Learning Forum

[destroy]

Hi everyone,

I am modeling Fluid- structure interaction phenomenon in the human tissue - aortic valve.
Generally I solved many problems with convergence and so on, but now Im having a difficult time with the structural side.

I applied a frictionless contact between the flexible walls, to avoid their collision - for the better moving mesh operation on the fluid side.
It worked very well, till I got the message:

The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.

Ofc I was reading about it and tried several ways to overcome the problem:
- reducing time step size
- in Analysis settings, changing number of substeps from 1 to 5
- in System Coupling, changing data transfer under relaxation factors
- analysis settings -> nonlinear controls -> stabilization - I tried to modify these settings

However, nothing helped.

Do you have any other ideas what could I try? 
I am also wondering if there is any other way to avoid structure collision than incorporating the contacts. Maybe some specific boundary condition / implementing construction geometry?

 

Kind regards

Destroy

[BenjaminStarling]

Hi Destroy,

How is it that you are certain that the contact is causing convergence difficulties? Are you solving with any other forms of non-linearity?

Not knowing a whole lot about aortic valves, how much contact is expected? Is the force transfer across the contact large?

There is pretty much no other methods other than contact for modelling body interactions in a structural solve. You can use joints and constraints but these typically do not model such scenarios accurately.

I do not have any knowledge on CFD or system coupling, but can definitely help you with contact related issues as well as non-linear structural analysis.

Your project sounds very complex. I would be interested to hear more details.

[destroy]

How is it that you are certain that the contact is causing convergence difficulties? Are you solving with any other forms of non-linearity?

Hi Benjamin, I dont have any other nonlinearities, material is linearly elastic. Im sure because Im quite familiar with such analysis like the one Im having problems, the only difference is added contact.

Not knowing a whole lot about aortic valves, how much contact is expected? Is the force transfer across the contact large?

The contact between the leaflets - I added it just to avoid the leaflet collision or penetration. This is for the purpose of the fluid side convergence - when the leaflets are connected/'penetrated", the fluid domain can collapse and there may be some problems with the moving mesh in Fluent. Thus I incorporated contact to avoid this problem - this way Im constantly having some small gap between the leaflets and my moving mesh model in Fluent works good.

Your project sounds very complex. I would be interested to hear more details

My project is related to the real aortic valve - the fluid-structure interaction. Ive got two solvers - Mechanical and Fluent. the data from fluent (integrated pressure field=force) is transferred to mechanical many times in every timestep till the transferred data as well as indivifual solvers are converged. The inlet velocity and outlet pressure in the aorta is changing in time.

 

There is pretty much no other methods other than contact for modelling body interactions in a structural solve. You can use joints and constraints but these typically do not model such scenarios accurately.

Thank you for the advice, could you tell me a little more about it? The contact itself isnt really necessary in aortic valves - just I want to avoid collision and remain some gap between the valve leaflets. 
And one question @Benjamin, from your experience - maybe it will be easier to achieve convergence when I will implement additional thin  cuboid bodies between the leaflets, and implement Contact between these and leaflets? I mean - maybe it will be easier to solve the nonlinear contact that is between the flat stationary wall and tricky-shaped leaflet, than between two tricky-shaped leaflets. What do you think? Below I attatched undeformed leaflets

 

[peteroznewman]

Hi Destroy,

Changing Frictionless to Frictional contact and using a small friction coefficient can help stabilize the mechanical solver and give it a better chance of convergence. This is especially helpful in structures that have low stiffness where the friction reduces chattering in the solver as it searches for equilibrium.

Another idea is that contacts can have an offset included in the definition. A small offset would allow the leaflet edges to have closed contact elements while there is still a small offset between the solid elements. I am not a CFD expert, but this might help the fluid mesh from collapsing to zero thickness and help the Fluent solver to continue. There would be some leakage if you use this method, but you can use a small enough offset where the leakage is insignificant.

Kind regards,

Peter

[BenjaminStarling]

I second Peters comment regarding frictional contact. Just a small coefficient can solve non-convergence issues in some applications.

My other comment would be timesteps. In a non-linear static structural I have often used up to 1000 substeps just to acheive convergence.

You are probably correct that a pseudo-body between the leaflets will help with convergence, but I would not be confident implementing such a solution as it would be difficult to understand any influence it is having on your results.

Another factor is the time step controls. You can set the contact to Predict for Impact. Although Im pretty sure the system coupling overwrites this setting so it may be useless/unavailable for this case. The next image shows the offset Peter mentioned at the bottom of the details window.

