[aminem]

Hi,

Can anyone explain me how I can introduce power heat (W) in chtMultiRegionFoam solver?

In my case I have 1.5 W in my LED.

Thanks

[zfaraday]

You have to use fvOptions in order to set up your heat source. Check this out!

Regards,

Alex

[aminem]

Hi Alex,

I have try to do a sample 2D test with fvOptions.

I think that fvOptions don't have any effect. I use OF-2.3.0 and chtMultiRegionFoam.

fvOptions:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    class    dictionary;
    format    ascii;
    location    "system";
    object    fvOptions;
}
cylindre_Source_scalar
{
    type    scalarSemiImplicitSource;
    selectionMode    cellZone;
    cellZone    cylindre;
    active    true;
    scalarSemiImplicitSourceCoeffs
    {
        volumeMode    specific;
        injectionRateSuSp
        {
            h    (10 0);
        }
    }
}

My case (https://www.dropbox.com/s/snaqn957og...c4.tar.gz?dl=0).

Thanks

[zfaraday]

Originally Posted by aminem

Hi Alex,

I have try to do a sample 2D test with fvOptions.

I think that fvOptions don't have any effect. I use OF-2.3.0 and chtMultiRegionFoam.

fvOptions:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.6.x                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version    2.0;
    class    dictionary;
    format    ascii;
    location    "system";
    object    fvOptions;
}
cylindre_Source_scalar
{
    type    scalarSemiImplicitSource;
    selectionMode    cellZone;
    cellZone    cylindre;
    active    true;
    scalarSemiImplicitSourceCoeffs
    {
        volumeMode    specific;
        injectionRateSuSp
        {
            h    (10 0);
        }
    }
}

My case (https://www.dropbox.com/s/snaqn957og...c4.tar.gz?dl=0).

Thanks

Taking a quick glance over the case you uploaded, in your case I would try the following fvOptions:

cylindre_Source_scalar
{
    type    scalarSemiImplicitSource;
    selectionMode    all;
    active    true;
    scalarSemiImplicitSourceCoeffs
    {
        volumeMode    specific;
        injectionRateSuSp
        {
            h    (10 0);
        }
    }
}

It should work in your case, at least it works in my cases.

Btw, can you post your log file so that we can see if fvOptions is correctly read by the solver? In the output of the solver it says if any fvOptions have been read or not...

Best regards,

Alex

[aminem]

Hi Alex
I tried your solution but it's doesn't work.
This is my solve log
thanks

[zfaraday]

Originally Posted by aminem

Hi Alex
I tried your solution but it's doesn't work.
This is my solve log
thanks

Well, as you can see

Creating finite volume options from "system/fvOptions"

Selecting finite volume options model type scalarSemiImplicitSource
    Source: cylindre_Source_scalar
    - applying source for all time
    - selecting all cells
    - selected 176 cell(s) with volume 2.786796e-06

the solver is reading correctly the fvOptions file. If you state that it is not doing anything then maybe you set up your file with wrong units... I don't know what else I can say since I don't have enough info to be able to judge your case...

[derekm]

  scalarSemiImplicitSourceCoeffs     {        
 volumeMode    specific;        
 injectionRateSuSp        
 {             h    (10 0);         }     
}

and

Selecting finite volume options model type scalarSemiImplicitSource
    Source: cylindre_Source_scalar
    - applying source for all time
    - selecting all cells
    - selected 176 cell(s) with volume 2.786796e-06

means 28 microwatts are you expecting to see anything at that power?

to get 1.5W you need a number more like 5E5

[zfaraday]

Originally Posted by derekm

  scalarSemiImplicitSourceCoeffs     {        
 volumeMode    specific;        
 injectionRateSuSp        
 {             h    (10 0);         }     
}

and

Selecting finite volume options model type scalarSemiImplicitSource
    Source: cylindre_Source_scalar
    - applying source for all time
    - selecting all cells
    - selected 176 cell(s) with volume 2.786796e-06

means 28 microwatts are you expecting to see anything at that power?

Thanks Derek to point out that the "missing" info was in the post above... :P

Originally Posted by derekm

to get 1.5W you need a number more like 5E5

@aminem: Otherwise you can also use

  scalarSemiImplicitSourceCoeffs     {        
 volumeMode    absolute;        
 injectionRateSuSp        
 {             h    (1.5 0);         }     
}

Best regards,

Alex

[aminem]

Hi,

In my fvOptions I have put absolute in volumeMode. Now fvOptions have an effect on temperature.

