
[Sponsors] 
October 22, 2014, 06:25 
Compressor Simulation using rhoPimpleDyMFoam

#1 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi
I am simulating compressor stage of a turbocharger with the rhoPimpleDyMFoam solver. running moveDynamicMesh checkAMI was smooth without any errors which assures that my mesh rotates properly and i have defined my interfaces correctly , please point out if i am assuming this wrong. However running the solver my simulation crashes showing this Code:
/**\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ Build : 2.3.0f5222ca19ce6 Exec : rhoPimpleDyMFoam Date : Oct 22 2014 Time : 15:58:22 Host : "EATStandalone" PID : 4587 Case : /home/eatin/OpenFOAM/eatin2.3.0/run/tutorials/TurboCharger/Trial_4 nProcs : 1 sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). fileModificationChecking : Monitoring runtime modified files using timeStampMaster allowSystemOperations : Disallowing usersupplied system call operations // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 Selecting dynamicFvMesh solidBodyMotionFvMesh Selecting solidbody motion function rotatingMotion Applying solid body motion to cellZone FLUID_ROTOR PIMPLE: Operating solver in PISO mode Reading thermophysical properties Selecting thermodynamics package { type hePsiThermo; mixture pureMixture; transport sutherland; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } AMI: Creating addressing and weights between 1900 source faces and 32076 target faces AMI: Patch source sum(weights) min/max/average = 0.995594, 1, 0.999764 AMI: Patch target sum(weights) min/max/average = 0.432794, 1, 0.996788 AMI: Creating addressing and weights between 17748 source faces and 5456 target faces AMI: Patch source sum(weights) min/max/average = 0.435302, 1.03344, 1.00009 AMI: Patch target sum(weights) min/max/average = 0.816766, 1.00271, 0.999924 AMI: Creating addressing and weights between 17839 source faces and 1957 target faces AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108 AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992 Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting turbulence model type RASModel Selecting RAS turbulence model kEpsilon #0 Foam::error::printStack(Foam::Ostream&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::compressible::mutkWallFunctionFvPatchScalarField::calcMut() const in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #4 Foam::compressible::mutWallFunctionFvPatchScalarField::updateCoeffs() in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #5 Foam::fvPatchField<double>::evaluate(Foam::UPstream::commsTypes) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" #6 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::evaluate() in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" #7 Foam::compressible::RASModels::kEpsilon::kEpsilon(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #8 Foam::compressible::RASModel::adddictionaryConstructorToTable<Foam::compressible::RASModels::kEpsilon>::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #9 Foam::compressible::RASModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #10 Foam::compressible::turbulenceModel::addturbulenceModelConstructorToTable<Foam::compressible::RASModel>::NewturbulenceModel(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleRASModels.so" #11 Foam::compressible::turbulenceModel::New(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::fluidThermo const&, Foam::word const&) in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/lib/libcompressibleTurbulenceModel.so" #12 in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" #13 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #14 in "/home/eatin/OpenFOAM/OpenFOAM2.3.0/platforms/linux64GccDPOpt/bin/rhoPimpleDyMFoam" Floating point exception (core dumped) Thanks 

October 22, 2014, 06:35 

#2 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Coming to my simulation i have to simulate compressor stage of a turbocharger
Meshing was done using ANSYS ICEM CFD , i had 3 mesh files 1. Inlet&Outlet 2.Volute 3.Rotor I imported them to openfoam using fluent3DMeshToFoam and then used mergeMeshes to make the complete domain, after that used splitMeshRegions makeCellZones overwrite to distinguish between the rotating zone and stationary zone. I am attaching few pictures of the domain so you could get a clear picture.Please have a look at them 

October 22, 2014, 06:38 

#3 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
This is the complete domain of my simulation


October 22, 2014, 07:39 

#4 
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 
1. How are you merging your three meshes that you have imported from fluent?
2. How did you create AMI patches? 3. Do you have 'sets' folder (with several domains) inside the constant folder? 

