Issues with creating "regions" for conjugate heat transfer problem!!

vabishek · April 22, 2015, 12:25

Dear OpenFOAMers,

I am relatively new to the world of OpenFOAM. I am currently working on a problem that involves conjugate heat transfer. I have attached two PDFs that show snapshots of the geometry I am dealing with. I have ONE fluid region and FOUR solid regions surrounding it. The material properties of the solid regions are same except that a heat source is applied to two of these regions. The momentum equations are solved in the fluid region, while the energy equation is solved in both the fluid and solid regions.

I created the regions using blockMesh. I have the following issues:

1. In the case of original_geo.pdf, the problem seems to be with the creation of defaultFaces at the interface of the fluid-solid regions i.e. Region 1- Region 3 , Region1-Region 2 and so on. This happens as the regions on either side cannot "see" the face b/w the regions and hence default patches are created. This is not ideal as I need the temperature at the interface to be coupled.

2. As a workaround, I split the fluid region into two regions as shown in "Modified_geo".pdf. However, in this case the velocity is not continuous b/w the two fluid regions. The temperature coupling works fine in this case, though.

I am not sure how to work around this issue. Any help/suggestion would be greatly appreciated.

Thanks!!

zhengzh5 · April 22, 2015, 19:58

Quote:

Originally Posted by vabishek

Dear OpenFOAMers,

I am relatively new to the world of OpenFOAM. I am currently working on a problem that involves conjugate heat transfer. I have attached two PDFs that show snapshots of the geometry I am dealing with. I have ONE fluid region and FOUR solid regions surrounding it. The material properties of the solid regions are same except that a heat source is applied to two of these regions. The momentum equations are solved in the fluid region, while the energy equation is solved in both the fluid and solid regions.

I created the regions using blockMesh. I have the following issues:

1. In the case of original_geo.pdf, the problem seems to be with the creation of defaultFaces at the interface of the fluid-solid regions i.e. Region 1- Region 3 , Region1-Region 2 and so on. This happens as the regions on either side cannot "see" the face b/w the regions and hence default patches are created. This is not ideal as I need the temperature at the interface to be coupled.

2. As a workaround, I split the fluid region into two regions as shown in "Modified_geo".pdf. However, in this case the velocity is not continuous b/w the two fluid regions. The temperature coupling works fine in this case, though.

I am not sure how to work around this issue. Any help/suggestion would be greatly appreciated.

Thanks!!

i assume you used blockMesh-TopoSet-splitMeshRegion combination to create your 5-regions mesh.

in your blockMesh, create it as if there's 6 regions (basically what you did in the modified geometry), but then inside topoSet, make sure you combine the 2 fluid regions into one. This way, your fluid region will have 4 patches (one shared with each solid region). and patches will be defined properly between regions.

Have you tried that?

thiagopl · April 23, 2015, 08:54

Hi vabishek,

I think this tutorial will help you in creating your regions. It is the best tutorial on chtMultiRegion I've found.

Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0

Regards,

vabishek · April 23, 2015, 10:07

Quote:

Originally Posted by zhengzh5

i assume you used blockMesh-TopoSet-splitMeshRegion combination to create your 5-regions mesh.

in your blockMesh, create it as if there's 6 regions (basically what you did in the modified geometry), but then inside topoSet, make sure you combine the 2 fluid regions into one. This way, your fluid region will have 4 patches (one shared with each solid region). and patches will be defined properly between regions.

Have you tried that?

Hello Jace,

Thanks for replying. Yes, I did try that but I was unsuccessful. It probably has to do with how I defined the regions in both blockMesh and toposetDict files. I have attached the files. I have a feeling that the way I define the regions in blockMesh is preventing me from creating the regions using topoSet. I have also attached a log file that contains the error I get when running splitMeshRegions after running blockMesh and topoSet.

vabishek · April 23, 2015, 10:10

Quote:

Originally Posted by thiagopl

Hi vabishek,

I think this tutorial will help you in creating your regions. It is the best tutorial on chtMultiRegion I've found.

Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0

Regards,

Hi Thiago,

Thanks for the link. I also think it is one of the best out of there. It was the first tutorials I went through when I started learning about CHT. I pretty much tried to follow it, but haven't had any luck.

zhengzh5 · April 23, 2015, 17:11

Quote:

Originally Posted by vabishek

Hello Jace,

Thanks for replying. Yes, I did try that but I was unsuccessful. It probably has to do with how I defined the regions in both blockMesh and toposetDict files. I have attached the files. I have a feeling that the way I define the regions in blockMesh is preventing me from creating the regions using topoSet. I have also attached a log file that contains the error I get when running splitMeshRegions after running blockMesh and topoSet.

here's your solution:

blockMeshDict

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(

   (-0.00259  0.0578 0.000279)  //0
   (-0.00114  0.0578 0.000279)  //1
   (-0.00114  0.069  0.000279)  //2
   (-0.0031   0.069  0.000279)  //3
   (0.00114  0.0578 0.000279)	//4
   (0.00114  0.069  0.000279)   //5
   (0.00259  0.0578 0.000279)   //6 
   (0.0031  0.069  0.000279)    //7

