Modified pimpleFoam solver to MRFPimpleFoam solver

hiuluom · June 8, 2015, 08:18

Hi everyone,

I know MRFSimpleFoam solver is steady incompressible. But now I would like to simulation MRF zone with unsteady incompressible. Hence, I modified the pimpleFoam solver becoming MRFPimpleFoam. Here code:

MRFPimpleFoam.C

Code:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     |
    \\  /    A nd           | Copyright (C) 2011 OpenFOAM Foundation
     \\/     M anipulation  |
-------------------------------------------------------------------------------
License
    This file is part of OpenFOAM.

    OpenFOAM is free software: you can redistribute it and/or modify it
    under the terms of the GNU General Public License as published by
    the Free Software Foundation, either version 3 of the License, or
    (at your option) any later version.

    OpenFOAM is distributed in the hope that it will be useful, but WITHOUT
    ANY WARRANTY; without even the implied warranty of MERCHANTABILITY or
    FITNESS FOR A PARTICULAR PURPOSE.  See the GNU General Public License
    for more details.

    You should have received a copy of the GNU General Public License
    along with OpenFOAM.  If not, see <http://www.gnu.org/licenses/>.

Application
    MRFSimpleFoam

Description
    Steady-state solver for incompressible, turbulent flow of non-Newtonian
    fluids with MRF regions.

\*---------------------------------------------------------------------------*/

#include "fvCFD.H"
#include "singlePhaseTransportModel.H"
#include "RASModel.H"
#include "MRFZones.H"
#include "simpleControl.H"
#include "IObasicSourceList.H"

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

int main(int argc, char *argv[])
{
    #include "setRootCase.H"

    #include "createTime.H"
    #include "createMesh.H"
    #include "createFields.H"
    #include "initContinuityErrs.H"

    MRFZones mrfZones(mesh);
    mrfZones.correctBoundaryVelocity(U);

    simpleControl simple(mesh);

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

    Info<< "\nStarting time loop\n" << endl;

    while (simple.loop())
    {
        Info<< "Time = " << runTime.timeName() << nl << endl;

        // --- Pressure-velocity SIMPLE corrector
        {
            #include "UEqn.H"
            #include "pEqn.H"
        }

        turbulence->correct();

        runTime.write();

        Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s"
            << "  ClockTime = " << runTime.elapsedClockTime() << " s"
            << nl << endl;
    }

    Info<< "End\n" << endl;

    return 0;
}


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

pEqn.H

Code:

{
    p.boundaryField().updateCoeffs();

    volScalarField rAU(1.0/UEqn().A());
    U = rAU*UEqn().H();
    UEqn.clear();

    phi = fvc::interpolate(U, "interpolate(HbyA)") & mesh.Sf();
    mrfZones.relativeFlux(phi);
    adjustPhi(phi, U, p);

    // Non-orthogonal pressure corrector loop
    while (simple.correctNonOrthogonal())
    {
        fvScalarMatrix pEqn
        (
            fvm::laplacian(rAU, p) == fvc::div(phi)
        );

        pEqn.setReference(pRefCell, pRefValue);
        pEqn.solve();

        if (simple.finalNonOrthogonalIter())
        {
            phi -= pEqn.flux();
        }
    }

    #include "continuityErrs.H"

    // Explicitly relax pressure for momentum corrector
    p.relax();

    // Momentum corrector
    U -= rAU*fvc::grad(p);
    U.correctBoundaryConditions();
    sources.correct(U);
}

uEqn.H

Code:

    // Momentum predictor

    tmp<fvVectorMatrix> UEqn
    (
        fvm::div(phi, U)
      + turbulence->divDevReff(U)
      ==
        sources(U)
    );

    mrfZones.addCoriolis(UEqn());

    sources.constrain(UEqn());

    UEqn().relax();

    solve(UEqn() == -fvc::grad(p));

After that, I test with mixerVessel2D model in tutorial OpenFOAM. The result was very good
https://onedrive.live.com/redir?resi...hint=folder%2c

When I simulated with 3D model as turbine. I think it is inaccurate. I do not see the vortex after tubine.
https://onedrive.live.com/redir?resi...nt=photo%2cpng

I don't know velocity not change. Could anybody show me my mistake, please?

