Hello,

I have been trying to perform a really simple FSI simulation with water flowing past two closely spaced cylindrical shafts. I used CFX tutorial # 21 (Oscillating Plate) as a template, but CFX multifield solver is just not cooperating. I changed the step time, meshing options, etc but I keep receiving a fatal error. The project files and results (.out) files are contained in the link provided with this posting. I kindly ask that you review them, if possible, and then advise/assist me on how to proceed (other than throw my laptop across the room). Thank you for your generous time. FSI project file link

Best,

Aaron

Hi Aaron

Here are a few tips for your FSI simulations.

-- Do you really need a two-way FSI for this problem? Just reconsider this question. Can your problem be solved with one way coupling?

-- Run CFD and FEM solver separately for the same problem without FSI coupling in order to see if all settings in your models are alright. If your uncoupled solution do not converge or give errors then your FSI will never converge.

-- Use your uncoupled CFD solution as an initial guess for the fluid field in the FSI simulations.

-- choose proper time scales/steps for both fluid and structure solvers. See/think if they both have to be same or not. Time step (DT) should be chosen on the basis of frequency (f) you want to resolve. Your DT should be 10-20 times smaller of the corresponding time-period. Time in simulations is not the clock time rather it is a physical time scale of your problem (this is due to the fact that the rotation of earth around its axis or around sun has nothing to do with your problem).

-- Assign your boundary conditions in the CFD solver carefully. For instance, in your model there is no outlet. Think what will happen if you keep on pumping a liquid/gas inside a box or balloon which is rigid/inflexible? Yes it will explode and so the solver. This is just an analogy and not a proper reasoning for the crash. The solver might be crashing due to many reasons. One reason, I see in your model improper boundary conditions.

-- Other reasons for the crash may lie in the fact that the flow rate, dimensions and corresponding flow model (Laminar/turbulent) for the CFD domain are unrealistic. To me it seems that you have a huge fluid force acting on the solid body. You may estimate roughly this force analytically and try to run the FEM simulation (without FSI) with this estimated force and consequently determine the reasonable time step needed by the FEM solver. Your time-steps may be too large and the grid is deforming too much.

-- If you have very large structural deformation, it is very important that you give little freedom to fluid-side grid to deform properly. That is why you should move away the symmetry (and other boundaries, if needed) boundaries in your problem far away from your deforming body. Otherwise you will have very acute angles in the fluid-side grid and hence the grid will be highly skewed.

-- Use proper numerical parameters in the solver control area of CFX. Max. number of Coefficient loop iteration should be around at least above 8-10. There is a danger choosing insufficient iterations. Have a look at Naveier-Stokes residuals in CFX, within each stagger iteration, your residuals must come to reasonable levels. Set at least 10 stagger iterations per time-step and use low under-relaxation factors for the stagger iterations.

-- On the structure side, employ beta-damping for the frequencies you do not want to see in your solution.

Finally, carrying out an FSI analysis can be very challenging. Even if your simulations run without crash, you have to know a few basic things which ensure that your results are close to reality and depict actual physics.

Otherwise, one can readily draw wrong conclusions, e.g. simulations results do not agree with that from the experiments and other similar lousy conclusions.

Remember: simulations only do what you ask them to do and simulations demand much more that just click-click operations.

I hope this mail will help to properly formulate your problem.

cheers

One other thing to check - mesh stiffness in CFX. You can define this by stiffening small elements or by stiffening elements near the wall. See where the elements are folding over in Post and see if switching the stiffness definition will help. You may also need to play around with the exponent as well - reduce it to 1 or 2, and increase it beyond the default of 10 to see if it makes a difference.