CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

fvSchemes

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   February 21, 2011, 08:18
Default fvSchemes
  #1
jms
Member
 
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
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
Attached Images
File Type: png schemes_lift.png (5.3 KB, 444 views)
File Type: png schemes_drag.png (4.9 KB, 341 views)
Attached Files
File Type: txt fvSchemes.txt (1.9 KB, 283 views)
jms is offline   Reply With Quote

Old   February 21, 2011, 08:23
Default
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
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 and sh.d like this.
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   February 21, 2011, 08:30
Default
  #3
jms
Member
 
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
Thank you very much. It makes sense
Any suggestion for the results presented? Using such a fvSchemes file?
jms is offline   Reply With Quote

Old   February 21, 2011, 08:33
Default
  #4
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to 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;"
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   February 21, 2011, 08:41
Default
  #5
Senior Member
 
Felix L.
Join Date: Feb 2010
Location: Hamburg
Posts: 165
Rep Power: 9
FelixL is on a distinguished road
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.
FelixL is offline   Reply With Quote

Old   February 21, 2011, 08:56
Default
  #6
jms
Member
 
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
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
jms is offline   Reply With Quote

Old   February 23, 2011, 02:17
Default
  #7
New Member
 
Alexandre Rubel
Join Date: Dec 2010
Location: Launceston, Tasmania AUSTRALIA
Posts: 28
Rep Power: 6
alex_rubel is on a distinguished road
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
alex_rubel is offline   Reply With Quote

Old   February 23, 2011, 03:57
Default
  #8
Member
 
Alex
Join Date: Apr 2010
Posts: 32
Rep Power: 7
aloeven is on a distinguished road
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)
aloeven is offline   Reply With Quote

Old   February 23, 2011, 04:02
Default
  #9
jms
Member
 
José
Join Date: Jan 2011
Posts: 73
Rep Power: 6
jms is on a distinguished road
there you are Alex I:
Wrong calculation of nut in the kOmegaSST turbulence model
jms is offline   Reply With Quote

Old   February 23, 2011, 05:57
Default
  #10
New Member
 
Alexandre Rubel
Join Date: Dec 2010
Location: Launceston, Tasmania AUSTRALIA
Posts: 28
Rep Power: 6
alex_rubel is on a distinguished road
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 : Submarine with SimpleFoam

Alex
alex_rubel is offline   Reply With Quote

Old   May 24, 2011, 15:19
Default anything about div(thing)
  #11
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 543
Rep Power: 18
chegdan will become famous soon enough
Quote:
Originally Posted by hjasak View Post
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
chegdan is online now   Reply With Quote

Old   May 24, 2011, 23:16
Default
  #12
oky
New Member
 
Oky Andytya
Join Date: Nov 2010
Posts: 26
Rep Power: 6
oky is on a distinguished road
Hi everyone,

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

Regrads,

Oky
oky is offline   Reply With Quote

Old   May 24, 2011, 23:25
Default
  #13
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 543
Rep Power: 18
chegdan will become famous soon enough
Quote:
Originally Posted by oky View Post
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/
chegdan is online now   Reply With Quote

Old   May 25, 2011, 02:52
Default
  #14
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to 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.
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   May 25, 2011, 10:42
Default
  #15
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 543
Rep Power: 18
chegdan will become famous soon enough
Quote:
Originally Posted by makaveli_lcf View Post
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
chegdan is online now   Reply With Quote

Old   August 30, 2013, 04:01
Default Gauss linear corrected
  #16
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
Hi Dr. Alexander
i need formulation of Gauss linear corrected. but i dont found it!
please can you help me?
sh.d is offline   Reply With Quote

Old   August 30, 2013, 04:04
Default
  #17
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
Pardon, what do you need and for which term (diffusive, convective)?
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   August 30, 2013, 04:19
Post
  #18
Member
 
xuhe-openfoam
Join Date: Aug 2013
Location: DaLian,china
Posts: 82
Rep Power: 3
bieshuxuhe is on a distinguished road
Quote:
Originally Posted by jms View Post
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!
bieshuxuhe is offline   Reply With Quote

Old   August 30, 2013, 04:26
Default
  #19
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 213
Rep Power: 10
makaveli_lcf is on a distinguished road
Send a message via ICQ to 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
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Advanced Process Simulation of
Solidification and Melting"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

Franz-Josef-Str. 18
A - 8700 Leoben
Österreich / Austria
Tel.: +43 3842 - 402 - 3125
http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   August 30, 2013, 07:02
Default
  #20
Member
 
Join Date: Oct 2012
Posts: 47
Rep Power: 4
sh.d is on a distinguished road
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
sh.d is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
fvschemes and fvsolutions in MRFSimpleFoam renyun0511 OpenFOAM Running, Solving & CFD 23 August 3, 2011 04:07
OpenFOAM fvSchemes: laplacianScheme, thomek Main CFD Forum 1 October 18, 2010 05:17
Implementation issues of fvSchemes / laplacianScheme, in particular gaussLaplacianSch thomek OpenFOAM Programming & Development 0 October 18, 2010 05:10
General help for fvSchemes and fvSolution settings harly OpenFOAM Running, Solving & CFD 4 September 7, 2009 10:31
Doubt in term representation in the fvSchemes dictionary titio OpenFOAM Running, Solving & CFD 0 July 17, 2009 13:21


All times are GMT -4. The time now is 23:25.