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

Error when running BuoyantBoussinesqSimpleFoam

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 18, 2020, 06:16
Default Error when running BuoyantBoussinesqSimpleFoam
  #1
Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6
b.simpson is on a distinguished road
Hi,

I am trying to run a simulation using the BuoyantBoussinesqSimpleFoam solver in OpenFOAM v-1812. The simulation is of a naturally ventilated building with space on the outside for the external environment.

Currently when I try running BuoyantBoussinesqSimpleFoam the simulation is exiting due to an error. The error is as follows:

Code:
-------------------------------------------------------
Primary job  terminated normally, but 1 process returned
a non-zero exit code.. Per user-direction, the job has been aborted.
-------------------------------------------------------
--------------------------------------------------------------------------
mpirun detected that one or more processes exited with non-zero status, thus causing
the job to be terminated. The first process to do so was:

  Process name: [[5190,1],1]
  Exit code:    142
--------------------------------------------------------------------------
Does anyone have an idea of what might be causing the error and/or how I should go about troubleshooting this?

Any help on this issue would be much appreciated.

Kind regards,
Ben


My boundary conditions are as follows:
Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 1e5;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmax"
    {
        type            totalPressure;
        p0              $internalField;
    }
    "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ|Inlet"
    {
        type            fixedFluxPressure;
        value           $internalField;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 293;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmin|zmax|Ceiling|Floor|EWall|NWall|SWall|WWall|Inlet"
    {
        type            fixedValue;
        value           uniform 293;
    }
    PC
    {
        type            fixedGradient;
		gradient		uniform 100;
    }
    Occ
    {
		type            fixedGradient;
		gradient		uniform 130;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 0);

boundaryField
{
    "xmin|xmax|ymin|ymax|zmax"
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
	"zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            noSlip;
    }
	Inlet
    {
        type            fixedValue;
        value           uniform (0 0.00047 0);
		//value           uniform (0 1 0);
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      alphat;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmax|Inlet"
    {
        type            calculated;
        value           uniform 0;
    }
	"zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            alphatJayatillekeWallFunction;
        Prt             0.85;
        value           uniform 0;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      CO2;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmax"
    {
        type            inletOutlet;
        inletValue      $internalField;
        value           $internalField;
    }
    "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            zeroGradient;
    }
	Inlet
    {
        type            fixedValue;
        value           uniform 1.0;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

//epsilonInlet  0.03; // Cmu^0.75 * k^1.5 / L ; L =10

dimensions      [0 2 -3 0 0 0 0];

internalField   uniform 0.01;

boundaryField
{
   "xmin|xmax|ymin|ymax|zmax"
    {
        type            inletOutlet;
        inletValue      uniform 0.01;
        value           uniform 0.01;
    }
    "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            epsilonWallFunction;
        value           $internalField;
    }
	Inlet
    {
        type            fixedValue;
        value           $internalField;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

kInlet          1.5;   // approx k = 1.5*(I*U)^2 ; I = 0.1

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

internalField   uniform 0.1;

boundaryField
{
   "xmin|xmax|ymin|ymax|zmax"
    {
        type            inletOutlet;
        inletValue      uniform 0.01;
        value           uniform 0.01;
    }
    "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            kqRWallFunction;
        value           uniform 0.1;
    }
	Inlet
    {
        type            fixedValue;
        value           uniform 0.1;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmax|Inlet"
    {
        type            calculated;
        value           uniform 0;
    }
    "zmin|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ"
    {
        type            nutkWallFunction;
        value           uniform 0;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}

FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 1e5;

boundaryField
{
    "xmin|xmax|ymin|ymax|zmin|zmax|Ceiling|Floor|EWall|NWall|SWall|WWall|PC|Occ|Inlet"
    {
        type            fixedFluxPressure;
        rho             rhok;
        value           uniform 0;
    }
	
	#includeEtc "caseDicts/setConstraintTypes"
}
b.simpson is offline   Reply With Quote

Old   June 19, 2020, 20:15
Default
  #2
Member
 
Lisandro Maders
Join Date: Feb 2013
Posts: 98
Rep Power: 13
Lisandro Maders is on a distinguished road
Hello,

Can you run other cases in parallel (tutorials?).. Doesn't look like a case problem, but some wrong mpi setup or similar..

