Hi,

I am working on a conjugate heat transfer project. Inside the fluid domain, there is a fan. The purpose of the fan is to provide force convection to uniform the temperature inside the fluid domain. This is a transient case. How to setup BCs for the fan?

The volume where the fan occupied was cut out. here, there are: walls, + one face for fan intake and one face for fan outlet.

For the intake side, I am using: inlet velocity (toward inside the fan) with zero gradient for temperature.

For the outlet side (flow into the fluid domain), I am using:

inlet velocity (toward the fluid domain)

temperature: calculate average temperature from the intake side, then, assign the average temperature to this surface face.

Is this reasonable? Any suggestion?

Thanks!

phsieh2005

1) Do you have any outlets or openings in the model? Or is the fan blowing and sucking from a single closed region?

The reason I ask is because if there are no outlets you will have problems if the flow into the domain does not *exactly* match the flow out of the domain. If this happens, the amount of fluid inside the domain will increase or decrease unrealistically with time, the pressure will be unrealistic and the problem will not converge. Even if you specify the same velocity in CFX-Pre, you will find that small numerical differences will occur and cause problems during the solution.

So if you have no other outlet or opening boundary in the model, you would be better off using an pressure outlet condition or opening condition to model the *back* of the fan instead of an inlet. This should make your calculation much more stable.

(If you do have other pressure outlets or openings in the model your method should work)

2) What temperature are you using on your inlet that sends fluid into your domain? How are you going to make sure that the temperature going into the back of the fan is the same as the temperature coming out of the front of the fan?!! If you are doing a cooling simulation this is very important!

There are several ways of doing this.

One possible way is as follows: You should search for the word "Dirichlet" in the CFX11 help system - this leads to the momentum source page of the manual. If you mesh the region occupied by the fan you can use the method the manual describes to impose a prescribed velocity in this region. If you do this then the same air that goes into the fan comes out at the front, and you can be sure that the temperature coming out of the fan is correct. This would be my preferred method.

Another way to get the right inlet temperature is to couple the inlet temperature to the air temperature at the outlet using CEL expressions. I have never tried that myself.

3) Don't forget that fans generate swirl and turbulence! You should try and assess if this will be important for your model.

Good luck, Andy

Sorry - I should not have assumed you are using CFX!! This is not the CFX forum. :-P Please see below for a corrected version!

I suggest you tell us which code you want to use, then you will get more specific answers.

Regards, Andy

1) Do you have any outlets or openings in the model? Or is the fan blowing and sucking from a single closed region?

The reason I ask is because if there are no outlets you will have problems if the flow into the domain does not *exactly* match the flow out of the domain. If this happens, the amount of fluid inside the domain will increase or decrease unrealistically with time, the pressure will be unrealistic and the problem will not converge. Even if you specify the same velocity at both faces, you will find that small numerical differences will occur and cause problems during the solution.

So if you have no other outlet or opening boundary in the model, you would be better off using an pressure outlet condition or opening condition to model the *back* of the fan instead of an inlet. This should make your calculation much more stable.

(If you do have other pressure outlets or openings in the model your method should work)

2) What temperature are you using on your inlet that sends fluid into your domain? How are you going to make sure that the temperature going into the back of the fan is the same as the temperature coming out of the front of the fan?!! If you are doing a cooling simulation this is very important!

There are several ways of doing this.

One possible way is as follows: You can use user defined sources to impose a particular velocity inside the fan on most codes. (If you are using CFX you should search for the word "Dirichlet" in the CFX11 help system - this leads to the momentum source page of the manual. For other codes you will have to search yourself or ask in the correct forum) If you do this then the same air that goes into the fan comes out at the front, and you can be sure that the temperature coming out of the fan is correct. This would be my preferred method.

Another way to get the right inlet temperature is to couple the inlet temperature to the air temperature at the outlet using your code's expression language or by coupling it to Fortran code.

3) Don't forget that fans generate swirl and turbulence! You should try and assess if this will be important for your model.

Good luck, Andy

Hi, Andy,

Thanks for the reply!

I am using ELMER (www.csc.fi/elmer).

There is no outlet in the fluid domain. If, on the fan intake side, I want to use pressure BC, what pressure value should I use? This is a transient problem. Pressure could change due to change in temperature.

I calculate the average temperature on the fan intake side, and use it on the fan outlet side (will be inlet into the fluid domain). This is assuming that temperature change is negligible. In this case, I will calculate average temperature on the fan intake side at every iteration/time step. I am not sure if this will be stable.

I am also assuming swirling is not critical. I am more interested in general temperature distribution.

I am not sure what you mean by using Dirichlet BC if I mesh the volume occupied by the fan. Can you explain? I have no problem meshing the volume occupied by the fan, just don't know how to deal with it.

phsieh2005

I've got to say that tools such as FLOTHERM and ICEPAK have this capability already built in. You really would be better off using that type of application specific tool.

Hi, Robin,

Thanks for the suggestion. But, the purpose here is to learn/understand how to model internal fans.

phsieh2005

A thought that comes to mind is to cut your grid inside the fan housing and impose a pressure jump there.

I have done a similar thing in 2D to model a ceiling fan in a room, using divergence-free finite elements. These (Hermite) FE involve the stream function as well as the velocity components, and I imposed a difference in stream function at the nodes at the tip of the blades, which fixed the flow from/through the fan. With the divergence-free FEM the pressure is decoupled and not involved in the velocity computation, but this implies a pressure jump when the pressure is recovered from the velocity.