
[Sponsors] 
reactingTwoPhaseEulerFoam  stability of subcooled boiling simulation 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 27, 2018, 09:21 
reactingTwoPhaseEulerFoam  stability of subcooled boiling simulation

#1 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Dear Foamers,
I have a problem with computational stability of boiling case with reactingTwoPhaseEulerFoam. It diverges and floating point error occurs. Description: I would like to simulate subcooled boiling of water on the attached geometry. Preferably to simulate all heat transfer stages (vapour blanket, nucleate boiling, natural convection). Current case: Heat transfer is from the patch called solid_wall. The temperature of the wall is elevated highly beyond the saturation temperature of water at given pressure (Currently constant temperature, no all heat transfer stages needs to be currently observed). Fluid domain is a cylinder tank full of water with outlet on the top (patch called fluid_top). The fluid is not agitated. The geometry is modelled as wedge (axisymmetric). At the outlet, reverse flow of the liquid phase is allowed. Due to nature of the problem, one can expect abrupt changes and so stability issues. The case setup is based on the tutorial $FOAM_TUTORIAL/multiphase/reactingTwoPhaseFlow/RAS/wallBoiling. The main differences are that no inlet is present in my case and very high temperature of the heated wall is used. Computational Attempts:
controDict Code:
application reactingTwoPhaseEulerFoam; startFrom latestTime; startTime 0; stopAt endTime; endTime 40; deltaT 1e7; writeControl adjustableRunTime; writeInterval 0.002; purgeWrite 0; writeFormat ascii; writePrecision 9; writeCompression uncompressed; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 0.01; maxDeltaT 0.0001; Code:
ddtSchemes { default Euler; } gradSchemes { default Gauss linear; } divSchemes { default none; "div\(phi,alpha.*\)" Gauss vanLeer; "div\(phir,alpha.*\)" Gauss vanLeer; "div\(alphaRhoPhi.*,U.*\)" Gauss limitedLinearV 1; "div\(phi.*,U.*\)" Gauss limitedLinearV 1; "div\(alphaRhoPhi.*,Yi\)" Gauss limitedLinear 1; "div\(alphaRhoPhi.*,(he).*\)" Gauss limitedLinear 1; "div\(alphaRhoPhi.*,K.*\)" Gauss limitedLinear 1; "div\(alphaPhi.*,p\)" Gauss limitedLinear 1; "div\(alphaRhoPhi.*,(kepsilon).*\)" Gauss upwind; "div\(phim,(kepsilon)m\)" Gauss upwind; "div\(\(\(\(alpha.*\*thermo:rho.*\)\*nuEff.*\)\*dev2\(T\(grad\(U.*\)\)\)\)\)" Gauss linear; } laplacianSchemes { default Gauss linear uncorrected; } interpolationSchemes { default linear; } snGradSchemes { default uncorrected; } fluxRequired { default no; } wallDist { method meshWave; nRequired yes; } Code:
