Negative cell volume detected - Sugestions
 

Hi. I started working with dynamic meshes and some problems came up such us the negative cell volume. I already understood the root of the problem and I'm looking forward to suggestions in order to fix this problem. The attached file represents my problem. It's an airfoil that moves on the vertical axis without rotation. My questions are: What techniques should I use? Is the mesh appropriated? Is any UDF coding needed?

EDIT: Looking for something like this: https://www.youtube.com/watch?v=2N1FJBwDlOg

Welcome to the world of dynamic meshing. So, if I understand your problem correctly, your airfoil is translating up and down, right? I'm just trying to get some more info here.

As for the negative cell volume, are you experiencing it as you are running the simulation, or when you "preview mesh motion"? I know how to view it from the former, but not so much the latter.

Lastly, what are your dynamic mesh settings? We could suggest things to you, but they wouldn't really help if we don't know where you are starting from. As a good starting point, I find it best to enable "Smoothing" and "Remeshing" in the "Mesh Methods" section ("Layering" is best for hexahedrals, which you don't have). If you click the "Settings" button, I usually end up setting the "Method" to "Diffusion", as I find it gives pretty good results for a multitude of applications. For the "Diffusion Function", you are going to have to see which case is more applicable to you, and then apply it (read through the manual and/or try both to see). I find that setting the "Diffusion Parameter" to "2" gives good results (the "Diffusion Parameter" can only be set from 0 to 2).

Hope this helps, and post whatever worked for you!

First of all, thanks for your suggestions @RaiderDoctor. The error was detected in the preview mesh motion, since I use this feature first to see if there will be any problem in the calculation process. I have dedicated this last week to understand the basics of dynamic meshing by testing every feature with different parameters. You recommended the diffusion method that in my case was not suitable, since the required time step to have a successful result was very small. The problem here is the leading edge, where the mesh shows some irregularities and with a certain time step, the error comes up. Reducing the time step helps in some situations, but sometimes the time step is so small that will make the calculation process really long. After testing almost all parameters, I found out that there must be the perfect balance between the mesh configuration (size, methods, inflation), time step and dynamic mesh settings. In my case, the "Smoothing" Spring method was the most efficient where I used a very low spring constant (0.0001) with a high number of iterations. In the remeshing, the default settings were enought. Layering option was disabled.

Thanks once again for your answer,

Emanuel Camacho