rhoSimplecFoam Mach0.8 no pressure values

CFDnewbie147 · October 31, 2013, 10:56

Hello together,

I'm trying to simulate a kind of rocket with rhoSimplecFoam and the following start-up conditions(it's laminar without any turbulence modell and a coarse mesh built with snappyhexmesh, the values are for standard atmosphere in 0km):

Code:

p
dimensions      [1 -1 -2 0 0 0 0];
internalField   uniform 101325;
boundaryField
{
    flange_CATIA
    {
        type            zeroGradient;
    }
 
    inlet
    {
        type            fixedValue;
  value  uniform 101325;
    }
 
    outlet
    {
        type            zeroGradient;
    }
 
 upperWall
 {
 
  type   zeroGradient;
 }
 
 lowerWall
 {
  type   zeroGradient;
 }
 
 frontAndBack
    {
        type            zeroGradient;
 }
}

Code:

T
dimensions      [0 0 0 1 0 0 0];
internalField   uniform 288.16;
boundaryField
{
    flange_CATIA
    {
        type            fixedValue;
        value           uniform 288.16;
    }
    inlet
    {
        type            fixedValue;
        value           uniform 288.16;
    }
    outlet
    {
        type            zeroGradient;
    }
 
 upperWall
 {
  type   zeroGradient;
 }
 
 lowerWall
 {
  type   zeroGradient;
 }
 
 frontAndBack
    {
        type            zeroGradient;
 }
}

Code:

U
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (272.215 0 0);
boundaryField
{
    flange_CATIA
    {
        type            fixedValue;
  value  uniform (0 0 0);
    }
 
    inlet
    {
        type            fixedValue;
  value  uniform (272.215 0 0);
    }
 
    outlet
    {
        type            zeroGradient;
    }
 
 upperWall
 {
  type  freestream;
 freestreamValue uniform (272.215 0 0);
 phi  phi;
 }
 
 lowerWall
 {
  type  freestream;
 freestreamValue uniform (272.215 0 0);
 phi  phi;
 }
 
 frontAndBack
    {
        type  freestream;
 freestreamValue uniform (272.215 0 0);
 phi  phi;
 }
}

for fvSolution I have:

Code:

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-06;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      2;
        nPostSweeps     2;
        nFinestSweeps   2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }
    "(U|e|k|epsilon)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        nFinestSweeps   2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }
}
SIMPLE
{
    nNonOrthogonalCorrectors 3;
    rhoMin          rhoMin [1 -3 0 0 0] 0.1;
    rhoMax          rhoMax [1 -3 0 0 0] 1.7;
    transonic       yes;
    residualControl
    {
        p               1e-3;
        U               1e-4;
        e               1e-3;
        // possibly check turbulence fields
        "(k|epsilon|omega)" 1e-3;
    }
}
 
relaxationFactors
{
    fields
    {
        p               0.1;
        rho             0.2;
    }
    equations
    {
        p               0.1;
        U               0.1;
        e               0.1;
        k               0.1;
        epsilon         0.1;
    }
}

and for fvSchemes:

Code:

ddtSchemes
{
    default             steadyState;
}
gradSchemes
{
    default             Gauss linear;
}
divSchemes
{
    default             none;
    div(phi,U)          bounded Gauss upwind;
    div((muEff*dev2(T(grad(U)))))      Gauss linear;
    div(phi,e)          bounded Gauss upwind;
    div(phi,epsilon)    bounded Gauss upwind;
    div(phi,k)          bounded Gauss upwind;
    div(phid,p)         bounded Gauss upwind;
    div(phi,Ekp)        bounded Gauss upwind;
    div((phi|interpolate(rho)),p)  Gauss upwind;
}
laplacianSchemes
{
    default         Gauss linear corrected;
}
interpolationSchemes
{
    default         linear;
}
snGradSchemes
{
    default         corrected;
}
fluxRequired
{
    default         no;
    p;
    pCorr;
}

Ouput looks like:

Code:

GAMG:  Solving for Ux, Initial residual = 3.5620403e-05, Final residual = 1.145979e-07, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.0016973702, Final residual = 6.0027881e-06, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.001536366, Final residual = 4.8191816e-06, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.00045292245, Final residual = 1.9744077e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.14242369, Final residual = 0.032751031, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.090691613, Final residual = 0.030714924, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.052047365, Final residual = 0.028755893, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.038641847, Final residual = 0.027810481, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.033185164, Final residual = 0.027251068, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.030303116, Final residual = 0.026959392, No Iterations 1000
time step continuity errors : sum local = 0.00026140328, global = -7.6367694e-16, cumulative = -1.1835275e-13
rho max/min : 1.5 1.1663043
ExecutionTime = 16521.99 s  ClockTime = 16533 s

if i reconstructPar and foamToVTK the last writen timestep and look at it in paraview i see a "normal" velocity distribution but when i look at pressure p there is all over the slice the standard pressure of 101325Pa which i dictate in the startup conditions. even if u look at the value range of p there's only this entry!

Can anyone help me and tell me, where is the problem or failure?
best regards,
cfdnewbie147

CFDnewbie147 · November 5, 2013, 05:33

That everybody knows what i mean:
When i look at my written solution file U i see:

Code:

dimensions [0 1 -1 0 0 0 0];
internalField nonuniform List<vector> 
31816
(
(272.215 5.221145e-12 -1.7181269e-12)
(272.215 5.7207594e-12 -1.4172429e-12)
(272.215 -3.0062849e-13 -8.1789221e-14)
(272.215 8.1848292e-14 -8.1992441e-14)
(272.215 5.7952553e-12 -1.5504855e-12)
(272.215 9.2944646e-13 4.9986554e-12)
(272.215 3.4030351e-13 -8.3896778e-13)
(272.215 -1.2806153e-12 1.5817917e-13)
(272.215 5.5325204e-13 3.0713544e-13)
(272.215 7.3076711e-14 -1.2613566e-12)
(272.215 -1.545563e-12 -9.7705242e-14)
(272.215 -2.0237993e-12 6.0391271e-12)
(272.215 1.3645437e-12 1.1097317e-12)
(272.215 1.1176496e-12 4.6202634e-12)
(272.215 5.9042102e-12 -1.8083531e-12)
(272.215 1.8823713e-12 -1.7038351e-12)
(272.215 -1.3134718e-12 6.0098351e-12)
...

