How to get wall heat flux from reactingFoam?
Dear OpenFomers,
I build a fluid domain for combustion simulation using reactingFoam. When I tried to use Code:
postProcess -func wallHeatFlux Code:
--> FOAM FATAL ERROR: (openfoam-2206) By the way, I've tested the wall boundary set at contant temperature or externalWallHeatFluxTemperature. Both boundary can't postProcess wallHeatFlux. Thank you formers! :) |
1/ Suggestion 1
Place wallHeatFlux computation in system/controlDict as in Code:
<existing controlDict> 2/ Suggestion 2 Add to Suggestion 1 your own wallHeatFlux file (thus overriding the default). Example is in the squareBend tutorial of rhoSimpleFoam. Observe that libs is set to fieldFunctionObjects. 3/ Suggestion 3 (requiring more witchcraft) Verify that the wallHeatFlux function is indeed provided by the shared object file as the wallHeatFlux tells us. fieldFunctionObjects is in the directory openfoam2012/platforms/linux64GccDPInt32Opt/lib . To verify that wallHeatFlux is indeed provided, use nm -g libfieldFunctionObjects.so | grep -I wallheatflux Let us know what you learn. |
Hi,
In addition to Domenico's points, try running: Code:
reactingFoam -postProcess -func wallHeatFlux In your case, postProcess utility does not load the turbulence model, but the wallHeatFlux function object needs it. When using reactingFoam -postProcess, the solver starts, loads all the models it needs, and then execute the function called by the -postProcess option. I don't have experience with reactingFoam so other problems might arise, but this is worth trying. Cheers, Yann |
Thank you @dlahaye and @Yann for such thorough procedures to solve my question.
I've tried using Yann's recommendation. It works. It will output a wallHeatFlux_step.dat in the postProcessing/wallHeatFlux folder. The suggestion1 of dlahaye is also working. The wall heat flux will be output to another file wallHeatFlux.dat in the same directory with the same output frequency as the result file. In the file, there are columns of time, patch, min, max, integral, it looks like below. Code:
# Wall heat-flux Does the 'integral' means the total heat flux through the path in unit of kW? For the minus sign (-), it mean the heat is going out through the patch. It makes me wonder, why there is plus (+) heat flux through wall_chamber (see the max)? One other thing which might not related to the postProcessing. I've asked reactingFoam with boundary heat transfer? to know if the OpenFOAM can have thin wall heat transfer as that in fluent. If any former can share, it will be appreciated. |
Yes on integral.
Yes on sign. No idea on wall_chamber patch. Requires seeing details. See other post for other question. |
All times are GMT -4. The time now is 04:39. |