zhyang-dev/openfoam
1
0
Fork 0
mirror of https://develop.openfoam.com/Development/openfoam.git synced 2025-11-28 03:28:01 +00:00
Code Issues Actions Packages Projects Releases Wiki Activity

ENH: Added ACMI tutorial case

Browse Source
This commit is contained in:
andy
2013-05-28 15:55:16 +01:00
parent 0aa5613dcf
commit 27fdf34f03
22 changed files with 1187 additions and 0 deletions
Download Patch File Download Diff File Expand all files Collapse all files

67
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/0.org/U Normal file
View File

@ -0,0 +1,67 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 1 -1 0 0 0 0];
internalField uniform (0 0 0);
boundaryField
{
inlet
{
type fixedValue;
value uniform (1 0 0);
}
outlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
walls
{
// type fixedValue;
type movingWallVelocity;
value uniform (0 0 0);
}
defaultFaces
{
type empty;
}
ACMI1_blockage
{
type fixedValue;
value uniform (0 0 0);
}
ACMI1_couple
{
type cyclicACMI;
value uniform (0 0 0);
}
ACMI2_blockage
{
type fixedValue;
value uniform (0 0 0);
}
ACMI2_couple
{
type cyclicACMI;
value uniform (0 0 0);
}
}
// ************************************************************************* //

67
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/0.org/epsilon Normal file
View File

@ -0,0 +1,67 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -3 0 0 0 0];
internalField uniform 1.8e-3;
boundaryField
{
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
walls
{
type epsilonWallFunction;
value $internalField;
}
defaultFaces
{
type empty;
}
ACMI1_blockage
{
type epsilonWallFunction;
value $internalField;
}
ACMI1_couple
{
type cyclicACMI;
value $internalField;
}
ACMI2_blockage
{
type epsilonWallFunction;
value $internalField;
}
ACMI2_couple
{
type cyclicACMI;
value $internalField;
}
}
// ************************************************************************* //

67
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/0.org/k Normal file
View File

@ -0,0 +1,67 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 3.75e-3;
boundaryField
{
inlet
{
type fixedValue;
value $internalField;
}
outlet
{
type inletOutlet;
inletValue $internalField;
value $internalField;
}
walls
{
type kqRWallFunction;
value $internalField;
}
defaultFaces
{
type empty;
}
ACMI1_blockage
{
type kqRWallFunction;
value $internalField;
}
ACMI1_couple
{
type cyclicACMI;
value $internalField;
}
ACMI2_blockage
{
type kqRWallFunction;
value $internalField;
}
ACMI2_couple
{
type cyclicACMI;
value $internalField;
}
}
// ************************************************************************* //

70
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/0.org/p Normal file
View File

@ -0,0 +1,70 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
location "0";
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions [0 2 -2 0 0 0 0];
internalField uniform 0;
boundaryField
{
inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}
walls
{
type zeroGradient;
}
couple1
{
type zeroGradient;
}
couple2
{
type zeroGradient;
}
defaultFaces
{
type empty;
}
ACMI1_blockage
{
type zeroGradient;
}
ACMI1_couple
{
type cyclicACMI;
value uniform 0;
}
ACMI2_blockage
{
type zeroGradient;
}
ACMI2_couple
{
type cyclicACMI;
value uniform 0;
}
}
// ************************************************************************* //

9
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/Allclean Executable file
View File

@ -0,0 +1,9 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial clean functions
. $WM_PROJECT_DIR/bin/tools/CleanFunctions
cleanCase
rm -rf 0

9
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/Allrun Executable file
View File

@ -0,0 +1,9 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
./Allrun.pre
runApplication $(getApplication)

13
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/Allrun-parallel Executable file
View File

@ -0,0 +1,13 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
./Allrun.pre
runApplication decomposePar
runParallel $(getApplication) 4
runApplication reconstructPar

17
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/Allrun.pre Executable file
View File

@ -0,0 +1,17 @@
#!/bin/sh
cd ${0%/*} || exit 1 # run from this directory
# Source tutorial run functions
. $WM_PROJECT_DIR/bin/tools/RunFunctions
runApplication blockMesh
runApplication topoSet -constant
# split the mesh to generate the ACMI coupled patches
runApplication createBaffles -overwrite
# remove zero-sized patches
runApplication createPatch -overwrite
cp -rf 0.org 0

