[wuyangzhen]

hello everyone,

im a beginner of openfoam. I have already made a case about double pipe heat exchanger with chtMultiRegionSimpleFoam. my case can run, but the result looks not good. i know there must be some mistakes in my case and the simulation time is also particularly short, but i cant find it, can someone help me to check it. so many thanks.

My case:

inner pipe (bottomWater): inner diameter 0.01m, the hot water flows through the inner pipe from pipe right to pipe left, the inlet temperature of hot water is 333K, velosity of hot water is 0.177m/s, it is transitional flow in inner pipe.
outer pipe (topWater): outer diameter 0.03m, the cold water flows through the outer pipe from pipe left to pipe right, the inlet temperature of cold water is 288K, velosity of cold water is 0.035m/s, it is laminar flow in outer pipe. the outer face of the outer pipe is insulated.
copper (midCopper): copper is the material of the inner pipe that used as a wall separating hot water and cold water. thermal conductivity of copper is 380 w/mk, copper thickness of inner pipe is 0.002m.

Length of pipe is 4.5m

i have updated my case file. no matter what the problem of this case have, please tell me, i will be very grateful.

[piu58]

What solver did you use? What happens if you run the simulation?

[wuyangzhen]

i use chtMultiRegionSimpleFoam. when i run the simulation, it goes well. but the simulation time is too short and the outlet temperature of hot water from the simulation is big difference with experimental data.

experimental data:
inlet temperature of hot water: 333K, outlet temperature of hot water is 318K
inlet temperature of cold water: 288K, outlet temperature of hot water is 298K

simulation result:
inlet temperature of hot water: 333K, outlet temperature of hot water is 299K
inlet temperature of cold water: 288K, outlet temperature of hot water is 298K

[Bloerb]

Attached is a cleaned up version of you case. I'll help you through this, since this is a good example case for heat transfer for many on here. The main things to do are:

Open the blockMesh file and edit the radii and length to your values. Play around with the mesh resolution. Afterwards set the T and U inlet conditions.

Inlet velocity profile
use flowRateInletVelocity and the extrapolatedProfile option or a fixedMean / fixedProfile option. fixedValue sets one constant value over the entire channel. The entry length will falsify your results. In reality the water will enter the heat exchanger with a velocity profile not a constant value. Again set up in the case attached. This is known as the Graetz Problem, make sure to read up on it.

turbulence model
Change your turbulence model to kOmegaSST. IMO this should give you better results for transitional flows. Calculate the inlet values of k and omega and set them accordingly.

mesh
to make sure your results are in good agreement with experimental data you need a resolved boundary layer. The attached blockMesh allows for this kind of refinement via grading. Eyeball the yPlus value and set your values accordingly. You can check with the yPlus function object if you are in the ballpark. For a well resolved boundary yPlus < 1 is a necessity. With values ~30 you should be able to reproduce the experiments.

residuals and convergence
check the residuals and outlet temperature for convergence. Additional function objects are attached. Use foamMonitor to check during run time if these are falling.

 
foamMonitor -l residuals.dat

Change to non constant thermal Properties.
Values for water can be found in the NIST webbook. Change your thermoPhysicalProperties files to polynomials once you were able to create a good solution with constant ones

Check back if there are other questions

[wuyangzhen]

Originally Posted by Bloerb

Attached is a cleaned up version of you case. I'll help you through this, since this is a good example case for heat transfer for many on here. The main things to do are:

Open the blockMesh file and edit the radii and length to your values. Play around with the mesh resolution. Afterwards set the T and U inlet conditions.

Inlet velocity profile
use flowRateInletVelocity and the extrapolatedProfile option or a fixedMean / fixedProfile option. fixedValue sets one constant value over the entire channel. The entry length will falsify your results. In reality the water will enter the heat exchanger with a velocity profile not a constant value. Again set up in the case attached. This is known as the Graetz Problem, make sure to read up on it.

turbulence model
Change your turbulence model to kOmegaSST. IMO this should give you better results for transitional flows. Calculate the inlet values of k and omega and set them accordingly.

mesh
to make sure your results are in good agreement with experimental data you need a resolved boundary layer. The attached blockMesh allows for this kind of refinement via grading. Eyeball the yPlus value and set your values accordingly. You can check with the yPlus function object if you are in the ballpark. For a well resolved boundary yPlus < 1 is a necessity. With values ~30 you should be able to reproduce the experiments.

residuals and convergence
check the residuals and outlet temperature for convergence. Additional function objects are attached. Use foamMonitor to check during run time if these are falling.

 
foamMonitor -l residuals.dat

Change to non constant thermal Properties.
Values for water can be found in the NIST webbook. Change your thermoPhysicalProperties files to polynomials once you were able to create a good solution with constant ones

Check back if there are other questions

Thank you very very much for your time and help.

