How to calculate drag coeff when using solids4Foam
 

The question is: How to calculate drag coeff when using solids4Foam on foam-extend 4.0? OR
Why execFlowFunctionObjects doesn't recognize regions in an FSI problem?

I went thru these steps:

1- solving:

Code:

---

user@linux$ solids4Foam

---

2- adding this to the end of controlDict:

Code:

---

  forceCoeffs1
  {
        type            forceCoeffs;
        region              fluid;     
        libs            ("libforces.so");
        outputControl      timeStep;
        outputInterval      1;
        patches            (interface);
        pName              p;
        UName              U;
        rhoName            rhoInf;
        log                true;
        rhoInf              1000;
        CofR                (0.5 0.1 0);
        dragDir    (1 0.0 0);
        magUInf    .2;
        lRef        .2;
        Aref        .04;
  }

---

3- executing this:

Code:

---

user@linux$ execFlowFunctionObjects

---

4- this error appears:

Code:

---

Create time

Create mesh for time = 0



--> FOAM FATAL ERROR:
Cannot find file "points" in directory "constant/polyMesh"

    From function Time::findInstance(const fileName&, const word&, const IOobject::readOption)
    in file db/Time/findInstance.C at line 148.

FOAM exiting

---

The Question again:
Why execFlowFunctionObjects doesn't recognize regions in an FSI problem?

regards
Ali

Quick answer: execFlowFunctionObjects was designed as a simply function objects execution application. It assumes that you used simpleFoam, pisoFoam or some other fluid flow solver.

Mmm... now that I think about it... inside which folder are you running that command?

inside the case folder as usual.

Hi Ali,

The function objects should work correctly when the solids4foam solver is running.

I do not have experience with execFlowFunctionObjects but possibly it does not work as expected when there are regions.

So one solution is to run your simulation again with the function objects included.

Philip

Access to solids4foam solver!!
 

Does anyone know how can i access to the solids4Foam solver ?

Hi Hamed,
Read this post.

Thank you Ali,
Dr Philip was very supportive in this field,

solids4Foam for neoHookeanElastic model
 

I am trying to use neoHookeanElastic model for FSI case of blood flow and living tissues interaction.

The FSI case consists of hyper-elastic Venous valves inside a blood vessel which demands the poisson`s ratio ~0.49 and Young M ~ 2e6.

The problem, however, is that for poisson`s ratio > 0.49, the solid part needs a very small time step (~1e-6) with many FSI iteration numbers(~35-40 iterations), and for higher time steps I got the following error :

From function void Foam::neoHookeanElastic::correct(surfaceSymmTensor Field& sigma) in filematerialModels/mechanicalModel/mechanicalLaws/nonLinearGeometryLaws/neoHookeanElastic/neoHookeanElastic.C at line 401-Material linearity enforced for stability!

mesh and geometry are attached,

thanks.

Hi,
Are you sure that it is an error? Isn't it only a warning?
Try these steps and see what happens:

• In system/controlDict, turn on adjustableTimeStep
• Use 1e-3 as absolute residual criteria for solid, fluid and outer fsi loop (By this, you actually loose the accuracy, but the procedure goes faster).
• Be sure that number of outer fsi loops are big enough that the residual is reached.

Best,
Ali

Hi Hamed,

Generally, the displacement-based approach taken by most of the solid models becomes very inefficient for large (>0.49) values of Poisson's ratio. Instead, a pressure-displacement approach may work better e.g. see Tukovic et al presentation at the OpenFOAM Workshop in Duisburg.

It may be sufficient for your work to assume a lower value.

Philip

Hi Dr. Philip and Mr Ali;

Considering my case (FSI on Venous valves interaction with blood flow), I thought the problem was more about the wrong Poisson`s ratio and Young`s Modulus, but after trying many different values for mechanical properties, I have the same deviation around the interfaces even if I use a very fine mesh.

I just made a few clarifying pictures to give you a better understanding of the problem. I would like to share my log file as well.

I would also like to share my case in a private email.

Thanks again for your kind supports.
-------
Hamed

Hi Hamed,

Does the gap become smaller as the FSI tolerance is tightened? Or alternatively, does it become larger as the FSI tolerance is loosened?

