
[Sponsors] 
July 12, 2010, 13:31 

#21 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
This one should work and run.
__________________
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. 

July 12, 2010, 22:01 

#22  
Member
Maolong LIU
Join Date: Apr 2010
Location: USA
Posts: 31
Rep Power: 9 
This is the p_rgh file now I use
//================================================== ============== FoamFile { version 2.0; format ascii; root ""; case ""; instance ""; local ""; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 1 2 0 0 0 0]; internalField uniform 0; boundaryField { bottomInlet { type zeroGradient; } topInlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } pipe { type zeroGradient; } defaultFaces { type empty; } } // ************************************************** *********************** // Take care of the object name is "p_rgh", not "p", and also the dimension is different to simpleFoam. Quote:


July 13, 2010, 10:33 
p_rgh

#23 
New Member
victor
Join Date: Jul 2010
Posts: 5
Rep Power: 9 
The last file itīs OK.
I' m actually using p_rgh for a wave tank in interFoam. I used your case to update the wave tank files where I found the p_rgh missing. Thanks for your help Victor 

August 2, 2010, 11:01 

#24 
New Member
Join Date: Jul 2010
Posts: 11
Rep Power: 9 
Hi, I'm also having the same problem trying to extract "twoStream.tar.gz". Would someone be willing to post a working version for v1.7 or as Victor requested provide some additional detail on how to fix the error "p_rgh at line 0"?
Thanks in advance! 

August 2, 2010, 11:06 

#25 
Member
Maolong LIU
Join Date: Apr 2010
Location: USA
Posts: 31
Rep Power: 9 
Try this
//================================================== ============== FoamFile { version 2.0; format ascii; root ""; case ""; instance ""; local ""; class volScalarField; object p_rgh; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 1 2 0 0 0 0]; internalField uniform 0; boundaryField { bottomInlet { type zeroGradient; } topInlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } pipe { type zeroGradient; } defaultFaces { type empty; } } 

August 2, 2010, 20:53 

#26 
New Member
Join Date: Jul 2010
Posts: 11
Rep Power: 9 
Thanks Maolong LIU!
When I use the your suggestion I get the following ======================= DILUPBiCG: Solving for alpha1, Initial residual = 0.00755434, Final residual = 2.4898e08, No Iterations 2 Phase 1 volume fraction = 0.501191 Min(alpha1) = 0 Max(alpha1) = 1 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 2.74871e12, No Iterations 3 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 9.82467e12, No Iterations 3 > FOAM FATAL IO ERROR: keyword p_rgh is undefined in dictionary "/home/hunts/Desktop/twoStream/system/fvSolution::solvers" file: /home/hunts/Desktop/twoStream/system/fvSolution::solvers from line 22 to line 73. From function dictionary::subDict(const word& keyword) const in file db/dictionary/dictionary.C at line 456. FOAM exiting ======================= Any ideas? My apologies. I'm relatively new to OpenFOAM. Thanks 

August 2, 2010, 21:14 

#27  
Member
Maolong LIU
Join Date: Apr 2010
Location: USA
Posts: 31
Rep Power: 9 
In the fvSoluction file, and also fvSchems file, because now you solve p_rgh equation in stead of p equation, so you need change p to p_rgh.
So just change all the word "p" to "p_rgh" in both those files. Quote:


August 2, 2010, 21:20 

#28  
Member
Maolong LIU
Join Date: Apr 2010
Location: USA
Posts: 31
Rep Power: 9 
This is my fvSolution file
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 1.6   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p_rgh { solver PCG; preconditioner DIC; tolerance 1e8; relTol 0; } p_rghFinal { solver PCG; preconditioner DIC; tolerance 1e8; relTol 0; } alpha1 { solver PBiCG; preconditioner DILU; tolerance 1e06; relTol 0; } U { solver PBiCG; preconditioner DILU; tolerance 1e08; relTol 0; } UFinal { solver PBiCG; preconditioner DILU; tolerance 1e08; relTol 0; } } PIMPLE { nOuterCorrectors 2; nCorrectors 2; nNonOrthogonalCorrectors 0; pRefCell 0; pRefValue 0; } Quote:


August 3, 2010, 01:09 

#29 
New Member
Join Date: Jul 2010
Posts: 11
Rep Power: 9 
Thank you!


