 |
 |
 |
|
|
|
[Sponsors] | ||||
Divergent temperature in chtMultiRegion(Simple)Foam |
 |
|
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 29, 2014, 04:43
|
Divergent temperature in chtMultiRegion(Simple)Foam
|
#1 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12  |
Hi,
first of all a summary of my installed software: Ubuntu 13.10 OpenFOAM 2.2.2 ParaView 3.12.0 enGrid 1.4.0 What I would like to achieve is a set up capable of assessing both heat transfer (conduction, convection and radiation) and flow in a rather complex structure. In best case a 3D steady state model as well as a 3D transient model will be achieved. Starting from both the tutorial cases 'multiRegionHeater' for the transient and steady state version of the chtMultiRegion-solver, I'm in the process of adapting the set up to my own needs, but useing a plane wall (and neglecting radiation) in order to link results to analytical solutions in a first step. By doing that I face the issue that my temperatures do not converge and causes the solver to stop with the following error: Code:
[2] --> FOAM FATAL ERROR: [2] Maximum number of iterations exceeded [2] [2] From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const [3] [3] [3] --> FOAM FATAL ERROR: [3] Maximum number of iterations exceeded [3] [3] From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const [3] in file /home/opencfd/OpenFOAM/OpenFOAM-2.2.2/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 76. [3] FOAM parallel run aborting
https://www.dropbox.com/s/x7b35dsaj6ao6r7/Geometry.pdf As I set it up as a 3D case, although I am aware that for this problem a 2D case is sufficient, apart from the depicted patches (in red) there are <regionname>_front and <regionname>_back patches. Regarding the mesh: The mesh is generated in enGrid (1.4.0) and then exported to OpenFOAM using the OpenFOAM (polyhedral) export function. My mesh related questions were already answered by wyldckat: http://www.cfd-online.com/Forums/eng...gion-case.html I am aware that a mesh generated by the blockMesh utility would suit that problem very well, but as I would like to go to a more complex structure, I try using the same process of setting up the case as I would do for future application. Due to the straightforward boundary layer refinement implemented in enGrid I would like to follow that path. What is important to note is that by using the enGrid export function, the OpenFOAM set up does not follow the process of splitMeshRegions and changeDictionaryDict to account for multiple regions. Regarding Boundary and initial conditions: As I'm using a k-epsilon turbulence model, I had a look at http://www.cfd-online.com/Tools/turbulence.php, the referred explanations on the single entities that are used for calculating k and epsilon as well as the OpenFOAM user guide, which explains on these within section 2.1.8 (Lid driven cavity flow tutorial). I ended up with the following equations: k = 3/2*(sqrt(U_x^2 + U_y^2 + U_z^2)*I)^2, where U_i are the mean flow velocities and I is the turbulence intensity epsilon = (C_mu^(0.75)*k^(1.5))/(l_t), where C_mu is a constant (0.09) and l_t is the turbulent length scale, which needs to be estimated. For the plane wall case I use l_t = L_char * 0.4*delta, where L_char is a characteristic length (1.5m x-dimension) and delta the boundary layer thickness (4.91*L_char/sqrt(Re_x)) I then set up the case using the derived k and epsilon values, according to the geometry, fluid properties and individual flow. Interestingly I face the reported error in the laminar region (U=0.1, U=1), but a turbulent case (U=10) works fine: https://www.dropbox.com/s/si9y50brwc...ady_U10.tar.gz Increasing the velocity to U=50 causes again troubles. None of the transient settings worked out: https://www.dropbox.com/s/gj62ozuik5...ent_U10.tar.gz To resolve that i had a closer look at http://openfoamwiki.net/index.php/Ge..._-_planeWall2D and the OF2.2 case. I ran the provided case (U0.1) without any troubles. Even U=1 without changing k and epsilon worked fine. Switching to a turbulent scenario (U=10) and applying the above mentioned equations to the scenario produced a solution. By the way I adapted the tutorial for running it in parallel. Please check the ChangeLog: https://www.dropbox.com/s/wwxv9y7zzi...arallel.tar.gz I realized that the k and epsilon values for the laminar region differs enormously from mine, so I used these values for my own set up, but again the solver crashes due to divergent temperature solutions, as stated above. So I really am confused about how to set the case. I also do not see big differences in the boundary and initial conditions after looking at them for two days. All fvSolution and fvSchemes are exactly the same. Sorry for the lengthy explanation, but I'm happy to share my documentation with the community after I resolved these issues. Greetings, Andreas |
