Hi YahhH,


Did you split your domain in half? This is possible because I think you are working a symmetrical case, ans it will decrease computing time.

Which boundary conditions do you use on the other boundaries?

Hi Gonzalo and flowris

thanks for reply,

A volumetric control? I guess you mean to use simple grading . I'm looking for doing that

I take

inlet : buoyantPressure for p, zeroGradient for alpha1, groovyBc for U (fixedValue (-10 0 0) below water surface, (0 0 0) above)

outlet, lowerwall, frontAndBack : buoyantPressure for p, zerogradient for U and alpha1

atmosphere : totalPressure for p , pressureInletOutletVelocity for U, inletOulet for alpha1

You're right, for a first step, I'll try the half of the domain.

Regards,

Yann

I was just wondering if anyone had been able to achieve quantatatively accurate results for the wigley hull yet, especially for the pressure forces. At the moment my pressure forces are about 20% too large (Froude 0.316).

Hi Chris,

Maybe it could be nice to create a new thread called 'wigley hull' where to share experience about this particular test case.

Are you using the grid of Prof. Eric Paterson ?
Which OpenFoam version are you using ?

- grid used (of Eric Patreson, structured, unstructured, sHM, ...)
- advices to improve the grid
- which OpenFOAM version
- settings (files in 0 directory)
- fvSchemes file
- fvSolution file
- tools (and tricks) to post-process the solution

Best regards,

Stephane.

Hi,
I am using a mesh that is semi structured (using blockMesh) but then have also used snappyHexMesh utility to add boundary layer cells, but not refinement (so the mesh is still conformal). The mesh is around 1.3million cells. I have used bouyantPresure as the pressure boundary condition for the hull. I am using version 1.6 of OpenFOAM.

Hello all,


When I run the wigley case from Eric Paterson in OpenFOAM-1.5-dev, I get the following error:

keyword nu is undefined in dictionary "/home/jmatthei/OpenFOAM/jmatthei-1.5-dev/run/wigley/constant/transportProperties"

file: /home/jmatthei/OpenFOAM/jmatthei-1.5-dev/run/wigley/constant/transportProperties from line 29 to line 70.

From function dictionary::lookupEntry(const word& keyword) const
in file db/dictionary/dictionary.C at line 213.

FOAM exiting


However, when I make a simple blockMesh (the ship is now a bar) and use the same files, this error is no longer present. The keyword nu is indeed defined in constant/transportProperties, for both phases.


What is the problem?

wigley on OF 170
 

Hi, i tried to set up wigley case by Eric Paterson (thanks for sharing!!) with interFoam 1.7.1 (laminar and ras). Now i d like to compare my results with some experimental data. Where can i found them?

Thanks in advance

Hi

this morning I downloaded the wigleyship case from Eric Paterson and tried to run it under OF-1.7.1 with the icoFoam solver as recommended in the attached PDF.
Unfortunately it seems that the syntax has been changed in between and so I got the following error message:

As previous in this thread suggested I replaced all pd's and gamma's by p's and alpha1's. I did this with the files in the 0 subdirectory as well as in the fvScheme file.
So actually I thought my problem was solved, but it just shortened the list of failures.
And for this last failure message I tried to find a file relating to this path but I couldn't find that either. Does anybody have any suggestions for solving this?
regards Colin

wigley on OF 170
 

Hi Colin. I tried wigley by Eric Paterson on OF 171 with interFoam (icoFoam is a single phase solver). You can download the case that i setted up for OF 171:

http://db.tt/OoAhgCi


The main changes are on p_rgh (zeroGradient -> buoyantPressure) and on nut/nuTilda/k/epsilon (zeroGradient -> specific wall functions on the hull patch)

Hi
thanks for your fast reply.
First I have to mention a typo of course I was talking about interFoam not icoFoam so exactly what you did was my intention.
Actually I thought I figured out what was wrong, I thought that the p_rgh the nut and the nuTilda files were missing, however that didn't fix it.

So I'm a little bit confused.
I'm assuming that I just have to type interFoam once I'm in the case directory you send me and that I nothing else have to execute, like blockMesh or what ever.

