[Benji]

Hey @all OpenFOAM users

After quite a long time I came back to using OpenFOAM for an experiment that I am currently working on. In the end, the 3D visualisation will be as important as the computation/the result itself.

Situation: A volume of water (shape: not important at the current stage) falls from a certain height into a basin (shape: not important at the current stage) filled with water. What I am interested in is the height of the water splash that follows the impact, as well as the waves that are generated an reflected by the walls of the basin.

In a first step I just altered the interFOAM dambreak case to a very simple 3D geometry with blockMesh. After that, I let the volume (here: box) of water fall down into the „basin“.



What I was wondering is the direction of the waves that follow the impact: It seems the the propagation of the waves that follow the impact is only in direction oft he x-axis and not (or at least not in the same manner/speed) in z-direction.



I have seen this also in some other 3D dambreak cases (examples on youtube).

Of course I can also upload code/files but I have the feeling that this is due to a rather trivial mistake, can someone help me fix this or have an expanlation?

I’d be really thankful for some help on this, or also just suggestions/ideas. Thanks!

Ben

PS: If someone has inputs to the following I'll take them gladly
2. I’ll change the shape of the basin from the rectangle to cylindric, heart-formed, etc. I think I will use snappyHexMesh. Does someone have tips or a better idea?
3. I will also alter the shape of the water volume to a sphere, „drop“,... Any tips what is a good way to do this?
4. Any recommendation on visualisation tools other than paraFOAM?

[guin]

Quick guess: may you have "empty" boundary conditions for the XY-patches?

[aow]

Benji,

I believe Rodrigo is correct. The default dambreak tutorial is performed as a 2D simulation with empty boundaries. To change this, go to the blockMeshDict and add the "front" and "back" faces, giving them the type "wall". You should add them into the "0" directory boundary condition files ("alpha.water", "U", "p_rgh", etc...) too, using the same conditions as those used for "leftWall", "rightWall", and "lowerWall". Once this is done correctly, all of the boundaries should behave as solid walls.

If that doesn't work, please post a .zip or .tar of your case files or at least provide sufficient details about your case setup so we can better understand what is going on.

Addressing your PS questions...

2. I’ll change the shape of the basin from the rectangle to cylindric, heart-formed, etc. I think I will use snappyHexMesh. Does someone have tips or a better idea?

snappyHexMesh can mesh around any shape that you can make a stereolithograpy (.stl file extension) file out of, which may be done manually (see the stereolithography Wikipedia page for the format and then generate the point and normal vector data with python, Matlab, etc...) or with Autodesk's Inventor (free for students) or other similar CAD programs. There are other options too such as foamyHexMesh.

3. I will also alter the shape of the water volume to a sphere, „drop“,... Any tips what is a good way to do this?

The setFields utility only works for rectangular regions to my knowledge so you'll have to try something different. After a quick search, I found funkySetFields, which seems to be a good option for setting non-uniform internal field values.

4. Any recommendation on visualisation tools other than paraFOAM?

For my work I've found that ParaView is the most suitable software, but I've also tried Tecplot, which makes some very nice looking visualizations of data.

Best regards,

Andrew

[Benji]

Hey

1. Thanks for the tipps, it wasn't exactly the empty patches at the walls, but rather ill defined walls in general, thanks for the direction

2. It did not get to work on this for too long, so far I have the cylindric mesh done still with blockMesh. I will try and post when I'm done with more complicated geometries, thanks for the tip with the stl-files!

3. Yup, funkySetFields seems to be it.

4. Hm, thanks again, never heard of Tecplot, but I'll give it a try.

I'll probably need some time now, but I'm sure I'll come back with more questions/problems/(results). Thanks

Ben

[Benji]

Hey everyone

I got to work on this a bit, although my goals/geometry have changed quite a bit. I still need to alter the initial conditions, but at the moment I have a more pressing thing: So far, I exported the results from paraview as jpgs/pngs and put them together with ffmpeg .

Depending on the angle there are some "un-nice" things like gaps in the surface, opacity where it shouldn't be, wrong colors at the borders between two blocks, and so on (see attachment). Does anyone have the same and/or have any tipps on how to make these images more smooth (some setting)?

Would be great, thanks.

Ben

[aow]

Hello again Benji,

I hope you've figured out how to improve the quality of your images, but if not how did you get that surface in paraview? I've been using the following post's (Multiphase 3D free wave surface post-processing visualization in paraview) instructions (see SirWombat's first reply) to get pretty decent results for the free surface. I do get some "tears" or "holes" in the surface though (see examples below). I've not really tried hard to fix this yet though so sorry I cannot give better advice.

[guin]

Again with a guess: Are you postprocessing a case in parallel? In such case, I'd suggest you to reconstruct the case before post-processing it. ParaView has usually problems with the interpolations across processor boundaries.

[aow]

Guin,

Thanks for the tip! I have indeed been using decomposed cases in Paraview. I'll give it a shot with a recomposed case and post the results when I can to verify if that's the issue.

Andrew

[aow]

I realize this is very late, but I did eventually get around to trying out using reconstructed case data instead of parallel case data as was suggested by guin who was correct about the "tears" in the free-surface contour being due to using parallel instead of reconstructed case data. I've attached an example of a case I reconstructed to show how much better it looks.

Thanks for the tip guin!