
[Sponsors] 
November 22, 2014, 20:44 
Problem with boundary conditions (heatTransfer)

#1 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
Hi there,
i'm new at this forum and also realtively new to OpenFoam. So here is my Problem: I want to solve a HeatTransfer problem, i want to examine the cooling of a cylinder in a wind tunnel. I have a .stl file of the cylinder and my wind tunnel is a hexagon made in the blockMeshdict. I used snappyHexMesh for the .stl file. Now i have the boundaries of the wind tunnel with the walls and the inlet and outlet as well as the boundaries windtunnel_to_cylinder and cylinder_to_windtunnel. First of all i only want to look at the cooling, without any turbulence models, so i set the turbulence to off. My Problem now is by using the chtMultiRegionFoam solver, that the temperature of the cylinder isn't changing. I think, that i don't set the boundary conditions for the temperature right. So here are the initial value files for the temperature of the wind tunnel and the cylinder. Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // //Cylinder dimensions [ 0 0 0 1 0 0 0 ]; internalField uniform 500; boundaryField { cylinder_to_windtunnel { type fixedValue; value uniform 500; } } // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // //Windtunnel dimensions [ 0 0 0 1 0 0 0 ]; internalField uniform 300; boundaryField { "(inletupperWalllowerWallfrontWallbackWall)" { type fixedValue; value uniform 300; } windtunnel_to_cylinder { type fixedValue; value uniform 300; } outlet { type zeroGradient: } } // ************************************************************************* // greetings Wirman 

November 24, 2014, 03:46 

#2 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
Hi,
you should make a sketch of your setup where you show all boundaries with their names. What means windtunnel_to_cylinder and cylinder_to_windtunnel? So there is a cylinder inside your wind tunnel, and cool air flows around that cylinder? Do you resolve the solid body (cylinder) with a mesh and solve for heat conduction in the solid? From what I can guess with the few information: Yes, your boundary conditions seem to be wrong. You have two general possibilities: 1) Fix the temperature at the surface. This means that the simulation can not change the temperature because it is a boundary condition for all time. Even with the highest cooling it will not change. This is what I think what happens here, because your cylinder seems to have a fixed temperature boundary condition. But: The heat flux inside / outside the cylinder can change. This is the temperature gradient at the surface. 2) Fix the gradient of the temperature. If you set the heat flux to zero that means, that your body will heat (or cool) until it gets the temperature of the surrounding fluid.
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 05:53 

