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

Open Foam for ship hydrodynamics

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   September 22, 2006, 06:50
Default Has anybody used OpenFoam to s
  #1
New Member
 
Alberto Fernandez
Join Date: Mar 2009
Posts: 2
Rep Power: 0
cognit is on a distinguished road
Has anybody used OpenFoam to study ship hidrodynamics? Would it be suitable/easy to do so? I mean, calculating free surface, drag, and so on as in a towing tank.
Thank you
cognit is offline   Reply With Quote

Old   September 22, 2006, 08:03
Default I have tried using the interFo
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
I have tried using the interFoam series of codes. At least I started trying before a more pressing project came along, and it seems to be doable. The main problem is wave transmissive/non-reflecting boundaries. Since the speed of the surface wave is dependent on its frequency and amplitude, its very difficult to build a filter to pass/remove these waves at the boundaries.

My workaround was to apply a spatially static viscosity ramp, basically freezing the waves before they hit the outlet boundary. I thik you could probably do something equivalent with an anisotropic porous media.

In addition, you will need a special outlet for pressure due to the numerics of the two-phase formulation. One of the components that make OpenFOAM VOF so robust is its use of a numerical interface compression term. Unfortunately, this same compresion term causes the pressure in the two fluids to vary sharply across the interface. If you add a fixed value pressure boundary to the mix, the result can be unpredictable (although this is not always the case). To get around this problem I used a boundary that applied fixed value pressure for the air-phase, but zeroGradient where there was water adjacent to the boundary.

If you are not scared off by the above contact me via e-mail, I might be able to help you out.
eugene is offline   Reply With Quote

Old   September 22, 2006, 08:19
Default If you are after a ensemble-av
  #3
Member
 
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 8
pierre is on a distinguished road
If you are after a ensemble-averaged approach, OpenFoam also provide reliable two-fluid codes that can be applied and modified for ship Hydrodyanmics.

Pierre
pierre is offline   Reply With Quote

Old   September 22, 2006, 09:50
Default Thank you for your quick respo
  #4
New Member
 
Alberto Fernandez
Join Date: Mar 2009
Posts: 2
Rep Power: 0
cognit is on a distinguished road
Thank you for your quick response.
I have never used OpenFoam. I have used other CFD codes and I got into them when doing part of my PhD work (parked some time ago for laboral reasons). I still collaborate with the university in testing and so on with the little spear time that I have.
I work on a naval design office and I trying to get back a little to CFD analysis. With the code that we use and helped develop (FEM based) we do get results but it dificult to have them reliable enough for consistent use in engineering.
I see that kind of analysis is somehow dificult with any kind of code. Comertial codes claim to solve it but in my experience not reliably enough.
With this I mean that I have seen some of the problems you mention.
I think I going to star looking into the documentation.
Also, how difficult is to create a mesh for this kind of problems that can have somehow complex boundaries?
Pierre, do you have any reference of an ensemble approach used for ship hydrodynamics?
Thank you again.
cognit is offline   Reply With Quote

Old   September 22, 2006, 10:39
Default Hi Alberto, Ref is: A polyd
  #5
Member
 
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 8
pierre is on a distinguished road
Hi Alberto,

Ref is: A polydisperse model for bubbly two-phase flow around a surface ship, International Journal of Multiphase Flow, Volume 25, Issue 2 , March 1999, Pages 257-305. P. M. Carrica, D. Drew, F. Bonetto and R. T. Lahey Jr.

Pierre
pierre is offline   Reply With Quote

Old   September 22, 2006, 11:09
Default Meshing isn't too difficult. Y
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Meshing isn't too difficult. You just have to make sure the submerged hull and any place the air-water interface goes is well resolved. Since the ship hull is generally quite smooth and the interface uses volume refinement, most commercial meshers will be able to this without a problem. The rest of the domain can be pretty coarse.

