Hi Im working on cooling analyses and need to define the heat load as openfoam BC.
I used fixed gradient (q/K)=(dt/dx)
And also externalwallheatflux
I also read that this BC turbulentHeatFluxTemperature also available. But I can't able to use it both the version from openfoam foundation and ESI.
So I wish to know to confirm whether this BC is no more supported by OpenFOAM
Hi,
I am not sure about "externalWallHeatFlux" boundary condition in OpenFOAM. However,
- openfoam.com v1912, externalWallHeatFluxTemperature
https://www.openfoam.com/documentation/guides/latest/api/classFoam_1_1externalWallHeatFluxTemperatureFvPatchScalarField.html#details
- openfoam.com, externalWallHeatFluxTemperature
https://cpp.openfoam.org/v7/externalWallHeatFluxTemperatureFvPatchScalarField_8H_source.html
Could these be used instead of "externalWallHeatFlux" in your case?
Also, I think that the functionality of " turbulentHeatFluxTemperature" was includes in the "externalWallHeatFluxTemperature". See the release notes of OpenFOAM 5.x
- https://openfoam.org/release/5-0/ (Energy, Heat Transfer and Thermophysical Modelling/Other)
and the corresponding commit on GIT
- https://github.com/OpenFOAM/OpenFOAM-dev/commit/e72e7c5625cc55315cb070120859577a526e3350
where the description starts with:
"by combining with and rationalizing functionality from turbulentHeatFluxTemperatureFvPatchScalarField. externalWallHeatFluxTemperatureFvPatchScalarField now replaces turbulentHeatFluxTemperatureFvPatchScalarField which is no longer needed and has been removed."
Best,
Martin
Hi Martin Isoz Martin I was specifying about externalWallHeatFluxTemperature only.
What is the difference between kappa and kappamethod...
I understood kappa means thermalconductivity. what is kappamethod. both kappa and kappamethod should be specified fluidThermo
Hi Ijaz Fazil Syed Ahmed Kabir ,
if you take a look into the source codes and documentation, you will find out that:
1. https://cpp.openfoam.org/v7/externalWallHeatFluxTemperatureFvPatchScalarField_8H_source.html
->
kappaMethod | Inherited from temperatureCoupledBase | inherited |
kappa | Inherited from temperatureCoupledBase | inherited |
2. https://github.com/OpenFOAM/OpenFOAM-7/blob/master/src/TurbulenceModels/compressible/turbulentFluidThermoModels/derivedFvPatchFields/temperatureCoupledBase/temperatureCoupledBase.H
->
Property | Description | Required | Default value kappaMethod | Thermal conductivity method | yes | kappa | Name of thermal conductivity field | no | none alphaAni | Name of the non-isotropic alpha | no | Anialpha
and
The thermal conductivity \c kappa may be obtained by the following methods: - 'lookup' : lookup volScalarField (or volSymmTensorField) with name defined by 'kappa' - 'fluidThermo' : use fluidThermo and default compressible::turbulenceModel to calculate kappa - 'solidThermo' : use solidThermo kappa() - 'directionalSolidThermo': uses look up for volSymmTensorField for transformed kappa vector. Field name definable in 'alphaAni', named 'Anialpha' in solid solver by default
(sorry for the bad formating, but it is nicely structured in the source code).
Long story short:
kappa -> name of the thermal conductivity field (if there is one)
kappaMethod -> method that is used to obtain the thermal conductivity
If you use kappaMethod "fluidThermo", then kappa is irrelevant and I believe it can hold anything you want. Therefore, you did not observe any crush using (incorrectly) "fluidThermo".
If you use kappaMethod "lookup", then you shold specify the name of the field to look for in kappa.
Best,
Martin
- Badges
- Science topic