October 23, 2014, 03:36 

#5 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
@vasava
As i have 3 mesh files 1.I created 3 case folders 1.Rotor 2.Volute 3.Inlet_Outlet 2. Placed the 3 mesh files into corresponding case folders and used fluent3DMeshToFoam fluent.msh scale 0.001 for each to convert to meters 3.merged Rotor and volute , and then merged the combined mesh with Inlet_Outlet 4.used splitMeshRegions makeCellZones overwrite to create cell zones of different regions , 3 in my case To create the AMI patches i used the createPatchDict, I will attach it for your reference Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; object createPatchDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Do a synchronisation of coupled points after creation of any patches. // Note: this does not work with points that are on multiple coupled patches // with transformations (i.e. cyclics). pointSync false; // Patches to create. patches ( { // Master side patch name AMI1; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI2; transform noOrdering; } constructFrom patches; patches (INT_STA_ROT_master); } { // Slave side patch name AMI2; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI1; transform noOrdering; } constructFrom patches; patches (INT_STA_ROT_slave); } { // Master side patch name AMI3; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI4; transform noOrdering; } constructFrom patches; patches (INT_ROT_STA_master); } { // Slave side patch name AMI4; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI3; transform noOrdering; } constructFrom patches; patches (INT_ROT_STA_slave); } { // Master side patch name AMI5; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI6; transform noOrdering; } constructFrom patches; patches (INT_OUTLET_HOUSING_master); } { // Slave side patch name AMI6; patchInfo { type cyclicAMI; matchTolerance 0.0001; neighbourPatch AMI5; transform noOrdering; } constructFrom patches; patches (INT_OUTLET_HOUSING_slave); } ); 

October 23, 2014, 05:50 

#6 
Senior Member

Hi,
Your problem seems to be in the turbulence model, I am guessing you have put epsilon equal to zero somewhere in either a boundary patch or the internalField. Change this to a sensible value for your case. Regards, Tom 

October 23, 2014, 09:01 

#7 
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 
Your mesh setup seems alright. I agree with tomf, get some appropriate values for turbulence and use them in initial condition.
Also can you post your boundary file here? 

October 27, 2014, 01:04 

#8 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi ,
Sorry for the late reply and thanks for your response I have checked my epsilon file and have not put zero anywhere and ya as you have suggested i am working on my initial and boundary conditions as this might be the source of error. @vasava Here is my boundary file Code:
FoamFile { version 2.0; format binary; class polyBoundaryMesh; location "constant/polyMesh"; object boundary; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // 16 ( WALL_HUB { type wall; inGroups 1(wall); nFaces 32413; startFace 16826280; } WALL_BACK_PLATE_ROT { type wall; inGroups 1(wall); nFaces 14330; startFace 16858693; } WALL_SHOURD { type wall; inGroups 1(wall); nFaces 36540; startFace 16873023; } WALL_BLADE { type wall; inGroups 1(wall); nFaces 96768; startFace 16909563; } WALL_HOUSING { type wall; inGroups 1(wall); nFaces 265149; startFace 17006331; } WALL_BACK_PLATE_STA { type wall; inGroups 1(wall); nFaces 39172; startFace 17271480; } WALL_FREESLIP_INLET { type wall; inGroups 1(wall); nFaces 6004; startFace 17310652; } WALL_FREESLIP_OUTLET { type wall; inGroups 1(wall); nFaces 17404; startFace 17316656; } OUTLET { type patch; nFaces 1957; startFace 17334060; } INLET { type patch; nFaces 2945; startFace 17336017; } AMI1 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 1900; startFace 17338962; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI2; } AMI2 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 32076; startFace 17340862; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI1; } AMI3 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 17748; startFace 17372938; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI4; } AMI4 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 5456; startFace 17390686; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI3; } AMI5 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 17839; startFace 17396142; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI6; } AMI6 { type cyclicAMI; inGroups 1(cyclicAMI); nFaces 1957; startFace 17413981; matchTolerance 0.0001; transform noOrdering; neighbourPatch AMI5; } ) // ************************************************************************* // 

October 27, 2014, 01:20 

#9  
Senior Member
Paritosh Vasava
Join Date: Oct 2012
Location: Lappeenranta, Finland
Posts: 732
Rep Power: 22 
Quote:
The boundary file looks ok but did you try any other turbulence setup?? 

