Hi

I am doing a FSI simulation of straight pipe flow using ANSYS-CFX coupling and facing a problem for quite sometime. The problem is related to size of the time-step (here onwards DT). It seems that there is a critical DT when goes smaller than a certain value, the coupling algorithm (i.e. stagger iterations) do not converge anymore. The usual value of DT which works in the simulations is equal to 1/20f, where f is the resonance frequency (first mode) of the structure. For further finer time-steps (e.g 1/32f) the coupling does not seem to work. I tried both shell and solid elements but the problem remains to be there.

From literature, I came to know about a numerical instability known as artificial added mass instability of staggered iterations. Here is the link for this reference:

http://www.mathematik.uni-stuttgart....s/2006pp09.pdf

Did anybody face a similar problem?

Is the problem known to ANSYS users and/or developers??

Hope to seeing a response.

many thanks in advance

The article you reference says that the instability only occurs in sequentially staggered codes. ANSYS-CFX is "strongly coupled" using the article terminology, so it doesn't apply.

With the smaller timestep do both the fluids and solids solutions converge individually (i.e. no coupling?). If you keep reducing the timestep does the problem persist? What's the typical value of f, could you be running into round-off error?

As stumpy mentioned by iterating within a timestep ANSYS eliminated any lag errors due to the sequential coupling. My thought would be that by reducing your timestep you are now able to capture physics which with the larger timestep were missed..perhaps some small scale vortex structures? I would attempt to spatially refine your mesh(s) and see if the problem goes away.

Yes the problem persists if I keep decreasing the time steps. Without FSI both fluid and structure simulations converge very well. I use typically f equal to 1000 Hz.

I also tried a beta damping of 1% (= 0.01/pi*1000) but it does not help. The problm is not related to round of errors. It seems to be a general problem, you may try with any material and fluid and will reproduce the error. But make it sure that f should be equal to the first eigen-mode of your structure.

Refining the spatial resolution does not help. I already tried it. Moreover there is no numerical reason why things should not work on coarse grids. My expereince with incompressible fluids that coarse meshes always produce much better convergence rates and this trend is general and that is why people successfully make use of multigrid algorithms.

Have you tried looking at the solution(flow and structural) in the timesteps before the convergence fails? And when you say it fails do you mean that the solution diverges? Or does it just not get below the cutoff value in the specified number of maximum iterations?

Solution diverges slowly with fluid forces (Fx,Fy and Fz) reaching to unphysical values and finally destroying the grid. It happens within the first time-step so there is nothing to observe before divergence. Note that this behavior can be observed in case of a pipe flow (I did not observe this behavior in FSI of external flows).

A material damping between 0.1%-1% (mp,damp,0.01) causes the solution to converge however giving totally wrong results (dynamics).

Hmm..I've not used the multi-field solver in ANSYS so my knowledge of the exact algorithms used is limited. What type of initial conditions are you using? Also have tried playing with the load transfer schemes?

Dear Dr. Kumar,

Which model are you using on the ANSYS side? Did you set the non-linear geometric parameters; otherwise, ANSYS will be using the small deformation approximation w/o geometry update and this could create the problem you have observed.

Though ANSYS <-> ANSYS CFX communicates both ways, there is no influence coefficient (linearization) between both solvers. Contact your help desk representative for ANSYS CFX and ask for additional recommendations regarding two-way FSI on the pipe flow/blood flow in artery problems.

Which version are you using 10.0 or 11.0?

Hope this helps,

Opaque.

Here is a copy of my solver options in the ANSYS input file:

antype,4 nlgeom,on ! Turn on Large Deformation

solc,on,on ! Turn on solution control with ability to use contact time prediction

kbc,1 ! stepped BC's

eqsl,sparse,,,,,1

resc,,none ! Do not keep any restart files

cntr,print,1 ! print out contact info and also make no initial contact an error

trnopt,full,,,,,hht

autots,on

timint,on

My ANSYS help-desk does not know much about this type of problem otherwise I would not have posted the problem on this forum.

This is problem with ANSYS that the support is distributed all over and sometimes your problem does not reach (or is not forwarded) to right persons.

1. How much relaxation do you have at the FSI interface (MFRE in the Ansys input file)? 2. What MFLC commands do you have in the Ansys input file? 3. Which version are you using? 4. Are you using a converged steady-state fluids solution as the initial guess so that the transient starts smoothly? 5. Ansys tech support should ask to get the case from you and run it to figure out the problem... which office are you dealing with?

couple more things... If you have a non-zero Reference Pressure in CFX, have you set "include pref in forces = t"? Have you pre-stressed/pre-deformed the structure before doing the full transient analysis? Do this by solving a transient case on the Ansys side with TIMINT,OFF while the CFX side is steady-state. You have to do it this way since you can't switch ANTYPE in Ansys when doing a restart.

1. I tried to use a relaxation from 0.1 to 0.7 but it does not help much.

2. some relevant MF commands are given below:

MFIT, 51, 1, 15

MFRELAX,DISP, 0.40000000 ,RELX

MFRELAX,FORC, 0.40000000 ,RELX

MFRELAX,TEMP, 0.40000000 ,RELX

MFRELAX,HFLU, 0.40000000 ,RELX

MFRELAX,HGEN, 0.40000000 ,RELX

MFRELAX,VELO, 0.40000000 ,RELX

MFRELAX,ALL , 0.40000000 ,RELX

MFRSTART, 0.00000000

MFPS, group1, ANSYS

MFPSIMUL, group2, CFX

MFSORDER, group1, group2

MFLCOMM, SURF,ANSYS,1,DISP,CFX,PIPE,Mesh Displacement,NONC

MFLCOMM, SURF,CFX,PIPE,Total Force Density,ANSYS,1,FORC,NONC

3. This problem I am facing for few months with ANSYS-10.

ANSYS-11 seems to be a bit better in a sense that it goes one step further (i.e. i can further refine the time steps by a factor of two). However I have not done thorough testing with ANSYS-11.

