compressibleInterFoam diverging Temperature/Velocity problem

shipman · January 11, 2016, 03:18

Hi to all,

I am trying to run laval Nozzle simulations using compressibleInterFoam. Nozzle has 3 inlets, 2 of them are liquid nitrogen whereas other one gas nitrogen.

I tried several boundary condition, however finally always getting number of iterations exceeded based on final Temp became negative whereas the velocity is too high. My boundary conditions are as follows:

alphaLiquid:

Code:

boundaryField
{
    inletliq1
    {
         type            fixedValue;
        value           uniform 1;
    }

	 inletliq2
    {
         type            fixedValue;
        value           uniform 1;
    }

	inletgas
    {
         type            fixedValue;
        value           uniform 0;
    }

    hotplate
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
       // type            calculated;
       // value           uniform 0;
        //type            inletOutlet;
       // inletValue      $internalField;
        
    }
    frontAndBack
    {
        type            empty;
    }
}

U:

Code:

inletliq1
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }

	inletliq2
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }
	
	inletgas
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }

    hotplate
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    outlet
    {
      // type            zeroGradient;
        
          type            inletOutlet;
          inletValue      uniform (0 0 0);
          value           uniform (0 0 0); 
    }
    frontAndBack
    {
        type            empty;
    }

p_rgh

Code:

boundaryField
{
    inletliq1
    {
         type            zeroGradient;
   /*   type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

	inletliq2
    {
         type            zeroGradient;
    /*  type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

	inletgas
    {
         type            zeroGradient;
    /*  type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

    hotplate
    {
        type            zeroGradient;
    //    gradient        uniform 0;
     //   value           uniform 100000;
    }
    outlet
    {
      type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 100000;
        value           uniform 100000;
        
    }
    frontAndBack
    {
        type            empty;
    }

T:

Code:

inletliq1
    {
        type            fixedValue;
        value           uniform 64;
    }

	inletliq2
    {
        type            fixedValue;
        value           uniform 64;
    }	

	inletgas
    {
        type            fixedValue;
        value           uniform 64;
    }

    hotplate
    {
        type            zeroGradient;
    }
	
    outlet
    {
        type             fixedValue;
        value            uniform 300;
    }
	
    frontAndBack
    {
        type            empty;
    }

For discraetization schemes I used following:

Code:

divSchemes
{
    div(phi,alpha)  Gauss vanLeer01; //vanLeer
    div(phirb,alpha) Gauss linear;

    div(rhoPhi,U)  Gauss upwind;
    div(phi,thermo:rho.N2liquid) Gauss upwind; //vanLeer01; 
    div(phi,thermo:rho.N2gas) Gauss upwind; //vanLeer01; //upwind; 
    div(rhoPhi,T)  Gauss upwind;
    div(rhoPhi,K)  Gauss upwind;
    div(phi,p)      Gauss upwind;
    div(phi,k)      Gauss upwind;

    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

And this is the last iterations (taken from log file) which results in error:

Code:

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047367522  Min(alpha.N2liquid) = -4.1378651e-09  Min(alpha.N2gas) = -8.197836e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00057059475, Final residual = 9.6696153e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017737476, Final residual = 2.5523847e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5862065e-05, Final residual = 5.1625609e-09, No Iterations 1
min(T) 1.0603252e-06
GAMG:  Solving for p_rgh, Initial residual = 4.5001306e-05, Final residual = 2.4484333e-14, No Iterations 1
max(U) 151.60039
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.1897599e-06, Final residual = 2.2659211e-15, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 3.8525366e-06, Final residual = 2.6463465e-16, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 3.8402215e-06, Final residual = 3.8142587e-23, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
ExecutionTime = 1132.48 s


Courant Number mean: 0.04020333 max: 0.24664585
deltaT = 3.4425687e-08
Time = 0.0008864852698

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047356642  Min(alpha.N2liquid) = -6.7193432e-08  Min(alpha.N2gas) = -3.1465242e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00056220914, Final residual = 9.531315e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017542992, Final residual = 2.5257089e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5606028e-05, Final residual = 5.0761703e-09, No Iterations 1
min(T) 2.073488e-07
GAMG:  Solving for p_rgh, Initial residual = 4.5783127e-05, Final residual = 2.5054008e-14, No Iterations 1
max(U) 151.69519
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.5587802e-06, Final residual = 2.2455038e-15, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.2241096e-06, Final residual = 2.7998571e-16, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 4.2032737e-06, Final residual = 4.560433e-23, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
ExecutionTime = 1132.52 s