That shows me, that the simulation runs because these are the calculated values...

But when I look at the written p file:

Code:

dimensions [1 -1 -2 0 0 0 0];
internalField nonuniform List<scalar> 
31816
(
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
101325
....

There's all over the internalfieldvalue without any discrepancy. Can anybody help me please?

Best regards,
CFDNewbie147

henrik · November 5, 2013, 05:55

Hi,

your pressure equation does not converge - 1000 Iterations!

Under normal conditions, you should not fix p AND U anywhere. Same is true for zeroGradient.

Try setting the pressure at the outlet and zeroGradient it at the inlet.

Henrik

CFDnewbie147 · November 5, 2013, 06:15

I changed as you said to:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
dimensions      [1 -1 -2 0 0 0 0];
internalField   uniform 101325;
boundaryField
{
    flange_CATIA
    {
        type            zeroGradient;
    }
 
    outlet
    {
        type            fixedValue;
 value  uniform 101325;
    }
 
    inlet
    {
        type            zeroGradient;
    }
 
 upperWall
 {
 
  type   zeroGradient;
 }
 
 lowerWall
 {
  type   zeroGradient;
 }
 
 frontAndBack
    {
        type            zeroGradient;
 }
}

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

and the others remain the same as before.
But it doesn't work either.
Output is:

Code:

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.2.1-57f3c3617a2d
Exec   : rhoSimplecFoam -parallel
Date   : Nov 05 2013
Time   : 11:07:51
Host   : "magnus08"
PID    : 4128
Case   : /z/pro/cfdtmp03/zachjoer/OpenFOAM/BA/HFK_SHM_gröber/Mach0080_turbulent
nProcs : 64
Slaves : 
63
(
"magnus08.4129"
"magnus08.4130"
"magnus08.4131"
"magnus08.4132"
"magnus08.4133"
"magnus08.4134"
"magnus08.4135"
"magnus07.21150"
"magnus07.21151"
"magnus07.21152"
"magnus07.21153"
"magnus07.21154"
"magnus07.21155"
"magnus07.21156"
"magnus07.21157"
"magnus06.22483"
"magnus06.22484"
"magnus06.22485"
"magnus06.22486"
"magnus06.22487"
"magnus06.22488"
"magnus06.22489"
"magnus06.22490"
"magnus05.23351"
"magnus05.23352"
"magnus05.23353"
"magnus05.23354"
"magnus05.23355"
"magnus05.23356"
"magnus05.23357"
"magnus05.23358"
"magnus04.22806"
"magnus04.22807"
"magnus04.22808"
"magnus04.22809"
"magnus04.22810"
"magnus04.22811"
"magnus04.22812"
"magnus04.22813"
"magnus03.23177"
"magnus03.23178"
"magnus03.23179"
"magnus03.23180"
"magnus03.23181"
"magnus03.23182"
"magnus03.23183"
"magnus03.23184"
"magnus02.23682"
"magnus02.23683"
"magnus02.23684"
"magnus02.23685"
"magnus02.23686"
"magnus02.23687"
"magnus02.23688"
"magnus02.23689"
"magnus01.23113"
"magnus01.23114"
"magnus01.23115"
"magnus01.23116"
"magnus01.23117"
"magnus01.23118"
"magnus01.23119"
"magnus01.23120"
)
Pstream initialized with:
    floatTransfer      : 0
    nProcsSimpleSum    : 0
    commsType          : nonBlocking
    polling iterations : 0
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time
Create mesh for time = 0

SIMPLE: convergence criteria
    field p  tolerance 0.001
    field U  tolerance 0.0001
    field e  tolerance 0.001
    field "(k|epsilon|omega)"  tolerance 0.001
Reading thermophysical properties
Selecting thermodynamics package 
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       sutherland;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleInternalEnergy;
}
Reading field U
Reading/calculating face flux field phi
Creating turbulence model
Selecting RAS turbulence model laminar
No finite volume options present

