the pseudo-transient approach.


      Thank you,


      Best Regards,


      Luthfi

    • DrAmine
      Ansys Employee

      pseudo-transient is a steady state solution method using implicit time marching under-relaxation.


       

    • farizanluthfi
      Subscriber

      I have tried to change the time-step method from automatic into user specified and also change the length scale from conservative to aggressive but both of them give me the diverged solution. In my case, I use automatic time step with timescale factor 0.1 and it can be run but the problem is the residuals keeps fluctuating even though I have run the simulation for almost 2 weeks in 175k iterations.


      Do you have a better recommendation according to my problem? I would be happy to hear that and try to implement it directly to see whether it's suitable or not 


      Thank you,


      Best Regards,


      Luthfi 

    • DrAmine
      Ansys Employee

      Can you show residual and monitor plot? As I said you can switch to transient solver if the fluctuations are quire high.

    • farizanluthfi
      Subscriber


      Above capture is the monitor and residual plot that you requested. As you can see in here, the residuals is sky rocketing when I turn the time step method into user specified of 1s pseudo time step from automatic time scale 0.1 


      But if I keep the automatic time scale 0.1, it always fluctuating which demonstrates it in the figure above.


      Thank you,


      Best regards,


      Luthfi

    • DrAmine
      Ansys Employee

      1 second is very large. That was not what I was suggesting. It looks like your rum is showing cylcing behavior can you try transient solver?

    • farizanluthfi
      Subscriber

      So I need to calculate the simulation from the beginning (first iteration) or just continue from last calculation then changed the approach into transient solver? Because of the lower mesh for this particular case, I use steady-state solver and it works well, but when I increase the mesh into doubled, it turns away into swinging like the picture that I provided in the last comments. Do you know why it could possibly happen in boiling case?


      Thank you for your kind responses.


      Best regards,


      Luthfi

    • farizanluthfi
      Subscriber

      For this case, I'm using RPI wall boiling model with Coupled Scheme. The spatial discretization is First Order Upwind for all schemes. For the pseudo transient explicit relaxation factors is described as follow:


      - pressure: 1


      - momentum: 1


      - density: 1


      - body forces: 0.5


      - volume fraction: 0.3


      - vaporization mass: 0.5


      - all turbulent forms: 0.3, 0.3, 0.5 respectively


      - energy: 0.6


      Thank you in advance,


      Best regards,


      Luthfi

    • farizanluthfi
      Subscriber

      k-epsilon Standard turbulence model with Standard wall function is used in this study to capture the boiling phenomena at the heated surface. Please check the following model and the last comments model that I used in this study. 


      Highly appreciated for your support and response.


      Thank you,


      Best regards,


      Luthfi

    • DrAmine
      Ansys Employee
      As I have couple of times said RPI does not like having fine near wall mesh. Make the mesh better finer off the wall and not at walls. I will always go for SST model for every engineering run.

      Finer mesh would resolve more effects which might not be captured by the deployed techniques.

      In case of unsteady I would start from results of steady run if well converged otherwise from scratch.
    • farizanluthfi
      Subscriber

      For unsteady case, I have ever read from the theory guide that it's better to use PC SIMPLE algorithm to solve the problem, so in your previous experience is it still relevant as well or how?


      Yeah for RPI model, the mesh option at the wall is not fine enough, the y+ is around 12-15. or is it still count as fine for the respective options?


      Okay, I will try your recommendation using SST model for the turbulence options.


      How about the solution control that I use for the simulation? Because if I use the default values, it will go diverged for the steady case.


      Thank you for your kindly support and response.


      Best regards,


      Luthfi

    • DrAmine
      Ansys Employee

      Yplus should be larger than 30-40.


      All segregated methods are almost equivalent with more merits for PISO when it comes to long time performance.


       


      I do not recommend changing default URFS for transient runs. Rather decreasing time step size at the beginning.


      Good Luck.

    • farizanluthfi
      Subscriber

      Thank you for your responses and assistance regarding this matter.


      How about the significant differences between the evaporation-condensation model and RPI wall boiling model for conducting the boiling case in ANSYS Fluent? As far as I know, they both have positive and negative value but according to the details of this case that I have shared in the previous posts, which one you will choose between the two options?


      Highly appreciated for your time and answer.


      Thank you,


      Best regards,


      Luthfi

    • DrAmine
      Ansys Employee
      Bulk phase change models without adjustments do not account for subgrid boiling. Evaporation is then underpredicted.
    • farizanluthfi
      Subscriber

      What kind of adjustment that we should need to do boiling simulation using bulk phase change models? So according to your experience, RPI wall boiling still better than the evaporation-condensation model?


      Thank you,


      Best regards,


      Luthfi

    • DrAmine
      Ansys Employee
      Check how much portion of the near wall cell us superheated and apply mass source plus secondary fluxes.
Viewing 17 reply threads
  • You must be logged in to reply to this topic.