Also, did you remember to source OpenFOAM?

Cheers,
Lisandro Maders is offline   Reply With Quote

Old   June 21, 2020, 15:36
Default
  #3
Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6
b.simpson is on a distinguished road
Thank you Lisandro, for your response.

I have tried running one of my other cases and the windaroundbuildings tutorial case, both run in parallel. Both ran to an endTime of 5000 without any errors.

I tried running my current case not in parallel and the solver stopped at a similar time to the parallel run, but without any error message or convergence message. I have copied the end of the log file below.

Can you explain what you mean by source OpenFOAM?

Kind regards,
Ben

Code:
Time = 499

DILUPBiCGStab:  Solving for Ux, Initial residual = 4.2035517e-12, Final residual = 4.2035517e-12, No Iterations 0
DILUPBiCGStab:  Solving for Uy, Initial residual = 1.3809356e-12, Final residual = 1.3809356e-12, No Iterations 0
DILUPBiCGStab:  Solving for Uz, Initial residual = 3.4626842e-11, Final residual = 3.4626842e-11, No Iterations 0
DILUPBiCGStab:  Solving for T, Initial residual = 5.7255095e-07, Final residual = 5.7255095e-07, No Iterations 0
DICPCG:  Solving for p_rgh, Initial residual = 4.8174887e-29, Final residual = 4.8174887e-29, No Iterations 0
time step continuity errors : sum local = 4.7379025e+47, global = 6.7267478e+38, cumulative = 1.3690775e+39
DILUPBiCGStab:  Solving for epsilon, Initial residual = 0.081559159, Final residual = 2.7467555e-07, No Iterations 1
bounding epsilon, min: -5.0589917e+76 max: 6.6333303e+104 average: 6.9901096e+98
DILUPBiCGStab:  Solving for k, Initial residual = 9.7152148e-06, Final residual = 9.7152148e-06, No Iterations 0
ExecutionTime = 12550.98 s  ClockTime = 12575 s

fieldMinMax fieldMinMax write:
    min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0)
    max(mag(U)) = 8.3277972e+51 in cell 58642 at location (-0.28756519 5.8448262 0.38346076)
    min(CO2) = -1.3654693e-08 in cell 2506767 at location (13.100119 16.077201 2.082341)
    max(CO2) = 1 in cell 471004 at location (7.8713678 2.5999999 1.2113401)
    min(p) = -3.6330321e+87 in cell 1506619 at location (-0.14127546 8.297961 3.4)
    max(p) = 1.0130987e+73 in cell 595727 at location (-0.018164488 7.8713315 3.1237291)
    min(T) = 292.99634 in cell 524500 at location (11.752019 15.324934 0.72123229)
    max(T) = 476.00394 in cell 267900 at location (13.908153 16.782254 3.3148686)

scalarTransport execute: CO2
DILUPBiCGStab:  Solving for CO2, Initial residual = 2.1732333e-28, Final residual = 2.1732333e-28, No Iterations 0

Time = 500

DILUPBiCGStab:  Solving for Ux, Initial residual = 1, Final residual = 0.0032024424, No Iterations 1
DILUPBiCGStab:  Solving for Uy, Initial residual = 1, Final residual = 0.0032024424, No Iterations 1
DILUPBiCGStab:  Solving for Uz, Initial residual = 1, Final residual = 0.0032024579, No Iterations 1
DILUPBiCGStab:  Solving for T, Initial residual = 1.1094197e-06, Final residual = 1.1094197e-06, No Iterations 0
b.simpson is offline   Reply With Quote

Old   June 21, 2020, 16:53
Default
  #4
HPE
Senior Member
 
HPE's Avatar
 
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 932
Rep Power: 12
HPE is on a distinguished road
Hi

- The maximum magnitude of the velocity field is nonphysically large. Also, that of epsilon field.
- Could you double-check the mesh metrics? `checkMesh -allGeometry -allTopology`?
- Could you run your case with another turbulence closure model, e.g. omega-based model?
HPE is offline   Reply With Quote

Old   June 22, 2020, 16:14
Default
  #5
Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6
b.simpson is on a distinguished road
Thank you for your response.

