CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   coupling temperature between two solids (http://www.cfd-online.com/Forums/openfoam-solving/83877-coupling-temperature-between-two-solids.html)

mirko January 13, 2011 16:54

coupling temperature between two solids
 
1 Attachment(s)
Hi,

I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.

My problem is that I don't know how to couple the temperature across the solid boundaries. I have tried using the solidWallMixedTemperatureCoupled, but that does not work

Code:

        air_to_plate
        {
        type          solidWallMixedTemperatureCoupled;
        neighbourFieldName T;
        K          K;
        value          293.15;
        }

(disregard the meaning of the `air' label - that is from a solid-fluid version of the problem when air was a fluid. Now I am treating it as solid).

As the problem in the solver that I am using or in the boundary condition?

Thanks,

Mirko

PS - I am attaching the problem files for a simple 2D problem.

mgc January 14, 2011 05:25

coupledMatrix
 
Did you try using the "coupledMatrix" instead? (See conjugateHeatFoam)

Marķa

maddalena January 14, 2011 10:55

Hi Mirko,
Quote:

Originally Posted by mirko (Post 290330)
Hi,
I am trying to figure out how to solve a temperature conduction problem between two solids using chtMultiRegionFoam. There are no fluids in this problem.

I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is:
constant/solid1/polymesh/boundary file:
Code:

    solid1_to_solid2
    {
        type            directMappedWall;
        nFaces          10;
        startFace      390;
        sampleMode      nearestPatchFace;
        sampleRegion    solid2;
        samplePatch    solid2_to_solid1;
        offset          (0 0 0);
    }

and 0/solid1/T file:
Code:

    solid1_to_solid2
    {
        type            solidWallMixedTemperatureCoupled;
        value          uniform 300;
        neighbourFieldName T;
        K              K;
    }

That's it! Hope it helps.
mad

mirko January 14, 2011 15:10

Quote:

Originally Posted by maddalena (Post 290442)
Hi Mirko,

I run a case like that as well, and the solution is as expected (at least in the temperature distribution). What I have is:
constant/solid1/polymesh/boundary file:
Code:

    solid1_to_solid2
    {
        type            directMappedWall;
        nFaces          10;
        startFace      390;
        sampleMode      nearestPatchFace;
        sampleRegion    solid2;
        samplePatch    solid2_to_solid1;
        offset          (0 0 0);
    }

and 0/solid1/T file:
Code:

    solid1_to_solid2
    {
        type            solidWallMixedTemperatureCoupled;
        value          uniform 300;
        neighbourFieldName T;
        K              K;
    }

That's it! Hope it helps.
mad

Thank you!

Yep, it helped me track down an incorrect entry in the changeDictionary/dictionaryReplacement/boundary/X_to_Y. I had incorrectly set the sampleRegion as X instead of Y.

I also used the coupling boundary condition compressible::turbulentTemperatureCoupledBaffle (I don't have a clue why that name. Looking at it's .H file the coupling condition looks very general).

Mirko

maddalena January 17, 2011 03:28

Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad

maddalena January 17, 2011 10:48

link
 
posted something on the subject here: http://www.cfd-online.com/Forums/ope...tml#post290772

mad

mirko January 17, 2011 12:00

Quote:

Originally Posted by maddalena (Post 290680)
Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad

I want to cleanup my setup & generate some benchmark cases. I will then post my setup and results.

Mirko

mirko January 19, 2011 18:58

2 Attachment(s)
Quote:

Originally Posted by maddalena (Post 290680)
Hi Mirko,
could you post the temperature change in time of some points of your domain and compare them with theoretical time variation? I have some doubts on results I have obtained so far...
Thank you

mad

Hi Maddalena,

(got busy with paperwork)

Unfortunately, I managed to break my two-region problem and loose the temperature connectivity across the interface.

FWIW I am attaching two archives:
  1. The broken two region problem that illustrates my predicament
  2. A simple 1D thermal conduction problem that I wanted to use for benchmarking of the above model. This is a very unphysical one: temperatures between 0 & 1. This simple model is working.
Thanks,

Mirko


All times are GMT -4. The time now is 13:53.