|
[Sponsors] |
[GUIDE] Switching from incompressible to compressible simulation |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
September 2, 2021, 09:11 |
[GUIDE] Switching from incompressible to compressible simulation
|
#1 | |
Member
Gabriel Felix
Join Date: May 2021
Location: Brazil
Posts: 35
Rep Power: 6 |
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; } } // ************************************************************************* // 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; } } // ************************************************************************* // 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); } // ************************************************************************* // 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; } //************************************************************************** // 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); } // ************************************************************************* // Quoting the user snak: Quote:
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 15:37. |
||
September 3, 2021, 13:39 |
|
#2 |
Senior Member
|
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. |
|
September 3, 2021, 13:45 |
|
#3 | |
Member
Gabriel Felix
Join Date: May 2021
Location: Brazil
Posts: 35
Rep Power: 6 |
Quote:
|
||
Tags |
compressible, incompressible, rhosimplefoam, simplefoam |
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
compressible vs incompressible flow | Nick R | Main CFD Forum | 1 | March 15, 2017 12:29 |
Compressible vs incompressible SGS model! | zhangyan | Main CFD Forum | 10 | June 4, 2016 05:39 |
Modify compressible solver to incompressible | mingzhao | OpenFOAM Programming & Development | 0 | September 18, 2015 18:46 |
Modify compressible solver to incompressible | mingzhao | OpenFOAM Running, Solving & CFD | 0 | September 18, 2015 13:50 |
compressible liquid simulation | kaiser | Main CFD Forum | 0 | October 13, 2002 05:32 |