[ashim]

Hi Jianxi Yao,

Thank you very much for your response. I have attached the link of case files here. Please check it and let me know your advice. I appreciate your kind help.

https://www.dropbox.com/s/e83368jwb3nz7f6/wigley.zip

Best regards,

Ali

[jianxiyao]

Originally Posted by ashim

Hi Jianxi Yao,

Thank you very much for your response. I have attached the link of case files here. Please check it and let me know your advice. I appreciate your kind help.

https://www.dropbox.com/s/e83368jwb3nz7f6/wigley.zip

Best regards,

Ali

Hello Ali,

I found some tutorials on the 7th OF workshop. See below:

http://www.openfoamworkshop.org/2012/OFW7.html

Please see the title named Marine Hydrodynamics by E. Patterson. You could download some useful materials via the link. My settings are very similar with E. Patterson.

If you still feel unhelpful. I can send you my case files later (not now).

Good luck.

Jianxi Yao

[ashim]

Hi Jianxi Yao,

Good morning. I have tried several settings in fvschemes and fvsolutions including Prof. E. Patterson settings to calculate the resistance using InterDyMFoam. But the results are not satisfactory still now. please note that, I did not add any boundary layer or free surface mesh, just mesh around the hull only. I have spent a lot of time,but no outcome. I am little bit puzzled now. I appreciate any kind of help.

Thank you

Ali

[jianxiyao]

Originally Posted by ashim

Hi Jianxi Yao,

Good morning. I have tried several settings in fvschemes and fvsolutions including Prof. E. Patterson settings to calculate the resistance using InterDyMFoam. But the results are not satisfactory still now. please note that, I did not add any boundary layer or free surface mesh, just mesh around the hull only. I have spent a lot of time,but no outcome. I am little bit puzzled now. I appreciate any kind of help.

Thank you

Ali

I am so sorry to reply you so late.
My settings in fvschemes and fvsolutions are

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
default Euler;
}

gradSchemes
{
default Gauss linear;
limitedGrad cellLimited Gauss linear 1;
}

divSchemes
{
div(rhoPhi,U) Gauss linearUpwindV grad(U);
div(phi,alpha) Gauss vanLeer;
div(phirb,alpha) Gauss interfaceCompression;
div(phi,k) Gauss upwind; //Gauss linearUpwind limitedGrad;
div(phi,omega) Gauss upwind; //Gauss linearUpwind limitedGrad;
div((muEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
default Gauss linear corrected;
}

interpolationSchemes
{
default linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p_rgh;
pcorr;
alpha.water;
}

and

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{
"alpha.water.*"
{
nAlphaCorr 1;
nAlphaSubCycles 2;
cAlpha 1;
icAlpha 0;

alphaOuterCorrectors yes;

MULESCorr yes;
nLimiterIter 100;
alphaApplyPrevCorr yes;

solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-10;
relTol 0;
minIter 1;
}

"pcorr.*"
{
solver PCG;
preconditioner
{
preconditioner GAMG;
tolerance 1e-05;
relTol 0;
smoother DICGaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nBottomSweeps 2;
cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
}
tolerance 1e-10;
relTol 0;
maxIter 100;
};

p_rgh
{
solver GAMG;
tolerance 1e-08;
relTol 0.01;
smoother DIC;
nPreSweeps 0;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
}

p_rghFinal
{
solver PCG;
preconditioner
{
preconditioner GAMG;
tolerance 2e-09;
relTol 0;
nVcycles 2;
smoother DICGaussSeidel;
nPreSweeps 2;
nPostSweeps 2;
nFinestSweeps 2;
cacheAgglomeration true;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
}
tolerance 2e-09;
relTol 0;
maxIter 20;
}

"(U|k|omega).*"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0;
minIter 1;
}

"cellDisplacement.*"
{
solver smoothSolver;
smoother symGaussSeidel;
nSweeps 1;
tolerance 1e-8;
relTol 0;
minIter 1;
}
}

PIMPLE
{
momentumPredictor yes;

nOuterCorrectors 1;
nCorrectors 3;
nNonOrthogonalCorrectors 0;

correctPhi yes;
moveMeshOuterCorrectors yes;
turbOnFinalIterOnly yes;
}

relaxationFactors
{
fields
{
}
equations
{
".*" 1;
}
}

cache
{
grad(U);
}


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

I hope it is helpful.

[ashim]

Dear Jianxi Yao,

Thank you so much. I will run the simulation using your settings. Do you have any suggestion about meshing? I have generated mesh using pointwise (with boundary layer) and snappyHexMesh (without boundary). I have found that Prof. E Patterson's mesh was generated using pointwise.

