PIMPLE at twoLiquidMixingFoam - p_rgh divergence - slow solving

pconen · July 26, 2019, 02:49

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.

gridley2 · August 1, 2019, 20:20

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.

pconen · August 5, 2019, 09:10

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.

pconen · August 6, 2019, 01:26

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.

gridley2 · August 6, 2019, 12:14

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)

pconen · August 16, 2019, 08:18

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!

pconen · August 16, 2019, 08:50

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.

Ramona · August 16, 2019, 08:59

Hello

could you plz somebody help me how can I choose inlet and outlet for geometry in openfoam?

Ramona · August 16, 2019, 09:03

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

pconen · August 16, 2019, 09:08

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?

gridley2 · August 16, 2019, 11:03

As for linear and non-linear, maybe that isn’t 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 Perric’s book or alternatively Patankar and Spalding’s 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 you’re using the the coupled velocity solver. I’ve 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 I’m 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.

Ramona · August 16, 2019, 11:10

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 · August 19, 2019, 03:15

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!

pconen · August 19, 2019, 03:16

Dear Ramona,

your welcome.

August 5, 2019, 09:10		#3
pconen Member Philipp Conen Join Date: Apr 2019 Location: GER, NRW Posts: 35 Blog Entries: 2 Rep Power: 7	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

August 16, 2019, 08:59	geometry	#8
Ramona New Member ramona Join Date: Apr 2019 Posts: 4 Rep Power: 7	Hello could you plz somebody help me how can I choose inlet and outlet for geometry in openfoam?

August 16, 2019, 09:03	openfoam	#9
Ramona New Member ramona Join Date: Apr 2019 Posts: 4 Rep Power: 7	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

August 16, 2019, 09:08		#10
pconen Member Philipp Conen Join Date: Apr 2019 Location: GER, NRW Posts: 35 Blog Entries: 2 Rep Power: 7	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

August 16, 2019, 11:03		#11
gridley2 New Member Gavin Ridley Join Date: Jan 2019 Location: Tennessee, USA Posts: 25 Rep Power: 7	As for linear and non-linear, maybe that isn’t 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 Perric’s book or alternatively Patankar and Spalding’s 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 you’re using the the coupled velocity solver. I’ve 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 I’m 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.

August 1, 2019, 20:20		#2
gridley2 New Member Gavin Ridley Join Date: Jan 2019 Location: Tennessee, USA Posts: 25 Rep Power: 7	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.

August 6, 2019, 12:14		#5
gridley2 New Member Gavin Ridley Join Date: Jan 2019 Location: Tennessee, USA Posts: 25 Rep Power: 7	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)

August 16, 2019, 11:10	thank you	#12
Ramona New Member ramona Join Date: Apr 2019 Posts: 4 Rep Power: 7	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.

August 19, 2019, 03:15		#13
pconen Member Philipp Conen Join Date: Apr 2019 Location: GER, NRW Posts: 35 Blog Entries: 2 Rep Power: 7	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

August 19, 2019, 03:16		#14
pconen Member Philipp Conen Join Date: Apr 2019 Location: GER, NRW Posts: 35 Blog Entries: 2 Rep Power: 7	Dear Ramona, your welcome. Ramona likes this. __________________ Greetings Philipp Conen

Thread Tools	Search this Thread
Show Printable Version Email this Page	Search this Thread: Advanced Search
Display Modes
Linear Mode Switch to Hybrid Mode Switch to Threaded Mode

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