Courant Number mean: 0.040201488 max: 0.24679589
deltaT = 3.4425687e-08
Time = 0.0008865196955

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047345767  Min(alpha.N2liquid) = -3.653193e-09  Min(alpha.N2gas) = -3.1586107e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00049636171, Final residual = 8.3886739e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.0001596781, Final residual = 2.2907359e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.3608802e-05, Final residual = 4.4344118e-09, No Iterations 1
min(T) -5.9874863e-07
GAMG:  Solving for p_rgh, Initial residual = 4.9065333e-05, Final residual = 2.5108673e-14, No Iterations 1
max(U) 151.78778
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 7.5718612e-06, Final residual = 2.1709276e-15, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 7.2286592e-06, Final residual = 2.5013507e-16, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 7.2137334e-06, Final residual = 3.0444005e-23, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
ExecutionTime = 1132.56 s


Courant Number mean: 0.040198901 max: 0.24695147
deltaT = 3.4425687e-08
Time = 0.0008865541212

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047334892  Min(alpha.N2liquid) = -3.2573147e-09  Min(alpha.N2gas) = -3.1638578e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00054769955, Final residual = 9.3002095e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017190608, Final residual = 2.4799912e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5173815e-05, Final residual = 4.9445499e-09, No Iterations 1
[8] 
[8] 
[8] --> FOAM FATAL ERROR: 
[8] Maximum number of iterations exceeded
[8] 
[8]     From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy>]
[8]     in file /opt/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.
[8] 
FOAM parallel run aborting
[8] 
[8] #0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
[8] #1  Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
[8] #2  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libfluidThermophysicalModels.so"
[8] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libfluidThermophysicalModels.so"
[8] #4  Foam::twoPhaseMixtureThermo::correct() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libtwoPhaseMixtureThermo.so"
[8] #5  ? in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/bin/compressibleInterFoam"
[8] #6  __libc_start_main in "/lib64/libc.so.6"
[8] #7  ? in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/bin/compressibleInterFoam"
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 8 in communicator MPI_COMM_WORLD 
with errorcode 1.

Is there anyone that can give some suggestion.

Thank you in advance.

Bloerb · January 11, 2016, 12:27

First and most important step.
You should run checkMesh. If your nonOrthogonality is above 50 add nonOrthogonalCorrectors. If it is above 60 consider remeshing. The aspect ratio is another big problem for the interfoam solvers from my experience. nOuterCorrectors can be increased and relaxation factors added. However those are all just measures to counteract bad meshes. Please post the checkMesh log. Are you using a turbulence model?

Some things that might help, but probably won't. You could try adding this to your grad schemes:

Code:

grad(U) cellLimited Gauss linear 1;

And you could try changing wall pressure boundaries to flixedFluxPressure instead of zeroGradient.

shipman · January 11, 2016, 20:21

Quote:

Originally Posted by Bloerb

First and most important step.
You should run checkMesh. If your nonOrthogonality is above 50 add nonOrthogonalCorrectors. If it is above 60 consider remeshing. The aspect ratio is another big problem for the interfoam solvers from my experience. nOuterCorrectors can be increased and relaxation factors added. However those are all just measures to counteract bad meshes. Please post the checkMesh log. Are you using a turbulence model?

Some things that might help, but probably won't. You could try adding this to your grad schemes:

Code:

grad(U) cellLimited Gauss linear 1;

And you could try changing wall pressure boundaries to flixedFluxPressure instead of zeroGradient.

Hi Stefan,

Thank you for your suggestions. I am running the case using 2D geometry and turbulence model is not so big deal. first, I just want to fix problem which I mentioned above. (Velocity is extremely increasing almost 15~20 times larger than inlet velocity, whereas Temp is going to negative...)

