[Xiaoyu Yang]

Dear All,

First of all, wish you all have a successful year in 2017! I am relatively new to this forum and to OpenFOAM and LES. Thanks for your suggestions in advance!

At the moment, I am trying to validate the code and the LES model via a fully developed incompressible turbulent channel case at Re_tau=180. The pisoFoam solver together with the dynamicKEqn LES model are used. Please I was wondering if anyone could give me some suggestions on how to choose a proper combination of numerical schemes. Instead of the default, I am seeking for higher order schemes for lower dissipation and better accuracy.

The geometry of this rectangular channel is (2\pi\delta, 2\delta, \pi\delta) in the (x, y, z) directions, respectively. For Re_tau=180, the Reynolds number based on the mean centreline velocity is Re_delta=3300, and the kinematic viscosity is scaled such that the half channel height is 1m and the mean centreline velocity is 1m/s. Accordingly, to drive the flow, a corresponding constant x-momentum source term is implemented as a dynamic code through fvOptions. In accordance with this case setup, the periodic boundary conditions (cyclic B.C.) are applied in both the streamwise and spanwise directions.

Comparison results of the mean velocity and the Reynolds stress with DNS (Moser, Kim, and Moin 1999) are attached. As can be seen, the numerical accuracy needs to be improved, and I am struggling with choosing a proper combination of numerical schemes for higher order accuracy. At the moment, the Crank Nicolson scheme with the coefficient 0.9 is used for time integration, and the Gauss cubic scheme is used for the gradient terms. Linear interpolation and Gauss linear corrected Laplacian terms are also used. The used fvSchemes, the fvSolution, and the turbulenceProperties files are also attached for clarity.

Particularly, if the Gauss cubic scheme is used for the divergence terms, the instantaneous flow structures show irregular discontinuities even though the solver could still run.

Besides, at this stage, my primary consideration is about the numerical schemes. To get more familiar with this flow solver, and to save time and get some quick answers, a coarse mesh is used for the current computation. The used grid density is about the half of the standard LES requirements in all the three directions, i.e. dx+=28, dz+=19, dy+_1st=0.36, and dy+_max=37. The noslip wall boundary condition is applied for the top and the bottom walls with the viscous sublayer resolved.

Currently, I am using OpenFOAM-v3.0+ version. It seems that the Crank Nicolson scheme is a good choice for time integration. However, when with the coefficient 1.0, this implementation of the code becomes unstable and the flow diverges. Therefore, I am using the coefficient 0.9. For spatial discretizations, generally, I am trying to find a fourth order combination, preferably with lower dissipation.

Please could anyone give me some suggestions for this.

Thanks for your time!

Xiaoyu

[ehsan]

Hello,

We have a similar problem, we tried cubic discretization for channel flow at Re_t=590. We used a relatively coarse grid but used a higher order discretization. The results lasted a lot and we did not get correct but underestimated solution. Would you please give any advice?
Regards

[Xiaoyu Yang]

Originally Posted by ehsan

Hello,

We have a similar problem, we tried cubic discretization for channel flow at Re_t=590. We used a relatively coarse grid but used a higher order discretization. The results lasted a lot and we did not get correct but underestimated solution. Would you please give any advice?
Regards

Hi Ehsan,

Good to know you are running similar simulations. For me, when the Gauss cubic scheme is used for div() terms, instantaneous flow structures show strange discontinuties. This looks like numerical disorders related to the schemes. Did you get this problem or not please? Do let me know if you get some progress.

Thanks in advance,

Xiaoyu

[ehsan]

Hello,

Thank you, no, we did not have this problem but our run time was really increased compared to the default setting of OpenFOAM. Another point: we used PIMPLEFoam solver for our simulation.

Best Regards

[Xiaoyu Yang]

Originally Posted by ehsan

Hello,

Thank you, no, we did not have this problem but our run time was really increased compared to the default setting of OpenFOAM. Another point: we used PIMPLEFoam solver for our simulation.

Best Regards

Hi Ehsan,

Thanks for your suggestions. Let me try the pimpleFoam solver shortly.

At the moment, with a combination of the backward time integration and Gauss linear spatial discretizations, I am getting some improved results using a fine mesh (81 x 161 x 81). For this, the mean velocity profile and the Reynolds stresses are attached in the following.

[Xiaoyu Yang]

Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

https://www.cfd-online.com/Forums/op...ctrum-les.html

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu

[Bashar]

Originally Posted by Xiaoyu Yang

Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

https://www.cfd-online.com/Forums/op...ctrum-les.html

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu

Hi,
So sorry to bother you ,but is it possible to share how you plot these results in your attachment? I am looking for away to post-process the results of my LES case . I have the data for UPrime2Mean and R and I want to extract it from the files in OpenFoam and then draw it.
Sorry again to ask you in your post.