#3 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
Hi,
thanks for your response. Sorry for being a bit vague, so here are some explanations. As an attachement i made a little image of my model in 2D, front and back Walls are the 3Dcase and the cylinder doesn't touches the front and the back wall (so it is complete in the wind tunnel, without touching any walls) In the .stl file of the cylinder i have only one region, named cylinder_to_windtunnel (so the points in the .stl file are all boundary points of the cylinder)  i think it could be a problem that there are no inner nodes?!?  this .stl file will be meshed with snappyHexMesh out of the blockMesh from the wind tunnel. I made the same with the wind tunnel to set up the wind tunnel without the cylinder. So i have the following boundaries in the polyMesh folders of Windtunnel and Cylinder: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // boundary Windtunnel 7 ( inlet { type patch; nFaces 100; startFace 207208; } outlet { type patch; nFaces 100; startFace 207308; } lowerWall { type wall; inGroups 1(wall); nFaces 200; startFace 207408; } upperWall { type wall; inGroups 1(wall); nFaces 200; startFace 207608; } frontWall { type wall; inGroups 1(wall); nFaces 224; startFace 207808; } backWall { type wall; inGroups 1(wall); nFaces 224; startFace 208032; } windtunnel_to_cylinder { type wall; inGroups 1(wall); nFaces 15625; startFace 208256; sampleMode nearestPatchFace; sampleRegion cylinder; samplePatch cylinder_to_windtunnel; } ) // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // boundary cylinder 1 ( cylinder_to_windtunnel { type wall; inGroups 1(wall); nFaces 15856; startFace 63660; sampleMode nearestPatchFace; sampleRegion windtunnel; samplePatch windtunnel_to_cylinder; } ) // ************************************************************************* // I see the point with the fixed Value, so i tried to change the boundary conditions to fixedGradient. So my new 0/cylinder/T file is the following: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [ 0 0 0 1 0 0 0 ]; internalField uniform 500; boundaryField { cylinder_to_windtunnel { type fixedGradient; gradient uniform 0; } } // ************************************************************************* // So here is a snapshot what chtMultiRegionFoam does: Code:
Solving for fluid region windtunnel diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.1691079, Final residual = 7.164976e08, No Iterations 28 DILUPBiCG: Solving for Uy, Initial residual = 0.1495004, Final residual = 5.141199e08, No Iterations 28 DILUPBiCG: Solving for Uz, Initial residual = 0.1496348, Final residual = 1.371065e08, No Iterations 30 DILUPBiCG: Solving for h, Initial residual = 0.1502954, Final residual = 5.238185e08, No Iterations 29 Min/max T:44.85127 776.2719 GAMG: Solving for p_rgh, Initial residual = 0.06935177, Final residual = 0.0003099182, No Iterations 5 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 7.980175e05, global = 2.0367e05, cumulative = 0.0003824869 GAMG: Solving for p_rgh, Initial residual = 0.06477691, Final residual = 6.725581e08, No Iterations 14 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 8.454755e09, global = 2.64765e09, cumulative = 0.0003824843 Solving for solid region cylinder DICPCG: Solving for h, Initial residual = 0.004598652, Final residual = 7.893509e07, No Iterations 2 Min/max T:min(T) [0 0 0 1 0 0 0] 500 max(T) [0 0 0 1 0 0 0] 500 ExecutionTime = 58.22 s ClockTime = 60 s Region: windtunnel Courant Number mean: 0.3687364 max: 8187.881 Region: cylinder Diffusion Number mean: 9.508806e05 max: 0.0002090919 Time = 0.83 i hope you have now enough information. Thanks for your effort. greetings Wirman 

November 24, 2014, 08:45 

#4 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
I don't know the details of that solver, but the log output sounds like you have the region "windtunnel" where the fluid flows and the region "cylinder" which is solid inside the cylinder. Is that correct?
PS: Wohoooo, this is my 1000th post.
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 09:20 

#5 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
yes that is correct.
i tried something that i found in the planeWall2D case, which is an example for the chtMultiRegionFoam solver. i set the boundaries windtunnel_to_cylinder and cylinder_to_windtunnel to mappedWall instead of wall and then i used for the 0 files: Code:
boundaryField { cylinder_to_windtunnel { type compressible::turbulentTemperatureCoupledBaffleMixed; Tnbr T; kappa solidThermo; kappaName none; value uniform 500; } } Code:
boundaryField { windtunnel_to_cylinder { type compressible::turbulentTemperatureCoupledBaffleMixed; Tnbr T; kappa fluidThermo; kappaName none; value uniform 300; } } here is the log of chtMultiRegionFoam Code:
Solving for fluid region windtunnel diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.02460263, Final residual = 3.736507e08, No Iterations 12 DILUPBiCG: Solving for Uy, Initial residual = 0.03327333, Final residual = 1.240097e08, No Iterations 14 DILUPBiCG: Solving for Uz, Initial residual = 0.3112729, Final residual = 8.590666e08, No Iterations 15 DILUPBiCG: Solving for h, Initial residual = 0.003709023, Final residual = 9.252748e08, No Iterations 12 Min/max T:76.66537 499.9691 GAMG: Solving for p_rgh, Initial residual = 0.6060488, Final residual = 0.004652162, No Iterations 4 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 1.789022e05, global = 1.050344e05, cumulative = 0.0001039832 GAMG: Solving for p_rgh, Initial residual = 0.1844631, Final residual = 4.072585e08, No Iterations 14 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 2.188366e10, global = 1.318627e10, cumulative = 0.0001039833 Solving for solid region cylinder DICPCG: Solving for h, Initial residual = 0.3283636, Final residual = 1.500188e08, No Iterations 4 Min/max T:min(T) [0 0 0 1 0 0 0] 499.6061 max(T) [0 0 0 1 0 0 0] 499.9998 ExecutionTime = 2.91 s ClockTime = 4 s Region: windtunnel Courant Number mean: 0.2657095 max: 21.11159 Region: cylinder Diffusion Number mean: 9.508806e05 max: 0.0002090919 Time = 0.03 

