[RaghavendraRohith]

Hi All,

I am trying to model a heat transfer problem for an adjacently placed meshes contacting through a patch. I need to define a heat transfer boundary condition on this patch to enhance the heat transfer between Mesh 1 and Mesh 2. I have also worked with chtMultiRegionFoam previously. This experience didnot help me as i am trying to solve incompressible flow and also using different meshes and volume scalar field. chtMultiRegionFoam helps in modelling heat transfer through mappedPatchBase called baffle between the meshes considered as boundaries. My geometries are complicated so i cannot use baffles.

I have searched some probabilties in interpolating or mapping volScalarField of one mesh to another. Can some body help me in modelling heat transfer using GroovyBC or by some other method by using meshToMesh etc.

Did somebody work on such complications.


Thanks in Advance.
Rohith

[ancolli]

Could u solve ur problem?

[Zeppo]

What's wrong with chtMultiRegionFoam? It seems to be ok in solving that kind of problem. And yes, "coupled" meshes shouldn't even be perfectly conformal - mapped boundary conditions can care for this.

[ancolli]

Originally Posted by Zeppo

What's wrong with chtMultiRegionFoam? It seems to be ok in solving that kind of problem. And yes, "coupled" meshes shouldn't even be perfectly conformal - mapped boundary conditions can care for this.

There are not problems with chtMultiRegionFoam, but how to use GroovyBC with differents regions is my key question. Do u know how to use it?

[Zeppo]

The thread starter said they want to model heat transfer between two mesh regions but they couldn't use chtMultiRegionFoam as the geometry they dealt with was very complex. I don't see how complexity of geometric model can prevent anyone from using chtMultiRegionFoam. Moreover, I can't see why bother with groovyBC, why not use turbulentTemperatureRadCoupledMixedFvPatchScalarFi eld as boundary conditions.

[ancolli]

Originally Posted by Zeppo

The thread starter said they want to model heat transfer between two mesh regions but they couldn't use chtMultiRegionFoam as the geometry they dealt with was very complex. I don't see how complexity of geometric model can prevent anyone from using chtMultiRegionFoam. Moreover, I can't see why bother with groovyBC, why not use turbulentTemperatureRadCoupledMixedFvPatchScalarFi eld as boundary conditions.

Well, in my case for several reasons.
1) I am using a simplified version of that solver, then turbulentTemperatureRadCoupledMixedFvPatchScalarFi eld is to complex and slow. If i use groovyBC with fluxa=fluxb and Ta=Tb, is converging far faster for a 1D problem.
2), I need to use another BC, Fluxa=fluxb but Ta a non linear function of Tb.
the problem with groovyBC is that i can not use it for a 2d or 3d problem, since it is taken an average flux and temperature in the complete boundary patch between 2 regions.
Do u know how to solve that?

[Zeppo]

What turbulentTemperatureRadCoupledMixedFvPatchScalarFi eld basically does is equalizing the fluxes from the left and right sides of an interface between regions. Poor performance (slow convergence) is caused by the fact that equalizing the fluxes is done in a segregated way: solve equations in regions alternately, one after another with explicit coupling on boundaries. I don't think groovyBC can help you overcome it.

Maybe you can adapt the code to your needs:
https://cpp.openfoam.org/v3/a10477_source.html#l00174

[ancolli]

Originally Posted by Zeppo

What turbulentTemperatureRadCoupledMixedFvPatchScalarFi eld basically does is equalizing the fluxes from the left and right sides of an interface between regions. Poor performance (slow convergence) is caused by the fact that equalizing the fluxes is done in a segregated way: solve equations in regions alternately, one after another with explicit coupling on boundaries. I don't think groovyBC can help you overcome it.

Maybe you can adapt the code to your needs:
https://cpp.openfoam.org/v3/a10477_source.html#l00174

in fact, I tried with turbulentTemperatureCoupledBaffleMixed coming by default in the chtmultiregionfoam tutorial. if i run my simple solver (laplace eq. in two regions) in 1D, with groovy takes 6 iterations, with turbulentTemperatureCoupledMixed 700 to reach the same final solution, starting from the same initial guess.
Addapting the code to my needs will take a lot of time TO ME. Is something that I will TRY to do just if i can not do what i need in an easy and fast way (groovyBC).
But thanks for the suggestion and for the time. I will try to improve my c++ undertanding....

[Zeppo]

How do you setup boundary conditions with groovyBC? What's in your 0/T file?

update: now i see your other thread where you explained the problem with groovyBC: https://www.cfd-online.com/Forums/op...r-regions.html

Unfortunatly, I have near to zero experience with groovyBC. You could probably ask Bernhard Gschaider (the core developer of groovyBC) for some help.

[ancolli]

Originally Posted by Zeppo

How do you setup boundary conditions with groovyBC? What's in your 0/T file?

update: now i see your other thread where you explained the problem with groovyBC: https://www.cfd-online.com/Forums/op...r-regions.html

Unfortunatly, I have near to zero experience with groovyBC. You could probably ask Bernhard Gschaider (the core developer of groovyBC) for some help.

yes, i am usign Dirichlet–Neumann partitioning
fluid BC in 0/Fluid/T:

  
"fluid_to_.*"
            {
        	type            groovyBC;
		gradientExpression "0";
		fractionExpression "1";
		valueExpression	"Ts";
		variables "Ts{solid_to_fluid/solid}=Tsolid;";
		value           $internalField;
            };

solid BC in 0/Solid/T:

 
"solid_to_.*"
            {
		type            groovyBC;
	
		gradientExpression "der";
		fractionExpression "0";
		valueExpression	"0";
		variables "der{fluid_to_solid/fluid}=-1/40*snGrad(Tfluid);";
		value           $internalField;
            };

about asking to Bernhard Gschaider, he already replied in other thread and I do not want to bother people (he has others things to do), he suggested replace {fluid_to_solid/fluid} (that works just in 1D since is averaging the field in the whole patch) by using mapped or neighbourField functions. (but, he is not sure whether this will work with mult-region cases). i tryed, but i groovyBC can not detect the other region without adding {fluid_to_solid/fluid} or at least i do not know where i am making a mistake.