It looks like your mesh is conformal; is that true? In that case, you can use the directMap approached instead of the GGI; you could also try RBF. Both are implemented in solids4foam.

Philip

Dear Hamed,
As I see infinity values in your omega field, it seems that your fluid flow is not solved properly. What do you think?
I suggest trying this simulation to solve only fluid and not interaction first. You can
do this by turning off fsi in :and then see what happens...

Dear Ali,

First, you’re right. The solver is getting problem with the omega field, that’s why the bounding term came in. This problem can be solved if I use fixed value velocity through inlet instead of being required to use time series velocity.
Second, following your suggestions, I just reduce the Tolerance for the FSI loop within each time-step from 1e-6 to 1e-3, and the solver takes a few quick iterations for convergence, and that’s much better right now. But, the deviation in between the interfaces is getting larger, and I hope that would be its maximum value.

Dear Philip,
If you mean the interfaces deviation gap, the time series velocity profile seems to be related problem as well. I don’t have that much deviation gap when I use fixed value velocity at the inlet patch.
I feel that the solver doesn’t work fine with some time series velocity BC.
Regarding the Method for transferring information between the interfaces, direct map approach doesn’t work well even if use a very fined conformal mesh created by ICEM CFD block structured approach. Plus, RBF works much better than GGI.

In sum, as I mentioned before, the procedure sounds to be much better now, but the deviation gap is widening over time, and I think this is becuase the FSI tolerance (1e-3) is too much. Lower FSI tolerance (1e-6), however, demands many iterations.
The other confusing point is that the current time step is 1e-5 with 0.0034 Co number, but if I take it 2-3 times bigger, the solver simply crashes.
Furthermore, the inlet patch is far from the FSI interface at the beginning, and it should take some time for flow field to reach there. But, the interface starts to move short after the start time.

Regards
Hamed

Hi Hamed,
Are you sure that it is not only a visualization problem? (Read this post.)
Have you turned on adjustableTimeStep in system/controlDict? This makes dT as big as possible based on maxCo entry which is also specified in system/controlDicrt.
If your initial velocity field (specified in 0/fluid/U.internalField) is not (0 0 0), then it is logical to see deformation right after the simulation starts.

Regards
Ali

Hi,

Does your case run properly when you solve for the fluid only case? How this so called time dependent velocity is formulated for inlet? Is the velocity variation smooth enough to prevent velocity jump during simulation?

If you are not sure the fluid part is producing stable and accurate solution, then heading directly to the fsi case can drastically increase time to diagnose the actual reason behind this behavior.

From past I recall that one should use combined pulsatile pressure/velocity boundary condition at inlet and outlet to obtain physically correct results.

Just be careful with loosening the fsi convergence tolerance!
You can do this when you are trying to determine the cause of instabilities but set it back to a tighter value when you are ready to run the final case.

As you have already observed, loosening the fsi tolerance may provide faster simulation but it also results in large gap between interfaces and your simulation will probably crash do the accumulation of errors. Specially in these cases as the simulation is strongly coupled with a low elastic modulus and density ratio ~ O(1).

Well there is a time dependent BC already implemented within solids4Foam toolkit which suggest the should not be any problem with time dependent BCs on the solver side.

Already answered this above, loosening fsi tolerance comes with a serious side effects. If you look into the HronTurekFsi3 tutorials, as strongly coupled case it needs 12-16 fsi iterations to converge in each time step and this is achieved by turning off the coupled switch which allow the fluid part to solve for a stable solution before starting to transfer the forces and receiving displacements.

One more thing, try setting pimple outer loop correction to 1 and see what happens.

Are you starting the simulation at rest?
What is the forces values being transferred to solid side at the beginning of the simulation before solving the fluid region?

I strongly suggest providing better initial condition for fluid region before starting a coupled solution.
If the velocity is pulsatile then run the fluid region for a single cycle before turning the coupled switch on.

Finally, why I don't see pressure equation getting solved in your log file?
It is just missing from the log or you are some how managed not to solve for it?

Regards,
D. Khazaei