CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

need help with conjugate heat transfer

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   February 19, 2014, 12:31
Default need help with conjugate heat transfer
  #1
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 5
skuznet is on a distinguished road
Hello Foamers!

I want to solve the conjugate heat transfer problem using chtMutiRegionFoam or chtMultiRegionSimpleFoam. It is a solid lattice with fluid flowing in the pores (please see the first picture attached).
I've generated solid and fluid meshes independently from STL geometry in HelyxOS (2nd and 3rd pictures). I defined interaction surface and other surfaces and set BC and used water properties from the tutorial chtMultiRegionFoam/multiRegionLiquidHeater
I was able to set up the case and it runs, however it gives non physical results.

Can any one tell me what I'm doing wrong?
Can I use non-comformal mesh? The mesh for solid and for fluid were generated intependently, therefor cell surfaces do not coincide.

Here is my case (its heavy, 93 megs):
chtMultiRegion Foam https://dl.dropboxusercontent.com/u/...tWaterH.tar.gz
chtMultiRegionSimpleFoam: https://dl.dropboxusercontent.com/u/..._Simple.tar.gz

Thank you!
Attached Images
File Type: jpg UCSmall.jpg (93.9 KB, 25 views)
File Type: jpg UCSolidMesh.jpg (76.2 KB, 20 views)
File Type: jpg UCFluidMesh.jpg (97.0 KB, 17 views)
skuznet is offline   Reply With Quote

Old   February 19, 2014, 14:33
Default
  #2
Member
 
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 7
zhengzh5 is on a distinguished road
Quote:
Originally Posted by skuznet View Post
Hello Foamers!

I want to solve the conjugate heat transfer problem using chtMutiRegionFoam or chtMultiRegionSimpleFoam. It is a solid lattice with fluid flowing in the pores (please see the first picture attached).
I've generated solid and fluid meshes independently from STL geometry in HelyxOS (2nd and 3rd pictures). I defined interaction surface and other surfaces and set BC and used water properties from the tutorial chtMultiRegionFoam/multiRegionLiquidHeater
I was able to set up the case and it runs, however it gives non physical results.

Can any one tell me what I'm doing wrong?
Can I use non-comformal mesh? The mesh for solid and for fluid were generated intependently, therefor cell surfaces do not coincide.

Here is my case (its heavy, 93 megs):
chtMultiRegion Foam https://dl.dropboxusercontent.com/u/...tWaterH.tar.gz
chtMultiRegionSimpleFoam: https://dl.dropboxusercontent.com/u/..._Simple.tar.gz

Thank you!
Hey, I think chtMultiRegionFoam requires conform mesh between regions, since it doesn't employ any AMI treatment. (someone please correct me if this is not the case.)

Since you have mesh the stl files independently, you must have the proper set up for the snappyHexMeshDict for each mesh, why not try to combine them, define cellZone for each stl-file, and mesh them together to get conformal boundary patches between the regions. Worth a try I think.

good luck!
zhengzh5 is offline   Reply With Quote

Old   February 19, 2014, 14:47
Default
  #3
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 5
skuznet is on a distinguished road
Thank you for your reply. Can you give me idea how can it do it - create conformal mesh. Can I do it in HelyxOS?
skuznet is offline   Reply With Quote

Old   February 19, 2014, 17:57
Default
  #4
Member
 
Jace
Join Date: Oct 2012
Posts: 77
Rep Power: 7
zhengzh5 is on a distinguished road
Quote:
Originally Posted by skuznet View Post
Thank you for your reply. Can you give me idea how can it do it - create conformal mesh. Can I do it in HelyxOS?
my snappyHexMeshDict:

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      autoHexMeshDict;
}

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

// Which of the steps to run
castellatedMesh true;
snap            true;
addLayers       false;


// Geometry. Definition of all surfaces. All surfaces are of class
// searchableSurface.
// Surfaces are used
// - to specify refinement for any mesh cell intersecting it
// - to specify refinement for any mesh cell inside/outside/near
// - to 'snap' the mesh boundary to the surface
geometry
{
    coolant.stl
    {
        type triSurfaceMesh;
	name coolant;
    }

    engine.stl
      {
    	type triSurfaceMesh;
    	name engine;
      }

    air.stl
      {
	type triSurfaceMesh;
	name air;
      }
};



// Settings for the castellatedMesh generation.
castellatedMeshControls
{

    // Refinement parameters
    // ~~~~~~~~~~~~~~~~~~~~~

    // If local number of cells is >= maxLocalCells on any processor
    // switches from from refinement followed by balancing
    // (current method) to (weighted) balancing before refinement.
    maxLocalCells 1000000;

    // Overall cell limit (approximately). Refinement will stop immediately
    // upon reaching this number so a refinement level might not complete.
    // Note that this is the number of cells before removing the part which
    // is not 'visible' from the keepPoint. The final number of cells might
    // actually be a lot less.
    maxGlobalCells 2000000;