Thank you again for your kind help,

Ali

[fondexx]

hi partners

I'm trying to make a CFD analysis of the KCS hull using interFoam, but I can't find the convergence and when I see the results on paraFoam I can see some interference or something, can you help me?

[CFD-Palma]

Dear All,

I have simulated a fast planing boat some time ago, and as I remember, the problem with interFoam (or interDyMFoam if you use dofs for the hull) was the shock of the sudden speed acting on the hull and the waves generated reflecting on the sides and end of the domain.

• The solution to the first problem was to put a strong dumping on the dof.

• For the second problem the solution was waveDymFoam, that has an absorption boundary that avoids reflections, allowing much smaller domains and therefore better refinement. (refinement, specially layers, should improve the force measurement)

waveDyMFoam is part of waves2Foam that you can find at: http://openfoamwiki.net/index.php/Co...d_Installation

Regards,
Carlos.

[cfdnew]

Hi Carlos

I am new to OpenFoam and I am trying to simulate free surface flow around ship hull with trim and sinkage. I have been able to compile waveDyMFoam and it works well for a small floating block in 2d as given in the video below,

https://www.youtube.com/watch?featur...&v=YKbj_7JMRl8

But when I try to simulate ship motions, it doesn't converge. It diverges in a few time steps. Please help to find the cause.

How to add dumping on a dof? Could you please give a reference.

Regards,

KM

Originally Posted by CFD-Palma

Dear All,

I have simulated a fast planing boat some time ago, and as I remember, the problem with interFoam (or interDyMFoam if you use dofs for the hull) was the shock of the sudden speed acting on the hull and the waves generated reflecting on the sides and end of the domain.

• The solution to the first problem was to put a strong dumping on the dof.

• For the second problem the solution was waveDymFoam, that has an absorption boundary that avoids reflections, allowing much smaller domains and therefore better refinement. (refinement, specially layers, should improve the force measurement)

waveDyMFoam is part of waves2Foam that you can find at: http://openfoamwiki.net/index.php/Co...d_Installation

Regards,
Carlos.

[CFD-Palma]

Hi KM,

Is a long time I am not working on this, but I attach the pointDisplacement file I was using.
My believe is that damping has no influence on the steady state but it helps to rich it.
Keep in mind that I was not imposing any waves nor studing the motion. I just wanted to get the trim and sinkage. Therefore, springs will affect the result but not dumping.
If you are using waves or studding the motion, this approach would not be correct.
Hoppe it helps.
Good luck and good results.
Regards,
Carlos.

[CFD-Palma]

Hi KM,

Is a long time I am not working on this, but I attach the pointDisplacement file I was using.
My believe is that damping has no influence on the steady state but it helps to rich it.
Keep in mind that I was not imposing any waves nor studding the motion. I just wanted to get the trim and sinkage. Therefore, springs will affect the result but not dumping.
If you are using waves or studding the motion, this approach would not be correct.
Hoppe it helps.
Good luck and good results.
Regards,
Carlos.

PD: Added waveProperties

[cfdnew]

Hi Carlos

Thank you for your response. I tried adding the two files in my simulation. But the solution still diverges. I have uploaded the files here http://www.mediafire.com/download/cs...1qv/wigley.zip .

If you can help.

With warm regards,

KM

[CFD-Palma]

Hi KM,

1. I had a look to your case and found that apparently the mass is not correct for the dimensions. If I am not wrong, your boat is about 40mx10mx3m approximately. with this dimensions your mass rho*volume should be at least 10 times bigger.
2. You apply the vertical spring 8 m aft of the G. I do not know the reason, but to avoid moments should be in the vertical of the G.
3. The RelaxationZone is only on the inlet and should be on outlet as well. The extension of the RZ should be reduced in the x direction, for example from 40-80 to 60-80.
4. Your domain appears to be a bit small and that produces strange results on the pressures.
5. Apparently you are running on single processor, it may take a day to finish if you succeed.

I have tried a run but it blows up after a wile, and is interesting that when that happens the boat a way above the water. My guess is that there is something wrong with the meshing or some other problem I do not see. I have to point out that my experience is very limited and you should go for the advice of an experienced member.
I am sorry not to be of more help.
Keep on trying, finally you will get there.
Best regards and good inspiration,
Carlos.

[cfdnew]

Hi Carlos

Thanks for the reply and your comments. I was our of town so couldn't read it earlier.

Could you please help me to understand the RelaxationZone startX and endX definition. In my case flow is along x axis. Relaxationzone is starting from x = 40 and ends at x = 80. When we write, startX (40 -40 0) and endX (80 40 0) what does it defines? Are they the opposite corners of the rectangle?

