[spelletier]

Hello all,

I am in the process of attempting to simulate a rather complex impinging jet problem and I feel as if I might be a little bit beyond my depth.

the problem in question involves multiple jet impingement on a heated surface with the goal of determining the heat transfer coefficient at various inlet settings. I am having a great deal of difficulty obtaining steady state results for the surface heat fluxes at the impingement surface. I am using kw SST, ideal gas law, sutherlands, atmospheric pressure outlets, and pressure inlets with velocities above 300 m/s. I have attached a few images of my grid and initial results showing the velocity profiles in mach number as well as residuals and heat fluxes.

I have a couple of theories as to why I cant achieve a steady state solution but I don`t think my understanding of CFD is strong enough. If anyone has any insight or resources I could study I would be greatly appreciative.

Theory 1) Even though the boundaries and flow are steady heat transfer itself is unsteady due to a variety of factors such as high turbulence, vortex's, and boundary layer separation?

Theory 2) The problem is steady state but my grid is either not a high enough resolution or is too low quality to produce steady state results?

Theory 3) I need to continue iterating using steady state and eventually the heat fluxes will level out?

[FMDenaro]

The problem in the lack of convergence in a RANS formulation is often debated. RANS assumes a "statistically" steady state.

Thus, the first issue to address is if your flow problem admits physically a statistically steady state (that is the statistically averaged variables do not depend on time). That has nothing to do with the unsteady, 3D character of the pointwise solution. That means that your problem must reach an energy equilibrium, that is production and dissipation of kinetic energy must balance. If in your case the internal energy is not in equilibrium the problem has not a statistically steady state and your RANS formulation correctly does not reach the convergence.
Conversely, if your flow problem admits a physical statistical steady state then the RANS solution exists and your issue depends on numerical and modelling issues. In such a case you should check for the iteration parameters, the grid resolution, the proper turbulence model...

[spelletier]

Thank you very much for taking the time to consider my problem

That has nothing to do with the unsteady, 3D character of the pointwise solution.

I'm not sure I quite understand, are you saying that the 3D physical flow characteristics themselves do not dictate whether a problem has a steady state solution?

That means that your problem must reach an energy equilibrium, that is production and dissipation of kinetic energy must balance.

If I understand correctly, an energy equilibrium in the system would mean there must be a steady state solution to the problem, In that case then a stationary system with constant boundary conditions such as mine will always have a steady state solution?

[FMDenaro]

- The key is that the steady state in the RANS formulation is considered for the statistical averaged variables. That means that a 3D, time dependent pointwise velocity field (showing vortical structures, strong fluctuations, etc) after the statistical averaging can become 2D and steady. That depends only on the specific physics of your problem.


- The steady (in statistical sense) BCs are a requisite but in your case we should see careful the type of BCs for the temperature. If they are prescribed in such a way that the heat flux balance over the boudaries, the system is in equilibrium. But if the temperature BCs, even if steady, allows for the averaged temperature to change in time (for example for an increasing or a decaying of the averaged temperature) then the averaged internal energy equation does not have a steady state.

[spelletier]

After working on this problem I have been able to successfully obtain steady state solution using first order methods, through which my monitors are all steady state and my residuals fall to below 1e-7. Unfortunately when I switch to second order to improve the accuracy of my results the system begins to oscillate erratically and not return anything of use.

Since the original post I have switched to a structured grid that has relatively good skewness and orthogonality, with the only potential problem being high aspect ratios at the boundary layer to achieve y+ ~ 1.

There is reverse flow at the outlets but this is true for both the second and first order so I don`t see why that would be an issue.

Is there a better approach to switching to second order other than switching all at the same time? Could switching one at a time or decreasing URF and then switching to second order help? Essentially I`m not exactly sure how to troubleshoot such a problem...

Ive read that the kOmega SST model can have convergence problems when deal with high gradients of "Omega" Although I don`t know how to determine If that is an issue in my simulation.


A secondary question that may sound rather defeatist:
I am doing a comparative study of various flow settings and don`t necessarily care about the absolute values would it be useless to compare first order results between simulations given that all other parameters remain the same?

Thank you again for your time professor as well as anyone else that has any insight.

[FMDenaro]

Problem in getting a convergent solution in RANS are quite common. As you verified, the first order scheme introduces a lot of numerical diffusion that has the ability to help convergence. However, such artificial diffusion can also be the cause of a poor solution.
Have you already tried to start from the first order solution you have obtained and run with second order scheme?

Try also differente turbulent models.

[spelletier]

Thank you for your suggestions!

the first order scheme introduces a lot of numerical diffusion that has the ability to help convergence. However, such artificial diffusion can also be the cause of a poor solution.

Is this numerical diffusion constant? As in will it cause similar error every time the simulation is run? For example if I had two runs on the same grid with varying inlet velocities would the diffusion effect them in the same way?

Have you already tried to start from the first order solution you have obtained and run with second order scheme?

I have tried starting from first order and then switching to second order after convergence which has been my main strategy so far although I have not been able to obtain second order convergence.

Try also differente turbulent models.

I have been able to obtain second order convergence using the k-e and k-e realizable schemes, however from prior research these give non-ideal results for impinging jet problems although if I can`t achieve second order convergence using k-w SST I may be forced to use k-e realizable to have results of which I at least know the relative "wrongness".

[FMDenaro]

The numerical diffusion of first order scheme has a magnitude proportional to the local grid size. Even if that says is the same magnitude when the grid is the same, you have to consider that the coefficient multiplies a second derivatives of the variable, it should be ensured that such term is always O(1)