Mesh Folding ... different experience!
2 Attachment(s)
hello dear CFDonline users!
I want to study on interaction of marine risers and water flows surround them (FSI problem)! So I decided to use Ansys MFX capability, but now I’ve faced with some problems: mesh folding! I’ve studied advices have been written on the forum, but somehow they are not very useful in my case. There are 3 main advices: 1)Increasing mesh quality: I think my mesh quality is ok! 2)Increasing mesh stiffness: I changed mesh stiffness near small volume (model component = 1000), but results didn’t change! 3)Decreasing time steps: I’ve uploaded two of my out files here. It seems by decreasing time steps results don't change! Let me know your idea please! … and another question: Does ‘under relaxation factor’ impress mesh folding? I set this factor to 0.5! Is it appropriate or not? Thanks in advance … Pouya! 
You might have to change your mesh deformation to 'unspecified' for the regions that are connected to multifield region (wall). If you give 'stationary' option to the moving walls, the mesh will definitely fold.
Also, a model exponent of '1000' is of no use as the stiffness values range from 1e15  1e15. So it doesn't matter how much exponent value you give. But first try the default 10 and then go for 20. In the expert controls change 'mesh displacement diffusion' to value of 3. depending on your elements monitor the orthogonal angle, which should be close to 90 for hex and close to 60 for tetra. HTH 
Please post an image of what you are modelling and a description of the sorts of motion you expect to undergo.

3 Attachment(s)
Hi & Thanks for your responses!
I’m studying a vertical riser vortex induced vibrations (VIV) under sheared current. The riser was made of a 9.63m brass pipe with an outer diameter of 0.02m and a wall thickness of 0.45mm. It was pinned at its two ends and the tension imposed on the two ends was 817N. Dear Mr. Galimutti this is why I think surface and bottom of domain (which are connected to multifield region) wouldn’t be affected by mesh deformation. I changed 'mesh displacement diffusion' to value of 3, but there was not a big change in results. Dear Mr. Horrocks let me say about VIV phenomenon. When water flows around a cylindrical body like the riser, it separates around the surface of riser. It frequently does so in an alternating series of vortices called the von Karman vortex street. This is known as vortex shedding. The effect of these vortices is to exert alternating forces on either side of the riser. If the periodicity of these forces coincides with the natural frequency of the riser string, a powerful resonance can be set up. I hopefully wait for your ideas. Thank you! 
I am well aware of von Karman vortex streets.
What motions does the cylinder possess? It sounds like there are no rotational modes. What about translational? X and Y (assumign flow in the X direction)? or just Y? 
X is in the flow direction and Y is the cross flow direction. Z direction coincides with riser axis. Cylinder has no motion at first. Its transitional degrees of freedom are constrained at 2 ends in X and Y directions (and Z direction at lower end of riser) and the tension of 817N is imposed on upper end of riser in Z direction. Rotational degrees of freedom are available at constraints. After vortex shedding riser would start to vibrating in both X and Y directions.

I see. How big are the motions relative to the cylinder diameter? Also, you say rotation is not constrained  does that mean the cylinder can rotate about its axis or some other axis?

5 Attachment(s)
Thank you for your reply! Yesterday, after your post, I tried my solid model without any rotational degrees of freedom. Unfortunately results were the same.
I post the RMS A/D ( normalized instantaneous vibration amplitude) pattern of crossflow response along the riser in the case of sheared current of U2=0.42 m/s and U2=0.84 m/s (These figures have been extracted from a paper written by Huang, Ching Chen & Rong Chen!!!). I ‘ve no more information about flow direction motions of riser. Thanks for your promising responses! 
The charts do not define the variables so I do not know what they are referring to.
But it is starting to look like this case is best done by a region around the cylinder which is quite stiff, so the motion can be absorbed by the larger mesh elements further out. You can do this with things like a mesh motion stiffness parameter which is a function of distance from the wall. 
3 Attachment(s)
Thank you Mr. Horrocks for your patience!
As you said I changed my stiffness. I used this function: [1/wall distance], but mesh folding occurred again! I changed my solid model and increased number of elements but results didn't change! These are pictures of Interface region after mesh folding! & another mesh stiffness function: [1/wall distance^2]. I tried it and I faced this problem: DIVIDEBYZERO 
What do those images show? I have no idea what that is.
Have you tried a smaller time step? 
What was your minimum orthogonal quality? You can see the 'min orthogonal quality' values in the monitors. Minimum orthogonal quality decrease with iterations or time (if it's transient) and once it falls below 5 or 6 you'll likely have mesh folding.

Thank you for your help! I tried your ideas, but I still face the same problem! I decreased time steps ... I found out smaller time steps would result in larger "negative SECTOR volume" and "negative ELEMENT volume"! I even tried larger time steps!!! Time steps larger than 0.025 sec would result in "Floating point exception: Overflow" error!
I tried coarse elements and decreased mesh density near solid boundary. According to mesh statistics (out file) minimum Orthogonality Angle in my case is 60.6 [deg]. I'm really confused! 
Minimum orthogonal quality of 60 is good. what kind of wall boundary condition you used at the top surface, is it given multifield too? i guess, due to tension the solid deforms in Y and hence shall the fluid. from what you said you only gave multifield to surface and bottom walls. I believe the top one is causing problems. When you see negative volume elements you should be able to see the locations. See where in you model negative elements are developing?

Problem in solving ansys FSI tutorial
hello everyone,
I am solving ansys tutorial to learn FSI, but in upto structural setup i solved it correctly but when i started with ansys cfx, pick face command is showing inactive which i want to create named selections. any body please help me sort out this problem. 
Hi everyone!
In the past few days I did something: I increased time steps to a value of 0.018 sec & changed turbulence model to SAS SST. My model used to crash after the first stagger iteration but now it works for the second stagger iteration and then it crashes. So I can check mesh quality after first stagger iteration! You were right Mr. Galimutti. It sees not very good! ++  Mesh Statistics  ++  Domain Name  Orthog. Angle  Exp. Factor  Aspect Ratio  +++++   Minimum [deg]  Maximum  Maximum  +++++  Default Domain  69.0 OK  10 ok  97 OK  +++++   %! %ok %OK  %! %ok %OK  %! %ok %OK  +++++  Default Domain  0 0 100  0 1 99  0 0 100  +++++ after first stagger iteration: ++  Mesh Statistics  ++  Domain Name  Orthog. Angle  Exp. Factor  Aspect Ratio  +++++   Minimum [deg]  Maximum  Maximum  +++++  Default Domain  29.8 ok  10 ok  540 ok  +++++   %! %ok %OK  %! %ok %OK  %! %ok %OK  +++++  Default Domain  0 1 99  0 1 99  0 1 99  +++++ I guess I have to change my mesh. I will write about the results. Thanks! 
one possible FSI folding mesh solution
Hi Pouya,
I recently had the same folding mesh "error 3840" problem. It was caused by the numerical instability of the fluid and solid "bouncing" back and forth with increasing amplitude until divergence and the wild mesh distortions you see. What fixed it for me was the knowledge resource video "2022119  Stabilizing strongly coupled 2way FSI simulations between FLUENT or CFX and Mechanical" :) Hope it works for you. You have to use trial and error to find just the right amount of damping so that it converges but also gets an accurate solution, I believe. My model is much smaller and liquid much more viscous than yours, but it could still work. 
All times are GMT 4. The time now is 20:03. 