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

interFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 16, 2012, 10:44
Question interFoam
  #1
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
lorraineshe is on a distinguished road
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?
Attached Files
File Type: gz Blasendynamik.tar.gz (14.7 KB, 7 views)
lorraineshe is offline   Reply With Quote

Old   November 16, 2012, 11:05
Default
  #2
Member
 
Join Date: Mar 2012
Location: Munich, Germany
Posts: 67
Rep Power: 5
treima is on a distinguished road
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
treima is offline   Reply With Quote

Old   November 16, 2012, 15:51
Default
  #3
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Mol, Belgium
Posts: 295
Rep Power: 13
Lieven will become famous soon enough
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
Lieven is offline   Reply With Quote

Old   November 20, 2012, 13:27
Default Bubble rising, interFoam
  #4
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
lorraineshe is on a distinguished road
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 is offline   Reply With Quote

Old   November 20, 2012, 13:41
Default
  #5
New Member
 
Join Date: Nov 2012
Posts: 3
Rep Power: 4
lorraineshe is on a distinguished road
Quote:
Originally Posted by treima View Post
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:
Attached Images
File Type: png Pressure.png (11.8 KB, 21 views)

Last edited by lorraineshe; November 20, 2012 at 14:11.
lorraineshe is offline   Reply With Quote

Old   November 20, 2012, 14:19
Default
  #6
Member
 
Michiel
Join Date: Oct 2010
Location: Delft, Netherlands
Posts: 97
Rep Power: 6
michielm is on a distinguished road
Quote:
Originally Posted by lorraineshe View Post
,
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
michielm is offline   Reply With Quote

Reply

Tags
interfoam bubble

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
InterFoam stops after deltaT goes to 1e14 francesco_b OpenFOAM Running, Solving & CFD 8 July 31, 2013 02:29
BoF-Group: interFoam - documentation and usage unnikrsn OpenFOAM Running, Solving & CFD 0 November 12, 2011 23:39
Segmentation fault in interFoam run through openMPI voingiappone OpenFOAM 16 November 2, 2011 07:49
Slow interFoam compared with other CFD tools? Ralph M OpenFOAM Programming & Development 1 November 17, 2010 07:46
Open Channel Flow using InterFoam type solver sxhdhi OpenFOAM Running, Solving & CFD 3 May 5, 2009 21:58


All times are GMT -4. The time now is 16:06.