December 10, 2010, 12:51 

#30 
Senior Member
Balkrishna Patankar
Join Date: Mar 2009
Location: Pune
Posts: 123
Rep Power: 10 
what does alphatab stand for ?


January 10, 2011, 13:15 

#31 
New Member
mehdoo
Join Date: Dec 2010
Posts: 3
Rep Power: 8 

January 25, 2011, 07:46 

#33 
New Member
Brendan Sloan
Join Date: Mar 2009
Posts: 24
Rep Power: 10 

January 25, 2011, 08:34 

#34 
Member
Maolong LIU
Join Date: Apr 2010
Location: USA
Posts: 31
Rep Power: 9 

January 25, 2011, 08:36 

#35 
New Member
Brendan Sloan
Join Date: Mar 2009
Posts: 24
Rep Power: 10 

January 25, 2011, 10:57 

#36 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,911
Rep Power: 28 
FYI, it is written in the code (createFields.H)
Code:
// Read the reciprocal of the turbulent Schmidt number dimensionedScalar alphatab(twoPhaseProperties.lookup("alphatab"));
__________________
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. 

July 8, 2011, 04:49 

#37 
New Member
Tanay Deshpande
Join Date: Aug 2010
Posts: 20
Rep Power: 9 
I'm trying to write a separate case for using twoLiquidMixingFoam in a customized form. First, I removed the variables 'p' and 'g' and 'gh' and instead operated everything in 'p_rgh'. Next, I removed 'alphatab' and now the diffusivity works solely on Dab.
In pEqn.H { volScalarField rAU = 1.0/UEqn.A(); surfaceScalarField rAUf = fvc::interpolate(rAU); U = rAU*UEqn.H(); surfaceScalarField phiU ( "phiU", (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rAU, rho, U, phi) ); adjustPhi(phiU, U, p_rgh); phi = phiU ;// ghf*fvc::snGrad(rho)*rAUf*mesh.magSf() for(int nonOrth=0; nonOrth<=nNonOrthCorr; nonOrth++) { fvScalarMatrix p_rghEqn ( fvm::laplacian(rAUf, p_rgh) == fvc::div(phi) ); p_rghEqn.setReference(pRefCell, getRefCellValue(p_rgh, pRefCell)); p_rghEqn.solve ( mesh.solver ( p_rgh.select ( finalIter && corr == nCorr1 && nonOrth == nNonOrthCorr ) ) ); if (nonOrth == nNonOrthCorr) { phi = p_rghEqn.flux(); } } U += rAU*fvc::reconstruct((phi  phiU)/rAUf); U.correctBoundaryConditions(); #include "continuityErrs.H" The problem is in the line fvm::laplacian(rAUf, p_rgh) == fvc::div(phi) And the output reads > FOAM FATAL IO ERROR: keyword laplacian(interpolate((1A(U))),p_rgh) is undefined in dictionary "/home/tanay/OpenFOAM/tanay1.7.1/run/roughMix/system/fvSchemes::laplacianSchemes" file: /home/tanay/OpenFOAM/tanay1.7.1/run/roughMix/system/fvSchemes::laplacianSchemes from line 54 to line 63. So, I tried adding this line to fvSchemes but it didn't work. Any suggestions on what's missing in fvSchemes? Here's the fvSchemes file if anyone wishes to view it ddtSchemes { default Euler; } gradSchemes { default Gauss linear; grad(U) Gauss linear; grad(muEff) Gauss linear; grad(p_rgh) Gauss linear; } snGradSchemes { default corrected; } divSchemes { default none; div(phi,U) Gauss limitedLinearV 1; div(phi,k) Gauss limitedLinear 1; div(phi,epsilon) Gauss limitedLinear 1; div(phi,R) Gauss limitedLinear 1; div(R) Gauss linear; div(phi,nuTilda) Gauss limitedLinear 1; div((nuEff*dev(grad(U).T()))) Gauss linear; div(phi,alpha1) Gauss limitedLinear 1; div(phi) Gauss limitedLinear 1; div(rhoPhi,U) Gauss limitedLinear 1; div(rho*phi,U) Gauss limitedLinear 1; } laplacianSchemes { default none; laplacian(nuEff,U) Gauss linear corrected; laplacian((1A(U)),p_rgh) Gauss linear corrected; laplacian(DkEff,k) Gauss linear corrected; laplacian(DepsilonEff,epsilon) Gauss linear corrected; laplacian(DREff,R) Gauss linear corrected; laplacian(DnuTildaEff,nuTilda) Gauss linear corrected; laplacian(Dab,alpha1) Gauss linear corrected; laplacian(rAUf,p_rgh) Gauss linear corrected; laplacian(muEff,U) Gauss linear corrected; } interpolationSchemes { default linear; interpolate(U) linear; } fluxRequired { default no; p_rgh ; alpha1 yes; } 

