| gabrielfelix |
September 2, 2021 08:11 |
[GUIDE] Switching from incompressible to compressible simulation
Hi folks
I'm simulating a propeller in steady-state incompressible flow using simpleFoam with the same boundary conditions as the pimpleFoam or pimpleDyMFoam marine propeller tutorial. I wanted to run my case in compressible flow and I faced some problems to which I could not find a direct guide to overcome them. I saw that there are many posts concerning the same problems I had, and I decided to create this guide, now that I managed to succesfully run my case with rhoSimpleFoam.
I tried to apply the same file configurations of the rhoSimpleFoam aerofoilNACA0012 tutorial in my case, however I had to make other modifications to be able to run the case.
I'm not expert on this compressible configurations, so the solutions I will come up here might not be the most adequate ones, but rather the ones I managed to run my case with after researching in many and many threads.
1. Add the alphat and T files to 0/
Compressible solvers deals with the Navier-Stokes flow energy equation, which is related to the flow temperature. Thus, temperature T and alphat (which I don't know what means) must be added to the boundary conditions.
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 0 0 1 0 0 0];
internalField uniform 298;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
inlet
{
type fixedValue;
value uniform 298;
}
outlet
{
type zeroGradient;
}
wall
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -1 0 0 0 0];
internalField uniform 0;
boundaryField
{
#includeEtc "caseDicts/setConstraintTypes"
wall
{
type compressible::alphatWallFunction;
value uniform 0;
}
inlet
{
type calculated;
value uniform 0;
}
outlet
{
type calculated;
value uniform 0;
}
}
// ************************************************************************* //
2. Add the density variable and its value to transportProperties file and create a thermophysicalProperties file
You must alter these files accordingly to your simulation altitude (i.e. rho = f(h) )
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
rho 1.225;
nu 1.8e-05;
// ************************************************************************* //
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
thermoType
{
type hePsiThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState perfectGas;
specie specie;
energy sensibleInternalEnergy;
}
mixture // air at room temperature (298 K)
{
specie
{
molWeight 28.96;
}
thermodynamics
{
Cp 1004.5;
Hf 0;
}
transport
{
mu 1.82e-05;
Pr 0.71;
Ts 116;
}
}
// ************************************************************************* //
3. Add new variables to fvSchemes, fvSolution and create fvOptions file
You must add the new state variables of the flow related to energy and temperature.
I used the same configs from the aerofoilNACA0012 tutorial in fvSchemes
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default steadyState;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) cellLimited Gauss linear 1;
grad(k) cellLimited Gauss linear 1;
grad(omega) cellLimited Gauss linear 1;
}
divSchemes
{
default none;
div(phi,U) bounded Gauss linearUpwind limited;
turbulence bounded Gauss upwind;
energy bounded Gauss linearUpwind limited;
div(phi,k) $turbulence;
div(phi,omega) $turbulence;
div(phi,epsilon) $turbulence;
div(phi,e) $energy;
div(phi,K) $energy;
div(phi,Ekp) $energy;
div(phid,p) Gauss upwind;
div((phi|interpolate(rho)),p) bounded Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear limited corrected 0.33;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default limited corrected 0.33;
}
wallDist
{
method meshWave;
}
// ************************************************************************* //
Add the energy equation solver and relaxation factors. It is also necessary to include rho in the relaxation factors. I used the same parameters as the tutorial.
I use potentialFlow to initialize the compressible simulation with an incompressible solution. nNonOrthogonalCorrectors in the SIMPLE section helps the solver when large pressure gradients appear in the flow.
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
"pcorr.*"
{
solver GAMG;
tolerance 1e-2;
relTol 0;
smoother DICGaussSeidel;
cacheAgglomeration no;
maxIter 50;
}
p
{
$pcorr;
tolerance 1e-5;
relTol 0.01;
}
pFinal
{
$p;
tolerance 1e-6;
relTol 0;
}
"(U|k|epsilon|e)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-6;
relTol 0.1;
}
"(U|k|epsilon|e)Final"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-6;
relTol 0;
}
}
SIMPLE
{
//correctPhi no;
//nOuterCorrectors 2;
//nCorrectors 1;
nNonOrthogonalCorrectors 1;
// Set up residual controls. Simulation stops when residual target is reached
residualControl
{
p 1e-6;
//U 1e-4;
//"(k|epsilon)" 1e-4;
}
}
potentialFlow
{
nNonOrthogonalCorrectors 1;
}
relaxationFactors
{
fields
{
p 0.3 ;
rho 0.01 ;
}
equations
{
U 0.7 ;
e 0.7 ;
k 0.7 ;
omega 0.7 ;
}
}
cache
{
grad(U);
}
// ************************************************************************* //
Create an fvOptions file to limit the temperature range and avoid getting non-physical values.
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
limitT
{
type limitTemperature;
min 101;
max 1000;
selectionMode all;
}
//************************************************************************** //
4. Change the forces or coefficients files if you use them
These files determines how the output forces and coefficients are printed by the solver. In incompressible flows, the rho = inf and the pressure is given by P = p/rho. Now that you have a finite density you must attribute its value to the files.
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
forces
{
type forces;
libs (forces);
writeControl timeStep;
timeInterval 1;
log yes;
patches ("propeller.*");
rho rho;
log true;
CofR (0 0 0); // Rotation around centre line of propeller
pitchAxis (0 1 0);
}
// ************************************************************************* //
5. Change the dimension of pressure its value in 0/p file
Quoting the user snak:
Quote:
In an incompressible solver, N-S equation is divided by a uniform density rho. This causes (1) the dimension of pressure of [0 2 -2 0 0 0 0] and (2) the kinematic viscosity nu in laplacian term. In an incompressible solver, pressure is assumed to be relative. The atmosphere will be 0 usually.
In a compressible solver, N-S equation is not divided by density. So, the dimension of pressure is [1 -1 -2 0 0 0 0] as usual. The dinamic viscosity mu appears in laplacian term. In a compressible solver, The absolute pressure is must be provided in p file because the value of pressure will be used to calculate other physical properies. The atmosphere will be 1e5 usually.
|
Code:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v2012 |
| \\ / A nd | Website: www.openfoam.com |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 101325;
boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 101325;
}
wall
{
type zeroGradient;
}
#includeEtc "caseDicts/setConstraintTypes"
}
// ************************************************************************* //
|
