CFD Online Discussion Forums - Time dependant pressure boundary condition

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Verification & Validation (https://www.cfd-online.com/Forums/openfoam-verification-validation/)

- - Time dependant pressure boundary condition (https://www.cfd-online.com/Forums/openfoam-verification-validation/115401-time-dependant-pressure-boundary-condition.html)

Time dependant pressure boundary condition

Dear all

Does anyone know validation result for unsteady icoFoam and smagorinsky model LES using pisoFoam ?
UNSTEADY here means both using 'unsteady solver' and 'time dependent boundary condition'

I have been using OpenFOAM about three month for aortic flow, but solver could not offer sufficient stabilities nor the results looks strange.
I need to solve identical geometry by unsteady pressure and unsteady velocity boundary conditions.
The result was identical in v2.1.1 and v1.6-ext.

Using inlet velocity curve was relatively stable, but chaos comes if time dependent pressure boundary condition is introduced.
I tested myself identical mesh in fluent 6.3.6 which gave 10 times smaller pressure ( pressure converted kinematic to real ) and fluent result matches measurement order.

The points I would like to ask is following.

1.
I found many comparisons with commercial softwares and experiments result unsteady calculation using time independent boundary condition, yet still can not find test result under unsteady boundary condition.
Is any such comparison available ? I am not fully confident with time dependent pressure boundary condition in OpenFOAM.

2.
What is the appropriate boundary condition settings for both time dependent velocity boundary condition and time dependent pressure boundary condition ?
Is anything wrong with my setting ?

-------------------------------------------------------------------
my setting for solving by time dependent pressure boundary (icoFoam)
-------------------------------------------------------------------
0/p

Quote:

inlet
{
type uniformFixedValue;
uniformValue tableFile;
tableFileCoeffs
{
fileName "$HOME/data/a0.5E-3.data";
outOfBounds clamp;
}
}

outlet
{
type fixedValue;
value uniform 0;
}

wall
{
type zeroGradient;
}

0/U
inlet
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

wall
{
type fixedValue;
value uniform (0 0 0);
}

note: I also test pressureInletOutletVelocity for inlet and outlet but result couldn't see notable difference.

---------------------------------------------------------------------
my setting for solving by time dependent velocity boundary (icoFoam)
---------------------------------------------------------------------
0/U

Quote:

inlet
{
type zeroGradient;
value uniform (0 0 0);
}

outlet
{
type zeroGradient;
value uniform (0 0 0);
}

wall
{
type fixedValue;
value uniform (0 0 0);
}

0/p
inlet
{
type uniformFixedValue;
uniformValue tableFile;
tableFileCoeffs
{
fileName "$HOME/FOAM/kim2010/p_diff1.0E-5.data";
outOfBounds clamp;
}
}

wall
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 0;
}

yosuke

hello yosuke,

First, i would not use icoFoam for transient case: use pisoFoam or pimpleFoam instead.

Then i would say your BC settings are not optimal.
1) I do not see any difference between your time dependent velocity and pressure case, just the file you use: this is typo ?

2) You are setting P at inlet and outlet, and zeroGradient for velocity for inlet / outlet. This is clearly unstable/not physical if p is not constant at inlet or outlet, which is your case at inlet.
I have not the correct answer here, but you could try:
0/p
inlet: uniformFixedValue;// with your changing P field.
outlet: fixedValue 0
0/U
inlet: advective
outlet: advective (or zeroGradient).

But setting velocity at outlet (then zeroGradient for p), will clearly work here.

Your trouble come from the zeroGradient for velocity at inlet, since pressure is not constant. And you just discovert that your Fluent inlet/outlet is not a zeroGradient condition exactly.

Hope this help.

regards,
olivier

Dear Olivier

Thank you very much for your reply. It worked.

Doubt with implementation of transient velocity b.c

Hi guys;

I am relatively new to the forum.
I am trying to inject an air bubble into a fluid of ethanol and see the flow of the air bubble through a rectangular 2D channel as an initial step based on a paper.

I have a rectangular bubble which I would like to relax it from rectangular to (curved at edges due to the influence of surface tension). So, it can take around 0.003s. (Notice time scale is small and I deal with interFoam solver). After, relaxing i inject with a uniform velocity of 0.0167m/s for a brief period of time say 0.01s.

Could you please let me know what sort of a boundary condition is to be used for the inlet and also at the outlet. :confused:

Thanks a lot for your patience and help.