1. first i edit the radius and length with my value but i cant understand the blockMeshdict that you have made.

convertToMeters 0.001;


// necessary variables
radiusI 5; // inner solid radius in mm
radiusM 7; // outer solid radius in mm
radiusA 15;   // outer fluid radius in mm
length -4500;  //mm
xa 5;   // Netzfeinheit radiale Richtung
ya 10;  // Netzfeinheit Umfangsrichtung
za 100; // Netzfeinheit in Rohrrichtung

// automatically calculated values (i cant understand this part, like 0.30*$radiusI*sin(degToRad(45.0)), what does it mean?)

c1p #calc "0.30*$radiusI*sin(degToRad(45.0))"; 
c2p #calc "0.70*$radiusI*sin(degToRad(45.0))";
c3p #calc "1.00*$radiusI*sin(degToRad(45.0))";
c4p #calc "1.00*$radiusM*sin(degToRad(45.0))";
c5p #calc "1.00*$radiusA*sin(degToRad(45.0))";
c1n #calc "-1.0*$c1p";
c2n #calc "-1.0*$c2p";
c3n #calc "-1.0*$c3p";
c4n #calc "-1.0*$c4p";
c5n #calc "-1.0*$c5p";

PRI #calc "0.25*$radiusI";
NRI #calc "-1.0*$PRI";

PRM #calc "0.70*$radiusI";
NRM #calc "-1.0*$PRM";

PRA #calc "1.00*$radiusI";
NRA #calc "-1.0*$PRA"; 

PRS #calc "1.00*$radiusM";
NRS #calc "-1.0*$PRS"; 

PRB #calc "1.00*$radiusA";
NRB #calc "-1.0*$PRB"; 

   vertices
   (
    // fluidA 
    ($c1n $c1n $length) // 0 
    ($c1p $c1n $length) // 1 
    ($c1p $c1p $length) // 2 
    ($c1n $c1p $length) // 3 

    ($c2n $c2n $length) // 4 
    ($c2p $c2n $length) // 5    
    ($c2p $c2p $length) // 6 
    ($c2n $c2p $length) // 7 

    ($c3n $c3n $length) // 8 
    ($c3p $c3n $length) // 9    
    ($c3p $c3p $length) // 10 
    ($c3n $c3p $length) // 11
     
    ($c1n $c1n 0) // 12       
    ($c1p $c1n 0) // 13
    ($c1p $c1p 0) // 14 
    ($c1n $c1p 0) // 15 
 
    ($c2n $c2n 0) // 16
    ($c2p $c2n 0) // 17    
    ($c2p $c2p 0) // 18
    ($c2n $c2p 0) // 19

    ($c3n $c3n 0) // 20
    ($c3p $c3n 0) // 21     
    ($c3p $c3p 0) // 22
    ($c3n $c3p 0) // 23   
    //solid
    ($c4n $c4n $length) // 24
    ($c4p $c4n $length) // 25   
    ($c4p $c4p $length) // 26 
    ($c4n $c4p $length) // 27  
    
    ($c4n $c4n 0) // 28
    ($c4p $c4n 0) // 29     
    ($c4p $c4p 0) // 30
    ($c4n $c4p 0) // 31    
    // fluidB
    ($c5n $c5n $length) // 32 
    ($c5p $c5n $length) // 33   
    ($c5p $c5p $length) // 34 
    ($c5n $c5p $length) // 35  
    