104
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/README Normal file
View File

@ -0,0 +1,104 @@
oscillatingInletACMI2D
This tutorial case gives an example of the Arbitrarily Coupled Mesh Interface
(ACMI) usage. The mesh is composed of two mesh regions: an inlet channel which
oscillates in the +/- Y-direction, and a fixed mesh region.
Each ACMI patch requires the specification of a 'non-overlapping' patch. In
this example, the non-overlapping patches are described as walls, e.g. taken
from the constant/polyMesh/boundary file:
1. First ACMI poatch pair applied to the inlet channel outlet
ACMI1_blockage
{
type wall;
nFaces 40;
startFace 43680;
}
ACMI1_couple
{
type cyclicACMI;
nFaces 40;
startFace 43720;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
}
1. Second ACMI poatch pair applied to the fixed mesh region inlet
ACMI2_blockage
{
type wall;
nFaces 96;
startFace 43760;
}
ACMI2_couple
{
type cyclicACMI;
nFaces 96;
startFace 43856;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI1_couple;
nonOverlapPatch ACMI2_blockage;
}
In the above, the ACMI1_blockage and ACMI1_couple patches occupy the same space,
with duplicate points, edges and faces. The ACMI2_blockage and ACMI2_couple
patches are created similarly.
The duplicate patches are initially created using the createBaffles utility.
Firstly, the original (non-duplicated) patch faces are collected into zones
using the topoSet utility.
Each ACMI/no-overlapping patch pair is specified using a master-slave approach.
However, since we are generating boundary patches (which are always master
patches) the slave patches are simply defined using 'dummy' entries, e.g.:
type faceZone;
zoneName couple1Faces;
patches
{
// create blockage patch
master
{
//- Master side patch
name ACMI1_blockage;
type wall;
}
slave1 // dummy entries only
{
//- Slave side patch
name ACMI1_blockage;
type wall;
}
// create cyclic ACMI patch
master2
{
//- Master side patch
name ACMI1_couple;
type cyclicACMI;
matchTolerance 0.0001;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
transform noOrdering;
}
slave2 // dummy entries only
{
//- Slave side patch
name ACMI1_couple;
type patch;
}
}
Boundary conditions must then be applied to all geometric patches in the usual,
manner, and the cases can be executed in parallel (as shown when running the
Allrun-parallel script) without any speacial treatment, i.e. the case set-up is
the same as when operating in serial mode.

25
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/RASProperties Normal file
View File

@ -0,0 +1,25 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object RASProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
RASModel kEpsilon;
turbulence on;
printCoeffs on;
// ************************************************************************* //

36
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/dynamicMeshDict Normal file
View File

@ -0,0 +1,36 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object dynamicMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dynamicFvMesh solidBodyMotionFvMesh;
motionSolverLibs ( "libfvMotionSolvers.so" );
solidBodyMotionFvMeshCoeffs
{
cellZone inletChannel;
solidBodyMotionFunction oscillatingLinearMotion;
oscillatingLinearMotionCoeffs
{
amplitude (0 0.5 0);
omega 3.14; // rad/s (.5 rps)
}
}
// ************************************************************************* //

103
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/polyMesh/blockMeshDict Normal file
View File

@ -0,0 +1,103 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
convertToMeters 1;
vertices
(
(0 0.3 0)
(1 0.3 0)
(1 0.7 0)
(0 0.7 0)
(0 0.3 0.1)
(1 0.3 0.1)
(1 0.7 0.1)
(0 0.7 0.1)
(1 0 0)
(3 0 0)
(3 1 0)
(1 1 0)
(1 0 0.1)
(3 0 0.1)
(3 1 0.1)
(1 1 0.1)
);
blocks
(
// hex (0 1 2 3 4 5 6 7) (20 20 1) simpleGrading (1 1 1)
// hex (8 9 10 11 12 13 14 15) (40 48 1) simpleGrading (1 1 1)
hex (0 1 2 3 4 5 6 7) (80 40 1) simpleGrading (1 1 1)
hex (8 9 10 11 12 13 14 15) (80 96 1) simpleGrading (1 1 1)
);
edges
(
);
boundary
(
inlet
{
type patch;
faces
(
(0 4 7 3)
);
}
outlet
{
type patch;
faces
(
(10 14 13 9)
);
}
walls
{
type wall;
faces
(
(3 7 6 2)
(1 5 4 0)
(11 15 14 10)
(9 13 12 8)
);
}
couple1
{
type patch;
faces
(
(2 6 5 1)
);
}
couple2
{
type patch;
faces
(
(8 12 15 11)
);
}
);
mergePatchPairs
(
);
// ************************************************************************* //

