T-junction simulation using interFoam

cmoreno98 · March 5, 2020, 13:25

Hello everybody,

I'm new to OpenFOAM and I'm trying to run a simulation of a T-junction (air entering through one inlet and water through the other) in microgravity conditions (g approximately 0). Since a picture is worth a thousand words, I show you the geometry and the mesh:

The mesh is done in Ansys and exported in .msh format. Then, the fluent3DMeshToFoam command is used to convert it from ASCII format to foam format.
The diameter of the channels is 1 mm, through the horizontal inlet (inlet1, walls1) enters air and through the vertical inlet (inlet2, walls2) enters water, both at 0.1 m/s.

I can consider the two flows to be incompressible, so I use interFoam solver. I know that the results should be something like this:

Air should advance through the horizontal pipe, meet the water at the junction and generate some bubbles. But when I run the simulation, air is not advancing through the channel and it's getting 'stucked' at the inlet like this:

I attach the three directories "0" (alpha.air, p_rgh and U files), "constant" (g, transportProperties and turbulenceProperties files) and "system" (controlDict, fvSchemes and fvSolution files) in the following link because I don't know where the problem is:
https://www.mediafire.com/file/60tv4...ction.rar/file

Some parameters:

inlet1 velocity: uniform (0.1 0 0); inlet2 velocity: uniform (0 -0.1 0)

deltaT = 5e-6; endTime = 0.2; writeInterval = 0.0016 (total of 125 directories)

How could I fix this problem? Thank you in advance,

Carlos.

crubio.abujas · March 6, 2020, 07:04

Hi Carlos,

The problem is on the boundary definition of the pressure. You have to tell OpenFOAM to calculate the required pressure to provide a specific flux, not just set it to 0.
Than can be done using fixedFluxPressure BC. You have to do it with both inlet1 and inlet2.

0/p_rgh:

Code:

    inlet1
    {
            type                 fixedFluxPressure;
            value                uniform 0;
     }

Hope it works!

cmoreno98 · March 6, 2020, 12:38

Quote:

Originally Posted by crubio.abujas

Hi Carlos,

The problem is on the boundary definition of the pressure. You have to tell OpenFOAM to calculate the required pressure to provide a specific flux, not just set it to 0.
Than can be done using fixedFluxPressure BC. You have to do it with both inlet1 and inlet2.

0/p_rgh:

Code:

    inlet1
    {
            type                 fixedFluxPressure;
            value                uniform 0;
     }

Hope it works!

Thank you very much Carlos, now the air moves

But I have another problem: the simulation is not behaving as expected when the two fluids meet at the junction. These are the results at t = 0.0112 (everything is OK):

This is the last time step where the results are the ones that I expect. From this point on, air and water mix in a strange way (screenshot at t = 0.0192):

The Courant number blows up, causing the simulation to stop (the last directory that I obtain is t = 0.0272, when it should end at t = 0.2).

I don't know if the problem is that the mesh is not good enough or that some files are not OK. For instance, inside "system" directory, I don't know if decomposeParDict or setFieldsDict are mandatory files

I didn't include them... (soy nuevo en OpenFOAM y puede que haya cosas básicas que esté haciendo mal, no sé si el problema estará en el mallado o en alguno de los archivos)

Anyone knows how to solve this problem? Thanks

crubio.abujas · March 9, 2020, 04:19

Hello again Carlos,

It seems that you have some issues with the BC of the phases. On the file alpha.air you have fixed the value of the walls to always be 0 (water). I don't know if that is a design requirement but it seems that is blowing up your simulation. Try changing it to zeroGradient, that would make the simulation more stable.

You can check your mesh using the command checkMesh, that will tell you if some mesh metrics is wrong, altough if you use an external mesher you may have that information from it. The mesh do not seem to be too distorted, although the cell size can be too big to capture the interphase properly or other flux phenomenon. If you want to play around with mesh size you can use refineMesh to create a more resolute version of the current mesh.

Concerning the files you mentioned, the file decomposeParDict is for paralleling your simulation. It tells OF how to split your mesh in sections for each parallel process.

The file setFieldDict is for imposing a set of values inside your domain. Neither of these file is strictly mandatory.

Hope that helps you!

cmoreno98 · March 10, 2020, 18:39

Good night Carlos,

Quote:

Originally Posted by crubio.abujas

It seems that you have some issues with the BC of the phases. On the file alpha.air you have fixed the value of the walls to always be 0 (water). I don't know if that is a design requirement but it seems that is blowing up your simulation. Try changing it to zeroGradient, that would make the simulation more stable.

