Dynamic mesh setting problem
 

Hi all,
I'm working on a 3D wing dynamic bending simulation. Wing motion is controlled by DEFINE_GRID_MOTION, and mesh is generated in ANSYS Meshing. Dynamic mesh is active in this case. I use smoothing and remeshing method. But I often have negative cells problem, and I find that remeshing doesn't work at all, I don't see any mesh part being remeshed. I've read some related posts, but none of them apply to me. There are still some questions confused me:

1/Dynamic Mesh Zones setting problem:
I believe I've seen two posts with opposite opinion on Dynamic Mesh Zones setting. One said that wing (wall) boundary should be set as User_defined, and the adjacent zone such as interior should be set as Deforming; However, the other post said if I set adjacent zone as Deforming, remeshing method will not work. I'm wondering which of these two statements is right? Does this mean there is a conflict between deforming and remeshing?

2/SET_DEFORMING_THREAD_FLAG()
I often see this code in DEFINE_GRID_MOTION and I know it marks the cells in adjacent zone and set it as deforming. If the later statement in last question is correct, shall I delete this line from my UDF?

3/Remeshing parameters setting
Before I do this wing job, I tried a simpler 2D airfoil pitching and plunging motion simulation. As many tutorials said, I use default settings for Max/Min cell size and skewness. But the result is even bad. After reading official help document, I found sizing function may suit my problem. Has anyone tried sizing function? Is there any additional requirements on grid when using sizing function?

One more question
 

4/Boundary layer and dynamic mesh
I’m using a mesh generated in ANSYS meshing without inflation, and the y plus is very high. However, mesh with boundary layer always face difficulty in dynamic mesh. Does anyone has a solution on this issue?

Dynamic Mesh
 

1. Dynamic mesh objects are set only for boundaries and never for cell zones. So, be it rigid body, deforming, user-defined, or some other, these should be applied only to boundaries. The deformation in the cell zone is determined on the basis of method chosen and options given for the boundary within Dynamic Mesh object.

2. This option should be maintained and not removed.

3. Default settings work provided the initial mesh is of good quality. If the initial mesh itself has a high skewness, then remeshing will fail. Furthermore, the motion in a single time-step should not cause displacement of the object larger than a cell size adjacent to the object.

4. It doesn't matter which tool is used to generate mesh as long as it is tetrahedral. requirements come from wall treatment and not governed by dynamic mesh. However, very coarse mesh implies a lot of deformation before remeshing takes place and that could lead to failure.

Hi vinerm,
Thank you for your reply. Your answer help me a lot. I check the mesh quality and it really needs improvement. I will try again with updated mesh. What's more, for the 4th question, I'm not quite sure which smoothing strategy is suitable for mesh with boundary layer. I used spring in my previous case and set spring constant factor close to 0, shall I use diffusion method instead? Does diffusion performs better than spring on tetrahedral mesh with boundary layer?

3/Remeshing parameters setting
Before I do this wing job, I tried a simpler 2D airfoil pitching and plunging motion simulation. As many tutorials said, I use default settings for Max/Min cell size and skewness. But the result is even bad. After reading official help document, I found sizing function may suit my problem. Has anyone tried sizing function? Is there any additional requirements on grid when using sizing function?

You need to three things. Mesh quality, mesh/domain strategy and optimal settings of re meshing to properly execute dynamic mesh problems. Default sizing function is good enough if you use smoothing with it. Otherwise you may need to optimize this. For more accurate results, one need to trial and rectify.

Hi arunraj,
Thank you for your reply. I tried different settings but they didn't improve much. I think I should reduce the skewness of my mesh. Although the average skewness is 0.2-0.3, the maximum skewness is up to 0.86. And those poor quality cells are around the wing tip, which is also the place with the largest displacement. But I found it difficult to reduce max skewness in ansys meshing. Maybe I should try other meshing tools.

Use dedicated meshing softwares like ICEM CFD or Pointwise. Even ansys meshing is good enough if you plan well.

Sorry for bothering again. I met another problem when I used remeshing. I have marked all negative volume cells in wingMesh.jpg file. Smoothing and remeshing settings are shown in other files. Mesh quality of adjacent zone became very bad. If remeshing is disabled, this problem can be solved but only small deformation of the wing is allowed. something wrong with my remeshing setting or smoothing setting? Or maybe I should use diffusion for smoothing instead?