|
|
|
|
|
January 29, 2014, 05:48
|
|
#2 |
|
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 |
hello,
Did you check where your temperature drop rise to the limit ? Because i suspect that you get bad temperature value at wall boundary, using turbulence k-e model. If this is the case, you may try to check / modify your wall BC (turbulence, mut, T). In some case, switching to another (adapted) turbulence model may solve your trouble. Another way is to switch back to 1order upwind for turbulence and temperature, and use limiter. Anyway, if you find a better solution, don't hesitate to post here. Regards, olivier |
|
|
|
|
|
|
January 29, 2014, 11:05
|
|
#3 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
Hi Oliver,
thank you very much for your hints. Indeed the issues occur within the boundary layer. What I am surprised about is that in the 2D Wiki cases everything works fine. As soon as I use my mesh (3D) and the same settings as in the 2D Wiki cases including the front and back faces as symmetryPlane the solver crashes in all cases except when U=10. Does the additional dimension influence the turbulence model that much? I am aware that turbulent flows are much more complex in 3D but I thought the model could handle that. You are suggesting to switch to another turbulence model. What exactly are you thinking of? A k-omega-STT model? Andreas |
|
|
|
|
|
|
January 29, 2014, 11:35
|
|
#4 |
|
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 |
Hello,
I faced once this use, but i don't remember how i solved this. This clearly come from the boundary layer, which i suspect to not behave well with temperature gradient, thus viscosity/density gradient. Try to switch from k-e realizable to RNG or the opposite, or kwSST. Check also your mut BC (? try the mutSpaldingWallFunction). Anyway if you find the root of this issue, post it. regards, olivier |
|
|
|
|
|
|
January 30, 2014, 09:55
|
|
#5 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
Hi,
I've tried now the following turbulence models:
Additionally I tried both mutUWallFunction and mutUSpaldingWallFunction, but both were unsuccessful. I really wonder that there is no solution to this issue as I see several threads in this forum discussing this particular error. Unfortunately all provided tutorials run in a laminar case. But I assume that a lot of heat transfer problems are related to turbulent flows. So I guess more people would have faced this before. |
|
|
|
|
|
|
January 30, 2014, 10:12
|
|
#6 |
|
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 |
hello,
Did you check if you have T oscillation in this boundary layer ? or temperature just rise ? - What is your Y+ ? - try to relax more T eq. - try to initialise with constant properties (density, viscosity, ...) - try SA turbulence model. What is you outlet BC (T and velocity/pressure). if you got a spot in pressure at outlet, this can explain the instability. regards, olivier |
|
|
|
|
|
|
January 31, 2014, 04:44
|
|
#7 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
Hi Olivier,
thanks again for your input! By looking at the minT values within the log file, I see that that value is oscillating but dropping in a general trend. What is interesting: the amplitude is in the beginning not that big (at most 50K) but right before the solver crashes the temperature value drops by more than 250K. To answer the Y+ question: I used the formulas given on http://www.cfd-online.com/Wiki/Y_plu...nce_estimation but rearranged the last equation for y+. For the y input I used the height of the very first cell at the wall boundary. So I get a y+ = 46. I'm not sure whether my understanding here is right. With respect to the BC for the cold region: alphat Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
