|
[Sponsors] |
Compressible 2D airfoil rhoSimpleFoam fatal error volScalarField none |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
July 22, 2016, 12:01 |
Compressible 2D airfoil rhoSimpleFoam fatal error volScalarField none
|
#1 |
New Member
Join Date: May 2016
Posts: 4
Rep Power: 10 |
Hello everyone,
note: there might be a number of writing errors, but my spelling checker isn't in English and as such isn't much help here. I'm trying to bring the incompressible 2D airfoil tutorial into the compressible solver. To begin with, I don't really care for the results. If it diverges because my conditions are off it's ok, for now i'm just trying to figure how to make it get past the first iteration. In an effort to keep it simple, I tried to re-use the rhoSimpleFoam tutorial, only changing the mesh and boundary conditions. To that end, I copied the constant/polymesh folder from the 2D airfoil I changed the boundary conditions in the 0/ folder. I also added the pRefCell and pRefVAlue to the fvSolution file. When i submit the job (via the rhoSimpleFoam comand), I get the following error message: Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Create time Create mesh for time = 0 SIMPLE: convergence criteria field p tolerance 0.001 field U tolerance 0.0001 field e tolerance 0.001 field "(k|epsilon|omega)" tolerance 0.001 Reading thermophysical properties Selecting thermodynamics package { type hePsiThermo; mixture pureMixture; transport sutherland; thermo hConst; equationOfState perfectGas; specie specie; energy sensibleInternalEnergy; } Reading field U Reading/calculating face flux field phi Creating turbulence model Selecting RAS turbulence model kEpsilon kEpsilonCoeffs { Cmu 0.09; C1 1.44; C2 1.92; C3 -0.33; sigmak 1; sigmaEps 1.3; } No MRF models present No finite volume options present Starting time loop Time = 1 GAMG: Solving for Ux, Initial residual = 1, Final residual = 0.099384, No Iterations 1 GAMG: Solving for Uy, Initial residual = 1, Final residual = 0.0794446, No Iterations 1 GAMG: Solving for e, Initial residual = 1, Final residual = 0.0101396, No Iterations 1 --> FOAM FATAL ERROR: request for volScalarField none from objectRegistry region0 failed available objects of type volScalarField are 15 ( thermo:mu thermo:psi nut rho k rhorAtU (1|A(U)) (1|((1|(1|A(U)))-H(1))) thermo:psi_0 alphat p T e epsilon thermo:alpha ) From function const Type& Foam::objectRegistry::lookupObject(const Foam::word&) const [with Type = Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>] in file /opt/OpenFOAM/OpenFOAM-v3.0+/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 193. FOAM aborting #0 Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so" #1 Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so" #2 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const& Foam::objectRegistry::lookupObject<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> >(Foam::word const&) const in "/opt/OpenFOAM/OpenFOAM-v3.0+/platfo rms/linux64Gcc48DPInt32Opt/lib/libfluidThermophysicalModels.so" #3 Foam::freestreamPressureFvPatchScalarField::updateCoeffs() in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/lib/libfiniteVolume.so" #4 Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>::GeometricBoundaryField::updateCoeffs() in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rhoSimpleFoam" #5 Foam::fvMatrix<double>::fvMatrix(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::dimensionSet const&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rhoSimpleFoam" #6 Foam::tmp<Foam::fvMatrix<double> > Foam::fv::optionList::operator()<double>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::word const&) in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rhoSimpleFoam" #7 ? in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rhoSimpleFoam" #8 __libc_start_main in "/lib64/libc.so.6" #9 ? in "/opt/OpenFOAM/OpenFOAM-v3.0+/platforms/linux64Gcc48DPInt32Opt/bin/rhoSimpleFoam" Aborted Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object alphat; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -1 0 0 0 0]; internalField uniform 0; boundaryField { walls { type compressible::alphatWallFunction; Prt 0.85; value uniform 0; } inlet { type calculated; value uniform 0; } outlet { type calculated; value uniform 0; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object epsilon; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -3 0 0 0 0]; internalField uniform 200; boundaryField { walls { type epsilonWallFunction; Cmu 0.09; kappa 0.41; E 9.8; value uniform 200; } inlet { type freestream; freestreamValue uniform 200; } outlet { type freestream; freestreamValue uniform 200; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object k; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -2 0 0 0 0]; internalField uniform 1; boundaryField { walls { type kqRWallFunction; value uniform 1; } inlet { type freestream; freestreamValue uniform 1; } outlet { type freestream; freestreamValue uniform 1; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object nut; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 2 -1 0 0 0 0]; internalField uniform 0.14; boundaryField { wall { type nutkWallFunction; Cmu 0.09; kappa 0.41; E 9.8; value uniform 0; } inlet { type freestream; freestreamValue uniform 0.14; } outlet { type freestream; freestreamValue uniform 0.14; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object p; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [1 -1 -2 0 0 0 0]; internalField uniform 33000; boundaryField { walls { type zeroGradient; } inlet { type freestreamPressure; } outlet { type freestreamPressure; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volScalarField; object T; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 0 0 1 0 0 0]; internalField uniform 229; boundaryField { walls { type zeroGradient; } inlet { type freestream; freestreamValue uniform 229; } outlet { type freestream; freestreamValue uniform 229; } frontAndBack { type empty; } } // ************************************************************************* // Code:
/*--------------------------------*- C++ -*----------------------------------*\ | ========= | | | \\ / F ield | OpenFOAM: The Open Source CFD Toolbox | | \\ / O peration | Version: v3.0+ | | \\ / A nd | Web: www.OpenFOAM.com | | \\/ M anipulation | | \*---------------------------------------------------------------------------*/ FoamFile { version 2.0; format ascii; class volVectorField; object U; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // dimensions [0 1 -1 0 0 0 0]; internalField uniform (25.75 3.62 0); boundaryField { walls { type fixedValue; value uniform (0 0 0); } inlet { type freestream; freestreamValue uniform (25.75 3.62 0); } outlet { type freestream; freestreamValue uniform (25.75 3.62 0); } } // ************************************************************************* // Thank you for any information you might provide JF |
|
August 1, 2016, 05:01 |
|
#2 |
New Member
Join Date: May 2016
Posts: 4
Rep Power: 10 |
Hello,
Has no one had that issue yet or any hint as to how to fix it? Thanks |
|
August 20, 2016, 19:18 |
|
#3 | |
Retired Super Moderator
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 10,981
Blog Entries: 45
Rep Power: 128 |
Quick answer:
Quote:
__________________
|
||
January 12, 2017, 11:18 |
|
#4 |
New Member
Joshua
Join Date: Oct 2016
Posts: 5
Rep Power: 10 |
Spot on, I have the exact same problem and took to comparing the source code between openfoam 3.0+ and 3.0.x and found that the field rhoName has been set to ("none") in freestreamPressure. The script in 3.0.x defines the fields by their names and sets defaults whereas it doesn't in 3.0+
From 3.0.x Code:
Foam::freestreamPressureFvPatchScalarField:: freestreamPressureFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF ) : zeroGradientFvPatchScalarField(p, iF), UName_("U"), phiName_("phi"), rhoName_("rho") {} Code:
Foam::freestreamPressureFvPatchScalarField:: freestreamPressureFvPatchScalarField ( const fvPatch& p, const DimensionedField<scalar, volMesh>& iF ) : zeroGradientFvPatchScalarField(p, iF), UName_("U"), phiName_("phi"), rhoName_("none") {} Edit: It runs find in serial but the error shows up again in parallel runs, totally at lost for what to do aside from changing all freestreamPressure boundaries to zeroGradient. Code:
inlet { type freestreamPressure; rho rho; } Code:
inlet { type freestreamPressure; } Code:
#!/bin/sh clear grep -rl 'freestreamPressure; *'/home/vmw_ubuntu/Desktop/case_dir | xargs sed -i '/freestreamPressure;/a \ \ \ \ \ \ \ \ \ rho rho;' # replace /home/vmw_ubuntu/Desktop/case_dir with the directory of your file. Last edited by firev1; January 14, 2017 at 02:47. |
|
September 28, 2017, 07:28 |
|
#5 | |
Member
Join Date: Oct 2013
Posts: 92
Rep Power: 13 |
Quote:
This post just saved me 3 days of bewilderment! It is absolutely important to know what your BCs require and what values they use implicitly!! |
||
Tags |
rhosimplefoam error, volscalarfield none |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Airfoil with simpleFoam and kOmegaSST: high drag values? | Tsiolkovsky | OpenFOAM Running, Solving & CFD | 6 | November 21, 2018 06:56 |
compressible flow calculation error using rhoSimpleFoam solver | student4326 | OpenFOAM Running, Solving & CFD | 7 | November 2, 2015 12:34 |
rhoSimpleFoam for compressible fluid through an orifice | WillemvdM | OpenFOAM Running, Solving & CFD | 2 | June 20, 2012 04:54 |
Compressible flow over airfoil | student123a | FLUENT | 2 | October 1, 2009 20:07 |
Compressible transonic airfoil RAE2822 simulation | Stefano | Siemens | 9 | June 21, 2006 11:47 |