Heat transfer between multiple solids and fluids

Update: June 1, 2017
OpenFOAM 4.x

Case directory

$FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam/multiRegionHeater

Summary

We consider an analytical domain filled with air in the upper region and water in the lower region. The upper and lower regions are separated by a solid region. Assuming that a heating element is set at the bottom of the solid domain, we calculate the temperature and flow of the entire system from 0 sec to 100 sec. The domain consists of five subdomains as shown below.

Model geometry (region heater) Model geometry (region "heater")
Model geometry (region leftSolid) Model geometry (region "leftSolid")
Model geometry (region rightSolid) Model geometry (region "rightSolid")
Model geometry (region bottomWater) Model geometry (region "bottomWater")
Model geometry (region topAir) Model geometry (region "topAir")

In the region "topAir", air flows in from the X minimum plane at 0.1 m/s and flows out from the X maximum plane. In the region "bottomWater", water flows in from the X minimum plane at 0.001 m/s and flows out from the X maximum plane.

The bottom of the region "heater" is fixed at a temperature of 500 K. The boundary temperature between the "heater" and the other regions is set to 300 K. The heat transfer conditions are set between the regions, but only a layer with thermal conductivity is set between the region "heater" and the region "leftSolid". This makes it difficult for heat to be transferred between the region "heater" and the region "leftSolid".

After the calculation, the utility "paraFoam" is used to generate .OpenFOAM files for each region. To visualize them, open each .OpenFOAM file from [File]-[Open] in the menu after starting ParaView.

Display all regions Display all regions

The meshes are as follows, and the number of mesh is 3000.

Meshes (region heater) Meshes (region "heater")
Meshes (region leftSolid) Meshes (region "leftSolid")
Meshes (region rightSolid) Meshes (region "rightSolid")
Meshes (region bottomWater) Meshes (region "bottomWater")
Meshes (region topAir) Meshes (region "topAir")

The calculation result is as follows.

Temperature in solid region (T) Temperature in solid region (T)
Temperature on XY-plane (T) Temperature on XY-plane (T)
Flow velocity on the XY-plane in the air side (U) Flow velocity on the XY-plane in the air side (U)
Flow velocity on the XY-plane in the water side (U) Flow velocity on the XY-plane in the water side (U)

Commands

cp -r $FOAM_TUTORIALS/heatTransfer/chtMultiRegionFoam/multiRegionHeater multiRegionHeater
cd multiRegionHeater

blockMesh
topoSet
splitMeshRegions -cellZones -overwrite

rm -f 0*/heater/{nut,alphat,epsilon,k,U,p_rgh}
rm -f 0*/leftSolid/{nut,alphat,epsilon,k,U,p_rgh}
rm -f 0*/rightSolid/{nut,alphat,epsilon,k,U,p_rgh}

changeDictionary -region bottomWater
changeDictionary -region topAir
changeDictionary -region heater
changeDictionary -region leftSolid
changeDictionary -region rightSolid

decomposePar -allRegions
mpirun -np 4 chtMultiRegionFoam -parallel
reconstructPar -allRegions

paraFoam -touchAll
paraFoam

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

Calculation time

1 minutes 10.38 seconds *4 parallel, Inter(R) Core(TM) i7-2600 CPU @ 3.40GHz 3.40GHz

Reference