value 0;
internalField uniform $value;
boundaryField
{
c_left
{
type calculated;
value uniform $value;
}
c_right
{
type calculated;
value uniform $value;
}
s_bottom_cold
{
type compressible::alphatWallFunction;
Prt 0.85;
value uniform $value;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
value 19.09;
internalField uniform $value;
boundaryField
{
c_left
{
type inletOutlet;
inletValue uniform $value;
value uniform $value;
}
c_right
{
type fixedValue;
value uniform $value;
}
s_bottom_cold
{
type compressible::epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform $value;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
value 0.375;
internalField uniform $value;
boundaryField
{
c_left
{
type inletOutlet;
inletValue uniform $value;
value uniform $value;
}
c_right
{
type fixedValue;
value uniform $value;
}
s_bottom_cold
{
type compressible::kqRWallFunction;
value uniform $value;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object mut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
value 0;
internalField uniform $value;
boundaryField
{
c_left
{
type calculated;
value uniform $value;
}
c_right
{
type calculated;
value uniform $value;
}
s_bottom_cold
{
type mutUSpaldingWallFunction;//mutUWallFunction;
value uniform $value;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
value 1e5;
internalField uniform $value;
boundaryField
{
".*"
{
type calculated;
value uniform $value;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
value 1e5;
internalField uniform $value;
boundaryField
{
c_left
{
type fixedValue;
value uniform $value;
}
c_right
{
type fixedFluxPressure;
value uniform $value;
}
s_bottom_cold
{
type fixedFluxPressure;
value uniform $value;
}
c_bottom
{
type symmetryPlane;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
value 293.15;
internalField uniform $value;
boundaryField
{
c_left
{
type fixedValue;
value uniform $value;
}
c_right
{
type zeroGradient;
}
s_bottom_cold
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
neighbourFieldName T;
kappa fluidThermo;
kappaName none;
value uniform 293.15;
}
c_bottom
{
type symmetryPlane;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
value (50 0 0);
internalField uniform (50 0 0);
boundaryField
{
c_left
{
type fixedValue;
value uniform $value;
}
c_right
{
type inletOutlet;
inletValue uniform (50 0 0);
value uniform (50 0 0);
}
s_bottom_cold
{
type fixedValue;
value uniform (0 0 0);
}
c_bottom
{
type symmetryPlane;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
}
// ************************************************************************* //
p Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
value 1e5;
internalField uniform $value;
boundaryField
{
s_left
{
type calculated;
value uniform $value;
}
s_right
{
type calculated;
value uniform $value;
}
s_top_shell
{
type calculated;
value uniform $value;
}
s_bottom_shell
{
type calculated;
value uniform $value;
}
s_front
{
type symmetryPlane;
}
s_back
{
type symmetryPlane;
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
value 443.15;
internalField uniform $value;
boundaryField
{
s_left
{
type zeroGradient;
}
s_right
{
type zeroGradient;
}
s_top_shell
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
value uniform $value;
neighbourFieldName T;
kappa solidThermo;
kappaName none;
}
s_bottom_shell
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
value uniform $value;
neighbourFieldName T;
kappa solidThermo;
kappaName none;
}
s_front
{
type symmetryPlane;
}
s_back
{
type symmetryPlane;
}
}
// ************************************************************************* //
By setting the thermophysicalProperties as follows, I thought I would end up with constant properties: Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant/bottomAir";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleEnthalpy;
}
mixture
{
specie
{
nMoles 1;
molWeight 28.9;
}
thermodynamics
{
Cp 1000;
Hf 0;
}
transport
{
mu 1.8e-05;
Pr 0.7;
}
}
// ************************************************************************* //
