[Kina]

Hey Guys,
whenever I start a 2-way FSI in Fluent, my solution tells me that only 1 percent of the area has been mapped. Has anybody experienced this kind of problem before and knows how to solve it?
Thanks!
K

[stumpy]

As a quick check just run for 1 step then load the Fluent and Mechanical results in CFD-Post and look at the two sides of the FSI interface. They should overlap, but there must be a gap if you only get 1% mapping.

[Kina]

Thank you very much!
I am a little confused. I just tried to build the exact same fsi again and it worked out perfectly. At least the percentage of mapped area. Now I only have to figure out why I get mixed error codes because of negative volumes or distorted elements in my static analysis. The model is properly constrained meaning one fixed support and the rest is fs-interface. Stumpy, do you have experience in setting up 2 way fsi in fluent? I am dealing with this problem for almost 3 weeks now and it is really annoying

K

[stumpy]

Could you give a quick summary of the case.

[Kina]

Sure, sorry.
The setup is a hydrofoil made of fiberglass in a flow volume of water with speed = 10 m/s. Since it is made of plastic, it is deflected very much and I get negative cell volumes. Then I improved my model and got highly distorted elements. Then I removed nearly all skewed cells in my volumes and now Fluent throws a floating point exception. The set is showed in the picture.
I can send you the files for sure if you have a free minute to look at it.
I suppose it is due to the large deflection since it runs smoothly for air as fluid. That's why I chose to apply the forces and deflections ramped for 50% of the iterations. However, at iteration 15, I get the floating point error with an error in pressure correction. Lowering the URF or choosing a different p-v coupling did not have any effect on the results. I use a tet-prism mesh created in ansys meshing with an inflation first layer thickness of 1e-4m for k-epsilon with enhanced wall fn. Everything runs good until inner iteration 15 when k and continuity of fluent freak out.

[stumpy]

Probably the classic FSI instability. Create a monitor for the pressure integral on the hydrofoil. If it's oscillating and diverging from one coupling iteration to the next within the same time step (not one time step to the next, and not one Fluent iteration to the next) then it's an FSI instability. Solution Stabilization under Dynamic Mesh > Solver Controls is used to fix this, but it's not that easy to use. If you can get on the ANSYS Customer Portal and search for "Fluent FSI" in the training section then you can download the FSI training material which will cover this.

[Kina]

I didn't know there was a "classic FSI instability". However, I read about stabilization when using incompressible fluids. I have set my volume stability factor to 0.1 and had Fluent repair the last left-handed cells of my mesh. It is currently running. I am not expecting it to work now but I hope it gives at least a different error statement
Thanks for now!

EDIT: Still crashes. Error Code: 2 now.

[Kina]

Okay, it is still giving me various errors but I don't seem to find the cure for the virtial mass added effect. Playing around with the URF did not help and switching to transient also did not have any effect. I read in this thread a lot: http://www.cfd-online.com/Forums/cfx...-fsi-case.html
However, i don't manage to find a way to manupulate the mass flux pressure coefficient. Does is also apply to my problem?

[stumpy]

The Solution Stabilization value (when using the coefficient based option) is the same thing as the mass flux pressure coefficient. You'll have to play with this value and watch the response of a force monitor point on the FSI boundary.

[Kina]

First of all, thank you very much for your help, stumpy!
The solution stabilization kinda seems to work. I employed a UDF that ramps up my velocity to avoid a large step of the pressure at the interface. Now I get a negative volume error at the iteration where it was originally about to crash. Does using smaller time steps help now? I am currently ramping the velocity from 0 to 10m/s in 20 steps aka 0.5s and then keep 10m/s for another 20 steps. Should I choose a smoother ramp or rather increase the overall number of time steps?

[stumpy]

When you get the negative volume it's important to find out why. Was a force monitor point oscillating from one coupling iteration to the next (FSI instability), or is it just that Fluent isn't handling the imposed displacement (so force would be smooth and well converged, but the mesh becomes too skewed)?

[Kina]

It is some kind of weird what's happening in the calculation.
This set of data was taken with two different stabilization factors for a velocity change of 0.3m/s per timestep.

Here, it overshoots slightly and has a slight bump in the middle of iteration 4. This causes the pressure correction to freak out or the continuity gets larger.

this is from the last calculation. I ran it with only 15 fluent iterations per inner coupling iteration so it could not recover from the overshoot properly. This caused very high pressure at the interface and the mechanical part dropped the work. I figure it could work if I am able to kinda damp out the straight overshoot and let the pressure drop more smoothly with the velocity change. Ramping it up over 60 timesteps, however, did not turn out to be too reasonable.
I hope there is any solution to this.
Thank you!

[Kina]

Apparently, the divergence and hence the negative cell volume has nothing to do with the choice of time step. This is a screen I took from the latest calculation using time steps of 0.005 and 120 steps to reach full velocity.

It's just weird since nothing is oscillating. It just breaks apart at a random point.
Now that I think about it, it looks like it has something to do with the moving mesh. So elements may get very skewed and they cause this pressure explosion. Is there any smart way to prevent something like that? As far as I know, inflation layers are mostly skewed.

[stumpy]

I think you are right - probably the mesh becomes skewed and causes the flow solution to fail. By the way, if you are fully converging the pressure/force in each coupling iteration (not coupling step) then there's no point in using Solution Stabilization.
So to fix the mesh I would use version 15.0. 14.5 uses a cell centered solution for calculating the displacements but 15.0 uses a more robust node based solution.

[Kina]

Do you know if there is any valuable FSI meshing tutorial or a set of tricks and tips anywhere online? Or is it more like iteratively trying to get a mesh that is not skewed after 40mm tip displacement?

[stumpy]

I don't know of anything specific for meshing with FSI.

[Kina]

Alright, then I'll see if I can get this guy to work. Thank you very much for all your suggestions. I will let you guys know how it turned out and what the problem probably was.
Alex