[atul1018]

Hello All

I am trying to solve particle-laden backward facing step case using DPMFoam. fluid phase has turbulent flow condition. I am using mappedPatch bc to get fully developed turbulent flow at inlet. Firstly, I was using RANS models to get the fluid fields and using fluid solution to model particle motion (including dispersion models) using solver DPMFoam. I am comparing time avearged fluid velocity profiles (normalized using max velocity) at several locations. For fluid phase (using RANS), I was getting really good agreement with experimental data (fluid velocity profiles) but particle phase velocity are far from measured profiles. The particles are not dispersed below the steps especially at measurement locations. despite several efforts to improve the results for particle phase, no success was achieved.

Then I shifted to LES models for fluid phase and use it to model motion of particles using same solver (DPMFoam). In doing so, I refined my mesh and used different LES models along the different delta functions. But unfortunately, this time I am not getting good results even for fluid phase (which I was getting, in RANS simulations). Partciles are slightly more in numbers but still far from measured values. in short in LES, both fluid and particle phase veocity profiles are far from measured values.

In my knowledge, the LES gives instantaneous fluid fields upto certain scales and may requires longer time to get stastically independet flow fileds, so avraging time, start and end of averaging affects the averaged values significantly. on the other hand, RANS gives time averaged values as solution, so averaging time will not affect the values (time avearge of time averaged values (RANS) is same; <<U>>=<U>). That was the reason, I was getting good match with experimental velocity profiles for fluid phase.

my question is: how much time should LES be run before start averaging, in order to get ststically independ solution? I was running for 1 sec, out of which averaging is done for last 0.3 sec. It seems that which is not sufficient to get stastically independent solutions, may require longer duration.

[oswald]

Hi Atul,


nice to see that you are still trying to find out what's wrong!



I find the approach of switching to LES quite interesting. It prevents difficulties in dispersion modelling. Unfortunately, it can be quite hard to get a reasonable model for LES. First of all: Are you still doing this in 2D? If so, I'd suggest switching to 3D.


You're approach to start averaging after some initial time is okay, I think. I don't know the residence time in your geometry (how long does it take from inlet to outlet in general?), but I'd suggest to let the simulation run at least for this time, preferably longer, before you start averaging. You can then set up some probes for the mean velocity and have a look on its behaviour. There should be some fluctuations at the beginning of the averaging process, but at some point it will level out to a quasi-steady state. How long this takes is hard to tell in advance. Just try it out.

[atul1018]

Hello Oswald




Thanks that you replied this time also to my thread and willing to help me out.

I find the approach of switching to LES quite interesting. It prevents difficulties in dispersion modelling. Unfortunately, it can be quite hard to get a reasonable model for LES. First of all: Are you still doing this in 2D? If so, I'd suggest switching to 3D.

I tried both with 2D and 3D cases. However for 3D cases, mesh is relatively coarse (eg. grid size of 2mm in z-direction) and symmetry bc is applied in z-direction. For both 2D and 3D cases, the fluid velocity profiles are very sensitive to LES models (which might be due to coarser mesh resolution). On the other hand, particle motion and its dispersion are very similar for all run 2D/3D LES cases. I am also wondering about mesh refinement, I cannot have extreme refined mesh because of requirement of high computational and time resources. I tried to optimize the mesh using grading in wall-normal direction and also using wall functions in some cases, but no significant improvement.

You're approach to start averaging after some initial time is okay, I think. I don't know the residence time in your geometry (how long does it take from inlet to outlet in general?), but I'd suggest to let the simulation run at least for this time, preferably longer, before you start averaging. You can then set up some probes for the mean velocity and have a look on its behaviour. There should be some fluctuations at the beginning of the averaging process, but at some point it will level out to a quasi-steady state. How long this takes is hard to tell in advance. Just try it out.

yes, you raised really good point of residence time (flow through time). My geometry has a length of 1068mm in x-direction and provided mean flow velocity at inlet is 9.39 m/s. so residence time (flow through time) is 1.068/9.39 =0.114 sec.I am doing simulation for 1 sec (~9*residence time), out of which averaging was done for last 0.3 sec (~2.5*residence time). I read in some literature, there they used total sim. duration = 83*residence time, out of which last 27*residence time was used to perform averaging. However in my case, it will take weeks to finish this kind simulation settings.




I don't know whether the inaccuracy is due to relatively coarser mesh or due to smaller simulation duration. increasing mesh resolution/simulation time would require a lot of computational and time resources.


Best Regards
Atul Jaiswal

[oswald]

Two thoughts regarding resolution:


The cell center of your first cell at the wall should preferably either be in the viscous sublayer (y+ < 1), in that case you don't need wall functions. Or you put in in the logarithmic region (30 < y+ < 100) and use wall functions. (iirc, OpenFOAM is also able to calculate appropriate values in the buffer region.) yPlus can be calculated with postProcess functionality.