What I have been trying yesterday was to extrude the mesh at the inlet to account for a developed boundary layer as soon as the flow hits the shell interface. I did this because I thought that it might be that I get a transition zone at the outlet. But unfortunately this didn't help. I will now take a look at the SA turbulence model and relaxation factors. Regards, Andreas |
|
|
|
|
|
|
February 1, 2014, 11:01
|
|
#8 |
|
Member
Michael Page
Join Date: Mar 2009
Location: Quebec, Canada
Posts: 36
Rep Power: 17 |
Hi,
I got a problem similar than yours. To get convergence, I started the simulation with laminar model. After 50 iterations, I copied new turbulence files (k, omega, mut, etc...) in the time folder a I activated my turbulence model. The model converge after that. Good luck, |
|
|
|
|
|
|
February 3, 2014, 03:12
|
|
#9 |
|
Senior Member
Olivier
Join Date: Jun 2009
Location: France, grenoble
Posts: 272
Rep Power: 17 |
hello,
Seem that your trouble came from your BCs. You use fixedValue for both velocity and pressure. You should _never_ do that. Regards, olivier |
|
|
|
|
|
|
February 4, 2014, 03:06
|
|
#10 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
Hi Michael,
Hi Olivier, thank you for your advice. Olivier was right. The pressure BC caused the trouble. The hint, to start off a laminar solution will be useful soon. Still all the investigating the root cause of the error taught me a lot on how to deal with OF and CFD itself. Thanks again for all your input. I ran a few test cases and for now it seems that a k-epsilon RNG model is the most stable one. Greetings, Andreas |
|
|
|
|
|
|
March 19, 2014, 13:21
|
|
#11 | |
|
New Member
Pam
Join Date: Feb 2011
Posts: 15
Rep Power: 15 |
Quote:
I am also facing the same problem with chtMultiRegionSimpleFoam and Laminar case. Could you please share your BC files if possible for my reference. Thank you,
__________________
Pam |
||
|
|
|
||
|
March 20, 2014, 04:15
|
|
#12 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
Hi Pam,
here are my changeDictionaryDict files: region cold: Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dictionaryReplacement
{
boundary
{
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
U
{
internalField uniform (0.0099585 0 0);
boundaryField
{
c_left
{
type fixedValue;
value uniform (0.0099585 0 0);
}
c_right
{
type inletOutlet;
inletValue uniform (0 0 0);
value uniform (0.0099585 0 0);
}
cold_to_shell
{
type fixedValue;
value uniform (0 0 0);
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
ce_top
{
type slip;
}
}
}
T
{
internalField uniform 293.15;
boundaryField
{
c_left
{
type fixedValue;
value uniform 293.15;
}
c_right
{
type zeroGradient;
}
cold_to_shell
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
neighbourFieldName T;
kappa fluidThermo;
kappaName none;
value uniform 293.15;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
ce_top
{
type zeroGradient;
}
}
}
epsilon
{
internalField uniform 0.01;
boundaryField
{
c_left
{
type fixedValue;
value uniform 0.01;
}
c_right
{
type inletOutlet;
inletValue uniform 0.01;
value uniform 0.01;
}
cold_to_shell
{
type compressible::epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0.01;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
ce_top
{
type zeroGradient;
}
}
}
k
{
internalField uniform 0.1;
boundaryField
{
c_left
{
type fixedValue;
value uniform 0.1;
}
c_right
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
cold_to_shell
{
type compressible::kqRWallFunction;
value uniform 0.1;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
ce_top
{
type zeroGradient;
}
}
}
p
{
internalField uniform 1e5;
boundaryField
{
".*"
{
type calculated;
value uniform 1e5;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
}
}
p_rgh
{
internalField uniform 1e5;
boundaryField
{
c_left
{
type zeroGradient;
}
c_right
{
type fixedValue;
value uniform 1e5;
}
cold_to_shell
{
type fixedFluxPressure;
value uniform 1e5;
}
c_front
{
type symmetryPlane;
}
c_back
{
type symmetryPlane;
}
c_bottom
{
type symmetryPlane;
}
ce_top
{
type fixedFluxPressure;
value uniform 1e5;
}
}
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dictionaryReplacement
{
boundary
{
s_front
{
type symmetryPlane;
}
s_back
{
type symmetryPlane;
}
}
T
{
internalField uniform 443.15;
boundaryField
{
s_left
{
type zeroGradient;
}
s_right
{
type zeroGradient;
}
shell_to_hot
