[jms]

Hi all!

I have been using OpenFOAM for 2 months, so I am quite new with this software.
I am using it to do a study in 2D of the flow over a NACA0015, at Re=2x10^6 at steady state. Using simpleFoam and the k-omega SST turbulence model.
I have been doing a sensitivity study of the numerical schemes. Thus, I have been changing the divSchemes. I have tried changing all the entries in there to QUICK/QUICKV, linear, linearUpwind and upwind. I couldn´t change the entry "div((nuEff*dev(grad(U).T())))" to any of those (I have to keep at as linear, otherwise the programme does not recognize it), why?
I have upload the file fvSchemes used so you can have a look at it.
I have also uplodaded a figure showing the results obtained compared with a reference. They do not look as expected since the closest solution obtained for the lift coefficient calculations is for the upwind numerical scheme, while this one should give the worst results, shouldn´t it?

Thank you for your attention.

I will really appreciate your help.

Regards,

José

[hjasak]

It does not recognise it because this is a straightforward div(thing) term and not convection div(phi, thing).

Therefore you cannot do upwinding, since there's no flux to decide the direction from.

Hrv

[jms]

Thank you very much. It makes sense
Any suggestion for the results presented? Using such a fvSchemes file?

[makaveli_lcf]

1. To change the scheme for "div((nuEff*dev(grad(U).T())))" you should define the flux variable by hand (see the User Guide p. 112 for interpolation schemes)

2. There are issues regarding wrong calculation for the viscous term for k-omega SST in OF on this forum. Its is different from other model for the value of sqrt(2). Perhaps that is the case for your comparison witrh reference solution.

3. "Gauss linear limited 1;" in your laplacian section is the same as "Gauss linear corrected;"

[FelixL]

Hello, José,


these are pretty neat results you have there. It is interesting to see how different divergence schemes affect the results.

However, did you perfom a grid sensitivity analysis when you compare your results? It would be a bit more meaningful if you'd analyze how the discretization error of each scheme is reduced when grid spacing is e.g. halfed.

The good reproduction of experimental data of lift coefficient when using upwinding really is surprising, but I wouldn't say upwinding is more accurate in this case. Especially at high lift coefficients separation occurs and this is where the choice of turbulence modeling becomes much more important than in attached cases. My guess is that k-Omega-SST is not able to reproduce the separation at high angle of attacks of this airfoil, but the increased diffusivity caused by using a first order scheme like upwinding sort of "accidently" corrects this shortcoming.

A comparison using different turbulence models (Spalart-Allmaras or LowRe-K-Epsilon) would make sense, but it of course also means many more simulations.



Greetings,
Felix.

[jms]

Thank you for your answers. Comments to Alex´s reply:

1) I will have a look at it.
2) I already corrected this issue.
3) Ok.

Comments to Felix´s reply:

I had already thought on that but I don´t know if I will have time enough to see this (I am doing a master thesis...).
Good to know that this can be coincidence. I will have a look at it! I was advised to use k-omega SST since it was predicting better the stall region. I also did some computations previously using Spalart Allmaras but the results obtained were very similar. Anyway...I may check other turbulence models.

Thank you for your help.

More suggestions are very welcome.

Regards,

José

[alex_rubel]

Hi all,
I'm using simpleFoam with kOmegaSST and I get accuracy issues with my Drag coefficient.
Can you tell me more about what you said Alex :

2. There are issues regarding wrong calculation for the viscous term for k-omega SST in OF on this forum. Its is different from other model for the value of sqrt(2). Perhaps that is the case for your comparison witrh reference solution.

Alex

[aloeven]

There was a bug in the kOmegaSST model regarding the computation of nut (missing sqrt(2)). This was fixed on 12 November 2010 in the git repository of OpenFOAM-1.7.x.

So you have to check your version. If you have 1.6.x or 1.7.1, then you have to fix the bug yourself.

You can check the files and fix here:
https://github.com/OpenCFD/OpenFOAM-...f7a0b26d64265d

Good luck,
Alex (another one)

[jms]

there you are Alex I:
http://www.cfd-online.com/Forums/ope...nce-model.html

[alex_rubel]

Thanks that's good to know, I got the 1.6.8 version I think.
I hope this will lead to improvement in my case.
Anyway, here is the link of my topic maybe you can help me : http://www.cfd-online.com/Forums/ope...implefoam.html

Alex

[chegdan]

Originally Posted by hjasak

It does not recognise it because this is a straightforward div(thing) term and not convection div(phi, thing).

