[Slaninář]

Hello,
I'm trying to simulate two MRFs in OpenFOAM 11. MRFProperties is:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  11
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       dictionary;
    location    "constant";
    object      MRFProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


MRF1
{
    cellZone    Rotor;
    active      yes;

    // Fixed patches (by default they 'move' with the MRF zone)
    nonRotatingPatches (Rotor_in Rotor_out );

    origin    (0 0 0);
    axis      (0 0 1);
    // omega     -151.843644923507;
    rpm       -1450;
}


MRF2
{
    cellZone    Mrot;
    active      yes;

    // Fixed patches (by default they 'move' with the MRF zone)
    nonRotatingPatches (Mrot_out Mrot_in );

    origin    (0 0 0);
    axis      (0 0 1);
    rpm       -1450;
}




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

However, for incompressibleFluid solver, this error occurs:

/*---------------------------------------------------------------------------*\ 
  =========                 | 
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox 
   \\    /   O peration     | Website:  https://openfoam.org 
    \\  /    A nd           | Version:  11 
     \\/     M anipulation  | 
\*---------------------------------------------------------------------------*/ 
Build  : 11 
Exec   : foamRun 
Date   : Apr 27 2024 
Time   : 13:06:18 
Host   : "slaninar-extreme4" 
PID    : 105828 
I/O    : uncollated 
Case   : /media/slaninar/0f1eafad-3b93-4c73-9544-109935e24a87/Programy/OpenFOAM/slaninar-10/run_org/PumpOFI/OpenFOAM_1 
nProcs : 1 
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE). 
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10) 
allowSystemOperations : Allowing user-supplied system call operations 

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

Create mesh for time = 0 

patchToPatch: Calculating couplings between 2660 source faces and 10952 target faces 
    Source min/average/max coverage = 0.860403/0.99973/1 
    Target min/average/max coverage = 0.90105/0.999733/1 
    Source average openness/error/depth/angle = 1.34718e-16/2.43049e-15/3.25552e-16/0 
    Source max openness/error/depth/angle = 7.97206e-16/2.43812e-14/2.90293e-15/0 
    51018 couplings calculated in 0.296447s 
patchToPatch: Calculating couplings between 10796 source faces and 20636 target faces 
    Source min/average/max coverage = 0.623984/0.999557/1 
    Target min/average/max coverage = 0.225696/0.999953/1 
    Source average openness/error/depth/angle = 1.21878e-16/0.000701521/0.000723702/0.126176 
    Source max openness/error/depth/angle = 6.64406e-16/0.38887/0.158765/24.1916 
    126220 couplings calculated in 0.654447s 
patchToPatch: Calculating couplings between 33155 source faces and 21924 target faces 
    Source min/average/max coverage = 0.5/0.999924/1 
    Target min/average/max coverage = 0.726963/0.999915/1 
    Source average openness/error/depth/angle = 1.35812e-16/0.00186038/0.0220941/0.75074 
    Source max openness/error/depth/angle = 1.83427e-15/0.385519/0.480225/32.9898 
    214126 couplings calculated in 1.56214s 
fvMeshStitcher: Connecting 
    Cell min/avg/max openness = 0/4.93197e-17/3.68435e-16 
Selecting solver incompressibleFluid 
Selecting viscosity model constant 
Selecting turbulence model type RAS 
Selecting RAS turbulence model realizableKE 
RAS 
{ 
    model           realizableKE; 
    turbulence      on; 
    printCoeffs     on; 
    A0              4; 
    C2              1.9; 
    sigmak          1; 
    sigmaEps        1.2; 
} 

Creating MRF zone list from MRFProperties 
    creating MRF zone: MRF1 
    - selecting cells using cellZone Rotor 
    - selected 2354137 cell(s) with volume 0.00201508 
    creating MRF zone: MRF2 
    - selecting cells using cellZone Mrot 
    - selected 79156 cell(s) with volume 0.0001888 

SIMPLE: Convergence criteria found 
        p: tolerance 1e-06 
        U: tolerance 1e-06 
        "(k|omega)": tolerance 1e-06 


SIMPLE: Operating solver in steady-state mode with 1 outer corrector 
SIMPLE: Operating solver in SIMPLE mode 



Starting time loop 

Constructing face momentum Uf 


--> FOAM FATAL ERROR:  
MRFZoneName not specified 

    From function const Foam::MRFZone& Foam::MRFPatchField::MRFzone(const Foam::objectRegistry&) const 
    in file cfdTools/general/MRF/derivedFvPatchFields/MRFPatchField/MRFPatchField.C at line 78. 

