[Traction]

Hey foamers,
In various interFoam and interFlow (interFoam with isoAdvector) trials I observed that the damBreak tutorial case does not lead to a steady and stable fluid behavior over time– even after increasing the simulation time to 1000s. I expected to observe some kind of damping which finally results in a smooth fluid behavior but right now I can see a lot of vertices, instabilities and artificial flows arising in both phases. It looks like they are formed in the air phase and pass through the gas/fluid interface to induce vertices inside the water phase.
For testing purposes I extended the damBreak tutorial case to “simulate” a calm fluid by just filling half of the domain with water. In doing so I also observed vertices in a similar manner which is physically wrong in my opinion.
I reproduced that with different OF versions (3.0.x, 4.1, foundation-dev, v1606+)

My main concern is that this disturbance also influences flows with low velocity areas or low velocity flows in general and as a consequence leads to wrong results. I noticed that by simulating low velocity channels.
Consequently I think this is an important topic to have a focus on and to exchange views about.

Has anyone experienced a similar behavior ? What is the reason for this ? Is it possible to achieve accurate results without spoiling physics / numerics ?
Maybe there also some ongoing projects to contribute to !?

[thomasArk47]

Hello,

I'm interested (sorry my english is bad) to analyze your case.

OpenFOAM is a wonderfull toolbox but there are some pitchfalls around numerical behavior. Mainly with unstructured meshes and multiphase flows.

So can you send me all your files related to your case please? I will try to see if your problem falls into something I have already done.

[vatavuk]

Hi,

I think it would be interesting to report that issue in the bug tracking page in this link:
https://bugs.openfoam.org/my_view_page.php

Best Regards,
Paulo

[Traction]

Hi,

I prepared 2 interFoam cases to reveal the main points I am concerned about. These cases were tested with the foundation-dev version.

The first one is a modified damBreak tutorial case. I initialized it with a uniform water level in the whole domain - so I basically excluded the dynamic break to have a more or less static situation. As you can see this leads to the generation of vertices and an unaccountable flow field in general.

The second example is a simple 2D channel with a low velocity inflow. As long as the inflow velocity is above 1.0m/s the flow field seems to be reasonable. By decreasing the inflow velocity to a value of 0.5m/s the oscillations start to form. These effects increase by decreasing the inflow velocity further on.
I attached an example with a velocity of 0.2m/s where you can see that the flow field is not like the expected uniform / parabolic flow. The resulting velocity peaks are above 0.3m/s !
Besides the physical aspects this extends the computational time - especially for large 3D cases.

For both cases I tried different configurations (BCs, turbulence, etc) to eliminate that this problem is related to inconsistent BC´s. By now I was not able to achieve improvements doing so.

As thomasArk47 mentioned maybe this is an expected numerical behavior ? I am not able to judge this because of my limited numerical knowledge so I am very interested to hear your thoughts.

[thomasArk47]

Hello,

thanks for the input files.

I will try to inspect closely your cases.

PS: I have other things to do so don't worry if I take time...

[akidess]

Originally Posted by Traction

As thomasArk47 mentioned maybe this is an expected numerical behavior ? I am not able to judge this because of my limited numerical knowledge so I am very interested to hear your thoughts.

It's a well known problem. Typically in papers you'll find the test case of a static droplet, which is prone to exactly the same problems. Small errors in curvature calculation lead to stresses at the interface. You can find lot's of literature and threads on this very forum on "parasitic" or "spurious" currents.

[thomasArk47]

Hello,

i have a look at your dambreak case and as Akidess says it falls into "something" like spurious current.

Nevertheless, in your case it is not related directly to the surface tension but rather to the density jump via the gravity field (g.X \nabla rho). A few remarks:
1- the magnitude of the oscillations is dependent on the mesh resolution (it converges say)
2- strongly dependent on the underlying integration scheme (mainly spatial one). Both on U and on alpha (it is better to use explicit integration for alpha with low Courant number, something like 0.1, possibly with sub cycling)

It seems that Jasak has recently worked aroung a new procedure to reduce this type of spurious currents. But I believe he didn't released the work (maybe he did it in the naval hydro pack but it is not free of charge)

I will have a look at your pipe simulation in order to check it is the same problem.

[bramDeJaegher]

Hi all

I'm currently struggling with the same issue, are there any updates on this post?

Regards,
Bram