
[Sponsors] 
May 26, 2010, 16:14 

#21  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
The upwind schemes does not require anything: div(phi, U) Gauss upwind; The gradient scheme is used, for example, by the linearUpwind scheme: div(phi, U) Gauss linearUpwind Gauss linear; Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 26, 2010, 17:28 

#22 
Member
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 16 
hi alberto,
thanks a lot for your reply. i want to limit k and epsilon and dont know how to make that. e.g. for k, would it work like that? div(phi, k) Gauss linearUpwind Gauss limitedLinear 1e10 30; if not, could you give me an example? thanks a lot, Moritz 

May 26, 2010, 22:54 

#23  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
If the equations do not include that physical limit, I would not use a limiter, but a bound, as done in the codes already. The syntax, explained at page U113 of the user's guide, is, for example: div(phi, U) Gauss limitedVanLeer a b; where a and b are the bounds of your range [a,b]. Schemes that support the limitation in this way are listed in the same page. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 27, 2010, 05:08 

#24  
Member
Moritz Wied
Join Date: Mar 2010
Location: suttgart, germany
Posts: 35
Rep Power: 16 
Quote:
What i dont understand is, that in these Schemes you calculate divergence and divgrad, but not the scalar values themselves, so can you limit the values themselves there? Quote:
Quote:
what parameters have to be given, when you use e.g. limitedVanLeerV? Thank you so much for your time!! 

May 27, 2010, 17:11 

#25  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
Let's try to understand what is the cause. What solver are you using, what turbulence model, and what boundary condition setup? Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 27, 2010, 22:43 

#26 
Senior Member

Hi Alberto, I have a similar problem with my case using kOmegaSST model. However, I ran many different but similar meshes of this external flow and they all converge. Only this case diverges on k. All the BCs and other parameters are identical.
Also, the case runs fine in laminar, although it doesn't converge... Could my mesh be the only cause of the divergence? Thanks, Louis 

May 27, 2010, 23:10 

#27 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Let me guess: is the mesh tetrahedral (maybe generated with Salomé)?
Please run checkMesh, and if you have very skewed cells and/or a high degree of nonorthogonality, yes, the mesh can be the reason of the problem. In this case you can easily see where this happens by saving solutions right before the crash and looking for peaks of values in the diverging variables. Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 28, 2010, 11:26 

#28 
Senior Member

Hi Alberto,
it is a hexmesh, from snappyHexMesh. Yes, it does have skewed faces but those skewed faces didn't seem to create a problem on my other meshes (well at least the bound on k worked for those other meshes). Thanks for your advice, I will try to slightly modify my snappyHexMesh parameters to get a slightly different mesh! Cheers, Louis 

May 28, 2010, 16:02 

#29  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

May 29, 2010, 10:18 

#30 
Senior Member

I got it to converge by modifying the mesh on the triSurface file.stl I gave to snappyHexMesh.. Not the best solution but works as a fix
Thx, Louis 

June 15, 2010, 10:27 
MRFSimpleFoam bounding k & epsilon

#31 
Member
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 16 
Hi Foamers,
I have a great problem using MRFSimpleFoam with OF 1.6. I'm studing (fluent Vs OpenFOAM) a 3D fan (mesh imported from GAMBIT) using the kepsilon model and upwind schemes for convective fluxes, the under relaxation factors are 0.3, 0.7, 0.5, 0.5 for pressure, velocity, k and epsilon. After 5600 iterations my OF residuals are very low and the message "bounding epsilon..." is printed very few times but the solution is far from the one obtained by Fluent using UDS. Trying to relaunch OF case from the 5600th iteration I faced the k and epsilon diverging and I haven't changed settings. I'm struggling to know what's going wrong.Can you please help me? Is there anybody who know about bugs in MRFSimpleFoam in OF 1.6? How to let kepsilon converge? Thanks Aldo 

June 15, 2010, 16:10 

#32 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Hi,
we do not have enough details to answer. P.S. Please, when you have a question, open a new thread. Thanks! :)
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 16, 2010, 04:01 

#33  
Member
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 16 
Quote:
Resume: MRFSimpleFoam 1st order upwind> convergence of u, p, k, epsilon untill 5800 iterations> stop and restart> residuals stepup (3 order) and divergence of k and epsilon (under zero) without any change in settings (I thought to get crazy but it's true). MRFSimpleFoam 2nd order upwind> divergence of k and epsilon (under zero), It seem there is not the possibility using other discretization schemes. How to set up a 2nd order disc. scheme without any problem? Is there anybody who know have tested MRFSimpleFoam comparing it to fluent? How arethe resulting fields? Thanks aldo 

