
[Sponsors] 
September 11, 2009, 15:48 

#41  
Member
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Quote:
you mean Bcs of sonicFoam case ????? As far as schemes are concerned , i used Minmod perfectly , ,However for rhoCentralFoam im not sure, as it is a completely different ballgame .. 

September 16, 2009, 08:24 

#42  
Member
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 10 
Quote:
It would be very interesting for me to see your 0/p, 0/U, 0/T files, as well as the system/fvSchemes and maybe also the system/fvSolution dictionary. Perhaps, there is something in, I don't already know.
__________________
grid generation: ICEM CFD 13.0 solver: CFX 13.0 

September 16, 2009, 10:41 

#43  
Member
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Quote:
Code:
type waveTransmissive; internalField uniform 1; boundaryField { inlet { type calculated; value uniform 1; } outlet { type calculated; // value uniform 3; } } Code:
boundaryField { inlet { /*type totalPressure; p0 uniform 1.0135e5; U U; phi phi; rho none; psi none; gamma 1.4; */ type fixedValue; value uniform 54000; } outlet { type zeroGradient; /* type waveTransmissive; value uniform 8800; field U; gamma 1.4; phi phi; rho rho; psi psi; lInf 0.01; fieldInf 8800; */ } Code:
internalField uniform 281; boundaryField { inlet { type fixedValue; value uniform 273; } outlet { type zeroGradient; } HTML Code:
[CODE]internalField uniform (260.39 0 0); boundaryField { inlet { type fixedValue; value uniform (380 0 0); } outlet { type inletOutlet; inletValue uniform (10 0 0); value uniform (10 0 0); //type zeroGradient; /*type waveTransmissive; value uniform (10 0 0 ); field U; gamma 1.4; phi phi; rho rho; psi psi; lInf 0.01; fieldInf (10 0 0 ); */ [/CODE] Last edited by mihir1310; September 16, 2009 at 10:58. 

September 16, 2009, 10:55 

#44 
Member
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Code:
solvers { rho diagonal {}; rhoU diagonal {}; rhoE diagonal {}; U smoothSolver { smoother GaussSeidel; nSweeps 2; tolerance 1e09; relTol 0.01; }; h smoothSolver { smoother GaussSeidel; nSweeps 2; tolerance 1e10 relTol 0; }; } Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(tauMC) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; reconstruct(rho) vanLeer; reconstruct(U) vanLeerV; reconstruct(T) vanLeer; } snGradSchemes { default corrected; } 

September 16, 2009, 11:33 

#45 
Member
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 10 
Thanks Mihir!
However, I am a little bit confused, because you said that you use Minmod for the discretization of the divergent terms and backward for the convective terms. By the way, are you simulating a CD nozzle, as well?
__________________
grid generation: ICEM CFD 13.0 solver: CFX 13.0 

September 16, 2009, 11:35 

#46  
Member
Mihir
Join Date: Mar 2009
Posts: 40
Rep Power: 10 
Quote:
heres for sonicFoam Code:
ddtSchemes { default backward; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } divSchemes { default none; div(phi,U) Gauss Minmod; div(phid,p) Gauss Minmod; div(phi,e) Gauss Minmod; } laplacianSchemes { default none; laplacian(mu,U) Gauss linear corrected; laplacian(mu,e) Gauss linear corrected; laplacian((rho*(1A(U))),p) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; 

September 16, 2009, 11:54 

#47 
Member
Julian Krick
Join Date: May 2009
Location: Guelph
Posts: 88
Rep Power: 10 
Okay, thanks. I think I'll try your settings. Let's see what it produce.
By the way: With rhoCentralFoam I noticed that a change of the lInf value (of the waveTransmissive BC) from 0.01, over 0.05, 0.5, 5, 50, 500 and finally 5000 does not have any effect on the result of my simulation. Which is, that the pressure waves are not transmitted across the outlet. Thus, I assume that rhoCentralFoam is (by any reason) not capable to apply the waveTransmissive BC. However, sonicFoam does apply the waveTransmissive BC, and changes of lInf resulted in very different behaviours. Does anyone know, why a certain BC does not work with a certain solver?
__________________
grid generation: ICEM CFD 13.0 solver: CFX 13.0 

April 21, 2010, 05:08 

#48 
Member
Join Date: Apr 2010
Posts: 53
Rep Power: 9 
hi at all!
i read all the comments concerning the growing courant nr. problem because mine is the same i set up a case with the icoFoam solver to achieve a first solution which i can improve later with other solver that display the reality better. i took the controlDict, fvSchemes and fvSolutions from the "icoFoam cavity tutorial". unfortunately not even this simplified calculation works because after round about 8 to 10 time steps the courant nr. is increased to something over e+100 (well i'd say this is a bit more than 1 ) first i tried to decrease the time step to 3.5e6 and change the writeControl to "adjustableRunTime"... but when looked at the runlogs, the timestep didn't change and remained constant. then i tried to limit the courant number with "maxCo 1", but i read that it doesn't work for "icoFoam", because its a simple solver. is this correct? do you have any idea, what i can do to achieve a solution that doesn't abort? 