FOAM exiting

If only one MRF zone is in MRFProperties everything works.
I found this thread but it is old and it doesn't solve my problem.
Does anybody know how to solve it?

[Marcelinus]

Hi there,



I got the same error a couple days ago and this was my fix:


In the velocity boundary file you need to specify the name of the MRF zone if there are multiple. Like this:

MRFRegion1
            {
                    type                 MRFnoSlip;
                    MRFZoneName    zone1;
            }

          MRFRegion2
            {
                    type                  MRFnoSlip;
                    MRFZoneName     zone2;
             }

You can get the name of the zone from the MRFProperties file. Hope this helps.

zone1
         {

                   cellZone    cell_1;
                   active       yes;

                   //nonRotatingPatches ();

                   origin    (-5.480-0.3003.000);
                   axis      (-0.346410.2000);

                   //omega     12.566370;
                   rpm            365;
          }

          zone2
          {
                   cellZone        cell_2;
                   active           yes;

                   //nonRotatingPatches ();

                   origin      (4.7752550.7071074.085786);
                   axis        (0.367423-0.2121320.424264);

                   //omega     12.566370;
                   rpm            69;
          }

[Slaninář]

It works. Now incompressible solver calculates two MRFs and results look believable. Thank you very much!

[luise_]

Unfortunately, this did not work. Are there any other ideas for solving the problem?

[Marcelinus]

Hello Luise,

what exactly did not work for you? What is the error message?

Kind regards

Marcelinus

[luise_]

Hello Marcelinus,

thanks for the fast reply!

I receive the same error message as Slaninář.

Pstream initialised with:
floatTransfer : false
nProcsSimpleSum : 0
commsType : nonBlocking
polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Selecting solver incompressibleFluid
Selecting viscosity model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
bounding k, min: 0 max: 0 average: 0
RAS
{
RASModel kOmegaSST;
turbulence on;
printCoeffs on;
alphaK1 0.85;
alphaK2 1;
alphaOmega1 0.5;
alphaOmega2 0.856;
gamma1 0.555556;
gamma2 0.44;
beta1 0.075;
beta2 0.0828;
betaStar 0.09;
a1 0.31;
b1 1;
c1 10;
F3 false;
}

Creating MRF zone list from MRFProperties
creating MRF zone: MRF_CW
- selecting cells using cellZone cellMRF_CWzone
- selected 2228629 cell(s) with volume 0.00503231
creating MRF zone: MRF_CCW
- selecting cells using cellZone cellMRF_CCWzone
- selected 2229399 cell(s) with volume 0.00503207
creating MRF zone: MRF_CW_f
- selecting cells using cellZone cellMRF_CW_fzone
- selected 2227378 cell(s) with volume 0.00503237
creating MRF zone: MRF_CCW_b
- selecting cells using cellZone cellMRF_CCW_bzone
- selected 2227898 cell(s) with volume 0.00503223

SIMPLE: No convergence criteria found


SIMPLE: Operating solver in steady-state mode with 1 outer corrector
SIMPLE: Operating solver in SIMPLE mode



Starting time loop

forces forcesCoeffs:
Not including porosity effects
forceCoeffs forcesCoeffs:
Not including porosity effects
forces forces:
Not including porosity effects
forceCoeffs forcesCoeffs write:
Cm = 0
Cd = 0
Cl = 0
Cl(f) = 0
Cl(r) = 0

forces forces write:
sum of forces:
pressure : (0 0 0)
viscous : (0 0 0)
porous : (0 0 0)
sum of moments:
pressure : (0 0 0)
viscous : (0 0 0)
porous : (0 0 0)

Constructing face momentum Uf
[0] --> FOAM FATAL ERROR:
[0] MRFZoneName not specified
[0]
[0] From function const Foam::MRFZone& Foam::MRFPatchField::MRFzone(const Foam:bjectRegistry&) const
[0] in file cfdTools/general/MRF/derivedFvPatchFields/MRFPatchField/MRFPatchField.C at line 78.
[0]
FOAM parallel run exiting

I tried what you suggested here:

MRF_CW
{

    cellZone    cellMRF_CWzone;
    active      yes;
    
    nonRotatingPatches ("drone.*");

    origin   (-0.176876 -0.176876 0.0639516);
    axis      (0 0 1);

    rpm       -6000;
}

MRF_CCW
{

    cellZone    cellMRF_CCWzone;
    active      yes;
    
        nonRotatingPatches ("drone.*");

    origin   (0.176876 -0.176876 0.0639516);
    axis      (0 0 1);

    rpm       6000;
}


MRF_CW_f
{

    cellZone    cellMRF_CW_fzone;
    active      yes;
    nonRotatingPatches ( "drone.*");
   // nonRotatingPatches (inlet "propeller_CCW.*" "propeller_CCW_b.*" "propeller_CW.*" outlet "drone.*");

    origin   (0.176876 0.176876 0.0639516);
    axis      (0 0 1);

    rpm       -6000;
}

MRF_CCW_b
{

    cellZone    cellMRF_CCW_bzone;
    active      yes;
    
        nonRotatingPatches ("drone.*");

    origin   (-0.176876 0.176876 0.0639516);
    axis      (0 0 1);

    rpm       6000;
}

and

 
MRFRegion1
    {
             type                 MRFnoSlip;
             MRFZoneName   MRF_CW;
    }

     MRFRegion2
     {
      type                  MRFnoSlip;
      MRFZoneName     MRF_CCW;
      }
             
	MRFRegion3
        {
              type                  MRFnoSlip;
              MRFZoneName     MRF_CW_f;
        }
       MRFRegion4
       {
              type                 MRFnoSlip;
              MRFZoneName    MRF_CCW_b;
       }

Maybe I am just missing something. I am happy about any help.

[Slaninář]

Hi,
I don't see any problem in your previous post, luise_. I may have missed something. However is it possible to provide full U file? Are you using OpenFOAM V11 and incompressible solver? I have no experience with OF V12 yet.

[luise_]

Hello,

yes I am using OF11 and incompressible Solver. Here is my full U file:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  11
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"
    
         "propeller_CW.*"
    {
        type            MRFnoSlip;
    }
           "propeller_CCW.*"
    {
        type            MRFnoSlip;
    }
    "propeller_CW_f.*"
    {
        type            MRFnoSlip;
    }
    
        "propeller_CCW_b.*"
    {
        type            MRFnoSlip;
    }
            "drone.*"
    {
        type           noSlip;
    }   

    inlet
    {
        type                freestreamVelocity;
        freestreamValue0    (0 0 0);
        freestreamValue     $internalField;
    }
    
    outlet
    {
        type                freestreamVelocity;
        freestreamValue0    (0 0 0);
        freestreamValue     $internalField;
    }
   
    MRFRegion1
    {
             type                 MRFnoSlip;
             MRFZoneName   MRF_CW;
    }

     MRFRegion2
     {
      type                  MRFnoSlip;
      MRFZoneName     MRF_CCW;
      }
             
	MRFRegion3
        {
              type                  MRFnoSlip;
              MRFZoneName     MRF_CW_f;
        }
       MRFRegion4
       {
              type                 MRFnoSlip;
              MRFZoneName    MRF_CCW_b;
       }
             
           
}

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

[Slaninář]

I think I know where the problem is. There are MRFnoSlip boundaries in the U file located in different MRF zones. Is that so? However, for these boundaries, MRFZoneName isn't defined. I think the U file should look like this:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  11
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    format      ascii;
    class       volVectorField;
    location    "0";
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    #includeEtc "caseDicts/setConstraintTypes"
    
    "propeller_CW.*"
    {
        type            MRFnoSlip;
        MRFZoneName   MRF_CW;
    }
    "propeller_CCW.*"
    {
        type            MRFnoSlip;
        MRFZoneName     MRF_CCW;
    }
    "propeller_CW_f.*"
    {
        type            MRFnoSlip;
        MRFZoneName     MRF_CW_f;
    }
    
    "propeller_CCW_b.*"
    {
        type            MRFnoSlip;
        MRFZoneName    MRF_CCW_b;
    }
    "drone.*"
    {
        type           noSlip;
    }   

    inlet
    {
        type                freestreamVelocity;
        freestreamValue0    (0 0 0);
        freestreamValue     $internalField;
    }
    
    outlet
    {
        type                freestreamVelocity;
        freestreamValue0    (0 0 0);
        freestreamValue     $internalField;
    }
}

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

I removed the MRFRegionsX boundary because I think there's been a misunderstanding. Of course, if MRFRegionsX are rotating walls in MRF zones then it is necessary to define these as well.