CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Request for dictionary transportProperties region0 failed

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By Yann
  • 1 Post By dandanTT

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 22, 2024, 03:13
Default Request for dictionary transportProperties region0 failed
  #1
New Member
 
Zhicheng Kai
Join Date: Oct 2024
Posts: 8
Rep Power: 2
dandanTT is on a distinguished road
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.
Other than that I defined the transportProperties, thermalPhysicalProperties and turbulentProperties in folder constant. The transportProperties is attached below.
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

// ************************************************************************* //
Thank you all for helping.
dandanTT is offline   Reply With Quote

Old   October 22, 2024, 05:07
Default
  #2
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,227
Rep Power: 28
Yann will become famous soon enough
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
dandanTT likes this.
Yann is offline   Reply With Quote

Old   October 22, 2024, 22:37
Default
  #3
New Member
 
Zhicheng Kai
Join Date: Oct 2024
Posts: 8
Rep Power: 2
dandanTT is on a distinguished road
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.
Yann likes this.
dandanTT is offline   Reply With Quote

Reply

Tags
#openfoam #debug, #openfoam #sonicfoam, #transportproperties

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 12:38.