Starting time loop
Time = 0.001
GAMG:  Solving for Ux, Initial residual = 0.99999977, Final residual = 0.057843227, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 1, Final residual = 0.0057390397, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 1, Final residual = 0.005994265, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.99999813, Final residual = 0.011565501, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.53767394, Final residual = 0.042120368, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.40405034, Final residual = 0.039739205, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.19331502, Final residual = 0.026101031, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.11284094, Final residual = 0.019926848, No Iterations 1000
time step continuity errors : sum local = 0.002175723, global = 2.3026111e-17, cumulative = 2.3026111e-17
rho max/min : 1.2250034 1.221886
ExecutionTime = 27.95 s  ClockTime = 28 s
forceCoeffs output:
    Cm    = -1.320359e-05
    Cd    = 0.093371132
    Cl    = -1.03555e-07
    Cl(f) = -1.3255368e-05
    Cl(r) = 1.3151813e-05
Time = 0.002
GAMG:  Solving for Ux, Initial residual = 0.00060043462, Final residual = 2.0503577e-05, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.082441175, Final residual = 0.00049357056, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.11074134, Final residual = 0.00068867064, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.0041800268, Final residual = 4.1992587e-05, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.5304093, Final residual = 0.04458336, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.36752576, Final residual = 0.038220884, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.18137599, Final residual = 0.025174498, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.108366, Final residual = 0.019873609, No Iterations 1000
time step continuity errors : sum local = 0.002175922, global = 5.3378713e-17, cumulative = 7.6404824e-17
rho max/min : 1.2294214 1.2213151
ExecutionTime = 69.49 s  ClockTime = 70 s
regIOobject::readIfModified() : 
    Re-reading object controlDict from file "/z/pro/cfdtmp03/zachjoer/OpenFOAM/BA/HFK_SHM_gröber/Mach0080_turbulent/processor0/../system/controlDict"
forceCoeffs output:
    Cm    = -1.3143246e-05
    Cd    = 0.093271678
    Cl    = -1.0385113e-07
    Cl(f) = -1.3195172e-05
    Cl(r) = 1.3091321e-05
Time = 0.003
GAMG:  Solving for Ux, Initial residual = 0.00037857059, Final residual = 8.5052485e-06, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.044059488, Final residual = 0.00028399619, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.064196449, Final residual = 0.00042835073, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.0021000954, Final residual = 1.8270224e-05, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.50388282, Final residual = 0.040716606, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.33629964, Final residual = 0.03360745, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.17019278, Final residual = 0.022648336, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.1026526, Final residual = 0.018258963, No Iterations 1000
time step continuity errors : sum local = 0.0021761224, global = 9.5011782e-17, cumulative = 1.7141661e-16
rho max/min : 1.2346406 1.2205626
ExecutionTime = 97.24 s  ClockTime = 97 s
forceCoeffs output:
    Cm    = -1.3086146e-05
    Cd    = 0.093173218
    Cl    = -1.0438748e-07
    Cl(f) = -1.313834e-05
    Cl(r) = 1.3033952e-05
Time = 0.004
GAMG:  Solving for Ux, Initial residual = 0.00029835602, Final residual = 4.6544107e-06, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.031149037, Final residual = 0.00020970957, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.048156363, Final residual = 0.00033464271, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.0014066861, Final residual = 1.0578563e-05, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.47831378, Final residual = 0.038590737, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.3080249, Final residual = 0.031021751, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.15908332, Final residual = 0.021173073, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.096633434, Final residual = 0.017030443, No Iterations 1000
time step continuity errors : sum local = 0.0021763272, global = 1.2815543e-16, cumulative = 2.9957203e-16
rho max/min : 1.2400847 1.21968
ExecutionTime = 139.14 s  ClockTime = 139 s
forceCoeffs output:
    Cm    = -1.3031053e-05
    Cd    = 0.093075976
    Cl    = -1.0516642e-07
    Cl(f) = -1.3083637e-05
    Cl(r) = 1.297847e-05
Time = 0.005
GAMG:  Solving for Ux, Initial residual = 0.00025412598, Final residual = 2.8360233e-06, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.024940148, Final residual = 0.00016987267, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.040378206, Final residual = 0.00028347182, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.001061219, Final residual = 6.8777058e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.44372922, Final residual = 0.036002632, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.28758996, Final residual = 0.029753192, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.15212154, Final residual = 0.020341676, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.093066532, Final residual = 0.017055932, No Iterations 1000
time step continuity errors : sum local = 0.0021765357, global = 1.5571698e-16, cumulative = 4.5528902e-16
rho max/min : 1.2453618 1.2187083
ExecutionTime = 180.69 s  ClockTime = 181 s
forceCoeffs output:
    Cm    = -1.2976731e-05
    Cd    = 0.092980081
    Cl    = -1.0631692e-07
    Cl(f) = -1.302989e-05
    Cl(r) = 1.2923573e-05
Time = 0.006
GAMG:  Solving for Ux, Initial residual = 0.00022470774, Final residual = 1.8258374e-06, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.021459541, Final residual = 0.00014443178, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.03597171, Final residual = 0.00024868834, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.0008551344, Final residual = 4.767277e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.41873944, Final residual = 0.034360238, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.26954847, Final residual = 0.027546949, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.14318594, Final residual = 0.020450321, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.088867609, Final residual = 0.01662983, No Iterations 1000
time step continuity errors : sum local = 0.0021767679, global = 1.9269832e-16, cumulative = 6.4798733e-16
rho max/min : 1.2502182 1.2176803
ExecutionTime = 222.19 s  ClockTime = 222 s
forceCoeffs output:
    Cm    = -1.2923706e-05
    Cd    = 0.092885572
    Cl    = -1.0766722e-07
    Cl(f) = -1.2977539e-05
    Cl(r) = 1.2869872e-05
Time = 0.007
GAMG:  Solving for Ux, Initial residual = 0.00020301393, Final residual = 1.214904e-06, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.019284991, Final residual = 0.00012594988, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.033408597, Final residual = 0.00022331514, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.00071877212, Final residual = 3.4481471e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.392023, Final residual = 0.032911925, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.25364493, Final residual = 0.026367517, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.13814654, Final residual = 0.019546314, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.086155724, Final residual = 0.015924053, No Iterations 1000
time step continuity errors : sum local = 0.0021770555, global = 1.9641971e-16, cumulative = 8.4440704e-16
rho max/min : 1.2545031 1.2166215
ExecutionTime = 263.64 s  ClockTime = 264 s
forceCoeffs output:
    Cm    = -1.2873292e-05
    Cd    = 0.092792417
    Cl    = -1.0917299e-07
    Cl(f) = -1.2927879e-05
    Cl(r) = 1.2818706e-05
Time = 0.008
GAMG:  Solving for Ux, Initial residual = 0.00018599158, Final residual = 8.2619823e-07, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.017834814, Final residual = 0.0001112848, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.031957113, Final residual = 0.00020336741, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.00062225315, Final residual = 2.5766043e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.36825807, Final residual = 0.031599221, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.23882483, Final residual = 0.025922063, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.13136105, Final residual = 0.01864055, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.08279768, Final residual = 0.015756884, No Iterations 1000
time step continuity errors : sum local = 0.0021773878, global = 2.5142653e-16, cumulative = 1.0958336e-15
rho max/min : 1.2581417 1.215552
ExecutionTime = 305.17 s  ClockTime = 305 s
regIOobject::readIfModified() : 
    Re-reading object controlDict from file "/z/pro/cfdtmp03/zachjoer/OpenFOAM/BA/HFK_SHM_gröber/Mach0080_turbulent/processor0/../system/controlDict"
forceCoeffs output:
    Cm    = -1.2827066e-05
    Cd    = 0.092700554
    Cl    = -1.1079009e-07
    Cl(f) = -1.2882462e-05
    Cl(r) = 1.2771671e-05
Time = 0.009
GAMG:  Solving for Ux, Initial residual = 0.00017209101, Final residual = 5.7049672e-07, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.016795727, Final residual = 9.8895364e-05, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.031131225, Final residual = 0.00018609196, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.00055064953, Final residual = 1.9676097e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.34989204, Final residual = 0.029939648, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.22819607, Final residual = 0.024709557, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.12779538, Final residual = 0.01867555, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.080116272, Final residual = 0.015209984, No Iterations 1000
time step continuity errors : sum local = 0.002177766, global = 2.4235564e-16, cumulative = 1.3381892e-15
rho max/min : 1.2611139 1.2144872
ExecutionTime = 346.67 s  ClockTime = 347 s
forceCoeffs output:
    Cm    = -1.2785563e-05
    Cd    = 0.092609912
    Cl    = -1.1228936e-07
    Cl(f) = -1.2841708e-05
    Cl(r) = 1.2729418e-05
Time = 0.01
GAMG:  Solving for Ux, Initial residual = 0.00016042696, Final residual = 3.9853703e-07, No Iterations 1
GAMG:  Solving for Uy, Initial residual = 0.015963236, Final residual = 8.7946467e-05, No Iterations 1
GAMG:  Solving for Uz, Initial residual = 0.030476925, Final residual = 0.00016997212, No Iterations 1
GAMG:  Solving for e, Initial residual = 0.00049567157, Final residual = 1.528501e-06, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.33324438, Final residual = 0.028036589, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.21835329, Final residual = 0.022957868, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.12379308, Final residual = 0.018037857, No Iterations 1000
GAMG:  Solving for p, Initial residual = 0.077487114, Final residual = 0.014877161, No Iterations 1000
time step continuity errors : sum local = 0.0021781888, global = 2.8736122e-16, cumulative = 1.6255504e-15
rho max/min : 1.264078 1.2134386
ExecutionTime = 388.21 s  ClockTime = 388 s
forceCoeffs output:
    Cm    = -1.2753832e-05
    Cd    = 0.092520433
    Cl    = -1.1351413e-07
    Cl(f) = -1.2810589e-05
    Cl(r) = 1.2697074e-05
End
Finalising parallel run

