CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

PIMPLE at twoLiquidMixingFoam - p_rgh divergence - slow solving

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree3Likes
  • 1 Post By gridley2
  • 1 Post By Ramona
  • 1 Post By pconen

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   July 26, 2019, 02:49
Unhappy PIMPLE at twoLiquidMixingFoam - p_rgh divergence - slow solving
  #1
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Greetings to all!

I am still new to OpenFOAM and actually work on my thesis. I am facing a problem with twoLiquidMixingFoam by using PIMPLE. Ich wanted to try out PIMPLE because I'd like to speed up my simulation an get a higher stability.
But at the moment I can't generate a fast an stable PIMPLE solution. I think the problem is the p_rgh which does not converge. So the residualControll can't work an the advantage from the PIMPLE algorythm is not given anymore.
So here my concret questions.
1) What can I do when my p_rgh is not sinking with PIMPLE? PISO is working fine, but also slow!
2) How can I speed up the PIMPLE in general?
3) Is there an easy Way to get a higher deltaT than 1E-06?

I would be very happy if there is someone who can help me with this.

Here are my Options:
fvSolution
Code:
solvers
{
    "alpha.*"
    {
        nAlphaCorr          1;
        nAlphaSubCycles     1;
        cAlpha              1;

        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-4;
        relTol          0;
        nSweeps         1;
    }

//If not using GAMG for pressure choose PCG Solver. For faster Solving tol:1e-4 and relTol 0.05.
       p_rgh
    {
        solver            PCG;
        preconditioner        DIC;
        tolerance        1e-3;        //StartVals:1e-5,StartVals:1e-6
        relTol            0.001;        //StartVals:0.01,StartVals:0.001
        minIter            3;
        maxIter            100;
    }

    p_rghFinal
    {
        solver            PCG;
        preconditioner        DIC;
        tolerance        1e-4;        //StartVals:1e-5,StartVals:1e-6
        relTol            0.000;        //StartVals:0.01,StartVals:0.001
        minIter            5;
        //maxIter            100;
    }

//For the Velocity - coupled (increasing stability).
    U
    {
        type            coupled;
        solver            PBiCCCG;
        preconditioner        DILU;
        tolerance        (1e-3 1e-3 1e-3);
        relTol            (0.1 0.1 0.1);
        minIter            3;
        maxIter            100;
    }

    UFinal
    {        
        type            coupled;
        solver            PBiCCCG;
        preconditioner        DILU;
        tolerance        (1e-4 1e-4 1e-4);
        relTol            (0 0 0);
        minIter            3;
        maxIter            100;
    }    

    "(k|omega)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-03;
        relTol          0.1;
    }

    "(k|omega)Final"
    {
        $U;
        tolerance       1e-04;
        relTol          0.1;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 3;
    nCorrectors          3;
    nOuterCorrectors    50;
    turbOnFinalIterOnly false;
 
    residualControl
{
    U               5e-03;
    p_rgh              5e-03;
    k               5e-03;
    omega           5e-03;
    alpha.adblue    5e-03;
    ".*"            5e-03;
}
}

relaxationFactors
{
    fields
    {
        p      0;
        pFinal   1;
    }
    equations
    {
        "(U|k|epsilon)"     0.7;
        "(U|k|epsilon)Final"   1;
    }
}
fvSchemes
Code:
ddtSchemes
{
    default         Euler;  
}

gradSchemes
{
    default         cellLimited Gauss linear 0.5; 
    grad(U)         cellLimited Gauss linear 0.5;

}

divSchemes
{
    default         none;
    div(rhoPhi,U)   Gauss upwind;
    div(phi,alpha)  Gauss vanLeer;    
    div(phi,k)      Gauss upwind;  
    div(phi,omega)  Gauss upwind;
    div(phi,e)        Gauss upwind; 
    div((nuEff*dev2(T(grad(U))))) Gauss linear; 
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

/*
divSchemes
{
    default         none;
    div(rhoPhi,U)   Gauss linearUpwind grad(U);
    div(phi,alpha)  Gauss vanLeer;
    div(rhoPhi,U)  Gauss upwind;     //linear;
    div(phi,alpha)  Gauss vanLeer;
    div(phi,k)      Gauss upwind;     //limitedLinear 1;
    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}*/

laplacianSchemes
{
    default         Gauss linear limited 0;    //Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         limited 0; 
}

wallDist
{
    method    meshWave;
}
controlDict
Code:
application     twoLiquidMixingFoam;

startFrom       latestTime;

startTime       0;

stopAt          endTime;    //endTime; writeNow;

endTime         20;

deltaT          0.0000000005;

writeControl    adjustableRunTime;

writeInterval   0.00005;

purgeWrite      0;

writeFormat     binary;

writePrecision  7;

writeCompression off;

timeFormat      general;

timePrecision   6;

runTimeModifiable yes;

adjustTimeStep  on;

maxCo           0.5;
maxAlphaCo      0.5;
maxDeltaT       1;

functions
{
    #includeFunc residuals
    #includeFunc pressureDifferencePatch
}
Here are the residuals