Thank you so much

blais.bruno · June 8, 2015, 11:41

If you look at the original article proposing the MRF method, by

J. Luo, R. Issa, A. Gosman, Prediction of impeller induced flows in mixing vessels using multiple frames of reference, in: Institution of Chemical
Engineers Symposium Series, Vol. 136.

They mention that this method is not valid for unsteady state. Actually, there are some underlying hypotheses to the MRF method, which make it inappropriate for unsteady simulations.
So it might work in 2D because you converge to a steady state and your unsteady solver becomes a relaxed steady solver. However, it will not be an appropriate approach in 3D.

Why not use sliding mesh (AMI) instead? I know it is slightly more expensive, but still...

hiuluom · June 8, 2015, 13:28

Hi Bruno,

Thanks your reply.

The turbine model has AMI sliding mesh. I have already run with MRFSimpleFoam and it's convergence. I would like to run with unsteady because I change the inlet velocity to oscilatingValued instead of fixValued.
Here is formula: u = 2.7 + 1.6(sìn2(pi)t/16).

MRFSimpleFoam only run steady state with simple interpolation that is reason I modified pimpleFoam. How can run MRF simulation with inlet velocity above?

P/s: I do not want to use pimpleDymFoam.

sharonyue · June 8, 2015, 13:50

Hello!

I dont think MRF can not be applied into unsteady state situations. In OpenFOAM, multi-phase solvers such as interFoam and twoPhaseEulerFoam can use MRF to simulate stirred tanks.

Which version r u using? pimpleFoam2.3.x can handle MRF by itself.

Best,

hiuluom · June 8, 2015, 22:07

Hi Dongyue,

I am using OF 2.1.1. I can not upgrade 2.3.x because I am running on server.

By the way, can pimpleFoam in 2.3.x version solve MRF? Which can MRF solver run with "oscillatingFixedValue" inlet BCs?

hiuluom · June 10, 2015, 02:35

Dear all,

I show the velocity result MRFSimpleFoam sovler OF 2.1.1 and pimpleFoam solver OF 2.3.0.

The MRFSimple give very good result, but in pimpleFoam does not see the rear vortex of turbine. In pimpleFoam OF 2.3.0, I only added fvoption

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

MRF1
{
    type            MRFSource;
    active          true;
    selectionMode   cellZone;
    cellZone        fluid_MRF;

    MRFSourceCoeffs
    {
        origin      (0 0 0);
        axis        (1 0 0);
        omega       2;
    }
}


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

If a model want to run MRF with pimpleFoam solver, is it only add fvOption into system directory?

Thank you so much.
Thanh

sharonyue · June 10, 2015, 03:29

Quote:

Originally Posted by hiuluom

Dear all,

If a model want to run MRF with pimpleFoam solver, is it only add fvOption into system directory?

Thank you so much.
Thanh

Oops, maybe Im wrong. Sorry,

I just check the code, in two-phase solver, MRF is embeded into pimple algorithm not by fvOptions but by mrfZone class, so maybe even fvOptions can deal with MRF(for steady-state), but it can not be used for pimpleFoam(transient). I guess.

Also, I checked with u original code MRFpimpleFoam, u make ur Ueqn() to be cleared in time step. This is not rite, u need UEqn to upgrade to solve pEqn 2 or 3 times. This is piso algorithm. Maybe u can merge pimpleFoam+mrfZone class instead of doing modifications on simpleFoam.

I make a MRFPimpleFoam solver based on pimpleFoam and tried on the mixer2D case, looks its rite. If u can upload a case to make a test that will be better.

hiuluom · June 10, 2015, 03:53

Hi sharonyue,

Here is my BCs:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*  Windows port by Symscape (www.symscape.com)                              *\
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -3 0 0 0 0];
internalField   uniform 0.598;
boundaryField
{
    stator
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    rotor
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    symmetry
    {
        type            epsilonWallFunction;
        value           uniform 10.935;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.598;
    }
    outlet
    {
        type            zeroGradient;
    }
    wing1
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    wing2
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    wing3
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    wing4
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    wing5
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    wing6
    {
        type            epsilonWallFunction;
        value           uniform 1;
    }
    AMI1_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI2_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
}
// ************************************************************************* //