[Xiaoyu Yang]

Originally Posted by Bashar

Hi,
So sorry to bother you ,but is it possible to share how you plot these results in your attachment? I am looking for away to post-process the results of my LES case . I have the data for UPrime2Mean and R and I want to extract it from the files in OpenFoam and then draw it.
Sorry again to ask you in your post.

Hi Bashar,

I assume that you got your Umean, UPrime2Mean, and RMean files from the solver. Then, for the channel case, you can use the tool --- postChannel to collapse the data down to single-line profiles. By default, this tool does not calculate the sub-grid-scale stresses, i.e. the RMean part. Therefore, you need to modify it a little bit. This should be straight-forward. Look for the way how the resolved Reynolds stresses are calculated. Then, copy paste and change to RMean values.

Let me know if you need further assistance.

Good luck......

Xiaoyu

[aerosjc]

Hi!

I'm also trying to validate my DNS results of channel flow at Re_tau = 180, but with codes in Flux Reconstruction method. There are 2 problems I want to discuss with you.

1. How to specify Re_tau = 180? The way I'm using is illustrated in http://desperadoshi.github.io/Notes/...del/index.html. Bother you to check if it's correct. Basically it's using Dean's law.

2. How to prove the results are DNS? Of course, we can compare with published results from well-known paper. However, how can we prove it's DNS with our own framework. Do you think the convergence of the FFT of time history of pressure or velocity could prove it's indeed DNS? Maybe there is somewhat connection between turbulence energy spectra and such spectra I described above, but I guess the convergence of turbulence energy spectra should be used to prove it's DNS, instead of FFT of time history, is that true? Apart from FFT way or turbulence energy spectra way, how do you prove your results are DNS?

[Bashar]

Originally Posted by Xiaoyu Yang

Hi Bashar,



I assume that you got your Umean, UPrime2Mean, and RMean files from the solver. Then, for the channel case, you can use the tool --- postChannel to collapse the data down to single-line profiles. By default, this tool does not calculate the sub-grid-scale stresses, i.e. the RMean part. Therefore, you need to modify it a little bit. This should be straight-forward. Look for the way how the resolved Reynolds stresses are calculated. Then, copy paste and change to RMean values.



Let me know if you need further assistance.



Good luck......



Xiaoyu

Thanks a lot for your input. So , to clarify, I need to execute this tool in my case directory, then it will print the data , which I can plot it using any program of my choice?
Regarding, the part that I need to modify the tool , that I did not understand how to do it. I will search to see how to do that since I never did such thing.
Best wishes and many thanks .
Bashar


Sent from my iPhone using CFD Online Forum mobile app

[Xiaoyu Yang]

Originally Posted by aerosjc

Hi!

I'm also trying to validate my DNS results of channel flow at Re_tau = 180, but with codes in Flux Reconstruction method. There are 2 problems I want to discuss with you.

1. How to specify Re_tau = 180? The way I'm using is illustrated in http://desperadoshi.github.io/Notes/...del/index.html. Bother you to check if it's correct. Basically it's using Dean's law.

2. How to prove the results are DNS? Of course, we can compare with published results from well-known paper. However, how can we prove it's DNS with our own framework. Do you think the convergence of the FFT of time history of pressure or velocity could prove it's indeed DNS? Maybe there is somewhat connection between turbulence energy spectra and such spectra I described above, but I guess the convergence of turbulence energy spectra should be used to prove it's DNS, instead of FFT of time history, is that true? Apart from FFT way or turbulence energy spectra way, how do you prove your results are DNS?

Hi Jingchang,

Good to know you are running similar cases.....

For DNS case setup, the Dean's correlation is ok. I feel probably the key thing is to determine the correlation between the inner and outer scales, or equivalently the corresponding Reynolds numbers. For Retau=180, the centreline Reynolds number Remax = Umax*delta/nu is about 3300. This gives fairly accurate inner and outer scales with relative error less than 2%. For a given combination of the half channel height "delta" and the kinematic viscosity "nu", than the friction velocity "u_tau" and and the centreline velocity "Umax" may be determined. Then, the channel model should be while defined, based on Reynolds number similarity. For higher friction Reynolds number cases, I guess you need to find the corresponding "Remax".

For DNS results, I guess it depends on the way how they are computed. In my mind, by definition, DNS means that the N-S equations are solved directly without any extra turbulence models, such as RANS models or LES SGS models. So I feel basically in a DNS simulation, all scales of turbulent motions are resolved directly, rather than modelled. So far this is still limited to relatively low Reynolds number flows, due to heavy computational intensity. On the other hand, once discretized, numerical issues arise such as stability, dissipation and dispersion of a particular scheme, etc. Therefore, special treatment may be needed to get a set of accurate converged solutions. But this should be a different topic. Then, for validation or benchmark purpose, I guess you might want to compare your DNS results with other available datasets, such as the mean statistics, the Reynolds stress budgets, and the spectrum, etc......

