OpenFoamのサンプル確認（パラメータやキーワードの覚書）です。
チュートリアルフォルダ：チュートリアル場所（windows）
次ページ：メッシュの置き換え
ベース
バージョン : Windows版（OpenFOAM-v2106-windows-mingw.exe）
引用元
<チュートリアルフォルダ>\multiphase\interFoam\laminar\damBreakWithObstacle
結果図
気層、液相のモデルになります。
作業
基本的な流れはT703 OpenFoam tipsと同じです。（または作業）
//チュートリアルからサンプルをコピーしておきます。// //0.origから0へ（.org削除） //コマンド:メッシュ作成 blockMesh //コマンド実行 topoSet subsetMesh -overwrite c0 -patch walls setFields //計算実行// interFoam //ParaView用VTK変換// foamToVTK
モデル
設定値の抜粋まとめ
全体構造
//初期フォルダ・ファイル構成 damBreakWithObstacle ├ 0.orig │ ├ alpha.water │ ├ k │ ├ nut │ ├ omega │ ├ p_rgh │ └ U ├ constant │ ├ dynamicMeshDict │ ├ g │ ├ transportProperties ：物性値 │ └ turbulenceProperties ├ system │ ├ blockMeshDict :ブロックメッシュ定義 │ ├ controlDict ：解析ジョブ設定 │ ├ decomposeParDict :未使用（win） │ ├ fvSchemes ：ソルバー設定 │ ├ fvSolution ：ソルバー設定 │ ├ setFieldsDict │ └ topoSetDict ├ Allclean └ Allrun
0.orig
設定確認 alpha.water
dimensions [0 0 0 0 0 0 0];
internalField uniform 0;
boundaryField
{
walls
{
type zeroGradient;
}
obstacle
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}
k
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0.00015;
boundaryField
{
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
"(obstacle|walls)"
{
type kqRWallFunction;
value $internalField;
}
}
nut
dimensions [0 2 -1 0 0 0 0];
internalField uniform 5e-07;
boundaryField
{
atmosphere
{
type zeroGradient;
}
"(obstacle|walls)"
{
type nutkRoughWallFunction;
Ks uniform 100e-6;
Cs uniform 0.5;
value $internalField;
}
}
omega
dimensions [0 0 -1 0 0 0 0];
internalField uniform 2;
boundaryField
{
atmosphere
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
"(obstacle|walls)"
{
type omegaWallFunction;
value $internalField;
}
}
p_rgh
dimensions [1 -1 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
walls
{
type fixedFluxPressure;
phi phiAbs;
value uniform 0;
}
obstacle
{
type fixedFluxPressure;
phi phiAbs;
value uniform 0;
}
atmosphere
{
type totalPressure;
p0 uniform 0;
}
}
U
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
atmosphere
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
"(obstacle|walls)"
{
type uniformFixedValue;
uniformValue (0 0 0);
}
}
constant
dynamicMeshDict
dynamicFvMesh dynamicRefineFvMesh;
// How often to refine
refineInterval 1;
// Field to be refinement on
field alpha.water;
// Refine field inbetween lower..upper
lowerRefineLevel 0.001;
upperRefineLevel 0.999;
// If value < unrefineLevel unrefine
unrefineLevel 10;
// Have slower than 2:1 refinement
nBufferLayers 1;
// Refine cells only up to maxRefinement levels
maxRefinement 2;
// Stop refinement if maxCells reached
maxCells 200000;
// Flux field and corresponding velocity field. Fluxes on changed
// faces get recalculated by interpolating the velocity. Use 'none'
// on surfaceScalarFields that do not need to be reinterpolated.
correctFluxes
(
(phi none)
(nHatf none)
(rhoPhi none)
(alphaPhi0.water none)
(ghf none)
(alphaPhiUn none)
);
// Write the refinement level as a volScalarField
dumpLevel true;
g
dimensions [0 1 -2 0 0 0 0]; value (0 0 -9.81);
設定確認 transportProperties
phases (water air);
water
{
transportModel Newtonian;
nu 1e-06;
rho 1000;
}
air
{
transportModel Newtonian;
nu 1.48e-05;
rho 1;
}
sigma 0.07;
turbulenceProperties
simulationType laminar;
system
設定確認 blockMeshDict
scale 1;
vertices
(
(0 0 0)
(1 0 0)
(1 1 0)
(0 1 0)
(0 0 1)
(1 0 1)
(1 1 1)
(0 1 1)
);
blocks
(
hex (0 1 2 3 4 5 6 7) (32 32 32) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
atmosphere
{
type patch;
faces
(
(3 7 6 2)
);
}
walls
{
type wall;
faces
(
(0 4 7 3)
(2 6 5 1)
(1 5 4 0)
(0 3 2 1)
(4 5 6 7)
);
}
);
mergePatchPairs
(
);
設定確認 controlDict
application interFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 2; deltaT 0.001; writeControl adjustable; writeInterval 0.02; purgeWrite 0; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable yes; adjustTimeStep yes; maxCo 0.5; maxAlphaCo 0.5; maxDeltaT 1;
decomposeParDict
numberOfSubdomains 6; method scotch;
設定確認 fvSchemes
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
}
divSchemes
{
div(rhoPhi,U) Gauss upwind;
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss linear;
div(phi,k) Gauss upwind;
div(phi,omega) Gauss upwind;
div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear corrected;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default corrected;
}
wallDist
{
method meshWave;
}
設定確認 fvSolution
solvers
{
"alpha.water.*"
{
nAlphaCorr 1;
nAlphaSubCycles 3;
cAlpha 1;
}
p_rgh
{
solver GAMG;
tolerance 1e-08;
relTol 0.01;
smoother DIC;
cacheAgglomeration no;
}
p_rghFinal
{
$p_rgh;
relTol 0;
}
"pcorr.*"
{
$p_rghFinal;
tolerance 0.0001;
}
U
{
solver smoothSolver;
smoother GaussSeidel;
tolerance 1e-06;
relTol 0;
nSweeps 1;
}
"(k|omega|B|nuTilda).*"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-08;
relTol 0;
}
}
PIMPLE
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
pRefPoint (0.51 0.51 0.51);
pRefValue 0;
}
設定確認 setFieldsDict
defaultFieldValues
(
volScalarFieldValue alpha.water 0
volVectorFieldValue U (0 0 0)
);
regions
(
boxToCell
{
box (0 0 0) (0.6 0.1875 0.75);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);
topoSetDict
actions
(
{
name c0;
type cellSet;
action clear;
}
{
name c0;
type cellSet;
action invert;
}
{
name c0;
type cellSet;
action subtract;
source boxToCell;
box (0.375 0.375 0) (0.625 0.625 0.25);
}
);
その他
次ページ以降
コメント