Thanks, it makes sense to change it to zeroGradient. It is not a design requirement to have water at the walls.

Quote:

Originally Posted by crubio.abujas

You can check your mesh using the command checkMesh, that will tell you if some mesh metrics is wrong, altough if you use an external mesher you may have that information from it. The mesh do not seem to be too distorted, although the cell size can be too big to capture the interphase properly or other flux phenomenon. If you want to play around with mesh size you can use refineMesh to create a more resolute version of the current mesh.

Regarding the mesh, I changed it a little bit in order to have smaller cells near the walls:

Using the command checkMesh on this mesh, the result is the following:

Code:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 6-fa1285188035
Exec   : checkMesh
Date   : Mar 10 2020
Time   : 17:27:50
Host   : "carlos"
PID    : 4375
I/O    : uncollated
Case   : /home/carlos/OpenFOAM/carlos-6/run/prueba
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           42144
    internal points:  37871
    faces:            227803
    internal faces:   221109
    cells:            95071
    faces per cell:   4.72186
    boundary patches: 5
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     7200
    prisms:        54228
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    33643
    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: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    inlet1              582      500      ok (non-closed singly connected)  
    walls1              4174     2138     ok (non-closed singly connected)  
    inlet2              756      639      ok (non-closed singly connected)  
    walls2              600      640      ok (non-closed singly connected)  
    outlet              582      500      ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 -0.0005 -0.0005) (0.006 0.0015 0.0005)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (-3.83452e-17 -8.17958e-17 -2.72592e-17) OK.
    Max cell openness = 1.39693e-15 OK.
    Max aspect ratio = 38.1396 OK.
    Minimum face area = 1.38676e-10. Maximum face area = 1.38029e-08.  Face area magnitudes OK.
    Min volume = 5.93772e-15. Max volume = 4.59938e-13.  Total volume = 5.50062e-09.  Cell volumes OK.
    Mesh non-orthogonality Max: 58.5843 average: 13.0879
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.52523 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

 End

Is it good enough? Maybe I should make smaller cells.

Quote:

Originally Posted by crubio.abujas

Concerning the files you mentioned, the file decomposeParDict is for paralleling your simulation. It tells OF how to split your mesh in sections for each parallel process.

The file setFieldDict is for imposing a set of values inside your domain. Neither of these file is strictly mandatory.

Hope that helps you!

Thank you for the explanation. I won't set up these files by the moment since they are optional.

So, following your recommendations, alpha.air, p_rgh, U and controlDict files should be like this?

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }

    inlet2
    {
        type            fixedValue;
    value        uniform 0;
    }

    walls1
    {
        type            zeroGradient;
    }

    walls2
    {
        type            zeroGradient;
    }

    outlet
    {
        type            zeroGradient;
    }
}

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

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedFluxPressure;
    value        uniform 0;
    }

    inlet2
    {
        type            fixedFluxPressure;
    value        uniform 0;
    }

    walls1
    {
        type            zeroGradient;
    }

    walls2
    {
        type            zeroGradient;
    }

    outlet
    {
        type            fixedValue;
    value        uniform 0; //Atmospheric pressure (Pgage)
    }
}

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

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     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
{
    inlet1
    {
        type            fixedValue;
        value           uniform (0.1 0 0);
    }

    inlet2
    {
        type            fixedValue;
        value           uniform (0 -0.1 0);
    }

    walls1
    {
        type            noSlip;
    }

    walls2
    {
        type            noSlip;
    }

    outlet
    {
        type            zeroGradient;
    }
}

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

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     interFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         0.2;

deltaT          0.000005;

writeControl    adjustableRunTime;

writeInterval   0.0016;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;

adjustTimeStep  no;

maxCo           2;
maxAlphaCo      1;

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

I have run the simulation again and I get a strange behavior of the air: it goes inside the vertical channel of water, like this:

It doesn't make sense and causes the Courant number to blow up after some iterations. Why is this happening? Is there a way to restrict the entrance of air into the vertical pipe? Or is happening because the cells of the mesh are not small enough? I could improve the mesh but I should decrease the time step in order to ensure that $Co=U\frac{\Delta t}{\Delta x}<1$ (and this simulation already took me 3.5 hours...).