This is checkMesh:

Code:

Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           127512
    internal points:  0
    faces:            252530
    internal faces:   125020
    cells:            62925
    faces per cell:   6
    boundary patches: 6
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     62925
    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                  
    inletliq1           20       42       ok (non-closed singly connected)  
    inletliq2           20       42       ok (non-closed singly connected)  
    inletgas            25       52       ok (non-closed singly connected)  
    hotplate            1060     2124     ok (non-closed singly connected)  
    outlet              535      1072     ok (non-closed singly connected)  
    frontAndBack        125850   127512   ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (0 -0.008 -0.0001) (0.024 0.008 0.0001)
    Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
    Mesh has 2 solution (non-empty) directions (1 1 0)
    All edges aligned with or perpendicular to non-empty directions.
    Boundary openness (-2.4370059e-17 -1.1251536e-17 1.1104837e-15) OK.
    Max cell openness = 2.178075e-16 OK.
    Max aspect ratio = 4.517634 OK.
    Minimum face area = 3.2677224e-10. Maximum face area = 3.2916764e-08.  Face area magnitudes OK.
    Min volume = 6.5354449e-14. Max volume = 2.3984089e-12.  Total volume = 3.509564e-08.  Cell volumes OK.
    Mesh non-orthogonality Max: 46.2859 average: 5.8587258
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 1.0520423 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End

And I changed the wall pressure BC to fixedFluxPressure. However, this solver needs p and p_rgh files during running the case. Could you tell me that the boundary conditions should be set same for both p and p_rgh or different? I set p as same as p_rgh.

I set also the fvSolution as you suggested:

Code:

PIMPLE
{
    momentumPredictor yes;
    transonic       no;
    nOuterCorrectors 3;
    nCorrectors     4;//2;
    nNonOrthogonalCorrectors 1;
}

however T again is going to negative and gives same error.

Any other request?

Thank you.

shipman · January 12, 2016, 04:26

As an adiditon, I also commented out TEqn.H to see whether it affects or not velocity increasing. However, no solution. still velocity is increasing extremely high and giving same error which i post at #1.

Any suggestion will be appreaciated.

thank you

Bloerb · January 12, 2016, 15:40

Your mesh seems alright. Therefore it is most likely a boundary condition.

You set T at your outlet to fixedValue. This needs to be zeroGradient. You can not define it as fixedValue on both inlet and outlet. Did not even see this before.

For p_rgh you might try setting hotPlate to fixedFluxPressure. Everything within the p file should be set to calculated.

Turbo_hrf · June 20, 2016, 18:49

Quote:

Originally Posted by shipman

Hi to all,

I am trying to run laval Nozzle simulations using compressibleInterFoam. Nozzle has 3 inlets, 2 of them are liquid nitrogen whereas other one gas nitrogen.

I tried several boundary condition, however finally always getting number of iterations exceeded based on final Temp became negative whereas the velocity is too high. My boundary conditions are as follows:

alphaLiquid:

Code:

boundaryField
{
    inletliq1
    {
         type            fixedValue;
        value           uniform 1;
    }

	 inletliq2
    {
         type            fixedValue;
        value           uniform 1;
    }

	inletgas
    {
         type            fixedValue;
        value           uniform 0;
    }

    hotplate
    {
        type            zeroGradient;
    }
    outlet
    {
        type            zeroGradient;
       // type            calculated;
       // value           uniform 0;
        //type            inletOutlet;
       // inletValue      $internalField;
        
    }
    frontAndBack
    {
        type            empty;
    }
}

U:

Code:

inletliq1
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }

	inletliq2
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }
	
	inletgas
    {
        type            fixedValue;
        value           uniform (15 0 0);
    }

    hotplate
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    outlet
    {
      // type            zeroGradient;
        
          type            inletOutlet;
          inletValue      uniform (0 0 0);
          value           uniform (0 0 0); 
    }
    frontAndBack
    {
        type            empty;
    }

p_rgh

Code:

boundaryField
{
    inletliq1
    {
         type            zeroGradient;
   /*   type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

	inletliq2
    {
         type            zeroGradient;
    /*  type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

	inletgas
    {
         type            zeroGradient;
    /*  type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 2.8e5;
        value           uniform 2.8e5;*/
    }

    hotplate
    {
        type            zeroGradient;
    //    gradient        uniform 0;
     //   value           uniform 100000;
    }
    outlet
    {
      type            totalPressure;
        phi             rhoPhi;
        rho             rho;
        psi             none;
        gamma           1.4;
        p0              uniform 100000;
        value           uniform 100000;
        
    }
    frontAndBack
    {
        type            empty;
    }

T:

Code:

inletliq1
    {
        type            fixedValue;
        value           uniform 64;
    }

	inletliq2
    {
        type            fixedValue;
        value           uniform 64;
    }	

	inletgas
    {
        type            fixedValue;
        value           uniform 64;
    }

    hotplate
    {
        type            zeroGradient;
    }
	
    outlet
    {
        type             fixedValue;
        value            uniform 300;
    }
	
    frontAndBack
    {
        type            empty;
    }

For discraetization schemes I used following:

Code:

divSchemes
{
    div(phi,alpha)  Gauss vanLeer01; //vanLeer
    div(phirb,alpha) Gauss linear;

    div(rhoPhi,U)  Gauss upwind;
    div(phi,thermo:rho.N2liquid) Gauss upwind; //vanLeer01; 
    div(phi,thermo:rho.N2gas) Gauss upwind; //vanLeer01; //upwind; 
    div(rhoPhi,T)  Gauss upwind;
    div(rhoPhi,K)  Gauss upwind;
    div(phi,p)      Gauss upwind;
    div(phi,k)      Gauss upwind;

    div(((rho*nuEff)*dev2(T(grad(U))))) Gauss linear;
}

And this is the last iterations (taken from log file) which results in error:

Code:

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047367522  Min(alpha.N2liquid) = -4.1378651e-09  Min(alpha.N2gas) = -8.197836e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00057059475, Final residual = 9.6696153e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017737476, Final residual = 2.5523847e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5862065e-05, Final residual = 5.1625609e-09, No Iterations 1
min(T) 1.0603252e-06
GAMG:  Solving for p_rgh, Initial residual = 4.5001306e-05, Final residual = 2.4484333e-14, No Iterations 1
max(U) 151.60039
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.1897599e-06, Final residual = 2.2659211e-15, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 3.8525366e-06, Final residual = 2.6463465e-16, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 3.8402215e-06, Final residual = 3.8142587e-23, No Iterations 1
max(U) 151.60044
min(p_rgh) 100000
ExecutionTime = 1132.48 s


Courant Number mean: 0.04020333 max: 0.24664585
deltaT = 3.4425687e-08
Time = 0.0008864852698

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047356642  Min(alpha.N2liquid) = -6.7193432e-08  Min(alpha.N2gas) = -3.1465242e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00056220914, Final residual = 9.531315e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017542992, Final residual = 2.5257089e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5606028e-05, Final residual = 5.0761703e-09, No Iterations 1
min(T) 2.073488e-07
GAMG:  Solving for p_rgh, Initial residual = 4.5783127e-05, Final residual = 2.5054008e-14, No Iterations 1
max(U) 151.69519
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.5587802e-06, Final residual = 2.2455038e-15, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 4.2241096e-06, Final residual = 2.7998571e-16, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 4.2032737e-06, Final residual = 4.560433e-23, No Iterations 1
max(U) 151.69523
min(p_rgh) 100000
ExecutionTime = 1132.52 s


Courant Number mean: 0.040201488 max: 0.24679589
deltaT = 3.4425687e-08
Time = 0.0008865196955

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047345767  Min(alpha.N2liquid) = -3.653193e-09  Min(alpha.N2gas) = -3.1586107e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00049636171, Final residual = 8.3886739e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.0001596781, Final residual = 2.2907359e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.3608802e-05, Final residual = 4.4344118e-09, No Iterations 1
min(T) -5.9874863e-07
GAMG:  Solving for p_rgh, Initial residual = 4.9065333e-05, Final residual = 2.5108673e-14, No Iterations 1
max(U) 151.78778
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 7.5718612e-06, Final residual = 2.1709276e-15, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
GAMG:  Solving for p_rgh, Initial residual = 7.2286592e-06, Final residual = 2.5013507e-16, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
GAMGPCG:  Solving for p_rgh, Initial residual = 7.2137334e-06, Final residual = 3.0444005e-23, No Iterations 1
max(U) 151.78782
min(p_rgh) 100000
ExecutionTime = 1132.56 s


Courant Number mean: 0.040198901 max: 0.24695147
deltaT = 3.4425687e-08
Time = 0.0008865541212