June 16, 2010, 10:48 

#34  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Quote:
You might want to try
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

June 16, 2010, 12:15 

#35  
Member
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 16 
Quote:
Sorry, I'm quite new in OF, can you please correct my fvSchemes dict (expecially the laplacian schemes)? __________________________________________________ ______ ddtSchemes { default steadyState; } gradSchemes { default cellLimited Gauss linear 1; grad(p) cellLimited Gauss linear 1; grad(U) cellLimited Gauss linear 1; } divSchemes { default none; div(phi,U) Gauss linearUpwindV cellMDLimited Gauss linear 1; div(phi,k) Gauss linearUpwind cellLimited Gauss linear 1; div(phi,epsilon) Gauss linearUpwind cellLimited Gauss linear 1; div((nuEff*dev(grad(U).T()))) Gauss linearUpwind cellLimited Gauss linear 1;//Gauss linear; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; } __________________________________________________ ___ Thanks 

June 19, 2010, 12:33 
MRF Divergence

#36 
Member
Aldo Iannetti
Join Date: Feb 2010
Posts: 48
Rep Power: 16 
Hi Alberto,
I tried to follow your advices but It diverges after 4000 iter. and I don't understand why, can you please have a look at the attached log and fvSchemes files in order to correct my mistakes? Thanks Aldo 

June 20, 2010, 15:10 

#37 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36 
Are there zones of the system where you can observe some unphysical behaviour (velocity too high, for example?
Additionally, what underrelaxation factors are you using? Did you try to reduce them for k and epsilon? P.S. You wrote you use OpenFOAM 1.6. Did you update it to 1.6.x? Best,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541) OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

February 5, 2014, 12:01 
How can I bound own Scalar value in equations?

#38 
New Member
Mahdi
Join Date: Jul 2013
Posts: 1
Rep Power: 0 
Thanks all for information about bounded schemes
I need a method to bound own volScalarField that is solved in an equation has div , laplacian ,... for example C1 in the concentration equation must be between [0,1] anybody can tell me how can i add this limiter to the equation and force C1 to be in [0,1]? thank you. 

September 21, 2016, 04:31 

#39  
Member
annn
Join Date: Jun 2016
Posts: 40
Rep Power: 10 
Quote:
for example say the bounding value for epsilon is 3 and the calculated was to be 2000, so the bounding epsilon would show up to be 1997? and so in the next iteratio they will use epsilons value as 3 instead of the calculated 2000? 

July 12, 2017, 08:59 
accuracy of simpleFoam  bounding epsilon/k

#40  
New Member
rmz
Join Date: May 2017
Location: Paris
Posts: 12
Rep Power: 9 
Hello,
I am working on a simulation of wind on buildings with a complex Mesh. I am using a RASModel kEspilon with the simpleFoam solver. I am applying ABL conditions (atmospheric boundary layer). I am facing problems with bounding K and bounding epsilon. the problem of bounding k and epsilon is caused by skew faces in my mesh. I searched for schemes that can fix the problem, and found a modification that improved my simulation: changing "laplacianSchemes" from "Gauss linear limited 1" to Gauss linear limited 0.333 changing "snGradSchemes" from "limited 1" to limited 0.333 simpleFoam ran for 800 steps before the "bounding k" / "bounding epsilon" warning appears. the following is an output from the last steps of simpleFoam: Quote:
simpleFoam is stable and converging. my question is: is simpleFoam converging to a correct solution (for p and U)? what is the accuracy of p and U results, does the bounding k and epsilon problem influence the results too much? thank you 

Tags 
bounding error, simplefoam stability 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Bounding epsilon or bounding omega  Stylianos  OpenFOAM  8  February 23, 2018 13:41 
SimpleFoam k and epsilon bounded  nedved  OpenFOAM Running, Solving & CFD  16  March 4, 2017 08:30 
MRFSimpleFOAM goes divergenced!  renyun0511  OpenFOAM Running, Solving & CFD  0  November 19, 2009 02:11 
SimpleFoam k and epsilon bounded  nedved  OpenFOAM Running, Solving & CFD  1  November 25, 2008 20:21 
Bounding epsilon and K with rasInterFoam  openfoam_user  OpenFOAM Running, Solving & CFD  0  October 23, 2008 08:48 