[bullmut]

Hi All
I am running a simulation around a heating element.
I have a container i would like to see the effect of inlet velocity and outlet placement on the internal temperature of the air. I have a heating element whose temperature i fix with fvOptions. I apply the cellset through topoSet so that i can adjust its location easily.

heatSource
{
    type scalarFixedValueConstraint;
    active true;
    selectionMode cellSet;
    cellSet heater;
    fieldValues
    {
        T 400;
    }
    scalarFixedValueConstrainteCoeffs
    {


     selectionMode cellSet;
     
    }
}

I am using the following thermophysicalProperties

thermoType
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}

mixture
{
    specie
    {
        molWeight   28.9;
    }
    thermodynamics
    {
        Cp          1007;
        Hf          0;
    }
    transport
    {
        As          1.4792e-06;
        Ts          116;
    }
}

the code runs but i get the following warning:

--> FOAM Warning :
From function virtual void Foam::fv:ption::checkApplied() const
in file cfdTools/general/fvOptions/fvOption.C at line 125
Source heatSource defined for field T but never used

I am guessing that when i solve for "e" my T field in the 0 folder gets included.

smoothSolver: Solving for e, Initial residual = 1, Final residual = 0.0172392, No Iterations 2

I am however lost on how to include a cellSet/cellZone of fixed temperature into the solver using fvOptions. should i be applying a h or e value instead of T?

[RobertHB]

Originally Posted by bullmut

heatSource
{
    type scalarFixedValueConstraint;
    active true;
    selectionMode cellSet;
    cellSet heater;
    fieldValues
    {
        T 400;
    }
    scalarFixedValueConstrainteCoeffs
    {


     selectionMode cellSet;
     
    }
}

I am guessing that when i solve for "e" my T field in the 0 folder gets included.

I am however lost on how to include a cellSet/cellZone of fixed temperature into the solver using fvOptions. should i be applying a h or e value instead of T?

Your fvOptions term applies to the variable "T". If you don't have a T variable in your 0/ folder or your solver does not use the T variable from your 0/ folder your fvOptions term does not apply.

I just did a quick look-over of the rhoPimpleFoam files and it does not seem to use the T variable.

[bullmut]

Hi Robert
Thanks for the reply
I am using the angledDuct case as my base.
It uses a T field in the 0 folder.

tutorials/compressible/rhoPimpleFoam/RAS/angledDuct:
├── 0
│ ├── alphat
│ ├── epsilon
│ ├── k
│ ├── nut
│ ├── p
│ ├── T
│ └── U
├── Allrun
├── constant
│ ├── fvOptions
│ ├── thermophysicalProperties
│ └── turbulenceProperties
└── system
├── blockMeshDict.m4
├── controlDict
├── fvSchemes
└── fvSolution

Which confuses me. I assume T would be included in the rhoPimpleFoma solver but when i looked at he .C file i did not see it.

[RobertHB]

If we select the hePsiThermo thermophysical model, the temperature field T is calculated from the solved energy variable in the following function [...] The above function calculate() is called by rhoPimpleFoam, rhoSimpleFoam and sonicFoam etc. from the line “thermo.correct()” after solving the energy conservation equation EEqn

Source: http://caefn.com/openfoam/temperature-calculation

Have a look for yourself but i would think that the T file is included to provide BC's and not the variable itself. Thus it does not include the fvOptions term. But i don't work with your solver or anything temperature related. So i might be wrong afterall.

[bullmut]

Yeah, i saw this post before.

Source: http://caefn.com/openfoam/temperature-calculation

Which makes me think i need to specify enthalpy (h) and not temperature in fvOptions

I am however lost on how to include a cellSet/cellZone of fixed temperature into the solver using fvOptions. should i be applying a h or e value instead of T?

Will try the enthalpy approach and let you know

[clapointe]

What you're probably looking for is fixedTemperatureConstraint. I've not tested it myself for rhoPimpleFoam, but it is used here (https://github.com/OpenFOAM/OpenFOAM...tant/fvOptions) for a rhoSimpleFoam tutorial so there's no reason it shouldn't work.

Caelan

[bullmut]

Hi All


Thanks for the info and help.
I ended up using an stl (since the heater is a simple box) and then with snappy i assigned a patch name. this name was then use in the T file of my 0 folder to set the temperature.


Allowed me to move my heater around easy enough and meant i could set the temperature directly.


Cheers