    ($c5n $c5n 0) // 36
    ($c5p $c5n 0) // 37     
    ($c5p $c5p 0) // 38
    ($c5n $c5p 0) // 39     
   );                

   blocks
   (
    //fluidA Inner 
    hex (0  1  2  3 12 13 14 15) fluidA  ($ya $ya $za) simpleGrading (1 1 1)
    hex (0  4  5  1 12 16 17 13) fluidA  ($xa $ya $za) simpleGrading (1 1 1)
    hex (2  6  7  3 14 18 19 15) fluidA  ($xa $ya $za) simpleGrading (1 1 1)
    hex (1  5  6  2 13 17 18 14) fluidA  ($xa $ya $za) simpleGrading (1 1 1)
    hex (3  7  4  0 15 19 16 12) fluidA  ($xa $ya $za) simpleGrading (1 1 1)    
    // fluidA Boundary Layer
    hex (9  5  4  8 21 17 16 20) fluidA  ($xa $ya $za) simpleGrading (1 1 1)    
    hex (11 7  6 10 23 19 18 22) fluidA  ($xa $ya $za) simpleGrading (1 1 1)    
    hex (10 6  5  9 22 18 17 21) fluidA  ($xa $ya $za) simpleGrading (1 1 1) 
    hex (8  4  7 11 20 16 19 23) fluidA  ($xa $ya $za) simpleGrading (1 1 1)     
    // solid
    hex (25 9  8  24 29 21 20 28) solid  ($xa $ya $za) simpleGrading (1 1 1)    
    hex (26 10 9  25 30 22 21 29) solid  ($xa $ya $za) simpleGrading (1 1 1)    
    hex (27 11 10 26 31 23 22 30) solid  ($xa $ya $za) simpleGrading (1 1 1) 
    hex (24 8  11 27 28 20 23 31) solid  ($xa $ya $za) simpleGrading (1 1 1)  
    // fluidB
    hex (33 25 24 32 37 29 28 36) fluidB ($ya $ya $za) simpleGrading (1 1 1)    
    hex (34 26 25 33 38 30 29 37) fluidB ($ya $ya $za) simpleGrading (1 1 1)    
    hex (35 27 26 34 39 31 30 38) fluidB ($ya $ya $za) simpleGrading (1 1 1) 
    hex (32 24 27 35 36 28 31 39) fluidB ($ya $ya $za) simpleGrading (1 1 1)    
   );

   edges
   ( 
    // fluidA
    arc 0 1     (0    $NRI $length)
    arc 1 2     ($PRI 0    $length)
    arc 2 3     (0    $PRI $length)
    arc 3 0     ($NRI 0    $length) 

    arc 4 5     (0    $NRM $length)
    arc 5 6     ($PRM 0    $length) 
    arc 6 7     (0    $PRM $length)
    arc 7 4     ($NRM 0    $length)
    
    arc 8 9     (0    $NRA $length)
    arc 9 10     ($PRA 0    $length)
    arc 10 11     (0    $PRA $length)
    arc 11 8     ($NRA 0    $length)   
   
    arc 12 13     (0    $NRI 0)
    arc 13 14     ($PRI 0    0)
    arc 14 15     (0    $PRI 0)
    arc 15 12     ($NRI 0    0)

    arc 16 17     (0    $NRM 0)
    arc 17 18     ($PRM 0    0)
    arc 18 19     (0    $PRM 0)
    arc 19 16     ($NRM 0    0)
    
    arc 20 21     (0    $NRA 0)
    arc 21 22     ($PRA 0    0)
    arc 22 23     (0    $PRA 0)
    arc 23 20     ($NRA 0    0)
    // solid
    arc 28 29     (0    $NRS 0)
    arc 29 30     ($PRS 0    0)
    arc 30 31     (0    $PRS 0)
    arc 31 28     ($NRS 0    0)    
    
    arc 24 25     (0    $NRS $length)
    arc 25 26     ($PRS 0    $length)
    arc 26 27     (0    $PRS $length)
    arc 27 24     ($NRS 0    $length)     
    // fluidB
    arc 36 37     (0    $NRB 0)
    arc 37 38     ($PRB 0    0)
    arc 38 39     (0    $PRB 0)
    arc 39 36     ($NRB 0    0)    
    
    arc 32 33     (0    $NRB $length)
    arc 33 34     ($PRB 0    $length)
    arc 34 35     (0    $PRB $length)
    arc 35 32     ($NRB 0    $length)     
   );
   
defaultPatch
{
    name walls; (here walls represent the outer face of pipe)
    type wall;
}   

boundary
(
    inlet
    {
        type patch;
        faces
        (
         (0  1  2  3 )
         (4  5  1  0 )
         (3  2  6  7 )
     (4  0  3  7 )
     (1  5  6  2 )
         (10 6  7  11)
         (9  5  6  10)
         (8  9  5  4 )
         (8  4  7  11)
     (39 31 30 38)    
     (38 30 29 37)    
     (37 29 28 36)    
     (36 28 31 39)         
        );
    } 
    outlet
    {
        type patch;
        faces
        (
     (13 12 15 14)         
     (17 16 12 13)
     (12 16 19 15)
     (17 13 14 18)
     (14 15 19 18)    
     (23 19 18 22)
     (20 16 19 23)
     (21 17 16 20)
     (22 18 17 21)
     (35 27 24 32)    
     (32 24 25 33)    
     (33 25 26 34)    
     (34 35 27 26)    
    );
    }        
);