I have run check mesh and couldnt see any issues in the log file.

Code:
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0

Enabling all (cell, face, edge, point) topology checks.

Enabling all geometry checks.

Time = 0

Mesh stats
    points:           349461
    faces:            1004544
    internal faces:   961536
    cells:            327680
    faces per cell:   6
    boundary patches: 7
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     327680
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Topological cell zip-up check OK.
    Face-face connectivity OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                   Bounding box
    xmin                2560     2709     ok (non-closed singly connected)   (-3 -3 0) (18.7 -3 3.4)
    xmax                2560     2709     ok (non-closed singly connected)   (-3 18.7 0) (18.7 18.7 3.4)
    ymin                2560     2709     ok (non-closed singly connected)   (-3 -3 0) (-3 18.7 3.4)
    ymax                2560     2709     ok (non-closed singly connected)   (18.7 -3 0) (18.7 18.7 3.4)
    zmin                16384    16641    ok (non-closed singly connected)   (-3 -3 0) (18.7 18.7 0)
    zmax                7920     8360     ok (non-closed singly connected)   (-3 -3 3.4) (18.7 18.7 3.4)
    zmax_ceiling        8464     8649     ok (non-closed singly connected)   (0 0 3.4) (15.7 15.7 3.4)

Checking faceZone topology for multiply connected surfaces...
    No faceZones found.

Checking basic cellZone addressing...
    No cellZones found.

Checking geometry...
    Overall domain bounding box (-3 -3 0) (18.7 18.7 3.4)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (4.4299191e-16 4.4299191e-16 -7.1450608e-15) OK.
    Max cell openness = 1.2245107e-16 OK.
    Max aspect ratio = 1.0239131 OK.
    Minimum face area = 0.027777776. Maximum face area = 0.029122167.  Face area magnitudes OK.
    Min volume = 0.0047222218. Max volume = 0.0049507683.  Total volume = 1601.026.  Cell volumes OK.
    Mesh non-orthogonality Max: 0 average: 0
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.2789791e-13 OK.
    Coupled point location match (average 0) OK.
    Face tets OK.
    Min/max edge length = 0.16666666 0.17065218 OK.
    All angles in faces OK.
    Face flatness (1 = flat, 0 = butterfly) : min = 1  average = 1
    All face flatness OK.
    Cell determinant (wellposedness) : minimum: 0.1249674 average: 0.93518669
    Cell determinant check OK.
    Concave cell check OK.
    Face interpolation weight : minimum: 0.49409237 average: 0.49993708
    Face interpolation weight check OK.
    Face volume ratio : minimum: 0.97664544 average: 0.99975127
    Face volume ratio check OK.

Mesh OK.

End
I have also just tried running the k-omegaSST turbulence model instead of k-epsilon. This ran without error past where the k-epsilon model usually failed. Unfortunately I was unable to run the model until convergence as my computer decided to crash several hours in

Here is the end of the log file before my computer died.

Code:
Time = 1613

DILUPBiCGStab:  Solving for Ux, Initial residual = 0.0022768434, Final residual = 3.8302314e-05, No Iterations 1
DILUPBiCGStab:  Solving for Uy, Initial residual = 0.00087106937, Final residual = 1.5127342e-05, No Iterations 1
DILUPBiCGStab:  Solving for Uz, Initial residual = 0.0016276516, Final residual = 2.8328342e-05, No Iterations 1
DILUPBiCGStab:  Solving for T, Initial residual = 0.0012589984, Final residual = 6.7196765e-05, No Iterations 1
DICPCG:  Solving for p_rgh, Initial residual = 0.0089650297, Final residual = 8.7014216e-05, No Iterations 55
time step continuity errors : sum local = 1.5389332e-05, global = -1.902396e-06, cumulative = -0.0041707033
smoothSolver:  Solving for omega, Initial residual = 0.00039958681, Final residual = 2.8080538e-05, No Iterations 3
DILUPBiCGStab:  Solving for k, Initial residual = 0.00018173884, Final residual = 4.1791532e-06, No Iterations 1
ExecutionTime = 17547.01 s  ClockTime = 17682 s