Therefore you cannot do upwinding, since there's no flux to decide the direction from.

Hrv

Hello Foamers,

I just had a simple question about the div((nuEff*dev(grad(U).T()))) term in fvSchemes for a simpleFoam simulation. I know that one cannot just use Gauss upwind since there is no flux and the direction of flux is not known. One can simply provide a phi as

div((nuEff*dev(grad(U).T()))) Gauss upwind phi 1;

Is this correct and usable? I ask because the default is linear and I thought that the cell Peclet number would have an effect (lead to unbounded results for this term) for central differencing...hence why upwinding with a prescribed phi=1 would be better. What is a good 1st order scheme and a good second order scheme...or should Gauss linear always be sufficient for div(thing) terms? Thanks for your help.

Dan

[oky]

Hi everyone,

I need help, how to get the value of convection coefficient [h] from Fluent directly?
Thank you.

Regrads,

Oky

[chegdan]

Originally Posted by oky

Hi everyone,

I need help, how to get the value of convection coefficient [h] from Fluent directly?
Thank you.

Regrads,

Oky

Wish I could help...try the Fluent forum instead. This is an openfoam forum. Good luck.

http://www.cfd-online.com/Forums/ansys/

[makaveli_lcf]

Dan,

you can use predefined flux to use the upwind scheme for your diffusion term. I didn't find any advantages applying this approach and usually your convection term produces unboundedness not the diffusion one.

[chegdan]

Originally Posted by makaveli_lcf

Dan,

you can use predefined flux to use the upwind scheme for your diffusion term. I didn't find any advantages applying this approach and usually your convection term produces unboundedness not the diffusion one.

Thanks for the input. After looking around more it seems that most posts referring to changing to 1st or second order schemes leave this term alone as Gauss linear. Thanks again.

Dan

[sh.d]

Hi Dr. Alexander
i need formulation of Gauss linear corrected. but i dont found it!
please can you help me?

[makaveli_lcf]

Pardon, what do you need and for which term (diffusive, convective)?

[bieshuxuhe]

Originally Posted by jms

Hi all!

I have been using OpenFOAM for 2 months, so I am quite new with this software.
I am using it to do a study in 2D of the flow over a NACA0015, at Re=2x10^6 at steady state. Using simpleFoam and the k-omega SST turbulence model.
I have been doing a sensitivity study of the numerical schemes. Thus, I have been changing the divSchemes. I have tried changing all the entries in there to QUICK/QUICKV, linear, linearUpwind and upwind. I couldn´t change the entry "div((nuEff*dev(grad(U).T())))" to any of those (I have to keep at as linear, otherwise the programme does not recognize it), why?
I have upload the file fvSchemes used so you can have a look at it.
I have also uplodaded a figure showing the results obtained compared with a reference. They do not look as expected since the closest solution obtained for the lift coefficient calculations is for the upwind numerical scheme, while this one should give the worst results, shouldn´t it?

Thank you for your attention.

I will really appreciate your help.

Regards,

José

divSchemes
{
default none;
div(phi,U) Gauss QUICKV cellLimited Gauss linear 1;
div(phi,k) Gauss QUICK cellLimited Gauss linear 1;
div(phi,omega) Gauss QUICK cellLimited Gauss linear 1;
div((nuEff*dev(grad(U).T()))) Gauss linear cellLimited Gauss linear 1;
}


The above is your divschemes. Does the number "1" in every schemes indicate the non-orthogonal correction? thank you!

[makaveli_lcf]

From User Guide: Some TVD/NVD schemes require a coefficient ψ, 0 ≤ ψ ≤ 1 , where ψ = 1 corresponds to TVD conformance, usually giving best convergence and ψ = 0 corresponds to best accuracy. Running with ψ = 1 is generally recommended

[sh.d]

thanks
yes i need it for diffusive : laplacian(muEff,U) Gauss linear corrected
i need the formulation of corrected snGradient.i see Hrvoj.jasak thesis but I could not find it...
please help me