November 24, 2014, 09:30 

#6 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
Ok, again: I never used that solver, but you need a coupled boundary condition for this fluid / solid intersection. This sounds familiar and makes sense. Glad it works now.
The other problem sounds like a numerical failure. Some questions: 1) Is this a transient solver? 2) Can you post more than one time step log output? 3) Can you post fvSchemes and fvSolution?
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 09:55 

#7 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
sure i can ;)
1.) chtMultiRegionFoam is a transient solver, the steadystate version is the chtMultiRegionSimpleFoam. 2. ) Here is the complete log of the solver. Unfortunately it terminates after 3 time steps: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create fluid mesh for region windtunnel for time = 0 Create solid mesh for region cylinder for time = 0 *** Reading fluid mesh thermophysical properties for region windtunnel Adding to thermoFluid Selecting thermodynamics package { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } Adding to rhoFluid Adding to UFluid Adding to phiFluid Adding to gFluid Adding turbulence Selecting turbulence model type laminar Adding to ghFluid Adding to ghfFluid Selecting radiationModel none Adding to KFluid Adding to dpdtFluid Adding fvOptions No finite volume options present *** Reading solid mesh thermophysical properties for region cylinder Adding to thermos Selecting thermodynamics package { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } Adding to radiations Selecting radiationModel none Adding fvOptions No finite volume options present Region: windtunnel Courant Number mean: 0.1320233 max: 6.178983 Region: cylinder Diffusion Number mean: 4.754403e05 max: 0.0001045459 Region: windtunnel Courant Number mean: 0.1320233 max: 6.178983 Region: cylinder Diffusion Number mean: 4.754403e05 max: 0.0001045459 Time = 0.005 Solving for fluid region windtunnel diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 1.70178e08, No Iterations 10 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 4.406888e08, No Iterations 8 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 7.053572e08, No Iterations 8 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 4.709673e08, No Iterations 13 Min/max T:300 499.9901 GAMG: Solving for p_rgh, Initial residual = 0.9248417, Final residual = 0.002323891, No Iterations 2 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 4.026599e05, global = 2.333879e05, cumulative = 2.333879e05 GAMG: Solving for p_rgh, Initial residual = 0.5507993, Final residual = 5.446465e08, No Iterations 13 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 8.541335e11, global = 4.909502e11, cumulative = 2.333874e05 Solving for solid region cylinder DICPCG: Solving for h, Initial residual = 1, Final residual = 1.22016e07, No Iterations 3 Min/max T:min(T) [0 0 0 1 0 0 0] 499.8234 max(T) [0 0 0 1 0 0 0] 500 ExecutionTime = 1.78 s ClockTime = 2 s Region: windtunnel Courant Number mean: 0.1322938 max: 11.29372 Region: cylinder Diffusion Number mean: 4.754403e05 max: 0.0001045459 Time = 0.01 Solving for fluid region windtunnel diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.1074785, Final residual = 1.815122e08, No Iterations 11 DILUPBiCG: Solving for Uy, Initial residual = 0.022709, Final residual = 8.128951e08, No Iterations 8 DILUPBiCG: Solving for Uz, Initial residual = 0.2808652, Final residual = 1.207978e08, No Iterations 11 DILUPBiCG: Solving for h, Initial residual = 0.002674789, Final residual = 1.18252e08, No Iterations 9 Min/max T:86.33847 499.9713 GAMG: Solving for p_rgh, Initial residual = 0.2937693, Final residual = 0.001758145, No Iterations 4 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 2.432616e06, global = 7.712725e07, cumulative = 2.256746e05 GAMG: Solving for p_rgh, Initial residual = 0.1388996, Final