PIMPLE: iteration 1
MULES: Solving for alpha.N2liquid
Liquid phase volume fraction = 0.047334892  Min(alpha.N2liquid) = -3.2573147e-09  Min(alpha.N2gas) = -3.1638578e-09
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for Ux, Initial residual = 0.00054769955, Final residual = 9.3002095e-11, No Iterations 2
smoothSolver:  Solving for Uy, Initial residual = 0.00017190608, Final residual = 2.4799912e-11, No Iterations 2
smoothSolver:  Solving for T, Initial residual = 1.5173815e-05, Final residual = 4.9445499e-09, No Iterations 1
[8] 
[8] 
[8] --> FOAM FATAL ERROR: 
[8] Maximum number of iterations exceeded
[8] 
[8]     From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar)const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar)const) const [with Thermo = Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >; Type = Foam::sensibleInternalEnergy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy>]
[8]     in file /opt/OpenFOAM/OpenFOAM-3.0.x/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.
[8] 
FOAM parallel run aborting
[8] 
[8] #0  Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
[8] #1  Foam::error::abort() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libOpenFOAM.so"
[8] #2  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::calculate() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libfluidThermophysicalModels.so"
[8] #3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::perfectFluid<Foam::specie> >, Foam::sensibleInternalEnergy> > > >::correct() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libfluidThermophysicalModels.so"
[8] #4  Foam::twoPhaseMixtureThermo::correct() in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/lib/libtwoPhaseMixtureThermo.so"
[8] #5  ? in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/bin/compressibleInterFoam"
[8] #6  __libc_start_main in "/lib64/libc.so.6"
[8] #7  ? in "/opt/OpenFOAM/OpenFOAM-3.0.x/platforms/linux64Gcc48DPInt32Opt/bin/compressibleInterFoam"
--------------------------------------------------------------------------
MPI_ABORT was invoked on rank 8 in communicator MPI_COMM_WORLD 
with errorcode 1.

Is there anyone that can give some suggestion.

Thank you in advance.

Hi, I have the same problem when using the compressibleInterFoam, All the boundary conditions, fvScheme, fvSolution are the same with you. Do you solve this problem? Why the velocity goes extremely high and temperature goes to negative?

your reply is most appreciated.

Bloerb · June 22, 2016, 08:53

You should add the changes I talked about. Change the Temperature outlet boundary condition to zeroGradient. Change p_rgh at walls to fixedFluxPressure etc.

SmokedJuggler · August 14, 2016, 15:46

Hello everyone,

I am using CompressibleInterFoam for a test case of a rectangular computational domain. In my case instead of what Shipman had, I have two walls on the left boundary and an Inlet in the middle. Top and Bottom Patches are free surfaces. And the Right patch is outlet. And as a test case I initialize all the regions to be air.

I was getting negative temperature before but using zeroGradiaent at the inlet fixed that problem. (Thanks for all the useful information here)

The temperature decreases rapidly but does not become negative anymore. However, I am getting the following error:

Code:

Courant Number mean: 0.017525563 max: 0.36055112
deltaT = 3.1316128e-05
Time = 0.01149259369

PIMPLE: iteration 1
MULES: Solving for alpha.water
Liquid phase volume fraction = 0.99838497  Min(alpha.water) = 0  Min(alpha.air) = -6.1014024e-05
diagonal:  Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
smoothSolver:  Solving for T, Initial residual = 0.0020526023, Final residual = 0.0023329173, No Iterations 1000
min(T) 0.93072415
GAMG:  Solving for p_rgh, Initial residual = 0.17359627, Final residual = 6.6372495e-05, No Iterations 1
max(U) 34.502714
min(p_rgh) 52859.589
#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::sigFpe::sigHandler(int) at ??:?
#2  ? in "/lib/x86_64-linux-gnu/libc.so.6"
#3  Foam::PCG::solve(Foam::Field<double>&, Foam::Field<double> const&, unsigned char) const at ??:?
#4  Foam::fvMatrix<double>::solveSegregated(Foam::dictionary const&) at ??:?
#5  Foam::fvMatrix<double>::solve(Foam::dictionary const&) at ??:?
#6  ? at ??:?
#7  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#8  ? at ??:?
Floating point exception (core dumped)

My B.C are:

alpha.water

Code:

    object      alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    FrontAndBack
    {
        type            empty;
    }
    Inlet
    {
        type            zeroGradient;
    }
    Outlet
    {
        type            zeroGradient;
    }
    TopAndBottomPatches
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }
    Walls
    {
        type            zeroGradient;
    }
}