[destroy]

Thank you @Peter and @Benjamin,

 

Surely I will try the frictional contact! Do you have an idea how to find the appropriate friction coefficient that will not affect much the results and will lead to convergence? Maybe just do some trials? Im asking because I have to wait about two weeks till one trial reach the critical point (nonconverged timestep) *

Yeah, the offset is exactly what I set to have some gap im my model

 My other comment would be timesteps. In a non-linear static structural I have often used up to 1000 substeps just to acheive convergence.

This may be a good idea, but using 20 cores (HP Workstation) and 1 substep, the one cardiac cycle gets about 3 months to calculate. I tried with minimum substeps=10 and maximum=30 and I could calculate only 1 timestep more (1 cardiac cycle is 10k timesteps) *

You are probably correct that a pseudo-body between the leaflets will help with convergence, but I would not be confident implementing such a solution as it would be difficult to understand any influence it is having on your results.

I think (I will check it) that on the fluid side it could have non affect when I dont subtract the fluid domain by these bodies (which ofc willl make no sense). On the structural side - maybe there is some trick in Mechanical as setting the body as construction body?

Another factor is the time step controls. You can set the contact to Predict for Impact. Although Im pretty sure the system coupling overwrites this setting so it may be useless/unavailable for this case

The general timestep size will always be the one set in system coupling. But, I can set for example 5 substeps per timestep, it will work the way that mechanical will have more than 1 substep per timestep, just the data is transferred at the last substep (and computational time will be greater).

 Thank you again @Peter and @Benjamin, I will check your ideas as soon as possibly!

* here I just wanted to add,  that I wrote the results two timesteps before the solution collapse, but not every change in mechanical support the restarts,  for example the contact changes do not support restarts (nr of substeps supports it)

[BenjaminStarling]

I would start with a friction coefficient of 0.1.

Regarding timesteps and substeps (I am unfamiliar with system coupling) if you can set more substeps for mechanical when you know the leaflets will be in contacts, especial when the status changes from open to closed, this will help with convergance, hopefully not costing too mcuh computationally. I imagine the computation time is largely CFD?

If you were to use that pseudo contact surface, you can create "rigid" bodies to build the contact surface on. This is essentially equivalent to a construction body to the APDL solver, but not sure what influence it will have on the system coupling. You can use a real shell body with very low thickness, youngs modulus...etc. and then fix all displacements/rotations on that and use it as a contact surface. This will essentially act as a rigid surface and can be acheived without APDL commands.

[nindoumon]

Hello, I also did FSI of the aortic valve. 

Recently, I met many convergence problems and highly distortion problems.

Actually, in order to get a good contact deformation, maybe you should try to add the radius of the Pinball Region.

 

Also, I really hope you can look at  the problems of mine: /forum/forums/topic/update-failed-for-solution-component-in-system-coupling-2-way-fsi-of-aortic-valve-simulation/?order=all#comment-13dac592-0f60-477d-aa25-ab6700a1bb8b

If you have answers, please help me out of these problems. 

Anyway, we are fighting for the some problems. Thank you very much. 

[nindoumon]

Dear peteroznewman,

Thank you for helping us about ANSYS problems. 

I also met many problems about the FSI of aortic valve. 

My problems page site: 

/forum/forums/topic/update-failed-for-solution-component-in-system-coupling-2-way-fsi-of-aortic-valve-simulation/?order=all#comment-13dac592-0f60-477d-aa25-ab6700a1bb8b

I have attached the achive file in the web page.

Please help me. 

[destroy]

Hello again,

Now Im trying different settings as below:

- setting frictional contact instead of frictionless
- setting contact normal stifness as manual, with value 0.1 
- adding cuboid bodies between the leaflets (as I was describing)
- trim contact = off

These things practically do not change the solving time. But - I will try solutions that (probably) will change the solving time:
- option: add offset, ramped effects
- contact options -> time step controls -> predict for impact
- analysis settings-stabilization=constant, method=energy + activate for first substep = yes

Please assure me - for the above three options, is it necessary to set Mechanical number of substeps as greater than one? Im not sure, because in System Coupling we've got coupling iterations. I mean, each timestep consists of several coupling iterations, in the every such iteration Mechanical and Fluent is solved. Thus Im not sure if it is necessary to increase Mechanical number of substeps cause in the every timestep Mechanical is solved several times, sometimes over 20 times.

 

 PS
@nindoumon Im pretty sure that you should use some stabilization mechanisms, as: Stabilization factor in dynamic mesh panel, under relaxation factors, proper number of fluent and coupling iterations etc.