If you need more information to help me let me know it.
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 1, 2019, 20:20
Default
  #2
New Member
 
Gavin Ridley
Join Date: Jan 2019
Location: Tennessee, USA
Posts: 25
Rep Power: 4
gridley2 is on a distinguished road
Hi,


Your relaxation factor for p appears to be zero. Do you know why under-relaxation is desired? You should set that factor to be around 0.2-0.5 or 0.5-1 depending on whether you use vanilla PIMPLE or consistent PIMPLE respectively.



Could you try changing that relaxation factor to say, 0.2?


By the way, a rule of thumb to get decent convergence is relax_U+relax_p=1. I'm not sure why mathematically this works well, but it seems to.
gridley2 is offline   Reply With Quote

Old   August 5, 2019, 09:10
Default
  #3
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Gavin,

thank you for reply to my question.
I understood underrelaxtion as a function of stability and calculation speed. So I used 0 for a highly stable calculation.
I also used 0.1/0.3 and 1 as underrelaxtionfactor. With 1 the speed was high an p decreased. But p decreased very very slow an only up to 0.98. So this lead to no win in this case.

But I try again and save your thumb rule in my head.
Thank you really much. I subscribe back in some days.
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 6, 2019, 01:26
Default
  #4
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Gavin,

I let the calculation run over night. A URF = 0.2 doesnt change my Problem of slow and unstable calculation.
Code:
PIMPLE: Iteration 50
DILUPBiCG:  Solving for Ux, Initial residual = 0.001560208, Final residual = 1.034981e-13, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.001074642, Final residual = 9.620375e-14, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.001472009, Final residual = 4.359329e-14, No Iterations 2
DICPCG:  Solving for p_rgh, Initial residual = 0.2390144, Final residual = 0.01121177, No Iterations 175
DICPCG:  Solving for p_rgh, Initial residual = 0.01796031, Final residual = 0.0008353669, No Iterations 9
DICPCG:  Solving for p_rgh, Initial residual = 0.003443909, Final residual = 0.0009118244, No Iterations 1
DICPCG:  Solving for p_rgh, Initial residual = 0.001411461, Final residual = 0.0007466737, No Iterations 1
time step continuity errors : sum local = 2.034207e-10, global = -8.159711e-12, cumulative = -1.751579e-06
DICPCG:  Solving for p_rgh, Initial residual = 0.001202807, Final residual = 0.0006922544, No Iterations 1
DICPCG:  Solving for p_rgh, Initial residual = 0.0008900349, Final residual = 0.0008900349, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 0.0008900349, Final residual = 0.0008900349, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 0.0008900349, Final residual = 0.0008900349, No Iterations 0
time step continuity errors : sum local = 2.425377e-10, global = -1.069591e-11, cumulative = -1.75159e-06
DICPCG:  Solving for p_rgh, Initial residual = 0.0008933383, Final residual = 0.0008933383, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 0.0008933383, Final residual = 0.0008933383, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 0.0008933383, Final residual = 0.0008933383, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 0.0008933383, Final residual = 9.720371e-05, No Iterations 70
time step continuity errors : sum local = 2.648834e-11, global = -6.587787e-12, cumulative = -1.751597e-06
DILUPBiCG:  Solving for omega, Initial residual = 2.603568e-07, Final residual = 2.998042e-10, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 2.077727e-08, Final residual = 5.145305e-12, No Iterations 1
ExecutionTime = 48113.92 s  ClockTime = 50635 s

fieldValueDelta pressureDifferencePatch write:
    subtract(p) = 9.150395e+33

Courant Number mean: 3.484067e-07 max: 1.177855
Interface Courant Number mean: 0 max: 0
deltaT = 3.205731e-22
Time = 7.30141e-05
The residual control also doesn't do what I want
Code:
    residualControl
{
    U   			5e-06;
    p_rgh  			5e-03;
    k   			5e-06;
    omega   		5e-06;
    alpha.adblue	5e-06;
    ".*"			5e-06;
}
I am happy about other hints.
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 6, 2019, 12:14
Default
  #5
New Member
 