I would be hugely grateful if you can help me with this issue.

Thank you very much,

Carlos.

crubio.abujas · March 11, 2020, 11:20

Hi again!

Its hard to tell... I've tried your set up and it worked for me. Maybe is related with he OF version, what version are you using? I've tried it with OF6. You can find the results and the case definition I've used here.

I don't know it those are the expected results. The interface may be better resolved with a finer mesh, but that shouldn't make the entire simulation to crash.

Neither the residuals nor the courant number seems to have unreasonable values. By the way, you may find interesting to use PyFoam for plotting relevant information while solving.

Concerning the simulation times, you may consider using a parallel running. Add a decomposeParDict file to your system file. This file may have different configuration parameters but I recommend you to start using the scotch method, that takes care of splitting your domain for each processor. That should reduce the time of simulation.

system/decomposeParDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


// Change 4 to your machine number of cores.
numberOfSubdomains 4;

method          scotch;

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

For execute it in parallel just use:

Code:

# Split your domain in different regions, one for each process.
decomposePar

# Run in parallel. The -np value must be the same defined in the decomposeParDict
mpirun -np 4 interFoam -parallel

# Recompose the case to process the results
reconstructPar

Do not despair, beginnings are always hard!

cmoreno98 · March 13, 2020, 07:44

Quote:

Originally Posted by crubio.abujas

Hi again!

Its hard to tell... I've tried your set up and it worked for me. Maybe is related with he OF version, what version are you using? I've tried it with OF6. You can find the results and the case definition I've used here.

Thank you very much Carlos. Now this case is working perfect, you're great!

I'm using OF6 aswell.

Quote:

Originally Posted by crubio.abujas

I don't know it those are the expected results. The interface may be better resolved with a finer mesh, but that shouldn't make the entire simulation to crash.

That's exactly what I want to do right now. I want to improve the resolution of the simulation by implementing a finer mesh. I've created this one, with 500k cells and inflation around the walls.
You say that a finer mesh shouldn't make the entire simulation to crash, but it does

I have tried to make the time step smaller (from 5 $\mu s$ to 1 $\mu s$ ), but the Courant number gets very big and the simulation stops at time t = 0.01 s approximately (after running for 10 hours). Maybe the mesh is too fine? 500k cells are too many cells? (maybe I should try with 300k or so). I checked the mesh and it is OK:

Code:

/*---------------------------------------------------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
Build  : 6-fa1285188035
Exec   : checkMesh
Date   : Mar 13 2020
Time   : 12:27:15
Host   : "carlos"
PID    : 2305
I/O    : uncollated
Case   : /home/carlos/OpenFOAM/carlos-6/run/Structured/0.5_0.5_15
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 polyMesh for time = 0

Time = 0

Mesh stats
    points:           190032
    internal points:  175778
    faces:            1160192
    internal faces:   1136584
    cells:            503802
    faces per cell:   4.55889
    boundary patches: 5
    point zones:      0
    face zones:       1
    cell zones:       1

Overall number of cells of each type:
    hexahedra:     28800
    prisms:        223968
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    251034
    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: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    inlet1              1418     1126     ok (non-closed singly connected)  
    walls1              16604    8405     ok (non-closed singly connected)  
    inlet2              1784     1413     ok (non-closed singly connected)  
    walls2              2400     2480     ok (non-closed singly connected)  
    outlet              1402     1118     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 -0.0005 -0.0005) (0.006 0.0015 0.0005)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (8.67928e-17 -5.65932e-16 6.04785e-17) OK.
    Max cell openness = 8.52587e-16 OK.
    Max aspect ratio = 19.5164 OK.
    Minimum face area = 6.89058e-11. Maximum face area = 2.7508e-09.  Face area magnitudes OK.
    Min volume = 1.41624e-15. Max volume = 6.88307e-14.  Total volume = 5.54272e-09.  Cell volumes OK.
    Mesh non-orthogonality Max: 60.3291 average: 14.111
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 2.49182 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

I have also introduced the constantAlphaContactAngle boundary condition at both walls (beacuse I want to study the behavior of air when changing this parameter), like this:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  6
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      alpha.air;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet1
    {
        type            fixedValue;
        value           uniform 1;
    }

    inlet2
    {
        type            fixedValue;
        value		uniform 0;
    }

    walls1
    {
        type            constantAlphaContactAngle;
        theta0          165;
        limit           gradient;
        value           uniform 0;
    }

    walls2
    {
        type            constantAlphaContactAngle;
        theta0          165;
        limit           gradient;
        value           uniform 0;
    }

    outlet
    {
        type            zeroGradient;
    }
}

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

But now that I see it I think that the contact angle condition at walls2 is useless since there is only water inside this channel. I'll change it for the next simulation.

