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

Tutorial Hemida for OF-1.6

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 28, 2010, 04:16
Default Tutorial Hemida for OF-1.6
  #1
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Hello,


I am currently trying the InterFoam tutorial, written by Hassan Hemida, which can be found at http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2007/. I think this tutorial has been written for an older version of interFoam. The laminar case was easily runned, but for the RAS case, I needed to change quite a lot of the files. The files I downloaded were written for reasInterFoam, while in OpenFOAM-1.6, RAS simulation is integrated in the normal interFoam solver.

The case I set up was more or less a mixture between the original files from Mr. Hemida and the RAS damBreak tutorial.

When running the case, I received time step continuity errors in the first time step. My log file looks like this:


Create time

Create mesh for time = 0


Reading g
Reading field p

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 RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}

time step continuity errors : sum local = 9.77995e-06, global = -9.77995e-06, cumulative = -9.77995e-06
DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 7.62511e-09, No Iterations 178
DICPCG: Solving for pcorr, Initial residual = 4.89025e-10, Final residual = 4.89025e-10, No Iterations 0
time step continuity errors : sum local = 7.45727e-14, global = -9.41208e-16, cumulative = -9.77995e-06
Courant Number mean: 0.000122101 max: 0.0277845

Starting time loop

Courant Number mean: 0.000878914 max: 0.2
deltaT = 0.000719825
Time = 0.000719825

MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220225 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220401 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220577 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220753 Min(alpha1) = 0 Max(alpha1) = 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00876324, No Iterations 94
DICPCG: Solving for p, Initial residual = 3.10228e-06, Final residual = 2.79213e-08, No Iterations 40
DICPCG: Solving for p, Initial residual = 0.000594512, Final residual = 5.7006e-06, No Iterations 92
DICPCG: Solving for p, Initial residual = 3.78488e-05, Final residual = 3.60187e-07, No Iterations 42
DICPCG: Solving for p, Initial residual = 0.00218362, Final residual = 1.99928e-05, No Iterations 86
DICPCG: Solving for p, Initial residual = 3.32376e-05, Final residual = 3.11412e-07, No Iterations 37
DICPCG: Solving for p, Initial residual = 0.00169515, Final residual = 1.46306e-05, No Iterations 82
DICPCG: Solving for p, Initial residual = 1.52903e-05, Final residual = 9.49297e-08, No Iterations 84
time step continuity errors : sum local = 2.1649e-09, global = 9.53018e-12, cumulative = -9.77994e-06



Can anyone help? (I am am not sure that I really understand what a time step continuity error means)
flowris is offline   Reply With Quote

Old   April 28, 2010, 07:07
Default
  #2
New Member
 
John.B
Join Date: Mar 2009
Posts: 14
Rep Power: 8
johnb is on a distinguished road
Hi,

You will always see "time step continuity errors" during your simulations, ideally it should be zero. So as long as it it is small and not increasing during simulation everything is fine.

If it explodes you have either specified incorrect BC or your mesh quality might be poor.

Regards,
John
johnb is offline   Reply With Quote

Old   April 29, 2010, 03:41
Default complete log file
  #3
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Thank you. I didn't give the complete log file, but it shows some more errors:

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.6 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 1.6-f802ff2d6c5a
Exec : interFoam
Date : Apr 29 2010
Time : 09:32:01
Host : rmawsynab105478
PID : 3037
Case : /home/jmatthei/OpenFOAM/jmatthei-1.6/run/tutorials_chalmers/turbFillBottleKEps_1
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).

