I have a problem with deforming mesh. When translating a structure (located centrally in a structured mesh) in a circular motion, folds starts appearing in the mesh. For each such circular motion the folds are getting larger and larger, and seems to result in the creation of negative volume elements in the longer runs.

Is there any way to ensure that the mesh carries no history of previous deformations, that is, once the structure in the mesh has returned to it's original position, the mesh should return to it's original form as well.

Any help is muchly appreciated.

Anders T. Svendsen, Aalborg University, Denmark

I forgot to mention that I am using CFX 10.0 and that I use fortran routines to govern the mesh deformation, by moving the structure and setting the mesh stiffness in the domain.

Hi,

Large mesh motion is difficult to do in CFX as it is difficult not to fold the mesh while doing it. Really the only option you have is to start being tricky with the mesh stiffness. Maybe if you locally increase the mesh stiffness near the moving body it can help? You can also do things like making the mesh stiffness higher for small elements or some combination of small elements and proximity to the moving body.

Glenn Horrocks

Anders,

As Glenn has suggested, you can increase the stiffness of the mesh in the domain. What you want to make sure the motion of the mesh is properly diffused away from the moving body. A few things you can try are:

1. Mesh stiffness - you can try setting the mesh stiffness as a function of wall distance and volume of finite volume. [1]
2. Transient timestep - as mesh motion is only available in transient simulation, by reducing the timestep, you effectively reduce the motion of the mesh. This allows the mesh displacement to converge easier and faster.
3. Mesh displacement equation - either increase the coefficient loops and/or lower (tighter) convergence criteria for the mesh displacement equation (Under Solver Control -> Equation Class -> Mesh Displacement). This should the same net effect as reducing timestep.

You can try one of the above or combination of them and see which one works better for you.

Good Luck!

jakjak

Ref: [1] ANSYS CFX-Solver, Release 10.0: Modelling, pp. 18-19

Thank you both for the feedback.

I am currently meddling with the mesh stiffness (1[m^(2+n) s^-1]/(wall distance)^n for n=1,2,3..) which reduces the problem, but doesn't quite resolve it.

I will try to reduce my timesteps and see if I can optimize the solver criterias as jakjak suggests.

Thanks again,

- Anders