[baran_foam]

Greeting All,
I am trying to solve a case in chtMultiRegionSimpleFoam for a geometry of cavity is surrounded by some thickness of insulation.

My question is how to calculate the heat flow from outside of insulating wall to the environment in openfoam 2.1.1.....

Please sugeest how should I do this thing? I have gone through some threads in CFD forum but can't get properly.....

Regards,
baran

[zfaraday]

Hi Baran,

I think what you need is wallHeatFlux utility. This is a post processing tool that computes the heat flux across all boundaries of your geometry. These boundaries need to be specified as wall, if they are previously specified as patch instead I think wallHeatFlux won't compute any flux across them.

Hope it helps!


Regards,

Alex

[baran_foam]

@ alex ....thanks fro your suggestion....
I tried with

wallHeatFlux

postProcessing utility.....it is working...for fluid region properly.....
but for solid region it is not working....
for my case I want to calculate how much heat is flowing from solid wall to environment....which is having mixed boundary condition of h & Tamb.....

Regards,
baran

[zfaraday]

Have you tried the -region flag? If boundaries have been defined as wall it must work.

Regards

Alex

[baran_foam]

Greeting all,

@alex ..I tried with this command but it is searching for file..

thermophysicalProperties

and showing fatal error.......
...it is not reading.....

solidThermoPhysicalProperties

for solid region...

please suggest something.......

Regards,
baran

[baran_foam]

Hello all,
I just went through solver of the utility...wallHeatFlux...and it is meant for fluid region...

surfaceScalarField heatFlux
(
fvc::interpolate(RASModel->alphaEff())*fvc::snGrad(h)
);

Can you suggest how to give heat flux.....command for...solid region....

Regards,
baran

[karoltomek]

I am using chtMultiRegionSimpleFoam solver (OF 2.3 and 2.2) and wallHeatFlux utility works for me. Do you have all needed files?
In fluid region directory I have:
- g
- RASProperties
- thermophysicalProperties
- turbulenceProperties
In solid region directory I have:
- radiationProperties
- thermophysicalProperties

And look at my fvSchemes settings file for solid region:

ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
}

divSchemes
{
default none;
}

laplacianSchemes
{
default none;
laplacian(alpha,h) Gauss linear uncorrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default uncorrected;
}

fluxRequired
{
default no;
}

[baran_foam]

Hello,
I am using OF 2.1...here for solid region file name is ..

solidThermoPhysicalProperties

this wallHeatFlux utility is unable to read this file for solid region....

Regards,
baran

[zfaraday]

Are you sure that the file is called solidThermoPhysicalProperties instead of simply thermophysicalProperties??

I have never worked with OF 2.1.1 but i have tried OF 2.2.1 and 2.3.x and the file name in these versions is the second one.

Can you post the whole message given out by OF so that it could be easier for the experts (not me) to find the problem?


Regards,

Alex

[baran_foam]

[bg8743@INDUX08 wallHeatFlux_consT]$ wallHeatFlux
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.1.1-221db2718bbb
Exec : wallHeatFlux
Date : Sep 23 2014
Time : 13:37:19
Host : "INDUX08.in.com"
PID : 24470
Case : /home/bg8743/OpenFoam/tutorials/heatTransfer/chtMultiRegionSimpleFoam/wallHeatFlux_consT
nProcs : 1
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 mesh for time = 0

Time = 0


--> FOAM FATAL IO ERROR:
cannot find file

file: /home/bg8743/OpenFoam/tutorials/heatTransfer/chtMultiRegionSimpleFoam/wallHeatFlux_consT/constant/thermophysicalProperties at line 0.

From function regIOobject::readStream()
in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting

[bg8743@INDUX08 wallHeatFlux_consT]$

may be solid region is not included for wallHeatFlux utility....
please suggest how to modify this for solid region....

[zfaraday]

The problem is that the file is being searched within the constant folder instead of the constant/solidRegion folder. Besides that you are executing wallHeatFlux instead of WallHeatFlux -region solidRegion.

Regards,

Alex

[baran_foam]

Greeting all,

@Alex....in my case i am unaware oe the command...given by you..so I make a folder of each region separately to check the wall heat flux......
by the command ..

wallHeatFlux -region <NAME>

same error is showing.........

for further study...I name this solidThermophysicalProperties as thermophysicalProperties.....so i got this kind of comment.....

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Time = 0
Selecting thermodynamics package constSolidThermo


--> FOAM FATAL ERROR:
Unknown basicThermo type constSolidThermo

Valid basicThermo types are:

26
(
ePsiThermo<pureMixture<constTransport<specieThermo <eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<eConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
ePsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hPsiThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hPsiThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<incompressible>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<constTransport<specieThermo <hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<icoPoly3ThermoPhysics>>
hRhoThermo<pureMixture<icoPoly8ThermoPhysics>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<hConstThermo<perfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<isobaricPerfectGas>>>>>
hRhoThermo<pureMixture<sutherlandTransport<specieT hermo<janafThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsPsiThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<constTransport<specieTherm o<hConstThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<constTransport<specieTherm o<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<hConstThermo<perfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<isobaricPerfectGas>>>>>
hsRhoThermo<pureMixture<sutherlandTransport<specie Thermo<janafThermo<perfectGas>>>>>
)



From function basicThermo::New(const fvMesh&)
in file basicThermo/basicThermoNew.C at line 60.

FOAM exiting

Regards,
baran

[zfaraday]

Have you defined properly both solid and fluid regions in the "constant/regionProperties" file?

[baran_foam]

@ alex...I hope I defined this properly......
but it is not built for solid region.......

Regards,
baran

[zfaraday]

Then I don't know what the problem can be... Maybe if you upload your case someone could check it out in order to help you.

Regards and cheer up!

Alex

[baran_foam]

Greeting all,
In this way i have modified wallHeatFlux utility...for OF 2.1.1 ...now it working properly.....
In createField.H

autoPtr<basicSolidThermo> thermo
(
basicSolidThermo::New(mesh)
);
const volScalarField& T = thermo->T();
tmp<volScalarField> tkappa = thermo->K();
//tmp<volSymmTensorField> tkappa = thermo.directionalkappa();
const volScalarField& kappa = tkappa();

In wallHeatFlux.C ..

surfaceScalarField heatFlux
(
fvc::interpolate(kappa)*fvc::snGrad(T)
);

In Make/option

EXE_INC = \
    -I$(LIB_SRC)/turbulenceModels \
    -I$(LIB_SRC)/turbulenceModels/compressible/RAS/RASModel \
    -I$(LIB_SRC)/thermophysicalModels/specie/lnInclude \
    -I$(LIB_SRC)/thermophysicalModels/basicSolidThermo/lnInclude \
    -I$(LIB_SRC)/finiteVolume/lnInclude

EXE_LIBS = \
    -lcompressibleRASModels \
    -lfiniteVolume \
    -lgenericPatchFields \
    -lspecie \
    -lbasicSolidThermo

Now it working properly...may be useful for some oher foamer...

Regards,
baran