There are agein 1000 Iterations...

Sorry for my incompetence...:/

CFDnewbie147 · November 5, 2013, 11:26

When I try some different Solver for p like this:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.2.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
solvers
{
    p
    {
        solver          PBiCG;
 preconditioner diagonal;
        tolerance       1e-05;//1e-08
        relTol          0.5;//0.1
        smoother        DILUGaussSeidel;//GaussSeidel
        nPreSweeps      2;
        nPostSweeps     4;
        nFinestSweeps   2;
        cacheAgglomeration off;
        nCellsInCoarsestLevel 100;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }
    "(U|e|k|epsilon)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        nFinestSweeps   2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 100;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }
}
SIMPLE
{
    nNonOrthogonalCorrectors 1;
    rhoMin          rhoMin [1 -3 0 0 0] 1.0;
    rhoMax          rhoMax [1 -3 0 0 0] 1.5;
    transonic       yes;
    residualControl
    {
        p               1e-3;
        U               1e-4;
        e               1e-3;
        // possibly check turbulence fields
        "(k|epsilon|omega)" 1e-3;
    }
}
relaxationFactors
{
    fields
    {
        p               0.2;
        rho             0.5;
    }
    equations
    {
        p               0.2;
        U               0.3;
        e               0.3;
        k               0.3;
        epsilon         0.3;
    }
}
// ************************************************************************* //

I get the same solution file for p as for the first solver GAMG and my Output looks like:

Code:

GAMG:  Solving for Ux, Initial residual = 4.922311e-10, Final residual = 4.922311e-10, No Iterations 0
GAMG:  Solving for Uy, Initial residual = 5.2654842e-09, Final residual = 5.2654842e-09, No Iterations 0
GAMG:  Solving for Uz, Initial residual = 1.7094164e-08, Final residual = 9.0853684e-11, No Iterations 1
GAMG:  Solving for e, Initial residual = 9.9583003e-09, Final residual = 9.9583003e-09, No Iterations 0
diagonalPBiCG:  Solving for p, Initial residual = 0.044142169, Final residual = 0.016692135, No Iterations 1
diagonalPBiCG:  Solving for p, Initial residual = 0.022796388, Final residual = 0.0057005063, No Iterations 1
time step continuity errors : sum local = 0.00017012542, global = -6.1272094e-05, cumulative = -0.049840115
rho max/min : 1.2224959 1.1601203
ExecutionTime = 99.81 s  ClockTime = 101 s
forceCoeffs output:
    Cm    = -7.6045523e-06
    Cd    = 0.075369208
    Cl    = 1.8001372e-08
    Cl(f) = -7.5955516e-06
    Cl(r) = 7.6135529e-06
Time = 0.1
GAMG:  Solving for Ux, Initial residual = 4.8521402e-10, Final residual = 4.8521402e-10, No Iterations 0
GAMG:  Solving for Uy, Initial residual = 5.211509e-09, Final residual = 5.211509e-09, No Iterations 0
GAMG:  Solving for Uz, Initial residual = 1.6856978e-08, Final residual = 8.9579104e-11, No Iterations 1
GAMG:  Solving for e, Initial residual = 1.0037838e-08, Final residual = 5.5905957e-11, No Iterations 1
diagonalPBiCG:  Solving for p, Initial residual = 0.043558749, Final residual = 0.0058719703, No Iterations 1
diagonalPBiCG:  Solving for p, Initial residual = 0.025481547, Final residual = 0.0091210457, No Iterations 1
time step continuity errors : sum local = 0.00017012541, global = -6.1272111e-05, cumulative = -0.049901388
rho max/min : 1.2224959 1.1601203
ExecutionTime = 99.94 s  ClockTime = 101 s
forceCoeffs output:
    Cm    = -7.6045524e-06
    Cd    = 0.075369208
    Cl    = 1.8001385e-08
    Cl(f) = -7.5955517e-06
    Cl(r) = 7.6135531e-06
End
Finalising parallel run

Why does this solver not work either???

wyldckat · November 9, 2013, 15:37

Greetings to all!

