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

hydrodynamic losses of a ship

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 19, 2007, 05:53
Default hydrodynamic losses of a ship
  #1
James Downing
Guest
 
Posts: n/a
hello,

i would like to calculate tha hydrodynamic losses of a hull in star cd. it is the first time that i try to do that in star and i have a lot of questions, so if there is anyone expert on this please answer me.

my questions are: 1) i have to create the water and the ship and the air? or only the water and the ship?

2) what kind of interfaces i have to apply? between which parts?

3) how can i apply the weight of the ship and the velocity ?

4) what else i have to do? 5) is it better to simulate that in star cd or in star ccm?

6)is there any tutorial???

i also have cfx but my director need that in star so... which do you believe is better software for that?

thanks a lot James

  Reply With Quote

Old   November 20, 2007, 16:01
Default Re: hydrodynamic losses of a ship
  #2
Ship in the hut
Guest
 
Posts: n/a
you need star-ccm+ to do this but it is ok because it uses the same license. There are macros especially for this. There is also a training course (cheap). Go to www.cd-adapco.com and fill the request form in the front page.

  Reply With Quote

Old   November 21, 2007, 04:18
Default Re: hydrodynamic losses of a ship
  #3
James Downing
Guest
 
Posts: n/a
i fill the request for, but there is no reply. can you send me any material like info or examples how to set it up?

best regards
  Reply With Quote

Old   November 27, 2007, 13:23
Default Re: hydrodynamic losses of a ship
  #4
Dan
Guest
 
Posts: n/a
James,

When you say hydrodynamic losses of the hull can you be more specific? If you are trying to do a problem involving 6 DOF motion, you will need to use Comet. If you are looking for resistance / wave making, to simulate a tow tank type calm water test, star ccm+ works great. You need a domain that contains both air and water if you want to capture the wave surface. This will be a VOF simulation, for which you will need to write a few very simple field functions in star CCM+ to define the level of your free surface, and also the hydrostatic pressure. You won't require any interfaces in your model.

My experience is with star ccm+, i know that cfx has a new coupled VOF solver, but i have never used it before.
  Reply With Quote

Old   November 27, 2007, 16:28
Default Re: hydrodynamic losses of a ship
  #5
JAMES DOWNING
Guest
 
Posts: n/a
I WANT TO CALCULATE THE POWER THAT A BOAT NEEDS TO RUN WITH 20 KNOTS ON THE SEA SURFACE WITH NO WAVES AND WITH 1 METER WAVES.

THE BOAT WILL HAVE A INITIAL VELOCITY AND WE WOULD LIKE TO SEE THE HYDRODYNAMIC LOSSES DUE TO THE CONTACT WITH THE WATER.

I DO NOT KNOW ANYTHING ABOUT THE COMET SOFTWARE .

CAN YOU TELL ME HOW TO SETUP THIS ANALYSIS ???

THANKS YOU SAVE ME...
  Reply With Quote

Old   November 27, 2007, 16:43
Default Re: hydrodynamic losses of a ship
  #6
Dan
Guest
 
Posts: n/a
Comet is an older code, where the VOF scheme in Star CD and Star CCM+ was originally developed and validated. It's not normally distributed any more, but it has 6 DOF motion, and overlapping mesh schemes that I don't believe are available yet for Star CCM+. The latest I had heard, these were planned to be released for January, in CCM+, but we'll have to wait and see.

Until then I'd suggest you start with the calm water analysis. You'll likely want to start by producing a simplified hullform above the waterline, to ease mesh creation / convergence.

Beyond that it's rather simple actually, you need to write a VOF field function setting the initial free surface height, and the height at the inlet (also possibly at the outlet too, depending on your choice of BC's). Also, you need a simple field function for the hydrostatic pressure on your outlet and for the initial conditions.

I'd suggest starting by running through the CCM+ tutorials on free surface flows first to make yourself familair with the solver, and how it works before attempting the whole ship problem.
  Reply With Quote

Old   November 27, 2007, 16:48
Default Re: hydrodynamic losses of a ship
  #7
JAMES DOWNING
Guest
 
Posts: n/a
i saw every tutorial and i did not find anything.... i am going crazy.. i contact cd adapco but i still have not got an answer (3 weeks), if you have any tutorial.. it would be great. where can i see about comet?

thanks a lot my friend
  Reply With Quote

Old   November 27, 2007, 17:05
Default Re: hydrodynamic losses of a ship
  #8
Dan
Guest
 
Posts: n/a
When you open ccm+, bring up help, go to training guide, and select multi phase tutorials, that will go through the VOF setup.

If you don't see multi phase tutorials, make sure you have the most up to date version of ccm+, the current release is 2.10.013

CD-Adapco no longer distributes Comet, so if you don't have a license for it at your institution it will likely be hard to get. It is used as a development code, and is rather hard to use to say the least. I would recommend starting with CCM+, and only look for Comet after you have gained considerable expertise with CCM+
  Reply With Quote

Old   November 28, 2007, 00:49
Default Re: hydrodynamic losses of a ship
  #9
JAMES DOWNING
Guest
 
Posts: n/a
JUST ONE MORE QUESTION...