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*  Windows port by Symscape (www.symscape.com)                              *\
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 0.0055;
boundaryField
{
    stator
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    rotor
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    symmetry
    {
        type            kqRWallFunction;
        value           uniform 0.135;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 0.0055;
    }
    outlet
    {
        type            zeroGradient;
    }
    wing1
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    wing2
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    wing3
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    wing4
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    wing5
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    wing6
    {
        type            kqRWallFunction;
        value           uniform 1;
    }
    AMI1_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI2_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
}
// ************************************************************************* //

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*  Windows port by Symscape (www.symscape.com)                              *\
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 0;
boundaryField
{
    stator
    {
        type            zeroGradient;
    }
    rotor
    {
        type            zeroGradient;
    }
    symmetry
    {
        type            zeroGradient;
    }
    inlet
    {
        type            zeroGradient;
    }
    outlet
    {
        type            fixedValue;
        value           uniform 0;
    }
    wing1
    {
        type            zeroGradient;
    }
    wing2
    {
        type            zeroGradient;
    }
    wing3
    {
        type            zeroGradient;
    }
    wing4
    {
        type            zeroGradient;
    }
    wing5
    {
        type            zeroGradient;
    }
    wing6
    {
        type            zeroGradient;
    }
    AMI1_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI2_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
}
// ************************************************************************* //

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*  Windows port by Symscape (www.symscape.com)                              *\
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (-6.2 0 0);
boundaryField
{
    stator
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    rotor
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    symmetry
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    inlet
    {
        type            fixedValue;
        value           uniform (-6.2 0 0);
    }
    outlet
    {
        type            zeroGradient;
    }
    wing1
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wing2
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wing3
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wing4
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wing5
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    wing6
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    AMI1_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
    AMI2_fluid_MRF
    {
        type            cyclicAMI;
        value           $internalField;
    }
}
// ************************************************************************* //

boundaryDIct:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

/*  Windows port by Symscape (www.symscape.com)                              *\
\*---------------------------------------------------------------------------*/

FoamFile
{
    version                 2.0; 
    format                  ascii; 
    class                   polyBoundaryMesh; 
    location                "constant/polyMesh"; 
    object                  boundary; 
}

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

13
(
    stator
    {
        type                    wall; 
        nFaces                  4352; 
        startFace               9025787; 
    }

    rotor
    {
        type                    wall; 
        nFaces                  5288; 
        startFace               9030139; 
    }

    symmetry
    {
        type                    wall; 
        nFaces                  3676; 
        startFace               9035427; 
    }

    inlet
    {
        type                    patch;  //Velocity-inlet
        nFaces                  514; 
        startFace               9039103; 
    }

    outlet
    {
        type                    patch;  //Pressure-outlet
        nFaces                  516; 
        startFace               9039617; 
    }

    wing1
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9040133; 
    }

    wing2
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9068557; 
    }

    wing3
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9096981; 
    }

    wing4
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9125405; 
    }

    wing5
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9153829; 
    }

    wing6
    {
        type                    wall; 
        nFaces                  28424; 
        startFace               9182253; 
    }

    AMI1_fluid_MRF
    {
        type                    cyclicAMI; 
        nFaces                  7712; 
        startFace               9210677; 
        matchTolerance          0.0001; 
        neighbourPatch          AMI2_fluid_MRF; 
        transform               noOrdering; 
    }

    AMI2_fluid_MRF
    {
        type                    cyclicAMI; 
        nFaces                  7712; 
        startFace               9218389; 
        matchTolerance          0.0001; 
        neighbourPatch          AMI1_fluid_MRF; 
        transform               noOrdering; 
    }

)

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

The first time I have simulated with MRFsimpleFoam OF2.1.1. After that, I would like to simulation with unsteady, so I modified pimpleFoam OF2.1.1 and it did not run. As you said, I install OF 2.3.0 and run pimpleFoam with MRF fvOption. The result pimpleFoam OF 2.3.0 still not good. I don't know what I missed file or BCs.

sharonyue · June 10, 2015, 04:12

Hi,

I updated my post, this solver should be the same with yours, but its based on pimpleFoam. Maybe u can upload your 3D case and make a simple test.

