buoyantBoussinesqSimpleFoam - continuity error
 

Hello all,

I am new to OpenFoam and I'm trying to solve a simple (at last I think it is...) case in which I have a heated rod inside a pipe. For natural convection it seems ok.

When I try to start a flow (inlet and outlet flows) I get a "continuity error message".

I based the configuration files on "hotRoom" OpenFoam's tutorial case.

The boundary conditions are:

p: inlet -> zeroGradient
outlet -> FixedValue uniform 0;
insideWall -> zeroGradient;
outsideWall -> zeroGradient;

U: inlet -> FixedValue (0 1 0)
outlet -> ZeroGradient (or calculated $internalField;
insideWall -> FixedValue (0 0 0);
outsideWall -> FixedValue (0 0 0);

T: inlet -> FixedValue 300;
outlet -> zeroGradient (or calculated $internalField);
insideWall -> FixedValue 1000;
outsideWall -> FixedValue 300;

So, any suggestions?
Thanks in advance.

Vitor

For your pressure, you should set the boundary condition to buoyantPressure

for the outlet velocity condition try pressureInletOutletVelocity with value (0 0 0).

I always use this bc in p_rgh

wall
{
type buoyantPressure;
rho rhok;
value uniform 0;
}

outlet
{
type zeroGradient;
}
inlet
{
type fixedValue;
value uniform 0;
}

Thanks guys. I got a better result, though not perfect. But with this buoyantPressure BC I'll try to tune my simulation.

Divergence problem solved by Greel's suggestion
 

@ Greel:

Boundary conditions for p_rgh suggested by you worked for my simulation.

I was having a divergence problem for buoyantBoussinesqSimpleFoam that got solved with those boundary conditions.

How good the results are, remains to be seen.

Thanks a lot
Ameya

How was the results?
I have similar doubts about p and p_rgh boundary conditions in buoyantBoussinesqSimpleFoam solver applied in simple pipe simulation...

thanks!

Dear Foamers,

It’s been a while that I’ve had the same problem in setting the correct BC for similar problems. Here is the review of how I solved this issue:

Problem: steady state open channel flow simulation. In this scenario, normally the simpleFoam is employed. The BCs are given by:


BCs: inlet, outlet, wall, topWall

U:

inlet
{
type fixedValue;
value uniform (0 0.1589 0);
}

outlet
{
type zeroGradient;
}

wall
{
type noSlip;
}

atmosphere
{
type slip;
}

p:

atmosphere
{
type zeroGradient;
}

inlet
{
type zeroGradient;
}
outlet
{
type fixedValue;
value uniform 0;
}

wall
{
type fixedFluxPressure; //remember that we cannot use Drichlet and Neuman BC at the same time
value uniform 0;
}


As one can see, selecting fixedValue BC for the outlet pressure is physically incorrect even though one can get result. To resolve this issue, I decided to use the hydrostatic pressure as the outlet BC for the pressure. To this end, one need to either define gravity in the governing equation or else use a steady state solver that has gravity in the equations. I went for the second approach. The only available solver for incompressible fluids that has this feature is buoyantBoussinesqSimpleFoam. When this solver is selected, the BCs needs to be defined for the U, p, and p_rgh. Generally, p_rgh=p-rho*g*h. I have searched a lot and finally could find the correct way of setting BC for the foregoing parameters.


U:

inlet
{
type fixedValue;
value uniform (0 0.1589 0);
}

outlet
{
type pressureInletOutletVelocity;
value uniform (0 0 0);
inletValue uniform (0 0 0);
}

wall
{
type noSlip;
}

atmosphere
{
type slip;
}


P:

atmosphere
{
type zeroGradient;
}

inlet
{
type zeroGradient;
}

outlet
{
type calculated;
value $internalField;
}

wall
{
type zeroGradient;

}



P_rgh

inlet
{
type fixedFluxPressure;
}

outlet
{
type fixedValue;
value uniform 0;
}

wall
{
type fixedFluxPressure;
}

atmosphere
{
type fixedFluxPressure;
}


let me know if it is not clear.

Keep Foaming