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 Tree12Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   June 7, 2010, 04:31
Default
  #61
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 6
flowris is on a distinguished road
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?
flowris is offline   Reply With Quote

Old   June 7, 2010, 06:14
Default
  #62
New Member
 
yannH
Join Date: Feb 2010
Posts: 26
Rep Power: 6
yannH is on a distinguished road
Hi Gonzalo and flowris

thanks for reply,

Quote:
Originally Posted by g.redondo View Post
Try to use a volumetric control at the free surface so you have more cells in there
A volumetric control? I guess you mean to use simple grading . I'm looking for doing that

Quote:
Originally Posted by flowris View Post
Which boundary conditions do you use on the other boundaries?
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
yannH is offline   Reply With Quote

Old   June 9, 2010, 17:15
Default
  #63
New Member
 
Chris Blake
Join Date: Jun 2010
Posts: 10
Rep Power: 6
c_blake is on a distinguished road
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).
c_blake is offline   Reply With Quote

Old   June 10, 2010, 07:55
Default
  #64
Senior Member
 
stephane sanchi
Join Date: Mar 2009
Posts: 299
Rep Power: 8
openfoam_user is on a distinguished road
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.
openfoam_user is offline   Reply With Quote

Old   June 13, 2010, 17:18
Default
  #65
New Member
 
Chris Blake
Join Date: Jun 2010
Posts: 10
Rep Power: 6
c_blake is on a distinguished road
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.
c_blake is offline   Reply With Quote

Old   July 7, 2010, 08:49
Default
  #66
Senior Member
 
Join Date: Apr 2010
Posts: 151
Rep Power: 6
flowris is on a distinguished road
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?
flowris is offline   Reply With Quote

Old   August 10, 2010, 12:12
Default wigley on OF 170
  #67
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
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

Last edited by nuovodna; August 30, 2010 at 06:12. Reason: question change
nuovodna is offline   Reply With Quote

Old   September 8, 2010, 06:52
Default
  #68
Senior Member
 
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 9
colinB is on a distinguished road
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:

Code:
Create time

Create mesh for time = 0

Reading field p_rgh



--> FOAM FATAL IO ERROR: 
cannot open file

file: /root/OpenFOAM/root-1.7.1/run/tutorials/multiphase/interFoam/wigley/0/p_rgh at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 61.

FOAM exiting
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
colinB is offline   Reply With Quote

Old   September 8, 2010, 07:08
Default wigley on OF 170
  #69
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
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)
nuovodna is offline   Reply With Quote

Old   September 8, 2010, 08:19
Default
  #70
Senior Member
 
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 9
colinB is on a distinguished road
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

Last edited by colinB; September 8, 2010 at 09:27. Reason: Update
colinB is offline   Reply With Quote

Old   September 8, 2010, 09:27
Default
  #71
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
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)
nuovodna is offline   Reply With Quote

Old   September 8, 2010, 09:46
Default
  #72
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 8
egp is on a distinguished road
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
egp is offline   Reply With Quote

Old   September 8, 2010, 11:02
Default
  #73
Senior Member
 
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 9
colinB is on a distinguished road
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
colinB is offline   Reply With Quote

Old   September 10, 2010, 06:52
Default wigley on OF 17x and 1.5-dev
  #74
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
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 Forces in OF15 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
Attached Images
File Type: png wigleyFr0_316_17x.png (5.2 KB, 103 views)

Last edited by nuovodna; September 10, 2010 at 12:00. Reason: link corrected
nuovodna is offline   Reply With Quote

Old   September 10, 2010, 11:10
Default
  #75
Senior Member
 
Join Date: Aug 2010
Location: Groningen, The Netherlands
Posts: 216
Rep Power: 9
colinB is on a distinguished road
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.
colinB is offline   Reply With Quote

Old   September 10, 2010, 12:27
Default
  #76
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
Link corrected

http://www.shipmotions.nl/DUT/Papers...909-DUT-92.pdf
nuovodna is offline   Reply With Quote

Old   September 14, 2010, 06:12
Default Results 1.7.x / 1.5-dev wigley
  #77
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
These are the results of X / Y / Z forces over the prof Paterson's wigley mesh
Attached Images
File Type: png Wigley_finalX.png (6.9 KB, 101 views)
File Type: png Wigley_finalY.png (8.8 KB, 84 views)
File Type: png Wigley_finalZ.png (8.8 KB, 74 views)
nuovodna is offline   Reply With Quote

Old   October 6, 2010, 06:17
Default
  #78
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 6
Ralph M is on a distinguished road
Quote:
Originally Posted by nuovodna View Post
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 Forces in OF15 post #152

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

www.shipmotions.nl/DUT/PapersReports/0909-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
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
Ralph M is offline   Reply With Quote

Old   October 6, 2010, 11:43
Default cd computation
  #79
Senior Member
 
Emanuele
Join Date: Mar 2009
Posts: 110
Rep Power: 7
nuovodna is on a distinguished road
Hi Ralph, thanks for your reply. A question: what value of S do you put in C_d formula?? S= Lenght * Draft * 2?
nuovodna is offline   Reply With Quote

Old   October 6, 2010, 11:52
Default
  #80
Senior Member
 
Ralph Moolenaar
Join Date: Aug 2010
Location: 's-Hertogenbosch, the Netherlands
Posts: 120
Rep Power: 6
Ralph M is on a distinguished road
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
Ralph M 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 12:01
Free Surface Flow for Ship sam FLUENT 6 October 24, 2003 06:29
viscous free surface flow past a ship hull lololo Main CFD Forum 0 June 13, 2002 00:02
meshing for surface ship flow boris FLUENT 0 April 24, 2002 21:27


All times are GMT -4. The time now is 15:48.