residual = 6.941843e08, No Iterations 13 diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 time step continuity errors (windtunnel): sum local = 8.460298e11, global = 4.874945e11, cumulative = 2.256751e05 Solving for solid region cylinder DICPCG: Solving for h, Initial residual = 0.307672, Final residual = 3.77194e08, No Iterations 3 Min/max T:min(T) [0 0 0 1 0 0 0] 499.6128 max(T) [0 0 0 1 0 0 0] 500.0002 ExecutionTime = 2.76 s ClockTime = 3 s Region: windtunnel Courant Number mean: 0.1322697 max: 8.331021 Region: cylinder Diffusion Number mean: 4.754403e05 max: 0.0001045459 Time = 0.015 Solving for fluid region windtunnel diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0 DILUPBiCG: Solving for Ux, Initial residual = 0.02061106, Final residual = 9.475351e08, No Iterations 12 DILUPBiCG: Solving for Uy, Initial residual = 0.02154275, Final residual = 5.186294e08, No Iterations 10 DILUPBiCG: Solving for Uz, Initial residual = 0.1588295, Final residual = 3.479565e08, No Iterations 13 DILUPBiCG: Solving for h, Initial residual = 0.002320682, Final residual = 7.601028e08, No Iterations 10 Min/max T:64.83592 499.9816 #0 Foam::error::printStack(Foam::Ostream&) in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #1 Foam::sigFpe::sigHandler(int) in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #2 in "/lib/x86_64linuxgnu/libc.so.6" #3 Foam::GAMGSolver::scale(Foam::Field<double>&, Foam::Field<double>&, Foam::lduMatrix const&, Foam::FieldField<Foam::Field, double> const&, Foam::UPtrList<Foam::lduInterfaceField const> const&, Foam::Field<double> const&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #4 Foam::GAMGSolver::Vcycle(Foam::PtrList<Foam::lduMatrix::smoother> const&, Foam::Field<double>&, Foam::Field<double> const&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::Field<double>&, Foam::PtrList<Foam::Field<double> >&, Foam::PtrList<Foam::Field<double> >&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #5 Foam::GAMGSolver::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libOpenFOAM.so" #6 Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/lib/libfiniteVolume.so" #7 Foam::fvMatrix<double>::solve(Foam::dictionary const&) in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam" #8 in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam" #9 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" #10 in "/soft/OpenFOAM/OpenFOAM2.3.x/platforms/linux64GccDPOpt/bin/chtMultiRegionFoam" Floating exception fvSchemes windtunnel Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) Gauss upwind; div(phi,K) Gauss linear; div(phi,h) Gauss upwind; div(phi,k) Gauss upwind; div(phi,epsilon) Gauss upwind; div(phi,R) Gauss upwind; div(R) Gauss linear; div((muEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; p_rgh; } // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { "(rhorhoFinal)" { solver PCG preconditioner DIC; tolerance 1e7; relTol 0; } p_rgh { solver GAMG; tolerance 1e7; relTol 0.01; smoother GaussSeidel; cacheAgglomeration true; nCellsInCoarsestLevel 10; agglomerator faceAreaPair; mergeLevels 1; } p_rghFinal { $p_rgh; tolerance 1e7; relTol 0; } "(UhkepsilonR)" { solver PBiCG; preconditioner DILU; tolerance 1e7; relTol 0.1; } "(UhkepsilonR)Final" { $U; tolerance 1e07; relTol 0; } } PIMPLE { momentumPredictor on; nCorrectors 2; nNonOrthogonalCorrectors 0; } relaxationFactors { fields { } equations { "h.*" 1; "U.*" 1; } } // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; } laplacianSchemes { default none; laplacian(alpha,h) Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } fluxRequired { default no; } // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // solvers { h { solver PCG; preconditioner DIC; tolerance 1e06; relTol 0.1; } hFinal { $h; tolerance 1e06; relTol 0; } } PIMPLE { nNonOrthogonalCorrectors 0; } // ************************************************************************* // 