U:

Code:

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

internalField   uniform (0 0 0);

boundaryField
{
    FrontAndBack
    {
        type            empty;        
    }
    Inlet
    {
        type            fixedValue;
        value           uniform (10 0 0);
    }
    Outlet
    {
        type            zeroGradient;
    }
    TopAndBottomPatches
    {
        type            pressureInletOutletVelocity;
        value           uniform (0 0 0);
    }
    Walls
    {
        type            noSlip;
    }

p:

Code:

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

internalField   uniform 1e5;

boundaryField
{
    FrontAndBack
    {
        type            empty;
    }
    Inlet
    {
        type            zeroGradient;
    }
    Outlet
    {
        type            fixedValue;
        value           uniform 1e5;

    }
    TopAndBottomPatches
    {
        type            totalPressure;
        p0              uniform 1e5;
    }
    Walls
    {
        type            zeroGradient;
    }
}

p_rgh

Code:

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

internalField   uniform 1e5;

boundaryField
{
    FrontAndBack
    {
        type            empty;
    }
    Inlet
    {
        type            zeroGradient;
    }
    Outlet
    {
        type            fixedValue;
        value           uniform 1e5;
    }
    TopAndBottomPatches
    {
        type            totalPressure;
        p0              uniform 1e5;
    }
    Walls
    {
        type            fixedFluxPressure;
        value           uniform 0;
 
    }
}

T

Code:

dimensions      [0 0 0 1 0 0 0];

internalField   uniform 300;

boundaryField
{
    FrontAndBack
    {
        type            empty;
    }
    Inlet
    {
        type            fixedValue;
        value           uniform 300; 
    }
    Outlet
    {
        type            zeroGradient;
    }
    TopAndBottomPatches
    {
        type            zeroGradient;
    }
    Walls
    {
        type            zeroGradient;
    }
}

I would appreciate if someone could give me some guidance on how to resolve the issue and help me understand why this error is happening.

Thanks to all,

lt123sss · May 30, 2017, 08:09

Have you solved your problem. I meet the same problem and cannot figure where the problem is? Your reply is highly appreciated.

JM27 · October 30, 2019, 12:24

Hi everyone,

I am having the same problem with diverging temperature and velocity using compressibleInterFoam. I am using OF v5.

I am using uniformFixedValue for p_rgh, calculated for p, zeroGradient for T, U and alpha but the simulation still crashes after few time-steps. I have tried several schemes but the simulation fails at more or less the same point in time.

Has anyone managed to solve this problem?

john myce · February 12, 2020, 12:25

Hey guys,

I know it is a old thread but be careful when you run simulation with Liquid N2.
Check in the following path according to your version : /src/thermophysicalModels/thermophysicalProperties/liquidProperties/N2/N2.C

If you have: mu_(32.165, 496.9, 3.9069, -1.08e-21, 10.0),
you need to add a minus to the coeff in bold because without this correction it compute a dynamic viscosity over 1e+24 Pa.s which is wrong.

See this link for more information: https://bugs.openfoam.org/view.php?id=3136

Maybe it can solve your problems with the velocity and temperature.

Cheers,

JM27 · May 7, 2020, 12:04

I am now running a different simulation for internal flow in compressibleInterFoam using air and water.

I still end up having the same problem, i.e. velocity and pressure keep on increasing and increasing until the simulation diverges

I've tried all sorts of boundary conditions and changed solver settings but it still keeps having the same issues although at different point in the simulation. I've also suppressed solution of the temperature equation to try and single out the issue but it seems that temperature is NOT causing the problem...

Can someone please tell me how they solved this problem??

Xinzhen · March 4, 2023, 01:51

Hi, I've been modifying the compressibleInterFoam solver recently as well, and ran into the problem you raised. I found that the calculations are correct when the grid is perfectly orthogonal, but quickly diverge when there are non-orthogonal parts of the grid. Did you solve this problem?

