[mactone]

Hi everyone,

I am a newbie to OpenFOAM. I used to use Fluent. In Fluent, the wall boundary of fluid domain can be set to have a 1D wall heat transfer with multiple layers.

I found the externalWallHeatFluxTemperature boundary seems to provide the same function as that in Fluent.

I use this on my wall boundary. However, the wall temperature seems remains constant even under the heat flow from the flame.

 {
        type            externalWallHeatFluxTemperature;

        mode            coefficient;

        Ta              constant 300.0;
        h               constant 10.0;
        thicknessLayers (0.1 0.2 0.3 0.4);
        kappaLayers     (1 2 3 4);

        kappaMethod     fluidThermo;

        value           $internalField;
    }

Anyone please help on the wall heat transfer issue in reactingFoam. Greatly appreciated.

[dlahaye]

Seems ok.

Suggest to run test lowering Ta or increasing h to get feel for the problem.

Happy to discuss further.

[JulioPieri]

You are making a very thick and insulated wall.

You are applying four layers of highly insulated materials.

Also, your outside h is very small, meaning that the heat flux is restricted, probably being transfered to the gas flow. You are essentially simulating a very insulated wall, which will make the temperature reasonably stable (and high).

If you don't want to use insulation, remove the kappaLayers stuff. Or at least try running with only one, with better values.

The h is the film coefficient of the OUTSITE wall, after the insulation. 10 W/m2K is a typical value for natural convection.

Try this:

{
        type            externalWallHeatFluxTemperature;

        mode            coefficient;

        Ta              constant 300.0;
        h               constant 100.0;
        thicknessLayers (0.05);
        kappaLayers     (33.5);

        kappaMethod     fluidThermo;

        value           $internalField;
    }

Lastly you may also try the "power" mode, instead of "coefficient".

The issue is most likely related to problem setup. Try applying the same numbers as you would in a Fluent case.

Other things to consider:
- Is your flame generating heat at all? Is your "Qdot" large enough (should be around 10^6 or such)?
- Is the reaction happening?
- Is your relaxation at a good number (high enough) so that it can actually allow changes in the fields?

[mactone]

wall_chamber
{
   type  externalWallHeatFluxTemperature;
   mode  coeficient;
   Ta   constant   300;
   h    constant   10;
   thicknessLayers  (25e-3 5e-3);
   kappaLayers       (0.16   40);
   kappaMethod   fluidThermo;
   value    $internalField;

When using $internalField as the value, the program can't run.
It shown
-->FOAM FATAL IO ERROR: (openfoam-2206)
compund has already been transferred from token
on line 21: moved compound of type List<scalar>

However, if I change the value to a constant value, say value constant 900;
It can run well.

I wonder which one is correct.

I am using openform 2206 running reactingFoam.

Thank you.

[JulioPieri]

Originally Posted by mactone

wall_chamber
{
   type  externalWallHeatFluxTemperature;
   mode  coeficient;
   Ta   constant   300;
   h    constant   10;
   thicknessLayers  (25e-3 5e-3);
   kappaLayers       (0.16   40);
   kappaMethod   fluidThermo;
   value    $internalField;

When using $internalField as the value, the program can't run.
It shown
-->FOAM FATAL IO ERROR: (openfoam-2206)
compund has already been transferred from token
on line 21: moved compound of type List<scalar>

However, if I change the value to a constant value, say value constant 900;
It can run well.

I wonder which one is correct.

I am using openform 2206 running reactingFoam.

Thank you.

"$internalField" is an alias to the "internalField" variable usually written in the beginning of the file, just below the header.

For the BC it acts almost as dummy ou "first iteration value". You can use "constant 900" if that makes the program run

[mactone]

Originally Posted by mactone

Hi everyone,

I am a newbie to OpenFOAM. I used to use Fluent. In Fluent, the wall boundary of fluid domain can be set to have a 1D wall heat transfer with multiple layers.

I found the externalWallHeatFluxTemperature boundary seems to provide the same function as that in Fluent.

I use this on my wall boundary. However, the wall temperature seems remains constant even under the heat flow from the flame.

 {
        type            externalWallHeatFluxTemperature;

        mode            coefficient;

        Ta              constant 300.0;
        h               constant 10.0;
        thicknessLayers (0.1 0.2 0.3 0.4);
        kappaLayers     (1 2 3 4);

        kappaMethod     fluidThermo;

        value           $internalField;
    }

Anyone please help on the wall heat transfer issue in reactingFoam. Greatly appreciated.

Coming back to see my stupid question, the thicknessLayers is of dimension meter. It is quite thick in this setting. I think it might be the reason why I can't see the outer surface temperature change at that time.