[realanony87]

In my steady state FSI simulation of a 3D wing with ansys v11 CFX, I get negative volumes at the trailing edge of the wing. Now the trailing edge is not sharp, but blunt, and since my mesh is structured (similar to the mesh used in the wing-body tutorial of ICEM CFD),
I have high aspect ratio elements right at the trailing edge( around 100) . The elements near the tip on the trailing edge give me the first negative elements in the FSI simulation.
I also have a fine boundary layer which may be causing the problem ( y+=2)
So I am guessing that the elements along the trailing edge which were flat and thin, become curved, but since their stiffness is high , then a problem with solving the node displacements occur . Or is the diffusion equation solved according to the nodes and curvature doesn't play a role ?
I have experimented with different values for the stiffness model exponent (1,2,3,5,10) and both models included in ansys cfx v11, namely distance from the wall and element size. For all values used, I get the same "first negative volume) location being exactly the same, with the same value for the negative volume.

I am thinking of starting the FSI simulation with low inlet velocity boundary conditions and then ramping up the velocity so that the wing deformation isn't drastic between the time steps. but that might take a while considering I have a not-so fast computer and 1.5m elements.
Or maybe there is a suitable CEL expression for my case ? I tried something like:

(1/Volume of finite volumes)^2 *1[m^8 s-1] + (Aspect ratio^4)*1[m^2 s-1]

But I cannot seem to get it to work since ansys complains about division by zero for the (1/Volume of finite volumes) term ( although there is no zero volume in the actual mesh, it works fine for an uncoupled CFD run)

Any help would be greatly appreciated ! thanks

[realanony87]

Picture of folded mesh. Notice that the boundary layer nodes do not move !It seems that the diffusion equation solver is not doing anything

[realanony87]

In ansys CFX Under Solver control -> Equation class settings -> Mesh displacement
I set the maximum coeff. loops to 20 and the convergence criteria to 1e-4 max. Now I do not have any problems and my mesh retains its quality.