October 27, 2014, 01:30 

#10 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi vasava,
Do you mean any of these two? I started with KEpsilon as it was the basic turbulence model to start with. 1.Komega SST 2.SpalartAllmaras I am attaching my 0 folder , please take a look at my initial and boundary conditions and help me correct them. I have copied and modified the files from annularThermalMixer tutorial. 

October 27, 2014, 04:16 

#11 
Senior Member

You have provided a relative pressure of 0 Pa, you should put the absolute pressure. OpenFOAM does not use a "gauge pressure" or similar for compressible solvers. The solver now tried to solve for an absolute vacuum, which it could not do. I guess it only found out when density was required to calculated some part of the turbulence model.
For incompressible cases 0 m2/s2 is allowed since in that case the absolute pressure does not matter. Regards, Tom 

October 27, 2014, 05:02 

#12  
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Quote:
I changed the pressure file as suggested by you creating a pressure difference between inlet and outlet but i still end up getting the same error . Alexeym has suggested this might be the cause of my error: Hi, as you've got FPE in mutkWallFunctionFvPatchScalarField::calcMut(), look at the source of the wall function: Code:
tmp<scalarField> mutkWallFunctionFvPatchScalarField::calcMut() const { const label patchi = patch().index(); const turbulenceModel& turbModel = db().lookupObject<turbulenceModel>("turbulenceModel"); const scalarField& y = turbModel.y()[patchi]; const scalarField& rhow = turbModel.rho().boundaryField()[patchi]; const tmp<volScalarField> tk = turbModel.k(); const volScalarField& k = tk(); const scalarField& muw = turbModel.mu().boundaryField()[patchi]; const scalar Cmu25 = pow025(Cmu_); tmp<scalarField> tmutw(new scalarField(patch().size(), 0.0)); scalarField& mutw = tmutw(); forAll(mutw, faceI) { label faceCellI = patch().faceCells()[faceI]; scalar yPlus = Cmu25*y[faceI]*sqrt(k[faceCellI])/(muw[faceI]/rhow[faceI]); if (yPlus > yPlusLam_) { mutw[faceI] = muw[faceI]*(yPlus*kappa_/log(E_*yPlus)  1); } } return tmutw; } 1. rhow[faceI] == 0 2. muw[faceI] == 0 3. k[faceCellI] < 0 4. E_*yPlus <= 0 (this is not the case, cause yPlus > yPlusLam_) So you need to check if any of conditions 13 is true in your case. I am able to figure out that these conditions come from the equations to have a proper solution but unable to understand which values i should correct.Please explain me if you can interpret what the problem exactly is. Thanks 

October 27, 2014, 05:09 

#13 
Senior Member

Could you just show the p file, I was not talking about a pressure difference between inlet and outlet, I meant that you cannot have 0 Pa anywhere in the domain (internalField or any boundary condition), it should be around your absolute operating pressure (101325 Pa for standard atmosphere conditions).
I guess it should look something like this: Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format binary; class volScalarField; location "0"; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 1 2 0 0 0 0]; internalField uniform 101325; boundaryField { WALL_HUB { type zeroGradient; } OUTLET { type fixedValue; value uniform 101325; } INLET { type zeroGradient; } WALL_BACK_PLATE_ROT { type zeroGradient; } WALL_SHOURD { type zeroGradient; } WALL_BACK_PLATE_STA { type zeroGradient; } WALL_BLADE { type zeroGradient; } WALL_HOUSING { type zeroGradient; } WALL_FREESLIP_INLET { type zeroGradient; } WALL_FREESLIP_OUTLET { type zeroGradient; } AMI1 { type cyclicAMI; value uniform 101325; } AMI2 { type cyclicAMI; value uniform 101325; } AMI3 { type cyclicAMI; value uniform 101325; } AMI4 { type cyclicAMI; value uniform 101325; } AMI5 { type cyclicAMI; value uniform 101325; } AMI6 { type cyclicAMI; value uniform 101325; } } // ************************************************************************* // Tom 

