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

Free Surface Ship Flow

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

Like Tree14Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 18, 2014, 08:40
Default
  #261
New Member
 
Ali
Join Date: Oct 2013
Posts: 25
Rep Power: 3
ashim is on a distinguished road
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
ashim is offline   Reply With Quote

Old   June 18, 2014, 09:35
Default
  #262
New Member
 
Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 6
jianxiyao is on a distinguished road
Quote:
Originally Posted by ashim View Post
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
jianxiyao is offline   Reply With Quote

Old   July 3, 2014, 17:20
Default
  #263
New Member
 
Ali
Join Date: Oct 2013
Posts: 25
Rep Power: 3
ashim is on a distinguished road
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
ashim is offline   Reply With Quote

Old   July 9, 2014, 09:24
Default
  #264
New Member
 
Jianxi Yao
Join Date: Apr 2011
Posts: 15
Rep Power: 6
jianxiyao is on a distinguished road
Quote:
Originally Posted by ashim View Post
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.
jianxiyao is offline   Reply With Quote

Old   July 9, 2014, 10:56
Default
  #265
New Member
 
Ali
Join Date: Oct 2013
Posts: 25
Rep Power: 3
ashim is on a distinguished road
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
ashim is offline   Reply With Quote

Old   August 12, 2014, 09:55
Default CFD problems KCS
  #266
New Member
 
David Fuentes
Join Date: May 2014
Posts: 4
Rep Power: 3
fondexx is on a distinguished road
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?
Attached Images
File Type: jpg Screenshot from 2014-08-12 09:19:38.jpg (46.8 KB, 64 views)
File Type: jpg Screenshot from 2014-08-12 09:42:59.jpg (81.0 KB, 62 views)
File Type: jpg Screenshot from 2014-08-12 09:44:02.jpg (80.4 KB, 51 views)
Attached Files
File Type: gz KCS_interFoam.2.tar.gz (7.6 KB, 10 views)
fondexx is offline   Reply With Quote

Old   August 13, 2014, 05:46
Default waves2Foam
  #267
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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.
ngj likes this.
CFD-Palma is offline   Reply With Quote

Old   August 13, 2014, 07:27
Default adding dumping on a dof
  #268
New Member
 
Kumar
Join Date: Aug 2014
Posts: 4
Rep Power: 2
cfdnew is on a distinguished road
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

Quote:
Originally Posted by CFD-Palma View Post
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 is offline   Reply With Quote

Old   August 13, 2014, 10:17
Default
  #269
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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.
Attached Files
File Type: txt pointDisplacement.txt (3.3 KB, 25 views)
CFD-Palma is offline   Reply With Quote

Old   August 13, 2014, 10:26
Default
  #270
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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
Attached Files
File Type: txt waveProperties.txt (1.7 KB, 22 views)
File Type: txt pointDisplacement.txt (3.3 KB, 13 views)
CFD-Palma is offline   Reply With Quote

Old   August 14, 2014, 05:06
Post
  #271
New Member
 
Kumar
Join Date: Aug 2014
Posts: 4
Rep Power: 2
cfdnew is on a distinguished road
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
cfdnew is offline   Reply With Quote

Old   August 15, 2014, 15:09
Default
  #272
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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.
CFD-Palma is offline   Reply With Quote

Old   August 26, 2014, 00:30
Default
  #273
New Member
 
Kumar
Join Date: Aug 2014
Posts: 4
Rep Power: 2
cfdnew is on a distinguished road
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
cfdnew is offline   Reply With Quote

Old   August 26, 2014, 04:27
Default
  #274
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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 likes this.
CFD-Palma is offline   Reply With Quote

Old   August 27, 2014, 05:13
Default
  #275
New Member
 
Kumar
Join Date: Aug 2014
Posts: 4
Rep Power: 2
cfdnew is on a distinguished road
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
cfdnew is offline   Reply With Quote

Old   August 28, 2014, 07:04
Default
  #276
Member
 
carlos
Join Date: Apr 2011
Posts: 37
Rep Power: 6
CFD-Palma is on a distinguished road
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.
CFD-Palma is offline   Reply With Quote

Old   August 28, 2014, 11:23
Default
  #277
New Member
 
saman
Join Date: Apr 2012
Posts: 4
Rep Power: 5
samy_20042004 is on a distinguished road
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
samy_20042004 is offline   Reply With Quote

Old   September 1, 2014, 00:47
Default
  #278
Member
 
Sachin
Join Date: Aug 2014
Location: India
Posts: 45
Rep Power: 2
Sachin m is on a distinguished road
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
Attached Images
File Type: jpg starting stage.jpg (53.3 KB, 44 views)
File Type: jpg free surfaceat 100.jpg (40.9 KB, 48 views)
File Type: jpg freesurfaceat 12000.jpg (26.5 KB, 43 views)
Sachin m is offline   Reply With Quote

Old   September 2, 2014, 13:45
Default Near-wall treatment for a k-omega SST model
  #279
New Member
 
Join Date: Oct 2013
Posts: 6
Rep Power: 3
jule is on a distinguished road
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!

Last edited by jule; September 3, 2014 at 13:57.
jule is offline   Reply With Quote

Old   October 16, 2014, 02:15
Lightbulb
  #280
Senior Member
 
zandi's Avatar
 
Fatema Zandi Goharrizi
Join Date: Mar 2009
Posts: 131
Rep Power: 8
zandi is on a distinguished road
Quote:
Originally Posted by eddi View Post
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
zandi is offline   Reply With Quote

Reply

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
Free-Surface Ship Flow - Boundary Conditions James Date CFX 1 February 19, 2013 06:42
ship free-surface analysis Andrea Mercuri CD-adapco 0 September 28, 2004 11:01
Free Surface Flow for Ship sam FLUENT 6 October 24, 2003 05:29
viscous free surface flow past a ship hull lololo Main CFD Forum 0 June 12, 2002 23:02
meshing for surface ship flow boris FLUENT 0 April 24, 2002 20:27


All times are GMT -4. The time now is 06:27.