fieldMinMax fieldMinMax write:
    min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0) on processor 0
    max(mag(U)) = 1.049388 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2
    min(CO2) = 0 in cell 0 at location (-2.9166667 -3 0.085) on processor 0
    max(CO2) = 1 in cell 277850 at location (1.899056 7.5999999 1.2113291) on processor 0
    min(p) = 99965.943 in cell 276497 at location (13.758831 15.718746 3.4) on processor 3
    max(p) = 100000 in cell 135893 at location (12.521604 15.718749 0) on processor 3
    min(T) = 293 in cell 0 at location (-2.9166667 -3 0.085) on processor 0
    max(T) = 1186.3781 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2

scalarTransport execute: CO2
DILUPBiCGStab:  Solving for CO2, Initial residual = 0.00036557033, Final residual = 6.8689503e-06, No Iterations 1

Time = 1614

DILUPBiCGStab:  Solving for Ux, Initial residual = 0.0029013552, Final residual = 4.6281166e-05, No Iterations 1
DILUPBiCGStab:  Solving for Uy, Initial residual = 0.0010731421, Final residual = 1.7715774e-05, No Iterations 1
DILUPBiCGStab:  Solving for Uz, Initial residual = 0.0017262862, Final residual = 2.9371945e-05, No Iterations 1
DILUPBiCGStab:  Solving for T, Initial residual = 0.0012577848, Final residual = 6.7378228e-05, No Iterations 1
DICPCG:  Solving for p_rgh, Initial residual = 0.0090579121, Final residual = 8.7629514e-05, No Iterations 43
time step continuity errors : sum local = 1.5462643e-05, global = -1.1040759e-06, cumulative = -0.0041718074
smoothSolver:  Solving for omega, Initial residual = 0.00039540712, Final residual = 2.8313504e-05, No Iterations 3
DILUPBiCGStab:  Solving for k, Initial residual = 0.00017238916, Final residual = 4.1214014e-06, No Iterations 1
ExecutionTime = 17560.16 s  ClockTime = 17698 s

fieldMinMax fieldMinMax write:
    min(mag(U)) = 0 in cell 0 at location (-2.9166667 -2.9166667 0) on processor 0
    max(mag(U)) = 1.046601 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2
    min(CO2) = 0 in cell 0 at location (-2.9166667 -3 0.085) on processor 0
    max(CO2) = 1 in cell 277850 at location (1.899056 7.5999999 1.2113291) on processor 0
    min(p) = 99965.943 in cell 271108 at location (1.9411685 15.718749 3.4) on processor 2
    max(p) = 100000 in cell 73613 at location (7.8713315 -0.018749525 0) on processor 1
    min(T) = 293 in cell 0 at location (-2.9166667 -3 0.085) on processor 0
    max(T) = 1180.8241 in cell 108330 at location (1.8558424 15.718582 3.3788139) on processor 2

scalarTransport execute: CO2
DILUPBiCGStab:  Solving for CO2, Initial residual = 0.00036510744, Final residual = 6.8622869e-06, No Iterations 1
Is there a reason why the k-omegaSST model would run without error but the k-epsilon model wont?

Kind regards,
Ben
b.simpson is offline   Reply With Quote

Old   June 22, 2020, 17:08
Default
  #6
HPE
Senior Member
 
HPE's Avatar
 
Herpes Free Engineer
Join Date: Sep 2019
Location: The Home Under The Ground with the Lost Boys
Posts: 932
Rep Power: 12
HPE is on a distinguished road
The culprit is the epsilon. There would be lots of reasons, I'm afraid. Please do search web - there should already be lots of insightful remarks about epsilon's numerical fragility.