I am still trying out simulations based on your comments. If someone else can also help me please.

Thanks

KM

[CFD-Palma]

Hi Kumar,

As you say, the coordinates are the points of a rectangular section volume where the relaxation is applied. (minX minY minZ) (maxX maxY maxZ)
After my previous reply, I noticed some omissions from my side:

• I did not apply any flow speed in 0/U, only in wave properties. Did not try your way, it may also work.
• The only function of the springs (in my case) was to apply dumping, so the spring constant should be very small (like e-3)to avoid affecting the position of the floating object and the rest position should not apply force.
• You must have the correct mass or the speed up or down may blow your simulation. Also the sea level (in wave properties) must be on your water line.
• The mesh is crucial. Start with a simple coarse mesh and once it works, refine it.
• Start at very low relative speeds, to avoid the high courant numbers.
• Read the old posts, we all have had the same problems in the beginning.

This is what comes to my mind now, if I remember something else I will let you know.
Regards,
Carlos.

[cfdnew]

Hi Carlos

Thanks a lot for the response again. I am now trying out first with a rectangular block instead of a ship shape. I have included your comments.

I have a question. What is Tsoft in the waveProperties dict file? When I keep it 0, the simulation seems to diverge. When I keep it 2, which I noticed in the some example file, I observe the water surface is no longer flat, there is a pulse shape formation near the inlet.

Regards,

KM

[CFD-Palma]

Hi Kumar,

I remember to have that issue with the Tsoft.
Unfortunately I do not recall why, but you will better ask in the waves2Foam forum.
I beleave it is a delay in the start of the wave, so when you use only current it can be 0, but if you apply waves is better to use something like 2 to avoid the first impact.
It is not clear to me in the example of the W2F file:
"
// Ramp time of 2 s // Foam::sin(2 * mathematicalConstant:i / (4.0 * Tsoft_) * Foam::min(Tsoft_, runTime.time().value() )) // and explicitly "1" for Tsoft = 0 Tsoft 2;
"
from:http://openfoamwiki.net/index.php/Contrib/waves2Foam
Regards,
Carlos.

[samy_20042004]

Hi all OpenFOAM users,

I am working on resistance calcualation of Wigley hull, very very repeated subject! I read all the posts here but I still have problem in forces results which are not suitable even for the OF222 Wigley tutorials without any changes, without motion !!! results for wave elevation have good agreement with experimental results but for forces are completely wrong for different Froude numbers!!! I try to use fvschemes and fvsolutions which Jianxiyao mentioned above but these files dosent work in OF222 and it also seems for moving case! If anyone have a suitable example or could help me to solve my problem I will be appreciate. If you need my files to check I will send it.

Regards,
Saman

[Sachin m]

Hi all,

I have run a drag force analysis of accustom hull using LTSInterFoam.
But after 12000 runs the free surface is seen above the ship hull. What could be the possible reason. Could it be because the solution is not yet stable. Should I run this for more number of iterations?

One more thing, I need to find the drag force on the hull. The function to write the force that I have asks for only one density value. How can that function give me the drag when it is a multiphase problem. There should be two values of density changing with the value of alpha1. Can anybody help me with this?

Below I am attaching few results:

1) The meshed hull with value of alpha1 shown. Blue region is air; red region is water.
2) Free surface after 100 iterations
3) free surface after 12000 iterations.

inlet is at left and outlet at the right

[jule]

Hi,
I would like to check that I am working under the right assumptions regarding the near wall treatment of my k-omega SST model.
I have applied the nutkRoughWallFunction to my hull patch so I expect the wall function to be used and I should not need to capture the laminar sublayer but instead can target the log law region with 30<y+<300?

Did I get it all wrong?

Also is the wall function “scalable”? Since my layer thicknesses are constant along the length of the model I am wondering what would happen if in one area of the model the first cell was contained within the laminar sublayer. Would the wall function recognise the transition to the composite region?

Thanks for your help!

[zandi]

Originally Posted by eddi

To my knowledge OpenFOAM doesn't include a surface following mesher (VOF with interface reconstruction) as would be necessary for efficient solution.

Or do you plan to use a phase fraction approach similar to the breaking dam example in the OpenFOAM manual? How would you balance the high/low mesh resolution close to the free surface and to the hull on the one hand side and in the distance on the oher hand side, all this while the free surface moves?

Eddi

Hi Eddi
OpenFOAM can do mesh adaption (tracking the moving surface) with dynamic mesh solvers such as interDyMFoam. in dynamicMeshDict the parameters would be difined and it is one of the capability of dynamic mesh of OpenFOAM. but as i know it just works for hexahedral meshes.
regards
Zandi