[MFWilliams]

Hello,


I have a problem with an FSI simulation that I am running to simulate blood flow that at the very start of my simulaiton I get relatively very high velocities at the outlets.


The first image attached to this shows the fluid velocity at 0.00015 seconds. From 0 seconds that band of high velocity starts moving from the outlets inwards.
The second image attached shows the velocity at 0.00146 seconds which is the longest I have been able to run my simulation for (not becuase of it breaking but because of time constraints). It shows how the high speed areas have moved into the model and at 0.00146 seconds there are maximum velocities of about 5m/s.


I have run a CFD sim using the exact mesh for the fluid domain in the FSI simulation and it does not have this problem and has a maximum velocity of 0.4m/s at the same times. The only thing that differs between the fluid part of the FSI and the CFD is that I have changed the pressure BC for the fluid interface to an extrapolatedPressure instead of a zero gradient.


The BC's of the fluid and solid are shown below:
Pressure

boundaryField
{
    outlet1
    {
        type        fixedValue;
        value       uniform 0;
    }
    outlet2
    {
        type        fixedValue;
        value       uniform 0;
    }
    inlet
    {
        type       zeroGradient;
    }
    fluidInterface
    {
        type       extrapolatedPressure;
        value      uniform 0;
    }

Velocity

boundaryField
{
    outlet2
    {
        type            zeroGradient;
    }
    inlet
    {
        type            groovyBC;
        refValue        uniform (0 0 0);
        refGradient     uniform (0 0 0);
        valueFraction   uniform 1;
        value           uniform (0 0 0);
        valueExpression "(a1*sin(b1*x+c1) + a2*sin(b2*x+c2) + a3*sin(b3*x+c3) + a4*sin(b4*x+c4) + a5*sin(b5*x+c5) + a6*sin(b6*x+c6) + a7*sin(b7*x+c7) + a8*sin(b8*x+c8))*(-normal())";
        gradientExpression "vector(0,0,0)";
        fractionExpression "1";
        evaluateDuringConstruction 0;
        cyclicSlave     0;
        variables       
25
(
"x=time();"
"a1=1.476;"
"b1=1.011;"
"c1=0.4674;"
"a2=1.206;"
"b2=1.132;"
"c2=3.477;"
"a3=0.05853;"
"b3=8.393;"
"c3=-0.2345;"
"a4=0.04648;"
"b4=16.76;"
"c4=-0.6503;"
"a5=0.00276;"
"b5=5.108;"
"c5=2.317;"
"a6=0.02639;"
"b6=33.52;"
"c6=-1.617;"
"a7=0.0228;"
"b7=25.14;"
"c7=-1.522;"
"a8=0.01827;"
"b8=41.87;"
"c8=-2.746;"
)
;
        timelines       (
);
        lookuptables    (
);
    }
    outlet1
    {
        type            zeroGradient;
    }
    fluidInterface
    {
        type            newMovingWallVelocity;
        value           uniform (0 0 0);
    }
}

Displacement:

boundaryField
{
    solidEnds
    {
        type            fixedDisplacement;
        value           uniform (0 0 0);
    }
    fluidInterfaceSolid
    {
        type            solidTraction;
        traction        uniform ( 0 0 0 );
        pressure        uniform 0;
        value           uniform (0 0 0);
    }
    outerSolidFace
    {
        type            solidTraction;
        traction        uniform ( 0 0 0 );
        pressure        uniform 2000;
        value           uniform (0 0 0);
    }
}

I have checked the inlet waveform for velocity and that produces correct results with the inlet velocity being about only 0.17m/s over the time scale that has been simulated in the FSI



The rest of the properties like schemes, solution methods, meshes are linked in post #1 of this thread: FSI case does not converge, foam extend 4.0

[ilhado]

Hi Merlin,

I already experienced this. I found that the velocity outlets BCs are important. I had divergences in velocity like that and I found in some cases that this was related to propagation phenomena that occurs when you numerically simulate flexible tubes with the traditional specified-pressure at the outlets, which reflect pressure and velocity waves. I suggest checking the 'advective' BC in foam-extend to be used for the velocity outlets, which is based on convective-BCs that "allow" waves propagation out of the domain.

Best
Iago

[MFWilliams]

That is very interesting, given that in a lot of literature on the topic it has been shown that specifying detailed outlets are less important. Although I think all of the ones saying that were using commercial solvers not OpenFOAM. I will look into them, thank you.


Merlin

[MFWilliams]

Adding on to this thread. I found out that the reason I was getting velocities at the outlet to my simulation was because I had an externally applied pressure to the outer face of the solid domain. Removing this means at the start of the simulation the velocity initialises from only the inlet.