@CFDnewbie147:

First problem that I can spot is this - you have this in your "fvSolution" file:

Code:

relaxationFactors
{
    fields
    {
        p               0.1;
        rho             0.2;
    }
    equations
    {
        p               0.1;
        U               0.1;
        e               0.1;
        k               0.1;
        epsilon         0.1;
    }
}

The relaxation factors are waaaaaaaaaaaaaaaaaaaaaay too low

This equates to the solver barely doing anything with the equations, since so little is used for the solution.
For comparison, the tutorial "compressible/rhoSimplecFoam/squareBend" uses these:

Code:

relaxationFactors
{
    fields
    {
        p               1;
        rho             1;
    }
    equations
    {
        p               1;
        U               0.9;
        e               0.9;
        k               0.9;
        epsilon         0.9;
    }
}

Second problem that I can spot is that the boundary condition at the "outlet" is undefined. In other words, you've defined both the pressure and velocity at the "inlet", which can lead to an undefined "outlet".
Third problem that I can figure out is that - and I'm guessing here - that you are trying to find the solution, without trying to solve the real physical problem. Let me explain what I mean with an example:
Imagine that instead of having to do this simulation with CFD, your problem was instead that you needed to fly a spaceship in the year 2013. Do you do simply do a quick read of the "quick starters guide into flying spaceships" in 15 minutes and then jump into the real spaceship and take-off with success?
If you had no previous experience whatsoever on anything similar at all, I don't expect you to have a safe take-off and landing!

With OpenFOAM - in fact with CFD in general - you should not try to simulate your final case before having enough practice with simpler cases. First you should start with a simple case and with slow (0.01 or 0.001 Mach?) flow speeds. Then gradually increase the complexity of your problem, so that you can understand what needs to change in order to have the new problem still converge.
In addition, you should try to solve cases that have known solutions, so that you can compare the results you are getting.

Otherwise, even if your case converges, it does not mean that the solution is correct. It only means that the solver converged to a solution, but it's not a 100% certainty that the solution is physically correct!

Best regards,
Bruno

CFDnewbie147 · November 10, 2013, 05:57

Dear Bruno,

first of all, thank you for your detailed answer.

3. I understand your example but that's not right at all. I'm working more than one year with CFD(TAU- Code) and now, for my bachelor thesis, I'm trying to solve the described problem with openfoam. With openfoam I don't have so much experience, only some simple work at university.

I made some tutorials before trying to simulate my real problem and tried to transfer my problem to the tutorial.

2. I thought, in comparison to the rhoSImplecFoam tutorial, I'm trying to solve the equations with more underrelaxation, so lower coefficients. I do not really have a feeling for this numbers, but i thought that for beginning, lower is better, but apparently not?

3.Yes that's true, i fix the pressure and velocity at the inlet (like in TAU). So do I have to fix only velocity at inlet and pressure at outlet?

I hope you will carry on guiding me to a solution.
Best regards,
CFDNewbie147

wyldckat · November 10, 2013, 06:15

Hi CFDnewbie147,

Quote:

Originally Posted by CFDnewbie147

3. I understand your example but that's not right at all. I'm working more than one year with CFD(TAU- Code) and now, for my bachelor thesis, I'm trying to solve the described problem with openfoam. With openfoam I don't have so much experience, only some simple work at university.

My apologies, I meant no disrespect. It's just I've seen on this forum several times in the past, new users of OpenFOAM trying to solve the final problem, without going through the normal learning curve necessary for understanding how OpenFOAM (and CFD) works.
But still, I'm guessing that TAU is a lot more user friendly than OpenFOAM, so consider this a whole other level of a spaceship

With OpenFOAM, most of the times we have to first assemble the spaceship ourselves, then to fill the gas tank, and so on...
With TAU, I'm guessing that one pays for the license and gets a key, a manual and all one has to do is to climb onto the spaceship, since it's ready to go.

Quote:

Originally Posted by CFDnewbie147

I made some tutorials before trying to simulate my real problem and tried to transfer my problem to the tutorial.

How many steps have you taken in evolving the case? More specifically, have you gradually increased the complexity of the problem, or did you jump directly to 0.8 Mach?

Quote:

Originally Posted by CFDnewbie147

2. I thought, in comparison to the rhoSImplecFoam tutorial, I'm trying to solve the equations with more underrelaxation, so lower coefficients. I do not really have a feeling for this numbers, but i thought that for beginning, lower is better, but apparently not?

You can try reducing gradually from 1 to 0.95, then 0.90 and so on, not jump directly to 0.1

In addition, check with the tutorials of OpenFOAM, to see the effect of reducing the relaxation parameters, so that you can get a better feel for them.

Quote:

Originally Posted by CFDnewbie147

3.Yes that's true, i fix the pressure and velocity at the inlet (like in TAU). So do I have to fix only velocity at inlet and pressure at outlet?

From my (limited) experience with OpenFOAM: yes, that's how it is able to work.

Best regards,
Bruno

CFDnewbie147 · November 10, 2013, 07:45

Dear Bruno,

no, that's OK you're right, OpenFOAM is more complex than TAU.

First of all, I took the motorbike tutorial with simpleFoam to look if my mesh works, after that I went to the square bend tutorial and made it running with my mesh and my boundary file without changing the values of the start up conditions. Then I changed some parameters in the startup conditions and looked if it worked...going to mach 0.8 because I think that's easier with subsonic than supersonic start up conditions. I decreased the underrelaxtion values but still doesn't work...and now I'm here because time is running away...

OK I will try underrelexation values near to 1 and I will fix velocity at inlet and pressure at outlet.
rest of my boundary conditions are OK? is the freestream condition better then slip conditions for the wall?

Any other improvements so far? Unfortunately I can change the values and run the case again at Tuesday...

So far, thanks for helping me.
Best regards,
CFDNewbie147

wyldckat · November 10, 2013, 09:31

Hi CFDNewbie147,

Well, from my experience, one should never be in a hurry when it comes to using OpenFOAM. The software is completely free, but it requires a lot more time in exchange. Although, once one has a full grasp of how to use, it can be as easy as running Allrun

As for the questions at hand: have a look at the sonicFoam tutorials. For example, "compressible/sonicFoam/ras/prism" does impose pressure on the inlet as well, but on the outlet it uses the "waveTransmissive" boundary condition. On the walls, it uses "supersonicFreestream", so I'm guessing that for subsonic, you can use the one you're using.

I would also advise you to check the code documentation: http://foam.sourceforge.net/docs/cpp/ - for example, the "freestream" page is this one: http://foam.sourceforge.net/docs/cpp...5.html#details

I don't have experience on this, so I have no idea if either one is suitable for your case

.

Good luck! Best regards,
Bruno

edit: I forgot about the under-relaxation details... my guess is that you should use the ones from the tutorial "squareBend" as a reference, not to just start using "1.0" is all equations and fields!