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

Create mesh for time = 0


Reading g
Reading field p

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 RASModel
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
sigmaEps 1.3;
}

time step continuity errors : sum local = 9.77995e-06, global = -9.77995e-06, cumulative = -9.77995e-06
DICPCG: Solving for pcorr, Initial residual = 1, Final residual = 7.62511e-09, No Iterations 178
DICPCG: Solving for pcorr, Initial residual = 4.89025e-10, Final residual = 4.89025e-10, No Iterations 0
time step continuity errors : sum local = 7.45727e-14, global = -9.41208e-16, cumulative = -9.77995e-06
Courant Number mean: 0.000122101 max: 0.0277845

Starting time loop

Courant Number mean: 0.000878914 max: 0.2
deltaT = 0.000719825
Time = 0.000719825

MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220225 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220401 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220577 Min(alpha1) = 0 Max(alpha1) = 1
MULES: Solving for alpha1
Liquid phase volume fraction = 0.0220753 Min(alpha1) = 0 Max(alpha1) = 1
DICPCG: Solving for p, Initial residual = 1, Final residual = 0.00877667, No Iterations 94
DICPCG: Solving for p, Initial residual = 3.10704e-06, Final residual = 2.79188e-08, No Iterations 40
DICPCG: Solving for p, Initial residual = 0.000594512, Final residual = 5.62055e-06, No Iterations 92
DICPCG: Solving for p, Initial residual = 3.73173e-05, Final residual = 3.68162e-07, No Iterations 42
DICPCG: Solving for p, Initial residual = 0.00218363, Final residual = 1.99515e-05, No Iterations 86
DICPCG: Solving for p, Initial residual = 3.3169e-05, Final residual = 3.11278e-07, No Iterations 37
DICPCG: Solving for p, Initial residual = 0.00169515, Final residual = 1.46307e-05, No Iterations 82
DICPCG: Solving for p, Initial residual = 1.52904e-05, Final residual = 9.53714e-08, No Iterations 84
time step continuity errors : sum local = 2.17497e-09, global = 9.60109e-12, cumulative = -9.77994e-06
#0 Foam::error:rintStack(Foam::Ostream&) in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#2 ?? in "/lib/libc.so.6"
#3 Foam::divide(Foam::Field<double>&, Foam::UList<double> const&, Foam::UList<double> const&) in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libOpenFOAM.so"
#4 void Foam::divide<Foam::fvPatchField, Foam::volMesh>(Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh>&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleTransportModels.so"
#5 Foam::tmp<Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> > Foam:perator/<Foam::fvPatchField, Foam::volMesh>(Foam::tmp<Foam::GeometricField<doub le, Foam::fvPatchField, Foam::volMesh> > const&, Foam::GeometricField<double, Foam::fvPatchField, Foam::volMesh> const&) in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#6 Foam::incompressible::RASModels::kEpsilon::correct () in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/lib/linux64GccDPOpt/libincompressibleRASModels.so"
#7 main in "/home/jmatthei/OpenFOAM/OpenFOAM-1.6/applications/bin/linux64GccDPOpt/interFoam"
#8 __libc_start_main in "/lib/libc.so.6"
#9 _start at /usr/src/packages/BUILD/glibc-2.9/csu/../sysdeps/x86_64/elf/start.S:116
Floating point exception
flowris is offline   Reply With Quote

Old   April 29, 2010, 04:49
Default
  #4
Senior Member
 
su_junwei's Avatar
 
su junwei
Join Date: Mar 2009
Location: Xi'an China
Posts: 151
Rep Power: 10
su_junwei is on a distinguished road
Send a message via MSN to su_junwei
Hi

It seems that you have set a zero value for k or epsilon on a certain boundary. Please try using a very small value instead.

Junwei
su_junwei is offline   Reply With Quote

Old   May 3, 2010, 05:19
Default small values for k and epsilon -> ok
  #5
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Thanks Junwei,

I had values of 0.1 for k and epsilon in the internal field of timestep 0, but values zero on some of the boundaries. When I changed to values of 0.1 everywhere in timestep zero, my tutorial ran fine.
flowris is offline   Reply With Quote