October 27, 2014, 05:31 

#14 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
@tomf,
Thank you very much. Just changed my pfile as suggested by you, now my simulation started running!! I was always worried about the mutfile , dint expect the error was in my pfile. For now the simulation is running but too slow,have to run it in parallel and maybe some changes in my fvSchemes and fvSolution will do. il come back to you in case of any queries, thanks a lot! 

November 6, 2014, 03:02 

#15 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi ,
I am simulating compressor of a turbocharger using rhoPimpleDyMFoam with kOmegaSST turbulence model. Boundary conditons are as follows: mass flow outlet : 0.04 kg/s total pressure inlet:101325 total temperature inlet:298k compressor rpm: 300,000 Can you help me with my FvSchemes and FvSolutions as to what modifications i should be doing for better results. let me know if you need any more details about the simulation. FvSchemes Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSchemes; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss linearUpwind grad(U); div(phi,h) Gauss linearUpwind grad(h); div(phi,K) Gauss linear; div(meshPhi,p) Gauss linear; div(phi,k) Gauss upwind; div(phi,omega) Gauss upwind; div((muEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p ; pcorr ; } // ************************************************************************* // Code:
/** C++ **\  =========    \\ / F ield  OpenFOAM: The Open Source CFD Toolbox   \\ / O peration  Version: 2.3.0   \\ / A nd  Web: www.OpenFOAM.org   \\/ M anipulation   \**/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object fvSolution; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { p { solver GAMG; smoother GaussSeidel; cacheAgglomeration on; agglomerator faceAreaPair; nCellsInCoarsestLevel 10; mergeLevels 1; tolerance 1e6; relTol 0.01; } pFinal { $p; relTol 0; } pcorr { $p; tolerance 1e2; relTol 0; } "(rhoUhkepsilonomega)" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e06; relTol 0.1; } "(rhoUhkepsilonomega)Final" { $U; relTol 0; } } PIMPLE { momentumPredictor yes; transonic no; nOuterCorrectors 1; nCorrectors 3; nNonOrthogonalCorrectors 1; rhoMin rhoMin [ 1 3 0 0 0 ] 0.5; rhoMax rhoMax [ 1 3 0 0 0 ] 2.0; } relaxationFactors { fields { } equations { "(Uhkepsilonomega).*" 1; } } // ************************************************************************* // 

November 6, 2014, 09:24 

#16 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,297
Rep Power: 26 
Whats the matter with your current results? Any problems?
__________________
The skeleton ran out of shampoo in the shower. 

November 6, 2014, 23:00 

#17 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi RodriguezFatz,
I have started running the simulation and each timestep is taking a lot of time. Is there anything to do with my FvSolution or FvSchemes files to speed up my simulation? I am already running it on 8 cores. 

