Hi

I want to specify both the temperature and heat flux at a modelled wall (its not a real wall, but a boundary for a porous reacting interface lying outside my Fluent model) Fluent doesn't allow this per se, but has anyone tried this using a udf to 'force' a specified heat flux.

I don't imagie anybody has, but if so please let me know.

Anybody got any ideas?, how to do it or approximate it with the existing options in Fluent??

Greg

Do you want to specify heat flux on both directions of the surface, or heat flux on one direction and temperature on the other? I have no experience with the former. The surface shadows are what you need for the latter.

Essentially I have a model with which I want to set the wall temperature and the heat flux from the surface. So the heat flux on the fluid side should be equal to that through the surface and on the other side.

I have set a wall temperature b/c and used the DEFINE_HEAT_FLUX uds to force the heat flux to the correct value by modifying in the heat transfer co-efficient. This seems to work.

In reality this is a coupled problem between a fluid and porous solid involving surface reaction. In this case the interface moves due to reaction and heat transfer (within te solid region drying, pyrolysis and thermo-mechanical breakdown of the solid all occur). These aspects are all too hard to model in fluent so I'm using a simple 1d heat balance model to force the right heat flux to account for the adverse mass flux, moving boundary and reaction at the wall.

I think this approach might work after playing around until 11pm last night. But one other question is - can one change the boundary condition's dynamically....

For example, below a critical temperature this could be a simple coupled heat transfer problem, but then above a critical temp, reaction kicks in and things get majorly painful (ie reaction, moving boundary). Because the wall temperature is governed by heat transfer from the fluid (actually a reacting packed bed), its a function of the solution.....anyway one step at a time!

I often wish I had a problem whre I could push some buttons on the gui ......

Thanks

Greg

(1). You need someone (like the GOD?) who knows ahead of the time what you will be doing, and develop a computer code for you, so that at the right time, it will be available to you. (2). If you fix the wall temperature, and also fix the heat flux, then in most cases, the temperature field is also known. (3). The problem basically is: people are using the pre-developed code for something beyond its capability. (day dreaming? I guess)

True, that fixes the temperature in the vicinity of the wall. But that doesn't necessarily fix the entire temperature field, unless the problem is simple (other constraints exist)??

True, also that this is a non-standard problem. I suppose there are three options (i) don't do the problem, (ii) use different code (your own maybe) or (iii) adapt fluent (or CFX, or your own) to do it.

Now (i) is easiest - but lets day that isn't an option.

Then we have to decide between (ii) and (iii). This is not that easy, although I know you don't trust anybody else's code. Fair enough.....

Greg

Just for clarification, the heat flux is not set to a constant value, but a value dependent upon the flow field temperature as well.

In essence Fluent would calculate the fluid side heat flux as

Qf = h*(Tcell - Twall) = k_fluid*dT/dn at wall

where wall is the wall temp and cell is adjacent fluid cell. Now this calculation by Fluent assumes a simple wall - ie no mass flux from the wall to the cell. If such a mass flux exists, then the heat transfer will be reduced. So we may say that we need to a new HTC as:

Qf_new = h_new*(Tcell - Twall)

where h_new depends upon the flow field near the wall. Similar arguments will hold if the wall is moving perpendicular to the fluid cell.

Greg

As long as you write a UDF you can have it dynamically change the heat flux. You just need to include an "if then" type statement.

I haven't given your problem too much thought but if you can get it to converge, I don't see why you couldn't force the heat flux as you proposed. Have you considered these other options: 1) Set the heat flux to your desired heat flux, then set the heat generation term such that the heat flux out = heat generated. This way you can indirectly force a certain temperature (in fact you can dynamically change the temperature by dynamically changing the heat generation term). 2) Set the wall temperature to your desired temperature (either constant or dynamically changing temperature), then set the heat generation term such that the heat flux out is adjusted to match your desired flux. 3) Model the entire porous zone yourself and have it as a UDF specifying heat flux and or mass flux at the porous boundaries. 4) Ignore the moving boundary term that you feel alters the heat flux, then let Fluent calculate everything as usual.

If you know the surface temperature and the heat flux, then you would be able to specify the cell temperature next to the wall:

q = -k*(T_wall - T_cell)/(delta n)

where I've assumed an orthogonal mesh. You could then write a user source term for the energy equation which would force the cell temperature to be that given in the above equation.

Their is an example of how to specify a value using user source terms; the example is to specify swirl to model a fan.

Thanks for your suggestions....

I have got a couple of things working:

a model as I originally proposed where I modify the HTC using a udf. This converges ok and exhibits the right qualitative behaviour - ie as fluid temperature increases, more water is evaporated, greater wall velocity etc.

I have already considered a case where I model surface reactions using udf's modified to allow the wall to be a reactant. In this case the wall velocity can be computed by how much solid is consumed. I then assumed that water evaporation is proportional to the solid consumption at the wall in order to determine the heat load behind the wall.

I haven't considered Scott's idea yet - but does anybody know how radiation fluxes are handled at a porous interface - ie can it be treated like a wall or is is treated as any other interior cell???? I couldn't find this in the manual.

Greg

I believe fluid-porous interfaces are treated like any other interior face.

[vikasy123]

i am not able to calculate heat flux in cfd post, it says error : heat flux not defined at this wall, any ideas!!