CFDnewbie147 · November 11, 2013, 09:29

You are right,
if anything is known, you can make a Allrun script, but the way to knowing everything in OpenFOAM is long and hard...

I thougth that the waveTransmissive condition is only for supersonic speed? But I don't know exactly, I've to look it up....or does anybody know this?

The unterrelaxation values I will use as reference and adapt to my case when it's running...

Do you know if rhoSimplecFoam can be used for mach numbers above 1? Or is this not possible because rhoSimplecFoam cannot solve the equations with the appearing shock waves?
I'm not sure about this...

Thank you for your help, and if anybody can answer some other questions I would be happy.

Best regards,
CFDNewbie147

CFDnewbie147 · November 12, 2013, 03:44

I checked my error file and found the following:

Code:

Duplicate entry Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2b1a63159437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE26addpatchConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2b1a7230c3de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b1a7230c76b]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b1a72325516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
Duplicate entry Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2b1a63159437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE32addpatchMapperConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2b1a7230c4de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b1a7230c793]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b1a72325516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
 
...
 
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2b79d49bd437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE32addpatchMapperConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2b79e3b704de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b79e3b70793]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b79e3b89516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2ad2a5ca5437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE31adddictionaryConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2ad2b4e585de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2ad2b4e587bb]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2ad2b4e71516]
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2b6c75140437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE32addpatchMapperConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2b6c842f34de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b6c842f3793]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b6c8430c516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b2ecc47d793]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2b2ecc496516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
#0 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZN4Foam5error14safePrintStackERSo+0x27) [0x2ace46fc6437]
#1 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so(_ZN4Foam12fvPatchFieldIdE32addpatchMapperConstructorToTableINS_14incompressible47alphatJayatillekeWallFunctionFvPatchScalarFieldEEC2ERKNS_4wordE+0xce) [0x2ace561794de]
#2 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2ace56179793]
#3 /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libincompressibleRASModels.so [0x2ace56192516]
Duplicate entry alphatJayatillekeWallFunction in runtime selection table fvPatchField
 
...
 
[magnus05:12296] [ 7] /opt/OpenFOAM/OpenFOAM-2.2.1/platforms/linux64Gcc48DPOpt/lib/libOpenFOAM.so(_ZNK4Foam10GAMGSolver5solveERNS_5FieldIdEERKS2_h+0x5c2) [0x2b6714195742]
[magnus05:12296] [ 8] rhoSimplecFoam [0x43a3da]
[magnus05:12296] [ 9] rhoSimplecFoam [0x4532c1]
[magnus05:12296] [10] rhoSimplecFoam [0x45359e]
[magnus05:12296] [11] rhoSimplecFoam [0x44de14]
[magnus05:12296] [12] /lib64/libc.so.6(__libc_start_main+0xf4) [0x2b6715104b54]
[magnus05:12296] [13] rhoSimplecFoam(__gxx_personality_v0+0x371) [0x41e109]
[magnus05:12296] *** End of error message ***
[magnus06][[20951,1],22][btl_tcp_frag.c:215:mca_btl_tcp_frag_recv] mca_btl_tcp_frag_recv: readv failed: Connection reset by peer (104)
[magnus01][[20951,1],62][btl_tcp_frag.c:215:mca_btl_tcp_frag_recv] mca_btl_tcp_frag_recv: readv failed: Connection reset by peer (104)
[magnus07][[20951,1],14][btl_tcp_frag.c:215:mca_btl_tcp_frag_recv] mca_btl_tcp_frag_recv: readv failed: Connection reset by peer (104)
--------------------------------------------------------------------------
mpirun noticed that process rank 30 with PID 12296 on node magnus05.cfd.lfk.eads.net exited on signal 8 (Floating point exception).
--------------------------------------------------------------------------

Why is there a error with libincompressibleRASModel? RhoSimplecFoam is compressible, isn't it?
And what's the duplicate entry error?
Does anybody know?

Best regards,
CFDNewbie147

wyldckat · November 15, 2013, 03:30

Hi CFDNewbie147,

If my memory doesn't fail me, that bug was corrected soon after OpenFOAM 2.2.1 was released. It means that there is a collision of object names, because "alphatJayatillekeWallFunction" exists for both compressible and incompressible and object-wise this is bad, since it can lead to the crash you have witnessed.

If possible, upgrade to OpenFOAM 2.2.2. Otherwise, you'll have to patch the code manually to correct the problem and then rebuild the affected OpenFOAM libraries.

Best regards,
Bruno

CFDnewbie147 · November 15, 2013, 12:08

Thank's a lot for answering this.

That means, perhabs al my simulations where this error occurs could be false and the results are not good/realistic?

Updating to OpenFOAM-2.2 is no opinion...but how to fix this bug manually?
Where do I find this specific patch and how to update the OF libraries?
Can anybody explain this to me?

Best regards,
CFDNewbie147

Claudio87 · November 21, 2013, 07:33

Dear Bruno and CFDnewbie147,

I add myself in your conversation because I think I have a relevant problem.

I introduce first the case.
To understand the geometry, I attached a slice, but the problem is 3D.
The flow moves from the right to the left side. The inlet BCs are applied on the inlet of the channel on the left; the outlet BCs on the outlet of the channel on the right. The air comes also from on high, from the external domain.

I'm using rhoSimplecFoam as solver, and kOmegaSST as turbulence model.
I got yet a first result, using the minimum flow rate for my problem; and everything seems good. I obtained the right value (I mean, as calculated) for the maximum velocity, and in
general the behaviour of the flow field seems reasonable.

Now, I'm trying to increase the flow rate, but without success...
Using the same parameters from the previous simulation, the solution diverges after few iterations.
I tried to change some of these parameters, in particular the under-relaxation factors.
I can obtain a converging simulation if I use a relaxation factor for p (0.9), but the solution is wrong:
1) it is veeeeery slow (but this isn't a real problem);
2) at the beginning, the velocity profile (with the new velocity) seems to move in the right direction, toward the nozzle;
3) then, it seems to come back!

The flow doesn't reach the nozzle, but comes back!
Considering the nozzle, downstream (on the right) nothing changes (p, rho, U....nothing!)

Instead, if I don't use any relaxation factor for p (so, I put just 1, as in the working case with minimum flow rate), it diverges after few iterations!

