Heat exchanger

OpenFOAM 4.x

Case directory

$FOAM_TUTORIALS/heatTransfer/chtMultiRegionSimpleFoam/heatExchanger

Summary

We calculate a heat exchanger. A fan is used to flow the cooled air around the porous material through which the hot fluid flows to perform heat exchange.

Model geometry (entire) Model geometry (entire)
Flow path with fan (region air) Flow path with fan (region air)
モデル形状（領域 leftSolid） Porous media (region porous)

In the region "air", the fluid flows in from the region "inlet" (white part) on the bottom surface at a temperature of 300 K and a velocity of (0, 0, 5) m/s. It is accelerated by the fan (green part), passes through the porous region (rectangular part), and then flows out from the region "outlet". On the other hand, in the porous region, fluid flows in from the x-maximum plane at a temperature of 400 K and a velocity of (0.01, 0, 0) m/s, and flows out from the x-minimum plane.

The fan is modeled using the MRF function as rotating at 47.7 rad/s with the Z-axis as the rotation axis. This setting is specified in the file constant/air/MRFProperties as follows.

MRF1
{
    cellZone    rotor;
    active      yes;
    
    nonRotatingPatches ();

    origin    (0.25 0.25 0.25);
    axis      (0 0 1);
    omega     47.7;
}

The porous media depends on the Darcy-Forchheimer law S_i = -\biggl(\mu D_{ij}+ \frac{1}{2}\rho\left \vert u \right \vert F\biggr) u_i, and the parameters that determine the porous media properties are specified in the file constant/air/fvOptions.

During configuration, the utility "paraFoam" is used to generate an .OpenFOAM file for each region. To visualize, open and visualize each .OpenFOAM file from the menu [File]-[Open] after starting ParaView.

Display all regions Display all regions

The meshes are as follows, and the number of mesh is 279000.

Meshes (region air) Meshes (region air)
Meshes (region air, zoomed) Meshes (region air, zoomed)
Meshes (region porous) Meshes (region porous)
Meshes (region porous, zoomed) Meshes (region porous, zoomed)

The calculation result is as follows.

Flow velocity on the XY plane of region air (U) Flow velocity on the XY plane of region air (U)
Temperature on the XY plane of region air (T) Temperature on the XY plane of region air (T)
Flow velocity on the XZ plane of region air (U) Flow velocity on the XZ plane of region air (U)
Temperature on the XZ plane of region air (T) Temperature on the XZ plane of region air (T)
Flow velocity on the XZ plane of region porous (U) Flow velocity on the XZ plane of region porous (U)
Temperature on the XZ plane of region porous (T) Temperature on the XZ plane of region porous (T)

Commands

cp -r $FOAM_TUTORIALS/heatTransfer/chtMultiRegionSimpleFoam/heatExchanger heatExchanger
cd heatExchanger

# Make meshes
blockMesh -region air
blockMesh -region porous

# Make rotor blades
topoSet -region air -dict system/topoSetDict.1

createBaffles -region air -overwrite

# Make a region for MRF
topoSet -region air -dict system/topoSetDict.2

rm -rf constant/air/polyMesh/sets

# Make dummy files for post-processing
paraFoam -touch -region porous
paraFoam -touch -region air

cp -rf 0.orig 0

decomposePar -region air
decomposePar -region porous

mpirun -np 4 chtMultiRegionSimpleFoam -parallel

reconstructPar -latestTime -region air
reconstructPar -latestTime -region porous

paraFoam

After ParaView has been started by the paraFoam command, each .OpenFOAM file must be opened from the menu [File]-[Open].

Calculation time

36 minutes 4.86 seconds *4 parallel, Inter(R) Core(TM) i7-2600 CPU @ 3.40GHz 3.40GHz