CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Community Contributions > OpenFOAM CC Toolkits for Fluid-Structure Interaction

Unusual high outlet velocities

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree2Likes
  • 1 Post By MFWilliams
  • 1 Post By MFWilliams

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   March 1, 2022, 07:59
Default Unusual high outlet velocities
  #1
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 3
MFWilliams is on a distinguished road
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

Code:
boundaryField
{
    outlet1
    {
        type        fixedValue;
        value       uniform 0;
    }
    outlet2
    {
        type        fixedValue;
        value       uniform 0;
    }
    inlet
    {
        type       zeroGradient;
    }
    fluidInterface
    {
        type       extrapolatedPressure;
        value      uniform 0;
    }
Velocity
Code:
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:
Code:
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
Attached Images
File Type: jpg 0.00015.jpg (40.0 KB, 4 views)
File Type: jpg 0.00146.jpg (47.0 KB, 3 views)
Chanikya_Valeti likes this.
MFWilliams is offline   Reply With Quote

Old   March 1, 2022, 09:27
Default
  #2
New Member
 
ilhado's Avatar
 
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 21
Rep Power: 9
ilhado is on a distinguished road
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
ilhado is offline   Reply With Quote

Old   March 1, 2022, 10:29
Default
  #3
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 3
MFWilliams is on a distinguished road
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
ilhado likes this.
MFWilliams is offline   Reply With Quote

Old   March 8, 2022, 06:06
Default
  #4
Member
 
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 3
MFWilliams is on a distinguished road
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.
MFWilliams is offline   Reply With Quote

Reply

Tags
boundary condition, fsi 2-way, fsi problem, high velocity flow

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
High velocities near walls in a cross junction PoSchwarz OpenFOAM Running, Solving & CFD 0 June 14, 2021 14:13
Pressure Outlet Guage pressure Mohsin FLUENT 36 April 29, 2016 18:16
UDF to extract particle positions and velocities at outlet marauder Fluent UDF and Scheme Programming 5 March 1, 2016 13:33
I'm getting too high velocities in simple 2D geometry logme FLUENT 0 June 17, 2015 17:43
HIgh pressure zone near the outlet? seasoul OpenFOAM Running, Solving & CFD 3 June 1, 2013 06:03


All times are GMT -4. The time now is 22:02.