   (0.00114  0.0578 0.000803)   //8
   (0.00259  0.0578 0.000803)   //9
   (0.0031   0.069  0.000803)   //10
   (0.00114  0.069  0.000803)   //11
   (-0.00259  0.0578 0.000803)  //12
   (-0.00114  0.0578 0.000803)  //13
   (-0.00114  0.069  0.000803)  //14
   (-0.0031   0.069  0.000803)  //15

   (-0.00114 0.0578 0.000889)   //16
   (0.00114  0.0578 0.000889)   //17
   (0.00114  0.069  0.000889)   //18
   (-0.00114 0.069  0.000889)   //19
   (-0.00259  0.0578 0.000889)  //20
   (-0.0031   0.069  0.000889)  //21
   (0.00259  0.0578 0.000889)   //22
   (0.0031   0.069  0.000889)   //23
);

blocks
(
    hex (13 8 11 14 16 17 18 19)  (30 30 30)    simpleGrading (1 1 1) 
    hex (1 4 5 2 13 8 11 14)      (30 30 30)    simpleGrading (1 1 1)
    hex (12 13 14 15 20 16 19 21) (30 30 30)    simpleGrading (1 1 1)
    hex (8 9 10 11 17 22 23 18)   (30 30 30)    simpleGrading (1 1 1)
    hex (0 1 2 3 12 13 14 15)     (30 30 30)    simpleGrading (1 1 1)
    hex (4 6 7 5 8 9 10 11)       (30 30 30)    simpleGrading (1 1 1)
); 

edges
(
);

boundary
(
  leftWall
  {
   type patch;
   faces
   (
    (0 12 15 3)
    (12 20 21 15)
   );
  }

  rightWall
  {
   type patch;
   faces
   (
    (6 9 10 7)
    (9 22 23 10)
   );
  }
 
   
  topWall
  {
   type patch;
   faces
   (
    //top
    (20 16 19 21)
    (16 17 18 19)
    (17 22 23 18)
   );
  }

  bottomWall
  {
   type patch;
   faces
   (
    (0 1 2 3)
    (1 4 5 2)
    (4 6 7 5)
   );
  }
   Inlet
  {
   type patch;
   faces
   (
    (0 1 13 12)
    (12 13 16 20)
    (1 4 8 13)
    (13 8 17 16)
    (4 6 9 8)
    (8 9 22 17)
     
   );
  }
  
  Outlet
  {
   type patch;
   faces
   (
     (15 14 2 3)
     (21 19 14 15)
     (14 11 5 2)
     (19 18 11 14)
     (11 10 7 5)
     (18 23 10 11)
        
   );
  }
);

mergeMatchPairs();
mergePatchPairs();
// ************************************************************************* //

topoSetDict

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
    // Heater
    {
        name    block1;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-0.00114 0.0578 0.000803 )(0.00114 0.069 0.000889);
        }
    }
    {
        name    block1;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (-0.00114 0.0578 0.000279)(0.00114 0.069 0.000803);
        }
    }
    {
        name    block1;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block1;           // name of cellSet
        }
    }

    // leftSolid
    {
        name    block2;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-0.0031 0.0578 0.000803 )(-0.00114 0.069 0.000889);
        }
    }
    {
        name    block2;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block2;
        }
    }

    // rightSolid
    {
        name    block3;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0.00114 0.0578 0.000803 )(0.0031 0.069 0.000889);
        }
    }
    {
        name    block3;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block3;
        }
    }

    // topAir
    {
        name    block4;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
	  box (-0.0031 0.0578 0.000279 )(-0.00114 0.069 0.000803);
        }
    }
    {
        name    block4;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block4;
        }
    }


    // bottomWater is all the other cells
    {
        name    block5;
        type    cellZoneSet;
        action  clear;
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block1;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block2;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block3;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block4;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  invert;
    }
    {
        name    block5;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block5;
        }
    }
);

// ************************************************************************* //

then run the following commands:

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite
paraFoam -touchAll

and view with paraview.

Good luck.

vabishek · April 23, 2015, 17:23

Quote:

Originally Posted by zhengzh5

here's your solution:

blockMeshDict

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;

vertices
(

   (-0.00259  0.0578 0.000279)  //0
   (-0.00114  0.0578 0.000279)  //1
   (-0.00114  0.069  0.000279)  //2
   (-0.0031   0.069  0.000279)  //3
   (0.00114  0.0578 0.000279)    //4
   (0.00114  0.069  0.000279)   //5
   (0.00259  0.0578 0.000279)   //6 
   (0.0031  0.069  0.000279)    //7

   (0.00114  0.0578 0.000803)   //8
   (0.00259  0.0578 0.000803)   //9
   (0.0031   0.069  0.000803)   //10
   (0.00114  0.069  0.000803)   //11
   (-0.00259  0.0578 0.000803)  //12
   (-0.00114  0.0578 0.000803)  //13
   (-0.00114  0.069  0.000803)  //14
   (-0.0031   0.069  0.000803)  //15

