How to properly set up an opening in buoyancy driven problems
 

Dear forum members,

I'm trying to setup an opening being the only boundary beside walls in a completely fluid domain. The fluid's density is independent of pressure but temperature sensitive. So I'm dealing with a buoyancy driven problem, the smooth no slip walls are defined with a heat transfer coefficient and an outside temperature lower than the initial domain temperature.

How to setup the opening? Due to temperature expansion, fluid will enter and exit through the same boundary, so an Opening should be my option of choice. For mass and momentum I chose Entrainment with a Relative pressure of 0 Pa and the Pressure Option set to Opening Pressure. For Turbulence I chose Zero Gradient and for Heat Transfer I chose an Opening Temperature equal to the initial domain temperature.

Concerning the buoyancy, I set the reference pressure also to 0 Pa and the reference density to an value between the density at the initial and opening temperature and the density at the outside temperature of the walls.

I constantly run into c_fpx_handler: Floating point exception: Overflow so I'm very grateful for any helpful suggestions.

Almost forgot, my mesh is high quality (4.4e+06 hexahedrons, block structured in ICEM) and the analysis type is transient, initial time step was set from 1e-09s to 1e-01s, all resulting in overflow. The attached image shows the fluid domain mostly covered by (cooling) walls marked in green and the opening with hemisphere shape colored grey supplying hot fluid. Gravity acts in negative y-axis direction.

i think there may be something wrong with your reference pressure ，it should be not 0pa，you can try 1 atm（101325pa）.

No one with any (other) suggestions?
 

First of all, thank you for your response.

Unfortunately, your suggestion did not help with my problem. Since the density of my fluid isn't pressure dependent, I didn't think that the buoyancy reference pressure would make any difference.

For additional information, I attached the solver's output file. As mentioned before, the mesh is still of descent quality, in the meanwhile I reduced the mesh density for a quicker trial and error process.

The whole domain is filled with fluid? The sphere acts like a basin and the fluid gets sucked into the tank-like structure?

Clarifications
 

Exactly, the entire domain is fluid (oil, temperature dependent but pressure independent material properties). Everything marked green is wall that’s cooling down the fluid (with decreasing temperature the density increases resulting in a volume reduction compensated by the opening).

The half sphere at the bottom acts like a source of hot fluid and I’m interested how much fluid is circling around in a steady state. The initial conditions of the fluid are not important to me, I’m not interested on how the steady state is reached.

Some comments:

* Your material properties do not have a continuous derivative. This often causes convergence difficulties. If you round off the discontinuous bits that can help convergence.
* Set your initial and minimum time step to 1e-10[s]. If it needs small time steps let it use them. If will automatically increase them if it can.
* Why do you run for 10 time steps? Make that lots to run to convergence. But I suspect this is just for development.
* Your boundary location is too close to the flow feature. You will need to move it back to somewhere the flow is simpler.
* I think you will find the pipe to the closed reservoir does not play any significant part in the final steady solution. So I would not bother modelling it.
* I doubt there is a steady solution for this anyway. It will probably be a periodic flapping flow.
* You have a tight conservation target (1e-3). Are you sure you need it this tight? Usually if you are using a transient simulation to march to a steady solution you use loose criteria to do the time steps quickly. It should start converging as you approach a steady result, or you might have to tighten it as you approach it.
* Consider making a coarser mesh to do this development work on. Once you have the basic model working remesh to a finer mesh for accuracy.