I have doubt on what BC I must put. As you can see in attached figure I want to put my solid in open air volume. I have put freestream BC, but I have this error:

Solving for fluid region fluide
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  double Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4  Foam::PBiCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#5  
 at ??:?
#6  
 at ??:?
#7  
 at ??:?
#8  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#9  
 at ??:?

What kind of BC I should put in open BC (freestream, InletOutlet, OutletInlet, ....)

Thanks for your help

[Cartuns11]

Hi aminem,

We could do a exchange.... I usually use inletOulet for U,T,p_rgh and I have obtained good results, however, you would also try with fixedPressure in p_rgh. My doubt is about injectRateSuSp inside a solid.... it doesn't work but if I use it inside a fluid, it works..... I don't know the problem, could you help me?

U
{
type inletOutlet;
inletValue uniform ( 0 0 0 );
value uniform ( 0 0 0 );
}

T
{
type inletOutlet;
inletValue uniform 300;
value uniform 300;
}

p_rgh
{
type inletOutlet;
inletValue uniform 1E5;
value uniform 1E5;
}

[Cartuns11]

My simulation is like your model, with atmospheric conditions but I have a bulb with a light-wire. The problem is the wire... it has 3D mesh and I want to introduce power/m^3 inside the wire using fvOptions. It hasn't worked.....the wire hasn't increased the temperature...... I checked the unit and these were correct....
In my fvOptions file:

heatSource
{
type scalarSemiImplicitSource;
active on;
selectionMode all;

scalarSemiImplicitSourceCoeffs
{
volumeMode specific;
injectionRate
{
h (5e+09 0);
}
}
}

thanks!

[zfaraday]

You need to provide more information Cartuns11, otherwise no one will be able to help you...

[Cartuns11]

ok!

The model is a chtMultiRegionSimpleFoam simulation without radiation. It consists in a bulb with wire and support inside the atmospheric air (openning conditions). The target is the temperatures of the bulb, wire, support and domain0 (air atmospheric). The input is the power of wire, which is a solid. The support is also a solid and the bulb and the air are a fluids.
The wire volume is 5e-09 [m^3] and I have to introduce 5e+09 [W/m^3]. The best way is fvOptions....but, when I carry out the solver, the temperature of wire doesnt increase.....it maintains same value.
I did proves which consisted in the power introducing in a fluid with the same method.......and inside the fluid, it worked..... I don't understand it....
I have loaded some image and some codes....All codes of wire.

fvOptions

heatSource
{
type scalarSemiImplicitSource;
active true;
selectionMode all;


scalarSemiImplicitSourceCoeffs
{
volumeMode specific;
injectionRateSuSp
{
h (5e+09 0);
}
}
　
}

fvSolution

solvers
{
p
{
solver GAMG;
tolerance 1e-7;
relTol 0.01;
smoother GaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
cacheAgglomeration on;
agglomerator faceAreaPair;
nCellsInCoarsestLevel 10;
mergeLevels 1;
}
U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
k
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
omega
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-8;
relTol 0.1;
nSweeps 1;
}
}
SIMPLE
{
nNonOrthogonalCorrectors 0;
}
potentialFlow
{
nNonOrthogonalCorrectors 10;
}
relaxationFactors
{
fields
{
p 0.5;
}
equations
{
U 0.7;
k 0.7;
omega 0.7;
}
}
cache
{
grad(U);
}

fvScheme

ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(U) cellLimited Gauss linear 1;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwindV grad(U);
div(phi,k) bounded Gauss upwind;
div(phi,omega) bounded Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
fluxRequired
{
default no;
p;
}

thermophisicalProperties

thermoType
{
type heSolidThermo;
mixture pureMixture;
transport constIso;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}
mixture
{
specie
{
nMoles 1;
molWeight 12;
}
transport
{
kappa 95;
}
thermodynamics
{
Hf 0;
Cp 176;
}
equationOfState
{
rho 19300;
}
}

thanks!

[derekm]

Need to see the solver log file

[aminem]

Hi Curtuns1,

1/We need to see your Log file to know if the fvOptions file is read.

2/You must put fvOptions in system/wire directory.

3/I think you need to put a cellZone indication in your fvOptions file?

For me it's work for one source. I try to do this with multiple sources.

