[90nash]

Hello Everyone,

I have been stuck on this problem for quite some time and would really appreciate any help.
I am working on a Womersley type flow with parabolic velocity profile specified at inlet (Time Period = 3 sec). Simulation type is laminar with max inlet Re=2077. A screenshot of the mesh has been attached. It shows underdeterminedCells in gray. The mesh is relatively coarse but i have tried a simulation with a finer mesh (0.6 million elements approx, also has underdetermined cells) and the simulation blows up in that case too.

I start up with first order schemes and then switch to second order after about 0.5 sec. I have tried various schemes available (mentioned in attached fvSchemes file in comments) but the simulation eventually blows up in every case after the flow reverses at around 3/4 Time Period (1.95 sec in this case). I have attached a screen shot of how velocity looks at this point.

Since the simulation was blowing for every permutation of fvschemes or relaxation factor (tried upto 0.3) near the inlet and outlet patches, i am led to believe that it is the underdeterminedCells that are causing the problem.

My Questions:
1. Is there a problem with the schemes that i have used? Can anyone suggest any improvement to the schemes to handle underdetermined cells or otherwise (I am a beginner with schemes).
2. The Mesh was created in ANSYS Fluent. I also tried running the same case in Fluent and it does not diverge. Is my thinking correct that OpenFoam solver is sensitive to underdeterminedCells? Can you suggest how to get rid of them?
3. Any other suggestion to improve is more than welcome.

I am using OF 2.2 along with swak4FOAM 2.x.
Here is how output look like at around 1.95 sec:

DICPCG:  Solving for p, Initial residual = 0.00154356, Final residual = 0.000846384, No Iterations 1
DICPCG:  Solving for p, Initial residual = 0.000886445, Final residual = 0.000886445, No Iterations 0
time step continuity errors : sum local = 1.07439e-08, global = -8.69841e-09, cumulative = -0.00108703
DICPCG:  Solving for p, Initial residual = 0.00154378, Final residual = 0.000846137, No Iterations 1
DICPCG:  Solving for p, Initial residual = 0.000886284, Final residual = 0.000886284, No Iterations 0
time step continuity errors : sum local = 1.07419e-08, global = -8.69717e-09, cumulative = -0.00108704
PIMPLE: converged in 8 iterations
ExecutionTime = 50761.6 s  ClockTime = 107754 s

Expression volFlowInlet :  sum=0.000157722
Expression volFlowOutlet1 :  sum=-3.60266e+11
Expression volFlowOutlet2 :  sum=3.51863e+11
Courant Number mean: 0.000444094 max: 1.02206
deltaT = 2.41579e-22
--> FOAM Warning : 
    From function Time::operator++()
    in file db/Time/Time.C at line 1039
    Increased the timePrecision from 661 to 662 to distinguish between timeNames at time 1.95279
Time = 1.9527872476915459909463379517546854913234710693359375

PS: I am really really sorry about such an extensive post. I can understand that it can be a pain to just read let alone reply. But i wanted to provide complete info.

Thanks a million
Nadish

checkMesh.txt

Mesh.jpg

Mesh_underdeterminedCells.jpg

Velocity_blown.jpg

case.tar.gz

[1988]

Hi
I have stuck in this problem the same as you but I found a post which is useful

http://www.cfd-online.com/Forums/openfoam-solving/132795-unexpected-deltat-decrease-pimplefoam-simulation.html

DId you find any way to iron out this problem?

[90nash]

Hello Ali,

Its really great to hear from you. I thought this post had faded out. Yes i was able to find the solution for this problem.

I was dealing with backflow problem and it was the nature of geometry itself that was causing the problem. I had to extend the outlets such that they lie in a region where the flow is not too perturbed. Actually another OpenFoam user, Hiroshiman, helped me with this problem. Check this post:

http://www.cfd-online.com/Forums/ope...-groovybc.html (Post #8)

If you are not dealing with backflow problem i suggest that you recheck the Boundary Conditions and geometry (including mesh). Other tips that might help:

1. Increase nOuterCorrectors to higher value, say 50, and observe the solution. If the solver converges at a time step it will not carry on to 50 iterations. But if the solution does not converge in 50 iterations consistently for successive timesteps, the solution will most likely diverge eventually at a later timestep.

2. Start of with default values for relaxation factors for U,k,epsilon i.e. 0.7. If the solution is not converging within specified (50) iterations, decreasing the relaxation factor will help.

3. You may use upwind divergence scheme and it is very likely that the solution will not diverge. However it is a first order scheme, thus too diffusive and you will not get a good solution.

Again i would like to iterate that i had tried numerous things with fvSchemes and fvSolution but the solution diverged everytime because the problem was with geometry and BC's.

Hope this helps!

Best,
Nadish

[1988]

Hi Nadish
thanks for your coplete answer.
what is your idea about sarting the solution with upwind scheme and then changing it to anoter one?But I dont know when is the right time to do that?
I just want to simulate laminar,incompressible,transient,newtonian flow in an artery to investigate the flow field ,do you think that changing the schemes has an great effect on the flow field?
I have meshed the eometry in gambit and I have 43000 tetrahedra cells.
thanks alot for your support

[90nash]

Hello Ali,

Sorry for being late on the reply.

At the starting since the flow field is not initialized you are bound to see a lot of oscillations. If you plot residuals these oscillations can be witnessed. Since first order schemes are more stable it is advisable to start the simulation with it. However continuing with it will not give you good results since they are diffusive. So once you see in residual plot that things look stable switch to second order convection schemes.

You might want to include prismatic cells on boundary surface to effectively capture boundary layer flow instead of all tet mesh.

Best,
Nadish