solvers { "alpha.*" { nAlphaCorr 1; nAlphaSubCycles 3; } p_rgh { solver GAMG; smoother DIC; tolerance 1e8; relTol 0.01; maxIter 100; minIter 2; } p_rghFinal { $p_rgh; relTol 0; } "U.*" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e6; relTol 0; minIter 1; } "(eh).*" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e12; relTol 0.001; minIter 1; maxIter 20; } "(kepsilonTheta).*" { solver smoothSolver; smoother symGaussSeidel; tolerance 1e8; relTol 0; minIter 1; } Yi { solver smoothSolver; smoother symGaussSeidel; tolerance 1e6; relTol 0; minIter 1; residualAlpha 1e8; } } PIMPLE { momnetumPredictor yes; nOuterCorrectors 250; nCorrectors 2; nNonOrthogonalCorrectors 0; nEnergyCorrectors 2; faceMomentum yes; residualControl { p_rgh { relTol 0; tolerance 1e4; } } } relaxationFactors { fields { iDmdt 0.1; p_rgh 0.1; p_rghFinal 0.6; } equations { ".*" 1; "h.*" 0.1; "U.*k.*epsilon.*alpha.*" 0.1; } } Code:
type thermalPhaseChangeTwoPhaseSystem; phases (gas liquid); volatile "water"; massTransfer on; gas { type multiComponentPhaseModel; diameterModel isothermal; constantCoeffs { d 0.00045; } isothermalCoeffs { d0 0.00045; p0 1e5; } Sc 0.7; residualAlpha 1e4; } liquid { type multiComponentPhaseModel; diameterModel constant; constantCoeffs { d 0.00045; } Sc 0.7; residualAlpha 1e4; } blending { default { type linear; continuousPhase liquid; minFullyContinuousAlpha.gas 0.7; minPartlyContinuousAlpha.gas 0.5; minFullyContinuousAlpha.liquid 0.7; minPartlyContinuousAlpha.liquid 0.5; } heatTransfer { type linear; continuousPhase liquid; minFullyContinuousAlpha.gas 1; minPartlyContinuousAlpha.gas 0; minFullyContinuousAlpha.liquid 1; minPartlyContinuousAlpha.liquid 0; } massTransfer { type linear; continuousPhase liquid; minFullyContinuousAlpha.gas 1; minPartlyContinuousAlpha.gas 0; minFullyContinuousAlpha.liquid 1; minPartlyContinuousAlpha.liquid 0; } } surfaceTension ( (gas and liquid) { type constant; sigma 0.07; } ); saturationModel { type polynomial; C<8> ( 308.0422 0.0015096 1.61589e8 1.114106e13 4.52216e19 1.05192e24 1.2953e30 6.5365e37 ); }; aspectRatio ( (gas in liquid) { type constant; E0 1.0; } (liquid in gas) { type constant; E0 1.0; } ); drag ( (gas in liquid) { type SchillerNaumann; residualRe 1e3; swarmCorrection { type none; } } (liquid in gas) { type SchillerNaumann; residualRe 1e3; swarmCorrection { type none; } } ); virtualMass ( (gas in liquid) { type constantCoefficient; Cvm 0.5; } (liquid in gas) { type constantCoefficient; Cvm 0.5; } ); interfaceComposition (); heatTransfer.gas ( (gas in liquid) { type spherical; residualAlpha 1e3; } (liquid in gas) { type RanzMarshall; residualAlpha 1e3; } ); heatTransfer.liquid ( (gas in liquid) { type RanzMarshall; residualAlpha 1e3; } (liquid in gas) { type spherical; residualAlpha 1e3; } ); massTransfer.gas (); massTransfer.liquid (); lift (); wallLubrication ( (gas in liquid) { type Antal; Cw1 0.01; Cw2 0.05; Cwc 10.0; Cwd 6.8; p 1.7; } ); turbulentDispersion ( (gas in liquid) { type Burns; sigma 0.7; Ctd 1.0; residualAlpha 1e3; } ); // Minimum allowable pressure pMin 10000; Code:
thermoType { type heRhoThermo; mixture multiComponentMixture; transport const; thermo hRefConst; equationOfState perfectGas; specie specie; energy sensibleEnthalpy; } dpdt yes; species ( water ); inertSpecie water; /* chemistryReader foamChemistryReader; */ /* foamChemistryFile "$FOAM_CASE/constant/reactions.gas"; */ water { specie { molWeight 18.0153; } equationOfState { rho 1; } thermodynamics { Hf 0; Cp 12078.4; Tref 373.55; Href 2675500; } transport { mu 1.2256e5; Pr 2.289; } } Code:
thermoType { type heRhoThermo; mixture multiComponentMixture; transport const; thermo hRefConst; equationOfState perfectFluid; specie specie; energy sensibleEnthalpy; } dpdt yes; species ( water ); inertSpecie water; "(mixtureH2Owater)" { specie { molWeight 18.0153; } equationOfState { R 3000; rho0 959; rho 959; } thermodynamics { Hf 0; Cp 4195; Tref 373.55; Href 417500; } transport { mu 2.8291e4; Pr 2.289; } } Code:
dimensions [1 1 2 0 0 0 0]; internalField uniform 100000; boundaryField { fluid_bottom { type fixedFluxPressure; } fluid_top { type prghTotalPressure; U U.liquid; p0 uniform 100000; value uniform 100000; } tank_wall { type fixedFluxPressure; } solid_wall { type fixedFluxPressure; } right { type wedge; } left { type wedge; } } Code:
gas min/max T 307.702909  2016.44048 liquid min/max T 359.969529  2389.91521 Tf.gasAndLiquid: min = 359.983643, mean = 367.376591, max = 403.907099 iDmdt.gasAndLiquid: min = 2137.69475, mean = 92.2414632, max = 2.62873604e23, integral = 0.000462413491 wDmdt.gasAndLiquid: min = 0, mean = 1.94094026, max = 22.9273172, integral = 2.7677863e07 dmdt.gasAndLiquid: min = 2114.76743, mean = 90.300523, max = 2.62873604e23, integral = 0.000462136713 smoothSolver: Solving for h.gas, Initial residual = 0.000705340909, Final residual = 1.52402318e13, No Iterations 1 smoothSolver: Solving for h.liquid, Initial residual = 0.0354795666, Final residual = 9.77502319e18, No Iterations 1 gas min/max T 307.726027  1868.00206 liquid min/max T 359.969529  2538.90673 Tf.gasAndLiquid: min = 359.983643, mean = 367.376596, max = 403.907099 iDmdt.gasAndLiquid: min = 2167.11375, mean = 92.7952508, max = 2.63187519e23, integral = 0.000411679688 wDmdt.gasAndLiquid: min = 0, mean = 1.94114191, max = 22.9373728, integral = 2.76781142e07 dmdt.gasAndLiquid: min = 2144.17637, mean = 90.8541089, max = 2.63187519e23, integral = 0.000411402907 GAMG: Solving for p_rgh, Initial residual = 0.232598235, Final residual = 7.74806493e17, No Iterations 2 GAMG: Solving for p_rgh, Initial residual = 0.246949424, Final residual = 1.06193819e16, No Iterations 2 PIMPLE: iteration 2 MULES: Solving for alpha.gas MULES: Solving for alpha.gas MULES: Solving for alpha.gas alpha.gas volume fraction = 0.000147084939 Min(alpha1) = 5.96787709e101 Max(alpha1) = 0.247168508 Constructing face momentum equations smoothSolver: Solving for h.gas, Initial residual = 0.668877348, Final residual = 7.52677685e06, No Iterations 2 smoothSolver: Solving for h.liquid, Initial residual = 