[jaroz]

Hello

I am trying my luck here, so I need to simulate the airflow in a data center and have issues defining boundary conditions.
First of all, floor tiles release air with constant mass flow rate (at pressure p+delta p) and a certain temperature setpoint T into the room. This seems ok

Next, there are servers, which host an internal fan, and are also a volumetric heat source.
I would need for the air to enter the server, which is defined as a Cell zone, and add a velocity source term for the fan, e.g. (50,0.0) , as well as a heat source term in W.
I am using buoyantBoussinesqSimpleFoam solver, which can only define temperature source term, so how to define heat source?

- Do I need to define cyclic boundaries on the inlet and Outlet of the server? But then i think Iit is not possible to model the heat transfer.

Finally, is it necessary to use chtmultiregionfoam for this problem and define the servers as solid regions? There it is possible to model conjugate heat transfer with source term h.

[arvindpj]

In order to specify volumetric heat source you could use the scalarSemiImplicitSource type in fvOptions as below:

heatSource
{
    type            scalarSemiImplicitSource;
    active          true;
 
    scalarSemiImplicitSourceCoeffs
    {
        selectionMode   all; // all, cellSet, cellZone, points
        cellSet         c1;
        volumeMode      specific; // absolute;
        injectionRateSuSp
        {
            T     (0.1 0);
        }
    }
}

Please refer this blog for more info.

Cheers

[jaroz]

Hello

Thanks very much for the post, especially the linked blog was very helpful for this!

If you don't mind I have developed some follow up questions:

1. So it seems for the Heat source term SC[K/s]:=q˙v/ρc. This means I can find out S_C by dividing the Total Heat (in W) by the density and capacity of the medium?

2. Is it possible to add Velocity source term to the cell zone, like described in
http://caefn.com/openfoam/fvoptions-meanvelocityforce
In addition to the heat source term?

For the Boussinesq simplification, that is described here, my Temperatures will vary approx. from 20°C-60°C (for hot spots). Is the Boussinesq approach okay here or Delta T too large?

Thanks

[arvindpj]

Hello

Thanks very much for the post, especially the linked blog was very helpful for this!

If you don't mind I have developed some follow up questions:

1. So it seems for the Heat source term SC[K/s]:=q˙v/ρc. This means I can find out S_C by dividing the Total Heat (in W) by the density and capacity of the medium?

yes

2. Is it possible to add Velocity source term to the cell zone, like described in
http://caefn.com/openfoam/fvoptions-meanvelocityforce
In addition to the heat source term?

yes, and have all in the same fvoption file.

For the Boussinesq simplification, that is described here, my Temperatures will vary approx. from 20°C-60°C (for hot spots). Is the Boussinesq approach okay here or Delta T too large?

Boussinesq simplification is valid if beta(T-T0) < 1; beta = thermal expansion coefficient; T0 = operating Temp (K)

[jaroz]

As a follow up question, my model is developed and solving nicely.
The issue I am facing is that the heat distribution in the medium doesn't seem to be homogeneous, but rather following a gauss-like curve with the following fvOptions code:

heatSource
    {
        type scalarSemiImplicitSource;
        active true;
        scalarSemiImplicitSourceCoeffs
        {
            selectionMode cellZone;
            cellZone servers;
            volumeMode specific;
            injectionRateSuSp
            {
                T ( 37.0 0);
            }

        }

    }

Higher heat load is clearly in the middle of the geometry. Is it possible to generate a uniform heat source term for the cell zone, where the center and boundaries are equally hot?

Cheers

[jaroz]

Sorry to bring up the post again, but I am still facing some issues. I have modeled the room successfully, but heat distribution remains uneven.

I have since figured out the source for this, air is recirculating from the back of the servers back into the server, this results in heating up.
The internal fan is modeled as a momentum source, is there a way to model the cell zone to deny backflow (with a boundary condition on the outflow side?)

[strobel]

Originally Posted by jaroz

Sorry to bring up the post again, but I am still facing some issues. I have modeled the room successfully, but heat distribution remains uneven.

I have since figured out the source for this, air is recirculating from the back of the servers back into the server, this results in heating up.
The internal fan is modeled as a momentum source, is there a way to model the cell zone to deny backflow (with a boundary condition on the outflow side?)

Hi, have you solved this issue? I usually try porous media to avoid this recirculation, but I don't know how this would fit on your modelling.