FSI Structural convergence problem
Hello there, I'm new to this forum as well as relatively new to ANSYS and CFX. I am attempting to simulate the deformation of a hyperelastic material shaped like an airfoil due to the airflow around it. Its a membrane that is looped around a trailing and leading edge support, basically a rubber band around two poles. For the membrane I have used the ANSYS predefined material of Neoprene Rubber.
I have tried to do this as a pesudo 2D analysis by the usual sweep method for the mesh in CFX, and by constraining the membrane in the structural set up so it cannot deform in the Z plane.
The CFX side has an initialised domain with the same flow conditions as the inlet, with the air at a preset velocity and angle of attack.
Whenever I conduct my FSI, my solution for the ANSYS solver always seems to diverge and result in an error stating that the mesh displacement could not be exported to the CFX solver. The ANSYS out file indicates that the solution has diverged rapidly. This is especially true whenever I set the initial conditions using the results of a previous CFX-only run with the same conditions.
I believe my problem stems from my structural set up, as I have found that (in analysing the transient solver on its own) whenever I apply a ramped uniform pressure to the upper side of the membrane, the structural solver will solve the displacement of the membrane quite happily. However when I try to apply an instantaneous pressure, the solution fails to converge, even for a very small timestep.
Does anyone have any advice on how to change the structural set up so it converges for an instantaneous pressure? Would it be better to somehow prestrain the membrane (which I admit I do not know how to do) before attempting the analysis? Or to start the FSI with a still, i.e. no flow, initial domain and let the flow increase gradually?
I would pre-stress by using a steady-state 2-way FSI, which you'll then have to restart as a transient.
Thank you for the reply. So just to clarify; I should run a steady-state solution, and then when restarting as transient define the initial conditions as the output from the steady state run (I have the transient and steady-state FSIs as seperate systems though off the same geometery and model)? Or just restart with the current solution data?
I've managed to run my first full steady-state and transient FSI. I realised that I had left the fluid turbulence model in laminar mode, which I changed to Shear Stress Transport, as well as drastically reducing my flow velocity from 10m/s to 1 m/s.
I'm going to try attempting this again at higher flow rates, along with what you've suggested. Would it be beneficial to attempt what was outlined in Solution #2022119? I saw you mention that in another thread and so had a look.
The first one - the transient run will use the steady state solution as the initial condition. This restart is not obvious. Try searching this forum for ANSYS.mf or TIMINT and you should find something. Make sure the transient boundary conditions represent a smooth continuation of the steady state solution - don't make any sudden pressure changes.
Solution 2022119 is probably needed for the transient solution. See if force/displacement monitor points on the interface oscillate and diverge at the start of the transient.
As a related question, would you please comment on the choice of suitable Mass flux pressure coefficient (following the instruction of 2022119 to achieve convergence)? This technique has helped achieve convergence, but I am not sure about the proper use of it.
Take my case as an example. My simulation has a sinusoidal actuation of 50 Hz, and I expect 5 sinusoidal waves in 0.1 sec for the flow rate across openings; please see the attached. I've tried three different pressure coefficients (PC), and the flow rate can differ significantly (Although the larger PC seems to give a better-looking sinusoidal wave). Is there any rule of thumb to pick a reasonable value?
Thank you for sharing your experience!
There's no reliable rule of thumb. All values should give the same solution *at convergence*, but different values will converge faster/slower. Use displacement/force monitor points to judge convergence, not residuals, and make sure those monitor points are fully convergence within each timestep - so you may need to force a certain minimum number of coupling iterations and/or CFX coefficient loops. The best value is the one that gives fastest convergence (smaller values) but does not oscillate/diverge (larger values).
I am modeling transient blood flow in a simple flexible tube,
The pressure distribution in this tube is oscillatory in time like this function: P= 1000*sin (t) (pa)
(This is not absolute pressure; absolute pressure is equal to 13332.2 pa)
When the pressure is positive my FSI analysis does not have any convergence problem but when the pressure is negative and its magnitude is greater than 100 pa it diverges and breaks the mesh and the broken mesh indicates that the tube is collapsing,
I also applied a constant pressure of -1000 pa to the inner wall of the this tube in the ansys structural by itself and it converges very well with a maximum mesh displacement of 10^-6, and the tube diameter is 0.3cm, why it is collapsing completely in FSI analysis,
I also decreased the under relaxation factor in cfx external coupling tab and decreased the time step size and set the Newton Raphson option to unsymmetric but none of them help.
interface convergence monitor:
structural convergence monitor:
Please help me to fix this,
Hope to see a response.
Hi Dear mrkmrk
I can suggest one thing to you at the moment.
Try changing your inlet boundary type from pressure to velocity or mass flow rate type. it can help if the source of your problem is negative pressure.
there are some well known velocity profiles for bio applications, like womersley velocity profile.
FSI Structural convergence problem
Thanks for your response,
my inlet boundary condition is Womersley velocity components,
Did you verify any FSI simulation results by Womersley analytical solution before? (Did you face this problem before?)
I'm trying to do that, but as you know in this analytical solution there are time intervals which in them the pressure is negative,
Both fluid and solid parts converge separately but when they are coupled solid part diverges,
All of the FSI converging problems that are reported in cfd online or other web pages are about diverging in the first/second/third time steps but my simulation diverges only when the pressure is negative.
2 way FSI and relative negative pressure
After testing the effect of all convergence control parameter that I know, I have a question:
Can Ansys model the behavior of flexible tube under the relative negative pressure by two way FSI simulation?:confused:
Everyone that has this problem should read this forum information first,
"Initializing transient analysis using static analysis in two-way FSI simulation ":rolleyes:
I haven't encountered such problem befor.
Did you solve this problem using initialization by static(steady) solver?
I do not know whether my experience about such an error could help someone or not, but I fixed this problem from ansys mechanical by changing the standard shape check to aggressive.
I hope It could be beneficial for someone
I will to try,
|All times are GMT -4. The time now is 00:24.|