81
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/polyMesh/boundary Normal file
View File

@ -0,0 +1,81 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev.ACMI |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
8
(
inlet
{
type patch;
nFaces 40;
startFace 21464;
}
outlet
{
type patch;
nFaces 96;
startFace 21504;
}
walls
{
type wall;
nFaces 320;
startFace 21600;
}
defaultFaces
{
type empty;
inGroups 1(empty);
nFaces 21760;
startFace 21920;
}
ACMI1_blockage
{
type wall;
nFaces 40;
startFace 43680;
}
ACMI1_couple
{
type cyclicACMI;
inGroups 1(cyclicACMI);
nFaces 40;
startFace 43720;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
}
ACMI2_blockage
{
type wall;
nFaces 96;
startFace 43760;
}
ACMI2_couple
{
type cyclicACMI;
inGroups 1(cyclicACMI);
nFaces 96;
startFace 43856;
matchTolerance 0.0001;
transform noOrdering;
neighbourPatch ACMI1_couple;
nonOverlapPatch ACMI2_blockage;
}
)
// ************************************************************************* //

22
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/transportProperties Normal file
View File

@ -0,0 +1,22 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object transportProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
transportModel Newtonian;
nu nu [ 0 2 -1 0 0 0 0 ] 1e-6;
// ************************************************************************* //

21
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/constant/turbulenceProperties Normal file
View File

@ -0,0 +1,21 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "constant";
object turbulenceProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
simulationType RASModel;
// ************************************************************************* //

53
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/controlDict Normal file
View File

@ -0,0 +1,53 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
application pimpleDyMFoam;
startFrom latestTime;
startTime 0;
stopAt endTime;
endTime 5;
deltaT 0.005;
writeControl adjustableRunTime;
writeInterval 0.05;
purgeWrite 0;
writeFormat ascii;
writePrecision 6;
writeCompression off;
timeFormat general;
timePrecision 6;
runTimeModifiable true;
adjustTimeStep true;
maxCo 0.5;
// ************************************************************************* //

107
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/createBafflesDict Normal file
View File

@ -0,0 +1,107 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createBafflesDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// Whether to convert internal faces only (so leave boundary faces intact).
// This is only relevant if your face selection type can pick up boundary
// faces.
internalFacesOnly false;
// Baffles to create.
baffles
{
ACMI1
{
//- Use predefined faceZone to select faces and orientation.
type faceZone;
zoneName couple1Faces;
patches
{
master
{
//- Master side patch
name ACMI1_blockage;
type wall;
}
slave // not used since we're manipulating a boundary patch
{
//- Slave side patch
name ACMI1_blockage;
type wall;
}
master2
{
//- Master side patch
name ACMI1_couple;
type cyclicACMI;
matchTolerance 0.0001;
neighbourPatch ACMI2_couple;
nonOverlapPatch ACMI1_blockage;
transform noOrdering;
}
slave2 // not used since we're manipulating a boundary patch
{
//- Slave side patch
name ACMI1_couple;
type patch;
}
}
}
ACMI2
{
//- Use predefined faceZone to select faces and orientation.
type faceZone;
zoneName couple2Faces;
patches
{
master
{
//- Master side patch
name ACMI2_blockage;
type wall;
}
slave // not used since we're manipulating a boundary patch
{
//- Slave side patch
name ACMI2_blockage;
type wall;
}
master2
{
//- Master side patch
name ACMI2_couple;
type cyclicACMI;
matchTolerance 0.0001;
neighbourPatch ACMI1_couple;
nonOverlapPatch ACMI2_blockage;
transform noOrdering;
}
slave2 // not used since we're manipulating a boundary patch
{
//- Slave side patch
name ACMI2_couple;
type patch;
}
}
}
}
// ************************************************************************* //

