November 21, 2018 at 5:23 pmGabrielLSubscriber
I'm now attempting to create a 3D simulation on the trim and draft behavior of a ship hull under both flat and wavy sea conditions using ANSYS Fluent 19.2 Academic. I have created a large rectangular geometry consisting of four bodies (i.e. flow domains) connected together, the top two being the atmosphere and the bottom two being the water zone. The ship hull (i.e. a cavity in the geometry) is drawn interfacing between the middle two bodies. The reason that I do so is to allow coarser mesh to be done on the top and bottom bodies, while denser and refined mesh can be done in the middle two bodies, thus capturing the water surface and ship movement in more detail. The sizes of the flow domain is much larger than the ship hull.
I have then generated the mesh using body sizing and refinement around the ship hull. This was then imported to Fluent to carry out analysis using VOF Open Channel Flow model. I chose k-omega standard viscous model, and assigned dynamic mesh to the ship hull using UDF to regulate its movement to pitch and heave only (z-direction displacement and rotation around y-axis). I used smoothing and remeshing method, with a spring constant factor of 0.5. The centre of gravity of the ship hull was defined 70% along the ship hull, with zero centre of gravity velocity. The inlet, outlet, atmosphere (pressure-outlet), ship hull (wall) and location of free surface were defined accordingly. I used a time step of 0.01s. For simplicity I did not assign any wave boundary conditions and the inlet velocity was kept at 0m/s. I initialized using hybrid initialization and flat condition.
After I run the calculation, I kept getting problematic results including reversed flow at outlet, as well as wild movements of the ship as it bounces up and down in a large magnitude, which eventually led to divergent error. I would have expected that the ship remains stationary and having a slight trim angle due to the hydrodynamic forces on the ship on the location of centre of gravity.
Can anyone here please help with my problem? The settings should be mostly correct but there were still erroneous results!
November 22, 2018 at 4:18 amKeyur KanadeAnsys Employee
From description set up looks ok.
You will need to check your UDF to see why there are forces to get wild movements.
November 22, 2018 at 4:32 amGabrielLSubscriber
Thank you very much for your help.
This is what I included in my UDF:
DEFINE_SDOF_PROPERTIES(stage, prop, dt, time, dtime)
prop[SDOF_MASS] = 7.257;
prop[SDOF_IYY] = 0.6165;
prop[SDOF_ZERO_TRANS_X] = TRUE;
prop[SDOF_ZERO_TRANS_Y] = TRUE;
prop[SDOF_ZERO_ROT_X] = TRUE;
prop[SDOF_ZERO_ROT_Z] = TRUE;
printf ("nstage: updated 6DOF properties");
I have also been wondering should I define the ship hull as a solid domain in fluent instead of simply creating a cavity in the fluid domain. However the latter seems to be the case for most online tutorials.
I have actually also found a similar fluent tutorial on "heave and pitch simulation of ship" but I could not find where to download the geometry and mesh file for that tutorial. Is there anywhere to download that specific file?
November 22, 2018 at 4:38 amKeyur KanadeAnsys Employee
Can you please insert image for you inlet conditions.
November 22, 2018 at 4:47 am
November 22, 2018 at 5:32 amKeyur KanadeAnsys Employee
Can you please try with shallow waves with first order wave theory. Please give details of wave height and wave length.
Is there any interface between two volumes? I see in the mesh that the mesh suddenly grows to bigger size. You may want to use conformal mesh with fine mesh. Please insert image of cross section of mesh. Also once you patch the volume, please check contours of vof before running.
November 22, 2018 at 6:35 amGabrielLSubscriber
November 22, 2018 at 5:26 pmRobAnsys Employee
The jump in cell size is very big, I usually aim for a volume change of around a factor of 2. Before remeshing, turn off the ship motion and see how the waves behave. If that fails review the mesh and repeat. Once the VOF bit works turn the moving ship back on.
November 23, 2018 at 4:34 amKeyur KanadeAnsys Employee
As Rob suggested, you have to work on your mesh first before you get into solver. Usually multiphase problems need a good mesh.
You will have to reduce that size jump. Also check quality of the mesh before going to solver. The min orthogonal quality should be more than 0.1
December 23, 2018 at 5:56 pm
December 23, 2018 at 7:05 pmraul.raghavSubscriber
You can visualize the regions where your mesh has skewed elements and try to focus on those regions to improve your mesh.
December 24, 2018 at 3:47 amKeyur KanadeAnsys Employee
please check the bad elements location. then take corrective action.
January 11, 2019 at 11:33 pmKevinsandovalSubscriber
Hello gabriel, I'm trying to simulate something similar to what you're doing, analyze the draft of a ship in calm sea situation, but I have not managed to make this simulation, maybe I have problems of boundary conditions or problems in the dynamic mesh, you have SETUP or messaging to guide me, I ask you please, I have not been able to find more information about this in the network, if you have more bibliography of this I will also be grateful, waiting for your message. thank you.
January 20, 2019 at 6:19 pmGabrielLSubscriber
Thank you very much for the kind assistance!
I have now been able to simulate the movement of the ship, but not completely. The only problem now I'm facing is that the model only works when the mass of the ship is larger than around 10kg. Below that (as what I intend to simulate a 7kg ship hull), non-physical and intense up-down movement of the hull is observed until the solution diverges. However, the model works perfectly fine with realistic physical pitch and heave behavior under no wave and wavy conditions when the mass is increased to a suitable value.
I thought this can be solved by reducing the under-relaxation factors or flow courant number to improve convergence. I also tried reducing the time-step to 10^-5s. I have also tried using k-omega SST or k-epsilon realizable viscous model. However, these didn't solve the issue. May also kindly advise the possible solutions?
For the setup of my model, please refer to the topmost post.
Thanks very much!
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- Suppress Fluent to open with GUI while performing in journal file
- Heat transfer coefficient
- What are the differences between CFX and Fluent?
- Floating point exception in Fluent
- Difference between K-epsilon and K-omega Turbulence Model
- Time Step Size and Courant Number
- The solver failed with a non-zero exit code of : 2
- Exporting Data Results
- Floating point exception