What I'm asking you is: there is some parameter I'm using in the wrong way?!
Thare is something I can do to obtain a converging simulation, physically correct?!

The fvSolution file:

Code:

solvers
{
    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        nFinestSweeps   2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }

    "(U|e|k|omega)"
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.1;
        smoother        GaussSeidel;
        nPreSweeps      0;
        nPostSweeps     2;
        nFinestSweeps   2;
        cacheAgglomeration true;
        nCellsInCoarsestLevel 20;
        agglomerator    faceAreaPair;
        mergeLevels     1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    rhoMin          rhoMin [1 -3 0 0 0] 0.1;
    rhoMax          rhoMax [1 -3 0 0 0] 5.0;
    transonic       yes;

    residualControl
    {
        p               1e-5;
        U               1e-5;
        e               1e-3;

        // possibly check turbulence fields
        "(k|omega)" 1e-3;
    }
}

relaxationFactors
{
    fields
    {
        p               1;
        rho             1;
    }
    equations
    {
        p               1;
        U               0.9;
        e               0.9;
        k               0.9;
        omega           0.9;
    }
}

and the fvScheme one:

Code:

ddtSchemes
{
    default             steadyState;
}

gradSchemes
{
    default             Gauss linear;
}

divSchemes
{
    default             none;

    div(phi,U)          bounded Gauss upwind;
    div((muEff*dev2(T(grad(U)))))      Gauss linear;
    div(phi,e)          bounded Gauss upwind;
    div(phi,epsilon)    bounded Gauss upwind;
    div(phi,k)          bounded Gauss upwind;
    div(phi,omega)      bounded Gauss upwind;
    div(phid,p)         Gauss upwind;
    div(phi,Ekp)        bounded Gauss upwind;
    div((phi|interpolate(rho)),p)  Gauss upwind;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p;
    pCorr;
}

I attach the 0 folder with the BCs for the old case (with minimum flow rate); in the new one I changed only the inlet flow rate and values for k and omega, updated for the new velocity.

I hope some of you could help me, because I don't know what I'm doing wrong...
Thank you in advance!

Best regards,
Claudio

wyldckat · November 23, 2013, 06:52

Greetings to all!

@CFDnewbie147:

Quote:

Originally Posted by CFDnewbie147

Updating to OpenFOAM-2.2 is no opinion...but how to fix this bug manually?
Where do I find this specific patch and how to update the OF libraries?

I'm not sure if you're going to like this, but since updating to 2.2.x or 2.2.2 is not an option, here are the steps necessary for patching the problem:

Go into the main OpenFOAM folder:
Code:
```
cd $WM_PROJECT_DIR
```
If OpenFOAM is installed as root at "/opt", then run also this command:
Code:
```
sudo -s
```

Run these commands for downloading the patch files:

Code:

wget "https://github.com/OpenFOAM/OpenFOAM-2.2.x/commit/c8c21905599e2bb94762eba73794a946c945a99b.patch"
wget "https://github.com/OpenFOAM/OpenFOAM-2.2.x/commit/b132ea81cfb4c1cdf6c134c300785c2afd47f971.patch"
wget "https://github.com/OpenFOAM/OpenFOAM-2.2.x/commit/c9f76c1b1b7f64d476592d1bd7d5eccedf2e36a2.patch"
wget "https://github.com/OpenFOAM/OpenFOAM-2.2.x/commit/e98f2a9217fff748e2a79ce36e8dad62de7f7985.patch"

Apply the patches:

Code:

patch -p1 < c8c21905599e2bb94762eba73794a946c945a99b.patch
patch -p1 < b132ea81cfb4c1cdf6c134c300785c2afd47f971.patch
patch -p1 < c9f76c1b1b7f64d476592d1bd7d5eccedf2e36a2.patch
patch -p1 < e98f2a9217fff748e2a79ce36e8dad62de7f7985.patch

Finally, build the necessary parts of OpenFOAM, by running Allwmake:
Code:
```
./Allwmake
```

By the way, the commits/patches in question are (as implied in step #3):

Best regards,
Bruno

wyldckat · November 23, 2013, 06:58

@Claudio:

Quote:

Originally Posted by Claudio87

I hope some of you could help me, because I don't know what I'm doing wrong...

Uhm... you left out a few very important details:

What is the overall dimension of the geometry?
What is the value of the minimum flow speed (not flow rate) in question at the inlet?
What is the value of the maximum velocity reached with the aforementioned flow speed?
What is the value of the new inlet flow speed?
What mesh resolution are you using?

Best regards,
Bruno

November 9, 2013, 15:37		#6
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,982 Blog Entries: 45 Rep Power: 128	Greetings to all! @CFDnewbie147: First problem that I can spot is this - you have this in your "fvSolution" file: Code: relaxationFactors { fields { p 0.1; rho 0.2; } equations { p 0.1; U 0.1; e 0.1; k 0.1; epsilon 0.1; } } The relaxation factors are waaaaaaaaaaaaaaaaaaaaaay too low This equates to the solver barely doing anything with the equations, since so little is used for the solution. For comparison, the tutorial "compressible/rhoSimplecFoam/squareBend" uses these: Code: relaxationFactors { fields { p 1; rho 1; } equations { p 1; U 0.9; e 0.9; k 0.9; epsilon 0.9; } } Second problem that I can spot is that the boundary condition at the "outlet" is undefined. In other words, you've defined both the pressure and velocity at the "inlet", which can lead to an undefined "outlet". Third problem that I can figure out is that - and I'm guessing here - that you are trying to find the solution, without trying to solve the real physical problem. Let me explain what I mean with an example: Imagine that instead of having to do this simulation with CFD, your problem was instead that you needed to fly a spaceship in the year 2013. Do you do simply do a quick read of the "quick starters guide into flying spaceships" in 15 minutes and then jump into the real spaceship and take-off with success? If you had no previous experience whatsoever on anything similar at all, I don't expect you to have a safe take-off and landing! With OpenFOAM - in fact with CFD in general - you should not try to simulate your final case before having enough practice with simpler cases. First you should start with a simple case and with slow (0.01 or 0.001 Mach?) flow speeds. Then gradually increase the complexity of your problem, so that you can understand what needs to change in order to have the new problem still converge. In addition, you should try to solve cases that have known solutions, so that you can compare the results you are getting. Otherwise, even if your case converges, it does not mean that the solution is correct. It only means that the solver converged to a solution, but it's not a 100% certainty that the solution is physically correct! Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

