Hello, I am using StarCD for A/C system analysis and I am looking for ways to model the flow through a heating device that looks like a car radiator. I was thinking about considering it as a porous medium, like a filter... Does anyone have experience or ideas ? Thanks.

Alexis

(1). I don't know what you are trying to achieve with this code and analysis. (2). A car radiator is designed to cool the water, and it is a cooling device. (3). A porous medium is something like sand, filter material, soil, where the detailed structure is somewhat small and random in most cases. In other words, it is not practical to model the detail structure for the lack of information at that level. (4). I am sure that a heating device is designed based on certain principle of heat transfer. My suggestion is why not model the heating device as a heating device? (It would be easier to send a Fax of the heating device picture to the code vendor to find out whether the code can handle the heating device or not.) (5).I don't think that a heating device is designed as if it is a porous medium. What do you think?

Hi

I am currently modelling fan heat-exchanger combinations and have written computationally more cost effective fan and heat exchanger models. I have used porous cells with user-defined resistance characteristics to model the heat exchanger. Depending on the type of heat exchanger modelled inlet flow losses due to oblique flow at the heat exchanger inlet can affect your results, so care must be taken.

Hi John

I posted my messages without reading yours. It depends whether you want the detail flow through the heat exchanger or whether you want the flow in the cavity or plenum chamber in front of the heat exchanger. If the latter is what needs to be resolved then using a porous heat exchanger model is adequate to model the effect of the heat exchanger, of course you will have to do a detail flow analysis if you want to resolve the flow field through the heat exchanger. The model I use can also heat up the air that passes through the heat exchanger. My results seem to compare favourably with experimental data (my own experimental data I might add).

regards

Chris

Chris, as a matter of fact, I am not interested in the flow pattern inside the radiator but I want to get a rough idea of what's going on in the chamber. So the porous medium model sounds good. However, I don't know where to start as far as estimating resistance properties... How did you do it ? Thank you very much for your help. Alexis

(1). Yes, if you don't want to know the detail flow field through the heat exchanger, you can always replaced it with a model. (2). Then it becomes an experimental problem to determine the characteristics of the model. And each heat exchanger design is somewhat different, then it becomes problem specific. (3). It is not a bad idea at all to do detailed flow analysis through an element of the heat exchanger to get the flow characteristics, then use it in the model later to simplify the calculations.

Hi

Yes, I agree in principle. I would refer to your proposed method as the "Total CFD approach". Of course one must firstly assume that the CFD code can accurately resolve the flow phenomena within the heat exchanger passages. In most applications flow seperation would occur. Another assumption is that your computer resources have enough "capacity" to deal with such flow details and the larger and more complex grids. My circumstances are propably unique as I have experiemntal facilities at my disposal but only limited computing power.

I am not necessarily unhappy concerning my position as it forces me to find a balance between the use of CFD and the need for experimental work. In this case I believe a little experimental work coupled with a heat exchanger model thrown in with a smaller less complex grid would be a more elegant solution than an all-out CFD approach. I know this is very much dependant on ones circumstances.

Lengthy replies seems to be infectious when in discussion with John. Sorry about that.

Use porous media for the "device". The manufacturer typcially has the pressure drop versus flow rate so you can determine the alpha and betas.

To model the actual heat exchange can be quite detailed. I have seen for automobile heat exchangers the use of a volumetic source term in the porous cells. Since the heat exhange (on the air side) is a function of the local velocity, perhaps you can scale the heat source term appropriately for each cell in the porous cells so that the sum equals the total heat exhange

I have developed a total heat exchanger model that handles the air flow losses as well as the heat addition. I refrained from using heat sources in the porous cells themselves but rather specified temperatures in the cells at the heat exchanger exit. Of course my heat transfer relations were formulated in such a way as to facilitate this method. The average velocity (needed to determine the outlet temperature of a given cell) I simply got from looking at the velocities of the porous cells lying inbetween the inlet and outlet cell. Things become even more interesting when severe flow distortions take place through the heat exchanger (recirculating flow).

(1). If I were you, I would follow the same approach you took. (2). The name you mentioned "the total CFD approach" sometimes has a different name for it. It is called "brute force approach--the Rambo style". (just kidding). (3). What I should say is: there has been some attempts to model the loss characteristics using CFD for flow over a small portion of the radiator in great detail. But it is not always practical.