CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   STAR-CCM+ (http://www.cfd-online.com/Forums/star-ccm/)
-   -   DFBI Seakeeping Simulation (http://www.cfd-online.com/Forums/star-ccm/102136-dfbi-seakeeping-simulation.html)

Forbin May 23, 2012 05:35

DFBI Seakeeping Simulation
 
Hi there!

I'm doing a seakeeping simulation with a small container-vessel for a student project and used the "boat in headwaves" tutorial as a guideline. The vessel is allowed to heave and pitch and I use the first order waves. The time-step is set in accordance to the CFL number. The mesh is valid.

Anyway I'm experiencing serious problems concerning my free surface. The free surface - especially the waves - behaves unphysical after some time and the water level in my region starts to rise. At this point the waves are badly scattered. This problem seems not to be connected to the mesh, because a tutor of me solved the simulation on the same mesh with COMET.

I assume that it may be related to the physics models I use and therefore would be glad for any help. The models used are:

- Multiphase Interaction
- Laminar
- Segregated Flow
- Gradients
- Implicit Unsteady
- Segregated Fluid Isothermal
- VOF Waves
- Gravity
- Multiphase Equation of State
- Volume of Fluid (VOF)
- Eulerian Multiphase
- Multiphase Mixture
- Three Dimensional

ping May 23, 2012 09:17

if your water level is rising it normally means you don't have vof wave inlet field function boundaries on ALL the boundaries other than the pressure outlet (which should have the vof wave hydrostatic field function). ensure you are watching a scalar plot (no smoothing) of volume fraction of water on one or two axial vertical sections to ensure the transition from air to water occurs across only one or two cells, since the iso surface 'hides' problems even though it displays the wave well. try shortening your times step and use 2nd order time is you want the waves to maintain their hieght. need about 20 cells vertical for a wave and 40 per wave length too (use anisotropic mesh refinement to achieve this). overset mesh will allow greater trim angles with a simpler mesh to capture the wave for sea keeping runs since the underlying mesh is stationary.

Forbin May 23, 2012 10:05

Quote:

Originally Posted by ping (Post 362680)
if your water level is rising it normally means you don't have vof wave inlet field function boundaries on ALL the boundaries other than the pressure outlet (which should have the vof wave hydrostatic field function).

Thank you ping, that is true. I only use one velocity inlet in front of my ship and one pressure outlet on the back, while the other sides of my region are symmetry planes. So I will change these to be velocity inlets as well...

abdul099 May 23, 2012 11:44

The water level should not rise due to symmetry planes instead of velocity inlet.

Did you use overlapping grid? Did every time step converge well?

ping May 23, 2012 11:54

sorry to contradict you abdul, but the top and bottom boundaries must be vof wave inlet boundaries if rigid body DFBI is being used in a case which has reasonable amounts of trim - Forbin says he/she is trying to replicate the boat tutorial which uses this technique - without this these cases go crazy. the way around this restriction is to use overset mesh when the base region is fixed and then there will be no problems

abdul099 May 23, 2012 16:48

ping, you're right. I did not think about top and bottom in an embedded motion case. I just thought about the sides. :(
So Forbin, forget my last post and listen to ping :cool:

Forbin May 24, 2012 04:16

Thanks for your quick response and help. I just started a simulation with the changes you suggested and I'm looking forward for the results...

And actually me is a "he"... :)

arun7328 October 15, 2013 10:27

Hello,

Did you get it running? I have the same problem when simulating a regular wave on a cylinder. The cylinder is only allowed to heave and pitch and I have used DFBI motion. It seems that after some time the cylinder sinks down or water level starts to increase. I have used velocity inlet at top and bottom. Any suggestions?

Thanks
Regards
Arun

Forbin October 17, 2013 09:36

Hey arun!

There was no real solution for this special problem. However, I managed to run the simulation correctly after exporting the mesh, followed by an import into a new simulation file. Therefore, I think that my original file was corrupted at some point. I hope this helps!


All times are GMT -4. The time now is 13:35.