2. i set up the inlet velosity in 0 file with flowRateInletVelocity and the extrapolatedProfile option as you say

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  v1606+                                |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0/fluidA";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [ 0 1 -1 0 0 0 0 ];

internalField   uniform ( 0 0 0 );

boundaryField
{
    inlet
    {
        type                          flowRateInletVelocity;
        volumetricFlowRate    0.000013889;
        extrapolateProfile        yes;
        value                         $internalField;
    }
    outlet
    {
        type                 inletOutlet;
        inletValue         $internalField;
        value               $internalField;
    }
    wall
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}

i dont know about the boundary of outlet with inletOutlet

outlet
    {
        type                 inletOutlet;
        inletValue         $internalField;
        value               $internalField;
    }

now the simulation are running. after that i will upload the result of simulation

[wuyangzhen]

Thank you very much for your time and help. i dont know why i cant reply with code file. the simulation is running., after it is finished, i will upload the result of the simulation.

fluidA: hot water flows through the inner pipe
fluidB: cold water flows through the outer pipe

[wuyangzhen]

hello Bloerb,

Thank you very much again.

i cant understand what you have said about mesh

mesh
to make sure your results are in good agreement with experimental data you need a resolved boundary layer. The attached blockMesh allows for this kind of refinement via grading. Eyeball the yPlus value and set your values accordingly. You can check with the yPlus function object if you are in the ballpark. For a well resolved boundary yPlus < 1 is a necessity. With values ~30 you should be able to reproduce the experiments.

it means i need change the simpleGrading in blockmeshdict, so that the yPlus can be < 1?

[piu58]

At which distance of the boundary layer you have to cover by the mesh depends on the model you run. RAND usually models around 30*yPlus. LES models at the space you have covered by the mesh. DNS models nothing, you have to make a very fine mesh until the friction is so large that no smaller vortices can arise.

[wuyangzhen]

Thank you for your help.

From the Simulation i get 2 pictures about yplus

fluidA: 1.5＜yPlus ＜2
fluidB: 2.25 ＜yPlus ＜2.3

it means i need to refine the mesh, so that the yPlus < 1?

[Bloerb]

Not necessarily. CHT requires two things:

1. The temperature on fluid and solid side are identical
2. heat flux fluid = - heat flux solid

So all the heat that is leaving the solid enters the fluid and vice versa. The amount of heat that goes over the boundary depends on the temperature and velocity gradient in the fluid. All the heat transfer happens inside the boundary layer of the fluid. Those are typically very thin for high Reynolds numbers. Hence you need to refine those. The y+ value tells you how well resolved your boundary layer is. For laminar flow you will get this right with only a few cells, for turbulent flow these boundary layers are however often so small (or to put it more correctly, the sublayers and hence your gradient needed for the correct cht results), that wall functions are needed. These will only function correctly if you are in the right y+ region. Hence you should aim for ~30 or if you can spare the expense fully resolve the boundary layer with y+<1. For a simple heat exchanger with transitional flow this might be overkill though.

What i meant is simpleGrading. Change this in such a way that your fluid boundary layers are resolved without drastically increasing the cell size. The values you have right now are perfectly fine however.

I also mentioned polynomial values for your fluid. After looking at your post again this is also overkill. The temperature range for your problem is simple to small for this to drastically effect your results.

The biggest problem right now is probably that your residuals for h are not falling in one of the regions. Why and which region is that? You might have to check mesh quality and the schemes and solution files.

[piu58]

> for turbulent flow these boundary layers are however often so small (or to put it more correctly, the sublayers and hence your gradient needed for the correct cht results)

The thickness of the layer of temperature changes is around 10% of the thickness of the Prandtl layer. To describe the temperature layer you should have a few cells there, for better accuracy around 10. Keep in mind that a refinement to the wall may destabilize your simulation.