Hi again @cecil_pabbathi!
I need to investigate this a bit more as the solver log unfortunately does not give the CFL number at this state of the simulation. Would get back to you as soon as I have created a successful run if that is okay. If you manage to fix the problem by yourself in the meantime, please let me know.
Best,
Jousef
Hi @jousefm
Thanks again ! Really need to get this case up and running. Out of curiosity, has the automatic timestep option been scrubbed altogether ?
Hi @cecil_pabbathi,
Not an expert on multi-phase DOF simulation but it seems like the issue you’re encountering are a result of a setup that still has issues rather than say a non ideal CFL number that causes your simulation to go into instability instantly.
Referring back to what Jousef referenced with regards to the 6DOF boat project, there are some irregularities that are in your simulation as compared to that.
For a start, your phase fraction sub-domain is being applied to a small area rather than the entire water domain which is occupied. This is what the 6DOF boat simulation project has done. You can start with that change and see if it helps.
The second irregularity I noticed was the boundary condition related to the object in the water, which is this case is your geometry. In the 6DOF boat simulation the geometry is defined as a moving wall velocity with zero values in the xyz direction, fixed flux pressure and a phase fraction value of gradient set to zero. Yours is a fixed value. Maybe this change might help.
Generally speaking if you’re running into issues like this I don’t think it is a CFL number issue. I would recommend looking into a successful simulation like the 6DOF boat project and to replicate it as closely as you can to every detail. Of course your case I believe is slightly different due the presence of the inlets having a set velocity so adjust as accordingly.
Hopefully this helps! Do let me know if it works.
Cheers.
Regards,
Barry
Hi @Get_Barried @jousefm ,
This was blatant ignorance from my side. Earlier I had set up a case with a smaller domain and the case ran well but I wasn’t happy with my force plots. I uploaded a newer model with bigger domains but I didn’t want to go through the pain of setting up my case again so I made a duplicate of my case set up and hence the water domain remained small. Sorry for the trouble I put you guys through but thanks again. 
As for the geometry being set up as moving wall velocity, I definitely have plans to study 6 DOF movement of the body under the influence of waves but at a later stage perhaps. For now, I am interested in the drag forces alone and optimizing the geometry accordingly.
Cheers,
Cecil
Hi @Get_Barried,
Coming out the CFL error, now I run into Fatal I/O error 
. I am using this project SimScale as reference because I feel it closely resembles what I want to study as well.
Hi @cecil_pabbathi,
I think I figured out the problem! So all you have to do is to set your outlet mean velocity to a positive value, which in your case is 3m/s. The negative value of the outlet means flow is somehow stuck and flowing back in through the outlet. I’ve copied your project over and it seems to be running fine so do try this and let me know.
Cheers.
Regards,
Barry
Hi @Get_Barried,
You’re a lifesaver ! Thanks mate. The simulation runs now. When using the other project as reference, it had a backflow outlet velocity defined as well. Really appreciate your time & valuable inputs. Cheers !
Regards,
Cecil
Hi @Get_Barried @jousefm ,
So I ran few simulations successfully. When I looked at the velocity contours, the velocity remains zero throughout(20 timesteps) without really changing much which makes no sense because an inlet velocity of 3 m/s was defined. Also had a look at a similar project (SimScale), the outlet mean velocity here is also defined in the opposite direction of the inlet velocity. Could that be the reason ? Would love to hear your thoughts. Cheers.
Regards,
Cecil
Hi @cecil_pabbathi,
Looking at your force plots for 20s, you will realize that something is seriously wrong. You’re getting moments of over 10k which means something went wrong somewhere. What the exact issue is I’m not too sure but the current simulation you are running (5s) is going well and checking the force plots you do have rather nominal values that should give out what you’re looking for.
Let it finish running and we’ll work from there.
Cheers.
Regards,
Barry
Hi @cecil_pabbathi!
The residuals for your last run look much smoother which not necessarily has to mean that the solution will be accurate or “correct” but looks much more promising than the last run (20sec) that you have created. Let’s see what we can derive from the post-processing.
Best,
Jousef
Hi @jousefm@ @Get_Barried
I took a short break from work so could not spend much time on the project either. The simulations ran well although I might need to decrease my end time length and increase my time step a bit to get more accurate results. I have a couple of questions as I am fairly new to transient and multiphase simulations.
Regarding the drag & lift, I want to specifically calculate how much drag is induced by water and likewise air. So i have split my CAD model into two parts, one part which will be immersed in water and the other exposed to air. So if I calculate the coefficients for both these parts and add them up it should give me a measure of the total drag & lift on the body, right ?
I have attached a short animation of my simulations. What you see is an isosurface of water phase at 0.5 colored by velocity magnitude. Towards the end of the simulation, there is a backflow phenomenon like water hitting against a wall, is that normal with the outlet bc I defined ?
Thanks for checking by,
Cheers,
Cecil
Hi @cecil_pabbathi,
Don’t worry, I’m even newer 
We’ll learn and solve along the way.
While you may be able to supposedly get the values out. I do not think that individually calculating both values and adding them up will give you a proper representation of the drag and lift on the body. This is due to (referring to the animation) water and air both “mixing” together and its very difficult to quantify exactly the lift and drag forces due to each medium. Fortunately, there is no need to do that. You can simply just obtain results directly from the body regardless of water or air and produce a lift and drag force value out. However, due to the nature of the results right now, this also may not accurate which brings me nicely to my next point which you already have kind of identified.
I suspect your outlet seems to be “blocking” the flow of water, hence the presence of a “back wave” occurs which will significantly affect your results. If the water were to instead “flow normally” per say and no backflow occurs then you can obtain direct results of lift and drag directly. As for how to fix this issue I am not exactly sure how. On one hand increasing the outlet velocity is one way, but referring to the sample case, the flow doesn’t behave like this despite the same outlet conditions. The backflow likely occurred due to the very strange sudden flow speed increase at around the 7s which is very strange. I suggest maybe increasing the area of the bounding box significantly to mitigate the effects of the wall and if this still continues, we’ll probably have to look into the side wall conditions.
Do let me know how it goes! Cheers.
Regards,
Barry
Hi @Get_Barried,
Thanks again for your valuable input mate. Trust me I am learning a lot from you along the way 
I will try a simulation with a bigger domain and see how that works out. Cheers.
Cecil
Hi @Get_Barried @jousefm,
Help ! I tried setting up a new sim with a bigger domain using the same boundary conditions but I keep getting plagued with the CFL error Here is the link to my project [Deleted by author]
HI @cecil_pabbathi, have you tried aligning your numeric with the example project you have linked? I would try reducing the courant number (alpha and normal co). Also the mesh for the example is much less locally refined. I found when I was doing my slosh analysis (although this was real transient not locally sidestepped) if I had excessive local refinements, the fluid passing into the refined cells would cause courant numbers to rapidly increase and cause divergence.
The animation above looks like the solution just became unstable and produced non physical results, Trying to ‘fix’ the outlet might not be necessary.
Hope this will help you get unstuck!
Darren
Hi @1318980 darren,
Your post was definitely informative and I coarsened my mesh like you said but still I have trouble getting the simulation to run. The simulation crashes as soon as it starts so the solver log isnt really helping either.
Regards,
Cecil
Hi @cecil_pabbathi, just so you know I have copied your project and will see what can be done, have you tried reducing the timestep?
Best,
Darren
Hi Darren @1318980,
Thanks for looking into my project and yes, I played around with different timesteps without any luck.
