|
[Sponsors] |
chtMultiRegionTwoPhaseEulerFoam thermo package not available |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
April 29, 2022, 12:34 |
chtMultiRegionTwoPhaseEulerFoam thermo package not available
|
#1 |
New Member
roham seif
Join Date: Jul 2020
Posts: 6
Rep Power: 6 |
Hi all,
I started from the tutorial of solidQuenching2D, changed the BCs to close the system, so maxY is not open anymore. I need to have heat loss at the two walls of the system. I used externalWallHeatFluxTemperature as BC and gave attention to set solidTehrmo for kappa method in <solid region> and fluidThermo for kappaMethod in <fluids region>. Still get the following error. Thank you very much in advance. OF version 2112 Geometry is the same as the tutorial file. Solid 0/T: PHP Code:
PHP Code:
PHP Code:
PHP Code:
PHP Code:
PHP Code:
PHP Code:
|
|
May 2, 2022, 12:59 |
|
#2 |
Senior Member
Julio Pieri
Join Date: Sep 2017
Posts: 107
Rep Power: 9 |
Have you try narrowing down the error to an specific BC/patch?
Try using another BC instead of externalWall[...] to see if the error is within that BC. Is that BC implemented in the chtMulti-twoPhase? |
|
May 2, 2022, 13:19 |
|
#3 |
New Member
roham seif
Join Date: Jul 2020
Posts: 6
Rep Power: 6 |
Thank you for the reponse.
-I set the BC to only one of the walls, still the same error. -I tried zeroGradient instead of externalWallHeatFluxTemperature and it worked fine. -using the "banana" trick: --> FOAM FATAL IO ERROR: (openfoam-2112 patch=220310) Unknown patchField type banana for patch type wall Valid patchField types : . . . externalWallHeatFluxTemperature . . |
|
May 2, 2022, 13:57 |
|
#4 |
Senior Member
Julio Pieri
Join Date: Sep 2017
Posts: 107
Rep Power: 9 |
Could you share your case? I'll try from my side
|
|
May 2, 2022, 16:12 |
|
#5 |
Senior Member
Julio Pieri
Join Date: Sep 2017
Posts: 107
Rep Power: 9 |
Actually I was able to reproduce the error from the tutorial case.
I did some research and the relevant part of the code is: Code:
switch (method_) { case mtFluidThermo: { typedef compressible::turbulenceModel turbulenceModel; { const auto* ptr = mesh.cfindObject<turbulenceModel> ( turbulenceModel::propertiesName ); if (ptr) { return ptr->kappaEff(patchi); } } { const auto* ptr = mesh.cfindObject<fluidThermo>(basicThermo::dictName); if (ptr) { return ptr->kappa(patchi); } } { const auto* ptr = mesh.cfindObject<basicThermo>(basicThermo::dictName); if (ptr) { return ptr->kappa(patchi); } } { const auto* ptr = mesh.cfindObject<basicThermo>("phaseProperties"); if (ptr) { return ptr->kappa(patchi); } } FatalErrorInFunction << "Using kappaMethod " << KMethodTypeNames_[method_] << ", but thermo package not available\n" << exit(FatalError); break; } ... In one of the comments, a user suggest to calculate kappa and create a kapp field to use with "lookup" kappaMethod, or to use fixedGradient. |
|
May 8, 2022, 08:06 |
|
#6 |
New Member
roham seif
Join Date: Jul 2020
Posts: 6
Rep Power: 6 |
Many thanks Julio.
I prefer not to keep the gradient constant. The other option sounds promissing but I do not know how can I define kappa for it. Any help is appreciated. |
|
May 9, 2022, 10:28 |
|
#7 |
Senior Member
Julio Pieri
Join Date: Sep 2017
Posts: 107
Rep Power: 9 |
You might have to modify the solver to create an IOobject. codedFunction might work here. It's a very simple operation, though. You can also use swak4Foam for that.
Check the available funcionObjects as it could have one for kappa (I'm not sure). To calculate Kappa, you can initially assume a constant for the material. Then get the temperature field and recalculate kappa in a spreadsheet for each cell. Then update the results in the kappa field file (you have to think some clever ordering here) and run the case for a while. You can iterate this a few times to "converge" the kappa method. I've never done this with kappa, but did similar procedure to calculate the "h" and "Ta" of the same BC and it gave me good results. |
|
April 9, 2024, 23:27 |
Governing equations
|
#8 |
New Member
Oscar Zagal
Join Date: Jan 2024
Posts: 16
Rep Power: 2 |
Hi dear all
Do you know where can I get the governing equations of the solver chtMultiRegionTwoPhaseEulerFoam? Thanks in advance. |
|
April 10, 2024, 09:41 |
|
#9 |
Senior Member
Julio Pieri
Join Date: Sep 2017
Posts: 107
Rep Power: 9 |
You should be able to find it for twoPhaseEuler (multiphaseEuler, etc) and for chtMultiRegion separately.
Try looking for similar solvers from other codes (commercial ones, for instance) as well, as the equation should most likely be the same. |
|
April 10, 2024, 11:36 |
|
#10 |
New Member
Oscar Zagal
Join Date: Jan 2024
Posts: 16
Rep Power: 2 |
Thanks for your advice, the source code is very complicated, is not like the basic solvers.
|
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[foam-extend.org] foam-extend-4.1 cannot compile on Centos8 | Ya_Squall2010 | OpenFOAM Installation | 2 | July 22, 2020 03:03 |
[foam-extend.org] paraview not runing? (foam extended 3.2 and ubuntu 15.04) | Milan2013 | OpenFOAM Installation | 23 | April 20, 2017 06:49 |
[OpenFOAM.org] Building OpenFOAM 3.0.1 on Ubuntu 16.04 - failed | erico | OpenFOAM Installation | 30 | February 2, 2017 10:24 |
OF 1.6 ext on Ubuntu 12.10 (64 bit) compilation errors | dreamilam | OpenFOAM Installation | 7 | April 21, 2013 06:43 |
Errors running allwmake in OpenFOAM141dev with WM_COMPILE_OPTION%3ddebug | unoder | OpenFOAM Installation | 11 | January 30, 2008 21:30 |