About ur boundaries, its right

hiuluom · June 10, 2015, 04:53

Everthing I post above. resultThe result ran with MRFSimpleFoam solver OF 2.1.1 very good. I would like to run oscilating velocity inlet. Hence, I must modified pimpleFoam OF 2.1.1 can run unsteady but it was not successful. The comparison MRFSimpleFoam and pimpleFoam result I posted at the first.

And now I am trying to simulate with pimpleFoam OF2.3.0. I only add fvoption. The result is not the same MRFSimpleFoam of2.1.1

I show test with mixerVessel pimpleFoam OF2.3.0, the result is good. But big model is not good.

Do you have any idea?

If you need more file, you can tell me.

sharonyue · June 10, 2015, 05:59

Quote:

Originally Posted by hiuluom

Everthing I post above. resultThe result ran with MRFSimpleFoam solver OF 2.1.1 very good. I would like to run oscilating velocity inlet. Hence, I must modified pimpleFoam OF 2.1.1 can run unsteady but it was not successful. The comparison MRFSimpleFoam and pimpleFoam result I posted at the first.

And now I am trying to simulate with pimpleFoam OF2.3.0. I only add fvoption. The result is not the same MRFSimpleFoam of2.1.1

I show test with mixerVessel pimpleFoam OF2.3.0, the result is good. But big model is not good.

Do you have any idea?

If you need more file, you can tell me.

Hello,

I test pimpleFoam 2.3.x with fvOptions, looks it can deal with MRF.
Also I test my solver(quite simple one), looks there is no difference. Attached is the comparison. I got this mesh from the propeller, but I make the mesh quite coarse.

I did not see any wrong on your boundary, maybe the impeller is rotating way too slow? or some setup is wrong I did not notice? How big is your mesh? U can upload your case.

hiuluom · June 10, 2015, 06:31

Hello,

Because the mesh is big I can not upload the file. My model is turbine as the same propeller. I show the checkMesh that you can imagine:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : checkMesh
Date   : Jun 10 2015
Time   : 16:25:14
Host   : "linuxserver"
PID    : 4211
Case   : /home/dfm/Working/phong-thanh/Case02_MSH-MRFPimpleFoam-of230
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           1236316
    faces:            9226101
    internal faces:   9025787
    cells:            4202604
    faces per cell:   4.34299
    boundary patches: 13
    point zones:      0
    face zones:       3
    cell zones:       2

Overall number of cells of each type:
    hexahedra:     0
    prisms:        1441472
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    2761132
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
   *Number of regions: 2
    The mesh has multiple regions which are not connected by any face.
  <<Writing region information to "0/cellToRegion"
  <<Writing region 0 with 3941656 cells to cellSet region0
  <<Writing region 1 with 260948 cells to cellSet region1

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    stator              4352     2297     ok (non-closed singly connected)  
    rotor               5288     2813     ok (non-closed singly connected)  
    symmetry            3676     1888     ok (non-closed singly connected)  
    inlet               514      283      ok (non-closed singly connected)  
    outlet              516      284      ok (non-closed singly connected)  
    wing1               28424    14232    ok (non-closed singly connected)  
    wing2               28424    14232    ok (non-closed singly connected)  
    wing3               28424    14232    ok (non-closed singly connected)  
    wing4               28424    14232    ok (non-closed singly connected)  
    wing5               28424    14232    ok (non-closed singly connected)  
    wing6               28424    14232    ok (non-closed singly connected)  
    AMI1_fluid_MRF      7712     4127     ok (non-closed singly connected)  
    AMI2_fluid_MRF      7712     4127     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-100 -39.9951 -40) (60 39.971 40)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-5.85408e-17 -4.19816e-18 6.51828e-16) OK.
    Max cell openness = 4.89647e-16 OK.
    Max aspect ratio = 14.5859 OK.
    Minimum face area = 1.07566e-06. Maximum face area = 59.4783.  Face area magnitudes OK.
    Min volume = 5.69289e-10. Max volume = 138.892.  Total volume = 802492.  Cell volumes OK.
    Mesh non-orthogonality Max: 64.5182 average: 19.8814
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.53318 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

MRFzone

Code:

zone1
{
    cellZone    fluid_MRF;
    active      yes;

    // Fixed patches (by default they 'move' with the MRF zone)
    nonRotatingPatches (AMI1_fluid_MRF AMI2_fluid_MRF stator symmetry inlet outlet);

    origin    (0 0 0);
    axis      (1 0 0);
    omega     constant 2;
}

I sent you the case in attach file.
I would like to see the vortex sam MRFSimpleFoam 2.1.1

hiuluom · June 14, 2015, 22:22

After waiting for a long time, the vortex appeared at the rear with MRFPimpleFoam 2.1.1 and pimpleFoam OF2.3.0. But in the wing MRF zone, I saw cell.