Quote:

Originally Posted by crubio.abujas

Neither the residuals nor the courant number seems to have unreasonable values. By the way, you may find interesting to use PyFoam for plotting relevant information while solving.

Concerning the simulation times, you may consider using a parallel running. Add a decomposeParDict file to your system file. This file may have different configuration parameters but I recommend you to start using the scotch method, that takes care of splitting your domain for each processor. That should reduce the time of simulation.

system/decomposeParDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
  =========                 |
  \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox
   \\    /   O peration     | Website:  https://openfoam.org
    \\  /    A nd           | Version:  7
     \\/     M anipulation  |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      decomposeParDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //


// Change 4 to your machine number of cores.
numberOfSubdomains 4;

method          scotch;

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

For execute it in parallel just use:

Code:

# Split your domain in different regions, one for each process.
decomposePar

# Run in parallel. The -np value must be the same defined in the decomposeParDict
mpirun -np 4 interFoam -parallel

# Recompose the case to process the results
reconstructPar

I'm more used to MATLAB than to Python, but I'll give it a look.
The parallel running is great! The simulation time is really shortened. Thank you very much again

Quote:

Originally Posted by crubio.abujas

Do not despair, beginnings are always hard!

I'm trying as hard as a I can to stay calm hahaha
It is really hard.

If you could help me with the new mesh problem I would be appreciated.

Saludos,

Carlos.

crubio.abujas · March 16, 2020, 10:38

Refinie the mesh may increase significantly the computation time. I can help you further without more details. If you say that the computation takes almost 10h to fail... It would be nice to share the computation log instead of let me waste those 10h .

If you don't know how to log the output, you can try piping the output.

Code:

# Show the results on screen AND store them into "interFoam.log"
interFoam | tee interFoam.log

You may use this with mpirun for parallel or any other command you wish.

Concerning PyFoam, altough it has been certainly written in python is not required to know python to use. When you install it (using pip its quite easy to do so) you get access to a bunch of executable fies with the name pyFoam...
For example:

Code:

# Launch interFoam and show the results. Automatically generates a log file.
pyFoamPlotRunner interFoam

# Read a log file and plot the relevant information.
pyFoamPlotWatcher interFoam.log

In any case, I've started with Matlab and switched to python some years ago. From my perspective is totally worth it!

cmoreno98 · March 19, 2020, 09:15

Quote:

Originally Posted by crubio.abujas

Refinie the mesh may increase significantly the computation time. I can help you further without more details. If you say that the computation takes almost 10h to fail... It would be nice to share the computation log instead of let me waste those 10h .

If you don't know how to log the output, you can try piping the output.

Code:

# Show the results on screen AND store them into "interFoam.log"
interFoam | tee interFoam.log

You may use this with mpirun for parallel or any other command you wish.

Concerning PyFoam, altough it has been certainly written in python is not required to know python to use. When you install it (using pip its quite easy to do so) you get access to a bunch of executable fies with the name pyFoam...
For example:

Code:

# Launch interFoam and show the results. Automatically generates a log file.
pyFoamPlotRunner interFoam

# Read a log file and plot the relevant information.
pyFoamPlotWatcher interFoam.log

In any case, I've started with Matlab and switched to python some years ago. From my perspective is totally worth it!

Hi Carlos,

I tried a new mesh of 428k cells. You can download the case folder here (I also included the .log file of the simulation).

I used 2 different time steps: 2e-6 and 5e-6. I also installed PyFoam as you recommended.

Results for 5e-6:
- Execution time: 9h 25min
- Residuals:

- Courant:

Results for 2e-6:
- Execution time: 22h 22min
- Residuals:

- Courant:

Comparison using ParaView:

- Time = 0.0064:

- Time = 0.0072:

- Time = 0.008:

Is it better to use a smaller time step? The max Courant number is smaller, but the results at ParaView are very simillar... I don't know if it's worth to "lose" 13h decreasing the time step to 2 microseconds when I get no substantial improvement.

