[Phicau]

Dear colleagues,

Now that I have released OLAFOAM (https://sites.google.com/site/olafoamcfd/) I open this thread to inform about code changes, gather questions, comments, bug reports and mainly anything you can think about.

You can find a general wiki page, which will be growing day by day here:

http://openfoamwiki.net/index.php/Contrib/OLAFOAM

I look forward to having some feedback from you.

Best,

Pablo


~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~

As a first major commit, I have added support for compilation in OpenFOAM v3.0+ (I just learned that such a thing existed yesterday..) and most important, modified the moving boundary condition to be compiled and used with Foam-Extend.

[C4l4M1TY]

Clean build of OpenFOAM-3.0.1 from source on Fedora 23 Workstation (x86_64).

After a successful build both the OlaFOAM boundary conditions and solvers (using olaFoamOF300) compiled with no issues. Thanks Pablo!

Steven

[ms411]

Hello everybody,

I am new here and I need help. I want to simulate waves on a dike in 2D and in 3D. I took for the 2D simulation the baseWaveFlume Tutorial and for the 3D simulation the irreg45degTank. In both tutorials I created an oblique wall at the "Outlet" (now it is defined as a wall) so that the waves can be reflected or run up the dike. When I now simulate this case in my opinion, the wave should come from the left side (Inlet-wave generation) and it runs up the dike at the right side. But if I view the case in paraview from the first time step on the right side at the "Outlet" (defined as a wall) there develop velocities in different directions, although the wave is neither generated nor it reaches the dike yet.

In the initial conditions I simulated two different cases for pressure. One time I set the pressure conditions to "zeroGradient" and another time I set it to "fixedfluxpressure".

Below I attach you the pictures from start of the case to a few time steps later. After it I copied my data from the initial conditions and important .dicts of my constant folder.

Do you have a solution ? I hope so, thank you very, very much for an answer!

Best regards

ms411
t0.png

t1.png

t2.png

t3.png

t4.png
alpha.water.org :

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet
{
type waveAlpha;
waveDictName waveDict;
value uniform 0;
}
frontAndBack
{
type empty;
}
outlet
{
type zeroGradient;
}
bottom
{
type zeroGradient;
}
atmosphere
{
type inletOutlet;
inletValue uniform 0;
value uniform 0;
}
}


p_rgh:

FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p_rgh;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
frontAndBack
{
type empty;
}
outlet
{
type zeroGradient;
}
inlet
{
type zeroGradient;
}
bottom
{
type zeroGradient;
}
atmosphere
{
type totalPressure;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
p0 uniform 0;
value uniform 0;
}
}


U:

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 waveVelocity;
waveDictName waveDict;
value uniform (0 0 0);
}
outlet
{
type fixedValue;
value uniform (0 0 0);
}
bottom
{
type fixedValue;
value uniform (0 0 0);
}
atmosphere
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
}
frontAndBack
{
type empty;
}
}


BlockMeshDict:

FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}

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

convertToMeters 1;

vertices
(
(0.0 -0.02 0.0)
(10.0 -0.02 0.0)
(14.0 -0.02 0.7)
(0.0 -0.02 0.7)
(0.0 0.0 0.0)
(10.0 0.0 0.0)
(14.0 0.0 0.7)
(0.0 0.0 0.7)
);

blocks
(
hex (0 1 5 4 3 2 6 7) (500 1 70) simpleGrading (1 1 1)
);

edges
(
);

patches
(
patch inlet
(
(0 4 7 3)
)
wall outlet
(
(1 5 6 2)
)
wall bottom
(
(0 1 5 4)
)
patch atmosphere
(
(3 2 6 7)
)
empty frontAndBack
(
(0 1 2 3)
(4 5 6 7)
)
);

mergePatchPairs
(
);


boundary:

FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

5
(
inlet
{
type patch;
nFaces 70;
startFace 69430;
}
outlet
{
type wall;
inGroups 1(wall);
nFaces 70;
startFace 69500;
}
bottom
{
type wall;
inGroups 1(wall);
nFaces 500;
startFace 69570;
}
atmosphere
{
type patch;
nFaces 500;
startFace 70070;
}
frontAndBack
{
type empty;
inGroups 1(empty);
nFaces 70000;
startFace 70570;
}
)

[Phicau]

Hi Martin,

these results really look nonphysical. First, you should definitely use fixedFluxPressure as p_rgh BC. Second, based on the limited information I can only guess that you have a huge non-orthogonality error due to your approach to create the mesh. You can try either creating a second block with a slope attached to the first one, or a longer one and use snappy to carve the slope.

Best,

Pablo

[Phicau]

Dear all,

I have included support to generate and absorb waves and currents simultaneously in olaFoam.

For further details: https://sites.google.com/site/olafoa...urrentsarehere

Best,

Pablo

[ms411]

Hello Pablo,

thank you for you very, very quick answer. I didn't answer so quick, because I tried to solve the problem. In fact you are right that my results look very non-physical because of the mesh. In the cfd-forum I found a post, where is the same problem discussed, but this guy was simulating with waves2foam.
Nevertheless, I think it makes no difference if I will simulate with OlaFoam or Waves2Foam, because both tools are based on interfoam/MULES.

My plan was now to divide my mesh. For the rectangular I will mesh rectangulars and for the triangle with triangles mesh. For this I used gmsh and I created my mesh in a *.msh file.

Now I have new Problems.

1. Gmsh doesn't create walls, it only patches.
2. I can't setFields because there are no coordinates written in the mesh.
3. Does the wave.dict know that waves should be produced at the inlet?

Thanks for an answer!!

I really want to find out, if the model is physical with this Mesh.

So please, Pablo or anyone else, help me!!

Thank you very, very much in advance!!

Best regards

Martin

[Phicau]

Hi Martin,

you can use only rectangles, only triangles or a mix of both to generate this simple mesh. There are lots of options.

And remember that google is your friend:

https://openfoamwiki.net/index.php/2...ial_using_GMSH

Best,

Pablo

[ingbay86]

Hi All,
i have just installed successfully the OpenFoam version OpenFOAM-v3.0+ and tried to install OLAFOAM but i got the following error:
olaFoam.C:80:28: fatal error: fvIOoptionList.H: File o directory non esistente
compilation terminated.
Is it a matter of OF compatibility? could you give me a help?
Thanks
Ing.

[Phicau]

Hi ingbay86,

I have just pushed a new commit, adding the solver for OpenFOAM v3.0+. Please update the code and try to recompile:

git checkout
git pull

Best,

Pablo

[ms411]

Dear Pablo,
since a few weeks I am trying to simulate waves on a dike. I need your help. I read a lot of papers for similar cases. I think the boundary conditions are right and the mesh is the problem. I read in the cfd forum, that other people had the same problem, due to the orthogonality of the mesh. This was my first mesh with the following results: Picture 01 02
So I tried to create it with snappyHexMesh.There seems to be a problem with the inlet at first time step. So do you know where my fault could be? Picture 03 04

Do I have to change something in the fvschemes or in the fvsolution? I load the case in a dropbox. Would you be so nice and have a look on it, I really don't know what to do.
https://www.dropbox.com/s/68apuhz3yq..._case.zip?dl=0

Thank you very, very much and best regards.

Martin

[Phicau]

Hi Martin,

to work with olaFoam, gravity needs to act in the negative Z direction.

Best,

Pablo

[ce73stargazer]

Hi there

I experience an error saying

Reading g
Reading field porosityIndex

Floating point exception (core dumped)


when i trying to start the case, then the process terminated, anyone have any idea of why?