June 8, 2015, 11:41		#2
blais.bruno Member Bruno Blais Join Date: Sep 2013 Location: Canada Posts: 64 Rep Power: 13	If you look at the original article proposing the MRF method, by J. Luo, R. Issa, A. Gosman, Prediction of impeller induced flows in mixing vessels using multiple frames of reference, in: Institution of Chemical Engineers Symposium Series, Vol. 136. They mention that this method is not valid for unsteady state. Actually, there are some underlying hypotheses to the MRF method, which make it inappropriate for unsteady simulations. So it might work in 2D because you converge to a steady state and your unsteady solver becomes a relaxed steady solver. However, it will not be an appropriate approach in 3D. Why not use sliding mesh (AMI) instead? I know it is slightly more expensive, but still... granzer likes this.

June 8, 2015, 13:50		#4
sharonyue Senior Member Dongyue Li Join Date: Jun 2012 Location: Beijing, China Posts: 848 Rep Power: 18	Hello! I dont think MRF can not be applied into unsteady state situations. In OpenFOAM, multi-phase solvers such as interFoam and twoPhaseEulerFoam can use MRF to simulate stirred tanks. Which version r u using? pimpleFoam2.3.x can handle MRF by itself. Best, __________________ My OpenFOAM algorithm website: http://dyfluid.com By far the largest Chinese CFD-based forum: http://www.cfd-china.com/category/6/openfoam We provide lots of clusters to Chinese customers, and we are considering to do business overseas: http://dyfluid.com/DMCmodel.html

June 8, 2015, 22:07		#5
hiuluom Senior Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 105 Rep Power: 13	Hi Dongyue, I am using OF 2.1.1. I can not upgrade 2.3.x because I am running on server. By the way, can pimpleFoam in 2.3.x version solve MRF? Which can MRF solver run with "oscillatingFixedValue" inlet BCs? Last edited by hiuluom; June 9, 2015 at 01:44.

June 10, 2015, 04:12		#9
sharonyue Senior Member Dongyue Li Join Date: Jun 2012 Location: Beijing, China Posts: 848 Rep Power: 18	Hi, I updated my post, this solver should be the same with yours, but its based on pimpleFoam. Maybe u can upload your 3D case and make a simple test. About ur boundaries, its right __________________ My OpenFOAM algorithm website: http://dyfluid.com By far the largest Chinese CFD-based forum: http://www.cfd-china.com/category/6/openfoam We provide lots of clusters to Chinese customers, and we are considering to do business overseas: http://dyfluid.com/DMCmodel.html

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[swak4Foam] Problem using swak4Foam in a modiefied solver	bastil	OpenFOAM Community Contributions	13	April 18, 2020 16:17
error while running modified pimple solver	R_21	OpenFOAM Programming & Development	0	May 28, 2015 07:59
compiling error(s) in a modified twoPhaseEulerFoam solver	foamer	OpenFOAM	14	June 20, 2014 09:51
CFX 5.5	Roued	CFX	1	October 2, 2001 17:49
Setting a B.C using UserFortran in 4.3	tokai	CFX	10	July 17, 2001 17:25

June 8, 2015, 13:28		#3
hiuluom Senior Member Huynh Phong Thanh Join Date: Aug 2013 Location: Ho Chi Minh City Posts: 105 Rep Power: 13	Hi Bruno, Thanks your reply. The turbine model has AMI sliding mesh. I have already run with MRFSimpleFoam and it's convergence. I would like to run with unsteady because I change the inlet velocity to oscilatingValued instead of fixValued. Here is formula: u = 2.7 + 1.6(sìn2(pi)t/16). MRFSimpleFoam only run steady state with simple interpolation that is reason I modified pimpleFoam. How can run MRF simulation with inlet velocity above? P/s: I do not want to use pimpleDymFoam.