[Cartuns11]

Hi,

I've loaded the solver log. The solver works but the temperature of wire doesn't increase...... I think that the solver reads fvOptions correctly..... In addition, The problem isn't the units, because I have put values between [-5E20 to 5E20]..... but the temperature hasn't moved..... In a other forum, I've read about this and the introducing power inside a solid using fvOptions doesn't work. It could be a problem of code....
The fvOptions is just in the wire folder.

BOMBILLADIRECCIO: bulb
CASQUILLODIRECCIO: support
FILAMENTODIRECCIO: wire
domain0:air

\*---------------------------------------------------------------------------*/
Build : 2.3.0-f5222ca19ce6
Exec : chtMultiRegionSimpleFoam -parallel
Date : Jun 10 2015
Time : 11:47:18
Host : "agonzalez-Precision-WorkStation-T7500"
PID : 713
Case : /home/agonzalez/Desktop/CloudFlow/Modelo_FOCO_SEAT/prbomb2
nProcs : 8
Slaves : 
7
(
"agonzalez-Precision-WorkStation-T7500.714"
"agonzalez-Precision-WorkStation-T7500.715"
"agonzalez-Precision-WorkStation-T7500.716"
"agonzalez-Precision-WorkStation-T7500.717"
"agonzalez-Precision-WorkStation-T7500.718"
"agonzalez-Precision-WorkStation-T7500.719"
"agonzalez-Precision-WorkStation-T7500.720"
)
Pstream initialized with:
floatTransfer : 0
nProcsSimpleSum : 0
commsType : nonBlocking
polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create fluid mesh for region BOMBILLADIRECCIO for time = 0
Create fluid mesh for region domain0 for time = 0
Create solid mesh for region CASQUILLODIRECCIO for time = 0
Create solid mesh for region FILAMENTODIRECCIO for time = 0
*** Reading fluid mesh thermophysical properties for region BOMBILLADIRECCIO
Adding to thermoFluid
Selecting thermodynamics package 
{
type heRhoThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
equationOfState icoPolynomial;
specie specie;
energy sensibleEnthalpy;
}
Adding to rhoFluid
Adding to UFluid
Adding to phiFluid
Adding to gFluid
Adding to turbulence
Selecting turbulence model type laminar
Adding to ghFluid
Adding to ghfFluid
Selecting radiationModel none
Adding fvOptions
No finite volume options present
*** Reading fluid mesh thermophysical properties for region domain0
Adding to thermoFluid
Selecting thermodynamics package 
{
type heRhoThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
equationOfState icoPolynomial;
specie specie;
energy sensibleEnthalpy;
}
Adding to rhoFluid
Adding to UFluid
Adding to phiFluid
Adding to gFluid
Adding to turbulence
Selecting turbulence model type laminar
Adding to ghFluid
Adding to ghfFluid
Selecting radiationModel none
Adding fvOptions
No finite volume options present
*** Reading solid mesh thermophysical properties for region CASQUILLODIRECCIO
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
*** Reading solid mesh thermophysical properties for region FILAMENTODIRECCIO
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
Creating finite volume options from fvOptions
Selecting finite volume options model type scalarSemiImplicitSource
Source: heatSource
- applying source for all time
- selecting all cells
- selected 3256 cell(s) with volume 5.422112e-09
Time = 1
　
Solving for fluid region BOMBILLADIRECCIO
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.005970245, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.006041075, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0007919736, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.01634446, Final residual = 0.0001542216, No Iterations 2
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.7937571, Final residual = 0.007827255, No Iterations 47
time step continuity errors : sum local = 0.159732, global = 2.600357e-10, cumulative = 2.600357e-10
Min/max rho:1.156291 1.156291
Solving for fluid region domain0
DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.009871374, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.008090986, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.0001421311, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.0006556001, Final residual = 6.4236e-06, No Iterations 2
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.9536995, Final residual = 0.00745634, No Iterations 34
DICPCG: Solving for p_rgh, Initial residual = 0.1693578, Final residual = 0.0016451, No Iterations 33
time step continuity errors : sum local = 0.004237694, global = 8.872091e-05, cumulative = 8.872117e-05
Min/max rho:1.170813 1.170813
Solving for solid region CASQUILLODIRECCIO
DICPCG: Solving for h, Initial residual = 0.5277625, Final residual = 0.0003224809, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
Solving for solid region FILAMENTODIRECCIO
DICPCG: Solving for h, Initial residual = 0.4530837, Final residual = 0.0004174483, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
ExecutionTime = 6.63 s ClockTime = 7 s
Time = 2
　
Solving for fluid region BOMBILLADIRECCIO
DILUPBiCG: Solving for Ux, Initial residual = 0.2284703, Final residual = 0.0001765353, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.2329958, Final residual = 0.0001731993, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.2032166, Final residual = 0.0001470408, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.9999981, Final residual = 0.006117996, No Iterations 4
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.8656138, Final residual = 0.007022698, No Iterations 47
time step continuity errors : sum local = 0.05913433, global = 1.469776e-10, cumulative = 8.872132e-05
Min/max rho:1.156291 1.156291
Solving for fluid region domain0
DILUPBiCG: Solving for Ux, Initial residual = 0.03329544, Final residual = 2.302509e-05, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.03612496, Final residual = 2.331844e-05, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.02318816, Final residual = 1.174436e-05, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.009117826, No Iterations 2
Min/max T:299.9999 300
DICPCG: Solving for p_rgh, Initial residual = 0.9949871, Final residual = 0.008860348, No Iterations 30
DICPCG: Solving for p_rgh, Initial residual = 0.08539426, Final residual = 0.0008468964, No Iterations 32