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
neighbourFieldName T;
kappa solidThermo;
kappaName none;
value uniform 443.15;
}
shell_to_cold
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
neighbourFieldName T;
kappa solidThermo;
kappaName none;
value uniform 443.15;
}
s_front
{
type symmetryPlane;
}
s_back
{
type symmetryPlane;
}
}
}
p
{
internalField uniform 1e5;
boundaryField
{
s_left
{
type calculated;
value uniform 1e5;
}
s_right
{
type calculated;
value uniform 1e5;
}
shell_to_hot
{
type calculated;
value uniform 1e5;
}
shell_to_cold
{
type calculated;
value uniform 1e5;
}
s_front
{
type symmetryPlane;
}
s_back
{
type symmetryPlane;
}
}
}
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.2 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object changeDictionaryDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dictionaryReplacement
{
boundary
{
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
}
U
{
internalField uniform (0.0099585 0 0);
boundaryField
{
h_left
{
type fixedValue;
value uniform (0.0099585 0 0);
}
h_right
{
type inletOutlet;
inletValue uniform (0 0 0);
value uniform (0.0099585 0 0);
}
hot_to_shell
{
type fixedValue;
value uniform (0 0 0);
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
he_bottom
{
type slip;
}
}
}
T
{
internalField uniform 593.15;
boundaryField
{
h_left
{
type fixedValue;
value uniform 593.15;
}
h_right
{
type zeroGradient;
}
hot_to_shell
{
type compressible::turbulentTemperatureCoupledBaffleMixed;
neighbourFieldName T;
kappa fluidThermo;
kappaName none;
value uniform 593.15;
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
he_bottom
{
type zeroGradient;
}
}
}
epsilon
{
internalField uniform 0.01;
boundaryField
{
h_left
{
type fixedValue;
value uniform 0.01;
}
h_right
{
type inletOutlet;
inletValue uniform 0.01;
value uniform 0.01;
}
hot_to_shell
{
type compressible::epsilonWallFunction;
Cmu 0.09;
kappa 0.41;
E 9.8;
value uniform 0.01;
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
he_bottom
{
type zeroGradient;
}
}
}
k
{
internalField uniform 0.1;
boundaryField
{
h_left
{
type fixedValue;
value uniform 0.1;
}
h_right
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
hot_to_shell
{
type compressible::kqRWallFunction;
value uniform 0.1;
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
he_bottom
{
type zeroGradient;
}
}
}
p
{
internalField uniform 1e5;
boundaryField
{
".*"
{
type calculated;
value uniform 1e5;
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
}
}
p_rgh
{
internalField uniform 1e5;
boundaryField
{
h_left
{
type zeroGradient;
}
h_right
{
type fixedValue;
value uniform 1e5;
}
hot_to_shell
{
type fixedFluxPressure;
value uniform 1e5;
}
h_front
{
type symmetryPlane;
}
h_back
{
type symmetryPlane;
}
h_top
{
type symmetryPlane;
}
he_bottom
{
type fixedFluxPressure;
value uniform 1e5;
}
}
}
}
// ************************************************************************* //
Apart from the mesh it happened also to me that due to the very slow flow in my domain, the buoyancy has a much bigger influence on the solution. Therefore consider switching off gravity by setting the gravity vector to (0 0 0) in constant/<fluidregions>/g Andreas |
|
|
|
|
|
|
March 20, 2014, 12:26
|
|
#13 | |
|
New Member
Pam
Join Date: Feb 2011
Posts: 15
Rep Power: 15 |
Quote:
Thanks again, Kind regards, Pam.
__________________
Pam |
||
|
|
|
||
|
March 24, 2014, 02:54
|
|
#14 |
|
New Member
akrasemann
Join Date: Dec 2013
Posts: 17
Rep Power: 12 |
The log file doesn't include an error output. But your density min and max value are probably at the maximum that is allowed. This indicates some issues there.
|
|
|
|
|
|
|
|
|
Similar Threads
|
||||
| Thread | Thread Starter | Forum | Replies | Last Post |
| whats the cause of error? | immortality | OpenFOAM Running, Solving & CFD | 13 | March 24, 2021 07:15 |
| Static Temperature / Opening Temperature | JulianP | CFX | 12 | April 10, 2019 18:00 |
| Problem with zeroGradient wall BC for temperature - Total temperature loss | cboss | OpenFOAM | 12 | October 1, 2018 06:36 |
| Calculation of the Governing Equations | Mihail | CFX | 7 | September 7, 2014 06:27 |
| is internalField(U) equivalent to zeroGradient? | immortality | OpenFOAM Running, Solving & CFD | 7 | March 29, 2013 01:27 |
Linear Mode
