|
[Sponsors] |
February 29, 2016, 10:06 |
heat flux with chtMultiRegionFoam
|
#1 |
New Member
Lucie
Join Date: Feb 2016
Posts: 6
Rep Power: 10 |
Hi,
I would like to know how integrate the heat flux option between a solid and a fluid region using chtMultiRegionFoam. I tried with this: "Solid_to_.*" { type compressible::turbulentHeatFluxTemperature; heatSource flux; q uniform 200; alphaEff alphaEff; Cp Cp; value uniform 300; } Or "Solid_to_.*" { type compressible::turbulentHeatFluxTemperature; heatSource flux 1000; q uniform 200; kappaName none; kappa solidThermo 0; value uniform 300; } But, I obtained this error : --> FOAM FATAL ERROR: lookup of thermophysicalProperties from objectRegistry domain0 successful but it is not a solidThermo, it is a heRhoThermo<pureMixture<const<hConst<perfectGas<sp ecie>>,sensibleEnthalpy>>> From function objectRegistry::lookupObject<Type>(const word&) const in file /opt/OpenFOAM/OpenFOAM-2.3.x/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 181. FOAM aborting Someone can help me please ? Thank you Lucie |
|
February 29, 2016, 14:03 |
|
#2 |
Member
Joćo Ferreira
Join Date: Nov 2014
Location: Braga, Portugal
Posts: 53
Rep Power: 11 |
Hi,
that error is related with the thermophysicalProperties dictionary, located on the constant folder (one for each region). Check the tutorials to see the differences when it's a solid or fluid region. https://github.com/OpenFOAM/OpenFOAM...tiRegionHeater To allow exchange of energy between regions I usually use this boundary type: compressible::turbulentTemperatureCoupledBaffleMix ed https://github.com/OpenFOAM/OpenFOAM.../bottomWater/T Hope it helps |
|
March 1, 2016, 03:19 |
|
#3 |
New Member
Lucie
Join Date: Feb 2016
Posts: 6
Rep Power: 10 |
Thanks. But with compressible::turbulentTemperatureCoupledBaffleMix ed, I can't have a heat flux as parameter, it is only the temperature at the interface.
For my case, I would like to have a heat flux in enter [W/m²] and I don't know the boundary condition which allows that ! Do you have an idea? Thank you Lucie |
|
March 1, 2016, 03:56 |
|
#4 |
Member
Joćo Ferreira
Join Date: Nov 2014
Location: Braga, Portugal
Posts: 53
Rep Power: 11 |
Having an imposed heat flux on a interface solid/fluid doesn't make sense to me. If it was a external wall, the boundary "externalWallHeatFluxTemperature" should do the work.
Anyway, as the error you mentioned it's not related with the boundary, try the one you were using (compressible::turbulentHeatFluxTemperature, I've never use it). |
|
March 1, 2016, 04:40 |
|
#5 |
New Member
Lucie
Join Date: Feb 2016
Posts: 6
Rep Power: 10 |
Oh yeah my mistake ! This boundary condition was for an external wall so I tried externalWallHeatFluxTemperature and it seems working. Thank you for your help !
I have another question ! By imposing an heat flux for an external boundary, all the other boundaries are coupled with the fluid or another solid and the boundaries conditions in the interface are: compressible::turbulentTemperatureCoupledBaffleMix ed; Do you know if it is possible to not imposed the temperature in the baffle because it is what I want to calculate ! Thank you so much Lucie |
|
March 1, 2016, 05:13 |
|
#6 |
Member
Joćo Ferreira
Join Date: Nov 2014
Location: Braga, Portugal
Posts: 53
Rep Power: 11 |
You define the initial value on the compressible::turbulentTemperatureCoupledBaffleMix ed, it will change accordingly as the simulation develops.
|
|
March 3, 2016, 17:04 |
|
#7 |
Senior Member
Join Date: Sep 2013
Posts: 353
Rep Power: 20 |
If you fix the temperature in the coupled patch why do you need to do a cht calculation? f the boundary wall temperature is known you can essentially solve the regions separately and do not need to couple them. You can however fix the gradient between the two.
You could check out the fvOptions for coupled patches interRegionHeatTransferModel - variableHeatTransfer - tabulatedHeatTransfer - constantHeatTransfer interRegionExplicitPorositySource |
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Total heat transf. rate vs Total surface heat flux | Renato Sousa | FLUENT | 1 | April 14, 2020 03:27 |
Radiation in semi-transparent media with surface-to-surface model? | mpeppels | CFX | 11 | August 22, 2019 07:30 |
Forced convective heat transfere with fixed heat flux? | BenFranklinIII | OpenFOAM Running, Solving & CFD | 0 | July 30, 2015 05:31 |
ChtMultiRegionFoam heat flux | grmb7 | OpenFOAM Running, Solving & CFD | 0 | June 24, 2015 21:00 |
Enforce bounds error with heat loss boundary condition at solid walls | Chander | CFX | 2 | May 1, 2012 20:11 |