July 10, 2011, 12:03 

#38 
Senior Member
Mieszko Młody
Join Date: Mar 2009
Location: POLAND, USA
Posts: 142
Rep Power: 10 
Hi Tanay,
I think that you can have a problem with an extra "bracket". An error says: laplacian(interpolate((1A(U))),p_rgh) so here u have : ...U)))  triple closing ) but in your laplacianSchemes you have : .... laplacian((1A(U)),p_rgh) Gauss linear corrected; .... and: A(U)) double closing ) so it seems that you have some typo in your code. Cheers ZMM 

July 11, 2011, 02:14 

#39 
New Member
Tanay Deshpande
Join Date: Aug 2010
Posts: 20
Rep Power: 9 
Yeah, thanks. That was a simple typo. Now, I'm getting a Courant number blowup.
Courant Number mean: 21.0277 max: 258.938 deltaT = 3.37996e06 Time = 0.0145817 #0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #1 Foam::sigFpe::sigFpeHandler(int) in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #2 Uninterpreted: #3 Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #4 Foam::GAMGSolver::solveCoarsestLevel(Foam::Field<d ouble>&, Foam::Field<double> const&) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #5 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMa trix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #6 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/opt/openfoam171/lib/linuxGccDPOpt/libOpenFOAM.so" #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/opt/openfoam171/lib/linuxGccDPOpt/libfiniteVolume.so" #8 in "/home/tanay/OpenFOAM/tanay1.7.1/applications/bin/linuxGccDPOpt/customizedTwoLiquidMixingFoam" #9 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6" #10 in "/home/tanay/OpenFOAM/tanay1.7.1/applications/bin/linuxGccDPOpt/customizedTwoLiquidMixingFoam" Floating point exception Lowering the time step just prolongs the blowup. All the fvSchemes (printed above) I've used correspond to a pimpleFoam tutorial and so they can't be too problematic. Where may be the error? 

July 15, 2011, 02:01 

#40 
New Member
Tanay Deshpande
Join Date: Aug 2010
Posts: 20
Rep Power: 9 
Well, ziemowit, I've given up trying to make the blowing up case converge since I tried everything from reducing the time step to decreasing the velocity and increasing laminar viscosity etc. So, now I'm trying to build a new solver based on PIMPLE to simulate twoLiquidMixing. In this, I've included a file called customTwoLiquid.H for laminar mixing. It reads as
surfaceScalarField muEff ("muEff", (alpha1*mu1 + (scalar(1)alpha1)*mu2)); volScalarField rho ("rho", (alpha1*rho1 + (scalar(1)alpha1)*rho2)); surfaceScalarField rhoIntoPhi ("rhoIntoPhi", rho*phi); Now this produces a compilation error. Can you please tell me what's wrong? 

Thread Tools  
Display Modes  