You can furthermore check the ratio of resolved TKE and SGS-TKE. Pope claims that it is sufficient to resolve 80% of the TKE, see https://iopscience.iop.org/article/1...30/6/1/035/pdf


I don't think it's necessary to simulate 83 times the residence time. Just check if your mean velocity is still changing. If not, I'd say it converged.

[atul1018]

The cell center of your first cell at the wall should preferably either be in the viscous sublayer (y+ < 1), in that case you don't need wall functions. Or you put in in the logarithmic region (30 < y+ < 100) and use wall functions. (iirc, OpenFOAM is also able to calculate appropriate values in the buffer region.) yPlus can be calculated with postProcess functionality.

for all of my Mesh resolutions, the first cell lies between 5 to 20, which is in the buffer region. So I must use wall function in order to get better results?

You can furthermore check the ratio of resolved TKE and SGS-TKE. Pope claims that it is sufficient to resolve 80% of the TKE, see https://iopscience.iop.org/article/1...30/6/1/035/pdf

What do you think about the checking the value of eddy-viscosity. I check the eddy viscosity values for all my LES cases with different models and delta functions. I found that 3D case (110400 cells) with kEqn (with VanDriest delta) gives lower values of nut (order of ~10^-5) than other models (which is of order ~10^-4). Does smaller value of eddy viscosity represent near to correct solution. It is worth to mention, molecular viscosity is 1.5*10^-5. So it means that only my 3D model predicts eddy viscosity in range of molecular viscosity. In other cases, eddy viscosity is 10 times higher than molecular viscosity.

I don't think it's necessary to simulate 83 times the residence time. Just check if your mean velocity is still changing. If not, I'd say it converged.

Yes, I will try now until I see no change in averaged values.



Best Regards
Atul Jaiswal

[atul1018]

Hello Oswald

Two thoughts regarding resolution:


The cell center of your first cell at the wall should preferably either be in the viscous sublayer (y+ < 1), in that case you don't need wall functions. Or you put in in the logarithmic region (30 < y+ < 100) and use wall functions. (iirc, OpenFOAM is also able to calculate appropriate values in the buffer region.) yPlus can be calculated with postProcess functionality.

I calculated the yPlus value at 1st cell manually but I want to crosscheck the value by comparing it with calculated value of yPlus using function object in OpenFoam. To do the same I have added the following in controlDict:

 yPlus1
    {
        type            yPlus;
        libs            (fieldFunctionObjects);
        writeControl    writeTime;
}

Unfortunately OpenFoam reports that turbulence model doesn't found in data base.I tried with runtime postprocessing and postprocessing after the simulations but same error is reported. I tried also with different version of Openfoam (OpenFoam-v1912 and OpenFoam 8), but no success. Others have also reported it (see: yPlus twoPhaseEulerFoam)


if you know how to fix this, please let me know.


Regards
Atul

[oswald]

You can try

pimpleFoam -postProcess -func yPlus

It works with OpenFOAM-dev and quite sure also with OpenFOAM 8.

[atul1018]

Hello Oswald


I am usingmultiphase solver (DPMFoam) not single phase solver (pimpleFoam). I tried the following in OpenFoam 8. When I do postprocessing after the simulation from commandline:

DPMFoam -postProcess -func yPlus

I get the error that turbulence model not found:

--> FOAM FATAL ERROR: 
Unable to find turbulence model in the database

    From function virtual bool Foam::functionObjects::yPlus::execute()
    in file yPlus/yPlus.C at line 185.

FOAM exiting

As DPMFoam is based on pimpleFoam. I also tried with your suggestion:

pimpleFoam -postProcess -func yPlus

it reports:

Time = 0
Reading field p

Reading field U


--> FOAM FATAL ERROR: 
cannot find file "/home/workstation/OpenFOAM/workstation-8/run/LES_55000cells_Smagorinsky_vanDriest_avg(0.3-5)/BFS_LES_improvement_trial/0/U"

    From function virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::readStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
    in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 538.

FOAM exiting

I guess this error is due to the names of the files used in solving the case using DPMFoam. In my case the files are name by ending '.air' (e.g. U.air, k.air,etc), thats why when code: pimpleFoam -postProcess -func yPlus is run, it gives error that file U is not found.



The code: DPMFoam -postProcess -func yPlus should have worked but gives error saying turbulence model not found in the database. Probably the function objects such as yPlus, wallShearStress are not working with multi-phase solvers as reported by others too.


Regards
Atul

[oswald]

You can try to rename "U.air" to "U" in the time folders of interest and revert the changes afterwards.