|
[Sponsors] |
Request for dictionary transportProperties region0 failed |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
October 22, 2024, 03:13 |
Request for dictionary transportProperties region0 failed
|
#1 |
New Member
Zhicheng Kai
Join Date: Oct 2024
Posts: 8
Rep Power: 2 |
Hi all,
I'm setting up for sonicFoam with k-omega SST RAS, but got an error that I have no idea where it comes from. Here is the full error message. My geometry is in a single domain, i.e. I don't think there should exist the need for region0? Code:
--> FOAM FATAL ERROR: (openfoam-2012) request for dictionary transportProperties from objectRegistry region0 failed available objects of type dictionary are 7(MRFProperties turbulenceProperties fvSchemes fvOptions fvSolution thermophysicalProperties data) From const Type& Foam::objectRegistry::lookupObject(const Foam::word&, bool) const [with Type = Foam::IOdictionary] in file ~/OpenFOAM/OpenFOAM/OpenFOAM-v2012/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 463. Code:
/*--------------------------------*- C++ -*----------------------------------*\ ========= | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox \\ / O peration | Website: https://openfoam.org \\ / A nd | Version: 6 \\/ M anipulation | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class dictionary; location "constant"; object transportProperties; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Transport model selection (use compressible gas model) transportModel sutherland; // Sutherland model coefficients for air (for high-speed compressible flow) SutherlandCoeffs { As 1.458e-6; // Sutherland constant (for dynamic viscosity) Ts 110.4; // Sutherland temperature [K] } // Thermophysical properties for the gas thermoType { type hePsiThermo; mixture pureMixture; transport sutherland; // Sutherland's law for viscosity thermodynamics hConst; // Constant specific heat equationOfState perfectGas; // Ideal gas law for compressible flow specie { molWeight 28.97; // Molecular weight of air [g/mol] } energy sensibleEnthalpy; } // Gas properties gas { molWeight 28.97; // Molecular weight of air [g/mol] Cp 1005; // Specific heat at constant pressure [J/(kg.K)] Hf 0; // Enthalpy of formation (set to 0 for ideal gas) } // Optional properties for Prandtl numbers Pr 0.71; // Prandtl number (typically for air) Prt 0.85; // Turbulent Prandtl number // ************************************************************************* // |
|
October 22, 2024, 05:07 |
|
#2 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,227
Rep Power: 28 |
Hello,
There should be no need for a transportProperties file in a compressible solver such as sonicFoam (which use thermophysicalProperties instead) My best bet is that there is something wrong in your case setup which is trying to access to a transportProperties file. I would first check the boundary conditions, more specifically the wall functions you use for alphat, which should start with compressible::. (might be another one though). FYI, region0 is the default name when there is a single region. Regards, Yann |
|
October 22, 2024, 22:37 |
|
#3 |
New Member
Zhicheng Kai
Join Date: Oct 2024
Posts: 8
Rep Power: 2 |
Thanks a lot, that works. It is the issue of the wall function of alphat. I was using
wall { type alphatJayatillekeWallFunction; Prt 0.85; value uniform 0; } and I replaced that with wall { type compressible::alphatWallFunction; // or compressible::alphatJayatillekeWallFunction; Prt 0.85; value uniform 0; } which both work. So the key is the "compressible::" for this error. |
|
Tags |
#openfoam #debug, #openfoam #sonicfoam, #transportproperties |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Paraview 5.10.1 - error - openfoam 11 - ubuntu 22.04 lts | gu1 | OpenFOAM Bugs | 5 | July 29, 2024 11:50 |
Foam::error::printStack(Foam::Ostream&) with simpleFoam -parallel | U.Golling | OpenFOAM Running, Solving & CFD | 52 | September 23, 2023 04:35 |
[OpenFOAM] ParaView/Parafoam error when making animation | Disco_Caine | ParaView | 6 | September 28, 2010 10:54 |
user subroutine error | CFDUSER | CFX | 2 | December 9, 2006 07:31 |
user defined function | cfduser | CFX | 0 | April 29, 2006 11:58 |