|
[Sponsors] |
March 1, 2022, 07:59 |
Unusual high outlet velocities
|
#1 |
Member
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5 |
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; } 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); } } 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); } } 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 |
|
March 1, 2022, 09:27 |
|
#2 |
New Member
Iago Lessa de Oliveira
Join Date: May 2015
Posts: 23
Rep Power: 11 |
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 |
|
March 1, 2022, 10:29 |
|
#3 |
Member
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5 |
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 |
|
March 8, 2022, 06:06 |
|
#4 |
Member
Merlin Williams
Join Date: Nov 2021
Posts: 71
Rep Power: 5 |
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.
|
|
Tags |
boundary condition, fsi 2-way, fsi problem, high velocity flow |
Thread Tools | Search this Thread |
Display Modes | |
|
|
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 |