    // The surface refinement loop might spend lots of iterations
    // refining just a few cells. This setting will cause refinement
    // to stop if <= minimumRefine are selected for refinement. Note:
    // it will at least do one iteration (unless the number of cells
    // to refine is 0)
    minRefinementCells 10;

    // Number of buffer layers between different levels.
    // 1 means normal 2:1 refinement restriction, larger means slower
    // refinement.
    nCellsBetweenLevels 2;



    // Explicit feature edge refinement
    // ~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

    // Specifies a level for any cell intersected by its edges.
    // This is a featureEdgeMesh, read from constant/triSurface for now.
    features
    (
        {
            file "coolant.eMesh";
	    level 0;
            //levels ((0 2)(1.5 1)(3 0));
        }

	{
	  file "engine.eMesh";
	  level 0;	
	}

	{
	  file "air.eMesh";
	  level 0;	
	}
       
    );



    // Surface based refinement
    // ~~~~~~~~~~~~~~~~~~~~~~~~

    // Specifies two levels for every surface. The first is the minimum level,
    // every cell intersecting a surface gets refined up to the minimum level.
    // The second level is the maximum level. Cells that 'see' multiple
    // intersections where the intersections make an
    // angle > resolveFeatureAngle get refined up to the maximum level.

    refinementSurfaces
    {
        coolant
        {
	  // Surface-wise min and max refinement level
	  level (0 2);

	  faceZone coolant;
	  cellZone coolant;
	  cellZoneInside inside;
        }

	engine
	  {
	    level (0 2);
	    faceZone engine;
	    cellZone engine;
	    cellZoneInside inside;
	  }
	air
	  {
	    level (0 2);
	    faceZone air;
	    cellZone air;
	    cellZoneInside inside;
	  }
       
    }

    // Resolve sharp angles
    resolveFeatureAngle 30;


    // Region-wise refinement
    // ~~~~~~~~~~~~~~~~~~~~~~

    // Specifies refinement level for cells in relation to a surface. One of
    // three modes
    // - distance. 'levels' specifies per distance to the surface the
    //   wanted refinement level. The distances need to be specified in
    //   descending order.
    // - inside. 'levels' is only one entry and only the level is used. All
    //   cells inside the surface get refined up to the level. The surface
    //   needs to be closed for this to be possible.
    // - outside. Same but cells outside.

    refinementRegions
    {
        //refinementBox
        //{
        //    mode inside;
        //    levels ((1E15 4));
        //}
    }


    // Mesh selection
    // ~~~~~~~~~~~~~~

    // After refinement patches get added for all refinementSurfaces and
    // all cells intersecting the surfaces get put into these patches. The
    // section reachable from the locationInMesh is kept.
    // NOTE: This point should never be on a face, always inside a cell, even
    // after refinement.
    locationInMesh (0.001 -12.501 0.001);
    //locationInMesh (0.1 0.1 0.1);

    // Whether any faceZones (as specified in the refinementSurfaces)
    // are only on the boundary of corresponding cellZones or also allow
    // free-standing zone faces. Not used if there are no faceZones.
    allowFreeStandingZoneFaces false;
}



// Settings for the snapping.
snapControls
{
    //- Number of patch smoothing iterations before finding correspondence
    //  to surface
    nSmoothPatch 3;

    //- Relative distance for points to be attracted by surface feature point
    //  or edge. True distance is this factor times local
    //  maximum edge length.
    tolerance 1.0;

    //- Number of mesh displacement relaxation iterations.
    nSolveIter 30;

    //- Maximum number of snapping relaxation iterations. Should stop
    //  before upon reaching a correct mesh.
    nRelaxIter 5;

    //- Highly experimental and wip: number of feature edge snapping
    //  iterations. Leave out altogether to disable.
    //  Of limited use in this case since faceZone faces not handled.
    nFeatureSnapIter 10;

    explicitFeatureSnap true;
    implicitFeatureSnap false;
    multiRegionFeatureSnap true;
}



// Settings for the layer addition.
addLayersControls
{
    relativeSizes true;

    // Per final patch (so not geometry!) the layer information
    layers
    {
        maxY
        {
            nSurfaceLayers 3;
        }
    }

    // Expansion factor for layer mesh
    expansionRatio 1.3;

    // Wanted thickness of final added cell layer. If multiple layers
    // is the thickness of the layer furthest away from the wall.
    // Relative to undistorted size of cell outside layer.
    finalLayerThickness 1;

    // Minimum thickness of cell layer. If for any reason layer
    // cannot be above minThickness do not add layer.
    // Relative to undistorted size of cell outside layer.
    minThickness 0.1;

    // If points get not extruded do nGrow layers of connected faces that are
    // also not grown. This helps convergence of the layer addition process
    // close to features.
    // Note: changed(corrected) w.r.t 17x! (didn't do anything in 17x)
    nGrow 0;

    // Advanced settings

    // When not to extrude surface. 0 is flat surface, 90 is when two faces
    // are perpendicular
    featureAngle 30;