SHOULD I PUT THE AIR AND THE WATER AS SINGLE MESH OR DIFFERENT MESH THE AIR AND DIFFERENT THE WATER AND PUT SOME INTARFACE BETWEEN THEM??? ALSO ABOUT THE SHIP, SHAL I PUT THE MESH IN THE AIR MESH AND APPLY A FORCE ON IT LIKE THE GRAVITY?

ANY IDEA??

THANKS A LOT YOU SAVE ME
  Reply With Quote

Old   November 30, 2007, 14:33
Default Re: hydrodynamic losses of a ship
  #10
Dan
Guest
 
Posts: n/a
You should build the mesh as a single mesh, the air and water levels are defined only by where you set the VOF level at the inlet (and you apply the same function under initial conditions as well). Your VOF field function is a simple if statement (if above waterline)?1:0 for the air phase, and the inverse for the water phase, check the user manual for the correct syntax for how to write the if function. Since it's not possible in Star CCM+ yet to have the ship move, and hence to account for sinkage and trim, your ship is simply a wall surface, placed in your CAD package according to where you want your still waterline. You should include gravity though since ocean waves behave as gravity waves. Hope that helps.
  Reply With Quote

Old   December 3, 2007, 05:25
Default Re: hydrodynamic losses of a ship
  #11
JAMES DOWNING
Guest
 
Posts: n/a
HELLO

i unterstand what you tell me, i should put the boat as a gavity part on the mesh and just put a wall on it, but how can i give the software the data to create the boat with gravity? to see how the boat acts as the wave hit it? or i can only put a boat at the place where the VOF is and see the losses witout move the boat...?

see that image http://www.cd-adapco.com/products/ST...ery/index.html there you can see a boat simulation... is this boat moving or is just fix?

thanks a lot james
  Reply With Quote

Old   December 3, 2007, 13:35
Default Re: hydrodynamic losses of a ship
  #12
Dan
Guest
 
Posts: n/a
Hi James,

The boat is likely just fixed, in order to move the boat to react to waves, you need to be able to change your mesh in an arbitrary manner, which is not a simple task.

You can work in an iterative manner, calculating the forces and moments on the ship at each time step, sinking and trimming the boat accordingly, re-meshing and solving at the next time step and so on. This would be quite a laborious task, but perhaps something you could script. Since this 6 DOF motion is something that will soon be in CCM+ (hopefully less than 6 mos?), I would suggest to get the static case working first, then if the scripting approach isn't feasablie, perhaps contact CD-Adapco to see if they can provide you either with Comet, or a beta version of CCM+ with this feature if it exists. (you can export your mesh from CCM+ to Star-CD and then eventually back to Comet).
  Reply With Quote

Old   December 14, 2007, 10:14
Default Re: hydrodynamic losses of a ship
  #13
Peter
Guest
 
Posts: n/a
James,

Using STAR-CCM+ for your application is going to lead to some issues unless you take a slightly different route.

For a VoF calculation involving a ship you need to capture the air/water interface accurately, including upstream of the boat to the inlet. So a fine mesh normal to the surface is required. However, in CCM+ using mesh refinement will refine the cells in all three directions, which is not good and will lead to a model that is much larger and therefore slower to run than in Comet, STAR-CD or other software. To get round this mesh problem you need to use a third party mesher. A basic model in CCM+ running free surface, boat static (not responding to waves) yes you can do it and extract the drag without trouble. Just watch the mesh size does not get out of hand.

The ignorance of adapco is nothing new and is frequently exploited by the competition. If this is a problem for you call Bill Clark at the Detroit office and give him an ear full.

The next version of STAR-CCM+ promises to have the functionality you need, but the withdrawal of Comet leaves adapco with only STAR-CD v4 for this application and this code is known to be wobbly on this application. I know of a Dutch company that dropped STAR v4 on this application because half of the runs fell over. I have also asked CD-adapco about delivery of 6DOF in CCM+ and having contacted people I can trust (not sales or management) the answer was the second half of 2008.

Until then you may well be high and dry.

Enjoy Christmas and don't think of work until January 2008,

Peter

  Reply With Quote

Old   December 15, 2007, 09:53
Default Re: hydrodynamic losses of a ship
  #14
Balduin Bankerotti
Guest
 
Posts: n/a
Just split the domain horizontal at waterlevel and create an interface there. Now you can have a subsurface and layered mesh parallel to the water level, which is what you want.
  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
Duct losses kk Main CFD Forum 1 February 29, 2008 15:03
Hydrodynamic of a ship James Downing CFX 0 November 18, 2007 23:05
friction losses Roux CFX 1 August 20, 2007 09:19
losses Pablo Cornejo FLUENT 0 December 19, 2005 10:31
Pressure losses René CFX 11 April 12, 2002 09:55


All times are GMT -4. The time now is 23:36.