Not quite sure, but hopefully these answer your questions......

Keep in touch,

Xiaoyu

[Xiaoyu Yang]

[QUOTE=Bashar;639260]Thanks a lot for your input. So , to clarify, I need to execute this tool in my case directory, then it will print the data , which I can plot it using any program of my choice?
Regarding, the part that I need to modify the tool , that I did not understand how to do it. I will search to see how to do that since I never did such thing.
Best wishes and many thanks .
Bashar


Hi Bashar,

Yes, in your case directory, execute the "postChannel" command, this tool will look for your time averaged datasets and collapse the data down to a single-line profile. Then, you could plot your results using other software packages, such as Tecplot or MatLAB.

To modify this tool, probably, you could search for some suggestions on how to modify an application under the OpenFOAM framework. Then, look through my previous posts to see how to add in the Rmean part.

Good luck,

Xiaoyu

[aerosjc]

Sorry for late reply.

Now, I modify the method I described and I'm sure it's correct.

Thank you for the reply.

[Elyas_Mosibat]

Originally Posted by Xiaoyu Yang

Hi Ehsan,

Here are the mean velocity and the Reynolds stresses profiles. As you can see, the mean flow seems acceptable with an relative error around 1%, and the log-law is captured. But the turbulence fluctuations and the Reynolds shear stress are much lower than the expected.

According to these two posts,

Relation between k and UPrime2Mean etc in LES

https://www.cfd-online.com/Forums/op...ctrum-les.html

it seems that, for LES, what I get from "UPrime2Mean" are the filtered/resolved turbulence stresses. The sub-grid scale modelled stresses have to be added into the above to get the full stresses, i.e. “total Reynolds Stress = UPrime2Mean + Subgrid_ReynoldsStress”. Have you done this before? To calculate the SGS part, is this line below correct?

(2.0/3.0)*I)*k_ - nuSGS_*twoSymm(fvc::grad(U_)

If so, I guess will have to play with the solver a little bit.

Still, based on the current results, it seems that these Reynolds stresses are under-estimated, since I feel the SGS part would not contribute that much. Any idea about this please?

Thanks in advance,

Xiaoyu

Hi Xiaoyu
If your turbulence model is Eddy viscosity , the GenEddyVisc is used to calculate the SGS part;
tmp<volSymmTensorField> GenEddyVisc::B() const
{
return ((2.0/3.0)*I)*k() - nuSgs_*twoSymm(fvc::grad(U()));
}
and if you are using another type of LES model , the GenSGSStress is used, and the SGS stress tensor will computed from your model

[Xiaoyu Yang]

Originally Posted by Elyas_Mosibat

Hi Xiaoyu
If your turbulence model is Eddy viscosity , the GenEddyVisc is used to calculate the SGS part;
tmp<volSymmTensorField> GenEddyVisc::B() const
{
return ((2.0/3.0)*I)*k() - nuSgs_*twoSymm(fvc::grad(U()));
}
and if you are using another type of LES model , the GenSGSStress is used, and the SGS stress tensor will computed from your model

Hi Elyas,

Thanks a lot! Let me check this......

Regards,

Xiaoyu

[kokab]

hello everybody
I also have a problem in validating my channel for Re_tau=395.
my channel is (2pi,2,pi) and LES model is WALE, all the set up are the same as channel395 in openFOAM tutorial.
I have attached my plots, can anyone tell me how to improve my result?
- mesh (60,60,60)
- openFOAM 3.0.1
- solver algorithm pimpleFoam
thanks all

[Xiaoyu Yang]

Hi Kokab,

It might be worth for you checking this technical report.

https://www.it.uu.se/research/public...4/2015-014.pdf

Hopefully, it can help you out.

Best wishes,

Xiaoyu

[kokab]

Hi Xiaoyu
thank you very much actually I had read mukha's thesis many times
my question was about the LES model, I mean by the WALE why can not valid my channel, however the mesh is very coarse but is there any other reason except that?
now I have changed my mesh to (128,128,128) with oneEqEddy and it is valid but WALE is still a big question...
again thanks a sea for your helping

[Tobi]

I will keep that thread in that forum because it has some analyzes
Please read the purpose of that sub-forum.

[ehsan]

Hello,

Any feedback on this new forum is welcome:

https://www.cfd-online.com/Forums/op...tml#post688964

Regards