[Ahmed Khattab]

Dear All,

i want to simulate convection heat transfer for flow exposed to constant wall temperature without including tube thickness. my problem is chtMultiRegionSimpleFoam is used for multiple Regions only.

thanks,

[Tobi]

Hi,

you are wrong.
cht can also used for one Region but is generated for Multi regions (conjugated heat Transfer).

If you want to simulate just one Region you can use buoyantSimpleFoam or buoyantBoussinesqSimpleFoam - or the Pimple for transient Solutions.

Regards

[Ahmed Khattab]

Originally Posted by Tobi

Hi,

you are wrong.
cht can also used for one Region but is generated for Multi regions (conjugated heat Transfer).

If you want to simulate just one Region you can use buoyantSimpleFoam or buoyantBoussinesqSimpleFoam - or the Pimple for transient Solutions.

Regards

Hi Tobias,

1- how could i use chtMultiRegionSimpleFoam for one region?

2- i think buoyantSimpleFoam is used for natural convection not forced convection. also, all thermo models available with it are for perfect gases not lequids.

thanks,
Ahmed

[Tobi]

Originally Posted by Ahmed Khattab

Hi Tobias,

1- how could i use chtMultiRegionSimpleFoam for one region?

2- i think buoyantSimpleFoam is used for natural convection not forced convection. also, all thermo models available with it are for perfect gases not lequids.

thanks,
Ahmed

Hi,

you could use cht for one region. You just have to use one region where is the problem?

the buoyantSimpleFoam are for natural convection but I think for forced convection you could also do it.

PS: you can use water as well - use icoPolynomial functions to describe your fluid.

[Ahmed Khattab]

Originally Posted by Tobi

Hi,

you could use cht for one region. You just have to use one region where is the problem?

the buoyantSimpleFoam are for natural convection but I think for forced convection you could also do it.

PS: you can use water as well - use icoPolynomial functions to describe your fluid.

Hi Tobias,

i want to use one fluid region and no solid regions, cht don't accept this. splitMeshRegions doesn't create mesh for only one region. also, cht must read regions to apply suitable equations.

thanks,
Ahmed

[Tobi]

Hi,

you are wrong.

Hmmm, you are not very familiar to the software, arent you?

I dont want to tell you step by step how to do it (no time) but some hints:


1. why do you need splitMeshRegions?
- you need it if you are using sHM with more than one region (--> cellZones)

2. just mesh your solid
3. move the mesh from constant/polyMesh into constant/solid/polyMesh
4. change the "regionProperties" - only solid is available
5. change the boundarys in constant/solid/polyMesh like you need
6. change 0/solid/* files to your application

-> start


You can simply check it out in the following way:

a) buoyantSimpleFoam tutorial -> buoyantCavity
b) make the mesh
c) move the mesh from buoyantCavity/constant/polyMesh into your cht case -> cht_case/constant/myRegion
d) move the files in 0 directory from buoyantCavity/0 into your cht case -> cht_case/0/myRegion
e) change the regionProperties so you have only one fluid (myRegion)
f) check that you have the fvSchemes and Solutions in system/myRegion

-> start

Be sure that the fluid files are in the constant/myRegion folder too.


Hope it will help you now.

PS: have a look at the source code then you will be able to understand how this solver is working

Regards
Tobi

[Tobi]

Originally Posted by Ahmed Khattab

Hi Tobias,

i want to use one fluid region and no solid regions, cht don't accept this. splitMeshRegions doesn't create mesh for only one region. also, cht must read regions to apply suitable equations.

thanks,
Ahmed

It does not matter if you just want to use one region for fluid or solid.

Therefor you should use buoyantSimpleFoam:

In the energy eqn you find the turbulent term

    fvScalarMatrix EEqn
    (
        fvm::div(phi, he)
      + (
            he.name() == "e"
          ? fvc::div(phi, volScalarField("Ekp", 0.5*magSqr(U) + p/rho))
          : fvc::div(phi, volScalarField("K", 0.5*magSqr(U)))
        )
      - fvm::laplacian(turbulence->alphaEff(), he)
     ==
        radiation->Sh(thermo)
      + fvOptions(rho, he)
    );