Another doubt that I have is that it seems that (is barely noticeable) the bubbles are being "sucked" at the outlet. There is a small bubble deformation, but I don't know why. The boundary conditions at the outlet are zeroGradient for alpha.air and U files and fixedValue (value 0) for p_rgh file.

Thank you very much,

Carlos.

crubio.abujas · March 19, 2020, 10:28

Hi, nice that you managed to solve it!

Concerning the mesh resolution, you have already performed some kind of mesh sensibility analisis. It is nice that the results are pretty simillar, it is a sign that you are going in the right track. What since is enough? That is something you have to determine. What is the purpuse of the simulation? Which error is acceptable?

I do not know how to help you further with the outlet issue. I am vaguely aware of wave reflection issie with some BC, but I never used them neither know if there is something implemented in OF.

Good luck with the model and your way with OF

cmoreno98 · March 20, 2020, 13:05

Quote:

Originally Posted by crubio.abujas

Hi, nice that you managed to solve it!

Concerning the mesh resolution, you have already performed some kind of mesh sensibility analisis. It is nice that the results are pretty simillar, it is a sign that you are going in the right track. What since is enough? That is something you have to determine. What is the purpuse of the simulation? Which error is acceptable?

I do not know how to help you further with the outlet issue. I am vaguely aware of wave reflection issie with some BC, but I never used them neither know if there is something implemented in OF.

Good luck with the model and your way with OF

The purpose of the simulation is to study the velocity, frequency and volume of the bubbles as a function of the inlet velocities (of air and water) and also the contact angle boundary condition.

Right now I would like to generate a plot like this:

It shows the fraction of air at two given surfaces (located at x=7 and x=8 mm in this case) with respect to time.
Do you know any way of generating two surfaces and extract the fraction of air at each time step? I think that I have to create some functions inside controlDict file but I don't know how to do it.

Is there a way to get this information using PyFoam? The volume of the bubbles for example. It would be extremely useful.

Thanks,

Carlos

najmehjafari · October 7, 2020, 09:52

Hi Carlos
I hope you are fine. I'm trying to run a simulation of a T-junction (cold water entering through one inlet and hot water through the other)
The mesh is done in Ansys and exported in .msh format. Then, the fluent3DMeshToFoam command is used to convert it from ASCII format to foam format.
but I don't understand why it doesn't work. It gets an error from me and I can not see it in Paraview. Can I take your Ansys file in this example?

crubio.abujas · October 8, 2020, 05:04

Quote:

Originally Posted by najmehjafari

Hi Carlos
I hope you are fine. I'm trying to run a simulation of a T-junction (cold water entering through one inlet and hot water through the other)
The mesh is done in Ansys and exported in .msh format. Then, the fluent3DMeshToFoam command is used to convert it from ASCII format to foam format.
but I don't understand why it doesn't work. It gets an error from me and I can not see it in Paraview. Can I take your Ansys file in this example?

Hello najmehjafari,

What kind of problems are you experiencing?

For exporting mesh from ANSYS to OpenFoam I think its needed to ensure that they are in ASCII format. By default they are in binary, so you just need to explore the exporting options of ANSYS Meshing to do so. Try that approach or share more information of the error you have so we can assest you better.

and2300 · October 10, 2020, 20:19

Hi Everyone

mumuaye · May 20, 2022, 16:45

Hello

I'm a new OpenFOAMer and I'm trying to run a similar question. The blockMesh has always been unsuccessful, can you give me the blockMesh file?

Thank you.

Berin Šeta · May 21, 2022, 14:31

Quote:

Originally Posted by mumuaye

Hello

I'm a new OpenFOAMer and I'm trying to run a similar question. The blockMesh has always been unsuccessful, can you give me the blockMesh file?

Thank you.

I think that mesh above was generated by Ansys Fluent. You could share your blockMeshDict and error you get, so someone could help you with that.

BR

kumar.kyutech · July 25, 2023, 01:10

Quote:

Originally Posted by crubio.abujas

Hi, nice that you managed to solve it!

Concerning the mesh resolution, you have already performed some kind of mesh sensibility analisis. It is nice that the results are pretty simillar, it is a sign that you are going in the right track. What since is enough? That is something you have to determine. What is the purpuse of the simulation? Which error is acceptable?

I do not know how to help you further with the outlet issue. I am vaguely aware of wave reflection issie with some BC, but I never used them neither know if there is something implemented in OF.