0.0363311226, Final residual = 1.12267408e17, No Iterations 1 gas min/max T 10269.4458  2197.07427 liquid min/max T 359.969529  2702.79741 [6] #0 Foam::error::printStack(Foam::Ostream&)Tf.gasAndLiquid: min = 359.983642, mean = 367.375326, max = 403.881676 at ??:? [6] #1 Foam::sigFpe::sigHandler(int) at ??:? [6] #2 ? in "/lib/x86_64linuxgnu/libc.so.6" [6] #3 Foam::sqrt(Foam::Field<double>&, Foam::UList<double> const&) at ??:? [6] #4 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam::sqrt<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > const&) at ??:? [6] #5 Foam::heatTransferModels::RanzMarshall::K(double) const at ??:? [6] #6 Foam::BlendedInterfacialModel<Foam::heatTransferModel>::K(double) const at ??:? [6] #7 Foam::ThermalPhaseChangePhaseSystem<Foam::MomentumTransferPhaseSystem<Foam::twoPhaseSystem> >::correctThermo() at ??:? [6] #8 ? at ??:? [6] #9 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [6] #10 ? at ??:? [MAEROWRK:25098] *** Process received signal *** [MAEROWRK:25098] Signal: Floating point exception (8) [MAEROWRK:25098] Signal code: (6) [MAEROWRK:25098] Failing at address: 0x3e80000620a [MAEROWRK:25098] [ 0] /lib/x86_64linuxgnu/libc.so.6(+0x354b0)[0x7f3cc8e714b0] [MAEROWRK:25098] [ 1] /lib/x86_64linuxgnu/libc.so.6(gsignal+0x38)[0x7f3cc8e71428] [MAEROWRK:25098] [ 2] /lib/x86_64linuxgnu/libc.so.6(+0x354b0)[0x7f3cc8e714b0] [MAEROWRK:25098] [ 3] /home/robin/OpenFOAM/OpenFOAM5.0/platforms/linux64GccDPInt32Opt/lib/libOpenFOAM.so(_ZN4Foam4sqrtERNS_5FieldIdEERKNS_5UListIdEE+0x28)[0x7f3cca329f58] [MAEROWRK:25098] [ 4] /home/robin/OpenFOAM/OpenFOAM5.0/platforms/linux64GccDPInt32Opt/lib/libreactingTwoPhaseSystem.so(_ZN4Foam4sqrtINS_12fvPatchFieldENS_7volMeshEEENS_3tmpINS_14GeometricFieldIdT_T0_EEEERKS8_+0x10a)[0x7f3cce32d20a] [MAEROWRK:25098] [ 5] /home/robin/OpenFOAM/OpenFOAM5.0/platforms/linux64GccDPInt32Opt/lib/libreactingEulerianInterfacialModels.so(_ZNK4Foam18heatTransferModels12RanzMarshall1KEd+0x7d)[0x7f3ccdf79a2d] [MAEROWRK:25098] [ 6] /home/robin/OpenFOAM/OpenFOAM5.0/platforms/linux64GccDPInt32Opt/lib/libreactingTwoPhaseSystem.so(_ZNK4Foam23BlendedInterfacialModelINS_17heatTransferModelEE1KEd+0x410)[0x7f3cce393fa0] [MAEROWRK:25098] [ 7] /home/robin/OpenFOAM/OpenFOAM5.0/platforms/linux64GccDPInt32Opt/lib/libreactingTwoPhaseSystem.so(_ZN4Foam29ThermalPhaseChangePhaseSystemINS_27MomentumTransferPhaseSystemINS_14twoPhaseSystemEEEE13correctThermoEv+0xa0e)[0x7f3cce394ebe] [MAEROWRK:25098] [ 8] reactingTwoPhaseEulerFoam[0x436585] [MAEROWRK:25098] [ 9] /lib/x86_64linuxgnu/libc.so.6(__libc_start_main+0xf0)[0x7f3cc8e5c830] [MAEROWRK:25098] [10] reactingTwoPhaseEulerFoam[0x44bb69] [MAEROWRK:25098] *** End of error message ***  mpirun noticed that process rank 6 with PID 25098 on node MAEROWRK exited on signal 8 (Floating point exception).  I enclose part of the case and a few pictures. Any recommendation/suggestion is welcomed. Thanks, Robin 

