interFoam case blows up

jrrygg · November 11, 2012, 11:46

Hi,

I have made a 3D-case with a mesh imported from Ansys. I want water to enter through a cylinder ("jet") and enter the main domain. I have specified an alpha 1 in negative x-direction, and tried with velocities ranging from 0.01 to 40 m/s. I have also experimented with different options for fvSchemes, fvSolution, max courant-numbers and timesteps with no luck.

The error message I get is:

Code:

Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Reading field p_rgh

Reading field alpha1

Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
Selecting turbulence model type laminar

Reading g
Calculating field g.h

time step continuity errors : sum local = 4.67867e-10, global = -4.67867e-10, cumulative = -4.67867e-10
DICPCG:  Solving for pcorr, Initial residual = 1, Final residual = 6.66652e-11, No Iterations 111
time step continuity errors : sum local = 3.11808e-20, global = 5.16e-22, cumulative = -4.67867e-10
Courant Number mean: 2.33626e-08 max: 3.83881e-05

Starting time loop

Courant Number mean: 2.33626e-08 max: 3.83881e-05
Interface Courant Number mean: 0 max: 0
Time = 0.0001

MULES: Solving for alpha1
Phase-1 volume fraction = 2.33933e-10  Min(alpha1) = 0  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 4.67867e-10  Min(alpha1) = 0  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 1, Final residual = 0.0429735, No Iterations 47
time step continuity errors : sum local = 6.12373e-06, global = -1.9493e-07, cumulative = -1.95398e-07
DICPCG:  Solving for p_rgh, Initial residual = 0.0589919, Final residual = 0.00254961, No Iterations 8
time step continuity errors : sum local = 0.000113259, global = 1.82915e-06, cumulative = 1.63376e-06
DICPCG:  Solving for p_rgh, Initial residual = 0.0149289, Final residual = 9.11547e-08, No Iterations 73
time step continuity errors : sum local = 4.31244e-09, global = 3.18223e-10, cumulative = 1.63407e-06
ExecutionTime = 0.21 s  ClockTime = 1 s

Courant Number mean: 0.00757338 max: 12.278
Interface Courant Number mean: 0 max: 0
Time = 0.0002

MULES: Solving for alpha1
Phase-1 volume fraction = 7.05874e-05  Min(alpha1) = -2.93612e-24  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.000141174  Min(alpha1) = -3.28782e-25  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.0166851, Final residual = 0.000693113, No Iterations 59
time step continuity errors : sum local = 3.47964e-05, global = 3.5545e-06, cumulative = 5.18857e-06
DICPCG:  Solving for p_rgh, Initial residual = 0.113737, Final residual = 0.00554455, No Iterations 22
time step continuity errors : sum local = 0.000272306, global = 6.33387e-06, cumulative = 1.15224e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.0730375, Final residual = 9.70425e-08, No Iterations 115
time step continuity errors : sum local = 5.18939e-09, global = -2.03538e-10, cumulative = 1.15222e-05
ExecutionTime = 0.37 s  ClockTime = 1 s

Courant Number mean: 0.0331767 max: 3081.05
Interface Courant Number mean: 7.87481e-07 max: 0.00145705
Time = 0.0003

MULES: Solving for alpha1
Phase-1 volume fraction = 0.000141468  Min(alpha1) = -1.13757e-23  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.000141761  Min(alpha1) = -2.82471e-24  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.341486, Final residual = 0.014237, No Iterations 71
time step continuity errors : sum local = 0.00127742, global = -0.000206445, cumulative = -0.000194923
DICPCG:  Solving for p_rgh, Initial residual = 0.0948778, Final residual = 0.00473849, No Iterations 23
time step continuity errors : sum local = 0.00587709, global = -0.000116325, cumulative = -0.000311248
DICPCG:  Solving for p_rgh, Initial residual = 0.261779, Final residual = 9.31408e-08, No Iterations 160
time step continuity errors : sum local = 1.36897e-07, global = -1.75955e-09, cumulative = -0.00031125
ExecutionTime = 0.54 s  ClockTime = 1 s

Courant Number mean: 0.786892 max: 104531
Interface Courant Number mean: 7.91815e-07 max: 0.00161964
Time = 0.0004

MULES: Solving for alpha1
Phase-1 volume fraction = 0.000142055  Min(alpha1) = -2.23505e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.000142348  Min(alpha1) = -3.30942e-22  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.721516, Final residual = 0.15886, No Iterations 1001
time step continuity errors : sum local = 1.20394, global = -0.0632404, cumulative = -0.0635517
DICPCG:  Solving for p_rgh, Initial residual = 0.0976159, Final residual = 0.0607169, No Iterations 1001
time step continuity errors : sum local = 330.267, global = -19.6465, cumulative = -19.71
DICPCG:  Solving for p_rgh, Initial residual = 0.612786, Final residual = 5.75419, No Iterations 1001
time step continuity errors : sum local = 1.06021e+06, global = 110793, cumulative = 110773
ExecutionTime = 1.35 s  ClockTime = 2 s

Courant Number mean: 2.9712e+07 max: 1.21991e+12
Interface Courant Number mean: 89.6278 max: 214939
Time = 0.0005

MULES: Solving for alpha1
Phase-1 volume fraction = 0.00014264  Min(alpha1) = -17299.9  Max(alpha1) = 5670.03
#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  void Foam::MULES::limit<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::zeroField const&, Foam::zeroField const&, double, double, int, bool) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::MULES::explicitSolve(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, double, double) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
Floating point exception (core dumped)

May it be a mesh-problem?