Gavin Ridley
Join Date: Jan 2019
Location: Tennessee, USA
Posts: 25
Rep Power: 4
gridley2 is on a distinguished road
OK, I see your problem. It's OK to have nonlinear tolerances set around 1e-3 (what's in the convergence control part of fvSolution), but your linear tolerances have to be way below that. Look at your p_rgh linear solve section (the part where you can select PCG or GAMG). Your tolerance is 1e-3. This is way too high. This needs to be 1e-8, or even 1e-10 if you want to get linear nonlinear residual around 1e-7. In my experience, depending on the mesh, the linear residuals should be about three orders of magnitude smaller than the nonlinear residuals.


By the way, you may want to post the results of checkMesh, since that can SERIOUSLY impact solution convergence. (Especially if dropping your linear convergence criterion still doesn't help)
gridley2 is offline   Reply With Quote

Old   August 16, 2019, 08:18
Default
  #6
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Gavin,

sorry for my late reply, but thanks for your answer!
I tought I close calculations with PIMPLE, but I would like to try out your ideas.
So here are my new fvSolutions:
Code:
solvers
{
    "alpha.*"
    {
        nAlphaCorr          1;
        nAlphaSubCycles     1;
        cAlpha              1;

        solver          smoothSolver;
        smoother        GaussSeidel;
        tolerance       1e-8;
        relTol          0;
        nSweeps         1;
    }

//If not using GAMG for pressure choose PCG Solver. For faster Solving tol:1e-4 and relTol 0.05.
       p_rgh
    {
        solver            PCG;
        preconditioner        DIC;
        tolerance        1e-8;        //StartVals:1e-5,StartVals:1e-6
        relTol            0.001;        //StartVals:0.01,StartVals:0.001
    }

    p_rghFinal
    {
        solver            PCG;
        preconditioner        DIC;
        tolerance        1e-8;        //StartVals:1e-5,StartVals:1e-6
        relTol            0.000;        //StartVals:0.01,StartVals:0.001
    }

//For the Velocity - coupled (increasing stability).
    U
    {
        type            coupled;
        solver            PBiCCCG;
        preconditioner        DILU;
        tolerance        (1e-8 1e-8 1e-8);
        relTol            (0.1 0.1 0.1);
    }

    UFinal
    {        
        type            coupled;
        solver            PBiCCCG;
        preconditioner        DILU;
        tolerance        (1e-8 1e-8 1e-8);
        relTol            (0 0 0);
    }    

    "(k|omega)"
    {
        solver          smoothSolver;
        smoother        symGaussSeidel;
        tolerance       1e-08;
        relTol          0.1;
    }

    "(k|omega)Final"
    {
        $U;
        tolerance       1e-08;
        relTol          0.1;
    }
}

PIMPLE
{
    nNonOrthogonalCorrectors 1;
    nCorrectors          3;
    nOuterCorrectors    20;
    turbOnFinalIterOnly false;
 
    residualControl
{
    U               5e-03;
    p_rgh              5e-03;
    k               5e-03;
    omega           5e-03;
    alpha.adblue    5e-03;
    ".*"            5e-03;
}
}

relaxationFactors
{
    fields
    {
        p      0.2;
        pFinal   1;
    }
    equations
    {
        "(U|k|epsilon)"     0.2;
        "(U|k|epsilon)Final"   1;
    }
}
In my checkMesh it says:
Code:
Mesh stats
    points:           1720306
    faces:            4913997
    internal faces:   4744352
    cells:            1604851
    faces per cell:   6.018222
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     1501520
    prisms:        45802
    wedges:        0
    pyramids:      0
    tet wedges:    216
    tetrahedra:    0
    polyhedra:     57313
    Breakdown of polyhedra by number of faces:
        faces   number of cells
            4   13322
            5   11049
            6   11441
            7   13
            8   132
            9   10444
           10   3
           11   101
           12   6080
           13   4
           14   44
           15   3991
           17   3
           18   686

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
                    fans    71745    86100  ok (non-closed singly connected)
            inlet_adblue       26       39  ok (non-closed singly connected)
            inlet_exhgas     4116     4347  ok (non-closed singly connected)
                  outlet     4277     4573  ok (non-closed singly connected)
                   sheet     3315     4329  ok (non-closed singly connected)
                    wall    86166    90014  ok (non-closed singly connected)

Checking geometry...
    Overall domain bounding box (-0.15985 -0.15985 -1.687) (0.15985 0.15985 0.5)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (2.59768e-16 -2.335864e-16 1.8714e-16) OK.
    Max cell openness = 3.274699e-16 OK.
    Max aspect ratio = 9.2792 OK.
    Minimum face area = 9.54776e-08. Maximum face area = 3.987172e-05.  Face area magnitudes OK.
    Min volume = 1.279944e-09. Max volume = 1.729588e-07.  Total volume = 0.1752509.  Cell volumes OK.
    Mesh non-orthogonality Max: 58.76045 average: 6.463263
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 3.728606 OK.
    Coupled point location match (average 0) OK.