November 10, 2013, 09:31		#10
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,982 Blog Entries: 45 Rep Power: 128	Hi CFDNewbie147, Well, from my experience, one should never be in a hurry when it comes to using OpenFOAM. The software is completely free, but it requires a lot more time in exchange. Although, once one has a full grasp of how to use, it can be as easy as running Allrun As for the questions at hand: have a look at the sonicFoam tutorials. For example, "compressible/sonicFoam/ras/prism" does impose pressure on the inlet as well, but on the outlet it uses the "waveTransmissive" boundary condition. On the walls, it uses "supersonicFreestream", so I'm guessing that for subsonic, you can use the one you're using. I would also advise you to check the code documentation: http://foam.sourceforge.net/docs/cpp/ - for example, the "freestream" page is this one: http://foam.sourceforge.net/docs/cpp...5.html#details I don't have experience on this, so I have no idea if either one is suitable for your case . Good luck! Best regards, Bruno edit: I forgot about the under-relaxation details... my guess is that you should use the ones from the tutorial "squareBend" as a reference, not to just start using "1.0" is all equations and fields! __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM Last edited by wyldckat; November 10, 2013 at 09:35. Reason: see "edit:"

November 15, 2013, 03:30		#13
wyldckat Retired Super Moderator Bruno Santos Join Date: Mar 2009 Location: Lisbon, Portugal Posts: 10,982 Blog Entries: 45 Rep Power: 128	Hi CFDNewbie147, If my memory doesn't fail me, that bug was corrected soon after OpenFOAM 2.2.1 was released. It means that there is a collision of object names, because "alphatJayatillekeWallFunction" exists for both compressible and incompressible and object-wise this is bad, since it can lead to the crash you have witnessed. If possible, upgrade to OpenFOAM 2.2.2. Otherwise, you'll have to patch the code manually to correct the problem and then rebuild the affected OpenFOAM libraries. Best regards, Bruno __________________ OpenFOAM: FAQ \| Getting started Forum: How to get help, to post code/output and forum guide Read this before sending me PM

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Pulsatile pressure inlet with pressure outlet	a.lynchy	FLUENT	3	March 23, 2012 14:45
Fluent natural ventilation pressure boundary condition	pierresandre	FLUENT	24	November 8, 2011 15:32
Neumann pressure BC and velocity field	Antech	Main CFD Forum	0	April 25, 2006 03:15
Pressure outlet values	Eric	FLUENT	3	February 11, 2004 13:05
Hydrostatic pressure in 2-phase flow modeling (CFX4.2)	HB &DS	CFX	0	January 9, 2000 14:19

November 5, 2013, 05:55		#3
henrik Senior Member Henrik Rusche Join Date: Mar 2009 Location: Wernigerode, Sachsen-Anhalt, Germany Posts: 281 Rep Power: 18	Hi, your pressure equation does not converge - 1000 Iterations! Under normal conditions, you should not fix p AND U anywhere. Same is true for zeroGradient. Try setting the pressure at the outlet and zeroGradient it at the inlet. Henrik

November 10, 2013, 05:57		#7
CFDnewbie147 Member Join Date: Jul 2013 Posts: 62 Rep Power: 13	Dear Bruno, first of all, thank you for your detailed answer. 3. I understand your example but that's not right at all. I'm working more than one year with CFD(TAU- Code) and now, for my bachelor thesis, I'm trying to solve the described problem with openfoam. With openfoam I don't have so much experience, only some simple work at university. I made some tutorials before trying to simulate my real problem and tried to transfer my problem to the tutorial. 2. I thought, in comparison to the rhoSImplecFoam tutorial, I'm trying to solve the equations with more underrelaxation, so lower coefficients. I do not really have a feeling for this numbers, but i thought that for beginning, lower is better, but apparently not? 3.Yes that's true, i fix the pressure and velocity at the inlet (like in TAU). So do I have to fix only velocity at inlet and pressure at outlet? I hope you will carry on guiding me to a solution. Best regards, CFDNewbie147

November 10, 2013, 07:45		#9
CFDnewbie147 Member Join Date: Jul 2013 Posts: 62 Rep Power: 13	Dear Bruno, no, that's OK you're right, OpenFOAM is more complex than TAU. First of all, I took the motorbike tutorial with simpleFoam to look if my mesh works, after that I went to the square bend tutorial and made it running with my mesh and my boundary file without changing the values of the start up conditions. Then I changed some parameters in the startup conditions and looked if it worked...going to mach 0.8 because I think that's easier with subsonic than supersonic start up conditions. I decreased the underrelaxtion values but still doesn't work...and now I'm here because time is running away... OK I will try underrelexation values near to 1 and I will fix velocity at inlet and pressure at outlet. rest of my boundary conditions are OK? is the freestream condition better then slip conditions for the wall? Any other improvements so far? Unfortunately I can change the values and run the case again at Tuesday... So far, thanks for helping me. Best regards, CFDNewbie147

November 11, 2013, 09:29		#11
CFDnewbie147 Member Join Date: Jul 2013 Posts: 62 Rep Power: 13	You are right, if anything is known, you can make a Allrun script, but the way to knowing everything in OpenFOAM is long and hard... I thougth that the waveTransmissive condition is only for supersonic speed? But I don't know exactly, I've to look it up....or does anybody know this? The unterrelaxation values I will use as reference and adapt to my case when it's running... Do you know if rhoSimplecFoam can be used for mach numbers above 1? Or is this not possible because rhoSimplecFoam cannot solve the equations with the appearing shock waves? I'm not sure about this... Thank you for your help, and if anybody can answer some other questions I would be happy. Best regards, CFDNewbie147

November 15, 2013, 12:08		#14
CFDnewbie147 Member Join Date: Jul 2013 Posts: 62 Rep Power: 13	Thank's a lot for answering this. That means, perhabs al my simulations where this error occurs could be false and the results are not good/realistic? Updating to OpenFOAM-2.2 is no opinion...but how to fix this bug manually? Where do I find this specific patch and how to update the OF libraries? Can anybody explain this to me? Best regards, CFDNewbie147