Edit: I hope I'm not wrong but I first run now setFields what resulted in an other error message and so I updated all the data in the setFieldsDict changing any gamma to alpha1 that fixed at least the setFields errors but I still cannot run interFoam, I have still the same error-message

Edit 2: Its running now. Failure was, beside some gammas instead of alpha1's, that as initial Timestep in the controlDict file there was a 30 and not a 0 and therefore the solver was constantly looking for the p_rgh file in the folder 30 and not 0.
However I go and get now some coffee and let the computer do his work ;)

take a look in system/controlDict file... change startTime to 0 ( i forgot to change the value) then type interFoam and it should run. setFields is not required (alpha1 have been previously set on the entire domain)

I haven't been following this discussion much over the past several months due to workload. However, after the Overset Symposium later this month, I should have some time to fix the Wigley hull test case for 1.7.x.

Actually, I think it would be useful to collect a number of meshes and start building a repository for the Ship Hydro SIG over on the Extend Portal (http://www.extend-project.de/)

Eric

Dear Eric
actually that is exactly what I planed (apart form the repository for SH SIG, but that can be arranged). Currently I'm trying to get a running system for ship hydrodynamic calculation and then test it on different cases.
If you have any hints for me I would appreciate them since I'm not an expert in OF nor in CFD.
regards Colin

wigley on OF 17x and 1.5-dev
 

I made some tests on 1.5-dev and 1.7.x using wigley hull provided by Prof. Paterson (L=1, B=0.1, D=0.0625). The results are quite similar (I changed the boundary conditions on p_rgh (was pd) and k/epsilon/nut/nuTilda adding wallfunction on 1.7.x). The computation of forces in 1.5-dev required a modification of forces.C code like illustrated in this thread http://www.cfd-online.com/Forums/ope...es-of15-8.html post #152

But my results are away from the experimental data taken from this pdf :

http://www.shipmotions.nl/DUT/Papers...909-DUT-92.pdf (wigley III model)

My value of total drag forces on half hull is : 0,25 (pressure:0.062 viscous: 0.188) at Fr=0.316.
The drag coefficient results 8 * 10^-3 (2*F/0.5*rho*S*U^2) [note: the number "2" in front of F is necessary because the mesh includes half hull). I assume S is L*D*2 that is same order of the wetted surface.

Using the data provided with the previous pdf (L=3, B=0.3, D=0.1875, Resistence Force=9.97, Fr=0.3) i obtain a drag coefficient of 2.5*10^-3

This is the graph of forces obtained with 1.7.x.

I guess that viscous forces are overestimated. The pressure Force calculated in openFoam is close to the total Force given in the pdf. Certainly the Reynolds Number is different (L=1 and L=3) but I don't expect that it can explain a discrepancy like that.

These are the files of 1.7.x simulation

http://db.tt/7pVKy6R

short note: could it be that the delft link is only for people who are at TU Delft?
For I couldn't enter the page and reducing the link to (...).nl/live tells me I don't have permission to go on this page.

Link corrected

http://www.shipmotions.nl/DUT/Papers...909-DUT-92.pdf

Results 1.7.x / 1.5-dev wigley
 

These are the results of X / Y / Z forces over the prof Paterson's wigley mesh

I started a few days ago with OF and did also the Wigley case. My results from OF are more or less the same as yours but I'm afraid that you made a mistake with calculating the drag coefficient from the towing tank? I get a result of 6.69*10^-3 with your method.

This is still not the same as the results from OF but there is a significant speed difference between the two cases (1m/s vs 1.63m/s) which increases the pressure resistance.

Regards,

Ralph

cd computation
 

Hi Ralph, thanks for your reply. A question: what value of S do you put in C_d formula?? S= Lenght * Draft * 2?

Yes, I used your method.

with a resistance of 9.97N, rho=1000, Vinf=1.6275m/s, L=3.0, T=0.1875 I get:

Cd=9.97/(0.5*1000*1.6275^2*(3*0.1875*2)=6.69*10^-3 for a Froude speed of 0.30

Cheers,

Ralph