[Pit7512]

Hi,
I desperately trying to run a free surface simulation of an river section. The Problem is, that I can´t get a nice surface without refinement. I tryed almost everything. For testing I have a simpel rectangular channel with an laminar flow of 10 by 4m (20m long, Hex-mesh 0,4m max). The flow seems fine at the botton but gets turbulent close to the surface. At the Inlet the water close to the surface goes down as you can see in the attachment. At the Outlet it goes up again. Is there a way to get it straigt without refinement of the surface.
I would be thankful for any tip

[EvaS]

Hi.

Could you post your settings here? At least inlet and outlet condition.
Did you checked "Tutorial 9: Free Surface Flow Over a Bump"?

Eva

[Doginal]

I've been struggling with the same problem. I have not found any complete solutions. Problem seems to be ansys trys to flatten the surface between timesteps across the mesh which causes small waves to propogate across the surface. There really aren't any solutions found in any of the documents. I think its one of those things you have to try to limit its effects, cant get rid of.

Best thing to do is just refine the mesh at the surface.

[ghorrocks]

Spurious currents at the free surface is a common problem with free surface simulations. They are very hard to eliminate in a eularian approach. You can minimise them by careful adhustment of the free surface parameters - I can't remember which, try them all and see which ones work, that's how I found this out - but you will not be able to eliminate it.

Alternate free surface approaches such as level set and single phase VOF have the potential of eliminating this problem - but you will need to go to a different CFD code to do that, CFX does not support any other options.

[cfdesf1990]

Hi
I am going to simulate a submarine near the free surface. I read free surface over a Bump tutorial.After 1000 time steps when Max Residuals for momentum and masses are about 10e-4, there is a surface wave (attached file), though the inlet velocity is set to normal velocity.
In addition, as far as I got from CFX solver tutorial, we must choose a different time step for volume fraction so I used 0.1 as volume fraction time step and 1 as the total time step but the wave still exists. The question is how can I solve this problem? and what is the origin of this wave?
Generally, I use structured mesh near the free surface and unstructured mesh in the rest. In the solver setting, the first order option is set. BCs are like the tutorial and I do not think that the problem is due to BCs.

Meysam


http://i57.tinypic.com/mwazaq.jpg

[ghorrocks]

It could be:

* transient behaviour, free surface simulations do this a lot. Many free surface simulations require transient simulation despite being steady state.
* Generated by spurious currents at the free surface
* An incompatibility with your boundary conditions.

[highorder_cfd]

Originally Posted by ghorrocks

It could be:

* transient behaviour, free surface simulations do this a lot. Many free surface simulations require transient simulation despite being steady state.
* Generated by spurious currents at the free surface
* An incompatibility with your boundary conditions.

Hi Glen, just a question.

When I solve free surface flows I always try to refine the mesh near the free surface. Usually I put the body in a subdomain meshed with tet element.

In my experience, I often get a more wavy and rough free surface where tetraedrons are used, whereas the accuracy is much better for hex elements, with a smooth free surface. Any suggestions?

[ghorrocks]

Free surface models are very sensitive to mesh quality and work best with orthogonal mesh, that is hex meshes. The angled faces of tets cause additional dissipation and blur the interface and can create additional spurious currents.

So you are correct, you should use hex elements as much as possible near the free surface.

[cfdesf1990]

Originally Posted by ghorrocks

It could be:

* transient behaviour, free surface simulations do this a lot. Many free surface simulations require transient simulation despite being steady state.
* Generated by spurious currents at the free surface
* An incompatibility with your boundary conditions.

Thank You so much, Glen.
I simulated it in the steady state condition. Do you mean transient simulation probably solves this problem?

[ghorrocks]

Free surface simulations frequently require transient mode to achieve convergence. This is because the surface waves have very low dissipation and are very difficult to converge. A transient simulation is not stopped by these little waves so can converge easier, but will take much longer to run.

[cfdesf1990]

So I will apply A transient simulation as well.
One more question, when I use upwind scheme the convergence speed increases noticeably and the wave decreases, especially after the submarine as you see in the following figure. Can we conclude and guess something else? Do you have any other suggestion?


http://www.freeuploadsite.com/do.php?img=80764

[highorder_cfd]

Originally Posted by m.khatoonabadi

So I will apply A transient simulation as well.
One more question, when I use upwind scheme the convergence speed increases noticeably and the wave decreases, especially after the submarine as you see in the following figure. Can we conclude and guess something else? Do you have any other suggestion?


http://www.freeuploadsite.com/do.php?img=80764

The upwind is a first order accuracy numerical scheme, thus the numerical dissipation introduced in the elements is higher. It is more robust, but you will lose in terms of accuracy as compared to the high resolution (that is 2nd order) for example.

[cfdesf1990]

Thank you, highorder_cfd. I got the point.