
[Sponsors] 
Bigger wave height leads to crash (interFoam) 

LinkBack  Thread Tools  Search this Thread  Display Modes 
May 13, 2011, 11:35 
Bigger wave height leads to crash (interFoam)

#1 
Member
David GISEN
Join Date: Jul 2009
Location: Germany
Posts: 56
Rep Power: 12 
Hey Foamers,
currently I am using groovyBC to simulate Airy waves in a channel with interFoam. For a small wave height (H=0.1m, T=2s > L=4,74m) everything works fine. But when I try to change to bigger waves (H=0.22m, T=3s > L=7,68m) my case crashes after 3.48 s. The stunning part is, that the residuals look quite good until this point and it crashes all out of a sudden. I guess that my schemes and solution settings are responsible for this behavior, and ask you kindly, to provide me with some tips for improving those settings. The residual plots are: And the settings are: controldict Code:
adjustTimeStep yes; maxCo 0.6; maxAlphaCo 0.6; maxDeltaT 0.01; Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(p) Gauss linear; grad(U) Gauss linear; } //V=Vectorfield divSchemes { div(rho*phi,U) Gauss limitedLinearV 1.0; div(phi,alpha) Gauss vanLeer; div(phirb,alpha) Gauss interfaceCompression; div(phi,k) Gauss linear; div(phi,omega) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } /* corrected: unbounded, 2. order, conservative uncorrected: bounded, 1. order, nonconservative limited 0.5: blend corrected, uncorrected */ interpolationSchemes { default linear; //interpolate(U) linear; } snGradSchemes { default corrected; } fluxRequired { default no; p_rgh; pcorr; alpha1; } Code:
solvers { pcorr { solver PCG; preconditioner { preconditioner GAMG; tolerance 1e05; relTol 0; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 2; nBottomSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e06; relTol 0; maxIter 100; } p_rgh { solver PCG; preconditioner { preconditioner GAMG; tolerance 1e05; relTol 0; smoother DICGaussSeidel; nPreSweeps 0; nPostSweeps 2; nBottomSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e06; relTol 0; maxIter 100; } p_rghFinal { solver PCG; preconditioner { preconditioner GAMG; tolerance 1e06; relTol 0; nVcycles 2; smoother DICGaussSeidel; nPreSweeps 2; nPostSweeps 2; nFinestSweeps 2; cacheAgglomeration true; nCellsInCoarsestLevel 20; agglomerator faceAreaPair; mergeLevels 1; } tolerance 1e06; relTol 0; maxIter 100; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e06; relTol 0; nSweeps 1; } k { solver PBiCG; preconditioner DILU; tolerance 1e06; relTol 0; } omega { solver PBiCG; preconditioner DILU; tolerance 1e06; relTol 0; } } PISO { momentumPredictor no; nCorrectors 3; nNonOrthogonalCorrectors 0; // nonorthogonality Max < 70: 0, otherwise 12, max. 3 nAlphaCorr 1; nAlphaSubCycles 3; // # subcycles, 2: 2x half lengh time step within each actual time step cAlpha 1.0; // 0: no compression, 1: conservative compression, >1: enhanced compression } David 

May 19, 2011, 10:33 

#2 
Member
David GISEN
Join Date: Jul 2009
Location: Germany
Posts: 56
Rep Power: 12 
For the record: The crash was due to a poorly set inlet boundary condition.
But nevertheless, it would be interesting to know what's the difference between pcorr, p_rgh and p_rghFinal. Does somebody know that? Thanks in advance, David 

November 7, 2011, 02:29 

#3 
Member
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 76
Blog Entries: 1
Rep Power: 11 
Hi David,
I am also using groovyBC to generate waves. The simulation crashed at a certain point when high wave height or 3D wave tank were tried. The simulation for low wave height and 2D can run smoothly. I suspect I am facing the same problem as you did. Can you please post here the solution to your problem? Many thanks. Kind regards, Albert 

November 7, 2011, 03:00 

#4 
Senior Member
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,379
Rep Power: 25 
pCorr is a single correction done before the start of the time loop to improve the initial value of the pressure field. p_rgh refers to the pressure solution excluding the final correction, and p_rghFinal to the previously excluded final correction. It is beneficial for computational performance to solve p_rgh with a lower tolerance than p_rghFinal.


November 7, 2011, 05:12 

#5  
Member
David GISEN
Join Date: Jul 2009
Location: Germany
Posts: 56
Rep Power: 12 
Quote:
as far as I remember, it was a typo in the inlet BC. Recheck it with the sources, e.g. USACE CEM. Another tip is to translate the function by pi/2. By doing this, you start with a neutral water level and not with a crest or through at the inlet. Regards, David edit: thanks @ anton 

November 8, 2011, 05:10 

#6 
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 726
Rep Power: 17 
It doesn't look like it was the problem in this case, but in general a lot of the crashes in interFoam are caused by collapsing air pockets which, due to the large density differences, can drive the velocity to increase very rapidly. To address this you can instead use the "compressible" interFoam solver or put an explicit limiter on the air side velocity magnitude.


November 14, 2011, 02:53 

#7 
Member
Albert Tong
Join Date: Dec 2010
Location: Perth, WA, Australia
Posts: 76
Blog Entries: 1
Rep Power: 11 
Hi Eugene,
I saw a treatment suggested by Eric Paterson to ignore the convective term on airside by changing Ueqn to Code:
fvVectorMatrix UEqn ( fvm::ddt(rho, U) + gamma*fvm::div(rhoPhi, U) // change occurs here  fvm::laplacian(muf, U, "laplacian(mut,U)")  (fvc::grad(U) & fvc::grad(muf)) ); Can you please explain how to "use the compressible interFoam" and especially how to "put an explicit limiter on the air side" to address this problem? Or please give some references. Kind regards, Albert Edit: Thanks, David. 

Tags 
fvschemes, fvsolution, interfoam, waves 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
alpha becomes bigger than 1 in interFoam  ata  OpenFOAM  1  March 21, 2020 14:49 
How to generate waves of particular wave height...please help  nims  FLUENT  0  September 21, 2010 02:48 
Latest git 1.6.x: Crash when using inletOutlet for variable alpha1 in interFoam  carsten  OpenFOAM Bugs  6  September 23, 2009 09:46 
How to know the wave height at one point  Nicolas  FLOW3D  2  March 31, 2009 20:08 
WAVE HEIGHT AND FORCE  WARITH  Siemens  1  March 21, 2004 12:43 