fvSchemes

jms · February 21, 2011, 08:18

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 · February 21, 2011, 08:23

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 · February 21, 2011, 08:30

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

makaveli_lcf · February 21, 2011, 08:33

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 · February 21, 2011, 08:41

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 · February 21, 2011, 08:56

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 · February 23, 2011, 02:17

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 :

Quote:

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 · February 23, 2011, 03:57

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 · February 23, 2011, 04:02

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

alex_rubel · February 23, 2011, 05:57

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 · May 24, 2011, 16:19

Quote:

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 · May 25, 2011, 00:16

Hi everyone,

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

Regrads,

Oky

chegdan · May 25, 2011, 00:25

Quote:

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 · May 25, 2011, 03:52

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 · May 25, 2011, 11:42

Quote:

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 · August 30, 2013, 05:01

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

makaveli_lcf · August 30, 2013, 05:04

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

bieshuxuhe · August 30, 2013, 05:19

Quote:

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 · August 30, 2013, 05:26

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 · August 30, 2013, 08:02

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

February 21, 2011, 08:23		#2
hjasak Senior Member Hrvoje Jasak Join Date: Mar 2009 Location: London, England Posts: 1,907 Rep Power: 33	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 cfdivan, sh.d, smog and 1 others like this. __________________ Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk

February 21, 2011, 08:33		#4
makaveli_lcf Senior Member Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 256 Blog Entries: 1 Rep Power: 19	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;" __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

May 25, 2011, 03:52		#14
makaveli_lcf Senior Member Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 256 Blog Entries: 1 Rep Power: 19	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. __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

August 30, 2013, 05:01	Gauss linear corrected	#16
sh.d Member Join Date: Oct 2012 Posts: 47 Rep Power: 14	Hi Dr. Alexander i need formulation of Gauss linear corrected. but i dont found it! please can you help me?

August 30, 2013, 05:04		#17
makaveli_lcf Senior Member Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 256 Blog Entries: 1 Rep Power: 19	Pardon, what do you need and for which term (diffusive, convective)? __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

February 21, 2011, 08:30		#3
jms Member José Join Date: Jan 2011 Posts: 73 Rep Power: 15	Thank you very much. It makes sense Any suggestion for the results presented? Using such a fvSchemes file?

February 21, 2011, 08:41		#5
FelixL Senior Member Felix L. Join Date: Feb 2010 Location: Hamburg Posts: 165 Rep Power: 18	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.

February 21, 2011, 08:56		#6
jms Member José Join Date: Jan 2011 Posts: 73 Rep Power: 15	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

February 23, 2011, 03:57		#8
aloeven Member Alex Join Date: Apr 2010 Posts: 32 Rep Power: 16	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)

February 23, 2011, 04:02		#9
jms Member José Join Date: Jan 2011 Posts: 73 Rep Power: 15	there you are Alex I: http://www.cfd-online.com/Forums/ope...nce-model.html

February 23, 2011, 05:57		#10
alex_rubel New Member Alexandre Rubel Join Date: Dec 2010 Location: Launceston, Tasmania AUSTRALIA Posts: 28 Rep Power: 16	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

May 25, 2011, 00:16		#12
oky New Member Oky Andytya Join Date: Nov 2010 Posts: 26 Rep Power: 16	Hi everyone, I need help, how to get the value of convection coefficient [h] from Fluent directly? Thank you. Regrads, Oky

August 30, 2013, 05:26		#19
makaveli_lcf Senior Member Dr. Alexander Vakhrushev Join Date: Mar 2009 Posts: 256 Blog Entries: 1 Rep Power: 19	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 __________________ Best regards, Dr. Alexander VAKHRUSHEV Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics" Simulation and Modelling of Metallurgical Processes Department of Metallurgy University of Leoben http://smmp.unileoben.ac.at

August 30, 2013, 08:02		#20
sh.d Member Join Date: Oct 2012 Posts: 47 Rep Power: 14	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

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
fvschemes and fvsolutions in MRFSimpleFoam	renyun0511	OpenFOAM Running, Solving & CFD	23	August 3, 2011 05:07
OpenFOAM fvSchemes: laplacianScheme,	thomek	Main CFD Forum	1	October 18, 2010 06:17
Implementation issues of fvSchemes / laplacianScheme, in particular gaussLaplacianSch	thomek	OpenFOAM Programming & Development	0	October 18, 2010 06:10
General help for fvSchemes and fvSolution settings	harly	OpenFOAM Running, Solving & CFD	4	September 7, 2009 11:31
Doubt in term representation in the fvSchemes dictionary	titio	OpenFOAM Running, Solving & CFD	0	July 17, 2009 14:21