   (-0.00114 0.0578 0.000889)   //16
   (0.00114  0.0578 0.000889)   //17
   (0.00114  0.069  0.000889)   //18
   (-0.00114 0.069  0.000889)   //19
   (-0.00259  0.0578 0.000889)  //20
   (-0.0031   0.069  0.000889)  //21
   (0.00259  0.0578 0.000889)   //22
   (0.0031   0.069  0.000889)   //23
);

blocks
(
    hex (13 8 11 14 16 17 18 19)  (30 30 30)    simpleGrading (1 1 1) 
    hex (1 4 5 2 13 8 11 14)      (30 30 30)    simpleGrading (1 1 1)
    hex (12 13 14 15 20 16 19 21) (30 30 30)    simpleGrading (1 1 1)
    hex (8 9 10 11 17 22 23 18)   (30 30 30)    simpleGrading (1 1 1)
    hex (0 1 2 3 12 13 14 15)     (30 30 30)    simpleGrading (1 1 1)
    hex (4 6 7 5 8 9 10 11)       (30 30 30)    simpleGrading (1 1 1)
); 

edges
(
);

boundary
(
  leftWall
  {
   type patch;
   faces
   (
    (0 12 15 3)
    (12 20 21 15)
   );
  }

  rightWall
  {
   type patch;
   faces
   (
    (6 9 10 7)
    (9 22 23 10)
   );
  }
 
   
  topWall
  {
   type patch;
   faces
   (
    //top
    (20 16 19 21)
    (16 17 18 19)
    (17 22 23 18)
   );
  }

  bottomWall
  {
   type patch;
   faces
   (
    (0 1 2 3)
    (1 4 5 2)
    (4 6 7 5)
   );
  }
   Inlet
  {
   type patch;
   faces
   (
    (0 1 13 12)
    (12 13 16 20)
    (1 4 8 13)
    (13 8 17 16)
    (4 6 9 8)
    (8 9 22 17)
     
   );
  }
  
  Outlet
  {
   type patch;
   faces
   (
     (15 14 2 3)
     (21 19 14 15)
     (14 11 5 2)
     (19 18 11 14)
     (11 10 7 5)
     (18 23 10 11)
        
   );
  }
);

mergeMatchPairs();
mergePatchPairs();
// ************************************************************************* //

topoSetDict

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
    // Heater
    {
        name    block1;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-0.00114 0.0578 0.000803 )(0.00114 0.069 0.000889);
        }
    }
    {
        name    block1;
        type    cellSet;
        action  add;
        source  boxToCell;
        sourceInfo
        {
            box (-0.00114 0.0578 0.000279)(0.00114 0.069 0.000803);
        }
    }
    {
        name    block1;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block1;           // name of cellSet
        }
    }

    // leftSolid
    {
        name    block2;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (-0.0031 0.0578 0.000803 )(-0.00114 0.069 0.000889);
        }
    }
    {
        name    block2;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block2;
        }
    }

    // rightSolid
    {
        name    block3;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
            box (0.00114 0.0578 0.000803 )(0.0031 0.069 0.000889);
        }
    }
    {
        name    block3;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block3;
        }
    }

    // topAir
    {
        name    block4;
        type    cellSet;
        action  new;
        source  boxToCell;
        sourceInfo
        {
      box (-0.0031 0.0578 0.000279 )(-0.00114 0.069 0.000803);
        }
    }
    {
        name    block4;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block4;
        }
    }


    // bottomWater is all the other cells
    {
        name    block5;
        type    cellZoneSet;
        action  clear;
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block1;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block2;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block3;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  add;
        source  cellToCell;
        sourceInfo
        {
            set block4;
        }
    }
    {
        name    block5;
        type    cellSet;
        action  invert;
    }
    {
        name    block5;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set block5;
        }
    }
);

// ************************************************************************* //

then run the following commands:

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite
paraFoam -touchAll

and view with paraview.

Good luck.

Thanks a lot, Jace. Works like a charm.

April 23, 2015, 08:54		#3
thiagopl Member Thiago Parente Lima Join Date: Sep 2011 Location: Diamantina, Brazil. Posts: 65 Rep Power: 15	Hi vabishek, I think this tutorial will help you in creating your regions. It is the best tutorial on chtMultiRegion I've found. Tutorial to set up a case for chtMultiRegionFoam in OpenFOAM 2.0.0 Regards, __________________ Fields of interest: buoyantFoam, chtMultRegionFoam.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Heat transfer problem at nucleate boiling	MrStuebb	FLUENT	12	March 14, 2017 14:31
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 07:28
Heat Transfer mechanisms	tafaugl	CFX	1	November 7, 2012 19:46
Wall heat transfer coefficient (HTC) problem	Mohamed khamis	CFX	1	January 16, 2010 00:12
How can I increase Heat Transfer at Domain Interf?	B.Simon	CFX	3	October 28, 2008 19:53