November 24, 2014, 10:04 

#8 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
Ok, tell me if you don't get me. The fluid solver part is something like PIMPLE. Currently you run PIMPLE in PISO mode, because you did not set nOuterCorrectors to anything higher than "1" (actually, you didn't set it at all, thus I see from your log it is set to "1").
Now, your max. Courant number is much too high for the PISO solver. Normally, this leads to numerical instabilities. I recommend to make the time step 20 times smaller, so the max. Co becomes about "0.5". See what happens.
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 10:32 

#9 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
i think i can follow you, but i haven't dealt with the theory behind the solvers. Are there any manuals of the theory behind e.g. the chtMultiRegionFoam?
To your suggestion: There is another fvSolution file in the system ordner and there the nOuterCorrectors is set to 1. 1 or lower is PISO Mode, what are other numbers? When i make the time steps about 100 times smaller the Courant number looks good (<0.5, beetween something about 0.04 at the beginning and 0.3 at the end where it terminates) but it terminates nevertheless at a t about 0.0004. Moreover the change in temperature in the solid is very small, but that is maybe because of the short time. But the heavily decrease of the temperature in the fluid is still there... 

November 24, 2014, 10:38 

#10 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
Your "min" value in the fluid should not become less than 300, is that what you say?
Try setting laplacian scheme to "uncorrected". Sometimes this can lead to negative wiggles.
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 10:54 

#11 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
yep, thats what im saying ... there is a fixed temperature of 300 at the inlet and the cylinder has a temperature of 500, so why should the minimum temperature be under 300? Correct me if i overlook something ...
Setting the laplacian schemes to uncorrected doesn't help 

November 24, 2014, 11:02 

#12 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
What does "checkMesh" show you?
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 11:10 

#13 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
checkMesh gives me an FOAM FATAL ERROR:
Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh for time = 0 > FOAM FATAL ERROR: Cannot find file "points" in directory "polyMesh" in times 0 down to constant From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&) in file db/Time/findInstance.C at line 203. FOAM exiting Code:
 constant  windtunnel  polyMesh  cylinder  polyMesh 

November 24, 2014, 11:50 

#14 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
I don't know how to use checkMesh for these kind of meshes, sorry.
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 11:57 

#15 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
any other ideas? i thought it is actually a primitive case, so it can't be that difficult to make the solver run correctly i really dislike openFoam maybe im too stupid to use it ...


November 24, 2014, 12:02 

#16 
Senior Member
Philipp
Join Date: Jun 2011
Location: Germany
Posts: 1,118
Rep Power: 16 
Don't give up that fast...
You need to spot the points where the temperature goes down in paraview. The numerics seem to be ok, so maybe it's some boundary condition error. Whatever, finding it will probably help. Edit: And you need to get checkMesh running...
__________________
The skeleton ran out of shampoo in the shower. 

November 24, 2014, 15:12 

#17  
Member
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 5 
Quote:
the other thing worth looking into is how you set your thermophysicalProperties for your fluid/solid regions. 