Btw, I spent a week looking at papers and theses of ocean wave/ship modelling and I can assure you there is no easy solution to the boundary problem.
eugene is offline   Reply With Quote

Old   November 6, 2006, 09:01
Default I am currently working on the
  #7
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
I am currently working on the following ship hydro benchmarks so that I can better understand OF

1. Wigley Hull
2. DTMB Model 5415
3. Suboff
4. Headform cavitation
5. Propeller flows

Has anyone already solved these benchmark problems? Which solvers did you use, or did you write a custom solver (e.g., steady-flow RANS surface capturing).

I am particularly interested in tracking vs. capturing capability for the free-surface problems, and will be studying this in the near future.

Eric Paterson
Penn State Univ
State College, PA USA
egp is offline   Reply With Quote

Old   January 12, 2007, 12:01
Default Hi Eric, I'm also really inter
  #8
clo
Member
 
clo
Join Date: Mar 2009
Posts: 36
Rep Power: 8
clo is on a distinguished road
Hi Eric, I'm also really interested in types of benchmark you refer. In particular, my final objectiv is to simulate a rotating machine as a marine propeller partially immersed in water. For the moment I'm really at the early stage learning OpenFoam and I'm learnig a simple two-phase flow case as the damBreak; then I would like to learn about moving mesh and finally put the 2 things together.
I don't know about your experience but do you think it's possible?

Thank you
ciao
clo is offline   Reply With Quote

Old   January 12, 2007, 17:16
Default Hello friends I looked at w
  #9
Senior Member
 
kumar
Join Date: Mar 2009
Posts: 112
Rep Power: 8
kumar2 is on a distinguished road
Hello friends

I looked at wave breaking over hydrofoils and compared with experimental work of Duncan ( very famous work , see jfm 1983.) excellent results from openfoam. ofcourse grid generation in openfoam using blockmesh is intended for simple geometry, propeller mesh would be hard with blockmesh. but the solver is excellent and we can read and modify all parts.

thanks

kumar
kumar2 is offline   Reply With Quote

Old   January 12, 2007, 17:49
Default Hi, I've been working with
  #10
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Hi,

I've been working with underwater and free surface hydrodynamics using FOAM and now OF since 1999 computing several benchmark cases including Wigley hulls, DTMB 5415, DARPA Suboffs etc using LES and VOF implementations. Most of the work is published or found in conference procedings. If you're interested please send me an email and I'll send copies of the papers.

Regards

/Eric
Sachin m likes this.
lillberg is online now   Reply With Quote

Old   January 22, 2007, 10:34
Default Hello Eric I am studing dr
  #11
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
Hello Eric

I am studing drag reduction using with microbubble injection in fluid.
So i want to model this case using LES implementation.
Do you have any experience in this field?
Or can you introduce me any references in this field?

Regards
Marhamat
marhamat is offline   Reply With Quote

Old   January 22, 2007, 10:54
Default Sorry, can't say I have. Very
  #12
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Sorry, can't say I have. Very interesting topic though, what kind of modelling did you have in mind for the bubbles?

Regards
Eric
lillberg is online now   Reply With Quote

Old   January 22, 2007, 18:04
Default I started my studing recently.
  #13
Senior Member
 
Marhamat Zeinali
Join Date: Mar 2009
Location: Tehran, Tehran, iran
Posts: 107
Rep Power: 8
marhamat is on a distinguished road
I started my studing recently.
So i didn't decide which model to use .
I inform you in near future.

Best regards
Marhamat
marhamat is offline   Reply With Quote

Old   January 22, 2007, 18:29
Default A thought: it seems there is a
  #14
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
A thought: it seems there is a few people interested in shpi hydrodynamics applications. If you are coming to Zagreb for the Workshop, it may be a good idea to add this as one of the topics. Any takers?

