CFD Online Discussion Forums

CFD Online Discussion Forums (
-   OpenFOAM (
-   -   Problem with interFoam; Wave/wiggle alpha1 behavior (

JonW May 12, 2011 07:48

Problem with interFoam; Wave/wiggle alpha1 behavior
4 Attachment(s)
Dear Foamers

I have a problem with interFoam (same with interDyMFoam) on a non-orthognal (and skewed) mesh :mad:.

The case file is "water_splash.tgz" for the interested. (for the very OpenFOAM newcomers, read the run_readme.txt file about how to run the case)

The mesh is not fancy as shown with "figure1.png"

The case file is typical of what I have to work with, I.e. I have to work with mesh systems where non-orthogonal and orthogonal meshes meets. The case file here is just artificially created, not for any purpose other than to demonstrate the problem with alpha1 and interface compression.

The case consists of water column flowing by the action of gravity, as shown below (time = 0 sec) as shown with "figure1.png"

The problem is shown in "figure2.png" and consist of that a wave (or wiggle) phenomenon occurs in alpha1 where two grid system meets :mad: :mad: (i.e. the orthogonal and the non-orthogonal).
I have the same problems with other types of non-orthogonal meshes, even where zero skewness is present. (The problem also persists when running interDyMFoam).

I have tried everything (I think :confused:),...
I have changed mesh configuration (making cell size in the two mesh system similar in size).
I have reduced time step (very much), reduced Courant numbers (also for alpha1)
put momentumPredictor to yes,
changed nCorrectors, nNonOrthogonalCorrectors, nAlphaCorr, nAlphaSubCycles.

NOTE: The only thing that solves this is if I put cAlpha to zero (“cAlpha 0;”). The result is shown with "figure3.png"

The solution putting cAlpha to zero, might suggest that the problem lies in the interface compression! ?? :confused:. But, as far as I can see, everything is correct for the compression in “alphaEqn.H”, so I don't understand this.

The problem of using cAlpha 0, is that the alpha1 get “diffused” throughout the system, and a clear boundary get "dissolved". Thus using cAlpha 0, is not a solution!

So any ideas?

Andrea_85 May 12, 2011 08:52

Hi Jon,
i do not know exactly if this is what you are looking for but....
i have worked a bit with interFoam and non orthogonal mesh, basically i have been able to find acceptable results by changing the fvSchemes to take into account bad mesh. I found good results using the pointLinear schemes instead of linear schemes for gradient and interpolation. Also leastSquares works fine for my simulation.
Hope this can help you


JonW May 12, 2011 10:02

pointLinear and leastSquares
Hi Andrea and thanks for the reply

Unfortunately, neither

default pointLinear;


default leastSquares;

...solved the problem

JonW February 23, 2013 21:41

how to avoid the problem alpha1 wave
3 Attachment(s)
Dear foamers, I know this post is old, but I think this is important, so here we go (part solution):

I was working on a project last week with interFoam. The system were such that the alpha wave problem should not occur (at least not in my mind), but there it was. In my problem, the aspect ratio of the mesh was greater than 1 (about 3) to save cpu time [aspect ratio = length of cell/width of cell, etc.]. Increasing the mesh resolution (and thus gaining aspect ratio of 1) made the alpha problem to go away.

I tried the same thing with the setup descriped in the beginning of this post, and the wave problem dissapered.

So here you have it,... one way in avoiding the problem, keep your aspect ratio close to 1 in your mesh system (if there is a wave problem).


All times are GMT -4. The time now is 01:57.