4. I always start with a steady converged solution as a starting field.

5. I am willing to provide the case to ansys tech support. In fact you take any arbitrary case of flow in a straight pipe and you will see this response from the code (provided your time step smaller than 1/20-40 f)

thanks

No i do not have a non-zero reference pressure in my fluid domain.

What is the motivation behind doing a pre-stressed analysis?

What acutually the solver does when both sides(ANSYS and CFX) one has the steady-state settings?? I am unable to grasp or understand the meaning of this coupling procedure. Can this type of coupling be applied to problems where flow field is unaffected by the motion in structure (e.g. one way fluid to solid coupling)??

The purpose of the pre-stressed/pre-deformed analysis is just to start the transient from a reasonable starting point. For example, lets say you have a straight pipe containing high pressure fluid flow. You perform a steady-state run in CFX only to get the initial flow field. Then you start your transient 2-way FSI. The first time ANSYS solves, it sees a high pressure and expands the pipe accordingly. Now CFX solves, but the pipe volume has been expanded. If your fluid is fairly incompressible then the absolute pressure will go very low or to zero and the simulation will fail. The smaller you make your timestep the worse this will get since CFX sees that the pipe has been expanded in a shorter time, so the pressure drop will be higher. A steady-state 2-way FSI simulation will allow the structure to deform to it's correct position based on the steady-state flow field. You can then get a smooth start to the transient. Note that it's not always necessary to do this, for example if you don't expect any deformation of the structure due to the steady-state flow field. It's not the same thing as 1-way coupling. Does this apply to your case? I have solved 2-way FSI pipe flow cases in the past with small timesteps (0.0001 [s]), but I'm not sure what my f was in these cases.

Use version 11.0, a lot changed from 10.0. If you open your 10.0 case in 11.0, then delete and recreate all the MF commands since things changed. In particular, in your MFLC commands make sure "Mesh Displacement" and "Total Force Density" get changed to "Total Mesh Displacement" and "Total Force". The commands you have are correct for version 10.0, they just need changed if you run in 11.0.

[taedeneo]

Hi all,
just wanna add one thing. Ansys-cfx uses fixed-point approach of doing FSI, therefore, one have to use small enough relaxation factors in order to make it "strongly coupled". However, it is very costly and may fail. However, it is wrong to say that the added mass instability is not relavant when using this approach. As long as you solve it with partitioned approach, this instability is relavant.

[stumpy]

First, I just want to clear up what "strongly coupled" means, since it can mean different things to different people. ANSYS-CFX FSI it iteratively implicit; you get an implicit FSI solution by iterating the FSI interface load transfer within each timestep. I not sure exactly what "stongly coupled" means, but just be clear that ANSYS - CFX FSI is not fully coupled in that it's not a single-matrix solution.
So, the relaxation factor has nothing to do with whether it is "strongly coupled". As long as you have converged the interface loads with a timestep then you have an implicit solution, and you can do this using no under-relaxation (relaxation factor = 1) and you'll have an implicit solution. Perhaps what was meant was that you need a small relaxation factor to achieve convergence of the interface loads? However, this is not true. Presented with an unstable FSI interface solution many people begin to reduce the relaxation factor to try to stabilise things. While this can work, it slows down convergence a lot. A much better approach is to use source term coefficients on the continuity equation. This is something ANSYS support recommends and is covered in their FSI training class. There's some info in the literature too on using this approach.

[taedeneo]

Hi Stumpy,
Yes, in some cases, it is possible to use relaxation factors equal to 1 and get convergence. From my experience, in many cases, when we try to solve flexible structure (high density ratio = solid density/fluid density), the relaxation factor has to be lowered so that the convergence of the interface loads can be achieved. It waste a lot of time to run in this way. At the moment, I am using artificial compressibility to run all my fsi run instead of applying relaxation factors(all relaxation factors are set to unity). It does improve the efficiency a lot. But the problem with the way I applied this technique is probably a bit inappropriate since i apply it via density(density=physical density+AC)(it does work in many cases though). Now i am trying to put it in source term instead. Do you mind explain how this can be done? For example, what is the expression you use for the source coefficient? I tried the expression explained in Degroote(2009)and Raback(2001)(see below) but it still keep diverging. I guess there must be somthing wrong in the way that i set it up. All i changed is that instead of putting the AC term via density, i put it in source term. Is there anyway I can get the document provide for the course without going to the course, which is currently available in the US only(I am in Australia)? Any help would be appreciated!

Degroote(2009):Simulation of fluid-structure interaction with the interface artificial compressibility method
Raback(2001):FLUID-STRUCTURE INTERACTION BOUNDARY
CONDITIONS BY ARTIFICIAL COMPRESSIBILITY

[stumpy]

I would recommend turning off the artificial compressibility you have on Density. Apply a continuity source term on the FSI interface (boundary source). Set the Mass Flux to 0 (we don't want to actually add mass!) then set a the Mass Flux Pressure Coefficient to a constant value. Start with something very small, say 1e-10 [I forgot the units]. This should make no difference to your convergence - if it does, then make it smaller. Monitor the force at the interface within each timestep. If you make that number larger you'll get a more damped response for the force at the interface, if you make it smaller you'll get a less damped response and move back towards the unstable solution. The optimal value with give a critically damped response and is best found through trial and error. There are some equations you can use to estimate this number up front, but to be honest it's not worth it since they are only approximations in any case.
Sorry, I don't know much about getting the FSI documents. You can probably purchase them from ANSYS without attending the training.