My case:

michielm · November 12, 2012, 02:22

Have you tried the option

Code:

adjustTimeStep     yes

and setting the maxCo to 0.1 or so?

My experience with interFoam is that a case that starts with an unphysical interface shape needs a couple of tiny timesteps in order to converge. It appears that your case is diverging because of a timestep which is too big.

jrrygg · November 12, 2012, 10:59

Thank you for your reply!

Yes I have tried with various settings in controlDict. It keeps blowing up. From my last run (Timestep 0.2):

My controlDict:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.1.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      controlDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

application     interFoam;

startFrom       startTime;

startTime       0;

stopAt          endTime;

endTime         1;

deltaT          0.001;

writeControl    adjustableRunTime;

writeInterval   0.005;

purgeWrite      0;

writeFormat     ascii;

writePrecision  6;

writeCompression uncompressed;

timeFormat      general;

timePrecision   6;

runTimeModifiable true;

adjustTimeStep  true;

maxCo           0.1;
maxAlphaCo      0.1;
maxDeltaT       1;


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

michielm · November 12, 2012, 11:47

could you post the last couple of solver steps and the error message for the case you show in your last post?! (with the adjustable timestep)

jrrygg · November 13, 2012, 08:27

Thank you for your help. The error message:

Code:

MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -4.52391e-23  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -1.04697e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -9.24491e-23  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -1.54047e-22  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.00448808, Final residual = 0.000210064, No Iterations 2
time step continuity errors : sum local = 3.12345e-11, global = 1.09597e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00371592, Final residual = 0.000166137, No Iterations 11
time step continuity errors : sum local = 2.4842e-11, global = -3.67525e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00332416, Final residual = 9.88164e-08, No Iterations 60
time step continuity errors : sum local = 1.49161e-14, global = 1.54071e-15, cumulative = -4.655e-05
ExecutionTime = 1389.81 s  ClockTime = 1546 s

Courant Number mean: 9.58414e-07 max: 0.102032
Interface Courant Number mean: 2.99141e-08 max: 0.00587784
deltaT = 2.98399e-14
Time = 0.201079196759357

MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -2.66929e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -1.20053e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -2.66929e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -2.66929e-22  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.00445708, Final residual = 0.000210387, No Iterations 2
time step continuity errors : sum local = 3.13306e-11, global = 1.726e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00371445, Final residual = 0.000164389, No Iterations 11
time step continuity errors : sum local = 2.46185e-11, global = -3.15885e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00332526, Final residual = 9.60067e-08, No Iterations 63
time step continuity errors : sum local = 1.45043e-14, global = -6.45223e-16, cumulative = -4.655e-05
ExecutionTime = 1389.9 s  ClockTime = 1546 s

Courant Number mean: 9.58448e-07 max: 0.102032
Interface Courant Number mean: 2.99091e-08 max: 0.00587354
deltaT = 2.92457e-14
Time = 0.201079196759386

MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -2.57925e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -4.52318e-23  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -1.49625e-22  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.00939034  Min(alpha1) = -1.49504e-22  Max(alpha1) = 1
DICPCG:  Solving for p_rgh, Initial residual = 0.00448914, Final residual = 0.000210085, No Iterations 2
time step continuity errors : sum local = 3.12323e-11, global = 1.09735e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00371613, Final residual = 0.000166175, No Iterations 11
time step continuity errors : sum local = 2.48435e-11, global = -3.67613e-14, cumulative = -4.655e-05
DICPCG:  Solving for p_rgh, Initial residual = 0.00332451, Final residual = 9.90195e-08, No Iterations 60
time step continuity errors : sum local = 1.4944e-14, global = 1.53605e-15, cumulative = -4.655e-05
ExecutionTime = 1389.98 s  ClockTime = 1546 s

Courant Number mean: 9.58483e-07 max: 0.102032
Interface Courant Number mean: 2.99043e-08 max: 0.00586926
deltaT = 2.86633e-14
Time = 0.201079196759415

#0  Foam::error::printStack(Foam::Ostream&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1  Foam::sigFpe::sigHandler(int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2   in "/lib/x86_64-linux-gnu/libc.so.6"
#3  void Foam::MULES::limiter<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::Field<double>&, Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::zeroField const&, Foam::zeroField const&, double, double, int) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  void Foam::MULES::limit<Foam::geometricOneField, Foam::zeroField, Foam::zeroField>(Foam::geometricOneField const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::zeroField const&, Foam::zeroField const&, double, double, int, bool) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::MULES::explicitSolve(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> const&, Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, double, double) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#6  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
Floating point exception (core dumped)

michielm · November 13, 2012, 11:51

ok, clearly something is completely blowing up and there are two common reasons: (i) mesh issues (ii) BC issues