Good luck with the model and your way with OF

Hi Carlos,
Could you help me with a similar problem?
I am trying to simulate capillary-driven flow in an open microchannel. But unfortunately with all the boundary conditions, I am getting this result:
open.JPG
This is obviously not correct.

I am attaching my case files here: PLEASE CHECK

Could you please let me know what's wrong?
I am able to simulate closed channel but facing this problem in open channel.

March 5, 2020, 13:25	T-junction simulation using interFoam	#1
cmoreno98 New Member Carlos Join Date: Feb 2020 Location: Barcelona Posts: 19 Rep Power: 6	Hello everybody, I'm new to OpenFOAM and I'm trying to run a simulation of a T-junction (air entering through one inlet and water through the other) in microgravity conditions (g approximately 0). Since a picture is worth a thousand words, I show you the geometry and the mesh: The mesh is done in Ansys and exported in .msh format. Then, the fluent3DMeshToFoam command is used to convert it from ASCII format to foam format. The diameter of the channels is 1 mm, through the horizontal inlet (inlet1, walls1) enters air and through the vertical inlet (inlet2, walls2) enters water, both at 0.1 m/s. I can consider the two flows to be incompressible, so I use interFoam solver. I know that the results should be something like this: Air should advance through the horizontal pipe, meet the water at the junction and generate some bubbles. But when I run the simulation, air is not advancing through the channel and it's getting 'stucked' at the inlet like this: I attach the three directories "0" (alpha.air, p_rgh and U files), "constant" (g, transportProperties and turbulenceProperties files) and "system" (controlDict, fvSchemes and fvSolution files) in the following link because I don't know where the problem is: https://www.mediafire.com/file/60tv4...ction.rar/file Some parameters: inlet1 velocity: uniform (0.1 0 0); inlet2 velocity: uniform (0 -0.1 0) deltaT = 5e-6; endTime = 0.2; writeInterval = 0.0016 (total of 125 directories) How could I fix this problem? Thank you in advance, Carlos.

March 6, 2020, 07:04		#2
crubio.abujas Senior Member Carlos Rubio Abujas Join Date: Jan 2018 Location: Spain Posts: 127 Rep Power: 11	Hi Carlos, The problem is on the boundary definition of the pressure. You have to tell OpenFOAM to calculate the required pressure to provide a specific flux, not just set it to 0. Than can be done using fixedFluxPressure BC. You have to do it with both inlet1 and inlet2. 0/p_rgh: Code: inlet1 { type fixedFluxPressure; value uniform 0; } Hope it works! ybapat and cmoreno98 like this.

March 9, 2020, 04:19		#4
crubio.abujas Senior Member Carlos Rubio Abujas Join Date: Jan 2018 Location: Spain Posts: 127 Rep Power: 11	Hello again Carlos, It seems that you have some issues with the BC of the phases. On the file alpha.air you have fixed the value of the walls to always be 0 (water). I don't know if that is a design requirement but it seems that is blowing up your simulation. Try changing it to zeroGradient, that would make the simulation more stable. You can check your mesh using the command checkMesh, that will tell you if some mesh metrics is wrong, altough if you use an external mesher you may have that information from it. The mesh do not seem to be too distorted, although the cell size can be too big to capture the interphase properly or other flux phenomenon. If you want to play around with mesh size you can use refineMesh to create a more resolute version of the current mesh. Concerning the files you mentioned, the file decomposeParDict is for paralleling your simulation. It tells OF how to split your mesh in sections for each parallel process. The file setFieldDict is for imposing a set of values inside your domain. Neither of these file is strictly mandatory. Hope that helps you! cmoreno98 likes this.