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Problem with interFoam; Wave/wiggle alpha1 behavior	JonW	OpenFOAM	10	February 4, 2023 07:27
UDF compiling problem	Wouter	Fluent UDF and Scheme Programming	6	June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem	JFDC	FLUENT	1	July 11, 2011 05:59
natural convection problem for a CHT problem	Se-Hee	CFX	2	June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem)	ParodDav	CFX	5	April 29, 2007 19:13

January 11, 2016, 12:27		#2
Bloerb Senior Member Join Date: Sep 2013 Posts: 353 Rep Power: 20	First and most important step. You should run checkMesh. If your nonOrthogonality is above 50 add nonOrthogonalCorrectors. If it is above 60 consider remeshing. The aspect ratio is another big problem for the interfoam solvers from my experience. nOuterCorrectors can be increased and relaxation factors added. However those are all just measures to counteract bad meshes. Please post the checkMesh log. Are you using a turbulence model? Some things that might help, but probably won't. You could try adding this to your grad schemes: Code: grad(U) cellLimited Gauss linear 1; And you could try changing wall pressure boundaries to flixedFluxPressure instead of zeroGradient. hogsonik likes this.

January 12, 2016, 04:26		#4
shipman Senior Member Baris (Heewa) Join Date: Jan 2013 Location: Japan Posts: 130 Rep Power: 13	As an adiditon, I also commented out TEqn.H to see whether it affects or not velocity increasing. However, no solution. still velocity is increasing extremely high and giving same error which i post at #1. Any suggestion will be appreaciated. thank you

January 12, 2016, 15:40		#5
Bloerb Senior Member Join Date: Sep 2013 Posts: 353 Rep Power: 20	Your mesh seems alright. Therefore it is most likely a boundary condition. You set T at your outlet to fixedValue. This needs to be zeroGradient. You can not define it as fixedValue on both inlet and outlet. Did not even see this before. For p_rgh you might try setting hotPlate to fixedFluxPressure. Everything within the p file should be set to calculated.

June 22, 2016, 08:53		#7
Bloerb Senior Member Join Date: Sep 2013 Posts: 353 Rep Power: 20	You should add the changes I talked about. Change the Temperature outlet boundary condition to zeroGradient. Change p_rgh at walls to fixedFluxPressure etc.

May 30, 2017, 08:09		#9
lt123sss New Member Tong Li Join Date: Mar 2017 Posts: 2 Rep Power: 0	Have you solved your problem. I meet the same problem and cannot figure where the problem is? Your reply is highly appreciated.

October 30, 2019, 12:24		#10
JM27 Member Join Date: Apr 2018 Location: UK Posts: 78 Rep Power: 8	Hi everyone, I am having the same problem with diverging temperature and velocity using compressibleInterFoam. I am using OF v5. I am using uniformFixedValue for p_rgh, calculated for p, zeroGradient for T, U and alpha but the simulation still crashes after few time-steps. I have tried several schemes but the simulation fails at more or less the same point in time. Has anyone managed to solve this problem?

February 12, 2020, 12:25		#11
john myce Member Join Date: Sep 2018 Location: France Posts: 62 Rep Power: 7	Hey guys, I know it is a old thread but be careful when you run simulation with Liquid N2. Check in the following path according to your version : /src/thermophysicalModels/thermophysicalProperties/liquidProperties/N2/N2.C If you have: mu_(32.165, 496.9, 3.9069, -1.08e-21, 10.0), you need to add a minus to the coeff in bold because without this correction it compute a dynamic viscosity over 1e+24 Pa.s which is wrong. See this link for more information: https://bugs.openfoam.org/view.php?id=3136 Maybe it can solve your problems with the velocity and temperature. Cheers,

May 7, 2020, 12:04		#12
JM27 Member Join Date: Apr 2018 Location: UK Posts: 78 Rep Power: 8	I am now running a different simulation for internal flow in compressibleInterFoam using air and water. I still end up having the same problem, i.e. velocity and pressure keep on increasing and increasing until the simulation diverges I've tried all sorts of boundary conditions and changed solver settings but it still keeps having the same issues although at different point in the simulation. I've also suppressed solution of the temperature equation to try and single out the issue but it seems that temperature is NOT causing the problem... Can someone please tell me how they solved this problem??

March 4, 2023, 01:51		#13
Xinzhen New Member Xinzhen Join Date: Nov 2022 Posts: 3 Rep Power: 3	Hi, I've been modifying the compressibleInterFoam solver recently as well, and ran into the problem you raised. I found that the calculations are correct when the grid is perfectly orthogonal, but quickly diverge when there are non-orthogonal parts of the grid. Did you solve this problem?