CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   hotRoom tutorial with atmosphere boundary condition (http://www.cfd-online.com/Forums/openfoam-solving/102227-hotroom-tutorial-atmosphere-boundary-condition.html)

Toorop May 25, 2012 09:51

hotRoom tutorial with atmosphere boundary condition
 
2 Attachment(s)
Hi,

I would like to specify atmosphere boundary condition in the hootRoom tutorials. The default case uses walls on the sides and at the top, so the only modification is the change in boundary conditions.
Code:

alphat
{
        type            calculated;
        value          uniform 0;
}

epsilon
{
        type            inletOutlet;
        inletValue      uniform 0.01;
        value          uniform 0.01;
}

k
{
        type            inletOutlet;
        inletValue      uniform 0.1;
        value          uniform 0.1;
}

kappat
{
        type            calculated;
        value          uniform 0;
}

nut
{
        type            calculated;
        value          uniform 0;
}

p
{
        type            calculated;
        value          0;
}

p_rgh
{
        type          totalPressure;
        p0              uniform 0;
        U              U;
        phi            phi;
        rho            rhok;
        psi            none;
        gamma      1;
        value        uniform 0;
}

T
{
        type            inletOutlet;
        inletValue      uniform 300;
        value          uniform 300;
}

U
{
        type            pressureInletOutletVelocity;
        value          uniform (0 0 0);
}

Unfortunately, the BC that I set is not giving me the results I'm looking for. The air won't exit the domain in the upward direction as expected, it makes an U shape path (picture attached). The solvers were buoyantBoussinesqPimpleFoam and buoyantBoussinesqSimpleFoam.

It would be great if someone could share his setup to achieve correct behaviour at the boundary. Thanks!

MartinB May 25, 2012 12:26

Hi,

you can try as BC for both p_rgh and U:
Code:

ceiling
{
      type zeroGradient;
}

Martin

Toorop May 29, 2012 06:13

1 Attachment(s)
Hi,

thanks for the tip. With the modifications the case produces a nice expected outflow in the early stages of the simulation. But then a crossflow develops across the domain - with both solvers. I think the pRefCell / pRefValue "hijacks" the flow - with the original BC there was no need for pRef. Any ideas how to overcome this situation?

Toorop May 31, 2012 10:50

2 Attachment(s)
Hi,

I have managed to solve the problem! :cool:

The combustion/fireFoam/les/smallPoolFire cases uses the boundary conditions I wanted to create, so I just copied and modified it to adjust to the buoyant solvers. I really don't now how on earth I couldn't find it sooner ...

Of course if anyone has some suggestion, please share it! Thanks.

tunkers June 2, 2012 10:03

Hello Tibor,


Thanks for posting this excellent example! In the past I've always had difficulty defining boundary conditions for the buoyant compressible flow solvers with inlets/outlets.

I've been trying to adapt your buoyantBoussinesqPimpleFoam solver example above so that it also works with the buoyantPimpleFoam solver (no boussinesq approximation). It runs for a while, but then the solver blows up after about 50 iterations with a "maximum iterations exceeded" error

Any ideas on how to get your example working in buoyantPimpleFoam?



--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function specieThermo<Thermo>::T(scalar f, scalar T0, scalar (specieThermo<Thermo>::*F)(const scalar) const, scalar (specieThermo<Thermo>::*dFdT)(const scalar) const) const
in file /mnt/data3/OpenFOAM/OpenFOAM-2.1.0/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 69.

FOAM aborting



Toorop June 4, 2012 05:35

2 Attachment(s)
Hi Eric,

I have altered the BC to conform with buoyantPimpleFoam and it runs without a problem, but doesn't produce the desired flow, or at least it looks strange (octopus shape).

Possible source of errors:
  • there's zero rho iterations in the log file
  • the system/fvSolution file rho solver section has 0 for tolerance and relTol (copied from the hotRoom tutorial) - changing it has no effect for me

I have limited experience with buoyant solvers so I have no idea how to fix it, maybe you can pinpoint the source of the problem.

tunkers June 5, 2012 07:20

Hi Tibor, Your modified buoyantPimpleFoam case is very helpful. I will experiment further with it to see if the results seem reasonable. Thanks for your help

Best Regards,

Eric

EOC June 21, 2013 02:26

Experimental results to validate the results
 
Hi everyone,

I am doing a similar simulation of natural convection from horizontal heated plate.Were you guys able to finish your simulation. I am doing a similar simulation and I got similar octopus shaped streamlines.

I want to ask if there is any data available to validate our simulation results. :)

Regards,
EOC


All times are GMT -4. The time now is 15:02.