Mesh OK.
I hope I unterstood you in a correct way. When I have any results I will give you an update.
Many thanks!
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 16, 2019, 08:50
Default
  #7
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Gavin,

as I can see the residualControl still does not work.
Here is my log of the solver:
Code:
ExecutionTime = 2664.28 s  ClockTime = 2706 s

...

PIMPLE: Iteration 19
DILUPBiCCCG:  Solving for Ux, Initial residual = 4.711859e-05, Final residual = 3.277177e-07, No Iterations (1 1 1)
DILUPBiCCCG:  Solving for Uy, Initial residual = 4.83186e-05, Final residual = 3.355973e-07, No Iterations (1 1 1)
DILUPBiCCCG:  Solving for Uz, Initial residual = 0.0001946199, Final residual = 1.360958e-06, No Iterations (1 1 1)
DICPCG:  Solving for p_rgh, Initial residual = 5.80858e-05, Final residual = 9.92059e-08, No Iterations 343
DICPCG:  Solving for p_rgh, Initial residual = 8.136671e-06, Final residual = 9.744144e-08, No Iterations 8
time step continuity errors : sum local = 4.032735e-11, global = -8.69936e-13, cumulative = 9.328705e-07
DICPCG:  Solving for p_rgh, Initial residual = 1.862189e-05, Final residual = 9.564784e-08, No Iterations 337
DICPCG:  Solving for p_rgh, Initial residual = 5.483464e-06, Final residual = 8.795988e-08, No Iterations 7
time step continuity errors : sum local = 3.640707e-11, global = 9.436154e-13, cumulative = 9.328715e-07
DICPCG:  Solving for p_rgh, Initial residual = 2.539553e-06, Final residual = 8.357301e-08, No Iterations 5
DICPCG:  Solving for p_rgh, Initial residual = 1.733912e-06, Final residual = 8.640904e-08, No Iterations 3
time step continuity errors : sum local = 3.576518e-11, global = 1.191871e-12, cumulative = 9.328727e-07
smoothSolver:  Solving for omega, Initial residual = 5.109694e-07, Final residual = 1.162782e-09, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 2.773506e-05, Final residual = 4.273729e-09, No Iterations 1
PIMPLE: Iteration 20
DILUPBiCCCG:  Solving for Ux, Initial residual = 0.0002354442, Final residual = 1.899741e-12, No Iterations (4 4 4)
DILUPBiCCCG:  Solving for Uy, Initial residual = 0.0002425355, Final residual = 1.873183e-12, No Iterations (4 4 4)
DILUPBiCCCG:  Solving for Uz, Initial residual = 0.0008617877, Final residual = 5.906528e-12, No Iterations (4 4 4)
DICPCG:  Solving for p_rgh, Initial residual = 0.153554, Final residual = 0.0001499837, No Iterations 350
DICPCG:  Solving for p_rgh, Initial residual = 0.07839407, Final residual = 7.580352e-05, No Iterations 333
time step continuity errors : sum local = 1.608803e-08, global = 1.087189e-10, cumulative = 9.329814e-07
DICPCG:  Solving for p_rgh, Initial residual = 0.04337104, Final residual = 4.208997e-05, No Iterations 348
DICPCG:  Solving for p_rgh, Initial residual = 0.007981723, Final residual = 7.981384e-06, No Iterations 342
time step continuity errors : sum local = 1.83341e-09, global = 1.948213e-13, cumulative = 9.329816e-07
DICPCG:  Solving for p_rgh, Initial residual = 0.004048247, Final residual = 3.857835e-06, No Iterations 350
DICPCG:  Solving for p_rgh, Initial residual = 0.001300558, Final residual = 9.93526e-08, No Iterations 371
time step continuity errors : sum local = 2.305758e-11, global = 8.214406e-14, cumulative = 9.329817e-07
DILUPBiCCCG:  Solving for omega, Initial residual = 5.757286e-05, Final residual = 2.727271e-07, No Iterations 1
DILUPBiCCCG:  Solving for k, Initial residual = 0.0004608179, Final residual = 1.510417e-06, No Iterations 1
ExecutionTime = 2664.28 s  ClockTime = 2706 s
Maybe you have another idea?

