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

[GUIDE] Switching from incompressible to compressible simulation

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

Like Tree1Likes
  • 1 Post By snak

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 2, 2021, 08:11
Default [GUIDE] Switching from incompressible to compressible simulation
  #1
New Member
 
Gabriel Felix
Join Date: May 2021
Location: Brazil
Posts: 26
Rep Power: 3
gabrielfelix is on a distinguished road
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"
}


// ************************************************************************* //

Last edited by gabrielfelix; September 3, 2021 at 14:37.
gabrielfelix is offline   Reply With Quote

Old   September 3, 2021, 12:39
Default
  #2
Member
 
shinji nakagawa
Join Date: Mar 2009
Location: Japan
Posts: 97
Blog Entries: 1
Rep Power: 15
snak is on a distinguished road
Hi Gabriel,

Thank you for summarizing the procedure.

Some important points are missing in this guide. The dimension and type of pressure and the physical property of viscosity depend on the type of solver (compressible or incompressible). We have to adjust these as switch the solvers.

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.
gabrielfelix likes this.
snak is offline   Reply With Quote

Old   September 3, 2021, 12:45
Default
  #3
New Member
 
Gabriel Felix
Join Date: May 2021
Location: Brazil
Posts: 26
Rep Power: 3
gabrielfelix is on a distinguished road
Quote:
Originally Posted by snak View Post
Hi Gabriel,

Thank you for summarizing the procedure.

Some important points are missing in this guide. The dimension and type of pressure and the physical property of viscosity depend on the type of solver (compressible or incompressible). We have to adjust these as switch the solvers.

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.
Thanks man! I forgot the pressure file changes. I'll add them to the guide. There are so many changes you gotta made that I took some of them for granted.
gabrielfelix is offline   Reply With Quote

Reply

Tags
compressible, incompressible, rhosimplefoam, simplefoam

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
compressible vs incompressible flow Nick R Main CFD Forum 1 March 15, 2017 11:29
Compressible vs incompressible SGS model! zhangyan Main CFD Forum 10 June 4, 2016 04:39
Modify compressible solver to incompressible mingzhao OpenFOAM Programming & Development 0 September 18, 2015 17:46
Modify compressible solver to incompressible mingzhao OpenFOAM Running, Solving & CFD 0 September 18, 2015 12:50
compressible liquid simulation kaiser Main CFD Forum 0 October 13, 2002 04:32


All times are GMT -4. The time now is 09:07.