- did you run checkMesh? - what was/is the result?
- do you have boundary conditions on alpha1 which might cause strong curvature?

jrrygg · November 13, 2012, 12:07

checkMesh seems fine I think (should I by the way use non-orthogonal correctors?):

Code:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           26691
    faces:            74600
    internal faces:   69400
    cells:            24000
    boundary patches: 4
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     24000
    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.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                  
    inlet               100      121      ok (non-closed singly connected)  
    atmosphere          2100     2191     ok (non-closed singly connected)  
    backWall            600      651      ok (non-closed singly connected)  
    symmetry            2400     2501     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 0 0) (0.5 0.5 0.5)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (-3.06208e-17 -3.24068e-16 1.6619e-16) OK.
    Max cell openness = 2.9343e-16 OK.
    Max aspect ratio = 113.772 OK.
    Minumum face area = 4.87918e-07. Maximum face area = 0.00423881.  Face area magnitudes OK.
    Min volume = 2.44101e-09. Max volume = 0.000106032.  Total volume = 0.125.  Cell volumes OK.
    Mesh non-orthogonality Max: 73.2231 average: 11.2647
   *Number of severely non-orthogonal faces: 80.
    Non-orthogonality check OK.
  <<Writing 80 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 0.843639 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

I have a water inlet on alpha1:

Code:

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

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    bucketwalls
    {
        type            zeroGradient;
    }
    rotif-rotating-solid
    {
        type            zeroGradient;
    }
    rotopen
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
    rotsym
    {
        type            symmetryPlane;
    }
    jetinlet
    {
        type            fixedValue;
        value           uniform 1;
    }
    jetsymmetry
    {
        type            symmetryPlane;
    }
    jetwall
    {
        type            zeroGradient;
    }
}

farhhad · November 13, 2012, 16:33

The number of non-orthognal faces is relatively high , I would use the following command to localise the faces and solve it:

foamToVTK faceSet -nonOrthoFaces

as I am currently dealing with them problem, i would say that the problem is absolutely from the mesh, unless you've set a non-physical condition in your BC. I've found out that interFoam or VOF is extremely sensitive with mesh, and hex mesh seems to work much better.

Farhad

michielm · November 14, 2012, 03:16

Additionally I remember that there used to be a bug in the symmetryPlane BC. Not sure whether that is still there in the latest OF version. You could easily try by temporarily changing the symmetryPlane BC to a fixedValue BC

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
interFoam vs icoFoam on a single-phase case	nuovodna	OpenFOAM Running, Solving & CFD	1	May 1, 2014 09:37
Interfoam blows on parallel run	danvica	OpenFOAM Running, Solving & CFD	16	December 22, 2012 02:09
SRFSimpleFoam tutorial case blows up on laptop (but runs on desktop?)	AHMeng	OpenFOAM Running, Solving & CFD	1	April 27, 2012 08:34
bc's of a komegaSST case	Zymon	OpenFOAM	11	July 25, 2010 09:36
Interfoam Droplet under shear test case	adona058	OpenFOAM Running, Solving & CFD	3	May 3, 2010 18:46

November 12, 2012, 02:22		#2
michielm Member Michiel Join Date: Oct 2010 Location: Delft, Netherlands Posts: 97 Rep Power: 15	Have you tried the option Code: adjustTimeStep yes and setting the maxCo to 0.1 or so? My experience with interFoam is that a case that starts with an unphysical interface shape needs a couple of tiny timesteps in order to converge. It appears that your case is diverging because of a timestep which is too big.

November 12, 2012, 11:47		#4
michielm Member Michiel Join Date: Oct 2010 Location: Delft, Netherlands Posts: 97 Rep Power: 15	could you post the last couple of solver steps and the error message for the case you show in your last post?! (with the adjustable timestep)

November 13, 2012, 11:51		#6
michielm Member Michiel Join Date: Oct 2010 Location: Delft, Netherlands Posts: 97 Rep Power: 15	ok, clearly something is completely blowing up and there are two common reasons: (i) mesh issues (ii) BC issues - did you run checkMesh? - what was/is the result? - do you have boundary conditions on alpha1 which might cause strong curvature?

November 13, 2012, 16:33		#8
farhhad New Member Farhad N. Join Date: Apr 2010 Posts: 6 Rep Power: 16	The number of non-orthognal faces is relatively high , I would use the following command to localise the faces and solve it: foamToVTK faceSet -nonOrthoFaces as I am currently dealing with them problem, i would say that the problem is absolutely from the mesh, unless you've set a non-physical condition in your BC. I've found out that interFoam or VOF is extremely sensitive with mesh, and hex mesh seems to work much better. Farhad

November 14, 2012, 03:16		#9
michielm Member Michiel Join Date: Oct 2010 Location: Delft, Netherlands Posts: 97 Rep Power: 15	Additionally I remember that there used to be a bug in the symmetryPlane BC. Not sure whether that is still there in the latest OF version. You could easily try by temporarily changing the symmetryPlane BC to a fixedValue BC