CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   interFoam (http://www.cfd-online.com/Forums/openfoam-solving/109395-interfoam.html)

lorraineshe November 16, 2012 09:44

interFoam
 
1 Attachment(s)
Hello,

i have done a simulation with interFoam. I got the error message like below:
Code:

/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.1.1                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 2.1.1-221db2718bbb
Exec  : interFoam
Date  : Nov 16 2012
Time  : 12:11:54
Host  : "manli-VirtualBox"
PID    : 8674
Case  : /home/manli/Blasendynamik
nProcs : 1
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


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 = 1.06596e+287, global = -6.315e+270, cumulative = -6.315e+270
GAMGPCG:  Solving for pcorr, Initial residual = 1, Final residual = 2.97882e-05, No Iterations 4
time step continuity errors : sum local = 3.1753e+282, global = -1.15191e+281, cumulative = -1.15191e+281
Courant Number mean: 2.76663e+287 max: 7.56694e+288

Starting time loop

Courant Number mean: 0.00365621 max: 0.1
Interface Courant Number mean: 0 max: 0
deltaT = 6.6077e-292
Time = 6.6077e-292

MULES: Solving for alpha1
Phase-1 volume fraction = 0.991857  Min(alpha1) = 0  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.991857  Min(alpha1) = 0.00111111  Max(alpha1) = 1
MULES: Solving for alpha1
Phase-1 volume fraction = 0.991857  Min(alpha1) = 0.00323727  Max(alpha1) = 1

Code:

......Reading field U

Reading/calculating face flux field phi

Reading transportProperties

Selecting incompressible transport model Newtonian
Selecting incompressible transport model Newtonian
#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/libc.so.6"
#3  void Foam::mag<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh>&, Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#4  Foam::tmp<Foam::GeometricField<double, Foam::fvsPatchField, Foam::surfaceMesh> > Foam::mag<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh>(Foam::GeometricField<Foam::Vector<double>, Foam::fvsPatchField, Foam::surfaceMesh> const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libfiniteVolume.so"
#5  Foam::interfaceProperties::calculateK() in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libinterfaceProperties.so"
#6  Foam::interfaceProperties::interfaceProperties(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<Foam::Vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::IOdictionary const&) in "/opt/openfoam211/platforms/linux64GccDPOpt/lib/libinterfaceProperties.so"
#7 
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
#8  __libc_start_main in "/lib/libc.so.6"
#9 
 in "/opt/openfoam211/platforms/linux64GccDPOpt/bin/interFoam"
Floating point exception
....

could someone tell me, how can I solve this problem?

treima November 16, 2012 10:05

Hello,

you have a Courant number of 0 and a timestep of approximatly 0, perhaps this is the problem.

Can you change this? For example a maximal Courant number of 0.1?


regards
treima

Lieven November 16, 2012 14:51

It seems to me that at there is already something seriously wrong immediately after initialization

time step continuity errors : sum local = 1.06596e+287

The extremely small time step (and related courant number) are, as I see it, a direct consequence of this. So I would recommend you to check boundary conditions and initial conditions of all variables (maybe the interfoam tutorial can help you).

Regards,

L

lorraineshe November 20, 2012 12:27

Bubble rising, interFoam
 
I have made the case simpler and checked the BC. I have made just:
all the variables zeroGradient at all sides except noslip for velocity at the inlet and fixvalue 0 for the pressure at the outlet. However, my case still doesn't work.

I wonder if it is because of the setFieldsDict, where I have used sphereToCell... to define the area of the air bubble.

who knows why...

lorraineshe November 20, 2012 12:41

1 Attachment(s)
Quote:

Originally Posted by treima (Post 392550)
Hello,

you have a Courant number of 0 and a timestep of approximatly 0, perhaps this is the problem.

Can you change this? For example a maximal Courant number of 0.1?


regards
treima

Hallo treima,
I have put deltaT 0.005, deltaX 1e-4, and the velocity of the bubble 0.02m/s, therefore the Co is 1.
The mesh is like below:


The Mesh is like below:

michielm November 20, 2012 13:19

Quote:

Originally Posted by lorraineshe (Post 393244)
,
I have put deltaT 0.005, deltaX 1e-4, and the velocity of the bubble 0.02m/s, therefore the Co is 1.

No!! this is only the case if you assume that you have no spurious velocities and with interFoam I am fairly certain that you do have those. The fact that the bubble velocity is 0.02 m/s does not mean that the maximum velocity in your domain is 0.02 m/s as well.

Use
Code:

adjustTimeStep yes;
in your controlDict to make sure that you get a maximum Co of the value you specify as
Code:

maxCo 0.1
in the controlDict.

By the way: if you have all zeroGradient boundaries the location of your bubble in your mesh is most likely the problem. Because then you have a zeroGradient U and a zeroGradient P at the boundary where the bubble is sticking through. This is only possible if both U and P are constant so with P constant this means that U=0 which means that the bubble cannot move over there. However, it wants to move in the rest of the domain due to buoyancy. I suggest you start of the bubble in the middle of your domain instead of halfway sticking through a boundary and see if that fixes the issue


All times are GMT -4. The time now is 19:07.