Old   May 28, 2010, 13:21
Default
  #6
New Member
 
rlobosco
Join Date: Nov 2009
Posts: 5
Rep Power: 7
rlobosco is on a distinguished road
I followed step by step of interFoam tutorial by Hassan Hemida. And applied exactly the same conditions to the geometry of a stepped spillway. But unreal oscillations appear at the interface, even more when I increase the length of the dam, as showed in the second picture attached. I realised that oscilations start from upper right coordenate of the box for defining alpha equal 1.
Can anyone give me a hint how to avoid this interface problem?
Someone tested this dambreak problem in 3D with geometry topology changes? The flow is also going from down the crest, it would stop to flow earlier.
Thanks for help.
With best regard,
Attached Images
File Type: png spillway1.png (2.3 KB, 30 views)
File Type: png spillway2.png (5.4 KB, 36 views)

Last edited by rlobosco; June 21, 2010 at 14:33.
rlobosco is offline   Reply With Quote

Old   May 11, 2012, 10:17
Default
  #7
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
Oscillations on the air-water interface are a common problem using interFoam. Mesh refinement and good fvSchemes are the key to improve. Find more info here:
Free Surface Ship Flow
flowris is offline   Reply With Quote

Old   August 21, 2013, 00:11
Default
  #8
Member
 
vishal
Join Date: Mar 2013
Posts: 54
Rep Power: 4
vishal_s is on a distinguished road
Hey flowris, I am also trying to simulate the InterFoam tutorial, written by Hassan Hemida, I have used the boundary conditions given below but unable to reproduce the same result as given in the tutorial for the laminar case (doing laminar case first). May you kindly look at the initial boundary conditions and let me know whether it is fine or not.

For U:

/*--------------------------------*- 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 volVectorField;
location "0";
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type fixedValue;
value uniform (0 -0.1 0);
}
inletWall
{
type fixedValue;
value uniform (0 0 0);
}
bottleWall
{
type fixedValue;
value uniform (0 0 0);
}
atmosphere
{
type inletOutlet;
inletValue uniform (0 0 0);
value uniform (0 0 0);
}
frontAndBack
{
type empty;
}
}


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

For P_rgh

/*--------------------------------*- 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 volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
inlet
{
type zeroGradient;

}
inletWall
{
type zeroGradient;
}
bottleWall
{
type zeroGradient;

}

atmosphere
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
value uniform 0;
}

frontAndBack
{
type empty;
}
}

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

For alpha1

/*--------------------------------*- 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 volScalarField;
location "0";
object alpha1;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet
{
type fixedValue;
value uniform 1;
}
inletWall
{
type zeroGradient;
}
bottleWall
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
frontAndBack
{
type empty;
}
}


// ************************************************** *********************** //
vishal_s is offline   Reply With Quote

Old   August 21, 2013, 02:35
Default
  #9
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
In comparison to the original case of Hamida, there are no differences in 0/U.

However, 0/pd and 0/gamma.org are:

Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4.1                                 |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

// Field Dictionary

FoamFile
{
    version         2.0;
    format          ascii;

    root            "/home/hassan/OpenFOAM/hassan-1.4.1/run/interFoam";
    case            "fillBottle";
    instance        "0";
    local           "";

    class           volScalarField;
    object          pd;
}

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


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

internalField   uniform 0;

boundaryField
{
    inlet           
    {
        type            zeroGradient;
    }

    inletWall       
    {
        type            zeroGradient;
    }

    bottleWall      
    {
        type            zeroGradient;
    }

    atmosphere      
    {
        type            fixedValue;
        value           uniform 0;
    }

    frontAndBack    
    {
        type            empty;
    }
}


// ************************************************************************* //
Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.4                                   |
|   \\  /    A nd           | Web:      http://www.openfoam.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/

FoamFile
{
    version         2.0;
    format          ascii;

    root            "";
    case            "";
    instance        "";
    local           "";

    class           volScalarField;
    object          gamma;
}

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


dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    inlet        
    {
        type            zeroGradient;
    }

    inletWall       
    {
        type            zeroGradient;
    }

    bottleWall       
    {
        type            zeroGradient;
    }

    atmosphere      
    {
        type            inletOutlet;
        inletValue      uniform 0;
        value           uniform 0;
    }

    defaultFaces    
    {
        type            empty;
    }
}


// ************************************************************************* //
you can still download the files here: http://www.tfd.chalmers.se/~hani/kurser/OS_CFD_2007/
flowris is offline   Reply With Quote