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 22, 2007, 19:58
Default Hi Hrv, I'm thinking of att
  #15
egp
Senior Member
 
egp's Avatar
 
Eric Paterson
Join Date: Mar 2009
Location: Blacksburg, VA
Posts: 197
Blog Entries: 1
Rep Power: 9
egp is on a distinguished road
Hi Hrv,

I'm thinking of attending the workshop, and would be very interested in a ship hydro session. If I we were further along, I would volunteer, but we are still novices. If you can get them to participate, I would nominate the group from Sweden (Alin, Fureby, Svennberg et al.) since they probably have the most experience using OpenFOAM in the ship hydro community.

Eric
egp is offline   Reply With Quote

Old   February 19, 2008, 21:30
Default hello Eric Lillberg I am ve
  #16
New Member
 
Miguel Quintero
Join Date: Mar 2009
Location: Honolulu, HI, USA
Posts: 4
Rep Power: 8
miguel_q is on a distinguished road
hello Eric Lillberg

I am very interested in the benchmark cases you mentioned above. Could you direct me in the right direction on where to find these papers/publications?

Miguel Q.
miguel_q is offline   Reply With Quote

Old   January 8, 2009, 16:34
Default I know this post is quiet abou
  #17
New Member
 
Francisco Blasco
Join Date: Mar 2009
Location: Santa Pola, Alicante, Spain
Posts: 1
Rep Power: 0
pacoblasco is on a distinguished road
I know this post is quiet about 1 year.

Does anybody have anything new on Ship Hydrodynamics using OpenFOAM??

I would like to know if somebody have any experience on it. I am very interested.

F. Blasco
pacoblasco is offline   Reply With Quote

Old   April 9, 2009, 09:23
Default
  #18
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 259
Blog Entries: 5
Rep Power: 11
tomislav_maric is on a distinguished road
I'm trying to simulate free surface flow around a ship using interFoam as a part of my semestral project. I've made libforces.so calculate forces and moments for water (phase1), at least I like to think so, but I keep getting floating point exception error and my gamma is turning negative during first time steps. checkMesh has gone through without warnings.
tomislav_maric is offline   Reply With Quote

Old   June 26, 2009, 02:51
Default
  #19
Member
 
Cem Albukrek
Join Date: Mar 2009
Posts: 50
Rep Power: 8
albcem is on a distinguished road
If your mesh is tetrahedral? Non-hex meshes tend to trigger instabilities in interFoam class solvers. I had had issues due to this a while back and could not refrain from banging my head against the wall as things looked perfectly fine with checkMesh. Thanks to Mark C., who pointed out hex meshes which you can produce with the snappyhexmesh utility is the way to go.

Cem
albcem is offline   Reply With Quote

Old   August 3, 2009, 09:30
Default
  #20
Senior Member
 
Tomislav Maric
Join Date: Mar 2009
Location: Darmstadt, Germany
Posts: 259
Blog Entries: 5
Rep Power: 11
tomislav_maric is on a distinguished road
Quote:
Originally Posted by albcem View Post
If your mesh is tetrahedral? Non-hex meshes tend to trigger instabilities in interFoam class solvers. I had had issues due to this a while back and could not refrain from banging my head against the wall as things looked perfectly fine with checkMesh. Thanks to Mark C., who pointed out hex meshes which you can produce with the snappyhexmesh utility is the way to go.

Cem
My current mesh is created with snappy and it's unstructured tetrahedral. Now I know that non orthogonality causes the gamma to become unbounded and that makes my runs explode.

Where can I find the tips on hex mesh for ships generation with snappy? What Open Surce software is best for meshing ships? Has anyone got any experience with Salome-Meca?

Thanks for the advice,
Tomislav
tomislav_maric 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
Ship hull hydrodynamics Costa Main CFD Forum 2 May 19, 2012 21:41
An Open Source mesh generator for Open Foam Ahmed Main CFD Forum 15 September 23, 2010 18:39
turbulence model for ship hydrodynamics ettax CD-adapco 0 January 20, 2009 06:02


All times are GMT -4. The time now is 22:25.