November 26, 2014, 13:17 

#18 
New Member
Join Date: Nov 2014
Posts: 10
Rep Power: 2 
okay, so new try:
first of all i got checkMesh running with the region option (thanks to zhengzh5) it says that the mesh is ok, but i don't know exactly what it does, so here are the log files: checkMesh cylinder: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh cylinder for time = 0 Time = 0 Mesh stats points: 33596 faces: 79516 internal faces: 63660 cells: 23292 faces per cell: 6.147003 boundary patches: 1 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 21416 prisms: 424 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 1452 Breakdown of polyhedra by number of faces: faces number of cells 4 40 5 344 6 372 9 268 12 212 15 132 18 84 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology cylinder_to_windtunnel 15856 16354 ok (closed singly connected) Checking geometry... Overall domain bounding box (0.124999 0 0.124315) (0.124999 0.01 0.124315) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (2.007952e18 9.761436e16 1.672787e18) OK. Max cell openness = 2.747404e16 OK. Max aspect ratio = 4.733498 OK. Minimum face area = 9.65406e07. Maximum face area = 1.294591e05. Face area magnitudes OK. Min volume = 8.679143e10. Max volume = 4.122625e08. Total volume = 0.0004866705. Cell volumes OK.: Mesh nonorthogonality Max: 37.56666 average: 7.999011 Nonorthogonality check OK. Face pyramids OK. Max skewness = 1.115269 OK. Coupled point location match (average 0) OK. Mesh OK. End Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create polyMesh windtunnel for time = 0 Time = 0 Mesh stats points: 90587 faces: 223881 internal faces: 207208 cells: 66936 faces per cell: 6.440316 boundary patches: 7 point zones: 0 face zones: 0 cell zones: 0 Overall number of cells of each type: hexahedra: 54757 prisms: 724 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 0 polyhedra: 11455 Breakdown of polyhedra by number of faces: faces number of cells 5 376 6 3004 9 6523 12 1000 15 540 18 12 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology inlet 100 121 ok (nonclosed singly connected) outlet 100 121 ok (nonclosed singly connected) lowerWall 200 231 ok (nonclosed singly connected) upperWall 200 231 ok (nonclosed singly connected) frontWall 224 261 ok (nonclosed singly connected) backWall 224 261 ok (nonclosed singly connected) windtunnel_to_cylinder 15625 16119 ok (closed singly connected) Checking geometry... Overall domain bounding box (0.5 0.25 0.25) (0.5 0.25 0.25) Mesh (nonempty, nonwedge) directions (1 1 1) Mesh (nonempty) directions (1 1 1) Boundary openness (3.994897e17 3.968973e17 1.058756e16) OK. Max cell openness = 2.883646e16 OK. Max aspect ratio = 3.224365 OK. Minimum face area = 1.049937e06. Maximum face area = 0.002505055. Face area magnitudes OK. Min volume = 1.671137e09. Max volume = 0.000125249. Total volume = 0.2495132. Cell volumes OK. Mesh nonorthogonality Max: 41.73929 average: 11.41158 Nonorthogonality check OK. Face pyramids OK. Max skewness = 1.23016 OK. Coupled point location match (average 0) OK. Mesh OK. End thermophysicalProperties windtunnel (air) Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType { type heRhoThermo; mixture pureMixture; transport const; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } mixture { specie { nMoles 1; molWeight 28.96; } transport { mu 1.8e05; Pr 0.7; } thermodynamics { Hf 2.544e+06; Cp 1004.5; } } // ************************************************************************* // Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // thermoType { type heSolidThermo; mixture pureMixture; transport constIso; thermo hConst; equationOfState rhoConst; specie specie; energy sensibleEnthalpy; } mixture { specie { nMoles 1; molWeight 12; } transport { kappa 80; } thermodynamics { Hf 0; Cp 450; } equationOfState { rho 8000; } } // ************************************************************************* // 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Overflow Error in Multiphase Modelling with Two Continuous Fluids  ashtonJ  CFX  6  August 11, 2014 14:32 
Boundary Conditions problem  o_mars_2010  Main CFD Forum  2  July 8, 2013 02:10 
Problem with pressure boundary conditions  GunGur  OpenFOAM Running, Solving & CFD  0  June 20, 2013 21:31 
An error has occurred in cfx5solve:  volo87  CFX  5  June 14, 2013 17:44 
Problem with periodic boundary conditions  jm_ngs  FLUENT  7  April 27, 2012 02:32 