November 7, 2014, 02:33 

#19 
Member
Abhijit
Join Date: Jul 2014
Posts: 75
Rep Power: 11 
Hi tobi,
My simulation has been running from past 1 day and still going on Here is the output Code:
Courant Number mean: 0.000114809 max: 1 deltaT = 1.41799e09 Time = 5.81839e07 solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.81839e07 transformation: ((0 0 0) (0.999958 (0.00913938 0 0))) AMI: Creating addressing and weights between 1900 source faces and 32076 target faces AMI: Patch source sum(weights) min/max/average = 0.99546, 1, 0.999763 AMI: Patch target sum(weights) min/max/average = 0.467982, 1, 0.996805 AMI: Creating addressing and weights between 17748 source faces and 5456 target faces AMI: Patch source sum(weights) min/max/average = 0.538509, 1.06046, 1.00015 AMI: Patch target sum(weights) min/max/average = 0.685009, 1.00305, 0.999864 AMI: Creating addressing and weights between 17839 source faces and 1957 target faces AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108 AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992 GAMG: Solving for pcorr, Initial residual = 1, Final residual = 0.00998453, No Iterations 47 GAMG: Solving for pcorr, Initial residual = 0.0244185, Final residual = 0.00465247, No Iterations 1 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 rhoEqn max/min : 2.15688 0.182153 smoothSolver: Solving for Ux, Initial residual = 3.26172e05, Final residual = 2.14196e09, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.00157835, Final residual = 1.29594e07, No Iterations 1 smoothSolver: Solving for Uz, Initial residual = 0.00176688, Final residual = 1.35932e07, No Iterations 1 smoothSolver: Solving for h, Initial residual = 0.000933756, Final residual = 7.49315e08, No Iterations 1 GAMG: Solving for p, Initial residual = 7.71888e05, Final residual = 3.25475e13, No Iterations 1 GAMG: Solving for p, Initial residual = 1.49854e09, Final residual = 1.49854e09, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.00014808, global = 0.000129601, cumulative = 0.0697627 rho max/min : 2 0.5 GAMG: Solving for p, Initial residual = 1.52653e07, Final residual = 1.52653e07, No Iterations 0 GAMG: Solving for p, Initial residual = 1.52653e07, Final residual = 1.52653e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.000148089, global = 0.000129601, cumulative = 0.0698923 rho max/min : 2 0.5 GAMG: Solving for p, Initial residual = 1.52573e07, Final residual = 1.52573e07, No Iterations 0 GAMG: Solving for p, Initial residual = 1.52573e07, Final residual = 1.52573e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.000148089, global = 0.000129601, cumulative = 0.0700219 rho max/min : 2 0.5 smoothSolver: Solving for omega, Initial residual = 2.31798e06, Final residual = 1.30867e10, No Iterations 1 bounding omega, min: 6301.47 max: 5.70133e+09 average: 2.17771e+06 smoothSolver: Solving for k, Initial residual = 2.69839e05, Final residual = 1.04992e09, No Iterations 1 ExecutionTime = 62085.4 s ClockTime = 83417 s Courant Number mean: 0.000114789 max: 1 deltaT = 1.41799e09 Time = 5.83257e07 solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.83257e07 transformation: ((0 0 0) (0.999958 (0.00916165 0 0))) AMI: Creating addressing and weights between 1900 source faces and 32076 target faces AMI: Patch source sum(weights) min/max/average = 0.995459, 1, 0.999763 AMI: Patch target sum(weights) min/max/average = 0.468157, 1, 0.996805 AMI: Creating addressing and weights between 17748 source faces and 5456 target faces AMI: Patch source sum(weights) min/max/average = 0.537877, 1.06201, 1.00015 AMI: Patch target sum(weights) min/max/average = 0.681757, 1.00303, 0.999863 AMI: Creating addressing and weights between 17839 source faces and 1957 target faces AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108 AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992 GAMG: Solving for pcorr, Initial residual = 1, Final residual = 0.00918253, No