time step continuity errors : sum local = 0.02833294, global = -0.0002961078, cumulative = -0.0002073865
Min/max rho:1.170812 1.170813
Solving for solid region CASQUILLODIRECCIO
DICPCG: Solving for h, Initial residual = 0.8983162, Final residual = 0.0002216541, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
Solving for solid region FILAMENTODIRECCIO
DICPCG: Solving for h, Initial residual = 0.2041466, Final residual = 0.0002220012, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
ExecutionTime = 7.46 s ClockTime = 8 s
Time = 3
　
Solving for fluid region BOMBILLADIRECCIO
DILUPBiCG: Solving for Ux, Initial residual = 0.2255419, Final residual = 0.0002050287, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.1777021, Final residual = 0.0001137957, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.7969785, Final residual = 0.0006711936, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.4353527, Final residual = 0.001637115, No Iterations 4
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.6657176, Final residual = 0.005987832, No Iterations 46
time step continuity errors : sum local = 0.02866349, global = -2.892586e-11, cumulative = -0.0002073865
Min/max rho:1.156291 1.156291
Solving for fluid region domain0
DILUPBiCG: Solving for Ux, Initial residual = 0.1704313, Final residual = 9.563561e-05, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.1710087, Final residual = 6.118017e-05, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.05492389, Final residual = 8.961354e-05, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.9856835, Final residual = 0.005686893, No Iterations 2
Min/max T:299.9969 300.0023
DICPCG: Solving for p_rgh, Initial residual = 0.8956926, Final residual = 0.00844547, No Iterations 38
DICPCG: Solving for p_rgh, Initial residual = 0.001688192, Final residual = 1.664736e-05, No Iterations 35
time step continuity errors : sum local = 0.006222197, global = 0.001343636, cumulative = 0.001136249
Min/max rho:1.170803 1.170825
Solving for solid region CASQUILLODIRECCIO
DICPCG: Solving for h, Initial residual = 0.8825567, Final residual = 0.0003003737, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
Solving for solid region FILAMENTODIRECCIO
DICPCG: Solving for h, Initial residual = 0.1137917, Final residual = 0.000146549, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
ExecutionTime = 8.34 s ClockTime = 9 s
Time = 4
　
Solving for fluid region BOMBILLADIRECCIO
DILUPBiCG: Solving for Ux, Initial residual = 0.1771537, Final residual = 0.0001553637, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.1853754, Final residual = 0.0001522035, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.6621283, Final residual = 0.0005294418, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.280204, Final residual = 0.001580275, No Iterations 4
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.7542199, Final residual = 0.005754844, No Iterations 44
time step continuity errors : sum local = 0.01850979, global = -1.039983e-10, cumulative = 0.001136249
Min/max rho:1.156291 1.156291
Solving for fluid region domain0
DILUPBiCG: Solving for Ux, Initial residual = 0.1450099, Final residual = 0.001142569, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.1362821, Final residual = 0.001065343, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.1069051, Final residual = 0.0009845638, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.5549841, Final residual = 0.003314565, No Iterations 2
Min/max T:299.9962 300.0023
DICPCG: Solving for p_rgh, Initial residual = 0.1746192, Final residual = 0.001707782, No Iterations 40
DICPCG: Solving for p_rgh, Initial residual = 0.001101075, Final residual = 1.08441e-05, No Iterations 39
time step continuity errors : sum local = 0.00453244, global = 0.001133385, cumulative = 0.002269634
Min/max rho:1.170803 1.170828
Solving for solid region CASQUILLODIRECCIO
DICPCG: Solving for h, Initial residual = 0.5303216, Final residual = 0.0001219209, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
Solving for solid region FILAMENTODIRECCIO
DICPCG: Solving for h, Initial residual = 0.06639977, Final residual = 8.910753e-05, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
ExecutionTime = 9.44 s ClockTime = 10 s
Time = 5
　
Solving for fluid region BOMBILLADIRECCIO
DILUPBiCG: Solving for Ux, Initial residual = 0.140732, Final residual = 0.0001026456, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.2060334, Final residual = 0.0001278458, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.1182916, Final residual = 7.821812e-05, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.4115059, Final residual = 0.003101837, No Iterations 4
Min/max T:300 300
DICPCG: Solving for p_rgh, Initial residual = 0.5854837, Final residual = 0.004143481, No Iterations 44
time step continuity errors : sum local = 0.007204766, global = 2.257701e-10, cumulative = 0.002269634
Min/max rho:1.156291 1.156291
Solving for fluid region domain0
DILUPBiCG: Solving for Ux, Initial residual = 0.1652503, Final residual = 0.001428339, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.1539691, Final residual = 0.001333403, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.1358239, Final residual = 3.548498e-05, No Iterations 2
DILUPBiCG: Solving for h, Initial residual = 0.4827221, Final residual = 7.081489e-05, No Iterations 4
Min/max T:299.9895 300.0014
DICPCG: Solving for p_rgh, Initial residual = 0.1503564, Final residual = 0.001128931, No Iterations 35
DICPCG: Solving for p_rgh, Initial residual = 0.004037298, Final residual = 4.023457e-05, No Iterations 29
time step continuity errors : sum local = 0.003569743, global = -0.0009190757, cumulative = 0.001350558
Min/max rho:1.170807 1.170856
Solving for solid region CASQUILLODIRECCIO
DICPCG: Solving for h, Initial residual = 0.4428948, Final residual = 0.0001086157, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
Solving for solid region FILAMENTODIRECCIO
DICPCG: Solving for h, Initial residual = 0.05024991, Final residual = 7.156336e-05, No Iterations 2
Min/max T:min(T) [0 0 0 1 0 0 0] 300 max(T) [0 0 0 1 0 0 0] 300
ExecutionTime = 10.33 s ClockTime = 11 s