Old   August 21, 2013, 06:19
Default
  #10
Member
 
vishal
Join Date: Mar 2013
Posts: 54
Rep Power: 4
vishal_s is on a distinguished road
flowris, thanks for the prompt reply.But why in the initial dynamic pressure field , the boundary condition for the atmosphere field is kept "fixed zero".Don't you think as the as the water
starts entering the atmosphere, the dynamics pressure is going to have some finite value??
vishal_s is offline   Reply With Quote

Old   August 21, 2013, 06:33
Default
  #11
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 7
flowris is on a distinguished road
That is totally reasonable. If I remember well, the tutorial case ends before the bottle is completely filled. All I did was giving you the BCs of the original tutorial, I am not saying they are the most physically correct ones. Did you try it with these?
flowris is offline   Reply With Quote

Old   August 26, 2013, 15:07
Default
  #12
Member
 
vishal
Join Date: Mar 2013
Posts: 54
Rep Power: 4
vishal_s is on a distinguished road
Flowris,I tried both BCs and it doesn't makes much difference. I would be really grateful, if you may kindly look at the initial boundary conditions for turbulence, I am trying for last few days but unable to get the proper result.May you kindly tell what is the mistake.

File for epsilon :

/*--------------------------------*- 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 volScalarField;
location "0";
object epsilon;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0.1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0.1;
}
inletWall
{
type epsilonWallFunction;
value uniform 0.1;
}
bottleWall
{
type epsilonWallFunction;
value uniform 0.1;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
frontAndBack
{
type empty;
}
}


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

FIle for k :

/*--------------------------------*- 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 volScalarField;
location "0";
object k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0.1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0.1;

}
inletWall
{
type kqRWallFunction;
value uniform 0.1;
}
bottleWall
{
type kqRWallFunction;
value uniform 0.1;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0.1;
value uniform 0.1;
}
frontAndBack
{
type empty;
}
}


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

FIle for nut :

/*--------------------------------*- 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 volScalarField;
location "0";
object nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0.1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0.1;
}
inletWall
{
type nutkWallFunction;
value uniform 0.1;
}
bottleWall
{
type nutkWallFunction;
value uniform 0.1;
}
atmosphere
{
type calculated;
value uniform 0;
}
defaultFaces
{
type empty;
}
}


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

File for nuTilda:

/*--------------------------------*- 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 volScalarField;
object nuTilda;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0.1;

boundaryField
{
inlet
{
type fixedValue;
value uniform 0;
}

inletWall
{
type fixedValue;
value uniform 0;
}

bottleWall
{
type fixedValue;
value uniform 0;
}

atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}

frontAndBack
{
type empty;
}
}

// ************************************************** *********************** //
vishal_s is offline   Reply With Quote

Reply

Tags
continuity error, hemida, interfoam

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
Problem on Fluent Tutorial: Horizontal Film Boilig Feng FLUENT 2 April 13, 2013 05:34
k-omega-SST model (OF 1.6) - turbulent flat plate cboss OpenFOAM Running, Solving & CFD 23 November 13, 2011 02:28
TwoPhaseEulerFoam bed tutorial case crashes in 1.6. Stable in 1.5 hemph OpenFOAM Bugs 2 February 17, 2010 09:10
TwoPhaseEulerFoam bed tutorial case stable in 1.5, crashes in 1.6 hemph OpenFOAM 3 December 5, 2009 05:19
Install of OpenFOAM 1.6 Error 1 Error 2 & run tutorial potac OpenFOAM Installation 3 August 27, 2009 09:04


All times are GMT -4. The time now is 23:45.