    // Maximum number of snapping relaxation iterations. Should stop
    // before upon reaching a correct mesh.
    nRelaxIter 3;

    // Number of smoothing iterations of surface normals
    nSmoothSurfaceNormals 1;

    // Number of smoothing iterations of interior mesh movement direction
    nSmoothNormals 3;

    // Smooth layer thickness over surface patches
    nSmoothThickness 2;

    // Stop layer growth on highly warped cells
    maxFaceThicknessRatio 0.5;

    // Reduce layer growth where ratio thickness to medial
    // distance is large
    maxThicknessToMedialRatio 1;

    // Angle used to pick up medial axis points
    // Note: changed(corrected) w.r.t 17x! 90 degrees corresponds to 130 in 17x.
    minMedianAxisAngle 90;

    // Create buffer region for new layer terminations
    nBufferCellsNoExtrude 0;

    // Overall max number of layer addition iterations. The mesher will exit
    // if it reaches this number of iterations; possibly with an illegal
    // mesh.
    nLayerIter 50;
}



// Generic mesh quality settings. At any undoable phase these determine
// where to undo.
meshQualityControls
{
    //- Maximum non-orthogonality allowed. Set to 180 to disable.
    maxNonOrtho 80;

    //- Max skewness allowed. Set to <0 to disable.
    maxBoundarySkewness 20;
    maxInternalSkewness 4;

    //- Max concaveness allowed. Is angle (in degrees) below which concavity
    //  is allowed. 0 is straight face, <0 would be convex face.
    //  Set to 180 to disable.
    maxConcave 80;

    //- Minimum pyramid volume. Is absolute volume of cell pyramid.
    //  Set to very negative number (e.g. -1E30) to disable.
    minVol 0;

    //- Minimum quality of the tet formed by the face-centre
    //  and variable base point minimum decomposition triangles and
    //  the cell centre.  Set to very negative number (e.g. -1E30) to
    //  disable.
    //     <0 = inside out tet,
    //      0 = flat tet
    //      1 = regular tet
    minTetQuality 1e-30;

    //- Minimum face area. Set to <0 to disable.
    minArea -1;

    //- Minimum face twist. Set to <-1 to disable. dot product of face normal
    //- and face centre triangles normal
    minTwist 0.02;

    //- minimum normalised cell determinant
    //- 1 = hex, <= 0 = folded or flattened illegal cell
    minDeterminant 0.001;

    //- minFaceWeight (0 -> 0.5)
    minFaceWeight 0.02;

    //- minVolRatio (0 -> 1)
    minVolRatio 0.01;

    //must be >0 for Fluent compatibility
    minTriangleTwist -1;


    // Advanced

    //- Number of error distribution iterations
    nSmoothScale 4;
    //- amount to scale back displacement at error points
    errorReduction 0.75;
}


// Advanced

// Flags for optional output
// 0 : only write final meshes
// 1 : write intermediate meshes
// 2 : write volScalarField with cellLevel for postprocessing
// 4 : write current intersections as .obj files
debug 0;


// Merge tolerance. Is fraction of overall bounding box of initial mesh.
// Note: the write tolerance needs to be higher than this.
mergeTolerance 1e-6;


// ************************************************************************* //
I have highlighted the interesting parts in red, you can rename those *.stl accordingly. Once the mesh is properly created, you can use

Code:
splitMeshRegions -cellZones -overwrite
to split the mesh into individual regions.

Good luck!
zhengzh5 is offline   Reply With Quote

Old   February 19, 2014, 21:57
Default
  #5
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 5
skuznet is on a distinguished road
Jace, thank you for posting it!

I'm going to try it now.

What are the *.eMesh files? Where do you get them from?

Also I can see you are using coolant in your case. Is it liquid? Which thermophysical model do you use?
skuznet is offline   Reply With Quote

Old   February 21, 2014, 13:29
Default
  #6
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 5
skuznet is on a distinguished road
Jace,

it looks like AMI is being used.
http://www.openfoam.org/version2.1.0/ami.php
skuznet is offline   Reply With Quote

Old   February 26, 2014, 16:52
Default
  #7
Member
 
Sergey
Join Date: Nov 2013
Posts: 87
Rep Power: 5
skuznet is on a distinguished road
Jace, thank you for the help! I was able to mesh both regions simultaneously, now have conformal mesh!
skuznet is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Question about heat transfer coefficient setting for CFX Anna Tian CFX 1 June 16, 2013 06:28
Error finding variable "THERMX" sunilpatil CFX 8 April 26, 2013 07:00
Heat Flux at wall in a conjugate heat transfer problem Chander CFX 2 July 9, 2011 22:22
Convective / Conductive Heat Transfer in Hypersonic flows enigma Main CFD Forum 2 November 1, 2009 23:53
Convective Heat Transfer - Heat Exchanger Mark CFX 6 November 15, 2004 16:55


All times are GMT -4. The time now is 21:09.