[Rockytime]

Hi All,

I'm currently running a simulation about Wells turbine, and I have problem in running the CFX- Solver Manager and it finish without completing the run. The picture below shows where the CFX solver manager stop.



I'm not sure which information you guys need in order to let all of you understand my problem. If u guys need more information, do let me know. Thanks.

Your help will be much appreciated. Thank you.

[urosgrivc]

First try what it says and switch your outlet BC for an opening type one.

Overflow usualy means:
Your simulation is diverging probably because of bad boundary conditions.

Quick thought:
Probably something is trying to get in to the domain threw the outlet boundary condition some backflow or something,
but it cant becouse outlet boundary condition does not let this to happen outlet is strictly out that means that presure and other properties in the domain can extrapolate and diverge. Opening alows flow to flow back
in to the domain with the properties you define. this doesent mean that it will flow into the domain through the outlet surface
but it keps the simulation stable threw the iterations

[Rockytime]

Hi Uro,

Thanks for your reply. I have changed my outlet into opening boundary condition. My solver completed the run but the graph keep fluctuating. Can I know what is the meaning of this graph?

[urosgrivc]

ok now that is interesting.

More details will be needed to figure this one out.
setings of the simulation etc..

Ou ok , I see now that you are runing transient, and also that your RMS courant number is 999+ that is way too high, you will definitley need to reduce the timstep size, and this is probably the answer.

Graph meens that the solution si badly converged and is going up and down becouse (I am guesing here-)you are probably rotating something so convergence is sometimes bad and sometimes a bit better.

[Rockytime]

Hi Uro, Thanks for your advice.

I will reduce the timestep to check the result again. Regarding simulation setup, I not sure which simulation setup you need so I will attached the whole coding for you on the next post. Appreciate if you can help me find the mistake inside.

Besides that, I'm not sure whether I setup the periodic boundary condition correctly. Can you advise me on this?

FYI, Im using periodic boundary condition because turbine is symmetry around the axis of rotation.

[Rockytime]

Attached below is the Celcode. If you need any further information to understand my mistake, do let me know. Thank you very much.

[ghorrocks]

It appears your simulation has many problems. Please look at my post on your other related thread for some comments (Problem to get force value on blade surface)

[urosgrivc]

If i see corectly:

You are doing a CHT (conjugated heat transfer simulation) but your gas properties are isothermal 25°C.
Why do you have solid (blades) domain in the simulation, are these heated up or are you interested in heat transfer betwen blades solid and air fluid domain? do you want to know heat transfer coeficient or what?

isothermal fluid and buoyancy - i dont know if this has any meaning,
as usualy buoyancy needs to be activated if density diference driven flow has a major impact on the results, and density diference usualy comes in the form of temperature diference for buoyancy.

-at 100 rev/min you should calculate maximum velocity that might ocure at the tip of the rotor (Omega*R) if it is high enough (70+ m/s) you should consider switching to air ideal gas.

also you have set the convergence criteria to 1e-6 this needs to be reached when solving the problem but in you case it cannot be as your timesteps are too long and max coef. loops limited to 5.
So you do have quite some time steping and convergence problems.
Is it not posible to make a steady state simulation?

If you are new to the cfd, try starting off slowley (something simpler), you need to walk first to than run
Cfd transient heat transfer multidomain simulations are not a walk in the park

--------------------
There is some problems (I hawe writen some above) and I do not know what you are trying to achieve with the simulation so I can not give you a direct ansver, these are only some thoughts.

But this is definitely not a -Problem about CFX Solver Manager- its all about setings of the simulation

[ghorrocks]

Rocky: I have posted almost the same post as urosgrivc did on your other thread. Please post a message stopping discussion on one of your threads as having the same discussion simultaneously on two threads is not useful. You can choose which thread discussion stops and which continues