Fluids

Fluids

Regarding total time steps or flow time

    • KSD
      Subscriber

      I want to solve a transient supersonic nozzle flow problem.

      For which there are no experimental data available, because of which I don't know how much total time, should the simulation take in order to stop the simulations.

      Based on the smallest grid size and using CFL < 1 , I am able to determine the time step size to be of order 1e-8.

      But I don't know, how many time steps or flow time I should give.

      I am interpolating the steady state solution then running the transient settings by giving arbitrary number of time steps

      So from the starting of iterations itself I am not seeing any change in mass imbalance monitor curve. Only residuals is oscillating with constant amplitude and frequency, I guess.

      And also I have checked the animation of contour of Mach number, it is not showing any change in behavior, it exactly looks like steady state solution plot.

      I am not sure whether is it happening because I am checking the results too early means do I need to wait for days, weeks or months to see any change.

      I really don't have any idea about what should be my waiting period time in order to get a confidence to accept the solution for further post processing.

    • DrAmine
      Ansys Employee
      Some flow-through times are a minimum and rule of thumb it to run till a sort of pattern settles in.
      Flow through time: if you launch a couple of massless particles from inlet (pulse injection): you should expect them at the outlet after first complete flow passage. That is the reference time which you can use. Another estimate using the mean velocity and length of the nozzle.
    • KSD
      Subscriber
      Sir, I tried plotting stream line from nozzle inlet and it shows it cannot find interface for particle --Abort, is it because my one flow passage is not yet completed means I should wait for more number of time steps.
      Regarding Reference Time
      This is the steady state solution velocity magnitude curve of nozzle flow interacting with crossflow of Mach 2.
      I am assuming roughly 2000 m/s to be mean velocity of nozzle, and the length of right part of domain is around 5080e-3 m.
      Does that mean approximately ( 5080e-3 /2000) = 0.0025400 seconds the flow will take to pass the domain.
      And for given time step size of 1e-8 calculated based on CFL < 1 and smallest grid size, I should give total number of time steps as (0.0025400/1e-8) = 254000
      So, after 254000 one flow passage will occur and for accuracy of the solution we wait for 3-4 flow passage, which means I have to wait for 3*254000 = 762000 time steps in total to do further post processing.
      Is this the way, I should do it.
      Please correct me if I am doing wrong, because it seems like huge number of time steps which will take lot of days for one simulation.

    • DrAmine
      Ansys Employee
      Sounds good as rough estimate. What is the motivation to run unsteady?
    • KSD
      Subscriber
      Sir, thanks for confirming the steps.
      Sir, the reason for doing unsteady simulation is I am not getting my mass imbalance perfectly constant it keeps on fluctuating even though the mass imbalance is of order 1e-4 but still it never remain constant e.g. 0.000145 : next iter 0.000124 : next iter 0.000154 an so on. It is not remaining constant like 0.000145 : next iter 0.000145 : next iter 0.000145.
      Above is the plot of mass imbalance for steady simulation it looks like constant but actually it isn't.
      If you look at below Mach contour of steady state solution, there are recirculation regions present, because of it, I think circulation region is slightly changing in size, which might be the reason I am not getting constant mass imbalance.
      Thus for that reason only I am think I should do a transient simulation as well.
      Is this reason good enough to do unsteady simulation ?

    • KSD
      Subscriber
      And also sir my cd plot (Don't focus on the values as I have selected all walls) for steady state solution look like this even though the value is fluctuating around 30463 but it is never constant.

      Doesn't it indicates that I should run fully transient analysis.
      But still the number of time steps is around 10 lacks and considering 20/iter, it will take so much time even using HPC.
      Is this actually the way, how I should approach for transient analysis.
      As I am new to transient analysis, I think it will take months to do simulation for different parameters like changing crossflow Mach number, changing angle etc...
      Sir, can you please suggest some ways to reduce my simulation time. I am already using adaptive time steps but it is not changing the time step that much from initial time step value.
      Please guide me.
    • Rob
      Ansys Employee
      How constant do you expect the result to be? Around 0.1 in 30463.8 looks pretty constant to me. Similarly, we're after a mass balance within about 0.5% of the minimum flow boundary. If you monitored the experiment to that level of precision what kind of sensors would you be using?
    • KSD
      Subscriber
      Sir, If it looks constant to you then it means, my understanding was wrong. I thought the value should not change in case of steady solution, it should remain same.
      Thank you for clarifying it.
      So Sir, does that mean doing transient simulation (URANS) here is meaning less? Could you please confirm that as well.
      Because considering the time taken by the transient simulation, I would like a confirmation on it whether I should really proceed with it or not. As my main objective is to find the nozzle thrust coefficient and how pressure is acting on outside of nozzle surface.
    • Rob
      Ansys Employee
      You need to decide if the simulation results in steady state are suitable for your application. Monitors, residuals and fluxes play a part in that, along with images to figure out what the flow is doing. The above looks pretty steady, but does take it's time to converge. What does your supervisor think?
    • KSD
      Subscriber
      Sir, till now I didn't see a single research paper related to my particular work where I can validate my results, only thing I have done is grid independence test for assuring the accuracy of solution. Regarding monitors, as you have already seen is constant for both drag and mass imbalance which indicates the solution is steady.
      As you can see above steady state solution Mach contour plot, there are recirculation region present, thus my supervisor believes that there can be variation in size of circulation and If I run (URANS) I might observe that changes.
      I have been running transient run for last two days only 2lakh time steps have been completed (On Clusters using 22 parallel processes ), and for total time steps of 40 lakh+ I think it will take more than 40 days just to complete one simulation.
      And I have to do the same for different crossflow Mach number which seems like it will take n number of months.
      I am calculating time step size as follows as my smallest mesh size is 1e-5 (due to presence of high grid density across wall or inflation layers) and maximum velocity is around 4200 m/s so based on that I am getting time step size of order 1e-9. Thus just for one flow time I need to do around 17 lakh time steps and for ensuring more than 2-3 flow time it will easily cross 40 lakh time steps which is humungous.
    • Rob
      Ansys Employee
      I cannot tell you that the steady solver is correct as you're seeing some variations in the monitors: I also haven't told you the result is wrong. I am NOT ALLOWED to give specific engineering advice to comply with the rules. Hence me giving you as much guidance on looking at the results as possible so you can decide if the extra compute cost is worth it to potentially trim another fraction of a percent of a tiny fluctuation.
      or don't operate under the same rules, so can be less subtle in their responses.
    • KSD
      Subscriber
      Sir, I can understand. Thank you for helping me and tagging others for answering my queries is really appreciable.
Viewing 11 reply threads
  • You must be logged in to reply to this topic.