[zfaraday]

Are you sure the fvSolution's code you provided above belongs to the wire? I don't think so...

Regarding what you say about a problem in the code, you are wrong, there's no problem in the code, I have run several simulations with heat sources in solids and they work well for me...

With regard to the units, as per what you say, the bulb is providing only 1W. I don't know if it is correct or not but it seems a low value...

Have you set up properly your initial and boundary conditions?

[Cartuns11]

I've checked all.... but I haven't found any error.... may be, there is one but I haven't seen it.
The units are correct, because the wire volume is 5e-09 m^3 and the heat flux is 5e+09 W/m^-3, therefore I have 25 W inside wire.
I'm going to carry out other models...

I'll tell you if I achieve to solve the problem.

Thanks.
Greetings

[Cartuns11]

Hi everybody,

I have found the ""error/solution"".............
The heat source of fvOptions works, if the model is no steadyState..... All time, I've been carrying out steadyState simulations (chtMultiRegionSimpleFoam) but when I have used chtMultiRegionFoam the heat source has been introduced....

I would like to do the model in steadyState with chtMultiRegionFoam...... any idea? could I do it? is it possible?

I'm thinking that the problem is in fvSchemes and fvSolution

Thanks

[zfaraday]

Hi Cartuns11,

I'm glad you could make it work in a transient state solver, however, it must work in steady state too because I have been working with chtMultiRegionSimpleFoam with solid generating regions for a while with no problem...

I suggest you something... Why don't you try to run one of the tutorial cases you can find within the "$FOAM_TUTORIALS/heatTransfer/chtMultiRegionSimpleFoam" directory first? You should add a heat source in one of the regions since no one of the tutorials contains volumetric heat generation, but if you are able to make the tutorial run properly obtaining physical results (I'm sure you can do it!) you can then adapt the geometry of your case to the parameters (fvSolution, fvSchemes...) used in the tutorial.

Hope it helps,

Alex