Heat transfer between multiple solids and fluids
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 "leftSolid")
Model geometry (region "rightSolid")
Model geometry (region "bottomWater")
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
The meshes are as follows, and the number of mesh is 3000.
Meshes (region "heater")
Meshes (region "leftSolid")
Meshes (region "rightSolid")
Meshes (region "bottomWater")
Meshes (region "topAir")
The calculation result is as follows.
Temperature in solid region (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 water side (U)
Commands
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