By the way I would like to ask what you mean with linaer and non-linear.
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 16, 2019, 08:59
Default geometry
  #8
New Member
 
ramona
Join Date: Apr 2019
Posts: 4
Rep Power: 4
Ramona is on a distinguished road
Hello

could you plz somebody help me how can I choose inlet and outlet for geometry in openfoam?
Ramona is offline   Reply With Quote

Old   August 16, 2019, 09:03
Default openfoam
  #9
New Member
 
ramona
Join Date: Apr 2019
Posts: 4
Rep Power: 4
Ramona is on a distinguished road
hello every one

could you please tell me which class is good for openfoam I am new in this field and I want to learn openfoam and get certificate

best regards
____________
Ramona
Ramona is offline   Reply With Quote

Old   August 16, 2019, 09:08
Default
  #10
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Ramona,

I think this Thread is not the best place for this question.
But I allready answered to your inlet/outlet question.
The secound question I do not understand. What do you mean with class?
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 16, 2019, 11:03
Default
  #11
New Member
 
Gavin Ridley
Join Date: Jan 2019
Location: Tennessee, USA
Posts: 25
Rep Power: 4
gridley2 is on a distinguished road
As for linear and non-linear, maybe that isnít the exactly correct term to use. Inner and outer pressure-velocity coupling iterations would be more correct to say, since the pressure-velocity coupled problem is a purely linear one. If you want more details on that coupling, I recommend checking out either Ferziger and Perricís book or alternatively Patankar and Spaldingís if you want something more mathematically mild.

So, a few things. In your relaxation terms, you have both field and equation relaxation. Your equation relaxation can usually be 1, since this is usually not the unstable part of the problem. Field relaxation is what you need. You should see a pretty solid speed-up when you remove equation relaxation. Of course, if you find that this makes your solve crash, you should add back some equation relaxation. Stabilization of the linear solve can usually be done with modest under-relaxation factors of .7 or .9, usually not low like .2.

I see that youíre using the the coupled velocity solver. Iíve not messed with that; it does the pressure-velocity coupling in a wholly different way from the usual CFD solve. This may have to do with why stuff here is working different than what Iím used to (segregated p/U coupling).

Another possibility could be your nonorthogonal terms making an issue. Does your fvSchemes use a corrected laplacian scheme? If so, you may also want to consider under-relaxing the nonorthogonal correction term, which is done in the fvSchemes file. You may also want to have two nonorthogonal corrections rather than just one, given that your mesh nonorthogonality is around 50.
pconen likes this.
gridley2 is offline   Reply With Quote

Old   August 16, 2019, 11:10
Default thank you
  #12
New Member
 
ramona
Join Date: Apr 2019
Posts: 4
Rep Power: 4
Ramona is on a distinguished road
Dear Pconen

I am very new with openfoam I used to use sim scale and for openfoam I want to learn step by step and I am looking for good source for start to learn openfoam

thank you I saw your answered for inlet and outlet thanks
pconen likes this.
Ramona is offline   Reply With Quote

Old   August 19, 2019, 03:15
Default
  #13
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Gavin,

thank you very much!
At the moment I have hard work with my thesis. But I will try your ideas as soon as possible.
Thanks!
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Old   August 19, 2019, 03:16
Default
  #14
Member
 
Philipp Conen
Join Date: Apr 2019
Location: GER, NRW
Posts: 35
Blog Entries: 2
Rep Power: 4
pconen is on a distinguished road
Dear Ramona,

your welcome.
Ramona likes this.
__________________
Greetings

Philipp Conen
pconen is offline   Reply With Quote

Reply

Tags
divergence, pimple, p_rgh, slow, twoliquidmixingfoam

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
chtMultiRegionSimpleFoam: maximum number of iterations excedeed. Nkl OpenFOAM Running, Solving & CFD 19 October 10, 2019 02:42
decompose dependent solution arionfard OpenFOAM 3 December 10, 2018 09:36
Adapt Fluent Mesh to weirOverflow tutorial WaterHammer1985 OpenFOAM Running, Solving & CFD 2 July 5, 2018 02:37
Segmentation fault when using reactingFOAM for Fluids Tommy Floessner OpenFOAM Running, Solving & CFD 4 April 22, 2018 12:30
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20


All times are GMT -4. The time now is 00:37.