April 21, 2010, 05:25 

#49 
Member
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 10 
hi bephi,
try to use bounded schemes like "upwind" or a TVDScheme for the divschemes. i think the convective terms produce an unbounded solution so you have to limit them. icofoam solves the NSEqs. I haven't testet this solver but i tested simplefoam and there its nearly the same problem. Joern 

April 21, 2010, 05:52 

#50 
Member
Join Date: Apr 2010
Posts: 53
Rep Power: 9 
hi joern!
thanks a lot for the quick reply! so you say I should change this: Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss linear; // change into "Gauss upwind" } laplacianSchemes { default none; laplacian(nu,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(HbyA) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } would it be okay when the mean value of the conr. is <1 or should the max CoNr <1 as well? if also needed, here are my files: p and U starting files: Code:
dimensions [0 2 2 0 0 0 0]; internalField uniform 0.000000; boundaryField { symmetry { type symmetryPlane; } inlet { type fixedValue; value uniform 452.38; } outlet { type zeroGradient; } dimensions [0 1 1 0 0 0 0]; internalField uniform ( 0.000000 0.000000 1.000000 ); boundaryField { symmetry { type symmetryPlane; } inlet { type fixedValue; value uniform ( 0.000000 0.000000 1.000000 ); } outlet { type zeroGradient; } Code:
application icoFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 1e3; deltaT 3.5e6; writeControl adjustableRunTime; writeInterval 10; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 1.0; Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; } laplacianSchemes { default none; laplacian(nu,U) Gauss linear corrected; laplacian((1A(U)),p) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p; } Code:
solvers { p PCG { preconditioner DIC; tolerance 1e06; relTol 0; }; U PBiCG { preconditioner DILU; tolerance 1e05; relTol 0; }; } PISO { nCorrectors 2; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } Last edited by bephi; April 21, 2010 at 08:16. 

April 21, 2010, 09:16 

#51 
Member
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 10 
the maxconum should not be much larger than 1 because the discretisation of OF ist just semi implicit.
the decoupling in OF causes explicit factors. In my test cases (for my diploma thesis) the solver simplefoam was only stable with maxCoNum<1.5. Try maxCoNum<1. 7 is too much for OF, i think. That would just work with a full implicit solver. Add: If you use "Gauss linear" for all discretisations you get an central that is instable for ALL Delta t. 

April 22, 2010, 00:53 

#52  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
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. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 22, 2010, 00:54 
help

#53 
Member
mohsen kh
Join Date: Nov 2009
Posts: 41
Rep Power: 8 
hi everyone
I have a new solver for twophase modeling. but there is a problem while running any case (dam break for instance). when in ControlDict I put the write interval one second the solution diverge quickly but if I put it .05 second the solution converges. I could not understand how the write interval affects the convergence of the system. please help as soon as possible 

April 22, 2010, 00:59 

#54  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
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. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 22, 2010, 01:02 

#55  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
Please open a new thread, and provide more information to increase the chances someone can help. 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. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

April 22, 2010, 01:58 

#56  
Member
Join Date: Apr 2010
Posts: 53
Rep Power: 9 
Quote:
you are right that it doesn't make sense to fix pressure and velocity at the inlet! i changed it but now my max. CoNo is increasing again to around about 7... is this a problem? greets! Last edited by bephi; April 22, 2010 at 02:22. 

April 22, 2010, 03:38 

#57  
Member
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 10 
Quote:
@bephi: a maxconum of 7 is now problem as long as your solution is ok ^^ take a look at the results (paraview) if they look physical ok. or try to calculate a bit longer to look if the solver stays stable. have you tried smaller timesteps to see if the maxconum stays smaller? 

April 22, 2010, 05:31 

#58 
Member
Join Date: Apr 2010
Posts: 53
Rep Power: 9 
hi!
at the moment my problem is the following: i calculated a time step of 3.5e6 s because my highest velocity is 26.83 m/s² and the smalest element lenght is 0.0001m the fluid needs round about 0.3 to 0.5 s to flow through the model so it would take 100000 steps which is too much in my in opinion.. so i increased the timestep to 0.0003 and after that to 0.00003 but then the conumber increases again until the calculation crashes... i didn't thought that a simple laminar calculation would be so difficult?! 

April 22, 2010, 08:30 

#59 
Member
Joern Bader
Join Date: Mar 2009
Posts: 33
Rep Power: 10 
if it takes to many steps, try a coarser mesh.
but if your mesh is too fine you need smaller timesteps, thats normal. are you sure about your max. velocity? i dont know the eigenvalues of the NSeqs but for the eulerequations the max. velocity isnt just the max. u, its max.(u+c) with the speed of sound c. my tip: try smaller timesteps, you will see if the solver stays stable. btw: how many cells does your testcase have? 

April 22, 2010, 08:48 

#60 
Member
Join Date: Apr 2010
Posts: 53
Rep Power: 9 
now a calculation with 100 timesteps was successful...i think i'll set up 100 additional steps and look what happens...
when do i know that the solution is converged? my model has 116112 trias, 622697 tetras and 198870 pentas 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
How to get the Global Node Number by UDF : Fluent  Yusuke  FLUENT  1  October 23, 2015 10:55 
CFL number  Daniele  CFX  5  July 19, 2012 19:11 
Number of interation?  Tu  Phoenics  1  September 28, 2008 14:12 
SOS! HELP! max number of cells :(  Jas  Phoenics  4  February 14, 2004 11:12 
Boundary region number limitation  Pablo Barreiro  Siemens  1  May 2, 2001 11:13 