[plakiasge98]

Hello, this is my first post in CFD-Online and thank you for your help till now with all threads posted.

I am currently trying to model the flow around a non moving sphere (open channel simulation). I am trying to modell it in CFX however I face the following issue. It seems like the free surafce is lowering at the end of the domain, so I tried a higher inlet velocity (20m/s) in order to figure out the issue. I am trying to figure out what is going wrong in my BC or setup. I have followed and totally understood the two tutorials provided by CFX (tutorial 9 and 30). It seems like the free surafce cannot stay horizontal, can you explain me the reason?

- Steady state
- Buoyancy model: Buoyant
- Homogenous model , Standard Free Surface Model
- Water inlet 1m/s, Water Volume Fraction = 1, Air Volume Fraction = 0
- Opening on the top side

Thank you for your help.

[AtoHM]

Your post is missing the most critical information: how did you set up the outlet boundary?
It looks like you have relative pressure 0 at the outlet. I feel you want your water level somewhere near the sphere, so you have to apply a static pressure profile equivalent to the hydrostatic pressure at the outlet.


Also I would suggest to move at least your outlet boundary further away from the sphere.

[plakiasge98]

Thank you for your reply. You are right I have missed reffering the outlet conditions. You are right the pressure in the outlet is 0 Average Static pressure. That is correct I have to apply hydrostatic pressure with the use of expressions. I will keep you updated.

[Stel]

Please, provide us with more detail about your setup. AtoHM's reply regarding the implementation of a static pressure profile at the outlet is indeed a good one. It also seems that you have a couple of openings at the outlet section, why so? Could you provide as with more detail about them?

[plakiasge98]

Indeed, with changing the outlet boundary condition to hydrostatic pressure, the free surafce is horizontal. I have to check now my results if they are physically correct because there is something strange at the end of the domain near the oulet.
Stel there were no openings in the outlet, I have just separated the outlet face in the height of the free surface.
Another question I have and I would appreciate your opinion is which of the two FLUENT or CFX is more suitable for Hull Prediction? Most of the papers and validation models are done with Star CCM+ and FLUENT. Do you know the reason that CFX is not suggested? Thank you again for your time.

[Stel]

Not quite sure but that could be because CFX only has one interface capturing scheme, the compressive scheme. Fluent (and maybe other commercial packages) will have other methods and features such as geo reconstruct, level set, anti-diffusion procedures, more interfacial area density models, etc.

Does that mean that CFX is bad for free surface flow? Not at all. CFX is a VERY ROBUST numerical solver, and this is a very nice virtue for free surface flows. CFX's compressive model has been tested and validated for many problems now and it works well for several problems. And don't think that other packages are perfect either. Right now, for example, I'm having a hard time solving a free surface flow problem in Fluent because of interface diffusion. I've tested a lot of things and realized that using the gradient interfacial area density (Fluent's equivalent to CFX's Free Surface IAD) is very diffusive. I don't have this problem in CFX. Also, free surface flows usually demand all of those profiles for boundaries and initialization, and implementing them in Fluent is not as user friendly as in CFX.

Also, this "software A is better than software B to simulate something" thing is usually more related to lack of knowledge of the software usage itself than what is really implemented in it.

[plakiasge98]

Thank you very much for your reply. All these details sound really interesting for having an overall image of software capabilities. I will try some benchmark geometries as this is my first project involving multiphase and free surafce modelling and I will decide the most suitable software. For sure I wanted to figure out where I was wrong, even if I come up with using other software.

[karachun]

There is CFX tutorial "Chapter 9: Free Surface Flow Over a Bump", do you make it? If not, then make it to become familiar with CFX free surface flow basics.

Some free surface flow with waves may have transient nature and therefore you need transient simulation to capture flow effects.

Free surface flow requires good mesh resolution near a free surface, based on your pictures it looks like the mesh is coarse. Perform mesh convergence study to investigate mesh size.

Waves may reflect from BC (symmetry, outlet, etc) one of solutions is to make mesh near BC coarse so waves will be artificially damped.

If you want to perform Ship Hull drag calculation then I can recommend to start with the KRISO Experimental case. This is a popular “Classical” example.

Here is a link to geometry.
https://www.nmri.go.jp/institutes/fl...container.html
And here is a link to a paper with measurement results.
https://www.researchgate.net/publica...al_ship_models

[plakiasge98]

Thank you very much for yur reply karachun

There is CFX tutorial "Chapter 9: Free Surface Flow Over a Bump", do you make it? If not, then make it to become familiar with CFX free surface flow basics.

I have tried the tutorial but I did not understand the importance of the hydrostatic pressure in the outlet bc.

Some free surface flow with waves may have transient nature and therefore you need transient simulation to capture flow effects.

Free surface flow requires good mesh resolution near a free surface, based on your pictures it looks like the mesh is coarse. Perform mesh convergence study to investigate mesh size.

Waves may reflect from BC (symmetry, outlet, etc) one of solutions is to make mesh near BC coarse so waves will be artificially damped.

I totally inderstand that I should use a more fine mesh this case was just a test case just to see that everything works fine and I needed it to run as fast as possible.

If you want to perform Ship Hull drag calculation then I can recommend to start with the KRISO Experimental case. This is a popular “Classical” example.

Here is a link to geometry.
https://www.nmri.go.jp/institutes/fl...container.html
And here is a link to a paper with measurement results.
https://www.researchgate.net/publica...al_ship_models

I know about this benchmark case and thank you very much for the reference. I fully appreciate it. Do you have to recommend me any simpler model in order to check also the rigid motion? This one would be my next step.

[karachun]

Originally Posted by plakiasge98

I have tried the tutorial but I did not understand the importance of the hydrostatic pressure in the outlet bc.

Originally Posted by plakiasge98

Do you have to recommend me any simpler model in order to check also the rigid motion?

No, I have solved only the problem with stationary mesh.

Originally Posted by plakiasge98

and I needed it to run as fast as possible

Then run 2D case - flow around infinite cylinder, you can reduce mesh size if you model only one layer of elements.
https://www.cfd-online.com/Wiki/Ansy...tion_in_CFX.3F