Good luck.

PS:Might be wise to check with other epsilon-based models, e.g. kepsilonphitf or rngkepsilon. etc.
HPE is offline   Reply With Quote

Old   June 23, 2020, 20:31
Default
  #7
Member
 
Lisandro Maders
Join Date: Feb 2013
Posts: 98
Rep Power: 13
Lisandro Maders is on a distinguished road
You could try to under-relax the fields a little bit. The BC's looks fine. This could be a mesh problem, can you share some image of a slice of your mesh?

Also, can you share the fvSchemes and fvSolution files you are using? Did you use the same files for both k-epsilon and kOmega-SST?
Lisandro Maders is offline   Reply With Quote

Old   June 24, 2020, 08:05
Default
  #8
Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6
b.simpson is on a distinguished road
Thanks for the replies.

I have been looking into better defining my BC's (especially for k and epsilon) previously they were just taken from tutorials.

As for the fvSolutions and fvSchemes, I have copied them below. For the Omega run I used the same solutions and schemes as this but jut added Omega. For that I copied the Omega relevant parts from the motorbike tutorial. I will try a run with under-relaxing the fields.

Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         steadyState;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    default         none;
	
    div(phi,U)      bounded Gauss upwind;
    div(phi,T)      bounded Gauss upwind;
    div(phi,k)      bounded Gauss upwind;
    div(phi,epsilon) bounded Gauss upwind;
	div(phi,CO2) 	bounded Gauss upwind;
    div((nuEff*dev2(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}


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

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
    p_rgh
    {
        solver          PCG;
        preconditioner  DIC;
        tolerance       1e-06;
        relTol          0.01;
    }

    "(U|T|h|k|epsilon|CO2)"
    {
        solver          PBiCGStab;
        preconditioner  DILU;
        tolerance       1e-05;
        relTol          0.1;
    }

    G
    {
        $p_rgh;
        tolerance       1e-05;
        relTol          0.1;
    }
}

SIMPLE
{
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;

    residualControl
    {
        p_rgh           1e-4;
        U               1e-4;
	CO2             1e-4;
        T               1e-4;
	h               1e-4;
        G               1e-4;

        // possibly check turbulence fields
        "(k|epsilon|omega)" 1e-4;
    }
}

relaxationFactors
{
    fields
	{
	rho             1.0;
        p_rgh           0.9;
    }
    equations
    {
        U               0.3;
	CO2             0.3;
	h               0.9;
        T               0.5;
        "(k|epsilon|R)" 0.7;
	P		0.8;
	G               0.7;
    }
}


// ************************************************************************* //
Thanks again for the support.

Kind regards,

Ben
b.simpson is offline   Reply With Quote

Old   June 26, 2020, 09:18
Default
  #9
Member
 
Ben Simpson
Join Date: Dec 2019
Location: UK
Posts: 32
Rep Power: 6
b.simpson is on a distinguished road
I have been able to get my model running by adjusting the relaxation factors for epsilon as you suggested. A value of 1 allowed my model to run without errors.

I still need to go back a better define my BC's but at least I have a functioning model for the time being.

Thanks for all the support with this issue.

Regards,
Ben
b.simpson is offline   Reply With Quote

Reply

Tags
buoyancy driven flow, buoyantboussinesqsimple, openfoam 1812

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
Simulation just stops output writing, but keeps running blaise OpenFOAM Running, Solving & CFD 6 March 27, 2024 04:49
Running Case in Parallel Typ Main CFD Forum 5 May 11, 2020 03:43
[swak4Foam] swak4foam openfoam 7 installation problem Andrea23 OpenFOAM Community Contributions 1 February 17, 2020 18:11
Error problem while running sadia d lts tutorial kane OpenFOAM Running, Solving & CFD 2 May 26, 2018 03:38
Error Running Design of Experiments in ANSYS Fluent tytrzecki FLUENT 0 April 22, 2018 15:01


All times are GMT -4. The time now is 09:01.