Thanks in advance

[Phicau]

Hi Zhifang,

with that amount of information I can only tell you that you are dividing by 0 somewhere.

http://www.cfd-online.com/Forums/ope...-get-help.html

Best,

Pablo

[ce73stargazer]

Originally Posted by Phicau

Hi Zhifang,

with that amount of information I can only tell you that you are dividing by 0 somewhere.

http://www.cfd-online.com/Forums/ope...-get-help.html

Best,

Pablo

Hi Pablo

Thanks for the reply and the link, thats really handy for checking

[ce73stargazer]

Hi there

I recently came across a question when i am using multiPistonMovement. After i finished doing all the preparation, blockMesh, setField etc and try to run the case it shows

/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.4.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 2.4.0-f0842aea0e77
Exec : olaDyMFoam
Date : May 24 2016
Time : 13:49:05
Host : "ubuntu14.04"
PID : 14994
Case : /home/zhifang/OpenFoamTests/OLAFOAM_Test/B203
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Create mesh for time = 0

Selecting dynamicFvMesh dynamicMotionSolverFvMesh
Selecting motion solver: displacementLaplacian
Selecting motion diffusion: inverseDistance

PIMPLE: Operating solver in PISO mode

Reading field porosityIndex

Porosity NOT activated

Reading field p_rgh

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

No finite volume options present

DICPCG: Solving for pcorr, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0, global = 0, cumulative = 0
Reading/calculating face velocity Uf

Courant Number mean: 0 max: 0

Starting time loop

Reading surface description:
topFreeSurface

Interface Courant Number mean: 0 max: 0
Courant Number mean: 0 max: 0
deltaT = 0.00119048
Time = 0.00119048

PIMPLE: iteration 1
Point displacement BC on patch inlet
Initial water depth Paddle_inlet = 0.24

--> FOAM FATAL IO ERROR:
wrong token type - expected Scalar, found on line 13327 the punctuation token ')'

file: /home/zhifang/OpenFoamTests/OLAFOAM_Test/B203/constant/multiPistonMovementDict.timeSeries at line 13327.

From function operator>>(Istream&, Scalar&)
in file lnInclude/Scalar.C at line 93.

I really dont understand why, the multiPistonMovementDict file looks perfectly fine to me. Any suggestions?

[ms411]

Originally Posted by Phicau

Hi Martin,

to work with olaFoam, gravity needs to act in the negative Z direction.

Best,

Pablo

Dear Pablo,

thank you for your support! It seems that there are waves running up on the dike. I have now another question, but I am not sure, if it is the right thread here. Now I want to calibrate the runup height on the dike by changing the roughness of the ground and of the dike surface. I postprocess with Paraview. Is there a possibility, how I can find out, how high my waves run up on the dike? Or can I act on the assumption, that OlaFoam simulates the right wave runup heights due to a realistic szenario?

Thank you again for your support!

Best regards

Martin

[Phicau]

Hi,

Zhifang, your dictionary file is not right. OpenFOAM looks for a scalar value and finds the end of the file. Check the number of elements on your time series.

Martin, CFD always need validation, you can never assume that the model performs well unless you prove so. There are a number of ways to obtain runup, I suggest that you take a look at the sampling utility in OpenFOAM.

Best,

Pablo

[ce73stargazer]

Hi Pablo

Thanks for the reply. I am pretty sure the time series have the same elements as the piston movements, thats why I am confused.

The attachment is the zip file of the multiPistonMovementDic, would u mind having a look at it?

Cheers
Zhifang

[Phicau]

Zhifang, your dictionary is not good at all and it is very easy to tell. You say that your time series has 13928 elements, yet your series starts at line 31 and ends at line 13328. Do the math.

Best,

Pablo

[handsomedog]

Hi, Pablo. I think the Olafoam can be used to simulate the longshore currents whatever in practical field and laboratory. But I did not find any publications or reports about this in recent days. Could you give me some suggestions how to use the Olafoam to calculate the 2D or 3D longshore currents ?
Best regards
Chunping