54
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/createPatchDict Normal file
View File

@ -0,0 +1,54 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object createPatchDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
// This application/dictionary controls:
// - optional: create new patches from boundary faces (either given as
// a set of patches or as a faceSet)
// - always: order faces on coupled patches such that they are opposite. This
// is done for all coupled faces, not just for any patches created.
// - optional: synchronise points on coupled patches.
// 1. Create cyclic:
// - specify where the faces should come from
// - specify the type of cyclic. If a rotational specify the rotationAxis
// and centre to make matching easier
// - always create both halves in one invocation with correct 'neighbourPatch'
// setting.
// - optionally pointSync true to guarantee points to line up.
// 2. Correct incorrect cyclic:
// This will usually fail upon loading:
// "face 0 area does not match neighbour 2 by 0.0100005%"
// " -- possible face ordering problem."
// - in polyMesh/boundary file:
// - loosen matchTolerance of all cyclics to get case to load
// - or change patch type from 'cyclic' to 'patch'
// and regenerate cyclic as above
// Do a synchronisation of coupled points after creation of any patches.
// Note: this does not work with points that are on multiple coupled patches
// with transformations (i.e. cyclics).
pointSync false;
// Patches to create.
patches
(
// none
);
// ************************************************************************* //

30
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/decomposeParDict Normal file
View File

@ -0,0 +1,30 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
numberOfSubdomains 4;
method scotch;
hierarchicalCoeffs
{
n (1 4 1);
delta 0.001;
order xyz;
}
// ************************************************************************* //

63
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/fvSchemes Normal file
View File

@ -0,0 +1,63 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
ddtSchemes
{
default Euler;
}
gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) cellLimited Gauss linear 1;
}
divSchemes
{
default none;
// div(phi,U) Gauss upwind;
div(phi,U) Gauss linearUpwind grad(U);
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div((nuEff*dev(T(grad(U))))) Gauss linear;
}
laplacianSchemes
{
default Gauss linear limited corrected 0.33;
}
interpolationSchemes
{
default linear;
}
snGradSchemes
{
default limited corrected 0.33;
}
fluxRequired
{
default no;
pcorr ;
p ;
}
// ************************************************************************* //

80
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/fvSolution Normal file
View File

@ -0,0 +1,80 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
pcorr
{
solver GAMG;
tolerance 1e-2;
relTol 0;
smoother GaussSeidel;
cacheAgglomeration no;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
maxIter 50;
}
p
{
$pcorr;
tolerance 1e-5;
relTol 0.01;
}
pFinal
{
$p;
tolerance 1e-6;
relTol 0;
}
"(U|k|epsilon)"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-6;
relTol 0.1;
}
"(U|k|epsilon)Final"
{
$U;
tolerance 1e-6;
relTol 0;
}
}
PIMPLE
{
correctPhi no;
nOuterCorrectors 1;
nCorrectors 2;
nNonOrthogonalCorrectors 0;
}
relaxationFactors
{
// "(U|k|epsilon).*" 1;
}
cache
{
grad(U);
}
// ************************************************************************* //

89
tutorials/incompressible/pimpleDyMFoam/oscillatingInletACMI2D/system/topoSetDict Normal file
View File

@ -0,0 +1,89 @@
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: dev |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object topoSetDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
actions
(
// Get both sides of ami
// ~~~~~~~~~~~~~~~~~~~~~
// Create faceZone for patch couple1
{
name couple1Faces;
type faceSet;
action new;
source patchToFace;
sourceInfo
{
name couple1;
}
}
{
name couple1Faces;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet couple1Faces;
}
}
// Create faceZone for patch couple2
{
name couple2Faces;
type faceSet;
action new;
source patchToFace;
sourceInfo
{
name couple2;
}
}
{
name couple2Faces;
type faceZoneSet;
action new;
source setToFaceZone;
sourceInfo
{
faceSet couple2Faces;
}
}
// Create cellZone for moving cells in inlet channel
{
name inletChannel;
type cellSet;
action new;
source boxToCell;
sourceInfo
{
box (-100 -100 -100) (1.0001 100 100);
}
}
{
name inletChannel;
type cellZoneSet;
action new;
source setToCellZone;
sourceInfo
{
set inletChannel;
}
}
);
// ************************************************************************* //