Iterations 49 GAMG: Solving for pcorr, Initial residual = 0.0244148, Final residual = 0.00465114, No Iterations 1 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 rhoEqn max/min : 2.15666 0.1872 smoothSolver: Solving for Ux, Initial residual = 3.25967e05, Final residual = 2.1407e09, No Iterations 1 smoothSolver: Solving for Uy, Initial residual = 0.00157519, Final residual = 1.29333e07, No Iterations 1 smoothSolver: Solving for Uz, Initial residual = 0.00176436, Final residual = 1.35799e07, No Iterations 1 smoothSolver: Solving for h, Initial residual = 0.000915801, Final residual = 7.35108e08, No Iterations 1 GAMG: Solving for p, Initial residual = 7.69707e05, Final residual = 3.22893e13, No Iterations 1 GAMG: Solving for p, Initial residual = 1.49221e09, Final residual = 1.49221e09, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.000148538, global = 0.000130024, cumulative = 0.0701519 rho max/min : 2 0.5 GAMG: Solving for p, Initial residual = 1.51827e07, Final residual = 1.51827e07, No Iterations 0 GAMG: Solving for p, Initial residual = 1.51827e07, Final residual = 1.51827e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.000148547, global = 0.000130024, cumulative = 0.0702819 rho max/min : 2 0.5 GAMG: Solving for p, Initial residual = 1.51748e07, Final residual = 1.51748e07, No Iterations 0 GAMG: Solving for p, Initial residual = 1.51748e07, Final residual = 1.51748e07, No Iterations 0 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors : sum local = 0.000148547, global = 0.000130024, cumulative = 0.0704119 rho max/min : 2 0.5 smoothSolver: Solving for omega, Initial residual = 2.31335e06, Final residual = 1.3162e10, No Iterations 1 bounding omega, min: 3196.96 max: 5.70337e+09 average: 2.17777e+06 smoothSolver: Solving for k, Initial residual = 2.69244e05, Final residual = 1.05185e09, No Iterations 1 ExecutionTime = 62226.4 s ClockTime = 83606 s Courant Number mean: 0.000114768 max: 1 deltaT = 1.41798e09 Time = 5.84675e07 solidBodyMotionFunctions::rotatingMotion::transformation(): Time = 5.84675e07 transformation: ((0 0 0) (0.999958 (0.00918393 0 0))) AMI: Creating addressing and weights between 1900 source faces and 32076 target faces AMI: Patch source sum(weights) min/max/average = 0.995457, 1, 0.999763 AMI: Patch target sum(weights) min/max/average = 0.468334, 1, 0.996805 AMI: Creating addressing and weights between 17748 source faces and 5456 target faces AMI: Patch source sum(weights) min/max/average = 0.537262, 1.06316, 1.00015 AMI: Patch target sum(weights) min/max/average = 0.678559, 1.00301, 0.999883 AMI: Creating addressing and weights between 17839 source faces and 1957 target faces AMI: Patch source sum(weights) min/max/average = 0.86998, 1, 0.999108 AMI: Patch target sum(weights) min/max/average = 0.991279, 1, 0.99992 

November 7, 2014, 02:54 

#20 
Super Moderator
Tobias Holzmann
Join Date: Oct 2010
Location: Tussenhausen
Posts: 2,708
Blog Entries: 6
Rep Power: 51 
Hi,
my simulations are running on 40 cores 2 weeks ... But you time step is very small and your density is wrong (I think) Code:
rho max/min : 2 0.5 I dont know what because you do not share many details. You should check out you time steps... maybe your pressure, velocity, k, epsilon are expoding. As I can see, you should use the correct form of the PIMPLE algorithm. Maybe it will be stabilized. Checkout my blog or also available at the wiki.
__________________
Keep foaming, Tobias Holzmann 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Study of the EEqn.H in rhoPimpleDyMFoam.  Horacio Aguerre  OpenFOAM Programming & Development  11  August 19, 2022 02:47 
Developing a rhoPimpleDyMFoam solver  bvieira  OpenFOAM Programming & Development  20  October 9, 2014 12:12 
rhoPimpleDymFoam  jvd.mechanic  OpenFOAM Running, Solving & CFD  0  June 15, 2014 05:20 
Divergence in rhoPimpleDyMFoam  bvieira  OpenFOAM Running, Solving & CFD  1  July 19, 2012 02:22 