March 11, 2020, 11:20		#6
crubio.abujas Senior Member Carlos Rubio Abujas Join Date: Jan 2018 Location: Spain Posts: 127 Rep Power: 11	Hi again! Its hard to tell... I've tried your set up and it worked for me. Maybe is related with he OF version, what version are you using? I've tried it with OF6. You can find the results and the case definition I've used here. I don't know it those are the expected results. The interface may be better resolved with a finer mesh, but that shouldn't make the entire simulation to crash. Neither the residuals nor the courant number seems to have unreasonable values. By the way, you may find interesting to use PyFoam for plotting relevant information while solving. Concerning the simulation times, you may consider using a parallel running. Add a decomposeParDict file to your system file. This file may have different configuration parameters but I recommend you to start using the scotch method, that takes care of splitting your domain for each processor. That should reduce the time of simulation. system/decomposeParDict: Code: /--------------------------------- C++ -----------------------------------\ ========= \| \\ / F ield \| OpenFOAM: The Open Source CFD Toolbox \\ / O peration \| Website: https://openfoam.org \\ / A nd \| Version: 7 \\/ M anipulation \| \---------------------------------------------------------------------------/ FoamFile { version 2.0; format ascii; class dictionary; location "system"; object decomposeParDict; } // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // // Change 4 to your machine number of cores. numberOfSubdomains 4; method scotch; // ************************************************************************* // For execute it in parallel just use: Code: # Split your domain in different regions, one for each process. decomposePar # Run in parallel. The -np value must be the same defined in the decomposeParDict mpirun -np 4 interFoam -parallel # Recompose the case to process the results reconstructPar Do not despair, beginnings are always hard! sersol and cmoreno98 like this.

March 16, 2020, 10:38		#8
crubio.abujas Senior Member Carlos Rubio Abujas Join Date: Jan 2018 Location: Spain Posts: 127 Rep Power: 11	Refinie the mesh may increase significantly the computation time. I can help you further without more details. If you say that the computation takes almost 10h to fail... It would be nice to share the computation log instead of let me waste those 10h . If you don't know how to log the output, you can try piping the output. Code: # Show the results on screen AND store them into "interFoam.log" interFoam \| tee interFoam.log You may use this with mpirun for parallel or any other command you wish. Concerning PyFoam, altough it has been certainly written in python is not required to know python to use. When you install it (using pip its quite easy to do so) you get access to a bunch of executable fies with the name pyFoam... For example: Code: # Launch interFoam and show the results. Automatically generates a log file. pyFoamPlotRunner interFoam # Read a log file and plot the relevant information. pyFoamPlotWatcher interFoam.log In any case, I've started with Matlab and switched to python some years ago. From my perspective is totally worth it! cmoreno98 likes this.

March 19, 2020, 10:28		#10
crubio.abujas Senior Member Carlos Rubio Abujas Join Date: Jan 2018 Location: Spain Posts: 127 Rep Power: 11	Hi, nice that you managed to solve it! Concerning the mesh resolution, you have already performed some kind of mesh sensibility analisis. It is nice that the results are pretty simillar, it is a sign that you are going in the right track. What since is enough? That is something you have to determine. What is the purpuse of the simulation? Which error is acceptable? I do not know how to help you further with the outlet issue. I am vaguely aware of wave reflection issie with some BC, but I never used them neither know if there is something implemented in OF. Good luck with the model and your way with OF cmoreno98 likes this.

October 7, 2020, 09:52		#12
najmehjafari New Member najmeh Join Date: Oct 2020 Posts: 1 Rep Power: 0	Hi Carlos I hope you are fine. I'm trying to run a simulation of a T-junction (cold water entering through one inlet and hot water through the other) The mesh is done in Ansys and exported in .msh format. Then, the fluent3DMeshToFoam command is used to convert it from ASCII format to foam format. but I don't understand why it doesn't work. It gets an error from me and I can not see it in Paraview. Can I take your Ansys file in this example?

October 10, 2020, 20:19		#14
and2300 New Member Andersson Romero Join Date: Oct 2020 Posts: 3 Rep Power: 6	Hi Everyone Last edited by and2300; October 22, 2020 at 22:59. Reason: Solved the problem.

May 20, 2022, 16:45	Can you help me	#15
mumuaye New Member mumu Join Date: May 2022 Posts: 3 Rep Power: 4	Hello I'm a new OpenFOAMer and I'm trying to run a similar question. The blockMesh has always been unsuccessful, can you give me the blockMesh file? Thank you.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Transient Simulation in CFX	ashtonJ	CFX	1	September 28, 2018 02:18
restarting paused transient simulation using reactingFoam	JMDag2004	OpenFOAM Running, Solving & CFD	1	August 10, 2015 11:15
Strange error in multithread simulation with interFoam	davidmd	OpenFOAM Running, Solving & CFD	3	December 13, 2014 21:45
setting up a simulation with multiple interactions	phandy	OpenFOAM Running, Solving & CFD	1	October 6, 2014 04:16
Discrete event simulation vs. fixed time (discrete time simulation)	jenjon	FLUENT	0	March 10, 2013 07:58