[Silmaril]

I was trying to run a simulation with mesh deformation in a HEXA grid. In order to have a simple "bellow-like" deformation motion, I divided the domain in several sub-domain connected by "sliding" GGI interfaces. Unfortunatly I didn't get the "bellow-like" motion but some strange mesh distortion occurs at some boundaries.

To study the possible causes of the problem I made a simplified 2D model similar to the sub-domain that shown mesh distortion:

2D Wedge with low angle (~20°) with inclined walls closing in the vertical direction (see attached figure).
With the settings shown in the figure for the mesh deformation I was hoping to obtain a uniform distribution of the nodes in the lateral walls similar to a bellow-like motion. Unfortunately distortion occurs at the high angle corners (shown in the right part of the figure). I tried different parameters for the mesh stiffness (exponent or values...) with little change in the result (a slightly better behaviour is obtained if the exponent is decreased from 10, default value, to 1).

Anyone knows how can I solve such a problem? (possibly wothout having to impose each node displacement with User Fortran Routines

Thanks

[stumpy]

Under Expert Parameters try 'meshdisp diffusion scheme = 3'. If that doesn't help then it would be best to define the motion of each node using a subdomain, but you don't need User Fortran for that. Create a weighting function that varies linearly from 0 on the stationary boundary to 1 on the moving boundary, then multiply that by the imposed displacement. For a Cartesian aligned rectangle the weighting function is trivial, for a wedge it still not too difficult.

[Silmaril]

Thanks very much, I've tried the expert parameter and the weighting function too, both give quite good results, even if some problem still arises. With this improvement probably I can just run a simulation for long enough till mesh start to degenerate, stop the calculation, and restart with a fresh-new mesh until the motion ends.

By the way, what's the difference between the mesh diffusion scheme 2 and 3? Why there's such a difference in element distortion?

Thank you again

[stumpy]

That parameter changes the numerics of the diffusion scheme. According to the documentation it changes the interior and boundary nodes to positive definite values. Basically I think that means you avoid wiggles in the solution. Positive definite values can give unphysical solutions, but in this case there is no real physics tied to the diffusion equation that is being solved so it doesn't matter if it's "physical". The boundary displacements are explicitly defined (they're not part of the solution), so it's not applicable here.

[vidhya]

hi,
i am quite new to sliding mesh technique. i have done simulation using MFR. can u giv a gist of how to perform sliding mesh in CFX.. i have read about SM method in articles still i dont understand properly... and also in cfx while defining interfaces, we have an option for pitch change. does that have anything connected to sliding mesh??? please help me...

[stumpy]

In CFX you usually don't want to use a "sliding mesh" for an MFR case. CFX has a transient rotor-stator interface to deal with relative motion between rotating/stationary components. Some codes don't have that, so they have to physically clock the rotating mesh, hence you get a sliding mesh at the interface.