June 28, 2018, 20:27 

#2 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hi Robin,
I am not very familiar with this solver, but I have two questions: (1) Can the reactingTwoPhaseEulerFoam simulate the subcooled boiling flow? Because I have seen many guys developed their own solvers based on twoPhaseEulerFoam to simulate this kind of problems. (2) Have you analysize the source code of the reactingTwoPhaseEulerFoam to figure out the models implemented in the solver? Do the models suitable for your simulation? Best regards, Qinhao 

June 29, 2018, 11:43 

#3 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinh,
Firstly, thank you for the reply. Despite it should be done earlier, I have been going through the source code just now. I will understand soon its capabilities much better. Certainly, I have been reading phd of Henrik Rusche and paper from Chalmers university called "Description of reactingTwoPhaseEulerFoam solver with a focus on mass transfer modelling terms". I am going to have a look further for boiling with twoPhaseEulerFoam. Cheers, Robin 

July 6, 2018, 08:46 

#4 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
Have you simulated subcooled boiling successfully using reactingTwoPhaseEulerFoam or other Foam? I hope you can give some hints on solving the same problems. Best regards, Qinhao 

July 8, 2018, 16:43 

#5 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
well, I have been able to run subcooled boiling with reactingTwoPhaseEulerFoam. However, I have not done any qualitative assessment. Moreover, I still make some changes to adequatly simulate exact case. Do you want some general hints or discuss your case? Cheers, Robin 

July 8, 2018, 21:25 

#6 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I have tried to use reactingTwoPhaseEulerFoam to simulate subcooled boiling flow under 4.5MPa, just like the experiment conducted by Bartolomej for subcooled boiling heat transfer to water (CFD modelling of subcooled boiling—Concept, validation and application to fuel assembly design). However, the temperature and the pressure increases above the prescribed saturation values and no vapour is formed. I think it may due to the thermal physical properties. For example, in the tutorial wallBoiling/constant/thermophysicalProperties.liquid, the Pr of water is 2.289, but it should be 1.75. I don't know how to set them. Do you have some hints? Thanks a lot! Best regards, Qinhao 

July 9, 2018, 05:03 

#7 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
just a quick question. Have you changed the saturationModel in constant/phaseProperties? The polynom in wallBoiling tutorial does not seem to be valid approximately above 0.5 MPa. My case is at atmospheric pressure. I will have a further look later. Best regards, Robin 

July 9, 2018, 06:57 

#8 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hi Robin,
Yes, the unphysical simulation results may due to the improper saturation model settings. But how to modify it to fit different pressure？ I have not find relevent statement about the model. Beat regards, Qinhao 

July 9, 2018, 09:35 

#9 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
if you use as saturationModel the polynomial one then it is defined as Code:
Polynomial equation for the saturation vapour temperature in terms of the vapour pressure (in Pa). T_sat = sum_i C_i*p^i where p is the pressure in Pa and C are the coefficients. I have just calculated a few values and found out that the polynom given in wallBoiling tutorial gives nonsense for the pressure above 0.5 MPa. You can either make other polynom in the pressure range you need or have a look on other models provided in OF. Let me know how it goes. Best regards, Robin 

July 10, 2018, 02:40 

#10 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hi Robin,
You are right, I have found that the default polynomial is suitable for pressure between 5000 Pa to 0.14 MPa. I fit a new fomula for pressure between 2.3MPa to 7.4MPa, and the simulation result for a 4.5MPa seems resonable. Additionally, I still puzzled about the therma dynamics in the constant/thermalphysicalProperties, what do the Href mean? The Tref may mean the satruation temperature. The figure shows the fitting formula: https://www.dropbox.com/s/ijvyr1qlbzeuznm/fit.tif?dl=0 and https://www.dropbox.com/s/5m5j5pla6b...omial.tif?dl=0 Best regards, Qinhao Last edited by Qinh; July 10, 2018 at 05:35. 

July 10, 2018, 12:42 

#11 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
for having a look at Hf, Cp, Tref, Href it is necessary to have a look at definition of thermoType dictionary an for options of thermo and equationOfState. In the case of wallBoiling/constant/thermophysicalProperties.gas
In hRefConstThermoI.H can be see: Hf is equal to Hc. Hc is chemical enthalpy. Href and Tref are values used to calculate Ha and Hs. Ha is Absolute enthalpy and Hs is Sensible enthalpy. Ha: Code:
return Cp_*(TTref_) + Href_ + Hf_ + EquationOfState::H(p, T); Code:
return Cp_*(TTref_) + Href_ + EquationOfState::H(p, T); H(p. T) is zero because we use EquationOfState perfectGas viz. perfectGasI.H The code mean that Ha=Hs for our case. Also, if current temperature T is equal to Tref, Hs = Hf = Href. Overall, the values Cp, Tref, Href must correspond same state of specie. According to ThermalPhaseChangePhaseSystem.C the saturation temperature is taken from saturationModel (not the value Tref. in thermophysicalProperties) as could be expected. Hence the values of Tref and Href in thermophysicalProperties do not have to be defined at the saturation point. Cheers, Robin 

