CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   Change of B.C after solving !!! (http://www.cfd-online.com/Forums/openfoam/81116-change-b-c-after-solving.html)

maysmech October 16, 2010 11:53

Change of B.C after solving !!!
 
Dear Foamers,

i used buoyantBousiesqPimpleFoam to simulate a room ventilation. i defined B.C of inlet as temperature fixedValue 290K as seen below.

Code:

boundaryField
{
    wall
    {
        type            zeroGradient;
    }
    inlet
    {
        type            fixedValue;
        value          uniform 290;
    }
    windows
    {
        type            fixedValue;
        value          uniform 305;
    }
    door
    {
        type            fixedValue;
        value          uniform 300;
    }
}

After solving all grids have temperature of more than 300K:confused:
why is boundary fixed value changed?

marupio October 16, 2010 13:08

It shouldn't do that. Did you change the right files? OpenFOAM only reads the [case]/0 files when starting from time = 0. If you are resuming a run with existing data, it will read from whatever time value it needs. You'd have to change those ones.

fcollonv October 16, 2010 14:10

Hello maysam,

Your settings for a ventilation case look strange for me. Why don't you have an outlet boundary condition? I presumed that you expect the flow coming from the window and outgoing by the door (or the opposite).
At the outlet I will preferably use an InletOutlet boundary condition.

Frederic

maysmech October 16, 2010 22:05

Thanks David and Fredric for your replies,
that was 0/T of my case. U is:
Code:

dimensions      [0 1 -1 0 0 0 0];

internalField  uniform (0 0 0);

boundaryField
{
    wall
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
    inlet
    {
        type            fixedValue;
        value          uniform (0 0 -0.1);
    }
    windows
    {
        type            fixedValue;
        value          uniform (0 0 0);
    }
    door
    {
        type            inletOutlet;
        inletValue      uniform (0 0 0);
        value          uniform (0 0 0);
    }

}

i,ve revised door from aeroGradient ti inletOutlet.
and P is:
Code:

dimensions      [0 2 -2 0 0 0 0];

internalField  uniform 0;

boundaryField
{
    wall
    {
    type    zeroGradient;
    }
    inlet
    {
        type            zeroGradient;
    }
    windows
    {
  value          uniform 0;

    type    zeroGradient;
    }
    door
    {
        type            fixedValue;
        value          uniform 0;
    }

}

the problem is i don't know how OF can use all of these 3 B.C with each other. you know we should define only one of P or U in other codes. Can this be the cause of problem?

fcollonv October 19, 2010 10:59

Setting boundary condition
 
Hello Maysam,

Could you tell me which version of OpenFOAM you are using?

For the boundary conditions, I would switch the door velocity and temperature condition to zeroGradient. I presumed you are not expecting the flow coming in from there.

One important thing:
For the pressure, you will have to use the "buoyantPressure" condition and not zeroGradient (have a look to the tutorial cases).

Hope that those small hints will help you.

Regards,
Frederic

maysmech October 19, 2010 15:30

Quote:

Originally Posted by fcollonv (Post 279808)
Hello Maysam,

Could you tell me which version of OpenFOAM you are using?

For the boundary conditions, I would switch the door velocity and temperature condition to zeroGradient. I presumed you are not expecting the flow coming in from there.

One important thing:
For the pressure, you will have to use the "buoyantPressure" condition and not zeroGradient (have a look to the tutorial cases).

Hope that those small hints will help you.

Regards,
Frederic

I use OpenFOAM 1.7.0

The problem is setting ceiling fan inlet temperature cooler than walls and internal temperature, velocity arises to ceiling which remove the velocity of fan and contour of velocity shows a worse flow to top instead of down and it is not true in real.

I think HeatTransfer solvers of OpenFOAM are not suitable for simulation of a room with having flow input and output because all of tutorials have no inlet or outlet patches. :confused:

Any suggestion for ventilation simulation of a room?

fcollonv October 22, 2010 09:12

Quote:

Originally Posted by maysmech (Post 279852)
I use OpenFOAM 1.7.0

The problem is setting ceiling fan inlet temperature cooler than walls and internal temperature, velocity arises to ceiling which remove the velocity of fan and contour of velocity shows a worse flow to top instead of down and it is not true in real.

I think HeatTransfer solvers of OpenFOAM are not suitable for simulation of a room with having flow input and output because all of tutorials have no inlet or outlet patches. :confused:

Any suggestion for ventilation simulation of a room?

Hello Maysam,

I don't see why it shouldn't work. If I understand you right, you don't really know in advance, what the structure of the flow will be. So I presumed you have to change your boundary condition. I would try : for the "pressure" (p_rgh) along the walls "buoyantPressure" and fixedValue at the opening (need to take into account the gravity) and for the velocity put at the opening pressureInletOutletVelocity.
I will also try first buoyantBoussinecqSimpleFoam to have a steady state solution to have a better idea of the mean flow.

Good try,

Frederic


All times are GMT -4. The time now is 21:50.