taedeneo
 

Hi Stumpy,
Thanks a bunch for the information. It is working now with a few of my test cases(all incompressible flow). what i did wrong is that i put the source in the whole domain instead of the boundary. This also agree with the comment made by Degroote(2009) that the source term should be applied only to interface elements. However, i also test it with one compressible flow problem (engine mount system).The bulk modulus of the fluid(oil)is 2e9 Pa. It turned out even if i put the largest number possible(4E37) for the source coefficient, the solvers can still not be able to achieve stability. Any idea on this? I am wondering if it is because of the fact that the fluid is compressible since from all the literatures i have read, all of them model their fluids as incompressible flow(such as blood flow). Any thoughts would be appreciated. Is there anything else you know from the FSI training class I should know?:)

Compressible flow with oil? Are you resolving "water" hammer? I suspect the instability is coming from elsewhere. If it occurs on start up and it's a transient case then perhaps the fluid and solid initial conditions were not in equilibrium, so you get a "bump" in the first timestep, which creates a pressure spike in the fluid that cannot be recovered from. The best approach to resolve this is to perform a steady-state 2-way FSI simulation first, so that you can get a smooth start to the transient. That's not trivial to do though.

Or maybe ramp the flow up from nothing so the initial spike is softened?

taedeneo
 

It is hydraulic engine mount system. I am trying to simulate interaction between hydraulic oil and rubber parts of the mount. The fluid is modeled as slightly compressible with bulk modulus of 2e9 Pa. This means that with only small change in volume, pressure inside the mount could be very high). However, I think the source of instability is still the added mass because when I tried to reduce fluid density and increase solid density(this makes density ratio smaller, which theoretically will make the system more stable), by doing this I got a stable solution even though it 's not the result I want. The pressure inside the mount is still the same, just the density ratio that is changed. Also I always ramp up applied load on the mount slowly. Therefore, all these evidences point out that the problem is still the added mass effect which depends on density ratio. For some unknown reasons , the source term (that make the coupling become stable in other problems such as blood flow and some external flows) fails to make an impact in this engine mount problem. Any ideas??? so confused!

The fact the source term coefficient has no effect is certainly strange. Do you want to post the CCL for the FSI boundary? How far does the solution progress - far enough to stop it and get a res file to examine? If you haven't already, add monitor point such as
maxVal(Total Mesh Displacement)@FSI_Interface
maxVal(Pressure)@Domain
minVal(Pressure)@Domain
force_x()@FSI_Interface, etc
Then make sure 'monitor coefficient loop convergence' is turned on. If it's truely unstable then the applied load shouldn't make a difference - so try zero load and let it run (round off at the interface will likely introduce a perturbation, which will grow if unstable).

taedeneo
 

links below are the file I use for the simulation (I think this way it will be more clear about what i did). I simplified the the problem to fluid in enclosure with a solid surround it. I tried running with no load at all, still it is unstable. To avoid confusion, the fluid is modeled as slightly compressible with bulk modulus of 2e9 Pa, therefore density =rho+rho*P/bulk modulus.

By the way, you said that by applying mass flux pressure coefficient is not actually introducing physical mass into the system, unlike using mass flux. Do you mind explaining this? What I understand is that mass flux pressure pressure coefficient will be multiplied with pressure at each cell, while mass flux is an exact amount of mass flux you want to introduce. Am I right to say that?

(like Sp=Sp' P+Sc)??. This is confusing to me because I know that CFX is using coupled solver and I thought there is no pressure in continuity equation. How is this work really?

Thanks for you helps



CFX
http://uploading.com/files/2a63c9e3/FSI_enclosure.cfx/
Solid input file
http://uploading.com/files/979a9ce9/FSI_enclosure.inp/
Solid simulation file
http://uploading.com/files/83m4fc3b/FSI_enclosure.dsdb/

taedeneo
 

I forgot one thing. If you want to try to run it, double precision should be turned on since the bulk modulus is a very big number

It looks like you just forgot to define a source coefficient on one of the FSI interfaces in CFX - only 1 of the 2 boundaries had this set. I did change the structural side too so that it was only running 1 substep, but other than speeding things up I doubt that made much difference. With zero load I found a source coeff of 1.0 kept things stable (monitor points for force_y()@fsiinterfaces stay close to 0). Once you add a load you'll probably need to change this source coefficient; for the zero load case we are basically solving 0 = 0, so it was impossible to tell if the source coeff of 1.0 gives the critically damped response we are looking for.

The size of the number makes no difference to single or double precision (for numbers of engineering significance). The difference between single and double precision is it allows more significant digits. For instance a single precision number could not tell the difference between 1.000000001 and 1.0, but double precision can.

Yes, Glenn is correct. Big numbers don't require double precision. When you have a big range in scales for a given quantity then you need double precision. In this case the mesh deformations are likely a small fraction of the domain size, so you should use double precision, just not for the reasons you thought.

taedeneo
 

the reason why i said that it is necessary to use double precision is that the bulk modulus is very big. This means that even a very small change in volume can make a big different in pressure. So if you do not have enough precision for the change in volume, the pressure change due to volume change of 0.000010000001 will be the same with that due to volume change of 0.00001.

Stumpy, did you use double precision when you test the case and see that it 's stable with coefficient of 1.0? I tried it out but it turns out it is not stable with double precision but stable with single precision. It doesn't make sense to me but that is the evidence I have. Note that every test I did is with no load.

I'll need to check (and download the files again - hope they are still there). I will get back to you at some point, but it may be a few days.

taedeneo
 

I just found out that it works on CFX12 (before I used CFX11). So it 's all good now. but I still have doubt in my mind about how the coefficient works and helps the instability. I got the document with me. According to the document, the coefficient will be multiplied by pressure difference not pressure. So Is this mean that pressure difference (as in pressure correction term in pressure equation, which is a form of continuity equation) is the solution variable in Continuity equation used by CFX? What form exactly is the continuity equation CFX? The document also claims that at convergence the influence of the coefficient will vanish since the pressure change approach zero. Any idea anyone??

taedeneo
 

By the way, why does it work in v12. not v11.? What did they change?? anyone?

Don't know what changed. The discussion on pressure difference goes back to the fundamentals of how you solve the linear system of equations. The linear system is usually written as [A][x] = [b]. [A] is your coefficient matrix. [x] is the solved variables, but your are actually solving for a change in the variable from the previous iteration. So at convergence [x] = 0, since the solution is not changing from one iteration to the next. So if [x] -> 0, then the coefficients in [A] cannot affect a converged solution, then only affect the path to convergence (i.e. stability, convergence rate).

Hello,
I had a problem, that seems to be the same as that one of Dr. V. Kumar.

When the timesteps are to small, the FSI simulations stops in the first timestep. The reason is an error in element formulation in the structure simulation. The volflow, that is written out by CFX, equals zero.

To solve the problem, I changed the inlet and outlet boundary condition: Instead of "Inlet", and "Outlet" I chose "Opening".

The background is probably the following:
The structure (at my simulation it is prestressed) has a very low "noise of displacements". So the structure moves towards the inlet. Therefore there would be an outflow at the inlet and an inflow at the outlet. But these flowdirections aren't allowed at the boundary conditions. So unrealistic under- and overpressures can occure. And thus the structure will be displaced too much, by what the simulation will stop.

May be this will help anyone.

Richard