July 11, 2018, 22:02 

#12  
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I have a silly question. Quote:
Best regards, Qinhao 

July 12, 2018, 06:34 

#13 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I learned that Tref is the saturation temperature at the system pressure. Href is the enthalpy at Tref and system pressure. They all can be referred in the lookup table. Best regards, Qinhao 

July 12, 2018, 09:19 

#14 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
yes, you are right. You can get those values from any thermodynamic property table. Only to clarify, as I have already mentioned, the data do not have to be necessarily for saturation point. However, it is sensible to define state point at which you compute (the setup mentioned previously means that cp is constant), hence the saturation point for you. Cheers, Robin 

July 13, 2018, 06:50 

#15 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I have a another question, and I hope you can give me some hints. The code will easily crash when I simulate a 3D case, so I have to simulate a simplfied 2D case  transfer the pipe to a wedge type geometry. I tied to create a wedge using ICEM. However, the angle between the faces is suggested to be no more than 5 degrees, which will lead to a mesh of low quality. How to solve the problem? Or how did you create your geometry at the very beginning? Thank you in advance! Best regards, Qinhao 

July 14, 2018, 13:01 

#16 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
I have also started my computation with wedge geometry. However, I switched to simplified 3D geometry. I have not got a problem with the mesh quality. In the case of wedge BC, some level of cell skewness is inevitable. Surely, you should keep it as low as possible. Keep the mesh quality high, as usually you would do, especially in the plane your mesh is straddling. To be honest, I do not know how the wedge BC treat the third direction. I have read somewhere that the skewness is not a big issue in this case (for the direction perpendicular to the coordinate plane your mesh is straddling). Overall, if you are not able to make the mesh better in the third direction, carry on in the computation and just be aware of it. If you find some new information in this topic let me know or somebody else might add some note. Anyway, have you run checkMesh utility and it has given you some warning? Cheers, Robin 

July 14, 2018, 21:15 

#17 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I create the mesh of the wedge by using ICEM, and the quality is as shown in the attached figure. https://www.dropbox.com/s/tv9g2mnnpv...ality.JPG?dl=0 I think the quality is low. Fortunately, there is no warning when I run checkMesh. So it seems that the mesh can be adopted in the simulation. Best regards, Qinhao 

July 15, 2018, 15:16 

#18 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
I was not able to load the dropBox page. Anyway, if the checkMesh shows you Mesh OK, than go ahead. Surelly, the checkMesh ok does not automatically mean that the mesh is perfect. According to your nonortagonality value you might want to setup nNonOrthogonalCorrectors. Cheers, Robin 

July 15, 2018, 20:32 

#19 
New Member
Richard
Join Date: Apr 2018
Posts: 24
Rep Power: 6 
Hello Robin,
I'm sorry about the link, and the website is attached again. https://www.dropbox.com/s/tv9g2mnnpv...ality.JPG?dl=0 Just as you said, I set the nNonOrthogonalCorrectors as 2, and the calculation seems reasonable. Best regards, Qinhao 

July 18, 2018, 14:45 

#20 
Member
Robin Kamenicky
Join Date: Mar 2016
Posts: 74
Rep Power: 10 
Hi Qinhao,
from the little I know about your case, it is difficult to judge the mesh but at the first glance it looks fine. Cheers, Robin 

Tags 
boiling, multiphase flow, reactingtwophaseeulerfoam, stability 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Fluent simulation subcooled boiling at low pressure  cscfx  Fluent Multiphase  1  August 9, 2017 20:54 
Twophase Eulerian model for nucleate subcooled boiling  Edy  OpenFOAM  5  February 11, 2017 16:21 
Wall boiling  subcooled boiling  kskong  CFX  2  March 9, 2011 20:02 
nucleate boiling simulation in CFX  Anil  CFX  3  August 25, 2010 14:18 
Boiling simulation using Fluent  Jake Lee  FLUENT  0  February 10, 2005 02:09 